Select three linear axes for machining with FUNCTION PARAXMODE

Application

Use the PARAXMODE function to define the axes the control is to use for machining. You program all traverses and contour descriptions in the main axes X, Y and Z, independent of your machine.

Requirement

Description of function

If the PARAXMODE function is active, the control uses the axes defined in the function to execute the programmed traverses. If the control is to move the main axis deselected by PARAXMODE, you can identify this axis by additionally entering the & character. The & character then refers to the main axis.

Moving the main axis and the parallel axis

Define three axes with the PARAXMODE function (e.g., FUNCTION PARAXMODE X Y W) to be used by the control for programmed traverses.

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.

The Positions workspace

FUNCTION PARAXMODE OFF

Use the PARAXMODE OFF function to deactivate the parallel-axis function. The control then uses the main axes defined by the machine manufacturer.

The control resets the PARAXMODE ON parallel-axis function via the following functions:

  • Selection of an NC program
  • End of program END PGM
  • 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.

 
Tip

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 main 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.

Straight line L

To traverse a deselected main axis:

    1. Select L

    1. Define coordinates
    2. Select deselected main axis (e.g., &Z)
    3. Enter a value
    4. Define the radius compensation, if necessary
    5. Define the feed rate, if necessary
    6. Define a miscellaneous function, if necessary
    7. Confirm your input

    Notes

    • You must deactivate the parallel-axis functions before switching the machine kinematics.
    • In order for the control to offset the main axis deselected with PARAXMODE, enable the PARAXCOMP function for this axis.
    • Additional positioning of a main 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.
    • Position displays

    Notes about machine parameters

    • In the machine parameter noParaxMode (no. 105413), you define whether the control provides the functions PARAXCOMP and PARAXMOVE.
    • 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).
      • If the machine parameter has not been defined for the main axis or has been defined with FALSE, the offset only applies to the axis programmed with &. The coordinates of the parallel axis still reference the workpiece preset. Despite the offset, the parallel axis will move to the programmed coordinates.
      • If the machine parameter for the main axis has been defined with TRUE, the offset applies to the main axis and the parallel axis. The presets of the main and parallel axis coordinates are shifted by the offset value.