gsk GSK980MD User Manual

GSK980MD MILLING CNC SYSTEM

User Manual

PREFACE

d

n

f

t

Warning！

 Before installation, programming and operation, read this manual an

the machine builder manual carefully and perform the relevant

operations strictly by the instructions in the manuals. Or else it may

result in product and machine damage, workpiece scrap, even serious

personal hurt.

 The functions, technical specifications（such as precision, speed）introduced in

this manual are only suitable for this product and those machines fixed with this product. The actual function configurations and technical performance are depended on the machine builder’s design. And the CNC machine functio configuration and technical specifications are defined by machine builder’s manual.

 Though this system is employed with integrated operator panel, the functions o

the keys on the panel are defined by PLC program (ladder). It should be noted tha the keys functions are narrated for the standard PLC program in this manual.

 For the panel key functions and significance, please refer to the machine builder’s

manual.

NOTE！

The content of this manual is subject to change without further notice.

GSK980MD milling CNC system

CAUTIONS

■ Transportation and Storage

 The product package box stacking should not exceed 6 layers.  Don’t crawl, stand or place heavy object on the product package box.  Don’t draw or move this product by the cables connected with it.  Don’t collide to or scratch panel and displayer.  The product package box should be prevent from moisture, insolation and drenching.

■ Check by opening box

 Whether the product is the ordered one after opening the package.  Whether the product is damaged during transiting.  Whether the parts are complete or damaged by ordering sheet.  If the product model doesn’t correspond to the ordered one, subsidiaries are lacking or damaged in

transiting, please contact us in time.

■ Wiring

 Wiring and check should be done by the qualified technicians.  This product must be securely grounded with a grounding resistance less than 4Ω, and the

grounding wire can’t be replaced by a neutral wire (zero wire)

 The wiring must be correct and secure to protect against product fault or unexpected result.  The surge diode connected with this product must be joint by the specified direction or this product

may be damaged.

 The power supply of this product must be cut off prior to pluging or opening the product cabinet.

■ Reparation

 Cut off the power supply before reparation or component replacement.  If short-circuit or overloading occurs, check the fault first, then restart after the fault is eliminated.  Don’t switch on or off power frequently, the interval should be at least 1 minute for the repowering

after power off.

PART 1

Part 1 Programming

PROGRAMMING

Contents

CHAPTER 1 PROGRAMMING ..................................................................................................Ⅰ-1

1.1 GSK980MD Brief............................................................................................................Ⅰ-1

1.2 Execution of the Program ................................................................................................Ⅰ-7

1.2.1 Order of the program execution.............................................................................Ⅰ-7

1.2.2 Execution order of command word within block...................................................Ⅰ-8

CHAPTER 2 MSTF COMMAND................................................................................................Ⅱ-1

2.1 M Command (Miscellaneous Function) ..........................................................................Ⅱ-1

2.1.1 EP (End of program) M02......................................................................................Ⅱ-1

2.1.2 End-of-run M30 .....................................................................................................Ⅱ-2

2.1.3 Subprogram call M98 ............................................................................................Ⅱ-2

2.1.4 Return from subprogram M99...............................................................................Ⅱ-2

2.1.5 Macro program call M9000~M9999......................................................................Ⅱ-3

2.1.6 M command defined by standard PLC ladder diagram .........................................Ⅱ-4

2.1.7 Program stop M00..................................................................................................Ⅱ-4

2.1.8 Spindle CCW, CW, stop control M03, M04 and M05...........................................Ⅱ-4

2.1.9 Coolant control M08, M09 ....................................................................................Ⅱ-4

2.1.10 Lubricant control M32, M33................................................................................Ⅱ-5

2.2 Spindle Function ..............................................................................................................Ⅱ-6

2.2.1 Spindle speed switching value control................................................................... Ⅱ-6

2.2.2 Spindle speed analog voltage control.....................................................................Ⅱ-6

2.2.3 Spindle override.....................................................................................................Ⅱ-7

2.3 Tool Function ...................................................................................................................Ⅱ-8

2.4 Feeding Function..............................................................................................................Ⅱ-8

2.4.1 Cutting feed (G94/G95, F command).................................................................... Ⅱ-8

2.4.2 Manual feed .........................................................................................................Ⅱ-10

2.4.3 MPG/ Step feed....................................................................................................Ⅱ-10

2.4.4 Automatic acceleration or deceleration ...............................................................Ⅱ-10

CHAPTER 3 G COMMAND........................................................................................................Ⅲ-1

3.1 Brief .................................................................................................................................Ⅲ-1

3.1.1 Modal, non-modal and initial................................................................................. Ⅲ-3

3.1.2 Examples................................................................................................................Ⅲ-3

3.1.3 Related definition................................................................................................... Ⅲ-3

3.1.4 Address definition..................................................................................................Ⅲ-4

3.2 Rapid Positioning G00.................................................................................................. Ⅲ-6

3.3 Linear Interpolation G01.................................................................................................. Ⅲ-7

3.4 Arc and Helical Interpolation G02, G03..........................................................................Ⅲ-8

3.5 Dwell G04......................................................................................................................Ⅲ-12

3.6 Plane Selection Command G17, G18 and G19..............................................................Ⅲ-13

3.7 Conversion of Inch and Metric G20 and G21.........................................................Ⅲ-14

3.8 Reference Point Return G28..........................................................................................Ⅲ-15

3.9 Return From Reference point G29.................................................................................Ⅲ-16

3.10 The 2nd, 3rd and 4th Reference Point Return G30.........................................................Ⅲ-17

3.11 Skip Function G31 .......................................................................................................Ⅲ-19

3.12 Tool Radius Compensation C (G40, G41 and G42) .................................................... Ⅲ-21

3.13 Tool Length Compensation (G43, G44, G49).............................................................. Ⅲ-23

Part 1 Programming

I

GSK980MD Milling CNC System

3.14 Workpiece Coordinate system G54~G59 ............................................................... Ⅲ-26

3.15 Compound Cycle Command........................................................................................ Ⅲ-28

Part 1 Programming

3.15.1 Brief for canned cycle........................................................................................... Ⅲ-28

3.15.2 Description for canned cycle................................................................................ Ⅲ-32

3.15.3 Cautions for canned cycle..................................................................................... Ⅲ-53

