Content .. 245 246 247 248 ..

FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION) - page 247

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1930 -

The CNC is in a mode other than the JOG, HNDL (INC), or REF mode.

The CNC is at an emergency stop.

The reset button on the MDI unit is held pressed.

A reset signal is input from the machine side.

The CNC is in an alarm condition.

The CNC is undergoing automatic operation (start, pause, or stop).

The CNC is in the tool-noose radius compensation mode (G41/G42 mode).

With this function, shifted coordinate systems are returned to the previous state by the first T code in the
next session of automatic operation, and axis movement occurs by the amount of canceled shifting, thus
resuming the position and coordinate systems of the inherent movement type.

Example:

If the amounts of wear compensation are: T1 = 0.1, T2 = 0.2, and T3 = 0.4
1)

The state that T1 compensation is applied during automatic operation (compensation of 0.1 axis
movement type):

The coordinate system is shifted by -0.1 (= T2 - T1) from the state mentioned in step 1 when
tool T2 is selected in manual tool compensation.

When compensation T3 is applied again during automatic operation, the coordinate system is
shifted by 0.2 (= T3 - T2), that is, totally by 0.3. The coordinate system, which has been shifted
by -0.1 in step 2, is shifted back to the previous state.

Once the T3 compensation command has been executed, the same position and coordinate system as
would be when the T3 compensation command is issued in the T1 compensation state are resumed.

When manual tool compensation ends properly, the T code modal changes to one where manual tool
compensation was carried out (the tool function code signals T00 to T31<Fn026 to Fn029> also change).

11.1.6

Y Axis Offset

Overview

When the Y axis, one of the basic three axes, is used with a lathe system, this function performs Y axis
offset.
When tool geometry/wear compensation is enabled (bit 6 (NGW) of parameter No.8136 is 0), both tool
geometry offset and tool wear offset are effective to Y axis offset. This function is enabled when bit 1
(YOF) of parameter No. 8132 is set to 1.

Explanation

Y axis offset results in the same operation as tool offset. For an explanation of the operation, related
parameters, and the like, refer to the item “Tool Offset.”

11.1.6.1

Support of arbitrary axes for Y axis offset

Overview

In a lath system, Y axis offset has been usable with the basic three axes only. This function enables Y axis
offset to be used with arbitrary axes other than the Y axis, which is one of the basic three axes.

Parameter

5043

Axis number for which Y-axis offset is used

[Input type] Parameter input

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1931 -

[Data type] Byte path

[Valid data range] 0 to 24

Set the number of an axis for which Y-axis offset is used.
If 0 or a value beyond the valid data range is set, the Y-axis offset is applied to the Y-axis
of the basic three axes. If setting is made for the X- or Z-axis of the basic three axes, the
standard tool offset for the X- or Z-axis is not used, and only the Y-axis offset is used.

11.1.7

4th/5th Axis Offset

Overview

This function enables tool offset for the 4th axis and 5th axis following the basic three axes (X, Y, and Z
axes). As with tool offsets based on the basic three axes (X, Y, and Z axes), 32 sets of 4th/5th axis tool
offsets are available. When tool geometry/wear compensation is enabled (bit 6 (NGW) of parameter
No.8136 is 0), tool geometry offset and tool wear offset are enabled. Moreover, the number of sets can be
increased from 32 to 64, 99, 400, 999, or 2000.
A tool offset value can be applied to arbitrary axes by setting an axis number (1 to the maximum number
of controlled axes) to be used for 4th axis offset in parameter No. 5044 and setting an axis number (1 to
the maximum number of controlled axes) to be used for 5th axis offset in parameter No. 5045. By setting
bit 1 (NO5) of parameter No. 11400 to 1, 5th axis offset is enabled.
If the same axis as used with the Y axis offset function is specified, however, a Y axis offset value is
applied to the specified axis, and a 4th axis offset value or 5th axis offset value is invalidated.
Tool offset values can be input through an I/O device.

