gsk GSK988T User Manual

Page 1

In this user manual we have tried to describe the matters concerning the operation of this CNC system to the greatest extent. However, it is impossible to give particular descriptions for all unnecessary or unallowable operations due to length limitation and

products application conditions；Therefore, the items not presented

herein should be regarded as “impossible” or “unallowable”.

Copyright is reserved to GSK CNC Equipment Co., Ltd. It is illegal for any organization or individual to publish or reprint this manual. GSK CNC Equipment Co., Ltd. reserves the right to ascertain their legal liability.

Page 2

GSK988T Turning CNC System User Manual

Preface

Your Excellency,

We are honored by your purchase of this GSK 988T Turning CNC

System made by GSK CNC Equipment Co., Ltd.

This book is User Manual “Programming and Operation”.

To ensure safe and effective running, please read this manual carefully

before installation and operation.

Warning

Accident may occur by improper connection and operation！This

system can only be operated by authorized and qualified personnel.

Special caution:

The power supply fixed on/in the cabinet is exclusively used for the

CNC system made by GSK.

It can't be applied to other purposes, or else it may cause serious

danger!

Page 3

Cautions

■ Delivery and storage

● Packing box over 6 layers in pile is unallowed.

● Never climb the packing box, stand on it or place heavy objects on it.

● Do not move or drag the products by the cables connected to it.

● Forbid collision or scratch to the panel and display screen.

● Avoid dampness, insolation and drenching.

■

Open-package inspection

● Confirm that the products are the required ones.

● Check whether the products are damaged in transit.

● Confirm that the parts in packing box are in accordance with the packing list.

● Contact us in time if any inconsistence, shortage or damage is found.

Contents

■ Connection

● Only qualified personnel can connect the system or check the connection.

● The system must be earthed, and the earth resistance must be less than 0.1Ω.

The earth wire cannot be replaced by zero wire.

● The connection must be correct and firm to avoid any fault or unexpected consequence.

● Connect with surge diode in the specified direction to avoid damage to the system.

● Switch off power supply before plugging out or opening electric cabinet.

■ Troubleshooting

● Switch off power supply before troubleshooting or changing components.

● Check the fault when short circuit or overload occurs. Restart can only be done

after troubleshooting.

● Frequent switching on/off of the power is forbidden, and the interval time should be at least 1 min.

III

Page 4

GSK988T Turning CNC System User Manual

ANNOUNCEMENT!

z This manual describes various possibilities as much as possible. However,

operations allowable or unallowable cannot be explained one by one due to

so many possibilities that may involve with, so the contents that are not

specially stated in this manual shall be regarded as unallowable.

WARNING！

z Please read this manual and a manual from machine tool builder carefully

before installation, programming and operation, and strictly observe the

requirements. Otherwise, products and machine may be damaged,

workpiece be scrapped or the user be injured.

CAUTION！

z Functions, technical indexes (such as precision and speed) described in

this user manual are only for this system. Actual function configuration and

technical performance of a machine tool with this CNC system are

determined by machine tool builder’s design, so functions and technical

indexes are subject to the user manual from machine tool builder.

z Though this system adopts standard operation panel, the functions of the

keys on the panel are defined by PLC program (ladder diagram). It should be

noted that the keys functions described herein are for the standard PLC

program (ladder diagram).

z For functions and effects of keys on control panel, please refer to the user

manual from machine tool builder.

Page 5

Contents

Safety Responsibility

Manufacturer’s Responsibility

——Be responsible for the danger which should be eliminated and/or controlled on design and configuration of the provided CNC systems and accessories. ——Be responsible for the safety of the provided CNC systems and accessories. ——Be responsible for the provided information and advice for the users.

User’s Responsibility

——Be trained with the safety operation of CNC system and familiar with the safety operation procedures. ——Be responsible for the dangers caused by adding, changing or altering to the original CNC systems and the accessories.

——Be responsible for the failure to observe the provisions for operation, adjustment,

maintenance, installation and storage in the manual.

This manual is subject to change without further notice.

This manual is reserved by end user. We are full of heartfelt gratitude to you for supporting us in the use of GSK’s products.

Page 6

GSK988T Turning CNC System User Manual

Page 7

Contents

Ⅰ PROGRAMMING ..........................................................................................................................1

Chapter I Programming Fundamentals ............................................................................................3

1.1 GSK988T Introduction ........................................................................................................3

1.2 CNC system of machine tools and CNC machine tools......................................................5

1.3 Programming Fundamentals...............................................................................................7

1.3.1 Coordinates definition ...............................................................................................7

1.3.2 Increment system .....................................................................................................9

1.3.3 Max. travel ..............................................................................................................10

1.3.4 Reference position..................................................................................................10

1.3.5 Machine coordinate system ....................................................................................10

1.3.6 Workpice coordinate system................................................................................... 11

1.3.7 Local coordinate system ......................................................................................... 11

1.3.8 Interpolation function ..............................................................................................11

1.4 Coordinate Value and Dimension......................................................................................12

1.4.1 Absolute programming and incremental programming ...........................................12

1.4.2 Diameter programming and radius programming ...................................................13

1.4.3 Decimal programming.............................................................................................14

1.4.4 Conversion between the metric and the inch ..........................................................14

1.4.5 Linear axis and rotary axis ......................................................................................15

1.5 Structure of an NC Program..............................................................................................15

1.5.1 Program name ........................................................................................................16

1.5.2 Block format............................................................................................................16

1.5.3 Word .......................................................................................................................17

1.5.4 Block number..........................................................................................................26

1.5.5 Main program and subprogram...............................................................................26

1.6 Program Run ....................................................................................................................27

1.6.1 Sequence of program run .......................................................................................27

1.6.2 Execution sequence of word...................................................................................28

Chapter II G Commands ................................................................................................................29

2.1 Summary ..........................................................................................................................29

2.1.1 G command classification .......................................................................................29

2.1.2 Omitting word input.................................................................................................31

2.1.3 Related definitions ..................................................................................................33

2.2 Rapid Traverse (Positioning) G00.....................................................................................33

2.3 Linear Interpolation G01 ...................................................................................................34

2.4 Arc Interpolation G02, G03 ...............................................................................................35

2.5 Dwell G04 .........................................................................................................................38

2.6 Cylindrical Interpolation 7.1...............................................................................................39

2.7 Polar Coordinate Interpolation G12.1, G13.1 ....................................................................43

2.8 Metric/Inch Switch G20, G21 ............................................................................................45

2.9 Stored Travel Check G22, G23 .........................................................................................45

2.10 Skip Interpolation G31 ....................................................................................................46

2.11 Automatic Tool Offset G36, G37 ...................................................................................48

2.12 Reference Position Function...........................................................................................50

VII

Page 8

GSK988T Turning CNC System User Manual

2.12.1 Reference position return G28.............................................................................. 50

2.12.2 2

2.13 Related Function of Coordinate System .........................................................................52

2.13.1 Selecting machine coordinate system position G53 .............................................53

2.13.2 Workpiece coordinate system setting G50 ...........................................................54

2.13.3 Workpiece coordinate system selection command G54～G59............................. 55

2.13.4 Local coordinate system setting G52....................................................................57

2.13.5 Level selection command G17～G19 ................................................................... 59

2.13.6 Exact stop mode G61/cutting mode G64.............................................................. 59

2.14 Fixed Cycle Command ...................................................................................................60

2.14.1 Axial cutting cycle G90 .........................................................................................60

2.14.2 Radial cutting cycle G94 .......................................................................................63

2.15 Multiple Cycle Commands .............................................................................................. 66

2.15.1 Axial Roughing Cycle G71.................................................................................... 66

2.15.2 Radial Roughing Cycle G72 ............................................................................... 72

2.15.3 Closed Cutting Cycle G73 ....................................................................................77

2.15.4 Finishing Cycle G70 .............................................................................................82

2.15.5 Axial Grooving Multiple Cycle G74 .......................................................................83

2.15.6 Radial Grooving Multiple Cycle G75 .....................................................................86

2.15.7 Notes for multi cycle machining ............................................................................ 89

2.16 Threading Cutting ........................................................................................................... 90

2.16.1 Thread Cutting with Constant Lead G32............................................................... 90

2.16.2 Thread cutting with variable lead G34 ..................................................................93

2.16.3 Thread cutting cycle G92......................................................................................95

2.16.4 Multiple thread cutting cycle G76..........................................................................97

2.17 Constant Surface Speed Control G96, Constant Rotational Speed Control G97..... 103

2.18 Feedrate per Minute G98, Feedrate per Rev G99 ................................................... 105

2.19 Drilling/Boring Fixed Cycle Command ..........................................................................106

2.19.1 End drilling cycle G83 /side drilling cycle G87 ....................................................107

2.19.2 End Boring CycleG85 / Side Boring Cycle G89 .................................................. 111

2.19.3 Cancelling Drilling/Boring G80............................................................................ 112

2.19.4 Notes for Drilling/Boring Cycle ............................................................................ 112

2.20 Tapping Cycle Command.............................................................................................. 112

2.20.1 Tapping Mode ..................................................................................................... 113

2.20.2 End Rigid Tapping Cycle (G84) / Side Rigid Tapping Cycle (G88)...................... 114

2.20.3 End Common Tapping Cycle (G84) /Side Common Tapping Cycle (G88) .......... 120

2.21 Automatic Chamfering Function.................................................................................... 123

2.22 Macro Command ..........................................................................................................126

2.22.1 Variable...............................................................................................................126

2.22.2 System variable ..................................................................................................127

2.22.3 Operation and jump command ...........................................................................131

2.22.4 Macro program statement and NC statement ..................................................... 136

2.22.5 Macro program call ............................................................................................. 136

, 3rd, 4th reference position return G30 .............................................................51

Chapter Ⅲ MSTF Commands..................................................................................................... 139

3.1 M (Miscellaneous Function) ............................................................................................139

3.1.1 End of program M02 .............................................................................................139

VIII

Page 9

Contents

3.1.2 End of program run M30 .......................................................................................139

3.1.3 Program stop M00 ................................................................................................139

3.1.4 Optional stop M01.................................................................................................140

3.1.5 Subprogram call M98 .........................................................................................140

3.1.6 Subprogram Call M198.........................................................................................141

3.1.7 Return from Subprogram M99............................................................................141

3.1.8 The Following M commands for standard ladder(some functions modified by K

parameters)......................................................................................................................142

3.1.9 M Commands defined by standard PLC ladder ....................................................143

3.2 Spindle Function .............................................................................................................143

3.2.1 Spindle speed analog voltage control ...................................................................143

3.2.2 Spindle override....................................................................................................144

3.3 Tool Function ..................................................................................................................144

3.3.1 Tool offset .............................................................................................................144

3.3.2 Tool Life Management ..........................................................................................147

Chapter IV Tool Nose Radius Compensation...............................................................................151

4.1 Application ......................................................................................................................151

4.1.1 Overview...............................................................................................................151

4.1.2 Imaginary tool nose direction ................................................................................152

4.1.3 Compensation value setting..................................................................................155

4.1.4 G40/G41/G42 command function .........................................................................156

4.1.5 Compensation direction ........................................................................................157

4.1.6 Cautions ...............................................................................................................159

4.1.7 Application ............................................................................................................1

4.2 Tool Nose Radius Compensation Offset Path.................................................................161

4.2.1 Inner and outer side ..............................................................................................161

4.2.2 Tool traversing when starting tool .........................................................................161

4.2.3 Tool traversing in Offset mode ..............................................................................163

4.2.4 Tool traversing in Offset canceling mode ..............................................................168

4.2.5 Tool interference check......................................................................................... 169

4.2.6 Commands for canceling compensation vector temporarily .................................171

4.2.7 Particulars.............................................................................................................174

Ⅱ OPERATION ...........................................................................................................................181

Chapter Ⅰ Overview.....................................................................................................................183

1.1 Operation Overview ........................................................................................................183

1.2 System Setting................................................................................................................184

1.3 Display ............................................................................................................................185

1.4 System............................................................................................................................187

1.4.1 System panel........................................................................................................187

1.4.2 System key definitions ..........................................................................................188

1.5 Machine Operation Panel ...............................................................................................190

1.5.1 Division of machine operation panel ..................................................................... 190

1.5.2 State indicator and press key definition on the panel............................................191

Chapter Ⅱ Power on, Power off and Safety Protection ................................................................196

Page 10

GSK988T Turning CNC System User Manual

2.1 Power on ........................................................................................................................196

2.2 Power off.........................................................................................................................197

2.3 Overtravel Protection ......................................................................................................197

2.4 Overtravel Protection in Memory Travel Limit .................................................................197

2.5 Emergence Operation..................................................................................................... 199

2.5.1 Reset ....................................................................................................................199

2.5.2 Emergency stop.................................................................................................... 199

2.5.3 Feed hold..............................................................................................................199

2.5.4 Cutting off power supply ....................................................................................... 199

Chapter Ⅲ Windows ................................................................................................................... 200

3.1 Position Display Window ................................................................................................205

3.1.1 Absolute coordinate window ................................................................................. 206

3.1.2 Relative coordinate display................................................................................... 207

3.1.3 Machine coordinate display ..................................................................................208

3.1.4 Comprehensive coordinate...................................................................................208

3.1.5 Setting the relative coordinate ..............................................................................209

3.1.6 Switching between the mode and the comprehensive message ..........................210

3.1.7 Clearing workpiece count ..................................................................................... 211

3.1.8 Clearing run time .................................................................................................. 211

3.2 Program Window ............................................................................................................ 212

3.2.1 Local directory and U disk directory......................................................................212

3.2.2 MDI program......................................................................................................... 213

3.2.3 Item/times ............................................................................................................. 214

3.3 System Window .............................................................................................................. 214

3.3.1 System parameter setting and rewriting window ..................................................215

3.3.2 Screw pitch compensation setting and rewriting window...................................... 218

3.3.3 System message and operation authority levels ..................................................219

3.3.4 System file management ......................................................................................222

3.3.5 Ladder diagram ....................................................................................................223

3.4 Setting Window............................................................................................................... 229

3.4.1 Tool offset setting.................................................................................................. 229

3.4.2 CNC setting window .............................................................................................233

3.4.3 Macro variable window .........................................................................................238

3.5 Message Window ...........................................................................................................239

3.5.1 Alarm message check window .............................................................................240

3.5.2 Alarm record check window.................................................................................. 241

3.5.3 Diagnosis window................................................................................................. 242

3.5.4 Oscillograph window............................................................................................. 245

3.5.5 GSK-CAN window ................................................................................................248

3.6 Graph Window ................................................................................................................ 249

3.6.1 Setting graph parameter .......................................................................................249

3.6.2 Processing graph path.......................................................................................... 250

3.6.3 Simulation graph................................................................................................... 251

3.7 Help Windows................................................................................................................. 252

Chapter Ⅳ Editing and Managing a Program .............................................................................254

Page 11

Contents

4.1 Searching, Creating, Executing and Opening a Program ...............................................254

4.1.1 Searching a program ............................................................................................254

4.1.2 Creating a program ...............................................................................................254

4.1.3 Executing a program.............................................................................................255

4.1.4 Opening a program...............................................................................................256

4.2 Renaming, Outputting, Deleting and Arraying Programs, Saving a Program as.............257

4.2.1 Renaming a program ............................................................................................257

4.2.2 Saving a program as.............................................................................................258

4.2.3 Deleting a program ...............................................................................................259

4.2.4 Outputting a program............................................................................................259

4.2.5 Arraying programs ................................................................................................260

4.3 Editing and Rewriting a Program ....................................................................................260

4.3.1 Editing a program .................................................................................................260

4.3.2 Rewriting a program .............................................................................................261

4.3.3 Shortcut key..........................................................................................................262

4.4 Block Comment...............................................................................................................263

4.5 Generating a Block Number............................................................................................263

4.6 Background Editing a Program .......................................................................................263

Chapter Ⅴ Manual Operation .....................................................................................................264

5.1 Manual Reference Position Return .................................................................................264

5.2 Manual Feed...................................................................................................................265

5.3 Increment Feeding ..........................................................................................................266

5.4 MPG Feeding...............................................................................................................

...267

Chapter Ⅵ Auto Operation............................................................................................................270

6.1 Auto Running ..................................................................................................................270

6.1.1 Selecting the running program..............................................................................270

6.1.2 Program running ...................................................................................................271

6.1.3 Running from any block ........................................................................................272

6.1.4 Skip.......................................................................................................................272

6.1.5 G31 skip ...............................................................................................................273

6.1.6 Stop auto running..................................................................................................273

6.2 MDI Running ...................................................................................................................274

6.2.1 Editing and running the program in MDI mode .....................................................274

6.2.2 Running from any block ........................................................................................275

6.2.3 Stop MDI running .................................................................................................. 275

6.3 DNC Running..................................................................................................................275

6.4 Auto Running Control......................................................................................................278

6.4.1 Machine and miscellaneous function lock.............................................................278

6.4.2 Dry run..................................................................................................................279

6.4.3 Single block running .............................................................................................280

6.4.4 Feedrate override .................................................................................................280

6.4.5 Rapid traverse override ........................................................................................281

Chapter Ⅶ Tool Offset and Setting Tools ....................................................................................282

7.1 Setting the Tool Offset and the Wearing Values..............................................................282

Page 12

GSK988T Turning CNC System User Manual

7.1.1 Direct input method ..............................................................................................282

7.1.2 Measuring mode................................................................................................... 283

7.1.3 +input mode.......................................................................................................... 284

7.1.4 C input method .....................................................................................................285

7.1.5 Clearing the offset value or the wearing value ......................................................286

7.2 Fixed-Point Tool Setting ..................................................................................................287

7.3 Trial Cut Toolsetting ........................................................................................................287

7.4 Position Record ..............................................................................................................290

7.5 Automatic Tool Compensation ........................................................................................290

Chapter Ⅷ Setting and Display Graphs ...................................................................................... 292

8.1 Setting the Graph Parameter .......................................................................................... 292

8.2 Path Graph Display and Operation ................................................................................. 293

8.3 Simulation graph display and operation ..........................................................................294

Chapter Ⅸ U disk Use ................................................................................................................ 296

9.1 Sending a Program......................................................................................................... 296

9.2 Backup Value..................................................................................................................297

9.2.1 System file backup ...............................................................................................297

9.2.2 Servo parameter backup ......................................................................................298

Chapter Ⅹ Processing Examples ................................................................................................. 301

10.1 Outer End Face Machining ...........................................................................................301

10.2 Compound Machining................................................................................................... 304

Chapter Ⅺ Parameters ............................................................................................................... 310

11.1 Parameters Related to System Setting ......................................................................... 311

11.2 Parameters Related to Interfaces of Input and Output .................................................. 311

11.3 Parameters Related to Axis Control/Setting Unit........................................................... 311

11.4 Parameters Related to Coordinate System................................................................... 315

11.5 Parameters Related to the Stroke Detection................................................................. 317

11.6 Parameters Related to Feedrate ................................................................................... 320

11.7 Parameters Related to Control of Acceleration and Deceleration ................................. 324

11.8 Parameters Related to Servo and Backlash Compensation .........................................326

11.9 Parameters Related to Input/Output .............................................................................330

11.10 Parameters Related to Display and Editing................................................................. 332

11.11 Parameters Related to Programming .......................................................................... 334

11.12 Parameters Related to Screw Pitch Error Compensation ...........................................336

11.13 Parameters Related to the Spindle Control................................................................. 339

11.14 Parameters Related to the Tool Compensation........................................................... 344

11.15 Parameters Related to the Canned Cycle................................................................. 347

11.15.1 Parameter of the Drilling Canned Cycle ............................................................347

11.15.2 Parameters Related to the Thread Cutting Cycle.............................................. 348

11.15.3 Parameters Related to the Combined Canned Cycle .......................................348

11.16 Parameters Related to the Rigid Tapping.................................................................... 349

11.17 Parameters Related to the Polar Coordinate Interpolation.......................................... 351

11.18 Parameters Related to the User Macro Program ........................................................ 352

XII

Page 13

Contents

11.19 Parameters Related to Skip Function..........................................................................353

11.20 Parameters Related to Graphic Display ......................................................................355

11.21 Parameters Related to Run Hour and Parts Count Display.........................................355

11.22 Parameters Related to MPG Feed ..............................................................................356

11.23 Parameters Related to PLC Axis Control ....................................................................357

11.24 Parameters Related to Basic Function........................................................................360

11.25 Parameters Related to GSK-CAN Communication Function ......................................361

Appendix 1 Alarm List ..................................................................................................................363

1.1 Program Alarms (P/S Alarms) .........................................................................................363

1.2 Parameter Alarms ...........................................................................................................372

1.3 Pulse Encoder Alarms.....................................................................................................373

1.4 Servo Alarms ..................................................................................................................373

1.5 Overtravel Alarms ...........................................................................................................373

1.6 Spindle Alarms................................................................................................................374

1.7 System Alarms................................................................................................................374

1.8 Communication prompt on the operation panel ..............................................................375

1.9 GSK-CAN Communication Prompts ...............................................................................375

1.10 Servo Inner Alarms .......................................................................................................377

Appendix 2 Standard Ladder Function Allocation.........................................................................381

2.1 X, Y Addresses Definition................................................................................................381

2.2 Standard Operation Panel...............................................................................................384

2.2.1 Address X .............................................................................................................384

2.2.2 Address Y .............................................................................................................386

2.3 Standard PLC Parameter Instruction ..............................................................................389

2.3.1 Parameter K..........................................................................................................389

2.3.2 Parameter DT .......................................................................................................390

2.3.3 Parameter DC.......................................................................................................391

2.3.4 Parameter D .........................................................................................................391

2.4 PLC(Address A) Alarms (the Followings are Referred to V2.03b)...................................392

Appendix 3 Installation .................................................................................................................394

3.1 GSK988T Appearance Dimension ..................................................................................394

3.2 Machine Operation Panel MPU02A of GSK988T............................................................395

3.3 Machine Operation Panel MPU02B Appearance dimension of GSK988T ......................396

3.4 GSK988T-H Appearance Dimension...............................................................................397

3.5 Appearance Dimension of GSK988T-H Operation panel................................................397

Appendix 4 Operation List............................................................................................................399

XIII

Page 14

GSK988T Turning CNC System User Manual

XIV

Page 15

Chapter 1 Programming Fundamentals

Ⅰ Programming

Ⅰ PROGRAMMING

Page 16

GSK988T Turning CNC System User Manual

Ⅰ Programming

Page 17

Chapter Ⅰ Programming Fundamentals

Chapter I Programming Fundamentals

1.1 GSK988T Introduction

GSK988T is exclusive to the slant bed CNC turning machine and turning center with the horizontal and the vertical structures. It uses 400MHz high-performance process to control 5 feed axes(including Cs axis) and 2 spindles, communicates with the servo unit through GSK-CAN serial

bus, and its matched servo motor uses the high-resolution absolute encoder to realize 0.1μm

position precision, which can meet the requirements of high-precision turning and milling compound machining. It has the network interface to support the remote monitor and file transmission and to meet the network teaching and workshop management. GSK988T is the best choice for the slant bed CNC turning and turning center.

