gsk GSK983Ma User Manual

Download

Page 1

This user manual describes all proceedings concerning the

operations of this CNC system in detail as much as possible. However, it is

impractical to give particular descriptions for all unnecessary or unallowable

system operations due to the manual text limit, product specific applications

and other causes. Therefore, the proceedings not indicated herein should

be considered impractical or unallowable.

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

rights are 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.

Page 2

GSK983Ma Milling Machine Center CNC System User Manual

Preface

Your Excellency,

It’s our pleasure for your patronage and purchase of this GSK983Ma Milling machining center CNC system made by GSK CNC Equipment Co., Ltd.

GSK983Ma User Manual divides into three parts, that is, “Programming”, “Operation” and “Appendix”.

Special prompt: 24V switch power box matched with the system is the

special power offered by our company.

User can not use the power to other purpose. Otherwise, the

enormous danger may occur!

Page 3

Safty Caution

！ Accident may occur by improper connection and operation！This system

can only be operated by authorized and qualified personnel. Please

carefully read this manual before using！

Refer to user manual issued by the manufacturer carefully

before installing, programming and operating this product, and

the relative operation should be performed based upon the user

manual strictly.

III

Page 4

GSK983Ma Milling Machine Center CNC System User Manual

Statement

● In this manual we have tried as much as possible to describe all the

various matters. However, we cannot describe all the matters which must not be done, or which cannot be done, because there are so many possibilities. Therefore, matters which are not especially described as possible in this manual should be regarded as “impossible”

Notice

● The product function and qualification (such as the accuracy, speed)

described in this manual is only for this product, which is installed the CNC machine of this product. The actual function configuration and technical capacity are determined by the setting of the manufacturer.

● The system is matched with the standard operation panel, but its

function of each key is defined by the PLC program (ladder diagram). It is very important to note that the function of the key in this manual is described for the standard PLC program!

● Refer to the manual issued by the manufacturer for the function of

each key on the operation panel and the meaning.

Page 5

Cautions

■ Transportation and storage

● Do not pile the carton more than six layers.

● Do not climb, stand or place the heavy on the carton.

● Do not drag or move the production using the cable connected with the

production.

● Do not bump the carton or scratch the panel and the display screen.

● The product packing should be avoid the damp, sun and rain.

■ Checking

● Confirm whether it is your purchased product after opening the packing.

● Confirm whether the product is being damaged during transporting.

● Confirm whether the spare parts are completed or being damaged.

● If the unconfirmed type, the lack of accessories or the damage of transportation

may occur, touch our company freely.

■ Wiring

● The wiring or checking should be performed with the professional.

● Refer to the Connection Manual for the wiring.

● The product should be grounded, and the grounding resistance should be less

than 0.1Ω. The neutral line (zero line) can not be replaced by the grounding.

● The wiring should be correct and firm, so that the product malfunction or undesired result may occur.

● The surge absorber diode connected with this product should be connected in the specified direction, or the product may be damaged.

● The power should be cut off when Inserting or pulling out the plug or opening the machine of the product

■ Detection

● The man who is the professional can be detected the machine.

● The power should be cut off before detecting or repairing or changing the

elements.

● Checking the malfunction when the short-circuit or the overloading occurs, it can be started after the malfunction is eliminated.

● Never attempt to turn on/off the product frequently, if you want to start it again after the power is turned off, it is necessary to wait for 1min at least.

Page 6

GSK983Ma Milling Machine Center CNC System User Manual

Security Responsibility

Security responsibility for manufacturer

——Manufacturer should be take responsibility for the danger of the motor and the

accessories which have been eliminated and/ or controlled in design and in structure.

——Manufacturer should be take responsibility for the security of the motor and

accessories.

——Manufacturer should be take responsibility for use information and suggestion

offered to the user.

Security responsibility for the user

——User should be know and understand about the content for security operation by

learning and training the security operation of the motor.

——User should be take responsibility for the security and danger about the increase,

change or original motor modification or accessory by themselves.

——User should be take responsibility for operating, adjusting, maintaining, installing

and storing the products without following the descriptions of this manual,

All specifications and design are subject to change without further

notice.

This manual is reserved by final user.

Sincere thanks for your friendly patronage for the products

made by GSK CNC Equipment Co., Ltd.

Chinese version of all technical documents in Chinese and

English languages is regarded as final.

Page 7

List

Programming

Programming .......................................................................................................................................1

Chapter One General........................................................................................................................1

1.1

GENERAL............................................................................................................................................ 1

CAUTIONS FOR READING THIS MANUAL ............................................................................................... 1

1.2

Chapter Two Specification.................................................................................................................3

Chapter Three Programming ..........................................................................................................13

3.1

WHAT IS PROGRAMMING..................................................................................................................... 13

PROGRAM STRUCTURE........................................................................................................................ 13

3.2

3.2.1 Block .....................................................................................................................................14

3.2.2 Program Word ..................................................................................................................... 14

3.2.3 Input format.......................................................................................................................... 16

3.2.4 Decimal point programming ..............................................................................................17

3.2.5 The maximum command value......................................................................................... 18

3.2.6 Program number................................................................................................................. 19

3.2.7 Sequence number .............................................................................................................. 20

3.2.8 Skip to optional block ......................................................................................................... 20

DIMENSION WORD .............................................................................................................................. 21

3.3

3.3.1 Controlled axis..................................................................................................................... 21

3.3.2 Setting unit ...........................................................................................................................22

3.3.3 The maximum stroke.......................................................................................................... 24

3.3.4 Program origin and coordinate system............................................................................ 24

3.3.5 The coordinate system and the machining start point................................................... 24

3.3.6 Workpiece coordinate system........................................................................................... 25

3.3.7 Reference (position) point ................................................................................................. 25

3.3.8 Absolute and incremental commands.............................................................................. 26

FEED FUNCTION (F FUNCTION) ........................................................................................................... 27

3.4

3.4.1 Rapid traverse rate............................................................................................................. 27

3.4.2 Cutting Feedrate ................................................................................................................. 27

3.4.3 Feedrate decelerates to 1/10.......................................................................................... 28

3.4.4 Synchronous feed (feed/rev.)............................................................................................ 28

3.4.5 F1-digit Feed ....................................................................................................................... 29

3.4.6 Automatic acceleration/deceleration................................................................................ 30

3.4.7 Automatic Corner Modification.......................................................................................... 31

PREPARATION FUNCTION (G FUNCTION) ............................................................................................. 34

3.5

3.5.1 Plain Selection (G17, G18, G19)...................................................................................... 37

3.5.2 Positioning (G00)................................................................................................................ 37

3.5.3 Single Direction Positioning (G60) ................................................................................... 38

3.5.4 Linear interpolation (G01)................................................................................................ 39

3.5.5 Circular Interpolation (G02, G03)..................................................................................... 41

3.5.6 Sine curve interpolation ..................................................................................................... 44

3.5.7 Thread Cutting (G33) ...................................................................................................... 45

～

3.5.8 Automatic reference position return (Reference position G27

3.5.9 Dwell (G04) ..........................................................................................................................51

3.5.10 Exact stop check (G09) ...................................................................................................51

3.5.11 Exact stop check (G60) and cutting mode (G64)......................................................... 51

3.5.12 Coordinate system setting (G92) ................................................................................... 51

～

3.5.13 Workpiece coordinate system (G54

G59).................................................................. 53

3.5.14 Workpiece coordinate system changes by the program command.......................... 55

3.5.15 Automatic coordinate system setting............................................................................. 55

3.5.16 Inch/Metric conversion (G20, G21)................................................................................ 56

3.5.17 Stored stroke limit (G22, G23)........................................................................................ 56

3.5.18 Skip Function (G31) ......................................................................................................... 59

COMPENSATION FUNCTION ................................................................................................................. 60

3.6

G30)........................ 47

VII

Page 8

GSK983Ma Milling Machine Center CNC System User Manual

3.6.1 Tool length compensation (G43, G44, G49) ...................................................................60

～

3.6.2 Tool position offset (G45

3.6.3 Cutter compensation (G40

G48)........................................................................................63

～

G42)....................................................................................70

3.6.4 Functions D and H ............................................................................................................101

3.6.5 External tool offset ............................................................................................................102

3.6.6 Enter offset value from the program (G10)..................................................................102

3.6.7 Scaling (G50, G51) ...........................................................................................................102

3.6.8 Coordinate system rotation (G68, G69).........................................................................105

THE FUNCTION OF CYCLE MACHINING .............................................................................................. 113

3.7

3.7.1 The function of the external operation........................................................................... 113

～

3.7.2 Canned cycle (G73, G74, G76, G80

G89)................................................................. 113

3.7.3 The initial point and point R in the canned cycle (G98, G99).....................................134

3.7.4 Rigid tapping cycle (G180, G184)...................................................................................135

SPINDLE FUNCTION (S FUNCTION), TOOL FUNCTION (T FUNCTION), MISCELLANEOUS FUNCTION (M

3.8 FUNCTION), THE 2

MISCELLANEOUS FUNCTION (B FUNCTION) ............................................................138

3.8.1 Spindle function (S function)............................................................................................139

3.8.2 Constant surface speed control ......................................................................................139

3.8.3 Tool function (T function)..................................................................................................141

3.8.4 Miscellaneous function (M function)...............................................................................141

3.8.5 The 2nd Miscellaneous Function (B function)...............................................................142

SUB-PROGRAM..................................................................................................................................142

3.9

3.9.1 The Manufacture of the Sub-pr ogram............................................................................142

3.9.2 The Performance of the Sub-program...........................................................................143

3.9.3 Special usage ....................................................................................................................143

USER MACRO PROGRAM.................................................................................................................145

3.10

3.10.1 General Brief....................................................................................................................145

3.10.2 Variable.............................................................................................................................145

3.10.3 Type of the Variable........................................................................................................147

3.10.4 Operation command .......................................................................................................157

3.10.5 Control command............................................................................................................160

3.10.6 The Compilation of the User Macro Program Body and Memory............................164

3.10.7 Macro Call command......................................................................................................167

3.10.8 The Relationships with Other Functions......................................................................177

3.10.9 Special Codes and Words Used in User Programs................................................... 178

3.10.10 Restrictions....................................................................................................................179

3.10.11 The Description of the P/S Alarm ...............................................................................179

3.10.12 Examples of User Macro .............................................................................................180

3.10.13 External Output Command..........................................................................................181

3.10.14 Macro interruption function (Macro B)....................................................................... 183

TOOL LIFE MANAGEMENT ..............................................................................................................184

3.11

3.11.1 Setting of the Tool Groups .............................................................................................184

3.11.2 Specification in the Machining process........................................................................186

3.11.3 Performance of the Tool Life Management.................................................................187

3.11.4 The Display and Input of the Tool Data........................................................................187

3.11.5 Other Cautions.................................................................................................................188

THE INDEXING FUNCTION OF THE INDEX WORKTABLE ..................................................................189

3.12

3.12.1 Instruction method ..........................................................................................................189

3.12.2 The Minimum Movement Unit: 0.001 degree/pulse...................................................189

3.12.3 Feedrate ...........................................................................................................................189

3.12.4 The Clamping and Release of the Indexing Worktable.............................................190

3.12.5 JOG/Step/MPG................................................................................................................191

3.12.6 Other Cautions ................................................................................................................191

Chapter Four Operation................................................................................................................ 193

POWER ON/OFF...............................................................................................................................193

4.1

4.1.1 Power ON ...........................................................................................................................193

4.1.2 Power OFF .........................................................................................................................193

PROGRAM LOCK................................................................................................................................193

4.2

RELATED OPERATIONS TO MACHINE PANEL ....................................................................................194

4.3

VIII

Page 9

List

4.3.1 Machine Panel................................................................................................................... 194

4.3.2 Emergency Stop (red)...................................................................................................... 196

4.3.3 Mode Selection ................................................................................................................. 196

4.3.4 Operations Related to Manual Operatio n...................................................................... 198

4.3.5 Manual Reference Point Return (reference position).................................................. 205

4.3.6 Related Operations in Automatic Running.................................................................... 205

4.3.7 MPG (manual pulse generator) Interruption ................................................................. 221

4.3.8 Manual Spindle Function .................................................................................................222

4.3.9 Manual Auxiliary Function ............................................................................................... 223

DISPLAY AND OPERATION OF THE NC UNIT WITH LCD CHARACTER DISPLAYER........................... 224

4.4

4.4.1 State Display ..................................................................................................................... 228

4.4.2 Key Input ............................................................................................................................ 230

4.4.3 Display of Program Number and Sequence Numbers................................................ 231

4.4.4 Alarm Display (functional key ALARM )..................................................................... 232

4.4.5 Operation Information (the content of external alarm message)............................... 232

4.4.6 Current Position Display and Reset (functional key POSITION )........................... 233

4.4.7 Display of Command Value (functional key COMMAND ) ...................................... 234

4.4.8 Setting (functional key SETTING ).............................................................................. 235

4.4.9 MDI Operation (functional key COMMAND )............................................................. 239

4.4.10 MDI Start and Running .................................................................................................. 240

4.4.11 Reset ................................................................................................................................240

4.4.12 Offset of the Tool Position............................................................................................. 241

4.4.13 Setting and Display of Workpiece Origin Point Offset............................................... 242

4.4.14 The method of Measuring Tool Length ....................................................................... 243

4.4.15 Program Display (Functional key PROGRAM).......................................................... 243

4.4.16 Program Number Retrieving (functional key PROGRAM)....................................... 245

4.4.17 Input a Single Program File ............................................................................................. 245

4.4.18 Input Program File with Multiple Programs.................................................................... 246

4.4.19 Input Programs by Keys................................................................................................ 246

4.4.20 Deletion of a Program.................................................................................................... 248

4.4.21 Deletion of All Programs................................................................................................ 248

4.4.22 Output a Program........................................................................................................... 248

4.4.23 Output All Programs.......................................................................................................... 248

4.4.24 Sequence Number Search............................................................................................ 248

4.4.25 Restart the Program....................................................................................................... 249

4.4.26 Comparison and Stop Function for Block ................................................................... 252

4.4.27 Input Offset Value (any functional key).......................................................................... 252

4.4.28 Output Offset Value(functional key: OFFSET) .............................................................. 252

：

4.4.29 Display Parameter (functional key

PARAMETER )................................................ 253

4.4.30 Program Edit (functional key：PARAMETER )......................................................... 253

4.4.31 Display of Running Time ............................................................................................... 262

4.4.32 Menu Switch Function.................................................................................................... 262

4.4.33 Operation for LCD Soft Functional Key....................................................................... 264

4.4.34 Input/Output of NC Parameter...................................................................................... 273

GRAPHIC FUNCTION............................................................................................................................ 274

4.5

4.5.1 Display Type of The Graphic........................................................................................... 274

4.5.2 Graphic Parameter Setting.............................................................................................. 274

4.5.3 The Meaning of Graphic Parameter............................................................................... 275

4.5.4 Drafting............................................................................................................................... 280

APPENDIX ......................................................................................................................................282

Appendix 1 System Version Display................................................................................................282

Appendix 2 G Codes List.................................................................................................................283

Appendix 3 Range of Command Values..........................................................................................285

Appendix 4 Nomographs .................................................................................................................286

Appendix 5 Parameters ...................................................................................................................289

Appendix 6 Alarm List......................................................................................................................329

Appendix 7 Status when Turning Power on, Reset and Cleared .....................................................338

Appendix 8 Stored Pitch Error Compensation Function................................................................340

Page 10

GSK983Ma Milling Machine Center CNC System User Manual

Appendix 9 Operation List ...............................................................................................................347

Appendix10 Program Lock ..............................................................................................................351

Appendix 11 USB Interface Parameter Transfer Operation .............................................................353

Appendix 12 System Clock Setting and PLC Programming ............................................................354

Appendix 13 The supplement of the GSK983Ma Milling Machining Center CNC System User

Manual.............................................................................................................................................359

Page 11

Chapter One General

Programming

Chapter One General

1.1 General

GSK983Ma Milling machining center CNC system (The following are abbreviated to

“System”), which is a medium and high grade manufactured goods with high speed, high accuracy,

high stability, and high cost performance. It has been developed base on the stable and reliable and

the market requirement and the updated technical development by the GSK CNC Equipment

Company.

This horizontal type/vertical type installation of this system adopts the 8.4

Part 1 Programming

inch/10.4 inch HR, hi-lite LCD screen separately. The system uses the full paster

automatic product technology and built-in PLC. The operating interpolation is

distributed processing by the multiply high-speed microprocessors, which owns the

treatment capacity for 500 blocks per second. The special hardware circuit is externally

connected the raster rule, which can be controlled of the position full-close. It has the

boundary CNC alarm detecting function, which is used for the serial high-speed, high

accuracy, Hi-Rel.

1.2 Cautions for Reading this Manual

The capacity of the CNC machine are determined by the CNC system, machine

structure, strong current control and the servo system (the mechanical operation pane

included), this manual is only described for the GSK983Ma CNC system.

This manual is introduced the function (Selection function included) of the system

with detailed, but the actual device is not included all the selection function. The function

of the CNC system is not only determined by the NC, but also the mechanical part, the

strong circuit of the machine side, servo system and the machine operator panel. It is

very hard to describe the whole functions of the system, programming and operation

thoroughly; it is only expressed from the angle of the system.

