FANUC Series 0i-MC. OPERATOR’S MANUAL

8. COORDINATE VALUE

B-64124EN/01

PROGRAMMING

AND DIMENSION

Either inch or metric input can be selected by G code.

8.3

INCH/METRIC

CONVERSION

(G20,G21)

Format

G20 ; Inch input

G21 ;_{mm input}

This G code must be specified in an independent block before setting the

coordinate system at the beginning of the program. After the G code for

inch/metric conversion is specified, the unit of input data is switched to

the least inch or metric input increment of increment system IS-B or IS-C

(II-2.3). The unit of data input for degrees remains unchanged.The unit

systems for the following values are changed after inch/metric

conversion:

- Feedrate commanded by F code

- Positional command

- Work zero point offset value

- Tool compensation value

- Unit of scale for manual pulse generator

- Movement distance in incremental feed

- Some parameters

When the power is turned on, the G code is the same as that held before

the power was turned off.

WARNING

G20 and G21 must not be switched during a program.

When switching inch input (G20) to metric input (G21) and vice versa, the tool compensation

value must be re-set according to the least input increment.

However, when bit 0 (OIM) of parameter 5006 is 1, tool compensation values are automatically

converted and need not be re-set.

CAUTION

For the first G28 command after switching inch input to metric input or vice versa, operation from

the intermediate point is the same as that for manual reference position return. The tool moves

from the intermediate point in the direction for reference position return, specified with bit 5

(ZMI) of parameter No. 1006.

NOTE

When the least input increment and the least command increment systems are different, the

maximum error is half of the least command increment. This error is not accumulated.

The inch and metric input can also be switched using settings. (See III-11.4.3)

103

8. COORDINATE VALUE

AND DIMENSION

PROGRAMMING

B-64124EN/01

Numerical values can be entered with a decimal point. A decimal point

8.4

can be used when entering a distance, time, or speed. Decimal points can

DECIMAL POINT

be specified with the following addresses:

PROGRAMMING

X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, and F.

Explanations

There are two types of decimal point notation: calculator-type notation

and standard notation.

When calculator-type decimal notation is used, a value without decimal

point is considered to be specified in millimeters inch,or deg. When

standard decimal notation is used, such a value is considered to be

specified in least input increments.Select either calculator-type or

standard decimal notation by using the DPI bit (bit 0 of parameter

3401).Values can be specified both with and without decimal point in a

single program.

Examples

Pocket calculator

Standard type decimal

Program command

type decimal point

point programming

programming

X1000

1000mm

1mm

Command value without

Unit : mm

Unit : Least input increment

decimal point

(0.001 mm)

X1000.0

1000mm

Command value with

Unit : mm

decimal point

WARNING

In a single block, specify a G code before entering a value. The position of decimal point may

depend on the command.

Examples:

G20;

Input in inches

X1.0 G04;

X1.0 is considered to be a distance and processed as X10000. This command

is equivalent to G04 X10000. The tool dwells for 10 seconds.

G04 X1.0;

Equivalent to G04 X1000. The tool dwells for one second.

NOTE

1 Fractions less than the least input increment are truncated.

Examples:

X1.23456;

Truncated to X1.234 when the least input increment is 0.001 mm.

Processed as X1.2345 when the least input increment is 0.0001 inch.

2 When more than eight digits are specified, an alarm occurs. If a value is entered with a decimal

point, the number of digits is also checked after the value is converted to an integer according

to the least input increment.

Examples:

X1.23456789; P/S alarm 0.003 occurs because more than eight digits are specified.

X123456.7; If the least input increment is 0.001 mm, the value is converted to integer

123456700. Because the integer has more than eight digits, an alarm occurs.

104

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64124EN/01

When a value is specified after address S, the code signal and strobe signal

9.1

are sent to the machine to control the spindle rotation speed.

SPECIFYING THE

A block can contain only one S code. Refer to the appropriate manual

SPINDLE SPEED

provided by the machine tool builder for details such as the number of

digits in an S code or the execution order when a move command and an

WITH A CODE

S code command are in the same block.

9.2

The spindle speed can be specified directly by address S followed by a

max.five-digit value (min^-1). The unit for specifying the spindle speed

SPECIFYING THE

may vary depending on the machine tool builder. Refer to the appropriate

SPINDLE SPEED

manual provided by the machine tool builder for details.

