gsk GSK928TE II User Manual

GSK928TEⅡ Turning CNC System User Manual

The user manual describes all items concerning the operation of

the system in detail as much as possible. However, it is

impractical to give particular descriptions of all unnecessary

and/or unavailable works of the system due to the length limit of

the manual, specific operations of the product and other causes.

Therefore, the operations not specified herein may be

considered impractical or unavailable.

This user manual is the property of GSK CNC Equipment Co., Ltd.

All rights reserved. It is against the law for any organization or

individual to publish or reprint this manual without the express written

permission of GSK and the latter reserves the right to ascertain their

legal liability.

1

Dear user,

GSK928TEⅡ Turning CNC System User Manual

We are really grateful for your patronage and purchase of GSK928

TEⅡ

Turning CNC

system made by GSK CNC Equipment Co., Ltd.

Caution

This system can only be operated by authorized and qualified personnel as

improper operations may cause accidents. Please carefully read this user

manual before use!

Before Use:

z Connect the emergency stop button of the system firmly and correctly, otherwise an

emergency stop alarm will occur when switch on the system, so that the system cannot

work properly.

z Set the reference point of the program of the system according to the actual mounting

position of the tool of the machine that the system controls.

Note: The power supply of the sy stem inst alled in the cabinet is exclusiv e to GSK’

CNC systems.

Must not take the power supply as other uses, otherwise, there maybe

cause great accidence!

Chinese version of all technical documents in Chinese and English

languages is regarded as final.

All specifications and designs are subject to change wi thout notice.

All rights reserved.

We are full of heartfelt gratitude to you for supporting us in the use of GSK’s
products.

2

GSK928TEⅡ Turning CNC System User Manual

Contents

Suggestions for Safety ....................................................................................................................... 1

Operation..............................................................................................................................................7

Chapter One Overview ................................................................................................................. 7

Chapter Two Technical Specifications........................................................................................ 8

Chapter Three Operator Panel..................................................................................................... 9

Chapter Four System Operation ............................................................................................... 14

4.1 System ON/OFF.................................................................................................................. 14

4.2 CNC System Operating Mode............................................................................................. 15

4.3 EDIT Mode........................................................................................................................... 15

4.4 Manual Mode....................................................................................................................... 28

4.5 AUTO Mode......................................................................................................................... 47

4.6 Parameter Setting................................................................................................................ 58

4.7 Tool Offset Setting Mode ..................................................................................................... 69

4.8 Diagnosis ............................................................................................................................. 70

4.9 Alarm of Emergency Stop and Overtravel........................................................................... 74

4.10 Drive Unit Switch Control .................................................................................................. 75

Programming ..................................................................................................................................... 76

Chapter 1 Programming Fundamentals ................................................................................... 76

1.1 Coordinate Axis and its Direction ........................................................................................ 76

1.2 Machine Zero....................................................................................................................... 76

1.3 Programming Coordinate .................................................................................................... 76

1.4 Workpiece Coordinate System............................................................................................ 78

1.5 Reference Point................................................................................................................... 78

Chapter 2 Program Structure..................................................................................................... 79

2.1 Character ............................................................................................................................. 79

2.2 Word .................................................................................................................................... 79

2.3 Block Number ...................................................................................................................... 80

2.4 Block .................................................................................................................................... 80

2.5 Program Structure ............................................................................................................... 80

Chapter 3 Commands and their Functions.............................................................................. 81

3.1 G commands — Preparatory Function .......................................................................... 81

3.2 M function — Miscellaneous Function.............................................................................113

3.3 S function — Spindle Function ........................................................................................118

3.4 T Function — Tool Function ..........................................................................................119

3.5 F function — Feedrate Function .................................................................................. 120

Chapter Four Programming Rules .......................................................................................... 121

I

Contents

4.1 Some Commands in One Block ........................................................................................ 121

4.2 Modal and Initial State of Commands ............................................................................... 121

4.3 Other Rules ....................................................................................................................... 122

4.4 Programming Example ...................................................................................................... 122

4.5 Alarm List........................................................................................................................... 129

Appendix 1 GSKRS232 Communication Use......................................................................... 132

Appendix 2 C5.1 FLASH Chip Copy and Check.................................................................. 141

Connection....................................................................................................................................... 143

Chapter One Interface .............................................................................................................. 143

1.1 Interface Layout................................................................................................................. 143

1.2 Total Frame........................................................................................................................ 144

1.3 Total Connection Layout .................................................................................................... 145

Chapter Two Interface Function .............................................................................................. 146

2.1 Specifications..................................................................................................................... 146

2.2 Interface Graph.................................................................................................................. 147

Chapter Three CNC Device Connection................................................................................. 148

3.1 X1 Communication Interface ............................................................................................. 148

3.3 X3 Spindle Encoder Interface............................................................................................ 150

3.4 X4 Tool Post Device Interface ........................................................................................... 152

3.5 X5 Feed Drive Unit Interface............................................................................................. 154

3.5.3.3 Pulse signal.......................................................................................................................155

3.6 X Switching Value Input Interface ..................................................................................... 163

3.7 X7 Switching Value Output................................................................................................ 165

3.8 X7 Spindle Converter Interface ......................................................................................... 167

Appendix 1 GSK928TEⅡ Tool post Controller Circuit Diagram ......................................... 170

Appendix 2 Interface Circuit Diagram..................................................................................... 171

Appendix 3 Machine Zero Return Mode ................................................................................. 174

Appendix 5 GSK928TEⅡ Integrated Wiring Table................................................................ 177

Appendix 6 Appeara nce Installation Dimension of GSK928TEⅡ Tur ning CNC System.. 181

II

GSK928TEⅡ Turning CNC System User Manual

Suggestions for Safety

The user must carefully read the suggestions for the system before installing and operating the

system.

The user must follow the suggestions of the system to ensure that the person is not hurt and the

equipments are not damaged.

The user must follow the related suggestions for safety described in the manual, and must not

operate it until the manual is read completely.

Follow safety instructions for the machine that the system will control. Do not run the machine

until you have completely read both the instructions and this manual.

User must follow the suggestions of safety described in the user manual from the machine

manufacture

User can operate the machine or compile the program to control the machine after completely

reading the User Manual and the one from the machine manufacturer.

The power supply of the system installed in the cabinet is exclusive to GSK’ CNC systems. Must

not take the power supply as other uses, otherwise, there maybe cause great accidence!

1

Safety Warning

Ⅰ.Graphic symbol

Caution Operation against the instructions may cause the operator serious injuries.

Alarm Wrong operation may injure the operator and damage the system.

Warning Improper operation may result in damage to the machine, as well its products.

Important information

Shield

Earthing (PE)

Encoder

Coil of contact or relay

Exchange

Connecting terminal

2

GSK928TEⅡ Turning CNC System User Manual

Ⅱ. Notes

1）Check before acceptance

Warning ● The damaged or defect product must not be used.

2）Delivery and storage

Warning ●Moistureproof measures are needed while the system is delivered and stored.

Never climb the packing box, neither stand on it, nor place heavy items on it. Do

not put over five packing boxes in piles. Take particular care of the front panel

and the display of the system.

3）Installation

Warning ●Protect the system from sunlight and raindrops. The shell of the system is not

waterproof.

Warning ●Prevent dust, corrosive air, liquid, conductors and inflammable substances from

entering the system.

●Keep the system away from inflammable and explosive substances. Avoid

places where there is powerful electromagnetic interference.

●Install the system firmly without vibration.

4）Wiring

Caution ●Only qualified persons can connect the system or check the connection. The

connecting wires cannot be damaged. Do not press or open the cover of the

system with power on.

Caution ●The voltage and the polarity of connecting plugs must accord with the manual.

●Wet hands are dangerous to grasp the plug or the switch.

Warning ●The connection must be proper and firm.

●The system must be earthed.

5）Debugging

Warning ●Make sure that the parameters of the system is correct before the system runs.

●No parameter is beyond the setting limit in the manual.

3

Safety Warning

6）Operation

Caution ●Only qualified operators can operate the system.

●Ensure the switch is OFF before connecting the power supply.

Warning ●The operator can not leave the system to work alone.

●Do not switch on the system until making sure the connection is correct.

●The emergency stop button is able to disconnect all power supplies when the

system breaks down. Do not switch on/off the system frequently

Warning ●Prevent the system from the environmental interference.

7）Troubleshooting

Caution ●Unqualified persons cannot repair the system.

Warning ●After alarms, do not restart the system until the breakdown is fixed.

4

GSK928TEⅡ Turning CNC System User Manual

Ⅲ. Safety Suggestions for Programming

1）Setting a coordinate system

Incorrect coordinate system may cause the machine not to work as expected even if the

program is correct, which may injure the operator, and damage the machine as well as its

tool and workpiece.

2) Rapid traverse (positioning)

When G00 rapid traverse performs the positioning( nonlinear motion to position between

its starting point and end point), make sure that the path for the tool is safe before

programming. The positioning is to perform the rapid traverse, and when the tool and the

workpiece are interfered, the tool, the machine and the workpiece may be damaged, and

even the operator injured.

3) Applicability of user manual

The manual introduces in detail all functions of the system, including optional functions

and max. controllable ranges, which are subject to change with the machine. If there is

any doubt, please read the instruction for the machine。

4) Functions of CNC system and machine

CNC machines depend on CNC systems, but also power voltage cabinets, servo systems,

CNC and the operator panels. It is hard to explain all the integrated functions,

programming and operation. Do not use integrated instructions not included in the manual

until they have been tested successfully.

5

Safety Warning

Ⅳ. Notes and Safety Suggestions for Operating Machine

1）Test the machine without workpieces or tools. Make sure that the machine runs well before

it starts to work.

2）Check the input data of the system carefully before operating the machine. Incorrect input

data may cause the machine to work improperly, so as to damage the workpiece and the

tool, as well injure the operator.

3）Make sure that the input feedrate of the system is suitable for the expected operation.

Feedrate has a maximum for each machine, and the amount of the feed rate is subject to

change with operation. Choose the maximum according to the instructions of the machine.

Improper feedrate leads the machine to work wrongly, so as to damage the workpiece and

the tool, as well injure the operator.

4 ） When tool compensation is needed, check the direction and the amount of the

compensation. Improper compensation causes the machine to work wrongly, so as to

damage the workpiece and the tool, as well injure the operator.

5）If the machine is to run in Manual mode, check the current position of the tool and the

workpiece, and correctly specify the moving axis, moving direction and the feedrate.

MPG(Handwheel) control with great override, such as 100, may damage the machine and

its tool, even injure the operator.

6）If the tool is return to the reference point, make sure that the machine has been equipped

with the device to detect the reference point, otherwise, the tool can not reach the

reference point, which may damage the machine and its tool, and even injure the operator.

6

GSK928TEⅡ Turning CNC System User Manual

Operation

Chapter One Overview

With 480×240 lattice TFT color graphic LCD, GSK 928TEⅡ CNC system takes as key control the

high-speed CPU and the complex programmable logic device of super-large-scale integrated

circuits. ISO CNC code is used to write part programs. The system is characterized by μ-level

precision control, a full screen editing, Chinese operation interface, real time demonstration of the

machining process, and high cost-performance ratio. By means of programming, the system can be

used to control stepper motors, so as to machine outer cylinders, end faces, grooves, tapers,

circular arcs, and threads.

7

Operation Chapter Two System Operator Panel

Chapter Two Technical Specifications

2.1 Controlled axes 2 (X, Z axis)

2.2

Link axes 2 (X, Z axis)

2.3

Min. setting unit 0.001 mm

2.4

Min. motion unit X: 0.0005mm; Z: 0.001mm

2.5

Max. dimension for programs ±8000.000 mm

Max. traverse rate 15000 mm/min

2.6

Feedrate 5-6000 mm/min (G98/G99)

2.7

Capacity of part program 62KB

2.8

2.9

Max. number of part programs 100

2.1

Graphic LCD 480×240 lattice TFT color LCD

Communication interface Standard RS-232

2.11

2.12

Tool selection 4（up to 8）

Compensation Tool compensation, clearance compensation

2.13

2.14

MPG(MPG) ×0.001 ×0.01 ×0.1

S1, S2, S3, S4 direct output; S0～S15 output

Spindle

2.15

2.16

G codes

2.17

Thread functions

with BCD code; three automatic gear shifting with

0～10V analog output; 1024p/r, 1200p/r spindle

encoder available

24 codes，including the fixed /compound cycles, Z

threading

Metric/inch single and multiple straight, taper

thread, high-speed retraction with setting the

retraction distance

8

928TE-II

GSK928TEⅡ Turning CNC System User Manual

Chapter Three Operator Panel

EDIT

JOG

AUTO

PARAM ETER

OFFSET

DI AG NOS IS

Introduction of GSK 928TEⅡ Turning CNC System operator panel as follows:

3.1 LCD display: CNC man-machine dialogue interface. Resolution 480×240 lattice TFT color

LCD display.

3.2 Digit key: input all kind: Input all kinds of data（0-9）.

3.3 Address keys：Input English letters in word addresses of part programs.

3.4 Function key s ：All function keys are based on Numerical Contr ol of Machine-Symbol.

INCREASI NG RAPID OVER RIDE TRA VERSE OVERRIDE: Increase rapid traverse

override in JOG mode and G00 rapid traverse override in AUTO mode.

REDUCING RAPID TRAVERSE OVERRIDE: Reduce rapid traverse override in JOG

mode and G00 rapid traverse override in AUTO mode.

INCREA SING FEEDRATE OVERRIDE: Increase feedrate override in JOG mode

and G01 feedrate override in AUTO mode.

9

Operation Chapter Two System Operator Panel

REDUCING FEEDATE OVERRIDE: Reduce feedrate override in JOG mode and G01

feedrate override in AUTO mode.

X PROGRAM REFERENCE POINT(PROGRAM ZERO) RETURN : It is valid in

JOG/AUTO mode.

Z PROGRAM REFERENCE POINT (PROGRAM ZERO) RETURN : It is valid in

JOG/AUTO mode.

X MACHINE ZE RO RETU RN : It is valid in JOG/AUTO mode.（whether machine zero is

valid is defined by Bit7 of P12 ）.

Z MACHINE ZERO RETURN: It is valid in JOG/AUTO mode.（whether machine zero is

valid is defined by Bit7 of P12 ）.

DRY RUN: In AUTO mode, DRY RUN tests a program without G, S, M, and T functions

output. In EDIT mode, moves the cursor directly to the first character behind the block

number. The machine coordinate data become white from yellow besides LED ON after it

is pressed.

SINGLE BLOCK : A single block runs in AUTO mode.

EDIT mode

JOG mode

AUTO mode

PARAMET E R mode

10

OFFSET mode

DIAGNOSIS mode

3.5 Edit/state key

Switch the input method in EDIT mode—- INSERT/REWRITE .

Delete a number, a letter, a block or a whole program.

Cancel the current input all kind of data or escape from the current operation state.

GSK928TEⅡ Turning CNC System User Manual

Input all kind of data or select the required or run program or create a new part program.

Press ENTER to confirmation.

PAGE UP: page up to search programs or parameters in EDIT/PARAMETER/OFFSET

operation mode.

PAGE DOWN: page down to search programs or parameters in EDIT/ PARAMETER/

OFFSET mode.

Cursor moving up：the cursor moves up one line in EDIT/PARAMETER/OFFSET mode.

Cursor moving down: the cursor moves down one line in EDIT/PARAMETER/OFFSET

mode.

Cursor moving left: the cursor moves one character position left in EDIT mode.

Cursor moving right: the cursor moves one character position right in EDIT mode.

3.6 Cycle start and feed hold button

11

Operation Chapter Two System Operator Panel

Start and pause programs in AUTO mode.

CYCLE START: Start to run programs in AUTO mode.

FEED HOLD: Motor reduces to pause in JOG or AUTO mode.

3.7 Manual axis control key

The selected axis and its direction in JOG mode:

X axis moves negatively in JOG mode.

X axis moves positively in JOG mode.

Z axis moves negatively in JOG mode.

Z axis moves positively in JOG mode.

RAPID TRAVERSE/FEED Switching rapid traverse and feed.

MANUAL STEP Selecting each step width or MPG feed in STEP/ MPG(Handwheel)

mode.

X MPG(Handwheel) X motion is controlled by the MPG(Handwheel) (when the control

is valid, other control keys related to the axis moving are invalid) .

Z MPG Z motion is controlled by the MPG(Handwheel) (when the control is valid, other

control keys related to the axis moving are invalid).

STEP/JOG mode Switch STEP/JOG mode.

3.8 Manual tool change and auxiliary function keys

Select directly the next tool number and control the machine to complete auxiliary functions as

follows：

12

GSK928TEⅡ Turning CNC System User Manual

Spindle rotation (CCW) Spindle rotates counterclockwise.

Spindle stop Spindle stops.

Spindle rotation (CW) Spindle rotates clockwise.

Cooling control Cooling ON/OFF

Spindle gear shifting Select the speed of each gear when the machine is equipped

with multi-gear (up to 16 gears) spindle motor and control

loops.

Tool change Select the next tool number neighboring to the current one.

Note

：

The above-mentioned pressing keys are valid in JOG, AUTO and DIAGNOSIS mode when X,

Z does not move, but only cooling control is valid

.

3.9 Reset key

System reset When the system resets, all axes stop motion, all auxiliary function

outputs are invalid, and the machine stops and returns to the initialization.

3.10 State indicator

It indicates the current state of CNC system. There are 15 function keys with LED indicator.

When LED ON, its function of corresponding key is valid, otherwise it is invalid.

13

GSK928TEⅡ Turning CNC System User Manual

Chapter Four System Operation

This chapter introduces operations of GSK928TEⅡ Turning CNC system. Please read carefully

before operation.

4.1 System ON/OFF

GSK928TE Turning CNC System is not equipped with the system power switch. User installs it Ⅱ

according to the different machine to avoid bad effects to CNC system owing to the impaction of

power supply.

CNC system is turned on as follows:

1. The master power switch of machine is turned on.

2. Connect with the power switch of the CNC system. Press
GSK mark and caption, at the time, the system displays the software and hardware version
number, delivery date by pressing other keys persistently except for the reset key.

CNC system is turned off as follows：

1. The power switch of the CNC is turned off.

2. the power switch of the machine is turned off.

Note : The system should be initialized when it is turned on firstly.

The initialization operations are as follows:

Press the reset key and “9” key, and then release firstly the reset key and then “9” to enter the
debugging window.

1. CNC PAR P01—P26 DY3

2. CNC PAR P01—P26 DA98

3. CLEAR PRO %00—%99

4. DEBUG

5. COPY FLASH 29C010

0. ESC PLEASE INPUT

Pressing 1: initialize the system parameters for stepper motor
Pressing 2: initialize the system parameters for servo motor
Pressing 3: delete all part programs
Pressing 4: enter the system development system
Pressing 5: FLASH copy and check
Pressing 9: escape from the system EDIT menu

and the system displays

Note 1: Measure the machine backlash of X, Z，and input their values to the machine parameters

P07 and P08. For input methods, see Section Operation, Parameter mode.

