gsk GSK928MA User Manual

GSK928MA

Milling Machine CNC System

User Manual

GSK CNC Equipment

The operating manual describes all matters concerning the operation of the system in detail as

much as possible. However, it is impractical to give particular descriptions of all unnecessary

and/or unavailable works on the system due to the text size limit of the manual, specific operations

of the product and other causes. Therefore, the matters not specified herein may be considered

impractical or unavailable.

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.

Dear user,

We are really grateful for your patronage and purchase of GSK928M milling CNC system made by

GSK CNC Equipment Co., Ltd.

Company Profile

As an industrial base of numerical control (NC) products in south China and an enterprise undertaking the

state’s Plan 863 “Middle-grade Numerical Control System Industrialization Supporting Technology”, GSK

has been committed to the development and manufacture of NC systems for machine tools and

servo/step motor drive units for years. GSK actively promotes machine tool NC innovation and offers NC

technical training and trade services of numerical controlled machine tools – integrating science,

engineering and trading. Our products support more than 50 domestic manufacturers of machine tools

with after-sales service network through the country. With a yield in the lead in China for four years in

succession, GSK series products are in great demand in the domestic demand and have sold as far as to

Southeast Asia at high cost-performance ratio.

Field T echni cal Support Service

Field support services are available when you encounter problems insolvable through telephone. GSK

CNC Equipment Company Limited will designate a technical support engineer to the field to solve

technical problems for you.

All specification and designs are subject to change without notice。

Sincerely thanks for your friendly support for our products.

Contents

Programming

1 Introduction..................................................................................................................................................5

1.1 Axis Definition .....................................................................................................................................5

1.2 Machine zero........................................................................................................................................5

1.3 Reference point...................................................................................................................................5

1.4 Coordinate System .............................................................................................................................5

1.5 Programming Coordinates................................................................................................................6

1.6 Input Unit and Range of Coordinate.................................................................................................6

1.7 Program Configuration.......................................................................................................................6

1.8 Tool Path of Rapid Position ing.........................................................................................................8

1.9 Offset of System Coordinate.............................................................................................................8

1.10 Initial and Modal of Sy stem..............................................................................................................8

1.11 Initial Status of System.....................................................................................................................8

1.12 Start of Program................................................................................................................................9

1.13 End of Program.................................................................................................................................9

1.14 Main Program and Subprogram......................................................................................................9

1.15 Backlash Compensation................................................................................................................10

1.16 R Reference Plane...........................................................................................................................10

2 S, T, M Function, D, H, F, FEED%............................................................................................................11

2.1 S Function..........................................................................................................................................11

2. 2 T Function .........................................................................................................................................11

2.3 M Function (Auxiliary Function )......................................................................................................11

2.4 D, H Function.....................................................................................................................................13

2.5 F, Feed%.............................................................................................................................................13

3 G Function (Preparatory Function).........................................................................................................14

3.1 G Function for Defining Programming State of the System .......................................................14

3. 2 G0 Rapid Positioning (Modal, Initial).............................................................................................14

3. 3 G1 Linear Interpolation (Modal)......................................................................................................15

3.4 G2, G3 Circular Interpolation (Modal).............................................................................................15

3. 5 G4 Dwell.............................................................................................................................................16

3. 6 G10 G11 Rough Milling in Concave Groove of Inner Circular ...................................................16

3. 7 G12 /G13 Finish Milling of Inner Circle..........................................................................................17

3. 8 G14 /G15 Fine Milling of Outer Circle............................................................................................18

3. 9 G22 System Parameter Setting (Modal)........................................................................................18

3.10 G23 Conditional Jump....................................................................................................................19

3.11 G27 Machine Zero Inspection........................................................................................................19

3.12 G28 Rapid Traverse to Reference Point via Middle Point..........................................................20

3.13 G31 Rapid Return to the R Reference Plane...............................................................................20

3.14 G34/ G35 Rough Milling of the Rectangle–concave Groove.....................................................20

3.15 G36/ G37 Fine Milling Within the Rectangle-concave Groove..................................................21

3.16 G38/ G39 Finish Milling Outside of the Rectangle......................................................................22

3.17 Summary to G Function of Fixed Cycle.......................................................................................22

3.18 G73 High Speed Drilling Cycle......................................................................................................24

3.19 G74 Tapping Cycle with Left-hand................................................................................................24

3.20 G81 Drilling Cycle............................................................................................................................25

3.21 G82 Drilling Cycle............................................................................................................................25

3.22 G83 Deep Hole Drilling (Perki ng)Cycle........................................................................................26

3.23 G84 Right-hand Tapping cycle......................................................................................................26

3.24 G85 Boring Cycle............................................................................................................................27

3.25 G86 Boring Cycle (drilling along head)........................................................................................27

3.26 G89 Boring Cycle............................................................................................................................28

3.27 G92 Floating Coordinate System Setting....................................................................................28

4 Parameter Programming..........................................................................................................................29

Operation

5 Introduction................................................................................................................................................31

5.1 Control Panel and Function buttons..............................................................................................31

5.2 Adjusting of LCD Brightness...........................................................................................................32

5.3 Indicators and Function Keys .........................................................................................................32

5.4 Operation Mode and Incremental Input..................................................................................... .....35

5.5 Resetting Power On..........................................................................................................................35

5.6 Operation of Menu.............................................................................................................................35

5.7 Main Menu for the Sy stem...............................................................................................................36

6 Parameter Setting......................................................................................................................................37

6.1 Description of Parameter.................................................................................................................37

7 Manual Mode..............................................................................................................................................43

7.1 Manual Operation..............................................................................................................................43

7.2 Display (Disp).....................................................................................................................................45

７.3 Zero Return Function (ZERO)........................................................................................................46

7.4 Command Function (COMM)...........................................................................................................47

8 Auto Mode..................................................................................................................................................49

8.1 Auto Operation..................................................................................................................................49

8.2 Display Function (Disp)....................................................................................................................51

8.3 Command Function (Comm)...........................................................................................................51

8.4 Run to Current Block in Dry Run and Positioning Run...............................................................53

8.5 Escape from Auto Mode (end).........................................................................................................54

8.6 Executing a Part Program.................................................................................................

