Circle calculation folder

Application

In the Circle calculation folder of the Insert NC function window, the control provides the functions FN 23 and FN 24.

These functions allow you to calculate the center of the circle and the radius of the circle from the coordinates of three or four circle points, for example the position and size of a partial circle.

Description of function

The Circle calculation folder contains the following functions:

Icon

Function

ProgramFn23Icon

FN 23: Determining the CIRCLE DATA from three points
Example: FN 23: Q20 = CDATA Q30

ProgramFn24Icon

FN 24: Determining the CIRCLE DATA from four points
Example: FN 24: Q20 = CDATA Q30

You save the coordinates in the working plane of the respective points in consecutive variables. You must save the coordinates of the main axis before the coordinates of the secondary axis, e.g. X before Y for tool axis Z.

Designation of the axes on milling machines

Circle calculation with three circle points

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.

11 FN 23: Q20 = CDATA Q30

The coordinate pairs of three points on a circle must be saved in Q30 and the five subsequent parameters—in this case, up to Q35.

The control then saves the circle center in the principal axis (X if spindle axis is Z) in parameter Q20, the circle center in the minor axis (Y if spindle axis is Z) in parameter Q21, and the circle radius in parameter Q22.

Circle calculation with four circle points

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.

11 FN 24: Q20 = CDATA Q30

The coordinate pairs of four points on a circle must be saved in parameter Q30 and the seven subsequent parameters—in this case, up to Q37.

The control then saves the circle center in the principal axis (X if spindle axis is Z) in parameter Q20, the circle center in the minor axis (Y if spindle axis is Z) in parameter Q21, and the circle radius in parameter Q22.

Note

Note that FN 23 and FN 24 automatically overwrite the resulting parameter and the two following parameters.