Note 2: Set P11 according to the electric circuit design and the motor’s direction of the machine.

Note 3: Adjust parameters P05, P06, P17～P22 according to the load of machine, which make it

14

GSK928TEⅡ Turning CNC System User Manual

run efficiently and stably.

Fig. 1 System initialization display

4.2 CNC System Operating Mode

GSK928TEII CNC System uses operating mode keys to select directly the operating mode,

which is helpful to directly change operating modes, easy, convenient and direct operations.

After GSK928TE CNC System is switched on, the dynamic display window iⅡ s as Fig. 1. The

window is displayed circularly until any key is pressed except for

the operating mode which is that of last power off.

, the system will enter

4.3 EDIT Mode

In EDIT mode, the user manually inputs or modifies the content of part program by operation

panel. In EDIT mode, create, select and delete part programs by keyboard, and insert, modify

and delete the content of selected part program. Besides, transmit part programs of the system

to the external PC or the edited part programs of external PC to CNC system by the serial

connection between RS232 communication interfaces and general-purpose PC.

After pressing

to enter EDIT mode, the system displays program names of all part

programs stored in the current program, the byte amount contained in current program and the

available memory bytes of system. See Fig. 2:

15

Edit keys in EDIT mode

GSK928TEⅡ Turning CNC System User Manual

Fig. 2 EDIT operating mode

(1)

cursor UP key

The cursor moves to the first character behind the block number of the upper block when the

key is pressed once.

The key being pressed down, the cursor sequentially moves up till the first block of block or

the key is released.

(2)

cursor DOWN key

The cursor moves to the first character behind the block number of the next down block

when the key is pressed once.

The key being pressed down, the cursor sequentially moves down till the last block number

of block or the key is released.

(3)

cursor LEFT key

The cursor moves left one character when the key is pressed once.

The key being pressed down, the cursor sequentially moves left till the first character of

block or the key is released.

(4)

cursor RIGHT key

The cursor moves right one character when the key is pressed.

The key being pressed down, the cursor sequentially moves right till the last character of block

or the key is released.

：

Note

Cursor — prompt identifier to indicate the current editable character position. There are

two states of CNC system.

A. The cursor is displayed to a horizontal line under a character in Insert mode.

B. The cursor is displayed to the pointed character in inverse and highlight. The two

cursors can be switched by

16

.

GSK928TEⅡ Turning CNC System User Manual

（5） DRY Run key

The cursor moves to the head of block or the head of first word of this block by pressing

continuously.

（6）

STEP/JOG mode

The cursor moves to the behind of the last character of this block.

（7）

REWRITE key

Switch INSERT/REWRITE mode once when the key is pressed once, and the cursor will
change correspondingly. The cursor in Insert mode is a flashing horizontal line, but that in
Rewrite is a character in flashing highlight.

（8）

When the key is pressed once, the program number with 2-digit is input to create a

new program, select or delete the existing program and all programs.

（9） PAGE UP Search the program number and display the content of previous page.

(10) PAGE DOWN Search the program number and display the content of next page.

(11)

Double functions key. Each key has

two definitions. Pressing it once is the first definition value，namely, U W I K D R. The same

key is pressed again, the system will automatically rewrite the previous input value into the
second definition value, namely / E P N L

. If the same key is pressed continuously, the

input value will be switched between the first definition value and the second one. ‘/’ is the
skip block character，‘

’is the space character.

4.3.1 Searching Directory of Part Program

In EDIT mode, the system displays the program name list of all part programs, all part program
amount and the leftover bytes in the part program memory area of CNC system. In EDIT mode,
the system displays the program name list of all part programs, all part program amount and the
leftover bytes in the part program memory area of CNC system.

Press in EDIT mode or press or when editing programs as Fig. 3:

17

GSK928TEⅡ Turning CNC System User Manual

Fig. 3 Searching a part program catalog / creating, selecting and deleting part programs

Most %00～%99 program names are displayed in each screen. When part programs in memory

area are over 100, they are displayed by paging. Press

list of next page and press

to display again the program number list of first page till the

to display the program number

last page.

4.3.2 Creating, Selecting, Deleting, Renaming and Copying a Part Program

The above-mentioned operations can be executed in the state of catalog search of part program or

in the course of editing program content.

The system displays as Fig. 4 when

program.

4.3.2.1 Creating a New Part Program

(1) Press

in the state of catalog search of part program.

(2) Input a new program number which does not exist in the program catalog list with 2-digit by

keyboard. See Fig. 4.

is pressed in the state of catalogue search of part

(3) Press

.

(4) After part programs are created, the system will automatically enter EDIT mode.

Example: Creating %20 program: Press to input and press

. So the program has been created to enter EDIT mode of %20 program. See

Fig. 5:

18

GSK928TEⅡ Turning CNC System User Manual

Fig. 4 Inputting a program number

Fig. 5 Creating a new part program

4.3.2.2 Deleting a Part Program

(1) Press

in the state of catalog search of part program.

(2) Input the required deleted program number by keyboard.

(3) Press

and the system will display Confirm ？.

(4) Press to delete the part program which program number has been input; press any

keys to cancel the deletion.

Example: Deleting %03 program: press and then orderly , ,

and

, so the program is deleted as Fig. 6:

19

GSK928TEⅡ Turning CNC System User Manual

4.3.2.3 Selecting a Part Program

Fig. 6 Deleting a part program

(1) Press

in the state of catalog search of part program.

(2) Input the required selected program number by keyboard.

(3) Press

.

(4) The part program is selected completely and the system displays its content to enter EDIT

mode.

Example: Selecting %01 part program.

Press

See Fig. 7:

to input and then press , so the selection is completed.

：

Note 1

After the first power on, the system enters EDIT mode or there is no content in the

Fig. 7 Selecting a part program

memory area of part program, it will automatically create and select %00 program. The

system will consider %00 as the current program after it be initialized.

Note 2: After the system has selected one program, the required one is changed only by

selecting it. Even if the system powers off, the selected program number cannot be

changed once it is selected.

20

GSK928TEⅡ Turning CNC System User Manual

4.3.2.4 Outputting a Part Program

Output part programs from CNC system internal memory to the external computer.

1. Connect the communication cable between CNC system and the computer when power off.

1. After CNC powers on, select EDIT mode.

2. Select the required part program according to Section Operation, 4.3.2.3 Select a part

program (do not select it if the current program is to be sent).

3. Press

, and the system prompts Ready To Send ！.

4. Keep the computer in the state of waiting for the receiving（See appendix: GSKR 232
communication program specification）.

5. After the computer is ready, if

is pressed, the system will prompt Sending … , and

so the system sends the selected program to the computer.

6. After the sending has completed, the system prompts Finished ！ , and any keys are

pressed to return to EDIT mode.

7. Press

to pause the sending.

4.3.2.5 Inputting a Part Program

Input the stored part program from the external PC to CNC system.

(1) Connect the communication cable between CNC system and the computer when power off.

（2）After CNC system powers on, select EDIT mode.

（3）Press

and the system prompts Ready To receive！.

(4) Keep the computer in the state of output. (See Appendix GSKTR communication

program specification ).

(5) After the system is ready, if

is pressed, the system will prompt Receiving … ,

and so the system sends the selected program to the CNC system.

(6) After the receiving is completed ,the system prompts Finished ！ and returns to EDIT

mode if any keys are pressed. The system displays the input program name in the catalog

list of part program.

(7) Press

to interrupt the receiving.

Note 1: In the course of inputting part program, CNC system considers the character string “%

XX” contained in the first block of the sent program from the computer as the program

21

GSK928TEⅡ Turning CNC System User Manual

name to save. If the sent program name is the same as one in CNC system, the system

cannot display the program name content of the sent program name, and will display it if

the old one is deleted.

Note 2: Send/receive part programs between 2 GSK928TE

Ⅱ

CNC systems according to the

above–mentioned methods. 2 CNC systems separately operate according to part

program input/output ways.

Note 3: It must have the block number of part program when the part program is sent from PC to

CNC system, otherwise there is a mistake.

4.3.2.6 Deleting All Part Programs

Delete all programs once in the program memory area of CNC system.

Press

Input ⑵

Press⑶

in the state of catalog search of part program.

, by keyboard.

，and the system prompts Confirm ？

Press⑷ to delete all part programs. Press other keys, and the system does not execute

the deletion and returns to EDIT mode.

Note: Press and then , release and then to delete all part program.

4.3.2.7 Renaming a Part Program

Rewrite the current program name to another one.

Press ⑴

, and the system displays % .

Input the program name which does not exist in the program name list, and press ⑵

to rewrite the current program name to the input program name.

Example: Rename the current program name %00 to % 05.

Press

to input , and press , so the renaming is

completed.

22

GSK928TEⅡ Turning CNC System User Manual

4.3.2.8 Copying a Part Program

Copy the content of current program to another new one and consider it as the current one.

Press⑴

, and the system displays % .

In⑵ put a program name which does not exist in the program name list, and press to

copy all contents of current program to the program whose number is input.

The new program name becomes the current one.

Example: Copy program of current program name % 00 to that of %05.

Press

to input , and press , so the copy is completed.

Note: If the input program name exists, the system will prompt File Existed . At the moment,

press any keys to input again the program name which does not exist in the program area,

and then press

, So the copy is completed.

4.3.3 Inputting/Editing Content of Part Program

CNC machining is defined that the system automatically completes the machining of workpiece

according to the part program sequence input by user. Each program is composed of many

blocks and each block consists of a block number, codes and data. Start the machine and gain

the standard workpiece after inputting the part program content according to the technology flow.

EDIT mode of CNC system uses the full-screen and part programs are employed with the file
management mode.

4.3.3.1 Automatically Creating a Block Number

Each part program contains many blocks and each block begins with the block number“ N**** ”;

After a new program is created, the system will automatically generate the first block

number“ N0000 ”; After one block is input and

is pressed, the system will generate the

next block number. In the course of input, the increment of block number is defined by P23.
When a block is inserted, the system will automatically consider the 1/4 integer value of P23 as
the increment to generate the block number. When M98, M97, M91, M92, M93, M94 and others
codes related with the block number are executed, there are no repetitive block numbers in the
program, otherwise the system will alarm. If the above codes are not executed, the block number
can be repeated.

See Fig. 8 for a program generation and inserting a block number in a block (P23 value is 10).

23

GSK928TEⅡ Turning CNC System User Manual

Fig. 8 automatically creating block number and inputting program content

4.3.3.2 Inputting Content of Program

EDIT mode of the CNC system is employed with the full screen. Inputting content of program is

executed in EDIT mode.

(1) Create a new program according to the creating method of new part program.

(2) After the block number N0000 is displayed, input the content of one block by keyboard.

(3) Input completely one block and then press .
(4) The system will generate the sequence number of next block and the content of program

should be input continuously.

(5) Input completely the last block and press

to end the input of content of program.

(6) The cursor rapidly moves in the block.

Press

once, and the cursor will point to the head of word; press it again，and the

cursor points to the head of block, and the above steps are executed circularly.

Press

once, the cursor points to the end of block.

(7) Insert a block in the first block.

Move the cursor to the head of the first block and then press .

Note: There are 255 characters at most in one block. When the characters exceed the screen,

pressing

displays one character left.

4.3.3.3 Inserting a Block

Insert one or more blocks between two blocks.

24

GSK928TEⅡ Turning CNC System User Manual

(1) Press to move the cursor to the first one of two blocks.

(2) Press

to move the cursor to the behind of last character, or press to move

directly the cursor to the behind of last character.

(3) Press , and the system will generate a new block number between two blocks (the

increment of sequence number is 1/4 integral value of P23, and if there is not enough, the
block number of the next block is rewritten.) and blank one block.

(4) Input the content of required block.

(5) After the content is input,

is pressed to insert blocks. When only one block is inserted,

the operation is not executed.

(6) The inserting is completed.

(7) If the block is inserted before the first block,

is pressed to move the cursor to the

under “N” of the first block, and the system will generate a new block number before the first

block after is pressed.

Note

：

After one block is inserted behind the last block and is pressed, the system will

automatically generate the next block number.

Example：Insert a new block M3 between N0020 and N0030 in Fig. 8 as follows:

(1) Press to move the cursor to N0020 , and press to move the

cursor to the behind of Z0.0.

(2) Press

， and the system will automatically generate one block number and blank a

block to display N0022 as Fig. 9. The cursor points to the first input character of the new

block.

(3) Input

.

(4) The inserting is completed as Fig. 10.

25

GSK928TEⅡ Turning CNC System User Manual

Fig 9. Generating a new block number after

Fig. 10 Input and end the insertion

4.3.3.4 Deleting a Block

Delete all content in one block (including block number).

(1) Press

to move the cursor to the required block.

is pressed

(2) Press

to move the cursor to the under of the address N of required block.

(3) Press .
(4) Delete all content of the selected blocks.

4.3.3.5 Inserting a Word in a Block

(1) Ensure the current input operation is in Insert mode, i.e. the cursor displays to the under of

block. If

(2) Press

26

is not pressed, switch Input to Insert mode.

or to move the cursor to the address character behind the required

GSK928TEⅡ Turning CNC System User Manual

inserting position.

(3) Input the inserting content.

(4) Insert the content before the address character pointed by the cursor.

Example：Insert 1 between X and 0 of N0020 G0 X0.0 Z0.0. Move the cursor to

the under of O behind of X ，and input 1 . N0020 G0 X10.0 Z0.0 is displayed.

：

Note

The system requires there is a space between each word (a letter adding the following

digits) in block. The system can automatically judge and generate a space in the course

of inputting when the program is edit, but cannot automatically judge in the course of

inserting, and so the user will input the space to ensure the complete program.

4.3.3.6 Deleting a Word in a Block

Delete the invalid content.

(1) Press to move the cursor to the required address character.

(2) Press

to delete the address character.

4.3.3.7 Modifying a Word in a Block

Adopt two methods to modify an address character of block according to the input mode

(INSERT/REWRITE).

INSERT mode: use the insert and the delete methods together.

(1) Press

，move the cursor to the required address character.

(2) Input the new word.

(3) Delete the invalid word according to the operation of deleting the content of block.

REWRITE mode: modify the character where the cursor points.

(1) Press

to switch to REWRITE mode (the cursor pointing to the address character in

highlight square).

(2) Press

to the required address character.

(3) Input the new address character, and the cursor points to the next one.

Example：Rewrite X of N0020 G0 X0.0 Z0.0 to U .
(1) Switch to Rewrite mode.
(2) Move the cursor to the under of X .
(3) Input U .

27

GSK928TEⅡ Turning CNC System User Manual

The end is ：N0020 G0 U 0.0 Z0.0.

4.3.3.8 Skipping a Block

Add / before the block number N of block, and the system will skip the block to execute
the next one when executing the program.

(1) Switch to INSERT mode.

(2) Move the cursor to the required block and press

the block number N of block.

(3) Sequentially press two times: the first time, insert before N ; the second

time, insert / before N .

to move the cursor to the under of

4.4 Manual Mode

In “Manual” mode, the motion of slider, the starting/stopping of spindle, cooling ON/OFF, manual tool
change, the program reference point return and the machine zero return in X, Z direction, and other
functions can be completed by operating the keyboard. When P11 Bit3 is set to 1, the actual spindle
speed can be displayed real time; when P11 Bit3 is set to 0, the programming spindle speed is
displayed. When the machine is equipped with the hydraulic chuck and the tailstock, the system can
control the operation of the hydraulic chuck and the tailstock by a pedal switch or external keys. They
keep interlock between the hydraulic chuck, the tailstock and the spindle.

Press

to enter Manual mode. There are JOG Jog mode and JOG Step mode. The initial

mode is JOG. Press to switch between JOG mode and Step mode. If the system is equipped
with the MPG, the system can adopt MPG control mode. JOG mode. is as follows:

Fig.11 JOG mode

4.4.1 Manual JOG

In JOG mode, press down a manual feed direction key, and the slider will continuously

28

GSK928TEⅡ Turning CNC System User Manual

traverse along the selected axis and direction. The slider will stop once the key is released.
The traverse speed will be executed according to the selected rapid traverse speed or feedrate.
Meanings of manual feed direction keys in JOG mode are as follows:

X negative key

X positive key

Z negative key

Z positive key

Note 1： Press the feed key in JOG mode, and the slider will traverse when the external spindle

and the feed hold knob are permitted to feed; press the manual feed key, and the

slider does not traverse in the state of feed hold.

Note 2: Even though the feed key is released, because the system automatically

accelerates/decelerates, the slide will continuously traverse not to stop when the

motor runs rapidly. The actual moving distance is determined by max. speed of the

motor, the acceleration/deceleration time and the feedrate override. The more the

acceleration /deceleration time is and the rapider the speed is, the longer the moving

distance of motor decelerating is, otherwise the moving distance is shorter.

4.4.2 Manual(JOG) Step

In STEP mode, the moving distance of slider each time is preset. The slider will traverse one

setting step in the selected coordinate axis and its direction when the manual feed direction key

is pressed once. When the key is pressed down, the slider feeds as one step until the last step

after it is released. The step width value is displayed with black.

Manual Step feed mode as Fig. 12：

Fig. 12 Manual step feed mode

29

GSK928TEⅡ Turning CNC System User Manual

Its step width is divided into 6 grades: 0.001 0.01 0.1 1.0 10.0 50.0

Press

to select each step width. The step width degrades one grade if it is pressed once. It

returns to the first grade after the last one is selected.

Note 1: In STEP mode, press

to stop slider traversing. When the key is pressed down,
the slider stops and the unfinished step will not be reserved, and then the feed key is
pressed to execute the next step feed. X step width is the moving distance in diameter.

Note 2: When the manual feed key is pressed, the external spindle and the feed hold knob are

permitted to feed, the slider traverses. When the manual step feed key is pressed, the

slider does not traverse in the state of feed hold.

Note 3: When the slider is traversing and the feed hold knob rotates to the feed hold position,

the slider will decelerate to stop and the unfinished step width will not be reserved.

4.4.3 Manual MPG (Handwheel) Control

In MPG mode, the micro motion of slider is controlled by rotating the manual pulse generator

(MPG). Press

or to enter MPG mode and select the coordinate axis controlled by

the MPG at the same time. See Fig. 13 (taking X axis as example).

Fig. 13 MPG control

z Rotate the MPG after selecting the required coordinate axis to move. The selected axis will

move along with the MPG rotating.

The MPG rotates (CW), the axis moves positively.

The MPG rotates (CCW), the axis moves negatively.

z There are three gears for each motion amount of MPG: 0.001, 0.01, 0.1mm. Press

to switch among them. The system will automatically select 0.1 mm when the previous step
size exceeds 0.1 from STEP mode to MPG mode.

z The system does not display the current speed of the spindle in MPG mode.

30

GSK928TEⅡ Turning CNC System User Manual

Note 1: The MPG speed of should be lower than 5 rev/s, otherwise the motor still moves even if

the MPG has stopped, which causes the moving distance does not correspond with the

scale.

