FANUC Series 0i-MC. OPERATOR’S MANUAL

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64124EN/01

It is possible to change the operating mode for two or more specified axes

20.1

to either synchronous operation or normal operation by an input signal

SIMPLE

from the machine.

SYNCHRONOUS

Synchronous control can be performed for up to four pairs of axes with

the Series 16, or up to three pairs with the Series 18, according to the

CONTROL

parameter setting (parameter No. 8311).

The following operating modes are applicable to machines having two

tables driven independently by separate control axes. The following

example is of a machine with two tables driven independently by the Y

axis and V axis. If the axis names and axis sets that are actually being used

differ from those in the example, substitute the actual names for those

below.

Fig. 20.1

Example of axis configuration of the machine operated

by simple synchronous control

Explanations

D Synchronous operation

This mode is used for, for example, machining large workpieces that

extend over two tables.

While operating one axis with a move command, it is possible to

synchronously move the other axis. In the synchronous mode, the axis

to which the move command applies is called the master axis, and the axis

that moves synchronously with the master axis is called the slave axis.

In this example, it is assumed that Y axis is the master axis and V axis is

the slave axis. Here, the Y axis and the V axis move synchronously in

accordance with program command Yyyyy issued to the Y axis (master

axis).

Synchronous operation is possible during automatic operation, jog feed,

manual handle feed using the manual pulse generator, and incremental

feed, but is not possible during manual reference position return.

404

B-64124EN/01

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

D Normal operation

This operating mode is used for machining different workpieces on each

table. The operation is the same as in ordinary CNC control, where the

movement of the master axis and slave axis is controlled by the

independent axis address (Y and V). It is possible to issue the move

commands to both the master axis and slave axis in the same block.

(1) The Y axis moves normally according to program command Yyyyy

issued to the master axis.

(2) The V axis moves normally according to program command Vvvvv

issued to the slave axis.

(3) The Y axis and the V axis move simultaneously according to program

command YyyyyVvvvv.

Both automatic and manual operations are the same as in ordinary

CNC control.

D Switching between

For how to switch between the synchronous operation and normal

synchronous operation

operation modes, refer to the relevant manual published by the machine

and normal operation

tool builder.

D Automatic reference

When the automatic reference position return command (G28) and the

position return

2nd/3rd/4th reference position return command (G30) are issued during

synchronous operation, the V axis follows the same movement as the Y

axis returns to the reference position. After the return movement is

complete, the reference position return complete signal of the V axis goes

on when that of the Y axis goes on.

As a rule, commands G28 and G30 must be issued in the normal operating

mode.

D Automatic reference

When the automatic reference position return check command (G27) is

position return check

issued during synchronous operation, the V axis and Y axis move in

tandem. If both the Y axis and the V axis have reached their respective

reference positions after the movement is complete, the reference position

return complete signals go on. If either axis is not at the reference

position, an alarm is issued. As a rule, command G27 must be issued in

the normal operating mode.

D Specifying the slave axis

When a move command is issued to the slave axis during synchronous

operation, a P/S alarm (No. 213) is issued.

D Master axis and slave

The axis to be used as the master axis is set in parameter No. 8311.

axis

The slave axis is selected by an external signal.

D Displaying actual speed

Setting bit 7 (SMF) of parameter No. 3105 to 1 suppresses display of the

for master axis only

actual speed of the slave axes.

405

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64124EN/01

Limitations

D Setting a coordinate

In synchronous axis control, commands that require no axis motion, such

system

as the workpiece coordinate system setup command (G92) and the local

coordinate system setup command (G52), are set to the Y axis by program

command Yyyyy issued to the master axis.

D Externally-requested

For signals such as external deceleration, interlock, and machine lock,

deceleration, interlock,

only the signals issued to the master axis are valid in the synchronous

and machine lock

operating mode. Signals issued to other axes are ignored.

D Pitch error

Both the pitch error and backlash are compensated independently for the

compensation

master axis and the slave axis.

D Manual absolute

Turn on the manual absolute switch during synchronous operation. If it

is off, the slave axis may not move correctly.

D Synchronization error

The difference between the master axis and slave axis in servo positional

check using positional

deviation is always monitored. If the difference exceeds the parameter-

deviation

set limit, an P/S alarm (No. 213) is issued.

D Synchronization error

The difference between the master axis and slave axis in machine

check using machine

coordinates is always monitored. If the difference exceeds the parameter-

coordinates

set limit, an servo alarm (No. 407) is issued.

D Synchronization

When the power is turned on, compensation pulses are output for the slave

axis to match the machine position of the master axis with the machine

position of the slave axis.

