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

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1914 -

NOTE

1 When G50 X_Z_T_ ; is specified, the tool is not moved.

The coordinate system in which the coordinate value of the tool position is (X,Z) is
set. The tool position is obtained by subtracting the offset value corresponding to
the tool offset number specified in the T code.

2 The G codes in the 00 group other than G50 must not be specified in the same

block as that containing a T code. If any one of G28, G29, G30, and G53 is
specified in the same block together with a T code, alarm PS0245, "T-CODE NOT
ALLOWED IN THIS BLOCK", is issued.

Compensation with coordinate shift

The work coordinate system is shifted by the X, Y, and Z tool offset amounts. Namely, the offset amount
corresponding to the number designated with the T code is added to or subtracted from the absolute
coordinates.

Fig. 11.1.3 (b) Offset operation with coordinate shift

Starting and canceling offset by specifying a T code

Specifying a tool offset number with a T code means to select the tool offset value corresponding to it and
to start offset. Specifying 0 as a tool offset number means to cancel offset.
For offset with tool movement, whether to start or cancel the offset can be specified with bit 6 (LWN) of
parameter No. 5002.
For compensation with coordinate shift, the offset is started and canceled when a T code is specified. For
the cancellation of geometry compensation, its operation can be selected with bit 5 (LGC) of parameter
No. 5002.

Table 11.1.3 (b)

Compensation method

Bit 6 (LWN) of parameter No. 5002=0

Bit 6 (LWN) of parameter No. 5002=1

Tool movement

When a T code is specified

When an axial movement is specified

Coordinate shift

When a T code is specified

(Note that geometry compensation can be canceled only if bit 5 (LGC) of parameter

No. 5002 = 1.)

Canceling offset with reset

Tool offset is canceled under one of the following conditions:
<1>  The power to the CNC is turned off and turned back on
<2>  The reset button on the MDI unit is pressed
<3>  A reset signal is input from the machine to the CNC
In cases <2> and <3> above, it is possible to select a cancel operation using bits 3 (LVC) of parameter No.
5006 and 7 (TGC) of parameter No. 5003.

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1915 -

Table 11.1.3 (c)

Compensation method

Parameter

LVC=0

TGC=0

LVC=1

TGC=0

LVC=0

TGC=1

LVC=1

TGC=1

Tool

movement

Wear compensation

Not

canceled.

Canceled.

(When axial movement

is specified)

Not

canceled.

Canceled.

(When axial movement

is specified)

Geometry compensation

Coordinate

shift

Wear compensation

Not

canceled.

Canceled.

Not

canceled.

Canceled.

Geometry compensation

Not

canceled.

Not canceled.

Canceled.

Notes and restrictions

Helical interpolation (G02, G03)

Tool position offset cannot be specified in a block in which helical interpolation is used.

Coordinate system rotation (G68.1)

Coordinate system rotation is executed on the command program first, followed by tool position
offset.

3-dimensional coordinate conversion (G68.1)

If tool position offset is used, tool position offset with coordinate shift cannot be used. Offset with
tool movement must be specified inside a nest of 3-dimensional coordinate conversion. At the
beginning block of the 3-dimensional coordinate conversion, tool does not move for a converted tool
offset value.

Example)

G68.1 ... ;

T0101;

T0100;

G69.1 ... ;

Workpiece coordinate system preset (G50.3)

When the bit 7(WTC) of parameter No.1205 is 0, performing workpiece coordinate system preset
causes tool position offset with tool movement to be canceled; this does not cause tool position
offset with coordinate shift to be canceled.

When the bit 7(WTC) of parameter No.1205 is 1, performing workpiece coordinate system preset
does not cause neither tool position offset with tool movement nor tool position offset with
coordinate shift to be canceled.

Machine coordinate system setting (G53), reference position return (G28), second, third, and fourth
reference position return (G30), and manual reference position return

Basically, before performing these commands or operations, cancel tool position offset. These operations
do not cause tool position offset to be canceled. The actions in the Table 11.1.3 (d) take place:

Table 11.1.3 (d)

When the command or operation is

specified

When the next axial movement command

is specified

Tool movement

The tool offset value is temporarily canceled.

The tool offset value is reflected.

Coordinate shift

Coordinates with the tool offset value
reflected are assumed.