3.15.4 Examples for modal data specified in canned cycle............................................. Ⅲ-55

3.15.5 Examples for canned cycle and tool length compensation................................... Ⅲ-56

3.16 Absolute and Incremental Commands G90 and G91 .................................................. Ⅲ-58

3.17 Workpiece Coordinate System Setting G92 ................................................................ Ⅲ-58

3.18 Feed per min. G94, Feed per rev. G95......................................................................... Ⅲ-59

3.19 G98、G99.................................................................................................................... Ⅲ-60

3.20 Chamfering Function................................................................................................... Ⅲ-60

3.20.1 Linear chamfering.............................................................................................. Ⅲ-60

3.20.2 Circular chamfering........................................................................................... Ⅲ-62

3.20.3 Special................................................................................................................ Ⅲ-64

3.21 Macro Command ............................................................................................................ Ⅲ-65

3.21.1 Macro Variable................................................................................................... Ⅲ-65

3.21.2 Operation and transfer command G65............................................................... Ⅲ-66

CHAPTER 4 CUTTER RADIUS COMPENSATION.................................................................Ⅳ-1

4.1 Application for Cutter Radius Compensation.................................................................. Ⅳ-1

4.1.1 Brief....................................................................................................................... Ⅳ-1

4.1.2 Compensation value setting................................................................................... Ⅳ-2

4.1.3 Command format................................................................................................... Ⅳ-2

4.1.4 Compensation direction......................................................................................... Ⅳ-2

4.1.5 Caution................................................................................................................... Ⅳ-3

4.1.6 Example for application......................................................................................... Ⅳ-4

4.2 Offset Path Explanation for Cutter Radius Compensation.............................................. Ⅳ-5

4.2.1 Conception for inner side or outer side.................................................................. Ⅳ-5

4.2.2 Tool movement in start-up..................................................................................... Ⅳ-5

4.2.3 Tool movement in offset mode.............................................................................. Ⅳ-7

4.2.4 Tool operation in offset cancellation mode.......................................................... Ⅳ-12

4.2.5 Interference check................................................................................................ Ⅳ-13

4.2.6 Command of compensation vector cancel temporarily ....................................... Ⅳ-15

4.2.7 Exceptional case .................................................................................................. Ⅳ-16

II

Chapter 1 Programming Fundamental

CHAPTER 1 PROGRAMMING

1.1 GSK980MD Brief

The new generation popular milling machine CNC GSK980MD is an upgrade production of the GSK980MC

which is developed by GSK Company. It has adopted 32 bits high-capability CPU and super large scale programable

parts FPGA. Real-time multitask control technology and hardware interpolation technologies are performed; so the

µm level precision motion control and PLC logic control are achieved.

MST

RESET

INSERT

EOB CANCELDELETE

ALTER

INPUT

OUTPUT

CHANGE

Part 1 Programming

OFFSET

ALARM SETTING

EDIT MPGMDI

AUTO

×1 ×10 ×100

MST

JOG CW PAUSE

DRYSKIPSINGLE

COOLANT

JOG

LUR.

STOP

TOOL

CCW

RAPID

FEEDRATESPINDE OVERRIDEOVERRIDE OVER RIDE

RUN

The Technical Characters of Product：

 Three controllable axes X, Y and Z, three linked axes X, Y and Z, 0.001mm interpolation precision,

maximum speed 30/min.

 The minimum command unit 0.001mm, the electronic gear ratio of command（1～32767）/（1～32767）  The PLC is built-in that it can achieve various controls of automatic tool post and the spindle automatic gear

shift. The ladder diagram can be edited, uploaded and downloaded.

 DNC function.  Compensation functions for screw-pitch error, backlash, tool length and tool nose radius.  Straight-line and exponential type acceleration or deceleration control for obtain high-speed and high

precision machining.

 Functions for rough-milling of the round groove and rectangle groove; and also the functions of

finish-milling of the whole circle and rectangle inside and outside.

 Tapping function.  Automatic chamfering function.  Tool life management function.  Metric and inch systems conversion.

Ⅰ-1

 Full screen parts program editing, 22MB program capacity.  Parameter backup and data communication.

Part 1 Programming

 Integrated multilingual display interface chosen by the parameter.  Multilevel operation password function convenient for the equipment administration.  Bidirectional communication between CNC and CNC, CNC and PC; the CNC software and the PLC program

can be upgraded by communication.

The Technical Specification Table

Controllable axes: three axes (X, Y and Z); simultaneous control axes (interpolation axes):

three axes (X, Y and Z)

Interpolation functions: X, Y and Z axes linear, helical and optional two axes circular

interpolation. Position command range: -9999.999～9999.999mm; minimum command unit: 0.001mm Electronic gear ratio: command multiplier 1～32767，command frequency divisor 1～32767

Operation

control

G command

Rapid traverse speed: maximum 30000mm/min

Rapid override: F0, 25%, 50%, 100% four levels real-time adjustment.

Cutting feedrate: maximum 15000mm/min or 500mm/rev. (feed per revolution) Feedrate override: 0～150% sixteen-level real-time adjustment Manual feedrate: 0～1260mm/min sixteen-level real-time adjustment

MPG feed: 0.001, 0.01, 0.1mm three gears

Acceleration or deceleration: the rapid traverse by S acceleration or deceleration, the cutting

feed by exponential acceleration or deceleration.

The automatic chamfering function

62 kinds of G codes: G00, G01, G02, G03, G04, G10, G17, G18, G19, G20, G21, G28,

G29, G30, G31, G40, G41, G42, G43, G44, G49, G54, G55, G56, G57, G58, G59, G65,

G73, G74, G80, G81, G82, G83, G84, G85, G86, G88, G89, G90, G91, G92, G94, G95,

G98, G99, G110, G111, G112, G113, G114, G115, G134, G135, G136, G137, G138, G139,

G140, G141, G142, G143.

27 kinds of arithmetic, logical operation and skip can be achieved by macro command G65.

