Use the PARAXMODE function to define the axes the control is to use for machining. You program all traverse movements and contour descriptions in the principal axes X, Y and Z, independent of your machine.
Application
Requirement
- Parallel axis is calculated
If your machine manufacturer has not yet activated the PARAXCOMP function as default, you must activate PARAXCOMP before you can work with PARAXMODE.
Defining behavior when positioning parallel axes with FUNCTION PARAXCOMP
Description of function
If the PARAXMODE function is active, the control uses the axes defined in the function to execute the programmed traverse movements. If the control is to move the principal axis deselected by PARAXMODE, you can identify this axis by additionally entering the character &. The & character then refers to the principal axis.
Moving the principal axis and the parallel axis
Define 3 axes in the PARAXMODE function (e.g. FUNCTION PARAXMODE X Y W) to be used by the control for programmed traverse movements.
If the FUNCTION PARAXMODE function is active, the control displays an icon in the Positions workspace. The icon for FUNCTION PARAXMODE may cover an active icon for FUNCTION PARAXCOMP.
FUNCTION PARAXMODE OFF
Use the PARAXCOMP OFF function to switch off the parallel-axis function. The control then uses the principal axes defined by the machine manufacturer.
- The control resets the PARAXMODE ON parallel-axis function via the following functions:
- Selection of NC program
- End of program
- M2 and M30
- PARAXMODE OFF
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 FUNCTION PARAX MODE X Y W | ; Execute programmed traversing movements with axes X, Y and W. |
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION PARAX MODE | Syntax initiator for axis selection for machining |
OFF | Deactivate the parallel axis function Optional syntax element |
X, Y, Z, U, V or W | Three axes for machining Only for FUNCTION PARAX MODE |
Moving the principal axis and the parallel axis
If the PARAXMODE function is active, you can traverse the deselected main axis with the & character within the straight line L.
| ||
| ||
|
Notes
- You must deactivate the parallel-axis functions before switching the machine kinematics.
- You can deactivate the programming of parallel axes with the machine parameter noParaxMode (no. 105413).
- In order for the control to offset the principal axis deselected with PARAXMODE, switch the PARAXCOMP function on for this axis.
- Additional positioning of a principal axis with the & command is done in the REF system. If you have set the position display to display ACTUAL values, this movement will not be shown. If necessary, switch the position display to REF values.
- Your machine manufacturer will define the calculation of possible offset values (X_OFFS, Y_OFFS and Z_OFFS from the preset table) for the axes positioned with the & operator in the presetToAlignAxis machine parameter (no. 300203).