HEIDENHAIN ITNC 530 User Manual page 177

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
The function of M101 can vary depending on the individual
machine tool. The machine tool manual provides further
information.
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 changed automatically
after the net NC block after expiration of the tool life, or
at latest one minute after tool life expires (calculation is for a
potentiometer setting of 100%)
If the tool life ends during an active M120 (look ahead),
the TNC waits to change the tool until after the block in
which you canceled the radius compensation with an R0
block.
The TNC automatically changes the tool even if a fixed
cycle is being run.
The TNC does not automatically change the tool as long
as a tool change program is running.
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 "Three-Dimensional Tool Compensation (Software Option 2),"
page 182. 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 greater than zero, 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.
HEIDENHAIN iTNC 530 177