gsk GSK980T User Manual

GSK980T

Turning Machine CNC System

User Manual

GSK980T CNC SYSTEM USER MANUAL

Ⅰ

INTRODUCTION······························································································································1

1.1 Introduction································································································································· 1

1.2 Type Signification························································································································ 1

1.3 Type Table ··································································································································· 1

II. Programming ······································································································································2

2.1 General······································································································································ 2

2.1.1 Axes Definition ·················································································································· 2

2.1.2 Reference Point (Machine Zero Point) ··············································································· 2

2.1.3 Coordinate value and direction and dimension··································································· 2

2.1.4 Unit and Range of coordinate····························································································· 3

2.1.5 Initial and Modal Status of the Command ·········································································· 3

2.1.6 The Start of a Program········································································································3

2.1.7 The End of a Program········································································································· 3

2.1.8 Program Configuration······································································································· 3

2.1.9 Program Configuration······································································································· 3

2.2 controlled Axis·························································································································· 5

2.2.1 Number of Controlled Axis ································································································ 5

2.2.2 Unit Setting ························································································································ 5

2.2.3 Maximum Strokes ·············································································································· 5

2.3 Preparatory Function (G Function)···························································································· 6

2.3.1 Positioning(G00) ················································································································ 7

2.3.2 Linear Interpolation (G01)·································································································· 7

2.3.3 Circular Interpolation (G02,G03) ······················································································· 8

2.3.4 Thread Cutting (G32) ······································································································· 11

2.3.5 Return to Reference Point Automatically (G28) ······························································· 14

2.3.6 Dwell(G04) ······················································································································ 14

2.3.7 Work Coordinate System Setting(G0) ··············································································14

2.3.8 Feed per Minute (G98) ····································································································· 15

2.3.9 Feed per Revolution(G99) ································································································ 15

2.3.10 Constant Surface Speed Control(G96, G97)··································································· 17

2.3.11 Canned Cycle(G90, G92 G94)························································································ 20

2.3.12 Multiple Repetitive Cycle (G70~G75) ··········································································· 25

2.3.13 Notes on Multiple Repetitive Cutting Cycle (G70~G75)················································ 34

2.4 Spindle Function(S Function)·································································································· 34

2.4.1 Spindle Speed Command·································································································· 34

2.5 Tool Function·························································································································· 35

2.5.1 Procedures of tool Change································································································ 35

2.5.2 Tool selection (Change) Related Parameters ···································································· 36

2.6 Auxiliary Function(M function) ······························································································ 36

2.6.1 Description of M F unction ······························································································ 37

2.6.2 M function Related Data··································································································· 37

2.7 Program Configuration············································································································ 39

2.7.1 Program···························································································································· 39

2.7.2 Program Number ·············································································································· 41

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.7.3 Sequence Number and Block···························································································· 42

2.7.4 Word and Address ············································································································ 42

2.7.5 Basic Addresses and Ranges of Command Values···························································· 43

2.7.6 End of Program ················································································································ 43

2.8 Coordinate Values and Dimensions························································································· 43

2.8.1 Absolute Commands and Incremental Commands ··························································· 43

2.8.2 Decimal Point Programming ···························································································· 45

2.8.3 Diameter Designation and Radius Designation ································································45

2.9 Tool Offset ······························································································································ 46

2.9.1 Geometry Tool Offset ······································································································· 46

2.9.2 T Code for Tool offset ······································································································ 46

2.9.3 Tool Offset Value Input by Moving the Tool To a Fixed Point ········································· 47

2.9.4 Direct Input of Tool Offset by Trial Cutting ·····································································47

2.10 Automatic Acceleration and Deceleration ············································································· 49

2.10.1 Speed Control In the Corner Between Blocks ···································································50

2.11 The Macro Program to User ·································································································· 50

2.11.1 The Macro Command ········································································································ 51

2.11.2 The Macro Program Body ······························································································ 51

2.11.3 Operation and Transfer Dictate（G65） ··········································································· 52

2.11.4 The Note about the Macro Program Body ······································································ 54

2.11.5 Example for User··············································································································· 55

III. Operation·········································································································································56

3.1 Operation Panel······················································································································· 56

3.1.1 LCD/MDI Panel ··············································································································· 56

3.1.2 Screen Change Keys········································································································· 57

3.1.3 Explanation of Key Board ································································································ 57

3.1.4 Machine Operation Panel ································································································· 58

3.2 Manual Operation···················································································································· 59

3.2.1 Manual Reference Point Return························································································ 59

3.2.2 Manual start Point Return································································································· 59

3.2.3 Manual Continuous Feed·································································································· 60

