Defining behavior when positioning parallel axes with FUNCTION PARAXCOMP
Application
The FUNCTION PARAXCOMP function is used to define whether the control takes parallel axes into account in the traversing movements with the associated main axis.
Description of function
If the FUNCTION PARAXCOMP 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 PARAXCOMP DISPLAY
Use the PARAXCOMP DISPLAY function to activate the display function for parallel axis movements. The control includes movements of the parallel axis in the position display of the associated main axis (sum display). Therefore, the position display of the main axis always displays the relative distance from the tool to the workpiece, regardless of whether you move the main axis or the parallel axis.
FUNCTION PARAXCOMP MOVE
The control uses the PARAXCOMP MOVE function to compensate for movements of a parallel axis by performing compensation movements in the associated main axis.
For example, if a parallel-axis movement is performed in the negative W-axis direction, the main axis Z is moved simultaneously in the positive direction by the same value. The relative distance from the tool to the workpiece remains the same. Application in gantry-type milling machines: Retract the spindle sleeve to move the cross beam down simultaneously.
FUNCTION PARAXCOMP OFF
Use the PARAXCOMP OFF function to switch off the PARAXCOMP DISPLAY and PARAXCOMP MOVE parallel axis functions.
The following actions cause the control to reset the PARAXCOMP parallel-axis function:
- Selection of NC program
- PARAXCOMP OFF
When FUNCTION PARAXCOMP is not active, the control does not display the corresponding icon and the additional information after the axis designations.
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 PARAXCOMP MOVE W | ; Compensate for movements of the W axis by means of a compensating movement in the Z axis |
The NC function includes the following syntax elements:
Syntax element | Meaning |
---|---|
FUNCTION PARAXCOMP | Syntax initiator for the behavior when positioning parallel axes |
DISPLAY, MOVE or OFF | Calculate the values of the parallel axis with the main axis, compensate for or do not take into account movements with the main axis |
X, Y, Z, U, V or W | Affected axis Optional syntax element |
Notes
- The PARAXCOMP MOVE function can be used only in connection with straight-line blocks (L).
- The control allows the use of one active PARAXCOMP function per axis only. If you define an axis both in PARAXCOMP DISPLAY and in PARAXCOMP MOVE, the last executed function will be active.
- Using offset values, you can define a parallel axis shift for the NC program (e.g., in the W axis). This allows machining of workpieces with different heights using the same NC program, for example.
Notes about machine parameters
The machine manufacturer uses the optional machine parameter presetToAlignAxis (no. 300203) to define for each axis how the control is to interpret offset values. For FUNCTION PARAXCOMP, the machine parameter applies to the parallel axes (U_OFFS, V_OFFS, and W_OFFS) only. If there are no offsets, the control behaves as described in the functional description.
Basic transformation and offset
- If the machine parameter has not been defined for the parallel axis or has been defined with FALSE, the offset is only active in the parallel axis. The preset of the programmed parallel-axis coordinates is shifted by the offset value. The coordinates of the main axis still reference the workpiece preset.
- If the machine parameter for the parallel axis has been defined with TRUE, the offset will be active in the parallel and main axes. The presets of the programmed parallel and main axis coordinates are shifted by the offset value.
Example
This example shows the effect of the optional machine parameter presetToAlignAxis (no. 300203)
Machining is done on a gantry-type milling machine using a spindle sleeve as the W axis (parallel to the main Z axis). The W_OFFS column of the preset table contains the value –10. The Z value of the workpiece preset is located at the machine datum.
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 Z+100 W+0 R0 FMAX M91 | ; Position the Z and W axes in the machine coordinate system M-CS |
12 FUNCTION PARAX COMP DISPLAY W | ; Activate the sum display |
13 L Z+0 F1500 | ; Position the Z axis at 0 |
14 L W-20 | ; Move the W axis to working depth |
In the first NC block, the control positions the Z and W axes relative to the machine datum, i.e. independent of the workpiece preset. In the RFACTL mode, the position display indicates the values Z+100 and W+0. In the ACTL. mode, the control takes W_OFFS into account and displays the values Z+100 and W+10.
In NC block 12, the control activates sum display for the ACTL. and NOML. modes of the position display. The control displays the movements of the W axis in the position display of the Z axis.
The result depends on the setting of the presetToAlignAxis machine parameter:
FALSE or not defined | TRUE |
---|---|
The control takes the offset into account in the W axis only. The value of the Z axis display remains unchanged. | The control takes the offset into account in the W and Z axes. The ACTL. display of the Z axis is changed by the offset value. |
Position-display values:
| Position-display values:
|
In NC block 13, the control moves the Z axis to the programmed coordinate 0.
The result depends on the setting of the presetToAlignAxis machine parameter:
FALSE or not defined | TRUE |
---|---|
The control moves the Z axis by 100 mm. | The coordinates of the Z axis reference the offset. To reach the programmed coordinate 0, the axis must move by 110 mm. |
Position-display values:
| Position-display values:
|
In NC block 14, the control moves the W axis to the programmed coordinate –20. The coordinates of the W axis reference the offset. To reach the programmed coordinate, the axis must move by 30 mm. Since the sum display has been activated, the control displays the movement in the ACTL. display of the Z axis as well.
The values in the position display depend on the setting of the presetToAlignAxis machine parameter:
FALSE or not defined | TRUE |
---|---|
Position-display values:
| Position-display values:
|
|
|
If you only move the W axis while the PARAXCOMP DISPLAY function is active, the control takes the offset into account only once, independent of the setting of the presetToAlignAxis machine parameter.