VALUE DIRECTLY

(S5-DIGIT

COMMAND)

106

9. SPINDLE SPEED FUNCTION

B-64124EN/01

PROGRAMMING

(S FUNCTION)

Specify the surface speed (relative speed between the tool and workpiece)

9.3

following S. The spindle is rotated so that the surface speed is constant

CONSTANT

regardless of the position of the tool.

SURFACE SPEED

CONTROL (G96, G97)

Format

D Constant surface speed

control command

G96 Sfffff ;

↑ Surface speed (m/min or feet/min)

Note : This surface speed unit may change according to machine tool

builder’s specification.

D Constant surface speed

control cancel command

G97 Sfffff ;

↑ Spindle speed (min^-1)

Note : This surface speed unit may change according to machine tool

builder’s specification.

D Constant surface speed

controlled axis

G96 Pα ;_{P0 : Axis set in the parameter (No. 3770)}

command

P1 : X axis, P2 : Y axis, P3 : Z axis, P4 : 4th axis

D Clamp of maximum

spindle speed

G92 S_ ;

The maximum spindle speed (min^-1) follows S.

107

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64124EN/01

Explanations

D Constant surface speed

G96 (constant surface speed control command) is a modal G code. After

control command (G96)

a G96 command is specified, the program enters the constant surface

speed control mode (G96 mode) and specified S values are assumed as a

surface speed. A G96 command must specify the axis along which

constant surface speed control is applied. A G97 command cancels the

G96 mode.When constant surface speed control is applied, a spindle

speed higher than the value specified in G92S_; (maximum spindle

speed) is clamped at the maximum spindle speed. When the power is

turned on, the maximum spindle speed is not yet set and the speed is not

clamped.S (surface speed) commands in the G96 mode are assumed as S

= 0 (the surface speed is 0) until M03 (rotating the spindle in the positive

direction) or M04 (rotating the spindle in the negative direction) appears

in the program.

Spindle speed (min^-1)

The spindle speed (min^-1) almost

coincides with the surface speed

(m/min) at approx. 160 mm (radius).

Surface speed

S is 600 m/min.

radius (mm)

Fig. 9.3 (a) Relation between workpiece radius, spindle speed

and surface speed

D Setting the workpiece

To execute the constant surface speed control, it is necessary to set the

coordinate system for

work coordinate system , and so the coordinate value at the center of the

constant surface speed

rotary axis, for example, Z axis, (axis to which the constant surface speed

control

control applies) becomes zero.

Fig. 9.3 (b) Example of the workpiece coordinate system for

constant surface speed control

108

9. SPINDLE SPEED FUNCTION

B-64124EN/01

PROGRAMMING

(S FUNCTION)

D Surface speed specified

in the G96 mode

G96 mode

G97 mode

Specify the surface speed in m/min

(or feet/min)

G97 command

Store the surface speed in m/min

(or feet/min)

Specified

Command for

The specified

the spindle

spindle speed

speed

(min^-1) is used

Not specified

The surface speed (m/min or

feet/min) is converted to the

spindle speed (min^-1)

Commands other than G96

G96 command

Specified

The specified

surface

Command

speed is used

for the surface

speed

Not specified

The stored surface speed (m/min or

feet/min) is used. If no surface speed

is stored, 0 is assumed.

Restrictions

D Constant surface speed

The constant surface speed control is also effective during threading.

control for threading

Accordingly, it is recommended that the constant surface speed control

be invalidated with G97 command before starting the scroll threading and

taper threading, because the response problem in the servo system may

not be considered when the spindle speed changes.

D Constant surface speed

In a rapid traverse block specified by G00, the constant surface speed

control for rapid traverse

control is not made by calculating the surface speed to a transient change

(G00)

of the tool position, but is made by calculating the surface speed based on

the position at the end point of the rapid traverse block, on the condition

that cutting is not executed at rapid traverse.

109

10. TOOL FUNCTION

B-64124EN/01

PROGRAMMING

(T FUNCTION)

10.1

By specifying an up to 8-digit numerical value following address T, tools

can be selected on the machine.

TOOL SELECTION

One T code can be commanded in a block. Refer to the machine tool

FUNCTION

builder’s manual for the number of digits commandable with address T

and the correspondence between the T codes and machine operations.

When a move command and a T code 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 T function

commands.

(ii)Executing T function commands upon completion of move command

execution.