The specification of the operation panel, the capacity of the CNC machine, the

machine programming and operation method of the character CNC machine are

performed by referring the manual issued by the manufacturer.

Page 12

Note: The notes are described for some items. However, when the notes without any expresses are

described in this manual, just skip the notes until you return to read it again after finishing this

manual, it is very easy to understand for this manual.

Part 1 Programming

GSK983Ma Milling Machine Center CNC System User Manual

Page 13

No.

Chapter two Specification

Chapter Two Specification

Name Specification

item

1 Controlled axes

No. of

simultaneously

controlled axes

3 Increment system

Standard: 3 axes (X, Y and Z)

(It can be set to the 4

address of 4

is selected from A, B, C, U, V and W, the 4th axis is

axis or the 5th axis based on the order. The

straight line axis or rotation one which is set by parameter; and the

address of the 5

axis is selected from U, V, W, A, B and C, the 5th axis

is straight line axis or the rotation one which is set by parameter, too).

The standard is 3 axes and 3-linkage simultaneously. (It can be set to the 4 axes and 3-linkage, 4 axes and 4-linkage, 5 axes and 3-linkage and 5 axes and 4-linkage base on the order).

Note: The functions, such as the rigid tapping and the feed per revolution, can not be used by the 5 axes.

The least

setting

0.001mm 0.0001inch 0.001°

increment

The least input

0.001mm 0.0001inch 0.001°

increment

Part 1 Programming

The least input increment by metric based on the parameter setting is

0.01mm.

4 Digit check device Pulse encoder

±99999.999mm

The Max.

±9999.9999inch

command value

±99999.999°

Use the formats, such as, changeable block, changeable character and

6 Input format

the changeable address.

Decimal point

The digit can be inputted with the decimal point, the addresses with

programming

decimal point: X, Y, Z, A, B, C, U, V, W, I, J, K, Q, R and F.

The axis direction speed is up to 60.000m/min or 2400inch/min. The

8 Rapid traverse

rapid traverse speed can be modified into F0, 25%, 50% and 100%

using the rapid traverse override (selection).

The feedrate can be set within the following range: 1mm/min ～

30,000mm/min, the upper limited speed of cutting feed 0.01inch/min～

9 Cutting feedrate

1200.00 inch/min can be set by the parameter. The feedrate override

10% is regarded as a gear which can be selected a feedrate within the

Page 14

GSK983Ma Milling Machine Center CNC System User Manual

range of 0～200%, the unit of feedrate set by parameter can be

modified into 0.01 mm/min, 0.001 mm/min or 0.001inch/min.

Automatic

acceleration/decele

ration

Absolute/increment

Part 1 Programming

value command

Coordinate system

setting (G92)

13 Positioning (G00)

Linear interpolation

(G01)

The linear acceleration or deceleration mode can be used at the rapid

traverse rate regardless of the manual or Auto to shorten the positioning

time.

Either the absolute programming or increment programming can be

selected by the G code.

G90: Absolute value programming

G91: Incremental value programming

The command value followed with the G92 can be used to set a

coordinate system, the tool position coordinate value is the command

value of this coordinate system.

Each axis can separately and rapidly move to the end then stops by

specifying G00, and whether the machine can be performed the

in-position (whether the machine is reached the specified position)

check by the parameter setting.

Use the G01 code, the linear interpolation can be performed based on

the feedrate specified by F code.

15 Buffer register

16 Dwell (G04)

Exact stop check

(G09)

Checking mode of

exact stop/cutting

mode (G61, G64)

Miscellaneous

function (M2 digit)

The next block can be read to the buffer register in advance before the

former block is performed. In this case, avoid the intermittence of NC

command because the time for reading. When the data is inputted to

the buffer register, the BUF is displayed at the lower right of LCD.

The next block movement can be delayed using the G04 code.

The delay time can be specified by the address P or X.

Specify a block of G09, it decelerates to 0 when the block ends, and

then performs the following block after positioning.

If the G61 is specified, the movement command followed with the G61

decelerates to 0 at the end of each block, and then performs the

following block after positioning.

If the G64 is specified, the movement command followed with the G64

other than the position does not decelerate but perform the following

block immediately, generally, it is for cutting mode.

The command after the address M followed 2-digit can be controlled for

the ON/OFF signal of the machine side. Only one M code can be

specified in a block.

20 Dry run

In the dry run mode, the feedrate becomes JOG.

The rapid traverse holds invariable in G00 command, the rapid traverse

override (selection) is still valid. Whether the rapid feedrate is run based

Page 15

Chapter two Specification

upon the dry run which is determined by the parameter setting.

Each axis can be separately forbidden the feed of the commanded axis,

21 Interlocking

if any commanded axis is added an interlocking during movement, all of

the axes of machine may decelerate and then stops. The machine

accelerates then starts as long as the interlocking releases.

22 Single block One block command can be performed once.

The block with / (slash) code (A / (slash) code followed by a block) can

23 Optional block skip

be omitted the start by switching on the optional block skip switch

installed on the machine side.

The movement direction or the mirror image of X, Y and 4

External mirror

program command and the MDI command can either set using MDI &

image

LCD panel or using the switches (selected function) at the machine

side.

Whether the movement amount of the tool is moved by manual

operation is added to the absolute coordinate value can be selected by

Manual absolute

turning the manual absolute switch on or off on the machine side.

ON/OFF

When the switch is turned off: added

When the switch is turned off: do not add

axis

Part 1 Programming

Miscellaneous

function lock

27 Machine lock

Z-axis command

cancel

29 Feed hold

Override

cancellation

31 ESP

External resetting,

resetting signal

The BCD code signal and strobe signal of M, S, T and B function are

forbidden to send to the machine side.

The machine does not move, but the position display is still enabled as

the machine is moving, the machine locking is enabled even if the block

is performing.

This function is only valid to the Z axis lock; use this function to check

NC program by drawing.

The feed of all axes can be temporarily stopped, the resetting can be

performed by pressing the cycle start button, before the feed resetting,

the manual operation can be performed in the mode of manual.

The cutting feedrate can be fixed on the 100% based on the signal

(selection function) from machine side.

All feed commands are being stopped (immediately interrupted) by

pressing the ESP button, the machine is stopped simultaneously.

NC can be reset from NC external. All of the feed commands are

stopped with this signal by resetting, and the machine decelerates to

stop. Additional, during the resetting button of MDI & LCD, ESP and

external resetting added; input a resetting signal to the machine side.

When the machine motion components arrived to the end of the stroke,

33 Overtravel

the arrival signal is received, the axis is decelerated then stopped, and the overtravel alarm may issue simultaneously.

Page 16

GSK983Ma Milling Machine Center CNC System User Manual

When the power is turned on and when NC is at the controllable state,

34 Ready NC signal

35 Ready servo signal

Part 1 Programming

36 NC alarm signal The signal from NC issues at the alarm state.

37 Distributed signal

Cycle operation

signal

Cycle operation

start indicator

signal

Feed hold indicator

signal

send this signal to the machine side; when the power is turned off or the

controllable unit is overheat, stop to send any signal to the machine

side.

Send a signal to the machine side after a servo system is ready. The

axis must be braked in this signal which does not send out is locked.

The NO READY is displayed on LCD when this signal is not executed.

When the movement command ends, NC outputs this signal. If the M,

S, T or B function and movement command in a block, this signal is

issued after movement command is performed, and the M, S, T or B

function can be performed.

NC sends out this signal in the cycle operation.

NC sends out this signal in cycle start.

NC issues this signal when the feed hold is on the dwell state.

Manual

consecution feed

42 Incremental feed

Sequence number

index

Program number

index

Interval

compensation

(1) JOG feed The JOG feedrate can be shifted in 24-step using the

rotation switch. The ratio of the 24-step is geometric series. (Standard

panel matches 20-step)

(2) Manual rapid traverse The rapid traverse can be performed by

manual, the rapid override can be used the rapid traverse of the

parameter setting.

The manual consecution is valid in 2-axis simultaneously.

The increment position control and high-efficiency manual position

(selection function) can be performed

The increment can be performed in 2-axis simultaneously. (the feed of

increment)

The sequence number within program for currently selected can be

indexed using MDI & LCD panel.

The program number of 4 digits followed with O can be indexed using

MDI & LCD panel.

It is a compensation function for the machine movement vector. The

compensation value is set by parameter within the range 0~255, which

is regarded as a unit of the least movement for each axis.

46 Locking of program

This function is forbidden a display, setting or edit of the program

number (9000～9899) by the locking.

Page 17

Chapter two Specification

(1) Ambient temperature

Work temperature: 0℃～45℃

Storage and transportation temperature: -20℃～55℃

(2) Relative humidity

≤90% (condensing), ≤95% (40 )℃

47 Ambient condition

Self-diagnosis

function

(3) Vibration

Work vibration<0.5G,

Storage and transportation vibration<1G

(4) Ambient temperature

When the NC device is used at the high concentration

circumstances, such as in the dust, cutting oil or the organic solvent, is

important to touch the manufacturer.

(1) Servo system

a. When the error of error register is more than the setting value of

stop state, the alarm issues.

b. When the value of error register is more than the maximum

setting value, the alarm issues.

c. When the position check system is abnormal, the alarm issues.

d. When the drifting voltage is excessive large, the alarm issues.

e. When the speed control unit is abnormal, the alarm issues.

(2) NC

Part 1 Programming

S function/T

function (BCD

2-digit)

S4-digit (Binary

system 12-digit

output) A/S4 digit

(analog output) A

a. When the memory is abnormal, the alarm occurs.

b. When ROM or RAM is abnormal, the alarm occurs.

c. When the MPU is abnormal, the alarm occurs.

(3) State display

a. Display the NC state on LCD.

b. Display I/O state on LCD.

2-digit command is followed with address S and T, the code signal of

BCD2-digit can be sent out once the command is performed, the S or T

code is separately sent out with other codes till to the following S or T is

specified.

The binary system 12-digit corresponding with the spindle speed or the

analog voltage outputs to the machine side, the maximum analog

voltage is ±10V, 2mA. The spindle speed (r/min) is directly specified by

S4, the spindle speed can be modified within the 50%, 60%, 70%, 80%,

90%, 100%, 110% or 120% based on the contact signal of the machine

side.

51 S4-digit (Binary When the spindle speed (r/min) is directly specified by S4-digit, output

Page 18

GSK983Ma Milling Machine Center CNC System User Manual

system 12-digit

output) A/S4 digit

(analog output) B

Thread cutting/

synchronic feed

Part 1 Programming

53 Position encoder

Constant surface

Speed control

The 2

function (B3-digit)

the current spindle speed voltage based upon the selected gear

number 1~4. The shift of gear is performed during strong circuit, and its

consequent GRA or GRB signal outputs to the side of NC. The higher

2-digit of S4 or lower 2-digit number of NC program command is

outputted in terms of the BCD code.

The position encoder is installed on the spindle; the thread cutting can

be performed by using the pulse speed of position encoder.

To achieve the above-mentioned feed as the spindle rotation, a

frequency can be introduced to connect it on the spindle directly and the

pulse voltage device which becomes a proportion to the number of

spindle rotation, 1024 pulses for each revolution.

Usually, the surface speed is specified with S code, in this case, when

the tool position is changed, the spindle speed is correspondingly

changed, and the surface speed is always equalled to the linear speed

specified with S code.

Three-digit command followed with address B is performed once, the

auxiliary

BCD three-digit code signal is sent out immediately for specifying the

index table positioning.

T function

(BCD4-digit)

57 Code standard

58 Rapid override

Reference position

return A

Reference position

return B

and the 4th

The 3

reference position

Four-digit command followed with address T is performed once, the

BCD three-digit code signal is sent out immediately, the T code is sent

out with other codes separately until they are reserved to the following T

code is specified.

ISO code (ISO840) and EIA code (EIARS-244-A) can be used by the

program code, which they can automatically and distinguishingly

performed.

The rapid traverse rate of Auto or Manual can be set based upon the

four gears, namely, F0, 25, 50 and 100%. F0 can be set a certain speed

by a parameter.

Reference position return A contains of the following items:

(1) Manual reference position return

(2) Reference position return check (G27)

(3) Automatically reference position return (G28)

The reference position return B is not only contained of the function of

reference position return B but also the 2

reference position return

(G30).

Set the distance of the 1st reference position by the parameter, the 3rd

and the 4

reference position can be set, and these reference positions

return

can be returned.

Page 19

Chapter two Specification

As for the stored stroke limit 1, the area other than the one of parameter

Stored stroke limit

Stored pitch error

compensation

The selection of

workpiece

coordinate system

setting is the forbidden area. As for the stored stroke limit 2, the internal

or the external area specified with parameter or program is forbidden

area. The enabled or disabled of stored stroke limit 2 is determined by

the G code.

G22: Enabled G23: Disabled

This function is used for the pitch error compensation caused by the

mechanical wearing of screw feed to improve the mechanical precise

and prolong the mechanical life. The compensation data is stored in the

memory which is regarded as a parameter; in this case, the relative

operations such as dog and the compensation structure are omitted.

One of the six workpiece coordinate systems can be set in advanced by

using six G codes, namely, G54~G59; and the following program should

be performed within the selected coordinate system.

The tool position offset can be performed using the G45~G48

commands. Tool position offset is the corresponding move command

extends or cuts an offset using the D or H code along axis. 1~184

Part 1 Programming

Tool position offset

commands can be specified by the D or H code, the maximum value of

offset is ±999.999 mm or ±99.999 inch.

(G45~G48)

G45: Extend the setting number.

G46: Short the setting number.

G47: Extend 2 times of setting number.

G48: Short 2 times of setting number.

When the manual reference position return is performed, the coordinate

The setting of

system can be set for setting the parameter in advance, namely, the

automatical

automatical performance is same as the G92 specified with reference

coordinate system

position.

The tool position offset (tool length compensation) can be performed in

the Z axis direction using G43 and G44 codes.

Tool length

The selection of offset number can be specified with 01~184 using H

compensation

code.

(G43, G44, G49)

The maximum value of offset is indicated as ±999.999 mm or

±99.999inch.

compensation (Tool

compensation) B,

C (G40~G42)

Cutter

radius

Cutter compensation can be performed using the G40~G42 codes. The

selection of offset number is specified within 1~184 using D code, the

maximum value of offset is ±999.999 mm or ±99.999inch.

The tool of the inner angle is less than 90° which can not use a tool

compensation B.

The tool of the inner angle is less than 90° which can use a tool

Page 20

GSK983Ma Milling Machine Center CNC System User Manual

compensation C.

After the standard tool is positioned at the fixed point, and then the tool

Tool length

measure

Tool life

Part 1 Programming

administration

function

Additional offset

memory A

Additional offset

memory B

Additional offset

memory C

to be measured is fixed at the same mechanical fixed position manually.

The length offset value of this tool is input regarded as an offset as long

as the Z INPUT is pressed.

The tool is divided into several groups within the tool magazine. Specify

a life to the tool of each group, when the tool of each group is used, the

accumulation is regarded as a criterion of the tool life for the tool

machining time or machining frequency. After the tool has been reached

the tool life, namely, the next tool is automatically selected within the

same group in advance

Tool position offset, the number of the cutter compensation can be

extended up to 64.

Tool position offset, the number of the cutter compensation can be

extended up to 64

The number of the tool compensation can be extended up to 184.

Once when the number of one-digit of 1~9 followed F is specified, the

74 F1-digit feed

External motion

function

Canned cycle A

(G80,G81,G82,G8

4,G85,G86,G89)

Canned cycle B

(G73, G74, G76,

G80~G89)

Inch/Metric

conversion (G20,

G21)

feedrate of corresponding number is then set. Specify the F0 is a rapid

traverse rate, the speed change signal issued from the side of machine,

the feedrate of the selected number can be increased or decrease by

the MPG.

After the X or Y axis is positioned, the external motion signal is output

by using the G81 command code, and G80 cancels this function

therefore.

Six canned cycles can be performed, for example, the drilling cycle,

tapping cycle and boring cycle etc.

Twelve canned cycles can be performed, namely, the peck drilling

cycle, finishing boring cycle, tapping cycle and counter-tapping cycle.

The inch or metric input can be switched by the G code.

G20: Inch input G21: Metric input

Specify G02 (or G03), the feedrate specified with F code is achieved an

optional arc interpolation within the rage of 0°～360°.

G02: Clockwise (CW) G03: Counterclockwise (CCW)

Circular arc

Interpolation

(G02,G03)

80 Sine curve In the helical interpolation command, when one axis within an arc plane

Page 21

Chapter two Specification

interpolation does not move (this axis is treated as an imagination axis), the other 2

axes can be performed a sine curve interpolation.

The circular

compensation is

performed using

radius R

programming

External

deceleration

External workpiece

number index A

84 External data input

In the arc interpolation, the radius value R instead of I, J and K is

directly specified a radius to simplify a program. The arc more than or

less than 180° can be performed.

The mechanical vibration during stopping at the end of stroke which can

be reduced to the least by this function, and the valid stroke can be

increased to the maximum, the additional axis does not an external

deceleration function. (Selected function)

Input any of the program number from 1~31 to NC from the machine

side and these programs (Selected function) are selected from NC

memory.

