FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 43

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 300 -

- Duration specification (LTM=1)

After all registered tool life management data is deleted, programmed
tool life management data is registered.
If a tool group command (T code) is specified, a tool whose life has
not expired is selected from the specified tool group. Then, life
management for the selected tool is started by a tool change command
(M06).    Life management (counting) is performed by measuring the
time during which the tool is actually used in the cutting mode at
regular intervals (every second or 0.1 second). The life count
interval is specified by bit 0 (FCO) of parameter No. 6805.    The time
required for single block stop, feed hold, rapid traverse, dwell,
machine lock, and interlock operations is not counted.
Setting bit 2 (LFV) of parameter No. 6801 enables the life count to be
overridden as directed by tool life count override signals.  An
override from 0 times to 99.9 times can be applied.  If 0 times is
specified, counting is not performed.

If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specification method as for the M series applies.
See the description for the M series.
The following explains the specification method for the turret type (bit
3 (TCT) of parameter No. 5040 = 0):

- Use count specification (LTM=0)

If a tool group command (T

○○

99 code) is issued, a tool whose life

has not expired is selected from the specified tool group, and the life
counter for the selected tool is incremented by one. Unless a tool life
count restart M code is specified, selection of a new tool and the
increment operation can be performed only if a tool group number
command and a tool change command are issued for the first time
since the entry of the control unit into the automatic operation start
state from the reset state.

CAUTION

No matter how many times the same tool group

number is specified in a program, the use count is
not incremented, and no new tool is selected.

- Duration specification (LTM=1)

If a tool group command (T

○○

99 code) is specified, a tool whose

life has not expired is selected from the specified tool group, and tool
management for the selected tool starts.
Life management (counting) is performed by measuring the time
during which the tool is actually used in the cutting mode at regular
intervals (every second or 0.1 second). The life count interval is
specified by bit 0 (FCO) of parameter No. 6805. The time required
for single block stop, feed hold, rapid traverse, dwell, machine lock,
and interlock operations is not counted.

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 301 -

Setting bit 2 (LFV) of parameter No. 6801 enables the life count to be
overridden according tool life count override signals. An override
from 0 times to 99.9 times can be applied. If 0 times is specified,
counting is not performed.

NOTE

1 When a tool is selected, tools are searched starting

from the current tool toward the last tool to find a
tool whose life has not expired. When the last tool
is reached during this search, the search restarts
from the first tool. If the search does find any tool
whose life has not expired, the last tool is selected.
When the tool currently used is changed by the tool
skip signal, the next new tool is selected using the
method described here.

2 If tool life counting indicates that the life of the last

tool in a group has expired, the tool change signal
is output. If the life count type is duration
specification, the signal is output as soon as the life
of the last tool in the group has expired. If the life
count type is use count specification, the signal is
output when the CNC is reset by a command such
as M02 or M30 or when the tool life count restart M
code is specified after the life of the last tool in the
group has expired.

3 If a T command is specified, a group and a tool in

the group are selected while the T command is
buffered. This means that if a block to be buffered
contains a T command specifying a group while
machining is being performed with that group
selected, the next T command is already buffered
even if the tool life expires during machining, so the
next tool is not selected. To prevent this, if the life
count type is duration specification and a T
command is to be specified to select the same
group successively, insert an M code for
suppressing buffering into a place immediately
before the T command.

4 When the tool life is counted, the remaining life of a

group (the life value minus the life counter value) is
compared with the remaining life setting, and the
status of the tool life expiration prior notice signal is
changed according to the result of the comparison.

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 302 -

- M99

If the life count is specified by use count and bit 0 (T99) of parameter
No. 6802 is 1, the tool change signal TLCH<Fn064.0> is output and
the automatic operation is stopped if the life of at least one tool group
has expired when the M99 command is executed. If the life count
type is duration specification, the tool change signal is output
immediately when the life of at least one tool group has expired; when
the M99 command is specified, the automatic operation is stopped, but
no more tool change signal is output.

If the life count is specified by use count, a tool group command (T
code) issued after the M99 command selects, from a specified group,
a tool whose life has not expired, and the next tool change command
(M06) increments the tool life counter by one.

If the life count is specified by use count, when a tool group command
(T code) is specified after the M99 command is specified, a tool
whose life has not expired is selected from a specified group, and the
tool life counter is incremented by one.
If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specifications as for the M series apply.

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 303 -

10.5.5

Tool Life Count Restart M Code

Explanation

If the life count is specified by use count, the tool change signal is
output if the life of at least one tool group has expired when a tool life
count restart M code is issued. A tool group command (T code)
issued after the tool life count restart M code selects, from a specified
group, a tool whose life has not expired, and the next tool change
command (M06) increments the tool life counter by one. This
enables the tool life to be counted by a tool change command (M06)
even if the command is not the first tool change command (M06)
issued since the entry of the CNC into the automatic operation start
state from the reset state. The tool life count restart M code is
specified in parameter No. 6811.

Example:

Suppose that M16 is a tool life count restart M code and that the
tool life management ignore number is 100.

Also suppose that the life count is specified by use count.

T101 ; A tool whose life has not expired is selected from group 1.

M06 ; Tool life management is performed for group 1.

(The tool life counter is incremented by one.)

T102 ; A tool whose life has not expired is selected from group 2.

M06 ; Tool life management is performed for group 2.

(The tool life counter is incremented by one.)

M16 ; Tool life counting is restarted.

T101 ; A tool whose life has not expired is selected from group 1.

M06 ; Tool life management is performed for group 1.

(The tool life counter is incremented by one.)

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 304 -

If the tool change type is the ATC type (bit 3 (TCT) of parameter No.
5040 = 1), the same specifications as for the M series apply.    See the
description for the M series.
The following explanation assumes that the tool change type is the
turret type (bit 3 (TCT) of parameter No. 5040 = 0).
If the life count is specified by use count, the tool change signal is
output if the life of at least one tool group has expired when a tool life
count restart M code is specified.    A tool group command (T code)
issued after the tool life count restart M code selects a tool whose life
has not expired from a specified group, and the tool life counter is
incremented by one.  This enables the tool life to be counted by a
tool group command (T code) even if the command is not the first tool
group command issued since the entry of the CNC into the automatic
operation start state from the reset state.    The tool life count restart M
code is specified in parameter No. 6811.

Example:

Suppose that M16 is a tool life count restart M code.

Also suppose that the life count is specified by use count.

T199 ; A tool whose life has not expired is selected from group 1.

Tool life management is performed for group 1.

(The tool life counter is incremented by one.)

T299 ; A tool whose life has not expired is selected from group 2.

Tool life management is performed for group 2.

(The tool life counter is incremented by one.)

M16 ; Tool life counting is restarted.

T199 ; A tool whose life has not expired is selected from group 1.

Tool life management is performed for group 1.

(The tool life counter is incremented by one.)

NOTE

1 The tool life count restart M code is treated as an M

code not involved in buffering.

2 If the life count type is use count specification, the

tool change signal is output if the life of at least one
tool group has expired when the tool life count
restart M code is specified. If the life count type is
duration specification, specifying the tool life count
restart M code causes nothing.

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 305 -

10.5.6

Disabling Life Count

Explanation

If bit 6 (LFI) of parameter No. 6804 is “1”, the tool life count disable
signal LFCIV can be used to select whether to cancel the tool life
count.

If the tool life count disable signal LFCIV is “1”, the tool life count
disabled signal LFCIF becomes “1”, and the tool life count is
disabled.
If the tool life count disable signal LFCIV is “0”, the tool life count
disabled signal LFCIF becomes “0”, and the tool life count is enabled.

NOTE

No buffering should occur when the state of the
tool life count disable signal LFCIV is changed.
So, use, for example, M codes not involved in
buffering to change the signal state. If M06 (for
the M series) or a tool change T code (for the T
series) is issued in a block that follows directly a
block in which an auxiliary function code with
buffering enabled is used to turn on or off the tool
life count disable signal LFCIV, it is likely that a
command for specifying whether to count may
become incorrect.

11.AUXILIARY FUNCTION

PROGRAMMING

B-63944EN/03

- 306 -

AUXILIARY FUNCTION

Overview

There are two types of auxiliary functions ; auxiliary function (M
code) for specifying spindle start, spindle stop, program end, and so
on, and secondary auxiliary function (B code) for specifying index
table positioning.
When a move command and auxiliary function are specified in the
same block, the commands are executed in one of the following two
ways:
(1) Simultaneous execution of the move command and auxiliary

function commands.

(2) Executing auxiliary function commands upon completion of

move command execution.

The selection of either sequence depends on the machine tool builder's
specification. Refer to the manual issued by the machine tool builder
for details.

Chapter 11, "AUXILIARY FUNCTION", consists of the following
sections:

11.1  AUXILIARY FUNCTION (M FUNCTION).........................307
11.2  MULTIPLE M COMMANDS IN A SINGLE BLOCK.........308
11.3  M CODE GROUPING FUNCTION ......................................309
11.4  SECOND AUXILIARY FUNCTIONS (B CODES) .............314

B-63944EN/03

PROGRAMMING

11.AUXILIARY FUNCTION

- 307 -

11.1

AUXILIARY FUNCTION (M FUNCTION)

When a numeral is specified following address M, code signal and a
strobe signal are sent to the machine. The machine uses these signals
to turn on or off its functions.
Usually, only one M code can be specified in one block. Depending
on the setting of bit 7 (M3B) of parameter No. 3404, up to three M
codes can be specified.
Which M code corresponds to which machine function is determined
by the machine tool builder. The machine processes all operations
specified by M codes except those specified by M98, M99,M198 or
called subprogram(Parameter No.6071 to 6079), or called custom
macro (Parameter No.6080 to 6089). Refer to the machine tool
builder's instruction manual for details.

Explanation

The following M codes have special meanings.

- M02,M30 (End of program)

This indicates the end of the main program.
Automatic operation is stopped and the CNC unit is reset. (This differs
with the machine tool builder.)
After a block specifying the end of the program is executed, control
returns to the start of the program.
Bits 5 (M02) and 4 (M30) of parameter No. 3404 can be used to
disable M02, M30 from returning control to the start of the program.

- M00 (Program stop)

Automatic operation is stopped after a block containing M00 is
executed. When the program is stopped, all existing modal
information remains unchanged. The automatic operation can be
restarted by actuating the cycle operation. (This differs with the
machine tool builder.)

- M01 (Optional stop)

Similarly to M00, automatic operation is stopped after a block
containing M01 is executed. This code is only effective when the
Optional Stop switch on the machine operator's panel has been
pressed.

- M98 (Calling of subprogram)

This code is used to call a subprogram. The code and strobe signals
are not sent. See the subprogram II-13.3 for details.

- M99 (End of subprogram)

This code indicates the end of a subprogram.
M99 execution returns control to the main program. The code and
strobe signals are not sent. See the subprogram section II-13.3 for
details.

Content .. 41 42 43 44 ..