Circular path C

Application

You use the circular path function C to program a circular path around a circle center point.

Requirement

Description of function

The control moves the tool on a circular path from the current position to the defined end point. The starting point is the end point of the preceding NC block. You can use at most two axes to define the new end point.

If you want to program a full circle, then define the same coordinates for the starting and end point. These points must lie on the circular path.

 
Tip

In the machine parameter circleDeviation (no. 200901) you can define the permissible deviation of the circle radius. The maximum permissible deviation is 0.016 mm.

With the direction of rotation you define whether the control moves along the circular path in a clockwise or counterclockwise direction.

Definition of the direction of rotation:

  • Clockwise: direction of rotation DR– (with radius compensation RL)
  • Counterclockwise: direction of rotation DR+ (with radius compensation RL)

Input

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 C X+50 Y+50 LIN_Z-3 DR- RL F250 M3

; Circular path with linear Z-axis superimpositioning

To navigate to this function:

Insert NC function All functions Path contour C

The NC function includes the following syntax elements:

Syntax element

Meaning

C

Syntax initiator for a circular path around a circle center

X, Y, Z, A, B, C, U, V, W

End point of the circular path

Number or numerical parameter

Entry: absolute or incremental

Optional syntax element

LIN_X, LIN_Y, LIN_Z, LIN_A, LIN_B, LIN_C, LIN_U, LIN_V or LIN_W

Axis and value of the linear superimposition

Number or numerical parameter

Entry: absolute or incremental

Linear superimpositioning of a circular path

Optional syntax element

DR

Rotational direction of the arc

Optional syntax element

R0, RL, RR

Tool radius compensation

Tool radius compensation

Optional syntax element

F, FMAX, FZ, FU, FAUTO

Feed rate

Feed rate F

Number or numerical parameter

Optional syntax element

M

M function

Miscellaneous Functions

Number or numerical parameter

Optional syntax element

Note

Example

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.

5 CC X+25 Y+25

6 L X+45 Y+25 RR F200 M3

7 C X+45 Y+25 DR+