Cartesian coordinates
With the G00 and G01 NC functions, you program a straight movement in rapid traverse or with a machining feed rate in any desired direction.
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.
N110 G00 Z+100 M3 | ; Straight line at rapid traverse |
N120 G01 X+20 Y-15 F200 | ; Straight line at machining feed rate |
If the feed rate was programmed using a numerical value, it is active only up to the NC block in which a new feed rate is programmed. G00 is active only for the NC block in which it was programmed. When the NC block programmed with G00 has been executed, the feed rate programmed most recently with a numerical value becomes active again.
Make sure to program rapid traverse movements exclusively with the G00 NC function instead of very high numerical values. This is the only way to ensure that rapid traverse is active on a block-by-block basis and that you can control rapid traverse independently of the machining feed rate.
G00 and G01 correspond to the L Klartext syntax with FMAX and F.