HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 462)

Programming: Turning Operations
14.4 Tools in turning mode (Option #50)
14
462
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
Tool compensation in the program
With FUNCTION TURNDATA CORR you can define additional
compensation values for the active tool. In FUNCTION TURNDATA
CORR 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.
FUNCTION TURNDATA CORR is always effective for the active
tool. A renewed
T deactivates compensation again. When you exit
the program (e.g. PGM MGT), the TNC automatically resets the
compensation values.
When you enter the function
FUNCTION TURNDATA CORR you can
specify by soft key the effect of the tool compensation:
FUNCTION TURNDATA CORR-TCS: The tool compensation is
effective in the tool coordinate system
FUNCTION TURNDATA CORR-WCS: The tool compensation is
effective in the workpiece coordinate system
Tool compensation FUNCTION TURNDATA CORR-
TCS is always effective in the tool coordinate system,
even during inclined machining.
Defining tool compensation:
Show the soft-key row with special functions
Select the menu for TURNING PROGRAM
FUNCTIONS
Select
FUNCTION TURNDATA
Select TURNDATA CORR
NC syntax
21 FUNCTION TURNDATA CORR-TCS:Z/X DZL:0.1 DXL:0.05
...