yaskawa J300L Programming Manual

Download

A A h

CNC SYSTEM FOR TURNING APPLICATIONS

YASNAC J300L

PROGRAMMING MANUAL

Upon receipt of the product and prior to initial operation, read these

instructions thoroughly, and retain for future reference.

REFERENCE

YASNAC J300L OPERATING MANUAL

TOE-C843-”1 3.20

YASUNNA MANUAL NO. TOE-C843-1 3.21

FOREWORD

This manual gives the information necessary for creating a program u;ing the YASNAC J300L (with basic NC operation panel, 9-inch CRT).

Some information is given in tables in the Appendix so that readers can easily find the necessary information. In the G code table, section numbers are given for each G code to allow quick access to a detailed explanation if necessary.

The YASNAC J300L comes with an operation manual in addition to this programming manual. Use these manuals in conjunction with each other to ensure prclductive operation.

CAUTIONS

This manual describes all the option functions (identified by the “*” symbol) but some of these may not be available with your YASNAC J300L. To determine the option functions installed in your NC, refer to the specification document or manuals published by the machine tool builder.

Unless otherwise specified, the following conditions apply in programming explanations and programming examples.

● Metric system for input and metric system for output/movement

●

: Zero point in the base coordinate system

●

: Reference point

Yaskawa has made every effort to describe individual functions and their relationships to other functions as accurately as possible. However, there are many things t;~at cannot or must not be performed and it is not possible to describe all of these. Accordingly, readers are requested to understand that unless it is specifically stated that something can be performed, it should be assumed that it cannot be performed.

Also bear in mind that the performance and functions of an NC machine tool are not determined solely by the NC unit. The entire control system consists of the mechanical system, the machine operation panel and other machine related equipment in addition to the NC. Therefore, read the manuals published by the machine tool builder for detailed information relating to the machine.

General Precautions

● Some drawings in this manual are shown with the protective cover or shields removed,

in order to describe the detail with more clarity. Make sure all covers and shields are replaced before operating this product, and operate it in accordance with the directions in the manual.

● The figures and photographs in this manua Ishow arepresentative product for reference

purposes and may differ from the product actually delivered to you.

● This manual maybe modified when necessary because of improvement of the product,

modification, or changes in specifications. Such modification is made as arevision by renewing the manual No.

● To order a copy of this manual, if your copy has been damaged or lost, contact your

Yaskawa representative listed on the last page stating the manual No. on the front page.

● If any of the nameplates affixed to the product become damaged or illegible, please

send these nameplates to your Yaskawa :representative.

● Yaskawa is not responsible for any modification of the product made by the user since

that will void our guarantee.

NOTES FOR SAFE OPERATION

Read this programming manual thoroughly before installation, operatiorl , maintenance or inspection of the YASNAC J300L.

The functions and performance as NC machine tool are not determined oily by an NC unit itself. Before the operation, read thoroughly the machine tool builder’s documents relating to the machine tool concerned.

In this manual, the NOTES FOR SAFE OPERATION are classified as “WARNING” “CAUTION’.

Indicates a potentially hazardous situa;ion which, if

~ WARNING

m!mi!l

Even items described inl ~ In either case, follow these important items.

Please note that symbol mark used to indicate caution differs between 1S0 and JIS.

not avoided, could result in death or serious injury to personnel. Symbol uct.

Indicates a potentially hazardous situa;ion which, if not avoided, may result in minor or mo,ierate injury to perscmnel and damage to equipment. It may also be used to alert against unsafe practice.

is used in labels attached to the prod-

CAUTION I may result in a vital accident insome situations.

In this manual, symbol mark stipulated by 1S0 is usecl.

On products, caution symbol marks of 1S0 and JIS are used in labels. Please follow the same safety instructions concerning caution.

Ill

KEY TO WARNING LABELS

The following warning labels are used with the YASNAC J300L.

Electric shock hazard Do not touch the terminals while the power is on, and for 5 minutes after switching off the power supply!

Location of label

NC unit

— Warning label

——

.—.

— .-

Grounding wires must be conr ected to the unit’s grounding terminals.

Use proper grounding techniques.

ILJI

Location of label

I ~ WARNING I “

Location of label

NC operation panel with 9 inch CRT

~~——

Rear face

Warning Iab[?l

FOREWORD . . . . .. .. . .. .. . .. .. . . . .. . . . .. . .. . . . .. . . . .. . .. . .

NOTES FOR SAFE OPERATION . . . . . . . . . . . . . . . . . . . . . . . . . . . .

KEY TO WARNING LABELS . . . . . .. . . . .. . . . .. . .. .. . .. . . . .. . .

1. PROGRAMMING BASICS

1.1 FUNDAMENTALS OF PROGRAMMING TERMINOLOGY . ...1-2

1,141

1.1.2 Least lnputlncrement and Least Output Increment . . . . . . . . . . . . . . . . . 1-3

1.1,3 Maximum Programmable Values for Axis Movement........,.. . . . . . 1-5

1.1.4 Tape Format . . . . . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-6

1.1,5 Program Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-9

1.1.6 OptionalBlockSkip(/1),(/2to/9) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-17

1.1,7 Buffer Register and Multi-active Register . . . . . . . . . . . . . . . . . . . . . . . . . 1-18

1.2 BASICS OF FEED FUNCTION . ., . . .. . . . .. . . . .. . . . . . . ...1-19

1.2.1

1.2.2 Cutting Feed (FCommand) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-20

1.2.3 Switching between Feed per Minute Modeand Feed per

1.2.4 Automatic Acceleratio nandDeceleration . . . . . . . . . . . . . . . . . . . . . . . . . 1-27

Numerically Controlled Axesandthe Number of Simultaneously

Controllable Axes . . .. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ,. 1-2

Rapid Traverse . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-19

Revolution Mode (G98/G99) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-26

!,,

Ill

2. COMMANDS CALLING AXIS MOVEMENTS

2.1 INTERPOLATION COMMANDS ..,... . . . . . . .. .. . .. . . . . ...2-3

2.1.1

2.1.2 Linear interpolation (GOl) . . . . . . . . . . . . . . . ., . . . . . . . . . . . . . . . . . . . ...2-5

2.1.3 Circular interpolation (G02, G03, G22, G23) . . . . . . . . . . . . . . . . . . . . . . . 2-9

2.1.4 Chamfering (Gil) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ,2-14

2,1.5 Rounding (G12) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ,2-16

2.1.6 Cylindrical interpolation (G124)G125) . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-18

2.1.7 Polar Coordinate interpolation (G126, G127)* . . . . . . . . . . . . . . . . . . . . 2-21

2.2 USING THE THREAD CUTTING FUNCTION . . . . . . . . . . . ...2-28

2.2.1 Thread Cutingand Continuous Thread Cutting (G32) . . . . . . . . . . . . . . 2-28

2.2.2

2.2.3 Variable Lead Thread Cutting (G34)* ,, ., . . . . . . . . . . . . . . . . . . . . . ...2-37

2.3 REFERENCE POINT RETURN . . . .. . ., . . . . .. .. . .. . . . . ...2-39

2.3.1

2.3.2 Reference Point Return Check (G27) . . . . . . . . . . . . . . . . . . . . . . . . . ...2-44

2.3.3 Return from Reference Point Return (G29) . . . . . . . . . . . . . . . . . . . . . . . 2-45

2.3.4 Second to Fourth Reference Point Return (G30)* . . . . . . . . . . . . . . . . . 2-49

Positioning (GOO,G06) . . . . . . . . . . . . . . . . . ,,, ,, ...,,,.,.........,.2-3

Multiple-thread Cuttirlg(G32)* . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...2 -34

Automatic Return to Fieference Point (G28) . . . . . . . . . . . . . . . . . . . . . . 2-39

3. MOVEMENT CONTROL COMMANDS

3.1 SETTING THE COORDINATESYSTEM . .. .. . .. . . . . . . .. ...3-3

3.1.1 Base”Coordinate System (G!jO) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-3

3.1.2 Workpiece Coordinate System (G50T, G51) * . . . . . . . . . . . . . . . . . . . . . . 3-7

3.2 DETERMINING THE COOFIDINATE VALUE

INPUT MODES . . . . .. . . . .. . . . . . .. . . . .. . . . . . . . . .. . . . ...3-16

3.2.1

3.2.2 Diametric and Radial Commands for X-=is . . . . . . . . . . . . . . . . . . . . . . 3-19

3.2.3 Inch/Metric Input Designation (G20, G21) . . . . . . . . . . . . . . . . . . . . . . . . 3-20

Absolute/lncremental Desigrlation . . . . . . . . . . . . . . . . . .1 . . . . . . . . . ...3-16

3.3 TIME-CONTROLLING COMMANDS . . . . . .. . . . .. . . ~~. .. ...3-22

3.3.1

Dwell (G04) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-22

3.4 TOOL OFFSET FUNCTIONS . . .. . . . . . . . . . . . . . .. . . ... ...3-23

3.4.1

3.4.2 Tool Position Offset . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-24

3.4.3 Nose ROffset Function (G4(l, G41/G42) . . . . . . . . . . . . . . . . . . . . . . . . . 3-29

Tool Offset Data Memory . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .. 3-23

3.5 SPINDLE FUNCTION (S FIJNCTION) . . . . . . . . . . . . . ... ...3-75

3.5.1

3.5.2 Maximum Spindle Speed Command (G50S) . . . . . . . . . . . . . . . . . . . . . 3-76

3.5.3 Constant Surface Speed Control (G96, G97)* . . . . . . . . . . . . . . . . . . . . 3-77

3.5.4 Rotary Tool Spindle Selection Function . . . . . . . . . . . . . . . . . . . . . . . . . . 3-81

Spindle Command (S5-digit Command) . . . . . . . . . . . . . . . . . . . . . . . . . . 3-75

3.6 TOOL FUNCTION (T FUNCTION) . . . . . . . . . . . . . . . . . . . ...3-82

3.6.1

3.6.2 T6-digit Command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-82

T4-digit Command . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-82

3.7 MISCELLANEOUS FUNCTION (M FUNCTION) . . . . c. . . ...3-83

3.7.1

3.7.2 internally Processed M Codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3- 84

3.7.3 General Purpose M Codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-85

. .—.——-—- ..— ..—.-—-----

MCodes Relating to Stop Operation (MOO, MOl, M02, M30) . . . . . . . . 3-83

vii

——— .- .._—-.—...—..-. -—-.-.... ..—— ..-.. - .—, -—-.. —.-..-,— . .. —.-—.——

4. ENHANCED LEVEL (COMMANDS

4.1 PROGRAM SUPPORT FUNCTIONS(l) ,.. .: .,............4-3

4.1.1

4.1.2 Multiple Repetitive Cycles (G70to G76)* . . . . . . . . . . . . . . . . . . . . . . . . 4-16

4.1.3 Multiple Chamfering/Rounding on Both Ends of Taper (Gill) * . . . . . . 4-56

4.1.4 Multiple Chamfering/Rounding on Arc Ends (G112) *. , . . . . . . . . . . . . . 4-70

4.1.5

4.2 PROGRAM SUPPORT FUNCTIONS

4.2.1

4.2.2 Programmable Data lnput(GIO) *.... . . . . . . . . . . . . . . . . . . . . . . . ...4-104

4.2.3 Subprogram Call Up Function (M98, M99) . . . . . . . . . . . . . . . . . . . . . . . 4-106

4.2.4 Stored Stroke Limit B(G36to G39) . . . . . . . . . . . . . . . . . . . . . . . . . ...4-108

Canned Cycles (G9Cl. G92. G94) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-3

Hole-machining Canned Cycles

(G80to G89, G831, G841, G861) . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...4-79

(2) , . . . . . . . . . . . . . . ...4-94

Solid Tap Function (G84, G841) *..... . . . . . . . . . . . . . . . . . . . . . . . . ..4-g4

4.3 AUTOMATING SUPPORT FUNCTIONS . . . . .. . . . . . . . . . . .4- 114

4,3.1

4.3.2 Tool Life Control Function (G122, G123) . . . . . . . . . . . . . . . . . . . . . . . . 4-117

4,4 MICROPROGRAMS . . .. .. . . . .. . .. . . . .. . .. .. . .. . . . .. . 4-126

4.4.1

4.4.2

4.4.3 Variables, . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...4 -138

4.4.4 Operation instructions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...4-162

4.4.5 Control instructions .,, ,,, . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...4-164

4,4,6 Registering the Microprogram . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...4 -170

4.4.7 RS-232C Data Output 2( BPRNT, DPRNT) . . . . . . . . . . . . . . . . . . . . . . 4-171

4.4.8 Microprogram Alarm Numbers,,,. , . . . . . . . . . . . . . . . . . . . . . . . . ...4-176

4.4.9 Examples of Microprograms, ,., ,, ., . . . . . . . . . . . . . . . . . . . . . . . ...4-177

Skip Function (G31) *.....,,.,...,.. . . . . . . . . . . . . . . . . . . . . . . ...4-114

Differences from Subprograms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4-126

Microprogram Call (G65, G66, G67)*. . . . . . . . . . . . . . . . . . . . . . . ...4-128

APPENDIX 1 G CODE TABLE

APPENDIX l.l GCODE TABLE . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Al-2

APPENDIX 2 INDEX

Vlll

PROGRAMMING BASICS

Chapter 1 describes the basic terms used in programming and

the feed functions.

1.1

FUNDAMEN”rALS OF PROGRAMMING

TERMINOLOGY. . . . . . . . . . . . . . . . . . . . .1-2

1.1,1

Numerically Controlled Axes and the Nulmber

of Simultaneously Controllable Axes . . . . . . . . 1 -2

1.1,2

1.1.3

1,1.4 1,1.5

1.1.6 Optional Block Skip (/1), (/2 to /9) * . . . . . . . . 1-17

1.1.7

1.2

BASICS OF I=EED FUNCTION . . . . . i .. 1-19

1.2.1

1.2.2 Cutting Feed (F Command) . . . . . . . . . . . . . . 1-20

1.2.3

1.2.4

Least Input Increment and Least Output

Increment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ‘1-3

Maximum Programmable Values for Axis

Movemen t . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-5

Tape Format . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-6

Program Format . . . . . . . . . . . . . . . . . . . . . . . . . 1-9

Buffer Register and Multi-active Registel’ . . . 1-18

Rapid Traverse . . . . . . . . . . . . . . . . . . . . . . . . . 1-19

Switching between Feed per Minute Mode and Feed per Revolution Mode (G98/G$19) . 1-26

Automatic Acceleration and Deceleration . . . 1-27

1.1

FUNDAMENTALS OF PROGRAMMING TERMINOLOGY

This section describes the basic terms used in programming.

1.1.1

Numerically Controlled Axes and the Number of Simultaneously Controllable Axes

The numerically controlled axes and the number of axes that can be controlled simultaneously are indicated in Table 1.1.

