HEIDENHAIN TNC 620 (340 56x-01) - Manual (Page 133)

HEIDENHAIN TNC 620 133
5.2 T
ool D
a
ta
Calling tool data
A TOOL CALL block in the part program is defined with the following
data:
 Select the tool call function with the TOOL CALL key.
 Tool number: Enter the number or name of the tool.
The tool must already be defined in a TOOL DEF block
or in the tool table. The TNC automatically places the
tool name in quotation marks. The tool name always
refers to the entry in the active tool table TOOL.T. If
you wish to call a tool with other compensation
values, also enter the index you defined in the tool
table after the decimal point. To select a tool from the
tool table, press the SELECT soft key. The TNC
shows the contents of the tool table. Use the arrow
keys to select a tool, and press OK to transfer it to the
pocket table
 Working spindle axis X/Y/Z: Enter the tool axis.
 Spindle speed S: Enter the spindle speed directly in
rpm. Alternatively, you can define the cutting speed
Vc in m/min. Press the VC soft key.
 Feed rate F : F [mm/min or 0.1 inch/min] is effective
until you program a new feed rate in a positioning or
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.
Example: Tool call
Call tool number 5 in the tool axis Z with a spindle speed of 2500 rpm
and a feed rate of 350 mm/min. The tool length is to be programmed
with an oversize of 0.2 mm, the tool radius 2 with an oversize of
0.05 mm, and the tool radius with an undersize of 1 mm.
The character D preceding L and R designates delta values.
Tool preselection with tool tables
If you are working with tool tables, use TOOL DEF to preselect the next
tool. Simply enter the tool number or a corresponding Q parameter, or
type the tool name in quotation marks.
20 TOOL CALL 5.2 Z S2500 F350 DL+0.2 DR-1 DR2+0.05