GSK980MD Milling CNC System

Operation

mode

Tapping

Precision

compensati

M command

T command

2

Ⅰ-

on

Seven operation modes: Edit, Auto, MDI, DNC, machine zero return, MPG/increment and

Manual operation. Tapping function; pitch: 0.001～500mm or 0.06～25400 teeth/inch Spindle encoder: encoder linear number can be set （0～5000p/r） The drive ratio between encoder and spindle:（1～255）：（1～255） Backlash compensation: (X, Y and Z axes) 0～2.000mm

Pitch error compensation: X, Y and Z axes, each of them have 255 compensation points, the compensation amount of each point: -0.255～0.255mm

Tool compensation: 32 groups tool length compensation, tool nose radius compensation (compensation type C)

Special M commands (redefinition is not allowed): M02、M30、M98、M99、M9000～M9999

Other M □□ commands are defined or disposed by PLC program M commands defined by standard PLC program: M00、M03、M04、M05 M08、M09、

M10、M11、M32、M33、

Up to 32 tool number（T01～T32），the tool change time sequence is achieved by PLC program. Tool life management function

Chapter 1 Programming Fundamental

The control mode of speed switching value: S □□ command is defined or deposed by PLC

Spindle

speed

control

PLC

function

Display

interface

Program

edit

Communica

tion

Suited drive

G Command Table

G code Command function G code Command function

G00

*G01

G02 G03 G04 G10

program; the standard PLC programs S1, S2, S3 and S4 directly ouput; The output of S1, S2, S3, and S4 are closed by S0.

The control mode of speed analog voltage: the spindle speed per minute is commanded by S code, output 0～10V voltage to spindle converter, the spindle stepless shift supporting 4 gears spindle mechanical gear.

9 kinds of basic command and 23 kinds of function command, 2-level PLC program that has 5000 steps and the processing time is 2µs for each step. The first level program refresh cycle is 8ms; it can offer the edit software for the ladder and PLC program communication download.

Integrated machine panel: 41 points input (key), 42 points output (LED) Basic I/O: 32 points input/ 32 points output

Displayer: 320×240 lattice, 5.7’’ mono-color LCD, CCFL back light

Display mode: multilingual interface set by parameters, which can display the machining

path.

Program capacity: 22MB, it supports the calling of the user macro, and the subprogram 4

level nesting.

Edit mode: full-screen editing, support the relative, absolute and mixed coordinates.

Bilateral program,parameter transmission between CNC and PC, CNC and CNC, supports

the system software and the download upgrade of the PLC program serial port, DNC

communication between CNC and PC

DA98 series digital AC servo or DY3 series step drive equipment by using the pulse+direction

signal input.

Positioning (rapid traverse)

Linear interpolation (cutting feed)

circular/helical interpolation by CW

circular/helical interpolation by CCW

dwell, exact stop

offset setting

G81 G82 G83 G84 G85 G86

Drilling cycle (point-drilling cycle)

Drilling cycle (counterbore cycle)

Peck drill cycle

Tapping cycle

Boring cycle

Drilling cycle

Part 1 Programming

*G17

G18 G19 G20 G21 G28 G29 G30

G31

*G40

G41 G42

XY plane selection

ZX plane selection

YZ plane selection

Inch input

Metric input

Reference point return

Return from reference point

Return from reference point (the 2nd,

3rd, 4th reference points)

Skip function

Tool radius compensation cancellation

Tool radius compensation left

Tool radius compensation right

G88 G89

*G90

G91 G92 G94 G95 G98

G99

G110 G111 G112

Boring cycle

Absolute programming

Incremental programming

Coordinate system setting

Feeding per minute

Feeding per revolution

Return to the initial plane in canned cycle

Return to the R (point) plane in canned

cycle

Round groove inner rough mill in CCW

Round groove inner rough mill in CW

Whole-circle inner finish mill in CCW

Ⅰ-3

GSK980MD Milling CNC System

G43 G44

Part 1 Programming

*G49 *G54

G55 G56

G57 G58 G59 G65 G73 G74

*G80

PLC Command Table

Basic

command

LD

LDI OUT AND

ANI

Tool length offset positively

Tool length offset negatively

Tool length offset concellation

Workpiece coordinate 1

Workpiece coordinate 2

Workpiece coordinate 3

Workpiece coordinate 4

Workpeice coordinate 5

Workpiece coordinate 6

Macro command

High-speed peck drill cycle

Left-hand tapping cycle

Canned cycle cancellation

Function

Read normally open contact

Read normally closed contact

Output loop

Normally open contact series connection

Normally closed contact series connection

G113 G114 G115 G134 G135 G136

G137 G138 G139 G140 G141 G142 G143

Function

command

TMRB CODB ROTB

MOVN

DECB

Whole-circle inner finish mill in CW

Excircle finish mill in CCW

Excircle finish mill in CW

Rectangle groove rough mill in CCW

Rectangle groove rough mill in CW

Rectangle groove inner finish mill in

CCW

Rectangle groove inner finish mill in CW

Rectangle outer finish mill in CCW

Rectangle outer finish mill in CW

Rectangle path series punch in CW

Rectangle path series punch in CCW

Circular path series punch in CW

Circular path series punch in CCW

Function

Timer

Binary system (Bit) transfer

Binary system(Bit) spin control

Data copy

Binary system(Bit) decoding

OR

ORI ORB ANB

Function

command

END1 END2

SET RST CMP

CTRC

GSK980MD Configuration Software: GSKCC

The GSKCC is run in the condition of the WIN98/2000/XP operation system, so, the machine manufacturer can

perform the GSK980MD ladder diagram, parts program, parameter, pitch error compensation data and tool

compensation data on the PC to finish the upload and download of the files between PC and GSK980MD system.

Normally open contact parallel connection

Normally closed contact parallel connection

Parallel connection of the series circuit block

Series connection of the parallel circuit block

Function

First level program ending

Second program ending

Setting

Resetting

Comparison setting

Counter

JMPB

SP

SPE

ADDB SUBB

ALT

DIFU DIFD

MOVE

PARI

LBL

CALL

Program skip

Subprogram numbering

Subprogram end

Binary (Bit) data addition

Binary (Bit) data subtraction

Alternative output

Up setting

Down setting

Logical AND

Parity check

Program skip numbering

Subprogram call

Ⅰ-

4

Chapter 1 Programming Fundamental

Part 1 Programming

GSK980MD Communication Software: TDComm

The TDComm is run in the condition of the WIN98/2000/XP, which is provided to the end user to finish the

bidirectional transmission of the parts program, the parameter, pitch error compensation data and tool compensation

data between PC and CNC.

