Omron NY532-5400, NJ501-5300 Installation Manual

Machine Automation Controller
Industrial PC Platform

NJ/NY-series

G code
Instructions Reference Manual

NJ501-5300
NY532-5400

O031-E1-02

NOTE

All rights reserved. No part of this publication may be reproduced, stored in a retrieval system, or transmitted, in
any form, or by any means, mechanical, electronic, photocopying, recording, or otherwise, without the prior
written permission of OMRON.

No patent liability is assumed with respect to the use of the information contained herein. Moreover, because
OMRON is constantly striving to improve its high-quality products, the information contained in this manual is
subject to change without notice. Every precaution has been taken in the preparation of this manual. Neverthe­less, OMRON assumes no responsibility for errors or omissions. Neither is any liability assumed for damages
resulting from the use of the information contained in this publication.

Trademarks

• Sysmac and SYSMAC are trademarks or registered trademarks of OMRON Corporation in Japan and other
countries for OMRON factory automation products.

• Microsoft, Windows, Excel, and Visual Basic are either registered trademarks or trademarks of Microsoft Corpora­tion in the United States and other countries.

• EtherCAT® is registered trademark and patented technology, licensed by Beckhoff Automation GmbH, Germany.

• ODVA, CIP, CompoNet, DeviceNet, and EtherNet/IP are trademarks of ODVA.

• The SD and SDHC logos are trademarks of SD-3C, LLC.

• Intel and Intel Core are trademarks of Intel Corporation in the U.S. and / or other countries.

Other company names and product names in this document are the trademarks or registered trademarks of their
respective companies.

Copyrights

Microsoft product screen shots reprinted with permission from Microsoft Corporation.

Introduction

Thank you for purchasing an NJ/NY-series NC Integrated Controller. (“NJ/NY-series NC Integrated
Controller” is sometimes abbreviated as “NC Integrated Controller”.)

This manual contains information that is necessary to use the NC Integrated Controller. Please read
this manual and make sure you understand the functionality and performance of the NC Integrated
Controller before you attempt to use it in a control system.

Keep this manual in a safe place where it will be available for reference during operation.

This manual only describes functions that are added to NJ501-5300 or NY532-5400.

When you use NJ501-5300, also consult manuals for the NJ-series listed in Related Manuals on page
21 for functions common to NJ501- Series including NJ501-1.

When you use NY532-5400, also consult manuals for the NY-series listed in Related Manuals on page
21 for functions common to NY532- Series including NY532-1.

Introduction

Intended Audience

This manual is intended for the following personnel, who must also have knowledge of electrical sys­tems (an electrical engineer or person with equivalent skills).

- Personnel in charge of introducing FA systems

- Personnel in charge of designing FA systems

- Personnel in charge of installing and maintaining FA systems

- Personnel in charge of managing FA systems and facilities

This manual is also intended for personnel who understand the following contents.

• For programming, this manual is intended for personnel who understand the programming language
specifications in international standard IEC 61131-3 or Japanese standard JIS 3503.

• For NC programming, this manual is intended for personnel who understand the programming lan­guage specifications in international standard ISO 6983-1 or Japanese standard JIS 6315.

Applicable Products

This manual covers the following products.

• NJ-series NC Integrated Controller

NJ501-5300

• NY-series NC Integrated Controller

NY532-5400

NJ/NY-series G code Instructions Reference Manual (O031)

1

Relevant Manuals

Relevant Manuals

The following table lists the relevant manuals for this product. Read all of the manuals that are relevant
to your system configuration and application before you use this product.

Most operations are performed from the Sysmac Studio and CNC Operator Automation Software.

Refer to the Sysmac Studio Version 1 Operation Manual (Cat. No. W504) for information on the Sys-
mac Studio, and CNC Operator Operation Manual (Cat. No. O032) for the CNC Operator.

Relevant Manuals for NJ Series

Basic information

NJ-series CPU Unit

Hardware User’s Manual

Manual

NJ/NX-series CPU Unit Built-in

NJ/NX-series CPU Unit

Software User’s Manual

NJ/NX-series Instructions

Reference Manual

NJ/NX-series CPU Unit Motion

Control User’s Manual

Instructions Reference Manual

NJ/NX-series Motion Control

EtherCAT

NJ/NX-series CPU Unit Built-in

EtherNet/IP™ Port User’s Manual

NJ/NY-series NC Integrated

Controller User’s Manual

NJ/NY-series G code

Instructions Reference Manual

NJ/NX-series

Troubleshooting Manual

®

Port User’s Manual

Purpose of use

Introduction to NJ-series Controllers 

Setting devices and hardware

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Software settings

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using numerical control 

Writing the user program

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using numerical control 

Programming error processing 

Testing operation and debugging

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using numerical control 









2

NJ/NY-series G code Instructions Reference Manual (O031)

Purpose of use

Basic information

NJ-series CPU Unit

Hardware User’s Manual

NJ/NX-series CPU Unit

Software User’s Manual

Relevant Manuals

Manual

NJ/NX-series Instructions

Reference Manual

NJ/NX-series CPU Unit Motion

Control User’s Manual

NJ/NX-series Motion Control

Instructions Reference Manual

NJ/NX-series CPU Unit Built-in

EtherCAT

®

Port User’s Manual

EtherNet/IP™ Port User’s Manual

NJ/NX-series CPU Unit Built-in

NJ/NY-series NC Integrated

Controller User’s Manual

NJ/NY-series G code

Instructions Reference Manual

NJ/NX-series

Troubleshooting Manual

Learning about error management and

corrections

Maintenance

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

*1. Refer to the NJ/NX-series Troubleshooting Manual (Cat. No. W503) for the error management concepts and the error items. However,

refer to the manuals that are indicated with triangles () for details on errors corresponding to the products with the manuals that are
indicated with triangles ().

*1



 

NJ/NY-series G code Instructions Reference Manual (O031)

3

Relevant Manuals

Relevant Manuals for NY Series

Basic information

NY-series Industrial Panel PC

Hardware User’s Manual

Purpose of use

NY-series Industrial Box PC

Hardware User’s Manual

Manual

NY-series Industrial Panel PC / Industrial Box PC

Setup User’s Manual

Software User’s Manual

NY-series Industrial Panel PC / Industrial Box PC

NY-series

Instructions Reference Manual

Motion Control User’s Manual

NY-series Industrial Panel PC / Industrial Box PC

NY-series Motion Control

Instructions Reference Manual

NY-series Industrial Panel PC / Industrial Box PC

Built-in EtherCAT Port User’s Manual

Built-in EtherNet/IP Port User’s Manual

NY-series Industrial Panel PC / Industrial Box PC

NJ/NY-series

NC Integrated Controller User’s Manual

G code Instructions Reference Manual

NJ/NY-series

Troubleshooting Manual

NY-series

Introduction to NY-series Panel PCs 

Introduction to NY-series Box PCs 

Setting devices and hardware 

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Making setup

Making initial settings

Preparing to use Controllers

Software settings

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using numerical control 

Writing the user program

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using CNC functions 

Programming error processing 

Testing operation and debugging

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

Using numerical control 

Learning about error management and

corrections

Maintenance

Using motion control 

Using EtherCAT 

Using EtherNet/IP 

*1

*2











 



*1. Refer to the NY-series Industrial Panel PC / Industrial Box PC Setup User’s Manual (Cat. No. W568) for how to set up

and how to use the utilities on Windows.

*2. Refer to the NY-series Troubleshooting Manual (Cat. No. W564) for the error management concepts and the error items.

However, refer to the manuals that are indicated with triangles () for details on errors corresponding to the products with
the manuals that are indicated with triangles ().

4

NJ/NY-series G code Instructions Reference Manual (O031)

Manual Structure

4-9

4 Installation and Wiring

NJ-series CPU Unit Hardware User’s Manual (W500)

stinUgnitnuoM3-4

4

stnenopmoCrellortnoCgnitcennoC1-3-4

4-3 Mounting Units

The Units that make up an NJ-series Controller can be connected simply by pressing the Units together
and locking the sliders by moving them toward the back of the Units. The End Cover is connected in the
same way to the Unit on the far right side of the Controller.

1 Join the Units so that the connectors fit exactly.

2 The yellow sliders at the top and bottom of each Unit lock the Units together. Move the sliders

toward the back of the Units as shown below until they click into place.

Precautions for Correct UsePrecautions for Correct Use

4-3-1 Connecting Controller Components

Connector

Hook

Hook holes

Slider

Lock

Release

Move the sliders toward the back
until they lock into place.

Level 1 heading
Level 2 heading
Level 3 heading

Level 2 heading

A step in a procedure

Manual name

Special information

Level 3 heading

Page tab

Gives the current
headings.

Indicates a procedure.

Icons indicate
precautions, additional
information, or reference
information.

Gives the number
of the main section.

The sliders on the tops and bottoms of the Power Supply Unit, CPU Unit, I/O Units, Special I/O
Units, and CPU Bus Units must be completely locked (until they click into place) after connecting
the adjacent Unit connectors.

Page Structure and Symbols

The following page structure and symbols are used in this manual.

Manual Structure

Note This illustration is only provided as a sample. It may not literally appear in this manual.

NJ/NY-series G code Instructions Reference Manual (O031)

5

Manual Structure

Precautions for Safe Use

Precautions for Correct Use

Additional Information

Version Information

Special Information

Special information in this manual is classified as follows:

Precautions on what to do and what not to do to ensure safe usage of the product.

Precautions on what to do and what not to do to ensure proper operation and performance.

Additional information to read as required.

This information is provided to increase understanding and ease of operation.

Information on differences in specifications and functionality for NC Integrated Controller with
different unit versions and for different versions of the Sysmac Studio and the CNC Operator
are given.

Note References are provided to more detailed or related information.

6

NJ/NY-series G code Instructions Reference Manual (O031)

1

2

3

4

A

1

2

3

4

A

Basic Information on NC Programming

G Code

M Code

PROGRAM CODES

Appendices

Sections in this Manual

Sections in this Manual

NJ/NY-series G code Instructions Reference Manual (O031)

7

CONTENTS

CONTENTS

Introduction ..............................................................................................................1

Intended Audience....................................................................................................................................... 1

Applicable Products..................................................................................................................................... 1

Relevant Manuals .....................................................................................................2

Relevant Manuals for NJ Series .................................................................................................................. 2

Relevant Manuals for NY Series.................................................................................................................. 4

Manual Structure ......................................................................................................5

Page Structure and Symbols....................................................................................................................... 5

Special Information...................................................................................................................................... 6

Sections in this Manual ...........................................................................................7

Terms and Conditions Agreement ........................................................................12

Warranty, Limitations of Liability ................................................................................................................ 12

Application Considerations ........................................................................................................................ 13

Disclaimers ................................................................................................................................................ 13

Safety Precautions .................................................................................................14

Precautions for Safe Use....................................................................................... 15

Precaution for Correct Use....................................................................................16

Regulations and Standards...................................................................................17

Versions ..................................................................................................................18

Checking Versions..................................................................................................................................... 18

Related Manuals .....................................................................................................21

Terminology ............................................................................................................ 24

Revision History .....................................................................................................25

Section 1 Basic Information on NC Programming

Instructions ............................................................................................................................................... 1-2

Instruction Parameters.............................................................................................................................. 1-5

G Code Descriptions.................................................................................................................................1-7

What is Modal?......................................................................................................................................... 1-9

Section 2 G Code

Interpolation Functions.................................................................................................................. 2-3

G00 Rapid Positioning.............................................................................................................................. 2-4

G01 Linear Interpolation ...........................................................................................................................2-6

G02, G03 Circular Interpolation................................................................................................................2-8

G31 Skip Function ..................................................................................................................................2-13

Dwell .............................................................................................................................................. 2-15

G04 Dwell ...............................................................................................................................................2-16

Feed Functions ............................................................................................................................. 2-17

Feedrate Function (F function) ............................................................................................................... 2-18

8

NJ/NY-series G code Instructions Reference Manual (O031)

CONTENTS

Acceleration Time, Deceleration Time, Jerk Time .................................................................................. 2-19

G09 Exact Stop ...................................................................................................................................... 2-20

G61 Exact Stop Mode ............................................................................................................................ 2-21

G64 Continuous-path Mode ................................................................................................................... 2-22

G500, G501 Multi-block Acceleration/Deceleration Rate ....................................................................... 2-24

Coordinate System ....................................................................................................................... 2-27

G52 Local Coordinate System Set......................................................................................................... 2-28

G53 Dimension Shift Cancel .................................................................................................................. 2-29

G54 to G59 Select Work Coordinate System......................................................................................... 2-30

G17, G18, G19 Plane Selection............................................................................................................. 2-31

G20 Inch Input, G21 Metric Input ........................................................................................................... 2-32

G90 Absolute Dimension, G91 Incremental Dimension ......................................................................... 2-33

Reference Point ............................................................................................................................ 2-35

G28 Return to Reference Point.............................................................................................................. 2-36

G30 Return to 2nd, 3rd and 4th Reference Point................................................................................... 2-38