Note 2: In MPG mode, all the functions related to the axis moving including JOG, zero return,

incremental/absolute movement are invalid, but S, M, T and other auxiliary functions

are valid.

Note 3: Even if the MPG is shaken, the slider does not traverse when the external spindle and

the feed hold knob forbid the slider to traverse. The spindle speed cannot be changed

real time.

Note 4: When the bigger override (X 100) is selected, the motor will rapidly traverse if the MPG

is rotated rapidly. At the moment, because the system automatically accelerates/

decelerate, the motor will traverse not to stop although the MPG stops. The actual

moving distance is determined by max. speed of motor, the acceleration/ deceleration

time, the feedrate override and the MPG speed. The rapider the speed is, the longer the

acceleration/deceleration time is and the rapider the MPG speed is, the longer the

moving distance of motor decelerating is, otherwise the shorter the moving distance of

motor is.

4.4.4 Manual Feedrate

Select the feedrate override in JOG feed mode.

The feedrate override increases one gear by pressing it once. Max. value :150%.

The feedrate override degrades one gear by pressing it once. Min. value : 0%.

Note 1: In JOG or MPG feed mode, select the feedrate override and then traverse the axis by

pressing manual feed direction key or rotating the MPG.

Note 2: In Step feed mode, select the feedrate override or increase/decrease the feedrate

override in the course of moving to change the feedrate.

Feedrate override (16 gears) as follows:

Feed override

0 0

10 7.5

20 22

30 38

40 60

50 82

60 110

70 180

80 240

90 300

100 420

110 525

31

Feedrate（mm/ min ）

GSK928TEⅡ Turning CNC System User Manual

120 675

130 850

140 1000

150 1260

4.4.5 Manual Rapid Traverse Speed/Feedrate

Select the rapid traverse speed/feedrate in JOG feed mode. The rapid traverse speed can be

selected by rapid traverse override divided into four gears 25%, 50%, 75%, 100%.

The actual feedrate is defined by the rapid traverse speed and the rapid traverse override:

X actual rapid traverse speed = P06 ×rapid traverse override

Z actual rapid traverse speed = P05 ×rapid traverse override

Selecting the manual rapid feed and the rapid traverse override is as follows:

Press

and rapid traverse override is displayed in a highlight square. Press
manual feed mode. See Fig. 14 for manual rapid traverse mode:

Switch feed/ rapid traverse.

Increase one gear of rapid traverse speed by pressing it once (Max. 100%).

Reduce one gear of rapid traverse speed by pressing it once (Min. 25%).

to switch to manual rapid traverse with the indicator ON. The feedrate override

again to switch to

Fig. 14 Manual rapid traverse

Note 1: In JOG feed mode, select the rapid traverse override and then press the coordinate axis

feed key.

Note 2: In Step feed mode, select the rapid traverse override or increase/reduce the rapid traverse

override in the course of traversing to change the rapid traverse speed.

32

GSK928TEⅡ Turning CNC System User Manual

4.4.6 Creating a Workpiece Coordinate

GSK928TE CNC system Ⅱ uses a floating workpiece coordinate which is the benchmark of

toolsetting and related dimension. After the system is installed, the workpiece coordinate must be

created firstly. When the actual position is inconsistent with that of the workpiece coordinate, the

coordinate is created again as follows:

（1） Install the trial workpiece reliably on the machine, and select a tool (usually select the first

one used in machining).
Select the proper spindle speed, and then start the spindle. Traverse the tool in “Manual”
mode, and cut a small sidestep of the workpiece.
X does not move but Z does to the safe position, and stop the spindle.

Measure the diameter of the cut sidestep. Press

to display Setting , and then

press to display Setting X, at last, input the metrical diameter and press ,

so the system creates automatically X workpiece coordinate, if is pressed , the
system cancels the creation of X workpiece coordinate.

（2） Start the spindle again and traverse the tool to cut a face on the workpiece in “Manual”

mode.

（3） Do not move Z but X to the safe position, and stop the spindle.

Select a datum mark (it is a fixed point on the machine, such as the face of chuck, the datum
plane of fixture, which can ensure the created new workpiece coordinate system coincides
with the previous broken one). Measure Z distance from the cut end face to the datum mark.

Press

to display Setting and press to display Setting Z , at last, input

the metrical diameter and press , the system creates automatically Z workpiece

coordinate, if
coordinate.

is pressed , the system cancels the creation of Z workpiece

Clear out the previous system offset after the workpiece coordinate system has been

created as the above-mentioned operation. If the workpiece coordinate system is not

created, there is warp between the current X, Z coordinate values displayed and the actual

tool position. Initialize the system before creating the workpiece coordinate system.

4.4.7 Setting Program Reference Point

The program reference point can be any position on the machine. Once the program reference
point is created, the slider anywhere else will return to this point by executing the program

33

GSK928TEⅡ Turning CNC System User Manual

reference point return (G26, G27, G29) or pressing the reference point return keys, at the
moment, cancel the tool compensation and the system offset. There are two methods to modify
the tool offset values(absolute input and incremental input) as follows:

The first method:

Move the cursor to the required tool offset number, press

to display Setting, and then

press to display Program Reference Point ?, at the moment, the point is the program

reference point by pressing . Cancel the setting of reference point by pressing .
There is no responding by pressing other keys.

The second method:

move the cursor to the required tool offset number, directly input the tool offset value and press

to complete the tool offset modification.

After the program reference point set, the previous reference point coordinate values do not be

changed in the new one if the workpiece coordinate is created again, and at the moment, the

program reference point needs to be set again. The initial value of program reference point is

X=150, Z=150.

4.4.8 Incremental Movement of Coordinate Axis

In “Manual” mode, traverse one axis according to the distance and direction input by user instead

of the step size defined by the system. Operations are as follows:

（1） Select the required axis to traverse. Press

displays Move U; press

to traverse Z, the system displays Move W.

to traverse X axis, and the system

（2） Input the required actual moving distance by keyboard. Input X, Z values with negative sign.

X value is in diameter. Press

to delete the wrong input. Press to cancel

the input and return to “Manual” mode.

（3） After inputting the data, press

, and the system displays “Run ？”; press

to traverse the selected axis according to the input distance and the direction.

Press

to cancel the movement and return to “Manual” mode.

（4） The incremental speed is the current selected manual speed.

34

GSK928TEⅡ Turning CNC System User Manual

Example：X moves negatively 15.8 mm from the current position as follows:

Press U – 1 5 . 8

, and the system displays Run ？; press , and

X moves negatively 15.8 mm.

4.4.9 Absolute Movement of Coordinate Axis

In “Manual” mode, traverse directly one axis from the current position to the input coordinate
position. Operations are as follows:

1. Select the required axis. Press

to move X axis, and the system displays Move X ; press

to move Z axis, the system displays Move Z.

2. Input the required actual coordinate value to reach the position (X value is in diameter) by

keyboard, and press

to delete the wrong input. Press to cancel the input and

return to “Manual” mode.

3. After inputting the data, press , the system automatically counts the required moving

distance and direction. With Run ？on the screen, press to move to the input coordinate

position. Press to stop and return to “Manual” mode.

4. The absolute speed is the current defined manual speed.

Example: Modify it into 85 if Z coordinate value is 50.

Press Z 8 5 and , the system displays Run ?, and the coordinate is

modified into 85 by pressing .

Note: In “Manual” mode, only one axis can be executed the incremental or absolute movement

at the current selected manual speed

.

4.4.10 MDI Function

In “Manual” mode, M functions can be executed by inputting M codes. Press

to display M,

and then input one or two-digit and press to execute the corresponding M function, or

press

to cancel the execution of M function.

Press ‘M’, ‘0’, ‘3’ to start the spindle rotating (CCW). Input and execute the following M codes:

35

GSK928TEⅡ Turning CNC System User Manual

M03 M04 M05 M08 M09 M10 M11 M32 M33 M21 M22 M23 M24. Omit it if

the first digit of M code is zero. The function is the same that in AUTO mode. For the explanations

of M codes, see Programming.

When MDI is error, the system prompts “DATA INVALID” and disappears by pressing

MDI mode, when the data is input or the coordinate is set,

instead of is

pressed, the system prompts “DATA INVALID” to escape. For example: input orderly T22 and

press , the system prompts “DATA INVALID” and escapes.

4.4.11 Manual Spindle Control

In “Manual” mode, the rotation (CCW/CW) and stop of spindle can be controlled by the keyboard

(if the feed/spindle hold knob is set in the position where the spindle is forbidden to rotate, the

spindle cannot be started even if the spindle rotation (CCW/CW) key is pressed. See User

Manual from the machine manufacture for gears of feed hold knob and mark symbols, and
Connection in the manual if the spindle needs to be connected separately).

Spindle rotation (CCW)

Displaying：SPINDLE CCW and LED ON

. In

Spindle stop
Displaying：SPINDLE STOP and LED OFF

Spindle rotation (CW)

Displaying：SPINDLE CW and LED ON

Note: Whether its brake signal is output is defined by MSP bit of P12 when the spindle stops. If

P12 MSP is 1, there is the brake signal when the spindle stops. If MSP is 0, there is

nothing. The time sequence relationships of the spindle brake, starting and stopping

signal are as follows:

1） In pulse control mode，M3, M4, M5, MSP output time sequence：

M3 or M4

M5
MSP

T1

T1

T2

T3

36

GSK928TEⅡ Turning CNC System User Manual

2） In level control mode，M3, M4, M5, MSP output time sequence

M3 or M4
M5

T1

T2

MSP

T3

T1：In pulse control mode，M3, M4, M5 signal duration is set by P15；

T2：Setting value: 0.2s；

T3：The output duration of spindle braking signal MSP is set by P16.

4.4.12 Manual Spindle Speed Control

For the machine with the multi-gear motor, press
to control the speed in JOG mode.

(1) Mechanical gear shifting control

When the P12 bit 0=0 (spindle speed controlled by the mechanical gear shifting), the output

mode of gear signal with multi-gear control is selected by P11 Bit4. When P12 bit 0=1, P11

Bit4 is invalid.

P11 Bit4=0: the gear signal is directly output for each bit. Each gear signal corresponds to an

output point from S0 to S4. S0 means that all output is invalid.

P11 Bit4=1: the gear signal is output according to the code. At the moment, the specific

spindle speed is gained from S00 to S15 by the external power circuit decode as

follows:

Code

Output point

S00 S01 S02 S03 S04 S05 S06 S07 S08 S09 S10 S11 S12 S13 S14 S15

or directly input the spindle speed code

S1 ★ ★ ★ ★ ★ ★ ★ ★

S2 ★ ★ ★ ★ ★ ★ ★ ★

S3 ★ ★ ★ ★ ★ ★ ★ ★

S4 ★ ★ ★ ★ ★ ★ ★ ★

“ ” means the output of corresponding output point is invalid.★

Spindle speed control operation：

Input S codes by keyboard to control the spindle speed. Pressing“ S” inputs the required speed

code; press

, and the system outputs the control signal according to the selected S code

mode.

Example: Select the eighth gear spindle speed.

37

GSK928TEⅡ Turning CNC System User Manual

Input orderly S 8

, and S8 signal is output with the displaying Prg. Speed S08.

Besides, press to change the spindle speed. If it is pressed once, the spindle speed is

output circularly S1, S2, S3, S4,(P11 bit 4=0) or S0～S15 ((P11 bit 4=1). The spindle speed

switches from S2 to S1 by pressing

three times when the spindle speed only has

two-gear.

(2) Frequency conversion control:

Select the converter to control the spindle speed when P12 Bit =1. Directly input the speed to
control the spindle when the machine is equipped with the converter to control the spindle.

Press

key to display S and input the required speed, then press , the system

converts the speed to 0-0V analog voltage by the output interface to output to the converter.

z To settle problems of the converter with low speed and torque, the system can execute

automatically the three-gear output signal, matching with the converter to ensure the

machine gain the low speed and power torque under the high frequency.

The system

provides three codes: M41, M42, M43 and three parameters: P09, P10, P24.

P09: Reach max. speed when the reduction gear of spindle is positioned on the low gear.

P10: Reach max. speed when the reduction gear of spindle is positioned on the high gear.

P24: Reach max. speed when the reduction gear of spindle is positioned on the medium gear.

M41: Output the low gear signal and use max. speed set by P09.

M42: Output the medium gear signal and use max. speed set by P24.

M43: Output the high gear signal and use max. speed set by P10.

Use M41, M42, M43 to select the required gear of spindle and then input directly the required

speed, and the system will automatically convert the output voltage to control the speed of

converter according to the current position of reduction gear. After power on, the system will

fault M43, i.e. the spindle is positioned on the high gear.

z Display the spindle speed: when P11 Bit 3=0, the programmed spindle speed is displayed

on the screen. When P11 Bit 3=1, the actual spindle speed is displayed.

z Detecting the encoder lines of spindle: the system directly detects the pulse amount per rev

of spindle encoder in “Manual” mode as follows:

Start the spindle and press

, and the system displays the pulse amount per rev of

spindle encoder. The system will prompt Encoder Error if the spindle is not started or the

encoder does not be installed. Press any keys to end the detection and return to “Manual”
mode.

38

GSK928TEⅡ Turning CNC System User Manual

Note 1: The spindle speed is controlled by P12 Bit0. When Bit0=0: it is the multi-gear control; when

Bit0=1: it is 0-10V analog voltage control.

Note 2: When P12 Bit0=1, P11 Bit4 is invalid, i.e. the spindle is always controlled by the converter. At

the moment, the output point S1, S2, S3, S4 is controlled by M41, M42, M43, and the

corresponding output point cannot be controlled by the spindle gear shifting key.

4.4.13 Manual Cooling Control

In “ Manual “ mode, press the key to control the cooling ON/OFF.

Cooling ON/OFF

Press

to switch the cooling ON/OFF. Start the cooling, and the system displays the

cooling is ON and LED is ON; stop the cooling, and the system displays the cooling OFF
and LED OFF.

4.4.14 Manual Tool Change Control

This system can control the tool post with 4 tool selections. It also can be extended to 8 tool

selections when T5～T8 tool selection signals are input in code mode. Three kinds of tool

change methods are as follows:

● Set P12 Bit1 to 0 and press

once, and the tool post rotates to the next controllable tool

number and the system displays the corresponding one.

● Set P12 Bit1 to 1, press once and , and the tool post rotates to the next

controllable tool number and the system displays the corresponding controllable tool number. If

is pressed, the tool post cannot execute the tool change when other keys are pressed.

● Input T * O directly by keyboard (* standing for rotating to the required controllable tool number)

and then press , and the tool post rotates to * which is pointing to the controllable tool,
and 0 stands for canceling the tool offset.

Note 1: For the first two methods, do not execute the tool compensation but the tool change, but

for the third, execute the corresponding tool compensation after inputting the tool

compensation number behind * .

39

GSK928TEⅡ Turning CNC System User Manual

Example: Input T22: switching to No. 2 tool and executing its compensation.

Input T31: switching to No. 3 tool and executing its compensation.

Input T40: switching to No. 4 tool and executing its compensation.

Input T00: canceling the tool change and the tool compensation.

Note 2: If the rotation tool post is failure, the system displays Tool NO. Lost , which indicates that

the system has not found the corresponding tool number in the specified time.

Note 3: The system is employed with the absolute tool change. When adopting the rotation tool

post, the tool number is fixed on the tool post. It ensures the tool number on the tool post

is the same as the one displayed on the screen.

Note 4: When P11 Bit5 is 1, select the line-up tool post. There is no signal output when executing

the tool change.

Note 5: When using the third method, execute the tool compensation by traversing the slider or

modifying the system coordinate which is defined by P11 Bit6.

Bit6=0: do not modify the coordinate but traverse the slider to execute the tool

compensation.

Bit6=1: do not traverse the slider but modify the coordinate to execute the tool

compensation.

4.4.15 Manual Toolsetting Operations

Usually, several tools are used in the course of machining a workpiece. Owing to the installation

and tool offset, the cutting position to which each tool rotates cannot coincide with that of the tool

nose. To avoid the tool offset in programming, this system set the automatic toolsettig method

according to the tool offset. User does not consider the tool offset but edits the part program

according to the workpiece drawing and the cutting technology, and calls the corresponding tool

compensation in the tool change command during the course of machining (For the usage, see

Program, tool compensation function).

Here are the two methods in this system:
GSK928TE CNC system has set the trial cutting and the fixed point toolsetting, and user can Ⅱ

select anyone. The specifications are as follows:

Trial cutting toolsetting mode:

(Create the workpiece coordinate system before adopting the trial cutting toolsetting mode. The

operations are the same those of ones after setting the workpiece coordinate system or

executing the program reference point return〔program home return〕)

1. Prepare for the toolsetting.

2. Input T00 to cancel the previous tool offset and then execute the toolsetting when the tool

offset number is not zero，otherwise the system will count all values between the previous tool

offset value and the new one (the operations must be executed when the tool is worn and

needed to execute the toolsetting again). If necessary, execute the toolsetting with the tool

40

GSK928TEⅡ Turning CNC System User Manual

offset.

3. Select any one tool after the workpiece is fixed on the machine (usually, the tool is the first one

used in machining).

4. Start the spindle with the proper speed. Traverse the tool to cut a little sidestep on the

workpiece in “Manual” mode.

5. X does not move but Z does to the safe position, and stop the spindle.

6. Measure the diameter of sidestep cut. Press

to display Offset X and input the

metrical diameter, and then press to display T * X (* standing for the current

controllable tool number) and press to count X tool offset value and store the value to
X tool offset parameter area to which * corresponds. The offset value can be searched and

modified in OFFSET mode. When T * X is displayed on the screen, input the digit 1～8 and

press to count the tool offset value and store it to X tool offset parameter area to

which the input digit corresponds. Press not

but to cancel the count and the

storage of tool offset.

7. Start the spindle again and traverse the tool to cut a face in “Manual” mode.

8. Z does not move but X does to the safe position, and stop the spindle. Select a point as a
datum mark (usually, the datum mark is a fixed point such as the chuck face, the fixture
datum plane, which is contributed to find easily the previous datum mark when executing the
toolsetting again), and measure X distance from the cut face to the selected datum mark.

Press

to display Offset Z and input the metrical data, and then press to

display T * Z(* standing for the current tool position No.), and last press to count Z

tool offset value and store it to Z tool offset parameter area to which * corresponds. The offset

value can be searched and modified in OFFSET mode. When T *Z is displayed on the

screen, input the number 1～8 and press to count the tool offset value and store it to

Z s tool offset parameter area to which the input number corresponds. Press not

but

to cancel the count and the storage.

9. Change another tool and repeat the above-mentioned operations 1-6 to execute other

toolsetting.

10. If the workpiece coordinate system has not been changed, all toolsettings are executed like

the above-mentioned. The toolsetting is easy and convenient when the tool is worn or

41

GSK928TEⅡ Turning CNC System User Manual

needed to tune. Firstly, cancel the tool compensation (T00) or execute program reference

point return (program home) when the tool compensation cannot be input or the counting

data is wrong.

