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
Requirements
- Pole CC
You must define a pole CC before programming with polar coordinates.
- 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.
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 | |
F, FMAX, FZ, FU, FAUTO | |
M |
Notes
- The pole is not the center of the contour circle!
- The Form column allows toggling between the syntaxes for Cartesian and polar coordinate input.
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.
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 |