Circular path CR

Application

You use a radius to program a circular path with the circular path function CR.

Description of function

The control moves the tool on a circular path, with the radius R, 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.

The starting and end points can be connected with four different circular paths of the same radius. The correct circular path is defined with the CCA center angle of the circular path radius R and the direction of rotation DR.

The algebraic sign of the circular path radius R is decisive for whether the control selects a center angle that is greater than or less than 180°.

The radius has the following effects on the center angle:

  • Smaller circular path: CCA<180°
  • Radius with a positive sign R>0

  • Longer circular path: CCA>180°
  • Radius with a negative sign R<0

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)

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.

10 L X+40 Y+40 RL F200 M3

11 CR X+70 Y+40 R+20 DR-

; Circular path 1

or

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 CR X+70 Y+40 R+20 DR+

; Circular path 2

or

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 CR X+70 Y+40 R-20 DR-

; Circular path 3

or

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 CR X+70 Y+40 R-20 DR+

; Circular path 4

For a full circle, program two circular paths in succession. The end point of the first circular path is the starting point of the second. The end point of the second circular path is the starting point of the first.

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 CR X+50 Y+50 R+25 LIN_Z-2 DR- RL F250 M3

; Circular path with linear Z-axis superimpositioning

To navigate to this function:

Insert NC function All functions Path contour CR

The NC function includes the following syntax elements:

Syntax element

Meaning

CR

Syntax initiator for a circular path with a radius

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

R

Radius of an arc

Number or numerical parameter

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

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

The distance between the starting and end points must not be greater than the circle diameter.