Fixed point toolsetting mode:

1. Select anyone tool (usually it is the first one used in machining) as a reference tool after

installing the trial cutting workpiece on the machine.

2. Start the spindle with the proper speed.

3. Select the proper manual feedrate, traverse the tool to the specified toolsetting point on the

workpiece in the manual feed mode, and stop the movement when the tool coincides with
the toolsetting point.

4. Press

highlight, then press continuously

, and the system display the current tool number and tool offset number in

two times, and the system displays normally the
current tool number and tool offset number, and automatically records the current coordinate
and considers it as the toolsetting reference of other tools (the operation cannot executed if
it is not the reference tool). It is necessary to execute the following operation for the
reference tool.

5. Press

and then (if the tool wears, press to execute the toolsetting
by taking the executed toolsetting tool as a reference), and the system displays normally the
current tool number and tool offset number, counts the offset value of the current
corresponding tool number and stores it to the corresponding parameter area. The offset
value can be searched and modified in OFFSET mode.

6. Traverse the tool to the tool change position from the toolsetting position in “Manual” mode

and rotate the next required one to the cutting position by manual tool change.

7. Repeat the above-mentioned operations 2, 3, 5 until all toolsettings have been completed.

Note 1: When adopting the optic toolsetting instrument, do not start the spindle but fix the

toolsetting point on the cross point of the toolsetting instrument, other operations are

the same as the above-mentioned.

Note 2: The tool offset automatically created by the system can be displayed and modified in

OFFSET mode. See OPERATION, OFFSET mode.

Note 3: If the tool is worn to change or a new one is installed, select another one which has been

executed the toolsetting as the reference tool. Firstly, fix the tool to the selected point on

the workpiece according to the toolsetting of reference tool (as the above-mentioned

operation No. 4 instead of No. 5), then, return to the safe position, last, change the new

tool and repeat the above No. 2, 3, 5 step to execute the toolsetting (the previous offset

value is not always zero).

Note 4: When the line-up tool post toolsetting is used and the tool is on the other side of

workpiece, X input metrical value is negative in the course of trial cutting toolsetting.

42

GSK928TEⅡ Turning CNC System User Manual

When the fixed point toolsetting is executed by hand, X tool offset value sign related to

the tool number is changed, i.e. “+” is changed into “-”and“-”into “+”.

4.4.16 Manual Program Reference Point Return

X, Z zero return (program zero return, machine zero return) operations must be executed at the

same time. If only one axis is being executed, the other maybe bring the unexpected motion.

Press the following keys to execute the program reference point return at any moment after

defining the program reference point.

Press

X program reference point return

to return from the current point to X program reference point at the selected

speed.

Z program ref er ence point return

Press

to return from the current point to Z program reference point at the selected

speed.

Note: Cancel separately the tool offset and the system offset in the corresponding axis after

executing the reference point return. After executing X, Z reference point return, the

system returns the state of canceling the tool offset and the system offset, displaying T * 0

(* is the current tool number).

4.4.17 Manual Machine Zero Return (Machine Reference Point Return)

Each machine has a fixed point as a reference point. The accumulative error can be deleted by

returning to the machining starting point after executing the machine zero return each time.

Before machining, firstly execute the machine zero return, and then specify the starting point of

machining, at last, write down its coordinate. For restarting the machine after power off, firstly

execute the machine zero return, and then return to the machining starting point written down to

start programs, which make the actual position accord with the system coordinate caused by

man moving the machine. Cancel the machine zero return when P12 Bit7 is 0.

X machine zero return

Press to move X positively to the machine zero at the selected rapid traverse speed.

43

GSK928TEⅡ Turning CNC System User Manual

Z machine zero return

Press to move Z positively to the machine zero at the selected rapid traverse speed.

Operations of machine zero return with the machine zero signal (P12 Bit4=0) are as follows:

1. The slider positively traverses along the selected axis at the rapid traverse speed. After the

mechanical stopper pushes down the deceleration signal of machine zero return, the slider

begins to decelerate to the lowest traverse speed (it is defined by P17 or P18), and traverses

continuously till the mechanical stopper disengages from the deceleration signal of machine

zero return.

2. The slider traverses continuously at the lowest traverse rate. When this system receives the

signal of one rev of motor encoder, the slider reaches the machine zero and stops the motion.

Such is the operation of machine zero return. The coordinate is set to the data defined by T9X

or T9Z in the course of tool compensation.

Operations of machine zero return without the machine zero signal are as follows:

1. The slider positively traverses along the selected axis at the rapid traverse speed. After the

mechanical stopper pushes down the deceleration signal of machine zero return the slider

begins to decelerate to the lowest traverse speed (it is defined by P17 or P18), and traverses

continuously. The coordinate is set to the data defined by T9X or T9Z in the course of tool

compensation.

2. Stop the motion when the mechanical stopper disengages from the deceleration signal of

machine zero return, and so the operation of machine zero return is completed.

Note 1: The machine zero return is positive. Ensure that the tool post is placed in the negative

direction of the machine zero before executing the machine zero return.

Note 2: If the machine is not equipped with the deceleration signal of machine zero, the P12 Bit7

must be set to 0 to cancel the machine zero return, otherwise the tool post moves at

max. speed to cause accidents.

Note 3: Cancel the system offset and the tool offset after executing the machine zero return.

4.4.18 Hydraulic Chuck Control Function

When P25 Bit1 is 1, the system has the hydraulic chuck control function. Separately select the
clamping mode and the output signal mode of chuck according to P25 Bit2 and Bit4 when the
hydraulic chuck control is valid. Whether the in-position signal is detected is defined by P25 Bit3;
the hydraulic chuck control and the spindle control have a relationship of interlock.
Bit2=0：the hydraulic chuck is outside chuck mode;

Bit2=1：the hydraulic chuck is inside chuck mode；
Bit4=0：the hydraulic chuck control signal uses the level control；

44

GSK928TEⅡ Turning CNC System User Manual

Bit4=1：the hydraulic chuck control signal uses the pulse control; its width is defined by the time

of P15；

Bit3=0：the hydraulic chuck needs to receive the in-position feedback signal；

Bit3=1：the hydraulic chuck does not need to receive the in-position feedback signal.

In outside chuck mode: After M10 is executed, the system outputs the chuck clamping signal
from X 7.19 (the output pulse or the level signal is selected by the parameter) and the chuck
clamping operation ends without needing the in-position feedback signal; when needing the
in-position feedback signal, the chuck clamping operation ends after detecting the in-position of

chuck clamping within 5 seconds, otherwise the system prompts “Chuck Ready Failure ”;

After M11 is executed, the system outputs the chuck releasing signal from X 7.18 (the output
pulse or the level signal is selected by the parameter), the chuck releasing operation ends
without needing the in-position feedback signal; when needing the in-position feedback signal,
the chuck releasing operation ends after detecting the chuck releasing in-position signal,

otherwise the system prompts “Chuck Ready Failure”;

In inside chuck mode: after M10 is executed, the system outputs the chuck clamping signal from
X 7.18, (the output pulse or the level signal is selected by the parameter), and the chuck
clamping operation ends without needing the in-position feedback signal; when needing the
in-position feedback signal, the chuck clamping operation ends after detecting the chuck

clamping in-position signal within 5 seconds, otherwise the system prompts “Chuck Ready

Failure”;

After M11 is executed, the system outputs the chuck releasing signal from X 7.19, (the output
pulse or the level signal is selected by the parameter), the chuck releasing operation ends
without needing the in-position feedback signal; when needing the in-position feedback signal,
the chuck releasing operation ends after detecting the chuck releasing in-position signal,

otherwise the system prompts “Chuck Ready Failure”

Besides commands, other ways are employed to control the hydraulic chuck, including the

external pedal switch. The system switches the clamping/releasing by M10/M11 when the pedal
switch is stepped once.

input

signal

input
signal

]

M10

M10

M11

M11

Time sequence of pulse control mode Time sequence of level control mode

Note 1: When the hydraulic chuck control is valid, the previous user input commands

(M91/M92/M93/M94) are invalid; when the hydraulic chuck control is invalid, the output
point is still used to the general one without interlocking with the spindle; the input point
is still used by the user, and M91/M92/M93/M94 are still valid.

Note 2: When the hydraulic chuck control is valid, the system defaults the chuck releasing after

power on, the first control input of chuck is valid and the system outputs the signal of
chuck clamping.

Note 3: The chuck control invalid when the spindle rotates.
Note 4: When the spindle rotates in the state of chuck releasing, the system prompts “Chuck

Ready Failure” and the spindle stops at the same time.

Note 5: In the course of automatic (continuous) run, the pedal switch control is invalid whether

the spindle rotates or not. When executing M10/M11 in the course of spindle rotating,

45

GSK928TEⅡ Turning CNC System User Manual

the system prompts “Spindle Ready Failure” to stop executing the next block; when
executing M3 or M4 in the state of chuck releasing, the system prompts: “Chuck Ready

Failure” to stop executing the next block.

4.4.19 Hydraulic Tailstock Control Function

When P25 Bit0 is 1, the system has the hydraulic tailstock control function. The output signal
mode of tailstock is defined by P25 Bit2 (level or pulse mode) when the hydraulic tailstock
control is valid. The hydraulic chuck control and the spindle control have a relationship of
interlock.
Bit4=0: the hydraulic tailstock control signal is employed with the level control;
Bit4=1: the hydraulic tailstock control signal is employed with the pulse control; the pulse width is

defined by the time of P15.

After M78 is executed, the system outputs the tailstock forward signal from X 7.5(the output
pulse or level signal is selected by the parameter), the tailstock forward operation ends; when
executing M78 in the course of the spindle rotating, the system prompts “Spindle Ready Failure”

After M79 is executed, the system outputs the tailstock backward signal from X 7.16(the output
pulse or the level signal is selected by the parameter), the tailstock backward operation ends;
when executing M79 in the course of the spindle rotating, the system prompts “Spindle Ready
Failure”.

Besides the commands, other ways are employed to control the hydraulic tailstock, including the
pedal switch. The system will switch the forward/backward by M78/M79 when the pedal switch is
stepped once.

input

signal

M78

M79

Time sequence of pulse control mode Time sequence of level control mode

Note 1: When the hydraulic tailstock control is valid, the previous user input M21/M22/M23/M24

is invalid; when the hydraulic tailstock function is invalid, the output point is still used for
the general one and the input point is used for the in-position signal input.

Note 2: When the hydraulic tailstock function is valid, the system defaults the state of the

tailstock retracting after power on. The system outputs the forward signal of tailstock
when the first chuck control input is valid.

Note 3: The operation of tailstock is invalid when the spindle is rotating.

Note 4: In the course of automatically continuous machining, the tailstock control input is invalid

whether the spindle rotates or not. When executing M78/M79 in the course of spindle
rotating, the system prompts: “Spindle Ready Failure” to stop executing the next block.

input

signal

M78

M79

46

GSK928TEⅡ Turning CNC System User Manual

4.5 AUTO Mode

In AUTO mode, CNC system executes the selected part programs orderly to machine the

qualified workpiece.

Press
block machining run or the continuous machining run in AUTO mode. See Fig. 15:

to enter AUTO mode. Select the dry run or the machining run; select the single

Fig. 15 AUTO mode

4.5.1 Function Keys in AUTO Mode

Switch Single/( Contiuous) Run mode

Switch Single block/(continuous) Run by pressing

Single mode and Auto Run is displayed in AUTO (Continuous) Run mode.

In AUTO (Continuous) Run mode, the system stops executing the next block by pressing the key,

and press

Switch Dry/Machining run mode

In AUTO mode, switch dry run/ machining run mode by pressing
RUN mode, but LED is OFF in machining mode.

47

to run continuously the next block.

, Au to BLK is displayed in AUTO

. LED is ON in DRY

GSK928TEⅡ Turning CNC System User Manual

In DRY RUN mode, the slider does not traverse and other auxiliary function controls are invalid
when programs run.

Select the required block by pressing

Select block number

and start to run from the selected block by pressing

.

Program run key

Execute one block in Single mode and one operation in cycle commands by pressing the key.

Execute the the whole program in AUTO(Continuous) Run mode by pressing the key.

Feed hold key

The slider will reduce to stop by pressing the key when programs are running, displaying
Pause! in highlight in the top right corner on the screen. Continue to execute the unfinished

programs by pressing . The system does not execute the unfinished program to return to

the first block by pressing

4.5.2 Automatic Run a Part Program

.

Enter AUTO mode after preparations for machining are ready. The system runs the selected part
program orderly to machine the workpiece automatically.

4.5.2.1 Running a Part Program from the First Block
After entering AUTO mode, the system automatically displays the previous two blocks on the

screen, and * is displayed in the front of the first block number. After pressing
the automatic run, the workpiece is machined automatically. The first block is the current running
one and the second one is ready to run.

4.5.2.2 Running a Part Program from a Specified Block

In some special conditions, it is necessary to start to run from some block in a part program. This
system allows starting any one block of current part program and placing the tool post in any
position.
The particular steps are as follows:

1. Confirm the specified run block. Execute G50 in Single mode and select the required run block
when using G50 to define the coordinate system and running a program from the specified
block.

(1) The system displays the first block of current running program by pressing

.

(2) The system displays the content of previous or next block by pressing

The system escapes from the selected block and displays the previous one by pressing

to start

.

.

48

GSK928TEⅡ Turning CNC System User Manual

2. After selecting the required block and pressing , the system prompts “Run?” to wait the
next execution.

3. After pressing
starting point of selected block and start to execute the block. The system escapes from the

selected block and return to the first block after pressing .

Press to execute the program from the selected block.

Note 1: The specified block cannot be in canned cycles, compound cycle bodies or subprograms,

otherwise there is the unexpected run.

Note 2: When using the coordinate system defined by G50 in the program, after power on, do not

run the program from the specified one before the system creates the coordinate system
by G50, otherwise there is a mistake run.

Note 3: When running the program from the specified block, the selected block should be for

executing linear movement or S. M. T. Ensure the coordinate of tool and system must be
placed on the starting point of arc, otherwise the machined circular arc may be not
qualified.

4.5.2.3 Single and (Continuous) Run Mode of a Part Program

Select Single mode to ensure the program is right after editing the part program.

The program will automatically execute one block by pressing

with “Run ?”on the screen, the system will automatically traverse to the

once, observing whether

the machine running is the same that of the expected to decide the next execution. Press
again to execute orderly the program until it ends. Halt the run and return to the program reference
point and modify the program until it is right if there are different between the expected run and the
actual one, and then select (Continuous) Run to execute the continuous machining.
Switch Single/(Continuous) Run by pressing .

Single and (Continuous) Run

z Press

the selected run mode is displayed on the screen.

z Press

executing the next one after executing the block. The system displays Halt in highlight on

the screen as Fig. 16. Press to execute the continuous run not to switch to Single

mode. Press

on the screen). Stop/cancel Single by pressing in the course of the program running.

to switch Single/ (Continuous) Run without executing the part program, and

to halt Single mode when the part program is continuously running, i.e. halt

to switch to Single mode after running the program (Halt in highlight

z When the part program is being executed in Single mode, pressing is invalid.

Note: The initial run is in (Continuous) Run mode when the system enters AUTO mode.

49

GSK928TEⅡ Turning CNC System User Manual

4.5.2.4 Dry Run and Machining Run
After editing a part program, ensure the coordinate data on the screen is the same that of the

actual one and the relationship between blocks is right to avoid the bad effect caused by
inputting mistake program data. Switch to the machining run mode to execute the machining if

there is no mistake in the dry run program. Switch dry/machining run by pressing
is ON in the top left corner when the program is running in DRY RUN mode.

Note 1: In DRY RUN mode, the slider does not traverse and other auxiliary functions are invalid.
Note 2: The initial run is the machining run mode when the system enters AUTO mode.

Fig.16 Single block stop

4.5.3 Displaying in a Part Program Running

When the part program is running, this system displays the running state, the dynamic run
coordinate, the workpiece planar solid graph, and the path of tool nose in the course of program
running, which is very convenient to monitor the running state of the machine and the program.
See the display as follows:

z The dynamic coordinate, the dynamic planar graph or the path of tool nose when running

the part program

z Content of current running block
z Running state of spindle, cooling, speed, tool and other auxiliary function

z Feedrate override

4.5.3.1 Coordinate Display in a Part Program Running

After entering AUTO mode, the system automatically selects the coordinate display mode as Fig.
17:

. LED

Fig.17 Program display in AUTO mode

50

GSK928TEⅡ Turning CNC System User Manual

Press to switch between the coordinates and the graphics display in AUTO mode. After
switching from the coordinates display to the graphics display in run, the path of tool nose after
switching is only displayed, the one before switching cannot be displayed.

4.5.3.2 Graphics Display in a Program Running

When there is no program to run in AUTO mode, press to display the planar solid in

highlight square and the analog tool shape according to the set workpiece dimension as Fig.18.

Fig. 18 Planar solid graph in AUTO mode

Fig. 19 Path of tool nose display in AUTO mode

4.5.3.3 Graphics Displaying Data Definitions

Because the display area of this system is limited, the different scale is employed to display the
whole graph of part. The length, the diameter of blank, the initial offset of tool and the display

scale are defined by the system. Press
coordinate display or the graphics display as Fig. 20:

to define the above-mentioned data of

51

GSK928TEⅡ Turning CNC System User Manual

Fig. 20 Data definition of graphics display

Length(LEN.)： Total length of blank Unit：mm
Diameter(DIA.)： Max. outer diameter of blank Unit：mm
Offset(OFFS.)： Z offset between the programmed benchmark point and the starting point of

blank, X programmed benchmark point is the center line of blank. Unit: mm

Example：length of blank：100mm

End face 2

End face 1

If the face 1 is the programmed benchmark point, the offset is 0.
If the face 2 is the programmed benchmark point, the offset is 100.

Scale: ensure the scale of workpiece shape displayed is irrelevant with the actual machining

one.
If the workpiece is bigger and the selected scale will be reduced; if the part is smaller and
the selected scale will be enlarged, which contribute to a better view effect.

4.5.3.4 Inputting Data of Graphics Display

When the program is not running or pauses in AUTO mode, press

to display the data

defined previously as Fig. 18 with the cursor pointing to the first digit of the length.

z Input the data (without the decimal point) and press , and the system will

automatically point to the next data. Recycle among the above-mentioned four data by

pressing

z Rewrite the scale: enlarge or reduce one gear by pressing or once when

52

continuously.

GSK928TEⅡ Turning CNC System User Manual

the cursor points to Scale .
The scale is defined by the system: 4:1, 3:1, 2:1, 1:1, 1:2, 1:3 and 1:4. User can select the
proper scale to realize the best view effect.

After rewriting the data, press

to return to AUTO mode, the system updates the

displaying range of blank according to the set display data in the graphics display mode.

When the set display data exceeds the screen displaying range, the system prompts Out Of

Graph, and the display data must be rewritten again.

Note 1: The starting point of tool must be out of the blank displaying range, otherwise the

machining process cannot be displayed exactly.