Programming Ⅰ

Fig. 1-1 GSK988T appearance

Technical characteristics

5 feed axes（including Cs axis）, 3-axis link, 2 analog spindles to realize the turning, milling compound

machining Command unit 1μm and 0.1μm, max. speed 60m/min（max. speed 24m/min in 0.1μm）

Optional to GSK-CAN servo unit to read/write the servo parameter and monitor servo unit Extended I/O unit and GSK-CAN axis through serial bus Nested many PLC programs, on-line editing, real-time monitoring PLC ladder Part programs edited on the background Network interface, remote monitoring and file transmission USB interface, U disc file operation, system allocation and software upgrading

8.4 inch truecolor LCD, two-dimensional motion path and solid graph display

Page 18

GSK988T Turning CNC System User Manual

Technical specifications

Controllable axes

Max. controllable axes：5（including Cs axis） Max. link axes：3

PLC controllable axes：5

Ⅰ Programming

Feed axis function

Least command unit：0.001mm, 0.0001mm Least command range：±99999999× least command unit

Rapid traverse speed：max. 60m/min in 0.001mm command unit, max. 24m/min in 0.0001mm

command unit Rapid override：F0, 25%, 50%, 100% real-timing tuning

Cutting feedrate:

0.01 mm/min～60000 mm/min or 0.01 inch/min～4000 inch/min（G98: feed per minute）

0.01 mm/rev～500 mm/r or 0.01 inch/rev～9.99 inch/rev（G99: feed per revolution） Feedrate override：0～150% 16-level real-time tuning

Interpolation mode: linear, arc, thread, polar interpolation, and rigid tapping

Thread function

Thread type: constant pitch straight thread/taper thread/end thread, variable pitch straight thread/taper thread/end thread Thread head：1~99 heads

Thread pitch： 0.01mm～500mm（metric thread）or 0.01inch～9.99inch（inch thread） Thread run-out：thread lenght, angle, speed can be set

Acceleration/deceleration function

Cutting feed: linear, exponential Rapid traverse: linear

Thread cutting: linear, exponential Initial speed, terminal speed and time of acceleration/deceleration are set by the parameter

Spindle function

2-channel 0V～10V analog voltage output，2-channel spindle encode feedback, double-spindle

control Spindle speed: spindle speed specified by S or PLC signal, its range: 0rpm～20000rpm

Spindle override：50%～120% 8-level real-time tuning

Spindle constant surface control Rigid tapping

Tool function

Tool length compensation（tool offset）：99 groups Tool wear compensation：99 groups of tool wear compensation data

Tool nose radius compensation（C type）

Toolsetting mode: fixed-point toolsetting, trial-cutting toolsetting, reference position return toolsetting Offset execution mode: modifying coordinate mode, tool traverse mode

Precision compensation

Backlash compensation: compensation range (-9999~9999)× check unit Memory pitch error compensation：1024 compensation points，compensation point number of each is

set by the parameter, each point compensation range (-700~700) × check unit

PLC function

13 basic commands, 30 functional commands

Page 19

Chapter Ⅰ Programming Fundamentals

PLC ladder on-line edit, real-time monitoring

2-level PLC program, up to 5000 steps, the 1 Many PLC programs（up to 16 programs），the current running PLC program can be selected

level program refresh period

I/O unit

Basic I/O：40 input /32 output Operation panel I/O：96 input/96 output

Human-computer interface

Display in Chinese, English and others Two-dimensional tool path and solid graph display

Servo state monitoring Servo parameter on-line allocation Real-time clock On-line help

Operation management

Operation mode: Auto, Manual, Edit, MDI, DNC, MPG, Reference position return Multi-level operation Authorization Management

Alarm log Timed stop

Program edit

Program capacity：36M, 10000 programs（including subprogram and macro program） Edit mode: full-screen edit, part program edit on the background

Edit function：searching, modifying and deleting program/block/word, copying/deleting block

Program format: ISO code, word without blank space, relative coordinates, absolute coordinate compound programming Macro command: statement macro command program Program call: macro program call with parameters, 12-level subprogram nesting Grammar check: executing the rapid grammar check for the program(do not run the program) after it has been edit

Communication function

RS232 interface: part program and parameter transmission, DNC machining, upgrading PLC program and system software U disc USB：U disc file operation, U disc file directly machining, upgrading PLC program and system

software U disc LAN： remote monitoring, network DNC machining, file transmission, remotely upgrading PLC

program, system software

Safety function

Emergency stop Hardware travel limit

Many storage travel checks Data backup and recover

Programming Ⅰ

1.2 CNC system of machine tools and CNC machine tools

CNC machine tool is an electro-mechanical integrated product, composed of Numerical Control Systems of Machine Tools, machines, electric control components, hydraulic components, pneumatic components, lubricating, cooling and other subsystems (components), and CNC systems of machine tools are control cores of CNC machine tools. CNC systems of machine tools are made up of computerized numerical control(CNC), servo (stepper) motor drive devices, servo (or stepper) motor

Page 20

GSK988T Turning CNC System User Manual

etc. Operational principles of CNC machine tools: according to requirements of machining technology, edit user programs and input them to CNC, then CNC outputs motion control commands to the servo (stepper) motor drive devices, and last the servo (or stepper) motor completes the cutting feed of machine tool by mechanical driving device; logic control commands in user programs to control

Ⅰ Programming

spindle start/stop, tool selections, cooling ON/OFF, lubricant ON/OFF are output to electric control systems of machine tools from CNC, and then the electric control systems control output components including buttons, switches, indicators, relays, contactors and so on. Presently, the electric control systems are employed with Programmable Logic Controller (PLC) with characteristics of compact, convenience and high reliance. Thereof, the motion control systems and logic control systems are the main of CNC machine tools. The system has simultaneously motion control and logic control function to control two axes of CNC machine tool to move, and has PLC function. Edit PLC programs (ladder diagram) according to requirements of input and output control of machine tool and then download them to GSK988T Turning Machine CNC system, which realizes the required electric control requirements of machine tool, is convenient to electric design of machine tool and reduces cost of CNC machine tool. Softwares used for controlling GSK988T Turning Machine CNC system are divided into system software (NC for short) and PLC software (PLC for short). NC system is used for controlling display, communication, edit, decoding, interpolation and acceleration/deceleration, and PLC system for controlling explanations, executions, inputs and outputs of ladder diagrams. Standard PLC programs are loaded (except for the special order) when GSK980TDa Turning Machine CNC System is delivered, concerned PLC control functions in following functions and operations are described according to control logics of standard PLC programs, marking with “Standard PLC functions” in GSK980TDa Turning CNC System User Manual. Refer to Operation Manual of machine manufacturer about functions and operations of PLC control because the machine manufacturer may modify or edit PLC programs again. Programming is a course of workpiece contours, machining technologies, technology parameters and tool parameters being edit into part programs according to special CNC programming G codes. CNC machining is a course of CNC controlling a machine tool to complete machining of workpiece according requirements of part programs. Technical flow of CNC machining is shown in Fig. 1-2.

Page 21

Chapter Ⅰ Programming Fundamentals

Analyse workpiece drawings and confirm machining processing

Edit part programs and record into CNC

Test part programs and execute trial run

O0001； G00 X3.76 Z0； G01 Z-1.28 F50； … M30；％

Programming Ⅰ

Execute toolsetting and set tool offsets and coordinates

Run part programs and machine workpiece

Check part dimension and modify part programs and compensations

The machining ends and the workpiece is formed

Fig. 1-2

1.3 Programming Fundamentals

1.3.1 Coordinates definition

The following figure is the sketch of CNC turning:

Page 22

GSK988T Turning CNC System User Manual

Ⅰ Programming

Fig. 1-3

GSK988T uses a rectangular coordinate system composed of X, Z axis. X axis is perpendicular with axes of spindle and Z axis is parallel with axes of spindle; negative directions of them approach to the workpiece and positive ones are away from it.

Parameter NO.1020 can set and modify program names for each axis and their responding relationship is as follows:

Table 1-3（a）

Axis name Setting value Axis name Setting value

X 88 Z 90

Y 89 A 65

B 66 C 67

There is a front tool post and a rear tool post of NC turning machine according to their relative position between the tool post and the spindle, Fig. 1-5 is a coordinate system of the front tool post and Fig. 1-6 is a rear toolpost one. It shows exactly the opposite of X axes, but the same of Z axes from figures. In the manual, it will introduce programming application with the front tool post coordinate system in the following figures and examples.

Fig.1-4 Front tool post coordinate system Fig.1-5 Rear tool post coordinate system

Page 23

Chapter Ⅰ Programming Fundamentals

1.3.2 Increment system

Increment system includes least input increment (input) and least command increment (output). Least input increment is the least unit of programming movement distance. Least command increment is the least unit of tool movement on the machine tool. Their unit: mm, inch or degree. Increment systems are separately IS-B and IS-C. Bit 1 of NO. 1004 decides to select IS-B or IS-C. Bit 1 (ISC) setting of No.1001 is applied to all axes. For example: increment system of all axes is set to IS-C when the parameter selects IS-C.

Table 1-3（b） increment system IS-B

Least input increment Least command increment

Metric machine

Inch machine

Least input increment Least command increment

Metric machine

Inch machine

Whether the least input increment is mm or inch is determined by the machine based on the parameter INM(1001#0). The least input increment can be switched between the inch and the mm input, which is controlled by G codes( G20 or G21) or the set parameter.

mm input

Inch input

mm input

Inch input

mm input

Inch input

mm input

Inch input

0.001mm（diameter）

0.001mm（radius）

0.001deg

0.0001inch（diameter）

0.0001inch（radius）

0.001deg

0.001mm（diameter）

0.001mm（radius）

0.001deg

0.0001inch（diameter）

0.0001inch（radius）

0.001deg

Table 1-3（c） increment system IS-C

0.0001mm（diameter）

0.0001mm（radius）

0.0001deg

0.00001inch（diameter）

0.00001inch（radius）

0.0001deg

0.0001mm（diameter）

0.0001mm（radius）

0.0001deg

0.00001inch（diameter）

0.00001inch（radius）

0.0001deg

0.0005mm

0.001mm

0.001deg

0.0005inch

0.001inch

0.001deg

0.00005mm

0.0001mm

0.001deg

0.00005inch

0.0001inch

0.001deg

0.00005mm

0.0001mm

0.0001deg

0.00005inch

0.0001inch

0.0001deg

0.000005mm

0.00001mm

0.0001deg

0.000005inch

0.00001inch

0.0001deg

Programming Ⅰ

Page 24

GSK988T Turning CNC System User Manual

1.3.3 Max. travel

Max. travel=least command increment X（±）99999999

Table 1-3 (d) max. travel IS-C

Ⅰ Programming

IS-B

IS-C

Note 1: The unit is diameter value in diameter programming, is radius value in radius programming in the

above table.

Note 2: The input command cannot exceed max. travel command. Note 3: The actual travel decides the machine tool.

Increment system Max. travel

Metric machine system ±99999.999mm

±99999.999deg

Inch machine system ±9999.9999inch

±9999.9999deg

Metric machine system ±9999.9999mm

±9999.9999deg

Inch machine system ±999.99999inch

±9999.9999deg

1.3.4 Reference position

Reference position is a fixed point on the machine tool. The tool can move to the position by executing the reference position return function. Generally, the reference position is used to tool change and setting coordinate system. GSK988T Turning CNC System can set 4 reference positions by parameters as follows:

reference point

Machine zero

reference point

Fig. 1-6 reference position

1.3.5 Machine coordinate system

Machine tool coordinate system is a benchmark one used for CNC counting coordinates and a

fixed one on the machine tool. Machine tool zero is a fixed point which position is specified by zero switch or zero return switch on the machine tool. Usually, the zero return switch is installed on max. stroke in axis positive direction. After the system is turned on, the reference position return is executed to set machine coordinate system. The machine coordinate system is not keeping until the system is turned off.

Note: For the machine with the incremental encoder, must execute the reference position return every time to

set the machine coordinate system after power-off; for the machine with the multi-coil absolute encoder, need not execute the reference position return every time after power-off.

Page 25

Chapter Ⅰ Programming Fundamentals

1.3.6 Workpice coordinate system

The workpiece coordinate system is a rectangular coordinate system based on the part drawing, also called floating coordinate system. The workpiece coordinate system is set by the system in advance, can be changed by moving its coordinate origin point. The established workpiece is valid till it is replaced by a new one. The system has preset 6 workpice coordinate systems (G54-G59).

1.3.7 Local coordinate system

When the system compiling programs in the workpiece coordinate system, sub-coordinate system of workpiece coordinate system can be set for easily programming, called local coordinate system as follows:

Local coordinate system

Workpiece coordinate system

Programming Ⅰ

Machine coordinate system

Fig. 1-7 local coordinate system

1.3.8 Interpolation function

Interpolation is defined as a planar or three dimensional contour formed by path of 2 or multiple

axes moving at the same time, also called Contour control. The controlled moving axis is called link axis when the interpolation is executed. The moving distance, direction and speed of it are controlled synchronously in the course of running to form the required Composite motion path. Positioning control is defined that motion end point of one axis or multiple axes instead of the motion path in the course of running is controlled.

GSK988T has linear, arc and thread interpolation function.

Linear interpolation: Composite motion path of X, Z axis is a straight line from starting point to

end point.

Circular interpolation: Composite motion path of X, Z axis is arc radius defined by R or the circle

center (I, K) from starting point to end point.

Thread interpolation: Moving distance of X or Z axis or X and Z axis is defined by rotation angle

of spindle to form spiral cutting path on the workpiece surface to realize the thread cutting. For thread interpolation, the feed axis rotates along with the spindle, the long axis moves one pitch when the spindle rotates one rev, and the short axis and the long axis directly interpolate.

Note 1:Xp, Yp, Zp are separately X or its parallel axis, Y or its parallel axis, Z or its parallel axis. The followings

are the same as those.

Note 2: IP expresses the combination of X_Y_Z_(used in programming).

Page 26

GSK988T Turning CNC System User Manual

Example:

Ⅰ Programming

Fig.1-8

…

G32 W-27 F3；（B→C；thread interpolation） G1 X50 Z-30 F100； G1 X80 Z-50；（D→E；linear interpolation） G3 X100 W-10 R10；（E→F；arc interpolation）

…

M30；

1.4 Coordinate Value and Dimension

1.4.1 Absolute programming and incremental programming

The system has two methods to command the too traverse: absolute value and incremental value command. In the absolute programming, use the coordinate value programming of the end point; in the incremental programming, use the traverse distance programming. In the system, using the absolute programming or incremental programming is depended on the word of the command as follows:

Table 1- 4（a）

Absolute value command Incremental value command

X movement command X U

Y movement command Y V

Z movement command Z W

C movement command C H

A movement command A None

B movement command B None

The system can select the incremental programming or the absolute programming mode, or the incremental/absolute compound programming; the absolute command and the incremental command can be in the same block as follow:

X100.0 W100.0;

When the absolute command and the incremental command of one axis are in the same block, the following command value is valid.

Page 27

Chapter Ⅰ Programming Fundamentals

The axis word can exist repetitively in the same block and the later value is valid, but when No.3403 Bit 6 (AD2) is set 1, the alarm occurs. U, W in other G command has bee specified to others. For example: in G73, the above conditions

1.4.2 Diameter programming and radius programming

Because the workpiece section is the circle in CNC turning controlled program, X dimension can use two kind of method; diameter programming command and radius programming command.

1. The user can select the radius programming or diameter programming, which is set by state parameter (No. 1006 Bit 3(DIAX)).

2. Parameters related to diameter/radius programming:

State parameter No.1006 BIT3 (DIAx):　

0—radius programming；

1—diameter programming；

State parameter No.5004 Bit1(ORC): 　

0—offset value is expressed with diameter; 1—offset value is expressed with radius;

Pay more attention to the conditions in the following table when X uses diameter programming:

Table 1- 4 (b) related addresses and data to the diameter or radius programming

Word Explanation Diameter

programming

X coordinate, polar coordinate G50 sets X coordinate Diameter

Diameter value

value

X increment Diameter

value

G71 infeed amount Radius value

X finishing allowance in

Parameter definition

G71, G72, G73

Related addresses to diameter/radius programming

tool retraction amount in G73 Clearance in G71, G72 Radius value Clearance after cutting in G75 Clearance to end point in G74 Taper in G90, G92, G94,

Radius value

Diameter value Diameter value

Radius value G76, radius in G02, G03, thread finishing amount in G76

I X amount of circle center Radius value

G32,G34,G92,Pitch long axis is X in G76

Radius value

X feedrate display Radius/rev, radius /min

Others X or U value of

position

Display Diameter

value

window

Radius programming Radius value

Radius value

Programming Ⅰ

Note: Besides the above-mentioned addresses and data related to the diameter programming or the radius

programming, other related to word and data related to X numerical value are expressed with radius value.

Page 28

GSK988T Turning CNC System User Manual

1.4.3 Decimal programming

Value can be input by decimal programming. Distance, time and speed can be input by decimal programming. The following addresses can use decimal point: X, Y, Z, A, B, C, U, V, W, H, I, J, K, R and F, and other addresses cannot use decimal programming.

Ⅰ Programming

There are two types of decimal point usage which is decided by No. 3401 Bit0(DPI).

When NO.3401 Bit 0(DPI) is set to 1, value without decimal point is with mm, inch.

When NO.3401 Bit0(DPI) is set to 0, input value is specified by least input increment.