GSK980MD DNC Communication Software: GcodeEdit

The GcodeEdit is run in the condition of the WIN98/2000/XP. which is provided to the manufacturer or the end

user to finish the DNC program transmission between PC and CNC.

Ⅰ-5

GSK980MD Milling CNC System

Part 1 Programming

Ⅰ-

6

Chapter 1 Programming Fundamental

1.2 Execution of the Program

1.2.1 Order of the program execution

The GSK980MD can not open two or more programs at the same time; it can run the current opened program in

Auto mode. So, the GSK980MD can perform only one program at any time. The cursor is located at the beginning of

the row of the first block when a program is opened, and the cursor can be moved in Edit mode. Start the execution of

the program from the block the current cursor is located at by using the cycle start signal (

external cycle start key) in the halt state of Auto mode, usually, the blocks are executed one by one in the order of the

blocks editing, and the execution is stopped till the M02 or M03 code is executed. The cursor is moved along with the

program execution. The program execution sequence or state will be changed in the following conditions:

 The program execution will be stopped if the

RESET

key or the Emergency Stop button is pressed;

 The program execution will be stopped if the CNC alarm or PLC alarm is generated;  The operation mode is switched to the MDI or Edit mode when the program is being executed; or the

program is started from the block the cursor is located at when switching to Auto mode by single block stop

(The program pauses after the current block executed), and then the

key is pressed or external

cycle start signal is ON;

 The operation mode is switched to Manual, MPG, Step and Machine zero mode when the program being

executed. The program is held on, then switching to Auto mode, and then the communication is switched

key on the panel or

Part 1 Programming

on when the

key is pressed or external cycle start signal is ON, the program is operated from the

halt position;

 The program pauses when pressing

from stopped position when pressing

FEED HOLD

key or external pause signal is cut off, the program is operated

key or external cycle start signal is ON;

 The program pauses after each block is executed when the single block switch is opened, pressing

key or switching on external cycle start signal is needed, program is executed continuously from the next

block;

 The skip switch of the block is opened which it is skipped or inexecuted when the “/” is in front of the

block;

 The skip object block is turned to when the G65 skip command is performed

 When M98 or M9000~M9999 command is performed, to call corresponding subprogram or macro run; the

subprogram or macro run is ended, when the M99 command is to be performed, to call the next block run

as returning to the mainprogram (If M99 command specifies the return object block number, then run by

skipping to object block);

 When the M99 command is performed in main program (its run is not started up because others program

calls), then returning to the program first stage to continue run, so the current program will be run

circularly.

Ⅰ-7

GSK980MD Milling CNC System

1.2.2 Execution order of command word within block

R, M, S and T, most command words M, S and T are explained by NC before sending to PLC for processing, the

other command words are processed by NC directly. M98, M99, M9000~M9999, as well as S command word for

Part 1 Programming

spindle speed by rev/min, m/min units are all processed by NC directly.

When G command shares a same block with M00, M01, M02 and M30, the NC performs M command after

finishing G command, and then sending the corresponding M signal to PLC for processing.

When the G command shares a same block with the M98, M99, M9000~M9999, these M command words are

performed by NC after it finishes the G command (the M signal not sent to PLC).

As the M, S and T command words processed by PLC and the G command words are sharing the same block,

the M, S and T command words are performed with the G command words at the same time which they are

determined by PLC program (ladder diagram), or the M, S and T command words are performed after the G

command is finished. As for the performance order of the command words, refer to the explanation of the machine

tool manufacturer.

Ⅰ-

8

Chapter 2 MSTF Command

CHAPTER 2 MSTF COMMAND CHAPTER 2 MSTF COMMAND

2.1 M Command (Miscellaneous Function) 2.1 M Command (Miscellaneous Function)

The M command word composed by command address M and 1~2 or 4 digits after the command M is used for

controlling the program execution or outputting M code to PLC.

M □□□□ M □□□□

Command address

M98, M99 and M9000~M9999 are independently processed by NC, and the M code is not output to PLC.

The M02 and M03 are defined as program END command by NC, at the same time it also gives the M code to

PLC for using the I/O control (close spindle, close cooling etc.).

The PLC program can not change the meaning of the above-mentioned commands when the M98, M99 and

M9000~M9999 are regarded as program CALL commands and the M02 and M30 are regarded as program END

commands. The codes of other M commands are all given to PLC program for specifying the command function;

please refer to the manual issued by machine tool manufacturer.

One block only has one M command. The CNC alarm occurs when two or more M commands are displayed in

one block.

Command value (00~99、9000~9999，leading zero can be omitted)

Table 2-1 M command table for program execution

Part 1 Programming rt 1 Programming

Commands Functions

M02 End-of-Run

M30 End-of-Run

M98 Subprogram call

Return from the Subprogram; the program will be circularly executed

M99

M9000～M9999

if the command M99 is used for main program ending (namely, the

current program is not called by other programs).

Call macro program (Program No. more than 9000)

2.1.1 EP (End of program) M02

Format: M02

Command function: The M02 command is executed in the Auto mode. The automatic run is ended when the

other commands of current block are executed; now in order to not return to the program

beginning, the cursor is stop at block which the M02 located. If the program is executed

again the cursor should be stopped at the beginning of the program.

The function of command M02 also can be defined by the PLC ladder diagram other than the abovementioned

functions which are processed by NC. The standard ladder diagram can be defined as: the current input state of CNC

is not change after the command M02 is executed.

Ⅱ-1

GSK980MD Milling CNC System

g

2.1.2 End-of-run M30 2.1.2 End-of-run M30

Format: M30 Format: M30

Part 1 Programming

rt 1 Programming

Command function: If M30 command is executed in the Auto mode, the automatic run is ended when the other

commands of current block are executed; the system cancels the nose radius compensation and the

cursor returns to the beginning of the prgram when the machine pieces number is added by 1 (It is

up to parameter if the cursor returns to the beginning).

The cursor is not return to the beginning of the program when the BIT4 of parameter No.005 is set to 0 in CNC;

w

hen it is set to 1, the prgram is finished, so the cursor returns to the beginning of the program at once.

when it is set to 1, the prgram is finished, so the cursor returns to the beginning of the program at once.

