2 t ool d a ta – HEIDENHAIN TNC 410 User Manual

Page 64

HEIDENHAIN TNC 410

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 of the tool. The tool
must already be defined in a TOOL DEF block or in the
tool table.

Working spindle axis X/Y/Z: Enter the tool axis. Parallel
axes U, V and W are permitted.

Spindle speed S

Tool length oversize: Enter the delta value for the tool
length.

Tool radius oversize: Enter the delta value for the tool
radius.

Example:
Call tool number 5 in the tool axis Z with a spindle speed 2500 rpm.
The tool length is to be programmed with an oversize of 0.2 mm,
the tool radius with an undersize of 1 mm.

20 TOOL CALL 5 Z S2500 DL+0.2 DR-1

The character D preceding L and R designates delta values.

Tool preselection with tool tables
When you use a tool table, enter a TOOL DEF block to preselect the
next tool to be selected. Simply enter the tool number or a
corresponding Q parameter, or type a tool name in quotation marks.

Tool change

The tool change function can vary depending on the
individual machine tool. Your machine manual provides
more information on M101.

Tool change position
A tool change position must be approachable without collision. With
the miscellaneous functions M91 and M92, you can enter machine-
referenced (rather than workpiece-referenced) coordinates for the
tool change position. If TOOL CALL 0 is programmed before the
first tool call, the TNC moves the tool spindle in the tool axis to a
position that is independent of the tool length.

Manual tool change
To change the tool manually, stop the spindle and
move the tool to the tool change position:

Move to the tool change position under program
control.

Interrupt program run (see section 11.3 “Program
Run”).

Change the tool.

Resume the program run (see section 11.3
“Program Run”).

Automatic tool change
If your machine tool has automatic tool changing
capability, the program run is not interrupted. When
the TNC reaches a TOOL CALL, it replaces the
inserted tool by another from the tool magazine.

Automatic tool change if the tool life expires:
M101

This function can vary depending on the
individual machine tool. Your machine
manual provides more information on
M101.

The TNC automatically changes the tool if the tool
life TIME2 expires during program run. To use this
miscellaneous function, activate M101 at the
beginning of the program. M101 is reset with M102.

The tool is not always changed immediately, but,
depending on the workload of the control, a few NC
blocks later.

Prerequisites for standard NC blocks
with radius compensation R0, RR, RL
The radius of the replacement tool must be the
same as that of the original tool. If the radii are not
equal, the TNC displays an error message and does
not replace the tool.

5.2 T

ool D