Parameter setting Least command unit

Rotary axis is

Rotary axis

ROTx=1 Linear axis

Example: when the metric input, the least input increment unit are set to 0.001:

Program command The corresponding actual

X1000 without decimal command value

X1000.0 with decimal

command value

The decimal which is less than the least input increment unit is discarded in course of program being executed.

Example: X2.34567. When the least unit of input increment is 0.001mm, X2.34567 becomes X2.345, when the least unit is 0.0001inch, it becomes X2.3456.

The system alarms when the specified is more than 8-digit value.

not related to parameter INI

Metric

INI=1 Inch

value when DPI is 1

1000mm

Unit：mm

1000mm

unit：mm

ISC=0（ISC system）

ISC=1

（ISB system）

ISC=0（ISC system）

ISC=1（ISB system）

ISC=0（ISC system）

ISC=1（ISB system）

The corresponding actual value when DPI is 0

1 mm Unit: least input increment( set to 0.001)

1000mm

Unit：mm

0.001deg ROTx=0

0.0001deg

0.001mm INI=0

0.0001mm

0.0001inch

0.00001inch

1.4.4 Conversion between the metric and the inch

Metric input or inch input is set by NO.0000 Bit2(INI). G commands corresponding to metric/inch system is as follows:

G20： inch input ；

G21： mm input.

Input data unit becomes the inch or metric input unit when NO.0000 Bit2 (INI) setting is changed. But, the angle unit is not changed.

——F feedrate;

——position command;

——zero offset of workpiece;

——tool compensation value;

Page 29

Chapter Ⅰ Programming Fundamentals

——graduation unit of MPG; ——movement distance in incremental feed.

NO.1001 Bit0 (INM) can set MM or INCH input of least command increment in linear axis. 0：mm input( metric machine)

1：inch input（inch machine）

1.4.5 Linear axis and rotary axis

NO.1006 Bit0(ROTx) can set each axis to linear axis or rotary axis. NO. 1006 Bit 1 (ROSx) can

be used to select the rotary type for each axis.

Absolute coordinate value is displayed circularly with the movement per rev set by NO.1260 when the cycle function is executed, which can prevent the rotary axis from overflowing. The cycle function is valid when NO.1008 Bit 0(ROAx) is set to 1.

For absolute value command, the coordinate values is the corresponding angle cycle value of per rev set by NO. 1260 after the machine moves. When NO.1008 Bit 1(RABx) is set to 0, the machine rotates according to the shortest distance(to the target point). For incremental command, the machine moves according to the angle defined by the command.

Programming Ⅰ

1.5 Structure of an NC Program

User needs to compile part programs (called program) according to command formats of CNC system. CNC system executes programs to control the machine tool movement, the spindle starting/stopping, the cooling and the lubricant ON/OFF to complete the machine of workpiece.

Program example:

Fig. 1-9

O0001 ; (Program name) N0005 G0 X100 Z50; (Rapidly positioning to A point) N0010 M12; (Clamping workpiece) N0015 T0101; (Changing No.1 tool and executing its offset) N0020 M3 S600; (Starting the spindle with 600 r/min) N0025 M8 (Cooling ON) N0030 G1 X50 Z0 F600; (Approaching B point with 600mm/min)

Page 30

GSK988T Turning CNC System User Manual

N0040 W-30 F200; (Cutting from B point to C point) N0050 X80 W-20 F150; (Cutting from C point to D point) N0060 G0 X100 Z50; (Rapidly retracting to A point) N0070 T0100; (Canceling the tool offset)

Ⅰ Programming

The tool leaves the path of A→B→C→D→A after the above-mentioned programs are executed.

ending with “%”; a block begins with block number (omitted) and ends with “;” or “*”. See the general structure of program as Fig. 1-10:

Program name

N0080 M5 S0; (Stopping the spindle) N0090 M9; (Cooling OFF) N0100 M13; (Releasing workpiece) N0110 M30; (End of program, spindle stopping and Cooling OFF)

A program consists of a sequence of blocks, beginning with “OXXXX”(program name)and

Program annotation

Block skip character

Block number

Character for end of block

Fig. 1-10 Structure of a program

Word

Block

Program

1.5.1 Program name

Format: ○ △△△△

Program number (0000～9999, the leading zero can be omitted）

Address O

is number of a program name, its range is 4△△△△ -digit integer 0000～9999, the system

alarms when the negative program name is input. The system ignores NC commands when program are edited and other NC commands are edited in the first line.

1.5.2 Block format

1. Format: / N countless words; △△△△

/： skip character. A block can have or not it, generally, it is placed in the initial

position of a program; user can press “SKIP” on the operation panel to execute the operation when the skip function is valid, otherwise, the “SKIP” key on the operation panel is valid, i.e. the skip character in the block is invalid;

N△△△△△：block number. A block can have or not it; number following N is △△△△△

5-digit positive integer 00001～99999, and the system alarms when the

input number is decimal.

Page 31

Chapter Ⅰ Programming Fundamentals

Countless words: one block can input countless words, and one block can have one or

more words or have no words.

，：

“EOB” is a end character when one block is completed, “;” is displayed in

LCD, there must be have one end character for one block;

2. Format requirements

（1）

In one block, there can be no blank space between block number and word, and can

be countless blank space(the total characters of one block is within 255);

　（2）In one block, there can be not or be countless space between skip character and block

number or words;

（3）

In one block, there can be not or be countless space between end character of block

and its front word or blocks; Each block can be up to 255 characters, including skip character, block number, command, space, end character of block “;”;

（4）

The system automatically ignores the content with small bracket “（”,“）”.

Explanations of program annotation: Note: The annotation of program home as the total annotation of a program is displayed in the program

catalog window, the created program automatically creates the small brackets “（”、“）”, if they are

deleted, the system has no them and they can be replaced by “;”.

3．Parameters related block number:

（1）

whether the system automatically creates block number or not:

User can set whether the system automatically creates block number or not in editing program by setting Bit 5(SEQ) of NO.0000;

（2）

Note: Sprit(/) explanations:

1. When the sprit (/) is used to skip character, it is generally placed the beginning of block, otherwise , and the messages from the sprit to EOB code are ignored. For example: U10.G00/04; when the skip function is started, the system executes U10. G00;(G00 U10.), when it stops, the system executes U10. G0004;(G04 U10.);

2. For cycle command buffer, when a block reads from memory to buffer memory, whether the skip function is valid or not has been executed. After a block reads into buffer memory, i.e. the system changes skip switch state, but does not influence the block which has read into the buffer memory;

3. Sprit (/) (closed in bracket[]) and sprit(/) right to value statement “=” in <Expression> are taken as division operation character instead of skip character.

Use can set the interval value in automatically creating block number by setting

NO.3216.

Programming Ⅰ

1.5.3 Word

1. Format: address + number. There must not be space between address and number. Presently, the system permissively input addresses: G, M, S, T, F, X, Y, Z, U, V, W, P, Q, I, J, K, R,

L, A, B, C, H , N, O， and will add other;

Command number range following address is referred to the following table.

Table 1-5-1 word table

Address

Function mm input inch input Related G

Program name

Line label

Preparatory function See G code See G code

0～9999 0～9999

1～99999 1～99999

codes

Page 32

GSK988T Turning CNC System User Manual

Miscellaneous function

Spindle speed

Ⅰ Programming

Tool offset

Feedrate per minute

Feedrate per rev

Pitch

X absolute coordinate value((linear axis), delay time (*1)

Y absolute coordinate value(linear axis) (*1)

Z absolute coordinate value (linear axis) (*1)

A absolute coordinate value(linear axis) (*1)

B absolute coordinate value(linear axis) (*1)

C absolute coordinate value (rotary axis) (*1)

X relative coordinate value, finishing allowance in G71, G72, G73, X tool retraction distance and specified delay time(*1) in G73, (*1)

0～9999 0～9999

（G96） 0～20000 m/min

（G97） 0～20000 r/min

0000～9999 0000～9999

（ISB system）１～60000 mm/min

（ISC system）１～24000 mm/min

（ISB system）

0.01～500mm/r

（ISC system）

0.01～500mm/r

0.01～500 mm 0.01～9.99inch

（ISB system）

-99999.999～99999.999mm

（ISC system）

-9999.9999～9999.9999mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 deg

（ISC system）

-9999.9999～9999.9999 deg

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（G96） 0～2000 feet/min

（G97） 0～20000 r/min

（ISB system）

0.01～2400 inch/min

（ISC system）

0.01～960 inch/min

（ISB system）

0.01～9.99inch/r

（ISC system）

0.01～9.99 inch/r

（ISB system）

-9999.9999～9999.9999inch

-999.99999～999.99999inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-99999.999～99999.999 deg

（ISC system）

-9999.9999～9999.9999 deg

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

G98

G99

Relative commands for thread machining

Relative command of axis, G04

Relative command of axis

Relative command of axis,G71,G7 2,G73,G04

Page 33

Chapter Ⅰ Programming Fundamentals

Cut depth in G71(modify parameter manual) (*2)

Y relative coordinate value(linear axis) (*1)

Z relative coordinate value, Z finishing allowance in G71, G72, G73, Z tool retraction distance (*1) in G73 (*1)

Cut depth (*2) in G72 (*2)

Arc radius (*1)

Taper and thread taper (*1) in G90, G92, G94, G76 (*1)

Tool retraction（*2） in

G71,G72 （*2）

Roughing times in G73

Thread increment in variable pitch cutting

Tool retract movement after cutting in G74, G75 and tool retraction after cutting to end point （*2）

Finishing amount （*2）

in G76

Dwell time 0~99999999ms 0~99999999 ms G04

G30 returning to No.n reference position

Commands for macro program number, subprogram and subprogram call times

（ISB system）

0.001~99999.999 mm

（ISC system）

0.0001~9999.9999 mm （ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

0.001~99999.999 mm

（ISC system）

0.0001~9999.9999 mm （ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system） 0～99999.999 mm

（ISC system） 0～9999.9999 mm

1～999（times） 1～999（times）

0.01～500.000 mm

-0.01～-500.000 mm

（ISB system） 0～99999.999 mm

（ISC system） 0～9999.9999 mm

（ISB system）

0.001～99999.999 mm

（ISC system）

0.0001～9999.9999 mm

2,3,4 2,3,4

1～9999

（ISB system）

0.0001~9999.9999 inch

（ISC system）

0.00001~999.99999 inch （ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

0.0001~9999.9999 inch

0.00001~999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system） 0～9999.9999 inch

（ISC system） 0～999.99999 inch

0.01～9.99inch

-0.01～-9.99inch

（ISB system） 0～9999.9999 inch

（ISC system） 0～999.99999 inch

（ISB system）

0.0001～9999.9999 inch

（ISC system）

0.00001～999.99999 inch

1～9999

G71

Relative command of axis

Relative command of axis, G71, G72, G73,

G72

G02,G03

G90,G92,G 94,G76

G71,G72

G73

G34

G74,G75

G76

G30（default to 2）

G65,G66,M 98 （ default

times is 1）

Programming Ⅰ

Page 34

GSK988T Turning CNC System User Manual

Line number assignment in G70, G71, G72,G73

X cycle movement（*3）

Ⅰ Programming

in G74, G75

Thread cutting parameter in G76

Thread tooth height （*3） in G76

Line number assignment in G70, G71, G72, G73

Tool infeed amount(*3) in Z brokenly infeed in G74,G75

Min. cutting amount (*3) in G76 thread roughing

1st thread cutting depth （*3 ） in G76 thread

roughing Initial angle （*3）of 1

circle in thread cutting （*3）

Macro program call times assignment

Head quality of multi-thread

Relative starting point of arc center is in X

vector (*1)

Relative starting point of arc center is in Y vector (*1)

Movement in short axis when thread run-out is executed (*1)

Relative starting point of arc center is in Z vector (*1)

0～99999 0～99999

0 ～ 99999999

command unit

Including 3 parameters: Thread finishing times：1～

99 Thread run-out length：00～

99（*0.1 pitch） Angle between two teeth：

0°~99°

1 ～ 99999999

command unit 0～99999 0～99999

0 ～ 99999999

command unit

0 ～ 99999999

command unit

1 ～ 99999999

command unit

0 ～ 99999999

command unit （default to 0）

1～9999（default to 1） 1～9999（default to 1）

1～99（default to 1） 1～99（default to 1）

（ISB system）

-99999.999～99999.999mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

（ISB system）

-99999.999～99999.999 mm

（ISC system）

-9999.9999～9999.9999 mm

least

0～99999999×least command

unit

Including 3 parameters: Thread finishing times：1～99 Thread run-out length：00～99 （*0.1 pitch） Angle between two teeth ：

0°~99°

1～99999999×least command

unit

0～99999999×least command

unit

0～99999999×least command

unit

1～99999999×least command

unit

0～99999999×least command

unit

（default to 0）

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

（ISB system）

-9999.9999～9999.9999 inch

（ISC system）

-999.99999～999.99999 inch

G70,G71,G 72,G73

G74,G75

G76

G70,G71,G 72,G73

G74,G75

G76

G32,G34,G 92

G65,G66

G92

G02,G03

G32,G34,G 92

G02,G03

Page 35

Chapter Ⅰ Programming Fundamentals

THEN

GOTO

WHILE

END

SIN

ASIN

COS

ACOS

TAN

ATAN

SQRT

ABS

ROUN

FIX

FUP

EXP

XOR

AND

BIN

BCD

123456

789

Length in long axis when thread run-out is executed （*2）

Conditional judgement

TH Execution after IF conditional judgment is completed successfully

GO Non-conditional skip

WH Cycle judgment

Start to execute cycle

EN Return to WHILE

== Equal to

<> Not equal

> Greater

than

>= Greater

than or equal to

< Less than

<= Less than

or equal to

SI Sine

AS Anti-sine

CO Cosine

AC Anti-cosine

TA Tangent

AT Anti-tangent

SQ Square root

AB Absolute

value

RO Rounding-off

FI Down integer

FU Up integer

Nature

logarithm

EX Exponential

function

XO OR AND

AN AND

BI Converse

from BCD to BIN

BC Converse

from BIN to BCD

With to compose the value of word, the leading 0 can be omitted

Word is 0 and is different with Null value

Number count and number expression

（ISB system） 0～99999.999 mm

（ISC system） 0～9999.9999 mm

Judgement logic is used to brackets following IF, WHILE

Functional function is used to count expression value

（ISB system） 0～9999.9999 inch

（ISC system） 0～999.99999 inch

G32,G34,G 92

Programming Ⅰ

Page 36

GSK988T Turning CNC System User Manual

Skip command, selectively skip the commands

Ⅰ Programming

following the character

Floating point number with number

Variable assignment

[

Prior operation of expression and conditional judgement prompt

]

Var i a b l e

;

End of program in the block, following annotation

Annotation start in the block. Example: (X20.)W-10.;

(

not execute X20.

Annotation end in the block

)

End of program

Note 1: The 2-digit following the decimal point of F value is value, and the more following the two-digit is

ignored.

Note 2: The expression can follow the word, the value counted by the expression is taken as the value of the

word, and the expression should have[] , and there must not be the space between the word and the expression. For example X[#1-#110] Z[#1+SIN[#120]].

*1）：When the address values in the above table, X, Y, Z, C, A, B, C, U, V, W, H, I, J, K, R are taken

as word address, their value ranges are controlled by the following parameters:

（1）No.0000#2 INI

INI input unit 0：metric

1：inch

（2）No.1006#0 ROTx

ROTx set linear axis or rotary axis 0：linear axis

1：rotary axis

（3）No.0004#1 ISC

ISC set least input unit and least command increment

Table 1-5-2 set least input unit and least command increment

ISC Least setting unit For short

0 0.001mm, 0.001deg or 0.0001inch IS-B

1 0.0001mm, 0.0001deg or 0.00001inch IS-C

Table 1-5-3 least command unit and value range

Address Parameter setting Least

command unit

X,Y,Z,C,A,B,C,U,V,W,H ROTx=0

Rotary axis

Rotary axis is not

ISC=0 ISB

0.001deg

Range

-99999.999～

99999.999 deg

Page 37

Chapter Ⅰ Programming Fundamentals

X,Y,Z,C,A,B,C,U,V, W,H,I,J,K,R

ROTx=1 Linear axis

related to INI

INI=0 Metric

INI=1 Inch

ISC=1 ISC

ISC=0 ISB

ISC=1 ISC

ISC=0 ISB

ISC=1 ISC

0.0001deg

0.001mm

0.0001mm

0.0001inch

0.00001inch

-9999.9999～

9999.9999 deg

-99999.999～

99999.999 mm

-9999.9999～

9999.9999 mm

-9999.9999～

9999.9999 inch

-999.99999～

999.99999 inch

When these word addresses follow data, data precision is least command unit, and excessive data is ignored. When a word address follows variable number or has [] expression, the word value has decimal data, and its precision is the least command unit, but its excessive data rounds.

（4）No.3401#0 DPI

DPI can use decimal address. When the decimal is omitted, its setting is as follows: 0：least setting unit

1：unit: mm，inch，sec

When parameter DPI is set to 1, word range is referred to Table 1-5-3;

When DPI is set to 0, and word omits its decimal, its value range is -99999999～99999999, data

unit is the least command unit in Table 1-5-3.

*2）: Command value calculation method specified by U, W, R, K is the same that of *1）, they

Programming Ⅰ

meet the value range described in *1） and limit value range according to preparatory

function.

*3）: Position specified value commanded by P, Q is 0～99999999, data unit is the least command

unit in Table 1-5-3. value range is limit by specific preparatory function.

2. Word value and state will change when the system runs, the following table separately explains each word omit and state when the system is ON, resets.

Table 1-5-4 word state

Character Function

Program name Value

Preparatory function Initial mode in

Miscellaneous

function M00, M01, M02, M30, M98, M99

Analog spindle speed

Tool offset Value

Initial value

when

power-on

reserved by last power-on

each group

Current

0 Current

reserved by last power-on

Default

value

Current value

Modal value

value

Current value

Keep in the next block?

Yes Yes None

No parameter

No （ function

reserved）

Yes

Yes Current value

Value after

pressing reset

key

（ CLR ）

NO.3402#6

Current value Specified by

Current value，

output is invalid

explanation

None

PLC, set by parameter

Page 38

GSK988T Turning CNC System User Manual

Feedrate per minute Parameter

value

Ⅰ Programming

Feedrate per rev Null Current

Pitch Null Current

Delay time Null 0 No 0

X absolute coordinate value

Y absolute coordinate value

Z absolute coordinate value

C absolute coordinate value

Delay time Null 0 No Null

X relative coordinate value

X allowance in finishing

Cutting depth in G71 Parameter

Y relative coordinate value

Z relative coordinate value

Z allowance in finishing

0 Current

0 0 No Current value

Null 0 No Null

value

0 0 No Current value

空

Current value

value

Parameter value

0 No Null

Yes parameter

（ CLR ）

NO.3402#6

Yes Current value

Yes Parameter

value

Cutting depth in G72 Parameter

value

C increment value

Arc radius 0 0 No Current value

Taper G90, G92, G94 and thread taper

Tool retraction in G71, G72

Roughing times in G73

Clearance in G74,G75 Parameter

Clearance to end point in G74,G75

0 0 No Current value G00

0 0 No Current value Polar

0 0 Yes Current value

Parameter value

value

0 0 No Null

Parameter value

Yes Parameter

value

Yes Parameter

value

Yes Parameter

value

Yes Parameter

value

coordinate interpolation

Page 39

Chapter Ⅰ Programming Fundamentals

Finishing cutting amount in G76

Dwell time Null 0 No Null

G30 returning to No. n

reference position

Macro program

number, subprogram,

subprogram call times

Line assignment in G70, G71, G72, G73

X cycle movement in G74,G75

Thread cutting in G76 Parameter

Thread tooth height in G76

Line assignment in G70, G71, G72, G73

Parameter value

Null 2 No Null

Null Alarm No Null

Null 0 No Null

value

0 Alarm No Null

Null Alarm No Null

Parameter value

Yes Parameter

value

Yes Parameter

value

Programming Ⅰ

Z broken tool infeed amount in G74, G75

Least cutting amount in G76 roughing

1st thread cutting depth in G76 thread roughing

1st circle start angle in thread cutting

Check offset in spindle fluctuation check

Macro program call times assignment

X vector of circle center corresponding to starting point

X calculation direction in cancelling radius compensation

Y vector of circle center corresponding to starting point

Y calculation direction in cancelling radius compensation

Z vector of circle center corresponding

Null 0 No Null

Parameter value

Null Alarm No Null

Null 0 No 0

Null 0

1 1 No Null

0 0 No Current value

Null Null No Null

0 0 No Current value

Null Null No Null

0 0 No Current value

Parameter

alue

Yes Parameter

value

No （ the

parameter cannot be modified

Page 40

GSK988T Turning CNC System User Manual

to starting point

Pitch increment in variable pitch thread cutting

Ⅰ Programming

X travel lower limit value

Z calculation direction in cancelling radius compensation

Null 0 Yes Current value

Null Alarm No Current value

Null Null No Null

1.5.4 Block number

Format: N △△△△△

is 5△△△△△ -digit integer 00001～99999, and its leading zero can be omitted.