Transfer the data to NC from an external specified operation such as

the machine side, the input data are shown below:

(1) External workpiece number index C

(2) External tool compensation C

(3) External alarm information

Part 1 Programming

Automatical

acceleration of

cutting feed

Additional skip

block selection

87 Skip function (G31)

Restarting of

program

Single direction

position

(4) External operation information

The cutting feed and manual consecution feed can be set by the

parameter, the constant is accelerated or decelerated with exponential

at the time of 8ms～4000ms.

The 1~9 digits followed with the switch command / of the block, 9 skip

optional program switch can be set at the side of machine, when one

optional program skip switch n is turned on, the block with / n is

skipped.

When the X, Y, Z, the 4

or the 5th axis commands are followed with

G31, they are performed a linear interpolation as G01. When this

command is performed, if it skips to this signal from the external input,

the rest of part of this command is stopped to perform the next block.

Specify a sequence number to be restarted, and the restart is

performed from here.

The positioning can be performed from unique direction to eliminate an

interval for realizing a precise position.

Storable program

Superaddition of

number

96 programs can be added at the standard program, totally 191

programs.

Page 22

GSK983Ma Milling Machine Center CNC System User Manual

91 Scaling

The tool path specified in program can be scaled up or down with the

range of 0.001～99.999.

The pulse only uses a MPG which can be performed a tool movement

92 MPG insertion

Automatic corner

Part 1 Programming

modification

Manual optional

angle feed

Sequence number

comparative stop

Operation time

display

Menu switch

overlapped with the automatical operation command in the case of the

machining is consecutively performed.

In the state of cutter compensation, when the inner corner is cut, the

modification can be automatically added to perform a low-speed

machining within the set area.

Set an angle corresponding with the positive direction along X axis on

the calibrated scale of machine operator panel, the JOG feed is

performed on the setting direction by using the start button. In the XY

plane, this function is only valid of 5° interval increment with the range

of 0°～360°. (Selected function)

The block is same as the preset sequence number during the program

performance, after this program has been performed which becomes a

stop state of single block, and this function is used to check a program.

The NC automatic operation time in second, minute or hour can be

displayed on the LCD.

The switches on machine operation panel are replaced by the setting

operation by the MDI & LCD which can be controlled the ON/OFF of

some functions.

User macro

There are two function limits, one is A, the other is B. It belongs to the

program A, B

manufacturer and the inherent function of the user.

99 Graphic display Tool path can be described on LCD

The MPG installed on the machine panel can be performed a

micro-feed for the machine, MPG issues 100 pulses for each revolution,

100 MPG

the movement amount for each pulse can be shifted 1, 10 and 100 folds

based upon the signal of machine side.

PLC MODEL—B can be used.

101 PLC

PLC MODEL-B Numbers of input 192 points Numbers of output 128 points Steps of program Up to 5000 steps

Page 23

Chapter Three Programming

3.1 What is Programming

The CNC machine moves in terms of the compiled program. When the parts are machined in NC,

the tool path and other machining conditions should be edited into this program, and this program is

regarded as part program.

The process from part drawing to the machining program is being performed by NC, as follows:

Part drawing Machining plan Part programming NC performs machining

(1) Confirm the NC machining range and the selected NC machine. (2) Confirm the installation of the workpiece material on the machine and select

miscellaneous motion, based on the NC rule. Usually, these commands are written into block.

the required jig and tool.

(3) Cutting sequence (The cutting depth and tool path of machining process type,

tool start, rough cutting and finish cutting).

(4) Select the cutting tool and tool jig, and decide their installation position on the

machine.

(5) Cutting condition (Spindle rotation speed, feedrate or the coolant ect.).

The part program, reads the controllable tool path and the NC command from machine

The part program will describe in this chapter.

Part 1 Programming

3.2 Program Structure

The program is divided into main program and subprogram. Usually, the NC moved based on the

command of main program, when the command of subprogram calling on the main program, the NC

is then moved based upon the command of subprogram.

When the main program return command is performed in the subprogram command, NC returns

to the main program then moves in terms of the command of main program.

In NC memory, 95 main programs and subprograms can be stored separately, and one of the

main programs is selected. NC machine can be moved based on its command.

Page 24

GSK983Ma Milling Machine Center CNC System User Manual

Main program Subprogram

Part 1 Programming

Command 1 Command 2

┊ ┊ ┊ ┊

[Rotor program

command]

Command n

Command n+1

┊ ┊ ┊ ┊ ┊

[Return to the main

program command]

Note: The number function (selection) of the additional storage program is selected. The program

numbers to be stored is added to 191.

Refer to the [4 Operation] for the storage and selection methods of a program.

Command 1 Command 2

┊ ┊ ┊ ┊ ┊ ┊ ┊ ┊ ┊ ┊ ┊

3.2.1 Block

The program is composed of several command, a command unit in a program is called the block.

Distinguish the blocks using end code. EOB code is indicated with “;”.

For example: XXXX； XXXX； XXXX；

Note 1: The maximum character in one block is free. Note 2: EOB code: EIA code uses CR, ISO code uses LF.

3.2.2 Program Word

The element composed with block is program word. The program word consists of the address

and its following digit. The + or – can be performed before the digit.

X - 1000

Address Digit

Program word

The address is indicated using one of the A~Z which describes the meaning of its following

umbers, the address and meaning in this NC can be used as follows. Same address may have

different meanings based on the different preparation function command in program.

Page 25

Chapter Three Programming

Name Address Meaning

Program number

Sequence

number

Preparation

function

Coordinate word

Feed function F Feedrate specification

Spindle function S Specify a spindle rotation speed

Tool function T Specify the tool number or tool offset number

function

Offset number

Dwell

Specify a program

number

Specify a

sequence number

Times of repetition L

Parameter

For example, the following block can be formed using these program words.

； N— G— X— Y— F— S— T— M— ；

Sequence number

Preparation function

In the following blocks, one row means one block, one grid of a block means a program word.

Name S57.10.10

Program number 0（：）

2002

/ N G X Y Z A/B/C C/V/W R/I J K F S T M B H/D LPQ

：（ISO）/O（EIA）

N Sequence number

X、Y、Z

A、B、C、U、V、W

R Arc radius

I、J、K

M Specify the ON/OFF of the machine tool sideMiscellaneous B Such as the table index

H、D P、X

P Specify a subprogram number

P、Q、R

Coordinate number

Feed function

Spindle function

Program number

Command motion mode (linear, circular arc etc.)

Movement command of coordinate axis Movement command of additional axis

Coordinate of circular arc center

Specify an offset number Specify a dwell time

Specify a sequence number; the program is repeatedly performed in this number. The repetition count of program, the repetition of canned cycle.

Parameter of canned cycle

Tool function

Micellaneous function

Pag

e /

Part 1 Programming

；

N20 G92 X

100.0 Y 200.0 Z 300.0

N21 G00 X

196.0 Y 315.0 Z 500.0

N22 G01 F10.0

S400 T15 M03

；

Note: CR（EIA），LF（ISO）

Page 26

GSK983Ma Milling Machine Center CNC System User Manual

3.2.3 Input format

Each program word is composed of a block which must be specified in terms of the following

description. This input format of this system is a changeable block format, therefore, both the number

of program word of a block and the character number of one program word which can be changed, in

this case, it is very convenient for programming.

Part 1 Programming

(1) Input in metric NO4·G02·XL+053·YL053·ZL+053·

RD053 D02

αL+053·βL+053· ·F050· ·

ID053·JD053·KD+053 H02

S02 T02

· ·B03·M02；

S04 T04

(2) Input in inch NO4·G02·XL+044·YL+044·ZL+044·

RD044 D02

αL+053·βL+053· ·F032· ·

ID044·JD044·KD044 H02

S02 T02

· · B03·M02；

S04 T04

Note 1: α or β is one of the additional axes A, B, C, U, V and W. Note: The addresses and meanings which are described above format are shown below:

X L + 0 5 3

Three digits following with the decimal point

Five digits before the decimal point

Leading zero can be omitted

With symbol

Absolute or incremental

Address

J D 0 5 3

Five digits before the decimal point

Leading zero can be omitted

Incremental with symbol

Address

Three digits following with the decimal point

For example: when the tool move to the 50.123mm along X-axis at the rapid traverse rate, and its movement command is as follows:

Page 27

Chapter Three Programming

G00 X50 . 123 Three digits following with the decimal point Five digits before the decimal point is 00050.

Leading zero is omitted

G00 can not be omitted (G00 specifies a rapid feed) even if the leading zero is omitted.

Note 3: When an address is specified twice at one block, in principle, the last command is enabled, and

the alarm does not perform.

For example: G01 M03 S200 M08； In this case, M08 is enabled, and the M03 is invalid. G code of each group in a block is valid which is

specified at last. G90/G91 is in a block, which is separately valid in its specified place. (See the Section 3.3.8)

For example: G90 X10.0

Absolute Incremental

R is always valid when the R and I, J or K are specified simultaneously in circular arc interpolation

command, which is regardless of the command sequence.

Note 4: F050 can be changed into F051 in metric input format. Refer to the [Section 3.4.3 for the feedrate x

1/10]. Note 5: P or Q is omitted in the above-mentioned format due to it owns several meanings. Note 6: When inputting in decimal point, refer to the [Section 3.2.4 for the decimal point input]. Note 7: The number input in metric, namely, X, Y, Z, A, B, C, U, V, W, I, J, K, Q, and R are set by parameter

which multiplies 10 times.

RD052

XL+052·YL+052·ZL+052·αL+052·βL+052·

ID052·JD052·KD052

(α or β is A, B, C, U, V or W) (input in metric), refer to the [Section 3.3.2.2, the input unit multiplies 10] Note 8: Refer to the [Section 3.3.2.2, the input unit multiplies 10].

G91 Y20.0 ；

Part 1 Programming

3.2.4 Decimal point programming

Numerical values can be entered with a decimal point for this device. A decimal point is used for the number of which is regarded as a unit of the distance, time or speed. However, some addresses can not input in decimal point, the position of decimal points are indicated the one of the mm, inch, degree or second.

X15.0 X15mm or x15inch

F10.0 10mm/min or 10inch/min G04X1. Dwell 1s B90.0 B90deg

Decimal points can be inputted the following address:

X、Y、Z、A、B、C、U、V、W、I、J、K、R、Q、F

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

Note 1: When the dwell is specified, X, but P, can be input in the decimal point. (Because the P can be

specified in the sequence number)

Note 2: Change the position of decimal point using the G code, the G code should be specified in

advance even in the same block. G20: (Specify in metric)

X1.0G04；……The X1.0 does not indicate a time instead of a movement distance (inch), as for the

X10000G04, its dwell time of the consequence is 10 seconds. When G04 is inputted, the display becomes 10.0 from 1.0. G04X1.0: …… is regarded as G04X1000, the dwell time of its consequence is 1 second.

Note 3: Note that it is a large difference with or without decimal point; the program is different from the

electronic-computer.

G21: (Specify a metric) X1.……X1 X1……X0.001

G20: (Specify an inch) X1.……X1inch

Page 28

GSK983Ma Milling Machine Center CNC System User Manual

X1……X0.0001inch

Note 4: The numbers can be used with or without the decimal point

X1000 Y23.7； X10 Y22359；

Note 5: If the value specified is less than the value of the least input increment, and this value is then

omitted. When the X1.23456 is specified, it is treated as X1.234 in metric, and it is regarded as

1.2345 in inch. The accumulation error occurs when the incremental value is specified, the accumulation error does not issue but its error omitted when the absolute value is specified.

The specified digits can not exceed the maximum allowance digits. X1.23456789……has an error due to it exceeds 8 digits. X1.2345678……does not an error because it is within the 8 digits.

Note 6: When a number with a decimal point is input which is converted into an integer of the least

Part 1 Programming

number is more than 8 digits.

input increment.

(For example) X12.34 12340 (Input in Metric)

The converted integer should be checked, still.

(For example) X1234567.8 X1234567800 (Input in Metric). The alarm may occur due to this

3.2.5 The maximum command value

Note that the maximum commanded value range of NC device is expressed in the following table instead of the mechanical movement range of NC machine. For example, the movement of X axis for the NC device is about 100m (Input in Metric). As for a certain machine, the stroke distance of X axis may limit within 2m, as the feedrate. The cutting feedrate of NC device can be set to 30m/min, but the NC machine side may limit within 6m/min. In the actual programming, refer to this manual and the manual issued from the manufacturer at the same time. Program can be performed after comprehending the special machine program fully. The maximum command value of each address is shown below:

Table 3.5 The basis address and the range of command value (the additional selection

included)

Input in inch

±3937.0078in

0.01inch/min

1200.00inch/

0.01inch/min

1200.00inch/

Name Address

Program

number

Sequence

number

Preparation

function

：（ISO） O（EIA）

X、Y、Z、I、

Coordinate

word

J、K、Q、R、 A、B、C、U、

V、W

Feed per

minute

Feed per

minute

(feedrate

1/10)

(Parameter

setting) Spindle function

Tool function T

Miscellaneo M

Input in mm

Output in mm

1～9999

0～99

±99999.999mm

±99999.999°

1 mm/min～

30000mm/min

0.1 mm/min～

30000.0mm/min

Input in inch

Output in mm

Input in mm

Output in inch

As the left As the left

″ ″ ″

±3937.0078inc

±99999.999°

0.01 inch/min～

1200.00inch/mi n

0.01 inch/min～

1200.00inch/mi n

±99999.999mm

±99999.999°

1 mm/min～

30000mm/min

0.1 mm/min～

30000.0mm/min

0～30000 0～30000 0～30000 0～30000

0～9999

0～99

″ ″ ″ ″ ″ ″

Output in

inch

As the left

±9999.999°

～

min

～

min

Page 29

Chapter Three Programming

us function

Dwell X

Dwell P

0 s～

99999.999s

0ms~99999999

″ ″ ″

Sequence

number

1～9999

″ ″ ″

setting Times of repeated

Offset

number

D、H 0～184

1～9999

″ ″ ″

The 2nd

M.S.T

0～999

″ ″ ″

function

3.2.6 Program number

This controllable device can be stored several programs into the NC memory, the program number is added to each program to distinguish these programs. Program number O The solution range is from 1 to 9999, the leading zero can be

omitted. (Program O0000 is used for transforming during the program replication.)

4 digits

Program starts at the beginning of the program number which ends till met the M02, M30 or M99.

The program of O1111 The program of O2222

01111………………………M02； 02222………………………M30；

M02 and M30: the end of main program. M99: the end of subprogram.

05555………………………M99；

The subprogram of O5555

Note 1: The “:” before the program number is replaced by “O” in ISO code. Note 2: The block of the code with optional block skip, such as /M02; /M30 or /M99 which can not treat

as an end of program.

Note 3: When the program number does not at the beginning of the program, the first sequence number

of this program (N…) can be replaced by the program number, but the NO program number is unallowable.

Note 4: If neither the program number nor the sequence number is performed at the beginning of the

program, the program number should be specified by the MDI & LCD panel when the program is stored to the memory.

Note: When several programs are performed, the EOB code without a flag is skipped after the 2

program and before its followed program, but the end of the previous program is finished by the ER (EIA) RO % (ISO), the program at its beginning should be used the EOB code.

Note 6: The run can be performed without a sequence number. However, the subprogram must always

have a program number.

Note 7: In some cases, the program numbers from 9000 to 9899 are used for the manufacturer, but the

user can not employ it.

Part 1 Programming

Page 30

GSK983Ma Milling Machine Center CNC System User Manual

Note 8: When the selection is performed by the manipulator, the program numbers 9900～9999 are used

as a manipulator data.

Note 9: M02, M30 or M99 does not performed at the end of a program, which is followed with ER (EIA) %

(ISO) or next program number 0, the end of program is set by BIT3 (NEOP) of parameter 306.

Note 10: When the maloperation is performed to cause the program is more than 4 digits, the program

may not call for the subprogram. In this case, the characters more than 4 digits are deleted. Deletion method: editing-> program lock open-> move the cursor to the program O-> insert the “EOB”-> move the cursor to the program O again-> press “deletion” key after the “EOB” is pressed.

3.2.7 Sequence number

Part 1 Programming

At the beginning of the block, the numbers 1～9999 within 4-digit followed with address N can be

specified the sequence number, and the sequence of its sequence number is optional. Either the sequence number can be performed for all the blocks, or the sequence number is added at the required place during program.

The sequence number should be continuously specified in the key place, for example, when a

new tool is used when it is used, or the working table index transfers to the new machining surface.

Note: For compatibility with other program formats of NC device, the sequence number N0 does not used

3.2.8 Skip to optional block

The slash /n (n=1～9) followed with numbers are specified at the beginning of the block, and

when the skip optional block switch n is ON, during the DNC operation or automatic operation, the block with /n corresponding to the switch number n is then ignored.

The block with /n is enabled after the skip optional block n is OFF. Namely, operator can alternatively select the skip block which with /n. The 1 in the /1 can be omitted, however, it can not be omitted when there are 2 or above skip optional block switches at the same block.

When the optional block switch is ON, the ignored area is shown below: ；/2N123G01X4……………………；N7856 Ignored area

For example：N100X100；

N101/2z100； N102/2/3X200； N103/3z200；

In the above-mentioned example, when the No.2 switch is ON, the blocks N101 and N102 are skipped; and when the No.3 switch is ON, the blocks N102 and N103 are skipped.