—.. . . . . .,-. .. . . ... . ,, , -. ,.

[able 1.1 Numerically Uontroilea Axes ana tne NumDer oT Slmul[aneously

Controllable Axes

Description

IBasic axes lXand Z

Controlled axes

Number of simttltaneousl y controllable axes

Note 1: For polar coordinate interpolation* and cylindrical interpolation

XCor ZCplane. For details, see 2.1.7,’’Polar Coordinate Interpolation” and 2.1.6, “Cylindrical Interpolation”.

2: With a manual pulse generator, only one axis control is possible.

Series 1 control

Positioning (GOO) All axes

Linear interpolation ((301) Circular interpolation (G02,

G03) Manual operation

Aclditional axis control A*

Additional axis control B*

}

Xand Z+C

Expandable to 5 axes (Y-axis, B-axis, etc.)

AUaxes

2 axes

All axes

*, circular interpolation is possible on virtual

—

1-2

..—.- —

1.1 FUNDAMENTALS OF PROGRAMMING TERMINOLOGY

1.1.2 Least Input Increment and Least Output Increment

The least input and output increments vary depending cmthe type of controlled axis whether it is a rotary axis or a linear axis.

(1)

LeastInput Incrementand10-tilmeInputIncrement

The least input increment to express axis movement distance that is input by using punched tape or manual data input switches is indicated in Table 1,2.

Table 1.2 Least Input Increment (pml 000 DO=O)

! i 2 i ? q

Metric Input

Inch Input

By setting “l” for parameter pm1000 DO (pm1000 DO = 1), the “lO-time input increment” specifications indicated in Table 1.3 is selected.

Table 1.3 10-time Input Increment (pml 000 DO= 1)

Metric Input

Inch Input

Note: Selection of “mm-input” and “inch-input” is made by the setting parameter pmOO07[IOorbythespecification

ofG20/G21

Disregarding of the least input increment mode which has been select ed, tool.offset data are always written in units of 0.001 mm (or 0.0001 inch, or 0.001 deg.). Offset movement is possible in the specified the following operations and the commands for them must be given in units c}f0.01 mm.

●

Data writing in the MDI mode

‘X-’:zzz:::: :3

‘X-’::z ~:G:-”-3

vake. If the offset data are set in units of 0.01 mm,

●

Programming for the memory mode operation

●

Program editing

1. If an NC program written in units of 0.001 mm is executed while the 0.01 mm setting increment is selected, dimension commands are.all executed 10 times the specified value.

2. If the program stored in memory is executed in the memory mode after changing the setting for pm1000 DO (input increment setting parameter), dimension commands in the stored program are executed in either 1/10 or 10 times the specified value.

3. When a program stored in memory is output to a tape, the stored program is output as it is and not influenced by the setting for pm1000 DO (input increment setting parameter).

Least Output Increment

(2)

The least output increment indicates the “minimum unit” of axis movement that is determined by the mechanical system. By selecting the option, it is possible to select the output unit system between “mm” and “inches”.

Table 1.4 Least Output Unit (pml 000 DO = 1)

Linear Axes

(X-, ‘f-, Z-axis, etc.)

Metric Output 0.001 mm 0.001 deg.

Inch Output

0.0001inch

* C-axis

0.001 deg.

..—.— ———

“l-4

1.1 FUNDAMEN”rALS OF PROGRAMMING TERMINOLOGY

1.1.3 Maximum Programmable Values for Axis Movement

The maximum programmable values that can be designated for a move command are indicated in Table 1.5. The maximum programmable values indicated in these tables are applica-

ble to addresses I, J, K, R, A, and B which are used for designating “distance” in addition

to the move command addresses X, Y, Z, C, U, W, V, and H.

Table 1.5 Maximum Programmable Values for Axis Movement

Linear Axes

(X-, Y-, Z-axis, etc.)

Metric Output

Metric Input

Inch Input

Metric Input

Inch Output

Inch Input

+ 999999.999mm + 999999.999 deg.

+ 39370.0787inch t 999999.999 deg.

A999999.999 mm

+ 99999.9999 inch

—,

* C-axis

,—

—.

!199999.999deg.

k S199999.999deg.

In incremental programming, the values 10be designated must not exceed he maximum programmable values indicated above. In absolute programming, the mmw distance of each axis must not exceed the maximum programmable values indicated abclve. In addition to the notes indicated above, it must also be taken into consideration that the cumulative values of move command must not exceed the values indicted in Table 1.6.

Table 1.6 Maximum Cumulative Values

\ Metric Input ] + 999999.999mm I Inch Input I + 999999.9999inch

Note: The values indicated above do not depend on the “least output increment”.

I A 999999.999 deg. I

999999.999deg.

1-5

1.1.4 Tape Format

The following describes the important items concerning the tape format.

(1) Label and Label Skip

By entering “label” at the beginning of a punched tape, classification and handling of

tape can be facilitated. The label skip function disregards the data appearing before the first EOB code. With

this feature, label can contain address characters and function codes which are not supported by the NC. A code that does not match the selected parity scheme can also be used. The label skip function becomes enabled when the power is turned ON or when the NC is reset. While the li~belskip function is enabled, “LX” message is displayed on the screen.

Tape Start and Tape End

(2)

At the start and end of a tape, the same code (see Table 1.7) should be punched.

Table 1.7 Tape Start and Tape End

Description

F’:

● The ER code (rewind stop code) entered following the tape start label indicates

the rewind stop when the tape is rewound by the tape rewind command.

● The ER code, expressing the tape end, indicates the stop point when several

part programs are stored in NC memory.

Tape startflape end

.—

1-6

1.1 FUNDAMENTALS OF PROGRAMMING TERMINOLOGY l——

- Label

~=~

ER CR

‘— Program part

T T

Tape start

(Called as ‘(%” or “Rewind Stop” code)

Note:

As theendof program code, M02

are

used as the p;ogram end Mcode is determined according to the setting forparamt.terpm3005 D3.

Fig.1.1

Program start (Called as “EOW or “End of Block’’. code)

SingleMainProgramPunchedonTape(EIACocle)

‘~—

(

Comment y ,– part

orM99canbeusedinsteadof’M30.Whetherornotthe Wcodesindicatedabove

~—

1~1

Tape end

LF/NL

0/0

—=— Program part

=I=Q=

- “beITrlTI T

Tape start

Program part _

Fig. 1,2

Program start

M3O&-

Program — end

-p

Program part

Multiple Programs F’unched on Tape (EIA Code)

Tape end —-

Tape end

1-7

(3) Program Start and Program End

(a) Program start

When punching a program on a tape, the following code should be punched to declare the beginning of a program. This code cancels the label skip function.

Table 1.8 Program St:irt

Description

E=.

(b)

Program end

Program start

Any of the following codes indicated in Table 1.9 should be punched at the end of

a program to declare the program end.

Table 1.9 Program End

EIA 1s0 Description

M02CR

M30CR M99CR M99LFJNL Subprogram end

Note 1:

When “M02CR” or “M30LF,’NL” is executed, the equipment may or may not be reset or rewound depending

on equipment specifications.

Refer to the manual published by the machine tool builder.

When multiple part programs are started in the NC memory, control may move to the next part program after reading the program end code shown above.

Thisoccurs when part programs are entered by total input.

If ER or LF/NLcode is executed for a program in which neither M02 nor M30 is entered at the end of the program; the NC is reset.

Mo2LF/NL

M30LFINL Program end and rewind

Program end

. — —-

“I-8

1.1.5 Program Format

(1) Program Part

The section beginning with the prc)gram start code-and ending with the program end code is called the program part. The program part consists of blocks, and each block consists of words.

E R ;

1.1 FUNDAMENTALS OF PROGRAMMING TERMINOLOGY l——

Block

Note: In this manual, the “EOB” code is expressed by a semi-colon C).

- -

Block Block

Program part

- = z

,—

Fig. 1.3 Construction of Program

Program number

(a)

By entering a program number immediately after the program start cocle, it is possible to distinguish a specific program from other programs. A program number consists of address O and a mi~ximum of 5-digit number that follows address O.

The NC memory has a capacity to store a maximum of 99 prog]ams; this capacit y

can be optionally increased to store up to 299 or 999 programx.

(b)

Sequence number

A sequence number, consisting, of address N and a maximum of 5-digit integer that

follows address N, can be ente:red at the beginning of a block. Sequence numbers are used only for reference numbers of blocks and do not influence the contents and execution order of machining processes. Therefore, sequential or non-sequential numbers may be used for sequence numbers,

It is also allowed to leave blocks without assigning sequence nu:mbers. In addition, the same sequence number may be assigned to different blocks. Although there are no restrictions on using se-

quence numbers, it is recommended to assign sequence numblars in a sequential order. Before executing the sequence number search, it is necessary to execute the program number search to determine the program in which sequence number search should be executed.

——..

——-

———

1. If a sequence number consisting of 6 of more digits is designated, 5 digits from the least insignificant digit are regarded as a sequence number.

2. If address search is executed for a sequence number which is assigned to more than one block, the block searched first is read and search processing is completed

at that block.

3. For blocks for which a sequence number is not assigned, search is possible by the address search operation if address data in the block to be searched are designated as the object of address search operation.

4. When designating a sequence number following G25 or M99, designate a 4-digit

number.

A word consists of an address character included in the function characters and a numeral of several digits that follow the address character. For example, word “G02” consists of address character “G’ and numeral “2”.

The function character means a character that can be used in the significant data area. For details of address character and function character codes, refer to Tables

1.10 and 1.11.

1-1o

1.1 FUNDAMENTALS OF PROGRAMM ING TERMINOLOGY

Table 1.10 Table of Address Characters

1——

Address

F G H

I J

‘t----- ‘–

L M IMiscellaneous function

Designation of angle for GO1 and Gill, Designation of thread angle for S76 Designation of spindle shift angle for multiple thread cutting operation

Designation of angle for multiple chamfering and rounding

IC-coordinate

Designation of depth and number of cuts for G71 to G76 . Designation of precision feed, Designation of precision lead in thread cu.ting Designation of ordinary feed, Designation of ordinary lead in thread cutting Preparatory function Incremental command of C-axis X-coordinate of center of arc, Canned cycle parameter data, Chamfer size (radius) B, O Y-coordinate of center of arc

Z-coordinate of center of arc, Canned cycle parameter data, Chamfer sizti

Increment/decrement amount in variable-lead thread cutting

INumber of repetitions

Description

——

—.

Iol

o B B B o

B, O

t----i

I B,O I IBI

Dwell time, Designation of the first sequence number of a canned cycle, Iprogram ~ o

X IX-coordinate IBI

Note: B: Basic. O: O~tion

number, and macro program number Designation of tbe first sequence number of a subprogram and the end sequence B o

number of a canned cycle Depth of cut in a hole-machining canned cycle Radius of an arc, Amount of rounding, Nose-R amount, Point R coordinate in a B o

hole-machining canned cycle Spindle function, Clamp spindle speed

Tool function, Tool coordinate memory number

Incremental command of X-axis, Dwell time, Canned cycle parameter B, O Incremental command of Y-axis o Incremental command of Z-axis, lCannedcycle parameter

IY-coordinate IZ-coordinate

1-11

—, — —.

‘H

1-.-d

B, O

I B,O I

IBI

.-...—.—

Table 1.11 Table of Function Characters

EIA code ISO code Description

EIA: Error if designated in the significant in-

Blank NUL

formation area

ISO: Disregarded

BS BS Disregarded

Tab

Disregarded

CR LF/NL End of block (EOF)

CR Disregarded

SP SP Space

LC 2-4-5 bits 2-4-7 bits

+ —

— —

(

)

Rewind stop tJpper case Lower case Control out (Comment start) Qrrrtrol in (Comment end) Disregarded, User macro operator Minus sign, User macro operator

o-9 0-9 Numerals

A-Z

Del

A-Z

Address characters C)ptionalblock skip

tJser macro operator

DEL Disregarded (includes all punched holes)

Decimal point

Parameter setting # Symbol of sharp (Variable)

[

$ $

@ @

? ‘/

[

Asterisk (Multiplication operator) Equal symbol L,eftbracket Right bracket For comment in macro program For comment in macro program For comment in macro program For comment in macro program

For comment in macro program

Remarks

EIA:

Special code

EIA:

Special code

Note

1: If a codenot indicatedaboveis designatedinthesignificantinformationarea,it causesanerror.

2: Informationdesignatedbetweenthecontroloutandcontrolincodesis regardedasinsignificantinformation.

3: Input code (EIA/fSO) is automatically recognized, and output code is determined by the setting for parameter

pmOO04

DO.

1-12

1.1 FUNDAMENTALS OF PROGRAMMI NG TERMINOLOGY

(d) Block

● A block consists of words to define a single step of operatio]l. One block ends

with the EOB (end of block) code. The EOB code is expressed by “CR’ in the EIA code system and “;LF/NL” in the 1S0 code system. In this manual, it is expressed by a semicolon “;” ple.

● Characters not indicated in Tables 1.10 “Table of Addrew Characters” and

1.11 “Table of Function Characters” must not be used.

● One block can contain up to 128 characters. Note that inval id chamcters such

as “Del” are not counted.

to make the explanation sim-

.—

~=,,e,) +--A

(a) Adding a character for TV check (an error occurs if an even number of characters is coI Itained in a block.)

; NO058G03X .-. Z . . .

3 E“””” F’”; ,___!

L—____— ‘essth”’129 –

Fig. 1,4 Block

(2) Comment Part

A comment can be displayed by using the contrcd out and control in

(a) Entering a comment in a program

It is possible to display a required comment on the screen by enclosing it with the control out and control in codes in a part program. The information enclosed by

these codes is regarded as insignificant information.

characters in a block

(b) Number of valid characters atlowed in a block

codes.

(b) Entering the control out and control in codes

The control out and control in codes can be entered in.the same manner as entering ordinary characters.

● “(’’:Press the [U] key after pressing the [SHIFT] key.

● “)’’:Press the [V] key after pressing the [SHIFT] key.

(Operation panel with 9-inch CRT)

,GQ

o—

Note 1: The characters that can be entered between the control out and control in codes are those that are entered by

2: It is not allowed to use tbe control out and control in codes in the area which are already enclosed by the control

Fig. 1.5 Characters that can be Entered between Control Out and Control

using the keys enclosed by dark line in Fig. 1.5.

out and control in codes.

In Codes (Keys Enclosed by Dark Line)

-“

Charactersthat

“(” (control out) and “)” (control in) codes

can be entered between

1-14

1.1 FUNDAMEN1-ALS OF PROGRAMMIIQG TERMINOLOGY 1—

RUNNING RUN

(TESTPROGRAM); GOO X1OO.Z1OO.; Go1 XO ZO F1O.;

(DRILLEND); ABSOLUTE

xl 200.000

Z1 2.000

TOOL: TOIO1 ACT : S1

FEED: F. 71rev

MEM

INCREMENT xl 0.000 Z1 0000

MAX : S1 5000 G67 G133 COM: S1 10MI G69

- p] co. . . . SETING

“EEJmn@zElL2iA

Emilmmniiiiiil

Fig. 1.6

Programmable Range (Input Format)

(3)

Program Execution Display Screen

012345

NooO18

G/MCODE

G151

G Go1 G80 G97 G199 G99 G127 G40 G125

G123M03

STP

LSK

This model of NC adopts the variable block format which complies with .lIS B6313. Programmable range of individual addresses is indicated in Table 1.12. The numbers

given in this table indicate the allowable maximum number of digits. An example of input format is given below.

x+53

3 digits to the right of a decimal point

5 digits in integer part

Sign

Address is X

This varies depending on the dimensioning system

(Metric or inch).

See Table 1.12.

Input data should be entered without a decimal point. If a decimall point is used, the entered value is treated in a different manner. Leading zeros and the’ ‘+” (plus) sign can

be omitted for all kinds of address data including sequence numbers. Note that, howev-

er, the “-” (minus) sign cannot be omitted.

Table 1.12 Input Formal

Address

Program number

Sequence number

G function

Linear axis

(x z, L K u,

Coordinate words

Feed per minute (mm/min) function

Feed per revolution and thread lead

S function

T function

M function

W, R, Q,~J)

Rotary axis

(c, H)

Dwell

Metric Output Inch Output

MetricInput Inch Input MetricInput Inch Input

05 05 N5 G3 G3

a+63

F60 or F63

F33 F34

T(2+2) T(2+2) T(3+3) T(3+3)

U (P) 63 U (P) 63

a+54 a+63 a+54 B, O

b+63 b+63 o

F52 or F54 F60 or F63 F52 or F54

F24 F33 F24 F26 F34 F26

S5 S5

M3 M3

N5 B

B: Basic

O: Option

B B B B B

B B

Program number designation

Sequence number designation

Number of repetitions

Designation of angle of line

Designation of multiple-thread angle

Note: The input format for “feed per minute” is set by using parameter pm2004 DO,

P5 P5

c! (P) 5

L9 L9

A (B) 33 A (B) 33

B3 B3

Q(P)5

B, O

0 o

1-16

1.1,6 Optional Blclck Skip (/1), (/2 to /9) *

If a block containing the slash code “/n (n=l to 9)” is executed with the external optional block skip switch corresponding to the designated number set ON, the commands in the block following the slash code to the end of block code are disregarded. The slash code “/n” can be designated at any position in a block.

Example:

/ 2 N 1234 GOOX1OO / 3 Z200;

If the “/2” switch is ON, the entire block is disregarded, and if “/3” switch is ON, this block indicates the following.

1.1 FUNDAMENTALS OF PROGRAMMING TERMINOLOGY

SUPPLE-

MENT

N 1234

“l” can be omitted for “/1”.

2. The optional block skip function is processed when a part program is read to the

buffer register from either the tape or memory. If the switch is set ON after the block containing the optional block skip code is read, the block is not skipped.

3. ~le optional block skip function is disregarded for program reacling (input) and

punch out (output) operation.

GOOX1OO;

. .-. .—.....-. .—

1-17

— ....-. -—.--.. --.. —”---------

~—... ,-. —

_.-. —- ——. — ——. —

1.1.7 Buffer Register and Multi-active Register

By using the buffer register and multi-active register, the NC ensures smooth control of the machine by reading the blocks of data into the buffer register.

(1)

Buffer Register

In normal operation, two blocks of data are buffered to calculate the offset and other data that are necessary for the succeeding operation.

In the nose R offset mode (option), two blocks of data (a maximum of four blocks of data, if necessary) are buffered to calculate the offset data that are necessary for the succeeding operation. In both of the normal operation mode and nose R offset mode, the data capacity of one block is amaximum of 128 characters, including the EOB code.

(2)

Multi-active Registers *

With a part program enclosed by M93 and M92, a maximum of seven blocks of data are buffered. If the time required for automatic operation of these seven buffered blocks is longer than the time required for the buffering and calculation of the offset data for the next seven blocks, the program can be executed continuously without a stop between blocks.

Table 1,13 M92 and M9:3 Codes

M92 Multi-active registers OFF

Function

Multi-activeregistersON

1.2 BASICS OF FEED FUNCTION

This section describes the feed function that specifies feedrate (distance per minute, distance per revolution) of a cutting tool.

1.2.1 Rapid Traverse

1.2 BASICS CIF FEED FUNCTION

SUPPLEMENT

(ID

Rapid traverse is used for positioning (GOO)and manual rapid traverse (RAPID) operation. In the rapid traverse mode, each axis moves at the rapid traverse rate set for the individual

axes; the rapid traverse rate is determined. by the machine tool builder and :Setfor the individual axes by using parameters. Since the. axes move independently of each other, the axes reach the target point at different time. Therefore, the resultant tool paths are not a straight

line generally.

The rapic, traverse override function can adjust the set rapid traverse rate to Fo, 25%, 50%,

and 100%~where F. indicates a fixed feedrate set for parameter pm244’7.

1. Rapid traverse rate is set in the following units for the individual axes. Setting units of rapid traverse rate

2. The upper limit of the rapid traverse rate is 240,000 mm/min. Since the most appropriate value is set conforming to the machine capability, refer to the manuals published by the machine tool builder for the rapid traverse rate of your machine.

0.001 mm/min or

1 deg.lmin

1.2.2 Cutting Feed (F Command)

The feedrate at which a cutting tc)olshould be moved in the linear interpolation (GO1) mode or circular interpolation (G02, G03) mode is designated using address characters F and E. The axis feed mode to be used is selected by designating the feed function G code (G98 or G99) as indicated in Table 1.14. Select the required feed mode by designating the feed func-

tion G code before specifying an F and E code.

Table 1,14 Cutting Feecl Mode G Codes

G98

\ G99 IDesignation of feed per revolution (mm/rev) mode \ 10 I

Designation of feed per minute (mm/min) mode

! 1

Function

Group

See 1.2.3 “Switching between Feed per Minute Mode and Feed per Revolution Mode” for details of these G codes. F and IEcodes are modal and once designated they remain valid until another For E code is designated. If feed mode designation G codes are switched between G98 and G99, however, it is necessary to designate the F and E code again. If no new F and E codes are designated, alarm “0370” occurs. Note that it is not allowed to designate an E code in the G98 (feed per minute) mode. If an E code is designated in the G98 mode, alarm “0371” occurs.

————

.- ..— —. .— -—

1-20

1.2 BASICS OF FEED FUNCTION

(1) Feed per Revolution Mode (G99)

A feedrate of a cutting tool per revolution of the spindle (mm/rev, inch/rev) can be designated by a numeral specified following address character F or E.

Table 1.15 Programmable Range of F and E Commands

(Feed

perRevolutionMode)

Format

F33

mm input

mm output

inch input

mm input

inch output

inch input

I -

Note:!: Theallowablemaximumvalueforthe X-axisis1/2ofthe value indicatedin theta ble.

;!: The upper ]jmjt of feedrates could be re~tr-jcted

programmable feedrate range, refer to the manuals published by the machine tool builder.

The feedrate per revolution is further restricted as indicated in Table 1.16 due to spindle

speed S.

Table 1.16 Restrictions on F and E Commands by Spindle Speed

E34 F24 E26 F33 E34 F24 E26

FO.001.to F500.000 mm/rev EO.0001 to E500.0000 mm/rtv FO.0001 to F19.6850 inch/re’~ EO.000001 to E19.685000 inch/rev FO.001 to F1270.000 mm/re~ EO.0001 to E1270.0000 mm/rev FO.0001 to F50.0000 inch/re+~ EO.000001 to E50.00000 inch/rev

bytheservosystemand[hemechanical system. For the actual

Programmable

Range

An F command specified in the simultaneous 2-axis linear interpolation mode or in the circular interpolation mode represents the feedrate in the tangential direction.

Example of Programming (linear interpolation mode)

Whh the following program: G99 S1OOO(r/rein); GO1 U60. W40. FO.5;

F x S = 0.5 mm/rev x 1000 r/rein

= 500

mm/min

= ~~

Z-axis component

- X-axis component

Tangential velocity

mm/min

500

+x I 300

——

400 mm/min

mm/min

Fig. 1.7 F Command in Simultaneous 2-axis Control Linear Interpolation

(Feed per Revolution)

Example of Programming (circular interpolation mode)

With the following program: G99 S1OOO(r/rein); G03U. ”” W”.

F x S = 0.2 mm/rev x 1000 r/rein

= 200 mm/min

Note 1: An FOcommand causes an input error.

2: A feedrate in the X-axis direc(ion is determined by the radial value.

Fig. 1.8

F Command in the Simultaneous

1.. ”FO.2;

Center

I ‘\

/ I

mm/min

200

2-axis Control Circular

Interpolation (Feed per Revolution)

y&LE-

Do not specify a negative value for an F command. An F command with a negative value causes alarm “0102”.

1-22

1.2 BASICS 01: FEED FUNCTION

(2) Feed per Minute Mode (G98)

A feedrate of a cutting tool per minute (mm/min, inch/rein) can be designated by a numeral specified following address character F. It is possible to set ttle F60 format and

F63 format (mm input) by the setting for parameter pm2004 DO. T!he programmable range is indicated in Table 1.17.

pm2004

DO=O

pm2004

DO=l

‘“C’””’PU’=R

inch output

Table 1.17 f

inch input

“r

F54

Note1: The allowablemaximumvalue

2: The upper limit of feedrates could be restricted by the servo system and the mechanical system. For the actual

programmable feedrate range, refer to the manuals published by the machine tool builder.

‘ogrammable Range of F Commands (Feed per Minute Mode)

Programmable Range (Linear Axis)

F1to F240000mm/min

FO.01to F94488.18 inch/rein

F1 to F609600 mm/min

FO.01to F24000.00 inch/rein

FO.001 to F240000.000 min/min

FO.0001 to F94488.1890 inch/rein

FO.001 to F609600.000 mm/min

FO.0001 to F24000.0000 inch/rein

~i~a

for the X-axis is 1/2 of the value indicated in the table.

Programmable Range (Rotary Axis)

I F0.01toF240000.00 deg/min I

F1 to F240000 deg/min

FO.01 to F240CIO0.00deg/min

FO.001 to F240000.000 deg/min

FO.001 to F240000.0000 degjmin

FO.001 to F240000.000 deg/min

FO.0001 to F240100.0000deg/min

.—

(3) Simultaneous 2-axis Control

An F command specified in the simultaneous 2-axis linear interpolar ion mode or in the

circular interpolation mode represents the feedrate in the tangential direction.

Example of Programming (linear interpolation mode)

With the following program:

G98;

GO1 U60. W40. F500.;

F = 500 = ~3002 + 4002 (mm/min)

Fig, 1.9 F Command in Simultaneous 2-axis Control Linear Interpolation

(Feed per Minute)

..--—.-.___________________...__. _______ .. . .

. . .......... .

Tangential velocity

500 mm/mi I

~ z..mis component .X

X.axis component

\/’

1-23

\,~

——

400 mm/min

—..—...-. ———, —,.-,.

/’”

I 300 mm/min

— ___________

Example of Programming (circular

interpolation mode)

y+#E.

(II)

Whh the following program:

G98; G03X. .” Z”” l.”o F200.;

F = 200 = V’FX2+- FZ2

(mm/min)

Note 1: An FO command causes an input error.

2: A feedrate in the X-axis direetion is determined by the radial value.

Fig. 1.10

Do not specify a negative value for an F command. An F command with a negative value causes alarm “O102”.

F Command

Interpolation (Feed per Minute)

in the Simultaneous

Center

: ‘i, I

;

2-axis Control Circular

200 mm/min

1-24

1.2 BASICS CIF FEED FUNCTION

Rotary Axis and Linear Axis

(4)

An F command specified in the interpolation mode between a rotar,y axis and a linear

axis represents the feedrate in the tangential direction.

Example of Programming

G98; GOI.

W1O. H60. F1OO.;

● mm input (F60)

Distance = ~100002 + 600002

60827.625 = 0.6082

‘ime = 1000000

● inch input (F52)

Distance

Time =

Fig. 1,-11

Independent Rotary Axis Command

(5)

If a rotary axis command is specified independently, feedrate is det{,xmined according to the selected input increment systsm. In the case of inch input syst~m, the unit of fee-

drale is determined by the setting for parameter,

~1000002 + 600002 = 1166190.0379

LET:::!:::::;:::

11~o~o~~~79 = 0.1166 (rein) = 6.9 (s)

FCommand in Interpolation between Rotary Axis and Linear Axis

(Feed per Minute)

= 60827.625 C-axiscomponent

Z-l~is component

(rein) = 36.5 (s)

+-z ./=!’omm

Tangential velocity

100 mm/min

-- —... —

--, —-.

6[)deg

Ta131e1.18

1-25

,——-.———.—..—..——

—.—..—..——-- — _____________

1,2.3 Switching between Feed per Minute Mode and Feed per Revolution Mode

(G98/G99)

Before specifying a feedrate command (E, F), a G code that determines whether the specified feedrate command is interpreted as feed per minute value or feed per revolution value should be specified. These G codes (G9!3, G99) are modal and once they are specified they remain valid until the other G code is specified. When the feed mode designation G code is specified, the presently valid E and F codes are canceled. Therefore, an E and F code must be specified newly after switching the feed mc)de by designating G98 or G99 command. The initial status that is established when the power is turned on is set by parameter pm4000.

Table 1.19 Parameter pm4000 and Initial Status

l-%=%-f-

1 pmqooo D2 = I I

(1) Feed per Minute Mode ((398)

G99

By specifying “G98;”,

minute mode.

Table 1.20 Meaning of (>98 Command

mm input

’98

the F codes specified thereafter are all executed in the feed per

-+%+

L..___H!

(2) Feed per Revolution Mocle (G99)

By specifying “G99;”, revolution mode.

Table 1.21 Meaning of G99 Command

the F codes specified thereafter are all executed in the feed per

inch/rein

1-26

1.2.4 Automatic Acceleration and Deceleration

Automatic acceleration/deceleration control is provided for rapid traver:;e and cutting feed operation, respectively.

(1) Acceleration and Deceleration for Rapid Traverse and Manui4 Axis Feed Op-

eration

For positioning (GOO),manual rapid traverse (RAPID), manual cent inuous feed (JOG), and manual handle feed (HANDLE), linear pattern automatic acceleration/deceleration is applied. Rapid traverse rate and acceleration/deceleration time co:mtant for rapid traverse are set for following parameters.

1.2 BASICS OF FEED FUNCTION

Table 1.22 Parameters Used for Setting Rapid Traverse Rate and Accelera-

tion/Deceleration Time Constant

Rapid traverse rate Acceleration/deceleration time constant

,----,Pi,

Feedrate

GOO

:***

Time ~

Fig. 1.12 Automatic Accelera,tion/Deceleration in Linear Pi~ttern

-t

Acceleration and Deceleration for Cutting Feed

(2)

For cutting feed (GO1 to G03 mode), feedrate is controlled by the automatic acceleration/deceleration in the exponential pattern.

—---

Feed rate

L“=‘.

Fig. 1.13 Acceleration/Deceleration in Exponential Pattern

Time constant for cutting feed and feedrate bias are set for parameters. For tapping,

time constant and feedrate bias can be set independently.

Table 1.23 Parameters for Tapping

X-axis Z-axis

Feedrate time constant pm2501 Feedrate bias pm2821 Tapping time constant pm2511

Tapping feedrate bias pm2831

For the parameters indicated above, the most optimum values are set for respective machines. Do not attempt to change the setting unless necessary.

pm2502 pm2503

pm2822 pm2512 pm2513 pm2832 pm2833

3rd-axis

pm2823

4th-axis

pm2504 pm2824 pm2825 pm2514 pm2515 pm2834 pm2835

5th-axis

pm2505

1-28

COMMANDS CALLING A)(IS

MOVEMENTS

Chapter 2 describes the interpolation commands, thread cut-

ting function, and reference point return function.

2.1 INTERPOLATION COMMANDS . . . . . ...2-3

2.1,1

2.1.2

2.1.3

2.1.4

2.1.5

2.1.6

2.1.7

2.2 USING THE THREAD CUTTING

FUNCTION,, . . . . . . . . . . . . . . . . . . . . . . 2-28

2.2.1 Thread Cutting and Continuous Thread

2.2.2

2.2.3 Variable Lead Threacl Cutting (G34) * ., , . . . 2-37

Positiorling (GOO,G06) . . . . . . . . . . . . . .. . .. 2-3

Linear interpolation (Gil) . . . . . . . . . . . . . . . . 2-5

Circular Interpolation

(G02, G03, G22, G23) . . . . . . . . . . . . . . . . . . . 2-9

Chamfering (Gil) . . . . . . . . . . . . . . . . . . . . ..2-f14

Rounding (G12) . . . . . . . . . . . . . . . . . . . . . ..2-t6

Cylindrical Interpolation (G124, G1 25)* . . . . 2-18

Polar Coordinate Interpolation

(G126, G127) . . . . . . . . . . . . . . . . . . . . . . . . . . 2-21

Cutting (G32) . . . . . . . . . . . . . . . . . . . . . . . . .:!-28

Multiple-thread Cutting (G32) * . . . . . . . . . . 2-34

2-1

—.— ..—.—

2.3 REFERENCE POINT RETURN . . . . ...2-39

2.3.1

2.3.2

2.3.3

2.3.4

Automatic Return to Reference Point

(G28)” . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...2-39

Fteference Point Return Check (G27) . . . . . . 2-44

Fleturn from Reference Point Return (G29) . 2-45

Second to Fourth Reference Point Return

(GO)* .,.......,.........”..........,,, 2-49

2-2

2.1 INTERPOLATION COMMANDS

2.1

2.1.1

INTERPOLATION COMMANDS

This section describes the positioning commands and the interpolation cclmmands that control the tool path’ along the specified functions such as straight line and wc.

Positioning (GOO,G06)

In the absolute programming mode, the axes are moved to the specified pcint in a workpiece coordinate system, and in the incremental programming mode, the axes move by the specified distance from the present position at a rapid traverse rate,

For calling the positioning, the following G codes can be used.

Table 2,1 G Codes for Positioning

Positioning in the errcr detect ON mode

=+2!!+

(1) Positioning

Positioning in the errcr detect OFF mode

in the Error Detect CIN Mode (GOO)

When “GOOX(U) o“ . Z(W) 0. “ (*C(H) o “ . *Y(V) 0.. );” is designated, positioning is executed in the “error detect ON” mode, in which the program advances to the next block only when the number cf lag pulses due to servo lag are checked after the

completion of pulse distribution has reduced to the permissible val~e. In the GOOmode, positioning is made at a rapid traverse rate in the simultaneous 2-axis

(*5-axis) control mode. The axes not designated in the GOOblockdo not move. In positioning operation, the individual axes move independently of each other at a rapid traverse rate that is set for each axis. The rapid traverse rates set for t]le individual axes differ depending on the machine. For the rapid traverse rates of you] machine, refer to the manuals published by the machine tool builder.

Fig. 2.1

Positioning in Simultaneous 2-axis

Control Mode

2-3

——.—-—---

.——-— ..-,—..——--—-————-.

-D

—

GOOdetermines the speed for offset movement.

Designation of GOOcan be omitted

since it is a modal command.

—

1. In the GOOpositioning mode, since the axes move at a rapid traverse rate set for the individual axes independently, the tool paths are not always a straight line. Therefore, positioning must be programmed carefully-so that a cutting tool will not interfere with a workpiece or fixture during positioning.

2. The block where a T comlmand is specified must contain the GOOcommand. Designation of the GOO command is necessary to determine the speed for offset movement which is called by the T command,

Example of Programming

G50 X150. Z1OO. ; GOO TO1O1 S1OOO M03 ;

(GOO) X30. Z5. ; -

—

?,/”

---

@30. —

F‘i‘

Fig. 2.2

Positioning in the Error Detect OFF Mode (G06)

(2)

When “G06 X(U) .0 “ Z(W) “ “ o (* C(H). “ “ Y(V) c “ .);” is specified, positioning

is executecl in the “error detect OFF” mode. In the G06 mode, positioning is executed in the simultaneous 2 axis (*up to 5 axis) con-

trol mode. Note that the G06 command is not modal and valid only in the designated

block. In this mode, program advances to the next block immediately after the comple-

tion of pulse distribution.

2.1,2 Linear Interpolation (GOI )

With thecommaqds of ’’GOl X(U) “ “ . Z(W) “ “ “ (*C(H)” “ “Y(V) . ““)1F(E) ‘ “ “;“,linear interpolation is executed in the simultaneous 2-axis (*5-axis) control mode. The axes not designated in the GO1 block do not move. For the execution of the linear interpolation, the following commands must be specified.

(1) Command Format

To execute the linear interpolation, the commands indicated below must be specified.

(a) Feedrate

2.1 INTERPOLATION COMMANDS

SUPPLEMENT

(3)

Feedrate is designated by an For E code. The axes are controlled so that vector sum (tangential velocity in reference to the tool moving direcltion) of feedrate of the designated axes will be the specified feedrate.

F (mm/min) = ~Fx2 + FZ2+ (Fc2)

(Fx: feedrate in the X-axis direction)

If no F or E code is designated in the block containing GO1 or in the preceding blocks, execution of a GO1 block causes alarm “0370”.

● With an F code, axis feedrate is specified in either feed per spindle revolution

(mm/rev or inch/rev) or feed per minute (mm/min or inch/rein).

● If the optional C-axis is selected, the feedrate of X- and Z-axis and that of C-

axis differ from each other. Feedrates of these axes obtained by the same F code are indicated in Table 2.2 below.

Table 2.2 Feedrates of X-/Z-axis and C-axis (F Command)

\\ I/,

POINT

‘Q’

Minimum F Command Unit

1 mm/min 1 deg/min

0.1 inch/rein 1 mm/min

0.0001 inch/rein

0.001 mm/min 0.0003937 degjmin

0.0001 inch/rein

2.54 deg/min

0.3937 deg/min

0.1 deglmin

0.001 deg/min

0.00254 deg/min

0.0001 deg/min

pm2004

DO=O

pm2004

DO=l

F Function

(Feed

mm output

inch output

mm output

—

inch output

per Minute)

mm input F60

inch input F51

mm input F60

inch input F51 0.1 inch/rein

mm input F63 0.001 mm/min

inch input F54

mm input

inch input F54

F63

Feedrate of X-/Z-axis Feedrate of C-axis

For the C-axis, a feedrate cannot be specified in the feed per minute mode.

2-6

2.1 INTERPOLATION COMMANDS

(b) End Point

The endpoint can be specified in either incremental or absolute values corresponding to the designation of an address character or G90/G91. For details, see 3.2.1, “Absolute/Incremental Programming”.

1. z

Programmed point

;

Present tool position

— +Z

e ~:~

Fig.2,3

Example of Programming

G50 X1OO. Z60.; GOO T0202 S600 M03;

GO1 ZO F1.;

LinearInterpolation

x35. Z5.;

X60. FO.2;

Axes are

}

moved in the GO1 linear interpolation mcde,

)’

_________ ,. _. ._. ... .. . ._

Fig.2.4 Exampleof Programming

—.-— -—-—.. .—.-’..—--.. —.-

2-7

. . .--—-.——~

,—,.-... -——. .- .— .——.. —-——, —. —.-—-— -

(2) Angle-designated Linear Interpolation*

By selecting the optional angle-designated linear interpolation function, it is possible to execute linear interpolation by designating an angle.

With the commands of “GO1 X(U) “ 00 A “ “ “ F(E)” 0. ;“ or “GO1 Z(W) “ .0 A “ “ o

F(E) “ . “ ;“, linear interpolation is executed at an angle A which is measured from the +Z-axis to the end point specified by either X or Z coordinate as shown in Fig. 2.5.

Feedrate is specified by an F or E code along the tangential direction. Programmable range of an angle A is indicated in Table 2.3.

Table 2.3 Programmable Range of Angle (A)

Programmable Range of Angle (A)

How the angle designated by command A is measured is determined by the sign which precedes the specified value as indicated in Table 2.4.

Table 2.4 Definition of Angle

Definition

Angle

measured in the countercloc

l=-t-- *+Z

A-

wise direction from the +.-axis

Angle measured in the clockwise

direction from the +.-axis

A+

Starl point

1 I L-------

Fig. 2.5 Angle-designated

Start point

Linear Interpolation

2-8

Example of Programming

2.1 INTERPOLATION COMMANDS

GO1 X50. A150. FO.3; GO1 ZO. A-180.; .-

+— @)

Fig. 2.6 Angle-designated Linear Interpolation

2.1.3 Circular Interpolation (G02, G03, G22, G23)

By specifying the following commands in a program, the cutting tool mo~’es along the specified arc in the ZX plane so that tangential velocity is equal to the feedrate specified by the For E code.

G02(G03) X(U) .O” Z(W) ”C” I” C. K.””(R ““”) F(E).””;

Center

-—— +Z

Fig. 2.7 Circular Interpolaticm

2-9

——.——. ———=—.. —.——-. .—. -—-. —..—-—-. ——.. --... ———. —,—. .-—... ..—.-— ...—. ——.——... ..

(1) Command Format

To execute the circular interpolation, the commands indicated in Table 2.5 must be specified.

Table 2.5 Commands Necessary for Circular Interpolation

Item

Direction of Rotation

End Point Position z (w)

Distance fromthe Start

Point to the Center centerof arc

Radius of Circular

(a) Rotation direction

The direction of arc rotation should be specified in the manner indicated in Fig. 2.8.

Arc R

G02

Address Description

G02

G03

x (u) X coordinate of arc end point (diametric value)

*Y(V)

Clockwise (CW) Counterclockwise (CCW)

coordinate of arc end point Y coordinate of arc end point Distance along the X-axis from the start point to the

center of arc (radial value)

DistancealongtheZ-axisfromthe startpointto the

DistancealongtheY-axisfromthe startpointto the centerofarc

Distance to the center of arc from the start point

Clockwise direction (CW)

Counterclockwisedirection (CCW)

‘-

[

—~

Fig. 2.8

(b) End point

The end point can be specified in either incremental or absolute values correspond-

ing to the designation of G90 or G91.

Rotation Direction of Circular Arc

G02

G03

2-1o

2.1 INTERPOLATION COMMANDS

If the specified end point is not on the specified arc, the arc radius i:; gradually

changed from the start point to the endpoint to generate a spiral so that the endpoint

lies on the specified arc.

Example of Programming

GO1 Z1OO. XO F1O.;

G03 Z-50. K-1OO.;

(

!50. O

100.

‘\

—---l-

100. z

Example of Programming

GO1 Z50. XO; G03 Z- 100. K-50.;

Fig. 2.9

Interpolation with End Point off the Specified

-100

(a) End point positioned inside the circumference

(b) End point lying outside the circumference

Arc

The center of arccanbe specified in two methods - designation of the distance from the start point to the center of the arc and designation of the radius of the arc.

End point

!;tart point

—---

‘qk[

;

.l-.–_._—

+P-

Center

.0”

--L

Fig. 2.10

c Specifying the distance from the start point to the center

Independent of the designated dimensioning mode (G90 or G91), the center of an arc must be specified in incremental values referenced from the start point.

● Specifying the radius

When defining an arc, it is possible to specify the radius by using address R

instead of specifying the center of the arc by addresses I or K. This is called “circular interpolation with R desigmtion” mode.

o For the circular arc with the central angle of 180 deg. or smaller, use an R

value of “R > O“.

. For the circular arc with the central angle of 180 deg. or larger, use an R

value of “R < O“.

Example of Programming

.—— ———. —

Fig, 2.11

G02X(U) ””” Z(W) ””” R*”” ”F(E)”’ “;

or smaller

Start point

Circular interpolation with Radius R Designation

2-12

2.1 INTERPCILATION COMMANDS

SJJPJLE-

If an R command is used to specify the radius of an arc, G22 and (;23 can be used instead of G02 and G03. When G22 or G23 is used, the programming format is the same as used when G02 or G03 is specified with an exception of a G code. l[fG22 or

G23 is used, however, it is not allowed to define the center of the arc by I and K com-

mands. If these commands are used with G22 or G23, alarm “0162” occurs.

—

(2) Supplements to Circular Interpolation

A circular arc extending to multiple quadrants can be defined by the commands in a single block.

Example of Programming

GOIZ””” F. O”; G02 X60. Z-46.6 120. K-19.596 F . “. ;

\ AA

@ 100.

27.

R28. “\

I ~

b 60.

—.——

Fig. 2.12 Circular Interpolation over Multiple Quadrants

Table 2.6

F==t=-&’;’m1

‘?

–428::–202 = –fi = –Ig.sgfj “m

2.1.4 Chamfering (G11)

With thecommandsof’’Gll X(U) .00 K “ ‘ “ {orZ(W) .00 I “ c J}F(E) ~“ . ;“,chamfering

at corners is specified. In the designation of chamfering, single axis command of either Xaxis or Z-axis should be used.

Gll is a modal G code of 01 group. Once designated, it remains valid until other G code in

the 01 group is specified next.

(1) X-axis Chamfering

G1l X(U) O”. K+ ..” F(E)””;

——

Chamfer size

—

— Designation of chamfering direction

With the commands indicated above, X-axis chamfering is executed.

K- K+

End point \

L.-

Fig. 2.13 X-axis

\~ ‘

450

Start

point

X (diametric value)

Chamfering

(2) Z-axis Chamfering

G1l Z(W) ”O” I+

““. F(E)”””;

—.

— Chamfer size (radial value)

t---!--

— Designation of chamfering direction

With the commands indicated above, Z-axis chamfering is executed.

End point

-1

0’

450

1’

‘/

Start point

Fig. 2,14 Z-axis Chamfering

2-14

Example of Programming

GOOX30. ZO; Gll Z-20. 18. F30 ; — @ (Gil) X80. ,K-7. ;

.— Q)

20.

H+

2.1 lNTERPOLATION COMMANDS

SUPPLE. MENT

2.15 Example of Programming

Fig.

1. The following restrictions apply to the chamfer size K and I. \KICIU/2],l 11<1 Wl

The K and I values must be smaller than the total move distance 1n the direction

of the designated axis. A formad error occurs if a value exceeding this limit is specified.

2. Alarm “0445” occurs if both addresses X and Z are specified in the same block,

a block not including I or K is specified in the Gll mode, or I or K value is “O”.

3. The nose R offset offset function* is valid for the block where G 11 is specified.

4. It is possible to specify the Gll block in the commands of blocks that define fin-

ishing shape for a multiple repetitive cycle (G70 to G73).

5. It is possible to specify chamfering by specifying GO1 instead clf Gil. GOIX(U) .”” K””” {or Z(W) ””” I.”} F(E) o“”;

.— _______ ____. — ._ -—... ..

2-15

— . . . .. —. —.. ,— .-,. =-—.. ,-< ..—. .—. ———-— —-—

2.1.5 Rounding (G12)

With the commands of “G12 X(U) “ “ . K “ c “ {or Z(W) “ . “ I . “ “} F(E) o “ . ;“, corner rounding is executed. In the designation, single axis command of either X-axis or Z-axis should be used. Rounding is executed in a quarter circle.

G12 is a modal G code of 01 group. Once designated, it remains valid until other G code in

the 01 group is specified next.

(1) X-axis Rounding

G12X(U). ”.K* -“” F(E)..;

——

————

— Designation of rounding direction

Rounding size

With the commands indicated above, X-axis rounding is executed.

K- K+

End

point

‘\

L._

Fig. 2,16 X-axis Rounding

Start point

)( (diametric

value)

(2) Z-axis Rounding

G12Z(W)””” I* ““. F(E) ”.o;

~ –L—

~—

Rounding size (radial value) Designating of rounding direction

—-. ..

With the commands indicated above, Z-axis rounding is executed.

End point

—.. - —

-1

---1--w

Start point

Fig. 2.17 Z-axis Rounc!ing

2-16

Example of Programming

GOO X20. ZO ;

G12 Z-25. 19. F30 ; (G12) X70. K-6. F20 ;

$70.

— (b

+ @

25.

——

2.1 INTERPOLATION COMMANDS

$20.

G’:

Fig. 2.18 Example of Programming

1. The following restrictions apply to the rounding size K and 1. lKl<lU/21,111<lWl

The K and I values must be sma”ller than the total move distance in the direction

of the designated axis. A format error occurs if a value

specified.

2. Alarm “0445” occurs if both addresses X and Z are specified in Ihe same block, a block not including I or K is specified in the G12 mode, or I or K value is “O”.

exceeding this limit is

3. The nose R offset offset function* is valid for the block where G12 is specified.

4. It is possible to specify the G12 block in the commands of blocks that define finishing shape for a multiple repetitive cycle (G70 to G73).

5. It is possible to specify chamfering by specifying GO1 instead clf G12.

GOIX(U) ””” R.. ”{or Z(W) ””” R”””} F@)”””;

2-17

.—— — .—— —.-. .-— .. —-. .—- —

—.—

,=..—.. .— ..

——

—..—.————. .

2.1.6 Cylindrical Interpolation (GI 24, G125) *

The cylindrical interpolation function allows programming of machining on a cylindrical workpiece (grooving on a cylindrical workpiece) in the manner like writing a program in a plane using the cylinder developed coordinate system. This functions allows programming both in absolute commands (C, Z) and incremental commands (H, W).

(1) Programming Format

(a) Features of GI 24, G 125

The following G codes are used for cylindrical interpolation.

Table 2,7 G Codes Used for Cylindrical Interpolation

Cylindrical interpolation mode ON

Group

e ‘“”’’ion :

Cylindrical interpolation mode OFF

These G codes are buffering prohibiting G codes. Specify G124 and G125 in a block without other commands. If other G code is

specified with G124 or G125 in the same block, alarm “0161” (UNMATCH G

CODE) occurs, G124 and G125 are modal G codes of 20 group. Once G124 is specified, the cylin-

drical interpolation mode ON state remains until G125 is specified. When the power is turned ON or the NC is reset, the G125 (cylindrical interpolation mode OFF) state is set.

(b) Programming format

Cylindrical interpolation mode ON

G124CO”. ;

-=--Machining program in the cylindrical interpolation mode

G125 ;

+ Cylindrical interpolation mode OFF

where, C = Radius of cylindrical workpiece

(1 = 0.001 mm or 0.0001 inch)

‘Theradius of a cylindrical workpiece must always be specified. If a C command is not specified, alarm “0162” (LACK OF ADDRESS) occurs.

2-18

Feedrate

(c)

In the cylindrical interpolation mode, interpolation is executecl in the virtual C-Z plane. Therefore, after the entry to the cylindrical interpolation. mode, it is necessary to specify feedrates in the C-Z plane. value represents feedrates (mrn/min, inchhnin) in the C-Z plane.

● For cylindrical interpolation, use the G98 (feed per minute) mode. Cylindrical

interpolation is not possible in the GOOmode. To execute ~Jositiorling, cancel the cylindrical interpolation mode. Note that GOOmode nlay be specified in a plane other than the C-Z plane.

(2) Example of Programming

2.1 INTERPOLATION COMMANDS

lJse address F to specify feedrates. F

Cu”ng’oo’u----z

Example of programming

0100 ; G98 ; TO1O1; GOOX44.O CO; .— G124 C45.O ; c— GO1 G42 Z47.5 F1OO; C60.O; Z32.5 C120.O ;

C240.O; G03Z40.OC249.549R7.5; G02Z47.5C259.099R7.5; GO1C360.O; G40Z44.O; G125; M30; —

Positioning at the start point c,f cutting

Cylindrical interpolation mode ON

Machining program

Cylindrical interpolation mode OFF

Fig. 2.19 Coordinate System for Cylindrical Interpolation

———— ,.———=—..=— ... .... .. ... ..— ,,.—.—-.” .-. .

2-19

—.. -

——., —. —. —. —.. .-~ -=—— -.”-. ——. +—.. --—

Relationships between Cylindrical Interpolation and Operations

(3)

In the cylindrical interpolation mode, the following G codes maybe specified: (GOO), GO1, G02, G03, G04, G1O, G22, G23, G40, G41, G42, G65, G66, G67, (G90, G91), G98, and G134. Alarm “0161” (UNMATCH G CODE) occurs if a G code other than those indicated above is specified in the cylindrical interpolation mode.

1. In the GOOmode, only X.-axis can be specified.

2. G90 and G91 are valid only when special G code specification is selected. 3, In the G134 mode, only M commands maybe specified.

●

In the cylindrical interpolation mode, the tool radius offset function can be used. Turning ON/OFF of the tool radius offset function must be made in the cylindrical interpolation mode. The tool radius offset function is valid only in the cylindrical interpolation mode and the polar coordinate interpolation mode.

●

In the cylindrical interpolation mode, cutting in the linear interpolation (GO1) mode and circular interpolation (G02/G03) mode is available. Circular interpolation is permitted only in the C-Z plane. If circular interpolation commands are specified in other plane, an alarm occurs. For the definition of an arc, use either addresses I and K to specify the center of arc or address R to directly specify the radius of the arc. Note that designation of address R is optional.

●

The nose R offset function must be canceled before specifying G124.

●

It is not allowed to specify G124 with the mirror image function ON. Similarly, it is not allowed to turn ON the mirror image function in the G124 mode. If the mirror image function is turned ON in the G124 mode, an alarm occurs.

●

Tand S commands must not be specified in the cylindrical interpolation mode. Designation of M commands is possible in the cylindrical interpolation mode.

●

The spindle function is invalid in the cylindrical interpolation mode.

●

In the cylindrical interpolation mode, the manual absolute function is fixed to OFF.

2-20

● In the cylindrical interpolation mode, program restart is not possible. If pro-

gram restart is attempted from a block in the cylindrical interpolation mode,

alarm “0481” (PROG, ER.ROR IN G124 MODE) occurs.

restart is allowed for blocks in which the cylindrical interpolation mode blocks

are” included.

2.1.7 Polar Coordinate Interpolation (GI 2!6, G127) *

The polar coordinate interpolation function allows programming of machining that is

executed by the combination of tool movement and workpiece rotation in,a virtual rectangu-

lar coordinate system.

In the machining accomplished by the combination of a linear axis (X-axis) and a rotary axis

(C-axis), the C-axis is assumed to be a linear axis that is perpendicular to the X-axis. By assuming a rotary axis as a linear axis, machining an arbitrary shape that is defined by the Xand C-axis can be programmed easily in the X-C rectangular coordinate system. In this programming, both of absolute commands (X, C) and incremental commands (U, H) can be used.

2.1 INTERPOLATION COMMANDS

However, program

I//

POINT

(1) Programming Format

When G126 is specified, the polar coordinate interpolation mode is established and the virtual coordinate system is set in the X-C plane with the origin oft] le absolute coordinate system taken as the origin of this coordinate system. Polar

is executed in this plane. Note that polar coordinate interpolation si:arts when G126 is specified assuming the present position of the C-axis to be “O”.

Return the C-axis to the origin of the absolute coordinate system before specifying

G126.

coordinate interpolation

————_

————-—-.——.—._—. .—.’—— ... .

2-21

.—— .—,—. .- .— .- —.. —. ——— ——

(a) Features ofG126 ancjG127

The following G codes are used to turn ON/OFF the polar coordinate interpolation mode.

Table 2.8 G Codes Used for Turning ON/O FFthe Polar Coordinate interpola-

tion

~GW~ F.n.ti.n

Polar coordinate interpolation mode ON

~“

G127

Specify G126 and G12’7 in a block without other commands. If other G code is specified with G126 or G127 in the same block, alarm “0161” (UNMATCH G

CODE) occurs. G126 and G127 are moclal G codes of 19 group. Once G126 is specified, the polar

coordinate interpolation mode ON state remains until G127 is specified. When the power is turned ON or the NC is reset, the G127 (polar coordinate interpolation mode OFF) state is set.

(b)

Feed rates

In the polar coordinate interpolation mode, interpolation is executed in the X-C plane. It is necessary to specify feedrates after entering the polar coordinate interpolation mode. For the designation of feedrates, use address F. Feedrate F expresses feedrates (mm/min, inch/rein) in the X-C plane. In the polar coordinate interpolation mode, specify feedrates in the G98 (feed per minute) mode. It is not possible to specify GOO(G codes that include rapid traverse cycle). To execute positioning, cancel the polar coordinate interpolation mode. It is allowed to specify

GOOin a plane other than the X-C plane.

Polar coordinate interpolation mode OFF I 19 I

Group

—

o Restrictions on feedrates

The following must be satisfied so that the actual speed of the rotary axis does

not exceed rapid traverse rate:

F/D S (n/360) ;< (Rapid traverse rate of rotary axis)

F (mm/ rein) : F command x Feed override D (mm) : Diametric value when a cutting tool approaches closest

to the workpiece center (tool paths after offset if the tool radius offset function is used.)

2-22

2.1 INTEFIPOL.ATION COMMANDS

—

e Example of calculation

To find the maximum value of F command (override: 1.00%) Conditions:

To carry out grooving of 15 mm wide akmg the centerline

To use 12 mm diameter end mill

C-axis rapid traverse rate is 12000 deghin.

F/(15 - 12) S (z/360) X 12000 F 5314 From the result indicated above, it is possible to specify F300 in the program.

+12

———. ———. —

—-

Fig. 2.20

To find the minimum machining diameter with F comm;md of 80 mm/min. Conditions:

80/D S (n/360) X

Rapid traverse rate of the rotary axis is 12000 deg/min.

12000

D S 0.764

From the result indicated above, machining is not possible if the tool path after offset comes closer to the center of the work piece than the calculated value.

2-23

———.

. .—-..

.. ,- .—

..=. —

-.,

(2) Example of Programming

Virtual C-axis

A \

Example of programming

00001 ; G98 ;

TO1O1;

GOOX120.O CO; — G126 ; GO1

G42 X40.O

XO C40.O 1-20.0;

G03

X-25.O ;

GO1

X-40.O C25.O K-15.O ;

G03

co;

GO1

X20.O 120.0;

G03

G40 X120.O ;

GO1

F1OO.O;

G127 ; M30 ;

—

-.’

Cutting tool

X-axis

Positioning at the cutting start point Polar coordinate interpolation mode ON

Machining program using the polar coordinate

interpolation function

Polar coordinate interpolation mode OFF

Fig. 2.21 Coordinate System for Polar Coordinate Interpolation

2-24

2.1 INTERPOLATION COMMANDS

(3) Negative Polar Coordinate Specification

Fo the machines in which the positive/negative designation of the X-axis is reversed,

it is possible to select the negative X-axis specification. In this specification, the plus

and minus sign of the X-axis in the virtual X- Cplane is reversed. The coordinate system used for programming is shown in Fig. 2.22. Whether or not the neg.~tive X-axis specification is selected is specified by using parameter pm4019 D1.

pm4019 D1 = 1

pm4019 D1 = O Normal specification

Normal specification

Virtual C (+)

Q’)”-Q:)

Fig. 2.22 Coordinate System of Negative X-axis Specification Polar

Coordinate

Normal specification

Virtual C (+)

, G03

/’

..-

-“. ‘$

‘ G02

—.—

Normal specification

—

NegativeX-axisspecification

Negative X-axis specification

Virtual C (+)

Negative X-axis specification

Virtual C (+)

x (+)

Negative X-axis specification

“=

/’

.. .

. . .

) ’03

~ x (-)

G02

Fig. 2.23 Direction of Rotaticm for Arc Commands

2-25

Normal specification

Negative X-axis specification

SUPPt.E-

MENT

-1-

Virtual C (+)

——

x(-)

—

Virtual C (+)

-------- .—(

-------- -—

~-3

+—

Normal specification Negative X-axis specification

Fig. 2.24 Offset Direction of Tool Radius Offset Function

1. If the negative X-axis specification is selected, the direction of rotation for the arc commands (G02, G03) and the direction of offset for the tool radius offset (G41, G42) are reversed from those in the normal specification. This must be taken into consideration when writing a program.

2. Turn ON the polar coordinate interpolation mode when the X-coordinate is plus for the normal specification and when it is minus for the negative X-axis specification.

G41

G42

-m- x (+)

SIJPPLEMENT

cl)

(4) Relationships between Polar Coordinate Interpolation Function and Opera-

tions

In the cylindrical interpolation mode, the following G codes maybe specified: (GOO),

GO1, G02, G03, G04, G1O, 022, G23, G40, G41, G42, G65, G66, G67, (G90, G91), G98, and G 134. Alarm “0161° (UNMATCH G CODE) occurs if a G code other than

those indicated above is specified in the polar coordinate interpolation mode.

1. In the GOOmode, only X-axis can be specified.

2. G90 and G91 are valid only when special G code specification is selected.

3. In the G134 mode, only M commands maybe specified.

—

● In the polar coordinate interpolation mode, the tool radius offset function can

be used. Turning CIN/OFF of the tool radius offset function must be made in the polar coordinate interpolation mode. The tool radius offset function is valid only in the cylindrical interpolation mode and the polar coordinate interpolation mode.

2-26

—---

2.1 INTERPOLATION COMMANDS

M In the polar coordinate interpolation mode, cutting in the linear interpolation

(GO1) mode and circular interpolation (G02/G03) mode. Circular interpola-

tion is permitted only in the X-C plane. If circular interpolation commands

are specified in other plane, an alarm occurs. For the definition of an arc, use either addresses I and K to specify the center of arc or address R to directly specify the radius of the arc. Note that designation of add:ess R is optional.

. The nose R offset function must be canceled before speci~ying G126.

● It is not allowed to specify G126 with the mirror image function ON. Similar-

ly, it is not allowed to turn ON the mirror image function in the G124 mode. If the mirror image functicn is turned ON in the G126 mode, an alarm occurs.

● T and S commands must not be specified in the polar coordinate interpolation

mode. Designation of M commands is possible in the polar coordinate interpolation mode.

● The spindle function is invalid in the polar coordinate inkxpolation mode.

. In the polar coordinate interpolation mode, the manual alxolute function is

fixed to OFF.

● In the polar coordinate interpolation mode, program restart is not possible. If

program restart is attempted from a block in the polar coordinate interpolation mode, alarm “0483” (PROG, ERROR IN G126 MODE) occurs. However, program restart is allowecl for blocks in which the cylindrical interpolation mode blocks are included.

● If a command that causes the tool paths to pass the center of the polar coordi-

nate in the polar coordinate interpolation mode, alarm “0483” occurs since the C-axis feedrate becomes infinite.

- In the polar coordinate interpolation mode, selection is possible for the X- and C-axis commands whether they are specified in diametric values or radial values.

X- and C-axis commands are specified irldiameter.

* ‘--i

X- and C-axis commands are specified in radius.

——— —.-——— ..—

2-27

—

.- —-. ——

2.2 USING THE THREAD CUllTING FUNCTION

2.2.1 Thread Cutting and Continuous Thread Cutting (G32)

With the commands of “G32X (U) 00 “ Z (W) . “ “ F (E) “ “ “

;“, it is possible to cut straight thread, tapered thread, or scroll thread in the lead specified by an F (normal thread cutting) or E @recise thread cutting) command to the point specified by absolute coordinate values (X, Z) or incremental coordinate values (U, W). Note that chamfering of thread is not possible in the G32 mode. Use the CJ92or G76* mode to include chamfering in thread cutting.

(1) Programmable Range of F and E Codes

Table 2.9 indicates the programmable range of thread lead F and E.

Table 2.9 Programmable Range of F and E Commands

Format Programmable Range of F and E

mm input

F33

E34 EO.0001 - E500.0000 mm

mm output

F24 FO.0001 - F19.6850 inch

inch input

E26 F33 FO.001 - F1270.000 mm

mm input

E34 EO.0003 - E1270.0000 mm

inch output

F24

inch input

E26

FO.001 - F500.000 mm

—

EO.000004 - E19.685000 inch

—

FO.001 - F50.0000 inch

EO.OOOO1O- E50.000000 inch

— —

2-28

2.2 USING THE THREAD CUITING FUNCTION

(2) Direction of Thread Lead

The direction of thread lead specified by the F and E commands is indicated in Table 2.10.

Table 2.10 Direction of Threacl Lead

Taper Angle a

I -4

(X!Z)<

‘~+~ “. -’—~

Fig. 2.25 Thread Cutting

(3) Restrictions on F and E by Spindle Speed S

I as LISO I L-MCIintheZ-a:cis direction stmtikf be specified. I

Lead in the X-axis direction should be specified.

Direction of Thread Lead

—,

As indicated in Table 2.11, there are restrictions on the designation of F and E commands by Table 2. llspindle speed S. Concerning the X-axis feedrate component, its upper limit is 1/2 of the values indicated in Table 2.11.

Table 2.11 Restrictions on F and E Commands by Spindle :Speed S

I inch output I

F (E) x S S 24,000 inch/rein

(4) Programming Formats

Programming formats of thread cutting are indicated in Table 2.12.

Table 2.12 Programming Formats of Thread Cutting

Thread Type

Normal G31 Z(W) ...;...;

Straight thread

Precision G32Z(W). .. E;..;

Normal G32X(U) . .. Z(FO. .F O...

Tapered thread

Precision G32X(U) 0.. Z(Wj. .. E...;

Normal G32 X(U) ...;...; –

Scroll thread

Precision G32 X(U) ...;...;

● Example of programming for cutting straight thread

Command Format

Thread lead L = 5.0 mm

5.0 mm

al = IS2 = 3.0 mm

Depth of cut per pass = 1.0 mm

+-x

GOOU-42. ; _—

G32 W-68. F5.O ; ~@ GOOU 42. ;

:---;-w 68. ; u-44. ;

G32 W-68. ;

GOOU 44. ;

——

—

3—.

Fig, 2,26 Example of Programming for Cutting Straight Thread

2-30

2.2 [JSING THE THREAD CUl_HNG FUNCTION

● Example of programming for cutting tapered thread

Thread lead

Depth of cut per pass= 1.0 rnm

L = 4.0 rnm & = 3.0 rnm 52 = 2.0 rnm

GOOX13. _— G32 X38. W-35. F4.O; GOOX60. ;

W35. ;

X11. ; G32 X36. W-35. ; GOOX60.;

-Y

r—r-’---

:“

%-- L-=---l

Fig. 2.27 Example of Programming for Cutting Tapered Ttread

2-31

——.+.-.———— .—————... . .—

(5) Continuous Thread Cutting

Since the N-Chas buffer register, designation for continuous thread cutting is possible. In addition, continuous threads can be cut smoothly because the block-to-block pause time is “O” for thread cutting command blocks.

Example of Programming

\\ I//

POINT

G32X(U) ””” Z(W) .” F(E)”””; G32X(U)””” Z(W)”.; .—.— G32X(U). ”” Z(W)”””;

—--—.---—.

—Cl

;

—a

(a) Reinforced pipe coupling

Fig. 2.28 Continuous Thread Cutting

1. If designation of thread lead (F, E) is changed during thread cutting cycle, lead accuracy is lost at joints of blocks. Therefore, thread lead designation must not

be changed during threacl cutting cycle.

2. If continuous thread cutting is specified, M codes must not be specified. If an M code is specified, the cycle is suspended at the specified block and continuous thread cannot be cut.

(b) Worm screw

2-32

2.2 USING THE THREAD ICUITING FUNCTION

(6) Margin for Incomplete Thread Portions (81, 62)

At the start and end of thread cutting, lead error is generated. Therefore, margins al and 82 should be given at the start and end portions in thread cutting,

-+--_--.--f-+,

Fig. 2.29 Margins for Incomplete Threads

These margins 61 and b2 can be calculated as indicated in Table 2,13.

Table 2.13 Calculation of Margins for Incomplete Thread Portions

Approximate Value Meaning

(mm) : Thread lead

51> &(ln;-1)

62>&

S (r / rein) : K : Constant (normally 30) a(-)

Spindle speed

: Thread accuracy

–L . . . .

—

: Natural logarithm (log)

——

(Lead error)

EEE!EE3=EI

Example of calculation

Thread lead L = 3.0 mm Spindle speed S = 5.0 r/rein Thread accuracy =1/100

61 and b2for this case

61> ~(hl~-1) – 3.0

* , L*S

–3.0x500.=083rnm

60”K 60”K “

—

X 50(I

60 “K

x 3.61 = 3.0 mm

\\ I/,

POINT

~tiiia)

2.2.2 Multiple-thread Cutting (G32) *

Multiple-thread cutting (multiple threads in alead) is possible without shifting the thread cutting start point. In thread cutting operation, axis feed starts in synchronization with the startpoint pulse (1 pulse/turn) output from the spindle pulse generator attached to the spindle. Therefore, the thread cutting start point is always at the same point on the workpiece circumference. In multiple-thread cutting operation, axis feed starts when the spindle rotates by a

certain angle after the output of the start-point pulse from the spindle pulse generator.

Keep the spindle speed at the same value until one thread is cut. If the spindle speed is not maintained constant, accuracy could be lost due to servo lag.

———

1. During thread cutting, override operation and feed hold operation are disregarded.

2. If G32 is specified in the G98 (feed per minute) mode, alarm “0452” occurs.

3. If a thread cutting command is executed in the dry run mode, axes move at the jog feedrate.

Lead

--———.-

Fig, 2.30 Double-start Thread

With the commands of “G32 X (U) “ “ o Z (W) . “ “ F (E) “ “ “ B “ “ o ;“, the spindle rotates by the angle specified by address 11after the output of the start-point pulse of the spindle pulse

generator. After that thread cutting starts toward the point specified by X (U) and Z (W) at the lead specified by an For E cc)mmand.

234

2.2 USING THE THREAD CUTTING FUNCTION ——

(1) Address B Specified in Multi-thread Cutting

Least input increment : 0.0010 Programmable range : 0 S B <360.000

If decimal point input is used, “B1.” is equal to 10 (B1. = 10). B commands are nonmodal and valid only in the specified block.

(2) Number of Threads and B Command

In general, the thread cutting start points lie on the workpiece circumference; the intervals of these points are calculated by dividing 3600 by the number of t breads. Examples of multiple threads (double-start, triple-start, and quadra-start thre ads) are shown in Fig. 2.31.

Thread cutting start point

- double-start thread

1st thread : 2nd thread: B180.

Fig. 2.31

No B command

Number of Threads and B Commands

Thread cutting start point

- tripla-start thread

1st thread : No B command 2nd thread: B120. 3rd thread : B240.

Thread xtting sfart point

- quadra-start thread

1st thread : 2nd threacl: B90. 3rd thread : B1 80. 4th thread : B270,

No B command

2-35

(3) Spindle Rotating Angle from Start-point Pulse Specified by B Command

For the designation of spinclle rotating angle measured from the start-point pulse, the least detectable increment is 360°/4096 pulses ~ 0.08790/pulse since the pulses output from the spindle pulse generator (4096 pulses/rotation) are used. For a B command, an error of ~ 1 pulse of the spindle rotation detection pulses could be generated. An example of programming for double-start thread is indicated below.

Example of Programming

GOOU..; G32W”. ”F ”.”; GOOU..; w“””;

. . . .

u G32W U”;

Thread cutting of thread A

)

suPPt.E-

MEWf

GOOU O”; G32 W . . “ B180. ; GOOU”.; w“””;

. . . .

u G32WU”

Fig. 2.32 Spindle Rotation Angle from Start-point Pulse by E)Command

1. If a B command value is outside the programmable range (O to 360.000), alarm “0453” occurs,

2. If a B cc)mmand is specified for multiple-thread cutting, continuous thread cutting is not possible.

G32W . . . . B90

G32W . . . .

3. The spindle rotation angle from the start-point pulse is specified using a B com-

mand (C+to 360°) disreg~rding of the spindle rotating direction.

B180. ;

+ Since the operation is suspended at this block to wait for the

start-point pulse, continuous thread cannot be cut.

--)

Thread cutting of thread B

2-36

2.2.3 Variable Lead Thread Cutting (G34)*

With the commands of “G34 X (U) Z (W) c “ “ K “ ‘ “ F (E) . “ “ ;“, variable lead thread

can be cut; thread lead variation per one spindle rotation is specified by address K. The least input increment of a K command is 0.0001 mm/rev or 0.00001 inch/re~. If the setting for

parameter pm1000 DO = 1, the least input increment of a K command is 0.001 mm/rev or

0.0001 inch/rev.

2.2 USING THE THREAD ICUITING FUNCTION

Fig. 2.33 Variable Lead Thread

(1) Restrictions on Programmable Range of K Commands

The programmable range of K commands is restricted by the formula indicated below.

F: Fixed lead command (mm/rev or inch/rev) K: Variable lead command (mm/rev or inch/rev)

w: Distance along the Z-axis from the start point to the end pclint (mm or inch)

<“u” along the X-axis in the case of face thread cutting.>

s: Spindle speed (rev/mm)

N: Number of spindle revolutions from the start point to the end point (rev)

~ . -(F+ K/2) + ~:)z + 2“K”W

Feedrate at End Point

(2)

Specify the commands so that the feedrate at the end point will not exceed the upper limit indicated in Table 2.14.

Table 2.14 Upper Limit of Feedrate at End Point

T__l___ upper~mit

==+---+=+

S x (F + ~ + KN) S pm2800 (Max. cutting feedrate)

Feedrate at End Point

(3)

Specify the commands so that the feedrate at the end point will not be a negative value.

(F+~)2+2KW>0

1. In the continuous block thread cutting for variable lead thread cutting, distribu-

tion of command pulses is interrupted at joints between blocks.

2. If a K command is outside the programmable range, alarm “0450” occurs.

3. If G34 is executed in the dry run mode, the axes move at a feedrate designated

for the jog feedrate if “parameter pm2000 D1 = l“.

4. If address B is designated in the G34 block, alarm “0450” occurs.

2.3 REFERENCE POINT RETURN

2.3

REFERENCE POINT RETURN

2.3.1 Automatic Return to Reference Point (G28)

With the commands of “G28 X(U) 0. “ Z(W) . s “ (*C(H) 00 “ *Y(V) “ “);”, the numeri-

cal y controlled axes are returned to the reference point. The axes are first nloved to the specified position at arapid traverse rate and then to the reference point automal ically. This reference point return operation is possible in.up to simultaneous 2-axis (* 5-i~xis) control. The axes not designated in the G28 block are not returned to the reference pt)int.

Example of Programming

Intermediate positioning point

Positioning

Start point

——

d \

,–. i_. _._..~

~ ~ ‘L

,/—” —” -

—.

—

~ Reference point return operaticn

Z-axis deceleration LS

d !

Reference point

(A fixed point in the machine)

— +Z

Fig. 2.34

Reference Point Return

(1) Reference Point Return Operation

Reference point return operation is the series of operations in which the axes return to the reference point after the reference point return operation has beerl started manually.

Reference point return is accomplished in two ways:

(a) Low-speed reference point return

In low-speed reference point return operation, a deceleration Iirnit switch is used. In high-speed reference point return operation, the first return operation i.sexecuted in the low-speed type using a deceleration limit switch; the reference po int data are stored after the completion of the first reference point return and in subsequent reference point return operations is executed without using a deceleration limit

switch. Alarm “2061” to “2065” occurs if an attempt is made to start tile reference point

return operation from a position where return operation is impossible.

2-39

(b) High-speed reference point return

See parameter pm4003 D6 and D7, It is possible to use the “high-speed reference point return” in place of the “auto-

matic reference point return”.

In this case, the reference point return is executed

in the following manner.

● After the positioning at the intermediate positioning point B, the axes return

directly to the reference point at a rapid traverse rate. The axes can be returned to the reference point in a shorter time compared to the normal reference point

return operation that uses a deceleration limit switch for the individual axes.

c Even if point B is located outside the area in which reference point return is

allowed, the high-speed reference point return specification. allows the axes

to return to the reference point.

c High-speed reference point return is enabled only for the axes for which nor-

mal reference point return has been completed either manually (manual reference point return) or by executing the G28 command after turning ON the power.

● If low-speed reference point return has not been completed for the X- and Z-

axis either manually or by executing the G28 command after power-ON, Iow-

speed reference point return is executed for the axis (X- and/or Z-axis) which

is specified in the G28 block.

● High-speed automatic reference point return is valid only when reference

point return is called by G28, and it does not influence manual reference point

return operation.

2!-40

—- ... .

2.3 REFERENCEP OINTRETURN

(2) C-axis* Control integrated with Spindle Control

Reference point return is executed for the C-axis each time the control mode is changed over from the spindle control to the C-axis control.

Feedrate

Approach speed

~ / creep “’’”

Reference point

-ii--

Fig. 2.35 Reference Point Return Pattern of C-axis lntegri~ted with Spindle

For the C-axis integrated with the spindle, a deceleration limit switch in low-speed reference point return operation.

Reference pulse

Set for parameters

)

is not used even

(3) Supplements to the Automatic Reference Point Return Commands

. Concerning machine lock intervention, there are two types of operation: turn-

ing ON the machine lock after suspending axis movement by using the feed hold function, and turning OFF the machine lock after suspending axis movement again by using the feed hoid function. Table 2.15 shows how the machine operates according to the machine lock intervention.

Table 2.15 Machine Operation according to Machine Lock Intervention

Machine Lock

OFF + ON

Machine Lock

OFF - ON

- OFF

Low-

speed

type

l+igh-

speed

type

Low-

speed

type

High-

speed

type

kfachine Lock Intervention during

Positioning to Intermediate

Pcx3itioning Point

41though positioning is continued .Othe intermediate positioning point position data display only), movementto the reference point is not jxecuted. Display data are not updated, either.

41though positioning is continued :0the intermediate positioning Joint, the position is displaced by .he machine lock intervention lmount.

Machine Lock Intervention during

Positioning to Reference Point

Display data are infinitely updated. Although positioning is made at the reference point after the detection of the actuation of the deceleration limit switch, this cannot be detected due to machine lock and, therefore, the display data are infinitely updated.

In response to the machine lock intervention, the axes stops moving. After that, the display data (position data in the workpiece coordinate system) are updated until the reference point return is completed. (withoot axis movement)

The axes move to the reference point (position data display is offset by the machine lock intervention amount).

Actual axis position is displayed due to the intervention of machine lock. Accordingly, although the display data (position data in the workpiece coordinate system) agree with the reference point, the axes are not located at the reference point.

● Before specifying I:heG28 command, the tool position offset mode and nose

R offset mode should be canceled. If the G28 command is specified without canceling these modes, they are canceled automatically.

c It is possible to select valid/invalid of reference point return for each axis. If

the axis for which “reference point return invalid” has been set is specified in the G28 block, alar-m “0241” occurs. Refer to parameter pm4002 DO to D4.

2-42

2.3 REFERENCEPOINTRETURN

● Itispossible todisplay aliirm`<0411'' (>C-axis) to`` 0415''(5th-axis) when an

axis move command other than G28 is executed without completing reference point return after turning ON the power. Whether or not such alarm display should be given is determined by the setting for parameter pm4022. The direction of reference point return is set for pm4002 DO to D4 for the individual axes.

● The absolute coordinate values of the axes specified in the G28block are saved

to memory as the intermediate positioning point. For the axes not specified in the G28 block, the intermediate positioning point saved in the previous reference point return operation remains valid.

● If M and/or T command is specified with G28 in the same b .ock, the axes con-

tinue moving to the reference point disregarding whether or not the FIN processing is completed before the positioning of an axis at the intermediate positioning point. Therefore, DEN is output at the reference IIoint.

● The deceleration limit switch position must be carefully attended to when

executing the reference point return for the first time after turning ON the power. For details, refer to 2.4.2, “Manual Reference Point Return” of the Operating Manual.

——..- .... .. .. .. . ........ . . .. ____ . .-__, r._.._... ._. —

2-43

-.+..--—.—...—..-.....-.——

—,. -.-. —- ——, ——. -..

.- ..-. .—

2.3.2 Reference Point Return Check (G27)

This function checks whether the axes are correctly returned to the reference point at the completion of the part program which is created so that the program starts and ends at the reference point in the machine by specifying the commands of “G27 X(U)” “ cZ(W)” “ o (* C(H) .00

In the G27 mode, the function checks whether or not the axes positioned by the execution of these commands in the simultaneous 2-axis (* 3-axis) control mode are located at the reference point. For the axes not specified in this block, positioning and check are not executed.

(1) Operation after the Check

When the position reached after the execution of the commands in the G27 block agrees with the reference point, the reference point return complete lamp lights. The automatic operation is continuously executed when all of the specified axes are positioned at the reference point. reference point return check: error (alarm “0421” (X-axis) to “0425” (5th-axis)) occurs and the automatic operation is interrupted. In this case, the cycle start lamp goes OFF.

* Y(V “ “ “);”.

If there is an axis that has not been returned to the reference point,

(2) Supplements to the Reference Point Return Check Command and Other

Operations

● If G27 is specified in the tool position offset mode, positioning is made at the

position displaced by the offset amount and the positioning point does not agree with the reference point. It is necessary to cancel the tool offset mode before specifying (327. Note that the tool position offset function is not canceled by the G27 command.

● The reference point return check is not executed if G27 is executed in the ma-

chine lock ON state.

c The mirror image function is valid to the direction of axis movement in the

reference point return operation called by G27. To avoid a position unmatch error, the mirror image function should be canceled by specif ying G69 (mirror image OFF) before executing G27.

2-44

2.3.3 Return from Reference Point Return (G29)

The commands of “G29 X ““. Z .0. ;“ ihe axes, having been returned to the reference point by the execution of the automatic reference point return function (G28, G30), to the intermediate positioning point by back tracing the paths along which the reference point return has been executed.

Example of Programming

2.3 REFERENCE POINT RETURN

G28 XOO” Z” O”;

“~

PointB

G29

Point A ~ B - C (Reference point)

Point C+B~D

Point D

Positioning in rapid traverse

.&””-

Fig. 2.36 Return from Reference Point

~!=

‘).=O.

i *

C (reference point)

Reference pclint returrl

B (Intermediate positioning point)

(1) Intermediate Positioning Point

● It is not possible to specify the intermediate positioning point in the G29 block.

The axes return to the previous point at a rapid traverse rate along the paths

taken in the return to the reference point. Note that the axes not specified in the G29 block do not move.

● If G28 or G30 (see :2.2.4, “Second to Fourth Reference Point Return (G30)*”)

has been executed several times before the execution of G29, point B to be set for the execution of B29 is established at the intermediate positioning point set in the last G28 or Gr30 operation. The following program written in absolute commands explains how point B is set for the return operation from the reference point.

Coordinate values of intermediate positioning point

N20 N23 N24

GOO

X30.Z20.; X-40.Z-50.;

GOO

G28 Zlo. Z20. (lo., 20.) G28 X30. ; G29

X-4C). Z-50. ;

(30., 20.)

‘~ ~n~point

Intermediate positioning point

End point

2-46

Example of Programming

N31 T0300; N32 G28 U80. W20.; N33 T0400; N34 G29

U-80. W40.;

—1—1——

2.3 REFERENCEP OINTRETURN

(reference point)

Intermediate

(absolute coordinate values)

Fig. 2.37

● In the following cases, the intermediate positioning point used for the execu-

Coordinate Values c]f Point B for G29 Operation

tion of G29 does not agree with the intermediate positioning point specified for the execution of G28 or G30. Therefore, do not specify such commands or attempt such operation.

. Execution of the following before the execution of G29 after the comple-

tion of G28:

positioning point

——-+Z

Coordinate system setting (G50 or coordinate system setting operation in POS. job) Intervention of machine lock Intervention of manual operation with manual absohte OFF

o Execution of G28, or G30 or G29 in a block specified after the cancellation

of the mirror image at a position different from the position where the mirror image was started.

. Execution of G28, or M:30 or M29 after the intervention of manual opera-

tion with the manual absolute OFF.

(2)

Supplements to the Return Command from the Reference Point Return

Automatic reference point return

(a)

If G29 is specified without the execution of G28 or G30 after turning ON the power, alarm “0240” occurs.

Nose R offset and canned cycle

(b)

If G29 is specified in the nose R offset mode (G41, G42) or in a canned cycle (G70 to G76, G90, G92, G94, G81 to G89), alarm “0170” or “0182” occurs.

Tool position offset

(c)

It is necessary to cancel the tool position offset function before specifying G28, G30, or G29. If these G codes are executed in the offset mode, the intermediate positioning point B’ is also offset, causing the tool to move to point B. Note that the tool position offset function is not canceled by G29.

C (reference point)

D’ ----4

b“

$“

Fig. 2.38 G29 Operation Executed

B’

,~ >~ ~’e’ ‘Ount

B (intermediate positioning point)

in the Tool Position Offset Mode

2-48

——1

2.3.4 Second to Fourth Reference Point F~eturn(G30) *

With the commands of “G30 Pn X(U) I o“ Z(W) “ “ . (* C(H) “ “ oY(V) ..0 );”, the axes are moved to P2 (second reference point), P3 (third reference point*), or P4 (fourth reference point*) in the simultaneous 3-axis (* 5-axis) control mode after the positi oning at the specified intermediate positioning point. If “G30 P3 U-40. ‘W30.;” is specifiecl, the X- and Z-axis return to the third reference point. If “Pn” is omitted, the second reference point is selected.

The axes not specified in the G30 block do not move.

Reference Point Positions

(1)

The position of each reference point is determined in reference to the first reference point. The distance from the first reference point to each of the reference points is set for the following parameters.

2,3 REFERENCE POINT RETURN

Table 2.16 Reference Points

X-axia Z-axis

2nd reference point 3rd reference point 4th referenee point

(2)

Supplements to the 2nd to 4th Reference Point Return Commands

● For the points to be considered to for the execution of G30, ~efer to the supple-

pm6811 pm6821 pm6822 pm6823 pm6831

pm6812 pm6813

pm6832 pm6833 pm6834 pm6835

3rd-axis

ments in 2.2.1, “Automatic Return to Reference Point (G2!8)”.

c If G29 is specified after G30, positioning is made at the point specified with

G29 after passing the intermediate positioning point specified with G30. Only the coordinate value of intermediate positioning point of the axis specified

with G30 is updated,

● For the execution of G30, reference point return must have been completed

after power-ON either manually or by the execution of G28. If an axis for which reference point return has not been completed is included in the axes specified in the G30 block, alarm “0240” occurs.

4th axis

prn6B14

pmi5824

5th-axis

pm6815 pm6825

... —-...—_ ..—.__..._. .. . .. ...___. _______ ._

.—______ .

2-49

——— ...-—— ———------- ———. .. .,.- ——... —. —.—.—

,—-—...

MOVEMENT CONTROL COMMANDS

Chapter 3 describes the procedure used for settilllg and selecting the coordinate system and the programming for con-

trolling the movement of a cutting tool.

3.1 SEl17NG THE COORDINATE

SYSTEM . . . . . . . . . . . . . . . . . . . . . . . . . ...3-3

3.1.1 Base Coordinate System (G50) . . . . . . . . . . . . 3-3

3.1.2 Workpiece Coordinate System

(G50T, G51)* . . . . . . . . . . . . . . . . . . . . . . . . . . . 3“7

3>2 DETERMINING THE COORDINATE

VALUE INPUT MODES . . . . . . . . . . . ...3- 16

3.2.1

3.2.2 Diametric and Radial Commands

3.2.3 Inch/Metric Input Designation (G20, G21!) , , 3-20

3.3 TIME-CONTROLLING COMMANDS , ..3-22

3.3.1

3.4 TOOL OFFSET FUNCTIONS . . . . . . . ..3-23

3,4.1 TooIOffeet Data Memory . . . . . . . . ,,, . . ...3-23

3.4.2

3.4.3 Nose R Offset Function (G40, G41/G42) * . . 3-29

Absolute/incremental Designation . . . . . , . . . 3-16

for X-axis . . . . . . . . . . . . . . . . . . . . . . . . . .,...3-19

Dwell (G04) . . . . . . . . . . . . . . . . . . . . . . . . . ...3-22

Tool Position Offset . . . . . . . . . . . . . . . . . . ...3-24

3.5 SPINDLE FUNCTION (S FUNCTION) .3-75

3.5.1

3.5.2

3.5.3

3.5.4

Spindle Command (S5-digit Command) . . . . 3-75

Maximum Spindle Speed Command

(G50S) . . . . . . . . . . . . . . . . . . . . . . . . . . . . ...3-76

Constant Surface Speed Control

(G96, G97)* . . . . . . . . . . . . . . . . . . . . . . . . . . .3-77

I<otary Tool Spindle Selection Function * . . . 3-81

3.6 TOOL FUNCTION (T FUNCTION) . . ...3-82

3.6.1

3.6.2

T4-digit Command. . . . . . . . . . . . . . . . . . . ...3-82

‘r6-digit Command* . . . . . . . . . . . . . . . . . . ...3-82

3.7 MISCELLANEOUS FUNCTION

(M FUNCTION) . . . . . . . . . . . . . . . . . . ...3-83

3.7.1 ItiCodes Relating to Stop Operation

(MOO, MOI, M02, M30) . . . . . . . . . . . . . . . ...3-83

3.7.2

3.7.3

Internally Processed M Codes . . . . . . . . . . . . 3-84

General Purpose M Codes...,,. . . . . . . . . . 3-85

3-2

3.1 SElllNG THE COORDINATE SYSTEMI

3.1.1 Base Coordinate System (G50)

Before programming axis movement, a coordinate system must be set. “Nhen a coordinate system is set, a single absolute coordinate system is determined and absolute move commands specified after the setting of a coordinate system are all executed ill it. The G50 command sets the position of the origin of a coordinate system used for programming.

G50 is a non-modal G code that is valid (only in the specified block. The block in which the G50 command is specified must not contain other G codes, M codes, S codes, and T codes. Especially, if an S or T code is specified in a block with G50- like “G50 S” o “;“ or “G50T “ “ “

(1)

;“, such designation calls specific functions and does not set a coordinate system.

Commands

3.1 SEITING THE CCIORDINAT’E SYSTEM

For setting a coordinate system, both absolute and incremental comnlands may be used.

Coordinate system setting in absolute commands

(a)

With the commands of “G50 X. 0.0 Z “ “ “

(“c... *Y”. “) ;“, a coordinate system is set so that the present tool nose position has the absolute coordinate values specified in the G50 block (X, Z, C, B*, Y *). In other words, the addresses in the G50 block specify the distance from the point that should be set as the origin (O, O,O)of the coordinate system used for progmmming to the present tool nose position. Axis movement commands can be specified for up to 2 aces (* 5 axes max.) simultaneous y. Note that the axes not specified the G50 block do not move.

An example of coordinate system setting is shown in Fig. 3.1. In this example, the coordinate system is set at the position where reference poilnt return has been executed. A coordinate system can be set at any position.

Present tool nose

position

1.1

coordinate system

Fig. 3.1

Setting of Base Cc)ordinate System (G50) at Reference Return Position

3-3

—.. ——-. ——___. ——.. —......- .—.— .—.. -.. -———-—— --

Coordinate system setting in incremental commands

(b)

If addresses U, W, and IHare specified with the commands of “G50 X “ .0 Z o c . (* H... *VCO

o) ;“, a new coordinate system is set in reference to the present coordinate system by shifting it the distance specified in incremental values of U (X-axis direction), W (Z-axis direction), and H (C-axis direction).

This feature is effectively used in several applications - an operation that uses cutting tools having considerable differences, for example. In this case, the cutting tools should first be divided into two groups and the difference between the length of standard tool in one group and that in the other group should be entered in a program. Then, a new base coordinate system can be set for the second tool group.

Example of programming

G50 U1OO. W- 100.;

Fig. 3,2

(2)

Coordinate System and 100 I Position Offset

Setting of Coordinate System with Incremental Values

‘fpo.itiono~%’i’h5:’didtool

-+,

After setting the coordinate system by executing the commands of “G50 X80. Z62.;” taking the cutting tool No. 0“1,if the cutting tool No. 02 which has the tool position offset amount as shown in Fig. 3.3 is selected and offset is executed, the cutting tool No, 02 moves to point A.

Example of Programming

N3 G50 X80. Z62.; N4 GOO TO1O1;

●

N1O GOOT0202;

●

‘+ti~o’’oo’

G50 comma;d with No. 02 tool selected

= 40 mm

Fig. 3.3

Coordinate System and Tool Position Offset

As shown in Fig. 3.3, if the coordinate system is set in reference to the standard tool and offset data are set for other tools, it is possible to program all tool movements in a single coordinate system.

3-4

\\ I/,

POINT

3.1 SEITING THE CCIORDINATE SYSTEM

Automatic Coordinate System Setting

(3)

It is possible to set a coordinate system automatically at the completion of manual reference point return. To set the coordinate system in this manner, the sel:ting values should be set for parameters for each of mm and inch input operation as irndicated below.

Table 3.1 Parameters for “mm” Input and “inch” Input

3. Whether or not the automatic coordinate system setting functio:n is made valid

or not should be set for parameters pm4006 DO to D4 for the individual axes.

4. To use the workpiece coordinate system shift function, set the cocn-dinate system by adding the workpiece coordinate system shift values to the coordinate system setting values when setting the coordinates ystem using the autom atic coordinate system setting function.

5. The coordinate system that has been set using the automatic coordinate system

setting function becomes invalid when other coordinate system setting function such as G50 is executed.

.—. — —-- -—.——. — .——

3-5

.-. __, — .-_ —... _______ .—_—

.——.-——— ..- ,— ._-. _______

(4) Supplements to the Base Coordinate System Commands

. If a T code is specified in the block next to the one in which the G50 command

is specified, it is necessary to enter GOOin the block where the T code is specified to define the offset movement feedrate.

G50Xoo” Zo -.;

GOO S500 M03 TO1O1;

● Cancel the tool position offset and nose R offset function before specifying

G50.

● When the power is turned ON, coordinate values (O,O,O)is set for the present

tool position. Therefore, the coordinate system must always be set before starting an operation. Concerning the C-axis integral with the spindle, use the automatic coordinate system setting function - change the mode to the C-axis control and execute the reference point return, and the coordinate system is set for the C-axis at the position where the reference point return has been completed.

● Once the coordinate system is set, it is not influenced by the reset operation.

To reset the coordinate system, use either of the following operation.

“ To set “O” on the [ABS] function screen. “ To set “O”for the coordinate values by executing “G50 XO ZO(CO);” in the

MDI mode.

“ To turn OFF the power once and turn it ON again.

o The present tool position in the base coordinate system is displayed on the

[AIM] function name which is called in the [POSIT.] job.

● Whether or not the workpiece coordinate shift is valid when G50 is specified

is determined by the setting for parameter pm4012 DO.

3-6

3.1.2 Workpiece Coordinate System (GsOT, Gsl ) *

The function to set workpiece coordinate systems is provided to set the coordinate system for the individual cutting tools so that the program can be executed at the :same program origin even if the cutting tool to be used is changed by the tool selection operation.

(1) Tool Coordinate Data Memory (Number)

Before specifying “GSOT” commarid, it is necessary to write the cocxdinate data to the tool coordinate data memory for each of the cutting tools.

(a) Tool coordinate data memory

3.1 SETrlNG THE CCIORDINATE SYSTEM

The number of tool coordinate data memory areas corresponds to the number of

tool offset data memory area pairs. See Table 3.2.

Table 3.2 Tool Coordinate Data Memory

Number of Tool Offset Data Memory Area

Tool coordinate data memory numbers and tool numbers

(b)

Pairs

When Oto 16

When Ot 50

Tool Coordinate

Ddi~ Memory Areas

(Number)

51 to 66 (I6 areas) 51 to 99 (4!)areas)

---i

Tool coordinate data memory number “51” corresponds to tool rmmber’’Ol”. Sim-

ilarl y, tool coordinate data memory number” 52” corresponds to tool number “02”, and so on.

Table 3.3 Correspondence between Tool Coordinate Dat:~ Memory Num-

bers and Tool Numbers

Tool Coordinate

Memory No.

Data

51 52

Tool No,

01 02

3-7

The coordinate data (Xtn, Ztn) as shown in Fig. 3.4 are written to the tool coordinate data memory for the individual tools Tn.

‘X*H

Ae-

f >

(L 7, i 4

The workpiece coordinate system determined

by the operator at the workpiece measurement

value direct input operation.

Fig. 3.4 Tool Coordinate Data Memory

/’

At,,

Workpiece

The tool post or turret is at the position where the CNC’S present position data display is (O,0).

‘xtn/2

3-8

3.1 SEITING THE CCIORDINATE SYSTEM

(2) Commands

(a) Features of G50T and G51

Table 3.4 G Codes Related to Workpiece Coordinate Systsm

Setting a workplece coordinate system

=“’0”” %+

The G50T and G51 commands are both non-modal and valid o]dy in the specified block.

(b) Setting a workpiece coordinate system

G50T ❑ 0 AA;

A workpiece coordinate system is set by using the comrnaml format indicated

above; the value calculated in the following formula is used as the setting value of

the workpiece coordinate system. Workpiece coordinate system setting value

= [Present position display value in the NC]

+ [Value set at the specified tool coordinate data memory area] + [Value set at the specified tool offset memory area]

Here, the “present position display value in the NC” indicates t~llevalue displayed at the [EXTERN] function in the [POSIT.] job.

Return to the origin for present value display

~ Toed offset number designation (00 to 50)

Toc,l coordinate value memory number designation (51 to 99)

———-. ... ———. ——

● In normal operation, “00” should be set for A A (tool offset number designa-

tion part).

Example: G50 T51OO ;

3-9

..— ..——.. -—.. . .. . ......... . . ... -— ——— —.. —.,—..

If “00” is set, a workpiece coordinae system is set assuming that the data set in the tool offset memory area is “0.

.- ,—— —.. —.—

-—.

When the program as indicated in the example above is set when the tool post or turret is positioned at arbitrary position, the workpiece coordinate system that the operator has determined is set correctly.

T1 when the turret or tool post is positioned at an arbitrary position (-x, -z)

)

z~l

{ \ #

(L \

Workpiece coordinate system

Fig. 3.5

● With the commands of “G50 TOOOO;”,the workpiece coordinate system is

Workpiece Coordinate System Setting

-z

/ (-x/2) +x!, /2

(-z) +z~,

When the turret or tool post is positioned at (O,O)

- +Z

The workpiece coordinate is set using these values.

}

canceled. That is, the command TOOOOcauses the calculation of the present

position data with “value in tool coordinate data memory = O“ and “value in

tool offset data memory = O“ to set the workpiece coordinate system.

Returning to the origin for present position (G51 )

(c)

system

With arnachiningprograrn that uses the workpiece coordinate system setting function, the start point of machining should be set at the position where the present position data display is (,0,O). Therefore, after the completion of machining, G51

must be specified in the program so that the X- and Z-axis return to the start point of machining accurately. With theG51 command, both of the X- and Z-axis return to the start point at a rapid traverse. Note that G51 should be specified in a block independently without other commands.

3-1o

3.1 SElllNG THE COORDINATE SYSTEM

(3) Example of Programs

(a) Example program using a workpiece coordinate system

An example of program in which a workpiece coordinate systl>m is used is given

below.

The start point of machining is (O,O) of present position display.

N1 G50 T51OO; ~

N2 GOOTO1O1 M03 S1OO; ~

(Machining using tool No. 01)

Setting of a workpiece coordinate system for tool No. 01

Selection of tool No. 01 (Note)

N20

GOOXC”” ZO”” -

N21

G50 T5200; _

N22

GOO T0202; —

Positioning Setting of a workpiece coordinate system for

tool No. 02 Selection of tool No. 02 (Note)

(Machining using tool No. 02)

N40

G51; c

T02

Returning to the point of (O,O) (present position data display)

Position where position data display is (O,O)

N20

Workpiece coordinate system

(Machining with tool NCE. 01 and 02 is programmed in this coordinate system)

Note: The tool position offset command in TOIC1 and T0202 can be used for the compensaticln for tool wear. [t can also

be used for offsetting in taper cutting.

Fig. 3.6 Example Program Using Workpiece Coordinate Systelm

3-11

(b) Example of program in which operation in a workpiece coordinate system

is interrupted

If an operation is restarted from the beginning of the program without returning the cutting tool to the start point of machining after the interruption of the program given below, the cutting tool is positioned correctly at the first approach position.

Example of program in which operation in a workpiece coordinate system is interrupted

N1 G50 T51OO; N2 TO1O1; N3 G96 S150 M03; N4 GOO X20. Z2.5;

When the operation is restarted from the position

of (-20., -27.5) after the interruption

+-A

Workpiec~ coordinate system

A Approach position (20., 2.5)

(TooI coordinate data memory 51X= 80.

Machining start position = Present position data display (O,O)

51Z = 40.)

Fig. 3.7 Example of program in which operation in a workpiece coordinate

system is interrupted

The commands of “N1 (350 T51OO;” executed at point B sets a workpiece coordinate system using the values of X = 60. (-20. + 80.) and Z = 12.5 (-27.5 + 40.). Therefore, the workpiece coordinate system is saved and, accordingly, the approach position point A remains unchanged.

3.1 SEITING THE COORDINATE SYSTEM

An example of program and workpiece coordinates ystem setti ng values are indicated below for cases where tool change position differs by tclols.

Table 3,5 Tool Coordinate Data Memory

N1 G50 T51OO; N2 GOOTO1O1 M03 S1OOO;

“ (Machining with TO1)

N25 G50 TOOOO; N26 GOOX-50. Z-35.;

N27 G50 T5200; N28 GOO T0202 M03 S800;

. The coordinate system setting values used

“ (Machining with T02)

N48 G51;

z = 5“ T02

# 0100.

‘z

~. \--

$110.

47,5 Tol

J’f’

TO1

— Tool changepositionto

by these commands are: X= (-50.) + 110. =60. z = (-35.) + 40. = 5,

T02

Machining start position = Position where present position clata is (O,O)

i.-

-50./2

-35. -

T02 is (-50,, -35.).

X = 4J60.

+ +Z

Workpiece coordinate system

Fig. 3.8 If Tool Change Positions Differ in a Workpiece Coordinate System

(4) Workpiece Coordinate System Shift Amount

The coordinate system that is set using G50 or the workpiece coordinate system setting

function can be shifted by the required distance. It is possible to write the shift distance to the workpiece coordinate system shift data memory, which is No. 00 of the offset data

memory data, for the X-, Z- and C-axis in the same operation as writing the tool offset

data.

(a) Shift data written to the memory

The shift data written to the memory becomes valid at the following timing:

● Execution of the G50 coordinate system setting command

. Execution of the G50 T workpiece coordinate system setting command Q Execution of the automatic coordinate system setting function

● Execution of key operation for setting the coordinate system.

When any of the operation indicated above is executed, a coordinate system is set by simply adding the set shift amount. No cutting tool movement takes place. If

a positive value is set for AX, AZ, and AC, the coordinate system is shifted in

the direction indicated by the arrow symbol in Fig. 3.9. In this figure, ~ and Z. indicate the original coordinate system setting values.

+x +x

-tz ~ XO12

~m-

Shift

t AX/2 I

Originel coordinate system

+.p.+z

Coordinate system set after the shift

Fig. 3.9 Workpiece Coordinate System Shift Operation

The direction in which the coordinate system should be shifted can be changed by

changing the setting fclr parameter pm4012 D3. By setting DO, it is possible to make the shift amount invalid at the execution of G50.

yaskawa J300L Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

CONTENTS

PROGRAMMING BASICS

MOVEMENT CONTROL COMMANDS