3.2.4 Step Feed ·························································································································· 61

3.2.5 Manual Handle Feed (Optional function) ········································································· 62

3.2.6 Manual auxiliary operation······························································································· 62

3.3 Automatic Operation ··············································································································· 64

3.3.1 Automatic Operation mode ······························································································ 64

3.3.2 Starting Automatic Operation ··························································································· 65

3.3.3 Executing Automatic Operation ······················································································· 65

3.3.4 Stopping and Terminating Memory Operation ·································································65

3.4 TEST OPERATION················································································································ 67

3.4.1 All Axis Machine Lock ···································································································· 67

3.4.2 Auxiliary Function Lock ·································································································· 67

3.4.3 Feedrate Override ············································································································· 67

3.4.4 Rapid Traverse Override··································································································· 68

3.4.5 Dry Running····················································································································· 68

3.4.6 Restart After Feed Hold···································································································· 68

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

3.4.7 Single Block ····················································································································· 68

3.5 Safety Operation······················································································································ 69

3.5.1 Emergency Operation ······································································································· 69

3.5.2 Overtravel························································································································· 70

3.6 Alarm ······································································································································ 70

3.7 Program Storage ＆ Edit ······································································································· 70

3.7.1 Preparation for Part Program Storage ＆ Edit Operation ················································ 70

3.7.2 Registering Program to Memory ······················································································ 70

3.7.3 Program Number Searching ····························································································· 71

3.7.4 Deleting Program ············································································································· 71

3.7.5 Deleting All Program········································································································ 71

3.7.6 Output a program ············································································································· 72

3.7.7 Output All Programs········································································································· 72

3.7.8 Sequence Number Search································································································· 72

3.7.9 Inserting, Amending and Deleting of word······································································· 73

3.7.10 Number of Registered Programs····················································································· 76

3.7.11 Capacity of System Memory ·························································································· 76

3.8 Display and Setting Data········································································································· 76

3.8.1 Offset Amount ·················································································································· 76

3.8.2 The setting of setting parameter························································································ 77

3.8.3 The Setting and Display of Custom Macro Variable························································· 79

3.8.4 Parameter ························································································································· 80

3.8.5 Diagnoses ························································································································· 82

3.9 Display ···································································································································· 82

3.9.1 Status display···················································································································· 82

3.9.2 Display of key in data······································································································· 83

3.9.3 Program Number, Sequence Number Display ·································································· 83

3.9.4 The Display of Program Memory Used.··········································································· 84

3.9.5 Display of Command Value ([PRG] key) ········································································· 84

3.9.6 Current position display ([POS] key) ··············································································· 85

3.9.7 Display of Run Time and Parts Count ·············································································· 86

3.9.8 Alarm Display([ALM] key)······························································································ 86

3.9.9 Adjusting Brightness of LCD ··························································································· 87

IV CONNECTION·································································································································88

4.1 SYSTEM CONNECTION DIAGRAM··················································································· 88

4.1.1 Layout diagram of interfaces···························································································· 88

4.1.2 Descriptions of Interfaces································································································· 88

4.1.3 Connection Diagram········································································································· 89

4.2 Detail of connection ················································································································ 89

4.2.1 From CNC to Axis Driver ································································································ 89

4.2.2 Description of Signal········································································································ 90

4.3 Connection between CNC and Axis Driver············································································· 92

4.4 Spindle Encoder ······················································································································ 93

4.5 RS232-C Serial Interface(Optional) ························································································ 93

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

4-6 Spindle Analogue Control Interface(Optional) ······································································· 94

4-7 Handwheel ······························································································································ 94

4.8 Connection of power supply···································································································· 95

4.9 In put/output Interface············································································································· 96

4.9.1 Connecting Diagram········································································································· 96

4.9.2 Input Signals····················································································································· 96

4.9.3 Signal Description ············································································································ 97

4.9.4 Output Signal ················································································································· 100

4.9.5 Diagnose Address Table of Input and Output Signal ······················································ 101

V Adjustment of Machine ····················································································································102

5.1 Preparation before Power On ································································································ 102

5.2 Adjustment of Machine ········································································································· 102

5.2.1 Emergency Stop Button·································································································· 102

5.2.2 Adjustment of Drive Axis······························································································· 102

5.2.3 Toolpost Adjustment······································································································· 104

5.2.4 Spindle Adjustment ········································································································ 104

5.2.5 Single step/ Handle Feed ································································································ 104

5.2.6 Others Adjustment·········································································································· 104