8.7 Execution Order in Auto Mode........................................................................................................55

8.8 Run Times of Part Program.............................................................................................................55

8.9 DNC Operation...................................................................................................................................56

8.10 Power Down Protection..................................................................................................................56

...............54

9 Dry Run Mode............................................................................................................................................57

10 Edit Mode..................................................................................................................................................58

10.1 Full Screen Edit (1-EDIT)................................................................................................................58

10.2 List of Program (2-LIST).................................................................................................................60

10.3 Program Copy (3-COPY)................................................................................................................61

10.4 Part Program Memory Area Lock (4-LOCK)................................................................................61

10.5 Part Program Memory Area Unlock (5-UN LOCK).......................................................................61

10.6 Deleting a Program (6-DEL)...........................................................................................................62

10.7 Initialization of Part Program Memory Area (7-P INIT)...............................................................62

11 Communication Mode............................................................................................................................63

12 Notes and Procedure of Operation.......................................................................................................66

Connection

13 Interface Overview ..................................................................................................................................67

13.1 Interface Layout...............................................................................................................................67

13.2 Total Frame......................................................................................................................................67

13.3 Total Connection Graph...................................................................................................................68

14 Interface function....................................................................................................................................68

14.1 Interface Specification....................................................................................................................68

14.2 Interface Pin list and Interface Method.........................................................................................68

15 Interface connection...............................................................................................................................71

15.1 Connecting with PC.............................................................................................................................71

15.2 Connecting GSK928MA CNC System and Feed Drive Device......................................................71

15.3 Connecting GSK928MA CNC system and Toolpost..................................................................77

15.4 Connecting GSK928MA CNC System and Manual Pulse Generator(MPG)............................78

15.5 Connecting with spindle Encoder.................................................................................................79

15.6 CNC system Switching Value Input..............................................................................................79

15.7 Switching Value Output of the CNC System...............................................................................81

Appendix A: Introduction for GSK928MA...............................................................................................83

Appendix B: System Parameter List........................................................................................................85

Appendix C: M Function Word List..........................................................................................................87

Appendix D: G Function Word List..........................................................................................................89

Appendix E: Error Word List and Tr oubleshooting...............................................................................91

GSK928MA Machine Zero Return Mode..............................................................................................

GSK928MA Interface Circuit Diagram 1.......................................................................................................95

GSK928MA Interface Circuit Diagram 2.......................................................................................................96

GSK928MA Integrated System External Circuit Diagram..........................................................................97

GSK928MA Toolpost Controller Circuit Diagram.......................................................................................98

GSK928MA Contour Installation Dimension Diagram...............................................................................99

GSK928MA-L Contour Installation Dimension Diagram..........................................................................100

........94

GSK928MA CNC SYSTEM OPERATION MANUAL

Programming

1 Introduction

1.1 Axis Definition

This is the CNC system with three or four coordinates for the milling machine and drill machine etc. A rectangular coordinate system combined of X axis, Z axis, Y axis and C（or A）axis is used to execute the positioning and interpolation operation in this CNC system. X axis is denoted to left and right direction and Y axis to clockwise and counterclockwise direction for milling machine in the horizontal plane, Z axis is denoted to vertical one for worktable（or milling cutter）and C (A) axis is an additional one(the 4 Whether A or C is used as the 4th axis in programming axis is confirmed by the C bit of No.10 system parameter No.10. A positive direction is defined to the tool moving away from the workpiece; otherwise it is negative direction as follows:

axis).

刀具

工件

机床

1.2 Machine zero

Machine zero is a fixed point close to the proximity switch on a machine tool. Usually the reference point is set at the maximum stroke of X, Y, Z axis in the positive direction. Do not use its function, supported by the system without installing the machine zero. There must be a machine zero deceleration switch before machine zero. It is unavailable for the 4th axis to use the machine zero function

1.3 Reference point

The position used for executing part programs is defined to reference point), namely, the starting point of tool or the origin point of machining [instead of (0, 0) of coordinate system].

1.4 Coordinate System

In this system, a program is programmed based on the workpiece coordinate system (that’s to say the workpiece coordinate system is equal to the programming coordinate system), it is suggested that the user should position the X , Y, Z axis’s zero with G0 instruction at the first block in the program. It can also define a floating coordinate system by instruction G92 in the program, and for

the convenience of programming, G92 can be used repeatedly in the program. The system will remember the position of machine zero and reference point. After executing the instruction G27 (return to the machine zero and test the step out), G28 (return to the reference point through the specified point), M02, M30, M31, the system will be changed from the floating coordinate system to the workpiece coordinate system. Parameter from No.61 to No.84 is the position of G54 toG59 coordinate system in the reference workpiece coordinate system, which can be modified to change the position of No.1 to No.6 workpiece coordinate system in the reference workpiece coordinate system. And the coordinate of current coordinate system can also be set in Manual mode. If the current coordinate system is not the reference workpiece coordinate system, the corresponding code of current coordinate system will be displayed at the bottom of the screen in the Manual or Auto mode: G92/G54/…/G59. In “Manual mode”, the current coordinate system can be switched “instruction” operation, and the workpiece coordinate system can also be selected by G54～G59 instruction in program. After execution of G27/G28/M02/M30 instruction or machine zero return, the system will be switched to reference workpiece coordinate system. When the workpiece coordinate system is selected by G54～G59 instruction in part program, the instructions can be in the same program block with interpolation and rapid positioning G instruction , and it will be executed firstly.

GSK928MA CNC SYSTEM OPERATION MANUAL

1.5 Programming Coordinates

We can program with absolute coordinates (G90) and relative (incremental) coordinates (G91), incremental coordinates are contrast to the current position’s coordinate.

1.6 Input Unit and Range of Coordinate

Rectangle coordinate is used in the system. The least input unit of the coordinate value is 0.01mm. The maximum instruction value is ±99999.99.

Axis name

X axis 0.01mm 0.01mm Z axis 0.01mm 0.01mm Y axis 0.01mm 0.01mm

A(C) axis 0.01mm Actual move depending on the design of machine

1.7 Program Configuration

The part program consists of a number of program blocks. Each block specifies the S function of the spindle speed, tool function (H for tool length compensation, D for tool corner radius compensation), miscellaneous function (M function) and preparation function (G function) for rapid positioning and cutting feed. And each block consists of a number of words; the word begins with an English character followed by a value. The block begins with word N (block number), followed by other words, and ends with Enter key.

Each block must consist of a sequence number for indicating the CNC operation sequence at the

Least input unit

Least output unit

beginning of the block and a <Enter> code for indicating the end of the block. A Letter N followed by a numerical value specifies the sequence number.

For example: N10 G0 X50 Y100 Z20 ↙ Block No.10, rapid positioning N20 G91 G0 X-30 Z-10 ↙ Block No.20, relative programming, rapid positioning N30 G1 Z-50 F40 ↙ Block No.30, linear interpolation (linear cutting) N40 G17 G2 X-10 Y-5 R10 ↙ Block No.40, circular interpolation N50 G0 Y60 Z60 ↙ Block No.50, rapid positioning N60 G28 X0 M2 ↙ Block No.60, return to starting point, program ending

For the above, N30,G1,Z-50,F40 etc. are called for words, the beginning character of word stands for significance of word, and the following digits are the word value. For the expression of value range, here N4 represents that the word value range is 4-bit integer(0～9999). And the range for X±5.2 is from -99999.99 to +99999.99. (i.e. maximum 5 integral bit and maximum 2 decimal bit, + and- sign is allowable)

The configuration of one block of program in this system is designated as follows: / N5 X±5.2 Y±5.2 Z±5.2 A±5.2 C±5.2 I±5.2 J±5.2 K±5.2 U5.2 V5.2 W5.2 P5 Q5.2 R±5.2 D1 H1 L5 F5.2 S2 T1 M2

/ Optional block skip code. When a slash is specified at the beginning of a block, this block

is an optional block. When the optional block skip indicator on the operation panel is light, the information in the block with a slash heading will be ignored in Auto mode, and One touch of the <skip> key can switch off the optional skip function.

