Fundamentals

Depending on the machine and kinematics, it is possible to perform both milling and turning operations on milling machines. A workpiece can thus be machined completely on one machine, even if complex milling and turning applications are required.

In a turning operation, the tool is in a fixed position, whereas the rotary table and the clamped workpiece rotate.

NC fundamentals for turning

The assignment of the axes with turning is defined so that the X coordinates describe the diameter of the workpiece and the Z coordinates the longitudinal positions.

Machining is thus always done in the ZX working plane. The machine axes to be used for the required movements depend on the respective machine kinematics and are determined by the machine manufacturer. NC programs with turning functions are largely independent of the machine kinematics.

Workpiece preset for turning operations

On the control, you can simply switch between milling and turning mode within your NC program. In turning mode, the rotary table serves as lathe spindle, whereas the milling spindle with the tool is fixed. This way, it is possible to machine rotationally symmetric contours. The tool reference point must always be at the center of the lathe spindle.

Preset management

If you use a facing head, you can set the workpiece preset to a different location, since in this case the tool spindle performs the turning operation.

Using a facing head with FACING HEAD POS (#50 / #4-03-1)

Production processes

Depending on the machining direction and task, turning applications can be subdivided into different production processes, e.g.:

  • Longitudinal turning
  • Face turning
  • Recess turning
  • Thread cutting

The control provides several cycles for each of the various production processes.

Mill-turning cycles (#50 / #4-03-1)

You can run the cycles with an inclined tool in order to produce undercuts.

Inclined turning

Tools for turning operations

When managing turning tools, other geometric descriptions than those for milling or drilling tools are required. The cutting-edge radius must be defined, for example, in order to apply cutter radius compensation. The control provides a special tool table for turning tools. In the Form workspace of the tool management, the control displays only the required parameters for the current tool type.

Tool parameters

Tool radius compensation (TRC) with lathe tools (#50 / #4-03-1)

You can correct turning tool values in the NC program.

The control offers the following functions for this:

Notes

 
Warning
Caution: Danger to the operator and machine!
Very high physical forces are generated during turning, for example due to high rotational speeds and heavy or unbalanced workpieces. Incorrect machining parameters, neglected unbalances or improper fixtures lead to an increased risk of accidents during machining!
  1. Clamp the workpiece in the spindle center
  2. Clamp workpiece securely
  3. Program low spindle speeds (increase as required)
  4. Limit the spindle speed (increase as required)
  5. Eliminate unbalance (calibrate)
  • The orientation of the tool spindle (spindle angle) depends on the machining direction. The tool tip is aligned to the center of the turning spindle for outside machining. For inside machining, the tool points away from the center of the turning spindle.
  • The direction of spindle rotation must be adapted when the machining direction (outside/inside machining) is changed.

  • Overview of miscellaneous functions

  • During turning, the cutting edge and the center of the turning spindle must be at the same level. During turning, the tool therefore has to be pre-positioned to the Y coordinate of the turning-spindle center.
  • In turning mode, diameter values are displayed on the X axis position display. The control then shows an additional diameter symbol.
  • The Positions workspace

  • In turning mode, the spindle potentiometer is active for the turning spindle (rotary table).
  • In turning mode, no coordinate conversion cycles are permitted except for the datum shift.
  • Datum shift with TRANS DATUM

  • In turning mode, the SPA, SPB and SPC transformations from the preset table are not permitted. If you activate one of these transformations, the control will display the Transformation not possible error message if executing the NC program in turning mode.
  • The control does not use the BLK FORM function to generate the traverse paths for the turning cycles (#50 / #4-03-1). In this case, define FUNCTION TURNDATA BLANK.
  • Blank form update in turning with FUNCTION TURNDATA BLANK (#50 / #4-03-1)

  • The machining times determined using the graphic simulation do not correspond to the actual machining times. Reasons for this during combined milling-turning operations include the switching of operating modes.
  • The Simulation workspace