Note 2: After switching from the graphics display to the coordinate display in the course of

machining, the displaying is not the previous machining path but the next machining one.
Switch to the planar solid display in the course of the program running, the workpiece
shape may not be displayed normally until the next cycle is executed.

4.5.4 Manual Operation of Auxiliary Function

In AUTO mode, the auxiliary functions such as spindle control, cooling ON/OFF, and spindle
speed can be operated by pressing the corresponding keys without the program running, but the
cooling can be also controlled in the course of program running.

Spindle rotation (CCW): SPINDLE CCW and LED ON.

Spindle stop: SPINDLE STOP and LED OFF.

Spindle rotation (CW): SPINDLE CW and LED ON.

Cooling ON/OFF: After starting the cooling, the system displays Cooling ON and LED is

ON; after stopping the cooling, the system displays Cooling OFF and

LED is OFF.

Spindle gear shifting: S01～S04, displaying of corresponding spindle speed on the

screen.

When the hydraulic chuck control function is valid, operate the external button or the pedal switch

to control the clamping and releasing of chuck which state interlocks with the spindle one.
When the hydraulic tailstock control function is valid, operate the external button or the pedal
switch to control the forward or the backward of tailstock which state interlocks the spindle one.

Note ：The tool change cannot be executed by manual pressing keys in AUTO mode.

4.5.5 Override Tune

In AUTO mode, the running speed of program can be tuned by changing the feedrate override

without changing the set speed in programs or parameters

z Feedrate override tune the value defined by F in the program:

53

GSK928TEⅡ Turning CNC System User Manual

Actual feedrate = F×feedrate override
It has 16 gears from 0%-150% (increment of 10%). All the feedrate commands are controlled by
feedrate override. When the feedrate override is 0, the programs stop.

z Rapid traverse override tune the rapid traverse speed (G00)

X actual rapid traverse speed = P05×rapid traverse override

Z actual rapid traverse speed = P06×rapid traverse override

The rapid traverse override is divided into 25%, 50%, 75%, 100%. All feed commands and the
operations are controlled by the rapid traverse override.

The feedrate override will increase one gear by pressing

once (Max. 150%).

The feedrate override will reduce one gear by pressing

once (Min. 0%).

The rapid traverse override will increase one gear by pressing

once (Max. 100%).

The rapid traverse override will reduce one gear by pressing

once (Min. 25%).

Note: Whether programs are running or not, pressing the above-mentioned corresponding key

can change the rapid traverse speed. The speed of slider will be changed if the rapid
traverse speed override is changed when the programs are running.

4.5.6 Operations in a Part Program Running

The operations in the course of part program running are as follows:

z Feed hold

After pressing ，the tool post stops with Pause ！on the screen.

If the feed hold function is valid, the system will continuously execute the unfinished block by

pressing

. When is pressed, the system returns to the feed hold state not to
execute the following block and switches automatically to SINGLE BLOCK mode, and the
program automatically returns to the first block. In the state of feed hold, the feedrate override
key, the rapid traverse override key, the spindle start/stop key and the cooling ON/OFF key are
valid.

Note: After executing the feed hold, ensure the spindle is started before running to avoid the

unexpected accidence.

z Single block stop

Press
on the screen.

After single block stopping, press

press

54

to stop to execute the next program after finishing the current block with HALT

to execute continuously the program or

to return to AUTO mode and the program stops.

GSK928TEⅡ Turning CNC System User Manual

Note

：

The operation of single block stop is valid when the program is running in AUTO

(Continuous) Run mode, and pressing key is invalid when the program is running in
AUTO Single mode. When executing the canned cycle commands, the operation of
single block stop is valid after finishing each step of the canned cycle.

● Modifying offset

In AUTO mode, modify the offset, but cannot modify that of the current machining run.

Modify the offset value in automatic run:

In automatic run, the offset value can be modified. When the offset value which corresponds
to the current tool offset number is modified, the modified value will be valid in the next
execution. When the tool offset value which corresponds to the unexecuted tool offset number,
the modified value is value in this execution. The operations are as follows:

① Press

in automatic run, and the system switches to the modification offset

display window:

Press

again, and the system returns to AUTO mode, displaying the window

circularly.

② Press

to select the required modification offset number, press “X”, “Z” to

select the required modification axis.

③ Input the data. When the input data directly replaces the previous, is pressed.

Press

to modify the previous data. Press to cancel the input data.

Note 1: In inputting the data, the system can be switched to the display window in AUTO mode

anytime, and switched the display window in OFFSET mode, and the previous input
data is still kept and you can continuously input the new.

Note 2: In inputting the data, the system automatically returns the display window in AUTO

mode when the pause or end of program appears.

Note 3: In displaying the offset modification window, the pause, the modifying feedrate override

and other operations are valid in AUTO mode. The system can be switched to the

55

display window of offset modification to execute the offset modification in PAUSE mode.

● Cooling ON/OFF

GSK928TEⅡ Turning CNC System User Manual

Press

to switch cooling ON/OFF.

When the cooling is ON, the system displays Cooling ON and LED is ON in the top right corner;
when the cooling is OFF, the system displays Cooling OFF on the screen and LED is OFF in

the top right corner.

z Override
The feedrate override and the rapid traverse override are tuned when the program is running or
the feed hold is valid, and the speed is immediate valid after tuning. For the tuning operation,

see Section Operation, 4.5.5 Override tune.

Before executing each block, the system prompts Feedrate Zero when the feedrate override is
zero. When the feedrate override is tuned to zero in the course of program running, the program
will stop and the system has no the prompt. The program continues to run when the feedrate
override is not zero.

4.5.7 Program Reference Point Return in AUTO Mode

To simplifying operations, the part program can be started wherever the slider is placed after
defining the workpiece coordinate system and the program reference point. At the moment, the
first traverse command of part program must be G00 and must be positioned with X, Z absolute
coordinates. In this case, the operation of program reference point return by pressing key or with
G26/G27/G29 is to return to the defined program reference point. After using G26/G27/G29, use
G00 to again position Z/X absolute coordinate (i.e. G00 Z_ X_) to gain the qualified machining.
After executing the program reference point return by pressing key, the system will automatically

point to the first block. At the moment, if

is pressed, the system runs from the first

block.

4.5.8 Feed Hold Knob in Automatic Run

GSK928TEII CNC System is equipped with an external interface of feed/spindle hold knob.

Traverse or stop the spindle and the slider when the knob is placed on the different position. Use
the knob to control conveniently the starting/stopping of spindle and the slide. There are three
positions of feed hold knob and its function as follows:
Position 1: permit the spindle to rotate and the slider to traverse.
Position 2: permit the spindle to rotate and forbid the slider to traverse.
Position 3: forbid the spindle to rotate and the slider to traverse.

Note: see the specific symbol specification of feed

hold knob from the machine manufacture.

Feed hold knob

4.5.8.1 Specification of Feed Hold Knob
Before program running

56

GSK928TEⅡ Turning CNC System User Manual

Press the correspond keys to control the spindle starting/stopping when the feed hold knob is
placed to the position 1 and 2; but the spindle cannot be started when it is placed to the position

3.

In AUTO Single mode

When the knob is placed to the position 1, all commands run normally; when it is placed to the
position 2, the control commands for spindle run but the motion commands of X, Z do not run
until the knob is placed to the position 1, when it is placed to the position 3, no blocks run.

In AUTO (Continuous) Run mode

After starting programs, the feed hold knob can be rotated any time to control the spindle and
the slider.

When the knob is placed to the position 1, programs run normally.

When the knob is rotated from 1 to 2, the slider stops and the spindle still keeps the previous
state.

When the knob is rotated from 2 to 3, the spindle stops.

When the knob is rotated from 3 to 2, the spindle restores the previous state.

When the knob is rotated from 2 to 1, the slider starts to run.

The system will automatically escapes from the automatic machining state after

pressing

or the reset key in the course of the feed hold and the spindle stopping. The
previous state of spindle and the unfinished commands cannot be reserved. Programs are
restarted if the machining is executed continuously.

57

GSK928TEⅡ Turning CNC System User Manual

4.6 Parameter Setting

There are 25 parameters ( P01～P25) in this system. Each parameter is defined to execute a
certain operating mode of the CNC system and the machine, and so some parameters must be
modified when the machine is installed and tuned.

Press to enter Parameter setting mode. The displaying is from P01 to P09 on the first
screen as Fig. 21:

Fig. 21 Parameter setting mode

Pressing

can display the previous or next parameter and its Chinese definition.

4.6.1 Parameter Specification

After the parameter number is selected, it is displayed in highlight and its name is displayed with
Chinese under the screen. The specific definitions are as follows:

4.6.1.1 P01 P02—Z Positive/Negative Overtravel (Soft Limit)

P01, P02 defines separately Z max. stroke of tool post in positive and negative direction. If Z

coordinate is not less than what is defined by P01 (positive overtravel), Z does not move instead
positively but negatively. If Z coordinate is not more than what is defined by P02 (negative
overtravel), Z does not move negatively but positively. Unit: mm.

4.6.1.2 P03 P04—X Positive/Negative Overtravel (Soft Limit)

P03, P04 defines separately the max. stroke of tool post in X positive and negative direction. If X

coordinate is not less than what is defined by P03 (positive overtravel), X does not move instead
positively but negatively. If X coordinate is not more than what is defined by P04 (negative
overtravel), X does not move negatively but positively. Unit: mm

Note 1: Though the coordinates range is 8000-

distance cannot be more than 8000 in AUTO mode.

4.6.1.3 P05—Z Rapid Traverse Speed

P05 defines Z rapid traverse speed in “Manual” mode and G00. The actual rapid traverse speed
is also controlled by the rapid traverse override. Z actual rapid traverse speed = P05* rapid

58

or can page up or page down to display other parameters, and pressing

（

-8000）=16000，but the incremental moving

GSK928TEⅡ Turning CNC System User Manual

traverse override. Unit: mm/min

4.6.1.4 P06—X Rapid Traverse Speed

P06 defines X rapid traverse speed in “Manual” mode and G00. The actual rapid traverse speed

is also controlled by the rapid traverse override. X actual rapid traverse speed = P05* rapid
traverse override. Unit: mm/min

4.6.1.5 P07 P08—X, Z Backlash Value

P07 P08 separately defines X, Z backlash value of mechanically-driven. Unit: mm.
There are backlash clearance in the lead screw, the decelerator and other driving device, which
cause the error in the repeated motion of tool post. To avoid the error, set P07, P08, which make
CNC system automatically compensate the error when the machine changes its moving
direction.
Measurement method of mechanically-driven backlash (Example: Z axis):

z Select “Manual” mode and the proper feedrate.
z Install the dial indicator on the proper position of the machine, move the tool post to the

probe of the dial indicator and set its pointer to zero.

z Select STEP mode with the step size 1.0 mm.

z Press Z feed key to move the tool post to the dial indicator and make it point to zero when

rotating one circle.

z Press Z feed key to move reversely and the pointer of dial indicator turns around. The

pointer cannot return to zero because of the backlash. At the moment, D-value between the
pointed position of pointer and zero is Z backlash value.

Note 1: Repeat the above-mentioned operations many times to gain the exact measurement

value.

Note 2: The measurement method of X backlash is the same that of Z, but the D-value must

multiply 2 to convert to the diameter value.

Note 3: The compensation speed of X, Z backlash is the initial speed (P17, P18 value) of each

axis.

4.6.1.6 P09—Low Gear Speed of Spindle

P09 defines max. speed when the system is employed with the converter to control the spindle
with the low gear (M41 is valid) and the 10V analog output voltage of system. P09 is invalid when
the spindle is controlled with multi-gear switching value. Unit: r/min.

4.6.1.7 P10—High Gear Speed of Spindle

P10 defines max. speed when the system is employed with the converter to control the spindle
with the high gear (M43 is valid) and the 10V analog output voltage of system. P10 is invalid
when the spindle is controlled with multi-gear switching value. Unit: r/min.

Note: The system will consider P10 value as the output benchmark when the spindle has no

high/medium/low gear. At the moment, P09, P23 are invalid. The high gear is valid after
power on.

4.6.1.8 P11 P12—Bit Parameter 1, Bit Parameter 2

For the different requirements of different machine, some control functions of this system can be
realized by setting the corresponding Bit of P11, P12 to 0 or 1.

The Bit parameters from left to right are Bit７～Bit 0 . Each bit can be set to 0 or 1.

● P11 bit specification

59

GSK928TEⅡ Turning CNC System User Manual

Bit7 Bit6 Bit 5 Bit 4 Bit 3 Bit 2 Bit 1 Bit 0

Bit 7 0 in MPG mode, 0.1mm override is valid.

1 in MPG mode, 0.1mm override is invalid, enter the menu after the system has

been ON for 15s.

Bit 6 0 move the machine slider not to modify the coordinates when executing the offset.

1 modify the coordinates and do not move the machine slide when executing the

offset.

Bit 5 0 the system uses the general motor turret tool post.

1 the system uses the line-up tool post.

Bit 4 0 the spindle speed gear directly outputs S1～S4.

1 the spindle speed gear outputs S0～S15 16 codes, the output is as the following

code table.

Bit 3 0 do not check the encoder resolution in DIAGNOSIS, JOG mode, display the

spindle programmed speed in JOG, AUTO mode.

1 check the encoder resolution in DIAGNOSIS, JOG mode, display the spindle

actual speed in JOG, AUTO mode.

Bit 2 0 spindle encoder pulse: 1200 pulse/r.

1 spindle encoder pulse: 1024 pulse/r.（the spindle speed is more than 120r/min，

otherwise, the system does normally execute the check.

Bit 1 selecting Z motor rotation direction.

Bit 0 selecting X motor rotation direction.

Code table of S code:

Code

Output

S00 S01 S02 S03 S04 S05 S06 S07 S08 S09 S10 S11 S12 S13 S14 S15

point

S1 ★ ★ ★ ★ ★ ★ ★ ★
S2 ★ ★ ★ ★ ★ ★ ★ ★
S3 ★ ★ ★ ★ ★ ★ ★ ★
S4 ★ ★ ★ ★ ★ ★ ★ ★

“ ”: the output of corresponding ★ bit is valid.

Note 1: By setting DIRX and DIRZ as 0 or 1, the actual rotation direction of motor can be

changed without any external tune. Ensure the moving direction of tool post is the same
that of the defined one. After rewriting the parameter of motor direction and pressing

or power on again, the direction changed is valid.

Note 2: Bit7- Bit6 are not used.

● P12 bit specifications

Bit 7 Bit 6 Bit 5 Bit 4 Bit 3 Bit 2 Bit 1 Bit 0

P12 bit specifications

Bit 7 0 machine zero return(machine reference point) function is invalid.

1 machine zero return function is valid.

Bit 6 0 Z drive unit alarm input signal（Zalm）being HIGH, the system alarm “ Z drive

60

GSK928TEⅡ Turning CNC System User Manual

alarms ”

1 Z drive unit alarm input signal（Zalm）being LOW, the system alarm “ Z

drive alarms ”

Bit 5 0 X drive unit alarm input signal（Xalm）being HIGH, the system alarm “ X drive

alarms ”

1 X drive unit alarm input signal（Xalm）being LOW, the system alarm “ X drive

alarms ”

Bit 4 0 machine zero return method one: do not check the one-turn signal.

1 machine zero return method two: check the one-turn signal.

Bit 3 0 do not output the spindle brake signal when the spindle stops.

1 output the spindle brake signal when the spindle stops. (the holding time of

brake signal is determined by P16).

Bit 2 0 starting the spindle and cooling ON/OFF is controlled by the level(controlled by

M03/04/05 M08/09 ）.

1 starting the spindle and cooling ON/OFF is controlled by the pulse(other M

signals are controlled by the level).

Bit 1 0 the tool post immediately rotates to execute the tool change after

pressed.

1 the tool post rotates to execute the tool change after

and are

pressed.

Bit 0 0 spindle speed is controlled by the switching value.

1 spindle speed is controlled by 0—10VDC analog value( frequency controlling the

spindle).

4.6.1.9 P13—Most Tools

P13 sets most tools on the tool post. GSK928TE CNC System is collocated with 4 tool Ⅱ

selections. It can be up to 6～8 tool selections when the tool selection signals are input by the
specified code.

4.6.1.10 P14—Tool Post Reversing Time

P14 sets the locking signal duration of motor reversing when the rotation tool post is executing

the tool change. Unit: 0.1 second.

Note: The value of P14 should be changed properly with the different rotation tool post. If the

parameter value is too big, the motor will easily become hot and be damaged; if the
parameter value is too small, the tool post cannot be locked tightly. So use the different
parameter values and select the proper one.

is

4.6.1.11 P15—M Code Pulse Time

P15 defines the duration of pulse signal when the spindle, the cooling, the hydraulic
chuck/tailstock are employed with the pulse control mode. Unit: 0.1 second.

4.6.1.12 P16—Brake Signal Time of Spindle

61

GSK928TEⅡ Turning CNC System User Manual

P16 defines the duration of brake signal when the brake signal of spindle is output. Unit: 0.1
second.

4.6.1.13 P17—Z Lowest Initial Speed

P17 defines Z lowest initial speed with G00 or in “Manual” mode. Unit: mm/min.
When Z actual speed n is lower than the value of P17, there is no course of Z
acceleration/deceleration The value of P17 must be tuned to the proper one according to the
actual load of machine.

4.6.1.14 P18—X Lowest Initial Speed

P18 defines X lowest initial speed with G00 or in “Manual” mode. Unit: mm/min.
When X actual speed is lower than the value of P18, there is no course of the
acceleration/deceleration. The value of P18 must be tuned to the proper one according to the
actual load of machine.

4.6.1.15 P19—Z Acceleration/Deceleration Time

P19 defines Z acceleration time from the lowest initial speed (P17) to the max. speed (P5) in
linear movement with G00 or in “Manual” mode. Unit: millisecond.
The course of Z acceleration is longer when the value of P19 is bigger. So the value of P19
should be smaller as possible to improve the efficiency according to loading characteristics.

4.6.1.16 P20—X Acceleration/Deceleration Time

P20 defines X acceleration time from the lowest initial speed (P18) to the highest speed (P6) in
linear movement with G00 or in “Manual” mode. Unit: millisecond.
The course of X acceleration is longer when the value of P20 is bigger. So the value of P20
should be smaller as possible to improve the efficiency according to loading characteristics.

4.6.1.17 P21—Initial Feedrate

P21 defines the initial speed of G01, G02, G03 and other feed commands in AUTO mode. Unit:
mm/min. There is no course of acceleration/deceleration when F speed defined by the program
is lower than the value of P21.

4.6.1.18 P22—Feed Acceleration/Deceleration Time

P21 defines the acceleration/deceleration time of G01, G02, G03 and other feed commands from

the specified speed value by P21 to 6000 mm/min in AUTO mode. Unit: millisecond.

By tuning P5, P6, P17

～

P22, this system can fit the different motors or the machine with the

different load to improve the machining efficiency.

4.6.1.19 P23—Increment of Block Numbers

P23 defines the increment value of the previous and next block number when the system
automatically generates the block number in EDIT mode, i.e. D-value between blocks.