Explanation

The operation of 4th/5th axis offset is the same as the operation of tool offset. For the operation, see
Section 12.1.1, "TOOL OFFSET".

Setting of tool offset values with the G10 command

By programming, 4th/5th axis offset values can be input.

Format

G10 P_ X_ Y_ Z_ R_ Q_ E_ F_ ;

G10 P_ U_ V_ W_ C_ Q_ E_ F_;

P : Offset number

: Specifies a workpiece coordinate system shift value.

1 to 999

: Specifies a tool wear offset value.

10000+(1 to 999) : Specifies a tool geometry offset value, with a number (1 to 999)

representing an offset number.

X  : X axis offset value (absolute)
Y  : Y axis offset value (absolute)
Z  : Z axis offset value (absolute)
U  : X axis offset value (incremental)
V  : Y axis offset value (incremental)
W : Z axis offset value (incremental)
R  : Tool nose radius compensation value (absolute)
C  : Tool nose radius compensation value (incremental)
Q  : Virtual tool nose number
E  : 4th axis offset value (absolute)
F  : 5th axis offset value (absolute)

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1932 -

Explanation

As in the G10 format above, address E for inputting a 4th axis offset value and address F for inputting a
5th axis offset value allow absolute values only to be input.

NOTE

1 When compared with the conventional G10 format for changing tool offset

values, address E for specifying a 4th axis offset value and address F for
specifying a 5th axis offset value are newly added in the format above.

2 When a program based on the G10 format above is executed, only those offset

values that correspond to programmed axis addresses and offset numbers are
rewritten.

Address name changing of format

When bit 2 (OFS) of parameter No.11403 is set to 1, the specification address in "Y-axis offset and
4th/5th axis offset" can use axis name 'A' or 'B' instead of default specification addresses 'Y', 'E' and 'F'.

Example) When the following parameters are set, the command address 'A' and 'B' are used for setting of

a tool offset.
-

Parameter No.5044 is set to 4 (4th axis offset is the 4th axis)

Parameter No.5045 is set to 5 (5th

axis offset is the 5th axis)

Parameter No.1020 (4th

axis ,5th

axis) = 65, 66 (Address name of 4th /5th

axis offset is 'A' and

'B')

Bit 2 (OFN) of No.11403 is set to 1 (Address depend on parameter No.1020)

G10 P01 X_ Z_ A_ B_

G10 P02 X_ Z_ A_ B_

...

G10 P__ X_ Z_ A_ B_

A_ :

Tool compensation data (4th axis offset value in the example).

B_ :

Tool compensation data (5th axis offset value in the example).

The other addresses are the same as for the tool compensation amount.

NOTE

1 The axis name that can be used as a specification address is only 'A', and 'B'.

If 'A' or 'B' is used as the specification address in Y-axis offset, the address 'V'
(incremental command of Y-axis offset) cannot be used.

2 If the either of following is set, the default specification addresses 'Y', 'E', and 'F'

are used.
- Parameter No.1020 is set to axis name other than 'A(65)' or 'B(66)'.
- An extended axis name is used.

3 When bit 2 (OFN) of parameter No.11403 is set to 1, conventional offset data

cannot be read. If conventional offset data is read, set 0 to bit 2 (OFN) of
parameter No.11403.

Limitation

This function supports the common memory between each path.

This function does not support direct input/counter input of tool offset values measured.

This function does not support offset value writing using a custom macro variable.

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1933 -

This function does not support the PMC window function.

However, this function supports writing/reading of 4th/5th axis offset values to and from the C
Language Executor.

This function does not support external data input. So, no 4th/5th axis offset value can be modified
with a PMC ladder.

This function does not support the second geometry tool offset function.

This function does not support the tool management function.

This function does not support the wrong operation prevention function.

This function does not support the program coordinate switch screen function and the offset memory
switch function.