Note 1: The slash (/) must be placed at the beginning of the block, if it is placed at other places, the

information in which from / to the EOB code is then omitted, and the information in the front of the / is still effective.

Note 2: The TH and TV are still checked to the skipped part while the skip optional block switch is opened,

which is same as the switch OFF.

Note 3: The block to be skipped is identified when the memory transfers the information to the buffer. When

the block in front of the / has been read into the buffer, this block may not be ignored even if the optional block switch is ON.

Note 4: This function is enabled during the sequence number is indexed. Note 5: This function is disabled when this program is registered to the memory. The / followed with a block

can be read into a memory regardless of the switch of skip optional block.

Note 6: When the program is output from the memory, the program can be completely output regardless of the

state of skip optional block switch.

Note 7: Some skip optional block switches (from 1 to 9) may not used for some machines. So, it is necessary

to inquire the manufacturer how many switches can be used before operating.

Note 8: The system with the function of additional skip optional block, if a block is more than a flag of skip

optional block, the 1 of /1 can not be omitted, the /1 may specify in terms of the above-mentioned notes.

For example Wrong: //3 G00 X10.0；

Correct: /1/3 G00 X10.0；

Page 31

Chapter Three Programming

3.3 Dimension Word

The dimension word decides the movement of tool, which is composed some commands relative to the numerical value by the address of movement axis and the numerical value indicates the movement direction and quantity. They may vary from the absolute and increment modes. (See the Section 3.3.8)

Dimension word address Meaning

The address in the Cartesian coordinate system of each

Basic axis

Additional axis

interpolation

parameter

3.3.1 Controlled axis

X、Y、Z

A、B、C、U、V、W

R Specify a circular radius Circular arc

I、J、K

axis indicates the position of axis or the distance along the axis direction. The address of the 4

or 5th axis, which means an angle of rotation axis or a position and a distance of linear axis separately.

It means that the distance from start to circular center along the X, Y and Z axes or its parallel axis.

Part 1 Programming

The machine movement axis controlled by the NC system is called controlled axis. Each controlled axis can be called using the dimension word address of this device. The numbers of standard axis controlled by NC system are 3 axes (X, Y and Z) and can be

added to the 4

axis or the 5th axis.

The additional axis can be used any of the addresses, such as, A, B, C, U, V or W, it is better to

use A, B and C for the rotation axis, and use U, V and W for the linear axis.

The numbers of controlled axis can be controlled at the same block which is 3 axes. The number of simultaneously controllable axes can be added to 4 by the additional axis selection, the additional axis by controlling singly is only used for the simultaneous 3 axes control. The 3 axes control with an additional axis can be carried out, after the function of additional axis control is selected.

The numbers of simultaneous controlled axes

The numbers of

Simultaneous 3

controlled axes

axes selection

Simultaneous 3 axes selection +

Simultaneous 4

additional axes simultaneous

axes selection

controlled selection

3 4 5

Note 1: When an additional axis control function does not performed, if an additional axis (A, B, C, U, V or

W) is carried out, the No.17 alarm may occur. Note 2: The numbers of simultaneous axes are always 2 axes during the manual operation. Note 3: The following functions can not be performed when the system has the 5th axis.

① Never attempt to perform the thread cutting and synchronous feed. ② Never attempt to add the S4 digit analog output function (The spindle DA (digital-analog

conversion) module substitutes for the output analog function).

The constant surface speed cont③ rol function can not be added.

Do not perform the rigid tapping function④

The real⑤ -time spindle actual speed can not be displayed.

X、Y、Z

(The additional axis included)

The coordinate axes and motion symbols If the relationships between machine coordinate axis and tool movement symbol are provided

Page 32

GSK983Ma Milling Machine Center CNC System User Manual

with the machine, the serious mess may occur in programming, which the relative explanations have been described in the EIA RS-267-A or ISO841.

However, the following explanations should be noticed during programming: a) The program should be programmed based on the standard coordinate system (Right-hand

Cartesian coordinates);

b) In programming, suppose that the workpiece does not move but the tool moves round with the

workpiece

Part 1 Programming

3.3.2 Setting unit

3.3.2.1 The least input increment and the least movement unit

1) The least input increment (Input unit)

Input the least units of tool movement amount by the command, which are registered in mm, inch

or deg.

2) The least movement unit (Output unit)

The least movement units input to the machine are indicated in mm, inch or deg. Any of the

Page 33

Chapter Three Programming

following groups can be adopted.

The least input

The least

Input/output

increment

movement unit

Input in mm, output in mm 0.001mm 0.001mm

Input in inch, output in mm 0.0001inch 0.001mm

Linear

axis

Input in mm, output in inch 0.001mm

0.0001inch

Input in inch, output in

inch

0.0001inch

Rotation axis 0.001° 0.001°

Note: The increment system of rotation axis can not be converted in inch/metric system.

Whether the least movement unit is based on 0.001mm or 0.0001 inch which is determined by

the machine and it can be selected by the presetting BIT0 (SCW) of parameter 006.

The least input increment is 0.001mm or 0.0001inch can be selected by the G code or the

parameter setting of MDI & LCD panel.

G20 the least input increment of linear axis is 0.0001inch.

G21 the least input increment of linear axis is 0.001mm.

The G20 or G21 is unchangeable when the system is ON or OFF.

Part 1 Programming

3.3.2.2 10 folds input unit

The least input increment in mm can be changed into 0.01mm using the BIT 1 of parameter 006,

which the unit in inch can not be changed.

Address

Dimension word

Rotary axis

Dwell time

X、Y、Z、Q、R、I、J、K、U、V、W

A、B、C

It can not be changed in the following cases:

a) When the input is different from the above-mentioned dimension word.

b) Display unit

c) The maximum command value range.

d) Increment feed unit and manual feed unit

e) Offset input

The least input increment

Input in mm Input in inch

0.01mm

0.0001inch

0.01° 0.01°

0.01s 0.001s

f) Others

Note 1: The input unit is either 0.0001inch or 0.001mm in the latter explanations in the manual. Note 2: The display unit changes into 0.01mm or 0.01deg by setting the BIT 2 (MDL) of parameter 006.

Page 34

GSK983Ma Milling Machine Center CNC System User Manual

3.3.3 The maximum stroke

The maximum stroke can be commanded in this device is shown below:

Input/output in

±99999.999mm

±99999.999°

Part 1 Programming

Note: The above-mentioned strokes vary from one machine to another.

3.3.4 Program origin and coordinate system

The program origin and coordinate system can be affirmed during programming. Usually, some

point on workpiece is set to a program origin.

Input in inch/

output in mm

±3937.0078inch

±99999.999°

Input in mm/ output

in inch

±99999.999mm

±99999.999°

Input/output in

inch

±9999.9999inch

±99999.999°

This is an example of that coordinate system is a workpiece coordinate system

3.3.5 The coordinate system and the machining start point

The workpiece coordinate system should be used while the program is sent to NC, tool and

program are operated from the start point. However, NC must be realized the tool’s coordinate value

at its start point by the G92 code (coordinate setting).

Page 35

Chapter Three Programming

3.3.6 Workpiece coordinate system

Several workpieces have been installed in machine, which the installation positions of these

workpieces are different; therefore, several workpiece coordinate systems should be applied. In this

case, 6 coordinate systems set in the machine in advance which can be selected by the 6 G codes

(G54～G59), the followed program is performed within the selected coordinate system, each

coordinate system can be determined by the distance from the reference position (the fixed point on a

machine) to its coordinate origin along with each axis, refer to the following figure.

The setting of workpiece origin offset, refer to the Section 4.4.13.

Part 1 Programming

When using the above-mentioned workpiece coordinate system, establish a coordinate system

without using a G92 code. The coordinate system set by G92 which is replaced by G54～G59.

Generally, G92 does not perform together with G54～G59.

Note: When using the coordinate system set by G54～G59, return to the 1st reference position after the

power is turned on, a workpiece coordinate system can be automatically set by G54, so the

automatic coordinate system need not to be set.

3.3.7 Reference (position) point

Reference position is a fixed on a machine tool to which the tool returns to the reference position

by the reference position return function. So, the program can not be started from a certain point on

workpiece coordinate system, but it can be started from a reference position. In this case, because

the reference position is a certain point on the machine, and the program is organized based upon the

point on the workpiece is regarded as an origin. Therefore, the tool returns to the reference position

Page 36

GSK983Ma Milling Machine Center CNC System User Manual

which must be described in workpiece coordinate system using G92 code.

Part 1 Programming

Program origin

Reference point

Workpiece

G92 Xα　Yβ ；

Note: When using the workpiece coordinate system set by G54～G59, G92 is unnecessary.

3.3.8 Absolute and incremental commands

The tool operation distance of each axis can be programmed in incremental or absolute

commands.

The operation distance can be programmed directly in a block by the increment command (G91).

Tool end position in a block is expressed by the coordinate value in the workpiece coordinate

system.

The above figure is carried out by the increment command program:

G91 X-60.0 Y40.0；

However, it is carried out by the absolute command program:

G90 X40.0 Y70.0；

In order to make a compatibility with other NC systems for the program, each address in block

can not changed the G90/91 command method.

Page 37

Chapter Three Programming

3.4 Feed Function (F function)

3.4.1 Rapid traverse rate

In the rapid traverse rate, the machine of each axis moves based on the specified speed.

In general, the rapid traverse rate is set by the manufacturer. (It is set by the parameter 092～095,

428, and from RPDFX to RPDF4).

Each axis of machine is separately moved, so these axes are moved from start to end which are

spent different time.

For example: When the rapid traverse rate of X and Y axes are separately 5000mm/min and

8000mm/min, and the operation programs are shown below:

G91 X2000.0 Y2000.0；

The X and Y axes on the machine tool are operated in the time of 24s and 25s where from start

to end.

The tool path on the above figure is shown below:

Part 1 Programming

The override control of rapid traverse rate can be carried out by the switch on the machine

operator panel. (F0, 25%, 50%, 100%) F0 is determined by the parameter 113 (SPDFL), and its unit

is not indicated by the percentage (%), instead of the mm/min or inch/mm.

3.4.2 Cutting Feedrate

Specify a tool cutting feedrate based upon the feed distance of each minute, the feedrate is

specified with F which is shown below:

F1（1mm/min，0.01inch/min）

F15000（15000mm/min）or F60000（600.00inch/min）。

Page 38

GSK983Ma Milling Machine Center CNC System User Manual

This feedrate is clamped at the upper limit (maximum) value

This upper limit value (the maximum value) can be set by the parameter 106 (FEDMX) by the

manufacturer, the feedrate is also controlled to the override from 0 to 200% (10% for each step) by

the switch from the machine operator panel. The claming of the upper limit speed is also effective to

the override feedrate. Specify the feedrate by F code is suitable for the rotation axis, too.

For example: Metric input F050

Inch input F032

Part 1 Programming

The decimal point input is available when inputting in metric or inch, and the decimal point are at

the place of degree/minute.

Metric input F12 0.12deg/min

Inch input F12 0.12deg/min

Metric input F12.0 12deg/min

Inch input F12.0 12deg/min

Note 1: Except the procedure of acceleration/deceleration in NC operation,

Note 1: The calculation error of the command feed where from NC holds the within ±2% of the command

feed, and the error is calculated by spending the time for measuring the movement distance which is

more than 500mm, where is followed with the NC steady state.

Note 2: Up to 7 digits can be performed for the F code, if the inputted feedrate is more than the upper limit

value, which will clamp at this value if the movement command is performed.

3.4.3 Feedrate decelerates to 1/10

The metric speed input can be changed into 1/10 by the setting of BIT 3 (FMIC) of parameter

006.

Description The least input unit Range

Feed/min. 0.1mm/min

F1～F150,000 (0.1 mm/min～15000.0mm/min)

3.4.4 Synchronous feed (feed/rev.)

Specify the feedrate based on the spindle feed/rev. G95 specifies the synchronous feed; and

G94 specifies the feed/min. (The movement amount in minute is a feedrate.)

Feed/min. Synchronous feed

Meaning Tool feed amount in minute

Address F F

G code G94 G95

Input in

1 mm/ min～30000 mm/ min

Solution

(F1～F30000)

Tool feed amount of spindle of

each revolution

0.01 mm/r～1000.00 mm/r

(F1～F100000)

Page 39

Chapter Three Programming

Input in inch

0.01inch/ min～1200.0inch/ min

(F1～F60000)

0.0001inch/r～100.0000inch/r

The feed in minute and the synchronous feed are generated a clamping at a certain

Clamping

feedrate, this clamping value is set by the manufacturer (the feedrate with override

value

can be clamped only.)

Override

The override (10% for each gear) from 0 to 200% is valid to the feed/min. and the

synchronous feed.

The clamping value is set based on the mm/min or inch/min. The synchronous feedrate changes

into mm/min or inch/min as the following equations.

fm=fr×R

Wherein, fm: The unit of the feedrate per minute is mm/min or inch/min

Fr: The unit of synchronous feedrate is mm/r or inch/r.

R: The unit of spindle speed is r/min.

Note 1: G94 and G95 are modal, which are valid after the specification is performed once till the other G

codes are generated.

Note 2: The synchronous feed must be performed with the spindle installed a position encoder.

Note 3: It also can be used when the position encoder speed is up to 1r/min., the feedrate maybe irregular,

which does not affect the machining. However, the abnormity can not continue, otherwise, the

unexpected behavior may occur along the decrease of the speed.

Part 1 Programming

3.4.5 F1-digit Feed

One-digit number from 1 to 9 F is specified after F, namely, the feedrate corresponding this

number is set. Each number has been set its corresponding parameter in advance. The F0 is

regarded as a rapid traverse rate. After the F1-digit feedrate switch installed on the machine panel is

shifted ON, the feedrate corresponding to the number currently selected can be increased or

decreased by rotating the MPG.

The increment/decrement of feedrate

MAX

100

/per scale of the MPG]

F=△

Wherein:

: It is used for the feedrate upper limit of F1～F4 ------ it is set by parameter #171～

MAX1

174(FIDF1～4);

: It is used for the feedrate upper limit of F5～F9------ it is set by parameter #1751～

MAX2

179(FIDF5～9);

X: any number among 1～127 set by parameter.

The feedrate set or altered is kept even while the power is OFF. The current feedrate is displayed

on the LCD.

Page 40

GSK983Ma Milling Machine Center CNC System User Manual

3.4.6 Automatic acceleration/deceleration

When the feed is started or stopped, at a certain time constant, the automatic acceleration or

deceleration is performed to avoid the mechanical system vibration occur. Therefore, the acceleration

or deceleration may not perform during programming.

The pointed corner can not be machined due to the automatic acceleration or deceleration, the

dwell command code (G04) is added between two blocks to machine a sharp corner.

Part 1 Programming

The actual tool path is fit to the programmed one after the dwell command is inserted. The faster

the feedrate rotates, the bigger the acceleration/deceleration tome constant occurs, the bigger the

corner error is.

Note 1: The feedrate changes between the blocks of the specified different movement, as follows:

The previous block

New block

Positioning × × ×

Cutting feed × ○ ×

Not move × × ×

×: The next block is performed after the command speed is decelerated to zero.

○: Continue to perform the next block, so that the feedrate is not changed widely.

Note 2: The deceleration is performed on each axis separately (X or Z axis) and the feedrate of each axis

may occur between blocks. Therefore, the actual tool path does not match for the programmed

path. For example, if the tool only moves along X axis in a block, and along Z axis in the next

block, it is then decelerated along with the X axis direction nearby the corner, and then

accelerated along the Z axis direction. The actual tool path is shown below:

Positioning Cutting feed Not move

In the circular arc interpolation, the actual arc radius should be less than the programmed one (refer to

the appendix), this error can be carried out by reducing the time constant of acceleration or deceleration as

much as possible.

Page 41

Chapter Three Programming

3.4.7 Automatic Corner Modification

If the tool is performed a tough machining with tool compensation based on the program feedrate

within the inner corner and inner circular arc area, the tool cutting overload may occur. This function

can be automatically decrease the feedrate to reduce the overload of tool in the above-named area,

so than the smooth machining surface can be carried out.

3.4.7.1 The automatic modification of inner corner

1) Working conditions

When two blocks (the previous one and the latter one) are available for the following conditions,

the feedrate can be achieved the automatic modification.

a. G codes of group 01 are G01, G02 or G03.

b. In the offset mode, the value of offset does not 0.

c. The offset should be performed within the machining corner

d. The axis moves along with the offset surface.

e. G41 and G42 command codes are not performed in the following blocks.

f. G41 and G42 command codes are not performed in the previous blocks. Or, if the two

blocks are performed, this block does not start.

g. The inner corner is less than the θ set by parameter in advance.

The angle of programmed path

(I) Straight line to straight line

Part 1 Programming

(II) Straight line to arc

(III) Arc to straight line

Page 42

(IV) Arc to arc

Part 1 Programming

When θ≤ΘP, which is treated as an inner corner. The value of θP is set by parameter (NO·335)

GSK983Ma Milling Machine Center CNC System User Manual

(1°≤θP≤179°). Suppose that the θ and θP are equivalent, the estimation error less than 0.001° may

occur.

2) Operation range

After the corner is affirmed to an inner one, the feedrate is modified from the corner range from

Le in the corner intersection block to another. The straight line distance between Ls and Le is the

point from tool center path to the corner intersection. Le and LS are separately set by the parameters

(#355 and #356)

The feedrate is modified within the range from a to b.

