Content      ..      1      2      3      ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 2

B-64124EN/01

PROGRAMMING

1. GENERAL

Symbols of the programmed commands G01, G02, ... are called the

preparatory function and specify the type of interpolation conducted in

the control unit.

(a) Movement along straight line

(b) Movement along arc

G01 Y_ _;

G03X--Y--R--;

X- -Y- - - -;

Control unit

X axis

Tool

Interpolation

move-

ment

Y axis

a)Movement

along straight

line

b)Movement

along arc

Fig. 1.1 (c) Interpolation function

NOTE

Some machines move tables instead of tools but this

manual assumes that tools are moved against workpieces.

13

1. GENERAL

PROGRAMMING

B-64124EN/01

Movement of the tool at a specified speed for cutting a workpiece is called

1.2

the feed.

FEED-FEED

FUNCTION

mm/min

Tool

F

Workpiece

Table

Fig. 1.2 Feed function

Feedrates can be specified by using actual numerics. For example, to feed

the tool at a rate of 150 mm/min, specify the following in the program:

F150.0

The function of deciding the feed rate is called the feed function (See

II-5).

14

B-64124EN/01

PROGRAMMING

1. GENERAL

1.3

PART DRAWING AND

TOOL MOVEMENT

1.3.1

A CNC machine tool is provided with a fixed position. Normally, tool

change and programming of absolute zero point as described later are

Reference Position

performed at this position. This position is called the reference position.

(Machine-Specific

Position)

Reference position

Tool

Workpiece

Table

Fig. 1.3.1 Reference position

Explanations

The tool can be moved to the reference position in two ways:

(1) Manual reference position return (See III-3.1)

Reference position return is performed by manual button operation.

(2) Automatic reference position return (See II-6)

In general, manual reference position return is performed first after the

power is turned on. In order to move the tool to the reference position

for tool change thereafter, the function of automatic reference position

return is used.

15

1. GENERAL

PROGRAMMING

B-64124EN/01

1.3.2

Coordinate System on

Part Drawing and

Z

Coordinate System

Z

Specified by CNC -

Program

Y

Y

Coordinate System

X

X

Coordinate system

Part drawing

CNC

Command

Tool

Z

Y

Workpiece

X

Machine tool

Fig. 1.3.2 (a) Coordinate system

Explanations

D Coordinate system

The following two coordinate systems are specified at different locations:

(See II-7)

(1) Coordinate system on part drawing

The coordinate system is written on the part drawing. As the program

data, the coordinate values on this coordinate system are used.

(2) Coordinate system specified by the CNC

The coordinate system is prepared on the actual machine tool table.

This can be achieved by programming the distance from the current

position of the tool to the zero point of the coordinate system to be set.

Y

230

Present tool position

300

Distance to the zero point of a coor-

Program

dinate system to be set

zero point

X

Fig. 1.3.2 (b) Coordinate system specified by the CNC

16

B-64124EN/01

PROGRAMMING

1. GENERAL

The positional relation between these two coordinate systems is

determined when a workpiece is set on the table.

Coordinate system on

part drawing established

on the workpiece

Coordinate system spe-

cified by the CNC estab-

lished on the table

Y Y

Workpiece

X

X

Table

Fig. 1.3.2 (c) Coordinate system specified by CNC and coordinate

systemon part drawing

The tool moves on the coordinate system specified by the CNC in

accordance with the command program generated with respect to the

coordinate system on the part drawing, and cuts a workpiece into a shape

on the drawing.

Therefore, in order to correctly cut the workpiece as specified on the

drawing, the two coordinate systems must be set at the same position.

D Methods of setting the

To set the two coordinate systems at the same position, simple methods

two coordinate systems

shall be used according to workpiece shape, the number of machinings.

in the same position

(1) Using a standard plane and point of the workpiece.

Y

Workpiece’s

Fixed distance

standard point

Fixed distance

Program

zero point

X

Bring the tool center to the workpiece standard point.

And set the coordinate system specified by CNC at this position.

17

1. GENERAL

PROGRAMMING

B-64124EN/01

(2) Mounting a workpiece directly against the jig

Program zero point

Jig

Meet the tool center to the reference position. And set the coordinate system

specified by CNC at this position. (Jig shall be mounted on the predetermined

point from the reference position.)