The selection of either (i) or (ii) depends on the machine tool builder’s

specifications. Refer to the manual issued by the machine tool builder

for details.

111

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-64124EN/01

10.2

Tools are classified into various groups, with the tool life (time or

frequency of use) for each group being specified. The function of

TOOL LIFE

accumulating the tool life of each group in use and selecting and using

MANAGEMENT

the next tool previously sequenced in the same group, is called the tool

FUNCTION

life management function.

Tool group number m

Code specifying

Tool

Tool life

The first tool life

tool compensa-

number

management data

tion value

The nth tool life

management data

Fig. 10.2 (a) Tool life management data (number of n tools)

By choosing a tool from a tool group specified by a machining program,

the tool life can be managed.

Tool life management data

Machining program

Machine and CNC operations

Tool group number 1

Machine

CNC

Places a se-

Automatically selects, from

Tool

lected tool in

tool group m, a tool whose

selection

Command for selecting

the wait state

life has not expired.

Tool group number m

tool group m

Attaches the

Starts counting the life of

tool in the wait

Tool change command

the tool attached to the

state to

(M06)

spindle.l

the spindle

Tool group number p

(tool change).

Fig. 10.2 (b) Tool Selection by machining program

112

10. TOOL FUNCTION

B-64124EN/01

PROGRAMMING

(T FUNCTION)

10.2.1

Tool life management data consists of tool group numbers, tool numbers,

codes specifying tool compensation values, and tool life value.

Tool Life Management

Data

Explanations

D Tool group number

The Max. number of groups and the number of tools per group that can

be registered are set by parameter (GS1,GS2 No. 6800#0, #1) (Table

10.2.1).

Table 10.2.1 The Max. number of groups and tools that can be registered

GS1

GS2

Number of group

Number of tool

(No. 6800#0)

(No. 6800#1)

128

WARNING

When bits 0 or 1 of parameter GS1,GS2 No.6800 is

changed, re-register tool life management data with the

G10L3 command (for registering and deleting data for all

groups). Otherwise, new data pairs cannot be set.

D Tool number

Specify a four-digit number after T.

D Code specifying tool

Codes specifying tool offset values are classified into H codes (for tool

compensation value

length offset) and D codes (cutter compensation). The maximum number

of the tool compensation value specification code which can be registered

is 255 when there are 400 tool compensation values.

NOTE

When codes specifying tool offset values are not used,

registration can be omitted.

D Tool life value

Refer to II-10.2.2 and II-10.2.4.

113

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-64124EN/01

10.2.2

In a program, tool life management data can be registered in the CNC unit,

and registered tool life management data can be changed or deleted.

Delete of Tool Life

Management Data

Explanations

A different program format is used for each of the four types of operations

described below.

D Register with deleting

After all registered tool life management data is deleted, programmed tool

all groups

life management data is registered.

D Addition and change of

Programmed tool life management data for a group can be added or

tool life management

changed.

data

D Deletion of tool life

Programmed tool life management data for a group can be deleted.

management data

D Register of tool life count

Count types (time or frequency can be registered for individual groups.

type

D Life value

Whether tool life is to be indicated by time (minutes) or by frequency, it

is set by a parameter LTM (No. 6800 #2) .

Maximum value of tool life is as follows.

In case of minute:4300(minutes)

In case of frequency :9999(times)

114

10. TOOL FUNCTION

B-64124EN/01

PROGRAMMING

(T FUNCTION)

Format

D Register with deleting

Format

Meaning of command

all groups

G10L3 ;

G10L3 :Register with deleting all groups

PL ;

:Group number

THD ;

:Life value

THD ;

:Tool number

:Code specifying tool offset value

(H code)

:Code specifying tool offset value

PL ;

(D code)

THD ;

G11

:End of registration

THD ;

G11 ;

M02 (M30) ;

D Addition and change of

Format

Meaning of command

tool life management

data

G10L3P1 ;

G10L3P1 :Addition and change of group

PL ;

:Group number

THD ;

:Life value

THD ;

:Tool number

:Code specifying tool offset value

(H code)

:Code specifying tool offset value

PL ;

(D code)

THD ;

G11

:End of addition and change of

THD ;

group

G11 ;

M02 (M30) ;

D Deletion of tool life

Format

Meaning of command

management data

G10L3P2 ;

G10L3P2 :Deletion of group

P ;

:Group number

P ;

G11

:End of deletion of group

P ;

G11 ;

M02 (M30) ;

115

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-64124EN/01

D Setting a tool life cout

Format

Meaning of command

type for groups

G10L3

Q_ : Life count type (1:Frequency, 2:Time)

G10L3P1);

PL Q ;

THD ;

⋅

THD ;

⋅

PL Q ;

THD ;

G11 ;

M02 (M30) ;

CAUTION

When the Q command is omitted, the value set in bit 2 (LTM)

of parameter No.6800 is used as the life count type.

