Circular path CT

Application

You use the circular path function CT to program a circular path that connects tangentially to the previously programmed contour element.

Related topics

  • Programming a tangential connecting circular path with polar coordinates
  • Circular path CTP

Requirement

  • Previous contour element programmed
  • Before you can program a circular path with CT you must program a contour element to which the circular path can connect tangentially. This requires at least two NC blocks.

Description of function

The control moves the tool on a circular path, with a tangential connection, 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.

When contour elements uniformly merge into another without kinks, then this transition is referred to as tangential.

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 CT X+50 Y+50 LIN_Z-2 RL F250 M3

; Circular path with linear Z-axis superimpositioning

To navigate to this function:

Insert NC function All functions Path contour CT

The NC function includes the following syntax elements:

Syntax element

Meaning

CT

Syntax initiator for a circular path with a tangential connection

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

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 contour element and the circular path should contain both coordinates of the plane in which the circular path is executed.
  • The Form column allows toggling between the syntaxes for Cartesian and polar coordinate input.
  • The Form column in the Program workspace

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.

7 L X+0 Y+25 RL F300 M3

8 L X+25 Y+30

9 CT X+45 Y+20

10 L Y+0