(3) Mounting a workpiece on a pallet, then mounting the workpiece and

pallet on the jig

ÂÂÂÂÂÂÂ

ÂPalletÂÂÂÂÂ

 ÂÂÂÂ

Â

ÂÂ

Jig

Â

ÂÂ

Workpiece

Â

ÂÂ

ÂÂÂÂÂÂÂ

ÂÂÂÂÂÂÂ

(Jig and coordinate system shall be specified by the same as (2)).

18

B-64124EN/01

PROGRAMMING

1. GENERAL

1.3.3

How to Indicate

Command Dimensions

for Moving the Tool -

Absolute, Incremental

Commands

Explanations

Command for moving the tool can be indicated by absolute command or

incremental command (See II-8.1).

D Absolute command

The tool moves to a point at “the distance from zero point of the

coordinate system” that is to the position of the coordinate values.

Z

Tool

A

Y

X

B(10.0,30.0,20.0)

Command specifying movement from G90 X10.0 Y30.0 Z20.0 ;

point A to point B

Coordinates of point B

D Incremental command

Specify the distance from the previous tool position to the next tool

position.

Z

Tool

A

X=40.0

Y

Z=-10.0

B

X

Y=-30.0

Command specifying movement from

G91 X40.0 Y-30.0 Z-10.0 ;

point A to point B

Distance and direction for

movement along each axis

19

1. GENERAL

PROGRAMMING

B-64124EN/01

1.4

The speed of the tool with respect to the workpiece when the workpiece

is cut is called the cutting speed.

CUTTING SPEED -

As for the CNC, the cutting speed can be specified by the spindle speed

SPINDLE SPEED

in min^-1 unit.

FUNCTION

Tool

Tool diameter

Spindle speed N

min^-1

f D mm

V: Cutting speed

m/min

Workpiece

Examples

<When a workpiece should be machined with a tool 100 mm in

diameter at a cutting speed of 80 m/min. >

The spindle speed is approximately 250 min^-1, which is obtained from

N=1000v/πD. Hence the following command is required:

S250;

Commands related to the spindle speed are called the spindle speed

function (See II-9) .

20

B-64124EN/01

PROGRAMMING

1. GENERAL

1.5

When drilling, tapping, boring, milling or the like, is performed, it is

necessary to select a suitable tool. When a number is assigned to each tool

SELECTION OF TOOL

and the number is specified in the program, the corresponding tool is

USED FOR VARIOUS

selected.

MACHINING - TOOL

FUNCTION

Tool number

01

ATC magazine

02

Examples

<When No.01 is assigned to a drilling tool>

When the tool is stored at location 01 in the ATC magazine, the tool

can be selected by specifying T01. This is called the tool function (See

II-10).

21

1. GENERAL

PROGRAMMING

B-64124EN/01

1.6

When machining is actually started, it is necessary to rotate the spindle,

and feed coolant. For this purpose, on-off operations of spindle motor and

COMMAND FOR

coolant valve should be controlled.

MACHINE

OPERATIONS -

MISCELLANEOUS

Tool

FUNCTION

Coolant

Workpiece

The function of specifying the on-off operations of the components of the

machine is called the miscellaneous function. In general, the function is

specified by an M code (See II-11).

For example, when M03 is specified, the spindle is rotated clockwise at

the specified spindle speed.

22

B-64124EN/01

PROGRAMMING

1. GENERAL

A group of commands given to the CNC for operating the machine is

1.7

called the program. By specifying the commands, the tool is moved along

PROGRAM

a straight line or an arc, or the spindle motor is turned on and off.

CONFIGURATION

In the program, specify the commands in the sequence of actual tool

movements.

Block

Block

Tool movement sequence

Block

Program

Block

⋅

⋅

⋅

⋅

Block

Fig. 1.7 (a) Program configuration

A group of commands at each step of the sequence is called the block.

The program consists of a group of blocks for a series of machining. The

number for discriminating each block is called the sequence number, and

the number for discriminating each program is called the program

number (See II-12).

