Tool Change - HEIDENHAIN TNC 620 User Manual

4

Tool change

Automatic tool change
Refer to your machine manual.
The tool change function can vary depending on the
individual machine tool.
If your machine tool has automatic tool changing capability, the
program run is not interrupted. When the control reaches a tool call
with TOOL CALL, it replaces the inserted tool by another from the
tool magazine.
Automatic tool change if the tool life expires: M101
Refer to your machine manual.
The function of M101 can vary depending on the
individual machine tool.
When the specified tool life has expired, the control can
automatically insert a replacement tool and continue machining
with it. Activate the miscellaneous function M101 for this. M101 is
reset with M102.
Enter the respective tool life after which machining is to be
continued with a replacement tool in the TIME2 column of the tool
table. In the CUR_TIME column the control enters the current tool
life.
If the current tool life is higher than the value entered in the TIME2
column, a replacement tool will be inserted at the next possible
point in the program no later than one minute after expiration of
the tool life. The change is made only after the NC block has been
completed.
Danger of collision!
During an automatic tool change with M101, the control always
retracts the tool in the tool axis first. There is danger of collision
when retracting tools for machining undercuts, such as side
milling cutters or T-slot milling cutters!
Deactivate the tool change with M102
After the tool change the control positions the tool according to
the following logic, unless otherwise specified by the machine tool
builder:
If the target position in the tool axis is below the current
position, the tool axis is positioned last
If the target position in the tool axis is above the current
position, the tool axis is positioned first
138
NOTICE
HEIDENHAIN | TNC 620 | User's Manual for Setup, Testing and Running NC Programs | 10/2018
Tools | Tool data