Compensation Functions............................................................................................................. 2-39

G40, G41, G42 Cutter Compensation.................................................................................................... 2-40

G43, G44, G49 Tool Offset..................................................................................................................... 2-51

G50, G51 Scaling................................................................................................................................... 2-53

G50.1, G51.1 Mirroring........................................................................................................................... 2-55

G68, G69 Coordinate System Rotation.................................................................................................. 2-57

Utilities........................................................................................................................................... 2-59

G74 Left-handed Tapping Cycle ............................................................................................................. 2-60

G80 Fixed Cycle Cancel......................................................................................................................... 2-62

G84 Tapping Cycle ................................................................................................................................. 2-63

G98 Fixed Cycle Return to Initial Level .................................................................................................. 2-66

G99 Fixed Cycle Return to R Point Level............................................................................................... 2-67

Chamfer and Fillet Functions ................................................................................................................. 2-68

Section 3 M Code

Auxiliary Function Output.............................................................................................................. 3-3

M Code Descriptions................................................................................................................................ 3-5

Reservation Auxiliary Functions ................................................................................................... 3-7

M00 Program Stop ................................................................................................................................... 3-8

M01 Optional Stop.................................................................................................................................... 3-9

M02, M30 End of Program ..................................................................................................................... 3-10

Spindle Axis .................................................................................................................................. 3-11

Spindle Axis Rotation Function (S function)........................................................................................... 3-12

M03 Spindle CW .................................................................................................................................... 3-13

M04 Spindle CCW.................................................................................................................................. 3-14

M05 Spindle OFF ................................................................................................................................... 3-15

M19 Spindle Orientation......................................................................................................................... 3-16

Programming ................................................................................................................................ 3-19

M98 Subprogram Call ............................................................................................................................ 3-20

M99 Subprogram End ............................................................................................................................ 3-21

Section 4 PROGRAM CODES

4-1 Calculation and Logic Operation ......................................................................................... 4-2

4-1-1 Operator priority.......................................................................................................................... 4-2

4-1-2 Arithmetic operators.................................................................................................................... 4-2

4-1-3 Functions .................................................................................................................................... 4-3

4-1-4 Condition comparators................................................................................................................ 4-5

4-1-5 Conditional join operators........................................................................................................... 4-5

4-2 Branch and Repetition .......................................................................................................... 4-6

4-2-1 if/else .......................................................................................................................................... 4-6

4-2-2 switch/case ................................................................................................................................. 4-6

NJ/NY-series G code Instructions Reference Manual (O031)

9

CONTENTS

4-2-3 while............................................................................................................................................4-6

4-2-4 do/while....................................................................................................................................... 4-6

4-3 User Variables........................................................................................................................ 4-7

4-3-1 Local Variables (“L”) ....................................................................................................................4-7

4-3-2 Coordinate System Global Variables (“Q”).................................................................................. 4-7

4-3-3 Global Variables (“P”) ..................................................................................................................4-7

4-3-4 Variable Indirection......................................................................................................................4-7

Appendices

A-1 Program Parsing by CNC Operator .....................................................................................A-2

A-1-1 Intermediate code format ............................................................................................................A-2

A-1-2 Program Parsing Example ..........................................................................................................A-4

10

NJ/NY-series G code Instructions Reference Manual (O031)

CONTENTS

NJ/NY-series G code Instructions Reference Manual (O031)

11

Terms and Conditions Agreement

Terms and Conditions Agreement

Warranty, Limitations of Liability

Warranties

 Exclusive Warranty

Omron’s exclusive warranty is that the Products will be free from defects in materials and workman­ship for a period of twelve months from the date of sale by Omron (or such other period expressed in
writing by Omron). Omron disclaims all other warranties, express or implied.

 Limitations

OMRON MAKES NO WARRANTY OR REPRESENTATION, EXPRESS OR IMPLIED, ABOUT
NON-INFRINGEMENT, MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE OF
THE PRODUCTS. BUYER ACKNOWLEDGES THAT IT ALONE HAS DETERMINED THAT THE
PRODUCTS WILL SUITABLY MEET THE REQUIREMENTS OF THEIR INTENDED USE.

Omron further disclaims all warranties and responsibility of any type for claims or expenses based
on infringement by the Products or otherwise of any intellectual property right.

 Buyer Remedy

Omron’s sole obligation hereunder shall be, at Omron’s election, to (i) replace (in the form originally
shipped with Buyer responsible for labor charges for removal or replacement thereof) the non-com­plying Product, (ii) repair the non-complying Product, or (iii) repay or credit Buyer an amount equal
to the purchase price of the non-complying Product; provided that in no event shall Omron be
responsible for warranty, repair, indemnity or any other claims or expenses regarding the Products
unless Omron’s analysis confirms that the Products were properly handled, stored, installed and
maintained and not subject to contamination, abuse, misuse or inappropriate modification. Return of
any Products by Buyer must be approved in writing by Omron before shipment. Omron Companies
shall not be liable for the suitability or unsuitability or the results from the use of Products in combi­nation with any electrical or electronic components, circuits, system assemblies or any other materi­als or substances or environments. Any advice, recommendations or information given orally or in
writing, are not to be construed as an amendment or addition to the above warranty.

See http://www.omron.com/global/ or contact your Omron representative for published information.

Limitation on Liability; Etc

OMRON COMPANIES SHALL NOT BE LIABLE FOR SPECIAL, INDIRECT, INCIDENTAL, OR CON­SEQUENTIAL DAMAGES, LOSS OF PROFITS OR PRODUCTION OR COMMERCIAL LOSS IN ANY
WAY CONNECTED WITH THE PRODUCTS, WHETHER SUCH CLAIM IS BASED IN CONTRACT,
WARRANTY, NEGLIGENCE OR STRICT LIABILITY.

Further, in no event shall liability of Omron Companies exceed the individual price of the Product on
which liability is asserted.

12

NJ/NY-series G code Instructions Reference Manual (O031)

Application Considerations

Suitability of Use

Omron Companies shall not be responsible for conformity with any standards, codes or regulations
which apply to the combination of the Product in the Buyer’s application or use of the Product. At
Buyer’s request, Omron will provide applicable third party certification documents identifying ratings
and limitations of use which apply to the Product. This information by itself is not sufficient for a com­plete determination of the suitability of the Product in combination with the end product, machine, sys­tem, or other application or use. Buyer shall be solely responsible for determining appropriateness of
the particular Product with respect to Buyer’s application, product or system. Buyer shall take applica­tion responsibility in all cases.

NEVER USE THE PRODUCT FOR AN APPLICATION INVOLVING SERIOUS RISK TO LIFE OR
PROPERTY OR IN LARGE QUANTITIES WITHOUT ENSURING THAT THE SYSTEM AS A WHOLE
HAS BEEN DESIGNED TO ADDRESS THE RISKS, AND THAT THE OMRON PRODUCT(S) IS
PROPERLY RATED AND INSTALLED FOR THE INTENDED USE WITHIN THE OVERALL EQUIP­MENT OR SYSTEM.

Terms and Conditions Agreement

Programmable Products

Omron Companies shall not be responsible for the user’s programming of a programmable Product, or
any consequence thereof.

Disclaimers

Performance Data

Data presented in Omron Company websites, catalogs and other materials is provided as a guide for
the user in determining suitability and does not constitute a warranty. It may represent the result of
Omron’s test conditions, and the user must correlate it to actual application requirements. Actual perfor­mance is subject to the Omron’s Warranty and Limitations of Liability.

Change in Specifications

Product specifications and accessories may be changed at any time based on improvements and other
reasons. It is our practice to change part numbers when published ratings or features are changed, or
when significant construction changes are made. However, some specifications of the Product may be
changed without any notice. When in doubt, special part numbers may be assigned to fix or establish
key specifications for your application. Please consult with your Omron’s representative at any time to
confirm actual specifications of purchased Product.

Errors and Omissions

Information presented by Omron Companies has been checked and is believed to be accurate; how­ever, no responsibility is assumed for clerical, typographical or proofreading errors or omissions.

NJ/NY-series G code Instructions Reference Manual (O031)

13

Safety Precautions

Safety Precautions

Refer to the following manuals for safety precautions.

• NJ-series CPU Unit Hardware User’s Manual (Cat. No. W500)

• NY-series Industrial Panel PC Hardware User’s Manual (Cat. No. W557)

• NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030)

• CNC Operator Operation Manual (Cat. No. O032)

14

NJ/NY-series G code Instructions Reference Manual (O031)

Precautions for Safe Use

Refer to the following manuals for precautions for safe use.

• NJ-series CPU Unit Hardware User’s Manual (Cat. No. W500)

• NY-series Industrial Panel PC Hardware User’s Manual (Cat. No. W557)

• NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030)

• CNC Operator Operation Manual (Cat. No. O032)

Precautions for Safe Use

NJ/NY-series G code Instructions Reference Manual (O031)

15

Precaution for Correct Use

Precaution for Correct Use

Refer to the following manuals for precautions for correct use.

• NJ-series CPU Unit Hardware User’s Manual (Cat. No. W500)

• NY-series Industrial Panel PC Hardware User’s Manual (Cat. No. W557)

• NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030)

• CNC Operator Operation Manual (Cat. No. O032)

16

NJ/NY-series G code Instructions Reference Manual (O031)

Regulations and Standards

Refer to the following manuals for regulations and standards.

• NJ-series CPU Unit Hardware User’s Manual (Cat. No. W500)

• NY-series Industrial Panel PC Hardware User’s Manual (Cat. No. W557)

Regulations and Standards

NJ/NY-series G code Instructions Reference Manual (O031)

17

Versions

Versions

Hardware revisions and unit versions are used to manage the hardware and software in NJ/NY-series
Units and EtherCAT slaves. The hardware revision or unit version is updated each time there is a
change in hardware or software specifications. Even when two Units or EtherCAT slaves have the
same model number, they will have functional or performance differences if they have different hard­ware revisions or unit versions.

Checking Versions

You can check versions on the ID information indications or with the Sysmac Studio.

Checking Unit Versions on ID Information Indications

The unit version is given on the ID information indication on the side of the product.

 Checking the Unit Version of an NJ-series CPU Unit

The ID information on the NJ501-5300 is shown below.

ID information indication

CNC version

Unit model Unit version

NJ501 - 5300

CNC Ver.1.00

PORT1 MAC ADDRESS:
PORT2 MAC ADDRESS:

Lot No. DDMYY xxxx

Ver.1.








Hardware revision

HW Rev.

MAC addressLot number and serial number

 Checking the Unit Version of an NY-series Controller

The ID information on an NY-series NY52-1 Controller is shown below.





18

ID information indication

Unit version

CNC version



Ver.1.
CNC Ver.1.00

NJ/NY-series G code Instructions Reference Manual (O031)

Versions

Checking Unit Versions with the Sysmac Studio

You can use the Sysmac Studio to check unit versions. The procedure is different for Units and for Eth­erCAT slaves.

 Checking the Unit Version of an NJ-series CPU Unit

You can use the Production Information while the Sysmac Studio is online to check the unit version
of a Unit. You can do this for the CPU Unit, CJ-series Special I/O Units, and CJ-series CPU Bus
Units. You cannot check the unit versions of CJ-series Basic I/O Units with the Sysmac Studio.

Use the following procedure to check the unit version.

1 Double-click CPU/Expansion Racks under Configurations and Setup in the Multiview

Explorer. Or, right-click CPU/Expansion Racks under Configurations and Setup and select
Edit from the menu.

The Unit Editor is displayed.

2 Right-click any open space in the Unit Editor and select Production Information.

The Production Information Dialog Box is displayed.

 Checking the Unit Version of an NY-series Controller

You can use the Production Information while the Sysmac Studio is online to check the unit version
of a Unit. You can only do this for the Controller.

1 Right-click CPU Rack under Configurations and Setup - CPU/Expansion Racks in the Multi-

view Explorer and select Production Information.

The Production Information Dialog Box is displayed.

 Changing Information Displayed in Production Information Dialog Box

1 Click the Show Detail or Show Outline Button at the lower right of the Production Informa-

tion Dialog Box.

The view will change between the production information details and outline.

Outline View Detail View

The information that is displayed is different for the Outline View and Detail View. The Detail View
displays the unit version, hardware version, and software versions. The Outline View displays only
the unit version.

Note The hardware revision is separated by “/” and displayed on the right of the hardware version.

NJ/NY-series G code Instructions Reference Manual (O031)

19

Versions

 Checking the Unit Version of an EtherCAT Slave

You can use the Production Information while the Sysmac Studio is online to check the unit version
of an EtherCAT slave. Use the following procedure to check the unit version.

1 Double-click EtherCAT under Configurations and Setup in the Multiview Explorer. Or,

right-click EtherCAT under Configurations and Setup and select Edit from the menu.

The EtherCAT Tab Page is displayed.

2 Right-click the master on the EtherCAT Tab Page and select Display Production Information.

The Production Information Dialog Box is displayed.