G10L3P1 and G10L3L2 can be commanded only when the

extended tool life management feature is enabled.

(Parameter EXT (No.6801#6) = 1)

116

10. TOOL FUNCTION

B-64124EN/01

PROGRAMMING

(T FUNCTION)

10.2.3

Tool Life Management

Command in a

Machining Program

Explanations

D Command

The following command is used for tool life management:

Toooo; Specifies a tool group number.

The tool life management function selects, from a specified group, a

tool whose life has not expired, and outputs its T code. In oooo,

specify a number calculated by adding the tool life management cancel

number specified in parameter6810 to a group number. For example,

to set tool group 1 when the tool life management cancel number is

100, specify T101;.

NOTE

When oooo is less than a tool life management cancel

number, the T code is treated as an ordinary T code.

M06;

Terminates life management for the previously used tools,

and begins counting the life of the new tools selected with

the T code.

WARNING

When an option for speciofying multiple M codes is

selected, specify this code by itself or as the first M code.

H99;

Selects the H code of tool life management data for the tool

currently being used.

H00;

Cancels tool length offset

D99;

Selects the D code of tool life management data for the tool

currently being used.

D00;

Cancels cutter compensation

WARNING

H99 or D99 must be specified after the M06 command.

When a code other than H99 or D99 is specified after the

M06 command, the H code and D code of tool life

management data are not selected.

117

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-64124EN/01

D Types

For tool life management, the four tool change types indicated below are

available. The type used varies from one machine to another. For details,

refer to the appropriate manual of each machinde tool builder.

Table 10.2.3 Tool Change Type

Tool change

type

Tool group

Previously

Tools to be used next

number spe-

used tools

cified in the

same block

as the tool

change com-

mand (M06)

Tool life count

Life counting is performed for a tool in the

Life counting

timing

specified tool group when M06 is specified

is performed

next.

when a tool

in the tool

group speci-

fied in the

same block

as M06 is

specified.

Remarks

Normally, when a tool group

When only

number is specified by itself,

M06 is speci-

type B is used. However, no

fied, P/S

alarm is raised even if the

alarm No.

tool group number is speci-

153 is

fied by itself as type C.

issued.

Parameter

No. 6800#7

No. 6800#7 (M6T)=1

No.6801#7

(M6T)=0

No. 6801#7 (M6E)=0

(M6E)=1

No.6801#7

(M6E)=0

NOTE

When a tool group number is specified and a new tool is

selected, the new tool selection signal is output.

Examples

D Tool change type A

Suppose that the tool life management cancel number is 100.

T101; A tool whose life has not expired is selected from group 1.

(Suppose that tool number 010 is selected.)

M06; Tool life counting is performed for the tool in group 1.

(The life of tool number 010 is counted.)

T102; A tool whose life has not expired is selected from group 2.

(Suppose that tool number 100 is selected.)

M06T101; Tool life counting is performed for the tool in group 2.

(The life of tool number 100 is counted.)

The number of the tool currently used (in group 1) is

output with a T code signal. (Tool number 010 is

output.)

118

10. TOOL FUNCTION

B-64124EN/01

PROGRAMMING

(T FUNCTION)

D Tool change type B

and C

Suppose that the tool life management ignore number is 100.

T101;

A tool whose life has not expired is selected from group 1.

(Suppose that tool number 010 is selected.)

M06T102;Tool life counting is performed for the tool in group 1.

(The life of tool number 010 is counted.)

A tool whose life has not expired is selected from group 2.

(Suppose that toolnumber 100 is selected.

M06T103;Tool life counting is lperformed for the tool in group 2.

(The life of tool number 100 is counted.)

A tool whose life has not expired is selected from group 3.

(Suppose that tool number 200 is selected.)