（1）

Can or not input a block number in one block(must input block number in target block in

which program skips), when many block number are input in one block, only the last block number is valid;

（2）

Block number can be placed any position of block but it is suggested that it should be

placed at the initial position in order to search and read；

（3）

There can be many same block number in one program, but the block number of target

block of program skip has only one; otherwise, the program skips to the nearest block to the block;

（4）

block number can be placed at will.(it is suggested that it should be placed by the rising

or falling monotonously;

Note: When the block number exceeds the range, and the program runs or the grammatical check is done, the

relevant alarm occurs.

1.5.5 Main program and subprogram

To simply the programming, when the same or similar machining path and control procedure is used many times, its program commands are edited to a sole program to call. The main program is defined to call others and the subprogram is to be called. They both take up the program capacity and storage space of system. The subprogram has own name, and can be called at will by the main program and also can run separately. The system returns to the main program to continue when the subprogram ends as follows:

Page 41

1.6 Program Run

1.6.1 Sequence of program run

Chapter Ⅰ Programming Fundamentals

Programming Ⅰ

Fig.1-11

Running the current open program must be in Auto mode. GSK988T cannot open two or more programs at the same, and runs only program any time. When the first block is open, the cursor is located in the heading of the first block and can be moved in Edit mode. In the run stop state in Auto mode, the program starts to run by the cycle start signal (CYCLE START key is pressed or external cycle start signal)from a block pointed by current cursor, usually blocks are executed one by one according to their programming sequence, the program stops running till executing M02 or M30. The cursor moves along with program running and is located at the heading of the current block. Sequence and state of program running are changed in the followings:

z The program stops run after pressing RESET or EMERGENCY STOP button;

z The program stops running when the system or PLC alarms;

z The program runs and single block stops (the program run stops after the current block runs

completely) in Edit, MDI mode, and then a block pointed by the current cursor starts running after the system switches into Auto mode, the CYCLE START key is pressed or external cycle start signal is switched on;

z The program stops run in Manual(Jog), Handwheel (MPG), Single Block, Program

Reference position Return, Machine Reference position Return mode and it continuously runs from current position after the system is switched into Auto mode and the CYCLE START key is pressed or the external cycle start signal is switched on;

z The program pauses after pressing the FEED HOLD key or the external cycle start signal is

switched off, and it continuously runs from current position after pressing the CYCLE START key or the external cycle start signal is switched on;

z When Single Block is ON, the program pauses after every block is executed completely, and

then it continuously runs from the next block after the CYCLE START key is pressed or the external cycle start signal is switched on;

z Block with “/” in the front of it is not executed when the block skipping switch is ON;

z The system skips to the target block to run after executing G65;

z Please see Section Three G Commands about execution sequence of G70~73;

Page 42

GSK988T Turning CNC System User Manual

z Call corresponding subprograms or macro program to run when executing M98 or

M9000~M9999; the system returns to main program to call the next block when executing M99(if M99 specifies a target block number, the system returns to it to run) after the subprograms or macro programs run completely;

Ⅰ Programming

z The system returns to the first block to run and the current program is executed repetitively

when M99 is executed in a main program.

1.6.2 Execution sequence of word

There are many words (G, X, Z, F, R, M, S, T and so on) and most of M, S, T is transmitted to

PLC by NC explaining and others are directly executed by NC. M98, M99, M9000～M9999, S word

for specifying spindle speed (r/min, m/min) is directly executed by NC.

NC firstly executes G and then M commands when G codes and M00, M01, M02 and M30 are in

the same block.

NC firstly executes G and then M commands( without transmitting M signal to PLC) when G

codes and M98, M99, M9000～M9999 are in the same block.

When G codes and M, S, T executed by PLC are in the same block, PLC defines M, S, T and G to be executed simultaneously, or execute M, S ,T after G codes. Please see User Manual of machine manufacturer for execution sequence of commands.

Execution sequence of G, M (except for the above M codes), S, T defined by GSK988T PLC in

the same block is determined by PLC, which is divided into two methods:

a) Movement codes and M miscellaneous code are executed simultaneously.

b) Execute miscellaneous codes after executing movement codes.

Refer to the machine manufacture’s user manual for the concrete execution method.

The second method is executed when there is M9, M99, M13, M33 or M5 for our GSK ladder.

Note: When G28 or G30 and M01 are in the same block, the pause after zero return is done. When there is a

single block stop command without M01,the single block stop is executed at the middle point and zero

return completion position. When G28 or G30 and M01 are in the same block and the single block stop is

valid, the pause is executed after zero return.

Page 43

Chapter Ⅱ G Commands

Chapter II G Commands

2.1 Summary

G command consists of command address G and its following command value, used for defining the motion mode of tool relative to the workpiece, defining the coordinates and so on. Refer to G commands as Fig. 2-1.

Note 1: The leading zero of the command value can be omitted. Example: G02 is equivalent to G2, G01 to G1.

Note 2: The leading zero following the command value cannot be omitted. Example: G20 and G2 are

different G commands in the different group; G12.1 is legal but G12.10 is illegal.

Note 3: The command value can be up to 8-bit digit. Example: G00000002 is correct and valid, equivalent

to G02.

Note 4: Except for G12.1 and G13.1, other G command cannot be with the decimal point, otherwise, the

alarm occurs. For example: G20.0, G00.0, G18.are illegal.

Ⅰ Programming

2.1.1 G command classification

G commands are divided into: modal G command and non-modal G command.

After a G command is executed, its defined function or state remains valid till other G command is specified in the same group, this G command is called the modal. After the modal G command is executed, before its defined function or state is changed, the G command cannot be input again when the following block executes the G word.

After a G command is executed, its defined function or state is valid once, its word must be input again when it is executed, and so the G command is called the non-modal.

Example 1: G01 and G00 are modal.

G01 X_；

Z_； G01 is valid in the range

X_；

G00 Z_;

X_; G00 is valid in the range

G01 X_;

Example 2: G04 is non-modal. O0002；

G0 X50 Z5；（Rapid traverse to X50 Z5）

G04 X4；（Delay 4s） G04 X5；（Delay 5s again，G04 is non-modal and must be input again）

M30；

Table 2-1 G command list

G command Group Function Classification

*G00 01 Positioning(rapid traverse) Modal

Page 44

GSK988T Turning CNC System User Manual

G01

G02

G03

G04 dwell

G7.1

Ⅰ Programming

(G107)

G10 Programmable data input G11

G12.1

（G112）

*G13.1

（G113）

G17 XpYp level selection

*G18 ZpXp level selection

G19

G20 Inch input

*G21

*G22 Stored travel check ON

G23

G28 Return to reference position

G30

Linear interpolation

Circular interpolation(CW)

Circular interpolation(CCW)

Cylindrical interpolation

Programmable data input cancel

Polar coordinate interpolation mode

Polar coordinate interpolation mode cancel

YpZp level selection

mm input

Stored travel check OFF

Return to 2nd, 3rd, 4th reference position

Non-modal

Modal

Non-modal

G32 Constant pitch thread cutting

G34

*G40 Tool radius compensation cancel

G41 Cutter compensation left

G42

G50 Workpiece setting or max. spindle speed

G52 Local coordinate system setting

G53

*G54 Select workpiece coordinate system 1

G55 Select workpiece coordinate system 2

G56 Select workpiece coordinate system 3

G57 Select workpiece coordinate system 4

G58 Select workpiece coordinate system 5

G59

G61 Exact stop mode

*G64

G65 00 Non-modal macro program call Non-modal

G66 Macro program mode call

*G67

G70 Finishing cycle

G71 Axial roughing cycle

G72 Radial roughing cycle

G73 Closed cutting cycle

G74

Variable pitch thread cutting

Cutter compensation right

setting

Machine coordinate system setting

Select workpiece coordinate system 6

Cutting mode

Cancel macro program mode call

Axial grooving cycle

Modal

Non-modal

Modal

Non-modal

Page 45

Chapter Ⅱ G Commands

G75 Radial cutting multi-cycle

G76 Multi thread cutting cycle

*G80 Cancel drilling fixed cycle

G83 End drilling cycle G84 End rigid/common tapping cycle G85 End boring cycle G87 Side drilling cycle G88 Side rigid/common tapping cycle G89 G90 Axial cutting cycle

G92 Thread cutting cycle

G94

G96 Constant surface speed control

*G97

*G98 Feed per minute

G99

Note 1: G commands in Group 01, 05, 09 separately set their state in No.3402 Bit0(G01), Bit4 (FPM), Bit7

(G23) when the system is power-on, the G commands in Group 06 in No.0000 Bit2(INI); when the system is turned on, the modal G command in other groups are at the state designated by *.

Note 2: When the system resets, No.3402 Bit6 (CLR) is set to 0, the modal of the G command remains

unchanged; when it is set to 1, the modal is changed to the one which is at the power-on, but G22 and G23 in Group 09 and G20 and G21 in Group 06 remain unchanged.

Note 3: G commands in Group 00 are non-modal. Note 4: G commands in Group 00 and ones in Group 01 are specified in the same block, G commands in

Group 00 are valid, G commands in Group 01 only change their modal.

Note 5: Commands in Group 06, 09, 21 and ones in other groups cannot be in the same block, commands

in Group 12 and G65 are specified only in a separate block.

Note 6: When No.3403 Bit6(AD2) is set to 0, many G commands in the different groups can be specified in

the same block, and the G command specified at last is valid; when it is set to 11, the alarm occurs.

Note 7: When compiling a G command in one block needs a word, and the compiled cannot use the word,

the word is ignored(for example: G00 X_ Z_ R_ ，R_ is ignored); when the ignored word format is

not correct, the alarm occurs (For example: G00 X_ Z_ R2.3.1）.

Note 8: When compiling No.1020 does not have the axis word including the absolute address or

incremental address, the alarm occurs.

Modal

Side boring cycle

Modal

Radial cutting cycle

Modal

Constant speed control

Modal

Feed per revolution

Ⅰ Programming

2.1.2 Omitting word input

To simplify the programming, their command values are reserved after executing words in Table 2-2. If the words are contained in the previous blocks, they cannot be input when the words are used with the same values and definitions in the following blocks.

Page 46

GSK988T Turning CNC System User Manual

Table 2-2

Command

address

U Cutting depth in G71 №51 parameter value U Move distance of X tool retraction in G73 №53 parameter value

Ⅰ Programming

W Cutting depth in G72 №51 parameter value W Move distance of X tool retraction in G73 №54 parameter value

Move distance of tool retraction in G71, G72 cycle

R Cycle times of stock removal in turning in G73 №55 parameter value

Move distance of tool retraction after cutting in G74, G75

R Allowance of finishing in G76 №60 parameter value

R Taper in G90, G92, G94, G96 0

(G98) F Feedrate per minute(G98) №30 parameter value

(G99) F

Feedrate per rev (G99)

F Metric pitch(G32, G92, G76) 0

I Inch pitch(G32, G92) 0

S Spindle speed specified(G97) 0

Spindle surface speed specified(G96)

S Spindle speed switching value output 0

Finishing times of thread cutting in G76;

Tool retraction width of thread cutting in G76 Angle of tool nose of thread cutting in G76;

Q Min. cutting value in G76 №59 parameter value

Note 1: For the command addresses with functions (such as F, used for feedrate per minute, feedrate per

rev and metric pitch and so on), they can be omitted not to input when executing the same function to definite words after the words are executed. For example, after executing G98 F_ without executing the thread command, the pitch must be input with F word when machining metric thread.

Note 2: When the words in the aboved table (except for F, S) are not omitted, the input new command value

is written to the corresponding parameter.

Note 3: When X（U）, Y（V）, Z（W）, A, B or C（H）are used to the end point coordinates of the specified

block and their words in the block are not input, the system takes the absolute coordinates of the current X, Y, Z, A, B or C as the coordinates of the end point.

Example 1：（run after the first power-on）：

Function Initial value when power-on

№52 parameter value

№56 parameter value

№57 parameter value №19 parameter value №58 parameter value

O0003；

Example 2：

O0001；

G98 F500 G01 X100 Z100；（G98: feed/minute，500mm/min）

G92 X50 W-20 F2 ；（thread cutting, F must be input when it is the pitch）

G99 G01 U10 F0.01 ；（G99: feed/minute, F is input again

）

G00 X80 Z50 ；

M30；

G0 X100 Z100；（rapidly traverse to X100 Z100；the modal G0 is valid）

Page 47

X20 Z30；（rapidly traverse to X20 Z30；the modal G0 can be omitted）

G1 X50 Z50 F300；（linear interpolation to X50 Z50， 300mm/min； the modal G1 is

valid）

X100；（linear interpolation to X100 Z50，300mm/min；When Z coordinate

is not input, the current coordinate value Z50 is used; F300 is kept, G01 can be omitted when it is modal.）

G0 X0 Z0；（rapidly traverse to X0 Z0，the modal G0 is valid）

M30；

2.1.3 Related definitions

Definitions of word are as follows except for the especial explanations:

Starting point: position before the current block runs; End point: position after the current block ends;

X: X absolute coordinates of end point; Xp：absolute coordinate of X end point or one which is parallel to X;

U: different value of X absolute coordinate between starting point and end point; Y：Y absolute coordinate of end point;

Chapter Ⅱ G Commands

Ⅰ Programming

Yp：absolute coordinate of Y end point or one which is parallel to Y; V：different value of Y absolute coordinate;

Z: Z absolute coordinates of end point; Zp：absolute coordinate of Z end point or one which is parallel to Z;

W: different value of absolute coordinates between starting point and end point; C：C absolute coordinate of end point;

H：different value of C absolute coordinate between end point and starting point; A：A absolute coordinate of end point; B：B absolute coordinate of end point; F：cutting feedrate. IP：it is the combination of axes to execute the data provided by G command, the later

specified address is valid when the absolute address and relative address of one axis are defined and are in the same block to be edit. The range for each axis in corresponding parameter is as follows:

2.2 Rapid Traverse (Positioning) G00

Command function: In the absolute command, the tool rapidly traverses to the position

specified by the workpiece coordinate system; in the incremental command, the tool rapidly traverses to the position which offsets the specified value of the current position.

Command format：G00 IP__；

Command explanation: IP: it is the end point coordinate value of the tool traversing for the

absolute command; it is the tool traversing distance for the incremental command.

Page 48

GSK988T Turning CNC System User Manual

Command path:

Ⅰ Programming

Fig. 2-1 rapid traverse(positioning)

Execution process:

Program：（Diameter programming） G00 X40.0 Z56.0；（Absolute programming）or G00 U60.0 W-36.0；（Incremental programming）or G00 X40.0 W-36.0；（Compound programming）or G00 U60.0 Z56.0；（Compound programming）

Fig. 2-2 positioning example

Note 1: The rapid traverse speed(G00) is set in No.1420 and is not related to the commanded feedrate F

value in the block.

Note 2: Whether the initial mode of Group 01 when power-on is G00 or G01 is determined by No.3402

Bit0(G01).

2.3 Linear Interpolation G01

Command function: the tool executes the linear traverse.

Command format: G01 IP

Command explanation：IP_: it is the end point coordinate value of tool traversing for the

Feed mode

G98

ISB system

ISCsystem

F__；it can be omitted to G1

absolute command; it is the tool traversing distance for the incremental command. F_: it is the feedrate of the tool and its ranges is shown below.

Metric（mm）input

Inch (inch) input

１～60000 mm/min 0.01～2400 inch/min

１～24000 mm/min 0.01～960 inch/min

G99

ISB system

ISC system

0.01～500mm/r 0.01～9.99inch/r

0.01～500mm/r 0.01～9.99 inch/r

Page 49

Command path:

Chapter Ⅱ G Commands

Fig. 2-3 linear interpolation

Execution process：

Programming：（Diameter programming） G01 X40.0 Z20.0 F500；（Absolute programming） or G01 U20.0 W-26.0；（Incremental programming）or G01 X40.0 W-26.0；（Compound programming）or G01 U20.0 Z20.0；（Compound programming）

Fig. 2-4 Linear interpolation example

Note 1: The tool traverses to the specified position along the linear at the speed specified by F. Before the

new value is specified, each program is not needed to specify.

Note 2: The actual cutting feedrate is the product between the feedrate override and F command value. Note 3: The actual cutting feedrate is limited by max. cutting feedrate MFR of No. 1422.

Note 4: G04 supports the synchronous interpolation of linear axis and rotary axis. The command speed

includes the speed of rotary axis. When there is only the combination speed of linear axis, the display value of actual speed does not include the actual speed of rotary axis.

Ⅰ Programming

2.4 Arc Interpolation G02, G03

Command function: The tool traverses along an arc on the specified level. Command format：

02 _

Command explanations：

Command Description

G17 XpYp level selection

G18 ZpXp level selection

G19 YpZp level selection

G02 Arc interpolation (CW)

G03 Arc interpolation (CCW)

Xp_ Movement of X or an axis parallel to it (set by No.1022)

Yp_ Movement of Y or an axis parallel to it (set by No.1022)

Zp_ Movement of Z or an axis parallel to it (set by No.1022)

GXpYp F

GXpZp F

GYpZp F

⎨⎬ ⎨ ⎬

GIJ

⎩⎩

⎧⎧

18 _ _ _

⎨⎬ ⎨ ⎬

GIK

⎩⎩

⎧⎧

19 _ _ _

⎨⎬ ⎨ ⎬

GJK

⎩⎩

⎧⎧

17 _ _ _

⎫⎫

03 _ _

⎭⎭

02 _

⎫⎫

03 _ _

⎭⎭

02 _

⎫⎫

03 _ _

⎭⎭

Page 50

GSK988T Turning CNC System User Manual

I_ Distance between starting point of Xp axis to center of arc (with sign, its

range referred to the following table)

J_ Distance between starting point of Yp axis to center of arc (with sign, its

range referred to the following table)

K_ Distance between starting point of Zp axis to center of arc (with sign, its

Ⅰ Programming

R_ Arc radius (with sign, it is the radius value when machining, range referred to

Address Incremental system

range referred to the following table)

the following table) Feedrate along arc（its range is the same that of G01）

Metric input（mm）

Inch input (inch)

I, J, K, R

I, J, K have sign symbols according their directions, they are positive when their directions are the same those of Xp, Yp, Zp, otherwise, they are negative.

Command path（arc direction）：

ISB system

ISC system

-99999.999～99999.999 -9999.9999～9999.9999

-9999.9999～9999.9999 -999.99999～999.99999

Fig. 2-5

Fig. 2-6 Arc interpolation

Page 51

Execution process：（taking G02 as an example）

Fig. 2-7 G02 arc interpolation

Chapter Ⅱ G Commands

Ⅰ Programming

Note 1: One or all of Xp, Yp, Zp can be omitted. When one of them is omitted, it means the coordinate

values of the starting point and the end point of the axis is consistent; when all are omitted, it means the two points are in the same position.

Note 2: When I = 0, J=0, K = 0, they can be omitted; when I, J, K and R are 0, the system executes the linear

movement based on No. 3403 Bit5(CIR) or alarms.

Note 3: When I = 0, J = 0 or K = 0，and the command is executed, the tool linearly traverses to the end point. Note 4: When I and J, J and K, I and K, are input with R, only R is valid, I, J, K are invalid.

Note 5: When the starting point and the end point are the same one, I, K are the center value, G02/G03 path

is a full circle; When R is the arc radius, it means the circle is 0 degree.

