FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL

1. GENERAL

PROGRAMMING

B-63524EN/01

The tool moves along straight lines and arcs constituting the workpiece

1.1

parts figure (See II-4).

TOOL MOVEMENT

ALONG WORKPIECE

PARTS FIGURE-

INTERPOLATION

Explanations

D Tool movement along a

straight line

Tool

Program

G01 Z...;

Workpiece

Fig.1.1 (a) Tool movement along the straight line which is parallel to Z-axis

Program

Tool

G01 X ... Z... ;

Workpiece

Fig.1.1 (b) Tool movement along the taper line

D Tool movement along an

arc

Tool

Program

G02X ... Z ... R ... ;

G03X ... Z ... R ... ;

Workpiece

Fig. 1.1 (c) Tool movement along an arc

B-63524EN/01

PROGRAMMING

1. GENERAL

The term interpolation refers to an operation in which the tool moves

along a straight line or arc in the way described above.

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 Z__;

G03X--Z--;

X--Z----;

Control unit

X axis

Tool

Interpolation

movement

Y axis

a) Movement

along straight

line

b) Movement

along arc

Fig. 1.1 (d) Interpolation function

NOTE

Some machines move tables instead of tools but this

manual assumes that tools are moved against workpieces.

D Thread cutting

Threads can be cut by moving the tool in synchronization with spindle

rotation. In a program, specify the thread cutting function by G32.

Tool

Program

G32Z--F--;

Workpiece

Fig. 1.1 (e) Straight thread cutting

B-63524EN/01

PROGRAMMING

1. GENERAL

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

1.2

the feed.

FEED-

FEED FUNCTION

Chuck

Tool

Workpiece

Fig. 1.2 (a) Feed function

Feedrates can be specified by using actual numerics.

For example, the following command can be used to feed the tool 2 mm

while the workpiece makes one turn :

F2.0

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

II-5).

1. GENERAL

PROGRAMMING

B-63524EN/01

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)

Tool post

Chuck

Reference

position

Fig. 1.3.1 (a) 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.

B-63524EN/01

PROGRAMMING

1. GENERAL

1.3.2

Coordinate System on

Part Drawing and

Coordinate System

Specified by CNC -

Program

Coordinate System

Coordinate system

Part drawing

CNC

Command

Workpiece

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)

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.

Coordinate system specified by the CNC

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

230

Present tool position

300

Distance to the zero point of a coor-

Program

dinate system to be set

zero point

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

1. GENERAL

PROGRAMMING

B-63524EN/01

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

The following method is usually used to define two coordinate systems

two coordinate systems

at the same location.

in the same position

1. When coordinate zero point is set at chuck face

Workpiece

150

Fig. 1.3.2 (c) Coordinates and dimensions on part drawing

Workpiece

Fig. 1.3.2 (d) Coordinate system on lathe as specified by CNC

(made to coincide with the coordinate system on part drawing)

1. GENERAL

PROGRAMMING

B-63524EN/01

1.3.3

How to Indicate

Command Dimensions

for Moving the Tool -

Absolute, Incremental

Commands

Explanations

Methods of command for moving the tool can be indicated by absolute

or incremental designation (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.

Tool

Workpiece

φ30

110

Command specifying movement from point A to point B

G90X30.0Z70.0;

Coordinates of point B

Fig. 1.3.3 (a) Absolute command

B-63524EN/01

PROGRAMMING

1. GENERAL

D Incremental command

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

position.

Tool

φ60

φ30

Command specifying movement from point A to point B

U-30.0W-40.0

Distance and direction for

movement along each axis

Fig. 1.3.3 (b) Incremental command

D Diameter programming /

Dimensions of the X axis can be set in diameter or in radius. Diameter

radius programming

programming or radius programming is employed independently in each

machine.

1. Diameter programming

In diameter programming, specify the diameter value indicated on the

drawing as the value of the X axis.

Workpiece

φ40

φ30

Coordinate values of points A and B

A(30.0, 80.0), B(40.0, 60.0)

Fig. 1.3.3 (c) Diameter programming

B-63524EN/01

PROGRAMMING

1. GENERAL

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

1.4

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

V: Cutting speed

v m/min

φD

N min^-1

Workpiece

Fig. 1.4 Cutting speed

Examples

<When a workpiece 200 mm in diameter should be machined at

a cutting speed of 300 m/min. >

The spindle speed is approximately 478 min^-1, which is obtained from

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

S478 ;

Commands related to the spindle speed are called the spindle speed

function (See II-9).

The cutting speed v (m/min) can also be specified directly by the speed

value. Even when the workpiece diameter is changed, the CNC changes

the spindle speed so that the cutting speed remains constant.

This function is called the constant surface speed control function

(See II-9.3).

1. GENERAL

PROGRAMMING

B-63524EN/01

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

1.5

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

SELECTION OF

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

TOOL USED FOR

selected.

VARIOUS

MACHINING - TOOL

FUNCTION

Tool number

Tool post

Fig. 1.5 Tool used for various machining

Examples

When the tool is stored at location 01 of the tool post, the tool can be

selected by specifying T0101.

