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 traverse movements and contour descriptions in the principal 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 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.

Positions workspace

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.

 
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 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.

Straight line L

  1. To traverse a deselected main axis:
L

  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.
  • 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.
  • Position displays

  • 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).