Parameter

5044

Axis number for which 4th-axis offset is used

NOTE

When this parameter is set, the power must be turned off before
operation is continued.

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0, 1 to number of controlled axes

Set the number of an axis for which the 4th-axis offset is used.
When a value ranging from 1 to the number of controlled axes is set in this parameter, the
4th-axis offset is applied to the set axis number. If 0 or a value beyond the valid data
range is set, the 4th-axis offset is not used. For the basic two axes X and Z, the standard
tool offsets are used, so the 4th-axis offset cannot be used. When the axis set for the
Y-axis offset function is set in this parameter, the Y-axis offset is used for the axis, and
the 4th-axis offset is not used.

5045

Axis number for which 5th-axis offset is used

NOTE

When this parameter is set, the power must be turned off before
operation is continued.

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0, 1 to number of controlled axes

Set the number of an axis for which the 5th-axis offset is used.
When a value ranging from 1 to the number of controlled axes is set in this parameter, the
5th-axis offset is applied to the set axis number. If 0 or a value beyond the valid data
range is set, the 5th-axis offset is not used. For the basic two axes X and Z, the standard
tool offsets are used, so the 5th-axis offset cannot be used. When the axis set for the
Y-axis offset function is set in this parameter, the Y-axis offset is used for the axis, and
the 4th-axis offset is not used.
When settings are made so that both the 5th-axis offset and 4th-axis offset apply to the
same axis, only the 4th-axis offset is used, and the 5th-axis offset is not used.

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1934 -

5040

NO4

[Input type] Parameter input

[Data type] Bit path

#7 NO4

4th axis offset function is:

Used.

Not used.

11400

NO5

[Input type] Parameter input

[Data type] Bit path

#1 NO5

The fifth axis offset function is:

Not used.

Used.

11.2

TOOL FUNCTIONS OF MACHINING CENTER SYSTEM

Overview

Selection of tools can be done by commanding tool numbers with up to an 8-digit numeral after address
T.

Signal

Refer to “AUXILIARY FUNCTION/2ND AUXILIARY FUNCTION”

Parameter

3032

Allowable number of digits for the T code

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 1 to 8

Set the allowable numbers of digits for the T code.
When 0 is set, the allowable number of digits is assumed to be 8.

Note

NOTE

When a move command and a tool function are specified in the same block, the
commands are executed in one of the following two ways:
(i) Simultaneous execution of the move command and tool function commands.
(ii) Executing tool function commands upon completion of move command

execution.

The selection of either (i) or (ii) depends on the sequence program of PMC.

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1935 -

Reference item

Manual name

Item name

OPERATOR’S MANUAL (B-64694EN)

Tool selection command
Tool selection function

CONNECTION MANUAL (FUNCTION)
(This manual)

Auxiliary function

11.2.1

Tool Compensation Memory

Overview

Tool compensation values include geometry compensation values and wear compensation values.
Tool compensation values can also be used without discriminating between geometry and wear
compensation values.

Fig. 11.2.1 (a) Geometric compensation and wear compensation

Tool compensation values can be entered into CNC memory from the MDI or from a program.
A tool compensation value is selected from the CNC memory when the corresponding code is specified
after address H or D in a program.
The value is used for tool length compensation, cutter compensation, or the tool offset.

Unit of range of tool compensation value

A tool offset unit and valid data range can be chosen from the following by setting the parameters:

Table 11.2.1 (a)

Unit of range of tool compensation value (metric input)

OFE

OFD

OFC

OFA

Unit

Range

0.01mm

9999.99mm

0.001mm

9999.999mm

0.0001mm

9999.9999mm

0.00001mm

9999.99999mm

0.000001mm

999.999999mm

Unit of range of tool compensation value (inch input)

OFE

OFD

OFC

OFA

Unit

Range

0.001inch

999.999inch

0.0001inch

999.9999inch

0.00001inch

999.99999inch

0.000001inch

999.999999inch

0.0000001inch

99.9999999inch

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1936 -

Tool compensation memory

One of the tool compensation memory A/C can be selected according to the configuration of offset
amount.