23

1. GENERAL

PROGRAMMING

B-64124EN/01

Explanations

The block and the program have the following configurations.

D Block

1 block

N ffff G ff Xff.f Yfff.f M ff S ff T ff ;

Sequence Preparatory Dimension word Miscel-

Spindle Tool

number function

laneous

function func-

function

tion

End of

block

Fig. 1.7 (b) Block configuration

A block starts with a sequence number to identify the block and ends with

an end-of-block code.

This manual indicates the end-of-block code by ; (LF in the ISO code and

CR in the EIA code).

The contents of the dimension word depend on the preparatory function.

In this manual, the portion of the dimension word may be represent as IP_.

D Program

;

Offff;

Program number

Block

Block

Block

⋅

⋅

⋅

⋅

⋅

⋅

M30 ;

End of program

Fig. 1.7 (c) Program configuration

Normally, a program number is specified after the end-of-block (;) code

at the beginning of the program, and a program end code (M02 or M30)

is specified at the end of the program.

24

B-64124EN/01

PROGRAMMING

1. GENERAL

D Main program and

When machining of the same pattern appears at many portions of a

subprogram

program, a program for the pattern is created. This is called the

subprogram. On the other hand, the original program is called the main

program. When a subprogram execution command appears during

execution of the main program, commands of the subprogram are

executed. When execution of the subprogram is finished, the sequence

returns to the main program.

Main program

⋅

Subprogram #1

⋅

M98P1001

O1001

Program for

hole #1

⋅

⋅

⋅

M99

M98P1002

⋅

⋅

Subprogram #2

O1002

Program for

M98P1001^⋅

hole #2

⋅

⋅

⋅

M99

Hole #1

Hole #1

Hole #2

Hole #2

25

1. GENERAL

PROGRAMMING

B-64124EN/01

1.8

TOOL FIGURE AND

TOOL MOTION BY

PROGRAM

Explanations

D Machining using the end

Usually, several tools are used for machining one workpiece. The tools

of cutter - Tool length

have different tool length. It is very troublesome to change the program

compensation function

in accordance with the tools.

(See II-14.1)

Therefore, the length of each tool used should be measured in advance.

By setting the difference between the length of the standard tool and the

length of each tool in the CNC (data display and setting : see III-11),

machining can be performed without altering the program even when the

tool is changed. This function is called tool length compensation.

ÇÇÇ

ÂÂ

ÇÇÇ

ÂÂ

H1

H2

H3

H4

StandardÇÇ

ÂÂ

tool

ÇÇÇ

ÂÂ

ÇÇÇ

ÂÂ

ÇÇÇ

Workpiece

D Machining using the side

Because a cutter has a radius, the center of the cutter path goes around the

of cutter - Cutter

workpiece with the cutter radius deviated.

compensation function

(See II-14.4,14.5,14.6)

Cutter path using cutter

compensation

Machined part

figure

Workpiece

Cutter

If radius of cutters are stored in the CNC (Data Display and Setting : see

III-11), the tool can be moved by cutter radius apart from the machining

part figure. This function is called cutter compensation.

26

B-64124EN/01

PROGRAMMING

1. GENERAL

Limit switches are installed at the ends of each axis on the machine to

1.9

prevent tools from moving beyond the ends. The range in which tools can

TOOL MOVEMENT

move is called the stroke.

RANGE - STROKE

Table

Motor

Limit switch

Machine zero point

Specify these distances.

ÇÇÇÇÇÇ

ÇÇÇÇÇÇ

ÇÇÇÇÇÇ

Tools cannot enter this area. The area is specified by data in memory or

a program.

Besides strokes defined with limit switches, the operator can define an

area which the tool cannot enter using a program or data in memory. This

function is called stroke check (see III-6.3).

27

B-64124EN/01

PROGRAMMING

2. CONTROLLED AXES

2.1

CONTROLLED AXES

Item

0i-MC

No. of basic controlled axes

3 axes

Controlled axes expansion (total)

Max. 4 axes (included in Cs axis)

Basic simultaneously controlled axes

3 axes

Simultaneously controlled axes

Max. 4 axes

expansion (total)

NOTE

The number of simultaneously controllable axes for manual

operation jog feed, manual reference position return, or

manual rapid traverse) is 1 or 3 (1 when bit 0 (JAX) of

parameter 1002 is set to 0 and 3 when it is set to 1).