The unit version is displayed after “Rev.”

 Changing Information Displayed in Production Information Dialog Box

1 Click the Show Detail or Show Outline Button at the lower right of the Production Informa-

tion Dialog Box.

The view will change between the production information details and outline.

Outline View Detail View

20

NJ/NY-series G code Instructions Reference Manual (O031)

Related Manuals

Related Manuals

The following manuals are related. Use these manuals for reference.

Manual name Cat. No. Model numbers Application Description

NJ-series CPU Unit
Hardware User’s Manual

NJ/NX-series CPU Unit
Software User’s Manual

NJ/NX-series Instructions Ref­erence Manual

NJ/NX-series CPU Unit Motion
Control User’s Manual

NJ/NX-series Motion Control
Instructions Reference Manual

NJ/NX-series CPU Unit
Built-in EtherCAT Port
User’s Manual

NJ/NX-series CPU Unit

Built-in EtherNet/IP
User’s Manual

NJ/NY-series
NC Integrated Controller User’s
Manual

NJ/NY-series
G code Instructions Reference
Manual



Port

W500

W501

W502

W507

W508

W505

W506

O030

O031

NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NX701-



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



NJ501-5300
NY532-5400

NJ501-5300
NY532-5400

Learning the basic
specifications of the
NJ-series CPU Units,
including introductory
information, designing,
installation, and main­tenance.
Mainly hardware infor­mation is provided.

Learning how to pro­gram and set up an
NJ/NX-series CPU
Unit.
Mainly software infor­mation is provided.

Learning detailed
specifications on the
basic instructions of
an NJ/NX-series CPU
Unit.

Learning about
motion control set­tings and program­ming concepts.

Learning about the
specifications of the
motion control
instructions.

Using the built-in Eth­erCAT port on an
NJ/NX-series CPU
Unit.

Using the built-in Eth­erNet/IP port on an
NJ/NX-series CPU
Unit.

Performing numeri­cal control with
NJ/NY-series Control­lers.

Learning about the
specifications of the
G code/M code
instructions.

An introduction to the entire NJ-series system
is provided along with the following informa­tion on the CPU Unit.

• Features and system configuration

• Introduction

• Part names and functions

• General specifications

• Installation and wiring

• Maintenance and inspection

The following information is provided on a
Controller built with an NJ/NX-series CPU
Unit.

• CPU Unit operation

• CPU Unit features

• Initial settings

• Programming based on IEC 61131-3 lan­guage specifications

The instructions in the instruction set (IEC
61131-3 specifications) are described.

The settings and operation of the CPU Unit
and programming concepts for motion control
are described.

The motion control instructions are described.

Information on the built-in EtherCAT port is
provided.
This manual provides an introduction and pro­vides information on the configuration, fea­tures, and setup.

Information on the built-in EtherNet/IP port is
provided.
Information is provided on the basic setup, tag
data links, and other features.

Describes the functionality to perform the
numerical control. Use this manual together
with the NJ/NY-series G code Instructions
Reference Manual (Cat. No. O031) when pro­gramming.

The G code/M code instructions are
described. Use this manual together with the

NJ/NY-series NC Integrated Controller User’s
Manual (Cat. No. O030) when programming.

NJ/NY-series G code Instructions Reference Manual (O031)

21

Related Manuals

Manual name Cat. No. Model numbers Application Description

NJ/NX-series Troubleshooting
Manual

Sysmac Studio Version 1
Operation Manual

CNC Operator
Operation Manual

NY-series IPC Machine Con­troller Industrial Panel PC
Hardware User’s Manual

NY-series IPC Machine Con­troller Industrial Box PC Hard­ware User’s Manual

NY-series IPC Machine Con­troller Industrial Panel PC /
Industrial Box PC Setup
User’s Manual

NY-series IPC Machine Con­troller Industrial Panel PC /
Industrial Box PC Software
User’s Manual

NY-series Instructions Refer­ence Manual

NY-series IPC Machine Con­troller Industrial Panel PC /
Industrial Box PC Motion Con­trol User’s Manual

NX701-

W503

W504 SYSMAC-

O032 SYSMAC-

W557

W556

W568

W558

W560

W559



NX102-



NX1P2-



NJ501-



NJ301-



NJ101-



SE2

RTNC0D

NY532-1



NY512-1



NY532-1



NY512-1



NY532-1



NY512-1



NY532-1



NY512-1



NY532-1



NY512-1



Learning about the
errors that may be
detected in an
NJ/NX-series Con­troller.

Learning about the
operating proce­dures and functions
of the Sysmac Studio.

Learning an introduc­tion of the CNC Oper­ator and how to use
it.

Learning the basic
specifications of the
NY-series Industrial
Panel PCs, including
introductory informa­tion, designing, instal­lation, and
maintenance.
Mainly hardware infor­mation is provided.

Learning the basic
specifications of the
NY-series Industrial
Box PC, including
introductory informa­tion, designing, instal­lation, and
maintenance.
Mainly hardware infor­mation is provided.

Learning the initial set­tings of the NY-series
Industrial PCs and
preparations to use
Controllers.

Learning how to pro­gram and set up the
Controller functions of
an NY-series Industrial
PC.

Learning detailed
specifications on the
basic instructions of
an NY-series Indus­trial PC.

Learning about motion
control settings and
programming con­cepts of an NY-series
Industrial PC.

Concepts on managing errors that may be
detected in an NJ/NX-series Controller and
information on individual errors are described.

Describes the operating procedures of the
Sysmac Studio.

An introduction of the CNC Operator, installa­tion procedures, basic operations, connection
operations, and operating procedures for
main functions are described.

An introduction to the entire NY-series system
is provided along with the following informa­tion on the Industrial Panel PC.

• Features and system configuration

• Introduction

• Part names and functions

• General specifications

• Installation and wiring

• Maintenance and inspection

An introduction to the entire NY-series system
is provided along with the following informa­tion on the Industrial Box PC.

• Features and system configuration

• Introduction

• Part names and functions

• General specifications

• Installation and wiring

• Maintenance and inspection

The following information is provided on an
introduction to the entire NY-series system.

• Two OS systems

• Initial settings

• Industrial PC Support Utility

• NYCompolet

• Industrial PC API

• Backup & recovery

The following information is provided on the
NY-series Controller functions.

• Controller operations

• Controller functions

• Controller settings

• Programming based on IEC 61131-3 lan­guage specifications

The instructions in the instruction set (IEC
61131-3 specifications) are described.

The settings and operation of the Controller
and programming concepts for motion control
are described.

22

NJ/NY-series G code Instructions Reference Manual (O031)

Manual name Cat. No. Model numbers Application Description

NY-series Motion Control
Instructions Reference Manual

W561

NY532-1

NY512-1





Learning about the
specifications of the
motion control

The motion control instructions are described.

instructions of an
NY-series Industrial
PC.

NY-series IPC Machine Con­troller Industrial Panel PC /
Industrial Box PC Built-in Eth­erCAT Port User’s Manual

W562

NY512-1





Using the built-in Eth­erCAT port in an
NY-series Industrial
PC.

Information on the built-in EtherCAT port is
provided.
This manual provides an introduction and pro­vides information on the configuration, fea-

NY532-1

tures, and setup.

NY-series IPC Machine Con­troller Industrial Panel PC /
Industrial Box PC Built-in Eth-



erNet / IP

Port User’s Manual

W563

NY532-1

NY512-1





Using the built-in Eth­erNet/IP port in an
NY-series Industrial
PC.

Information on the built-in EtherNet/IP port is
provided.
Information is provided on the basic setup, tag
data links, and other features.

Related Manuals

NY-series Troubleshooting
Manual

W564

NY532-1

NY512-1





Learning about the
errors that may be
detected in an
NY-series Industrial
PC.

Concepts on managing errors that may be
detected in an NY-series Controller and infor­mation on individual errors are described.

NJ/NY-series G code Instructions Reference Manual (O031)

23

Terminology

Terminology

Term Description

NJ501-1 Represents NJ501-1300/-1400/-1500.

24

NJ/NY-series G code Instructions Reference Manual (O031)

Revision History

O031-E1-02

Revision code

Cat. No.

A manual revision code appears as a suffix to the catalog number on the front and back covers of the
manual.

Revision code Date Revised content

01 October 2017 Original production
02 July 2018 • Added information on the

• Corrected mistakes.

NX102-

Revision History

.

NJ/NY-series G code Instructions Reference Manual (O031)

25

Revision History

26

NJ/NY-series G code Instructions Reference Manual (O031)

Basic Information on NC Pro­gramming

This section provides the list of available instructions, and the descriptions of parame­ters and modal.

Instructions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-2

G Codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-2

M Codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-4

Instruction Parameters . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-5

G Code Descriptions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-7

What is Modal? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1-9

1

NJ/NY-series G code Instructions Reference Manual (O031)

1 - 1

1 Basic Information on NC Programming

Instructions

The following table lists the G codes and M codes supported by NJ501-5300 and NJ532-5400.

G Codes

Modal group Initial modal

00 Non-modal --- G04 Dwell Stops the CNC coordinate system for a predefined

00 Non-modal --- G09 Exact Stop Executes a forcible control deceleration stop

00 Non-modal --- G28 Return to Reference

00 Non-modal --- G30 Return to 2nd, 3rd or

00 Non-modal --- G31 Skip Function Provides Rapid Positioning (G00) and input stop.
00 Non-modal --- G52 Local Coordinate Sys-

00 Non-modal --- G53 Dimension Shift Cancel Runs commands in the machine coordinate sys-

01 Rapid Position­ing

02 Plane G17 G17 X-Y Plane Selection Changes a plane, the reference of Circular Interpo-

03 Distance G90 G90 Absolute command Enables absolute position mode for all axes in the

06 Unit Operation

G01 G00 Rapid Positioning Performs a point-to-point operation in the minimum

depends on
the Orthogo­nal Axis
Command
Unit setting

Instruc

tion

Point

4th Reference Point

tem Set

G01 Linear Interpolation Moves a CNC motor from the current position to a

G02 Circular Interpolation in

CW direction

G03 Circular Interpolation in

CCW direction

G18 Z-X Plane Selection
G19 Y-Z Plane Selection

G91 Incremental command Enables relative Incremental position mode for all

G20 Inch input Switches all the settings of the CNC coordinate

G21 Metric input

Name Outline of function

period of time.

together with the registration of in-position at the
termination of a block.

Moves the tool to the reference point (position 0)
via the middle point specified by an argument of
the instruction.

Moves the tool to the 2nd, 3rd and 4th reference
point.

Creates coordinates in the Work Coordinate Sys­tem.

tem.

time by following the restrictions of CNC motor set­tings.

specified position.
Moves the tool on an arc path on the XY, YZ, or ZX

plane.

lation (G02/G03), Cutter Compensation
(G40/G41/G42), and Coordinate System Rotation
(G68/G69).

CNC coordinate system, and moves the axes to a
specified position in the current coordinate system.

axes in the CNC coordinate system, and moves
the axes a certain distance from the last command
position.

system, command values, and the unit of current
values.

1 - 2

NJ/NY-series G code Instructions Reference Manual (O031)

1 Basic Information on NC Programming

Modal group Initial modal

07 Tool radius G40 G40 Cancels tool compen-

08 Tool length off­set

09 Fixed cycle G80 G74 Left-handed Tapping

10 Return level G98 G98 Fixed Cycle Return to

11 Scaling G50 G50 Cancel scaling Scales the current coordinate system.

14 Coordinate
System Selection

15 Path Control G64 G61 Exact Stop Mode Stops operation between blocks to prevent corner

16 Rotation G69 G68 Enables rotation Rotates the current coordinates.

22 Mirroring G50.1 G50.1 Cancel Mirroring Mirrors the current coordinates.

23 Multi-block
Accelera­tion/Deceleration
Rate

G49 G43 Tool Offset, positive Corrects the position in the Z-axis direction.

No Work
Coordinate
System is
selected (all
coordinate
axis have
zero offset).

G501 G500 Enables multi-block

Instruc

tion

sation
G41 Tool Compensation, left
G42 Tool Compensation,

right

G44 Tool Offset, negative
G49 Cancels tool offset

Cycle
G80 Fixed Cycle Cancel Cancels a fixed cycle.
G84 Tapping Cycle Performs tapping machining.

Initial Level
G99 Fixed Cycle Return to

R Point Level

G51 Scaling
G54 1st Work Coordinate

System selection
G55 2nd Work Coordinate

System selection
G56 3rd Work Coordinate

System selection
G57 4th Work Coordinate

System selection
G58 5th Work Coordinate

System selection
G59 6th Work Coordinate

System selection

G64 Continuous-path Mode When two or more sequential operations are

G69 Disables rotation

G51.1 Mirroring

acceleration/decelera-

tion rate
G501 Disables multi-block

acceleration/decelera-

tion rate

Name Outline of function

Enables selection of a tool for control, automati­cally moves the tool to the left side or right side of
the programmed path, and correct the radius of the
tool.

Performs reverse tapping machining.

