HEIDENHAIN TNC 640 (34059x-05) - Manual (Page 498)

Programming: Turning Operations
14.4 Tools in turning mode (Option #50)
14
498
TNC 640 | User's Manual
HEIDENHAIN Conversational 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
TOOL CALL 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
...