FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 37

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 252 -

- Multi-path system

The tool management data and cartridge management table are
common data among the paths. The spindle management table and
standby position table, however, are treated as independent data for
each path.
When the spindle table or standby position table is specified as a
cartridge from the PMC window, specify the following, in which the
path number is set in the hundred’s place:

Spindle position

First Second Third Fourth

First path

111(11)

112(12) 113(13) 114(14)

Second

path

211 212 213 214

Third

path

311 312 313 314

Fourth

path

411 412 413 414

Fifth

path

511 512 513 514

Sixth

path

611 612 613 614

Seventh

path

711 712 713 714

Eighth

path

811 812 813 814

Ninth

path

911 912 913 914

Tenth

path

1011 1012 1013 1014

Standby position

First Second Third Fourth

First path

121(21)

122(22) 123(23) 124(24)

Second

path

221 222 223 224

Third

path

321 322 323 324

Fourth

path

421 422 423 424

Fifth

path

521 522 523 524

Sixth

path

621 622 623 624

Seventh

path

721 722 723 724

Eighth

path

821 822 823 824

Ninth

path

921 922 923 924

Tenth

path

1021 1022 1023 1024

NOTE

When specifying 111, 121, and so on to specify the
first path, you may specify just 11, 21, and so on.

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 253 -

Tool management data

- Data of each tool such as type number, life status, and compensation number
- The number of sets of data is 64, 240, or 1000.

Cartridge management table

- This table indicates the cartridge and pot to which each set of tool management

data is assigned.

- Up to four cartridges are used.

Path 1

Path 10

Path 2

Standby position table

121 to 124 (21 to 24)

Spindle position table

111 to 114 (11 to 14)

Standby position table

221 to 224

Spindle position table

211 to 214

Standby position table

1021 to 1024

Spindle position table

1011 to 1014

. . . . . . . . . . .

- M/T series

The tool management data and cartridge management table are data
common to the M and T series.

- Tool life management and tool change

The CNC performs tool life management, regarding tools having the
same tool type number as a group.  When a tool type number (T
code) is specified by an NC program, the tool management data
registered in the CNC is searched to find a tool having the shortest life
among the tools with the same tool type number.
The cartridge number and pot number corresponding to the searched
tool are output as a T code signal to the PMC.    Based on the output
cartridge number and pot number, the PMC performs preparation for a
tool change (to the next tool).    A different tool can also be selected
on the PMC side.
The CNC performs tool life counting for each tool that is at a spindle
position in the spindle management table.

When the lives of all tools having the tool type number specified by
the T code have expired, alarm PS5317 is issued.    If there is a tool in
the spindle position or standby position, that tool is selected to
continue machining.
As the T code signal, a specified tool type number instead of the
cartridge number and pot number can also be output directly by
parameter setting.

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 254 -

There are two types of tool life management counting methods:
counting the number of use times and counting cutting time.    One of
the counting methods is set in tool information of tool management
data.

Other major specifications related to tool life management are as
follows:
Tool type number (T code):  Up to 8 digits (1 to 99,999,999)
Maximum tool life value:

99,999,999 times when the number of use times is specified

999 hours 59 minutes 59 seconds when time is specified

Life count interval when time is specified:

1 second

Tool life management count restart M code:

Enabled

Tool life count override:

Enabled

To specify a certain tool directly without performing tool life
management by tool type number, use the following format:

M (value in parameter No. 13252) T (cartridge number) (pot
number) ;

When parameter No. 13252 is set to 333, the cartridge number is 2,
and the pot number is 27, for example, the following command is
specified:

M333 T20027;

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 255 -

- Tool search order

Tools having a tool type number (T) specified by a program are
searched sequentially from tool management data number 1 while
registered data contents are checked. The following shows how a
search operation is made within the NC:

Is tool management data valid (is bit 0 (RGS) of tool information set to 1)?

Is tool being edited?

Does tool type number (T) match with specified number?

Is tool registered in cartridge (is cartridge number non-zero value)?

Is cartridge targeted for search (are bits 0 to 3 of parameter No. 13203 set to 0)?

Is tool registered at spindle position or standby position of another path?

Does tool life status indicate that tool management is not performed (0)?

Is tool excluded from management target a search target (is bit 4 (SEN) of tool information 1)?

Search end

Does tool life status indicate that life expired (3)?

Does tool life status indicate tool breakage (4)?

Regard tool with smallest remaining life or customize data value as candidate.
Bit 6 (SWC) of parameter No. 13203 (0: Check remaining life, 1: Check customize data)

Check of next tool?

