Fundamentals of coordinate definitions
You program a workpiece by defining the path contours and the target coordinates.
Depending on the dimensioning used in the technical drawing, you use Cartesian or polar coordinates with absolute or incremental values.
Cartesian coordinates
Application
A Cartesian coordinate system consists of two or three axes that are all mutually perpendicular. Cartesian coordinates are relative to the datum (origin) of the coordinate system, which is at the intersection of the axes.
With Cartesian coordinates you can uniquely specify a point in space by defining the three axis values.
Description of function
In the NC program you define the values in the linear axes X, Y, and Z, such as with a straight line L.
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 L X+60 Y+50 Z+20 RL F200 |
The programmed coordinates are modally effective. As long as the value of an axis remains the same, you do not need to program the value for further path contours.
Polar coordinates
Application
You define polar coordinates in one of the three planes of a Cartesian coordinate system.
Polar coordinates are relative to a previously defined pole. From this pole you define a point by its distance to the pole and the angle to the angle reference axis.
Description of function
Polar coordinates can be used in, for example, the following situations:
- Points on circular paths
- Workpiece drawings with angular information, such as bolt hole circles
You define the pole CC with Cartesian coordinates in two axes. These axes specify the plane and the angle reference axis.
The pole is modally effective within an NC program.
The angle reference axis is related to the plane as follows:
Plane | Angle reference axis |
---|---|
XY | +X |
YZ | +Y |
ZX | +Z |
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 CC X+30 Y+10 |
The polar coordinate radius PR is relative to the pole. PR defines the distance of this point from the pole.
The polar coordinate angle PA defines the angle between the angle reference axis and this point.
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 LP PR+30 PA+10 RR F300 |
The programmed coordinates are modally effective. As long as the value of an axis remains the same, you do not need to program the value for further path contours.
Absolute input
Application
Absolute input always references an origin. For Cartesian coordinates, the origin is the datum and for polar coordinates the origin is the pole and the angle reference axis.
Description of function
Absolute values define the target point for positioning.
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 L X+10 Y+10 RL F200 M3 | ; Position at point 1 |
12 L X+30 Y+20 | ; Position at point 2 |
13 L X+50 Y+30 | ; Position at point 3 |
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 CC X+45 Y+25 | ; Define the pole with two axes using Cartesian coordinates |
12 LP PR+30 PA+0 RR F300 M3 | ; Position at point 1 |
13 LP PA+60 | ; Position at point 2 |
14 LP PA+120 | ; Position at point 3 |
15 LP PA+180 | ; Position at point 4 |
Incremental entries
Application
Incremental input always references the previously programmed coordinates. For Cartesian coordinates these are the values in the X, Y and Z axes, and for polar coordinates the values of the polar coordinate radius PR and the polar coordinate angle PA.
Description of function
Incremental entries define the value by which the control positions. The previously programmed coordinates serve as the respective datum of the coordinate system.
You define incremental coordinates with an I before each axis designation.
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 L X+10 Y+10 RL F200 M3 | ; Position to point 1 absolutely |
12 L IX+20 IY+10 | ; Position to point 2 incrementally |
13 L IX+20 IY+10 | ; Position to point 3 incrementally |
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 CC X+45 Y+25 | ; Define the pole absolutely in two axes with Cartesian coordinates |
12 LP PR+30 PA+0 RR F300 M3 | ; Position to point 1 absolutely |
13 LP IPA+60 | ; Position to point 2 incrementally |
14 LP IPA+60 | ; Position to point 3 incrementally |
15 LP IPA+60 | ; Position to point 4 incrementally |