Note 6: When R is the arc radius, it is more than or less than 180°, and it is more than 180° arc when R is

negative; it is less than or equal to 180° when R is positive

Note 7: The alarm occurs when the radius difference between the starting point and the end point of arc

exceeds the set value(except for 0) of No. 3410. When the difference does not exceed the setting value or the set value is 0, the tool firstly executes the arc interpolation along the radius value between the arc and the center, and traverse linearly to the end point; in using R programming, R should be equal to or more than the half between the starting point and the end point; when the end point is not in the arc defined by R, the user can set whether the system alarms according to No. 3403 Bit4 (RER). It is suggested that the user should use R programming.

Note 8: In G02/G03 mode, the system alarms when the other axes exceeding the current level are

commanded in G02/G03

Note 9: The feedrate along the arc is related to not only F value and the override, but also the machining

precision(ISB, ISC) and the machining radius. For example, when the arc radius is smaller, the machining cannot be executed at the set feedrate to get the machining precision.

Note 10: The actual cutting feedrate is limited to max. cutting feedrate MFR of No.1422

Page 52

GSK988T Turning CNC System User Manual

G02/G03 compound programming example:

Ⅰ Programming

Φ22

R15

Fig. 2-8 Arc programming

Program：O0001 N001 G0 X40 Z5；（Rapidly traverse） N002 M03 S200；（Start the spindle） N003 G01 X0 Z0 F900； (Approach the workpiece) N005 G03 U24 W-24 R15；（Cut arc R15） N006 G02 X26 Z-31 R5；（Cut arc R5） N007 G01 Z-40； (Cut ф26) N008 X40 Z5； (Return to starting point) N009 M30；（End of program）

2.5 Dwell G04

Command function: execute the next block after dwelling the defined time.

Command format: G04 P__ ；or

G04 X__ ；or

G04 U__ ；or

G04；

Command specification: G04 is non-modal.

The dwell time is defined by the word P__, X__ or U__. X, U value can specify the decimal. P value cannot have the decimal, otherwise, the system alarms. Time of P__, X__ or U__ is shown below.

Address P U X

Unit

Note: DWT is the setting value of No. 1015 Bit 7(DWT).

DWT=1 0.001s

DWT=0

ISB 0.001s

ISC 0.0001s

s s

Page 53

Chapter Ⅱ G Commands

Value range of P__, X__ or U__ is shown below.

Address Incremental system Metric input Inch input

X, U

ISB system

-99999.999～99999.999 -9999.9999～9999.9999

ISC system

-9999.9999～9999.9999 -999.99999～999.99999

P ISB, ISC 0~99999999 0~99999999

Note 1: The system exactly stop a block when P, X, U are not input or P, X , U specify negative values. Note 2: X, U can command the negative value. The absolute value is taken as dwell time in G04, but the

address P cannot command the negative value.

Note 3: P time unit is set by No. 1015 Bit 7(DWT).

Note 4: P, X, U are in the same block, P is valid; X, U are in the same block, the later specified command is

valid.

Note 5: The dwell can be executed after the current delay time is completed in executing the feed hold in G04.

Note 6: When G04 and subprogram M98 /M99 P__ are in the same block, the number following P is the time

value of G04 dwell, and is also the message of M98/M99, i.e. subprogram skip message error.

Note 7: G04 and the interpolation command in Group 1(such as G00, G01) are in the same block, G04 is

valid, G0, G01 only change the modal value of G commands in Group 1.

Note 8: When No.3403 Bit 6(AD2) is 0, G04 and G commands in Group 00 are in the same block, and the

later specified command is valid.

Ⅰ Programming

2.6 Cylindrical Interpolation 7.1

Command function: the cylindrical interpolation is defined that the movement amount of

rotary axis specified by angle is converted into the movement distance

of linear axis along the surface in the CNC inside, which makes the

rotary axis and other axis execute the linear interpolation or circular

interpolation. After interpolation, the distance is converted into the

movement amount of the rotary axis, which is shown below:

Developed

Fig. 2-9

Command format：

Page 54

GSK988T Turning CNC System User Manual

X(U)

Y(V)

Z(W)

X(U)

Y(V)

Z(W)

⎫ ⎪ ⎪ ⎪

⎪

； Activate the cylindrical interpolation code. G07.1 can be written to G107

⎬ ⎪ ⎪ ⎪

⎪

⎭

or G7.1, but must not be with other command in a line;

⎫ ⎪ ⎪ ⎪

⎪

； Disable the cylindrical interpolation mode. It must not be with other

⎬ ⎪ ⎪ ⎪

⎪

⎭

⎧ ⎪ ⎪ ⎪

⎪

G07.1

⎨ ⎪

Ⅰ Programming

……；

⎪ ⎪

⎪

⎩

⎧ ⎪ ⎪ ⎪

⎪

G07.1

⎨ ⎪ ⎪ ⎪

⎪

⎩

command in a line;

Command explanation: G7.1 is non-modal; r is the cylindrical radius.

Note 1: The rotary axis in the cylindrical interplation mode is specified by No. 1022, X, Y, Z or the axis

parallel with it is also done. G17～G19 is specified to select the level for which the rotary axis is the

specified linear axis. For example, when the rotary axis is X, G17 must specify XY level which is

determined by the rotary axis and Y axis. The rotary axis in the cylindrical interpolation mode must be set to the only one.

Before the cylindrical interpolation, the level for cylindrical interpolation must be specified firstly,

otherwise, the alarm occurs; the alarm does when G17~G19 is specified to select the level when

the cylindrical interpolation is being executed; G17~G19 must be specified alone with the rotary

axis in the same block, otherwise, the alarm occurs.

Note 2: Even if the axis unspecified by the parameter commands the movement value in the cylindrical

interpolation mode, it does not execute the cylindrical interpolation;

Note 3: The specified feedrate is the speed of the unfolded cylindrical surface in the cylindrical

interpolation mode;

Note 4: One rotary axis and another linear axis can execute the circular interpolation in the cylindrical

interpolation mode. But the arc radius can be specified by only R instead of I, J and K. The usage

of the radius R is the same that of the circular interpolation;

The unit of the rotary axis is mm or inch instead of degree. For example, when the circular

interpolation is executed between Z and C axis, No. 1022 is set to 1 (X axis) for C axis; at the

Page 55

Chapter Ⅱ G Commands

moment, the circular interpolation command is: G18 Z__ C__； G02(G03) Z__ C__ R__；

For C axis, when No. 1022 is set to 2, the arc command is : G19 C__ Z__； G02(G03) Z__ C__ R__；

Note 5: Any tool radius compensation mode being executed must be cleared before the system enters the

cylindrical interpolation mode. Start and end the tool offset in the cylindrical interpolation mode;

the alarm occurs when the cylindrical interpolation is enabled in the used tool radius

compensation mode;

Note 6: In cylindrical interpolation mode, the movement amount of rotary axis specified by the angle is

converted into the movement distance of linear axis along outerside surface, which makes rotary

axis and another axis execute the linear interpolation or circular interpolation. After interpolation,

the distance is converted into the angle, and the movement amount for the conversion is rounded

to least input increment. So, when the diameter of the cylindrical is lesser, the actual movement

amount is not equal to the specified movement amount, but the error does not acculmulate.

MOTION_REV

amountmotion Actual

MOTION_REV：movement amount per rotation of rotary axis（its value is set by No.1260）；

R：Radius of workpiece； [ ]：Round to least input increment；

2π2

⎡ ⎢

××

valuecommand

⎣

2π2

MOTION_REV

⎤ ⎥

⎦

Ⅰ Programming

Note 7: In the cylindrical interpolation mode, the system alarms when the positioning operation (rapid

movement command G00 and other commands to bring rapid traverse, including G28, G53, G73,

G74, G76, G80～G89 ) cannot be specified;

Note 8: In the cylindrical interpolation mode, the system alarms when the workpiece coordinate system

（G50，G54～G59）or the local coordinate system is specified;

Note 9: In the cylindrical interpolation mode, the system resets to clear the cylindrical interpolation mode.

It must be specified again when the syste enters the cylindrical interpolation mode again;

Note 10: The tool offset must be specified before the cylindrical interpolation mode is set, and the alarm

occurs when the offset value is changed in the cylindrical interpolation mode.

Page 56

GSK988T Turning CNC System User Manual

Example：

O0001 (CYLINDRICAL INTERPOLATION);

N01 G00 Z100.0;

N02 M14; (the spindle is switched into

Ⅰ Programming

N03 G28 H0;(zero return of C axis )

N04 G18 C0;

N05 G07.1 C67.299;

N06 G01 G42 Z120.0 F250;

N07 C30.0;

N08 G03 Z90.0 C60.0 R30.0;

N09 G01 Z70.0;

N10 G02 Z60.0 C70.0 R10.0;

N11 G01 C150.0;

N12 G02 Z70.0 C190.0 R75.0;

N13 G01 Z110.0 C230.0;

N14 G03 Z120.0 C270.0 R75.0;

N15 G01 C360.0;

N16 G40 Z100.0;

N17 G07.1 C0;

N18 M15; ( the spindle is switched into speed

position control mode)

control mode)

N19 M30;

The above figure is the side unfolded cylindrical in the program. In the figure, when the

movement amount of rotary aixs (C axis) specified by the angle is converted into the distance of

linear axis of outside surface of the cylindrical, and the rotary axis and another linear axis (Z axis)

Page 57

Chapter Ⅱ G Commands

together execute interpolation, which is taken as the interpolation of Z-X level coordinate system

in G18 level.

When decoding “N07 C30.0”, the angle movement amount of the rotary axis C si converted into

the movment amount of linear axis:

67.299

=×=

Lmm

30 35.23

180

Thereafter, the operation result of C‘s linear movement and Z’s tool compensation is output to

the real-time interpolation value

2.7 Polar Coordinate Interpolation G12.1, G13.1

Command function: the contour is controlled by the programming command in the rectangle

coordinate system being switched into one linear motion (tool motion) and one turn motion (workpiece turn motion). The function is used to end face cutting.

Command format：G12.1； enter the polar coordinate interpolation mode, written to G112;

---------；

----------；

G13.1； cancel the polar coordinate interpolation mode, written to

G113;

Command explanation: G12.1, G13.1, are specified by an single block.

After the polar coordinate mode is activated, the linear or arc interpolation in the rectangular coordinate system which consists of the linear axis and the rotary axis can be commanded.

G12.1 activates the polar coordinate interpolation mode and select a

polar coordinate interpolation level, and the polar coordinate interpolation is completed in the level.

Ⅰ Programming

Fig. 2-10

Execution process: The polar coordinate interpolation program based on X (linear axis) and C

(rotary axis).

Page 58

GSK988T Turning CNC System User Manual

O0001； N10 T0202

…

N100 G00 X150 C0 Z0； N110 G12.1；

Path after tool nose radius compensation

N120 G42 G01 X80 F200;

Ⅰ Programming

N130 C20; N140 G03 X40 C40 R20;

Program path

N160

N150 G01 X-40; N160 G03 X-80 C20 R20; N170 G01 C-20;

N170

N180 G03 X-40 C-40 R20; N190 G01 X40;

N180

N200 G03 X80 C-20 R20; N210 G01 C0; N220 G40 X150.0; N230 G13.1; N240 Z100.0

…

N500 M30

Note 1: When the system is turned on or resets, the polar coordinate interpolation is cancelled(G13.1);

G12.1 and G13.1 are modal;

Note 2: The linear axis and turn axis for the polar coordinate interpolation must be set in advance in

NO.5460, NO.5461; the axis undefined by the parameter does not execute the polar coordinate interpolation in spite of specifying the movement value in the polar coordinate interpolation mode;

Note 3: The used level (selected by G17, G18 or G19) before G12.1 is cancelled; after G13.1 cancels the

polar coordinate interpolation, the level recovers; when the system resets, the polar coordinate interpolation is cancelled and the system uses the level selected by G17, G18 or G19;

Note 4: In the polar coordinate interpolation mode, the program commands use the rectangular coordinate

command in the polar coordinate level. The linear axis in the level uses the diameter or radius programming and the turn axis uses the radius programming;

Note 5: G codes in the polar coordinate interpolation mode can be used as follows: G01：linear interpolation; G02, G03：arc interpolation; G04：dwell; G40, G41, G42：tool nose radius compensation; G65, G66, G67：user macro program command; G98, G99：feed/rev, feed/minute; The system alarms when other G commands are executed in the polar coordinate interpolation mode. Note 6: F feedrate is the tangent speed with the polar coordinate interpolation level(rectangular coordinate

system) in the polar coordinate interpolation mode;

Note 7: The arc interpolation commanding the arc radius address is determined by the linear axis of the

interpolation level in the polar coordinate interpolation level as follows:

Use I and J when the linear axis is X or its parallel and the turn axis uses J; Use J and K when the linear axis is X or its parallel and the turn axis uses J; Use K and I when the linear axis is Z or its parallel and the turn axis uses I; Note 8: Must set a workpiece coordinate system before using G12.1, the center of the turn axis is the

origin of the coordinate system. The coordinate system must not be changed in G12.1 mode.

Note 9: Cannot start or cancel the polar coordinate interpolation mode; command G12.1 or G13.1 in G40;

otherwise, the system alarms;

Note 10: When the tool traverses near to the workpiece center in the polar coordinate interpolation mode,

C weight of feedrate changes, which exceeds max. C cutting speed to cause the system alarms.

Note 11: The program command uses the rectangular coordinate command in the polar coordinate level.

The axis address of the turn axis is taken as the one of the 2 When the system executes G12.1, the tool position of the polar coordinate interpolation starts

Virtual axis

N150

N140

N130

N120

N210

N190

N200

Fig.2-11

axis(imaginary axis) in the level.

Page 59

Chapter Ⅱ G Commands

from the angle 0. So, the spindle must be positioned before the polar coordinate interpolation is executed.

Note 12: The current position displays the actual coordinates in the polar coordinate interpolation.

However, the remainder distance is displayed according to the coordinates in the polar coordinate interpolation level(rectangular coordinate level).

Note 13: Must not switch the spindle gear in the polar coordinate interpolation. The system must be in the

spindle speed control mode when the gear shifting is needed.

2.8 Metric/Inch Switch G20, G21

Command function: realize the metric/inch switch of the system input mode. Command format: G20; inch input G21; metric input Command explanation: G20/G21 is modal in Group 6, and can be set to the initial mode by

No.0000 BIT2 (INI);

G20/G21

The units of the following value will change after they switch between the metric and the inch.

——F feedrate; ——position command; ——zero offset of workpiece; ——tool compensation value; ——scale unit of MPG; ——movement in incremental feed.

Note 1: The initial mode of G20/G21 is set by NO. 0000 BIT2 (INI) when the system is turned on. Note 2: When G20/G21 switches the current input mode, the system must set the beginning of the

program and specify in an alone block, otherwise, the system alarms.

Note 3: The tool compensation value must input the incremental unit and set it again. The tool

compensation value can automatically change and cannot be set again when NO.5006 Bit0 is 1.

Note 4: It modifies NO.0000 Bit2 (INI) when the system executes G20/G21. the displayed mode also

changes when NO.0000 Bit 2 (INI) is changed.

Ⅰ Programming

2.9 Stored Travel Check G22, G23

Command function: Create the forbidden area of stored travel limit check 2 and limit the tool

traverse range in one area.

Command format：G22； stored travel 2 check is turned on

---------；

G23； stored travel 2 check is turned off

Command explanation: G22: stored travel check is turned on; G23: stored travel check is turned off; Positive coordinates of the stored travel area is set by No.1322; Negative coordinates of the stored travel area is set by No. 1323; Limit area figure: taking examples of X, Y, Z limit area are as follows. X, Y, Z are positive

coordinates, I, J, K are negative.

Page 60

GSK988T Turning CNC System User Manual

Ⅰ Programming

Fig. 2-12

Note 1: The initial mode of G22/G23 can be set by No. 3402 Bit 7(G23) when the system is turned on again. Note 2: G22 stored travel check is limited to the stored travel limit check 2, and the detailed is referred to

OPERATION

Note 3: The data is set by the distance(min. command increment is taken as the unit) to the reference

position when the parameter sets the top point of the forbidden area;

Note 4: Whether the limit range is the inner side or outer side of the area is set by No. 1300 Bit0 (OUT) , and

it is the inner side when it is set to 0;

Note 5: The limit is valid after the system executes the reference position return; the system alarms when

the reference position is in the limit area in G22;

Note 6: The tool reversely traverses when the travel alarm appears; Note 7: G22/G23 is commanded in an alone block; Note 8: The system is switched from G23 to G22 in the forbidden area, there are as follows: the system

alarms in the next movement block when the forbidden area is in the inner side; alarms when the forbidden area is in the outer side;

Note 9: When the set forbidden area is set by mistaken sequence, the system executes the area check of

the two points as the top points;

Note 10: When No.1310 Bit 0(OT2x) of the stored travel limit check 2 is set to 1(executing the stored travel

limit 2 check), the system executes G22 and then the check; the system does not execute the check when it is G23.

;

2.10 Skip Interpolation G31

Command function: In the course of executing the command, when the outside skip signal

(X3.5) is input, the system stops the command to execute the next

block. The function is used to the dynamic measure (such as milling machine), toolsetting measure and so on of workpiece measure.

Command format：G31 IP_ F_；

Command explanations: non-modal G command (00 group);

Its address format is same that of G01; Cancel the tool nose radius compensation before using it; Feedrate should not be set to too big to get the precise stop

position;

The following block execution when skipping:

Page 61

Chapter Ⅱ G Commands

1. The next block of G31 is the incremental coordinate programming below.

Fig. 2-13

2．The next block of G31 is the absolute coordinate programming of one axis below.

Ⅰ Programming

Fig. 2-14

3. The next block of G31 is the absolute coordinate programming of two axes below

Program: G31 Z200 F100

G01 X100 Z300

Fig. 2-15

Skip signal explanation:

SKIP signal (SKIP): X3.5 Type: input signal

Function: X3.5 ends the skip cutting. I.e. in a block containing G31, the skip signal becoming the

absolute coordinate position of “1” is to be stored in the macro variable (#5061～

Page 62

GSK988T Turning CNC System User Manual

#5065, its last bit digit corresponds to the No. n axis of the system), at the same time, the movement in G31 block ends. No. 6200 Bit 19SK0) sets the invalid input state of the skip signal, and when it is set to 0, the input signal 1 is valid.

Operation: When the skip signal becomes “1”, CNC executes as follows: When the block is

Ⅰ Programming

executing G31, CNC stores the current absolute coordinates for each axis. CNC stops G31 to execute the next block, the skip signal detects its state instead of its RISING EDGE. So when the skip signal is “1”, it meets the skip conditions.

Note1: When the skip signal is input, the feedrate override, the dry run, and automatic acceleration/

deceleration are invalid in the course of movement by the skip function, which is to improve the tool positioning precision.

Note 2: The skip signal is valid, the system immediately stops the feed axis (without acceleration/

deceleration execution), and G31 feedrate should be as low as possible to get the precise stop position.

2.11 Automatic Tool Offset G36, G37

Command function: When the command is executed to make the tool move to the measured

position, the CNC automatically measures the difference between the current actual coordinates and the command coordinates to be the tool

offset value. The function is used to the automatic toolsetting. Command format: G36 X__; G37 Z__; Explanations: X absolute coordinate(only used to G36), Z absolute coordinate (only used to G37); Non-modal G command (00 group); Cancel the tool nose radius compensation before using it; Only use the absolute programming; Define the workpiece coordinate system before using the command; Specify the tool number and tool compensation number before using the command;

Measure position arrival signal: XAE(X3.6) ――――corresponding to G36 ZAE(X3.7) ――――corresponding to G37

Function: When the position measured by the program command is different from that where the

tool actually reaches (i.e. at the time, the measured position arrival signal becomes “1”), the difference of the coordinates is added to the current tool compensation value to update the compensation value. When G36X_(or G37Z_) is executed, the tool firstly rapidly traverses to the position measured by the command, and decelerates and temporarily stop the position before the measured position, and then, reaches to the measured position at the speed set by No.6241 (or No.6242). When the measured position arrival signal corresponding to G command becomes the state set by No. 6240#0, and the tool is in the measured position range ±ε, the system updates the offset compensation value and ends the block. When the measured position arrival signal does not become “1”, and after the tool reaches the measured position distance ε, the

Page 63

Chapter Ⅱ G Commands

CNC alarms, ends the block and does not update the offset compensation value.