Sets the return position of a fixed cycle to the initial
level.

Sets the return position of a fixed cycle to the R
point level.

Changes the current coordinate system to a speci­fied one defined by the user by using the offsets of
X-, Y-, Z-, A-, B-, and C-axis.

rounding and blending from being executed.

aligned, the former can be blended with the latter
and accelerated/decelerated.

Reads the path ahead, and adjusts the accelera­tion or deceleration rate.

Instructions

1

G Codes

NJ/NY-series G code Instructions Reference Manual (O031)

1 - 3

1 Basic Information on NC Programming

M Codes

Type Instruction Name Outline of function

Reservation
auxiliary func­tion output

Spindle Axis M03 Spindle CW Operates the Spindle axis in the positive direction at the speci-

Programming M98 Subprogram Call Calls a subprogram from the program currently running.

M00 Program Stop Stops the execution of the NC program at the block where M00

is commanded.

M01 Optional Stop As is the case with M00, stops the execution of the NC program

at the block where M01 is commanded.

M02/M30 End of Program Stops the NC program to enable reset mode.

fied speed.

M04 Spindle CCW Operates the Spindle axis in the negative direction at the speci-

fied speed.
M05 Spindle OFF Stops the Spindle axis.
M19 Spindle Orienta-

tion

M99 Subprogram End Terminates the subprogram currently running and returns to the

Uses this command to adjust orientation of the spindle axis

when you replace tools and carry out other tasks.

main program from which the subprogram was invoked.

1 - 4

NJ/NY-series G code Instructions Reference Manual (O031)

1 Basic Information on NC Programming

Instruction Parameters

Instruction Parameters

The following describes the parameters used in each instruction.

Parameter Description Relevant codes Recommended range

Target A-axis Position [com­mand units]

A

B

C

F

G G code --- Valid G code

I

J

K

L

M M Code --- Valid M code (M0 to M191)

P

Q Q-variable address --- Valid address (Q0 to Q4095)

R

S Spindle rotation speed [r/min] M03/M04/M19 0 ≤ S ≤ MAX speed (CNC motor setting)

A-axis middle point [command
units]

A-axis offset [command units] G52 -1,000,000 ≤ A ≤ 1,000,000
Target B-axis Position [com­mand units]
B-axis middle point [command
units]
B-axis offset [command units] G52 -1,000,000 ≤ B ≤ 1,000,000
Target C-axis Position [com­mand units]
C-axis middle point [command
units]
C-axis offset [command units] G52 -1,000,000 ≤ C ≤ 1,000,000
Feedrate [command units] G00/G01/G02/G03 0.000000001≤ F≤ MAX feedrate (CNC coordinate

Dwell time [s] G04 0≤F≤100,000

X-axis arc center [command
units]
X-axis scaling magnification G51 0.00001 ≤ I ≤ 10,000

Y-axis arc center [command
units]

-axis scaling magnification G51 0.00001 ≤ J ≤ 10,000

Y

Z-axis arc center [command
units]

Z-axis scaling magnification G51 0.00001 ≤ K ≤ 10,000

Number of repetitions G74/G84 0 ≤ K ≤ 10,000
L-variable address --- Valid address (L0 to L255)
Number of loops M98 0 ≤ L ≤ 10,000

P-variable address --- Valid address (P0 to P32767)
Dwell time [ms] G04/G74/G84 0≤P≤100,000,000
Reference point specification G30 Valid reference point number (P2 to P4)
All axes scaling magnification G51 0.00001 ≤ P ≤ 10,000
Program number M98 Programmed by Sysmac Studio

Arc radius [command units] G02/G03 -1,000,000 ≤ R ≤ 1,000,000
Rotation angle [deg] G68 -360 ≤ R ≤ 360
R Point Level [command units] G74/G84 -1,000,000 ≤ R ≤ 1,000,000

G00/G01/G02/G03 -1,000,000 ≤ A ≤ 1,000,000

G28/G30 -1,000,000 ≤ A ≤ 1,000,000

G00/G01/G02/G03 -1,000,000 ≤ B ≤ 1,000,000

G28/G30 -1,000,000 ≤ B ≤ 1,000,000

G00/G01/G02/G03 -1,000,000 ≤ C ≤ 1,000,000

G28/G30 -1,000,000 ≤ C ≤ 1,000,000

system setting)

G02/G03 -1,000,000 ≤ I ≤ 1,000,000

-10,000 ≤ I ≤ -0.00001

G02/G03 -1,000,000 ≤ J ≤ 1

-10,000 ≤ J ≤ -0.00001

G02/G03 -1,000,000 ≤ K ≤ 1,000,000

-10,000 ≤ K ≤ -0.00001

1000 to 2999

Programmed by HMI

3000 to 9999

,000,000

1

NJ/NY-series G code Instructions Reference Manual (O031)

1 - 5

1 Basic Information on NC Programming

Parameter Description Relevant codes Recommended range

Target X-axis Position [com­mand units]

Dwell time [s] G04 0≤X≤100,000

X

Y

Z

ta Acceleration time [ms] G01/G02/G03 0 ≤ ta ≤ 250,000
td Deceleration time [ms] G01/G02/G03 0 ≤ td ≤ 250,000
ts Jerk Time [ms] G01/G02/G03 0 ≤ ts ≤ 1

X-axis middle point [command
units]

X-axis center [command units] G50/G50.1/G68 -1,000,000 ≤ X ≤ 1,000,000
X-axis offset [command units] G52 -1,000,000 ≤ X ≤ 1,000,000
Target Y-axis position [com-

mand units]
Y-axis middle point [command

units]
X-axis center [command units] G50/G50.1/G68 -1,000,000 ≤ Y ≤ 1,000,000
Y-axis offset [command units] G52 -1,000,000 ≤ Y ≤ 1,000,000
Target Z-axis position [com-

mand units]
Z-axis middle point [command

units]
Z-axis center [command units] G50/G50.1/G68 -1,000,000 ≤ Z ≤ 1,000,000
Z-axis offset [command units] G52 -1,000,000 ≤ Z ≤ 1,000,000
Z-point position [command

units]

There is no modal group for feedrate F, spindle rotation speed S, acceleration time ta, deceleration time
td, and Jerk time ts, but it operates as the modal to maintain the commanded state.

G00/G01/G02/G03 -1,000,000 ≤ X ≤ 1,000,000

G28/G30 -1,000,000 ≤ X ≤ 1,000,000

G00/G01/G02/G03 -1,000,000 ≤ Y ≤ 1,000,000

G28/G30 -1,000,000 ≤ Y ≤ 1,000,000

G00/G01/G02/G03 -1,000,000 ≤ Z ≤ 1,000,000

G28/G30 -1,000,000 ≤ Z ≤ 1,000,000

G74/G84 -1,000,000 ≤ Z ≤ 1,000,000

25,000

1 - 6

NJ/NY-series G code Instructions Reference Manual (O031)

1 Basic Information on NC Programming

Effect range of G64

Effect range of G61

Word

Block

N02 M03 S 1000
N03 G64
N04 X20
N05 Y10

N06 G61
N07 X-20
N08 Y-10
N09 M30 // End of Program

N01 G17 G91 G01 ta1000 td1000 F1000

Writing comments
(Multiple line comments can be written.)
/*There are two ways of commenting multiple lines.*/

G Code Descriptions

The program format generally called the G code is defined by ISO 6983 (JIS B 6315).

A combination of characters such as G, M and X, and digits is called a word, and a line consisting of two
or more words are called a block. G codes are executed sequentially in units of a block. When execu­tion of the current block is completed, the next block is executed in principle. A line feed code indicates
the end of block. The length of one block must be 1020 bytes or less. These restrictions apply to blocks
after program parsing. Refer to Program Parsing by CNC Operator on page A-2 for program parsing.

The influential range varies depending on the word. A word that only has an effect in the block where it
is written is called non-modal, and one that continues to have an effect when omitted in subsequent
blocks is called modal. In the modal, a few words produce their effects exclusively. This is called a
modal group.

Comments can be entered by using “//” before the comment, which is valid to the end of the block. This
specification is not defined by ISO 6983.

The spindle operations, F, and M30 need to be described. M30 can be written as M02.

G Code Descriptions

1

NJ/NY-series G code Instructions Reference Manual (O031)

* G61 and G64 are in the same modal group and if another one is written, the subsequent modal
changes.

1 - 7

1 Basic Information on NC Programming

Optional Skip Block

If an optional signal is entered, the block where the related command is written is skipped.

*1

Enter the command as /N

*1. N is a constant from 1 to 31.

G17 G91 G01 ta1000 td1000 F1000 S1000 M03
G64

/1 X20 // The optional block skip can be written at the

/ Y10 // If N is omitted, /1 is assumed.

G61

/1/2 X-20 // Multiple numbers can be specified.

Y-10
M30

Note that the optional block skip can be used for G codes only.

It cannot be used for program codes.

.

beginning of line only.

1 - 8

NJ/NY-series G code Instructions Reference Manual (O031)

1 Basic Information on NC Programming

What is Modal?

There are two types of G codes: One that is valid only in its block, and the other that continues to be
valid until another G code of the same group is specified. The former is called non-modal G code, and
the latter modal G code.

Modal G codes are summarized into some G code groups. The group is called a modal group.

In the same modal group, G codes that cannot hold simultaneously are summarized. One of the
G-code states is always preserved. For example, G90 (Absolute Dimension) and G91 (Incremental
Dimension) are summarized into modal group 03.

Refer to Instructions on page 1-2 for information about which G code is summarized in which modal
group.

What is Modal?

1

NJ/NY-series G code Instructions Reference Manual (O031)

1 - 9

1 Basic Information on NC Programming

1 - 10

NJ/NY-series G code Instructions Reference Manual (O031)

G Code

2

This section describes the specifications of the G code.

Interpolation Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-3

Dwell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-15

Feed Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-17

Coordinate System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-27

Reference Point . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-35

Compensation Functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-39

Utilities . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2-59

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 1

2 G Code

2 - 2

NJ/NY-series G code Instructions Reference Manual (O031)

2

Interpolation Functions

Instruction Name Page

G00 Rapid Positioning P. 2-4
G01 Linear Interpolation P. 2-6
G02/G03 Circular Interpolation P. 2-8
G31 Skip Function P. 2-13

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 3

2 G Code

G00 Rapid Positioning

This instruction positions a tool.

Modal/Non-modal Modal
Modal group 01 Rapid Positioning
Instruction format G00 X- Y- Z- A- B- C-
Relevant G codes G90, G91

Parameters

X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Target Z-axis Position Specifies the destination position [command units] on the

A Target A-axis Position Specifies the destination position [command units] on the

B Target B-axis Position Specifies the destination position [command units] on the

C Target C-axis Position Specifies the destination position [command units] on the

Parameter Name Description

X-axis.

Y-a xi s.

Z-axis.

A-axis.

B-axis.

C-axis.

Function

Use this command to position a tool.

It moves the tool from the current position to a specified position in the minimum period of time with the
CNC motor parameters and CNC coordinate system parameters. Write the command according to the
instruction format. The description of each coordinate can be omitted.

This function does not guarantee the trace. If the linear trace is required, use the linear interpolation
(G01).

The command position follows the specifications for the Absolute Dimension (G90) and Incremental
Dimension (G91).

2 - 4

NJ/NY-series G code Instructions Reference Manual (O031)

Programming Example

Y

X

50

100

2 G Code

The following program performs positioning with the absolute dimensions.

:
N010 G90 // Absolute dimension
N011 G00 X100 Y50

G00 Rapid Positioning

2

Programming Example

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 5

2 G Code

G01 Linear Interpolation

This instruction performs linear interpolation.

Modal/Non-modal Modal
Modal group 01 Rapid Positioning
Instruction format G01 F- ta- td- ts- X- Y- Z- A- B- C-
Relevant G codes G90, G91, F, ta, td, ts

Parameters

F Target Velocity Specifies the target velocity [command units/min].
ta Acceleration Time Specifies the acceleration time [ms].
td Deceleration Time Specifies the deceleration time [ms].
ts Jerk Time Specifies the jerk time [ms].
X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Target Z-axis Position Specifies the destination position [command units] on the

A Target A-axis Position Specifies the destination position [command units] on the

B Target B-axis Position Specifies the destination position [command units] on the

C Target C-axis Position Specifies the destination position [command units] on the

Parameter Name Description

X-axis.

Y-a xi s.

Z-axis.

A-axis.

B-axis.

C-axis.

2 - 6

NJ/NY-series G code Instructions Reference Manual (O031)

Function

Y

X

50

100

Current position

This command moves the CNC motor with the specified velocity, acceleration time, deceleration time,
and jerk time to operate a tool linearly from the current position to a target position.

Unlike G00, if two or more continuous operating functions are aligned, the commands are blended to
accelerate or decelerate.

The command position follows the specifications for the Absolute Dimension (G90) and Incremental
Dimension (G91).

2 G Code

G01 Linear Interpolation

G01 uses the following settings for its operation.