Arbitrary speed threading

The alarm PS0528, “THREADING FORMAT ERROR” is issued when a T-code and the M-code for
starting arbitrary speed threading are specified in the same block.

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1916 -

Auxiliary function output in moving axis (G50.9)

The alarm PS5330, “G50.9 FORMAT ERROR” is issued when a T-code and auxiliary function
output in moving axis (G50.9) are specified in the same block.

Programmable parameter input (G10)

The alarm PS1144, “G10 FORMAT ERROR” is issued when a T-code is specified during
programmable parameter input.

Parameter

1205

WTC

[Input type] Parameter input

[Data type] Bit path

#7 WTC

When workpiece coordinate system preset is done, actual tool position offset by tool

movement is :
0:

Not considered.

Considered.

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 codes.
When 0 is set, the allowable number of digits is assumed to be 8.

3129

DAP

DRP

[Input type] Parameter input

[Data type] Bit path

#0 DRP

For relative coordinate display:

The actual position considering a tool offset (tool movement) is displayed.

The programmed position excluding a tool offset (tool movement) is displayed.

#1 DAP

For absolute coordinate display:

The actual position considering a tool offset (tool movement) is displayed.

The programmed position excluding a tool offset (tool movement) is displayed.

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.

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

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1917 -

NOTE

When tool offset memory A is selected with the M series, the tool
offset set in this parameter WOF is followed even if geometric
compensation and wear compensation are disabled (bit 6 (NGW) of
parameter No. 8136 is set to 1) 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.

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1918 -

5002

WNP

LWM

LGC

LGT

ETC

LWT

LGN

[Input type] Parameter input

[Data type] Bit path

#1 LGN

Geometry offset number of tool offset :

Is the same as wear offset number

Specifies the geometry offset number by the tool selection number

NOTE

This parameter is valid when tool geometry/wear compensation is
enabled (bit 6 (NGW) of parameter No.8136 is 0).

#2 LWT

Tool wear compensation is performed by:

Moving the tool.

Shifting the coordinate system.

NOTE

This parameter is valid when tool geometry/wear compensation is
enabled (bit 6 (NGW) of parameter No.8136 is 0).

#3 ETC

When a T-code command is two digits or shorter, the T code is:

Not extended.

Extended.

When this parameter is 1, two-digit or shorter T-code commands are extended.
(Three-digit or longer T-code commands are not extended.) The value after extension is
determined by the setting of the number of digits in the offset number in T-code
commands (parameter No. 5028).

Parameter No.

5028

Number of digits after

extension

Sample extension

Extended to two digits

Before extension: T1

→

After extension: T11

Extended to four digits

Before extension: T1

→

After extension: T0101

3 or greater

Not extended

[Example]

Parameter No. 5028 : 2

Parameter No. 3032 : 4 (Allowable number of digits in T code)

Before extension

→

After extension

→

T0101 (1-digit command is extended to 4 digits.)

T12

→

T1212 (2-digit command is extended to 4 digits.)

T112

→

T112 (Not extended)

T1122

→

T1122 (Not extended)

NOTE

1 The setting of the allowable number of digits in T code (parameter

No. 3032) indicates the number of digits in a specified command
(before being extended). If the number of digits in the command
exceeds the allowable number of digits in T code, the alarm
PS0003, “TOO MANY DIGIT” is issued.

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1919 -

NOTE

2 This parameter is dedicated to the lathe system. Tool change is

available with the turret type setting (bit 3 (TCT) of parameter No.
5040 = 0).

3 If the number of digits in the offset number in a T-code command

(parameter No. 5028) is set to 0, the value after extension is
determined by the number of digits in the number of tool
compensation values (parameter No. 5024).

4 Common variable #149 for calling a T-code macro is set to the

pre-extension value.

#4 LGT

Tool geometry compensation is:

Compensated by the shift of the coordinate system

Compensated by the tool movement

NOTE

This parameter is valid when tool geometry/wear compensation is
enabled (bit 6 (NGW) of parameter No.8136 is 0).

#5 LGC

When tool geometry compensation is based on coordinate shifting, the tool geometry

offset is:
0:

Not canceled by a command with offset number 0.

Canceled by a command with offset number 0.