5.3 Standard Parameter Setting and the Storage of Parameter, Diagnosis and Program ·············· 105

Appendix Ⅰ Parameter ·····················································································································106 Appendix II Diagnosis·························································································································114 Appendix III Alarm Code List·············································································································119 Appendix IV Binary to Decimal Conversion Table·············································································122 Appendix V Installation dimension·········································································································I

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

Ⅰ INTRODUCTION

1.1 Introduction

GSK980T is a well-pervading machine numerical-controlled system produced by my factory. As

a upgrading production of the economical CNC,GSK980T has following characteristic:

△ Adopting 16-bit CPU,CPLD and hardware interpolation to realize high-speed and um

level control

△ Adopting 4-layer PCB and having high integration, reasonable technology and high

reliability

△ Having Chinese display with LCD and friendly interface, convenient operation △ Being able to adjusting accelerating or decelerating speed, matching step- motor or servo

motor

△ Being able to adjust the ratio of electronic gear and having convenient application

1.2 Type Signification

GSK 980T — 。

Assembly form： none：small panel（420×260mm）

L： big panel（420×320mm） B： boxed assembly Sort symbol ：none： surface operation panel A： alloy-solid operation panel

1.3 Type Table

Order type specification

GSK980T GSK980T-L GSK980T-B

GSK980TA

GSK980TA-L

GSK980TA-B GSK980T-DF3A □□□ □

420×260mm surface operation panel 420×320mm surface operation panel GSK980T-L boxed assembly，line goes out from the hole of box bottom（line going out from the top of box must be specified） 420×260mm alloy-solid operation panel

GSK980TA being assembled with the additional panel of AP01，the size is 420×320mm GSK980TA-L boxed assembly Being assembled with DF3A with line going out from the bottom of box（from the bottom of box）

GUANGZHOU CNC EQUIPMENT CO., LTD.

Machine CNC of 980T series

Production symbol of GSK

GSK980T CNC SYSTEM USER MANUAL

GSK980T-DF3A □□□ □-B

GSK980T-DY3 □□□□

-B

GSK980T-DY3□□□□

Note ：“□□□□”is 4-bit digit. the first 2-bit means the specification of driver in X axis, the second 2-bit means the specification of driver in Z axis. assembled in that axis.

Being assembled with DF3A with line going out from back （from aerial socket in the back of box）

Being assembled with DY3 with line going out from back（from aerial socket in the back of box） Being assembled with DY3 with line going out from the bottom of box（from the bottom of box）

“00” means no driver being

II. Programming

2.1 General

2.1.1 Axes Definition

In this CNC system, the main two axis of motion of the lathe machine is referred to as X and Z axis in a right hand coordinate system. Since the spindle of the lathe is horizontal, the Z axis is horizontal as well, the cross axis is denoted by X.A positive motion in both X and Z direction moves the tool away from the workpiece. The figure below shows the coordinate system of front toolpost lathe system and rear toolpost lathe system. In the front toolpost system, a positive command moves the Z axis from left to right and the X axis from back to front. In this CNC system we use front toolpost system for introducing the programming. Front toolpost system Rear toolpost system

2.1.2 Reference Point (Machine Zero Point)

Reference point is a fixed position on a machine tool which the tool can easily be moved. Usually, the reference point is set at the max. travel position of each axis at positive direction. Don’t use the reference point return function (such as G28).if the reference point is not available on the corresponding machine tool.

2.1.3 Coordinate value and direction and dimension

In this system, there are two ways to command the travels of the tool, the absolute command and incremental command, the using of the absolute command and the incremental command depending

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

on the address used. Absolute and incremental commands can be used together in one block. The format of the address is as follows:

X axis X U Z axis Z W

Address Absolute command Incremental command

2.1.4 Unit and Range of coordinate

The least input of this system is 0.001mm and the maximum input is ±9999.99.

Axis Least input unit Least motion increment

0.001mm(Diameter program) 0.0005mm X axis

0.001mm(Radius program) 0.001mm

Z axis 0.001mm 0.001mm

2.1.5 Initial and Modal Status of the Command

Initial status is the status of the control before it is programmed. Modal status means after the command is specified; it is effective until another command in the same group is specified .

2.1.6 The Start of a Program

At the beginning of program executing, the tool tips of the first programmed tool(standard tool)should be the start point of the programmed workpiece coordinate system. Usually, the first programmed tool is used as a standard tool which its offset compensation value is (0,0).

2.1.7 The End of a Program

Command code M30 is specified in the last block of a program to end the executing of a program. Before ending the executing of grogram by M30, the tool must be programmed to return to the start point of the workpiece coordinate system, and the corresponding tool offset compensation must be cancelled.