This is called the tool function (See II-10).

B-63524EN/01

PROGRAMMING

1. GENERAL

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

1.6

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

COMMAND FOR

coolant valve should be controlled (See II-11).

MACHINE

OPERATIONS -

Coolant on/off

MISCELLANEOUS

FUNCTION

Chuck open/close

CW spindle rotation

Workpiece

Fig. 1.6 Command for machine operations

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.

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

the specified spindle speed.

1. GENERAL

PROGRAMMING

B-63524EN/01

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

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).

B-63524EN/01

PROGRAMMING

1. GENERAL

Explanations

The block and the program have the following configurations.

D Block

1 block

N fffff G ff Xff.f Zfff.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 begins with a sequence number that identifies that 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

⋅

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.

1. GENERAL

PROGRAMMING

B-63524EN/01

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

⋅

hole #2

⋅

M99

B-63524EN/01

PROGRAMMING

1. GENERAL

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-15.1)

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.

Rough

Thread

Standard

Finishing Grooving

cutting

tool

Workpiece

Fig. 1.8 Tool offset

1. GENERAL

PROGRAMMING

B-63524EN/01

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. Besides the stroke limits, data in memory can

RANGE - STROKE

be used to define an area which tools cannot enter.

Table

Motor

Limit switch

Machine zero point

Specify these distances.

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).

2. CONTROLLED AXES

PROGRAMMING

B-63524EN/01

2.1

CONTROLLED AXES

Series 16i

Series 160i

16i-TB

16i-TB, 160i-TB

Item

160i-TB

(two-path control)

Number of basic

2 axes

2 axes for each tool post

controlled axes

(4 axes in total)

Controlled axis expansion

Max. 8 axes

Max. 8 axes for each tool

(total)

(Included in Cs axis)

post (Included in Cs axis)

(Note)

Number of basic simulta-

2 axes

2 axes for each tool post

neously controlled axes

(4 axes in total)

Simultaneously controlled

Max. 6 axes

Max. 6 axes for each tool

axis expansion (total)

post

The table above lists the number of controlled axes of one-path control

and two-CPU two-path control. For the number of controlled axes of

one-CPU two-path control and two-CPU three-path control, refer to the

specifications.

NOTE

A two-path control system with the 7.2″/8.4″ LCD has up to

eight controlled axes.

The number of simultaneously controllable axes for manual

operation (jog feed, incremental feed, or manual handle

feed) is 1 or 3 (1 when bit 0 (JAX) of parameter 1002 is set

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

Series 18i

Series 180i

18i-TB

18i-TB, 180i-TB

Item

180i-TB

(two-path control)

Number of basic

2 axes

2 axes for each tool post

controlled axes

(4 axes in total)

Controlled axis expansion

Max. 6 axes

Max. 6 axes for each tool

(total)

(Included in Cs axis)

post (Included in Cs axis)

(Note)

Number of basic simulta-

2 axes

2 axes for each tool post

neously controlled axes

(4 axes in total)

Simultaneously controlled

Max. 4 axes

Max. 4 axes for each tool

axis expansion (total)

post

The table above lists the number of controlled axes of one-path control

and two-CPU two-path control.

For the number of controlled axes of one-CPU two-path control, refer to

the specifications.

2. CONTROLLED AXES

PROGRAMMING

B-63524EN/01

The names of two basic axes are always X and Z; the names of additional

2.2

axes can be optionally selected from A, B, C, U, V, W, and Y by using

NAMES OF AXES

parameter No.1020.

Each axis name is determined according to parameter No. 1020. If the

parameter specifies 0 or anything other than the nine letters, the axis name

defaults to a number from 1 to 8.

With two-path control, the names of two basic axes for one tool post are

always X and Z; the names of additional axes can be optionally selected

from A, B, C, U, V, W, and Y by using parameter No. 1020. For one tool

post, the same axis name cannot be assigned to multiple axes, but the same

axis name can be used with the other tool post.

Limitations

D Default axis name

When a default axis name (1 to 8) is used, the system cannot operate in

MEM, MDI, or RMT mode.

D Duplicate axis name

If the parameter specifies an axis name more than once, only the first axis

to be assigned that axis name becomes operable.

NOTE

When G code system A is used, the letters U, V, and W

cannot be used as an axis name (hence, the maximum of

six controlled axes), because these letters are used as

incremental commands for X, Y, and Z. To use the letters

U, V, and W as axis names, the G code system must be B

or C. Likewise, letter H is used as an incremental command

for C, thus incremental commands cannot be used if A or B

is used as an axis name.

With two-path control, when information

(such as the

current position) about each axis is displayed on the screen,

an axis name may be followed by a subscript to indicate a

tool post number (e.g., X1 and X2). This is axis name to help

the user to easily understand which tool post an axis

belongs to. When writing a program, the user must specify

X, Y, Z, U, V, W, A, B, and C without attaching a subscript.

In G76 (multiple-thread cutting), the A address in a block

specifies the tool nose angle instead of a command for axis

If C or A is used as an axis name, C or A cannot be used as

an angle command for a straight line in chamfering or direct

drawing dimension programming. Therefore, C and A

should be used according to bit 4 (CCR) of parameter No.

3405.

B-63524EN/01

PROGRAMMING

2. CONTROLLED AXES

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

2.3

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 degrees.

The increment system is classified into IS-B and IS-C (Tables 2.3 (a) and

2.3 (b)). Select IS-B or IS-C using bit 1 (ISC) of parameter 1004. When

the IS-C increment system is selected, it is applied to all axes and the 1/10

increment system option is required. The setting of parameter ISC (No.

1004#4) is valid for all axes. When IS-C is selected, for example, the

setting units for all axes are IS-C.

Table 2.3 (a) Increment system IS-B

Least input increment

Least command increment

Metric

0.001 mm (Diameter)

0.0005 mm

system

input

0.001 mm (Radius)

0.001 mm

machine

0.001 deg

inch

0.0001 inch (Diameter)

0.0005 inch

input

0.0001 inch (Radius)

0.001 inch

0.001 deg

Inch

0.001 mm (Diameter)

0.00005 mm

machine

input

0.001 mm (Radius)

0.0001 mm

system

0.001 deg

inch

0.0001 inch (Diameter)

0.00005 inch

input

0.0001 inch (Radius)

0.0001 inch

0.001 deg

Table 2.3 (b) Increment system IS-C

Least input increment

Least command increment

Metric

0.0001 mm (Diameter)

0.00005 mm

system

input

0.0001 mm (Radius)

0.0001 mm

machine

0.0001 deg

inch

0.00001 inch (Diameter)

0.00005 inch

input

0.00001 inch (Radius)

0.0001 inch

0.0001 deg

Inch

0.0001 mm (Diameter)

0.000005 mm

machine

input

0.0001 mm (Radius)

0.00001 mm

system

0.0001 deg

inch

0.00001 inch (Diameter)

0.000005 inch

input

0.00001 inch (Radius)

0.00001 inch

0.0001 deg

2. CONTROLLED AXES

PROGRAMMING

B-63524EN/01

The maximum stroke controlled by this CNC is shown in the table below:

2.4

Maximum stroke+Least command increment

99999999.

MAXIMUM STROKES

Table 2.4 Maximum strokes

Increment system

Maximum strokes

Metric machine

"99999.999 mm

system

"99999.999 deg

IS-B

Inch machine

"9999.9999 inch

system

"99999.999 deg

Metric machine

"9999.9999 mm

system

"9999.9999 deg

IS-C

Inch machine

"999.99999 inch

system

"9999.9999 deg

NOTE

The unit in the table 2.4 is a diameter value with diameter

programming and a radius value in radius programming.

A command exceeding the maximum stroke cannot be

specified.

The actual stroke depends on the machine tool.

3. PREPARATORY FUNCTION

B-63524EN/01

PROGRAMMING

(G FUNCTION)

PREPARATORY FUNCTION (G FUNCTION)

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.

G01X_;

Z_;

G01 is effective in this range

X_;

G00Z_;

There are three G code systems : A,B, and C (Table 3). Select a G code

system using bits 6 (GSB) and 7 (GSC) of parameter 3401. To use G code

system B or C, the corresponding option is needed. Generally, this

manual describes the use of G code system A, except when the described

item can use only G code system B or C. ln such cases, the use of G code

system B or C is described.

3. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-63524EN/01

Explanations

If the CNC enters the clear state (see bit 6 (CLR) of parameter 3402)

when the power is turned on or the CNC is reset, the modal G codes

change as follows.

(1) G codes marked with

in Table 3 are enabled.

(2) When the system is cleared due to power-on or reset, whichever

specified, either G20 or G21, remains effective.

(3) Bit 7 of parameter No. 3402 can be used to specify whether G22

or G23 is selected upon power-on. Resetting the CNC to the clear

state does not affect the selection of G22 or G23.

(4) Setting bit 0 (G01) of parameter 3402 determines which code,

either G00 or G01, is effective.

(5) When G code system B or C is used, setting bit 3 (G91) of

parameter 3402 determines which code, either G90 or G91, is

effective.

G codes of group 00 except G10 and G11 are single-shot G codes.

P/S larm (No.010) is displayed when a G code not listed in the G code

list is specified or a G code without a corresponding option is

specified.

G codes of different groups can be specified in the same block.

If G codes of the same group are specified in the same block, the G

code specified last is valid.

If a G code of group 01 is specified in a canned cycle, the canned cycle

is canceled in the same way as when a G80 command is specified. G

codes of group 01 are not affected by G codes for specifying a canned

cycle.

When G code system A is used, absolute or incremental programming

is specified not by a G code (G90/G91) but by an address word (X/U,

Z/W, C/H, Y/V). When G code system A is used for a drilling cycle,

only the initial level is provided at the return point.

G codes are displayed for each group number.

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 2