NOTE

This parameter is valid when tool geometry/wear compensation is
enabled (bit 6 (NGW) of parameter No.8136 is 0).

#6 LWM

Tool offset operation based on tool movement is performed:

In a block where a T code is specified.

Together with a command for movement along an axis.

#7 WNP

Imaginary tool tip number used for tool nose radius compensation, when the tool

geometry/wear compensation function is equipped, is the number specified by:
0:

Geometry offset number

Wear offset number

5003

TGC

[Input type] Parameter input

[Data type] Bit path

#7 TGC

A tool geometry offset based on a coordinate shift is:

Not canceled by reset.

Canceled by reset.

NOTE

This parameter is valid when tool geometry/wear compensation is
enabled (bit 6 (NGW) of parameter No.8136 is 0).

11. TOOL FUNCTIONS

B-64693EN-1/01

- 1920 -

5004

ORC

[Input type] Parameter input

[Data type] Bit path

#1 ORC

The setting of a tool offset value is corrected as:

Diameter value

Radius value

NOTE

This parameter is valid only for an axis based on diameter
specification. For an axis based on radius specification, specify a
radius value, regardless of the setting of this parameter.

5006

LVC

TGC

[Input type] Parameter input

[Data type] Bit

#1 TGC

If a T code is specified in a block where G50, G04, or G10 is specified:

No alarm is issued.

The alarm PS0245, “T-CODE NOT ALLOWED IN THIS BLOCK” is issued.

#3 LVC

A tool offset (geometry/wear) based on a tool movement and wear offset based on a

coordinate shift are:
0:

Not canceled by reset.

Canceled by reset.

5013

Maximum value of tool wear compensation

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (offset unit)

[Min. unit of data] The increment system of a tool offset value is followed.
[Valid data range] The settings of bits 3 to 0 (OFE, OFD, OFC, and OFA) of parameter No. 5042 are

followed.

For metric input

OFE

OFD

OFC

OFA

Valid data range

0 to 9999.99mm

0 to 9999.999mm

0 to 9999.9999mm

0 to 9999.99999mm

0 to 999.999999mm

For inch input

OFE

OFD

OFC

OFA

Valid data range

0 to 999.999inch

0 to 999.9999inch

0 to 999.99999inch

0 to 999.999999inch

0 to 99.9999999inch

B-64693EN-1/01

11. TOOL FUNCTIONS

- 1921 -

This parameter sets the maximum allowable tool wear compensation value. If an attempt
is made to set a tool wear compensation value, the absolute value of which exceeds the
value set in this parameter, the following alarm or warning is output:

Input from MDI

Warning: DATA IS OUT OF RANGE

Input by G10

Alarm PS0032: ILLEGAL OFFSET VALUE IN G10.

When 0 or a negative value is set, no maximum allowable value is applied.

[Example] When 30.000 is set

As a tool offset value, a value from -30.000 to +30.000 can be input.

5014

Maximum value of incremental input for tool wear compensation

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (offset unit)

[Min. unit of data] The increment system of a tool offset value is followed.
[Valid data range] The settings of bits 3 to 0 (OFE, OFD, OFC, and OFA) of parameter No. 5042 are

followed.

For metric input

OFE

OFD

OFC

OFA

Valid data range

0to9999.99mm

0to9999.999mm

0to9999.9999mm

0to9999.99999mm

0to999.999999mm

For inch input

OFE

OFD

OFC

OFA

Valid data range

0to999.999inch

0to999.9999inch

0to999.99999inch

0to999.999999inch

0to99.9999999inch

Set the maximum allowable value for the tool wear compensation value, input as an
incremental value. If the incremental input value (absolute value) exceeds the set value,
the following alarm or warning message is output:

Input from MDI

Warning: DATA IS OUT OF RANGE

Input by G10

Alarm PS0032: ILLEGAL OFFSET VALUE IN G10.

When 0 or a negative value is set, no maximum allowable value is applied.

5024

Number of tool compensation values

NOTE

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

[Input type] Parameter input

[Data type] Word path

[Valid data range] 0 to 999

Set the maximum allowable number of tool compensation values used for each path.
Ensure that the total number of values set in parameter No. 5024 for the individual paths
is within the number of compensation values usable in the entire system. The number of
compensation values usable in the entire system depends on the option configuration.

FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION) - page 245