Cycle 10 ROTATION

ISO programming

G73

Application

Within an NC program, the control can rotate the coordinate system in the working plane about the active datum.

The ROTATION cycle takes effect as soon as it has been defined in the NC program. It is also in effect in the Manual operating mode in the MDI application. The active angle of rotation is shown in the additional status display.

Reference axis for the rotation angle:

  • X/Y plane: X axis
  • Y/Z plane: Y axis
  • Z/X plane: Z axis

Reset

Program Cycle 10 ROTATION again and specify a rotation angle of 0°.

Notes

  • This cycle can be executed only in the FUNCTION MODE MILL machining mode.
  • Cycle 10 cancels an active radius compensation. If necessary, reprogram the radius compensation.
  • After defining Cycle 10, move both axes of the working plane to activate the rotation for all axes.

Cycle parameters

Help graphic

Parameter

Rotation angle?

Enter the angle of rotation in degrees (°). Enter the value as an incremental or absolute value.

Input: –360.000...+360.000

NC programs contained in this User's Manual are suggestions for solutions. The NC programs or individual NC blocks must be adapted before being used on a machine.

Change the following contents as needed:

  • Tools
  • Cutting parameters
  • Feed rates
  • Clearance height or safe position
  • Machine-specific positions (e.g., with M91)
  • Paths of program calls

Some NC programs depend on the machine kinematics. Adapt these NC programs to your machine kinematics before the first test run.

In addition, test the NC programs using the simulation before the actual program run.

 
Tip

With a program test you determine whether the NC program can be used with the available software options, the active machine kinematics and the current machine configuration.

Example

11 CYCL DEF 10.0 ROTATION

12 CYCL DEF 10.1 ROT+35