Tool Compensation In The Program - HEIDENHAIN TNC 640 User Manual

Turning | Tools in turning mode (option 50)

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.
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.
FUNCTION TURNDATA CORR is always effective for the active tool.
A renewed T deactivates compensation again. When you exit the
program (e.g. with PGM MGT), the control automatically resets the
compensation values.
When you enter the TURNDATA CORR FUNCTION you can specify
the effect of the tool compensation with a soft key:
FUNCTION TURNDATA CORR-TCS: The tool compensation is
effective in the tool coordinate system
FUNCTION TURNDATA CORR-WPL: 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.
Define the tool compensation:
Show the soft-key row with special functions
Press the TURNING PROGRAM FUNCTIONS soft
key
Press the FUNCTION TURNDATA soft key
Press the TURNDATA CORR soft key.
Example
N210 FUNCTION TURNDATA CORR-TCS:Z/X DZL:0.1 DXL:0.05*
...
HEIDENHAIN | TNC 640 | ISO Programming User's Manual | 10/2017
16
637