(1) Tool compensation memory A

There is no difference between geometry compensation memory and wear compensation memory in
tool compensation memory A. Therefore, amount of geometry offset and wear offset together is set
as the offset memory. There is also no differences between cutter compensation (D code) and tool
length compensation (H code).

(2) Tool compensation memory C

Memory for geometry compensation and wear compensation is separate in tool compensation
memory C. Geometry compensation and wear compensation can thus be set separately. Separate
memories are prepared for cutter compensation (for D code) and for tool length compensation (for H
code).

The above description is summarized as follows:

Table 11.2.1 (b)

Tool compensation memory

Compensation amount

Tool compensation amount (Geometry compensation value + Wear
compensation value)

Geometry compensation value for H code
Geometry compensation value for D code
Wear compensation value for H code
Wear compensation value for D code

Parameter

3109

DWT

[Input type] Parameter input

[Data type] Bit path

#1 DWT

Characters G and W in the display of tool wear/geometry compensation amount

The characters are displayed at the left of each number.

The characters are not displayed.

3205

OSC

[Input type] Parameter input

[Data type] Bit

#4 OSC

On the offset screen, offset value erasure by a soft key is:

Enabled.

Disabled.

3290

GOF

WOF

[Input type] Parameter input

[Data type] Bit path

#0 WOF

Setting the tool offset value (tool wear offset) by MDI key input is:

Not disabled.

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1937 -

Disabled. (With parameters Nos. 3294 and 3295, set the offset number range in
which updating the setting is to be disabled.)

NOTE

When tool offset memory A is selected with the M series, the tool
offset value set in this parameter is followed even if geometric
compensation and wear compensation are not specified with the T
series.

#1 GOF

Setting the tool geometry offset value by MDI key input is:

Not disabled.

Disabled. (With parameters Nos. 3294 and 3295, set the offset number range in
which updating the setting is to be disabled.)

3294

Start number of tool offset values whose input by MDI is disabled

3295

Number of tool offset values (from the start number) whose input by MDI is disabled

[Input type] Parameter input

[Data type] Word path

[Valid data range] 0 to 999

When the modification of tool offset values by MDI key input is to be disabled using bits
0 (WOF) and 1 (GOF) of parameter No. 3290, parameters Nos. 3294 and 3295 are used to
set the range where such modification is disabled. In parameter No. 3294, set the offset
number of the start of tool offset values whose modification is disabled. In parameter No.
3295, set the number of such values. In the following cases, however, none of the tool
offset values may be modified:
-

When 0 or a negative value is set in parameter No. 3294

When 0 or a negative value is set in parameter No. 3295

When a value greater than the maximum tool offset number is set in parameter No.
3294

In the following case, a modification to the values ranging from the value set in parameter
No. 3294 to the maximum tool offset number is disabled:
-

When the value of parameter No. 3294 added to the value of parameter No. 3295
exceeds the maximum tool offset number

When the offset value of a prohibited number is input through the MDI panel, the
warning "WRITE PROTECT" is issued.

[Example] When the following parameter settings are made, modifications to both of the tool

geometry offset values and tool wear offset values corresponding to offset numbers 51 to
60 are disabled:
-

Bit 1 (GOF) of parameter No. 3290 = 1 (to disable tool geometry offset value
modification)

Bit 0 (WOF) of parameter No. 3290 = 1 (to disable tool wear offset value
modification)

Parameter No. 3294 = 51

Parameter No. 3295 = 10

If the setting of bit 0 (WOF) of parameter No. 3290 is set to 0 without modifying the
other parameter settings above, tool geometry offset value modification only is disabled,
and tool wear offset value modification is enabled.

5013

Maximum value of tool wear compensation

[Input type] Parameter input

Content .. 245 246 247 248 ..