Circular path CP around pole CC

Application

You use the circular path function CP to program a circular path around the defined pole.

Related topics

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.

The distance from the starting point to the pole is automatically both the polar coordinate radius PR as well as the radius of the circular path. You define the polar coordinate angle PA that the control moves to with this radius.

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 CP PA+50 Z-2 DR- RL F250 M3

; Circular path

To navigate to this function:

Insert NC function All functions Path contour C

The NC function includes the following syntax elements:

Syntax element

Meaning

CP

Syntax initiator for a circular path around a pole

PA

Polar coordinate angle

Number or numerical parameter

Entry: absolute or incremental

Optional syntax element

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

Notes

  • The Form column allows toggling between the syntaxes for Cartesian and polar coordinate input.
  • If you define PA incrementally, you must define the direction of rotation with the same algebraic sign.
  • Consider this behavior when importing NC programs from earlier controls, and adapt the NC programs if necessary.

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.

18 LP PR+20 PA+0 RR F250 M3

19 CC X+25 Y+25

20 CP PA+180 DR+