Fundamentals of turning cycles

 
Machine

Refer to your machine manual.

Machine and control must be specially prepared by the machine manufacturer for use of this cycle.

Option 50 must have been enabled.

8xx

The pre-positioning of the tool has a decisive influence on the workspace of the cycle and thus the machining time. During roughing, the starting point for cycles corresponds to the tool position when the cycle is called. When calculating the area to be machined, the control takes into account the starting point and the end point defined in the cycle or of the contour defined in the cycle. If the starting point is within the area to be machined, then the control positions the tool at the set-up clearance beforehand in some cycles.

The direction of stock removal is longitudinal to the rotary axis for Cycles 81x and transverse to the rotary axis for Cycles 82x. In Cycle 815, the movements are contour-parallel.

The cycles can be used for inside and outside machining. The control takes the information for this from the position of the tool or from the definition in the cycle.

Working with turning cycles

For cycles in which a defined contour is machined (Cycles 810, 820, and 815), the direction set when programming the contour determines the machining direction.

In cycles for turning you can specify the machining strategies of roughing, finishing or complete machining.

 
Notice
Danger of collision!
The turning cycles position the tool automatically to the starting point during finishing. The approach strategy is influenced by the position of the tool when the cycle is called. The decisive factor is whether the tool is located inside or outside an envelope contour when the cycle is called. The envelope contour is the programmed contour, enlarged by the set-up clearance. If the tool is within the envelope contour, the cycle positions the tool at the defined feed rate directly to the starting position. This can cause contour damage.
  1. Position the tool at a sufficient distance from the starting point to prevent the possibility of contour damage
  2. If the tool is outside the envelope contour, positioning to the envelope contour is performed at rapid traverse, and at the programmed feed rate within the envelope contour.
 
Tip

The control monitors the length of the cutting edge CUTLENGTH in the turning cycles. If the cutting depth programmed in the turning cycle is greater than the length of the cutting edge defined in the tool table, then the control issues a warning. In this case, the cutting depth will be reduced automatically in the machining cycle.

Execution with a FreeTurn tool

The control supports the execution of the contours with FreeTurn tools in the cycles 81x and 82x. This method allows you to perform the most common turning operation with just one tool. Thanks to the flexible tool, machining times can be reduced because the control does not need to change tools as much.

 
Notice
Danger of collision!
The shaft length of the turning tool limits the diameter that can be machined. There is a risk of collision during machining!
  1. Check the machining sequence in the simulation
 
Tip
  • The NC program remains unchanged except for the calling of the FreeTurn cutting edges.
  • Example: Turning with a FreeTurn tool

  • If you use a FreeTurn tool for machining, the control will internally switch the kinematics. This can lead to movements changing the positions of the cutting edge. In this case, the control will display a warning message.
  • If the control displays a warning message during simulation, HEIDENHAIN recommends that you run the program once without a workpiece. It is possible that the control does not display a warning during program run because the simulation does not show all movements, such as PLC positioning movements. The simulation may thus differ from the actual machining process.