4.6.1.20 P24—Medium Gear Speed of Spindle
P24 defines the max. speed when the converter is used to control the spindle with the medium

gear and the 10V analog output voltage of system. P24 is invalid when the spindle is controlled
by the multi-gear switching value.
Unit: r/min.

4.6.1.21 P25—Bit Parameter 3

●P25 bit specifications

62

GSK928TEⅡ Turning CNC System User Manual

Bit 7 Bit 6 Bit 5 Bit 4 Bit 3 Bit 2 Bit 1 Bit 0

Bit 7 0 decelerating to zero is valid.

1 not decelerating to zero is valid.

The parameter decides that the connection method of two commands when the
system executes continuously the block in AUTO mode. If it is set to 1, after the
previous command ends and the run decelerates to zero, the next command is
executed. If it is set to 1, it is benefit for rapid transition of the tangent between arc
and arc, between arc and linear, which can avoid the trace on the workpiece.

Bit 6 0 run override of backlash is one.

1 run override of backlash is two times.

Bit 5 0 run override of backlash is four times.

1 run override of backlash is eight times.

Execution speed of backlash =lowest initial speed × (P25 Bit6) × (P25 Bit5).

P25d6/P25d5 can divide the multiple: 1, 2, 4, 8; the stepper motor should not
more than 1.
The stepper motor should not more than 1. the servo motor can be adjusted
according to the actual load.

Bit 4 0 the hydraulic chuck/tailstock control signal is LOW.

1 the hydraulic chuck/tailstock control signal is pulse. The pulse width is determined

by P15.

Bit 3 0 the hydraulic chuck control needs to check the clamp/release in-position signal.

1 the hydraulic chuck control does not check the clamp/release in-position signal.

Bit 2 0 the chuck clamp mode is outer.

1 the chuck clamp mode is inner.(clamp, release signal output is opposite to the

outer mode.)

Bit 1 0 the hydraulic chuck function is invalid.

1 the hydraulic chuck function is valid.

Bit 0 0 the hydraulic tailstock function is invalid.

1 the hydraulic tailstock function is valid.

4.6.1.22 P26—Bit Parameter 4

●P26 Bit specifications

Unused Unused Unused Unused Bit 3 Bit 2 Bit 1 Bit 0

Bit 3 0 do not set the position again. The system automatically check whether the current

coordinates are same that of the defined by G50.

1 automatically set the position again. The system does not return to the initial point

of program, and directly modifies the current position into the ones defined by G50.
The parameter determines G50 mode in AUTO mode. P26 Bit3=1, the system
does not response the corresponding prompt, and directly modifies the current
coordinates into the ones defined by G50 to execute the next block.

Bit 2 0 limit alarm deceleration.

1 limit alarm emergency stop.

63

GSK928TEⅡ Turning CNC System User Manual

r

D

The parameter specifies which method is used when the system runs upon the

hard limit. When it is set to 0, the system alarms and the motion axis decelerates
because the system runs upon the hard limit; when it is set to 1, the system
alarms and the motion axis stops suddenly and the coordinates are not same that
of the actual position because the system runs upon the hard limit.

Bit 1 0 automatic controllable spindle.

1 automatic uncontrollable spindle.

The system determines whether the spindle control is operated by pressing key in

AUTO mode.

Bit 0 0 spindle speed smoothness is invalid.

1 spindle speed smoothness is valid.

The parameter is used for thread cutting. Generally, when it is set to 0, it is benefit for

the system to trace the spindle speed. But with the extreme low speed to cut the
thread with extreme big pitch, it is set to 1, which is benefit to the stepper motor stably
running.

4.6.1.23 Parameter P27～P30

P27 — Z multiple indicating Z electric gear numerator.（1～255）
P28 — Z division indicating Z electric gear denominator.（1～255）
P29 — X multiple indicating X electric gear numerator.（1～255））
P30 — X division indicating X electric gear denominator.（1～255）

When the electric gear function is used with the different input and output unit, and the
backlash is measured by the system coordinate changing, the backlash can be input directly.
When the backlash is measured by the percentage form, the measured value should multiplex
the reciprocal of electric gear ratio. The coordinates of the trial-cutting toolsetting is also done so.

For example: Z electric gear ratio is 1:2, the measured Z dimension is 15mm, the input should be
KX2=30.

When the system uses the electric gear function, its max. speed and the output resolution will be
changed. When the electric gear numerator is more than its denominator, the permitted max.
speed will be reduced. Along with the electric gear ratio value changing, however the
relationship must be as follows:

The resolution output by the system is inverse proportion of the electric gear ratio value. The
bigger the electric gear ratio value, the smaller the system resolution is. Otherwise, the smaller
the electric gear ratio value is, the higher the resolution is.
To get the precise positioning and speed indicators, it is recommended that the electric gear ratio
is set to 1:1 and the actual electric gear ratio is set in the servo drive.
When the system is matched with the stepper drive, it is recommended that the drive unit with the
stepper division function is used, and as possible, the electric gear ratio is 1: 1 to avoid that the
difference between the numerator and denominator.

Numerator

eno

min

× F ≤ 15000

ato

Parameter list as follows:

64

GSK928TEⅡ Turning CNC System User Manual

No. Definition Unit Initial value

P01 Z positive limit value mm 8000.000

P02 Z negative limit value mm -8000.000

P03 X positive limit value mm 8000.000

P04 X negative limit value mm -8000.000

P05 Z max. traverse speed mm 6000

P06 X max. traverse speed mm 6000

P07 Z backlash mm 00.000

P08 X backlash mm 00.000

P09 Spindle low gear speed r/min 1000

P10 Spindle high gear speed r/min 3000

P11 Bit parameter 1 00000000

P12 Bit parameter 2 00000000

P13 Most tool 4

P14 Tool post CW time 0.1s 10

P15 M code time 0.1s 10

P16 Spindle brake time 0.1s 10

P17 Z lowest initial speed mm/min 50 / 150

P18 X lowest initial speed mm/min 50 / 150

P19 Z acceleration time ms 600 / 300

P20 X acceleration time ms 600 / 300

P21 Initial speed of cutting feed mm/min 50 / 100

P22 Acceleration/deceleration time of cutting feed ms 600 / 400

P23 Increment of block numbers 10

P24 Spindle middle gear speed r/min 2000

P25 Bit parameter 3 00000000

P26 Bit parameter 4 00000000

P27 Z multiple 1

P28 Z division 1

P29 X multiple 1

P30 X division 1

0～8000.000

-8000.000～0

0～8000.000

-8000.000～0

8～15000

8～15000

0～10.000

0～10.000

0～9999

0～9999

0～11111111

0～11111111

1～8

1～255

1～255

1～255

8～9999

8～9999

8～9999

8～9999

8～9999

8～9999

1～255

0～9999

0～11111111

0～11111111

1～255

1～255

1～255

1～255

Range

4.6.2 Parameter Input

The parameters are rewritten and tuned according to the actual condition of machine after being

installed on the machine although they are initialized before delivery.

Operations of inputting parameter content are as follows:

The first input:

z Select the parameter setting mode.

z Press to move the cursor to the parameter number in highlight to the required

one (displaying the selected parameter name in English in the below of screen at the same

65

GSK928TEⅡ Turning CNC System User Manual

time). Press to display the highlight.

z Input the parameter by keyboard. Press

to delete the wrong input value and input

it again.

● Press

to confirm the input.

Example ：rewrite the value of P05 to 4500 as Fig. 22.

Note

：

The inputting characters are more than 8 numbers（containing the decimal point without

）

the sign

.

The second input:

● Move the curse to the required parameter number, input directly the data to press

to complete the parameter modification.

Example ：rewrite the value of P05 to 4500 as Fig. 22.

：

Note

The inputting characters are more than 8 numbers（containing the decimal point without

）

the sign

.

or

Fig. 22 Parameter content input

● Press

● Press

to display the highlight.

to move the cursor in highlight to P05.

● Input 4 5 0 0 by keyboard.

● Press ，and the value of P05 is rewritten to 4500.

：

Note 1

66

Press to cancel the wrong input and input again.

GSK928TEⅡ Turning CNC System User Manual

Note 2

：

The input is invalid and the parameter content will not be changed if the input exceeds

the specified range.

Note 3：Press after inputting the data, and the input is invalid.

：

Note 4

“00” cannot be added to the ahead of it when max. tool number (the initial value is 004)

of P13 is rewritten and its units digit is directly input. Directly input “6” not to input “006” if
the tool number is rewritten to 6 on the tool post.

4.6.3 Parameter Initialization

When this system is switched on for the first time or the parameters are disordered, the
parameters must be initialized to make the parameters become the default value.

Initialize the parameters as follows:

1. The specific procedures of 928TEⅡ initialization:

● press simultaneously

● firstly release

.

and .

● then release

.

● appear：

1. CNC PAR P01—P26 DY3

2. CNC PAR P01—P26 DA98

3. CLEAR PRO %00—%99

4. DEBUG

5. COPY FLASH 29C010

0. ESC PLEASE INPUT

Pressing 1: system parameter initialization of optional stepper drive unit.
Pressing 2: system parameter initialization of optional servo drive unit.
Pressing 3: deleting all part programs.
Pressing 4: entering the system menu.
Pressing 5: FLASH chip copy and check.
Pressing 0: escape the system edit menu.

Note: After the system is initialized, it must return to EDIT mode to select the program again if it

needs to run automatically, otherwise it cannot execute the program and will alarm.

4.6.4 Searching and Modifying Each Bit Definition of Bit Parameter

To convenient operations, the definition of each digit of bit parameter can be displayed on the

screen in English and its content can be directly modified.

Press①

to move the cursor to the bit parameter P11 or P12.

After pressing②

67

,the most significant bit(MSB) of selected parameter is displayed in

GSK928TEⅡ Turning CNC System User Manual

highlight with its definition in English below the screen.

Press③

to move the cursor right or left to select the different bit, and the

definition of selected bit will be changed along.

After pressing ④

cursor still points to the previous bit parameter. Press

, if is pressed, the system escapes from the bit search but the

, and the system
escapes from the bit search but the cursor still points to the previous or the next bit
parameter.

Press the number key 0 or 1 to directly modify the value pointed by the cursor into 0 or 1 ⑤

when the cursor is pointing some bit. Press

, , and the

input value is valid. Press at the moment, the system will not save the input value and

the input operation is invalid.

68

GSK928TEⅡ Turning CNC System User Manual

4.7 Tool Offset Setting Mode

This system can define 8 groups tool offset value ( T1～T8). Each group offset has two data in X,
Z direction. The offset group amount automatically generated by manual toolsetting is the same
as the used tool ones. Other offset data must be input by keyboard. No. 9 offset value is the
coordinate setting value after executing the machine zero return (machine home return). Do not
use T*9 in the command, otherwise the system alarms “PARAMETER ERROR”.

Select

Fig. 23 Offset mode

4.7.1 Searching a Tool Offset Value

The particular content of each offset value can be viewed in OFFSET mode. Press or

to enter the offset setting mode as Fig. 23:

to search the pervious or the next offset value. Press or to search the

offset value of page up or page down, and 9 blocks offset value in each page are displayed.

4.7.2 Inputting a Tool Offset by Keyboard

Input the offset by keyboard：absolute and incremental input

Absolute input of offset

● Select the offset setting mode.

● Press

selected offset number is displayed under the screen when moving the cursor).

● The highlight square behind the offset number is displayed on the screen by pressing

● Input the offset value by keyboard. Press

again.

69

to move the cursor in highlight to the offset number to be modified (the

to cancel the wrong input value and input

.

GSK928TEⅡ Turning CNC System User Manual

● Press to confirm the input，and store it into the parameter area of current selected offset

number.

Incremental input of offset data

● Select the offset setting mode.

● Press

to move the cursor in highlight to the offset number to be modified (the
selected offset number is displayed under the screen at the same time when moving the
cursor).

●The highlight square behind the offset number is displayed on screen by pressing

●Input the data by keyboard. Press

to cancel the wrong input and input again. Press

to count the input value and the previous value of selected parameter. If the input
value is positive, the system adds the input value to the previous value and saves the sum
automatically. If the input value is negative, the system reduces the input value from the
previous value and saves the remaining value automatically.

4.8 Diagnosis

This system has the self-diagnosis function, displaying the state of external input/output interface
signal, the spindle speed and so on.

Press

to enter DIAGNOSIS mode as Fig. 24:

.

Fig. 24 Diagnosis mode

Note: If the P11 Bit3 is 0 (do not detect the spindle encoder), the encoder lines in Fig. 24 will

not be displayed. When the system is not equipped with the spindle encoder or the
spindle stops, Encode lines=0000 is displayed. Press the other mode keys to escape
from the display.

4.8.1 Diagnosis Definition of Input Interface

Input 1：

70

Input 2：

GSK928TEⅡ Turning CNC System User Manual

Signal name Input interface diagnosis

ALZ Z drive unit alarm

ALX X drive unit alarm

UI2 No. 2 user input

UI1 No. 1 user input

-LT X, Z negative travel limit

LT X, Z positive travel limit

PCZ Z zero

PCX X zero

A14 G31 check skip

Signal name Input interface diagnosis

DEZ Z deceleration zero

DEX X deceleration zero

SHL Hydraulic chuck pedal switch

TPS Hydraulic tailstock pedal switch

T4 No. 4 tool

T3 No. 3 tool

T2 No. 2 tool

T1 No. 1 tool

A15 Reserved

Note 1: In the display of input interface diagnosis, the corresponding bit is 0 when the external

signal is valid; the corresponding bit is 1 when the external signal is invalid.

Note 2: The signal diagnosis of input interface is circularly executed at the time, and the state of

current signal is displayed anytime.

Note 3: Press any keys to escape from DIAGNOSIS mode into another one.
Note 4: The rotation tool post of GSK928TEII CNC System is equipped with 4 tool selections,

which can expand to 6
T5-T8 codes are as follows:

T5=T1+T3 T6=T2+T3 T7=T1+T2

～

8 ones according to the special code mode. At the moment,

（

See Connection）

T8=T1+T4

4.8.2 Diagnosis Definition of Output Interface

Definitions of output diagnosis are as follows(sequence from left to right D7—D0):

Output 1：

71

GSK928TEⅡ Turning CNC System User Manual

Signal name Output interface diagnosis

TZL Tool post CCW

TFL Tool post CW

M03 Spindle CCW

M04 Spindle CW

M05 Spindle stop

M08 Cooling ON

M09/M79 Cooling OFF

MSP Spindle brake

A01 Alarm lamp red

Output 2：

Signal name Output interface diagnosis

M10 Workpiece clamped

S04 No. 4 gear spindle speed

M11 Workpiece released

S03 No. 3 gear spindle speed

U02/M78 No. 2 user output

S02 No. 2 gear spindle speed

U01 No. 1 user output

S01 No. 1 gear spindle speed

A02 Alarm lamp green

Note 1: The corresponding bit output is valid if each bit of output interface diagnosis is 1. When

the bit is 0, the corresponding bit output is invalid.

Note 2: The output interface diagnosis is displayed to the hold state of current each output bit. If

the signal is the pulse mode, the bit is displayed to 0 although its output is valid.

Note 3: Press the mode selection key to enter another mode.

4.8.3 Encoder — Spindle Encoder ands Spindle Rotating Test

If P11 Bit3 is set to 1, this system can detect and display the pulse/rev of spindle encoder, and
automatically set the encoder LINE Bit of P11 according to the detection after entering
DIAGNOSIS mode as Fig. 24. The spindle speed is the current actual speed. Unit: r/min.
The encoder lines are the pulse/rev.
z P11 Bit3 determines whether the system detects and displays the encoder lines in

DIAGNOSIS mode.

z The encoder diagnosis can display the actual value when the spindle encoder is installed

and the spindle is started, otherwise the system prompts: 0000.

z The spindle encoder rotates with the spindle synchronously, i.e. the encoder also rotates

one circle when the spindle rotates one circle, otherwise the detected spindle speed is not
coincident with the actual one.

In “Manual” mode, the spindle encoder lines are detected, but LINE bit of P11 cannot be set

72

GSK928TEⅡ Turning CNC System User Manual

automatically. Press

, the system starts to detect and display the spindle encoder
lines. The course of detection will be circularly executed at the time before pressing the
other keys to escape from the detection.

z Automatic detecting function of spindle encoder lines

When “Diagnosis spindle encoder” of P11 bit parameter is set to “1”, the system will
automatically detect the spindle encoder lines in “DIAGNOSIS” mode and automatically set
“Encoder lines ” of P11 bit parameter.

When the detected encoder lines are 1200, “encoder lines ” of P11 bit parameter is

automatically set to “0”.

When the detected encoder lines are 1024, “encoder lines ” of P11 bit parameter is

automatically set to “1”.

When the encoder lines detected are not 1024/1200, the bit parameter will not be changed.

4.8.4 Auxiliary Function Control of Machine

In DIAGNOSIS mode, the system can execute the auxiliary function of machine by pressing the

auxiliary function keys on the operator panel instead of inputting commands.

After

is pressed, the spindle rotates counterclockwise, LED is ON, the corresponding

bit of M3 in output 1 is 1 and that of M5 is 0.

After

is pressed, the spindle stops, LED is OFF, the corresponding bit of M3/M4 in output

1 is 0 and that of M5 is 1.

After

is pressed, the spindle rotates clockwise, LED is ON, the corresponding bit of M4

in output 1 is 1 and that of M5 is 0.

After

is pressed, the cooling ON/OFF is switched. When the cooling is ON, LED is ON,
the corresponding bit of M8 in output 1 is 1 and that of M9 is 0; when the cooling is OFF, LED is
OFF, the corresponding bit of M8 in output 1 is 0 and one of M9 is 1.

After
corresponding bit of S1

After
displayed in the corresponding bit of T4

is pressed, the spindle motor rotates circularly in S1～S4 or S0～S15 and the

～S4 in output 2 can be displayed accordingly.

is pressed, the tool post rotates to the next controllable tool and the tool state is

～T1 in input 1.

73

GSK928TEⅡ Turning CNC System User Manual

4.9 Alarm of Emergency Stop and Overtravel

There is an integrated safeguard in this GSK928TE II CNC System to guard the operator’s safety
and protect the machine from being damaged.

4.9.1 Emergency Stop

There is an input terminal of external emergency stop in the input interface. User should connect

Normally-closed contact of red mushroom emergency stop switch on the operator panel with the
input terminal of emergency stop. After Emergency stop switch is pressed in the state of
emergency, the system will be in the state of emergency stop and stop all feeds, the spindle, and
the cooling. The screen flashes as Fig. 25.

Fig. 25 Emergency stop alarm

After releasing the emergency switch, rotates it clockwise in the direction of its upper arrowhead
until automatically releasing. The system will escape from the state of emergence stop and
return to the previous mode by pressing any keys of the system keyboard. If there is not the
external emergency button, it should connect the input terminal of emergency stop with 0V,
otherwise this system cannot run normally.

After releasing the emergency switch, rotates it clockwise in the direction of its upper arrowhead
until automatically releasing. The system will escape from the state of emergence stop and
return to the previous mode by pressing any keys of the system keyboard.
If there is not the external emergency button, it should connect the input terminal of emergency
stop with 0V, otherwise this system cannot run normally.

4.9.2 Overtravel Switch Alarm

This system can detect it if the overtravel switch is installed on the machine. When the traversing

slider presses down the switch, the auxiliary functions do not stop, but feeds and programs stop,
displaying the overtravel alarm signal of the corresponding axis on the top right corner on the
screen.
After the overtravel switch alarms, select the manual mode and press the feed key opposite to
the limit direction, which make the system can escape from the overtravel and its alarm can
automatically disappear.

4.9.3 Drive Unit Alarm

When the alarm output signal of drive unit is transmitted to CNC system and the drive unit alarms,

this system automatically stops all feeds, displaying X Drive Unit Alarm or Z Drive Unit Alarm

on the top right corner. Program stop and close all output signals. At the moment, check the drive
unit and other devices to troubleshooting, and then turn on again.

74

GSK928TEⅡ Turning CNC System User Manual

4.9.4 Other Alarms

When there are other alarms, the system will prompt in English on the screen. Please deal with
them correspondingly according to the prompt and the troubleshooting in the manual.

4.10 Drive Unit Switch Control

In all non-running states, after pressing continuously twice, the drive unit is closed and the

motor is released. After pressing
the motor is locked (the drive unit switch function is invalid when the content of program is edit).

75

once in the state of its close, the drive unit is open and

GSK928TEⅡ Turning CNC System User Manual

Programming

Chapter 1 Programming Fundamentals

The automatic machining of CNC machine is the course of edited part programs automatically
running. The programming is defined that the drawing and the technology of machining workpiece
are described with CNC language and are edited to the part programs.
Here describes the definition of command and the programming mode of CNC part programs.
Please read carefully these contents before programming.

1.1 Coordinate Axis and its Direction

This system has defined the controlled axis and its motion according to GB/T 19660—2005/ISO

841 ： 2001 Industrial Automation System and Integration-Numerical Control of
Machines-Coordinate System and Motion Nomenclature. The two coordinate axes are

named with X and Z, which are perpendicular each other to form X—Z plane rectangular
coordinate system as Fig. 1.

Ｏ

Ｘ

Fig. 1 X—Z plane rectangular coordinate system

X：It is defined to be perpendicular with the rotary centerline of spindle. X positive direction is the

one that the tool leaves from the rotary center of spindle.

Z：It is defined to be coincident with the rotary centerline of spindle and Z positive direction is the

one that the tool leaves from the headstock.

1.2 Machine Zero

The reference point is a fixed point on the machine. Generally, it is set at the position of X, Z max.
stroke, the machine zero signal and the stopper are installed here. If the system is not equipped
with the machine zero signal and the stopper, please do not use this function, or set P12 Bit7 to

0.

Ｚ

1.3 Programming Coordinate

The absolute coordinates (X, Z word), the incremental coordinates(relative coordinates) (U, W
word) or the compound coordinates (X/W, U/Z word) can be applied to the programming in the

76

GSK928TEⅡ Turning CNC System User Manual

system.
For X axis, the system adopts the diameter programming (the dimension and the parameter in X
direction are described in diameter).

1.3.1 Absolute Coordinate Values

The absolute coordinate value is the distance to the coordinate origin, i.e. it is the coordinate

value of the tool traversing to the end point as Fig. 2:

Fig. 2 Absolute coordinate value

The commands of the tool traversing from A point to B point uses B point coordinate values as follows:
X 50 Z 70.

1.3.2 Incremental Coordinate Value

The incremental coordinate value is the distance from the previous position to the next one, i.e.

the actual moving distance of tool as Fig. 3:

Fig. 3 Incremental coordinate value

The commands of tool traversing from A to B with the incremental coordinate are as follows: U

-30 W -40 (X with diameter programming)

1.3.3 Compound Coordinate Value

The incremental coordinates and the absolute coordinates can be applied at the same time, but

one coordinate axis in one block can only be defined by one method, i.e. X , W or U , Z can be

77

GSK928TEⅡ Turning CNC System User Manual

applied, but the X ,U or Z ,W cannot be applied. For example, traverse the tool from A point to B

point as Fig. 3, X axis is applied with the absolute coordinates and Z axis with the incremental

coordinates as: X 5 0 W -4 0.

1.4 Workpiece Coordinate System

The workpiece coordinate system is defined that some point on the workpiece is considered as

the coordinate origin to create the coordinate system. Its axes are separately parallel with X, Z
axis in the same direction.

After the workpiece coordinates is created, all absolute coordinate values in programming are the

position values in the workpiece coordinate system. Generally, Z workpiece coordinate system is
set on the rotating centerline of workpiece.

According to the actual condition in programming, define the workpiece coordinate zero, i.e. the

programming home in the workpiece drawing and the coordinate origin of CNC system command.
The workpiece coordinate system is created by setting a workpiece coordinate.

1.5 Reference Point

The reference point set by the operator is at a safe and convenient position. Any position can be

set to the reference point but it is generally set at the safe position.

Once the reference point is defined, the tool can return to the reference point by executing the
reference point return function in “Manual” or AUTO mode. Even if the system is switched off, the
reference point still exists. If the stepper motor is employed, there is slight error caused by the
motor vibrating after the system is switched on again. Execute the reference point return again to
avoid the error.

The reference point is automatically set to X=150, Z=150 without setting the reference point after
the system is switched on firstly.

78

GSK928TEⅡ Turning CNC System User Manual

T

Chapter 2 Program Structure

CNC command set edited according to the requirement of machine moving is named as program.

According to the sequence of command, the tool traverses along the straight line and the circular
arc, or the spindle starts/stops, cooling is ON/OFF. The sequence of command is edited
according to the technology requirement of workpiece.

2.1 Character

Character is the basic unit to compose the program. The character includes English letters, digits

and other signs.

z 17 English letters are the address character of each command or data：D E F G I K L

M N P R S T U W X Z

z Digit is the specific data of each address character： ０，１，２，３，４，５，６，７，８，

９

z Sign：% — .

% ：the start sign of program number
—：negative data
. ：decimal point

Address character definitions and data ranges are as follows:

Address

character

% Program number

N Block number Block number 0000～9999（integer）
G Preparatory function Command run mode 00～99（integer）
M Auxiliary function Auxiliary operation command 00～99（integer）

T Tool function

S Spindle speed function Spindle speed command

F Feed function Feedrate mm/min 0～9999（integer）

X Z Absolute coordinates X, Z absolute coordinate value mm -8000.000～+8000.000

U W

I K

R

E Thread lead Inch thread lead Tooth/inch 100～0.25 tooth/inch

D Dwell time Dwell command 0.001ｓ 0.001～65.535

P

L Compound address

Function Specification Unit Range

Incremental
coordinates
Coordinates of circle
center
Arc radius or taper of
canned cycle

hread lead, entrance

of block

Program number of machining
workpiece

Tool number and compensation
number

X, Z incremental coordinates value mm -8000.000～+8000.000

X, Z circle center coordinate relative
to the starting point of arc

Radius of arc or cycle taper

Metric thread lead or calling the skip

command

Cycle amount, thread leads and
contour blocks in cycle

00～99（integer）

00～89（integer）

0～4 （multi-gear speed motor）
0～15
0～P11/12（frequency conversion
control）

mm -8000.000～+8000.000

mm

1～99

Radius 0～4199.000

0.25～100(thread lead)
0000～9999(integer)

2.2 Word

A word consists of an address character and the following numerical command. For example:

N000 12.8 W-23.45 and so on.

z Each word must have an address character (English letter) and the following number

character string.

79

Programming Chapter Three Commands and Functions

z The invalid 0 of digital character string can be omitted.
z The leading zero of command can be omitted. For example: G00 can be written to G0.
z The positive sign can be omitted, but the negative sign must not be omitted.

2.3 Block Number

A block number consists of the letter N and the following 4-digit integer. It can be automatically

generated by the system and be modified in EDIT mode. The range is 0000-9999.

2.4 Block

A block consists of a block number and words. One block can contain 255 characters at most

(including space between words). It is necessary to have the block number generated
automatically by the system and can be modified in EDIT mode.

N0120 G1 X130 W-40 F50 Enter

z N0120 Block number
z G1 Preparatory function
z X130 W-40 Motion data
z F50 Motion speed

z Enter End of block by pressing

Note 1: Each word of block is separated with the space generated automatically by the system,

but it is necessary to input the space manually by user when this system cannot
distinguish the words.

Note 2: The word can be placed on any position in a block.

without being displayed on the screen.

2.5 Program Structure

A block consists of commands arraying of one or several technology operations in the course of

machining. A part program consists of some blocks according to the machining technology
orderly. A block number (line number) is used for identifying blocks. A program name (or file
name) is used for identifying programs.

Each part program consists of one program number and blocks. A program contains 9999 blocks

at most. A block number is composed of N and the following 4-digit integer. A program number is
comprised of % and the following 2-digit integer.

80

GSK928TEⅡ Turning CNC System User Manual

Chapter 3 Commands and their Functions

Here describes the function and the specification of all commands of GSK928TE CNC System.Ⅱ

3.1 G commands — Preparatory Function

G commands are defined as the run mode of machine, composed of the character G and the

following 2-digit as the following table. G commands of GSK928TEII CNC System are as follows:

Command Function Modal Programming format Remark

G00 Rapid traverse movement

G01 Linear interpolation * G01 X(U) Z(W) F

G02 Circular interpolation (CW) *

G03 Circular interpolation (CCW) *

G33 Thread cutting * G33 X(U) Z(W) P(E) I K

G32 Tapping cycle G32 Z P(E)

G90 Inner and outer surface turning cycle * G90 X(U) Z(W) R F

G92 Thread cutting cycle *

G94 Outer and inner face (taper) cycle * G94 X(U) Z(W) R F

G74 Deep hole machining cycle on face G74 X(U) Z(W) I K E F

G75 Grooving cycle G75 X(U) Z(W) I K E F

G71 Outer roughing cycle G71 X I K F L

G72 Face roughing cycle G72 Z I K F L

G22 Part cycle start G22 L

G80 Part cycle end G80

G50 Create workpiece absolute coordinate system G50 X Z

G26 X, Z reference point return G26

G27 X reference point return G27

G29 Z reference point return G29

G31 Skip function G31 X(U) Z(W) F

G04 Dwell G04 D

G93 System offset G93 X（U） Z（W）
G98 Feed per minute * G98 F 1～6000 mm /min

G99 Feed per rev G99 F

Initial

state

G00 X(U)Z(W)

G02 X(U) Z(W) R F
G02 X(U) Z(W)I K F

G03 X(U) Z(W)R F
G03 X(U) Z(W)I K F

G92 X(U) Z(W) P(E) L I
K R

F:5-6000 mm
/min
F:5-3000 mm
/min

F:5-3000 mm
/min

Rapid traverse

in G00

Rapid traverse

in G00

Rapid traverse

in G00

0.01 ～ 99.99 mm
/rev

Note 1: The commands with * in above-mentioned table are the modal one which are still valid

even if the other G commands are not specified.

Note 2: Each block can have only one G command (Only G04 command can be applied with the

other G commands in one block).

Note 3: It is in G00 or G98 when the system powers on or resets.

3.1.1 G00 — Rapid Traverse Movement(Positioning)

Command format：G00 X（U） Z（W）

81

Programming Chapter Three Commands and Functions

The tool rapid traverses to the specified position with G00.

G00 X（U） Z（W） are the coordinate value of the specified point.

Fig. 4 G00 rapid traverse

Example：Traverse from A to B with G00 as Fig. 4：
Absolute programming:
N0010 G00 X18 Z0 ；
Incremental programming:
N0100 G00 U52 W-30；
When X and Z axis are commanded with G00, they traverse separately at max. rapid traverse
speed and the acceleration at the same time. One of them will not stop automatically until it
reaches the command position. The system will add the compensation value to G00 traverse
value to execute the operation to improve the working efficiency when the tool change command,
the tool compensation command and G00 are in the same block. So ensure the tool change
command and G00 are in the same block as possible when executing the tool change and the
compensation.
G00 can define separately X or Z.
The traverse speed in G00 is set by P05/06 and controlled by the rapid traverse override.

X actual rapid traverse speed = P05 ×rapid traverse override

Z actual rapid traverse speed = P06 ×rapid traverse override

The actual max. speed of machine is defined by its actual condition and matched motor. For
particular parameters, please see the manual from machine manufacture. `

G00 is the modal command and can be omitted in the next same block.
G00 can be omitted to G0, and G0 and G00 are equivalent.

Note: Ensure the tool is placed on the safe position to avoid the tools shocking each other when

X, Z move at the same time.

3.1.2 G01 — Linear Interpolation

Command format: G01 X（U） Z（W） F ；

The tool traverses at the specified feedrate by G01 from the current point to the specified point

X(U),Z(W).

X(U) Z(W) are the specified end point coordinates.

F-feedrate． Unit：mm / min

82

GSK928TEⅡ Turning CNC System User Manual

Fig. 5 G01 linear interpolation

Traverse from A to B with G01 and its speed is 150 mm/min as Fig. 5.

Absolute programming:
N0100 G01 X45 Z-35 F150 ；
Incremental programming:
N0100 G01 U25 W-35 F150 ；

G01 can define separately the motion of X or Z.
The feedrate with G01 is specified by F and controlled by the feedrate override. F value is modal
and can be omitted when it is not changed.
Actual feedrate = F × feedrate override
G01 is the modal command and can be omitted in the next block.

G01 can be omitted to G1, and G1 and G01 are equivalent.

3.1.3 G02 G03 — Circular Interpolation

Command format: G02 X(U) Z(W) I K F ; Programming with the center coordinate

G03 X(U) Z(W) I K F ;

or G02 X(U) Z(W) R F ;Programming with radius

G03 X(U) Z(W) R F ;

Words:

Word Specified content Specification
G02 Rotation direction Clockwise arc CW
G03 Rotation direction Counterclockwise arc CCW
X, Z Absolute coordinate Absolute coordinate value of arc end point
U, W Incremental coordinate Distance of arc from the starting point to the end

point
I, K Circle center coordinate Distance from the circle center to the starting point.
R Radius of arc Distance from any point on the arc to the circle

center

F Feedrate Feedrate along the arc

The tool can traverse along the specified arc path at the defined feedrate by G02, G03. G02 is
for the clockwise arc and G03 is for the counterclockwise. The arc direction is defined by

considering the circle center as the reference point: G02: clockwise arc; G03:

counterclockwise arc.

See Fig. 6：

83

Programming Chapter Three Commands and Functions

A

A

Fig. 6a G2/G03 Z negative direction Fig. 6b G02/G03 Z positive direction
X, Z or U, W defines the end point of arc. It can be described with the absolute or the incremental
coordinates. The incremental coordinate is the distance from the starting point to the end point of
arc.
I, K define the center coordinates: I, K separately correspond to X, Z coordinates, and are the
vector of starting point as the origin pointing to the circle center. It is X component (with diameter)
and K is Z vector. The direction of I, K is the positive /negative when it is the same time as X, Z
positive/negative direction as Fig. 7:

G02 X..Z..I..K..F..；

Or
G02 X..Z..R..F..；

bsolute coordinate value）

（

（ Diameter programming）

Arc center

R

I

G03 X..Z..I..K..F..；

Or
G03 X..Z..R..F..；

（

bsolute coordinate value）

（Diameter programming）

X

Z

Z

X

K

Z

Arc center

R

X

K

I

Z

X

Fig. 7 Circle center coordinates

I value is the diameter. Generally, the counted value of drawing is the radius which must be

multiplied 2 in programming. Use R to program without I, K.

The feedrate of clockwise interpolation from A to B is 100 mm/min as Fig. 8:：

N0100 G00 X20 Z60 ; Rapidly positioning to the starting point

of arc machining

84

GSK928TEⅡ Turning CNC System User Manual

N0110 G02 X60 Z40 I0 K-20 F100 ；Circle center programming.
N0110 G02 X60 Z40 R20 F100 ；Radius programming

or N0110 G02 U40 W-20 I0 K-20 F100 ；
N0110 G02 U40 W-20 R20 F100 ；

The feedrate of the counterclockwise interpolation from A to B is 100 mm/min.

N0100 G00 X20 Z60 ；Rapidly positioning to the starting point

of arc machining

N0110 G03 X60 Z40 I40 K0 F100 ；Circle center programming.
N0110 G03 X60 Z40 R20 F100 ；Radius programming.

or N0110 G03 U40 W-20 I40 K0 F100 ；

N0110 G03 U40 W-20 R20 F100 ;

Note 1: Max. R is not more than 4199 mm, otherwise the system cannot ensure its value is

right.

Note 2: the system will test whether the current coordinates (starting point), the end point

coordinates and the center coordinates are right when it adopts K

, I to execute the

programming. If the end point is not on the arc, and Z error will be more than 0.05 mm
or that of X will be more than 0.1 mm, the system alarms: “INCOMPATIBLE DATA”.
When the arc from the starting point to the end point is more than 180

°, the system

alarm :“OVERTRAVEL”.

Note 3: When the system adopts R programming and 2R is less than the distance from the

current point to the end point, otherwise the system alarms: “INCOMPATIBLE DATA”.

Programming example：

Absolute programming：
N0000 G0 X18 Z0 ；
N0010 G03 X30 Z-15 R20 F100 ；

Incremental programming：
N0000 G0 X18 Z0 ；
N0010 G03 U12 W-15 R20 F100 ；

3.1.4 G33 — Thread Cutting

Command format： G33 X (U)_ Z (W)_ P (E)_ K_ I_ D_；

X (U) Z (W)——absolute/incremental coordinate of thread end point( when X is omitted, it is the

straight thread).

P——metric thread lead. Unit: mm Range：0.25-100 mm

E——inch thread lead. Unit: tooth/inch Range：100-0.25 tooth／inch

K——X distance from the starting point to the end point of thread run-out. Unit: mm. When K is

omitted, do not execute the thread run-out.

When the straight thread K＞0 in machining and the thread run-out is being executed, X
positively moves; when K＜0 and the thread run-out is being executed, X negatively moves.
The sign of K in machining must be the same as X moving direction.

85

Programming Chapter Three Commands and Functions

I——it is X moving distance(diameter value) when executing the thread run-out. Unit: mm. When

there is K and I is omitted, the system defaults I=2×K( 45° thread run-out) and I is not

negative.

D ——rotary machining depth.（unit: mm ）

When G04 is with others, D is the delay time. When there is no K, there is no D, otherwise,

the system prompts “ILLEGAL PARAMETER”. K=0, I, D are invalid. When the taper

thread is machined, rotary machining cannot be used, i.e. there is no D, otherwise the

system prompts “ILLEGAL PARAMETER”.

The metric/inch straight thread, taper thread, inner and outer thread can be machined by G33.
When X（U）are not zero in G33, the taper thread is machined. When the spindle rotates

clockwise, the right-hand thread is cut positively and the left-hand thread is cut negatively.
When the spindle rotates counterclockwise, they are opposite.