(This is enabled only when the absolute

position detection function is used.)

D Compensation for

Compensation for out-of-synchronism (where the difference between

out-of-synchronism

the master and slave axes in servo positional deviation is always

monitored and the servo motor for the slave axis is compensated to reduce

the difference) is not performed.

D Manual reference

When the machine is manually returned to the reference position during

position return

synchronous operation, both the master axis and the slave axis move

synchronously until the acceleration movement is complete. However,

grid detection thereafter is carried out independently.

406

B-64124EN/01

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

The roll-over function prevents coordinates for the rotation axis from

20.2

overflowing. The roll-over function is enabled by setting bit 0 of

ROTARY AXIS

parameter ROAx 1008 to 1.

ROLL-OVER

Explanations

For an incremental command, the tool moves the angle specified in the

command. For an absolute command, the coordinates after the tool has

moved are values set in parameter No. 1260, and rounded by the angle

corresponding to one rotation. The tool moves in the direction in which

the final coordinates are closest when bit 1 of parameter RABx No. 1008

is set to 0. Displayed values for relative coordinates are also rounded by

the angle corresponding to one rotation when bit 2 of parameter RRLx No.

1008 is set to 1.

Examples

Assume that axis A is the rotating axis and that the amount of movement

per rotation is 360.000 (parameter No. 1260 = 360000). When the

following program is executed using the roll-over function of the rotating

axis, the axis moves as shown below.

Sequence

Actual

Absolute coordinate

G90 A0 ;

number

movement

value after movement

value

end

N1 G90 A-150.0 ;

-150

210

N2 G90 A540.0 ;

-30

180

N3 G90 A-620.0 ;

-80

100

N4 G91 A380.0 ;

+380

120

N5 G91 A-840.0 ;

-840

Relative

-360°

-0°

360°

coordinate value-720°

Absolute

-0°

coordinate value

210°(Absolute)

180°

100°

120°

NOTE

This function cannot be used together with the indexing

function of the index table.

407

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64124EN/01

When the angular axis makes an angle other than

90° with the

20.3

perpendicular axis, the angular axis control function controls the distance

ANGULAR AXIS

traveled along each axis according to the inclination angle. A program,

CONTROL

when created, assumes that the angular axis and perpendicular axis

intersect at right angles. However, the actual distance traveled is

controlled according to an inclination angle.

Program coordinate system

+Y Coordinate system actually used

(Angular axis)

+Z (Perpendicular axis)

θ : Inclination angle

Explanations

When the angular axis is the Y-axis and the perpendicular axis is the

Z-axis, the amount of travel along each axis is controlled according to the

formulas shown below.

The distance traveled along the Y-axis is determined by the following

formula:

Ya=Yp/cosθ

The distance traveled along the Z-axis is corrected by the inclination of

the Y-axis, and is determined by the following formula:

Za=Zp-Yp*tanθ

The speed component along the Y-axis is determined by the following

formula:

Fa=Fp/cosθ

Ya, Za, Fa : Actual distance and speed

Yp, Zp, Fp : Programmed distance and speed

D Method of use

The angular and perpendicular axes for which angular axis control is to

be applied must be specified beforehand, using parameters (No. 8211 and

8212).

Parameter AAC (No. 8200#0) enables or disables the inclined axis

control function. If the function is enabled, the distance traveled along

each axis is controlled according to an inclination angle parameter (No.

8210).

Parameter AZR (No. 8200#2) enables angular axis manual reference

point return only with a distance along the angular axis.

D Invalidity of normal axis

By setting the normal axis/angular axis control invalid signal NOZAGC

to 1, slanted axis control only for the angular axis can be available.

In this time the angular axis are converted to those along the slanted

coordinate system without affecting commands to normal axis.

D Absolute and relative

An absolute and a relative position are indicated in the programmed

position display

Cartesian coordinate system.

408

B-64124EN/01

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

D Machine position display

A machine position indication is provided in the machine coordinate

system where an actual movement is taking place according to an

inclination angle. However, when inch/metric conversion is performed,

a position is indicated which incorporates inch/metric conversion applied

to the results of inclination angle operation.

WARNING

After angular axis control parameter setting, be sure to

perform manual reference position return operation.

If once manual reference position return has been

performed along the angular axis, also perform manual

reference position return along the perpendicular axis.

P/S alarm No.090 is issued when an attempt is made to

manually return to the reference position along the

perpendicular axis although the angular axis is not on the

reference point.

Once the tool has been moved along the angular axis when

perpendicular/angular axis control disable signal NOZAGC

has been set to 1, manual reference position return must be

performed.