2.1.8 Program Configuration

The definition of the work coordinate system is depending on the start point of the tool in the corresponding work program by specifying a value after G50 is a floating coordinate, if G50 is not commanded the current absolute coordinate value is treated as the start point of the program. After a workpiece coordinate system is set, a point on the tool, such as the tool tip, is at specified coordinate.

2.1.9 Program Configuration

(1) Bock

The configuration of one block of program in this system is designated as follows:

N O O O O G O O X O O .O Z O O . O M O O S O O T O O O

N: Sequence Number

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

G: Preparatory Function X,Z: Dimension word M: Miscellaneous function S: spindle function T: Tool function

CR: End of block Each block of a program contains a sequence number for discriminating the executed sequence of each block the beginning of the block , and an end of bock code CR for indicating the end of the block..

(2)Program

Normally, a program number is specified at the beginning of the program, and a program end code M30 is specified at the end of the program.

CR:

00000:

M30CR

Program number Block Block Block

End of program

(3) Main Program and Subprogram

M98p1001

M98P1002

M98p1001

Subprogram #1

01001;

M99

Subprogram #2

01002;

M99

Program for

attern #1

Program for

attern #2

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

When machining of the same pattern appears at many sections of a workpiece program, a program for this pattern is created first, this is called the subprogram, on the other hand, the original program is called the main program. When a subprogram execution command is executed during the executing of the main program, commands of the subprogram are executed. When the executing of the subprogram is finished, the sequence returns to the main program.

2.2 controlled Axis

2.2.1 Number of Controlled Axis

Number of Controlled Axis 2 Axis (X, Z)

Number of Simultaneously control axis 2 Axis (X, Z)

2.2.2 Unit Setting

Input /Output The least input unit The least Command unit

X:0.001mm (Diameter designation)

Metric input /output

When radius Program is designated, the movement on X axis is program in Radius. Refer to the Operation manual issued by the machine builder for detail.

X:0.001mm (Radius designation )

Z:0.001 mm

X:0.0005mm

Z:0.001mm X:0.001mm Z:0.001mm

2.2.3 Maximum Strokes

Maximum Stroke = The least setting unit × 9999999

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.3 Preparatory Function (G Function)

A two-digit number following address G determines the meaning of the command for the concerned block. G codes are divided into the following two types: Type Meaning One-shot G code The G code is effective only in the block in which it is specified Modal G code The G code is effective until another G code in the same group is specified (Example) G01 and G00 are modal G code in the same group

G01X_; Z_; G01 is effective G00Z_ ; G00 is effective

G Code List

G Code Group Function

G00

*G01

G02 G03

G28 G32 01 Thread cutting G50 00 Coordination system setting G65 00 Macro command G70 Finishing cutting cycle G71 Outer diameter coarse cutting cycle G72 End face peck drilling cycle G73 Pattern repeating G74 End face peck drilling cycle G75 G90 Outer diameter/internal diameter slot cutting cycle G92 Thread cutting cycle G94 G96 Constant surface speed control enable G97

*G98 Feed per minute

G99

Note1: G codes marked with*are initial G codes when turning on power. Note2: The G codes of 2:00 are one-shot G codes. Note3: when a G code which is not listed in this G codes list or a G code without a corresponding option function is specified, alarm (No.010) is displayed. Note4: G codes of different groups can be specified in the same block of the program. If G codes of the same groups are specified in the same block, the last specified one is effective. Note5: The maximum spindle speed can be specified by G50 under the constant line speed control. Note6: G codes are displayed by each group number.

00 00

Positioning (Rapid traverse) Linear interpolation (Cutting feed) Circular interpolation CW Circular interpolation CCW Dwell, exactly stop G04 Return to reference point (Machine zero point)

Outer diameter/internal diameter slot cutting cycle

End face cutting cycle

Constant surface speed control disable

Feed per revolution

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

Note7: The clock wise or counterclockwise of G02,G03 commands are defined by the direction of the coordination system.

2.3.1 Positioning(G00)

The G00 command moves the tool to the specified position at a rapid traverse rate. Format:G00X((U)__Z(W)__;

The tool is positioned with the rapid traverse rate for each axis separately.

(Example)

Note: the Rapid traverse speed of the G00 command is set by the machine builder (ParameterNo.022~023), The rapid traverse feed rate for each axis of G00 command depends on the machine builder’s setting (Parameter No.022~023),it is controlled by Rapid traverse feed rate override switch on the operation panel. (F0,25%,50%,100%),rapid traverse can not be specified by F code.

56.0

φ40.0

on linear interpolation positioning

X (Diameter programming)

36.0

G00 U-60.0 W-36.0; G00 X40.0 Z56.0;or (Diameter programming)

30.0

2.3.2 Linear Interpolation (G01)

G01X (U) __Z (W) __F__;

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

This command specified a linear interpolation movement. Absolute or incremental dimension depends on the address X, Z/U, W .The feedrate is specified by address F, and is effective until a new value is specified .The feedrate need not be specified every time. (Example)

φ40.0

20.0

Start Point

End point

46.0

φ20.0

G00 U20.0 W-26.0; G01 X40.0 Z20.0;or Diameter Programming

2.3.3 Circular Interpolation (G02,G03)

The command below can move the tool along a circular arc on the specified plane.

G02 X__Z__ R_F

G03 X__Z__ I_K_F

Command Description G02 Clockwise direction(CW) G03 Counterclockwise direction(CCW)

X、Z U、Z I、K

R Radius of arc (radius value) F Feedrate along the arc

“Clockwise” and “Counterclockwise” on the Z-X plane of the Cartesian coordinate system are defined when the Z-X plane is views from the positive to negative direction of the Y-axis, as illustrated in the figure below:

The end point of the arc in the work coordinate system Distance from the start point to the end point Distance from the start point to the center of an arc

G03

G02

Cartesian coordinate system

GUANGZHOU CNC EQUIPMENT CO., LTD.

G03

GSK980T CNC SYSTEM USER MANUAL

(Diameter programming) (absolute value) G02 X..Z..R..F..; Or G02 X..Z..I..K..F..;

Center of arc

(Diameter Programming) (absolute value) G03 X..Z..R..F..; or G03 X..Z..I..k..F..;

The end point of the arc is specified by address X, Z or U, W. Address U and W specify the distance from the start point to the end point. The arc center is specified by address I and K for the X and Z axis. However, the value following K or I is a vector component in which the arc is seem from the start point, and is specified as an incremental value. As show below:

Center

Start point

End point (X, Z)

I, K must be signed according to the direction. The arc center also can be specified by address R. As show below:

G02 X_Z_R_F_;

G03 X_Z_R_F_; In this case, two types of arcs are considered (One arc is less than 180°, the other is more than 180°), as show in below figure. An arc exceeding 180° can not be commanded.

R=50

End point

R=50

Start point

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

(Example)

Absolute and increment programming:

G02 X50.0 Z30.0 125.0 F30;or

G02 U20.0 W-20.0 125.0 F30;or

G02 X50.0 Z30.0 R25.0 F30;or

G02 U20.0 W-20.0 R25. F30; The federate in circular interpolation is specified by address F, and the federate is controlled to be the feed rate along the arc (the tangential feedrate of the arc).

Note1:10, K0 can be omitted. Note2: When X and Z are omitted simultaneously, the end point is the same as the start point, and the center is specified with I and K, a 360° arc is specified G02 I_;(Full circle) When R is used ,an arc of 0° is specified: G02 R_; (The tool does not move) Note3: The error between the specified feedrate and the actual tool feedrate is ±2%. The feedrate is measured along the arc after the tool nose compensation is applied. Note4: If I, K and R addresses are specified simultaneously, the arc is specified by address R and the I and K address are ignored. Note5: When I and K are used, the difference in the radius values at the start point and the end point of the arc dose not cause an alarm…

φ50.0

30.0

50.0

10.0

15.0

R25.0

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.3.4 Thread Cutting (G32)

Equal lead straight thread, tapered screws and scroll threads can be cut by using Command G32.

Metric thread can be cut by using the below command (the lead of the thread is specified by F address):

G32 X (U) _Z(W) _F_;(Metric thread) F address specify the lead in long axis ranged from 0.001 to 500.000mm Inch thread can be cut by using the below command(the teeth number is specified by I address):

G32 X (U) _Z(W) _I_;(Inch thread) I address specified the teeth number per inch in long axis ranged from 0.060 to 254000.000 teeth/inch. (Example)

G32 X__Z__F__;

X axis End point

In general, the thread cutting need to repeat along the same path in rough cutting through finish cuts for a thread. Since the thread cutting starts when a I-revolution signal is output from the spindle position encoder, thread cutting is started at a fixed point and the tool path on the workpiece is unchanged for repeated threading cutting. The spindle speed must remain constant from rough cutting through finish cutting. if not, thread lead error will occur.