N Block sequence number ranged from 0 to 65535; it is a default, and it must be the first

sign of the block if it contains N. (It can be omitted in DNC.)

Preparatory function, several G instructions for defining states and one G instruction for

acting can be specified in the same block X ,Y,Z ,A,C

I,J,K The position K of the center of circle, which is relative to the starting point in circular

P Dwell time; Parameter number; Program number;

Coordinate value ranging from –99999.99 to 99999.99 in each axis;

Absolute(G90) or relative(G91) value;

Whether A or C is available in programming to the forth axis is confirmed by the C bit of

No.10 parameter.

interpolation.

K is denoted to the spindle speed in tapping.

GSK928MA CNC SYSTEM OPERATION MANUAL

R Arc radius, the reference plane(R plane) in the fixed cycle

D The number for tools(0～9);used for the tool radius compensation; L H F Cutting feedrate, the unit is mm/min or mm/r;

S Spindle speed; T The function of tool change;

Repetition count ranges from 0∼65535;The number of holes to be drilled;

The number for length of tools(0～9);used for the tool length compensation;

M Auxiliary function for the starting and stop of spindle ,water pump and the inputting and

outputting by user;

↙

Free format is used for program block. Except the requirement of the beginning with “/”, “N”, other word (a letter following by a numerical value) may be put in any sequence. And the block ends with the ENTER sign.

1.8 Tool Path of Rapid Positioning

The sequence of rapid positioning is as follows: It’s Z axis, X axis, Y axis, the 4th axis in turn when the direction of Z axis is positive. It’s X axis, Y axis, the 4th axis, Z axis in turn when the direction of Z axis is negative. It’s X axis, Y axis, the 4th axis in turn when there is no positioning in Z axis.

1.9 Offset of System Coordinate

The offset of the system coordinate (coordinate offset in X, Y, Z, C axis direction) can be set by parameter No. 55, 56, 57, and 58 respectively, which can be redound to adjust the machining remainder conveniently, without modifying the program.

nter code, End of block code;

GSK928MA CNC SYSTEM OPERATION MANUAL

1.10 Initial and Modal of System

Initial status is defined that t the programming status before the program runs. It is the default status of the system when power-on. The modal is defined that the corresponding word is valid after the instruction is specified until another block is specified. Another meaning for the modal: the word does not be input again in the following block for the same function after it is set.

1.11 Initial Status of System

The initial status of this system after power on is listed as follows:

Item Status Description Programming mode G90 Programming with the absolute coordinate G17 Selecting X-Y plane for circular interpolation G40 Canceling tool radius compensation G49 Canceling tool length compensation

Using reference coordinate system

Item Status Description G80 Modal data in non-fixed cycle G94 Speed state in feed per minute G98 Return starting point in fixed cycle

Modal G code G0 Rapid positioning

Rapid traverse rate Depending on parameter No.1 (G0 SPD) Cutting feedrate Depending on parameter No.2 (G1 F)

Current status: Item Description Work coordinate value Spindle Current status

1.12 Start of Program

At the beginning of program executing, the tool nose tool should be at the position in which the tool be changed. It is suggested that G00 X_ Y_Z_ should be programmed in the first block of the program to position the tool to the starting point in absolute coordinate; otherwise the program will not run normally.

1.13 End of Program

Usually, M2, M30, or M31 is specified in the last block of the program to end the executing of the program; M2: Indicating the end of the program and stopping the spindle, turning off the coolant pump. M30: End of program. M31: End program and restart the program; Before executing these instructions, make sure the tool back to the starting point of the workpiece coordinate system with the execution of G28 instruction. After the execution of the program, the system will return to workpiece coordinate system with the cancellation of tool offset.

GSK928MA CNC SYSTEM OPERATION MANUAL

Current coordinate, the tool position after the latest Auto operation or Manual operation.

1.14 Main Program and Subprogram

Subprogram comprised by a number of program blocks is contained in the main program is

identified by the sequence number of the first block of it. At the last block of the subprogram, M99 must be specified. Subprogram is generally arranged after M2 or M30 of the main program. The subprogram can be called by M98 instruction.

Three-embedded subprogram call at most can be executed using M98 instruction in this CNC

system.

For example: subprogram call using M98 instruction

N40 P1000 L10 M98 ↙ 10 times the subprogram No.1000 is to be repeated. … … N1000 G1 X-6 ↙ beginning of subprogram N1010 X-30 Z-30 ↙ N1020 Z-20 ↙ N1030 X-10 Z-30 ↙ N1040 G0 X45 Z80 M99 ↙ end of subprogram

1.15 Backlash Compensation

The backlash compensation value is stored as system parameter in the system parameter memory area, Parameter No. 11, 12,13,14 are used for X ,Y, Z and the 4th axis backlash compensation respectively. If the compensation value of each axis is set to 0.00, it means no compensation, if it is set other than 0.00 in this case, the backlash compensation will be given automatically by the CNC system (circular interpolation can backlash compensate automatically if the circular interpolation automatically exceeds the quadrant).

1.16 R Reference Plane

R reference plane is laid high from some height of X-Y plane. It ‘s higher than the workpiece but not too high, which can be redound to lift the cutting tool in Z direction and rapid traverse in X,Y direction at R reference plane while fixed cycle processing is in progress machining (drilling or groove rough milling). It can be defined by program using R word.

GSK928MA CNC SYSTEM OPERATION MANUAL

2 S, T, M Function, D, H, F, FEED%

2.1 S Function

S function is namely the S word in a block used for specifying the spindle speed. When using 4-bit switching value encoder output to specify the spindle speed: Set No. 54 to be of 4-bit switching value encoder output corresponding to 0.00, S0～S15 to control the spindle speed. At the same time, S0～S255 corresponds to output 0～10V analog voltage. When using analog signals (0～10V) to specify the spindle speed: S function can be used directly to specify the spindle speed (rev per minute) by setting No. 54, No.59 (the spindle speed when outputting 5V voltage signal) and S function is directly used for the

spindle speed. Please read the chapter: Parameter Setting.

