Circular path CT
Application
You use the circular path function CT to program a circular path that connects tangentially to the previously programmed contour element.
Related topics
- Programming a tangential connecting circular path with polar coordinates
Requirement
- Previous contour element programmed
Before you can program a circular path with CT you must program a contour element to which the circular path can connect tangentially. This requires at least two NC blocks.
Description of function
The control moves the tool on a circular path, with a tangential connection, from the current position to the defined end point. The starting point is the end point of the preceding NC block. You can use at most two axes to define the new end point.
When contour elements uniformly merge into another without kinks, 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 CT X+50 Y+50 LIN_Z-2 RL F250 M3 | ; Circular path with linear Z-axis superimpositioning |
To navigate to this function:
Insert NC function All functions Path contour CT
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
CT | Syntax initiator for a circular path with a tangential connection |
X, Y, Z, A, B, C, U, V, W | End point of the circular path Number or numerical parameter Entry: absolute or incremental Optional syntax element |
LIN_X, LIN_Y, LIN_Z, LIN_A, LIN_B, LIN_C, LIN_U, LIN_V or LIN_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 |
R0, RL, RR | |
F, FMAX, FZ, FU, FAUTO | |
M |
Note
- The contour element and the circular path should contain both coordinates of the plane in which the circular path is executed.
- 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.
7 L X+0 Y+25 RL F300 M3 |
8 L X+25 Y+30 |
9 CT X+45 Y+20 |
10 L Y+0 |