Z axis

Start point

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

Tapered thread

α≤45°

α＞45°

the lead is LZ

the lead is LX

The lead always is specified in radius. The lead can not be cut correctly due to reason of deceleration and acceleration in the beginning and ending of the threading cutting, To cut a correct lead, the programmed length of the thread must be longer than the actual length of the thread. Example: thread cutting

70mm

δ2

Lead of thread: 4mm

δ1=3mm δ2=1.5 mm

Depth of cutting in X-axis direction: 1MM(cut twice) (Metric input, diameter programming)

G00 U-62.0; G32 W_74.5 F4.0; G00 U62.0; W74.5 U-64.0;(Cut 1MM more in second cut ) G32 W-74.5 F4.0; G00 U64.0 W74.5;

GUANGZHOU CNC EQUIPMENT CO., LTD.

30mm

GSK980T CNC SYSTEM USER MANUAL

30mm

40mm

φ14.0

φ43.0

φ50.0

δ1

δ2

Lead of thread :In Z axis direction:3.5mm

δ1=2mm δ2=1mm

Depth of cutting in X axis direction:1MM(cut twice) Using the above mentioned data to program: (Metric Input, diameter programming)

G00 X12.0 Z72.0; G32 X41.0 Z29.0 F3.5; G00 X50.0 Z72.0; X10.0; (1MM more in second cut) G32 X39.0 Z29.0

G00 X50.0 Z72.0: Note1: When the previous block also was a thread cutting block, the cutting will start immediately without detecting the 1-revolution signal.

G32 Z__F__;

Z__; (1-revolution signal is not detected before the executing of this block)

G32__; (this block also is thread cutting block)

Z__F__;(1-revolution signal is also not detected)

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.3.5 Return to Reference Point Automatically (G28)

G28 X (U)__Z(W)__; This command can make the tools return to reference point automatically via an intermediate position, the intermediate position is specified by addresses X(U)__Z(W). (1)Positioning from the present position to the intermediate position of the designated axis at rapid

traverse rate(point A→point B). (2)Return to reference point from the intermediate position at rapid traverse rate(point B→point R).

(3)If the machine lock is turn off, when the tool has returned to the reference point, the reference point return completion led goes on.

Note1: If returning to the reference point manually has never been done after power on ,the motion of returning to the reference point automatically from the intermediate point in G28 is same as that in manual way. The direction of intermediate point is specified by parameter No.006(ZMX,ZMZ). Note2:If the start point of machining program is same as the reference point ,doing G28 can return to the start point of machining program. Note3:If the start point of machining program is not same as the reference point ,returning to the start point of machining program can be realized by rapid positioning command or operation of returning to the start point, not by G28.

G28 X40 Z50

Present Point A

Reference point R

Intermediate point

B (40, 50)

2.3.6 Dwell(G04)

By specifying a dwell, the execution of the next block is delayed by the specified time. Format:

G04 P__; or G04 X__; or G04 U__;

The unit of the delay time is second. Command value of the dwell time is from 0.001 to

99999.999second. If addresses P, X is omitted, this command can specified an exact stop.

2.3.7 Work Coordinate System Setting(G0)

A work coordinate system can be set using the following the blow command:

G50 X(x) Z(z); Use this command to set a coordinate system ,this coordinate system is referred as a workpiece coordinate system, so a point on the tool, such as the tool tip ,is specified as coordinate value(x, z). Once a workpiece coordinate system has been set, the absolute position of following blocks is specified according to this coordinate system When diameter programming, X address is specified by diameter value. When radius programming, X address is specified by radius value.

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

(Example) Coordinate system setting with diameter designation

G50 X100.0 Z150.0;

100.00mm

150.00mm Start point = reference point

As illustrated in above figure, the reference point on the turret is superposition with the start point, and the coordinate system is set by G50 at the start of the program. Thus, when an absolute command is carried out, The start point will move to the position commanded. In order to move the tool tip to the position commanded, the difference between the reference and the tool tip is compensated by the too offset.

Note: If the coordinate system setting is carried out by G50, a coordinate system in which the position prior to the effecting of the offset becomes the designated position, is set.

2.3.8 Feed per Minute (G98)

G98 specify the feed per minute, a number follows F specify the amount of feed of the cutting tool per minute. G98 is a modal code. Once a G98 is specified, it is available until a G99 (feed per revolution )is specified.

2.3.9 Feed per Revolution(G99)

G99 specified the feed per spindle revolution. A number follows F specified the amount of feed the cutting tool per spindle revolution. G99 is also a modal code, once a G99 is specified; it is available until a G98 is specified.

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

Table 2.3.9 Feed Per Minute and Feed Per Revolution

Feed per minute Feed per revolution

Address F F

Command

code

Command

ranges

Limitation value

Override

The limitation takes place at a certain specified speed for both feed per minute and feed per revolution. This clamping value is set by the machine tool builder. (Override is applied to implement clamping of speed) An override from 0~150%(10%per step)can be applied to both feed per minute mode and feed per revolution mode

G98 G99

1~8000mm/min

(F1~F8000)

0.01~500.00mm/rev (F1~F50000)

Note: when using feed per revolution mode, if it necessary to affix a position encoder to the spindle.

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.3.10 Constant Surface Speed Control(G96, G97)

When the surface speed is set by a value after address S, and the spindle speed is calculated according to the relative position between the tool and the workpiece to keep the surface speed always the specified value, so-called constant surface speed control. Voltage is fed to the spindle control section so that the spindle rotates to produce the correct surface speed. The units of the surface speed is as follows:

Input unit Surface speed unit Metric system m/min

The units of the surface speed depend on the setting of the machine tool builder. The Constant surface speed control is specified by the follow command:

G96 S__; The surface speed is set after address S. The constant speed control can be canceled by the following command:

G97 S__; The spindle speed is set after address S. It is necessary to apply the constant speed control on Z axis.

Spindle speed (rpm)

（n）

3000

2800

2600

2400

2200

2000

1800

1600

1400

1200

1000

800

600

400

200

40 60 80

GUANGZHOU CNC EQUIPMENT CO., LTD.

As show in the figure, the spindle speed (rpm) coincides with the surface4 speed (m/min) at approx. 160mm(radius).

为

100

120140 160

min

180

200220 240260280300

单位（mm）

GSK980T CNC SYSTEM USER MANUAL

(1)Spindle Speed Override

An override for the specified surface speed or the spindle speed can be specified in 50,60,70,80,90,100,110,120%

(2)Maximum Spindle Speed Limitation

The value follows G50 S specify the maximum spindle speed for constant surface speed control in rpm:

G50 S__; When the spindle speed in constant surface speed control reaches the value specified in the above command, the spindle speed is clamped at this maximum value.

(3)Constant Surface Speed Control for Rapid Traverse(G00)

For a Block in which G00is specified, the constant surface speed control is made by calculating the surface speed based on the position at the end point of the rapid traverse block instead of calculating the surface speed to a transient change of the tool position, Because at rapid traverse condition, cutting is not executed. (Example:)

1050

300 400 500 600 700 800 900 1000 1100 1200 1300 1400 1500

600

Programmed path

Path after compensation

N15

N14

400

N11

100

200

300

375

400

500

Radius value

600

700

675

(Diameter programming)

N8 G00 X1000.Z1400.; N9 T0303; N11 X400.Z1050.; N12 G50 S3000; (Designation of Maximum spindle speed) N13 G96 S200; (Surface speed 200m/,in) N14 G01 Z700. F1000; N15 X600. Z400.;

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

N16 Z....;

The CNC use the programmed coordinate value on the X axis to calculate the surface speed. When offset compensation is valid, this is not the value calculated according to the X axis coordinate after offset. At the end point N15 in example above is not the turret center, but the tool nose, that is to say at 600dia, the surface speed is 200m/min. If X axis coordinate value is negative, the CNC uses the absolute value.

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

2.3.11 Canned Cycle(G90, G92 G94)

For repetitive machining peculiar to turning, such as the metal removal in rough cutting, the cutting of the same path is made repetitively, by using these cycles. The said cutting specified in a range of three to several dozen blocks can be specified in one block. In addition, only the values to be changed need to be specified for repetition, the program using this cycle is very simple and useful. The drawings in the examples below are for diameter programming. In radius programming, change U/2 or X/2 to U or X respectively.

(1)Outer Diameter/Internal Diameter Cutting Cycle(G90)

(a)Cylinder cutting cycle

G90 X (U)__Z(W)__F__;

Z axis

X/2

2（F）

Xaxis

3（F）

4（R）

1（R）

U/2

F：Cutting feed

R:Rapid traverse

Tool

In incremental programming, the signs of the numbers following address U and W depend on the direction of paths1 and 2, in the cycle of above figure, the signs of U and W are negative. In single block mode, Operation of 1,2,3,4 are performed by pressing the cycle start key. (b)Taper cutting cycle

G90 X (U)__Z(W)__R__F__;

Z axis

X/2

2（F）

U/2

X axis

3（F）

1（R）

4（R）

F：Cutting feed R:Rapid traverse

Tool

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

In incremental programming, the relation between the signs of the numbers following the address U、 W、R, and the tool paths are as follows:

1) U <, W<0, R<0 2) U >0, W<0, R>0

U/2

3(F)

2(F)

U/2

1(R)

4(R)

3(F)

2(F)

U<0, W<0, R>0 4) U>0, W<0, R<0 But ︱R︱≤︱U/2︱ But ︱R︱≤︱U/2︱

1(R)

2(F)

3(F)

1(R)

4(R)

U/2

(2) Thread Cutting Cycle (G92)

(a) Straight thread cutting

G92X (U)__Z(W)__F__; (Metric thread)

G92X (U)__Z(W)__I__; (Inch thread)

GUANGZHOU CNC EQUIPMENT CO., LTD.

Pitch specified (L)

3(F)

2(F)

4(R)

1(R)

U/2

GSK980T CNC SYSTEM USER MANUAL

Note: Address I for inch thread is not a modal command.

Pitch specified (Number of teeth/inch)

Z axis

F：Cutting feel

R:Rapid traverse

X axis

Width of chanferring

2（F）

3（R）

4（R）

1（R）

X/2

U/2

Tool

In incremental programming, the signs of values of U and W commands depend on the direction of paths 1 and 2. It is to say, if the direction of path 1 is negative along X axis, the value of U is negative. The command of the lead of thread and the limitation of spindle is same with command G32. In single block mode, single block is effective for operation1,2,3,4. The length of the chamfering is set by parameter No.019THDCH. The width of the chamfering is set by parameter No.THDCH*1/10*L (lead of thread) Note 1:As mentioned in Note of G32.And, When the FEED HOLD key is pressed during the execution of the thread cutting block, the feed would not stop until path 3 is finished. (b)Taper Thread Cutting Cycle:

G92 X (U)__Z (W)__R__F__;

lead specified (L)

G92 X (U)__ Z (W)__R__I__;

lead specified (number of teeth/inch)

Note: Address I for inch thread is not a modal command.

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

X/2

U/2

X axis

3（R）

(3) End Face Cutting Cycle(G94)

(a)End Face Cutting Cycle

G94 X (U)__ Z(W)__F__;

2（F）

4（R）

Z axis

1（R）

F：Cutting feed

R:Rapid traverse

Tool

X axis

3（F）

2（F）

4（R）

1（R）

X/2

U/2

F：Cutting feed

R:Rapid traverse

Tool

Zaxis

In incremental programming, the signs of the value following address U and W depend on the direction of paths 1 and 2. That is, if the path 1 is negative along Z axis, the sign of the value of W is negative. In single running mode, press Cycle start Key to perform the operation 1,2,3 and 4. (b)Taper Face Cutting Cycle

G94 X (U)__Z (W)__R__F__;

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

Z axis

X/2

3（F）

U/2

2（F）

1（R）

4（R）

X axis

F：Cutting feed

R:Rapid traverse

In incremental programming, the relationship between the signs of the values of U, W and R and the tool paths is as follows:

1) U<0, W<0, R<0 2)U>0, W<0, R<0

U/2

2(F)

3(F)

4(R)

U/2

1(R)

3)U<0, W<0, R>0(︱R︱≤︱W︱) 4)U>0, W<0, R>0(︱R︱≤︱W︱)

2(F)

1(R)

3(F)

4(R)

1(R)

4(R)

2(F)

3(F)

U/2

2(F)

3(F)

1(R)

4(R)

U/2

Note 1: The data value of X (U), Z (W) and R of during canned cycle are modal as same as G90,G92 and G94, if X (U), Z (W) or R is not newly commanded, the previously commanded

GUANGZHOU CNC EQUIPMENT CO., LTD.

GSK980T CNC SYSTEM USER MANUAL

data is still effective.

In the example below, a canned cycle can be repeated only by specifying the new movement commands for X axis, but the Z axis movement need not be re-commanded. However, these data are cleared if a one-shot G code expect G04 or a G code, which is not in the same group with G90, G92 and G94, is command. (Example):

Z axis

X axis

The following program can perform the cycle in the above figure:

N030 G90 U-8.0 W-66.0 F4000;

N031 U-16.0;

N032 U-24.0;

N033 U-32.0;

2.3.12 Multiple Repetitive Cycle (G70~G75)

This optional canned cycle function is used to make the programming easy. For example, the data for the finish workpiece shape can be used as the data for rough cutting automatically.

(1)Multiple Repetitive Cycle for Outer Diameter (G71)

As in the figure below, a finished shape of A to A’ to B is given by a program, the specified area is removed by depth of cut △D, and the finish cutting allowance of △ U/2, and △W is left.

Program commanded path

△W

Aˊ

△U/2

Cutting feed

Rapid travers

△D

GUANGZHOU CNC EQUIPMENT CO., LTD.

+ 108 hidden pages