2.2

The names of three basic axes are always X, Y, and Z. The name of an

additional axis can be set to A, B, C, U, V, or W by using parameter 1020.

AXIS NAME

Parameter No. 1020 is used to determine the name of each axis.

Limitations

D Default axis name

When this parameter is set to 0 or a character other than the valid

characters is specified, an axis name from 1 to 4 is assigned by default.

When a default axis name (1 to 4) is used, operation in the MEM mode

and MDI mode is disabled.

D Duplicate axis names

If a duplicate axis name is specified in the parameter, operation is enabled

only for the axis specified first.

29

2. CONTROLLED AXES

PROGRAMMING

B-64124EN/01

2.3

The increment system consists of the least input increment (for input) and

least command increment (for output). The least input increment is the

INCREMENT SYSTEM

least increment for programming the travel distance. The least command

increment is the least increment for moving the tool on the machine. Both

increments are represented in mm, inches, or deg.

Set bit 1 (ISC) of parameter No. 1004 to select which increment system

to use. The setting of bit 1 (ISC) of parameter No. 1004 is applied to all

the axes. For example, when IS-C is selected, the increment system for

all the axes is IS-C.

Name of

Least input

Least command

Maximum

increment system

increment

increment

stroke

0.001mm

0.001mm

99999.999mm

IS-B

0.0001inch

0.0001inch

9999.9999inch

0.001deg

0.001deg

99999.999deg

0.0001mm

0.0001mm

9999.9999mm

IS-C

0.00001inch

0.00001inch

999.99999inch

0.0001deg

0.0001deg

9999.9999deg

The least command increment is either metric or inch depending on the

machine tool. Set metric or inch to the parameter INM (No.100#0).

For selection between metric and inch for the least input increment, G

code (G20 or G21) or a setting parameter selects it.

Combined use of the inch system and the metric system is not allowed.

There are functions that cannot be used between axes with different unit

systems (circular interpolation, cutter compensation, etc.). For the

increment system, see the machine tool builder’s manual.

2.4

Maximum stroke = Least command increment

99999999

See table 2.4 Incremen System.

MAXIMUM STROKE

Table 2.4 Maximum strokes

Increment system

Maximum stroke

Metric machine system

± 99999.999 mm

± 99999.999 deg

IS–B

Inch machine system

± 9999.9999 inch

± 99999.999 deg

Metric machine system

± 9999.9999 mm

± 9999.9999 deg

IS–C

Inch machine system

± 999.99999 inch

± 9999.9999 deg

NOTE

1

A command exceeding the maximum stroke cannot be

specified.

2

The actual stroke depends on the machine tool.

30

3. PREPARATORY FUNCTION

B-64124EN/01

PROGRAMMING

(G FUNCTION)

PREPARATORY FUNCTION (G FUNCTION)

3

A number following address G determines the meaning of the command

for the concerned block.

G codes are divided into the following two types.

Type

Meaning

One-shot G code

The G code is effective only in the block in which it is

specified.

Modal G code

The G code is effective until another G code of the

same group is specified.

(Example )

G01 and G00 are modal G codes in group 01.

G01X ;

Z;

G01 is effective in this range.

X;

G00Z ;

31

3. PREPARATORY FUNCTION

B-64124EN/01

PROGRAMMING

(G FUNCTION)

Table 3 G code list (1/3)

G code

Group

Function

G00

Positioning

G01

Linear interpolation

01

G02

Circular interpolation/Helical interpolation CW

G03

Circular interpolation/Helical interpolation CCW

G04

Dwell, Exact stop

G05.1

AI advanced control/AI contour control

G07.1 (G107)

