Straight line LP

Application

With the straight line function LP you program a straight traverse motion in any direction using polar coordinates.

Related topics

Requirement

Description of function

The control moves the tool in a straight line from its current position to the defined end point. The starting point is the end point of the preceding NC block.

You define the straight line with the polar coordinate radius PR and the polar coordinate angle PA. The polar coordinate radius PR is the distance from the end point to the pole.

The algebraic sign of PA depends on the angle reference axis:

  • If the angle from the angle reference axis to PR is counterclockwise: PA>0
  • If the angle from the angle reference axis to PR is clockwise: PA<0

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 LP PR+50 PA+0 R0 FMAX M3

; Straight line without radius compensation in rapid traverse

To navigate to this function:

Insert NC function All functions Path contour LP

The NC function includes the following syntax elements:

Syntax element

Meaning

LP

Syntax initiator for a straight line with polar coordinates

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

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.

12 CC X+45 Y+25

13 LP PR+30 PA+0 RR F300 M3

14 LP PA+60

15 LP IPA+60

16 LP PA+180