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.

Rotary axis positioning with MOVE

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.

Rotary axis positioning TURN

STAY

The control does not position any axes.

Rotary axis positioning with STAY

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.

 
Notice
Danger of collision!
The center of rotation is in the tool axis. In the case of large tool diameters, the tool may plunge into the material during tilting. During the tilting movement, there is a risk of collision!
  1. 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.

 
Tip

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.

 
Tip

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.

 
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.

Example

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.

 
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 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.

 
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 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.

 
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 PLANE SPATIAL SPA+45 SPB+0 SPC+0 STAY

Selecting STAY does not allow defining further syntax elements.

Note

 
Notice
Danger of collision!
The control does not automatically check whether collisions can occur between the tool and the workpiece. Incorrect or no pre-positioning before tilting the tool into position can lead to a risk of collision during the tilting movement!
  1. Program a safe position before the tilting movement
  2. Carefully test the NC program or program section in the Single Block mode