2. 2 T Function

T function is used for the control of tool change on the toolpost, in which the tool number is expressed by a digit from 0～8(The current tool can be directly used as No.0 tool without rotating

the toolpost). It is relative to the No.98 parameter of the CNC system：

When the No.98 parameter is less than or equal to 0.00, it means that the automatic toolpost for tool change is not fixed on the machine and the T function can be executed in Manual mode, but the locking time of the toolpost reverse rotation is very short, and the T word will not be shown without the execution of T function in the operation interface of Auto, Manual, Dry run mode etc.. While the Auto mode is running to the T function word, the system will pause, and the manual tool change can be performed by operator. Press <RUN> key to go on program execution after the tool change is done. When the No.98 parameter is more than 0.00, it means that the automatic toolpost for tool change has been fixed on the machine and the No.98 parameter represents the locking time (usually 1s) of toolpost reverse rotation. If the tool number expressed by digits is not the current tool when T function is being executed, the toolpost will be rotated to the required tool by the system instructions.

2.3 M Function (Auxiliary Function)

M0 — Program ends. After executing other instructions of the block, stop the spindle, and cut off

the coolant, point to the next block without the further running, waiting for pressing the RUN key to go on running the block.

M2 — End of program. Stop the spindle, switch off the coolant, and cancel the coordinate offset

specified by G92 and the tool offset to return to the initial block. After executing M2

instruction, the system will be switched to the reference workpiece coordinate system. M3 — Spindle clockwise rotation; M4 — Spindle counterclockwise rotation; M5 — Spindle stop;

M6 — Invalid compatible function; M8 — Coolant On;

M9 — Coolant Off;

M12 — Pause: waiting for pressing <RUN> key. (pressing <emergency> key to stop running). M20 —Setting the outputting of user 1 to 1; M21 —Setting the outputting of user 1 to 0; M22 —Setting the outputting of user 2 to 1;

M23 —Setting the outputting of user 2 to 0;

M24 —Setting the outputting of user 3 to 1;

M25 —Setting the outputting of user 3 to 0; M27 — The system coordinate to be zero, and cancel the machine zero return. M28 — Reset

the coordinate value of the 4th axis (A or C axis) .

M30 — End of program and cancellation of tool offset and return to the start block of the program

(without running). After a block containing M30 is executed, the CNC system will be switched to the reference workpiece coordinate system

M31 — End of program, processing cycle. Cancel the tool offset and return to the initial program.

After executing M31, the system is switched to the reference workpiece coordinate system.

M32 — Lubrication On; M33 — Lubrication Off; M60 —When the output of user 1 is 1, the system waits; when the output of user 1 is 0, the system

executes the other blocks in the same block or the next block.

M61 — When the output of user 1 is 0, the system waits; when the output of user 1 is 1, the system

executes the other blocks in the same block or the next block. M60/M61 may be in the same block with G function and be executed firstly which can improve the process execution speed instead of G90/G91 instruction.

M90 — The program skips to the block specified by D when the output of user 1 is 0.

GSK928MA CNC SYSTEM OPERATION MANUAL

Format : N_ M90 P_

P is the skipping block number (If the input is 1, executing the next block by sequence number)

M91 — The program skips to the block specified by D when the output of user 1 is 1.

Format: N_ M90 P_

P is the skipping block number (If the input is 0, executing the next block by sequence number)

M92 — Unconditional skip to the block specified by D,

Format: N_ M90 P_

P is the skipping block number

M93 —Skipping when output of user 2 is 0.

Format: N_ M90 P_

P is the skipping block number (If the input is 1, execute the next block in order)

M94 —Skipping when output of user 2 is 1.

Format: N_ M90 P_ P is the skipping block number (If the input is 0, execute the next block in order)

M98 — Calling of subprogram

Format: N_ D_ L_ M98 P is the start block number of subprogram, L is calling times (omission for once), and three-loop subprogram call at most can be executed using M98 instruction.

M99 — End and return of subprogram.

Note: 1) M0, M2, M30, M31, M99 after G function is executed;

2) M90, M91, M92, M93, M94, M98 is the single format (other G function can't be with G90, G91 function at a time)

3) Other M function which is in the same block with other functions will be executed first (i.e. It will be executed before G function).

GSK928MA CNC SYSTEM OPERATION MANUAL

2.4 D, H Function

D — Cutting tool radius number (0～9) which is used for tool radius compensation. The tool

radius value of D1-D9 can be set by parameter 15-23 respectively.

H — Cutting tool length number (0～9) which is used for and being used in tool length

compensation. The tool length value of H1-H9 can be set by parameter 24-32 respectively. The tool radius number can be specified by D word (D1-D9, D0 means tool radius value is 0) in program. The function of tool radius compensation is fit in V3.0 version software and above of the system. And all software versions are used for the tool radius compensation of circle groove and rectangle groove processing cycle. The tool length number can be specified by H word (H1-H9, H0 means tool length value is 0) in program and does tool length compensation with G43 or G44.

2.5 F, Feed%

F word can be used freely in the block for specifying cutting feedrate. F is effective till the new value of F is set (The rapid traverse speed and the initial cutting feedrate can also be set by Parameter NO.1 and No.2). F: 0.01～3000.00 mm/min

FEED％ is used as feedrate override, range: 0％,10％,20％,......, 150％, which can be adjusted

by pressing <↑Feed％> key and <↓Feed％>key. The feedrate override can be adjusted in running.

GSK928MA CNC SYSTEM OPERATION MANUAL

3 G Function (Preparatory Function)

3.1 G Function for Defining Programming State of the System

Programming state of system is specified by these G functions as follows. They are modal which means they are valid unless the programming state is changed. The initial is the programming state that the part program is to be executed. The following G can be used in one program block with other G functions and at most 6 G functions can be used in the same block. G17 — Initial state, select X-Y plane for circular interpolation G18 — Select Z-X plane for circular interpolation G19 — Select Y-Z plane for circular interpolation G40 — Initial state, cancel tool radius compensation G43 — Tool length compensation + G44 — Tool length compensation – G49 — Initial state, cancel tool length compensation G54 — Initial state, select the 1 G55 — Initial state, select the 2 G56 — Initial state, select the 3 G57 — Initial state, select the 4 G58 — Initial state, select the 5 G59 — Initial state, select the 6 G80 — Initial state, cancel the modal data of fixed cycle (use G98 instruction simultaneously) G90— Initial state, do programming with absolute coordinate. X, Y, Z word values mean the

absolute coordinate values.

G91— programming with incremental coordinate. X, Y, Z word values mean the incremental

coordinate values (the increment relative to the starting point of the current block).