Fig. 2-16

G36, G37 automatic tool offset command use

From the initial position to the measured position specified by Xa or Za in G36 or G37, the tool

rapidly traverses to A zone and stops at T point (Xa–γx or Za–γz) , and then traverses to B, C and D at the feedrate set by No.6241( or No.6242). The system alarms when the tool traverses in B zone and the measured point arrival signal of the end point is set to. The system alarms when the tool stops at V point. Parameter No. 6241, No. 6242, No.6254, No.6255 are set by the radius value.

Ⅰ Programming

Fig. 2-17

Example:

G50 X760 Z1100; create the workpiece coordinate system T0101; define No. 1 tool and execute its tool compensation G36 X200; traverse to X toolsetting point ( X toolsetting point coordinate:

200) T0101; execute X tool compensation again

G00 X204; retract a little G37 Z800; traverse to Z toolsetting point ( Z toolsetting point coordinate:

800) T0101; execute Z tool compensation again and the toolsetting is completed

Page 64

GSK988T Turning CNC System User Manual

M30;

Tool No.

Ⅰ Programming

Programming zero

Z measured position

Offset value (Before measure)

X measured position

Offset value (After measure)

Fig. 2-18

2.12 Reference Position Function

2.12.1 Reference position return G28

Command function: move from the starting point at the rapid traverse speed to the middle

position specified by IP_ and then return to the reference position.

Command format: G28 IP__ ；

Command explanation: G28 is non-modal. IP_: it is the middle point coordinates, is specified by the absolute

value and incremental value. Omit one or all command address for each axis, omitting some axis means the axis does not return to the reference position, omitting all means the middle point is the tool starting point in the current workpiece coordinate system, and the tool does not return to the reference position and keeps stopping.

Command execution process: (as Fig. 2-18):

（1）

Rapidly position from the current position to the middle position of the command

axis(A→B);

（2）

Rapidly position from the middle point to the reference position (B→R);

Page 65

Chapter Ⅱ G Commands

Fig. 2-19

Note 1: After the system is turned on, it does not execute the manual reference position return; when the

system executes G28 reference position return, it judges it alarms or executes like the manual reference position return according to No. 1002 Bit 3(AZR) to use the deceleration block to execute the reference position return. But, when the reference position setting function without the block(No.1002 Bit1 (DLZ)) is set to 1 or NO.1005 Bit 1(DLZx) is set to 1, it is unrelated to AZR setting, the system alarms when the system executes G28 before the reference position is created.

Note 2: Each axis separately moves at the rapid traverse speed from the starting point through the middle

point to the reference position, i.e. G00 mode.

Note 3: G28 or G30 in the tool radius compensation mode automatically cancels the tool radius

compensation, and automatically recovers it in the next movement command.

Note 4: Generally, G28 is specified in an alone line; when the system specifies simultaneously the same

parameter address word of G00 or G01, IP_ is specified to G28 parameter, G00 or G01 only change the modal value of the corresponding G groups and does not execute the motion.

Ⅰ Programming

2.12.2 2nd, 3rd, 4th reference position return G30

Command function: move at the rapidly traverse speed to the middle point specified IP_ and

then to the 2nd, 3rd and 4th reference position.

Command format：G30 P2 IP__ ；return to the 2

G30 P3 IP__ ；return to the 3

G30 P4 IP__ ；return to the 4

Command explanation: G30 is non-modal;

IP_: it is the middle point coordinates, is specified by the absolute value and incremental value. Omit one or all command address for each axis, omitting some axis means the axis does not return to the reference position, omitting all means the middle point is the tool starting point in the current workpiece coordinate system, and the tool does not return to the reference position and keeps stopping.

Command execution process (as Fig.2-18):

（1）

Rapidly position from the current position to the middle position of the command axis(A→B);

（2）

Rapidly position from the middle point to the reference position (B→R);

Note 1: Reference position position is set in NO.1241～NO.1243; Note 2: After the system is turned on, it executes the reference position return once before executing G30;

do not execute the reference position return firstly before executing G30 after the system with the absolute encoder is turned on;

Note 3: When P is omitted, the system executes it as P2 and returns to the 2 Note 4: The middle point will move to the new workpiece coordinate system when the workpiece

reference position

reference position;

Page 66

GSK988T Turning CNC System User Manual

coordinate system is changed;

Note 5: Each axis separately moves at the rapid traverse speed from the starting point through the middle

point to the reference position, i.e. G00 mode.

2.13 Related Function of Coordinate System

Ⅰ Programming

The tool position is expressed with the coordinate value of the coordinate system, the coordinate value is specified by the programmed axis. GSK988T system has three kinds of coordinate system:

1. machine coordinate system

2. workpiece coordinate system

3. local coordinate system

Fig.2-19 describes the relationship of the three coordinate systems:

G52

W0-54

G54

G50

G52

W0-59

G59

EXT

REF

Fig. 2-12

Page 67

Chapter Ⅱ G Commands

REF Reference position.

M0 Origin of machine coordinate system is a fixed point on the machine, No. 1240

value confirms the relative position of the reference position and the machine origin.

M2 The 2nd reference position, No.1214 set the 2nd reference position position in the

machine coordinate system.

EXT The outer origin offset can be set by No. 1220 or in the coordinate setting

window.

G50 The offset set by G50 is 0 when the system is turned on.

G54, 59 The offset of the workpiece coordinate system is set by No. 1221, No. 1226, and

is also set in the coordinate window.

W0-54,

W0-59

G52 The offset of the local coordinate system is 0 when the system is switched on. All

L0 Origin of the local coordinate system.

Note: The system has created the above coordinate system after the 1st reference position return is

Origin of the workpice coordinate system.

workpiece coordinate systems share, i.e. the local coordinate system offset set in one workpiece coordinate system can exist in other workpiece coordinate system.

executed. The coordinate system is created after the system is turned on with the absolute position encoder.

Ⅰ Programming

2.13.1 Selecting machine coordinate system position G53

A particular on the machine as the machining reference is called as the machine zero which is taken as the origin of the coordinate system is called as the machine coordinate system. After the system is turned on, executing the manual reference position return sets the machine coordinate system which keeps till the system is turned off.

Command format: G53 IP

Command function: when the position of the machine coordinate system is commanded, the

tool moves the position at the rapid traverse speed. Omitting one axis means the axis does not move; when the system only specifies G53 without specifying the

positions of any axes, the system does not execute the motion. Command explanation: G53 is non-modal; IP_: the absolute coordinate value for each axis in the machine

As the following figure: the specified axis rapidly moves from A (20,

;

coordinate system must be specified by the absolute value.

20) in the current workpiece coordinate system to B (-8, -10) in the machine coordinate system.

Page 68

GSK988T Turning CNC System User Manual

Ⅰ Programming

Fig.2-21

Note 1: G53 is non-modal, and is valid in other blocks; Note 2:G53 specifies the absolute position value in the machine coordinate system. The axis command is

ignored when some axis uses the incremental value command;

Note 3: When G53 is commanded, the system cancels the tool nose radius compensation; Note 4: After the system is turned on, the system performs the manual reference position return or G28

automatic reference position return, and automatically creates the origin position of the machine coordinate system according to the value set by No. 1240;

Note 5:The machine coordinate system must be set before the system commands G53. So, the system

must execute the manual reference position return or G28 automatic reference position return after it is turned on; the operation is not operated when the system uses the absolute position encoder;

Note 6: The system executes G53 and G00, G01 in Group 01 in the same block, G00 or G01 only modifies G

modal value in Group 01.

2.13.2 Workpiece coordinate system setting G50

The coordinate system used to machining the workpiece is called as the workpiece

coordinate system.

The workpiece coordinate system can be set in advance. The set workpiece can change its origin position to set again the position of workpice coordinate system in the machine coordinate system.

Command format: G50 IP__ ；

Command function: The absolute coordinate of the current position can be set by setting the

absolute coordinate of current position to create the workpiece coordinate system (called as the floating coordinate system). After the workpiece coordinate system is created, the absolute coordinate programming inputs the coordinate value in the coordinate system till

the new workpiece coordinate system in G50 is created. Command explanation: G50 is non-modal G; IP_: When the system uses the absolute command, it specifies the

new absolute coordinate position of the current point in the coordinate system; when the system uses the incremental command, after its executes G50, the absolute coordinate value of the current point is equal to the sum between the absolute coordinate value before execution and the coordinate incremental value.

Page 69

Chapter Ⅱ G Commands

Note 1: After G50 changes the workpiece coordinate system, other workpiece coordinate system also

performs the same offset;

Note 2: In G50, the system can omit one or all command addresses for each axis, the current coordinate

value is not input when the command value for each axis is not input. When the axis command address is omitted, the coordinate axis which is not input keeps its pervious coordinate value;

Note 3: When G50 and G command (G00, G01) are in the same block, the system only modifies the modal

value of Group 1, and the coordinate value in the block is specified by G50;

Note 4: When the system does not set G50 offset value, it can set No. 1202 Bit(G50) to forbid G50;

Note 5: After G50 sets the coordinate system, the system must be turned off and then on, the coordinate

values set by G50 remain unchanged before power off.

Note 6: In NC program, when LGT is set the coordinate offset mode to execute the tool offset, and the

system executes T function does not execute the absolute value command, the coordinate system is set by G50, the absolute coordinate value displayed by G50 is the one that the coordinate value set by G50 adding the tool compensation value which is not executed. The difference between the relative coordinates and the machine coordinates is （-80，10）when the system executes N4, the

difference value is caused because X100Z10 setting G50X20Z20 to create the workpiece coordinate system offset, i.e. the user does not think over the tool offset influence when G50 is set in NC program.

Program Absolute

N1 T0100 G00 X100 Z10

coordinate

X：100 Z：10 X：100 Z：10 X：100 Z：10

Relative

coordinate

Machine

coordinate

Ⅰ Programming

N2 T0101 （ No.01 tool

X：88 Z：-13 X：100 Z：10 X：100 Z：10

compensation value X12 Z23）

N3 G50 X20 Z20

N4 G00 X10 Z10

X：8 Z：-3 X：20 Z：20 X：100 Z：10

X：10 Z：10 X：22 Z：33 X：102 Z：23

2.13.3 Workpiece coordinate system selection command G54～G59

Command function: One of G54～G59 is specified, one of workpice coordinate system 1～6

can be selected. After the workpiece coordinate system is specified, the specified point in the block is in the specified workpiece till a new workpiece coordinate system is created as Fig. 2-21. The tool positions X60.0, Z20.0 in the workpiece coordinate system 3.

Fig. 2-22

Command format：G54 workpiece coordinate system 1；

Page 70

GSK988T Turning CNC System User Manual

G55 workpiece coordinate system 2； G56 workpiece coordinate system 3； G57 workpiece coordinate system 4； G58 workpiece coordinate system 5；

Ⅰ Programming

Command explanation: G54～G59 are modal.

Note 1: The workpiece is created after the system is turned on and executes the reference position

return. When the system is turned on, it automatically selects G54 as the current workpiece coordinate system;

Note 2: G54-G59 describing the 6 workpiece coordinate systems can change their positions by the

external workpiece zero offset value or workpiece zero offset value, and their relationship is as Fig. 2-22;

G59 workpiece coordinate system 6；

Fig. 2-23

Note 3: Use the following method to change:

1）MDI input changes the workpiece coordinate system zero; 2）Use G50 to move the workpiece coordinate system;

Specifying G50 IP_ makes the workpiece coordinate system（G54～G59）to set a new workpiece

coordinate system where the current tool position is consistent with the specified coordinates. When G50 specifies the relative value, the value adding the previous tool position coordinate value creates a new coordinate system, but the tool position does not change but the coordinate system executes the offset as Fig. 2-23:

Page 71

Chapter Ⅱ G Commands

Fig. 2-24

Note 4: The coordinate offset value created by G50 adds to the one of all workpiece zero to make ensure

that all workpiece coordinate systems offset the same value as Fig. 3-21:

Ⅰ Programming

Fig. 2-25

Note 5: The workpiece zero offset value of G54～G59 workpiece coordinate system can be set in the

parameters and input in the coordinate setting window;

Note 6: When the system is turned on, it defaults G54 as the current workpiece coordinate system; after

the system executes the reference position return, it creates the coordinate system, uses G55～

G59 to switch to other workpiece coordinate system; when the system resets, No.1201 Bit 7(WZR) determines whether the system returns to G54 workpiece coordinate system; when No. 3402 Bit 6(CLR) is set to 1, the modal returns to G54.

2.13.4 Local coordinate system setting G52

To be convenient to programming, the sub-coordinate system to set the workpiece coordinate system is called the local coordinate system. Command format: G52 IP__; set the local coordinate system …… G52 IP0; cancel the local coordinate system (IP0 means the absolute value

for each axis adds one zero)

Page 72

GSK988T Turning CNC System User Manual

Command function: commanding G52 in the program can set the local coordinate system in

the workpiece coordinate system G54~G59. The origin of the local coordinate system can set in the position specified by IP_ in the workpiece coordinate system. The corresponding relationship is as Fig. 2-26.

Ⅰ Programming

Fig. 2-26

Command explanation: G52 is non-modal;

IP_: when IP_ is absolute command, the system specifies the absolute coordinate value of origin of local coordinate system in the workpiece coordinate system; when IP_ is the incremental command, the system specifies the relative coordinate value of the origin of the local coordinate system related to the one of the workpiece coordinate system; Once the local coordinate system is created, its coordinates are used to the axis motion command. Using G52 to command the zero of the new local coordinate system( workpiece coordinate system) can change the position of the local coordinate system; Making the zero of the local coordinate system coincide with the one of the workpiece coordinate system can cancel the local coordinate system and returns to the workpiece coordinate system, i.e. command G52 X0 Z0.

Note 1: The local coordinate system setting does not change the workpiece coordinate system and

the machine coordinate system.

Note 2: Commanding G52 can temporarily cancel the offset in the tool nose radius compensation. Note 3: In local coordinate system, when G50 sets the workpiece coordinate system and the system

has not specified the coordinate values to all axes in the local coordinate system, the axis which is not specified in G50 in the local coordinate system still keeps, the local coordinate system corresponding to G50 axis is cancelled; For example:

……

G52 X50 Z50;

……

G50 X100; at the moment, Z coordinate value is not change, the local coordinate system

corresponding to X is cancelled ……

Note 4: When the system selects the workpice coordinate system command （G54～G59）to change

the workpiece coordinate system in the local coordinate system, the local coordinate system also moves to the new workpiece coordinate system.

Note 5: Whether the local coordinate system in reset is cancelled is determined by No.1202 Bit

3(RLC) , the local coordinate system is cancelled in reset when the parameter is set to 1.

Note 6: Whether the local coordinate system in manual reference position return is cancelled is

determined by No.1201Bit 2 (ZCL), the local coordinate system is cancelled in manual

Page 73

reference position return when the parameter is set to 1.

2.13.5 Level selection command G17～G19

Chapter Ⅱ G Commands

Command function: The level selection command is used to the arc interpolation and the

tool nose radius compensation selection level. Once the system has selected the level, it can execute the arc interpolation and tool nose

radius compensation on the level. Command format: G17 selects XpYp level; G18 selects ZpXp level; G19 selects YpZp level; Command explanation: G17, G18, G19 are modal G commands. Xp: X or its parallel axis Yp: Y or its parallel axis Zp: Z or its parallel axis

Note 1: Xp, Yp, Zp are determined by the axis addresses of G17, G18, G19 in the block; when the axis

addresses are omitted, the system defaults the omitted are the addresses of the basic axis; the level keeps when the system does not command G17, G18, G19 blocks.

Note 2: The parameter sets each axis to have three basic axes (X, Y, Z) or the parallel axis. Note 3: The level remains unchanged in the G17, G18, G19 not be specified. Note 4: When the system is turned on, its initialization is defaulted to G18 state, i.e. ZX level; Note 5: When the system repetitively specifies G17～G19 in the same block, and No.3403 Bit 6(AD2) is 0,

the last G17～G19 word is valid, the system alarms when the parameter is set to 1;

Note 6: The multi-compound cycle command（G70～G76） and the fixed cycle command（G90, G92, G94

are used to ZX basic axis level; when their functions are specified in other levels, the system alarms;

Note 7: The motion command is not related to the level selection, besides the arc interpolation and tool

nose radius compensation command, when the system commands the axis beyond the levels, it does not alarm and the axis can move; when the system selects the axis motion beyond the level in the arc interpolation command, the system alarms. For example:

……;

G17; G01 X100 Y50 Z20 F100; the system does not alarm, Z moves

……;

G02 X20 Z50 R100; the system alarms

……;

Example: the level selection: when X and A are parallel axis: G17 X_ Y_ ；select XY level G17 A_ Y_ ；select AY level G18 X_ Z_ ；select ZX level G17； select XY level

G17 A_ select AY level G18 Y_ select ZX level, Y motion is not relative the level

Ⅰ Programming

）

2.13.6 Exact stop mode G61/cutting mode G64

G61 function: After programmed axis of the block must exactly stop at the end pont of the

block, the next block is executed.

G64 function: When the programmed axis of each block following G64 starts to develerate (it

has not reached the programmed end point), the system starts to execute

Page 74

GSK988T Turning CNC System User Manual

the next block, the programmed contour in G64 is different from the actual,

and the difference condition is determined by F value and the angle between

two paths, the more the different is, the more F value is.

Command format： G61; （exact stop mode）

Ⅰ Programming

Command explanations:

1. A block including G61 eactaly stops the end point of the program before the system

executes the next block, which is used to process sharpt edges and corners. G61 is

modal and valid till G64 is commanded. The programmed contour is the same that of the

actual.

2. G64 is modal, valid and default before G61 is commanded. G64 path is different from that

of G61 as Fig. 2-27;

3. G61, G64 belong to Group 15, and their relations with other G groups are referred to

Group 5.

4. When G01 is executed, it is in the exact stop in cutting mode because it is non cutting

command.

5. When G61/G64 is specified, it is value in the next commanded block.

G64; （cutting mode）

Note: The system defaults G64 cutting mode.

Tool path in cutting mode

Fig. 2-27

Tangential point

Tool path when specifying exact stop

Tangential point

2.14 Fixed Cycle Command

To simplify programming, the system defines G command of single machining cycle with one block to complete the rapid traverse to position, linear/thread cutting and rapid traverse to return to the starting point:

G90: axial cutting cycle; G92: thread cutting cycle; G94: radial cutting cycle;

G92 thread cutting fixed cycle command is described in Thread Function.

2.14.1 Axial cutting cycle G90

Command function: From starting point, the cutting cycle of cylindrical surface or taper

Page 75

Chapter Ⅱ G Commands

surface is completed by radial feeding(X) and axial (Z or X and Z) cutting.

Command format：G90 X（U）__ Z（W）__ F__；（cylinder cutting）

G90 X（U）__ Z（W）__ R__ F__；（taper cutting）

Command specifications:

G90 is modal;

X_,Z_ Coordinates of longitudinal cutting (C point in the figure below)

U_,W_ Movement to end point (C point in the figure below) of longitudinal cutting

F_ Cutting feedrate

Taper（radius value, with direction, range referred to the table below

Ⅰ Programming

Address Incremental system

Cycle process:

ISB system

ISC system

① X rapidly traverses from starting point to cutting starting point; ② Cutting feed (linear interpolation) from the cutting starting point to cutting end point;

③ X executes the tool retraction at feedrate (opposite direction to the above-mentioned ①),

and return to the position which the absolute coordinates and the starting point are the same;

④ Z rapidly traverses to return to the starting point and the cycle is completed.

metric（mm）input

-99999.999～99999.999mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

Inch (inch) input

Fig.2-28

Page 76

GSK988T Turning CNC System User Manual

Ⅰ Programming

Fig. 2-29

Cutting path: Relative position between cutting end point and starting point with U, W, R, and tool

path of U, W, R with different sign symbols are as Fig. 2-28:

1） U>0，W<0，R>0 2） U<0，W<0，R<0

3） U>0，W>0，R<0 ,│R│≤│U/2│ 4） U<0，W>0，R>0,│R│≤│U/2│

Fig.2-30

Page 77

Example: Fig. 2-29, rod Φ125×110

Chapter Ⅱ G Commands

Ⅰ Programming

Fig.2-31

Program：

Program : O0002; M3 S300 G0 X130 Z3;

G90 X120 Z-110 F200; (A→D, cut Φ120) X110 Z-30;

X100; X90; X80; X70; X60; G0 X120 Z-30; G90 X120 Z-44 R-7.5 F150; Z-56 R-15 Z-68 R-22.5

Z-80 R-30 M30;

（A→B，6 times cutting cycle Φ60, increment of 10mm）

（B→C，4 times taper cutting）

2.14.2 Radial cutting cycle G94

Command function: From starting point, the cutting cycle of cylindrical surface or taper

surface is completed by radial feeding(X) and axial (Z or X and Z) cutting.

Command format: G94 X(U) __ Z(W) __ F__; (face cutting)

G94 X(U) __ Z(W) __ R__ F__; (taper face cutting)

Command specifications: G94 is modal;

X_,Z_ Coordinate of cutting end point(C point in the figure below)in the direction of

the bottom side

U_,W_ Movement to cutting end point (C point in the figure below)in the direction of

bottom side

F_ Cutting feedrate

Taper Taper（radius value, with direction, range referred to the table below

Page 78

GSK988T Turning CNC System User Manual

Address Incremental

system

Ⅰ Programming

Cycle process:

① Z rapidly traverses from starting point to cutting starting point;

② Cutting feed (linear interpolation) from the cutting starting point to cutting end point;

③ Z executes the tool retraction at the cutting feedrate (opposite direction to the

above-mentioned ①), and returns to the position which the absolute coordinates and the starting point are the same;

④ The tool rapidly traverses to return to the starting point and the cycle is completed.

ISB system

ISC system

Metric（mm）input

-99999.999～99999.999mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

Inch (inch) input

Fig. 2-32

Fig.2-33

Page 79

Chapter Ⅱ G Commands

Cutting path: Relative position between cutting end point and starting point with U, W is as Fig.2-32:

1） U>0 W<0 R<0 2） U<0 W<0 R<0

（3）U>0 W>0 R<0 （│R│≤│W│） 4）U<0 W>0 R<0 （│R│≤│W│）

Ⅰ Programming

Example: Fig. 2-35, rob Φ125×112

Program：

G00 X130 Z5 M3 S1； G94 X0 Z0 F200 End face cutting

X120 Z-110 F300；

G00 X120 Z0

Fig. 2-34

（cut outer Φ120）

Page 80

G94 X108 Z-30 R-10

X96 R-20 X84 R-30

X72 R-40 X60 R-50；

GSK988T Turning CNC System User Manual

（C→B→A，cut Φ60）

Ⅰ Programming

M30；

Note 1:These fixed cycle commands are used to ZX level. The system alarms when other axis motion in

the block of the fixed cycle command is commanded;

Note 2: After X(U) , Z(W) , R are executed in the canned cycle command, their command values are value if

X(U) , Z(W) ,R are not redefined by executing a new canned cycle commands. The command values of X(U) ,Z(W) ,R are cleared if non-modal G command(00 Group) except for G04 or G00, G01, G02, G03, G32 is executed;

Note 3: In MDI mode, the previous canned cycle can be executed by pressing the cycle start key after the

canned cycle is completed;

Note 4: One cycle cannot be executed repetitively in G90～G94 when the next block of G90～G94 is M, S, T

command; the previous cycle is executed repetitively in G90～ G94 when the next block is

ended( EOB;).

Example …

N010 G90 X20.0 Z10.0 F400； N011 ；（execute G90 one time again）

…

Note 5: Pause or single block is executed in G90, G94, the single block stops after the tool moves end

point of current path.

2.15 Multiple Cycle Commands

GSK988T multiple cycle commands include axial roughing cycle G71, radial roughing cycle G72, closed cutting cycle G73, finishing cycle G70, axial grooving multiple cycle G74, axial grooving multiple cycle G75 and multiple thread cutting cycle G76. When the system executes these commands, it automatically counts the cutting times and the cutting path according to the programmed path, travels of tool infeed and tool retraction, executes multiple machining cycle(tool infeed →cutting→retract tool→tool infeed), automatically completes the roughing, finishing workpiece and the starting point and the end point of command are the same one.

G76 multiple thread cutting cycle command is described in Thread Function.

2.15.1 Axial Roughing Cycle G71

Command function: G71 is divided into three parts:

: 1st blocks for defining the travels of tool infeed and retract tool, the ⑴

cutting feedrate, the spindle speed and the tool function when roughing;

: 2nd blocks for defining the block in⑵ terval, finishing allowance; : 3rd blocks for some continuous finishing path, counting the roughing ⑶

path without being executed actually when executing G71. According to the finishing path, the finishing allowance, the path of tool infeed and tool retract, the system automatically counts the path of

roughing，the tool cuts the workpiece in paralleling with Z, and the

roughing is completed by multiple executing the cutting cycle tool infeed→ cutting→tool retraction. The starting point and the end point

Page 81

are the same one. The command is applied to the formed roughing of non-formed rod.

Command format：G71 U（Δd

G71 P（ns）

Chapter Ⅱ G Commands

）

R（e） F S T Q（nf） U（Δu） W（Δw）； ⑵

；

⑴

N（ns）．．．．．；

Command specifications：

(1) ns～nf blocks in programming must be followed G71 blocks. If they are in the front of G71

blocks, the system automatically searches and executes ns ～ nf blocks, and then

executes the next program following nf block after they are executed, which causes the system executes ns～nf blocks repetitively;

(2) ns～nf blocks are used to count the roughing path and the blocks are not executed when

G71 is executed. F, S, T commands of ns～nf blocks are invalid when G71 is executed, at the moment, F, S, T commands of G71 blocks are valid. F, S, T of ns～nf blocks are valid when executing ns～nf to command G70 finishing cycle;

(3) For G71 (I type), ns block is only G00, G01 which has no Z (W) in Group 01, otherwise,

the system considers it G71 ( type)Ⅱ machining;

(4) X and Z dimensions must be changed monotonously (always increasing or reducing) for

the finishing path;

(5) In ns～nf blocks, there are only G commands: G01, G02, G03, G04, G96, G97, G98, G99,

G40, G41,G42 and the system cannot call subprograms(M98/M99); (6) G96, G97, G98, G99, G40, G41, G42 are invalid in G71 and valid in G70, G96, G97, G98, (7) When G71 is executed, the system can stop the automatic run and manual traverse, but

return to the position before manual traversing when G71 is executed again, otherwise,

the following path will be wrong; (8) When the system is executing the feed hold or single block, the program pauses after the

system has executed end point of current path; (9) d△ ， u are specified by the same U and different with or without being specified P,Q

commands; (10) G71 cannot be executed in MDI, otherwise, the system alarms;

Relevant definitions:

Finishing path

△

As Fig. 2-34, Part 3 of G71(ns～nf block)defines the finishing path, and the starting point

of finishing path (starting point of ns block)is the same these of starting point and end point of G71, called A point; the first block of finishing path(ns block)is used to X rapid traversing or tool infeed, and the end point of finishing path is called to B point; the end point of finishing path(end point of nf block)is called to C point. The finishing path is A→B→C

．．．．．．．．；．．．．F；．．．．S；．．．．

N（nf）．．．．．；

⑶

Ⅰ Programming

Page 82

GSK988T Turning CNC System User Manual

Roughing path

Δd

Ⅰ Programming

ns Block number of the first block of finishing path

nf Block number of the last block of finishing path

Δu X finishing allowance range is as the following table (diameter) with sign symbols. X

Δw Z finishing allowance range is as the following table (diameter) with sign symbols. X

F Cutting feedrate; S: Spindle speed; T: Tool number, tool offset number

The finishing path is the one after offsetting the finishing allowance（Δu, Δw）and is the

path contour formed by executing G71. A, B, C point of finishing path after offset corresponds separately to A’, B’, C’ point of roughing path, and the final continuous cutting path of G71 is B’→C’ point

It is each travel（radius value）of X tool infeed in roughing without sign symbols, and the direction of tool infeed is defined by move direction of ns block. The command value Δd is

reserved after executing U（Δd）and the value of NO.5132 is rewritten. The value of system

parameter NO.5132 is regarded as the travel of tool infeed when U（Δd）is not input

It is travel（radius value）of X tool retraction in roughing（radius value）without sign symbols,

and the direction of tool retraction is opposite to that of tool infeed, the command value e is

reserved and the value of system parameter NO.5133 is rewritten after R（e）is executed.

The value of system parameter NO.5133 is regarded as the travel of tool retraction when

R（e）is not input

coordinate offset of roughing path compared to finishing path, i.e. the different value of X absolute coordinates between A’ and A. The system defaults Δu=0 when U（Δu）

input, i.e. there is no X finishing allowance for roughing cycle

coordinate offset of roughing path compared to finishing path, i.e. the different value of X absolute coordinates between A’ and A. The system defaults Δw=0 when U（Δw）

input, i.e. there is no Z finishing allowance for roughing cycle

is not

M, S, T, F

Address Incremental system

U（Δd）

R（e）

U（Δu）

W（Δw）

P（ns）

Q（nf）

Execution process: as Fig. 2-36.

① X rapidly traverses to A’ from A point, X travel is Δu, and Z travel is Δw

They can be specified in the first G71 or the second ones or program ns～nf. M, S, T, F

functions of M, S, T, F blocks are invalid in G71, and they are valid in G70 finishing blocks

metric（mm）input

ISB system 0.001~99999.999 0.0001~9999.9999

ISC system 0.0001~9999.9999 0.00001~999.99999

ISB system

ISC system

ISB system

ISC system

ISB system

ISC system

0～99999.999 0～9999.9999

0～9999.9999 0～999.99999

-99999.999～99999.999 -9999.9999～9999.9999

-9999.9999～9999.9999 -999.99999～999.99999

-99999.999～99999.999 -9999.9999～9999.9999

-9999.9999～9999.9999 -999.99999～999.99999

1～99999 1～99999

inch(inch) input

Page 83

Chapter Ⅱ G Commands

② X moves from A’is Δd( tool infeed), ns block is for tool infeed at rapid traverse speed with

G0, is for tool infeed at feedrate F with G71, and its direction of tool infeed is that of A→B point;

③ Z executes the cutting feeds to the roughing path, and its direction is the same that of Z

coordinate A→B point;

④ X, Z execute the tool retraction e (45°straight line)at feedrate, the directions of tool

retraction is opposite to that of too infeed;

⑤ Z rapidly retracts at rapid traverse speed to the position which is the same that of Z

coordinate;

⑥ After executing X tool infeed (Δd+e)again, the end point of traversing tool is still on the

middle point of straight line between A’ and B’(the tool does not reach or exceed B’), and after executing the tool infeed (Δd+e)again, execute ③；after executing the tool infeed (Δd+e)again, the end point of tool traversing reaches B’ point or exceeds the straight line between A’→B’ point and X executes the tool infeed to B’ point, and then the next step is executed;

⑦ Cutting feed from B’ to C’ point along the roughing path;

⑧ Rapid traverse to A from C’ point and the program jumps to the next clock following nf

block after G71 cycle is ended.

Ⅰ Programming

Fig. 2-36 G71 cycle path

Coordinate offset direction with finishing allowance: Δu, Δw define the coordinates offset and its direction of finishing, and their sign symbols are

as follows Fig. 2-35: B→C for finishing path, B’→C’ for roughing path and A is the tool starting point

Page 84

GSK988T Turning CNC System User Manual

B’

Ⅰ Programming

C’

A’

B’

A’

C’

Fig.2-37

Example：Fig. 2-38

Fig.2-38

Program：O0004；

G00 X200 Z10 M3 S800；（Spindle clockwise with 800 rev/min）

G71 U2 R1 F200；（Cutting depth each time 4mm，tool retraction [in diameter]）

Page 85

Chapter Ⅱ G Commands

G71 P80 Q120 U0.5 W0.2；（roughing a---e，X machining allowance 0.5mm , Z 0.2mm N80 G00 X40 S1200；（Positioning）

G01 Z-30 F100 ；（a→b）

X60 W-30；（b→c） a→b→c→d→e blocks for finishing path

W-20；（c→d）

N120 X100 W-10；（d→e）

G70 P80 Q120；（a---e blocks for finishing path）

M30；（End of block）

G71 supports continuous grooving machining:

Direction of the shape in the 2

axis of the level (X axis in ZX level) is not necessary to

monotonous rise or fall, and there may be up to 10 groovings, which is shown below:

）

Ⅰ Programming

Fig. 2-39

But, external contour along Z must mononously rise or fall, and the following contour cannot be machined:

Monontone change is not observed along the Z axis

Fig. 2-40

The first tool must be vertical: the machining can be executed when the shape along Z changes

mononously, which is shown below:

Fig. 2-41 The tool retraction should be executed after turning, and the retraction amount is specified by R (e) or No 5133, which is shown below:

Page 86

GSK988T Turning CNC System User Manual

e（set by a parameter）

Ⅰ Programming

Fig. 2-42

Execution process sketch:

Fig. 2-43

Note 1: For grooving, X (U), Z(W) must be specified, and W0 is done when Z does not move. Note 2: For grooving, the finishinig allowance is specified to X direction, is invalid for Z direction.

Note 3: For grooving, the tool retraction amount is left to make the tool approach the workpiece(Label 25,

26) with G1 speed after the current grooving is done to execute the next grooving. When the

retraction amount is 0 or the left distance is less than retraction amount, the tool approaches the

workpiece with G1 speed.

Note 4: For grooving, the finishing path (ns～nf block), Z dimension must mononously change (always

increase or decrease)

Note 5: For G71 II type, when there is arc in finishing path (ns～nf), # 3410 parameter (the arc radius

permits error) cannot be non-zero, i.e., the permitting function of arc radius error cannot be

activated.

Note 6: Radius error is irrelevant to cutting allowance, and radius error is permitted and checks whether

the alarm occurs.

2.15.2 Radial Roughing Cycle G72

Command function：G72 is divided into three parts:

⑴

1st blocks for defining the travels of tool infeed and tool retraction, the cutting speed, the spindle speed and the tool function in roughing;

Page 87

Chapter Ⅱ G Commands

⑵ 2nd blocks for defining the block interval, finishing allowance; ⑶ 3rd blocks for some continuous finishing path, counting the roughing path without being

executed actually when G72 is executed. According to the finishing path, the finishing allowance, the path of tool infeed and retract

tool, the system automatically counts the path of roughing，the tool cuts the workpiece in

paralleling with Z, and the roughing is completed by multiple executing the cutting cycle tool infeed→cutting feed→tool retraction. The starting point and the end point of G72 are the same one. The command is applied to the formed roughing of non-formed rod.

Command format ：G72 W（Δd

）

R（e） F S T

；

⑴

Ⅰ Programming

Q（nf） U（Δu） W（Δw）； ⑵

⑶

G72 P（ns）

（ns）．．．．．；

．．．．．．．．；．．．．F；．．．．S；．．．．；

N （nf）．．．．．；

Command specifications:

1. ns～nf blocks in programming must be followed G72 blocks. If they are in the front of G72 blocks, the system automatically searches and executes ns～nf blocks, and then executes

the

next program following nf block after they are executed, which causes the system executes ns～nf blocks repetitively;

2. ns～nf blocks are used for counting the roughing path and the blocks are not executed when G72 is executed. F, S, T commands of ns～nf blocks are invalid when G72 is executed, at the moment, F, S, T commands of G72 blocks are valid. F, S, T of ns～nf blocks are valid when executing ns～nf to command G70 finishing cycle;

3. There are G00,G01 without the word X(U) in ns block, otherwise the system alarms;

4. X,Z dimensions in finishing path(ns～nf blocks) must be changed monotonously (always

increasing or reducing) for the finishing path;

5. In ns～nf blocks, there are only G commands: G01, G02, G03, G04, G96, G97, G98, G99,

G40, G41,G42 and the system cannot call subprograms(M98/M99);

6. G96, G97, G98, G99, G40, G41, G42 are invalid in G72 and valid in G70;

7. When G72 is executed, the system can stop the automatic run and manual traverse, but return to the position before manual traversing when G72 is executed again, otherwise, the following path will be wrong;

8. When the system is executing the feed hold or single block, the program pauses after the system has executed end point of current path;

9. d△ ， u are specified by the same U and different with or without being specified P,Q △

commands;

10. G72 cannot be executed in MDI, otherwise, the system alarms.

Relevant definitions:

Finishing path

the above-mentioned Part⑶ of G71(ns～nf block)defines the finishing path, and

Page 88

GSK988T Turning CNC System User Manual

the starting point of finishing path (i.e. starting point of ns block)is the same these of starting point and end point of G72, called A point; the first block of finishing path(ns block)is used for Z rapid traversing or cutting feed, and the end point of finishing path is called to B point; the end point of finishing path(end point of nf block)is called to C point. The finishing path is A→B→C.

Ⅰ Programming

Roughing path

Δd It is each travel of Z tool infeed in roughing without sign symbols, and the direction

e It is each travel of Z tool infeed in roughing without sign symbols, and the direction

ns Block number of the first block of finishing path.

nf Block number of the last block of finishing path.

Δu X finishing allowance in roughing, (X coordinate offset of roughing path compared

Δw Z finishing allowance in roughing, its value: -9999.999~9999.999 ( Z coordinate

F Cutting feedrate; S: Spindle speed; T: Tool number, tool offset number.

M, S, T, F

Address Incremental system

The finishing path is the one after offsetting the finishing allowance（Δu, Δw）and is

the path contour formed by executing G72. A, B, C point of finishing path after offset corresponds separately to A’, B’, C’point of roughing path, and the final continuous cutting path of G72 is B’→C’ point.

of tool infeed is defined by move direction of ns block. Δd is reserved after the

system executes W（Δd）and NO.5132 value is modified. The value of system

parameter NO.051 is regarded as the travel of tool infeed when W（Δd）is not input.

of tool retraction is opposite to that of tool infeed; after R(e) is executed, e value e is reserved and the system modifies No.5133 value. The value of system

parameter NO.5133 is regarded as the travel of tool retraction when R（e）is not

input.

to finishing path, i.e. the different value of X absolute coordinate between A’and A, diameter value with sign symbols).

offset of roughing path compared to finishing path, i.e. the different value of X absolute coordinates between A’ and A, with sign symbols).

They can be specified in the first G72 or the second ones or program ns～nf. M, S,

T, F functions of M, S, T, F blocks are invalid in G72, and they are valid in G70 finishing blocks.

Metric（mm）input

Inch (inch) input

W（Δd）

R（e）

U（Δu）

W（Δw）

P（ns）

Q（nf）

ISB system 0.001~99999.999 0.0001~9999.9999

ISC system 0.0001~9999.9999 0.00001~999.99999

ISB system

ISC system

ISB system

ISC system

ISB system

ISC system

0～99999.999 0～9999.9999

0～9999.9999 0～999.99999

-99999.999～99999.999 -9999.9999～9999.9999

-9999.9999～9999.9999 -999.99999～999.99999

-99999.999～99999.999 -9999.9999～9999.9999

-9999.9999～9999.9999 -999.99999～999.99999

1～99999 1～99999

Page 89

Chapter Ⅱ G Commands

ISC system

Execution process： Fig. 2-44

① X rapidly traverses to A’ from A point, X travel is Δu, and Z travel is Δw; ② X moves from m A’is Δd( tool infeed), ns block is for tool infeed at rapid traverse

speed with G0, is for tool infeed at G72feedrate F in G1, and its direction of tool infeed is that of A→B point;

③ X executes the cutting feeds to the roughing path, and its direction is the same that

of X coordinate B→C point;

④ X, Z execute the tool retraction e (45°straight line)at feedrate, the directions of tool

retraction is opposite to that of tool infeed ;

⑤ X rapidly retracts at rapid traverse speed to the position which is the same that of Z

coordinate;

⑥ After Z tool infeed (Δd+e)again is executed, the end point of traversing tool is still on

the middle point of straight line between A’ and B’(the tool does not reach or exceed B’), and after Z executes the tool infeed (Δd+e)again, is executed③ ；after the tool infeed (Δd+e) is executed again, the end point of tool traversing reaches B’ point or exceeds the straight line between A’→B’ point and Z executes the tool infeed to B’ point, and then the next step is executed;

⑦ Cutting feed from B’ to C’ point along the roughing path; ⑧ Rapidly traverse to A from C’ point and the program jumps to the next clock

following nf block after G71 cycle is completed.

1～99999 1～99999

Ⅰ Programming

Fig. 2-44

Coordinate offset direction with finishing allowance:

Δu, Δw define the coordinates offset and its direction of finishing, and their sign symbols

are as follows Fig. 2-45: B→C for finishing path, B’→C’ for roughing path and A is the starting point.

Page 90

GSK988T Turning CNC System User Manual

B’

A’

B’

Ⅰ Programming

C’

B’

C’

A’

C’

B’

Example：Fig. 2-46

Program：

O0005； G00 X176 Z10 M03 S500 （Change No.2 tool and execute its compensation,

Fig.2-45

80 20 15 20

Fig.2-46

Starting point

(176,10)

spindle rotation with 500 rev/min）

G72 W2.0 R0.5 F300；（Tool infeed 2mm, tool retraction 2mm）

G72 P10 Q20 U0.2 W0.1；（Roughing a--d，X roughing allowance 0.2mm and Z

0.1mm）

N10 G00 Z-55 S800 ；（Rapid traverse）

Page 91

G01 X160 F120；（Infeed to a point）

X80 W20；（Machining a—b

W15；（Machining b—c） Blocks for finishing path

N20 X40 W20 ；（Machining c—d）

G70 P050 Q090 M30；（Finishing a—d）

2.15.3 Closed Cutting Cycle G73

Command functions: G73 is divided into three parts:

⑴

Blocks for defining the travels of tool infeed and tool retraction, the cutting speed, the spindle speed and the tool function when roughing;

Blocks for defining the block interval, finishing allowance;⑵

Blocks for some continuous finishing p⑶ ath, counting the roughing

path without being executed actually when executing G73.

According to the finishing allowance, the travel of tool retraction and

the cutting times, the system automatically counts the travel of roughing offset，the travel of each tool infeed and the path of roughing,

the path of each cutting is the offset travel of finishing path, the cutting path approaches gradually the finishing one, and last cutting path is the finishing one according to the finishing allowance. The starting point and end point of G73 are the same one, and G73 is applied to roughing for the formed rod. G73 is non-modal and its path is as Fig.2-40.

Command forma：G73 U（Δi）

G73 P（ns）

W （Δk） R （d） F S T ； ⑴

Q（nf） U（Δu） W（Δw）； ⑵

Chapter Ⅱ G Commands

）

Ⅰ Programming

（ns）．．．．．；

．．．．．．．；

．．．．F；．．．．S；．．．．；

（nf）．．．．．；

Command specifications：

1. ns～nf blocks in programming must be followed G73 blocks. If they are in the front of G73 blocks, the system automatically searches and executes ns～nf blocks, and then

executes the next program following nf block after they are executed, which causes the system executes ns～nf blocks repetitively.

2. ns～nf blocks are used for counting the roughing path and the blocks are not executed when G73 is executed. F, S, T commands of ns～nf blocks are invalid when G71 is executed, at the moment, F, S, T commands of G73 blocks are valid. F, S, T of ns～nf

⑶

Page 92

GSK988T Turning CNC System User Manual

blocks are valid when executing ns～nf to command G70 finishing cycle.

3. There are only G00, G01 in ns block.

4. In ns～nf blocks, there are only G commands:G00, G01, G02, G03, G04, G96, G97,

G98, G99, G40, G41,G42 and the system cannot call subprograms(M98/M99)

5. G96, G97, G98, G99, G40, G41, G42 are invalid in G73 and valid in G70.

Ⅰ Programming

Finishing path

Roughing path It is one group of offset path of finishing one, and the roughing path times are the

6. When G73 is executed, the system can stop the automatic run and manual traverse, but return to the position before manual traversing when G73 is executed again, otherwise, the following path will be wrong.

7. When the system is executing the feed hold or single block, the program pauses after the system has executed end point of current path.

8. i△ ， u are specified by the same U and Δk△ ，Δw are specified by the same U, and they

are different with or without being specified P, Q commands.

9. G73 cannot be executed in MDI, otherwise, the system alarms.

10. Z must be the monotonous in the cycle body specified by P and Q. Z tool retraction and finishing allowance are set to 0 when the system executes X non-monotonous workpiece. When No. 5102 Bit0 (MRI) is set to 1, the system does not alarm.

11. When the programming is executed, and the initial positioning point retreats one tool infeed value in the direction of cutting but the result is in the contour range, the dry run is executed to observe whether its own path of the system has overcutting because the tool retraction direction is the same that of tool infeed in programming state.

Relevant definitions:

The above-mentioned Part 3 of G73(ns～nf block)defines the finishing path, and

the starting point of finishing path (start point of ns block)is the same these of starting point and end point of G73, called A point; the end point of the first block of finishing path(ns block)is called B point; the end point of finishing path(end point of nf block)is called C point. The finishing path is A→B→C.

same that of cutting. After the coordinates offset, A, B, C of finishing path separately corresponds to A

n, Bn, Cn

cutting path is A1, B1, C1 and the last one is A

of roughing path(n is the cutting times, the first

d, Bd, Cd

). The coordinates offset value

of the first cutting compared to finishing path is （Δi×2+Δu，Δw+Δk）（diameter

Δi

Δk

programming）, the coordinates offset value of the last cutting compared to finishing path is（Δu，Δw），the coordinates offset value of each cutting compared to the previous one is（Δi×2/d-1，Δk/d-1）.

Travel of X tool retraction in roughing is the following table（radius value with sign symbols）, Δi is equal to X coordinate offset value（radius value）of A1 point

compared to Ad point. The X total cutting travel(radius value) is equal to |Δi| in roughing, and X cutting direction is opposite to the sign symbol of Δi: Δi＞0, cut in X negative direction in roughing. It is reserved after Δi command value is executed and the system rewrites No.5135 value. NO.5135 value is regarded as the travel of X tool retraction of roughing when U（Δi）is not input.

Travel of Z tool retraction in roughing is the following table（radius value with sign symbols）, Δk is equal to X coordinate offset value（radius value）of A1point

compared to A

point. The Z total cutting travel(radius value) is equal to |Δk| in

Page 93

Chapter Ⅱ G Commands

roughing, and Z cutting direction is opposite to the sign symbol of Δk: Δk＞0, cut in Z negative direction in roughing. It is reserved after Δk command value is

executed and the system rewrites No.5136 value. NO.5136 value is regarded as the travel of X tool retraction of roughing when W（Δk）is not input.

d It is the cutting times and its range is referred to the following table. R5 means the

closed cutting cycle is completed by 5 times cutting. R（d）is reserved after it is

executed and the system rewrites NO.5137. The value of system parameter NO.5137 is regarded as the cutting times when R（d is not input.

ns Block number of the first block of finishing path.

nf Block number of the last block of finishing path. Δu It is X finishing allowance as the following table (diameter value with sign

symbols ) and is the X coordinate offset of roughing contour compared to finishing

path, i.e. the different value of X absolute coordinates of A

it is the offset of the last X positive roughing path compared to finishing path. The system defaults Δu=0 when U（Δu）

is not input, i.e. there is no X finishing

allowance for roughing cycle.

Δw It is Z finishing allowance as the following table -99.999~99.999 (unit: mm ) and is

the Z coordinate offset of roughing contour compared to finishing path, i.e. the

different value of Z absolute coordinate of A

compared to A. Δw＞0，it is the offset

of the last roughing path compared to finishing path in Z positive direction. The system defaults Δw=0 when W（Δw）

is not input, i.e. there is no Z finishing

allowance for roughing cycle.

F Feedrate; S: Spindle speed; T: Tool number, tool offset number.

M, S, T, F

They can be specified in the first G73 or the second ones or program ns～nf. M, S,

T, F functions of M, S, T, F blocks are invalid in G73, and they are valid in G70 finishing blocks.

Address Incremental system

Metric（mm）input

compared to A. Δu＞0，

Inch (inch) input

Ⅰ Programming

U（Δi）

ISB system

ISC system

W（Δk）

ISB system

ISC system

R（d）

U (Δu）

W（Δw）

ISB, ISC

ISB system

ISC system

ISB system

ISC system

Execution process:(Fig. 2-40).

① A→A ② First roughing A

1→B1

：Rapid traverse；

1→B1→C1

：Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in ns

block in G1；

-99999.999～99999.999 mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

-99999.999～99999.999 mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

1～999（times） 1～999（times）

-99999.999～99999.999 mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

-99999.999～99999.999 mm -9999.9999～9999.9999 inch

-9999.9999～9999.9999 mm -999.99999～999.99999 inch

：

Page 94

GSK988T Turning CNC System User Manual

B1→C1：Cutting feed.

③ C ④ Second roughing A

2→B2

block in G1;

Ⅰ Programming

2→C2

⑤ C

…………

No. n times roughing，A

n→Bn

ns block in G1;

n→Cn

n→An+1

…………

Last roughing，A

d→Bd

block in G1;

d→Cd

→A：Rapid traverse to starting point;

：Rapid traverse；

1→A2

2→B2→C2

：

：Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in ns

：Cutting feed.

：rapid traverse；

2→A3

n→Bn→Cn

：

：ns Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in

：Cutting feed.

：Rapid traverse;

d→Bd→Cd

：

：Rapid traverse speed in ns block in G0, cutting feedrate specified by G73 in ns

：Cutting feed.

Fig. 2-47 G73 run path

Coordinate offset direction with finishing allowance:

Δi, Δk define the coordinates offset and its direction of roughing, Δu, Δw define the coordinates offset and cut-in direction in finishing; Δi, Δk, Δu, Δw can consist of many groups. Generally, the sign symbols of Δi and Δu are consistent, the sign symbols of Δk and Δw are consistent, there are four kinds of combination as Fig. 3-48,A for start-up tool point, B→C for workpiece contour, B’→C’for roughing contour and B’’→C’’ for finishing path.

Page 95

Chapter Ⅱ G Commands

B”

B’

C”

C’

B”

B’

A”

A’

A”

A’

C’

C”

C’

C”

A’

A”

B’

B”

A’

A”

Ⅰ Programming

B’

B”

C’

C”

Example：Fig. 2-49

Program：O0006；

G99 G00 X200 Z10 M03 S500; （Specify feedrate per rev and position starting point

Fig.2-48

Fig.2-49

and start spindle）

G73 U1.0 W1.0 R3 ; （X tool retraction with 2mm, Z 1mm）

Page 96

GSK988T Turning CNC System User Manual

G73 P14 Q19 U0.5 W0.3 F0.3 ; （X roughing with 0.5 allowance and Z 0.mm）

N14 G00 X80 W-40 ; G01 W-20 F0.15 S600 ; X120 W-10 ;

Ⅰ Programming

W-20 ; Blocks for finishing

G02 X160 W-20 R20 ;

N19 G01 X180 W-10 ; G70 P14 Q19 M30; （Finishing）

2.15.4 Finishing Cycle G70

Command function：The tool executes the finishing of workpiece from starting point along

with the finishing path defined by ns～nf blocks. After executing G71, G72 or G73

to roughing, execute G70 to finishing and single cutting of finishing allowance is completed. The tool returns to starting point and execute the next block following G70 block after G70 cycle is completed.

；

）

Command format：G70 P（ns

Command specifications:

1. ns：Block number of the first block of finishing path

nf: Block number of the last block of finishing path.

G70 path is defined by programmed one of ns～nf blocks. Relationships of relative position

of ns, nf block in G70～G73 blocks are as follows:

．．．．．．．．

Q（nf

）

G71/G72/G73 ……；

（ns）．．．．．．

．．．．．．．．

· F

· S Blocks for finishing path

（nf）……

．．．

G70 P（ns） Q（nf）；

2. G70 is compiled following ns～nf blocks. If they are in the front of G71 blocks, the system automatically searches and executes ns～nf blocks, and then executes the next program following nf block after they are executed, which causes the system executes ns～nf

blocks repetitively.

3. F, S, T in ns～nf blocks are valid when executing ns～nf to command G70 finishing cycle.

4. G96, G97, G98, G99, G40, G41, G42 are valid in G70;

5. When G70 is executed, the system can stop the automatic run and manual traverse, but

return to the position before manual traversing when G70 is executed again, otherwise, the following path will be wrong.

6. When the system is executing the single block, the program pauses after the system has

．．．．．．

Page 97

Chapter Ⅱ G Commands

executed end point of current path.

7. G70 cannot be executed in MDI mode, otherwise, the system alarms.

2.15.5 Axial Grooving Multiple Cycle G74

Command function: Axial (X) tool infeed cycle compounds radial discontinuous cutting cycle:

Tool infeeds from starting point in radial direction(Z), retracts, infeeds again, and again and again, and last tool retracts in axial direction, and retracts to the Z position in radial direction, which is called one radial cutting cycle; tool infeeds in axial direction and execute the next radial cutting cycle; cut to end point of cutting, and then return to starting point (starting point and end point are the same one in G74), which is called one radial grooving compound cycle. Directions of axial tool infeed and radial tool infeed are defined by relative position between

end point X（U）Z（W） and starting point of cutting. The command is

used to machine radial loop groove or column surface by radial discontinuously cutting, breaking stock and stock removal.

Command format：G74 R（e）

G74 X（U）

；

Z（W） P（Δi） Q（Δk） R（Δd） F ；

Ⅰ Programming

Command specifications：

（1）The cycle movement is executed by Z（W）and P（Δk）blocks of G74, and the movement

is not executed if only “G74 R（e）

；” block is executed;

（2）Δd and e are specified by the same address and whether there are Z（W）and P（Δk）

word or not in blocks to distinguish them;

（3）The tool can stop in Auto mode and traverse in Manual mode when G74 is executed, but

the tool must return to the position before executing in Manual mode when G74 is executed again, otherwise the following path will be wrong.

（4）When the single block is running, programs pauses after each axial cutting cycle is

completed.

（5）R（Δd）

must be omitted in blind hole cutting, and so there is no distance of tool retraction

when the tool cuts to axial end point

Relevant definitions：

Starting point of axial cutting cycle

Starting position of axial tool infeed for each axial cutting cycle, defining with

(n=1,2,3……), Z coordinate of An is the same that of starting point A, the different

value of X coordinate between A

and A

is Δi. The starting point A1 of the first

n-1

axial cutting cycle is the same as the starting point A, and the X coordinate of starting point (A

End point of axial tool infeed

Starting position of axial tool infeed for each axial cutting cycle, defining with Bn(n=1,2,3……), Z coordinate of Bn is the same that of cutting end point, X coordinate of B

) of the last axial cutting cycle is the same that of cutting end point.

is the same that of An , and the end point (Bf ) of the last axial tool infeed is the

same that of cutting end point.

End point of radius tool retraction

End position of radius tool infeed(travel of tool infeed is Δd) after each axial cutting cycle reaches the end point of axial tool infeed, defining with C coordinate of C

is the same that of cutting end point, and the different value of X

(n=1,2,3……), Z

Page 98

GSK988T Turning CNC System User Manual

coordinate between Cn and An is Δd；

End point of axial cutting cycle

Ⅰ Programming

Cutting end point

R（e）

X X absolute coordinate value of cutting end point Bf (unit: mm)

U Different value of X absolute coordinate between cutting end point Bf and starting

Z Z absolute coordinate value of cutting end point Bf (unit: mm).

W Different value of Z absolute coordinate between cutting end point Bf and starting

P（Δi）

Q（Δi）

R（Δd）

End position of axial tool retraction from the end point of radius tool retraction, defining with D

(n=1,2,3……), Z coordinate of Dn is the same that of starting point, X

coordinate of Dn is the same that of Cn (the different value of X coordinate between it

and A

It is defined by X（U）

is Δd)；

Z（W） ,and is the end point Bf of last axial tool infeed.

It is the travel of tool retraction after each axial(Z) tool infeed without sign symbols as the following table. The command value is reserved after executing R（e）and the

value of NO.5139 is rewritten. The value of NO.5139 is regarded as the travel of tool retraction when R（e）is not input.

point.

Travel of radial(X) cutting for each axial cutting cycle without sign symbols, and the value range is referred to the following table.

Travel of Z discontinuous tool infeed without sign symbols in axial(Z) cutting, and the value range is referred to the following table.

Travel (radius value)of radial (X) tool retraction after cutting to end point of axial cutting. The value range is referred to the following table. The radial (X) tool retraction is 0 when R（Δd）

is omitted and the system defaults the axial cutting end point. The

radial (X) tool retraction is 0 when P（Δi）

Address Incremental system

P（Δi） Q（Δk

）

R（e） R（Δd

）

ISB system

ISC system

ISB system

ISC system

0~99999999（unit:0.001mm） 0~99999999（unit:0.0001inch）

0~99999999（unit:0.0001mm） 0~99999999（unit:0.00001inch）

0～99999.999mm 0～9999.9999 inch

0～9999.9999 mm 0～999.99999 inch

Command execution process: as Fig. 2-50.

① The system executes the axial (Z) cutting feed △k from the starting point A

axial cutting cycle; when Z coordinate of cutting end point is less than that of starting point, the system executes Z negative feed, otherwise, positive feed;

② The system executes the axial(Z) rapid tool retraction e and its direction is

opposite to the feed direction of ①;

③ The system executes Z cutting feed(Δk+e) again, the end point of cutting feed is

still in it between starting point A tool infeed; the system executes Z cutting feed (Δk+e)again and then executes ②; after it executes Z cutting feed (Δk+e)again, the end point of cutting feed is on

or is not between An and Bn , the system executes Z cutting feed to Bn and

then executes ○4；

metric（mm） input

of axial cutting cycle and end point Bn of axial

is omitted.

Inch (inch) input

④ Radial(X) rapid tool retraction △d（radius value）to C

; when X coordinate of Bf

Page 99

(cutting end point) is less than that of A (starting point), the system executes X positive tool retraction, otherwise, X negative tool retraction;

⑤ Axial(Z axial) rapid retract tool to Dn, No. n axial cutting cycle is completed. If the

current axial cutting cycle is not the last one, execute ⑥ ; if it is the previous one before the last axial cutting cycle, execute ⑦;

⑥ Radial(X axial)rapid tool infeed, and its direction is opposite to that of ④tool

retraction. When the end point of tool infeed is still on it between A and A (starting point of last axial cutting cycle) after the system executes X tool infeed (△d+△i) (radius value) , i.e. Dn→A next axial cutting cycle); after the system executes the tool infeed ( d+ i), the △△ end point reaches A executes ① to start the first axial cutting cycle;

⑦ X rapidly traverse to return to A, and G74 is completed.

Chapter Ⅱ G Commands

and then the system executes ① (start the

n+1

or is not between Dn and Af, X rapidly traverse to Af and

Ⅰ Programming

Example: Fig.2-51

Fig. 2-50 G74 path

Page 100

GSK988T Turning CNC System User Manual

Ⅰ Programming

Fig. 2-51

Program：

O0007； G0 X40 Z5 M3 S500；（Start spindle and position to starting point of machining） G74 R0.5 ；（Machining cycle） G74 X20 Z-20 P3000 Q5000 F50； (Z tool infeed 5mm and tool retraction 0.5mm each time;

rapid return to starting point(Z5) after cutting feed to end point(Z-20), X tool infeed 3mm and cycle the above-mentioned steps)

M30；（End of program）

2.15.6 Radial Grooving Multiple Cycle G75

Command function: Axial (Z) tool infeed cycle compounds radial discontinuous cutting

cycle: Tool infeeds from starting point in radial direction, retracts, infeeds again, and again and again, and last tool retracts in axial direction, and retracts to position in radial direction, which is called one radial cutting cycle; tool infeeds in axial direction and execute the next radial cutting cycle; cut to end point of cutting, and then return to starting point (starting point and end point are the same one in G75), which is called one radial grooving compound cycle. Directions of axial tool infeed and radial tool infeed are defined by relative position

between end point X（U）Z（W） and starting point of cutting. G75 is

used to machine the radial loop groove or column surface by radial discontinuously cutting, breaking stock and stock removal.

；

）

Command format：G75 R（e

G75 X（U）

Command explanations:

1. The cycle movement is executed by X（W）and P（Δi）

when there is no X(U) in G75 block. When only “G75 R（e）

No.5139 value is modified, the cycle operation cannot be executed;

2. Δd and e are specified by the same address R and whether there are X（U）and P（Δi）

words or not in blocks can distinguish them;

Z（W） P（Δi） Q（Δk） R（Δd） F ；

blocks of G75, G75 is not executed

；” block is executed and only

gsk GSK988T User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual