Content      ..      1      2      3      ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 2

1. GENERAL

GENERAL

B-63534EN/02

Related manuals of

The following table lists the manuals related to SERVO MOTOR a series

SERVO MOTOR a series

Specification

Manual name

number

FANUC AC SERVO MOTOR a seriesDESCRIPTIONS

B-65142

FANUC AC SERVO MOTOR a series

B-65150

PARAMETER MANUAL

FANUC AC SPINDLE MOTOR a seriesDESCRIPTIONS

B-65152

FANUC AC SPINDLE MOTOR α series

B-65160

PARAMETER MANUAL

FANUC SERVO AMPLIFIER a seriesDESCRIPTIONS

B-65162

FANUC SERVO MOTOR a series

B-65165

MAINTENANCE MANUAL

Either of the following servo motors and the corresponding spindle can

be connected to the CNC covered in this manual.

D FANUC SERVO MOTOR ai series

D FANUC SERVO MOTOR a series

This manual mainly assumes that the FANUC SERVO MOTOR i series

of servo motor is used. For servo motor and spindle information, refer to

the manuals for the servo motor and spindle that are actually connected.

6

GENERAL

1. GENERAL

B-63534EN/02

1.1

When machining the part using the CNC machine tool, first prepare the

program, then operate the CNC machine by using the program.

GENERAL FLOW OF

1) First, prepare the program from a part drawing to operate the CNC

OPERATION OF CNC

machine tool.

MACHINE TOOL

How to prepare the program is described in the Chapter II.

PROGRAMMING.

2) The program is to be read into the CNC system. Then, mount the

workpieces and tools on the machine, and operate the tools according

to the programming. Finally, execute the machining actually.

How to operate the CNC system is described in the Chapter III.

OPERATION.

Part

Part

drawing

programming

CNC

MACHINE TOOL

CHAPTER II PROGRAMMING

CHAPTER III OPERATION

Before the actual programming, make the machining plan for how to

machine the part.

Machining plan

1. Determination of workpieces machining range

2. Method of mounting workpieces on the machine tool

3. Machining sequence in every machining process

4. Machining tools and machining

Decide the machining method in every machining process.

Machining process

1

2

3

Hole

Face cutting

Side cutting

Machining procedure

machining

1. Machining method

: Rough

Semi

Finish

2. Machining tools

3. Machining conditions

: Feedrate

Cutting depth

4. Tool path

7

1. GENERAL

GENERAL

B-63534EN/02

Tool

Side cutting

Face cutting

Hole machining

Prepare the program of the tool path and machining condition

according to the workpiece figure, for each machining.

8

GENERAL

1. GENERAL

B-63534EN/02

1.2

NOTES ON READING

CAUTION

THIS MANUAL

1

The function of an CNC machine tool system depends not

only on the CNC, but on the combination of the machine

tool, its magnetic cabinet, the servo system, the CNC, the

operator ’s panels, etc. It is too difficult to describe the

function, programming, and operation relating to all

combinations. This manual generally describes these from

the stand-point of the CNC. So, for details on a particular

CNC machine tool, refer to the manual issued by the

machine tool builder, which should take precedence over

this manual.

2

Headings are placed in the left margin so that the reader can

easily access necessary information. When locating the

necessary information, the reader can save time by

searching though these headings.

3

This manual describes as many reasonable variations in

equipment usage as possible. It cannot address every

combination of features, options and commands that

should not be attempted.

If a particular combination of operations is not described, it

should not be attempted.

1.3

NOTES ON VARIOUS

CAUTION

KINDS OF DATA

Machining programs, parameters, variables, etc. are stored

in the CNC unit internal non-volatile memory. In general,

these contents are not lost by the switching ON/OFF of the

power. However, it is possible that a state can occur where

precious data stored in the non-volatile memory has to be

deleted, because of deletions from a maloperation, or by a

failure restoration. In order to restore rapidly when this kind

of mishap occurs, it is recommended that you create a copy

of the various kinds of data beforehand.

