HEIDENHAIN TNC 620, User Manual

Page: 145 / 521

Tools | Tool data
Prerequisites for a tool change with M101
As replacement tools, use only tools with the same
radius. The control does not automatically check the
radius of the tool.
If you want the control to check the radius of the
replacement tool, enter
M108
in the NC program.
The control performs the automatic tool change at a suitable point in
the program. The automatic tool change is not performed:
During execution of machining cycles
While radius compensation (
RR
/
RL
) is active
Directly after an approach function
APPR
Directly before a departure function
DEP
Directly before and after
CHF
and
RND
During execution of macros
During execution of a tool change
Directly after a
TOOL CALL
or
TOOL DEF
During execution of SL cycles
Overtime for tool life
This function must be enabled and adapted by the
machine manufacturer.
The tool condition at the end of planned tool life depends on e.g.
the tool type, machining method and workpiece material. In the
OVRTIME
column of the tool table, enter the time in minutes for
which the tool is permitted to be used beyond the tool life.
The machine manufacturer specifies whether this column is enabled
and how it is used during tool search.
Tool usage test
Requirements
Refer to your machine manual.
The tool usage test function must be enabled by your
machine tool builder.
To conduct a tool usage test, you must activate
Create tool usage
files
in the MOD menu.
Further information: "Generating a tool usage file", Page 354
4
HEIDENHAIN | TNC 620 | User's Manual for Setup, Testing and Running NC Programs | 01/2022
145