G94— Initial state, set the feedrate per minute. The unit of cutting feedrate set by F word is

mm/min, i.e. the millimetres of feeding per minute

G95 — Set the feedrate per rev. The unit of cutting feedrate set by F word is mm/r, i.e. the

millimetres of feeding per rev of spindle. The spindle pulse encoder (1200 pulses per rev)

must be fixed firstly before using G95 function. G98 — Initial state, return to the start plane in fixed cycle. G99 — Return to the R reference plane in fixed cycle. G09，G60，G61，G64 ：Invalid compatible function.

workpiece coordinate system

3. 2 G0 Rapid Positioning (Modal, Initial)

Format : N_ G0 X _Y_ Z _ C_( or A_)↙ X, Y,Z, C(or A) is the coordinate absolute value (G91) or relative value(G90) of end point to be positioned in work coordinate system. The needless axis can be omitted. The rapid traverse speed is specified by parameter No.1 and can be modified by pressing parameter key. The sequence of positioning is as follows: Position Z, X, Y, 4

axis in turn when Z axis is positive (the cutter rising off the workpiece).

It’s the X, Y, the 4th, Z axis in turn when the Z axis is negative. Whether A or C is valid in programming to the 4

GSK928MA CNC SYSTEM OPERATION MANUAL

axis is specified by C bit of parameter NO.10.

3. 3 G1 Linear Interpolation (Modal)

Format : N_ G1 X _Y_ Z _ C_( or A_) ↙ X, Y, Z is the end point coordinate absolute value or relative value to be interpolated in work coordinate system. The axis that has no movement can be omitted. F is feedrate, if it is omitted, the last feedrate F which has been executed will be used. The feedrate of initial state (initial modal data) can be specified by system parameter No.2. Whether A or C is valid in programming to the 4th axis is specified by C bit of system parameter NO.10.

3.4 G2, G3 Circular Interpolation (Modal)

Format : G17 G2 X_ Y_ ↙

N_ G18 Z_ X_ R_ F_ ↙

G19 G3 Y_ Z_ ↙

Or: G17 G2 X_ Y_ I_ J_↙ N_ G18 Z_ X_ I_ K_ F_ ↙ G19 G3 Y_ Z_ J_ K_↙

The first type of format is that the programming is done by arc radius R; the second type of format is that the programming is done by the position that the circle center relative to the starting point (current position):

G2: Clockwise direction (CW) G3: Counterclockwise direction (CCW), see diagram X,Y, Z: The end point coordinate value (absolute coordinate value

for G90, incremental coordinate value for G91) of arc in work coordinate system, can be omitted for the axis with no

moving I: Distance with X-direction from starting point to center point. J: Distance with Y-direction from starting point to center point. K: Distance with Z-direction from starting point to center point. R: Radius of arc. If R>0, the arc is less than or equal to 180° is

commanded;

Else, if R<0, the arc is more than or equal to 180°

G17,G18,G19

F: Feedrate along the arc, which can be omitted In circular

Select X-Y plane, Y-Z plane, Z-X plane respectively.

interpolation, the tool is feeding by cutting speed. In circular

interpolation, the tool is automatically cross quadrant with

the backlash compensation.

G17 — X-Y plane G18 — Z-X plane G19 — Y-Z plane

GSK928MA CNC SYSTEM OPERATION MANUAL

3. 5 G4 Dwell

Format: N_ G4 P_ ↙ or N_ G4 X_ ↙ The unit of P is 1%s, and X is s: e.g. P250 is 2.5s, X1.5 is 1.5s.

3. 6 G10 G11 Rough Milling in Concave Groove of Inner Circular

Format: G10—CCW rough milling inner circle: G10

N_ R_ Z_ I_ W_ Q_ K_ V_ D_ F_ ↙M02 G11— CW rough milling inner circle: G11

N_ R_ Z_ I_ W_ Q_ K_ V_ D_ F_ ↙M02

R The position of R reference plane. It is absolute coordinate value in Z direction in G90 and

relative plane far from the starting point in Z direction of current block in G91, which is easy to position in X-Y direction on R plane rapidly and lift tool in Z direction.

Z The height of concave groove. It is absolute coordinate value in G90 and position relative to

R plane in G91. I The radius of concave groove. It must longer than the radius of the current tool. W Q The increment in each cutting in Z direction. Q>0 K The width increment in cutting. It’s usually shorter than the diameter of tool. K>0. V The distance far from the last machining plane in fast cutting. W>V>0. D The number of tool radius (1-9), which can be specified by parameter No.15 to 23. D0 means

R, Z, W, V and Q are modal data in fixed cycle. The process of rough milling inner circle for concave groove is as follows: (1) Move the tool to R reference plane in Z direction rapidly. (2) Cut the height of W downward (cutting speed). (3) Mill an I-radius circle helically with the increment of K every time (compensation for the radius

(4) Return to R reference plane rapidly in Z direction. (5) Orient to the center of the circle in X-Y direction rapidly.

The first cutting height.（blow R reference plane）W>0.

tool radius value is 0.

of tool is specified automatically by system).

(6) Orient to the plane V from the last machining plane in Z direction rapidly. (7) Cut the height of (Q+V) downward in Z direction. (8) Repeat above procedure No. (3) to (7) to finish cutting the total height. (9) Return to the starting point in Z direction (G98) or R reference plane (G99). "r" in following graph is the radius of tool relative to D (compensation for the radius of tool is specified automatically by system).

GSK928MA CNC SYSTEM OPERATION MANUAL

3. 7 G12 /G13 Finish Milling of Inner Circle

Format: G12—CCW fine mill inner circle. G12 N_ I_ J_ D_ F_ ↙ G13—CW fine mill inner circle. G13

I The radius of the circle J The distance between the starting point and the center of the circle D The tool radius number (1-9), which can be specified by parameter No.15 to 23. D0 means

the radius value is 0.

The end point of the tool:

G12:1→2→3→4→5→6 G13:6→5→4→3→2→1

The letter r in following graph is the radius of tool relative to D (compensation for the radius of tool is specified automatically by system).

GSK928MA CNC SYSTEM OPERATION MANUAL

3. 8 G14 /G15 Fine Milling of Outer Circle

Format:

G14—CCW fine milling of outer circle. G14

N_ I_ J_ D_ F_ ↙

G15—CW fine mill of outer circle G15

I The radius of the circle J The distance between the starting point and the center of the circle D The tool radius number (1-9), which can be specified by parameter No.15 to 23. D0

means the radius value is 0.

The path of the tool:

G14:1→2→3→4 G15:4→3→2→1

The letter r in following graph is the radius of tool relative to D (The compensation for the radius of tool is specified automatically by system).

