HEIDENHAIN TNC 426 B User Manual page 92

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. To call a tool by the tool name,
enter the name in quotation marks. The tool name
always refers to the entry in the active tool table
TOOL .T.
Working spindle axis X/Y/Z: Enter the tool axis.
Spindle speed S: Enter the spindle speed directly or
allow the TNC to calculate the spindle speed if you are
working with cutting data tables. Press the S
CALCULATE AUTOMAT. soft key. The TNC limits the
spindle speed to the maximum value set in MP 3515.
Feed rate F: Enter the feed rate directly or allow the
TNC to calculate the feed rate if you are working with
cutting data tables. Press the F CALCULATE AUTO-
MAT. soft key. The TNC limits the feed rate to the
maximum feed rate of the „longest axis" (set in MP
1010). F is effective until you program a new feed rate
in a positioning block or a TOOL CALL block.
Tool length oversize: Enter the delta value for the tool
length.
Tool radius oversize: Enter the delta value for the tool
radius.
Tool radius oversize 2: Enter the delta value for the
tool radius 2.
Example:
Call tool number 5 in the tool axis Z with a spindle speed 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.
20 TOOL CALL 5 Z S2500 F350 DL+0.2 DR-1 DR2:+0.05
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.
76
www.EngineeringBooksPdf.com
5 Programming: Tools