FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION) — page 25

1. AXIS CONTROL

B-64693EN-1/01

- 154 -

- Servo axis

Diagnosis data No.3740 displays detection unit which is calculated by the following equation.

Detection unit = Least command increment / CMR

- Cs contour control axis

Detection unit of Cs contour control axis is set by bit 0 (CS360M) of parameter No.4005. Diagnosis data

No.3740 displays the following value. Diagnosis data No.3740 is displayed 0.0 by the hypothetical Cs

axis (bit 7 (CDMx) of parameter No.3740 = 1).

Table 1.4.5 (a) Detection unit of Cs contour control axis

Bit 0 (CS360M) of parameter No.4005

Diagnosis data No.3740

0

0.001

1

0.0001

- Spindle positioning axis

Detection unit of spindle positioning axis is set by gear ratio between spindle and position coder

(parameter Nos.3721, 3722). Diagnosis data No.3740 displays the following value.

Table 1.4.5 (b) Detection unit of spindle positioning axis

Gear ratio of spindle to position coder

Diagnosis data No.3740

1:1

0.088 (1x360/4096)

1:2

0.176 (2x360/4096)

1:4

0.352 (4x360/4096)

1:8

0.703 (8x360/4096)

…

…

1:N

(Nx360/4096)

Diagnosis data

3740

Detection unit

[Data type] Real axis

[Unit of data] mm, inch, deg (machine unit)

[Valid data range] 0.0 to 99.99

This diagnosis data displays detection unit.

#7

#6

#5

#4

#3

#2

#1

#0

3741

DEG

IN.

MM

[Data type] Bit axis

#0 MM

Detection unit is:

0: Not mm.

1: mm.

#1 IN.

Detection unit is:

0: Not inch.

1: inch.

#2 DEG

Detection unit is:

0: Not degree.

1: degree.

B-64693EN-1/01

1. AXIS CONTROL

- 155 -

1.5

SETTINGS RELATED WITH COORDINATE SYSTEMS

1.5.1

Machine Coordinate System

Overview

The point that is specific to a machine and serves as the reference of the machine is referred to as the

machine zero point. A machine tool builder sets a machine zero point for each machine.

A coordinate system with a machine zero point set as its origin is referred to as a machine coordinate

system.

A machine coordinate system is set by performing manual reference position return after power-on. A

machine coordinate system, once set, remains unchanged until the power is turned off.

Format

M

(G90)G53

IP

_ P1;

IP

_ : Absolute command dimension word

P1 : Enables the high-speed G53 function.

(G90)G53.2 G01

IP

＿

F

＿

;

IP

_ : Absolute command dimension word

F_ : Feedrate

T

G53

IP

_ P1;

IP

_ : Absolute command dimension word

P1 : Enables the high-speed G53 function.

G53.2 G01

IP

＿

F

＿

;

IP

_ : Absolute command dimension word

F_ : Feedrate

Explanation

- Selecting a machine coordinate system (G53)

When a command is specified the position on a machine coordinate system, the tool moves to the position

by rapid traverse. G53, which is used to select a machine coordinate system, is a one-shot G code; that is,

it is valid only in the block in which it is specified on a machine coordinate system. Specify an absolute

command for G53. When an incremental command is specified, the G53 command is ignored. When the

tool is to be moved to a machine-specific position such as a tool change position, program the movement

in a machine coordinate system based on G53.

- High-speed G53 function

The high-speed G53 function enables the rapid traverse block overlap function between the machine

coordinate system selection command (G53) block and positioning (rapid traverse) command (G00) block,

which allows the next rapid traverse command (G00) to be executed without decelerating and stopping

the tool at the end of the machine coordinate system selection command (G53). This function enables

high-speed positioning even when the machine coordinate system selection command (G53) is used.

The high-speed G53 function is enabled by specifying P1 in the G53 block.

1. AXIS CONTROL

B-64693EN-1/01

- 156 -

- Selecting a machine coordinate system with feedrate (G53.2)

Positioning of machine coordinate system at a feed rate is available with the command of G53.2. The feed

rate can be used in the modal of G01.

NOTE

The selecting a machine coordinate system with feedrate (G53.2) is an option.

To use this function, an option of the selecting a machine coordinate system with

feedrate is required.

G53.2 is one shot G code. Moreover, the tool offset value is temporarily canceled by G53.2 command like

G53.

As for the time constant, a usual feed rate are used. At the point of G53.2 command, the axis decelerates

to a stop once like G53 command.

Feed per minute, feed per revolution, and inverse time feed of G codes of 05 group are available.

When group 01 G-code except G00/G01 is commanded with G53.2, the alarm PS5372, “IMPROPER

MODAL G-CODE” is generated. And, when G53.2 is commanded while group 01 Modal G-code is the

one except G00/G01, the alarm PS5372 is generated.

Limitation

- Cancel of the compensation function

When the G53 command is specified, cancel the compensation functions such as the cutter compensation,

tool length offset, tool-nose radius compensation, and tool offset.

- G53 specification immediately after power-on

Since the machine coordinate system must be set before the G53 command is specified, at least one

manual reference position return or automatic reference position return by the G28 command must be

performed after the power is turned on. This is not necessary when an absolute-position detector is

attached.

Specification in the same block

M

Commands G50/G51, G50.1/G51.1, and G68/G69 cannot be specified in the same block where the G53

command is specified.

T

Commands G50/G51 (except for G code system A), G50.1/G51.1, and G68.1/G69.1 cannot be specified

in the same block where the G53 command is specified.

Reference

- Setting a machine coordinate system

When manual reference position return is performed after power-on, a machine coordinate system is set

so that the reference position is at the coordinate values of (

a

,

b

) set using parameter No.1240.

B-64693EN-1/01

1. AXIS CONTROL

- 157 -

b

Reference position

Machine coordinate system

Machine zero point

a

Fig. 1.5.1 (a)

Example (selecting a machine coordinate system with feedrate)

N1 G90 G01 ;

N2 G53.2 X50.0 Y100.0 F1000 ; Absolute command with feedrate F1000

N3 G53.2 X150.0 F500 ;

Absolute command with feedrate F500

Fig. 1.5.1 (b)

Parameter

1240

Coordinate value of the reference position in the machine coordinate system

NOTE

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

operation is continued.

[Input type] Parameter input

[Data type] Real axis

[Unit of data] mm, inch, deg (machine unit)

[Min. unit of data] Depend on the increment system of the applied axis

[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)

Set the coordinate values of the reference position in the machine coordinate system.

Alarm and message

Number

Message

Description

PS5372 IMPROPER MODAL G-CODE (G53.2)

In the G53.2 block, a G code in group 01 other than G00 or
G01 is specified. Alternatively, G53.2 is specified when the
modal G code in group 01 is other than G00 or G01.

Y axis

100

0

50 150 X axis

Temporarily decelerates and stops.

1. AXIS CONTROL

B-64693EN-1/01

- 158 -

Reference item

Manual name

Item name

OPERATOR’S MANUAL (B-64694EN)

Machine coordinate system

1.5.2

Workpiece Coordinate System/Addition of Workpiece

Coordinate System Pair

Overview

A coordinate system used for machining a workpiece is referred to as a workpiece coordinate system. A

workpiece coordinate system is to be set with the CNC beforehand (setting a workpiece coordinate

system).

A machining program sets a workpiece coordinate system (selecting a workpiece coordinate system).

A set workpiece coordinate system can be changed by shifting its origin (changing a workpiece

coordinate system).

1.5.2.1

Workpiece coordinate system

NOTE

To use the workpiece coordinate system, set 0 in bit 0 (NWZ) of parameter

No.8136.

- Setting a workpiece coordinate system

A workpiece coordinate system can be set using one of three methods:

(1) Method using a workpiece coordinate system setting G code

A workpiece coordinate system is set by specifying a value in the program after a workpiece

coordinate system setting G code.

(2) Automatic setting

If bit 0 (ZPR) of parameter No. 1201 is set to 1, a workpiece coordinate system is automatically set

when manual reference position return is performed.

This function is, however, disabled when the workpiece coordinate system is being used.

(3) Method using a workpiece coordinate system selection G code

Six workpiece coordinate systems can be set beforehand using the MDI unit. Program commands

G54 to G59 can be used to select the work axis to be used.

When using an absolute command, establish the workpiece coordinate system in any of the above ways.

CAUTION

The established workpiece coordinate system depends on diameter

programming or radius programming.

- Selecting a workpiece coordinate system

The user can choose from set workpiece coordinate systems as described below.

(1) Selecting a workpiece coordinate system set by workpiece coordinate system setting G code (G92,

G50) or automatic workpiece coordinate system setting

Once a workpiece coordinate system is selected, absolute commands work with the workpiece

coordinate system.

(2) Choosing from six workpiece coordinate systems set using the MDI unit

By specifying a G code from G54 to G59, one of the workpiece coordinate systems 1 to 6 can be

selected.

G54 . . Workpiece coordinate system 1

G55 . . Workpiece coordinate system 2

G56 . . Workpiece coordinate system 3

G57 . . Workpiece coordinate system 4

G58 . . Workpiece coordinate system 5

G59 . . Workpiece coordinate system 6

B-64693EN-1/01

1. AXIS CONTROL

- 159 -

Workpiece coordinate systems 1 to 6 are established after reference position return after the power is

turned on. When the power is turned on, G54 coordinate system is selected as default.

When bit 2 (G92) of parameter No. 1202 is set to 1, executing the G code command for coordinate system

setting (G92 <M series>, G50 <Tseries> (G92 with G code system B/C for T series)) results in the issue

of alarm PS0010, “IMPROPER G-CODE”. This is designed to prevent the user from confusing

coordinate systems.

CAUTION

The set workpiece zero point offset value depends on diameter programming or

radius programming.

- Changing workpiece coordinate system

The six workpiece coordinate systems specified with G54 to G59 can be changed by changing an external

workpiece zero point offset value or workpiece zero point offset value.

Three methods are available to change an external workpiece zero point offset value or workpiece zero

point offset value.

(1) Inputting from the MDI unit

(2) Programming (using a programmable data input G code or a workpiece coordinate system setting G

code)

(3) Using the external data input function

An external workpiece zero point offset value can be changed by input signal to CNC. Refer to

machine tool builder's manual for details.

Workpiece

coordinate system 1

(G54)

Workpiece

coordinate system 2

(G55)

Workpiece coordinate

system 3

(G56)

Workpiece coordinate

system 4

(G57)

Workpiece coordinate

system 5
(G58)

Workpiece coordinate

system 6

(G59)

ZOFS2

ZOFS3

ZOFS4

ZOFS5

ZOFS1

ZOFS6

Machine zero point

EXOFS :External workpiece zero point offset value
ZOFS1 to ZOFS6 : Workpiece zero point offset value

EXOFS

Fig. 1.5.2.1 (a) Changing an external workpiece zero point offset value or workpiece zero point offset value

Format

- Changing by inputting programmable data

G10 L2 Pp

IP

_;

p=0

: External workpiece zero point offset value

p=1 to 6 : Workpiece zero point offset value correspond to workpiece coordinate system 1 to 6

IP

_: For an absolute command, workpiece zero point offset for each axis.

For an incremental command, value to be added to the set workpiece zero point offset for each axis (the
result of addition becomes the new workpiece zero point offset).

1. AXIS CONTROL

B-64693EN-1/01

- 160 -

-

Changing by setting a workpiece coordinate system

M

G92

IP

_;

T

G50

IP

_;

Explanation

- Changing by inputting programmable data

By specifying a programmable data input G code, the workpiece zero point offset value can be changed

for each workpiece coordinate system.

- Changing by setting a workpiece coordinate system

By specifying a workpiece coordinate system setting G code, the workpiece coordinate system (selected

with a code from G54 to G59) is shifted to set a new workpiece coordinate system so that the current tool

position matches the specified coordinates (IP_).

Then, the amount of coordinate system shift is added to all the workpiece zero point offset values. This

means that all the workpiece coordinate systems are shifted by the same amount.

CAUTION

When a coordinate system is set with G code command for workpiece coordinate

system setting after an external workpiece zero point offset value is set, the

coordinate system is not affected by the external workpiece zero point offset

value. When G92X100.0Z80.0; is specified, for example, the coordinate system

having its current tool reference position at X = 100.0 and Z = 80.0 is set.

T

If IP is an incremental command value, the work coordinate system is defined so that the current tool

position coincides with the result of adding the specified incremental value to the coordinates of the

previous tool position. (Coordinate system shift)

When bit 0 (WAB) of parameter No. 11279 is set to 1, the setting of the workpiece coordinate system is

executed with absolute value even if the work coordinate system setting (G92) is commanded during the

incremental mode (G91) in the G-code system B/C of the lathe system.

Notes

- Manual reference position return

When the manual reference position return is performed, the value of the workpiece coordinate system set

by G code (G92, or G50 for the lathe system G-code system A) is cleared to 0. And when the automatic

reference position return (G28) is performed, this workpiece coordinate system is not cleared to 0 but

stored.

Parameter

#7

#6

#5

#4

#3

#2

#1

#0

11279

WAB

[Input type] Parameter input

[Data type] Bit

B-64693EN-1/01

1. AXIS CONTROL

- 161 -

#0 WAB

When the incremental mode (G91) is selected in the G-code system B/C of the lathe

system, if the setting of the workpiece coordinate system (G92) is commanded, the setting

of the workpiece coordinate system is executed with:

0: Incremental value.

1: Absolute value.

1.5.2.2

Workpiece coordinate system preset

NOTE

To use the workpiece coordinate system preset function, set 0 in bit 1 (NWC) of

parameter No. 8136.

Explanation

In reset state, execute Manual reference position return, a workpiece coordinate system is shifted by the

workpiece zero point offset value from the machine coordinate system zero point. Suppose that the

manual reference position return operation is performed when a workpiece coordinate system is selected

with G54. In this case, a workpiece coordinate system is automatically set which has its zero point

displaced from the machine zero point by the G54 workpiece zero point offset value; the distance from

the zero point of the workpiece coordinate system to the reference position represents the current position

in the workpiece coordinate system.

Reference position

G54 workpiece coordinate system

Workpiece zero point

Manual reference position return

Machine zero point

G54 workpiece

zero point offset

value

Fig. 1.5.2.2 (a)

If an absolute position detector is provided, the workpiece coordinate system automatically set at

power-up has its zero point displaced from the machine zero point by the G54 workpiece zero point offset

value. The machine position at the time of power-up is read from the absolute position detector and the

current position in the workpiece coordinate system is set by subtracting the G54 workpiece zero point

offset value from this machine position. The workpiece coordinate system set by these operations is

shifted from the machine coordinate system using the commands and operations listed below.

(a) Manual intervention performed when the manual absolute signal is off

(b) Move command executed in the machine lock state

(c) Movement by handle interrupt

(d) Operation using the mirror image function

(e) Shifting the workpiece coordinate system by setting the local coordinate system or workpiece

coordinate system

In the case of (a) above, the workpiece coordinate system is shifted by the amount of movement during

manual intervention.