D Tool change type D

Suppose that the tool life management ignore number is 100.

T101M06;A tool whose life has not expired is selected from group 1.

(Suppose that tool number 010 is selected.)

Tool life counting is performed for the tool in group 1.

T102M06;A tool whose life has not expired is selected from group 2.

(Suppose that tool number 100 is selected.)

Tool life counting is performed for the tool in group 2.

(The life of tool number 100 is counted.)

119

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-64124EN/01

10.2.4

The life of a tool is specified by a usage frequency (count) or usage time

(in minutes).

Tool Life

Explanations

D Usage count

The usage count is incremented by 1 for each tool used in a program.

In other words, the usage count is incremented by 1 only when the first

tool group number and tool change command are specified after the

CNC unit enters the automatic operation state from the reset state.

CAUTION

Even if the same tool group number is specified more than

once in a program, the usage count is only incremented by

1 and no new tools are selected.

D Usage time

When a tool change is specified (M06), tool life management is started

for the tools specified by the tool group number. In tool life

management, the time during which a tool is used in the cutting mode

is counted in four second increments., If the tool group is changed

before the incremental time of four seconds elapses, the time is not

counted. The time a tool is used for single block stop, feed hold, rapid

traverse, dwell, machine lock, and interlock is not counted.

NOTE

When a tool is selected from available tools, tools are

searched starting from the current tool towards the lasttool

to find a tool whose life has not expired. When thelast tool

is reached during this search, the search restartsfrom the

first tool. When it has been determined that there are no

tools whose life has not expired, the last tool is selected.

When the tool currently being used is changed by tool skip

signal, the next new tool is selected using the method

described here.

When tool life is counted by time, the life counting can be

overridden using the tool life count override signal. An

override from 0 to 99.9 can be applied. When 0 is specified,

time is not counted. Before the override capability can be

used, bit 2 of parameter LFV No.6801 must be set.

When tool life counting indicates that the life of the last tool

in a group has expired, the tool change signal is output.

When tool life is managed by time, the signal is output when

the life of the last tool in the group has expired. When tool

life is managed by usage frequency (count), the signal is

output when the CNC unit is reset or the tool life count

restart M code is specified.

120

B-64124EN/01

PROGRAMMING

11. AUXILIARY FUNCTION

AUXILIARY FUNCTION

General

There are two types of auxiliary functions ; miscellaneous function (M

code) for specifying spindle start, spindle stop program end, and so on,

and secondary auxiliary function (B code) for specifying index table

positioning.

When a move command and miscellaneous 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 miscellaneous

function commands.

ii) Executing miscellaneous function commands upon completion of

move command execution.

The selection of either sequence depends on the machine tool builder’s

specification. Refer to the manual issued by the machine tool builder for

details.

121

11. AUXILIARY FUNCTION

PROGRAMMING

B-64124EN/01

11.1

When a numeral is specified following address M, code signal and a

strobe signal are sent to the machine. The machine uses these signals to

AUXILIARY

turn on or off its functions.

FUNCTION

Usually, only one M code can be specified in one block. In some cases,

(M FUNCTION)

however, up to three M codes can be specified for some types of machine

tools.

Which M code corresponds to which machine function is determined by

the machine tool builder.

The machine processes all operations specified by M codes except those

specified by M98, M99,M198 or called subprogram(Parameter No.6071

to 6079), or called custom macro (Parameter No.6080 to 6089). Refer to

the machine tool builder’s instruction manual for details.

Explanations

The following M codes have special meanings.

D M02,M03

This indicates the end of the main program

(End of program)

Automatic operation is stopped and the CNC unit is reset.

This differs with the machine tool builder.

After a block specifying the end of the program is executed,

control returns to the start of the program.

Bit 5 of parameter 3404 (M02) or bit 4 of parameter 3404 (M30) can be

used to disable M02, M30 from returning control to the start of the

program.

D M00

Automatic operation is stopped after a block containing M00 is executed.

(Program stop)

When the program is stopped, all existing modal information remains

unchanged. The automatic operation can be restarted by actuating the

cycle operation. This differs with the machine tool builder.

D M01

Similarly to M00, automatic operation is stopped after a block containing

(Optional stop)

M01 is executed. This code is only effective when the Optional Stop

switch on the machine operator’s panel has been pressed.

D M98

This code is used to call a subprogram. The code and strobe signals are

(Calling of sub-

not sent. See the subprogram II- 12.3 for details .

program)

D M99

This code indicates the end of a subprogram.

(End of subprogram)

M99 execution returns control to the main program. The code and strobe

signals are not sent. See the subprogram section 12.3 for details.

D M198 (Calling a

This code is used to call a subprogram of a file in the external input/output

subprogram)

function. See the description of the subprogram call function (III-4.6) for

details.

NOTE

The block following M00, M01, M02, or M30 is not pre-read

(buffered). Similarly, ten M codes which do not buffer can

be set by parameters (Nos. 3411 to 3420). Refer to the

machine tool builder’s instruction manual for these M codes.

122

B-64124EN/01

PROGRAMMING

11. AUXILIARY FUNCTION

In general, only one M code can be specified in a block. However, up to

11.2

three M codes can be specified at once in a block by setting bit 7 (M3B)

MULTIPLE M

of parameter No. 3404 to 1. Up to three M codes specified in a block are

COMMANDS

simultaneously output to the machine. This means that compared with

the conventional method of a single M command in a single block, a

IN A SINGLE BLOCK

shorter cycle time can be realized in machining.

Explanations

CNC allows up to three M codes to be specified in one block.

However, some M codes cannot be specified at the same time due to

mechanical operation restrictions. For detailed information about the

mechanical operation restrictions on simultaneous specification of

multiple M codes in one block, refer to the manual of each machine

tool builder.

M00, M01, M02, M30, M98, M99, or M198 must not be specified

together with another M code.

Some M codes other than M00, M01, M02, M30, M98, M99, and

M198 cannot be specified together with other M codes; each of those

M codes must be specified in a single block.

Such M codes include these which direct the CNC to perform internal

operations in addition to sending the M codes themselves to the

machine. To be specified, such M codes are M codes for calling

program numbers 9001 to 9009 and M codes for disabling advance

reading (buffering) of subsequent blocks. Meanwhile, multiple of M

codes that direct the CNC only to send the M codes themselves

(without performing internal operations ) can be specified in a single

block.

Examples

One M command

Multiple M commands

in a single block

M40 ;

M40M50M60 ;

M50 ;

G28G91X0Y0Z0 ;

M60 ;

G28G91X0Y0Z0 ;

123

11. AUXILIARY FUNCTION

PROGRAMMING

B-64124EN/01

When a value is specified after address B, the code signal and strobe signal

11.3

are output. The code is retained until a B code is specified next.

THE SECOND

The functions are used for machine side operations such as indexing for

AUXILIARY

the rotation axis. Each block can contain only one B code. Setting

parameter No. 3460 enables the use of one of addresses A, C, V, and W,

FUNCTIONS

instead of address B. However, this address must be different from that

(B CODES)

for the controlled axis. For details, refer to the manual issued by the

machine tool builder.

Explanations

D Valid data range

0 to 99999999

D Specification

1. To enable the use of a decimal point, set bit 0 (AUP) of parameter

No.3450 to 1.

Command Output value

B10.

10000

B10

2. Use bit 0 (DPI) of parameter No. 3401 to specify whether the

magnification for B output will be

1000 or

1 when a decimal

point is omitted.

Command Output value

DPI=1

1000

DPI=0

3. Use bit 0 (AUX) of parameter No. 3405 to specify whether the

magnification for B output will be

1000 or

10000 when a

decimal point is omitted for the inch Input system

(only when DPI=1).

Command Output value

AUX=1

10000

AUX=0

1000

Restrictions

The address (B or the address specified with parameter No. 3460) used

with the second auxiliary functions cannot be used for the controlled axis

name (parameter No. 1020).

124

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

PROGRAM CONFIGURATION

General

D Main program and

There are two program types, main program and subprogram. Normally,

subprogram

the CNC operates according to the main program. However, when a

command calling a subprogram is encountered in the main program,

control is passed to the subprogram. When a command specifying a

return to the main program is encountered in a subprogram, control is

returned to the main program.

Main program

Subprogram

Instruction 1

Instruction 1Ȁ

Instruction 2

Instruction 2Ȁ

Follow the direction of the

subprogram

Instruction n

Instruction n+1

Return to the main program

Fig. 12 (a) Main program and subprogram

The CNC memory can hold up to 400 main programs and subprograms.

A main program can be selected from the stored main programs to operate

the machine. See III-9.3 or III-10 in OPERATION for the methods of

registering and selecting programs.

125

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

D Program components

A program consists of the following components:

Table 12 Program components

Components

Descriptions

Tape start

Symbol indicating the start of a program file

Leader section

Used for the title of a program file, etc.

Program start

Symbol indicating the start of a program

Program section

Commands for machining

Comment section

Comments or directions for the operator

Tape end

Symbol indicating the end of a program file

Leader section

Tape start

% TITLE

;

Program start

O0001 ;

(COMMENT)

Program section

Comment section

M30 ;

Tape end

Fig. 12 (b) Program configuration

D Program section

A program section consists of several blocks. A program section starts

configuration

with a program number and ends with a program end code.

Program section

configuration

Program number

O0001 ;

Block 1

N1 G91 G00 X120.0 Y80.0 ;

Block 2

N2 G43 Z-32.0 H01 ;

Block n

Nn Z0 ;

Program end

M30 ;

A block contains information necessary for machining, such as a move

command or coolant on/off command.Specifying a slash (/) at the start

of a block disables the execution of some blocks (see “optional block

skip” in II-12.2).

126

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

This section describes program components other than program sections.

12.1

See II-12.2 for a program section.

PROGRAM

COMPONENTS

Leader section

OTHER THAN

Tape start

% TITLE

;

Program start

PROGRAM

O0001 ;

SECTIONS

(COMMENT)

Comment section

Program section

M30 ;

Tape end

Fig. 12.1 (a) Program configuration

Explanations

D Tape start

The tape start indicates the start of a file that contains NC programs.

The mark is not required when programs are entered using SYSTEM P

or ordinary personal computers. The mark is not displayed on the screen.

However, if the file is output,the mark is automatically output at the start

of the file.

Table 12.1 (a) Code of a tape start

Name

ISO

EIA

Notation in this manual

code

Tape start

D Leader section

Data entered before the programs in a file constitutes a leader section.

When machining is started, the label skip state is usually set by turning

on the power or resetting the system. In the label skip state, all

information is ignored until the first end-of-block code is read. When a

file is read into the CNC unit from an I/O device, leader sections are

skipped by the label skip function.

A leader section generally contains information such as a file header.

When a leader section is skipped, even a TV parity check is not made. So

a leader section can contain any codes except the EOB code.

D Program start

The program start code is to be entered immediately after a leader section,

that is, immediately before a program section.

This code indicates the start of a program, and is always required to

disable the label skip function.

With SYSTEM P or ordinary personal computers, this code can be entered

by pressing the return key.

Table 12.1 (b) Code of a program start

Name

ISO

EIA

Notation in this manual

code

Program start

;

127

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

NOTE

If one file contains multiple programs, the EOB code for

label skip operation must not appear before a second or

subsequent program number.

D Comment section

Any information enclosed by the control-out and control-in codes is

regarded as a comment.

The user can enter a header, comments, directions to the operator, etc. in

a comment section.

Table 12.1 (c) Codes of a control-in and a control-out

Name

ISO

EIA

Notation in this

Meaning

code

manual

Control-out

(

2-4-5

(

Start of comment section

Control-in

)

2-4-7

)

End of comment section

When a program is read into memory for memory operation, comment

sections, if any, are not ignored but are also read into memory. Note,

however, that codes other than those listed in the code table in Appendix

A are ignored, and thus are not read into memory.

When data in memory is output on external I/O device(See III-8), the

comment sections are also output.

When a program is displayed on the screen, its comment sections are also

displayed. However, those codes that were ignored when read into

memory are not output or displayed.

During memory operation or DNC operation, all comment sections are

ignored.

The TV check function can be used for a comment section by setting

parameter CTV (bit 1 of No. 0100).

CAUTION

If a long comment section appears in the middle of a

program section, a move along an axis may be suspended

for a long time because of such a comment section. So a

comment section should be placed where movement

suspension may occur or no movement is involved.

NOTE

If only a control-in code is read with no matching

control-out code, the read control-in code is ignored.

The EOB code cannot be used in a comment.

128

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

D Tape end

A tape end is to be placed at the end of a file containing NC programs.

If programs are entered using the automatic programming system, the

mark need not be entered.

The mark is not displayed on the screen. However, when a file is output,

the mark is automatically output at the end of the file.

If an attempt is made to execute % when M02 or M03 is not placed at the

end of the program, the P/S alarm (No. 5010) is occurred.

Table 12.1 (d) Code of a tape end

Name

ISO

EIA

Notation in this

code

manual

Tape end

129

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

This section describes elements of a program section. See II-12.1 for

12.2

program components other than program sections.

PROGRAM SECTION

CONFIGURATION

% TITLE;

Program number

O0001 ;

N1 … ;

Sequence number

(COMMENT)

Comment section

Program section

Program end

M30 ;

Fig. 12.2 (a) Program configuration

D Program number

A program number consisting of address O followed by a four-digit

number is assigned to each program at the beginning registered in

memory to identify the program.

In ISO code, the colon ( : ) can be used instead of O.

When no program number is specified at the start of a program, the

sequence number (N

) at the start of the program is regarded as its

program number. If a five-digit sequence number is used, the lower four

digits are registered as a program number. If the lower four digits are all

0, the program number registered immediately before added to 1 is

registered as a program number. Note, however, that N0 cannot be used

for a program number.

If there is no program number or sequence number at the start of a

program, a program number must be specified using the MDI panel when

the program is stored in memory (See III-8.4 or III-10.1)

NOTE

Program numbers 8000 to 9999 may be used by machine

tool builders, and the user may not be able to use these

numbers.

130

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

D Sequence number and

A program consists of several commands. One command unit is called a

block

block. One block is separated from another with an EOB of end of block

code.

Table 12.2 (a) EOB code

Name

ISO

EIA

Notation in this

code

manual

End of block (EOB)

;

At the head of a block, a sequence number consisting of address N

followed by a number not longer than five digits (1 to 99999) can be

placed. Sequence numbers can be specified in a random order, and any

numbers can be skipped. Sequence numbers may be specified for all

blocks or only for desired blocks of the program. In general, however, it

is convenient to assign sequence numbers in ascending order in phase

with the machining steps (for example, when a new tool is used by tool

replacement, and machining proceeds to a new surface with table

indexing.)

N300 X200.0 Z300.0 ; A sequence number is underlined.

Fig. 12.2 (b) Sequence number and block (example)

NOTE

N0 must not be used for the reason of file compatibility with

other CNC systems.

Program number 0 cannot be used. So 0 must not be used

for a sequence number regarded as a program number.

D TV check (Vertical parity

A parity check is made for a block on input tape vertically. If the number

check along tape)

of characters in one block (starting with the code immediately after an

EOB and ending with the next EOB) is odd, an P/S alarm (No.002) is

output. No TV check is made only for those parts that are skipped by the

label skip function. Bit 1 (CTV) of parameter No. 0100 is used to specify

whether comments enclosed in parentheses are counted as characters

during TV check. The TV check function can be enabled or disabled by

setting on the MDI unit (See III-11.4.3.).

131

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

D Block configuration

A block consists of one or more words. A word consists of an address

(word and address)

followed by a number some digits long. (The plus sign (+) or minus sign

(-) may be prefixed to a number.)

Word = Address + number (Example : X-1000)

For an address, one of the letters (A to Z) is used ; an address defines the

meaning of a number that follows the address. Table 12.2 (b) indicates

the usable addresses and their meanings.

The same address may have different meanings, depending on the

preparatory function specification.

Table 12.2 (b) Major functions and addresses

Function

Address

Meaning

Program number

O (1)

Program number

Sequence number

Preparatory function

Specifies a motion mode (linear, arc,

etc.)

Dimension word

X, Y, Z, U,

Coordinate axis move command

V, W, A, B,

I, J, K

Coordinate of the arc center

Arc radius

Feed function

Rate of feed per minute,

Rate of feed per revolution

Spindle speed function

Spindle speed

Tool function

Tool number

Auxiliary function

On/off control on the machine tool

Table indexing, etc.

Offset number

D, H

Offset number

Dwell

P, X

Dwell time

Program number

Subprogram number

designation

Number of

Number of subprogram repetitions

repetitions

Parameter

P, Q

Canned cycle parameter

NOTE

In ISO code, the colon ( : ) can also be used as the address

of a program number.

X_ Y_

;

Spindle

Sequence Preparatory

Dimension Feed-

Tool

Miscellaneous

speed

number

function

word

function

Fig. 12.2 (c) 1 block (example)

132

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 5