Compensating turning tools with FUNCTION TURNDATA CORR (#50 / #4-03-1)

Application

With FUNCTION TURNDATA CORR you can define additional compensation values for the active tool. In the TURNDATA CORR FUNCTION you can enter delta values for tool lengths in the X direction DXL and in the Z direction DZL. The compensation values have an additive effect on the compensation values from the turning tool table.

The compensation can be defined in the tool coordinate system T-CS or in the working plane coordinate system WPL-CS.

Reference systems

Requirements

Description of function

The coordinate system in which the compensation is active can be defined:

  • FUNCTION TURNDATA CORR-TCS: Tool compensation is active in the tool coordinate system
  • FUNCTION TURNDATA CORR-WPL: Tool compensation is active in the workpiece coordinate system

With FUNCTION TURNDATA CORR-TCS you can define a cutter radius oversize DRS. This enables you to program an equidistant contour oversize. DCW allows you to correct the recessing width of a recessing tool.

Tool compensation FUNCTION TURNDATA CORR-TCS is always active in the tool coordinate system, even during inclined machining.

FUNCTION TURNDATA CORR is always effective for the active tool. A renewed TOOL CALL deactivates compensation again. When you exit the NC program, the control automatically resets the compensation values.

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 TURNDATA CORR-TCS:Z/X DZL:+0.1 DXL:+0.05 DCW:+0.1

; Tool compensation in Z direction, X direction and for the width of the recessing tool

To navigate to this function:

Insert NC function All functions Special functions Turning tool compensation TURNDATA

The NC function includes the following syntax elements:

Syntax element

Meaning

FUNCTION TURNDATA CORR

Syntax initiator for tool compensation of a turning tool

CORR-TCS:Z/X or CORR-WPL:Z/X

Tool compensation in the tool coordinate system T-CS or in the working plane coordinate system WPL-CS

DZL:

Delta value for the tool length in Z direction

Optional syntax element

DXL: or
DXL-DIAM:

Delta value for the tool length in X direction, given as a radius or diameter value

DXL-DIAM: only if CORR-WPL:Z/X has been selected

Optional syntax element

DCW:

Delta value for the recessing tool width

Only if CORR-TCS:Z/X was selected

Optional syntax element

DRS:

Delta value for the cutter radius

Only if CORR-TCS:Z/X was selected

Optional syntax element

Note

The control shows delta values from the tool management graphically in the simulation. For delta values from the NC program or from compensation tables, the control changes only the position of the tool in the simulation.

The values of the function FUNCTION TURNDATA CORR take the effect of delta values from the NC program.

Note in connection with the interpolation turning (#96 / #7-04-1)

During interpolation turning, the functions FUNCTION TURNDATA CORR and FUNCTION TURNDATA CORR-TCS are not active.

If you want to compensate for a turning tool in Cycle 292 CONTOUR.TURNG.INTRP., compensation needs to be performed in the cycle or in the tool table.

Cycle 292 CONTOUR.TURNG.INTRP. (#96 / #7-04-1)