Circular path CTP

Application

You use the CTP function to program a circular path with polar coordinates that connects tangentially to the previously programmed contour element.

Related topics

  • Programming a tangentially connecting circular path with Cartesian coordinates
  • Circular path CT

Requirements

  • Pole CC
  • You must define a pole CC before programming with polar coordinates.

  • Polar coordinate datum at pole CC

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

Description of function

The control moves the tool on a circular path, with a tangential connection, from the current position to the end point defined with polar coordinates. The starting point is the end point of the preceding NC block.

When contour elements uniformly merge into another, without kinks or corners, 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 CTP PR+30 PA+50 Z-2 DR- RL F250 M3

; Circular path

To navigate to this function:

Insert NC function All functions Path contour CT

The NC function includes the following syntax elements:

Syntax element

Meaning

CTP

Syntax initiator for a circular path with a tangential connection

PR

Polar coordinate radius

Number or numerical parameter

Entry: absolute or incremental

Optional syntax element

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

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.

12 L X+0 Y+35 RL F250 M3

13 CC X+40 Y+35

14 LP PR+25 PA+120

15 CTP PR+30 PA+30

16 L Y+0