Fig. 9 G33 thread cutting

1. G33 axial straight thread is as Fi.g 9-1

Starting point

End point

K sign decides the direction of the thread run-out; there is no the thread run-out when K is
omitted; when there is no I, I=2K.
For example：G00 Z100 X100； G33 W-40 K3 I5 P2；end point (Z60，X105)

2. G33 axial rotary machining straight thread: as Fig. 9-2.

End point

Starting point

K sign decides the direction of the rotary machining and the thread run-out; K cannot be omitted;
when there is no I, I=2K.

Example：G00 Z100 X100；

86

GSK928TEⅡ Turning CNC System User Manual

G33 W-40 K3 I5 D4.4 P2；

End point (Z60，X100.60)

3. G33 axial taper thread：(≤45°，U/2≤W) as Fig. 9-3

Starting point

End point

U sign decides the direction of the thread run-out; K sign is invalid; the machining cannot execute the
rotary machining; when there is no I, I=2K.

Example：G00 Z100 X20；

G33 W-40 K3 I5 U6.2 P2；

End point (Z60，X31.20)

3. G33 end face thread：(>45°，U/2>W) as Fig. 9-4

Starting point

End point

W sign decides the direction of thread run-out; K sign is invalid; the machining is rotary machine;

when there is no I, I=K/2.
Example：G00 Z100 X20；

G33 W-8.3 K3 I1.6 U20.7 P2；

End point (Z90.10，X40.70)

5. G33 end face straight thread: as Fig. 9-5.

87

Programming Chapter Three Commands and Functions

Starting point

End point

K sign decide the direction of the thread run-out; when K is omitted, there is no the thread run-out;
when there is no I, I=K/2.

Example：G00 Z100 X20；

G33 K3 I1.6 U20.7 P2；

End point (Z101.60，X40.70)

6. G33 end face rotary machining thread: as Fig. 9-6

Starting point

End point

K sign decide the direction of the thread run-out; when K is omitted, there is no the thread run-out;
when there is no I, I=K/2.

Example：G00 Z100 X20；

G33 K3 I1.6 D1.8 U20.7 P2；

End point (Z99.80，X40.70)

Generally, repeat the thread cutting many times in the same path from the roughing to the finish

turning when the thread is machined. The thread cutting starts after receiving 1-rotation signal

88

GSK928TEⅡ Turning CNC System User Manual

from the spindle encoder, and so the cutting points on the circle of machining workpiece are the
same when repeating the thread cutting many times, the spindle speed must not be changed at
the same time, otherwise there is the error of thread cutting.

The feedrate of thread cutting and the spindle speed are comfortable. If the spindle speed is high,

the system will not respond timely, which cause the thread to be damaged. The recommended
spindle speed is as follows: N × P ≤ 3000

N—spindle speed Unit：r/min Max. speed is less than 2000 r/min
P—thread lead Unit：mm Inch thread value must be converted to the metric one.
There is wrong screw lead caused by the acceleration/deceleration when the thread cutting is

started and ended. To avoid the above-mentioned problem, the thread length defined is longer
than the actual requirement. Generally, the length is more than 1.3 mm when the thread is cut
with the acceleration.

Fig. 10 Thread cutting

Example：thread lead: ２mm, cutting depth: 2.５mm（diameter value，cutting twice）as Fig. 10：
N0000 G00 X25 Z5 ；approach workpiece

N0010 G01 X23.5 F100 ；feed 1.5 mm (diameter programming)

N0020 G33 Z-50 P2 K2.5 ；the first thread cutting
N0030 G00 X26 ；tool retraction 2.５mm

N0040 Z5 ；return to the starting point

N0050 G01 X22.5 ；the second feeding 1mm

N0060 G33 Z-50 P2 K2.5 ；the second thread cutting

N0070 G00 X26 ；X tool retraction

N0080 Z5 ；z returns to starting point

Note 1: The feed hold key and the feedrate override are invalid in the course of thread cutting.

Note 2: In the course of thread cutting, the feed will stop once the spindle stops.

Note 3: The photoelectric encoder with 1200 or 1024 lines must be installed to rotate with the

spindle synchronously. The selected encoder lines are the same as the actual installed
ones. When the encoder lines are 1200, P11 Bit 4 is 0; when the encoder lines are 1024,
P11 Bit 4 is 1. If the setting of Bit 4 is wrong, the pitch will be mistake when the thread is
machined.

Note 4: For the thread with the thread run-out parameter in the command, the spindle speed, the

pitch, X acceleration time and X initial speed, I/K ratio in the program will affect the
length of thread run-out. The higher the speed is, the bigger the pitch is, the longer X
acceleration time is, the lower X initial speed is, the smaller I/K ratio is, the longer the
length of thread run-out is, vice versa, the shorter the length is. Relatively, I/K ratio has
more influence upon the length of thread run-out.

Note 5: When the previous block and the current one are the thread cutting command, do not

detect the thread head signal (only one per rev) but directly start the cutting feed.

89

Programming Chapter Three Commands and Functions

Example: G33 W-20 P3；the system detects 1-turn signal when the thread cutting is executed.
G33 W-30 P2; the system does not detect 1-turn signal when the thread cutting is

executed.

3.1.5 G32 — Z Tapping Cycle

Command format：G32 Z (W) P (E)；

Ｚ（Ｗ）—end point coordinates or length of tapping
Ｐ—pitch of metric thread
Ｅ—pitch of inch thread

G32 Z tapping process

1． Z feed

1. Stop the spindle

2. Wait for the spindle to stop completely.

3. Spindle rotates counterclockwise (opposite to the previous direction).

4. retract the tool to Z starting point of cycle.

5. Spindle stops.

Z

X

Fig. 11 G32 tapping cycle

Example：Single thread with 1.5 mm lead
N0010 G00 X0 Z20 ；rapidly positioning the starting point of workpiece

N0020 M3 S01 ；spindle CCW

N0030 G01 Z2 F500 ；Z approach the workpiece

N0040 G32 Z-30 P1.5 ；Z infeed tool

N0050 G00 Z20 ；leave the workpiece and return to program starting point

N0060 M02 ；end of program

Note 1: Determine the spindle direction according to the possible tapping direction before

tapping. The spindle will stop after the tapping ends. Restart the spindle when
continuously machining.

Note 2: G32 is for the rigid tapping. There is a deceleration time after the signal of spindle

stopping is valid. At the moment, Z feed will rotate along the spindle if the spindle does
not stop completely. Therefore, the actual bottom hole of machining is deeper than the
actual required. The actual depth should be determined by the spindle speed in tapping
and by whether the spindle’s brake is installed or not.

Note 3: The other cautions are the same those of G33.

`

90

GSK928TEⅡ Turning CNC System User Manual

3.1.6 G50 — Creating a Workpiece Coordinate System

Command format: G50 X Z;
G50 defines a coordinate system and confirms the current position of tool in the coordinate as X,
Z coordinate value.
The defined coordinate system by G50 is named as the workpiece coordinate system. The
absolute coordinate in the following command must be in it after the workpiece coordinate
system is set.
Z is defined on the rotation center of workpiece after the workpiece coordinate system is set and
X on the end face of chuck or workpiece as Fig. 12:

Fig. 12 G 50 creating a workpiece coordinate system

Fig. 12a：Ｇ５０ Ｘ１００ Ｚ8０ ；Z coordinate is positive in machining.
Fig. 12b：Ｇ５０ Ｘ１００ Ｚ3０ ；Z coordinate is negative in machining.

Note 1: When G50 is executed, the system automatically checks if the current coordinates are

the same those of the defined coordinates by G50. If they are same, execute the next

block; if not, the system prompts: Prog. Zero? .Press , the system will return to

the starting point of program by G50 to execute the next block. Press , the
system will not return to the starting point of program but directly modify the current
coordinates into the defined coordinate value by G50. Press other keys, the system will

not execute any operations. Press , the system will return to the previous state
before pressing the run keys. The course of returning to the starting point of program is
the same that of G00.

Note 2: Do not start to execute some block from the middle of program before executing 50 after

power on if the system uses G50 in the programming, otherwise maybe the coordinate
data is wrong. G50 is only in single block. Otherwise the system does not execute other
commands.

Note 3: If the system does not use G50 to execute the first block of program, X, Z absolute

coordinate must be positioned simultaneously with G00. The system will execute the
absolute coordinates by the system when the first traverse command uses the
incremental programming.

Note 4: If the system uses G50 to execute the previous block and does not use G50 to execute

the next one, the program reference point is still on the defined point by the previous
program. After executing the reference point return, the reference point still returns to the
previous position.

91

Programming Chapter Three Commands and Functions

3.1.7 G26 — Reference Point Return

Command format：G26 ;
The tool returns to the reference point( machining starting point) with G26, and the mode of the

reference point return with G26 is the same that of G00. See Fig. 13:

Fig. 13 G26 reference point return

Reference point return ：
After executing G commands, X, Z moves to the point defined by G50. Without G50 in the
program, move to the reference point defined in “Manual” mode with G26. Define the point with
G50 as the reference point if the user does not define the reference point in “Manual” mode. The
system defaults X=150，Z=150 as the reference point if it has never defined the reference point.
If the system executes the first motion after G26 in the program without G50, it must firstly
position with the command in X, Z absolute programming mode, otherwise the following
command after G26 cannot be executed rightly. X, Z move from A to the reference point B
simultaneously and respectively at max. rapid traverse speed and the speed defined by the rapid
traverse override.
When the system uses G50 in the program to define the reference point, the tool retracts to the
point defined by G50 after executing G26, and the following program is needed to execute the
programming. Without G50 in the program, G26 is executed according to the position of
reference point defined by user in “Manual” mode. Take the previous position defined by G50 as
the reference point which is not defined by user. The system will default X=250，Z=250 as the
reference point if the system has never defined it. When the system uses G26 without G50, must
position again with G0 before executing the traverse command behind G26, otherwise the
following command cannot be executed rightly.

Note 1: After the tool returns to the reference point with G26, it must position simultaneously X, Z

absolute coordinates with G00 to continuously traverse, which is contributed to the right
motion.

Note 2: The tool returns to the reference point with G26 at the speed defined (rapid traverse

speed) by G00 and controlled by the rapid traverse override.

Note 3: After the tool returns to the reference point with G26, the offsets of tool and system are

cancelled.

3.1.8 G27 — X Reference Point Return

Command format：G27 ;

After X returns to the reference point with G27 at the rapidest traverse speed controlled by the
rapid traverse override, X offsets of tool and system are cancelled. When Z offset value is also 0,
the tool offset number is displayed to 0.

92

GSK928TEⅡ Turning CNC System User Manual

3.1.9 G29 — Z Reference Point Return

Command format：G29 ;

After X returns to the reference point with G27 at the rapidest traverse speed controlled by the
rapid traverse override, Z offsets of tool and system are cancelled. When X offset value is also 0,
and the tool offset number is displayed to 0.

Note: The cautions of G27, G29 are the same those of G26.

3.1.10 G31 —Skip

Command format： G31 X（U）_ Z（W）_ F_ ；

X , Z — end point coordinates after the command ends.

U, W — incremental value counted by the theory end point.

F — feedrate.

Command function: execute G31 according to G01 run mode, and check the outer skip signal in

running. In spite of arriving or exceeding the theory end point, the run stops and

the current coordinates are changed to the theory values counted by X, Z or U,

W values in programs when the outer signal is valid.

Example：current coordinates X=100 Z=100

G31 Z30 F20；

The moving distance is Z70, Z runs with 20mm/min, no matter what it exceeds Z30, Z

always runs without the outer signal; when Z=28.37 and the outer signal is valid, Z

immediately stops and the current Z coordinate is changed to 30.

Note: G31 input interface: X4.14.

Attention: to get the accurate position, the run stops immediately and there is no deceleration course

once the system has checked the outer signal. So, the run speed in G31 cannot be high,

and it is recommended that it is should be less than the value of P21.

3.1.11 G04 — Dwell

Command format：G04 D ;

D—dwell time. Unit: second range：0.001－65.535s

G04 defines the meantime between two blocks.

Example：G04 D2.5 ；dwell for 2.5s.

3.1.12 Constant Surface Speed ON/OFF—G96/ G97

Command format：G96 S ;

G97 S;

S defines the constant surface speed in G96. Unit：m/min.
S defines the spindle speed in G97 after canceling the constant surface speed. Unit：r/min.

Note 1: The spindle speed is controlled actually by the constant surface speed control function

when the system adopts the spindle controlled by the converter, i.e. MDSP=1 of P12.

93

Programming Chapter Three Commands and Functions

Do not execute the constant surface speed control in G96 if the system adopts the
gear shifting spindle.

Note 2: The constant surface speed control is valid only in AUTO mode and the system will

automatically cancel the constant surface speed control after escaping from AUTO
mode or resetting.

Note 3: The constant surface speed control is valid in the end point in G00. Execute the constant

surface speed control anytime in G01, G02, G03.

Note 4: Max. speed of constant surface speed control is defined by P09, P10, and min. speed

set by the system is 25 r/min.

Note 5: The constant surface speed defined by S in the constant surface speed control is not

one after the tool compensation or the offset but the programming path.

Note 6: The rotary axis must be positioned on Z workpiece coordinate system (X=0) in the

constant surface speed control.

Note 7: G96 is modal. When G96 is valid, the single S command is taken as the new surface

speed data.

Note 8: In DRY RUN mode, the surface speed control is valid but the single S command cannot

update the previous surface speed.

Note 9: The constant surface speed control is valid when executing the thread cutting. Ensure

the constant surface speed control is invalid with G97 to make the spindle speed
constantly.

Note 10: Before using the constant surface speed control, it is necessary to make sure the

current spindle speed approaches the initial speed of constant surface speed. They
must coincide with each other by tuning the spindle speed to approach the initial speed
of constant surface speed if there is big different, otherwise the spindle speed is
suddenly changed which also be caused by the big tool compensation value when the
tool compensation is modified to the coordinate mode.

3.1.13 Single Canned Cycle

It is necessary to cut repeatedly the same machining path in the course of some special roughing.

To simplify the programming, improve the programming and the machining efficiency, the canned
cycle is set. The tool will automatically return to the coordinate position before execution when
executing the canned cycle once. If the cycle is executed again, do not rewrite the cycle
commands but execute the programming of feeding data again. Return to the starting point of
cycle after executing the cycle. If other commands G, M, S, T are contained in the block behind
the cycle ones, the cycle automatically ends.

3.1.13.1 G90 — Inner/Outer Surface Turning Cycle

Command format：G90 X(U) Z(W) R F ;

X（U）Z（W）—end point of cylindrical(taper) surface，The two axes must be given and the

incremental coordinates cannot be zero.

R—diameter difference between the starting point and the end point of cycle. It is the axis surface

cutting if R is omitted.

F—feedrate.

G90 cycle process：

1. X rapidly moves from A to B.

2. X, Z cut at F speed from B to C (X does not move without R).

3. X cut at F speed from C to D.

4. Z rapidly moves from D to A.

The tool is still at the starting point of cycle after G90 cycle ends. If only X coordinate of end point

is defined again (or incremental coordinate U), the above-mentioned cycle is repeated according
to the new X (U) coordinate value.

When using the incremental coordinates, U sign is defined by X from A to B, and W sign is

defined by Z from B to C.

94

GSK928TEⅡ Turning CNC System User Manual

Z

When executing the taper surface cutting cycle, R sign is determined by the X from C to B.

Z

X/2

R/2

W

Rapid traverse

Cutting feed

X

U/2

Fig. 14 Inner/outer cylindrical (taper) surface turning cycle

Relationships between the data behind U, W, R and the tool path are as follows:

(1)U＜0，W＜0，R＜0 (2)U＜0，W＜0，R＞0

Z

U/2

U/2

W

X

X from A to B is negative, so U<0;

Z from B to C is negative, so W<0;

X from C to B is negative, so R<0.

(3)U

＞0，W＜0，R＜0 (4)U＜0，W＜0，R＞0

X

X from A to B is negative, so U<0;
Z from B to C is negative, so W<0;
X from C to B is positive, so R>0.

W

Z

W

X

X from A to B is positive, so U>0;
Z from B to C is negative, so W<0;
X from C to B is negative, so R<0.

Z

X

Fig. 15 Relationships between signs of U, W, R and tool path in G90

X from A to B is positive, so U>0;
Z from B to C is negative, so W<0;
X from C to B is positive, so R>0.

Rapid traverse Cutting feed

95

Programming Chapter Three Commands and Functions

Example 1: Fig. 15a outer cylindrical surface: the first cutting feed= 5 mm, the second cutting

feed= 2 mm, F=100 mm/min.

N0010 G00 X47 Z62 ；rapidly position to A

N0020 G90 X40 Z30 F100

N0030 X35

N0040 X33

；cycle once A B C D A

；the first tool infeed to cycle once A B1 C1 D A

；the second tool infeed to cycle once A B2 C2 D A

The tool is still on A after executing the above-mentioned blocks.

Example 2: Fig. 15b taper surface: the cutting feed R=- 5 mm once, F=100 mm/min.

N0010 G00 X55 Z5 ；rapidly position to A

N0020 G90 X50 Z-20 R-5 F100

N0030 G90 X50 Z-20 R-10

N0040 G90 X50 Z-20 R-15

N0050 G90 X50 Z-20 R-20

N0060 G90 X50 Z-20 R-25

；cycle A B1 C D A

；cycle A B2 C D A

；cycle A B3 C D A

；cycle A B4 C D A

；cycle A B C D A

The tool is still on A after executing the above blocks.

Note 1: The directions of cylindrical machining and cutting feed are defined automatically by the

starting point of the cycle and X, Z coordinate values in the command.

Note 2: When the single block is running, Press

once to execute one cycle and stop at

the end point of each step of cycle.

Note 3: If the next command is not the single traverse command in X or Z direction but other G,

M after the cycle ends, the cycle will automatically end.

Note 4: Cautions of other single canned cycle are the same those of the front three items.

Note 5: When executing the cycle G90, G94, if there is taper cutting(R≠0), G90, X, Z, R cannot be

omitted.

3.1.13.2 G92 — Thread Cutting Cycle

Command format

：G92 X（U）_ Z（W）_ P（E）_ I_ K_ R_ L _ D_ ； I is not negative

value.

The tool is still on A after the system executes the above blocks.

Note 1: The directions of cylindrical machining and cutting feed are defined automatically by the

starting point of the cycle and X, Z coordinate values in the command.

Note 2: When the single block is running, Press

once to execute one cycle and stop at

the end point of each step of cycle.

Note 3: If the next command is not X, Z single motion command but other G, M after the cycle

ends, the cycle will automatically end.

Note 4: Cautions of other single canned cycle are the same those of the front three items.
Note 5: When executing the cycle G90, G94, if there is taper cutting(R≠0), G90, X, Z, R cannot

be omitted.

As Fig. 16 G92 thread machining .

1. G92 axial straight thread: as Fig. 16-1

96