HEIDENHAIN TNC 620 User Manual page 131

Tools | Tool data
Input parameter BT (block tolerance)
Depending on the NC program, the machining time can increase as a
result of the tool life verification and calculation of the automatic tool
change. You can influence this with the optional input parameter BT
(block tolerance).
If you enter the M101 function, the control continues the dialog by
requesting BT. Here you define the number of NC blocks (1 to 100)
by which the automatic tool change may be delayed. The resulting
time period by which the tool change is delayed depends on the
content of the NC blocks (e.g. feed rate, path). If you do not define
BT, the control uses the value 1 or, if applicable, a default value
defined by the machine manufacturer.
The higher the value of BT, the smaller will be the effect
of an extended program duration through M101. Please
note that this will delay the automatic tool change!
To calculate a suitable initial value for BT, use the
following formula:
t: average machining time of an NC block in seconds
Round the result up to an integer value. If the calculated
result is greater than 100, use the maximum input value
of 100.
If you want to reset the current age of a tool (e.g. after
changing the indexable inserts), enter the value 0 in the
CUR_TIME column.
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
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022
4
131