Before attempting to manually move the tool along the

angular and perpendicular axes simultaneously, set

perpendicular/angular axis control disable signal NOZAGC

to 1.

NOTE

If an inclination angle close to 0° or ±90° is set, an error can

occur. (A range from ±20° to ±90° should be used.)

Before a perpendicular axis reference position return check

(G27) can be made, angular axis reference position return

operation must be completed.

409

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64124EN/01

When enough torque for driving a large table cannot be produced by only

20.4

one motor, two motors can be used for movement along a single axis.

TANDEM CONTROL

Positioning is performed by the main motor only. The submotor is used

only to produce torque. With this tandem control function, the torque

produced can be doubled.

Main motor

Table

Ball screw

Submotor

Fig. 20.4 Example of operation

In general, the NC regards tandem control as being performed for one

axis. However, for servo parameter management and servo alarm

monitoring, tandem control is regarded as being performed for two axes.

For details, refer to the relevant manual published by the machine tool

builder.

410

1. GENERAL

OPERATION

B-64124EN/01

1.1

MANUAL

OPERATION

Explanations

D Manual reference

The CNC machine tool has a position used to determine the machine

position return

position.

(See Section III-3.1)

This position is called the reference position, where the tool is replaced

or the coordinate are set. Ordinarily, after the power is turned on, the tool

is moved to the reference position.

Manual reference position return is to move the tool to the reference

position using switches and pushbuttons located on the operator’s panel.

Reference position

Tool

Machine operator’s panel

Fig. 1.1 (a) Manual reference position return

The tool can be moved to the reference position also with program

commands.

This operation is called automatic reference position return (See Section

II-6).

414

B-64124EN/01

OPERATION

1. GENERAL

D The tool movement by

Using machine operator’s panel switches, pushbuttons, or the manual

manual operation

handle, the tool can be moved along each axis.

Machine operator’s panel

Manual

pulse

generator

Tool

Workpiece

Fig. 1.1 (b) The tool movement by manual operation

The tool can be moved in the following ways:

(i) Jog feed (See Section III-3.2)

The tool moves continuously while a pushbutton remains pressed.

(ii) Incremental feed (See Section III-3.3)

The tool moves by the predetermined distance each time a button is

pressed.

(iii) Manual handle feed (See Section III-3.4)

By rotating the manual handle,the tool moves by the distance

corresponding to the degree of handle rotation.

415

1. GENERAL

OPERATION

B-64124EN/01

1.2

Automatic operation is to operate the machine according to the created

program. It includes memory, MDI and DNC operations. (See Section

TOOL MOVEMENT

III-4).

BY PROGRAMMING-

Program

AUTOMATIC

01000

;

OPERATION

M_S_T

;

Tool

G92_X_ ;

G00...

;

G01

;

Fig. 1.2 (a) Tool movement by programming

Explanations

D Memory operation

After the program is once registered in memory of CNC, the machine can

be run according to the program instructions. This operation is called

memory operation.

CNC

Machine

Memory

Fig. 1.2 (b) Memory operation

D MDI operation

After the program is entered, as an command group, from the MDI

keyboard, the machine can be run according to the program. This

operation is called MDI operation.

CNC MDI keyboard

Machine

Manual program

input

Fig. 1.2 (c) MDI operation

D DNC operation

In this mode of operation, the program is not registered in the CNC

memory. It is read from the external input/output devices instead. This

is called DNC operation. This mode is useful when the program is too

large to fit the CNC memory.

416

B-64124EN/01

OPERATION

1. GENERAL

1.3

AUTOMATIC

OPERATION

Explanations

D Program selection

Select the program used for the workpiece. Ordinarily, one program is

prepared for one workpiece. If two or more programs are in memory,

select the program to be used, by searching the program number (Section

III-9.3).

In memory or on a tape

O1001

Program number

G92

------

Work-1 program

M30

O1002

Program number

G92

------

Work-2 program

Automatic

operation

M30

O1003

Program number

G92

------

Work-3 program

M30

Fig. 1.3 (a) Program selection for automatic operation

D Start and stop

Pressing the cycle start pushbutton causes automatic operation to start.

(See Section III-4)

By pressing the feed hold or reset pushbutton, automatic operation pauses

or stops. By specifying the program stop or program termination

command in the program, the running will stop during automatic

operation. When one process machining is completed, automatic

operation stops.