The function of command M30 can be defined by the PLC ladder diagram other than the abovementioned

fu

nctions processed by NC. The standard ladder diagram can be defined as: to close the M03, M04 or M08 signal

functions processed by NC. The standard ladder diagram can be defined as: to close the M03, M04 or M08 signal

output after the M30 command is executed, at the same time the M05 signal is given.

2.1.3 Subprogram call M98 2.1.3 Subprogram call M98

Format：M98 P○○○○□□□□ Format：M98 P○○○○□□□□

Command function: when the M98 command is executed in the Auto mode, CNC calls and executes the

subprogram specified by P, which can be performed 9999 times at most, when the other commands

of current block are executed. The M98 command is disabled in MDI.

The called subprogram No.（0000～9999）.The

leading zero of subprogram can be omitted when

the call frequency are not given; the subprogram

No. should be 4 digits when the calling frequency is

iven;

Calling frequency（1-9999），calling for once, the

input can be omitted

2.1.4 Return from subprogram M99 2.1.4 Return from subprogram M99

Format： M99 P○○○○ Format： M99 P○○○○

Command function: (in subprogram) as the other commands of current block are executed, the block specified

by P is performed continuously when the main program is returned. The next block is performed

continuously by calling current subprogram of M98 command when returning to the

mainprogram; because of the P is not given. If the main program is ended by using the M99

(namely, the current program is not called by other programs for execution), the current program

will be run circularly. So, the M99 command is disabled in MDI.

The block No. (0000～9999) to be executed

when a mainprogram is returned, the leading

zero can be omitted.

Example: Fig. 2-1shows that the execution route of the subprogram is called (the P command within M99). Fig.

2-2 shows that the execution route of the subprogram is called (the P command is not in M99).

2

Ⅱ-

Chapter 2 MSTF Command

N

O1009；

主程序

0010 ………;

0020……….;

0030……….;

0040 M98 P1010;

0050……….;

0060……….;

0070……….;

……..

Fig.2-1

O1010；

子程序

1020………;

1030………;

………

1100 M99 P0070;

%

Part 1 Programming rt 1 Programming

Ｏ0001;

G92 X100 Z100;

M3 S1;

G0 X0 Z0;

G1 X200 Z200 F200;

M98 P21006;

G0 X100 Z100;

M5 S0;

M30;

%

Mainprogram

Call

Return

Fig. 2-2

Ｏ1006;

G90 G1 X50 Z50;

G91 X100 Z200;

X30 Z-15 F250;

M99;

%

Subprogram

This GSK980MD can calls quadruple subprogram, namely, the other subprogram can be called from the

subprogram. (See Fig. 2-3)

Mainprogram

O 1001；

... ... ... M98P1002; ... ... ... ... M30;

Subprogram

O 1002；

... ... ... M98P1003; ... ... ... ... M99;

S in g le n e stification D o u b le nes tific a tio n

Subprogram

O 1003；

... ... ... M98P1004; ... ... ... ... M99;

Subprogram

O 1004；

... ... ... M98P1005; ... ... ... ... M99;

T rip lic a te n estification Q u a d ru p le n estification

Subprogram

O 1005；

... ... ... M98P1005; ... ... ... ... M99;

Fig. 2-3 Subprogram nestifications

2.1.5 Macro program call M9000~M9999

Format： M□□□□

9000

Command function: Call the macro program which is corresponded by the command value

Macro program: Program 09000~09999 is special space obligated for the machine tool manufacturer for using

editing and achieving speical function subprogram, which is called marco program. Two-level operation authority is

～

9999

（O9000～O9999）.

Ⅱ-3

GSK980MD Milling CNC System

needed when editing the program 09000~09999, the user can not modifiy or operate the macro program but the

macro calling command if his authority is 3~5 level. So the M9000~M9999 command operates invalidly in MDI.

Part 1 Programming

2.1.6 M command defined by standard PLC ladder diagram

The M commands other than the abovementioned commands (M02, M03, M98, M99, M9000~M9999) are

defined by PLC. The M commands are defined by standard PLC hereinafter. This GSK980MD milling machine is

used for machine control. About the function, meaning, control time sequence and logic etc. of the M command,

refer to the manual issued by the machine tool builder.

M command specified by standard PLC ladder diagram

Commands Functions Remarks

M00 Program pause

M03 Spindle CCW

M04 Spindle CW

*M05 Spindle stop

M08 Coolant on

*M09 Coolant off

M32 Lubrication on

*M33 Lubrication off

Function interlock,

state hold

Notes: The command with “*” specified by standard PLC is valid when the power is turned on.

2.1.7 Program stop M00

Format: M00

Command function: the program is stopped after executing the M00 command, the “pause” is displayed; the

program will continue when the key of Cycle Start is pressed.

2.1.8 Spindle CCW, CW, stop control M03, M04 and M05

Format: M03;

M04;

M05;

Command function: M03: spindle forward rotation (CCW);

M04: spindle reverse rotation (CW);

M05: spindle stop.

Note: The control time sequence and logic of M03, M04 and M05 are specified by standard PLC program, refer to the Appendix of this manual.

2.1.9 Coolant control M08, M09

Format: M08;

M09;

Command function: M08: cooling on;

M09: cooling off.

Note: The control time sequence and logic of M08 and M09 are specified by standard PLC program, refer to the Appendix of this manual.

4

Ⅱ-

Chapter 2 MSTF Command

2.1.10 Lubricant control M32, M33

Format: M32;

M33;

Command function: M32: lubrication on;

M33: lubrication off.

Note: The control time sequence and logic of M08 and M09 are specified by standard PLC program; refer to the Appendix of this manual.

Part 1 Programming

Ⅱ-5

2.2 Spindle Function 2.2 Spindle Function

GSK980MD Milling CNC System

Part 1 Programming rt 1 Programming

The spindle speed is controlled by S command, there are two ways to control spindle speed for GSK980MD. The spindle speed is controlled by S command, there are two ways to control spindle speed for GSK980MD.

Spindle speed switching value control mode: the S□□ (2-digit command value) command is processed by PLC

pr

ogram for exporting the switching value signal to machine, so that the step speed change of the spindle is achieved.

program for exporting the switching value signal to machine, so that the step speed change of the spindle is achieved.

