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
- Programming a circular path with Cartesian coordinates
Requirement
- Pole CC
You must define a pole CC before programming with polar coordinates.
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.
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 | |
F, FMAX, FZ, FU, FAUTO | |
M |
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.
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+ |