HEIDENHAIN TNC 320 - Calling the tool data

Tools | Tool data
5
222
HEIDENHAIN | TNC 320 | ISO Programming User's Manual | 10/2017
Calling the tool data
Before you can call the tool, you have to define it in a G99 block or
in the tool table.
A T in the NC program is programmed with the following data:
Press the TOOL CALL key
Tool number: Enter the number or name of the
tool. With the TOOL NAME soft key you can enter
a name. With the QS soft key you enter a string
parameter. The control automatically places the
tool name in quotation marks. You have to assign
a tool name to a string parameter first. Names
always refer to an entry in the active tool table
TOOL .T.
Alternative: Press the SELECT soft key
The control opens a window where you can
select a tool directly from the TOOL.T tool table.
To call a tool with other compensation values,
enter a decimal point followed by the index you
defined in the tool table.
Working spindle axis X/Y/Z: Enter the tool axis
Spindle speed S: Enter the spindle speed S in
revolutions per minute (rpm) Alternatively, you
can define the cutting speed Vc in meters per
minute (m/min). Press the VC soft key
Feed rate F: Enter feed rate F in millimeters per
minute (mm/min). The feed rate is effective until
you program a new feed rate in a positioning
block or in a T block
Tool length oversize DL: Enter the delta value
for the tool length
Tool radius oversize DR: Enter the delta value
for the tool radius
Tool radius oversize DR2: Enter the delta value
for the tool radius 2
If the number of the already inserted tool is entered in
the T block without specifying the tool axis, then only
the spindle speed will change.
If the tool axis is also entered in the T block, the control
will insert a replacement tool if a replacement tool was
defined.