Compensating turning tools with FUNCTION TURNDATA CORR (option 50)

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

Requirement

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 compensate 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 in effect for the active tool. A renewed TOOL CALL deactivates compensation. When you exit the NC program (e.g. with PGM MGT), 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

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:

Delta value for the tool length in X direction

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

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

If you wish to compensate for a turning tool in Cycle 292 CONTOUR.TURNG.INTRP., then you must perform this in the cycle or in the tool table.

Cycle 292 CONTOUR.TURNG.INTRP. (option 96)