3. 9 G22 System Parameter Setting (Modal)

Format: N_ G22 P_ L_ X_ Y_ Z_ ↙ P=1～99 : System parameter number, refer to chapter of system parameter setting for details. X, Y, Z: The data used to calculate

L=0～19 : Calculation factors as follows: L=0: Set the system parameter No.P =0”. L=1: Set system parameter No.P =X; L=2: Set system parameter No.P=-X. L=3: Set system Parameter No.P= Abs (X); (the absolute value of X) L=4: Set system parameter No.P＝original value + X L=5: Set system parameter No.P＝original value - X L=6: Set system parameter No.P ＝X+Y

L=7: Set system parameter No.P ＝X-Y L=8: Set system parameter No.P ＝-X+Y L=9: Set system parameter No.P ＝-X-Y L=10: Set system parameter No.P ＝2X L=11: Set system parameter No.P ＝X/2 L=12: Set system Parameter No. P＝X * (The value of lower byte of Y); The value of lower

byte: 0.00—0.25

L=13: Set system parameter No.P ＝X / (The value of lower byte of Y); The value of lower

byte: 0.00—0.25 L=14: Set system parameter No.P ＝X*Y/Z L=15: Set system parameter No. P＝Root(X*Y) L=16: Set system parameter No. P＝Root(X**2+Y**2) L=17: Set system parameter No. P＝Root(X**2-Y**2)

L=18: Set system parameter No. P＝max (X,Y)

L=19: Set system parameter No. P＝min (X,Y) L=20: Set system parameter No. P＝mod(X,Y)

The data which range are integers from -2147483648 to 2147483648 are stored by 4 bytes in the system. While calculating by parameters, be sure to use the effective data. It is 1 for the system while 0.01 is displayed. Notice: The calculation is done all by integers in the system, and 0.01 corresponds to 1 of the internal integers which range from -999999999 to 999999999.

GSK928MA CNC SYSTEM OPERATION MANUAL

3.10 G23 Conditional Jump

Format: N_ G23 P_ X_ Y_ Z_ L_ ↙

P: System parameter number 1～99; L: Sequence number of the block jump to(range: 0～65535);

X, Y, Z: Conditional value (there should be at least one conditional value to be specified in the

block):

If one of the conditions below is satisfied, control will jump to the block with sequence number

specified by L, else, control executes the next block sequentially.

If X is specified and the value of parameter = X, jump to No. L block; If Y is specified and the value of parameter >Y, jump to No. L block;

If Z is specified and the value of parameter <Z, jump to No. L block;

3.11 G27 Machine Zero Inspection

Format: N_ G27↙ The tool offset will be cancelled and system will return to workpiece coordinate system in G27. The system will be positioned to the machine zero and the stepout will be inspectioned by system. Before executing G27 instruction, make sure that the tool is in the negative direction of the reference point deceleration signal. If machine zero hasn’t been built by machine tool builder or the machine zero return operation has never been executed, alarm E45 will be displayed. If any step has been detected lost after the system executes the machine zero return, alarm E41/E42 /E43 will

be displayed. When Bit E41 of Parameter No.10 is 0 and stepout is detected, alarm E41/E42/E43 will be displayed. When Bit E41 of parameter No.10 is 1 and only the deviation is larger than

0.02mm, alarm E41/E42/E43 will be displayed. The system does not detect the stepout when G27, M28 instructions are in the same block, i.e. alarm E41/E42 /E43 will not be displayed. After the execution of G27/G28/M02/M30 instruction or machine zero return and reference point return operation, the system will be switched to the reference workpiece coordinate system.

GSK928MA CNC SYSTEM OPERATION MANUAL

3.12 G28 Rapid Traverse to Reference Point via Middle Point

Format: N_ G28 X_ Y_ Z_ A_(or C_)↙ This instruction is used to position the tool to the middle point, and then to traverse to the reference point at rapid traverse speed. The tool offset compensations is cancelled after reference point return. After the execution of G27/G28/M02/M30 instruction or machine zero return and reference point return operation, the system will be switched to the reference workpiece coordinate system.

3.13 G31 Rapid Return to the R Reference Plane

Format: N_G31 ↙ Return to the R reference plane in Z direction rapidly.

3.14 G34/ G35 Rough Milling of the Rectangle–concave Groove

Format: G34 —CCW milling G34

N_ R_ Z_ I_ J_ K_ W_ Q_ V_ U_ D_F_ ↙

G35—CW milling G35

R The position of R reference plane. It’s the absolute value in G90 and the position relative to

the starting point of the current block in G91.

Z The height of groove. It’s the absolute value in G90 and the position relative to the R

reference plane. W The cutting height in first milling, W>0. Q The incremental height in each cutting, Q>0. V The distance from the last machining plane when moving the tool rapidly, V>0. K The incremental width in each cutting and usually shorter than the radius of the tool, K>0. I The width of the rectangle-concave groove in X direction, I>0. J The width of the rectangle-concave groove in Z direction, J>0. U The corner radius of the rectangle-concave groove, U≥0. D The tool radius number (1-9), which can be specified by parameter No.15 to 23. D0

means the radius value is 0. R, Z, W, V, Q is the modal data in the fixed cycle.

The process is as follows (the rectangle center is the starting point): (1) Moving down to the R reference plane in Z direction.

(2) Cutting the height W at cutting feedrate. (3) Milling the rectangular plane with the increment K from center to outside. (The compensation

for the radius of tool is specified by system automatically.) (4) Return to the R reference plane rapidly in Z direction. (5) Orienting to the center of the rectangle rapidly in X-Y direction. (6) Moving down in Z direction and orienting to the position with the distance V from the last

machining plane. (7) Cutting the length (Q+V) down in Z direction. (8) Repeating the above procedure No. (3) to (7) to finish machining the rectangular plane for the

total cutting height. (9) Rapid return to the starting point in Z direction (G98) or to the R reference plane (G99). In following graph r is the radius of tool relative to D (The compensation for the radius of tool is specified automatically by the system).

GSK928MA CNC SYSTEM OPERATION MANUAL

3.15 G36/ G37 Fine Milling Within the Rectangle-concave Groove

Format: G36—CCW milling G36 N_ I_ J_ D_ K_ U_ F_ ↙

G37—CW milling G37

I, J The width of the rectangle along X and Y axis respectively K The distance between the starting point of program and the rectangle side in X direction. U The chamfer radius. There is no chamfer when U is omitted. D The tool radius number (1-9), which can be specified by parameter No.15 to 23. D0

means the radius value is 0.

The cycle process: G36:1→2→3→4 G37:4→3→2→1

The letter r in following graph is the radius of tool relative to D (The compensation for the radius of tool is specified automatically by the system).

GSK928MA CNC SYSTEM OPERATION MANUAL

3.16 G38/ G39 Finish Milling Outside of the Rectangle

Format :G38—CCW milling G38

N_ I_ J_ K_ U_ D_ F_ ↙

G39—CW milling G39

I,J The width of the rectangle along X and Y axis respectively K The distance between the starting point of program and the rectangle side. U The chamfer radius. D The tool radius number (1-9), which can be specified by parameter No.15 to

23. D0 means the radius value is 0.

The tool path:

G38:1→2→3→4 G39:4→3→2→1

The letter r in following graph is the radius of tool relative to D (The compensation for the radius of tool is specified automatically by system).