9

1. GENERAL

PROGRAMMING

B-63534EN/02

1.1

The tool moves along straight lines and arcs constituting the workpiece

parts figure (See II-4).

TOOL MOVEMENT

ALONG WORKPIECE

PARTS FIGURE-

INTERPOLATION

Explanations

The function of moving the tool along straight lines and arcs is called the

interpolation.

D Tool movement along a

straight line

Tool

Program

G01 X_ _ Y_ _ ;

X_ _ ;

Workpiece

Fig. 1.1 (a) Tool movement along a straight line

D Tool movement along an

arc

Program

G03X_ _Y_ _R_ _;

Tool

Workpiece

Fig. 1.1 (b) Tool movement along an arc

14

PROGRAMMING

1. GENERAL

B-63534EN/02

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.

15

1. GENERAL

PROGRAMMING

B-63534EN/02

1.2

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

the feed.

FEED-FEED

FUNCTION

mm/min

Tool

F

Workpiece

Table

Fig. 1.2 (a) 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).

16

PROGRAMMING

1. GENERAL

B-63534EN/02

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 (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.

17

1. GENERAL

PROGRAMMING

B-63534EN/02

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

18

PROGRAMMING

1. GENERAL

B-63534EN/02

The positional relation between these two coordinate systems is

determined when a workpiece is set on the table.

Coordinate system on

part drawing estab-

lished on the work-

Coordinate system spe-

piece

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.

19

1. GENERAL

PROGRAMMING

B-63534EN/02

(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)).

20

PROGRAMMING

1. GENERAL

B-63534EN/02

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

21

1. GENERAL

PROGRAMMING

B-63534EN/02

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 rpm 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 rpm, 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) .

22

PROGRAMMING

1. GENERAL

B-63534EN/02

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).

23

1. GENERAL

PROGRAMMING

B-63534EN/02

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.

24

PROGRAMMING

1. GENERAL

B-63534EN/02

1.7

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

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).

25

1. GENERAL

PROGRAMMING

B-63534EN/02

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).

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.

26

PROGRAMMING

1. GENERAL

B-63534EN/02

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

27

1. GENERAL

PROGRAMMING

B-63534EN/02

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.

28

PROGRAMMING

1. GENERAL

B-63534EN/02

1.9

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

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).

29

B-63534EN/02

PROGRAMMING

2. CONTROLLED AXES

2.1

CONTROLLED AXES

Series 16i, Series 160i,

16i-MB, 160i-MB,

16i-MB, 160i-MB,

Series 160is

Item

160is-MB

160is-MB

(two-path control)

No. of basic controlled

3 axes for each path

3 axes

axes

(6 axes in total)

Controlled axes

Max. 8 axes

Max. 8 axes for each path

expansion (total)

(included in Cs axis)

(included in Cs axis)

Basic simultaneously

2 axes for each path

2 axes

controlled axes

(4 axes in total)

Simultaneously controlled

Max. 6 axes

Max. 6 axes for each path

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).

Series 18i, Series 180i,

18i-MB5, 180i-MB5,

18i-MB, 180i-MB,

Item

Series 180is

180is-MB5

180is-MB

No. of basic controlled

3 axes

axes

Controlled axes expan-

Max. 6 axes (included in Cs axis)

sion (total)

Basic simultaneously

2 axes

controlled axes

Simultaneously controlled

Max. 5 axes

Max. 4 axes

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).

31

2. CONTROLLED AXES

PROGRAMMING

B-63534EN/02

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.

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

characters is specified, an axis name from 1 to 8 is assigned by default.

In two-path control, the basic three axis names are fixed to X, Y, and Z

for either path, but the name of an additional axis can be selected from A,

B, C, U, V, and W by parameter 1020. Duplicate axis names cannot be

used in the same path, but the same axis name can be used in different

paths.

Limitations

D Default axis name

When a default axis name (1 to 8) 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.

NOTE

In two-path control, axis information displayed on the CRT

screen, such as the current position, may contain an axis

name with a suffix indicating the related path (X1, X2, etc).

This is intended to provide a comprehensible indication of

the path to which the axis belongs. The suffix cannot be

used in a program ; the axis name should be specified as X,

Y, Z, U, V, W, A, B, or C.

32

B-63534EN/02

PROGRAMMING

2. CONTROLLED AXES

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.

The increment system is classified into IS-B and IS-C. 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.

Name of in-

Least input incre-

Least command

Maximum

crement sys-

ment

increment

stroke

tem

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.

33

2. CONTROLLED AXES

PROGRAMMING

B-63534EN/02

2.4

Maximum stroke = Least command increment

99999999

See 2.3 Incremen System.

MAXIMUM STROKE

Table 2.4 (a) 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.

34

3. PREPARATORY FUNCTION

B-63534EN/02

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 ;

35

3. PREPARATORY FUNCTION

B-63534EN/02

PROGRAMMING

(G FUNCTION)

G code list for M series (1/4)

G code

Group

Function

G00

Positioning

G01

Linear interpolation

G02

Circular interpolation/Helical interpolation CW

G03

01

Circular interpolation/Helical interpolation CCW

G02.2, G03.2

Involute interpolation

G02.3, G03.3

Exponential function interpolation

G02.4, G03.4

Three-dimensional circular interpolation

G04

Dwell, Exact stop

G05

High speed cycle machining

00

G05.1

AI contour/AI nano contour/Smooth interpolation

G05.4

HRV3 on/off

G06.2

01

NURBS interpolation

G07

Hypothetical axis interpolation

G07.1 (G107)

Cylindrical interpolation

G08

Advanced prevew control

G09

00

Exact stop

G10

Programmable data input

G10.6

Tool retract and return

G11

Programmable data input mode cancel

G12.1

Polar coordinate interpolation mode

21

G13.1

Polar coordinate interpolation cancel mode

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

G25

Spindle speed fluctuation detection off

24

G26

Spindle speed fluctuation detection on

37

3.

PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-63534EN/02

G code list for M series (2/4)

G code

Group

Function

G27

Reference position return check

G28

Automatic return to reference position

G29

Automatic return from reference position

G30

2nd, 3rd and 4th reference position return

00

G30.1

Floating reference point return

G31

Skip function

G31.8

EGB skip function

G31.9

Continuous high-speed skip function

G33

01

Thread cutting

G37

Automatic tool length measurment

00

G39

Corner offset circular interpolation

G40

Cutter compensation cancel/three-dimensional tool compensation cancel

G41

Cutter compensation left/three-dimensional tool compensation

G41.2

Three-dimensional cutter compensation (Tool side compensation) left side

07

G41.3

Three-dimensional cutter compensation (Leading edge offset)

G42

Cutter compensation right

G42.2

Three-dimensional cutter compensation (Tool side compensation) right side

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

G49

08

Tool length compensation cancel

G50

Scaling cancel

11

G51

Scaling

G50.1

Programmable mirror image cancel

22

G51.1

Programmable mirror image

38

3. PREPARATORY FUNCTION

B-63534EN/02

PROGRAMMING

(G FUNCTION)

G code list for M series (3/4)

G code

Group

Function

G52

Local coordinate system setting

00

G53

Machine coordinate system selection

G54

Workpiece coordinate system 1 selection

14

G54.1

Additional workpiece coordinate system selection

G54.2

23

Rotary table dynamic fixture offset

G55

Workpiece coordinate system 2 selection

G56

Workpiece coordinate system 3 selection

G57

14

Workpiece coordinate system 4 selection

G58

Workpiece coordinate system 5 selection

G59

Workpiece coordinate system 6 selection

G60

00

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

G69

Coordinate rotation cancel/three-dimensional coordinate conversion cancel

G72.1

Rotation copy

00

G72.2

Linear copy

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)

39

Content      ..      1      2      3      ..