Cylindrical interpolation

G08

00

Advanced preview control

G09

Exact stop

G10

Programmable data input

G11

Programmable data input mode cancel

G15

Polar coordinates command cancel

17

G16

Polar coordinates command

G17

XpYp plane selection

Xp: X axis or its parallel axis

G18

02

ZpXp plane selection

Yp: Y axis or its parallel axis

G19

YpZp plane selection

Zp: Z axis or its parallel axis

G20

Input in inch

06

G21

Input in mm

G22

Stored stroke check function on

04

G23

Stored stroke check function off

G27

Reference position return check

G28

Return to reference position

G29

00

Return from reference position

G30

2nd, 3rd and 4th reference position return

G31

Skip function

G33

01

Thread cutting

G37

Automatic tool length measurment

00

G39

Corner offset circular interpolation

G40

Cutter compensation cancel/Three dimensional compensation cancel

G41

07

Cutter compensation left/Three dimensional compensation

G42

Cutter compensation right

G40.1 (G150)

Normal direction control cancel mode

G41.1 (G151)

19

Normal direction control left side on

G42.1 (G152)

Normal direction control right side on

G43

Tool length compensation + direction

08

G44

Tool length compensation - direction

G45

Tool offset increase

G46

Tool offset decrease

00

G47

Tool offset double increase

G48

Tool offset double decrease

33

3.

PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64124EN/01

Table 3 G code list (2/3)

G code

Group

Function

G49

08

Tool length compensation cancel

G50

Scaling cancel

11

G51

Scaling

G50.1

Programmable mirror image cancel

22

G51.1

Programmable mirror image

G52

Local coordinate system setting

00

G53

Machine coordinate system selection

G54

Workpiece coordinate system 1 selection

G54.1

Additional workpiece coordinate system selection

G55

Workpiece coordinate system 2 selection

G56

14

Workpiece coordinate system 3 selection

G57

Workpiece coordinate system 4 selection

G58

Workpiece coordinate system 5 selection

G59

Workpiece coordinate system 6 selection

G60

00/01

Single direction positioning

G61

Exact stop mode

G62

Automatic corner override

15

G63

Tapping mode

G64

Cutting mode

G65

00

Macro call

G66

Macro modal call

12

G67

Macro modal call cancel

G68

Coordinate rotation/Three dimensional coordinate conversion

16

Coordinate rotation cancel/Three dimensional coordinate conversion

G69

cancel

G73

Peck drilling cycle

09

G74

Counter tapping cycle

G75

01

Plunge grinding cycle (for grinding machine)

G76

09

Fine boring cycle

G77

Direct constant-dimension plunge grinding cycle(for grinding machine)

G78

01

Continuous-feed surface grinding cycle(for grinding machine)

G79

Intermittent-feed surface grinding cycle(for grinding machine)

G80

Canned cycle cancel/external operation function cancel

G81

Drilling cycle, spot boring cycle or external operation function

G82

Drilling cycle or counter boring cycle

G83

Peck drilling cycle

G84

09

Tapping cycle

G85

Boring cycle

G86

Boring cycle

G87

Back boring cycle

G88

Boring cycle

G89

Boring cycle

34

3. PREPARATORY FUNCTION

B-64124EN/01

PROGRAMMING

(G FUNCTION)

Table 3 G code list (3/3)

G code

Group

Function

G90

Absolute command

03

G91

Increment command

G92

Setting for work coordinate system or clamp at maximum spindle speed

00

G92.1

Workpiece coordinate system preset

G94

Feed per minute

05

G95

Feed per rotation

G96

Constant surface speed control

13

G97

Constant surface speed control cancel

G98

Return to initial point in canned cycle

10

G99

Return to R point in canned cycle

G160

In-feed control function cancel (for grinding machine)

20

G161

In-feed control function (for grinding machine)

35

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.1

The G00 command moves a tool to the position in the workpiece system

specified with an absolute or an incremental command at a rapid traverse

POSITIONING

rate.

(G00)

In the absolute command, coordinate value of the end point is

programmed.

In the incremental command the distance the tool moves is programmed.

Format

G00

IP

_;

IP: For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance

the tool moves.

Explanations

Either of the following tool paths can be selected according to bit 1 of

parameter LRP No. 1401.

D Nonlinear interpolation positioning

The tool is positioned with the rapid traverse rate for each axis

separately. The tool path is normally straight.

