Rotary axis positioning
Application
The type of rotary axis positioning defines how the control tilts the rotary axes to the calculated axis values.
The selection depends in part on the aspects below:
- Is the tool near the workpiece during tilting to position?
- Is the tool at a safe tilting position during tilting to position?
- May and can the rotary axes be positioned automatically?
Description of function
The control offers three types of rotary axis positioning from which one must be selected.
Type of rotary axis positioning | Meaning |
---|---|
MOVE | If you perform tilting near the workpiece, then use this option. |
TURN | If the workpiece is so large that the range of traverse is not sufficient for the compensating movement of the linear axes, then use this option. |
STAY | The control does not position any axes. |
Rotary axis positioning with MOVE
The control positions the rotary axes and performs compensation movements in the linear main axes.
The compensation movements ensure that the relative position between the tool and the workpiece will not change during the positioning process.
The TNC7 basic can move up to four axes simultaneously. If an NC block commands movement of more than four axes, the control displays an error message. Note that the compensating movement is performed in up to three linear axes.
- Ensure sufficient distance between the tool and the workpiece
When DIST is not defined or when you define the value 0, the center of rotation and consequently the center of the compensation movements is in the tool tip.
When you define DIST with a value greater than 0, the center of rotation in the tool axis is shifted away from the tool tip by this value.
If you wish to tilt about a certain point on the workpiece, ensure the following:
- Prior to tilting to position, the tool is positioned directly above the desired point on the workpiece.
- The value defined in DIST matches exactly the clearance between the tool tip and the desired center of rotation.
Rotary axis positioning TURN
The control positions only the rotary axes. The tool must be positioned after tilting to position.
Rotary axis positioning with STAY
Both the rotary axes and the tool must be positioned after tilting to position.
Even with STAY, the control orients the working plane coordinate system WPL-CS automatically.
When selecting STAY, the rotary axes must be tilted to position in a separate positioning block after the PLANE function.
In the positioning block, use only the axis angles calculated by the control:
- Q120 for the axis angle of the A axis
- Q121 for the axis angle of the B axis
- Q122 for the axis angle of the C axis
The variable avoids entry and calculating errors. In addition, no changes are required after changing the values within the PLANE functions.
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 A+Q120 C+Q122 FMAX |
Input
MOVE
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 PLANE SPATIAL SPA+45 SPB+0 SPC+0 MOVE DIST0 FMAX |
Selecting MOVE allows defining the syntax elements below:
Syntax element | Meaning |
---|---|
DIST | Distance between center of rotation and the tool tip Input: 0...99999999.9999999 Optional syntax element |
F, F AUTO or FMAX | Feed rate definition for automatic rotary axis positioning Optional syntax element |
TURN
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 PLANE SPATIAL SPA+45 SPB+0 SPC+0 TURN MB MAX FMAX |
Selecting TURN allows defining the syntax elements below:
Syntax element | Meaning |
---|---|
MB | Retraction in the current tool axis direction before positioning the rotary axis Values with an incremental effect can be entered or a retraction up to the traverse limit can be defined by selecting MAX. Input: 0...99999999.9999999 or MAX Optional syntax element |
F, F AUTO or FMAX | Feed rate definition for automatic rotary axis positioning Optional syntax element |
STAY
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 PLANE SPATIAL SPA+45 SPB+0 SPC+0 STAY |
Selecting STAY does not allow defining further syntax elements.
Note
- Program a safe position before the tilting movement
- Carefully test the NC program or program section in the Single Block mode