Tool Life, Replacement Tool - HEIDENHAIN TNC 415 Technical Manual

15.1.2 Tool life, replacement tool

The operator is able to specify two different tool lives (TIME1 and TIME2) and a replacement tool
(RT) for every tool in the tool table.
If on TOOL CALL the current tool life (CUR.TIME) is greater than TIME2, the pocket number or tool
number (MP7480) of the replacement tool is automatically downloaded. If TIME2 is greater than
zero and no replacement tool is defined, a TOOL CALL for the replacement tool provokes the error
message "MAX. TOOL LIFE EXPIRED" when this time elapses.
If the current tool life is greater than TIME1, the NC sets flag M2094. Further action can be defined
by the machine tool manufacturer (e.g. output a PLC error message).
With the M function M101, the tool can be replaced automatically after a certain service life (TIME 1
or TIME 2). The replacement tool is not installed exactly when tool life ends but can vary by several
NC blocks depending on processor capacity. A T strobe M2046 is sent to the PLC and marker
M2404 is set. With automatic replacement tool installation (M101) the same radius must be defined
for the replacement tool as for the original tool in standard NC programs (NC blocks with RR, RL or
R0).
No radius correction is defined in NC blocks with surface-normal vectors. A delta value (DR, DL) for
length and radius can be defined for each tool in the tool table. The TNC uses these delta values in
NC programs with surface-normal vectors. If the radius of the replacement tool differs from that of
the original tool, then this must be defined in the "DR" field in the tool table. The delta value must
always be negative. If a positive delta value is defined then the error message "Tool radius too large"
will appear. This error message can be reset by M-function M107. M107 is reset by M108.
MP7680 can define whether the oversize for the tool radius (DR2) is considered when calculating
tool length for NC blocks with surface-normal vectors.
The current tool life is only counted from TOOL CALL to TOOL CALL in the automatic modes
("Program run/Single block" and "Program run/Full sequence"). It does not matter whether the spindle
is turning or the machine is traversing. The tool life counter does not stop until the program is
interrupted with "Internal Stop", M02, M30 or END PGM.
The tool life counter does not run in the manual modes ("Manual Operation", "El. Handwheel" and
"Positioning with manual input").
The operator can reset the current tool life by entering zero.
Marker Function
M2094 Maximum tool life elapsed
(TIME1 in tool table)
MP7680 Machine parameters with multiple function
Entry: %xxxxxxx
Bit 6
01.98 TNC 407/TNC 415/TNC 425
Tool length for blocks with surface normal vector
0 = Without DR2 from the tool table
1 = With DR2 from the tool table
15 Tool changer
Set Reset
NC NC; PLC
4-227