D Linear interpolation positioning

The tool path is the same as in linear interpolation (G01). The tool is

positioned within the shortest possible time at a speed that is not more

than the rapid traverse rate for each axis. However, the tool path is not

the same as in linear interpolation (G01).

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

The rapid traverse rate in G00 command is set to the parameter No. 1420

for each axis independently by the machine tool builder. In the

posiitoning mode actuated by G00, the tool is accelerated to a

predetermined speed at the start of a block and is decelerated at the end

of a block. Execution proceeds to the next block after confirming the

in-position.

“In-position ” means that the feed motor is within the specified range.

This range is determined by the machine tool builder by setting to

parameter (No. 1826).

In-position check for each block can be disabled by setting bit 5 (NCI)

of parameter No.1601 accordingly.

37

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.2

For accurate positioning without play of the machine (backlash), final

positioning from one direction is available.

SINGLE DIRECTION

POSITIONING (G60)

Overrun

Start position

Start position

Temporary stop

End position

Format

G60

_;

IP

IP : For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance

the tool moves.

Explanations

An overrun and a positioning direction are set by the parameter (No.

5440). Even when a commanded positioning direction coincides with

that set by the parameter, the tool stops once before the end point.

G60, which is an one-shot G-code, can be used as a modal G-code in

group 01 by setting 1 to the parameter (No. 5431 bit 0 MDL).

This setting can eliminate specifying a G60 command for every block.

Other specifications are the same as those for an one-shot G60 command.

When an one-shot G code is sepcified in the single direction positioning

mode, the one-shot G command is effective like G codes in group 01.

Examples

When one-shot

When modal

G60 commands are used.

G60 command is used.

G90;

G90G60;

Single direction

positioning mode start

G60

X0Y0;

X0Y0;

Single direction

Single direction

G60

X100;

X100;

positioning

positioning

G60

Y100;

Y100;

G04

X10;

G04X10;

G00

X0Y0;

G00X0Y0; Single direction

positioning

mode cancel

39

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Tools can move along a line

4.3

LINEAR

INTERPOLATION

(G01)

Format

G01

IP_F_;

_:For an absolute command, the coordinates of an end point ,

IP

and for an incremental commnad, the distance the tool moves.

F_:Speed of tool feed (Feedrate)

Explanations

A tools move along a line to the specified position at the feedrate

specified in F.

The feedrate specified in F is effective until a new value is specified. It

need not be specified for each block.

The feedrate commanded by the F code is measured along the tool path.

If the F code is not commanded, the feedrate is regarded as zero.

The feedrate of each axis direction is as follows.

G01ααββγγζζ

Ff ;

Feed rate of α axis direction : Fa +a

f

L

b

Feed rate of β axis direction :

F_b +

f

L

g

Feed rate of γ axis direction :

Fg +

f

L

z

Feed rate of ζ axis direction : F_z +

f

L

L + a2 ) b2 ) g2 ) z²Ǹ

The feed rate of the rotary axis is commanded in the unit of deg/min (the

unit is decimal point position).

When the straight line axis α(such as X, Y, or Z) and the rotating axisβ

(such as A, B, or C) are linearly interpolated, the feed rate is that in which

the tangential feed rate in the αandβ cartesian coordinate system is

commanded by F(mm/min).

β-axis feedrate is obtained ; at first, the time required for distribution is

calculated by using the above fromula, then the β -axis feedrate unit is

changed to deg 1min.

41

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

A calcula;tion example is as follows.

G91 G01 X20.0B40.0 F300.0 ;

This changes the unit of the C axis from 40.0 deg to 40mm with metric

input. The time required for distribution is calculated as follows:

^Ǹ20² ) 40²

8 0.14907

(min)

300

The feed rate for the C axis is

40

8

268.3 degńmin

0.14907

In simultaneous 3 axes control, the feed rate is calculated the same way

as in 2 axes control.

Examples

D Linear interpolation

(G91) G01X200.0Y100.0F200.0 ;

Y axis

(End position)

100.0

X axis

0

(Start position)

200.0

D Feedrate for the

rotation axis

G91G01C-90.0 G300.0 ;Feed rate of 300deg/min

(Start point)

90°

(End point)

Feedrate is 300 deg/min

42

Content      ..      1      2      3      ..