HEIDENHAIN TNC 426 B User Manual page 93

Tool change
The tool change function can vary depending on the
individual machine tool. Refer to your machine tool
manual.
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 11.4 "Program Run").
Change the tool.
Resume the program run (see section 11.4 "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. Refer to your machine tool manual.
The TNC automatically changes the tool if the tool life TIME1
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.
HEIDENHAIN TNC 426 B, TNC 430
www.EngineeringBooksPdf.com
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.
Prerequisites for NC blocks with
surface-normal vectors and 3-D compensation
(see Chapter 5.4 „Three-Dimensional Tool
Compensation")
The radius of the replacement tool can differ from
the radius of the original tool. The tool radius is not
included in program blocks transmitted from CAD
systems. You can enter the delta value (DR) either in
the tool table or in the TOOL CALL block.
If DR is positive, the TNC displays an error message
and does not replace the tool. You can suppress this
message with the M function M107 , and reactivate it
with M108.
77