3.17 Summary to G Function of Fixed Cycle

Circular concave groove rough milling cycle, rectangular concave groove rough milling cycle,

drilling cycle, boring cycle and taping cycle can be realized by G function of fixed which is comprised of G10,G11,G34,G35,G73～G89. The usual process is as follows:

(1) Orienting to the hole rapidly in X-Y plane (This function is not involved within G10, G11,

G34, and G35).

(2) Moving down to the R reference plane rapidly in Z direction (The R reference plane is

between the starting point and the X-Y plane of workpiece and close to the workpiece

cycle,

plane). (3) Milling the first height in Z direction. (4) Milling the height with the increment every time in Z direction. (5) Operation in hole bottom or plane. (6) Return to the R reference plane or to the starting point (G98) alongZ axis. (7) Circulate from (1) to (6) to perform drilling of the holes on the line if L word is in the

program (This function is not involved within G10, G11, G34, G35).

The usual format is as follows:

G98

N_ G_ X_ Y_ R_ Z_ W_ Q_ P_ U_ V_ L_ K_ F_ ↙

G99 X, Y The position of the hole in X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in G90 and the

position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the R reference

plane in G91). W The first cutting depth (calculate it from the R reference plane, W>0). Q The increment of cutting depth in Z direction. P The delay time in the hole bottom(unit: 1/100s) U The distance of lifting the tool during high speed drilling cycle (G73).U>0 V The distance from the last machining plane in high speed drilling cycle(G73) or deep hole

drilling cycle(G83), V>0. L K

F The machining speed. R Z W Q U V word is the modal value in fixed cycle. If they are specified in advance and not changed, they needn’t to be input again in the sequential blocks with the G function of fixed cycle. They can be cancelled by G80 instruction. It can return to the starting point of the block by using G98 instruction in Z direction after the cycle (initial and modal). It can return to the R reference plane in Z direction by using G99 instruction after the cycle (modal). If there is L word in the fixed cycle of G73-G98, L holes will be machined circularly on the line from the current X-Y plane to the end point with X-Y coordinate specified by the block. The distance between each adjacent hole is equal. There is no hole in the current position (the starting point of the block) and the last hole will be located in the end point. The illustration is as follows:

Drilling cycle of holes with the numbers L from the starting point (the starting point of the

block) to the position with the XY coordinate

The spindle speed per minute in G74, G84. It’s used to calculate the speed in

acceleration and deceleration in tapping.

GSK928MA CNC SYSTEM OPERATION MANUAL

End point

终点

Starting point

起点

3.18 G73 High Speed Drilling Cycle

Format: N_ G73 X_ Y_ R_ Z_ W_ Q_ U_ V_ F_ ↙

X,Y The hole position in X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position

in G90 and the position relative to the starting point of the block in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to

the R reference plane in G91). W U V Q The increment of cutting depth in Z direction, Q>0.

R Z W U V Q is the modal data in fixed cycle.

The cycle process is as follows:

(1) Rapid positioning to the X-Y plane. (2) Rapid traverse down to the R reference plane in Z direction.

(3) Cutting a depth equal to W firstly in Z direction. (4) Rapid traverse up a distance U. (5) Rapid traverse a distance (U-V) down. (6) Cutting a depth (Q+V) down.

(7) Repeating the procedure No. (4), (5), (6), till tool feeds to the bottom of the hole in Z

direction.

(8) Rapidly return to the starting point (G98) or the R reference plane (G99).

(9) If there is L word in the block, then repeating the procedure No.(1)-(8) to complete L holes.

The first cutting depth (calculating it from the R reference plane), W>0.

The distance of rapid lifting of cutters, U>0

The distance to the last machining plane in rapid cutting, U>0, U≥V

3.19 G74 Tapping Cycle with Left-hand

Format: Metric I_

N_ G74 X_ Y_ R_ Z_ P_ K_ ↙

Inch J_ X,Y The position of X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in

G90 and the position relative to the starting point in G91).

Z The hole depth (the absolute position in G90 and the position relative to the

R reference plane in G91).

GSK928MA CNC SYSTEM OPERATION MANUAL

I J P Number of initial pulse in tapping (0-1119) (When the machine installed with

K It is the spindle speed per minute, and it is used to calculate the speed in

R and Z are the modal data of the fixed cycle.

A 1200pulses/ rev. spindle encoder should be fixed for tapping. The operation procedure: (1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) Spindle rotating counterclockwise. (4) Tapping to the hole bottom. (5) Stopping the spindle. (6) The spindle rotating clockwise and tapping up to the R reference plane. (7) Stopping the spindle. (8) Rapidly return to the starting point (G98) or the R reference plane (G99). (9) If there is L word I in the block, then repeat the procedure (1)～(8) to complete holes.

For metric thread, tooth: 0.01～12.00(mm). For inch thread, tooth: 2.12～200.00.

a 1200pulses/ rev. encoder).Usually P can be omitted (i.e. P0).

acceleration and deceleration in tapping.

3.20 G81 Drilling Cycle

Format: N_ G81 X_ Y_ R_ Z_ F_ ↙ X,Y The position of X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in G90 and the

position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the R reference

plane in G91).

R and Z are the modal data. The operation procedure: (1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) Drilling down in Z direction. (4) Rapidly return to the starting point (G98) or the R reference plane (G99). (5) If There is L word in the block, then repeating the procedure (1)～(4) to complete L holes.

3.21 G82 Drilling Cycle

Format: N_ G82 X_ Y_ R_ Z_ P_ F_ ↙ X,Y The position of X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in G90 and the

position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the R reference

plane in G91).

R and Z are the modal data of fixed cycle.

The operation procedure: (1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) Drilling down in Z direction and pausing for the time specified by P at the hole bottom.

(4) Rapidly return to the starting point (G98) or the R reference plane (G99). If There is L word in the block, then repeating the procedure (1)～(4) to complete L holes.

GSK928MA CNC SYSTEM OPERATION MANUAL

3.22 G83 Deep Hole Drilling (Perking)Cycle

Format: N_G83 X_ Y_ R_ Z_ W_ Q_ V_ F_ ↙

X,Y The position of the hole in X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in

G90 and the position relative to the starting point of the block in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the

R reference plane in G91). W The first cutting depth (calculated from the R reference plane, W>0). V The distance to the last machining plane during rapidly traversing W>V>0. Q The machining increment in Z direction.

R W V Q are modal data of fixed cycle, Z is the non-modal data. If Z is omitted in the block, the tool will feed for W value, then rapidly move counterclockwise and stop. No alarm occurs in the CNC system.

The operation procedure:

(1) Positioning in X-Y plane.

(2) Rapidly traversing down to the R reference plane.

(3) Cutting a depth W firstly.

(4) Rapidly traversing up back to the R reference plane.