Start

Cycle start

Stop

Feed hold

Automatic operation

Reset

Program stop Stop caused

Program end

by program

Fig. 1.3 (b) Start and stop for automatic operation

417

B-64124EN/01

OPERATION

1. GENERAL

1.4

Before machining is started, the automatic running check can be

executed. It checks whether the created program can operate the machine

TESTING A

as desired. This check can be accomplished by running the machine

PROGRAM

actually or viewing the position display change (without running the

machine) (See Section III-5).

1.4.1

Check by Running the

Machine

Explanations

D Dry run

Remove the workpiece, check only movement of the tool. Select the tool

(See Section III-5.4)

movement rate using the dial on the operator’s panel.

Tool

Table

Fig. 1.4.1 (a) Dry run

D Feedrate override

Check the program by changing the feedrate specified in the program.

(See Section III-5.2)

Feed rate specified by program :

100 mm/min.

Tool

Feed rate after feed rate override (20%) :

20 mm/min.

Workpiece

Fig. 1.4.1 (b) Feedrate override

419

1. GENERAL

OPERATION

B-64124EN/01

D Single block

When the cycle start pushbutton is pressed, the tool executes one

(See Section III-5.5)

operation then stops. By pressing the cycle start again, the tool executes

the next operation then stops. The program is checked in this manner.

Cycle start

Tool

Stop

Cycle start

Workpiece

Stop

Fig. 1.4.1 (c) Single block

1.4.2

How to View the

Position Display

Change without

Running the Machine

Explanations

D Machine lock

(See Sections III-5.1)

MDI

Tool

Workpiece

The tool remains stopped, and only the

positional displays of the axes change.

Fig. 1.4.2 Machine lock

D Auxiliary function lock

When automatic running is placed into the auxiliary function lock mode

(See Section III-5.1)

during the machine lock mode, all auxiliary functions (spindle rotation,

tool replacement, coolant on/off, etc.) are disabled.

420

1. GENERAL

OPERATION

B-64124EN/01

1.6

The operator can display or change a value stored in CNC internal

memory by key operation on the MDI screen (See III-11).

DISPLAYING AND

SETTING DATA

Data setting

Data display

Screen Keys

MDI

CNC memory

Fig. 1.6 (a) Displaying and setting data

Explanations

D Offset value

Geometry

Wear com-

compensation

pensation

Setting

Tool compensation

number1

12.3

25.0

Tool compensation

number2

20.0

40.0

Tool compensation

number3

⋅ ⋅ ⋅

Screen Keys

Display

⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅

⋅ ⋅ ⋅

⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅ ⋅

⋅ ⋅ ⋅

MDI

CNC memory

Fig.1.6 (b) Displaying and setting offset values

The tool has the tool dimension (length, diameter). When a workpiece is

machined, the tool movement value depends on the tool dimensions.

By setting tool dimension data in CNC memory beforehand,

automatically generates tool routes that permit any tool to cut the

workpiece specified by the program. Tool dimension data is called the

offset value

(See Section III-11.4.1).

422

B-64124EN/01

OPERATION

1. GENERAL

1st tool path

Machined

shape

2nd tool path

Offset value of the 1st tool

Offset value of the 2nd tool

Fig. 1.6 (c) Offset value

D Displaying and setting

Apart from parameters, there is data that is set by the operator in

operator’s setting data

operation. This data causes machine characteristics to change.

For example, the following data can be set:

S Inch/Metric switching

S Selection of I/O devices

S Mirror image cutting on/off

The above data is called setting data (See Section III-11.4.3).

Setting data

Setting

⋅Inch/Metric switching

⋅Selection of I/O device

⋅Mirror image ON/OFF setting

⋅

Screen Keys

Displaying

⋅

CNC Memory

Operational

characteristics

Program

Automatic

operation

Movement of

the machine

Fig. 1.6 (d) Displaying and setting operator’s setting data

423

1. GENERAL

OPERATION

B-64124EN/01

D Displaying and setting

The CNC functions have versatility in order to take action in

parameters

characteristics of various machines.

For example, CNC can specify the following:

S Rapid traverse rate of each axis

S Whether increment system is based on metric system or inch system.

S How to set command multiply/detect multiply (CMR/DMR)

Data to make the above specification is called parameters (See Section

III-11.5.1).

Parameters differ depending on machine tool.

Parameter

Rapid traverse rate

Setting

Position control

Reference position return

Backlash compensation data

Pitch error compensation

Screen Keys

Display

data

⋅

MDI

⋅

CNC memory

Operational

characteristics

Movement

Program

Automatic

of the

operation

machine

Fig. 1.6 (e) Displaying and setting parameters

D Data protection key

A key called the data protection key can be defined. It is used to prevent

part programs, offset values, parameters, and setting data from being

registered, modified, or deleted erroneously

(See Section III-11).

