HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 187)

Tool data 5.2
5
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
187
Caution: Danger to the workpiece and tool!
Switch off the automatic tool change with M102 if
you are working with special tools (e.g. side mill
cutter) because the TNC at first always moves the
tool away from the workpiece in tool axis direction.
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 element
BT (block tolerance)
If you enter the
M101 function, the TNC continues the dialog by
requesting the BT. Here you define the number of NC blocks (1
- 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 TNC uses the value 1 or, if applicable, a default value
defined by the machine manufacturer.
The more you increase 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 output value for
BT use the
formula
BT = 10 : Average machining time of an
NC block in seconds . Round up to the next odd
integer. 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.
The
M101 function is not available for turning tools
and in turning mode.
Prerequisites for NC blocks with surface-normal vectors and
3-D compensation
The active radius ( R + DR) of the replacement tool must not
differ from the radius of the original tool. You can enter the delta
values (
DR) either in the tool table or in the T block. If there are
any deviations, 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.