As for the circular arc, this modification is effective for the EOB based on the following conditions.

① Distance within Le.

Page 43

Chapter Three Programming

The start and end points of circular are located on the same quadrant or the start is situated at ②

the adjacent one of the end quadrant.

The modification function of the start of the block is enabled based on the following conditions.

Distance within Ls.①

The start and end points of circular are located on the same quadrant or the end is situated at ②

the adjacent one of the start quadrant.

(For example) The circular disk

Part 1 Programming

The feedrate is modified from a to b and c to do for the program of an arc.②

3) Modification value

The modification value is set by the parameter #334. 1≤AOVOR (each gear 1%) ≤100 (%)

It is also enabled for the dry run and the F1-digit command. In the case of the F4-digit command,

the actual feedrate is as follows:

Fx (AOVOR) × (Feedrate modification)

4) Whether the inner corner modification is enabled

The inner corner modification can be determined by the G code, in the group 15, add the G62

between the G91 and G64, refer to the following table. These G codes are related with the exact stop

check mode.

Exact stop check Inner corner modification

G61 Enabled Disabled

G62 Disabled Enabled

G64 Disabled Disabled

Note 1: G64 state is performed when the power is turned on or off.

Note 2: G09 must be specified if the exact stop check is performed in the mode of G62.

Note 3: The inner arc cutting feedrate change is always effective which is not affected by the G codes,

refer to the Section 4.7.2.

3.4.7.2 The change of inner side arc cutting

In the case of the inner side arc offset cutting, the feedrate of programmed path is specified by

Page 44

GSK983Ma Milling Machine Center CNC System User Manual

the F code, and the actual feedrate is F×RC/RP (wherein, RC is a radius of tool center path; RP is a

radius of program path).

This change is also valid to the dry run and F1-digit command.

(For example 1)

Part 1 Programming

However, if RC is much smaller than RP, namely, RC/RP=0, the tool may stop then. Therefore,

after the least deceleration rate is set, when RC/RP≤AOVMDR, the actual feedrate is FX (AOVMDR).

The MDR is determined by the parameter #333. 1≤AOVMDR (each gear 1%) ≤100, which is also

used for F1-digit and the dry run. The acceleration rate of inner corner automatic modification is not

affected by the AOVMDR.

Note: If the inner side arc cutting is overlapped at the inner corner automatic modification, in this case, the

actual feedrate is F×

× (corner modification) × (feedrate override).

3.5 Preparation Function (G function)

Two numbers following address G determines the meanings of the command for the concerned

block.

G codes are divided into the following two types:

Type Meaning

One-shot G code The G code is effective only in the specified block.

Modal G code

(Example) G01 and G00 are modal G codes.

The G code is effective until another G code of the same group is

specified.

G01 X ；

Y ； G01 is valid in this range

X ；

G00 Y ；

Page 45

Chapter Three Programming

Table 3.5.1 G codes

G code Group Function

G00 Positioning (rapid traverse)

G01 Linear interpolation (feed)

G02 Circular interpolation CW (Clockwise)

G03

G04 Dwell

G07

G09 Exact stop check

G10

G17 XY plane selection

G18 ZX plane selection

G19

G20 Input in inch

G21

G22 Stored stroke limit ON

G23

G27 Reference position return check

Circular interpolation CCW (Counterclockwise)

Speed Sine curve control (Specify an imagination

axis)

Offset setting, workpiece zero offset setting

YZ plane selection

Input in mm

Stored stroke limit OFF

Part 1 Programming

G28 Return to the reference position

G29 Return From reference position

G30 2nd, 3rd and 4th reference position return

G31

G33 01 Thread cutting

G40 Tool compensation cancel

G41 Tool compensation – left side

G42

G43 Tool length compensation + direction

G44 Tool length compensation - direction

G49

G45 Tool position offset increase

G46 Tool position offset decrease

G47 Tool position offset double increase

G48

G50 Scaling off

G51

Skip cutting

Tool compensation – right side

Tool length compensation cancel

Tool position offset double decrease

Scaling on

G54 Workpiece coordinate system 1 selection

G55

Workpiece coordinate system 2 selection

Page 46

GSK983Ma Milling Machine Center CNC System User Manual

G56 Workpiece coordinate system 3 selection

G57 Workpiece coordinate system 4 selection

G58 Workpiece coordinate system 5 selection

G59 Workpiece coordinate system 6 selection

G60 00 Single direction positioning

G61 Exact stop check mode

G62 Automatic corner modification valid

Part 1 Programming

G64

G65 00 Simply call the Marco command

G66 Marco command modal call

G67

G68

G69

G73 Peck drilling cycle

G74 Counter tapping cycle

G76 Fine boring

G80 Canned cycle cancel

G81 Drilling cycle, spot boring

G82 Drilling cycle, counter boring

G83 Peck drilling cycle

G84 Tapping cycle

G85 Boring cycle

Cutting mode

Macro command modal call cancellation

Coordinate rotation ON

Coordinate rotation OFF

G86 Boring cycle

G87 Counter boring cycle

G88 Boring cycle

G89

Boring cycle

G90 Absolute command

G91

Increment command

G92 00 Setting for work coordinate system

G94 Feed per minute

G95

Feed per rotation

G98 Return to the initial point in canned cycle

G99

Return to point R in canned cycle

G96 Constant surface speed control

G97

Constant surface control cancel

G180 Cancel the rigid tapping in canned cycle

G184

Rigid tapping cycle

Page 47

Chapter Three Programming

Note 1: The G code with is a start G code of each group. Namely, when the power is turned on or the

resetting key is controlled when the system parameter of G code is specified, the G codes are set

up therefore. As for the G22 and G23, the G22 is selected when the power is turned on, G22 or

G23 (one of them is effective before resetting) is then set up.

The selection of start G codes state, such as G00, G01, G43, G44, G49, G90, G91 or G94，G95, which

is determined by the parameter 008.

The effective one between G20 and G21 is selected before the power is turned off or the resetting

key is pressed.

Note 2: G codes in group 00 are not modal, which are only valid in its block.

Note 3: When the G codes in the above table are specified, or when an undefined optional G code is

specified to a control device, the alarm (No.0/0) may occur, but the G38 and G39 are ignored.

Note 4: Some G codes can be specified at the same block even if they are not shared the same group.

When two or more G codes in a same group are specified at the block, the last specified G codes

are effective.

Note 5: In the canned cycle mode, if any of the G codes in group 01 are specified, the canned cycle will

automatically cancelled, and the system is then on the state of G80. However, G codes in group

01 are not affected by any G codes in the canned cycle.

Note 6: G70 and G71 can be separately replaced the G20 and G21 (particular G code) by setting the BIT 5

(GSP) of parameter 008.

Note 7: G codes of each group are displayed.

Part 1 Programming

3.5.1 Plain Selection (G17, G18, G19)

Select a plain for circular interpolation and tool compensation by the commands.

G17……XY plain

G18……ZX plain

G19……YZ plain

The movement command is regardless of the plain selection of G17/G18/G19, for example,

when the G17 Z _ is specified, the Z moves.

3.5.2 Positioning (G00)

Use this code, tool positioning is performed at each point of address X, Y, Z or A, B, C, U, V and

W programming, the coordinate value must be specified in the absolute command. The distance from

start to end must be specified in the increment command, and the tool is separately moved at the

rapid traverse rate of each axis, the tool path in positioning is not always a straight line.

Two axes (2 addresses) can be programmed at the same time in a block, but, only one can be

performed for the 4

axis.

Specify a G00 positioning G00α_____β_____；

（α·β=X、Y or Z）

For example: the rapid traverse feedrate is: X axis 9600mm/min

Page 48

GSK983Ma Milling Machine Center CNC System User Manual

The program of Y axis in 9600mm/min

G00G91 X25.0 Y-10.0

Part 1 Programming

Note 1: The rapid traverse feedrate in G00 command is set for each axis by the machine tool manufacturer,

therefore, it can not be specified by the a programming.

In the positioning of G00, the tool speeds up from the start till to the preset speed, which may rapidly

move thereafter till decelerate to the end, and the next block is performed after confirming the “appropriate

position” sequently. (Note 2)

Note 2: The “appropriate position” means that the motor feed is within the specified range (This range is

determined by the machine tool manufacturer).

Note 3: If the system is selected to a simultaneous 3 axes function which the following movement

command can be specified is shown below.

G00 X___Y___Z___；

In this example, X, Y and Z axes positions the tool to the specified location at the specified speed at the

same time.

When the system selection has a simultaneous control function of additional axis, both the address X, Y

and Z and the additional axis address are commanded. Three or four axes can be operated simultaneously if

the commands are performed.

For example: X500.0 Y300.0 Z25.0 B20.0；

3.5.3 Single Direction Positioning (G60)

The exact positioning without an offset can be finally positioned from one direction.

Start

End

(The last position direction is from right to left)

The G00 is replaced by G60: G60 α____β____γ____δ____；

(The α, β and γ= X, Y and Z or additional axes A, B, C, U, V or W, which are controlled in 3 axes

or 4 axes. the simultaneous control occasion for the 2 axes and 3 axes are included an additional

axis).

An overrun and a positioning direction are set by parameter. Even when a commanded

positioning direction coincides with that set by the parameter, the tool stops once before the end

point.

Page 49

Chapter Three Programming

Note 1: G60, which is a one-shot G code.

Note 2: During canned cycle for drilling, no single direction positioning is effected in Z axis.

Note 3: No single direction positioning is effected in an axis for which no overrun has been set by the

parameter

Note 4: When the move distance 0 is commanded, the single direction positioning is not performed.

Note 5: The direction set to the parameter is not effected by mirror image.

Note 6: The single direction positioning does not apply to the canned cycles of G76 and G87

3.5.4 Linear interpolation (G01)

G01α____β____F____；

Part 1 Programming

(α. β=X, Y, Z, A, B, C, U, V or W. Additional axis is carried out a simultaneous control with other

axes).

Actually, it is specified a linear interpolation mode. The values from α and β are defined a tool

movement distance, which is treated in the mode of the absolute and increment based on the current

state of G90/G91. The feedrate is specified by F code, and the F code is modal.

Program example: （G91）G01 X200.0 Y100.0 F200.0

Y End

0 Start 200.0 X

Specify the feedrate by F code is a tool movement speed, if the F code does not specify when

the power is turned on; the feedrate is then regarded as 0.

The movement command with simultaneous 3 axes control function is shown below.

G01 X____Y____Z____F____；

Simultaneous 3 axes linear interpolation can be performed by this command.

When the additional simultaneous control function is selected, The X, Y or Z can be replaced by

the 4

axis address (A, B or C), in this case, the simultaneous 3 axes control of the 4th axis can be

carried out.

For example: G01 X500.0 Y300.0 B20.0 F10.0；

The following commands can be performed when the system has an optional simultaneous 4

Page 50

GSK983Ma Milling Machine Center CNC System User Manual

axes function.

G01α____β____γ____δ____F____；

Wherein α, β, γ, δ= X, Y, Z, A, B, C, U, V or W.

Note 1: The feedrate of each axis direction is as follows:

ββ F f；

G01αα

Feedrate of α axis direction: Fα=

Part 1 Programming

Feedrate of β axis direction: Fβ=

Note 2: The feedrate of rotation axis can be determined by degree/minute (metric input: F050, Inch input:

For example: G91 G01 B90.0 F300；

Note 3: The 4th axis is included in the linear interpolation (Rotation axis A, B or C). The cutting feed unit

For example: G91 G01 X20.0 B40.0 F300.0；

Change the movement command unit (degree) of B axis into mm or inch, the machining time is as

follows:

F032).

(degree) comes into inch (or mm) and its feedrate is controlled in Cartesian coordinates of α—β

which is equaled to the speed specified by F code. Calculate the feedrate of rotation axis based

on the Note 1, and its unit becomes into degree/minute.

·f

4020

300

The feedrate of B axis is shown below:

=0.014907（min）

=268.3 deg/min

14907.0

Note 4: in simultaneous 3 or 4 axes, the calculation of Cartesian coordinate feedrate is same as the

simultaneous 2 axes control.

Note 5: The feedrate of rotation axis is up to 6000deg/min in metric or inch input, even if the specified

feedrate is more than the maximum speed, this speed must be fixed on the upper-limit value.

Page 51

Chapter Three Programming

3.5.5 Circular Interpolation (G02, G03)

3.5.5.1 Circular interpolation without an additional axis

The command below will move a tool along a circular arc.

Arc in the X——Y plane

G02 R____

G17 X____Y___ F____；

G03 I____J___

Arc in Z——X plane

G02 R____

G18 X____Z__ F____；

G03 I____K___

Arc in Y——Z plane

Part 1 Programming

G02 R____

G19 Y____Z___ F____；

G03 J____K___

Item Command code Meaning

G17 Circular arc on XY plane

1 Plain selection

2 Rotation direction

The G17 is effective as the start code of plane selection as long as the power is turned on.

CW or CCW is determined by left or right hand coordinates.

End

position

Distance from start to

Circular arc radius R Circular arc radius

G90 mode

G91 mode

center

Two axes from X,

Two axes from I, J

G18 Circular arc on ZX plane G19 Circular arc on YZ plane G02 Clockwise (CW) G03 Counterclockwise (CCW)

End position in workpiece coordinate

Y or Z

Distance from start to end

Y or Z

Distance from start to center

or K

system

The end point of an arc is specified by address X, Y or Z, and is expressed as an absolute or

Page 52

GSK983Ma Milling Machine Center CNC System User Manual

incremental value according to G90 or G91. For the incremental value, the distance of the end point

which is viewed from the start point of the arc is specified.

The arc center is specified by address I, J and K for the X, Y and Z axes, respectively. The

numerical value following I, J or K, however, is a vector in which the arc center is seen from the start

point, and is always specified as an incremental value irrespective of G90 and G91, as shown below.

End point (X，Y)

Part 1 Programming

Center

Start

I, J and K must be signed according to the direction.

The arc interpolation can be specified by address R instead of I, J or K. The command format is

as follows:

G02

X____Y____R____；

G03 There are two circular arcs during the arc interpolation (it is specified by radius) of R is used －

the arc is less than or more than 180°, as shown below:

Example for command:

1. The arc is less than 180°

G02 X6.0 Y2.0 R5.0；

Center

End point (Y，X)

Start

End point (Y，Z)

Start

Center

2. The arc is more than 180°

G02 X6.0 Y2.0 R-5.0；

Example of program

100

60 40

Origin

50R

60R

90 120 140 200

②

Y=50mm

End point

①

Y=50mm

Page 53

Chapter Three Programming

a) Absolute programming

（I） G92 Ｘ200.0 Y40.0 Z0；

G90 G03 X140.0 Y100.0 I-60.0 F300.0；

G02 X120.0 Y60.0 I-50.0；

（II） G92 X200.0 Y40.0 Z0；

G90 G03 X140.0 Y100.0 R60.0 F300；

G01 X120.0 Y60.0 R50.0；

b) Increment programming

（I） G91 G03 X-60.0 Y60.0 I-60.0 F300；

G02 X-20.0 Y-40.0 I-50.0；

（II） G91 G03 X-60.0 Y60.0 R60.0 F300；

G02 X-20.0 Y-40.0 R50.0；

Cutting feedrate of arc interpolation equals to the cutting feedrate specified by F code.

Note 1: In the arc interpolation, I0, J0 or K0 can be omitted.

Note 2: When the arc end point equals to the start point, and I, J and K are commanded a center. The X, Y

and Z can be ignored when the 360° arc (the whole circular) is programmed.

Note 3: Suppose that an arc radius 0 is programmed, the No.23 alarm may occur.

Note 4: The error between the specified feedrate and the actual tool feedrate is ±2% or less. When the

cutter compensation is performed, the actual tool feedrate is the speed of tool center path.

Note 5: If the address I, J, K and R are specified at a same block, the arc specified by R is effective and the

other are omitted.

3.5.5.2 Arc interpolation with additional axis

Part 1 Programming

Arc interpolation with an additional axis can be performed, the presetting axis (X, Y or Z) is

parallel with the additional axis, if the additional axis does not paralleled with any axis, the arc

interpolation can not be carried out. Specify a G code in the specified selection plane for the arc

interpolation command. Specify an address of an axis to perform the axes which is performed the arc

interpolation along the G code plane selection.

For example: Suppose that the additional axes U and W are separately paralleled with the X and

Y axes

a) G17X-Y-…………………XY plane

b) G17U-Y-…………………UYplane (U parallels with X)

c) G17Y-……………………XY plane

d) G17………………………XY plane

e) G17 X-Y-U-…………alarm

f) G18X-W-………………XW plane (W parallels with Z)

The arc center also can be specified by address I, J and K, which is same as the arc interpolation

without any additional axes. The parallel axes of X, Y and Z are separately used the addresses I, J

Page 54

GSK983Ma Milling Machine Center CNC System User Manual

and K.

The arc interpolation is specified by R is valid.

3.5.6 Sine curve interpolation

In the helical cutting command, the sine interpolation can be carried out when the arc

interpolation does not move (this axis is virtual axis) by specifying an arc command axis.

