Calling The Tool Data - HEIDENHAIN TNC 640 User Manual

6

Calling the tool data

Before you can call the tool, you have to define it in a TOOL DEF
block or in the tool table.
A TOOL CALL 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). Alternatively, you can define
the feed rate in millimeters per revolution (mm/1)
by pressing the FU soft key or in millimeters per
tooth (mm/tooth) by pressing FZ. The feed rate is
effective until you program a new feed rate in a
positioning block or in a TOOL CALL 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 TOOL CALL block without specifying the tool axis,
then only the spindle speed will change.
If the tool axis is also entered in the TOOL CALL
block, the control will insert a replacement tool if a
replacement tool was defined.
258
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
Tools | Tool data