Data Setting

Screen Keys

Protection Key

MDI

Registration / modification inhibition

Machine operator’s

panel

Program

Offset value

Data protection

Signal

Parameters

key

Setting data

CNC memory

Fig. 1.6 (f) Data protection key

424

B-64124EN/01

OPERATION

1. GENERAL

1.7

DISPLAY

1.7.1

The contents of the currently active program are displayed. In addition,

the programs scheduled next and the program list are displayed.

Program Display

(See Section III-11.2.1)

Active sequence number

Active program number

PROGRAM

1100

00005

G90 G17 G00 G41 D07 X250.0 Y550.0 ;

G01 Y900.0 F150 ;

X450.0 ;

G03 X500.0 Y1150.0 R650.0 ;

N5 G02 X900.0 R-250.0 ;

Program

G03 X950.0 Y900.0 R650.0 ;

content

N7 G01 X1150.0 ;

Y550.0 ;

X700.0 Y650.0 ;

N10 X250.0 Y550.0 ;

N11 G00 G40 X0 Y0 ;

MEM STOP * * *

* * *

13 : 18 : 14

PRGRM

CHECK

CURRNT

(OPRT)

Currently executed program

The cursor indicates the currently executed location

PROGRAM DIRECTORY

O0001 N00010

PROGRAM (NUM.) MEMORY (CHAR.)

USED:

3321

FREE:

429

O0001

(MACRO-GCODE.MAIN)

O0002

(MACRO-GCODE.SUB1)

O0010

(TEST-PROGRAM.ARTHMETIC NO.1)

O0020

(TEST-PROGRAM.F10-MACRO)

O0040

(TEST-PROGRAM.OFFSET)

O0050

O0100

(INCH/MM CONVERT CHECK NO.1)

O0200

(MACRO-MCODE.MAIN)

> _

EDIT **** *** ***

16:05:59

[ PRGRM ]

[

DIR+

]

[

]

[

]

[

(OPRT) ]

425

1. GENERAL

OPERATION

B-64124EN/01

1.7.2

The current position of the tool is displayed with the coordinate values.

The distance from the current position to the target position can also be

Current Position

displayed. (See Section III-11.1.1 to 11.1.3)

Display

Workpiece coordinate system

ACTUAL POSITION (ABSOLUTE)

O0003 N00003

X 150.000

Y 300.000

Z 100.000

PART COUNT 30

RUN TIME

0H41M CYCLE TIME 0H 0M22S

MEM

* * * *

* * *

19 : 47 : 45

ABS

REL

ALL

(OPRT)

1.7.3

When a trouble occurs during operation, alarm number and alarm

message are displayed on the screen. (See Section III-7.1)

Alarm Display

See APPENDIX G for the list of alarms and their meanings.

ALARM MESSAGE

O1000 N00003

010

IMPROPER G-CODE

MEM STOP

* * *

ALM

19 : 55 : 22

ALARM

MSG

HISTRY

426

B-64124EN/01

OPERATION

1. GENERAL

1.7.4

Run time and number of parts are displayed on the screen. (See Section

lll-11.4.5)

Parts Count Display,

Run Time Display

ACTUAL POSITION (ABSOLUTE)

O0003 N00003

X 150.000

Y 300.000

Z 100.000

PART COUNT 18

RUN TIME

0H16M CYCLE TIME 0H 1M 0S

MEM STRT

FIN

* * * *

20 : 22 : 23

ABS

REL

ALL

(OPRT)

1.7.5

Programmed tool movement can be displayed on the following planes:

(See Section III-12)

Graphic Display

1) XY plane

2) YZ plane

3) XZ plane

4) Three dimensional display

(1)

(2)

Display on the XY plane

Display on the YZ plane

(3)

(4)

Display on the XZ plane

Three dimensional display (isometric)

Fig. 1.7.5 Graphic display

427

1. GENERAL

OPERATION

B-64124EN/01

1.8

Programs, offset values, parameters, etc. input in CNC memory can be

output to paper tape, cassette, or a floppy disk for saving. After once

DATA INPUT /

output to a medium, the data can be input into CNC memory.

OUTPUT

Portable tape reader

FANUC PPR

Memory

Paper tape

Program

FANUC Floppy Cassette

Reader/puncher

FANUC Floppy

Offset

interface

cassette adaptor

Parameters

Floppy disk

SYSTEM P

CNC

Automatic programming system

Memory card

adapter

(incorporated CNC)

Fig. 1.8 Data Output

428

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 15