Part 1 Programming

The specification of the virtual axis is as follows: G07α0; (Specify α a virtual axis) G07α1; (Specify α a solid axis) (α= X, Y, Z or additional axis A, B, C, U, V and W) After the G07α0 is commanded, axis α is then regarded a virtual axis till the command G07α1 is

specified.

For the monocyclic Sine curve interpolation along Y-Z plane, X axis is a virtual one.

2+Y2

= r2 (r：Circular arc radius)

Y = rsin (

) Z (λ：Monocyclic Z axis movement)

Example for program

10.0

20.0

N001 G07 X0；

N002 G91 G17 G03 X-200 Y0.0 I-10.0 Z20.0 F100；

N003 G01 X10.0；

N004 G07 X1；

X axis is a virtual during the N002～N003 blocks.

In the N002 block, when the Z axis is regarded as a straight line, helical cutting command is then

Page 55

Chapter Three Programming

carried out, however, the X axis does not move, Y axis is moved when the Z axis is performed a Sine

interpolation.

In N003 block, the X axis does not move, the machine is on the state of dwell when the

interpolation ends.

Note 1: Virtual axis is only valid to the automatic operation, but the manual.

Note 2: The interlock, stroke limit and external deceleration are also effective to the virtual axis.

Note 3: The manual insertion is enabled to the virtual axis, too. Namely, this axis moves because the

manual insertion.

3.5.7 Thread Cutting (G33)

Threads with a specified pitch can be cut.

G33Z z F f；

Wherein Z: Thread length (Increment command) or thread end point (Absolute command).

f: Thread pitch

Part 1 Programming

The least input

Solution

increment

Input in mm 0.01mm

Input in inch 0.0001inch

F1～F50000（0.01mm～500.00mm）

F1～F500000（0.0001inch～50.0000inch）

The spindle speed limit is shown below:

1≤S≤

feedrate Maximum

or allowed position encoder speed

pitch Thread

Wherein:

S：Spindle speed (r/min)

Thread pitch: mm or inch

The maximum speed: mm/min or inch/min

Maximum command-specified feedrate for feed-per-minute mode or maximum feedrate that is

determined based on motor and machine tool restrictions including those related to motors,

whichever is smaller.

The speed under the position encoder: 4.000r/min (Position encoder A)

6.000r/min (Position encoder B)

Note 1: The spindle speed can be read consecutively from the position encoder installed on the spindle,

and converted into cutting feedrate-per-minute for cutting-feed.

Note 2: The converted cutting feedrate does not add an override but fixed on 100%.

Note 3: The converted cutting feedrate must be fixed.

Note 4: The feed hold is invalid during the thread cutting.

For example:

Page 56

Part 1 Programming

N20 G90 G00 X100.0 Y… S45 M03;

GSK983Ma Milling Machine Center CNC System User Manual

N21 Z200.0 ;

N22 G33 Z120.0 F5.0 ;

N23 M19;

N24 G00 X105.0

N25 Z200.0 M00;

N26 X100.0 M03;

N27 G04 X2.0 ;

N28 G33 Z120.0 F5.0 ;

Explanations:

N20, N21: Position the tool on the center of aperture, the spindle CW.

N22: The first thread cutting is performed, and its pitch is determined by address F.

N23: Spindle stops at a fixed position on the circle by M19. (M19: spindle stops at a fixed

position)

M24: Retract the tool along X axis direction.

N25: Move the tool on the hole: the program stops by M00, and the operator can adjust the tool

for thread cutting again.

N26: Put the tool center at the center of an aperture, the spindle CW.

N27: When the move command is short in N26 block, a dwell command should be added again

so that the spindle has enough time to be reached the rated speed.

N28: Perform the 2

thread cutting.

Page 57

Chapter Three Programming

3.5.8 Automatic reference position return (Reference position G27～G30)

3.5.8.1 Reference position return check (G27)

The point fixed on a machining plane is referred to as a reference position, if the reference

position return is performed manually, and the tool is then positioned at this point.

G27 command function check whether the tool is positioned at the reference position. G27α___β___；

(α, β: it is selected from addresses X, Y and Z and the additional axes A, B, C, U, V and W), tool

can be positioned at the reference position by these commands.

If the tool is on the reference position, the reference position return indicator with its

corresponding axis is then ON.

After the reference position is returned, if the M00 or M01 does not performed in the block, the

next block performs continuously. If each cycle does not need a reference position return, an optional

program skip function can be used then.

Part 1 Programming

If the system has a function of simultaneous 3 axes control, the G27 code can be expressed as

follows:

G27α___β___ r ___；

（Addresses α, β and r are selected by the X, Y, Z and the additional axes A, B, C, U, V and W.

However, if an additional axis simultaneous control does not selected, the additional axis only can be

controlled 1 axis simultaneously.

The following commands can be used when the simultaneous 4 axes control are selected. G27α___β___r___δ___；

Wherein, α, β, r, δ = X, Y, Z, A, B, C, U, V or W.

Note 1: In the cutter compensation, the tool position is the one added an offset value by G27. In this case,

if the tool does not at the reference position, the indicator of reference position return does not

ON. Generally, G27 is only on the compensation cancel mode.

Note 2: In the Inch mechanical system with metric input, the indicator is lighted up even if the tool

programmed position offsets 1μ from the reference position, because the least input increment is

less than the least move increment of mechanical system.

3.5.8.2 Automatically return to the reference position (G28)

G28 α___β___；

(Addresses α and β are selected by the X, Y, Z and the additional axes A, B, C, U, V and W.

However, if the function of additional simultaneous axis does not perform, the additional axis only can

be controlled alone).

This axis specified by this command can automatically position at the reference point, α and β

are move commands, which are specified based on the absolute/increment by G90/G91.

The end point of this command is called the “intermediate point”, and the coordinate value

Page 58

GSK983Ma Milling Machine Center CNC System User Manual

specified by this command is registered into NC.

The operations in G28 block are shown below:

Firstly, all of the controllable axes can be positioned to the intermediate point at the rapid

traverse rate. Then, return to the reference position from the intermediate point. If the machine does

not locked in this case, the indicator of reference position may be lighted up.

In this case, position to the intermediate point and reference position equals to the G00

positioning.

Part 1 Programming

The commands with simultaneous 3 axes are shown below: G28α___β___ r ___；

(Address α, β and r are selected from the X, Y, Z and the additional axes A, B, C, U, V and W)

The following commands can be used with the simultaneous 4 axes function: G28α___β___ r___δ___；

Wherein, α, β, r, δ= X, Y, Z, A, B, C, U, V or W。

Generally, the G28 command is used that the tool is automatically changed the ATC.

Note 1: In G28 block, the coordinate value of move command is not only registered, but also the

coordinate value of intermediate point. Namely, the axis does not specified in G28 block, the

coordinate value in the previous G28 command which is treated as a coordinate value of an

intermediate point of that axis.

For example: N1 G90 X100.0 Y200.0 Z300.0；

N2 G28 X400.0 Y500.0；

N3 G28 Z600.0；

Explanations:

N2：The intermediate point is (400.0, 500.0)

N3：The intermediate point is (400.0, 500.0, 600.0)

Note 2: After the power is turned on, the manual reference position return does not perform, and the G28

moves from the intermediate point which is same as the manual reference position return. In this

case, the move direction of intermediate point becomes the one of the reference position return by

parameter setting.

Note 3: G28 is specified by rotation axis, the move direction from intermediate point to the reference

position becomes the one of reference position by parameter setting. The movement amount is

within 360°.

3.5.8.3 Return from the reference position automatically (G29)

G29α___β___；

(Addresses α and β are selected from X, Y, Z and the additional axes A, B, C, U, V and W, if the

simultaneous control function of an additional axis does not select, the additional axis simultaneous

function can not be performed with any one of the others.)

Tool can be positioned at a specified point via an intermediate point based on this function.

Usually, this command followed with the G28 is used.

Page 59

Chapter Three Programming

α and β are movement commands which are specified by the absolute/increment values based

on the state of G90/G91

In the increment command, the increment value corresponding to the intermediate point should

be specified.

When the G29 block operation is performed, all specified axes can be reached to the appointed

point by the defined intermediate point by G28 code at the rapid traverse rate.

This positioning operation is from an intermediate point to the specified one which is similar as

the G00 positioning.

The application of G28 and G29 is shown below:

Reference point

The tool is changed at point R

Part 1 Programming

700

500

300

300 1,300 1,800

Intermediate point

X(MM)

When G91 is performed:

G28 X1000.0 Y200.0; (From A to B till to R)

M00；

G29 X500.0 Y-400.0; (From R to B till to C)

This example is expressed that programmer do not need to calculate the actual movement

distance where from the intermediate point to the reference position. If the simultaneous 3 axes

control function is performed for the system, the G29 code is as follows.

G29α___β___ r ___；

(Addresses α, β and r are selected from X, Y, Z and the additional axes A, B, C, U, V and W, if the

simultaneous control function of an additional axis does not select, the function of additional axis

simultaneous control can not be performed with any one of the others.)

The following commands can be performed when the simultaneous 4 axes function are

registered:

G29α___β___ r ___δ___；

Page 60

GSK983Ma Milling Machine Center CNC System User Manual

Wherein, α, β, r, δ = X, Y, Z, A, B, C, U, V and W.

Note: When the workpiece coordinate system is changed after the tool reaches the reference position

through the intermediate point by the G29/G30 command, the intermediate point also shifts to a

new coordinate system. If G29 is then commanded, the tool moves to the commanded position

through the intermediate point which has been shifted to the new coordinate system.

3.5.8.4 2nd, 3rd and 4th reference position return （G30）

Part 1 Programming

The following commands can be moved the specified axis to the 2

, 3rd or 4th reference position.

G30 P3 α___β___; (P2 can be omitted.) P4

P2: the 2

P3: the 3

P4: the 4

The 2

reference position

, 3rd or 4th reference position is used for the distance of the 1st reference position at the

scene debugging by the parameter setting in advance, this function is same as the G28 specification

of reference position except for the tool does not return to the 1

reference position instead of the 2nd,

3rd or 4th reference position. The G29 code is specified after G30 which the tool is positioned to the

specified place by G29 from the intermediate point has been set by G30, and it is same to specify the

G29 code after G28.

Usually, G30 code is used when the automatic tool-change position is different from reference

position. If the simultaneous 3 axes function is performed, the G30 code is as follows:

G30α___β___ r ___；

(Addresses α, β and r are selected from X, Y, Z and the additional axes A, B, C, U, V and W, if the

simultaneous control function of an additional axis does not select, the function of additional axis

simultaneous control can not be performed with any one of the others.)

The following commands can be performed when the simultaneous 4 axes function are

registered:

G30 P3 α___β___ r ___δ___；

Wherein, α, β, r, δ = X, Y, Z, A, B, C, U, V or W.

Note: After the power is turned on, the manual reference position return or automatic reference position

return must be performed once before performing the G30 code.

Page 61

3.5.9 Dwell (G04)

G04X（t）；or

Chapter Three Programming

G04P（t

）；

Any of the methods can be used for dwell, after the previous block is performed, the dwell

must be through the (t) ms time before the next block is performed.

The maximum code time is 99999.999s. The time error is about 16ms.

For example: Dwell 2.5s

G04 X2.5 or G04 P2500;

Note 1: Do not use a decimal point to program for address P.

Note 2: The following conditions can be used when the dwell delay is performed, which one is valid by the

BIT4 (CINP) parameter setting.

1. The dwell delay can be used after the previous block speed is set to 0.

2. The dwell delay can be used after the tool reaches to the specified value. (After the positioning

point check)

3.5.10 Exact stop check (G09)

A block including the G09, its feedrate decelerates to 0 at the end point; confirm the position state

(Note 2), and then next block is performed consecutively. This function is used for forming a sharp

pointedness. G09 is only valid in the specified blocks.

Note 1: The positioning point check is carried out automatically without a G09 positioning mode (G00,

G60).

Note 2: The positioning point means that the feed motor has been reached to the specified end range.

Part 1 Programming

3.5.11 Exact stop check (G60) and cutting mode (G64)

(1) Exact stop check mode (G61)

The movement command of each block after G61 should be decelerate to 0 at its end, till

encounter G64 code, and the next block is performed consecutively after the in-position state is

affirmed at the end point.

(3) Cutting mode (G64)

Each block followed with G64 does not decelerate, even in the G64 mode, but shift to the next

block immediately till to the end point of the movement command G61. However, in the positioning

command (G00 or G60) or in the block of the exact stop check (G09) is confirmed, or in those blocks

without any movement commands, the feedrate is still decelerate to 0 and perform a positioning

check.

3.5.12 Coordinate system setting (G92)

G92X（X）Y（Y）Z（Z）r（r）δ（δ）；

Page 62

GSK983Ma Milling Machine Center CNC System User Manual

The tool is moved to a certain point by the absolute command, and the coordinate system must

be preset which is set up by the following commands.

（r，δ= A、B、C、U、V、W） This command builds a coordinate system, the original of coordinate system is offered from the

appointed distance of the tool position. This is called workpiece coordinate system, once this system

is set up, the following absolute commands should be referred to a value from this workpiece

coordinate system.

Part 1 Programming

G92 X25.0 Z23.0；

G92 is used at the start of block to guarantee the tool is consistent with the program start point,

which is described in the above program.

G92 X600.0 Z1200.0；

As the above-mentioned, G92 will affirm the tool point is overlapped with the program start at the

beginning of program to perform an absolute command, this standard point is positioned at the

specified point. In order to position the nose at the specified place, the difference from tool nose to the

base point must be checked with the tool length compensation.

Note 1: If a coordinate system is set using G92 during tool length offset, a tool coordinate system at the

specified position is without an offset value.

Note 2: Cutter compensation is cancelled temporarily with G92.

Page 63

Chapter Three Programming

3.5.13 Workpiece coordinate system (G54～G59)

Specify a coordinate system without G92, six coordinate systems on machine tool can be preset,

which can be selected from G54 to G59.

G54………………… Workpiece coordinate system 1

G55………………… Workpiece coordinate system 2

G56………………… Workpiece coordinate system 3

G57………………… Workpiece coordinate system 4

G58………………… Workpiece coordinate system 5

G59………………… Workpiece coordinate system 6

Six coordinate systems can be set by distance (Workpiece point 0 offset values) of each axis

from the reference position to its 0 point.

For example: G55 G00 X100.0 Z20.0；

X15.5 Z25.5；

In the above example, position to the workpiece coordinate 2 (X =100.0, Z =20.0) and (X =15.5，

Part 1 Programming

Z =25.5).

Workpiece coordinate systems 1 to 6 are established after reference position return after the

power is turned on. G54 coordinate system is selected once the power is turned on.

Note 1: The compensation of workpiece 0 point offset of each axis is input from external data (optional), which

the solution is: 0～±0.7999mm or 0～±0.7999inch, check whether this function is performed in the

machine manual.

Note 2: The coordinate system is set without G92 when using G54～G59. If the G92 is used for establishing a

coordinate system, some special matters of the move coordinate system can be established using

G54～G59.

Page 64

GSK983Ma Milling Machine Center CNC System User Manual

Part 1 Programming

In the state of G54, when tool is positioned at the (200, 160), G92 X10 Y100; specify the workpiece

coordinate system 1 (X , Y ) is moved by vector A, and other workpiece coordinates are also offset the ˊˊ

vector A simultaneously.

Note 3: A function of coordinate system setting does not select, set the suitable parameter value #309.0～

3 (APX～AP4).

Functions of workpiece coordinate system measurement

Workpiece coordinate system measurement function can be set the current machine coordinate to the corresponding workpiece coordinate automatically by the measurement (MEASUR) directly, and it is convenient for the coordinate system setting.

(1) Page 1 (Workpiece coordinate offset 01)

Fig. 1

EXT: Workpiece coordinate system offset G54: Workpiece origin offset of workpiece coordinate system 1 G55: Workpiece origin offset of workpiece coordinate system 2 G56：Workpiece origin offset of workpiece coordinate system 3

(2) Page 2 (Workpiece coordinate offset 02)

Page 65

Chapter Three Programming

Part 1 Programming

Fig. 2

G57：Workpiece origin offset of workpiece coordinate system 4 G58：Workpiece origin offset of workpiece coordinate system 5 G59：Workpiece origin offset of workpiece coordinate system 6

The procedures of workpiece coordinate setting can be performed by the coordinate

measurement function:

(1) Move the cursor to the workpiece coordinate serial number to be changed. (2) Press X 0 ， Y 0 , Z 0 or 4TH/5TH 0,, and then press the soft function

key of measurement (MEASUR), namely, the current machine coordinate value can be set to the

workpiece coordinate system to be changed on workpiece origin offset.

3.5.14 Workpiece coordinate system changes by the program command

When the workpiece coordinate system is not enough (although 6 pieces have been performed

already) and in the case of the workpiece coordinate system should be moved in terms of the

requires, we can move them by the program commands.

G10 L2 P P

X Y Z r δ；

In this case: P=1～6: it corresponds to the coordinate system 1～6, X, Y, Z, r, δ (r or δ equals to

one of the A, B, C U,V or W)

The workpiece zero offset is absolute or increment which is determined by the G90 or G91.

Note: Set P= 0, change EXT: The offset of workpiece coordinate system.