Command Description Unit

F Target Velocity command unit/min
ta Acceleration Time ms
td Deceleration Time ms
ts Jerk Time ms

The F command calculates velocity by using X-, Y-, and Z-axis. If the user selects A-, B-, or C-axis, the
axis is operated at the rotational axis speed.

For relationship between acceleration time, deceleration time, and jerk time and the speed waveforms,
refer to the programming example of G64 Continuous-path Mode on page 2-22.

Programming Example

The following program performs linear interpolation with the absolute dimension.

:
N010 G90 // Absolute dimension
N011 G01 X100 Y50 F300

:

2

Function

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 7

2 G Code

G02, G03 Circular Interpolation

These instructions perform circular interpolation.

Modal/Non-modal Modal
Modal group 01 Rapid Positioning

Instruction format

Relevant G codes G90, G91, G17, G18, G19

Parameters

F Target Velocity Specifies the target velocity [command units/min].
ta Acceleration Time Specifies the acceleration time [ms].
td Deceleration Time Specifies the deceleration time [ms].
ts Jerk Time Specifies the jerk time [ms].
X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Target Z-axis Position Specifies the destination position [command units] on the

A Target A-axis Position Specifies the destination position [command units] on the

B Target B-axis Position Specifies the destination position [command units] on the

C Target C-axis Position Specifies the destination position [command units] on the

I X-axis arc center Specifies the arc center [command units] on the X-axis.
J Y-axis arc center Specifies the arc center [command units] on the Y-axis.
K Z-axis arc center Specifies the arc center [command units] on the Z-axis.
R Arc radius Specifies the arc radius [command units].

Circular
Interpola­tion
in CW
direction

Circular
Interpola­tion
in CCW
direction

Parameter Name Description

When specifying the arc
center

When specifying the arc G02 F- ta- td- ts- X- Y- Z- R- A- B- C-

When specifying the arc
center
When specifying the arc G03 F- ta- td- ts- X- Y- Z- R- A- B- C-

X-axis.

Y-a xi s.

Z-axis.

A-axis.

B-axis.

C-axis.

G02 F- ta- td- ts- X- Y- Z- I- J- K- A- B- C-

G03 F- ta- td- ts- X- Y- Z- I- J- K- A- B- C-

2 - 8

NJ/NY-series G code Instructions Reference Manual (O031)

Function

Y

X

50

90

10

10050

Current position

Center

Target Position

This command moves CNC motors with the specified velocity, acceleration time, deceleration time, and
jerk time to operate a tool in an arc motion from the current position to a target position.

For relationship between acceleration time, deceleration time, and jerk time and the speed waveforms,
refer to the programming example of G64 Continuous-path Mode on page 2-22.

When this command is executed, the arc path is calculated on the XY, YZ, or ZX plane. If you select an
axis other than those composing the plane to specify a position, the path is linear.

If both IJK and R are omitted, an error occurs. Also, if R0 is specified, the linear path is set.

Programming Example

 The following shows circular interpolation with Arc center specification

:

N010 G90 ..................Absolute dimension

N011 G17 ..................XY Plane selection

N010 G02 X100 Y90 I0 J40 F300

:

2 G Code

G02, G03 Circular Interpolation

2

Function

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 9

2 G Code

 The following shows circular interpolation with Arc radius specification

N010 G90 .................. Absolute dimension

N011 G17 .................. XY Plane selection

N012 G02 X140 Y50 R-40 F300

When radius < 0, a circle larger than a semicircle is drawn.

(radius < 0)

:

:

Y

90

50

10

Center

Current position

10050

Target Position

 The following shows circular interpolation with Arc radius specification

(radius > 0)

:

N010 G91 .................. Incremental dimension

N011 G17 .................. XY Plane selection

N012 G02 X40 Y40 R40 F300

:

When radius > 0, a circle smaller than a semicircle is drawn.

Y

X

2 - 10

90

50

10

Target Position

Current position

10050

NJ/NY-series G code Instructions Reference Manual (O031)

Center

X

2 G Code

-90

100

90

80

70

60

50

40

30

20

10

0

-40 -30 -20 -10 -90 10 20 30 40 50

X

Y

30

-50

-40

-30

-20

-10
0

10

20

30

40

50

0

10

20

30

40

50

60

70

80

90

100

25
20
15
10

5
0

Y

X

Z

 Spiral interpolation

N01 G17 G64 G91 F1000
N02 M03 S300
N03 G02 Y10 J50 // First rotation of spiral interpolation
N04 Y10 J40 // Second rotation of spiral interpolation
N05 Y10 J30 // Third rotation of spiral interpolation
N06 M05
N07 M30 // End of program

G02, G03 Circular Interpolation

2

Programming Example

 Helical interpolation

N01 G17 G64 G91 F1000
N02 M03 S300
N03 G02 J50 Z10 // First rotation of helical interpolation
N04 J50 Z10 // Second rotation of helical interpolation
N05 J50 Z10 // Third rotation of helical interpolation
N06 M05
N07 M30 // End of program

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 11

2 G Code

 Conical interpolation

N01 G17 G64 G91 F1000
N02 M03 S300
N03 G02 Y10 J50 Z10 // First rotation of conical interpolation
N04 Y10 J40 Z10 // Second rotation of conical interpolation
N05 Y10 J30 Z10 // Third rotation of conical interpolation
N06 M05
N07 M30 // End of program

30
25
20
15

Z

10

5
0

100

-50

-40

-30

-20

70

60

-10
0

10

X

20

30

40

50

10

0

30

20

50

40

90

80

Y

2 - 12

NJ/NY-series G code Instructions Reference Manual (O031)

G31 Skip Function

If a skip signal is input externally during execution of a movement command, the commanded move­ment is interrupted to execute commands in the next block.

Modal/Non-modal Non-modal
Modal group 00 Non-modal
Instruction format G31 X- Y- Z- A- B- C-
Relevant G codes G90, G91

2 G Code

G31 Skip Function

2

Parameters

X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Target Z-axis Position Specifies the destination position [command units] on the

A Target A-axis Position Specifies the destination position [command units] on the

B Target B-axis Position Specifies the destination position [command units] on the

C Target C-axis Position Specifies the destination position [command units] on the

Function

This command interrupts movement with Rapid Positioning (G00) and external input. Each CNC motor
assigned to a command axis operates independently to the command position.

All the CNC motors start moving simultaneously and operate according to respective parameters. If you
want to unify external inputs, set the same signal for all the inputs.

Each CNC motor also stops independently. Until all of the CNC motors stop, the process does not pro­ceed to the next block. This command is not blended with other operations.

If there is an input externally to a CNC motor, the motor is moved to the captured position. Otherwise, it
stops at the command position. The basic operation is the same as that of Rapid Positioning (G00). The
command position follows the specifications for the Absolute Dimension (G90) and Incremental Dimen­sion (G91). The velocity must be specified as the Skip Velocity (CNC motor setting). For details, refer to
the NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030). The user can read the posi-
tions captured by _CNC_CapturedPosition(), which are sorted in ascending order of CNC motor num­bers. For example, if the CNC coordinate system has CNC motors 1/3/4, _CNC_CapturedPosition(0)
indicates CNC motor 1, _CNC_CapturedPosition(1) indicates CNC motor 3, and _CNC_CapturedPosi­tion(2) indicates CNC motor 4.

For inputting skip signal, consult the instruction manual provided by the machine tool manufacturer.

Parameters

Parameter Name Description

X-axis.

Y-a xi s.

Z-axis.

A-axis.

B-axis.

C-axis.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 13

2 G Code

_

Drop

Trigger position

1S-series Servo Drive
EtherCAT communications
built-in type

Sensor

Programming Example

Use the skip function and measure the wear volume of tool length. In this example, the tool touches the
sensor and skip signal is input while it moves toward the cutting surface. The stop position is captured
using the skip signal, and notified to the sequence control program as an argument of M code output.
Based on the captured position, calculate the wear volume of tool length in the sequence control pro­gram. For the procedure for setting the wear volume of tool length that was calculated, refer to the How
to Enable Tool Replacement in the NJ/NY-series NC Integrated Controller User’s Manual (Cat. No.
O030).

N01 G17 G91 G64 F1000
N02 G28 X5 Y5 // Moves to the position to start measuring the

N03 G31 Z-10 // Moves to the cutting surface.
N04 M101 VA[_CNC_CapturedPosi-

tion2]
N05 M30

wear volume of tool length.

// Notification to the sequence control program

Use of M101 for transferring the captured data to the sequence control program is an example. When
using this command, refer to the instruction manual provided by the machine tool manufacturer.

Z

N03

CNC_CapturedPosition(2)

Stop

0

Sensor input

Time

2 - 14

NJ/NY-series G code Instructions Reference Manual (O031)

2

Dwell

Instruction Name Page

G04 Dwell P. 2-16

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 15

2 G Code

N010 N011 N012

Velocity

10 seconds

Time

G04 Dwell

This instruction stops the NC program only for a specified period of time.

Modal/Non-modal Non-modal
Modal group 00 Non-modal

Instruction format

Relevant G codes

Parameters

F Specification in seconds Specifies a stop time [s] of the NC program.
X Specification in seconds Specifies a stop time [s] of the NC program.
P Specification in millisec-

Function

The CNC coordinate system for which G04 is executed stops for the period of time specified by F, P, or
X parameter indicating the number of seconds. The unit of time period specified by F or X parameter is
second, and for P parameter is millisecond.

G04 F-

G04 P-

G04 X-

Parameter Name Description

Specifies a stop time [ms] of the NC program.

onds

The G04 command only stops axis motions. It does not affect the spindle axis and device functions
controlled by sequence control programs. If no parameter is specified, Dwell of 0 second, the default
value will be executed.

Programming Example

The following program waits for 10 seconds between linear interpolations.

:
N010 G01 X100 Y100 F50
N011 G04 X10
N012 G01 X200 Y200

:

2 - 16

NJ/NY-series G code Instructions Reference Manual (O031)

2

Feed Functions

Instruction Name Page

F Function Feedrate Function (F function) P. 2-18
ta/td/ts Acceleration Time, Deceleration

Time, Jerk Time
G09 Exact Stop P. 2-20
G61 Exact Stop Mode P. 2-21
G64 Continuous-path Mode P. 2-22
G500/G501 Multi-block Acceleration/Deceler-

ation Rate

P. 2-19

P. 2-24

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 17

2 G Code

Feedrate Function (F function)

This instruction specifies the feedrate.

Modal/Non-modal Modal
Instruction format F{data}
Relevant G codes G01, G02, G03

This instruction specifies the feedrate using a numeric value after the F code.

Zero (0) and a negative value cannot be specified.

The velocity is specified in command units/min. (the feedrate per minute).

The positioning axis is not operated simply by specifying the feedrate.

Use a feed command to move the positioning axis.

For relationship between the feedrate and speed waveforms, refer to the programming example of G64
Continuous-path Mode on page 2-22.

2 - 18

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

Acceleration Time, Deceleration Time, Jerk Time

Acceleration Time, Deceleration Time, Jerk

These instructions specify an acceleration time, deceleration time, and jerk time.

Modal/Non-modal Modal

Acceleration Time ta{data}

Instruction format

Relevant G codes G01, G02, G03

Specify the acceleration time with a numeric value after the ta code. Specify the deceleration time with
a numeric value after the td code. Specify the jerk time with a numeric value after the ts code.

The unit of time is in milliseconds.

For relationship between acceleration time, deceleration time, and jerk time and the speed waveforms,
refer to the programming example of G64 Continuous-path Mode on page 2-22.

Deceleration Time td{data}
Jerk Time ts{data}

Time

2

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 19

2 G Code

0

Feedrate

Time

N02 N03 N04 N05

G09 Exact Stop

This instruction stops deceleration upon termination of the block that is currently running.

Modal/Non-modal Non-modal
Modal group 00 Non-modal
Instruction format G09
Relevant G codes G01, G02, G03

Parameters

This command does not have any parameters to set.

Function

Executing G09 decelerates to a stop simultaneously with in-position check upon the termination of a
block. It is used to prevent blending operations with the next block, such as cutting corners with an
acute angle. This code is only valid for the current block.

Programming Example

Among movement commands between multiple blocks, the following program prevents blending opera­tions between certain blocks, and decelerates to a stop.

N01 G01 G91 G64 F500 // Continuous-path mode
N02 X10
N03 G09 X10 // N02 and N03 are not blended
N04 X10 G09 // N04 and N05 are not blended
N05 X10
N06 M30

2 - 20

NJ/NY-series G code Instructions Reference Manual (O031)

G61 Exact Stop Mode

2 G Code

G61 Exact Stop Mode

This instruction stops operation between blocks to prevent corner blending from being executed.

Modal/Non-modal Modal
Modal group 15 Path Control
Instruction format G61
Relevant G codes G01, G02, G03

Parameters

This command does not have any parameters to set.

Function

The G61 stops an operation between blocks to prevent the execution of blending of the corner and cut­ting corners with an acute angle during operation. When G61 is commanded, deceleration is applied to
the end point of the cutting block, then an in-position check of each block is executed. G61 maintains
the valid state until G64 (Continuous-path Mode) is commanded. Continuous-path Mode (G64) is the
default value at startup.

Programming Example

2

Parameters

Refer to the programming example of G64 Continuous-path Mode on page 2-22.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 21

2 G Code

G64 Continuous-path Mode

When two or more sequential operations are aligned, the former can be blended with the latter and

Parameters

accelerated/decelerated.

Modal/Non-modal Modal
Modal group 15 Path Control
Instruction format G64
Relevant G codes G01, G02, G03, G500, G501

This command does not have any parameters to set.

Function

When G64 is commanded, it is not decelerated to the end point of each block after the command, and
cutting is blended with the next block. This command maintains the valid state until G61 is commanded.
However, G64 causes the feedrate to be decelerated to 0, and an in-position check is executed in the
following cases:

• G00 Rapid Positioning

• G09 Exact Stop

• Block with no movement command in the next block

This does not apply to Multi-block Acceleration/Deceleration Rate Enable (G500).

Refer to G500, G501 Multi-block Acceleration/Deceleration Rate on page 2-24 for details.

Programming Example

In the process of a movement command drawing a rectangle, Continuous-path Mode is switched to
Exact Stop Mode.

N01 G17 G91 G01 ta1000 td1000 ts500 F1000
N02 M03 S1000
N03 G64 // Continuous-path mode
N04 X80
N05 Y40
N06 G61 // Exact stop mode
N07 X-80
N08 Y-40
N09 M30

2 - 22

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

0

40

X

Y

N07

80

N05

N04

N08

N06

td + ts

N04 N05

N07 N08

X
Y

ta + ts

1500

1000

500

0

-500

-1000

-1500

ts ts ts ts

Feedrate

Time

This shows the path of X-Y plane.

Shows the speed waveforms. The parameters shown in the figure are values ta=1000, td=1000, and
ts=500 that have been specified in the NC program.

G64 Continuous-path Mode

2

Programming Example

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 23

2 G Code

G500, G501 Multi-block Accelera­tion/Deceleration Rate

Modal/Non-modal Modal
Modal group 23 Multi-block Acceleration/Deceleration Rate
Instruction format G500, G501
Relevant G codes G01, G02, G03, G64

Parameters

This command does not have any parameters to set.

Function

When this command is enabled in Continuous-path Mode, the Controller reads the path ahead and
searches for a location where the limitation of position, velocity or acceleration may be exceeded.
When the location is found, it decelerates the path to control within the limit range. This change applies
retroactively to the path previously calculated, and is completed prior to actual execution.

G500 enables, and G501 disables. G500 must be used simultaneously with Continuous-path Mode
(G64). If G500 is used together with the Exact Stop Mode (G61), it operates in the Exact Stop Mode.

If the multi-block acceleration/deceleration rate is disabled, accelerate to the feedrate in the first block,
and decelerate in the last block. For this reason, if the specified travel distance is small in accelera­tion/deceleration operation, the operation is such that the maximum acceleration rate is exceeded.

When the multi-block acceleration/deceleration rate is enabled, accelerate or decelerate to the feedrate
across multiple blocks so that the maximum acceleration rate of each motor is not exceeded.

If the multi-block acceleration/deceleration rate is disabled (G501), the following restrictions apply.

• The maximum acceleration or deceleration (CNC motor setting) is made invalid.

• The Back Trace cannot be used.

2 - 24

NJ/NY-series G code Instructions Reference Manual (O031)

Programming Example

The following program shows a movement command which draws a line with a series of infinitesimal
movements when the multi-block acceleration/deceleration rate is enabled or disabled.

N01 G17 G64 G91 G01 F100
N02 M03 S300
N03 G500 // Enables multi-block acceleration/deceleration rate
N04 X1
N05 X1
N06 X1
N07 X1
N08 X1
N09 X1
N10 X1
N11 X1
N12 X1
N13 X1
N14 M05
N15 M30

2 G Code

G500, G501 Multi-block Acceleration/Decel-

eration Rate

2

Programming Example

V

F

0

Feedrate

N04

N05

N06

N07

VF: Velocity specified by F code

N08 N09

N10

N11

N12

N13

Time

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 25

2 G Code

0

Feedrate

Time

N04

N05 N06 N07 N08 N09 N10 N11 N12

N13

V

F

VF: Velocity specified by F code

N01 G17 G64 G91 G01 F100
N02 M03 S300
N03 G501 // Disables multi-block acceleration/deceleration rate
N04 X1
N05 X1
N06 X1
N07 X1
N08 X1
N09 X1
N10 X1
N11 X1
N12 X1
N13 X1
N14 M05
N15 M30

2 - 26

NJ/NY-series G code Instructions Reference Manual (O031)

2

Coordinate System

Instruction Name Page

G52 Local Coordinate System Set P. 2-28
G53 Dimension Shift Cancel P. 2-29
G54 to G59 Select Work Coordinate System P. 2-30
G17/G18/G19 Plane Selection P. 2-31
G20/G21 Inch Input/Metric Input P. 2-32
G90/G91 Absolute Dimension/Incremental

Dimension

P. 2-33

For coordinate system types, refer to the NJ/NY-series NC Integrated Controller User’s Manual (Cat. No.
O030).

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 27

2 G Code

G52 Local Coordinate System Set

This instruction creates coordinate system in the Work Coordinate System.

Modal/Non-modal Non-modal
Modal group 00 Non-modal

Instruction format

Relevant G codes G50, G51, G50.1, G51.1, G68, G69, G54 to G59

Parameters

Parameter Name Description

X X-axis offset Specifies an X-axis offset [command units] of the coordinate

Y Y-axis offset Specifies a Y-axis offset [command units] of the coordinate

Z Z-axis offset Specifies a Z-axis offset [command units] of the coordinate

A A-axis offset Specifies an A-axis offset [command units] of the coordinate

B B-axis offset Specifies a B-axis offset [command units] of the coordinate

C C-axis offset Specifies a C-axis offset [command units] of the coordinate

Local Coordinate
System Setting

Set a Local Coordinate Sys­tem.

Release a Local Coordinate
System.

system.

system.

system.

system.

system.

system.

G52 X- Y- Z- A- B- C-

G52 X0 Y0 Z0 A0 B0 C0

Function

This command adds an offset specified by the parameter to the current coordinate system.

To release the offset, either set it to zero (0) or omit the all axis parameters.

This command releases Scaling (G50/G51), Mirroring (G50.1/G51.1), and Coordinate System Rotation
(G68/G69).

2 - 28

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

G53 Dimension Shift Cancel

Parameters

This instruction runs commands in the machine coordinate system.

Modal/Non-modal Non-modal
Modal group 00 Non-modal
Instruction format G53 X- Y- Z- A- B- C-

Relevant G codes

Parameter Name Description

X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Target Z-axis Position Specifies the destination position [command units] on the

A Target A-axis Position Specifies the destination position [command units] on the

B Target B-axis Position Specifies the destination position [command units] on the

C Target C-axis Position Specifies the destination position [command units] on the

G50, G51, G50.1, G51.1, G68, G69, G52, G54 to G59, G40, G41, G42, G43, G44,
G49

X-axis.

Y-a xi s.

Z-axis.

A-axis.

B-axis.

C-axis.

G53 Dimension Shift Cancel

2

Parameters

Function

This command runs rapid positioning commands in the machine coordinates, i.e., coordinates without
compensation. The command values are always handled as absolute values, and other movement
behaviors follow G00 Rapid Positioning.

This command releases Scaling (G50/G51), Mirroring (G50.1/G51.1), Coordinate System Rotation
(G68/G69), and the Local Coordinate System Set (G52). It temporarily releases Zero Shift (G54 to G59)
during operation, and maintains the current status of Inch Input/Metric Input (G20/G21). Tool Offset
(G43/G44/G49) and Cutter Compensation (G40/G41/G42) must be released prior to execution of this
command.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 29

2 G Code

G54 to G59 Select Work Coordi­nate System

These instructions change the current Work Coordinate System.

Modal/Non-modal Modal
Modal group 14 Coordinate System Selection

Instruction format

Relevant G codes G50, G51, G50.1, G51.1, G53, G68, G69

Parameters

This command does not have any parameters to set.

Function

Changes the current coordinate system to a specified one defined by the user by using the offsets of
X-, Y-, Z-, A-, B-, and C-axis.

This command releases Scaling (G50/G51), Mirroring (G50.1/G51.1), and Coordinate System Rotation
(G68/G69).

For offset settings of work coordinate system, refer to the Work Coordinate System Offset Parameters
of NJ/NY-series NC Controller User’s Manual (Cat. No. O030).

1st work coordinate system G54
2nd work coordinate system G55
3rd work coordinate system G56
4th work coordinate system G57
5th work coordinate system G58
6th work coordinate system G59

2 - 30

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

G17, G18, G19 Plane Selection

Parameters

Function

These instructions select a plane to be the basis of instructions.

Modal/Non-modal Modal
Modal group 02 Plane

X-Y Plane G17

Instruction format

Relevant G codes G02, G03, G41, G42, G68, G69

Z-X Plane G18
Y-Z Plane G19

This command does not have any parameters to set.

This command selects a plane, the reference of Circular Interpolation (G02/G03), Cutter Compensation
(G40/G41/G42), and Coordinate System Rotation (G68/G69). You can specify XY (G17), ZX (G18),
and YZ (G19). XY is specified at startup. Refer to G02, G03 Circular Interpolation on page 2-8, G40,
G41, G42 Cutter Compensation on page 2-40, G68, G69 Coordinate System Rotation on page 2-57 for
details.

G17, G18, G19 Plane Selection

2

Parameters

Precaution for Usage

Depending on plane selection of G17/G18/G19, some G codes change operation while others do not
change operation. The following shows operations changed according to plane selection.

• G41/G42 (Cutter Compen­sation):

• G43/G44 (Tool Offset): The tool length is compensated for Z-axis regardless of the selected plane. No

• G74/84 (Fixed Cycle): During a fixed cycle, the cutting is executed in the Z-axis direction regardless of

Refer to the following table for the relationship between plane selection and each G code.

G Code

G17 (XY Plane Selec­tion)

G18 (ZX Plane Selection)

G19 (YZ Plane Selection)

The cutter radius is compensated for the selected plane. An error will occur if
planes are switched during cutter compensation.

error will occur even if planes are switched during tool offset.

the selected plane.

G41/G42 (Cutter Com-

pensation)

The cutter radius is com­pensated for the XY
plane.
The cutter radius is com­pensated for the ZX plane.
The cutter radius is com­pensated for the YZ plane.

G43/G44 (Tool Offset) G74/84 (Fixed Cycle)

The tool length is compen­sated in the Z-axis direc­tion.

Fixed cycle operation is
fixed to the Z-axis direc­tion.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 31

2 G Code

G20 Inch Input, G21 Metric Input

These instructions toggle the units.

Modal/Non-modal Modal
Modal group 06 Unit

Instruction format

Relevant G codes ---

Parameters

This command does not have any parameters to set.

Function

Switches all the settings of the CNC coordinate system, command values, and the unit of current val­ues. You can select “inch” or “mm” for the unit. For example, for the maximum velocity of a CNC coordi­nate system, only the interpretation of the unit system can be changed without changing values.

Inch input G20
Metric input G21

2 - 32

NJ/NY-series G code Instructions Reference Manual (O031)

G90 Absolute Dimension,

Y

X

G90
G91

N03

N03

N02

N04

N04

N05

N01 G01
N02 X4 Y-2
N03 X-2 Y3
N04 X-2 Y-1
N05 X0 Y0

G91 Incremental Dimension

These instructions set a feed command to the Absolute Dimension or Incremental Dimension com-

Parameters

mand.

Modal/Non-modal Modal
Modal group 03 Distance

Instruction format

Relevant G codes

Absolute command G90
Incremental command G91

G00, G01, G02, G03, G28, G30, G31, G74, G84,
G50, G51, G50.1, G51.1, G68, G69

2 G Code

G90 Absolute Dimension, G91 Incremental

Dimension

2

Parameters

This command does not have any parameters to set.

Function

Absolute position mode and Incremental position mode is provided for operating functions. Executing
G90 enables absolute position mode for all axes in the CNC coordinate system, and moves the axes to
a specified position in the current coordinate system. Executing G91 enables Incremental position
mode for all axes in the CNC coordinate system, and moves the axes a certain distance from the last
command position. By default, absolute position mode is enabled for all axes.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 33

2 G Code

2 - 34

NJ/NY-series G code Instructions Reference Manual (O031)

2

Reference Point

Instruction Name Page

G28 Return to Reference Point P. 2-36
G30 Return to 2nd, 3rd and 4th Refer-

ence Point

P. 2-38

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 35

2 G Code

G28 Return to Reference Point

Modal/Non-modal Non-modal
Modal group 00 Non-modal
Instruction format G28 X- Y- Z- A- B- C-

Relevant G codes

Parameters

This instruction returns the tool automatically to the reference point via the specified middle point.

X X-axis middle point Specifies a middle point [command units] on the X-axis.
Y Y-axis middle point Specifies a middle point [command units] on the Y-axis.
Z Z-axis middle point Specifies a middle point [command units] on the Z-axis.
A A-axis middle point Specifies a middle point [command units] on the A-axis.
B B-axis middle point Specifies a middle point [command units] on the B-axis.
C C-axis middle point Specifies a middle point [command units] on the C-axis.

Function

The G28 command moves the tool to the optional middle point at rapid feed, then returns it to the refer­ence point. If the middle point is not specified, the tool returns directly to the reference point.

• The tool is moved to the reference point (position 0) via the middle point.

• The middle point follows the specifications for the Absolute Dimension (G90) and Incremental Dimen­sion (G91).

• The only axis that operates is the one for which the middle point is specified.

• Motion to each point follows the Rapid Positioning (G00) specifications.

• After the middle point is reached, this command releases Scaling (G50/G51), Mirroring
(G50.1/G51.1), and Coordinate System Rotation (G68/G69). During motion between the middle point
and reference point, this command also releases Zero Shift (G54 to G59) temporarily. It maintains the
current status of Inch Input (G20) and Metric Input (G21). Tool Offset (G43/G44/G49) and Cutter
Compensation (G40/G41/G42) must be released prior to execution of this command.

G90, G91, G50, G51, G50.1, G51.1, G68, G69, G54 to G59, G40, G41, G42, G43,
G44, G49

Parameter Name Description

2 - 36

NJ/NY-series G code Instructions Reference Manual (O031)

Programming Example

0

N03

N08

N07

(10, 10)

N08

N04

N05

N06

Y

X

30

20

10

5010

Middle position

Reference point

(0, 0)

After cutting operation, the tool moves to the middle position (10, 10) and returns to the reference point
(0, 0).

N01 G17 G91 G64 F1000
N02 M03 S500
N03 G00 X10 Y20
N04 G01 X40
N05 Y10
N06 X-40
N07 Y-10
N08 G28 X0 Y-10 // Return to reference point
N09 M30

2 G Code

G28 Return to Reference Point

2

Programming Example

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 37

2 G Code

G30 Return to 2nd, 3rd and 4th Reference Point

This instruction returns the tool to the 2nd, 3rd, or 4th reference point.

Modal/Non-modal Non-modal
Modal group 00 Non-modal

Instruction format

Relevant G codes

Parameters

X X-axis middle point Specifies a middle point [command units] on the X-axis.
Y Y-axis middle point Specifies a middle point [command units] on the Y-axis.
Z Z-axis middle point Specifies a middle point [command units] on the Z-axis.
A A-axis middle point Specifies a middle point [command units] on the A-axis.
B B-axis middle point Specifies a middle point [command units] on the B-axis.
C C-axis middle point Specifies a middle point [command units] on the C-axis.
P Reference point setting Reference point

Return to 2nd,
3rd or 4th Ref­erence Point

Parameter Name Description

Return to 2nd Reference Point G30 X- Y- Z- A- B- C­Return to 2nd Reference Point G30 P2 X- Y- Z- A- B- C­Return to 3rd Reference Point G30 P3 X- Y- Z- A- B- C­Return to 4th Reference Point G30 P4 X- Y- Z- A- B- C­G90, G91, G50, G51, G50.1, G51.1, G68, G69, G54 to G59, G40,
G41, G42, G43, G44, G49

Function

This command moves the tool to the 2nd, 3rd, or 4th reference point. The reference points follows the
settings. The reference points are identified by the P word. The operation for this command is the same
as that for the Return to Reference Point (G28).

2 - 38

NJ/NY-series G code Instructions Reference Manual (O031)

2

Compensation Functions

Instruction Name Page

G40/G41/G42 Cutter Compensation P. 2-40
G43/G44/G49 Tool Offset P. 2-51
G50/G51 Scaling P. 2-53
G50.1/G51.1 Mirroring P. 2-55
G68/G69 Coordinate System Rotation P. 2-57

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 39

2 G Code

G40, G41, G42 Cutter Compensa­tion

These instructions compensate the path by considering the tool diameter.

Modal/Non-modal Modal
Modal group 07 Tool radius

Instruction format

Relevant G codes G01, G02, G03, G17, G18, G19

Parameters

This command does not have any parameters to set.

Cancels tool compensation G40
Tool Compensation, left G41
Tool Compensation, right G42

2 - 40

NJ/NY-series G code Instructions Reference Manual (O031)

Function

Y

X

: Path after correction
: Specified path

N01 G17 // XY plane
N02 G01 G90
N03 G41 // or G42
N04 X15 Y10
N05 Y20
N06 X40
N07 Y10
N08 G40
N09 Y0

G41
(Left)

G42
(Right)

X

Z

: Path after correction
: Specified path

G41
(Left)

G42
(Right)

N09 X0

N08 G40

N07 X10

N06 Z40

N05 X20

N04 Z15 X10

N03 G41 // or G42

N02 G01 G90

N01 G18 // ZX plane

This command assumes the correction of cylindrical tool radius orthogonal to a plane. The correction
offset adapts automatically to two axes vertical to the plane, and the corrected path shifts from the com­manded path by the tool radius.

This command acts on G01, G02, and G03. The user can select XY, YZ, or ZX plane with Plane Selec­tion (G17/G18/G19).

G40 is Cutter Compensation Cancel, G41 is Cutter Compensation Left, and G42 is Cutter Compensa­tion Right.

The compensation cannot be started with Circular Interpolation (G02/G03).

The travel distance at startup must be greater than the cutter radius. However, when the tool moves
inside the arc, the cutter radius must be smaller than the circular command.

The extent of correction depends on the selected tool.

2 G Code

G40, G41, G42 Cutter Compensation

2

Function

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 41

2 G Code

Y

Z

: Path after correction
: Specified path

G41
(Left)

G42
(Right)

N09 Z0

N08 G40

N07 Z10

N06 Y40

N05 Z20

N04 Y15 Z10

N03 G41 // or G42

N02 G01 G90

N01 G19 // YZ plane

Compensated circular speed

When Circular Interpolation (G02/G03) is used simultaneously with G40, G41, or G42, the path of the
tool center differs from the commanded path that applies to the tool edge. This makes the velocity dif­ferent between the tool center and the commanded path.

The user can select the tool center path after correction or the tool edge path contacting with the com­mand to move the tool at the specified velocity.

2 - 42

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

X

Y

: Path after correction
: Specified path

Arc added

Tool diameter compensation: Corner circular interpolation (Added Arc)

When the angle of a corner exceeds 270 degrees, this command automatically adds an arc with the
same radius as the cutter radius.

G40, G41, G42 Cutter Compensation

2

Tool diameter compensation: Corner circular interpolation (Added Arc)

Start of Correction at Inside the Corner

Programmed path Programmed path

Startup move Startup move

Tool center path Tool center path

Linear interpolation operation

Cutter Compensation Cutter

Compensation

Circular interpolation
operation

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 43

2 G Code

Programmed
path

Programmed
path

Corrected linear
interpolation operation

Corrected
circular
interpolation
operation

Tool center path Tool center path

Startup
move

Startup
move

Cutter Compensation Cutter Compensation

Cutter
Compensation

Programmed path

Programmed path

Arc added

Arc added

Corrected linear
interpolation operation

Tool center path

Corrected
circular
interpolation
operation

Tool center path

Startup
operation

Startup
operation

Cutter Compensation

Cutter

Compensation

Cutter
Compensation

Start of Correction at Outside the Corner

 No arc is added

 An arc is added

2 - 44

NJ/NY-series G code Instructions Reference Manual (O031)

Correction processing at Inside the Corner

Programmed path Programmed path

Linear interpolation
operation

Linear
interpolation
operation

Linear interpolation operation

Circular
interpolation
operation

Tool center path

Tool center path

Cutter
Compensation

Cutter
Compensation

Cutter
Compensation

Cutter
Compensation

Programmed path Programmed path

Circular
interpolation
operation

Circular
interpolation
operation

Linear interpolation operation

Circular
interpolation
operation

Tool center path

Tool center path

Cutter
Compensation

Cutter
Compensation

Cutter
Compensation

Cutter
Compensation

2 G Code

G40, G41, G42 Cutter Compensation

2

Tool diameter compensation: Corner circular interpolation (Added Arc)

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 45

2 G Code

Programmed path Programmed path

Linear interpolation
operation

Linear interpolation
operation

Arc added

Circular
interpolation
operation

Tool center path Linear interpolation

operation

Arc added

Tool center path

Cutter Compensation

Cutter
Compensation

Cutter Compensation

Cutter
Compensation

Programmed path

Programmed path

Linear interpolation
operation

Arc added

Circular
interpolation
operation

Circular interpolation
operation

Circular interpolation
operation

Tool center path Tool center path

Arc added

Cutter
Compensation

Cutter
Compensation

Cutter

Compensation

Cutter
Compensation

Programmed path Programmed path

Linear interpolation
operation

Linear interpolation
operation

Circular
interpolation
operation

Tool center path Linear interpolation

operation

Tool center path

Cutter Compensation Cutter Compensation

Cutter Compensation

Cutter Compensation

Correction processing at Outside the Corner

 Cutter radius correction of outside corner with a deep angle

2 - 46

NJ/NY-series G code Instructions Reference Manual (O031)

 Cutter radius correction of outside corner with a shallow angle

Programmed path Programmed path

Linear interpolation
operation

Circular
interpolation
operation

Circular interpolation
operation

Tool center path Tool center path

Cutter
Compensation

Cutter Compensation

Cutter
Compensation

Cutter
Compensation

Programmed path Programmed path

Move of
cancel

Move of
cancel

Linear interpolation operation

Circular
interpolation
operation

Tool center path Tool center path

Cutter Compensation Cutter

Compensation

Programmed path

Programmed
path

Move of
cancel

Move of
cancel

Corrected linear
interpolation operation

Corrected
circular
interpolation
operation

Tool center path Tool center path

Cutter
Compensation

Cutter
Compensation

Cutter
Compensation

Termination of Correction at Inside the Corner

2 G Code

G40, G41, G42 Cutter Compensation

2

Tool diameter compensation: Corner circular interpolation (Added Arc)

 Cancellation of cutter radius correction at inside the corner

Termination of Correction at Outside the Corner

 No arc is added

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 47

2 G Code

X

Y

: Path after correction

: Specified path

 An arc is added

Corrected linear

Tool center path Tool center path

Arc added Arc added

Cutter
Compensation

interpolation operation

Programmed path

Cutter
Compensation

Cutter
Compensation

Corrected
circular
interpolation
operation

Move of
cancel

Detection of Overcut

Move of
cancel

Programmed path

2 - 48

When an overcut is detected, the operation stops and an error occurs.

To detect an overcut, set the Overcut operation mode to Overcut detection. For details, refer to the
NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030).

NJ/NY-series G code Instructions Reference Manual (O031)

Prevention of Overcut

X

Y

: Path after correction

: Specified path

2 G Code

G40, G41, G42 Cutter Compensation

2

Prevention of Overcut

Programming Example

When an overcut is detected, some operations are skipped to prevent the overcut. If the tool passes
the inside of an arc that is smaller than the tool, the error cannot be prevented. The user needs to
use a tool smaller than the arc, or change the arc that causes the error to a straight line.

To prevent an over-cut, set the Over-cut operation mode to Prevention of over-cuts. For details, refer
to the NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030).

The following program executes a series of operations from the start to the end of cutter compensation.
The operations consist of the following three steps.

1. Startup operation: Movement to the cutting surface with the first operation command that enabled the
cutter compensation by G41/42.

2. Correction operation: Cutting with operation commands between the startup operation and cancel opera­tion.

3. Cancel operation: Leaving from the cutting surface with the first operation command that disabled the
cutter compensation by G40.

N01 G500 G17 G64 G91 G01 F100
N02 M100 VA1 // Tool change Tool ID #1 (Cutter radius: 5)
N03 S300 M03
N04 G41 // Enables cutter compensation
N05 X10 // Startup operation
N06 X10 // Correction operation
N07 G40 // Disables cutter compensation
N08 X10 Y0 Z0 // Cancel operation
N09 M30

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 49

2 G Code

Use of M100 for transferring the tool change request to the sequence control program is an example.
When using this command, refer to the instruction manual provided by the machine tool manufacturer.

Y

N06

N08N05

0

X

Cutter Compensation of G41/G42 has the following restrictions for operation during correction.

• A series of operations such as the startup operation, correction operation, and cancel operation must
be provided.

• The modal that can be used during the correction operation is G01/02/03.

• G02/03 cannot be used for the startup operation and cancel operation.

• G00 cannot be used for the startup operation.

• The travel distance of the startup operation and the cancel operation must be equal to or greater than
the cutter radius.

• Edge surfaces cannot be switched (between G41 and G42) during the correction operation. For the
operation that the tool intersects the edge surface, cancel it once with G40 before switching edge
surfaces.

• During tool compensation, M code for which the M code output timing (M code setting) is Synchro­nous, or M code for which parameters are specified cannot be used. For the M code output timing,
refer to the NJ/NY-series NC Integrated Controller User’s Manual (Cat. No. O030).

• During correction operation, a single block execution or the program stop by M00/M01 is not allowed.

2 - 50

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

Z

G43 (+)

G44 (-)

N01 G01 G91
N02 G43
N03 X10 Z15
N04 X10
N05 X10 Z-15
N06 X10
N07 G49

X

: Coordinates after correction
: Original coordinates

G43, G44, G49 Tool Offset

Parameters

Function

These instructions compensate the path by considering the tool length.

Modal/Non-modal Modal
Modal group 08 Tool length offset

Tool length correction, in
positive direction

Instruction format

Relevant G codes G01, G02, G03, G17, G18, G19

Tool length correction, in
negative direction
Cancels tool offset G49

G43

G44

This command does not have any parameters to set.

This command immediately corrects the position in the Z-axis direction. G43 corrects the position in the
positive direction, G44 in the negative direction, and G49 terminates the correction. The extent of cor­rection depends on the selected tool.

G43, G44, G49 Tool Offset

2

Parameters

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 51

2 G Code

Programming Example

The following program executes a series of operations from the start to the end of tool offsetting. This
sample programming shows the change of tool length during the cutting operation.

N01 G17 G64 G90 G01 F100
N02 M100 VA1 // Tool change Tool ID #1 (Tool length: 8)
N03 G43 // Enables tool offset
N04 X10 Z-10
N05 X20
N06 M100 VA2 // Tool change Tool ID #2 (Tool length: 6)
N07 G43 // Enables tool offset
N08 X30 Z-10
N09 X40
N10 G49 // Disables tool offset
N11 X50 Z0 // Cancels tool offset
N12 M30

Use of M100 for transferring the tool change request to the sequence control program is an example.
When using this command, refer to the instruction manual provided by the machine tool manufacturer.

Z

0

-2

-4

-8

-10

10

N04

N05

20 30 40 50

X

N11

Path when tool offset is enabled

Path when tool offset is disabled

N08

N09

2 - 52

NJ/NY-series G code Instructions Reference Manual (O031)

G50, G51 Scaling

2 G Code

These instructions magnifies or compresses a commanded shape.

Modal/Non-modal Modal
Modal group 11 Scaling

Instruction format

Relevant G codes G00, G01, G02, G03, G90, G91

Parameters

X X-axis center point Specifies a center point [command units] on the X-axis.
Y Y-axis center point Specifies a center point [command units] on the Y-axis.
Z Z-axis center point Specifies a center point [command units] on the Z-axis.
I X-axis scaling magnifica-

J Y-axis scaling magnifica-

K Z-axis scaling magnifica-

P Scaling ratio of all axes Specifies a magnification ratio of all axes.

Disables scaling G50

When specifying the X, Y and

Enables scaling

Parameter Name Description

tion

tion

tion

Z-axis scales simultaneously
When specifying the X, Y and
Z-axis scales separately

Specifies an X-axis magnification ratio.

Specifies a Y-axis magnification ratio.

Specifies a Z-axis magnification ratio.

G51 X- Y- Z- P-

G51 X- Y- Z- I- J- K-

G50, G51 Scaling

2

Parameters

Function

The G50 and G51 scale the current coordinate system. G50 disables the scaling and G51 enables it. X,
Y, and Z parameters indicate the center point. If any of them is omitted, the omitted value is handled as
the current position. The values of X, Y, and Z parameters are handled as absolute position. The P
parameter indicates the magnification ratio of all of the X-, Y-, and Z-axis, whereas I, J, or K parameter
is the magnification ratio of each axis. The I, J, and K parameters are the magnification ratio of X-, Y-,
and Z-axis respectively. If any of I, J, and K parameters is omitted, the omitted value is handled as the
same size. P parameter is prioritized over I, J, and K parameters.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 53

2 G Code

N14

N17

(20, 15)

Y

X

25

20

20

15

5

0

10

Center point

Programming Example

The following program enlarges the circle defined in the subprogram to double size.

N11 G64 G90 G01 F100
N12 M03 S300
N13 G51 X20 Y15 P2 // Sets scaling to double.
N14 M98 P1000 // Cuts the figure of double size (indicated by the solid

line in the following figure).
N15 G50 // Disables scaling
N16 G01 X0 Y0
N17 M98 P1000 // Cuts the figure of original size (indicated by the

broken line in the following figure).
N18 M05
N19 M30

// Subprogram drawing a circle
// NC Program No.1000
N01 G17 G01 X20 Y10
N02 G02 X20 Y20 R5
N03 G02 X20 Y10 R5
N04 M99 // End of the subprogram

2 - 54

NJ/NY-series G code Instructions Reference Manual (O031)

G50.1, G51.1 Mirroring

2 G Code

G50.1, G51.1 Mirroring

These instructions invert the path on the specified coordinate system.

Modal/Non-modal Modal
Modal group 22 Mirroring

Instruction format

Relevant G codes G00, G01, G02, G03, G17, G18, G19

Parameters

X X-axis center point Specifies a center point [command units] on the X-axis.
Y Y-axis center point Specifies a center point [command units] on the Y-axis.
Z Z-axis center point Specifies a center point [command units] on the Z-axis.

Function

The G50.1 and G51.1 mirror the current coordinates. G50.1 disables mirroring, and releases the mirror­ing of symmetric axes specified by X, Y, and Z parameters in the instruction format. G51.1 enables mir­roring. In the instruction format, X, Y, and Z parameters indicate the symmetric axes. If any of them is
omitted, the axis is not mirrored. The values of X, Y, and Z parameters are handled as absolute posi­tions.

Disables mirroring G50.1
Enables mirroring G51.1 X- Y- Z-

2

Parameters

Parameter Name Description

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 55

2 G Code

0

N14N17

Y

X

30

30 4020

10

5010

Programming Example

The following program reverses a figure defined in the subprogram across the symmetric axes.

N11 G64 G90 G01 F100
N12 M03 S300
N13 G51.1 X30 // Line symmetry to X=30
N14 M98 P1000 // Cuts the mirrored figure by calling the subprogram

(indicated by the solid line in the following figure).
N15 G50.1
N16 G01 X0 Y0
N17 M98 P1000 // Cuts the original figure by calling the subprogram

(indicated by the broken line in the following figure).
N18 M05
N19 M30

// Subprogram drawing a figure
// NC Program No.1000
N01 G17 G01 X10 Y10
N02 G01 X20 Y10
N03 G01 X20 Y30
N04 G01 X15 Y30
N05 G03 X10 Y25 R5
N06 G01 X10 Y10
N07 M99 // End of the subprogram

As shown in the above figure, the rotation direction of the spindle axis does not change in mirroring. As
Up cut/Down cut are not maintained, adjust the rotation direction of the spindle axis according to your
purpose.

2 - 56

NJ/NY-series G code Instructions Reference Manual (O031)

G68, G69 Coordinate System Rotation

2 G Code

G68, G69 Coordinate System Rotation

These instructions rotate a specified figure.

Modal/Non-modal Modal
Modal group 16 rotation

Instruction format

Relevant G codes G00, G01, G02, G03, G17, G18, G19

Parameters

X X-axis center point Specifies a center point [command units] on the X-axis.
Y Y-axis center point Specifies a center point [command units] on the Y-axis.
Z Z-axis center point Specifies a center point [command units] on the Z-axis.
R Rotation angle Specifies a rotation angle [deg].

Function

The G68 and G69 rotate the current coordinates. G69 disables rotations, and G68 enables rotation. In
the instruction format, X, Y, and Z indicate the center point. If any of them is omitted, the omitted value
is handled as the current position. The X, Y, and Z values are handled as absolute positions. R indi­cates a rotation angle, and if it is omitted, an error occurs. The user can select XY, ZX, or YZ plane by
using the G17, G18, or G19.

Enables rotation G68 X- Y- Z- R-
Disables rotation G69

Parameter Name Description

2

Parameters

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 57

2 G Code

N15

N17

R90

N13

0

Y

X

10

Programming Example

The following program rotates a figure defined in the subprogram.

N11 G17 G64 G91 G01 F1000
N12 M03 S500
N13 X10
N14 G68 X10 Y0 R90 // Sets the rotation angle to 90°
N15 M98 P1000 // Cuts the rotated figure (indicated by the solid

line in the following figure)
N16 G69 // Disables rotation
N17 M98 P1000 // Cuts the unrotated figure (indicated by the

broken line in the following figure)
N18 M05
N19 M30

// Subprogram drawing a triangle
// NC Program No.1000
N01 G17 G01 X10 Y3
N02 Y-6
N03 X-10 Y3
N04 M99 // End of the subprogram

2 - 58

NJ/NY-series G code Instructions Reference Manual (O031)

2

Utilities

Instruction Name Page

G74 Left-handed Tapping Cycle P. 2-60
G80 Fixed Cycle Cancel P. 2-62
G84 Tapping Cycle P. 2-63
G98 Fixed Cycle Return to Initial Level P. 2-66
G99 Fixed Cycle Return to R Point

Level

P. 2-67

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 59

2 G Code

G74 Left-handed Tapping Cycle

This instruction performs reverse tapping machining.

Modal/Non-modal Modal
Modal group 09 Fixed cycle
Instruction format G74 X- Y- Z- R- P- K-
Relevant G codes G80, G98, G99, G90, G91

Parameters

X Target X-axis Position Specifies the destination position [command units] on the

Y Target Y-axis Position Specifies the destination position [command units] on the

Z Z point Specifies the position of Z point [command units].
R R point Specifies the position of R point [command units].
P Dwell time Specifies a stop time [ms] at the Z point.
K Number of repetitions Specifies a number of repetitions of the fixed cycle.

Function

Parameter Name Description

X-axis.

Y-a xi s.

This command is convenient for tapping. Internally, it is substituted by the code corresponding to the
following. This command uses an M code. Therefore, in order to execute the Left-handed Tapping
Cycle (G74) or Tapping Cycle (G84) correctly, the M-code reset queue needs to be processed by the
sequence control program correctly.

The X and Y words indicate the initial level, Z word indicates the Z point, R word the R point level, P
word the dwell time, and K word the number of repetitions. If the K word is omitted, it is assumed to be
K=1.

 When the CNC coordinate system has the spindle axis

G74 Xx Yy Zz Rr Pp Kk

//if G91 and G98 are activated
M19
//Execute below code k times
G00 Xx Yy //Initial level
G00 Zr //R point level
G01 Zz //Z point
G04 Pp //dwell
G01 Z-z //R point level
G00 Z-r //Initial level
//End of repetition
M5

//if G91 and G99 are activated
M19
//Execute below code k times
G00 Xx Yy //Initial level (first time) -> R point level (from the second)
(G00 Zr //R point level (first time only))
G01 Zz //Z point
G04 Pp //dwell
G01 Z-z //R point level

//End of repetition
M5

2 - 60

The spindle axis internally functions as the C-axis. In this case, positions of Z-axis and spindle axis syn­chronize.

NJ/NY-series G code Instructions Reference Manual (O031)

2 G Code

F

S

Spindle speed = Z-axis movement amount ×

G98

G99

X

Z

X

Z

Initial level

R point level

Z point

Initial level

R point level

Z point

If the spindle axis is assigned to the coordinate system, the number of rotations of spindle axis from the

G74 Left-handed Tapping Cycle

R point level to the Z point is as follows.

 When the CNC coordinate system does not have the spindle axis

G74 Xx Yy Zz Rr Pp Kk

//if G91 and G98 are activated

//Execute below code k times
G00 Xx Yy //Initial level
G00 Zr //R point level
M19
M04
G01 Zz //Z point
G04 Pp //dwell
M03
G01 Z-z //R point level
M04
G01 Z-r //Initial level

//if G91 and G99 are activated

//Execute below code k times
G00 Xx Yy //Initial level (first time) -> R point level (from the second)
(G00 Zr //R point level (first time only))
M19
M04
G01 Zz //Z point
G04 Pp //dwell
M03
G01 Z-z //R point level
M04

2

Programming Example

In this case, the Z-axis and spindle axis positions can be synchronized by using the sequence control
program.

When the spindle axis is not assigned to the coordinate system and to determine the number of rota­tions of spindle axis, consult the instruction manual provided by the machine tool manufacturer.

Programming Example

Refer to the programming example of G84 Tapping Cycle on page 2-63.

NJ/NY-series G code Instructions Reference Manual (O031)

2 - 61

2 G Code

G80 Fixed Cycle Cancel

This instruction cancels a fixed cycle.

Modal/Non-modal Modal
Modal group 09 Fixed cycle
Instruction format G80
Relevant G codes G74, G84

Parameters

This command does not have any parameters to set.

Function

This command must be inserted into the end of a fixed cycle.

2 - 62

NJ/NY-series G code Instructions Reference Manual (O031)