Search end

Yes

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 256 -

- System variables

The following tool management data of the tool being used as a
spindle after a tool change by M06 and the tool to be used next which
is specified by a T code can be read through custom macro variables:

Being

used

Item

#8401

Tool management data number

#8402

Tool type number (T)

#8403

Tool life counter

#8404

Maximum tool life value

#8405

Tool notice life value

#8406

Tool life status

#8407

Customize data 0 (bit)

#8408 Tool

information

#8409

Tool length compensation number (H)

#8410

Cutter compensation number (D)

#8411

Spindle speed (S)

#8412

Cutting feedrate (F)

#8413

Tool geometry compensation number (G)

#8414

Tool wear compensation number (W)

#8431

Customize data 1

#8432

Customize data 2

#8433

Customize data 3

#8434

Customize data 4

#8435

Customize data 5

#8436

Customize data 6

#8437

Customize data 7

#8438

Customize data 8

#8439

Customize data 9

#8440

Customize data 10

#8441

Customize data 11

#8442

Customize data 12

#8443

Customize data 13

#8444

Customize data 14

#8445

Customize data 15

#8446

Customize data 16

#8447

Customize data 17

#8448

Customize data 18

#8449

Customize data 19

#8450

Customize data 20

#8451

Customize data 21

#8452

Customize data 22

#8453

Customize data 23

#8454

Customize data 24

#8455

Customize data 25

#8456

Customize data 26

#8457

Customize data 27

#8458

Customize data 28

#8459

Customize data 29

#8460

Customize data 30

#8461

Customize data 31

#8462

Customize data 32

#8463

Customize data 33

For machining
center systems

For lathe systems

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 257 -

Being

used

Item

#8464

Customize data 34

#8465

Customize data 35

#8466

Customize data 36

#8467

Customize data 37

#8468

Customize data 38

#8469

Customize data 39

#8470

Customize data 40

When a cartridge number of a spindle position (11 to 14) or standby
position (21 to 24) is specified in #8400, information about the
corresponding position can be read.
If the spindle position table or standby position table has an empty pot,
<empty> is read from #8402 to #8470.
Value 0 is read from #8401 (data number).

Therefore, machining conditions registered in tool management data
can be specified directly by coding, for example, D#8410, H#8409,
S#8411, and F#8412 with a tool change macro (such as M06).
Similarly, customize data can be referenced by a custom macro, and
machining programs can be customized according to the tool used.

NOTE

For the maximum number of tool management
function customization data items, refer to the
relevant manual issued by the machine tool builder.

10.TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63944EN/03

- 258 -

- Specifying a tool compensation number

When parameter No. 13265 is 0, a compensation number registered as
tool management data of a tool attached at a spindle position can be
selected by specifying H99 or D99.
(99 is treated as a special number, so 99 cannot be specified directly as
a compensation number.)
When other than 0 is set in parameter No. 13265, the number set in the
parameter can be specified instead of 99. For example, if parameter
No. 13265 is 3, specifying H3 specifies the tool length compensation
number registered for the tool at the spindle position.

When the tool management function is not used, a tool compensation
number is specified also with a T code; when the tool management
function is used, the T code is used only to specify a tool type number,
so a tool compensation number must be specified with address D.
Except the specifications for addresses, the specifications for the
number of permissible digits (parameter No. 3032) and the number of
digits consisting of a compensation number (parameter No. 5028),
separation of geometry compensation numbers and wear
compensation numbers (bit 1 (LGN) of parameter No. 5002), and so
on are the same as for T.

If parameter No. 13265 is set to 0, when a compensation number
registered for a tool attached at a spindle position is specified, the
specification format varies according to the number of digits as
follows, which is the same as for conventional T:
When the compensation number is 1 digit long:    D9
When the compensation number is 2 digits long:    D99
When the compensation number is 3 digits long:    D999
Because 9, 99, or 999 is treated as a special number, it cannot be
specified directly as a compensation number.
Unless parameter No. 13265 is set to 0, the number set in the
parameter can be specified instead of 9, 99, or 999.    When parameter
No. 13265 is set to 3, specifying D3 specifies the tool geometry
compensation number and tool wear compensation number registered
for a tool attached at the spindle position.

Multi-path system

Depending on whether the local path is a machining center system or a
lathe system, tool compensation numbers are specified by using one of
the above methods.

B-63944EN/03

PROGRAMMING

10.TOOL FUNCTION (T FUNCTION)

- 259 -

Spindle selection

When specifying compensation numbers of a tool attached to a spindle
other than the first spindle, specify the spindle number with address P
within the same block that contains H/D.    When specifying the first
spindle, you can omit P.
D99 P3;   Specifying compensation numbers registered for the tool
attached at the third spindle
D99   ; Specifying compensation numbers registered for the tool
attached at the first spindle

- Read/write operations for tool management data and cartridge management table

The tool management data and cartridge management table can be
read from and written to by using the CNC/PMC data window library
(FOCAS2).    Therefore, a specific tool management system including
all available tool data not registered in the CNC can be built easily by
using the OPEN CNC.

Similarly, the tool management data and cartridge management table
can also be read from and written to using the PMC window.

Tool management data of the tool being used as a spindle after a tool
change operation performed by M06 and the tool being selected by
specifying a T code can be read using a custom macro.

The user can modify tool management data by MDI from the tool
management function screen of the CNC.  Addition, modification,
and deletion of the above tool management data can be made from a
part program (G10).    Such data can also be input to and output from
external I/O equipment by using the ALL I/O screen and tool
management function screen.

- G10 format

Addition, modification, and deletion are performed for the tool
management data and cartridge management table from programs.
For use of this function, the programmable data input option function
is required.
If a format error is found in the commands from G10 L75/L76/L77 to
G11, or if a value beyond the valid data range is specified, alarm
PS5312 is issued.    In such a case, correct the program.    Within the
range from G10 to G11, no decimal point can be specified with any
address.    If a decimal point is specified, alarm PS0007 results.

Content .. 35 36 37 38 ..