(5) Rapidly traversing down to the position with the distance V from the end machining

plane. (6) Drilling a depth (Q+V) down. (7) Repeating the procedure (4) ～ (6) to reach the hole bottom. (8) Rapidly return to the starting point or the R reference plane. (9) If There is L word in the block, then repeating the procedure (1)～(8) to complete L holes.

3.23 G84 Right-hand Tapping cycle

Format: Metric I_

N_ G84 X_ Y_ R_ Z_ P_ K_↙

Inch J_

X,Y The position of X-Y plane.

R The coordinate value of the R reference plane (It’s the absolute position

in G90 and the position relative to the starting point in G91).

Z The hole depth(the absolute position in G90 and the position relative to

the R reference plane) I J P Number of initial pulse in tapping (0-1119) (when the machine installed

K It is the spindle speed per minute for thread cutting, and is used to

R and Z are the modal data for fixed cycle.

A 1200pulses/ rev. spindle encoder is used in tapping.

The operation procedure:

(1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) The spindle rotating clockwise. (4) Tapping to the hole bottom. (5) Stopping the spindle. (6) The spindle rotating counterclockwise and tapping up to the R reference plane. (7) Stopping the spindle.

(8) Rapidly return to the starting point (G98) or the R reference plane (G99).

If There is L word in the block, then repeating the procedure (1)～(8) to complete L holes.

For metric thread, tooth: 0.01～12.00(mm).

For inch thread, tooth: 0.01～200.00(teeth/inch).

with a 1200pulses/ rev. spindle encoder).Usually P can be omitted (i.e. P0).

calculate the speed in acceleration and deceleration in tapping by the

system.

GSK928MA CNC SYSTEM OPERATION MANUAL

3.24 G85 Boring Cycle

Format: N_G85_ X_ Y_ R_ Z_ F_ ↙

X,Y The position of X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in G90 and the

position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the R reference

plane in G91).

R and Z are the modal data. The operation procedure: (1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) Drilling down in Z direction with the speed specified by F word. (4) Rapidly traversing up to the R plane with the speed specified by F word. (5) If There is L word in the block, then repeating the procedure (1)～(4) to complete L holes. (6) Rapidly return to the starting point in G98.

3.25 G86 Boring Cycle (drilling along head)

Format: N_ G86 X_ Y_ R_ Z_ F_ ↙

X,Y The position of X-Y plane.

R The coordinate value of the R reference plane (It’s the absolute position in G90 and the

position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the R

reference plane in G91). R and Z are the modal data. The operation procedure:

(1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane. (3) Drilling down in Z direction at the speed specified by F.

(4) Stopping the spindle. (5) Rapidly return to the R reference plane (G99) or the starting point (G98).

(6) If There is L word in the block , then repeating the procedure (1)～(5) to complete L holes.

GSK928MA CNC SYSTEM OPERATION MANUAL

3.26 G89 Boring Cycle

Format: N_ G89 X_ Y_ R_ Z_ P_ F_ ↙

X,Y The position of X-Y plane. R The coordinate value of the R reference plane (It’s the absolute position in G90

and the position relative to the starting point in G91).

Z The hole depth(It’s the absolute value in G90 and the position relative to the

starting point in G91). R and Z are the modal data. The operation procedure: (1) Positioning the hole in X-Y plane. (2) Rapidly traversing down to the R reference plane.

(3) Drilling down in Z direction at the speed specified by F and pausing at the hole bottom

for the time specified by P. (4) Rapidly traversing up to the R reference plane at the speed specified by F in Z direction. (5) If There is L word in the block, then repeating the procedure (1)～(4) to complete L

holes.

(6) Rapidly return to the starting point in G98.

3.27 G92 Floating Coordinate System Setting

Format: N_ G92 X_ Y_ Z_ C(or A)_↙ X, Y, Z, and C: the floating coordinate value of current position.

An absolute positioning must be executed at the initial block of part program. For the convenience

of the programming, the floating coordinate system can be freely defined in the program. The system can automatically execute the conversion between reference point and machine zero. Furthermore, the system can automatically return to the workpiece coordinate system after executing G27, G28, M02, M30, M31 or return to the machine zero and reference point.

GSK928MA CNC SYSTEM OPERATION MANUAL

4 Parameter Programming

The parameter programming use the value of the system parameter as the value of certain words in the program block, A changeable parameter value can make the program flexible and versatile by applying the function of parameter programming (parameter can be modified by G22). Combining with the G23 function to skip, some complex cutting cycle and special cycle part programs for user can be achieved. There are a total of 99 parameters available in this system. The number of the parameter is ranged for 1∼99. For the parameter No.1～84,attention should be paid in programming for the influence of the parameter change to the relative function of the system. And parameter No.85∼99 can be used flexible in parameter programming by user. The words X, Y, Z, U, V, W, Q, F, I, J, K, R can be specified in parameter programming. The format of these words in parameter programming is expressed as follows:

Word letter + * + Parameter number.

Note: Only integer can be calculated in system, 0.01 corresponds to the interior integer 1.The

range of parameter value is -999999999 to 999999999. Be cautious to use G22 for preventing it from overflowing.

For example : N200 G0 X*70 Y*71 ↙

The value of the X is the value of parameter No.70; the value of the Y is the value of the parameter No. 71. Example: using parameter programming to achieve the triangle cutting cycle. The coordinate value of the starting point of the cycle in X-Y plane is (200.00, 300.00) and the tool has been positioned to the starting point. The program is as follows: N10 G0 X200 Z300 Z0↙ (Rapidly positioning ) N30 G22 P62 X8 L1 ↙ (Setting parameter No.62 P62＝8.00 : The first cutting

depth in X direction)

N40 G23 P62 Z150 L60 ↙ (judging: whether the total cutting depth in X direction<150.00? ) N50 G22 P62 X150 L1 ↙ ( false, cutting depth P62＝150.00 ) N60 P61 X*62 Y200 Z150 L14 ↙ (Parameter No.61: cutting depth in Y direction P61

L62*200/150)

N90 P60 X*62 L2 ↙ (Parameter No.60 P60＝ - P62 ) N100 P79 X*61 L2 ↙ (Parameter No.79 P79＝ - P61 ) N110 G91 G0 X*60 ↙ (Rapidly moving in X direction) N120 G1 X*62 Y*79 ↙ (Cutting slantwise) N130 G90 G0 Y*61 ↙ (Rapidly traversing to starting point in Y direction) N140 G23 P62 X150 L180 ↙ (If the total cutting depth in X direction =150, cycle ends) N150 G22 P62 X8 L4 ↙ (The cutting depth in X direction ＋ 8.00 ) N160 M92 D40↙ (Skipping to the block No.40, i.e. N40) N180 M2

↙ (Cycle ending: Stopping the spindle, end of program)

＝

+ 73 hidden pages

gsk GSK928MA User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual