Fundamentals of path functions
Application
When creating an NC program, you can use the path functions to program the individual contour elements. To do so, use coordinates to define the end points of the contour elements.
The control then uses the coordinate entries, the tool data, and the radius compensation to calculate the traverse path. The control simultaneously positions all machine axes that you programmed in the NC block of a path function.
Description of function
Inserting a path function
The gray path function keys initiate the dialog. The control inserts the NC block in the NC program and prompts you for each piece of necessary information.
Depending on the design of the machine tool, either the tool moves or the machine table moves. When programming a path function, you always assume that the tool is in motion.
Motion in one axis
If the NC block contains one coordinate, the control moves the tool parallel to the programmed machine axis.
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.
L X+100 |
The tool retains the Y and Z coordinates and moves to the position X+100.
Motion in two axes
If the NC block contains two coordinates, the control moves the tool in the programmed plane.
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.
L X+70 Y+50 |
The tool retains the Z coordinate and moves in the XY plane to the position X+70 Y+50.
You define the working plane by entering the tool axis when calling the tool with TOOL CALL.
Motion in more than two axes
If the NC block contains three coordinate entries, the control moves the tool spatially to the programmed position.
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.
L X+80 Y+0 Z-10 |
Depending on the kinematics of your machine, you can program up to six axes in a linear L block.
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.
L X+80 Y+0 Z-10 A+15 B+0 C-45 |
The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message.
If the axis position does not change, you can nevertheless program more than four axes.
Circles and arcs
Use the path functions for circular arcs to program circular motions in the working plane.
The control moves the tool in two axes simultaneously on a circular path relative to the workpiece. You can program circular paths with a circle center point CC.
Direction of rotation DR for circular motions
When a circular path has no tangential transition to another contour element, define the direction of rotation as follows:
- Clockwise direction of rotation: DR–
- Counterclockwise direction of rotation: DR+
Tool radius compensation
Tool radius compensation is defined in the NC block of the first contour element.
Do not activate tool radius compensation in an NC block for a circular path. Activate tool radius compensation in a preceding straight line.
Pre-positioning
- Program a suitable pre-position
- Check the sequence and contour with the aid of the graphic simulation