Spindle speed analog voltage control mode: the actual spindle speed is specified by the S□□□□ (4-digit

co

mmand value), the NC outputs the 0~10V analog voltage signal to the spindle servo device or transducer for

command value), the NC outputs the 0~10V analog voltage signal to the spindle servo device or transducer for

ac

hieving the stepless speed regulating of the spindle.

achieving the stepless speed regulating of the spindle.

2

.2.1 Spindle speed switching value control 2.2.1 Spindle speed switching value control

The spindle speed is on switching value control when the BIT4 of bit parameter NO.001 is set to 0. One block

only has one S command. The CNC alarm occurs when there are two or more S commands displayed in block.

When the S command shares the same block with the command word, the performance sequence is defined by

PLC program. For details, refer to the manual issued by the machine tool builder.

This GSK980MD milling machine is used for machining control when the spindle speed switching value is

controlled. The time sequence and logic for S command should be referred by the manual issued by the machine tool

builder. The following S command is defined by GSK980MD standard PLC, for reference only.

Command format: S□□Command format: S□□

～

00

04 (the leading zero can be omitted): 1～4 gears spindle speed

switching value control.

In spindle speed switching value control mode, the FIN signal is returned after the set time of data parameter

No.081 is delayed after the code signal of S command is sent to PLC. Now the time is called execution time of S

code.

The S01, S02, S03 and S04 output states are invariable when the CNC is reset.

The S1~S4 commands are ineffective output when the CNC is switched on. An arbitrary command is performed

from S01, S02, S03 and S04, the corresponding S signal output is effective and held on, at the same time the other 3 S

signal output are cancelled. The S1~S4 output are cancelled when performing the S00 command, only one of S1~S4

is effective in the meantime.

S code performs

Delay time

Subsequent command word or block

performs

2.2.2 Spindle speed analog voltage control

The spindle speed is analog voltage control when the BIT4 of current bit parameter is set to 1

Format

Command function: The CNC outputs 0~10V analog voltage to control the spindle servo or transducer for

：S OOOO

0000

～9999 (leading zero can be omitted): Spindle speed analog voltage control

achieving the stepless speed regulating of the spindle when the spindle speed is set. The S command

value is not memorized when the power is turned off; and then the parameter recovers to 0 when the

power is turned on.

Ⅱ-

6

Chapter 2 MSTF Command

The CNC owns four mechanical spindle shifts function. Counting the corresponding analog voltage value

specified by the speed based upon the current set value (corresponding to data parameter No.037~No.040) of the top

speed (output analog voltage is 10V) of the spindle shift when the S command is performed, then output the voltage

value to spindle servo or transducer, so that the consistency of actual speed and required speed of the spindle are

controlled.

The analog voltage output is 0V when the CNC is switched on. The output analog voltage value is invariable

(Unless the cutting feed in constant linear speed control and the absolute value of X axis absolute coordinate value

are changed) after the S command is executed. The analog voltage output is 0V when the command S0 is executed.

And the analog voltage output value is invariable when the CNC is reset or at urgent stop.

The parameter related to spindle speed analog voltage control:

Data parameter No.021: the output voltage offset for spindle top speed (the output analog voltage is 10V);

Data parameter No.043: the voltage offset for the zero spindle speed (the output analog voltage is 0V);

Data parameter No.037~No.040: The top speed for spindle 1~4 shifts (the output analog voltage is 10V);

2.2.3 Spindle override

Part 1 Programming

The spindle actual speed can be modified by using spindle override when the spindle speed analog voltage

control is effective, the actual speed modified by spindle override is limited by the top speed of current spindle shift,

and also it is controlled by the lowest spindle limitation value and the top spindle limitation value in constant linear

speed control mode.

This NC offers 8-level spindle override (50%~120%, the change is 10% per level).

modificative mode of the spinde

override are defined by PLC ladder diagram. Refer to the manual

The actual level and the

issued by the machine tool builder when attempting to use it. The following is function description is GSK980MD standard PLC ladder diagram, for reference only.

The spindle override defined by GSK980MD standard PLC ladder digaram has 8 levels. The spindle actual

real-time speed can be adjusted by using the spindle override key in the command speed range of 50%~120%, the

spindle override will be memorized when the power is turned off. Refer to the OPERATION of this manual for

modification operation of the spindle override.

Ⅱ-7

2.3 Tool Function

GSK980MD Milling CNC System

Part 1 Programming

There is no tool function in this 980MD system.

2.4 Feeding Function

2.4.1 Cutting feed (G94/G95, F command)

Format: G94F_; (F0001~F8000, leading zero can be omitted, for feed speed per minute, mm/min)

Command function: The cutting feedrate is specified by mm/min, G94 is modal G command. If the current

mode is G94 that it needs no G94 any more.

Format: G95F_; (F0.0001~F500, leading zero can be omitted)

Command fucntion: The cutting feedrate is offerred by the unit of mm/rev., G95 is modal G command. The G95

command can be omitted if the current mode is G95. When the CNC performs G95 F_, the cutting

feedrate is controlled by feedrate command based on the multiplication of F command value

(mm/rev) and current spindle speed (rev/min). The actual feedrate varies with the spindle speed. The

spindle cutting feedrate per revolution is specified by G95 F_, the even cutting line can be formed

on the face of workpiece. It is necessary to install spindle encoder when the G95 mode is operated.

The G94 and G95 are modal G commands at the same group, one of them is available only. The G94 is initial

state G command, so, it defaults the G94 when the CNC is switched on. The following below shows the conversion

formula of feed value per rev. and feed value per min:

F

= Fr×S

m

Thereinto: F

F

S: spindle speed (r/min).

The feedrate value is set by the CNC bit parameter No.053 when the CNC is switched on, the F value is

invariable after the F command is executed. The feedrate is 0 after F0 is executed. The F value is invariable when

CNC is reset or at urgent stop.

Note: In G95 mode, the cutting feedrate will be uneven when the spindle speed is less than 1 rev. /min. The following error will exist in the actual feedrate when the spindle speed vibration occurs. To guaranteen the machine quality, it is recommanded that the spindle speed selected in machining is not less than the lowest speed of available torque exported by spindle servo or transducer.

Cutting feed: The CNC makes tool movement path and the path (linear or circular arc) defined by command into

consistency (The circular interpolation can be performed by two axes in selected plane when it is

circular arc, the helical interpolation is formed by the third axis linear interpolation linkage), by which,

the CNC controls three directions movement for X axis, Y axis and Z axis at the same time. The

instantaneous speed of movement path in a tangential direction is consistent with the F command

value, so this is called CUTTING FEED or INTERPOLATION. The cutting feedrate is supplied by F

command, which it is disassembled to each interpolation axis according to the programming path

when the CNC performs the interpolation command (cutting feed).

: feed value per minute (mm/min);

m

: feed value per revolution (mm/r);

x

Ⅱ-

8

Chapter 2 MSTF Command

Linear interpolation: The CNC can controll the instantaneous speed in the directions of X axis, Y axis and Z

axis, so the vector resultant speed in these three directions are equal to the F command value.

=

f

x

f

=

y

f

=

z

F is vector resultant speed for the instantaneous speed in X, Y and Z axis directons

The d

is instantaneous increment of the X axis, the fx is instantaneous speed of X axis.

x

The d

is instantaneous increment of Y axis, the fy is instantaneous speed of Y axis.

y

The d

is instantaneous increment of Z axis, the fz is instantaneous speed of Z axis.

z

Circular interpolation (helical interpolation): Performing the arc interpolation in selected plane, the third axis

performs linear interpolation, so the F value is circular interpolation speed. An interpolation of linear and circular arc

has the following relation when the linear interpolation speed is f:

d

x

++

d

y

++

d

z

++

Ff ×=

F

•

222

ddd

zyx

F

•

222

ddd

zyx

F

•

222

ddd

zyx

length axis linear

lengtharc circular

Part 1 Programming rt 1 Programming

Tool p a th

F e e d ra te a long the circ le betw een 2 arc

interpolation axes is the specified one .

There are 16 levels feedrate override (0~150%, 10% per level) are offerred by NC. The actual feedrate series,

the memory performed or not when the power is turned off and the method of overriding are defined by PLC ladder

diagram. Refer to the manual issued by the machine tool builder. The function description of GSK980MD standard

PLC ladder diagram is as follows, for reference only.

By using the feedrate override key of the machine panel or external override switch it can performs real-time

modification for the cutting feedrate. The actual cutting feedrate can be adjusted in the range of command speed

0~150%, here, the feedrate is memorized when the power is turned off. How to operate the cutting feedrate

adjustment, refer to Chapter 3 OPERATION of this manual.

Related parameter:

CNC parameter No. 029: the exponential acceleration or deceleration time constant of cutting feed and manual

feed.

CNC parameter No.030: the initial (terminal) speed of exponential acceleration or deceleration for cutting feed.

CNC parameter No.031: the upper limit value (X axis, Y axis and Z axis are same) of the cutting feedrate.

Ⅱ-9

GSK980MD Milling CNC System

2.4.2 Manual feed

Manual feed: This GSK980MD can perform positive/negative movement of X, Y or Z axis by the current

Part 1 Programming

This NC offers 16 levels (0~150%, 10% each time) manual feedrate (override), see the following table 2-2. The

actual feedrate series and modification mode or the like in manual feeding, are defined by PLC ladder diagram. Refer

to the manual issued by the machine tool builder. The function description of GSK980MD standard PLC ladder

diagram is as follows, for reference only.

Feedrate

override(%)

Manual

feedrate

(mm/min) Note: The manual feedrate of X axis is diameter variation per minute; the feedrate defined by GSK980MD standard PLC ladder diagram is memorized when the power is turned off.

Related parameter: Data parameter No.029: for exponential acceleration or deceleration time constant in manual

manual feedrate in the Manual mode. X axis, Y axis and Z axis can be moved at one time.

Table 2-2

0 10 20 30 40 50 60 70 80 90 100 110 120 130 140 150

0 2.0 3.2 5.0 7.9 12.6 20 32 50 79 126 200 320 500 790 1260

feed.

Data parameter No.041: for speed lower limit of acceleration or deceleration in manual feed.

2.4.3 MPG/ Step feed

MPG feed: This GSK980MD can move positively or negatively in X, Y or Z axis by current increment in the

MPG mode. Only one of the axes can be moved at one time.

Step feed: This GSK 980MD can move positively or negatively for X, Y or Z axis by current increment in the

Step mode. One of the axes can be moved only at one time.

Only one mode is effective for the MPG or step mode at one time, it is up to Bit3 of CNC bit parameter No.001.

This NC offers 4 steps (0.001mm, 0.01mm, 0.1mm and 1mm) MPG/ step increment. The actual MPG/ step

increment series, the selection of increment and current effective axis or the like, are defined by PLC ladder diagram.

Refere to the manual issued by the machine tool builder.

Related parameter: Data parameter No.029: for exponential acceleration or deceleration time constant of cutting

feed and manual feed.

Data parameter No.041: for initial or terminal speed of exponential acceleration or deceleration in manual feed.

2.4.4 Automatic acceleration or deceleration

This GSK980MD performs automatically acceleration or deceleration in order to achieve the smooth transition

of the speed at the beginning of the axis movement or before the movement stops; this will diminish the impact when

the movement is start or stop. This GSK980MD adopts kinds of acceleration or deceleration as follows:

Rapid traverse: linear type front acceleration or deceleration

Cutting feed: exponential type rear acceleration or deceleration

Manual feed: exponential type rear acceleration or deceleration

MPG feed: exponential type rear acceleration or deceleration

Step feed: exponential type rear acceleration or deceleration

Ⅱ-

10

Chapter 2 MSTF Command

r

A

r

A

r

A

r

A

Speed after interpolation

Speed by acceleration or

deceleration control

Part 1 Programming

CNC

comm

ad

Pulse

assignment

(In terpolati

on)

cceleration or

deceleration control

cceleration or

deceleration control

cceleration or

deceleration control

Fig. 2-9

Drive control

FR: Rapid traverse rate

Set by data parameter No.022,

No.023 and No.024 parameter

: Rapid traverse acceleration o

T

R

deceleration time constant

Set by data parameter No.025,

No.026 and No.027 parameter

X axis

moto

Y axis

moto

Z axis

moto

Fig. 2-10 Curve for rapid traverse

Feedrate

cceleration or deceleration

time constant for cutting

feedrate

Time

FC: feedrate

TC: The acceleration or deceleration time constant of cutting feedrate

(Data parameter No.029)

Fig. 2-11 Curves for cutting and manual feedrate

Ⅱ-11

GSK980MD Milling CNC System

A

When the cutting feed is performed, this GSK980MD adopts exponential rear acceleration or deceleration, an

Part 1 Programming

arc transition will be formed for the acceleration or deceleration at the meeting point of the path for the adjacent two

rt 1 Programming

cu

tting feed blocks, when the BIT3 of the bit parameter No.007 is set to 0. A contour error exists between the actual

cutting feed blocks, when the BIT3 of the bit parameter No.007 is set to 0. A contour error exists between the actual

to

ol path and the programmed path when the positioning is not enough accurate at the meeting point of the two paths.

tool path and the programmed path when the positioning is not enough accurate at the meeting point of the two paths.

In

order to avoid this kind of error, the exact stop command (G04;) can be inserted between the two blocks or the

In order to avoid this kind of error, the exact stop command (G04;) can be inserted between the two blocks or the

B

IT3 of the CNC bit parameter No.007 is set to 1. Now, the previous block is decelerated to zero speed and it is

BIT3 of the CNC bit parameter No.007 is set to 1. Now, the previous block is decelerated to zero speed and it is

po

sitioned to the end of the block, and then the next cutting feed block is performed. The following block can be

positioned to the end of the block, and then the next cutting feed block is performed. The following block can be

pe

rformed because each block is accelerating from the initial speed and then decelerating to zero at last. If the

performed because each block is accelerating from the initial speed and then decelerating to zero at last. If the

pr

ogram time is increasing, it may cause the lower machining efficiency.

program time is increasing, it may cause the lower machining efficiency.

The BIT3 of bit parameter No.007 is set to 0, the transition between two adjacent blocks is processed according

to the table 2-3.

Table 2-3 Table 2-3

block

Next block Next block

block

Rapid positioningRapid positioning Cutting feed Cutting feed

Without move Without move

Rapid positioning X X X

Cutting feed X O X

Without move X X X

Note: X: The subsequent block is perfomed after the previous block is accurately positioning

at the end of he block.

O: Each axis speed is transitted according to the acceleration or deceleration between

the adjacent blocks; an arc transition is formed at the meeting point of the tool path. (Inaccurate positioning)

Example (The BIT3 of the bit parameter is set to 0)

G91 G01*-100; (X axis move negatively)

Z-200; (Z axis move negatively)

Y-300; (Y axis move negatively)

X

Z

Programmed path

ctual movement tool path

Fig. 2-12

12

Ⅱ-

Chapter 3 G Command

CHAPTER 3 G COMMAND CHAPTER 3 G COMMAND

3.1 Brief 3.1 Brief

The G command is composed by the command address G and the1 to 3 digits command value after the

command G. Many kinds of operations are specified such as tool movement relative to workpiece, coordinate set,

etc.See Table 3-1 for G commands.

G □□□G □□□

The G command words can be classified to 11 groups such as 00, 01, 02, 03, 05, 06, 07, 08, 09, 10 and 14. They

share the same block except for 01 and 00 groups, different groups G commands can be defined at the same block.

The last G command is valid when two or more same group G commands are introduced at the same block. Different

G command groups without common parameter (command word) can be defined at the same block, and their

functions are simultaneously valid regardless of sequence. If the G command or the optional G command other than

Command value (00~143, the leading zero can be omitted)

Command address G

Part 1 Programming art 1 Programming

Table 3-1 is employed, alarm occurs.

Table 3-1 G command word list

Command words Groups Functions Remarks

G04 Dwell, exact stop

G28 Machine zero return

G29 Return from reference point

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

G31 Skip function

G92 Coordinate system set

G65

G00 (initial G command) Rapid traverse

G01 Linear interpolation

G02 Circular interpolation (CW)

G03 Circular interpolation (CCW)

G73

G74

G80 (initial G command)

G81

G82 Drilling cycle (counterbore cycle)

00

Macro

01

Peck drilling cycle

Left-hand (counter) tapping cycle

Canned cycle cancellation

Drilling cycle (spot drill cycle)

Non-modal G

command

Modal G

command

G83

G84

G85 Boring cycle

G86

G88

Peck drilling cycle

Tapping cycle

Drilling cycle

Boring cycle

Ⅲ-1

GSK980MD Milling CNC System

Command words Groups Functions Remarks

Part 1 Programming

G17 (initial G command) XY plane selection

G90 (initial G command) Absolute programming

G89

G110 Circular groove inner rough-milling CW

G111 Circular groove inner rough-milling CCW

G112 Circular groove inner fine-milling CW

G113 Circular groove inner fine-milling CCW

G114 Excircle finish-milling CW

G115 Excircle finish-milling CCW

G134 Rectangle groove rough-milling CW

G135 Rectangle groove rough-milling CCW

G136 Rectangle groove inner finish-milling CW

G137 Rectangle groove inner finish-milling CCW

G138 Rectangle outter finish-milling CW

G139

G18 ZX plane selection

G19

G91

Boring cycle

Rectangle outter finish-milling CCW

02

YZ plane selection

03

Relative programming

Modal G

command

Modal G

command

G94 (initial G command)

G95

G20 Data input in inch

G21

G40 (initial G command) Tool nose radius compensation cancellation

G41 Tool nose radius compensation left

G42

G43 Tool length offset in + direction

G44 Tool length offset in - direction

G49 (initial G command)

G140 Rectangle path serially punch CW

G141 Rectangle path serially punch CCW

G142 Arc path serially punch CW

G143

G98 (initial G command) Return to initial level in canned cycle

G99

G54 (initial G command)

G55 Workpiece coordinate system 2

G56 Workpiece coordinate system 3

G57 Workpiece coordinate system 4

G58 Workpiece coordinate system 5

G59

05

06

07

08

09

10

14

Feed per minute

Feed per revolution

Data input in metric

Tool nose radius compensation right

Tool length offset cancellation

Arc path serially punch CCW

Return to R level in canned cycle

Workpiece coordinate system 1

Workpiece coordinate system 6

Modal G

command

Modal power

down memorize

Modal G

command

Modal G

command

Non-modal G

command

Modal G

command

Modal G

command

Ⅲ-

2