3.5.15 Automatic coordinate system setting

When the reference position is returned firstly, a coordinate system can be set at the preset

parameter (Set the parameters No. 375～378, 440 when the metric input is performed, and set the

parameters No. 379～382, 441 when the inch input is performed). That is to say, it is same as the

Page 66

GSK983Ma Milling Machine Center CNC System User Manual

G92 which the function of the reference position is automatically set the coordinate system.

Note: If the workpiece coordinate system setting function is used, all of the parameters No.375～378, 440

are set to 0 when the metric input is performed, and all of the parameters No. 379～382, 441 are set

to 0 when the inch input is performed.

If the setting value does not 0, the workpiece coordinate systems (1～6) offset may occur.

3.5.16 Inch/Metric conversion (G20, G21)

Part 1 Programming

Either inch or metric input can be selected by G code.

Unit G code The least input unit

Inch (Inch) G20 0.0001inch

Mm (Metric) G21 0.001mm

This two G codes must be specified in an independent block before setting the workpiece

coordinate system at the beginning of the program.

N10 G20；

N20 G92 X___Y___；

The following contents vary from the two G codes:

1) Feedrate commanded by F code

2) Position display

3) Offset value

4) Unit of scale for MPG.

5) Movement amount in incremental feed

6) A part of parameters

Note 1: When the power is turned on, the G code is the same as that held before the power was turned off.

Note2: G20 and G21 must not be switched during a program.

Note 3: When the unit system between machine and program are different, the maximum error is the half

of the least movement unit which this error value does not accumulate.

3.5.17 Stored stroke limit (G22, G23)

The movement range of the tool can be restricted by the following two methods.

(Tool can not enter the shadowed area)

Stored stroke limit 1:

Page 67

Chapter Three Programming

The boundary is set by the parameter, and the specified boundary is called forbidden area.

Usually, it is never changed after the manufactory is set. So, it is set at the maximum stroke of

machine which is equivalent the soft limit.

Stored stroke limit 2:

The boundary is specified by the parameter or command, the specified area (inside or outside) is

forbidden area, which is determined by BIT6 of parameter 009 (RWL).

G22 code can be stop the tool enters the forbidden area, and the G23 code can be lift the

forbidden area.

Creating or changing the forbidden area using a command

G22 X___Y___Z___I___J___K___；

Part 1 Programming

X＞I，Y＞J，Z＞K

X－I＞2000 (The least command increment)

Y－J＞2000 (The least command increment)

Z－K＞2000 (The least command increment)

When setting the area by parameters, points A and B in the figure below must be set.

1＞X2，Y1＞Y2，Z1＞Z2

＞2000 (The least command increment)

1－X2

＞2000 (The least command increment)

1－Y2

＞2000 (The least command increment)

1－Z2

If the forbidden area is set by parameter, the X Y Z I J K should be set by the least move unit

(output unit) of the mechanical coordinate system which is regarded as zero point by the reference

position.

If it is set by G22 code, the X Y Z I J K should be programmed by the least input increment (input

unit) of the mechanical coordinate system which is regarded as zero point by the reference position.

The programmed data is then became the numerical digit value of the least movement unit, which this

value is treated as parameter setting.

Page 68

GSK983Ma Milling Machine Center CNC System User Manual

Some part of cutter or jig must be checked to enter the forbidden area, so, the calculations

among the X Y Z I J K are different.

Part 1 Programming

Point a is set if check point A enters the forbidden area, it is same to the b.

If the point A is regarded as tool nose check, and if the tool length varies for each tool which is set

to the longest tool, the tool setting is also safe regardless of the modification.

Area can be set in overlaps.

Note 1: Each limit becomes effective after the power is turned on and manual reference position return or

automatic reference position return by G28 has been performed.

Note 2: After the power is turned on and manual reference position return has been performed, if the

reference position is in the forbidden area of each limit, the stored stroke limit is valid, an alarm is

generated immediately. (Only in G22 mode for stored stroke limit 2).

When G23 is switched to G22, and the tool is in the forbidden area, in this case, an alarm may generate in

the next block.

Note 3: In the case of Note 2, the tool does not move in the forbidden area, press the ESP switch to

release the forbidden condition or move the tool out of the forbidden area by G23. The setting

should be modified if it is set incorrect, the reference position return may perform again.

Note 4: The axis without a reference position return function which does not a forbidden area, an alarm

for this axis does not issue in the forbidden area.

Note 5: If two points setting for the forbidden area are same, the area is described as follows:

When the forbidden area is inside the specified area, then all areas are the moveable areas.

When the forbidden area is outside the specified area, then all areas are the forbidden areas in G22

mode.

Note 6: Unnecessary limits should be set beyond the machine stroke.

Note 7: If the tool enters a forbidden area and an alarm is generated, the tool can be moved only in the

backward direction.

Note 8: In the setting area, the rectangle formed by two top points may create a limit area, even if the

Page 69

Chapter Three Programming

sequence of coordinate value of the two points is set incorrectly.

Note 9: G22______; and G23; should be commanded in a single block.

Note 10: The additional axis can not be used the function of stored stroke limit 2.

3.5.18 Skip Function (G31)

Linear interpolation can be commanded by specifying move command following the G31, like

G01. If an external skip signal is input during the execution of this command, execution of the

command is interrupted and the next block is executed.

G31 can be used once, which is only valid in the specified block.

The operation after inputting the skip signal is determined by the next block is increment

command or absolute one.

1) The next block is increment command.

The increment operation is performed from the intermediate point:

For example: G31 G91 X100.0；

Y50.0；

2) Next block is an absolute command, (Only one axis)

Part 1 Programming

An axis is specified in a block which moves to the command position, and the unspecified axis

holds the position of which the skip signal is input.

For example: G31 G90 X200.0；

Y100.0；

3) Next block is absolute command (Specify 2 axes)

The next block will move to the specified position whenever a skip signal is input.

For example: G31 G90 X200.0；

X300.0 Y100.0；

Page 70

Part 1 Programming

Specify the feedrate of block (G31) by BIT 7 (SKPF) of parameter 306 is as follows:

a) Specify the feedrate by F code (It is can be specified at the previous place or in G31

block)

b) Set the feedrate by parameter No.342 (PSKPFL).

The coordinate values when the skip signal is turned on can be used in a custom Macro

GSK983Ma Milling Machine Center CNC System User Manual

because they are stored in the custom Macro system variable #5061～#5065, as follows:

#5061………………………X axis coordinate value when the skip signal is ON.

#5062………………………Y axis coordinate value when the skip signal is ON.

#5063………………………Z axis coordinate value when the skip signal is ON.

#5064………………………The 4

#5065………………………The 5

coordinate value when the skip signal is ON.

coordinate axis when the skip signal is ON.

The skip function can be used in the occasion of infinitive movement, so, it is suitable for the

following matters.

a) The standard dimension feed of the Milling machine.

b) It is measured by the tool touches with the sensor.

Note 1: In the efficient state of the cutter compensation C, an alarm of No.035 may occur once the

G31 command is performed. The tool compensation should be cancelled by G40 before G31

code.

Note 2: If the feedrate specified by G31 is related with the one of the parameter setting, it is still

related with the speed of parameter setting even the dry operation is performed.

Note 3: When the feedrate specified by G31 is related with the one of the parameter setting, the

automatic acceleration/deceleration is invalid. In this case, the automatic measurement

accuracy is improved when the skip function is applied.

3.6 Compensation Function

3.6.1 Tool length compensation (G43, G44, G49)

Page 71

Chapter Three Programming

G43

Z___H___； or G44

G43

H___；

G44

The setting of offset value in offset memory is moved in positive or negative for the end position

of movement command along with Z axis. This function can be used by setting the difference

between the tool length assumed during programming and the actual tool length of the tool used into

the offset memory, and the compensation can be carried out regardless of the program change. H

code can be set the offset value in the offset memory along the direction by G43, G44 code.

(1) Offset direction

G43 + (Positive) offset

G44 – (Negative) offset

When G43 is specified, the tool length offset value (stored in offset memory) specified with the H

code is added to the coordinates of the end position specified by a command in the program. When

G44 is specified, the same value is subtracted from the coordinates of the end position. The resulting

coordinates indicate the end position after compensation, regardless of whether the absolute or

incremental mode is selected.

G43

G91 Z0 H______； G44 Offset value offsets in positive along Z axis in G43, but it offsets in negative along Z axis in G44.

G43 and G44 are modal G codes, G codes without a same group after they are commanded

which are specified are valid. The G43 or G44, which one is valid after the power is turned on, which

Part 1 Programming

is determined by the parameter setting #8.1 and #8.4.

(2) Specify an offset value

Specify an offset number by H code, the setting of the offset value in the offset memory of this

code which adds or reduces to the program value of the Z axis. Offset number can be specified from

H00 to H184. When 184 D codes are used by the cutter compensation, the offset number can be

specified from the D01 to D184.

Note: Only one value can be input for one offset number, when one offset number is specified to tool

length compensation, the cutter compensation can not be specified any more.

Offset value corresponds to the offset number, which they can set in the offset memory by the

MDI &LCD or by the communication operation in advance, the setting of the offset value is as follows:

Metric input Inch input

Offset value

0mm～±999.999mm 0 inch～±999.999inch

Usually, the offset value of H00 corresponding with the offset number 00 is 0; therefore, the offset

value corresponding with the H00 does not set.

(3) Cancel G49 by tool length compensation

Page 72

GSK983Ma Milling Machine Center CNC System User Manual

Specify G49 or H00 when the tool length compensation will be cancelled. Once the H00 or G49

is specified, it may cancel and position again by the H00 or G49

Note 1: When the Z axis address followed with the G49 is omitted, the Z axis may position again, it is

necessary to notice that the Z axis address can not be ignored after the G49.

If the executed command is G43 last time, Z axis shifts an offset value towards negative direction, if

the performed command is G44 last time; the Z axis shifts an offset value towards positive

direction.

For example:

Part 1 Programming

N1 G0G90G43H1Z123.0； Position to the Z123+ offset value

N2 G49（or H0）； Position to Z123.0 again

N3 M30；

Note 2: In the tool length offset mode, the tool length offset vector is canceled when moving to the

reference position while the G28 Zz

modal G43/G44 is still displayed, and the modal code display does not shift to G49.

or G30 Zz is specified, however, the previously specified

(4) The example of tool length compensation (the machining of #1, #2, #3)

Page 73

Chapter Three Programming

H01= －4.0 (Offset value)

N1 G91 G00 X120.0 Y80.0 ；……………（1）

N2 G43 Z-32.0 H01 ；……………（2）

N3 G01 Z-21.0 F1000 ；……………（3）

N4 G04 P2000 ；……………（4）

N5 G00 Z21.0 ；……………（5）

N6 X30.0 Y-50.0 ；……………（6）

N7 G01 Z-41.0 ；……………（7）

N8 G00 Z41.0 ；……………（8）

N9 X50.0 Y30.0 ；……………（9）

N10 G01 Z-25.0 ；……………（10）

N11 G04 P2000 ；……………（11）

N12 G00 Z57.0 H00 ；……………（12）

N13 X-200.0 Y-60.0 ；……………（13）

Note 1: Offset value differs depending on the offset number, the new offset value does not add to the old

one.

H01…………Offset value 20.0

H02…………Offset value 30.0

G90 G43 Z100.0 H01；…… Z will be reached to 120.0

G90 G43 Z100.0 H02；…… Z will be reached to 130.0

Note 2: D code can not be used in tool length compensation. Other axes can be used the tool length

compensation other than the Z axis, which can be selected by BIT 1 of parameter 307 of which

axis is added the tool length compensation. The axis address α code can be used in the same

block of G43 and G44.

G43

α＿H＿；(α: alternative axis)

G44

Tool length compensation can be only added one axis simultaneously, an alarm may occur in the

following commands. Tool length compensation must be cancelled once before switching the tool length

compensation axis.

G43 Z＿H＿；

Part 1 Programming

G43 X＿H＿；(Alarm)

3.6.2 Tool position offset (G45～G48)

The travel distance of the specified axis can be increased or decreased by the digit set in the

offset memory by the commands G45～G48, refer to the table 6.2.

Page 74

Part 1 Programming

The G codes are one-shot code, which is only valid in the specified block.

Once the compensations are specified by D or H, which remains unchanged until other

compensations are selected.

Tool offset compensation is used H or D which is determined by BIT 3 (OFSD) of parameter 10.

When the tool radius value is set in offset memory, the tool path can be programmed by the

workpiece.

GSK983Ma Milling Machine Center CNC System User Manual

Table 6.2 Tool position offset and G codes

G code Function

G45 Increase an offset value

G46 Decrease an offset value

G47 Increase the offset value by twice

G48 Decrease the offset value by twice

The solution range of offset value

Metric input Inch input

Offset value

0mm～±999.999mm 0 inch～±99.9999inch

0°～±999.999° 0°～±999.999°

This offset function is also valid for the additional axis (the 4

axis).

The offset value always indicates 0 when the offset number is 00 (H00 or D00).

An increment and decrement may generate along the tool travel direction of this axis, which

moves from the end of previous block to the commanded position in the block of G45～G48, and then

the compensation of increase and decrease can be performed.

1) G45 code (Only for the increase offset value

～～～～～～～ Motion command value

Offset value

Actual motion value

a) Motion command+12.34 offset value +5.67 b) Motion command+12.34 offset value

-5.67

Page 75

Chapter Three Programming

c) Motion command-12.34 offset value +5.67 d) Motion command-12.34 offset value -5.67

2) G46 code (Only reduce an offset value)

Try to reverse the symbol of offset value in G45 code, and it is then same as the G46.

a) Motion command +12.34 offset value +5.67(b)～(d) is omitted

Part 1 Programming

3) G47 code (Increase the offset value by twice)

c) Motion command -12.34 offset value +1.23 d) Motion command -12.34 offset value -1.23

4) G48 code (Reduce the offset value by twice)

Try to reverse the symbol of offset value in G47 code, and it is then same as the G48.

a) Motion command +12.34 offset value +1.23(b)～(d) is omitted

Page 76

GSK983Ma Milling Machine Center CNC System User Manual

Only when the offset value is moved in increment code (G91) mode, the movement command is

0. When the movement amount in absolute code (G90) is set to 0, any operations may not be

performed.

Part 1 Programming

Offset value +12.34 (Offset number 01)

NC code G91 G45 X0

D01；

Equivalent

X12.34 X-12.34 X-12.34

G91 G46 X0 D01；

G91 G45 X-0

D01

G91 G46 X-0

D01；

X12.34；

command

Note 1: If one is specified from G45～G48 for the simultaneous 2 axes control, the tool offset is then valid

to the two axes.

In the case of the G45

Movement commands X1000.0 Y5000.0

Offset value +200.0 Offset number 02

Programmed command G45 G01 X1000.0 Y5000.0 D02;

Note 2: In the chamfer machining, if the tool offset is performed, the overcutting or the lack of cutting may

generate.

Page 77

Chapter Three Programming

F ； Y ；

；

G01 X G47 X

Part 1 Programming

G01 G45 X

G45 Y

F D ；

Y ；

；

Note 3: When the offset amount is more than the movement command value, the actual tool movement

direction becomes reverse to the programmed direction.

For example: G46 X2.50；

(Increment command)

Offset value + 3.70 It equivalents to the command X-1.20；

Note 4: As for the circular arc interpolation (G02, G03), tool offset can be generated by G45～G48 codes

only the command belongs to the 1/4 and 3/4 circular. Namely, tool compensation can be

Page 78

GSK983Ma Milling Machine Center CNC System User Manual

performed only when the command belongs to the 1/4 and 3/4 circular arc.

Refer to the 6.21: Offset value +20.0，Offset number 01

Refer to the program:

（G91）

G45 G03 X-70.0 Y70.0 I-70.0 D01；

Part 1 Programming

Refer to the 6.22: Tool position offset in circular interpolation

N1 G46 G00 X___Y___D___；

N2 G45 G01 Y___F___；

N3 G45 G03 X___Y___I___；

N4 G01 X___；

Programmed too path

Refer to the 6.23: Program using a tool offset

Cutter compensation

Actual tool path

Page 79

Chapter Three Programming

Part 1 Programming

1. G91 G46 G00 X80.0 Y50.0 D01；

2. G47 G01 X50.0 F120；

3. Y40.0；

4. G48 X40.0；

5. Y-40.0；

6. G45 X30.0；

7. G45 G03 X30.0 Y30.0 J30.0；

8. G45 G01 Y20.0；

9. G46 X0；……… The offset value only moves along – X direction

10. G46 G02 X-30.0 Y30.0 J30.0；

11. G45 G01 Y0；………… The offset value only moves along – Y direction

12. G47 X-12.0；

13. G47 Y-80.0；

14. G46 G00 X-80.0 Y-50.0；

Note 5: If the H code is used in G43 or G44 mode, only Z axis moves an offset value. Therefore, the D code

can be used instead H in the G45～G48 in the mode of G43, G44 as much as possible.

Note 6: During the canned cycle mode, the G45～G48 modes are ignored, the G45～G48 must be

programmed before specifying a canned cycle, and cancelled after the canned cycle is

performed.

Note 7: The tool offset mode (G45～G48) can not be performed in G41 or G42 (tool compensation) mode.

Otherwise, a P/S alarm may issue. (Alarm number: 36)

Page 80

GSK983Ma Milling Machine Center CNC System User Manual

3.6.3 Cutter compensation (G40～G42)

3.6.3.1 The function of cutter compensation

The tool with a radius R machines a workpiece specified in the Fig. A, the corresponding tool

center must be a B path of the radius R, in this case, tool removes a tool distance is called offset,

calculate the distance of the tool path (offset) by the function of tool compensation, refer to the

Part 1 Programming

following figure.

Programmer can edit a workpiece figure with the tool offset mode, if a tool radius (offset value) is

measured and set in NC in the machining, the tool path may be offset (path B) regardless of the

programmed path.

There are two tool compensation modes (B and C), only mode C is described in this section. The

difference between B and C are shown below:

In the tool compensation B, the corner equals to 90° or less than which can not be performed an

internal offset. In this case, a suitable inner corner arc should be programmed.

3.6.3.2 Offset value (D code)

Up to 32 offset values can be set to the offset memory (there 64, 99 or 184 pieces can be

selected), (32 offsets are separately used in the tool length compensation and too position offset).

The offset value based on the D specified on the block, and the bit parameter is set by the MDI &

LCD.

The setting range is as follows:

Input in mm Input in inch

Offset value 0mm ~ 999.999mm 0inch ~99.9999inch

The offset value corresponding to 00 or D00 always means 0.

It is impossible to set D0 to any other offset amount.

3.6.3.3 Offset vector

The offset vector is the two dimensional vector that is equal to the offset vector assigned by D

Page 81

Chapter Three Programming

code. It is calculated inside the control unit, and its direction is up-dated in accordance with the

progress of the tool feed of each axis. This offset vector (it is called vector in the following description)

generates from the control unit, so that the tool offset movement can be calculated, and the actual

path of tool radius offset programmed path can be carried out. This offset vector is deleted by reset.

This vector varies from the tool movement, it is very important to comprehend the vector when

the program is performed. Read the following description and distinguish how the vector generates.

3.6.3.4 Plane selection and vector

Offset calculation is carried out in the plane determined by G17, G18 and G19. This plane is called the offset plane. For example, the offset value can be carried out using the (X, Y) or (I, J) in block and then the vector is calculated after the XY plane has been selected. The axis is not affected for the coordinate value which is not in the offset plane. The programmed values are used as they are. In simultaneous 3 axes control, the tool path projected on the offset plane is compensated. The shift among plane selection must be performed in the offset cancellation mode. If the plane selection is performed in offset mode, an alarm (No.37) may generate.

G code Offset plane

G17

G18

G19

When the offset plane with an additional axis set, an additional axis should be set in advance in

parameter to which parallels with one of the X Y Z axes. The offset plane can not be defined when it

does not parallel to the axis.

X－Y plane

Z－X plane

Y－Z plane

Part 1 Programming

The offset plane with an additional axis and the G codes (G17, G18 and G19) can be specified

an additional axis simultaneously.

a) G17 X_Y_；……XY plane

b) G17 U_Y_；……UY plane (U parallels with X)

c) G17 Y_；………XY plane

d) G17；…………XY plane

e) G17 X_Y_U_；…… alarm

f) G18 X_W_；……XW plane (W parallels with Z)

3.6.3.5 G40，G41 and G42

The cancellation and generation of cutter compensation vector are specified by G40, G41 and

G42. The G40, G41 and G42 can be commanded with G00 or G01 simultaneously for deciding the

directions of offset vector and tool movement.

Page 82

GSK983Ma Milling Machine Center CNC System User Manual

G code Function

G40 Cutter compensation cancel

G41 Cutter compensation left

G42 Cutter compensation right

The system enters the cutter compensation mode with G41 or G42 code.

The system enters the cancel mode with G40 code.

Refer to the procedure of offset in the following figure.

Part 1 Programming

Start the block , the offset cancel mode becomes offset mode (G41) in this block. T① he tool

center is offset by the radius perpendicular to the next block path. The tool compensation value is

assigned by D07, namely, the offset number is 7, and the G41 means tool offset left.

The system is automatically performed a tool compensation after the workpiece

the programmed path movement in the end of block

——→P8→P9→P1 has been programmed and then started.

1→P2

In the block , tool returns to the start (offset cancel) by specifying G40. Tool center is vertical to ①

10.

○

The compensation cancel of G40 must be specified in the end of program.

The program of cutter compensation C shows an example:

G92G40 X0 Y0 Z0

a) N1 G90 G17 G00 G41 D07 X250.0 Y550.0； (Offset value is set to 07 by MDI in

advance.)

Page 83

Chapter Three Programming

b) N2 G01 Y900.0 F150；

c) N3 X450.0；

d) N4 G03 X500.0 Y1150.0 I-600.0 J250.0；

e) N5 G02 X900.0 I200.0 J150.0；

f) N6 G03 X950.0 Y900.0 I250.0 J0；

g) N7 G01 X1150.0；

h) N8 Y550.0；

i) N9 X700.0 Y650.0；

j) N10 X250.0 Y550.0；

k) N11 G00 G40 X0 Y0；

3.6.3.6 Details of cutter compensation C

The following descriptions provide a detailed explanation of the cutter compensation C

(1) Cancel mode

NC becomes clear state (BIT3 CLER of NC parameter 7 selects reset signal and whether the NC

becomes clear state) when the power is turned on or the M02 or M30 is performed by controlling the

reset key, the offset can be cancelled therefore.

In the cancel mode, vector always set to 0, the tool center path is overlapped with the

programmed path, and the cancel mode should be performed at the end of the program.

When the program is executed at the end of offset mode, the program positioning at the end of

program can not be carried out but the tool position offsets a vector value from the end position.

Part 1 Programming

（2）Start

In the cancel mode, when a block is available for the following conditions which is performed, the

system is then entered the offset state, in this case, this block is called the start block.

a) The G41 or G42 has been commanded, and the system enters the state of G41 or G42.

b) Tool compensation number is not D00.

c) The axis (Except the I, J, K) (even one axis can be performed) in the offset plane has been

specified and its movement value is not 0.

In the start block, the circular command (G02, G03) is unallowable, otherwise, the No.34 alarm

may issue, the NC stops. NC read two blocks in the start, the first block is read and performed; the

next block enters to the cutter compensation buffer register (The content of this register can not be

displayed).

Additional, two consecutive blocks are read while the single block mode is performed, and the

read block is stopped after it has been performed, usually, two blocks are then read previously. Three

blocks in the NC, namely, the performing block, next block and the another one.

Note: When an angle of intersection created by tool paths specified with move commands for two blocks

is over 180°, it is referred to as “inner side.” When the angle is between 0°～180°, it is referred to as

Page 84

GSK983Ma Milling Machine Center CNC System User Manual

“outer side.”

Part 1 Programming

(i) Machining around the inner side

Linear Linear

Thereafter, the following descriptions are indicated as below:

S indicates the single block dwell point

L indicates that the tool moves along a straight line

C indicates that the tool moves along an arc

Linear Circular arc

(ii) When the tool moves around the outside of a corner at an obtuse angle (90°≤α≤180°), tool

path in start-up has two types A and B, and they are selected by BIT 1 (SUPM) of parameter 011.

Type A: (Linear to linear)

Page 85

(Linear to Circular)

Chapter Three Programming

Part 1 Programming

Type B: (Linear to Linear)

The intersection point is an intersected point with the offset path which is calculated by the

two consecutive blocks.

(Linear to Circular)

The intersection described above-mentioned which the offset path is carried out from r

length by two blocks

(iii) When an acute angle is performed (α＜90° equals to the outer side）

Page 86

GSK983Ma Milling Machine Center CNC System User Manual

Type A (Linear Linear)

G42

(Linear Circular)

Part 1 Programming

Programmed path

Path of tool nose center

G42

r S

Path of tool nose center

Type B (Linear Linear)

G42

(Linear Circular)

Programmed path

Path of tool nose center

Page 87

Chapter Three Programming

Note: In the case of Type B, when tool moves around straight line at the inner side of the pointed angle is

less than 1 degree, the compensation is performed based on the following figure.

Part 1 Programming

(2) Offset mode

The circular arc must be performed an offset even if a linear interpolation is performed in the

offset mode.

In the offset mode, the block without a movement command instead of miscellaneous function or

dwell which can not be commanded in the two consecutive blocks, otherwise, either undercutting or

overcutting may occur.

An offset plane can not be changed in offset mode, otherwise, the alarm No.37 occurs and the

tool is stopped.

(i) Tool movement around an inner side of a corner (180°≤α)

Linear to Linear

Page 88

Linear to Circular

Part 1 Programming

Circular to Linear

GSK983Ma Milling Machine Center CNC System User Manual

Circular to Circular

A narrow pointed angle moves within 1° from linear to linear, in this case, the offset vector becomes excess large.

Page 89

Chapter Three Programming

Reader should infer in the same procedure, in case of arc to straight line, straight line to arc and

arc to arc.

(ii) Tool movement around the outside of a corner at an obtuse angle (90°≤α＜180°） Linear to Linear

Part 1 Programming

Linear to Circular

Circular to Linear

Circular to Circular

Page 90

(iii) Tool movement around the outside of a corner at an acute angle

Linear to Linear

Part 1 Programming

Linear to Circular

GSK983Ma Milling Machine Center CNC System User Manual

Programmed path

Path of tool nose center

Circular to Linear

Circular to Circular

Programmed path

Path of tool nose center

Programmed path

Path of tool nose center

When an end position for the arc is not on the arc

Programmed path

Page 91

Chapter Three Programming

When a leading is programmed on arc, the arc center switched with an arc end which is treated

as an imaginary arc. The imaginary circle is regarded an arc of tool compensation which is

compensated as a vector. The resulting is different with tool center path in which the tool

compensation is regarded as a straight line with arc leading.

The same description applies to tool movement between two circular paths.

There is no inner intersection

The arc intersection may occur on the compensation path when the offset value is insufficient,

the intersection may disappear when the offset value is increased, in this case, the No.33 alarm may

generate at the end of the previous block and the system stops.

Part 1 Programming

The above figure shows that compensation paths along arcs A and B intersect at P when a sufficiently small value is specified. If an excessively large value is specified, this intersection does not occur.

The center of the arc is overlapped with the start position or the end position. In this case, alarm No.38 may occur, and NC stops the program at the end of previous program.

（G41 mode） N5 G01 X1000； N6 G02 X1000 I0 J0； N7 G03 Y-1000 J-1000；

(3) Offset cancel

In the offset mode, when a block which satisfies any one of the following conditions is executed,

the system enters the offset cancel mode, and the function of this block is called the offset cancel.

Command mode:

Page 92

GSK983Ma Milling Machine Center CNC System User Manual

1) G40 has been commanded.

2) Treat the D00 as a tool compensation number The arc G02 or G03 can not be specified when the offset cancel is performed. An alarm No.34

may generate if it is commanded, and the NC stops.

When performing offset cancel, circular arc commands (G02 and G03) are not available. If a

circular arc is commanded, an alarm (No.034) is generated and the tool stops.

In the offset cancel, a read block which includes two blocks is executed to store on the buffer (without displaying) with respect to the cutter compensation. In the case of a single block mode, after reading one block, the control executes it and stops. By pushing the cycle start button once more, one block is executed without reading the next block.

Part 1 Programming

Then the control system is in the cancel mode, and normally, the block to be executed next will be stored in the buffer register and the buffer for cutter compensation does not perform.

(a) When the tool moves around the inner side of a corner (α≥180°）

Linear to Linear

Circular to Linear

(b) When tool moves along with a corner (90°≤α＜180° obtuse angle)

(i) Type A

Linear to Linear

Page 93

Circular to Linear

Chapter Three Programming

Part 1 Programming

(ii) Type B Linear to Linear

Circular to Linear

Page 94

Circular to Linear

Part 1 Programming

(ii) Type B

Linear to Linear

GSK983Ma Milling Machine Center CNC System User Manual

Circular to Linear

In the occasion of type B, when tool moves an acute angle within 1° with straight line to straight

line from outer side, the form of compensation is as follows:

(4) Cutter compensation G code in offset mode

The cutter compensation G codes (G41, G42) can be separately specified by offset mode, the

movement direction to the previous block is set an offset vector forming a correct angel, which is

regardless of the machining inner side or outer side.

Page 95

Chapter Three Programming

Suppose that the codes (G41, G42) are included in the arc command, which may not perform a

correct arc.

The compensation direction switch can be carried out by specifying cutter compensation G

codes (G41, G42), refer to the Note 2 “Switch offset direction in offset mode”.

Linear to Linear

Part 1 Programming

Circular to Linear

Change in the offset direction in the offset mode

The offset direction is decided by G codes (G41 and G42) for the sign of offset value as follows.

Sign of offset amount

＋－

G code

G41 Left side offset Right side offset G42 Right side offset Left side offset

An offset direction can be shifted by G41, G42 in offset mode for the special occasions. However, the start block and the next block can not be switched. In the occasion of offset direction, the concept of inner side or outer side is cancelled to suit all matters. Suppose that the offset value is positive in the following examples.

Linear to Linear

Linear to Circular

Page 96

Part 1 Programming

Circular to Linear

GSK983Ma Milling Machine Center CNC System User Manual

Circular to Circular

Generally, there is no intersection on tool path after the offset is added: If the switch of G41 and G42 are performed and there is no intersection of offset path If there is no offset path intersection but G41 and G42 are shifted from blocks A to B, then the

vector vertical to the programmed direction is set up with the start of block B.

a) Linear to Linear

Page 97

Chapter Three Programming

Part 1 Programming

b) Linear to Circular

c) Circular to Circular

The tool center path length from cutter compensation is more than the circumferential: Usually, the above-mentioned matter may not occur, it is possible that only when G41 and G42

are shifted, or G40 is specified by addresses I, J and K commands.

Page 98

GSK983Ma Milling Machine Center CNC System User Manual

Part 1 Programming

In the above occasion, tool center path does not move a circle instead of the arc of P1～P2.

Refer to the description which the alarm is caused for the interference check. If the tool will move along the entire circumference, and then this circumference must be commanded separately.

(5) Cancel the temporary offset, and perform the following commands in offset mode, then the “temporary offset cancel” may execute, and then the system will automatically recover to the offset mode.

Refer to the “Offset cancel” in the Section 6.3.6 (4) and the “Start” in the section 6.3.6 (2) for the

details.

(a) G28 returns to the reference position automatically

If the G28 is specified in offset mode, the offset is then cancelled at the intermediate point, and

then it is automatically recovered till to the reference position.

If the offset vector holds at the intermediate point, the vector of each axis has been performed to

return to the reference position by NC which is set to 0.

Intermediate point

G28

G00

G42

G00

Reference point

(b) G29 automatically returns from reference position If the G29 is specified in offset mode, the offset may be cancelled at the intermediate point, and

then automatically recovered in the next block again.

Directly specify G29 after G28.

G42

G00

Intermediate point

G28

G29

G00

Reference point

The occasion other than G29 is directly specified after G28.

Intermediate zone

G00

G42

G00

G29

Page 99

Chapter Three Programming

(6) The command is used for cancelling the offset vector temporarily. In the same offset mode, if the G92 (absolute 0 point programming) is specified; the offset vector

must be cancelled temporarily, and then recovered automatically.

In the case of, the offset cancel motion does not perform, tool directly moves to the point of specified offset cancel vector from intersection, and then the tool moves to the intersection when the offset mode is recovered.

Part 1 Programming

(G41 mode)

N5 G01 X3000 Y7000；

N6 X－3000 Y6000；

N7 G92 X1000 Y2000；

N8 G01 X4000 Y8000；

Note: In the single block mode, the SS indicates a point that tool stops twice.

(7) The block without a tool movement

There is no tool movement in the following blocks. The tool never moves even if the cutter compensation is valid in these blocks.

M05; M code output

S21 S code output

G04 X1000; Dwell time

G22 X100000; Machine area setting

G10 P01 X100 Offset value setting without moving

(G17) Z2000; Movement out of the offset panel

G90; G code only

G91 X0; Movement amount is 0

a) It is commanded when starting

If a block without a tool movement is specified at the start of program, the offset vector may not

generate.

G04 G91

N6 X1000.0 Y1000.0； N7 G41 X0； N8 Y-1000.0； N9 X1000.0 Y-1000.0；

b) It is specified in offset mode

A single block without a tool movement is specified in offset mode, and its vector is same to the tool center path without a command block (Refer to the Section 6.3.6 (a) for the offset mode); this block is performed at the stop position of this single block.

Page 100

GSK983Ma Milling Machine Center CNC System User Manual

Part 1 Programming

However, when the movement value is 0, the tool move of this block is same as the one which is

specified more than one block without any tool movement

Two or above blocks without any tool movement can not be specified consecutively, otherwise, the vector along with tool movement direction which may generate a length equals to an offset value and the direction is vertical to the previous block. Thereby, the overcutting may occur.

Note: SSS means that the tool is stopped thrice by single block.

c) It is specified with offset cancel

When a block without a tool movement is specified with offset cancel, a vector generates along the previous block tool movement direction which equals an offset value, this vector is cancelled in the next movement command.

N6 G91 X100.0 Y100.0；

N7 G40；

N8 X100.0 Y0；

(8) The content within offset plane in G40 and I___J___K___which is specified, and the

previous block mode is G41 or G42.

The above-mentioned command is specified in the offset mode which becomes an example as G17, the same as other occasions.

gsk GSK983Ma User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual