gsk GSK218M Operation Manual

Download

GSK218M CNC SYSTEM Programming and Operation Manual

This user manual describes all proceedings concerning the

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

it is impractical to give particular descriptions for all unnecessary or

unallowable system operations due to the manual text limit, product

specific applications and other causes. Therefore, the proceedings not

indicated herein should be considered impractical or unallowable.

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

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

individual to publish or reprint this manual without the express written

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

legal liability.

GSK218M CNC SYSTEM Programming and Operation Manual

Preface

Your excellency,

It’s our pleasure for your patronage and purchase of this GSK GSK218M CNC

system made by GSK CNC Equipment Co., Ltd.

This book is “Programming and Operation” manual.

！ Accident may occur by improper connection and operation！ This

system can only be operated by authorized and qualified personnel.

Please carefully read this manual before usage！

Special cautions:

The power supply fixed on/in the cabinet is exclusively used for the CNC system made by GSK. It can't be applied to other purposes, or else it may cause serious danger.

This manual is reserved by final user.

All specifications and designs herein are subject to change without further notice.

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

GSK218M CNC SYSTEM Programming and Operation Manual

Warning and Precautions

Warning, note and explanation

This manual contains the precautions to protect user and machine. The precautions are classified as warning and note by safety, and supplementary information is regarded as explanation. Read the warnings, notes and explanations carefully before operation.

Warning

Personnel may be hurted or equipment be damaged if operations and steps are not observed.

Note

Equipment may be damaged if operation instructions or steps are not observed by user.

Explanation

It is used for the supplementary information except for warning and note.

z Copy right is reserved.

III

GSK218M CNC SYSTEM Programming and Operation Manual

CONTENT

Ⅰ OVERVIEW..........................................................................................................................1

Ⅱ PROGRAMMING.................................................................................................................3

1 General.....................................................................................................................................4

1.1 Tool movement along workpiece contour —interpolation................................................4

1.2 Feed——Feed function...................................................................................................5

1.3 Cutting feedrate, spindle speed function.........................................................................6

1.4 Operation instruction——miscellaneous function............................................................6

1.5 Tool selection for various machining——Tool function.................................................... 6

1.6 Tool figure and tool motion by program...........................................................................7

1.6.1 Tool length compensation....................................................................................7

1.6.2 Tool radius compensation....................................................................................7

1.7 Tool movement range——stroke.....................................................................................8

2 Part Program Composition.....................................................................................................9

2.1 Program composition......................................................................................................9

2.1.1 Program name.....................................................................................................9

2.1.2 Sequence number and block .............................................................................10

2.1.3 Instruction word..................................................................................................10

2.2 General structure of a program.....................................................................................11

2.2.1 Subprogram edit ................................................................................................13

2.2.2 Subprogram call.................................................................................................13

2.2.3 Program end......................................................................................................14

3 Programming Fundamentals................................................................................................15

3.1 Controlled axis ..............................................................................................................15

3.2 Axis name.....................................................................................................................15

3.3 Coordinate system........................................................................................................15

3.3.1 Machine coordinate system ...............................................................................15

3.3.2 Reference point..................................................................................................15

3.3.3 Workpiece coordinate system............................................................................16

3.3.4 Absolute programming and relative programming .............................................17

3.4 Mode and non-mode.....................................................................................................18

3.5 Decimal point programming ..........................................................................................19

4 Preparatory Function: G code..............................................................................................20

4.1 Classification of G code ................................................................................................20

4.2 Simple G code ..............................................................................................................23

4.2.1 Rapid positioning G00........................................................................................23

4.2.2 Linear interpolation G01.....................................................................................24

4.2.3 Circular (helical) interpolation G02/G03.............................................................25

4.2.4 Absolute/ incremental programming G90/G91...................................................30

GSK218M CNC SYSTEM Programming and Operation Manual

4.2.5 Dwell(G04).........................................................................................................31

4.2.6 Unidirectional positioning (G60).........................................................................32

4.2.7 System parameter online modification (G10).....................................................33

4.2.8 Workpiece coordinate system G54～G59..........................................................34

4.2.9 Additional workpiece coordinate system............................................................36

4.2.10 Machine coordinate system selection G53 ......................................................37

4.2.11 Floating coordinate system G92 ......................................................................37

4.2.12 Plane selection G17/G18/G19 .........................................................................39

4.2.13 Polar coordinate system setup/cancel G16/G15..............................................40

4.2.14 Scaling in plane G51/G50................................................................................42

4.2.15 Coordinate system rotation G68/G69...............................................................46

4.2.16 Skip function G31.............................................................................................50

4.2.17 Inch/metric conversion G20/G21......................................................................51

4.2.18 Optional angle chamfering/corner rounding.....................................................52

4.3 Reference point G code................................................................................................53

4.3.1 Reference point return G28 ...............................................................................54

4.3.2 2nd, 3rd, 4th reference point return G30............................................................55

4.3.3 Automatic return from reference point G29........................................................56

4.3.4 Reference point return check G27.....................................................................57

4.4 Canned cycle G code....................................................................................................57

4.4.1 Rough milling of inner circular groove G22/G23 ................................................62

4.4.2 Fine milling cycle within a circle G24/G25..........................................................65

4.4.3 Outer circle finish milling cycle G26/G32 ...........................................................67

4.4.4 Rectangular groove rough milling G33/G34.......................................................70

4.4.5 Inner rectangular groove finish milling cycle G35/G36.......................................72

4.4.6 Rectangle outside finish milling cycle G35/G36.................................................74

4.4.7 High-speed peck drilling cycle G73....................................................................76

4.4.8 Drilling cycle, spot drilling cycle G81..................................................................78

4.4.9 Drilling cycle, counterboring G82 .......................................................................80

4.4.10 Drilling cycle with chip removal G83 ................................................................81

4.4.11 Right-handed tapping cycle G84......................................................................83

4.4.12 Left-handed tapping cycle G74........................................................................85

4.4.13 Fine boring cycle G76......................................................................................87

4.4.14 Boring cycle G85..............................................................................................88

4.4.15 Boring cycle G86..............................................................................................90

4.4.16 Boring cycle, back boring cycle G87................................................................92

4.4.17 Boring cycle G88..............................................................................................93

4.4.18 Boring cycle G89..............................................................................................95

4.4.19 Left-handed rigid tapping G74.......................................................................96

4.4.20 Right-handed rigid tapping G84 .......................................................................98

4.4.21 Peck drilling rigid tapping (chip removal) cycle ..............................................100

4.4.22 Canned cycle cancel G80..............................................................................102

4.5 Tool compensation G code.......................................................................................... 105

4.5.1 Tool length compensation G43, G44, G49.......................................................105

4.5.2 Tool radius compensation G40/G41/G42.........................................................108

4.5.3 Explanation of tool radius compensation .........................................................114

GSK218M CNC SYSTEM Programming and Operation Manual

4.5.4 Corner offset circular interpolation（G39） .....................................................131

4.5.5 Tool offset value and number input by pr ogram（G10）.................................133

4.6 Feed G code ...............................................................................................................133

4.6.1 Feed mode G64/G61/G63 ...............................................................................133

4.6.2 Automatic override for inner corners（G62） ..................................................134

4.7 Macro G code .............................................................................................................136

4.7.1 Custom macro..................................................................................................136

4.7.2 Macro variables................................................................................................137

4.7.3 Custom macro call...........................................................................................143

4.7.4 Operation and transfer instruction....................................................................143

4.7.5 Examples for custom macro.............................................................................148

5 Miscellaneous Function M code ........................................................................................150

5.1 M codes controlled by PLC .........................................................................................151

5.1.1 Forward and reverse rotation instructions（M03, M04） ..............................151

5.1.2 Spindle stop (M05)...........................................................................................152

5.1.3 Cooling on and off （M08, M09） ................................................................ 152

5.1.4 A axis release and clamping（M10, M11）...................................................152

5.1.5 Tool release and clamping（M16, M17） .....................................................152

5.1.6 Spindle orientation（M19） .............................................................................152

5.1.7 Tool search instruction（M21, M22） ...........................................................152

5.1.8 Magazine rotation instruction（M23, M24）..................................................152

5.1.9 Rigid tapping（M29）......................................................................................152

5.1.10 Lubricating on and off（M32, M33）...........................................................153

5.1.11 Helical chip remover on and off（M35, M36） ............................................153

5.1.12 Mirror image instructions（M40, M41, M42, M43） ...............................153

5.1.13 Spindle blowing on and off（M44, M45） ...................................................153

5.1.14 Auto tool change start and end（M50, M51）.............................................153

5.1.15 Tool judging after tool change（M53）..........................................................153

5.2 M codes used by program...........................................................................................153

5.2.1 Program end and return （M30, M02） .......................................................154

5.2.2 Program dwell（M00）....................................................................................154

5.2.3 Program optional stop（M01）........................................................................154

5.2.4 Subprogram calling （M98） ..........................................................................154

5.2.5 Program end and return（M99） .....................................................................154

6 S codes for Spindle Function.............................................................................................155

6.1 Spindle analog control.........................................................................................155

6.2 Spindle switch volume control.............................................................................155

6.3 Constant surface speed control (G96/G97).........................................................156

7 Feed Functions F code.......................................................................................................159

7.1 Traverse......................................................................................................................159

7.2 Cutting feedrate ..........................................................................................................159

7.2.1 Feed per minute（G94） .................................................................................160

7.2.2 Feed per revolution（G95） ............................................................................160

7.3 Tangential speed control.............................................................................................161

7.4 Feedrate override keys ...............................................................................................161

GSK218M CNC SYSTEM Programming and Operation Manual

7.5 Auto acceleration/deceleration....................................................................................162

7.6 Acceleration/deceleration for corner of a block ...........................................................163

8 Tool Function.......................................................................................................................164

8.1 Tool function................................................................................................................164

Ⅲ OPERATION....................................................................................................................165

1 Operator Panel ....................................................................................................................166

1.1 Panel layout................................................................................................................166

1.2 Explanation of the panel function................................................................................166

1.2.1 LCD area .........................................................................................................166

1.2.2 Edit area ..........................................................................................................167

1.2.3 Screen operation keys .....................................................................................168

1.2.4 Control area.....................................................................................................169

2 System Power On/Off and Safety Operations...................................................................173

2.1 System power on ........................................................................................................173

2.2 System power off ........................................................................................................173

2.3 Safety operations........................................................................................................ 174

2.3.1 Reset operation................................................................................................174

2.3.2 Emergency stop...............................................................................................174

2.3.3 Feed hold.........................................................................................................175

2.4 Cycle start and feed hold ............................................................................................175

2.5 Overtravel protection...................................................................................................175

2.5.1 Hardware overtravel protection........................................................................175

2.5.2 Software overtravel protection .........................................................................176

2.5.3 Release of the overtravel alarm .......................................................................176

3 Interface Display as well as Data Modification and Setting.............................................180

3.1 Position display.........................................................................................................180

3.1.1 Four types of position display...........................................................................180

3.1.2 The display of the run time, part count, programming speed and override, actual

speed etc.........................................................................................................182

3.1.3 Relative coordinate clearing and mediating .....................................................184

3.2 Program display..........................................................................................................185

3.3 The display, modification and setting of the parameters .............................................189

3.3.1 Parameter display............................................................................................189

3.3.2 Modification and setting of the parameter values.............................................190

3.4 Offset display, modification and setting.......................................................................191

3.4.1 Offset display...................................................................................................191

3.4.2 Modification and setting of the offset value......................................................193

3.5 Setting display.............................................................................................................193

3.5.1 Setting page.....................................................................................................193

3.5.2 Parameter and program switch page...............................................................195

3.5.3 Coordinate setting interface.............................................................................196

3.5.4 Display and setting of the machine soft panel..................................................197

3.5.5 Servo page.......................................................................................................198

3.5.6 Backup, restore and transfer of the data..........................................................199

VII

GSK218M CNC SYSTEM Programming and Operation Manual

3.5.7 Password authority setting and modification....................................................200

3.6 Graphic display ...........................................................................................................201

3.7 Diagnosis display........................................................................................................203

3.7.1 Diagnosis data display.....................................................................................203

3.7.2 Signal viewing..................................................................................................206

3.8 Alarm display ..............................................................................................................206

3.9 PLC display.................................................................................................................209

3.10 Index display.............................................................................................................211

4 Manual Operation................................................................................................................216

4.1 Coordinate axis movement .........................................................................................216

4.1.1 Manual feed.....................................................................................................216

4.1.2 Manual rapid traverse ......................................................................................216

4.1.3 JOG feedrate and manual rapid traverse speed selection...............................216

4.1.4 Manual intervention..........................................................................................217

4.2 Spindle control ............................................................................................................218

4.2.1 Spindle CCW ...................................................................................................218

4.2.2 Spindle CW......................................................................................................219

4.2.3 Spindle stop.....................................................................................................219

4.2.4 Spindle auto gear shift .....................................................................................219

4.3 Other manual operations.............................................................................................220

4.3.1 Cooling control.................................................................................................220

4.3.2 Lubricating control............................................................................................220

4.3.3 Chip removal....................................................................................................220

4.3.4 Work light control.............................................................................................220

5 Step Operation ....................................................................................................................221

5.1 Step feed.....................................................................................................................221

5.1.1 Selection of moving amount.............................................................................221

5.1.2 Selection of moving axis and direction.............................................................221

5.1.3 Step feed explanation ......................................................................................222

5.2 Step interruption..........................................................................................................222

5.3 Auxiliary control in Step mode.....................................................................................222

6 MPG Operation....................................................................................................................223

6.1 MPG feed....................................................................................................................223

6.1.1 Moving amount selection .................................................................................223

6.1.2 Selection of moving axis and direction.............................................................223

6.1.3 Explanation of MPG feed.................................................................................224

6.2 Control in MPG interruption.........................................................................................225

6.2.1 MPG interruption operation..............................................................................225

6.2.2 Relation of MPG interruption with other functions............................................226

6.3 Auxiliary control in MPG mode....................................................................................226

7 Auto Operation....................................................................................................................227

7.1 Selection of the auto run programs.............................................................................227

7.2 Auto run start...............................................................................................................227

7.3 Auto run stop...............................................................................................................228

7.4 Auto running from an arbitrary block ...........................................................................229

VIII

GSK218M CNC SYSTEM Programming and Operation Manual

7.5 Dry run........................................................................................................................229

7.6 Single block running....................................................................................................230

7.7 Running with machine lock .........................................................................................230

7.8 Running with M.S.T. lock.............................................................................................231

7.9 Feedrate and rapid override in auto run......................................................................231

7.10 Spindle override in auto run ......................................................................................232

7.11 Background edit in auto run ......................................................................................232

8 MDI Operation......................................................................................................................234

8.1 MDI instructions input..................................................................................................234

8.2 Run and stop of MDI instructions................................................................................235

8.3 Words modification and clearing of MDI instructions...................................................235

8.4 Modes changing..........................................................................................................235

9 Machine Zero Operation.....................................................................................................236

9.1 Conception of machine zero .......................................................................................236

9.2 Steps for machine zero ...............................................................................................237

9.3 Machine zero steps by program..................................................................................237

10 Edit Operation ...................................................................................................................239

10.1 Program edit .............................................................................................................239

10.1.1 Program creation ...........................................................................................240

10.1.2 Deletion of a single program ..........................................................................245

10.1.3 Deletion of all programs................................................................................. 245

10.1.4 Copy of a program.........................................................................................246

10.1.5 Copy and paste of blocks...............................................................................246

10.1.6 Cut and paste of block ...................................................................................247

10.1.7 Replacement of the blocks.............................................................................247

10.1.8 Rename of a program....................................................................................247

10.1.9 Program restart..............................................................................................248

10.2 Program management ..............................................................................................249

10.2.1 Program directory search...............................................................................249

10.2.2 Number of the program stored.......................................................................250

10.2.3 Memory capacity............................................................................................250

10.2.4 Viewing of the program list.............................................................................250

10.2.5 Program lock..................................................................................................250

11 Communication.................................................................................................................251

11.1 Serial communication................................................................................................251

11.1.1 Program start.................................................................................................251

11.1.2 Function introduction......................................................................................251

11.1.3 Software usage..............................................................................................252

11.2 USB communication..................................................................................................256

11.2.1 General and precautions................................................................................256

11.2.2 USB flash disk entry.......................................................................................256

11.2.3 USB part program operation steps .................................................................256

11.2.4 DNC processing operation steps ...................................................................257

11.2.5 USB flash disk system exit.............................................................................257

11.2.6 Remarks for USB flash disk model ................................................................257

GSK218M CNC SYSTEM Programming and Operation Manual

APPENDIX 1 ..............................................................................................................................259

1 Bit parameter .................................................................................................................260

2 Number parameter.........................................................................................................281

APPENDIX 2 ..............................................................................................................................310

Alarm List..................................................................................................................................310

GSK218M CNC SYSTEM Programming and Operation Manual

Ⅰ OVERVIEW

GSK218M CNC SYSTEM Programming and Operation Manual

1. Overview

This manual is comprised by following parts:

I Overview

It describes the chapter structure, system model available, relative instructions and the

note.

Ⅱ Programming

It describes G functions and the programming format, characteristics and restrictions

by NC language.

OperationⅢ

It describes the manual and auto operation, program input/output and editing methods.

Appendix

It describes parameter list, alarm list and programming data table.

The manual is used for GSK218M CNC system.

GSK218M CNC SYSTEM Programming and Operation Manual

Ⅱ PROGRAMMING

GSK218M CNC SYSTEM Programming and Operation Manual

1 General

1.1 Tool movement along workpiece contour —interpolation

1） Tool movement along a straight line

Fig. 1-1-1

2）

Tool movement along an arc

Fig. 1-1-2

The tool linear and arc motion function is called interpolation.

The programming instructions such as G01, G02 are called preparatory function, which is

used for interpolation for CNC device.

GSK218M CNC SYSTEM Programming and Operation Manual

a) Movement along straight line

G01 Y X Y ;

;

Interpolation

a) Movement along straight

line

b) Movement along arc

G03 X

Y R ;

X axis (Motor)

Y axis (Motor)

Tool movement

Fig.1-1-3

Note For some machines, it is the worktable moving other than tool moving in practice.

It is assumed that the tool moves relative to the workpiece in this manual. Refer to the machine actual movement direction in practice to protect against personnel hurt and machine damage.

1.2 Feed——Feed function

The feedrate specification is called feed function.

Fig. 1-2-1

To specify a speed to machine the part by tool is called feed and the machine speed is instructed by a numerical value. For example, the program instruction is F150 if tool feeds by 150mm/min.

GSK218M CNC SYSTEM Programming and Operation Manual

1.3 Cutting feedrate, spindle speed function

Tool

工件

Tool diameter

V: Cutting speed

(m/min）

RPM

workpiece

Fig. 1-3-1

The speed of tool relative to workpiece in cutting is called cutting feedrate. It can be

instructed by spindle speed RPM(r/min) by CNC.

Example: If the tool diameter is 10mm, cutting linear speed is 8 m/min, the spindle speed

is about 255RPM according to N=1000V/πD, so the instruction is: S255

Instructions related to spindle speed are called spindle speed function.

1.4 Operation instruction——miscellaneous function

When the workpiece is to be machined, to make the spindle run and supply coolant, the

machine spindle motor and cooling pump switches must be controlled by actual requirement.

Fig. 1-4-1

The programs or machine switch actions controlled by system NC instructions are called

miscellaneous functions, which are instructed by M code.

Example: If M03 is instructed, the spindle rotates clockwise by the speed specified.

(Clockwise direction means the direction viewed from the spindle –Z negative direction.)

1.5 Tool selection for various machining——Tool function

It is necessary to select a proper tool when drilling, tapping, boring, milling, etc. is performed. When a number is assigned for each tool and the number is specified in the program, the corresponding tool is selected.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 1-5-1

Example When the tool is placed at location 01 in the ATC magazine, the tool can be selected by specifying T01 code. This is called the tool function.

1.6 Tool figure and tool motion by program

1.6.1 Tool length compensation

Usually several tools are used for machining one workpiece. If instructions such as G0Z0 are executed in a same coordinate system, because tools have different tool lengths, the distances from tool end to workpiece are different. So it is very troublesome to change the program frequently.

Fig. 1-6-1-1

Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (usually the 1st tool), machining can be performed without altering the program even when the tool is changed. After the tool positioning in Z axis (e.g. G0Z0), the distances of the tool end to the workpiece are identical. This function is called tool length compensation.

1.6.2 Tool radius compensation

Because a tool has a radius, if the tool goes by the path given by program, the workpiece will

be cut off a part for a radius wide. To simplify the programming, the program can be run by CNC

around the workpiece with the tool radius deviated, while the transient path of the intersections of

the lines or the arcs can be processed automatically by system.

GSK218M CNC SYSTEM Programming and Operation Manual

Tool path using tool radius compensation

Workpiece

Machined part figure

Tool

Fig.1-6-2-1

If diameters of tools are stored in the CNC tool compensation list, the tool can be moved by tool radius apart from the machining part figure by calling different radius compensation according to program. This function is called tool radius compensation.

1.7 Tool movement range——stroke

The travel limit switches are fixed at the positive and negative maximum stroke of the machine X, Y, Z axis respectively. If the overtravel occurs, the moving axis slows down and stops after it touches the limit switch. And the overtravel alarm is issued. This function is usually called hardware limit.

The parameter setting can specify the safe tool running range, if the tool exceeds the range, the system stops all the axes moving with overtravel alarm given. This function is called stroke verification, namely, the software limit.

Fig. 1-7-1

GSK218M CNC SYSTEM Programming and Operation Manual

2 Part Program Composition

2.1 Program composition

A program is composed by many blocks which are formed by words. The blocks are separated by the end code (LF for ISO,CR for EIA). In this manual the end code is represented by “；”character.

O00002 N00180

EOB CODE

BLOCK

PROGRAM

END

S0000 T0100

PROGRAM

NAME

SEQUENCE

NO.

ADD: Ln：2

PROGRAM

O00002;

N60 X100 Y0； N120 X0；

N180 G01 X50 Y50 F2000 ；

N240 G41 X100 D1；

N300 G01 Y100；

N360 G02 X200 R50； N420 G01 Y0 F2500； N480 X0；

N540 M30；

WORD

EDIT

【◆PRG】

Fig. 2-1-1 Program structure

The set instructions to control the CNC machine tool to machine the parts are called program.

After the program edited is entered into the CNC system, the system controls the tool to move

【CUR

MOD】【DIR】【MDI】

【CUR/NXT】

along straight line, arc or make the spindle run or stop by these instructions. And the instructions should be edited by the machine actual movement sequence. The program structure is shown in Fig.2-1-1.

2.1.1 Program name

In this system the system memory may store many programs. In order to differentiate these programs, address O with five figures behind it is headed in the beginning of the program. And it is shown in Fig. 2-1-1-1.

Fig. 2-1-1-1 Program name composition

GSK218M CNC SYSTEM Programming and Operation Manual

2.1.2 Sequence number and block

A program is consisted by many instructions, and an instruction unit is called block (see Fig.

2-1-1). The blocks are separated by program end code (see Fig. 2-1-1). In this manual the block end code is represented by character“；”.

Address N with 4 figures sequence number behind it can be used at the beginning of the block (see Fig. 2-1-1), and the leading zero can be omitted. The sequence of the sequence number (insertion set by bit parameter No. 0 # 5) can be arbitrary, and the intervals between them can be inequal (set by Parameter P210). Sequence number can be either in all blocks, or in some important blocks. But by common machining sequence, the number should be arranged by ascending. That the sequence number is placed in important part of the program is for convenience. (e.g. in tool changing, or worktable indexed to a new plane).

2.1.3 Instruction word

Word is a factor to block composition. It is formed by an address and figures behind it

(sometimes +, - added before figures)

Fig.2-1-3-1 Word composition

The address is a character from English alphabetic table which defines the meaning of the

figure behind it. In this system, the usable addresses and their meaning as well as value range are

shown as Table2-1-3-1:

Sometimes an address has a different meaning for different preparatory function.

If 2 or more identical addresses appear in an instruction, the alarm for it will be set by

parameter N0. 32#6.

Table 2-1-3-1

Address Range Meaning

O N G

-99999.999～99999.999（mm）

0.001～9999.999（s） Dwell time

-99999.999～99999.999（mm） Y coordinate address

-99999.999～99999.999（mm）

0～99999 0～99999

00～99

Program name Sequence number Preparatory function X coordinate address

Z coordinate address Arc radius/angle displacement R level in canned cycle Arc center vector in X axis relative to start point

GSK218M CNC SYSTEM Programming and Operation Manual

Address Range Meaning

-99999.999～99999.999（mm）

0～99999（mm/min）

0.001～500(mm/r)

0～99999（r/min）

00～04

0～9999

00～99

1～99999.9999（ms）

1～99999

-99999.9999 ～ 99999.9999 （mm）

01～99

00～256 00～256

Arc center vector in Y axis relative to start point Arc center vector in Z axis relative to start point Feed in a minute Feed in a revolution Spindle speed Multi-gear spindle output Tool function Miscellaneous function output, program executing process, subprogram calling Dwell time Subprogram number calling Cutting depth or hole bottom offset in canned cycle Operator for G65 Length offset number Radius offset number

Special attention should be paid that the limits in table 2-1-3-1 are all for CNC device, but not

for machine tool. Therefore, programming should be done on a basis of good understanding of the

programming limitation of machine builder manual besides this manual.

2.2 General structure of a program

The program is classified for main program and subprogram. Generally, the CNC system is

acutated by the main program. If the main program contains the subprogram call, the CNC system

acts by the subprogram. If the subprogram contains the instruction of returning to main program,

the CNC system returns to the main program to go on execution. The program execution sequence

is shown as Fig.2-2-1.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig.2-2-1 Program execution sequence

The structure of the subprogram is same as that of the main program.

If there are fixed sequence blocks occurring repeatedly in a program, it can be taken as a subprogram which can be stored in the memory in advance with no need to be edited repeatedly. So it can simplify the program. The subprogram can be called in Auto mode, usually by M98 in the main program. And the subprogram called can also call other subprograms. The subprogram called from the main program is called the 1

level subprogram. 4 levels subprogram at most can be called in a program (Fig.2-2-2). The last block in the subprogram must be the returning instruction M99. After M99 execution, the control returns to next block following the block that calls the subprogram in the main program to go on execution. If the main program end is M99, the program execution can be repeated.

Fig. 2-2-2 Two-level subprogram nesting

A single subprogram call instruction can be continuously and repeatedly used to call a

subprogram up to 9999 times.

GSK218M CNC SYSTEM Programming and Operation Manual

2.2.1 Subprogram edit

Write out a subprogram by following format:

Write out the subprogram number behind the address O at the subprogram beginning, and

the M99 instruction at the subprogram end (M99 format as above).

2.2.2 Subprogram call

The subprogram is called out for execution by the main program or the subprogram. The

instruction format is as following:

Fig. 2-2-2-1

● If the repeat time is omitted, the default is 1.

Example M98 P1002L5 ；(It means No.1002 subprogram is continuously called for 5

times.)

● Execution sequence of subprogram call from main program

Subprogram call from subprogram are identical with that from main program.

Note 1、Alarm (PS 078) occurs if subprogram number specified by address P is not found.

2、No. 90000~99999 subprograms are the system reserved programs, if they are

called, they can be executed, and can be displayed.

GSK218M CNC SYSTEM Programming and Operation Manual

2.2.3 Program end

The program begins with program name, ends with M02, M30 or M99 (see Fig.2-1-1-1). For the

end code M02,,M30 or M99 detected in program execution: if M02, M30 specifies the end, the

program finishes and reset; and M30 can be set by bit parameter N0.33#4 for returning to the program

beginning, and M02 can be set by bit parameter N0.33#2 for returning to the program beginning. if

M99 specifies the end, the control returns to the program beginning to restart the program; if M99 、

M02 and M30 is at the end of the subprogram, the control returns to the program that calls the

subprogram and go on executing the following block.

GSK218M CNC SYSTEM Programming and Operation Manual

3 Programming Fundamentals

3.1 Controlled axis

Table 3-1

Item 218M

Basic controlled axes

Extended controlled axes (total) 4 axes

3.2 Axis name

The 3 primary axis names are always X, Y, or Z. And the controlled axes are set by number parameter No.5. The additional axis names are set by number parameter No.6 accordingly, such as A, B, C.

3 axes（X, Y, Z）

3.3 Coordinate system

3.3.1 Machine coordinate system

A special point on machine used as machine benchmark is called machine zero, which is set by the machine builder. The coordinate system set by machine zero taken as origin is called machine coordinate system. It is set up by manual machine zero return after power is on. Once set, it remains unchanged till the power off, system reset or emergency stop.

This system uses right-hand Cartesian coordinate system. The motion along spindle is Z axis motion. Viewed from spindle, the motion of headstock approaching the workpiece is negative Z axis motion, and departing for positive. The other directions are determined by right-hand Cartesian coordinate system.

3.3.2 Reference point

There is a special point on CNC machine tool for tool change and coordinate system setup, which is called reference point. It is a fixed point in machine coordinate system set by machine builder. By reference point return, the tool can easily move to this position. Generally this point in CNC milling system coincides with the machine zero, while the reference point of Machine Center is usually the tool change point.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 3-3-2-1

There are two methods to traverse the tool to reference point:

1. Manual reference point return (see“Manual reference point return”in Operation Manual )

2. Auto reference point return

3.3.3 Workpiece coordinate system

The coordinate system used for workpiece machining is called workpiece coordinate system

(or part coordinate system), which is preset by CNC system （to set workpiece coordinate system）。

Fig.3-3-3-1

In order to make the tool to cut the workpiece to the figure on drawing by instruction program according to drawing in the workpiece coordinate system specified by CNC, the relation of the machine coordinate system and the workpiece coordinate system must be determined.

The method to determine the relation of these two coordinate systems is called alignment. It

can be done by different methods such as part figure, workpiece quantity. .

) By part base pointⅠ ) When part is fixed on jigⅡ

GSK218M CNC SYSTEM Programming and Operation Manual

To align the tool center to the

workpiece base point, specify the workpiece

coordinate system by CNC instructions at

this position, and the workpiece coordinate

system coincides with the programming

coordinate system.

Workpiece coordinate system should be set for each processing program (to select a

workpiece coordinate system). The workpiece coordinate system set can be changed by moving its

origin.

There are two methods to set the workpiece coordinate system:

1. By G92, see 4.2.11 for details.

2. By G code from 54 to 59, see 4.2.8 for details.

Because the tool center can’t be

located at the workpiece base point, locate

the tool to a position (or reference point)

that has a distance to the base point, set

the workpiece coordinate system by this

distance(e.g. G92)

3.3.4 Absolute programming and relative programming

There are absolute and relative definitions to define the axis moving. The absolute definition

is the method of programming by the axis moving final point, which is called absolute

programming. The relative definition is the method of programming by the axis moving, which is

called relative programming (call incremental programming).

1) Absolute coordinate

It is the target position coordinate in the specified workpiece coordinate system, namely the

position the tool to move to.

Fig.3-3-4-1

Move the tool from point A to point B, using the B coordinate in G54 workpiece coordinate

system, the instruction is as following:

G90 G54X10 Y30 Z20 ；

GSK218M CNC SYSTEM Programming and Operation Manual

2) Incremental coordinate

It is the target position coordinate relative to the current position by taking the current

position as the origin.

Fig.3-3-4-2

For traversing the tool from point A to point B, the instruction is as following:

G0 G91 X-40 Y-30 Z-10；

3.4 Mode and non-mode

The mode means that the address value set by a block is effective till it is reset by another

block. Another significance of it is that if a functional word is set, it doesn’t need to be input again if it

is used in the following blocks.

¾ e.g. for following program:

G0 X100 Y100； (rapid positioning to the location X100 Y100)

X20 Y30； (rapid positioning to the location X120 Y30, G0 specified by mode can be

omitted)

G1 X50 Y50 F300； (interpolate to location X50 Y50 by straight line with the feedrate

300mm/min G0→G1 )

X100； (interpolate to location X100 Y50 by straight line with the feedrate 300mm/min ,

G1, Z50,F300 are all specified by mode and can be omitted )

G0 X0 Y0； (rapid positioning to the location X0 Y0)

The initial state is the default state after the system power-on. See table 4-1.

¾ For following program:

O00001

X100 Y100； (rapid positioning to the location X100 Y100, G0 is the initial state)

G1 X0 Y0 F100； (interpolate to location X0 Y0 by straight line with the feedrate

100mm/min, G98 is the initial power-on state )

Non-mode means that the relevant address value is effective only in the block contains

this address, if it is used in following blocks, it must be specified again. e.g. G functional

GSK218M CNC SYSTEM Programming and Operation Manual

instructions of 00 group in Table 4-1.

Refer to Table 3-4 for mode and non-mode description for functional word.

Table 3-4-1 Mode and non-mode for functional instruction

A group of G functions that can be cancelled by each other, once executed, they are effective till they are cancelled by other G functions in the same group. A group of M functions that can be cancelled by each other, once executed, they are effective till they are cancelled by other G functions in the same group. They are only effective in the block they are specified and cancelled at the block end.

They are only effective in the block they are specified.

Mode

Non-mode

Modal G

function

Modal M

function

Non-modal G

function

Non-modal M

function

3.5 Decimal point programming

Numerical values can be entered with a decimal point. A decimal point can be used when

entering a distance, time, or speed. Decimal points can be specified with the following addresses:

X, Y, Z, A, B, C, I, J, K, R, P, Q, and F.

Explanation:

1、 The decimal point programming are set by bit parameter NO：33#1. If bit parameter

NO：33#1=1, the programming value unit is mm, inch, or deg; if bit parameter

NO：33#1=0, the programming value unit is the min. moving unit which is set by bit

parameter NO：5#1.

2、 The decimal part that is less than the min. input incremental unit should be omitted.

Example:

X9.87654； When the min. input incremental unit is 0.001mm, it should be X 9.876.

When the min. input incremental unit is 0.0001mm, it should be X 9.8765.

GSK218M CNC SYSTEM Programming and Operation Manual

4 Preparatory Function: G code

4.1 Classification of G code

Preparatory function is represented by G code with the number behind it, which defines the

meaning of the block that contains it. G codes are devided by the following two types:

Classification Meaning

Non-mode G code Effective in the block in which it is specified

mode G code Effective till another G code of the same group is specified

Example G01 and G00 are mode G code in the same group.

G01 X ＿； Z ＿＿＿； G01 effective X ＿＿＿； G01 effective G00 Z＿＿； G00 effective

Note: Refer to system parameter list for details.

Table 4-1 G codes and their functions

G code Group Instruction format Function

*G00 G00 X_Y_Z_ Positioning (rapid traverse)

G01 G01 X_Y_Z_F_ Linear interpolation(cutting feed) G02 Circular interpolation CW

G03 G04

G10 *G11 *G12

G13 *G15 G15 Polar coordinate instruction cancel

G16

G02 R_ G03

G04 P_ or G04 X_ G10L_；N_P_R_

G11

G12 X_Y_Z_ I_J_K_ G13 X_Y_Z_ I_J_K_

G16

X_Y_

I_J_

F_；

Circular interpolation CCW Dwell, exact stop

Programmable data input Programmable data input cancel Storage stroke detection on Storage stroke detection off

Polar coordinate instruction

*G17

G18

G19

G20 Inch input *G21

Write in with other program in block, used for circular interpolation and tool radius compensation

Specified by a single block at the program beginning before the coordinate system set

XY plane selection ZX plane selection YZ plane selection

Metric input

GSK218M CNC SYSTEM Programming and Operation Manual

G22

G22_X_Y_Z_R_I_L_W_Q_V_D_F_K

G23 G23_X_Y_Z_R_I_L_W_Q_V_D_F_K

CCW inner circular groove rough milling

CW inner circular groove rough milling

G24 G24_X_Y_Z_R_I_J _D_F_K CCW fine milling cycle within a circle

G25 G25_X_Y_Z_R_I_J _D_F_K CW fine milling cycle within a circle

G26

G26_X_Y_Z_R_I_J _D_F_K CCW outer circle fine milling cycle

G27 G27 Reference point return detection

G28 G28 Reference point return

G29 G29 Return from reference point

X_Y_Z_

G30 G30Pn 2nd ,3rd, 4th reference point return

G31

Skip function

G32 G32_X_Y_Z_R_I_J _D_F_K CW outer circle finish milling cycle

G33

G33_X_Y_Z_R_I_L_W_Q_V_U_D_F_K CCW rectangular groove rough

milling

G34 G34_X_Y_Z_R_I_L_W_Q_V_U_D_F_K CW rectangular groove rough milling

G35

G36

G37

G38

G39 00 G39

*G40 G17 X_Y_ Tool radius compensation cancel

G41 G18 X_Z_ Left-hand tool radius compensation

G42

G35_X_Y_Z_R_I_J _L_U_D_F_K CCW inner rectangular groove finish

milling cycle

G36_X_Y_Z_R_I_J _L_U_D_F_K CW inner rectangular groove finish

milling cycle

G37_X_Y_Z_R_I_J _L_U_D_F_K CCW rectangle outside finish milling

cycle

G38_X_Y_Z_R_I_J _L_U_D_F_K CW rectangle outside finish milling

cycle

I_J_； I_J_； J_K_ or G39

Corner offset circular interpolation

G40 G41

G19

G42

Y_Z_ Right-hand tool radius

compensation

G43 G43 Positive tool length compensation

G44 G44 Negative tool length compensation

*G49

G49

Tool length compensation cancel

*G50 G51 Scaling cancel

G51

G53 00 Write into the program

G51 X_ Y_ Z_ P_ Scaling

Machine coordinate system selection

*G54 Workpiece coordinate system 1

G55 Workpiece coordinate system 2

G56 Workpiece coordinate system 3

G57 Workpiece coordinate system 4

Write into the block with other program, usually placed at the program beginning

G58 Workpiece coordinate system 5

G59

Workpiece coordinate system 6

G60 00 G60 X_ Y_ Z_ F_ Unidirectional position

G61 14 G61 Exact stop mode

GSK218M CNC SYSTEM Programming and Operation Manual

G62 G62 Automatic corner override

G63

Tapping mode

*G64 G64 Cutting mode

G65 00 G65 H_P# i Q# j R# k Macro program instruction

G68 G68 X_ Y_ R_ Coordinate system rotation

*G69

G73

G74

G76

G69 Coordinate system rotation cancel

G73 X_Y_Z_R_Q_F_； G74 X_Y_Z_R_P_F_； G76 X_Y_Z_R_P_F_K_；

Peck drilling cycle

Lef-hand tapping cycle

Fine boring cycle

*G80 Write into the block with other program Canned cycle cancel

G81

G82

G83

G84

G85

G86

G87

G88

G89

*G90 Absolute programming

G91

G81 X_Y_Z_R_F_； G82 X_Y_Z_R_P_F_； G83 X_Y_Z_R_Q_F； G84 X_Y_Z_R_P_F_； G85 X_Y_Z_R_F_； G86 X_Y_Z_R_F_； G87 X_Y_Z_R_Q_P_F_； G88 X_Y_Z_R_P_F_； G89 X_Y_Z_R_P_F_；

Write into the block with other program

Drilling cycle(spot drilling cycle)

Drilling cycle (counter boring cycle)

Peck drilling cycle

Tapping cycle

Boring cycle

Drilling cycle

Back boring cycle

Boring cycle

Incremental programming

G92 00 G92 X_Y_Z_ Coordinate system set

*G94

G95

G96

*G97

*G98

G99

G94

Feed per minute

G95 Feed per revolution

G96S_ Constant surface speed control

（cutting speed）

G97S_ Constant surface speed control

cancel（cutting speed）

Write into the block with other program

Return to initial point in canned cycle

Return to point R level (in canned cycle)

Note：1、If modal instruction and non-modal instruction share the same block, the

non-modal instruction is in priority, and the corresponding mode should be

changed according to the other modal instructions in the block, but the modal

instructions are not executed .

2、For the G code with * sign, when the power is switched on, the system is in the

state of this G code.

3、G codes except G10, G11 in 00 group are all non-modal G code.

4、Alarm occurs if G code not listed in this table is used or G code without the

GSK218M CNC SYSTEM Programming and Operation Manual

selection function is specified.

5、G codes from different groups can be specified in a block, but 2 or more G codes

from the same group can’t be specified in a block, otherwise alarm or tool

abnormity occurs.

6、If G codes from 01 group and 09 group share the same block, the G code from 01

group will be taken. In canned cycle mode, if G code from 01 group is specified,

the canned cycle will be cancelled automatically and the system turns into G80 state.

7、G codes are represented by group numbers repectively according to their types.

All G codes can be cleared by bit parameter No.35#0~7 and No.36#0~7 setting at

system reset and emergency stop.

8、if rotation scaling instruction and the instruction of 01 group or that of 09 group

share the same block, the rotation scaling instruction will be taken, and the 01

group or 09 group modes should be changed. If the rotation scaling instruction

and instruction of 00 group share the same block, alarm occurs.

4.2 Simple G code

4.2.1 Rapid positioning G00

Format: G00 X_Y_Z_

Function: G00 instruction moves the tool to the position in the workpiece system specified with

an absolute or an incremental instruction at a traverse speed by linear interpolation.

It is set by bit parameter NO:12#1 and uses the following two paths.( Fig. 4-2-1-1).

1． Linear interpolation positioning: The tool path is the same as linear interpolation（G01）.

The tool is positioned within the shortest possible time at a speed not more than the

traverse speed of each axis.

2． Nonlinear interpolation positioning: The tool is positioned with the traverse speed of each

axis respectively. The tool path is usually not straight.(the positioning is efficient ).

Fig. 4-2-1-1

Explanation:

1 After G00 is executed, the system changes the tool current move mode for G00

2 The tool doesn’t move if positioning parameter is not specified, and the system only

3 G00 are identical with G0.

4 G0 speed for X, Y, Z axis is set by number parameter P88~P92.

Restrictions

The traverse speed is set by parameter, if F is specified in G0 instruction，it is used for the

following cutting feedrate. For example:

G0 X0 Y10 F800； rapid traversing by system parameter set

G1 X20 Y50； by F800 feedrate

The rapid feedrate is adjusted by the key on operator panel with following override : F0，

25， 50， 100%, see Fig. 4-2-1-2. The speed for F0 is set by number parameter P93, and

they are used by all axes.

GSK218M CNC SYSTEM Programming and Operation Manual

mode. The G00 (parameter value is 0) or G01 (parameter value is 1) default mode

can be set by bit parameter No.031#0 while the power is switched on.

change the current tool move mode for G00.

Fig. 4-2-1-2 Rapid feedrate override key

Note: Attention for the positions of the workpiece and worktable when programming

should be paid to protect against tool collision.

4.2.2 Linear interpolation G01

Format: G01 X_ Y_ Z_ F_

Function: The tool moves along a line to the specified position at the feedrate (mm/min)

specified by parameter F.

Explanation:

1 X_ Y_ Z_ are the final point coordinate which concerns the coordinate system, refer to

3.3.1～3.3.3 sections.

2 The feedrate specified by F is effective till the new F code is specified. The feedrate by

F code is got by an interpolation along a line, if F code is not specified in program, the

feedrate uses the default value when the power is on.(see number parameter P87 for

the setting)

Program example (see Fig. 4-2-2-1)

GSK218M CNC SYSTEM Programming and Operation Manual

G01 X200 Y100 F200 ；

Note： Each axis feedrate is as following：

G01 Xα Yβ ZγFf ； In this block：

Feedrate in X axis：

Feedrate in Y axis：

Feedrate in Z axis：

L =

Fig. 4-2-2-1

Note: 1、 The instruction parameters except F are all positioning parameter. And the

upper limit of the feedrate F can be set by number parameter P94. If the actual

federate (using override) exceeds the upper limit, it is restricted to the upper

limit and its unit is mm/min. The lower limit of the feedrate F can be set by

number parameter P95. If the actual federate (using override) exceeds the

lower limit, it is restricted to the lower limit and its unit is mm/min.

2、 If the positioning parameter behind G01 is not specified, the tool doesn’t move,

and the system only changes the tool current mode for G 01 mode. The

system default mode at power-on can be set for G00 (value is 0) or G01 (value

is 1) by altering the system bit parameter NO:31#0.

4.2.3 Circular (helical) interpolation G02/G03

A Circular interpolation G02/G03

Prescriptions for G02 and G03:

The plane circular interpolation means that the arc path is to be finished by the specified

rotation and radius or circle center from the start point to the end point in the specified plane.

Because the arc path can’t be defined only by the start point and the end point, other

conditions are needed:

¾ Arc rotation direction（G02，G03） ¾ Circular interpolation plane（G17, G18, G19）

GSK218M CNC SYSTEM Programming and Operation Manual

¾ Circle center coordinate or radius, which gives two programming format: Circle center

coordinate I, J ,K or radius R programming

Only the three points above are all confirmed, could the interpolation operation be done

in coordinate system.

The circular interpolation can be done by the following instructions to make the tool to go

along an arc, it is shown as follows:

Arc in XY plane

G02 R_

G17

X_Y_

G03

F_；

I_J_

Arc in ZX plane

G02 R_

G18

X_Z_

G03

F_；

I_K_

Arc in YZ plane

G02 R_

G19

Y_Z_

G03

F_；

J_K_

Table 4-2-3-1

Item Content Instruction Description

G17 Arc specification on XY plane

1 To specify plane

G18 Arc specification on ZX plane

G19 Arc specification on YZ plane

To specify rotation

direction

G90

End position

G91

Distance from start point

to circle center

Two axes of X,Y, Z

Two axes of I,J, K

G02 CW

G03 CCW

End point coordinate in

axis

workpiece coordinate system

Coordinate of end point

axis

relative to start point

Coordinate of circle center

axis

relative to start point

Arc radius R Arc radius

5 Feedrate F Arc tangential speed

CW and CCW mean the directions viewed from the positive Z(or Y, Z) axis to the negative

in the right-hand Cartesian coordinate system regarding to XY ( or ZX, YZ)plane , as shown in Fig.

4-2-3-1.

GSK218M CNC SYSTEM Programming and Operation Manual

G03

G02

G17

G02

G03

G18

Fig. 4-2-3-1

G03

G02

G19

The default plane mode at power-on can be set by bit parameters NO:31#1, #2, #3.

The arc end point can be specified by parameter words X, Y, Z. It is an absolute value in G90, an incremental value that is a coordinate of the end point relative to the start point in G91. The circle center is specified by parameter words I, J, K, corresponding to X, Y, Z respectively. Either in absolute mode G90, or in incremental mode G91, parameter values of I, J, K are coordinates of circle center relative to the arc start point (for simplicity, the circle center coordinate when taking the start point as origin). They are incremental values with signs. See Fig. 4-2-3-2.

End point (X,Y)

End point (Z,X)

End point (Y,Z)

Start pointStart point

Center

Fig. 4-2-3-2

I, J, K are assigned with sign according to the circle center relative to the start point. The

circle center can also be specified by radius R besides I, J, K.

G02 X_ Y_ R_ ； G03 X_ Y_ R_ ；

1 Two arcs can be drawn out as following, one arc is more than 180°, the other one is

less than 180°. The radius of the arc more than 180° should be specified by a negative value.

(e.g. Fig. 4-2-3-3) as arc is less than 180° ①

G91 G02 X60 Y20 R50 F300 ；

Start point

as arc is more than 180°②

G91 G02 X60 Y20 R-50 F300 ；

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-3-3

2 The arc equal to 180° can be programmed either by I, J, K, or by R.

Example： G90 G0 X0 Y0；G2 X20 I10

Equal to G90 G0 X0 Y0；G2 X20 R10

F100；

F100

or G90 G0 X0 Y0；G2 X20 R- 10 F100

Note For the arc 180°, the positive or negative value of R doesn’t affect the arc path.

3 The arc equal to 360° can only be programmed by I, J, K.

(Program example)

Fig. 4-2-3-4

The tool path programming for Fig. 4-2-3-4 is as following:

1． Absolute programming

G90 G0 X200 Y40 Z0；

G3 X140 Y100 R60 F300；

GSK218M CNC SYSTEM Programming and Operation Manual

G2 X120 Y60 R50；

G0 X200 Y40 Z0；

G90 G3 X140 Y100 I-60 F300；

G2 X120 Y60 I-50；

2． Incremental programming

G0 G90 X200 Y40 Z0；

G91 G3 X-60 Y60 R60 F3000；

G2 X-20 Y-40 R50；

G0 G90 X200 Y40 Z0；

G91 G3 X-60 Y60 I-60 F300；

G2 X-20 Y-40 I-50；

Restriction

1. If address I, J, K and R are specified together in program, the arc specified by R is in priority

and others are ignored.

2. If both arc radius parameter and the parameter from the start point to the circle center are not

specified, error message will be issued by system.

3. If the circle is to be interpolated, only the parameters I, J, K from start point to circle center but

the parameter R can be specified.

4. Attention should be paid to the coordinate plane selection when the circular interpolation is

being done.

5. If X, Y, Z are all omitted, i.e. the start point and the final point coincides, as well as R is

specified (e.g. G02R50), the tool doesn’t move.

B Helical interpolation

Format:

G02/G03

Fig. 4-2-3-5

Function: It is used to move the tool to a position specified from current position by a feedrate

specified by parameter F in a helical path.

Explanation:

GSK218M CNC SYSTEM Programming and Operation Manual

Tool path

The feedrate along the circumference of two

circular interpolated axes is the specified feedrate

Fig. 4-2-3-6

The first two bits of the instruction parameter are positioning parameter. The parameter words are the two axes name (X, Y or Z) in current plane. These two positioning parameters specify the position the tool is to go to. The third parameter word of the instruction parameter is a linear axis except the circular interpolation axis. Its value is the helical height. The significance and restriction for other instruction parameters are identical with circular interpolation.

If the circle can’t be machined by the system specified instruction parameter, the system will give error message. And the system changes the current tool moving mode for G02/G03 mode.

Feedrate along the two circular interpolation axes are specified

A moving axis that is not circular interpolation axis is added as for the instruction method, and F instruction specifies the feedrate along an arc. So the feedrate of this linear axis is as following:

The feedrate should be ensured that the linear axis feedrate are not beyond any limit.

Restriction Attention should be paid to the coordinate plane selection set when the helical

interpolation is being done.

4.2.4 Absolute/ incremental programming G90/G91

Format: G90/G91 Function: There are 2 instructions for axis moving, the absolute instruction and the incremental

instruction. The absolute instruction is a method of programming by the axis moving end point coordinate, which is concerned with coordinate system. Refer to section

3.3.1～3.3.4.

The incremental instruction is a method of programming by the axis relative moving.

GSK218M CNC SYSTEM Programming and Operation Manual

The incremental value is irrelevant with the coordinate system concerned, it only uses moving direction and distance of the end point relative to the start point.

The absolute instruction and the incremental instruction are specified by G90 and G91 respectively.

Fig. 4-2-4-1

For the moving from start point to end point in Fig. 4-2-4-1, the programming by absolute instruction G90 and incremental instruction G91 are as follows: G90 G0 X40 Y70；

or G91 G0 X－60 Y40 ；

The action can be performed by both programming methods that can be expediently used by operator.

Explanation:

¾ No instruction parameter. It can be written into the block with other instructions. ¾ G90 and G91 are the same group mode, i.e. if G90 is specified while G91 not, the mode is

G90(default). If G91 specified while G90 not, the mode is G91.

System parameter

G90 mode ( parameter is 1) or G91 ( parameter is 1) mode specified for the default

positioning parameter at power-on can be set by bit parameter NO：31#4.

4.2.5 Dwell(G04)

Format: G04 X_ or P_ Function: The dwell is executed by G04, and the execution of next block is delayed by the time

specified. In addition, a dwell can be specified to make an exact stop check in cutting mode G64.

G04

0～9999.999

0～99999.9999

X for second P for millisecond

Explanation:

1 G04 is non-modal instruction, which is only effective in current line. 2 If parameters X, P both appear, parameter X is effective. 3 Alarm occurs if X, P value is set for negative. 4 Exact stop is executed if neither X nor P is specified.

GSK218M CNC SYSTEM Programming and Operation Manual

4.2.6 Unidirectional positioning (G60)

Format: G60 X_ Y_ Z_ F_

Overrun

Dwell

Start point

End point

Fig. 4-2-6-1

Function: For accurate positioning to eliminate machine backlash, G60 can be used for

accurate positioning in a direction.

Explanation:

Dwell

G60 is non-modal code（the modal value can be set by bit parameter NO. 48#0）, which is

only effective in a specified block.

For parameter X, Y, Z, they represent the end point coordinate in absolute programming; and

moving distance of tool in incremental programming.

When using unidirectional positioning in tool offset, the path of unidirectional positioning is the

tool compensation path.

The overrun marked in above figure can be set by system parameter P335，P336，P337，P338，

P339, and the dwell time can be set by parameter P334. The positioning direction can be

defined by the set positive or negative overrun, refer to system parameter for details.

Example 1:

G90 G00 X-10 Y10;

G60 X20 Y25; (1)

If the system parameter P334 = 1, P335 = -8, P336 = 5；as for statement (1), the tool path is

AB→dwell for 1s→BC

C(20,25)

A(-10,10)

—10 0

10 20 30

Fig. 4-2-6-2

B(28,20)

Dwell for 1s

System parameter:

GSK218M CNC SYSTEM Programming and Operation Manual

P334

P335

P336

P337

P338

P339

Dwell time of unidirectional positioning （unit：mm） Overrun and unidirectional positioning direction in X axis（unit：mm） Overrun and unidirectional positioning direction in Y axis（unit：mm） Overrun and unidirectional positioning direction in Z axis（unit：mm） Overrun and unidirectional positioning direction in 4th axis（unit：mm） Overrun and unidirectional positioning direction in 5th axis（unit：mm）

4.2.7 System parameter online modification (G10)

Function: It is used to set or modify the values of radius, length offset, external zero offset,

workpiece zero offset, additional workpiece zero offset, number parameter, bit

parameter and so on in program.

Format:

G10 L50 N_P _R_； Set or modify bit parameter G10 L51 N_ R_； Set or modify number parameter G11； Parameter input mode cancel

Parameter definition:

N： Parameter number. Sequence number to be modified.

P： Parameter bit number. Bit number to be modified.

R： Value. Parameter value after it modified.

The values can also be modified by following instructions, refer to relative sections for details: G10 L2 P_X_Y_Z_A_B_; Set or modify external zero offset or workpiece zero offset G10 L10 P_R_; Set or modify length offset G10 L11 P_R_; Set or modify length wear G10 L12 P_R_; Set or modify radius offset G10 L13 P_R_; Set or modify radius wear G10 L20 P_ X_Y_Z_A_B_; Set or modify additional workpiece zero offset

Note:

1、In parameter input mode, except annotation statement, other NC statement can’t be

specified.

2、G10 must be specified in a single block or the alarm occurs. It should be noted that

the parameter input mode must be cancelled by G11 for after G10 for program

normal use.

3、The parameter value modified by G10 must be within the system parameter range. If

GSK218M CNC SYSTEM Programming and Operation Manual

not, alarm occurs. 4、The canned cycle mode must be cancelled prior to G10 execution, or alarm occurs. 5、Those parameters above the user level and effective by restarting after power-off

can not be modified by G10.

4.2.8 Workpiece coordinate system G54～G59

Format: G54～G59 Function: It specifies the current workpiece coordinate system. It is used to select workpiece

coordinate system by specifying workpiece coordinate system G code in program.

Explanation:

1. No instruction parameter.

2. 6 workpiece coordinate systems can be set in the system, any of which can be selected

by G54~G59 instruction.

3. G54 (workpiece coordinate system 1) is selected automatically by system after machine zero return at power-on. The absolute position on displayer is the coordinate set in G54 coordinate system.

G54 ---------------- Workpiece coordinate system 1 G55 ---------------- Workpiece coordinate system 2 G56 ---------------- Workpiece coordinate system 3 G57 ---------------- Workpiece coordinate system 4 G58 ---------------- Workpiece coordinate system 5 G59 ---------------- Workpiece coordinate system 6

4. When different workpiece coordinate system is called by block, the axis for move by

instruction will be located in the new workpiece coordinate system; for the coordinate of the axis not move, it turns to the corresponding coordinate in the new workpiece coordinate system and the actual machine position doesn’t alter.

e.g. The corresponding machine coordinate for G54 coordinate system origin is （10,10,10）.

The corresponding machine coordinate for G55 coordinate system origin is （30，30，30）. When the program is executed by sequence, the absolute coordinate and the machine

coordinate of the end point are shown as follows:

Table 4-2-8-1

Program Absolute coordinate Machine coordinate

G0 G54 X50 Y50 Z50 50，50，50 60，60，60

G55 X100 Y100 100，100，30 130，130，60

X120 Z80 120，100，80 150，130，110

5. The external workpiece zero offset or workpiece zero offset can be altered by G10, which is

GSK218M CNC SYSTEM Programming and Operation Manual

shown as follows: By instruction G10 L2 Pp X_Y_Z_ P=0 ： External workpiece zero offset P=1 to 6 ： Workpiece zero offset of workpiece coordinate system from 1 to 6 X_Y_Z_ ： For absolute instruction（G90）, it is workpiece zero offset of each

axis

For incremental instruction（G91）, it is workpiece zero offset set

plusing each axis(the result is the new workpiece zero offset).

By G10 instruction, each coordinate system can be altered respectively.

Workpiece coordinate

system 1 （G54）

Machine zero

Machine coordinate origin

Workpiece coordinate

system 2

（G55）

Workpiece coordinate

system offset

Machine reference point

Fig. 4-2-8-1

Workpiece coordinate

system 3 （G56）

Workpiece coordinate

system 4 （G57）

Workpiece coordinate

system 5 （G58）

Workpiece coordinate

system 6

（G59）

As shown in Fig. 4-2-8-1, after power-on, the machine returns to machine zero by manual zero return. The machine coordinate system is set up by machine zero with the machine reference point generating and workpiece coordinate system to be defined. The corresponding values of offset number parameter P10～14 in workpiece coordinate system are the integral offset of the 6 workpiece coordinate system. The 6 workpiece coordinate system origins can be specified by coordinate offset input in MDI mode or set by number parameter P15～44. These 6 workpiece coordinate systems are set up by the distances from machine zero to each coordinate system origin.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-8-2

Example：

N10 G55 G90 G00 X100 Y20；

N20 G56 X80.5 Z25.5；

For the example above, when N10 block is being executed, it rapidly traverses to a position

（X=100，Y=20）in

When N20 block is being executed, the absolute coordinate value automatically turns to the

coordinate value （X=80.5，Z=25.5）in G55 workpiece coordinate system for rapid positioning.

G55 workpiece coordinate system.

4.2.9 Additional workpiece coordinate system

Except 6 workpiece coordinate systems (from G54 to G59), 50 additional workpiece coordinate systems can be used. Format: G54 Pn Pn: specified additional workpiece coordinate system code Range ： 1～50

The setting and restriction of the additional workpiece coordinate system are the same as

that of workpiece coordinate system from G54 to G59.

The workpiece zero offset in additional workpiece coordinate system can be set by G10, as

following:

By instruction G10 L20 Pn X_Y_Z_

n=1 to 50： Additional workpiece coordinate system code

X_Y_Z_ ： Set axis address and offset value for workpiece zero offset.

For absolute instruction (G90), the value specified is the new offset

value.

For incremental instruction (G91), the new offset value can be got by

adding the value specified to the current offset value.

By G10 instruction, each workpiece coordinate system can be changed respectively.

When the P address of the additional workpiece coordinate and the other instructions containing P address are in a same block, they share this P address together.

GSK218M CNC SYSTEM Programming and Operation Manual

4.2.10 Machine coordinate system selection G53

Format: G53 X_ Y_ Z_

Function: To rapidly position the tool to the corresponding coordinate location in the machine

coordinate system.

Explanation:

1 While G53 is used in program, the instruction coordinate behind it should be the

coordinate in the machine coordinate system and the machine will rapidly position to the location specified.

2 G53 is a non-modal instruction, which is only effective in block containing it, and it

doesn’t affect the coordinate system defined before.

Restriction

Machine coordinate system selection G53

When the position in the machine coordinate system is specified, the tool rapidly traverses

to this position. The G53 used for selecting machine coordinate system is a non-modal G code,

which is only effective for the block specifying the machine coordinate system. Absolute G90

should be specified for G53; if G53 is specified in incremental mode (G91), G91 is neglected

(G53 is still in G90 mode without changing G91 mode). The tool can be specified to move to a

special position, e.g. G53 can be used in program to position the tool to the tool changing point.

After power on

Machine coordinate system must be set before G53 is specified after power on. Therefore,

manual reference point return must be performed after power on(zero return in manual mode)

or auto reference point return must be performed specified by G28. If an absolute position

encoder is used, this operation is unneeded.

Note: when G53 is specified, the tool radius compensation and tool length offset are cancelled

temporarily and they will be restored in the next block.

4.2.11 Floating coordinate system G92

Format: G92 X_ Y_ Z_

Function: It is used to set floating workpiece coordinate system. The current tool absolute

coordinate values in the new workpiece coordinate system are specified by 3

instruction parameters. And this instruction doesn’t’ result in the axis movement.

GSK218M CNC SYSTEM Programming and Operation Manual

Explanation:

G92 floating coordinate system

Machine zero

Machine coordinate origin

Fig. 4-2-11-1

1、 As the figure shows, the origin of the G92 floating coordinate system is the value in

machine coordinate system, which is irrelevant to the workpiece coordinate system, it can

be set up after the machine zero return.

G92 setting is effective in the following conditions:

1) Before system power off

2) Before workpiece coordinate system is called

3) Before machine zero return

The G92 floating coordinate system is usually used for the alignment of temporary

workpiece machining and it will be lost after the power is off. And G92 is usually used at

the program beginning or specified in MDI mode before the program auto run.

2、 There are two methods for defining the floating coordinate system:

（1）By tool nose:

Fig. 4-2-11-2

As fig. 4-2-11-2 shows, for G92 X25 Z23，take the position the tool nose locates at as the

point（X25， Z23）in the floating coordinate system,

（2）By a fixed point in the arbor as a basic point:

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-11-3

As Fig. 4-2-11-3 shows, specify the workpiece coordinate system by block “G92 X600

Y1200”(by a basic point in the arbor as a start point). Regarding a basic point as the start point, if

the motion is specified by the absolute value in the program, the basic point is moved to the

specified position and it must be added the tool length compensation value, which is the

difference of the basic point to the tool nose.

Note： 1 If G92 is used for coordinate system setting in tool offset, the coordinate system

is the one set by G92 as to the tool length compensation without the offset

value added.

2 For tool radius compensation, the tool offset should be cancelled if G92 is

used.

Restriction

After floating coordinate system is set, the 1

canned cycle instruction should be in a

complete format, or the tool move will be wrong.

4.2.12 Plane selection G17/G18/G19

Format: G17/G18/G19

Function: For circular interpolation, tool radius compensation, drilling or boring, plane

selection is needed, which can be selected by G 17/G18/G19.

Explanation:

It has no instruction parameter. The system default at power-on is G17 plane if parameter is

not specified. It can also be set by bit parameter NO.31#1, #2, #3. The relation of the instruction

and the plane is as following:

G17-------------XY plane

G18-------------ZX plane

G19-------------YZ plane

GSK218M CNC SYSTEM Programming and Operation Manual

Plane is not changed if G17，G18，G19 is not specified in the block.

For example:

G18 X_ Z_； ZX plane

G0 X_ Y_； Plane unchanged (ZX plane)

In addition the moving instruction is irrelevant to the plane selection. e.g. in the following

instruction, Y axis is not in the ZX plane, so the Y axis moving is irrelevant to ZX plane.

G18Y_；

Annotation: Only the canned cycle in G17 plane is available in this system at present. For

criterion or astringency, plane should be expressly defined in the corresponding

block, especially in a system used by many users, which can avoid the incident

or abnormity caused by programming error.

4.2.13 Polar coordinate system setup/cancel G16/G15

Format: G16/G15

Function:

G16 is used for the setup of the polar

coordinate system of the positioning parameter.

G15 is used for the cancellation of the polar coordinate system of the positioning parameter.

Explanation:

No command parameter.

If G16 is set, the coordinate can be input by polar coordinate radius and angle. The positive of

angle is the CCW direction of the 1

axis positive direction in a plane selected; while the negative is

CW direction. Both the radius and angle can use the absolute or incremental instructions（G90 ，

G91）.

If G16 is used, the 1

represents the polar radius in polar coordinate system, the 2

axis of the positioning parameter of the tool moving command

axis of that represents the polar

angle in polar coordinate system.

If G15 is specified, the polar coordinate system can be cancelled and the control returns to

the Cartesian coordinate system.

The definition of the polar coordinate system origin:

1 In G90 absolute mode, if G16 is specified, the workpiece coordinate system origin is regarded

as the polar coordinate system origin.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-13-1

2 In G91 incremental mode, if G16 is specified, the current point is regarded as the polar

coordinate system origin.

Example: Bolt hole circle (the workpiece coordinate system zero point is set as the polar

coordinate system origin, selecting X-Y plane)

Fig. 4-2-13-2

z To specify angle and radius by absolute value

G17 G90 G16; To specify polar coordinate system and take the workpiece coordinate system

zero point in X-Y plane as the polar coordinate system origin

G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0; To specify 100mm distance and 30°angle

Y150; To specify 100mm distance and 150°angle Y270; To specify 100mm distance and 270°angle

G15 G80; To cancel the polar coordinate system

To specify angle by incremental value, polar radius by absolute value

G17 G90 G16; To specify the polar coordinate system and take the workpiece coordinate

system zero point in X-Y plane as the polar coordinate system origin

G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0; To specify 100mm distance and 30°angle

G91 Y120;

Y120;

G15 G80;

To specify 100mm distance and 150°angle

To specify 100mm distance and 270°angle

To cancel the polar coordinate system

Moreover, when programming by polar coordinate system, the current coordinate plane setting

should be considered. And the polar coordinate plane and the current coordinate plane are

GSK218M CNC SYSTEM Programming and Operation Manual

relevant. e.g. in G91 mode, if the current coordinate plane is specified by G17, the origin of it is defined by the X,Y axis components of the current tool position. If the current coordinate plane is specified by G18, the origin of it is defined by the Z, X axis components of the current tool position.

Fig. 4-2-13-3

If the positioning parameter of the 1

current position is the default positioning parameter of the hole cycle. The 1

hole cycle after G16 instruction is not specified, the tool

canned cycle

instruction after the current polar coordinate must be complete, or the tool moving will be wrong.

After G16 instruction, except the hole cycle, the words of the positioning parameter for tool moving involves with the special plane selection mode. While the polar coordinate system is cancelled by G15 which followed by a moving instruction, the tool current position is defaulted as the start point of the moving instruction.

4.2.14 Scaling in plane G51/G50

Format:

G51 X_ Y_ Z_ P_ (X、Y、Z: Absolute instruction for scaling center coordinate, P: axis scaling by

a same ratio) … Scaling processing blocks G50 Scaling cancel or G51 X_ Y_Z_ I_ J_ K_（scaling by different ratios （I, J, K）by each axis） … Scaling processing block G50 Scaling cancel

Function:

G51 is used for the programming figure scaling in a same or different ratio by a position

specified as the center. G51 is needed to be specified in a single block and cancelled by G50.

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-14-1 Scaling (P1'P2P3P4→ P1’P2’P3’P4')

Explanation:

1 Scaling center: G51 can be specified with 3 positioning parameters X_Y_Z_, which are

optional. These positioning parameters are used to specify the scaling center of G51. If they are not specified, the tool current position will be specified for the scaling center. Whether the positioning mode is absolute or incremental, the scaling center is specified by the absolute positioning mode. Moreover, in polar coordinate system G16 mode, the parameters in G51 are expressed by Cartesian coordinate system.

Example:

G17 G91 G54 G0 X10 Y10;

G51 X40 Y40 P2; Though in incremental mode, the scaling center means the

absolute coordinate（40,40）in G54 coordinate system

G1 Y90; By incremental mode as for parameter Y

2 Scaling: whether the current mode is G90 or G91, the scaling are always expressed by

absolute mode.

Except specified in program, the scaling can also be specified in parameters. The number

parameters P331~335 correspond to the scaling ratios of X, Y, Z, 4

and 5th respectively. If

no scaling is specified, the number parameter P330 can be used for scaling setting.

If the parameter P or I, J, K value specified are negative, the mirror image is made for the

corresponding axis.

3 Scaling setting: The effectiveness of the X axis scaling is set by bit parameter NO：47#3,

the effectiveness of the Y axis scaling is set by bit parameter NO：47#4, the effectiveness of

the Z axis scaling is set by bit parameter NO：47#5, and the scaling ratio of each axis is set

by bit parameter NO：47#6. (0: instructed with P, 1: instructed with I, J, K.)

4 Scaling cancellation: After the scaling is cancelled by G50 followed by a moving instruction, if

the coordinate rotation is cancelled by default, the current tool position is regarded as the

GSK218M CNC SYSTEM Programming and Operation Manual

start point of this moving instruction.

5 In scaling mode, G codes for reference point return （G27～G30 etc.）and coordinate system

specification（G52～G59 , G92 etc.）can’t be specified. If needed, they should be specified after the scaling is cancelled.

6 Even different scalings are specified for circular interpolation and axes, the ellipse path cann’t

be made by tool.

If the scaling ratios of the axes are different and the circular interpolation are programmed by R, the interpolation figure is shown as Fig. 4-2-14-2, (below the scaling ratio of X is 2, that of Y is 1)

G90 G0 X0 Y100; G51 X0 Y0 Z0 I2 J1; G02 X100 Y0 R100 F500;

Above commands are equivalent to the following one:

G90 G0 X0 Y0 Z0； G02 X200 Y0 R200 F500;

Scaling of radius R depends on I or J which is larger

Scaled shape

（0，0）

Fig. 4-2-14-2 Scaling of circular interpolation 1

（100，0）（200，0）

If the axes scaling ratio are different, and the circular interpolation is programmed by I, J, K. if the arc is failed, alarm for it occures by the system.

7 Scaling is ineffective for the tool radius compensation, tool length compensation and tool offset,

which is shown in Fig. 4-2-14-3.

GSK218M CNC SYSTEM Programming and Operation Manual

Programmed figure

Scaled figure

The tool radius compensation values are not scaled

F i g. 4-2-14-3 Scaling of tool radius compensation

Example for mirror image program: Main program

G00 G90; M98 P9000; G51 X50.0 Y50.0 I1 J-1; M98 P9000; G51 X50.0 Y50.0 I-1 J-1; M98 P9000; G51 X50.0 Y50.0 I-1 J1; M98 P9000; G50; Subprogram O9000 G00 G90 X60.0 Y60.0; G01 X100.0 F100; G01 Y100; G01 X60.0 Y60.0; M99;

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-2-14-4

Restriction

1 The moving scaling of Z axis is ineffective in following canned cycles: 1） The cut-in value Q and retraction value d of peck drilling cycle（G83, G73） 2） Fine boring cycle（G76）. 3） Offset value Q of X axis and Y axis in back boring cycle（G87）.

2 In MANUAL mode, the traverse distance can’t be in creased or de creased by scaling .

Note: 1 The position is displayed by scaling coordinates. 2 The result for an axis performing mirror image in a specified plane is as

following:

1）Circular instruction……………….reverse direction of rotation 2）Tool radius compensation C……….reverse direction of offset 3）Coordinate system rotation…………….reverse direction of rotation angle

4.2.15 Coordinate system rotation G68/G69

A programmed shape can be rotated. When a workpiece comprises some identical shapes, this function can be used for programming by prepairing a subprogram for the shape unit, then calling it by rotation function.

Format:

Function: G68 is used for the programming shape in plane rotating by a center point specified

G17 G68 X_ Y_ R_

or G18 G68 X_ Z_ R_ or G19 G68 Y_ Z_R_

G69

as an origin. G69 is used for cancellation of coordinate system rotation.

GSK218M CNC SYSTEM Programming and Operation Manual

Angle of rotation

Explanation:

1 G68 is an optional parameter with 2 positioning parameters that are used for specifying

the rotation center. If the rotation center is not specified, the tool current position is regarded as the center by system. The positioning parameters are relevant to the current coordinate plane, while X, Y for G17; Z, X for G18; Y, Z for G19.

2 Whether the current positioning mode is absolute or incremental, the rotation center

can only be specified by absolute positioning of Cartesian coordinate system.

G68 can be followed by a command parameter R, the value of the parameter is the angle to be rotated. The positive value is for CCW rotation and the angle unit is degree. If no rotation angle is specified in this function, the angle will be set by number parameter P329.

3 In G91 mode, the rotation angle by increment is set by bit parameter NO: 47#0 (rotation

angle of coordinate system, 0: by absolute instruction; 1: by G90/91 instruction ).

Center of rotation

Fig. 4-2-15-1

4 When the system is in rotation mode, plane selection is not allowed, or errors will be

shown. Attention should be paid in programming.

5 In coordinate system rotation mode, G codes for reference point return （G27～G30

etc.）and coordinate system specification（G52～G59 , G92 etc.）can’t be specified. They should be specified after the scaling is cancelled if needed.

6 After coordinate system rotation, the tool radius compensation, tool length

compensation, tool offset and other compensation operation will be performed.

7 If coordinate system rotation is performed in scaling mode(G51), the rotation center

coordinate values will be scaled. but the rotation angle is not scaled, when the moving instruction is given, the scaling will be executed first, then the coordinate system rotation.

Example 1: Rotation

G92 X-50 Y-50 G69 G17; G68 X-50Y-50 R60;

GSK218M CNC SYSTEM Programming and Operation Manual

G90 G01 X0 Y0 F200; G91 X100; G02 Y100 R100; G3 X-100 I-50 J-50; G01 Y-100; G69 ; M30

Tool path after rotation

Originally programmed tool path

Rotation center

Example 2: Scaling and rotation

G51 X300 Y150 P0.5; G68 X200 Y100 R45; G01 G90 X400 Y100; G91 Y100; X-200; Y-100; X200; G69 G50;

（0，0）

60°

（-50，-50）

Fig. 4-2-15-2

M30

GSK218M CNC SYSTEM Programming and Operation Manual

When scaling and coordinate

system rotation are applied

200

100

100 200 300 400

Example 3 : Repetition of G68

By program (main program)

G92 X0 Y0 Z20 G69 G17; M3 S1000;

When only coordinate system rotation is applied

When only scaling is applied

Cutting progam

Fig. 4-2-15-3

G0Z2 ; G51 X0 Y0 I1.2 J1.2 G42 D01； (offset setting) M98 P2100 (P02100); (subprogram call) M98 P2200L7； (calling for 7 times) G40 G50 G0 G90 Z20; X0Y0 M30;

Subprogram 2200 O2200 G68 X0 Y0 G91 R45.0; (relative rotation angle) G90; M98 P2100; (subprogram O2200 calling subprogram O2100) M99；

Subprogram O2100 O2100 G90 G0 X0 Y-20； (Right-hand tool compensation setup) G01Z－2 F200； X8.284； X14.142 Y-14.142；

M99;

GSK218M CNC SYSTEM Programming and Operation Manual

Programmed path

（0，0）

When offset is applied

（0，-20）

(14.142,-14.142)

(8.284,-20)

subprogram

Fig. 4-2-15-4

4.2.16 Skip function G31

Format: G31 X_Y_Z_ Function: The linear interpolation can be specified like G01 after G31 instruction. During the

execution of G31, the current instruction execution will be interrupted to execute next block if an external skip signal is entered. While the working end point is specified not by programming but by signals from machine, this function can be used (e.g. used for grinding). It can also be used for measuring the workpiece dimensions.

Explanation:

1、 G31 is a non-mode G code that is only effective in a specified block. 2、 Alarm occurs if G31 is given during the tool radius compensation. The tool radius

compensation should be cancelled before G31 in struction .

Example:

The block after G31 is a single axis moving specified by incremental values, as Fig. 4-2-16-1 shows:

Skip signal is input here

100

Fig. 4-2-16-1 A single axis moving specified by incremental values of next block

Actual motion

Motion without skip signal

GSK218M CNC SYSTEM Programming and Operation Manual

The block after G31 is a single axis moving specified by abso lute values, as F ig. 4-2-16-2 shows:

G31 G90 X200 F100; Y100;

Y100

Skip signal is input here

X200

Actual motion

Fig. 4-2-16-2 Single axis moving specified by absolute values of next block

The block after G31 is 2-axis moving specified by absolute values, as Fig. 4-2-16-3 shows:

Skip signal is input here

100

(300,100)

Motion without skip signal

Actual motion

Motion without skip signal

100 200 300

Fig. 4-2-16-3 2-axis moving specified by absolute values of next block

4.2.17 Inch/metric conversion G20/G21

Format: G20： input by inch system

G21： input by metric system

Function: They are used for the inch/metric input conversion in program. Explanation:

1 This function must be specified by a single block at the beginning of the program before

the coordinate system setup.

2 Change the unit of the following item after the inch/metric conversion:

Feedrate specified by F code Position instruction Workpiece zero offset value Tool compensation value

GSK218M CNC SYSTEM Programming and Operation Manual

Scale unit of MPG

Mov i ng di s tanc e i n incremental feeding

The G code status at power-on is the same as that in power-off.

Note： 1 Inch/metric conversion can’t be executed during the program execution.

2 The tool compensation value must be preset by the minimum incremental

input unit when inch system is converted to metric system or the reverse.

3 For the 1

G28 instruction, th e running from the intermediate point is the same as the MANUAL reference point return when inch system is converted to metric system or the reverse.

4 When the minimum incremental input unit is different from the minimum

command unit, the maximum error that is not accumulated is the half of the

minimum command unit . 5 The inch/metric system for program input can be set by bit parameter NO:00#2. 6 The inch/metric system for program output can be set by bit parameter NO:03#0.

4.2.18 Optional angle chamfering/corner rounding

Format: L_：chamfering R_：corner rounding

Function: When the above instruction is added to the end of a block that specifies linear

interpolation（G01）or circular interpolation（G02, G03）, a chamfering or corner rounding is automatically done in the machining. Blocks specifying chamfering and corner rounding can be specified consecutively.

Explanation:

1、 Blocks specifying chamfering and corner rounding can only be inserted between the linear

interpolation blocks.

2、 The chamfer ing after L is used to specify the distance from the virtual corner point to the

start and the end point. The virtual corner point is the corner point that exists if chamfering is not performed. As the following figure shows:

GSK218M CNC SYSTEM Programming and Operation Manual

（1）G91 G01 X100 ,L10; （2）X1 00 Y100;

Inserted charming blcok

Fig. 4-2-18-1

3、 The corner rounding after R is used to specify the radius for corner. As the following figure

shows:

（1）G91 G01 X100 ,R10; （2）X100 Y100;

Center of a circle with radius R

Fig. 4-2-18-2

Restriction

Virtual corner intersection

1 Chamfering and corner rounding can only be performed in the plane specified, and

these functions can’t be performed for parallel axes.

2 If the inserted chamfering or corner rounding block causes the tool to go beyond the

original interpolation move range, alarm is issued. 3 Corner rounding can’t be specified in a threading block。 4 The chamfering and corner rounding value can’t be negative, or alarm is issued.

4.3 Reference point G code

The reference point is a fixed point on a machine tool to which the tool can easily be moved by the reference point return function. There are 3 instructions for reference point as is shown in Fig. 4-3-1-1, the tool can be automatically moved to the reference point via an intermediate point along an axis specified by G28; or from the reference point automatically to a specified point via an intermediate point along a specified axis by G29.

GSK218M CNC SYSTEM Programming and Operation Manual

(3)

R (Reference position)

(2) (4)

(1)

(Intermediate point)

(return to the start point

of reference position)

Fig. 4-3-1

(5)

(return to target point

from reference position)

4.3.1 Reference point return G28

Format: G28 X_ Y_ Z_ Function: It is used for the operation to return to the reference point (a special point on

machine) via an intermediate point.

Explanation: Intermediate point:

An intermediate point is specified by an instruction parameter in G28, which can be expressed by absolute or incremental instructions. During the execution of this block, the coordinate value of the intermediate point of the axis specified is stored that is to be used for the G29(returning from the reference point) instruction.

Note: The coordinate value of the intermediate point is stored in the CNC system. Only

the axis coordinate value specified by G28 is stored each time, for the other axes not specified by G28, the coordinate values specified by G28 before are used. If the intermediate point defaulted by the system is not ensured by user when using G28 instruction, it is better to specify all the axes. Take a consideration by N5 block in the following example 1.

(3)

R (reference position)

(2) (4)

(1)

(5)

Fig. 4-3-1-1

GSK218M CNC SYSTEM Programming and Operation Manual

1 The action of the G28 block can be analyzed as following: （refer to Fig.4-3-1-1）：

(1) Positioning to the intermediate point of the specified axis from the current position (point

A→point B) at a traverse speed.

(2) Positioning to the reference point from the intermediate point (point B →point R) at a

traverse speed.

2 G28 is a non-mode instruction which is only effective in current block.

3 The combined reference point return of a single axis or multiple axes is available in this system.

And the intermediate point coordinate is saved by system during the workpiece coordinate

system change.

Example 1:

N1 G90 G54 X0 Y10； N2 G28 X40 ； Set the intermediate point of X axis for X40 in G54 workpiece coordinate

N3 G29 X30 ； Return to the point (30，10) via point（40,10）from reference point, i.e. target

N4 G01 X20；

N5 G28 Y60 ； Intermediate point(X40，Y60), which is substituted by X40 specified by G28

N6 G55； Due to workpiece coordinate system change, the intermediate point (40，60)

system, and return to reference point via point（40,10）, i.e. reference point

return of single X axis

point return of single X axis

before due to it is not specified in X axis.

Note The intermediate point is not （20，60）.

in G54 workpiece coordinate system is changed for (40，60) in G55

workpiece coordinate system.

N7 G29 X60 Y20； Return to the point (60, 20) via the intermediate point (40，60) in G55

workpiece coordinate system from reference point

The G28 instruction can automatically cancel the tool compensation and this instruction is only used in automatic tool change mode( changing tool at the reference point after reference point return). So the tool radius compensation and tool length compensation should be cancelled

before using this instruction. See the 1

reference point setting in number parameter P45～P49.

4.3.2 2nd, 3rd, 4th reference point return G30

There are 4 reference points in machine coordinate system. In a system without an

absolute-position detector, the

the auto reference point return（ G28） or manual reference point return is performed.

Format:

G30 P3 X_ Y_ Z_； the

G30 P2 X_ Y_ Z_； the 2nd reference point return (P2 can be omitted)

2nd, 3rd, 4th reference point return functions can be used only after

3rd reference point return

GSK218M CNC SYSTEM Programming and Operation Manual

G30 P4 X_ Y_ Z_； the 4

Function: It is used for the operation of returning to the specified point via the intermediate point

specified by G30 from the reference point.

Explanation:

1 X_ Y_ Z_； Instruction for specifying the intermediate point (absolute/ incremental)

The specification and restriction for G30 instruction is the same as G28 instruction.

reference point return

See number parameter P50～64 for the

3 The G30 code can also be used together with G29 code (return from reference

point), whose setting and restriction are identical with G28 code.

2nd, 3rd, 4th reference point setting.

4.3.3 Automatic return from reference point G29

Format:

Function: It is used for the operation of returning to a specified point via the intermediate

Explanation:

1 The action of the G29 block can be analyzed as following: （refer to Fig.4-3-1-1）：

2 G29 is a non-modal instruction which is only effective in current block. Usually return from

G29 X_ Y_ Z_

point specified by G28, G30 from the reference point (or current point).

(1) Positioning to the intermediate point (point R→point B) specified by G28, G30 from the

reference point at a traverse speed.

(2) Positioning to a specified point from the intermediate point (point B →point C) at a

traverse speed.

reference point should be specified immediately after G28, G30 instruction.

3 The optional parameters X,Y and Z in G29 instruction are used for specifying the target point

(i.e. point C in Fig. 4-3-1-1) from the reference point, which can be expressed by absolute or

incremental instruction. The instruction specifies the incremental value from the intermediate

point in incremental programming. If an axis is not specified it means the axis has no moving

relative to the intermediate point. The G29 instruction followed by an axis is a single axis

return with no action taken by other axes.

Example 1

G90 G0 X10 Y10；

G91 G28 X20 Y20； Reference point return via the intermediate point(30，30)

G29 X30； Return to (60，30) from the reference point via the intermediate point(30，

30).

Note: The component in X axis should be 60 in incremental programming.

The intermediate point of G29 instruction is assigned by G28, G30. Refer to G28

explanation for the definition, criterion and system default of the intermediate point.

GSK218M CNC SYSTEM Programming and Operation Manual

4.3.4 Reference point return check G27

Format: G27 X_ Y_ Z_

Function: It is used for the reference point return check; the reference point is specified by

X_ Y_ Z_ (absolute/incremental instruction).

Explanation:

1、 G27 instruction positions the tool at a traverse speed. If the tool reaches the reference

point, the reference point return indicator lights up. However, if the position reached by the

tool is not the reference point, an alarm is issued.

2、 In machine lock mode, even G27 is specified and the tool has automatically returned to the

reference point, the indicator for return completion doesn’t light up.

3、 In an offset mode, the position to be reached by the tool with G27 instruction is the position

obtained by adding the offset. Therefore, if the position with the offset added is not the

reference point, the indicator does not light up, and an alarm is issued. Usually the tool

offset should be cancelled before G27 instruction.

4.4 Canned cycle G code

Canned cycle make it easier for the programmer to creat programs. With a canned cycle, a

machining operation by multiple blocks can be realized by a single block which contains G function.

(In this system only canned cycle in G17 plane is available)

The general process of canned cycle:

A canned cycle consists of a sequence of 6 operations, as Fig. 4-4-1 shows:

Fig. 4-4-1

GSK218M CNC SYSTEM Programming and Operation Manual

Operation 1: Positioning of axes X and Y (may including another axis)

Operation 2: Traverse to point R level

Operation 3: Hole machining

Operation 4: Operation at the bottom of a hole

Operation 5: Retraction to point R level

Operation 6: Traverse to the initial point

The hole machining can be performed in Z axis if positioned in XY plane. It defines that a

canned cycle operation is determined by 3 types. They are all specified by G code.

1) Data type

G90 absolute mode； G91 incremental mode

2) Return point plane

G98 initial level； G99 R level

3) Groove machining type G22、G23、G24、G25、G26、G32、G33、G34、G35、G36、G37、G38。

4) Hole machining type

G73， G74， G76， G81～G89

Initial level and R level

Initial level It is the absolute position where the tool locates in Z axis before the canned

cycle.

R level It is also called safe plane, it is a position in Z axis when the traverse is switched

to the feeding in canned cycle, which is usually positioned at a distance from the

workpiece surface to prevent the tool from colliding with the workpiece and

provide a sufficient distance to finish the acceleration. The instructions of G73/G74 /G76/G81 ～ G89 specify all the data( hole location data, hole

machining data, repetition) , by which a block is constituted.

The format for hole machining is shown as following:

Therein, the significance of the hole location data and machining data is as following Table 4-4-1:

Table 4-4-1

Designation

Hole

machining

Parameter

word

Refer to Table 4-4-3，note the restrictions above。

Explanation

Data for hole

location

Data for hole

machining

GSK218M CNC SYSTEM Programming and Operation Manual

The hole location is specified by absolute value or

X，Y

incremental value and the control is identical to the G00 positioning.

As Fig. 4.4.2(A) shows, the distance from point R level to the hole bottom is specified by incremental value, or the hole

bottom coordinate is specified by absolute value. And the feedrate is the speed specified by F in operation 3; while in operation 5, it is a traverse speed or a speed specified by F code due to the different machining type.

In Fig. 4.4.2(B), the distance from the initial level to point R

level is specified by incremental value or point R level coodinate is specified by absolute value. The speeds in operation 2 and 6 are both traverse.

It is used to specify the cut-in value or the parallel moving value in G76 or G87.

It is used to specify the dwell time at the hole bottom. The canned cycle instruction can be followed by a parameter P_ ,

which specifies the dwell time after the tool reaches the Z plane. The time unit is ms. The min. value of the parameter can be set by number parameter P281, and the max. value by number parameter P282.

F It is used to specify the cutting feedrate.

The repetition is specified in parameter K_, which is effective only in the specified block. It can be omitted and the default is

one time. The max. drilling times are 99999. If a negative value is specified, it executes by absolute values. If zero is specified, the mode is changed without drilling operation.

Restriction

¾ The canned cycle is mode instruction, which is effective till it is cancelled by a G code.

¾ G80 and G codes in 01 group are used for cancelling canned cycle.

¾ The processing data once specified in canned cycle are effective till the canned cycle is

cancelled. Therefore, after all the processing data required for hole machining are specified in the beginning of the canned cycle, only the data to be changed is needed to be respecified in the following canned cycle.

Note

1 The feedrate specified by F remains effective even the canned cycle is cancelled.

2 In single mode, the canned cycle has 3 stage working type, positioning→R level→initial level

3 In canned cycle, the data of hole machining and hole position will be eliminated if the system is

reset. The instance of dada retained and eliminated is shown as following table:

GSK218M CNC SYSTEM Programming and Operation Manual

Table 4-4-2

No.

① ②

Designation of

data

G00X-M3； G81X-Y-Z-R-F-；

Specify values for Z, R, F in the beginning.

Explanation

G81，Z-R-F- can be omitted due to the identical hole

Y-；

③

machining mode and data specified in ②. Drill the hole for the length Y once by G81.

④

G82X-P-；

Move in X axis relative to hole . Do the hole machining ③ by G82 and data Z，R，F specified in and P in . ②④

⑤ G80X- Y- Hole machining is not performed. Cancel all the hole data.

Because all data are cancelled in , Z, R needs to be ⑤

G85X-Z-R-P-；

⑥

respecified and F that remains can be omitted. P is saved but not needed in this block.

⑦

⑧

⑨

X- Z-；

G89X-Y-；

G01X-Y-；

It is a hole machining with a different Z value to . And ⑥ there is moving only in X axis. Do the hole machining by G89 according to the data Z specified in , R, P in⑦ and F in .⑥② Cancel the hole machining mode and data.

A Absolute instruction and incremental instruction in canned cycle G90/G91

The change of G90/G91 along drilling axis is shown as Fig. 4-4-2. (Usually it is programmed by

G90, if it is programmed by G91, Z and R are regarded as negative values.)

（A）（B）

Fig. 4-4-2

B Return to initial level in canned cycle G98/G99

After the tool reaches the bottom of a hole, it may return to the point R level or the initial level.

GSK218M CNC SYSTEM Programming and Operation Manual

These operations can be specified by G98 and G99.

Generally, G99 is used for the 1

drilling operation and G98 is used for the last drilling operation. The initial level does not change even drilling is performed in G99 mode. The following figure illustrates the operation of G98 and G99.

G98 is the system default mode.

G9 8 (re tu rn to in itia l lev e l )

Initia l l e v e l

G99 (return to point R level)

Fig. 4-4-3

The following symbols are used for the canned cycle illustration:

Positioning ( rapid traverse G0)

Cutting feed (linear interpolation G1)

Initia l le v e l

Point R

Manual feed

Offset ( rapid traverse G0)

Dwell

Fig. 4-4-4

Canned cycle comparison table（G22～G89）

Table 4-4-3

G code

Drilling (-Z

direction)

G22 Feed G23 Feed G24 Feed G25 Feed G26 Feed G32 Feed

Operation at

the hole

bottom

Retraction(+Z

direction)

Rapid C CW inner circular groove rough milling Rapid CW inner circular groove rough milling Rapid Rapid Rapid Rapid

Application

CCW finish-milling within a circle cycle CW finish-milling within a circle cycle CCW outer circle finish-milling cycle CW outer circle finish-milling cycle

GSK218M CNC SYSTEM Programming and Operation Manual G33 Feed G34 Feed

G35 Feed

G36 Feed

G37 Feed G38 Feed

G73

G74 Feed

G76 Feed

G80 Cancel

G81 Feed Rapid feed

G82 Feed Stop Rapid feed

Intermittent

feed

Rapid feed High-speed peck drilling cycle

Dwell→spindle

Oriented

spindle stop

Rapid

Feed Counter tapping cycle

Rapid feed Fine boring

CCW rectangle groove rough milling CW rectangle groove rough milling CCW inner rectangle groove finish-milling

cycle CW inner rectangle groove finish-milling

cycle CCW rectangle outside finish-milling cycle CW rectangle outside finish milling cycle

Drilling，spot drilling

Drilling，counterboring

G83

G84 Feed

G85 Feed Feed Boring

G86 Feed Spindle stop Rapid feed Boring

G87 Feed Spindle CCW Rapid feed Boring

G88 Feed

G89 Feed Dwell Feed Boring

Restriction

In canned cycle, tool offset is ignored.

Intermittent

feed

Rapid feed Peck drilling cycle

Dwell 

spindle CCW

Dwell 

spindle CCW

Feed Tapping

MANUAL Boring

4.4.1 Rough milling of inner circular groove G22/G23

Format: G22 G98/G99 X_ Y_ Z_ R_ I_ L_ W_ Q_ V_ D_ F_ K_ G23 Function: They are used for circular interpolations from the circle center by helical type till the

circular groove programmed is machined.

GSK218M CNC SYSTEM Programming and Operation Manual

Explanation:

G22： CCW inner circular groove rough milling G23： CW inner circular groove rough milling X、Y：The start point within X, Y plane Z： Machining depth, which is absolute position in G90 and position to R reference

level in G91

R： R reference level, which is absolute position in G90 and position to start point of this block in

G91 I： Circular groove radius, it should be over the current tool radius L： Cut width increment within XY plane, less than tool diameter but more than 0; W：Initial cut depth in Z axis, which is the distance below R reference level and it

is over 0( if the initial cut depth exceeds the groove bottom, it should machine by

this bottom) ; Q：Cut depth of each feed; V：Distance to the end surface at rapid tool traverse, which is over 0; D：Tool diameter number, ranging within 0 ~ 256, D0 is defaulted for 0. The current tool

diameter value is got by the given number.

K：Repetitions.

Cycle process:

Rapid t⑴ o a location in XY plane;

Rapid down to R level; ⑵

⑶ To cut W depth downward by cutting feedrate; ⑷ From center outward to mill a circle surface with a radius I helically by a L increment

each time; Z axis rapidly returns to R level;⑸ X, Y⑹ axes rapidly position to the circle center; Z axis rapid downward to a location with a distance V to the end surface; ⑺ To cut a⑻ （Q+V）depth downward in Z axis; Repeat the actions from ⑼ （4）~（8）till the total depth of circle surface is finished; Return⑽ to initial level or R level according to G98 or G99 instruction.

Instruction path:

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-4-1-1

G22: CCW inner circle groove rough milling

2I-D

Note：D is the tool diameter value is the helical radius coefficient

Tool

Tool center path

Circle groove border

Feed point

Fig. 4-4-1-2

G23: CW inner circle groove rough milling

2I-D

Note：D is the tool diameter value is the helical radius coefficient

Tool

Tool center path

Circle groove border

Feed point

Fig. 4-4-1-3

GSK218M CNC SYSTEM Programming and Operation Manual

Note：1、The NO: 12#1 should be set to 1 when the instruction is used. 2、When the helical radius coefficient in groove cycle is set to 0, the system uses linear feed

instead of helical ; if the programmed speed is over F15, it feeds by the speed of F15, if the programmed speed is less than F15, it feeds by the programmed one.

Example: To rough mill a groove within a circle by canned cycle G22 instruction, which is as

follows:

Fig. 4-4-1-4

G90 G00 X50 Y50 Z50； (G00 rapid positioning)

G99 G22 X25 Y25 Z-50 R5 I50 L10 W20 Q10 V10 F800；

(Groove rough milling cycle within a circle)

G80 X50 Y50 Z50； (Canned cycle cancel and return from R level)

M30；

Cancellation：G codes of 01 group (G00 to G03), G60 modal G code (bit parameter NO: 48#0

is set to 1) and G22/G23 cannot be specified in a same block, or G22/G23 will

be cancelled.

Tool offset：The tool radius offset in canned cycle is ingnored.

4.4.2 Fine milling cycle within a circle G24/G25

Format:

G24

G98/G99 X_ Y_ Z_ R_ I_ J_ D_ F_ K_

G25

Function: They are used to fine mill a circle by a radius I and direction specified and the tool

returns after milling.

Explanation:

G24： CCW fine milling within a circle

G25： CW fine milling within a circle

X、Y：The start point position within X, Y plane

Z：Machining depth which is absolute position in G90 and position to R reference level

GSK218M CNC SYSTEM Programming and Operation Manual

in G91

R： R reference level which is absolute position in G90 and position to start point of this block in

G91

I： Milling circle radius, ranging within 0 mm ~9999.999mm, use absolute value if it is a

negative one;

J： Distance of fine milling start point to circle center, ranging with 0 mm ~9999.999mm,

use absolute value if it is a negative one;

D：Tool diameter number, ranging within 0 ~256. D0 is defaulted for 0. The tool

diameter value is obtained by the given number.

K：Repetitions

Cycle process:

Rapid to a location within XY plane;⑴

Rapid down to R le⑵ vel;

Feed to the hole bottom;⑶

⑷ To position to the start point from current position at the bottom;

To interpolate by the transition arc 1 from the start point;⑸

⑹To make circular interpolation for the whole circle by inner arc path of finish-milling.

To make circular interpolation by transition arc 4 and return to the start ⑺

point;

Return to the initial level or R level according to G98 or G99 instruction.⑻

Instruction path:

Fig. 4-4-2-1

Note：The NO: 12#1 should be set to 1 when this instruction is used.

Example: To fine mill a circular groove that has been rough milled as following by canned cycle

G24 instruction:

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-4-2-2

G90 G00 X50 Y50 Z50； (G00 rapid positioning)

G99 G24 X25 Y25 Z-50 R5 I50 J10 F800；

(Canned cycle starts, and goes down to the bottom to perform the inner circle fininsh milling)

G80 X50 Y50 Z50； (To cancel canned cycle and return from R level)

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G24/G25 cannot be specified in a same block,

or G24/G25 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.3 Outer circle finish milling cycle G26/G32

Format:

G26

G98/G99 X_ Y_ Z_ R_ I_ J_ D_ F_ K_；

G32

Function: They are used to finish mill a circle outside a circle by the specified radius and

direction and the tool returns after milling.

Explanation:

G26： CCW outer circle finish milling cycle

G32： CW outer circle finish milling cycle

X、Y：The start point within X, Y plane

Z：Machining depth, which is absolute position in G90 and position to R reference level

in G91

R：R reference level, which is absolute position in G90 and position to start point of this block in

G91

I： Finish milling circle radius, ranging within 0 mm ~9999.999mm, use the absolute

value if it is a negative one.

GSK218M CNC SYSTEM Programming and Operation Manual

J： Distance from the milling start point to milling circle center, ranging within

0 mm ~9999.999mm, use the absolute value if it is a negative one

D：Tool radi us number, ranging within 0 ~256, D0 is defaulted for 0. The current tool

radius value is obtained by the given number.

K：Repetitions.

Cycle process:

Rapid to a location within XY plane;⑴

Rapid down to R level;⑵

Feed to the hole bottom;⑶ ⑷ To position to the start point from current position at the bottom;

⑸ To interpolate by the transition arc 1 from the start point; ⑹ To make circular interpolation for the whole circle by arc 2, arc 3 ⑺ To make circular interpolation by transition arc 4 and return to the start point; Return to the initial level or R level according to G98 or G99 instruction.⑻

Instruction path:

G26: CCW outer circle finish milling cycle

2I+D

Center of circle

Outer circle border

Tool

Tool center path

Fig. 4-4-3-1

Feed position

GSK218M CNC SYSTEM Programming and Operation Manual

G32: CW outer circle finish milling cycle

2I+D

Center of circle

Outer circle b o rde r

Tool

Feed position

( X0, Y0 )

Tool center path

Fig. 4-4-3-2

Explanation:

In outer circle finish milling, the interpolation directions of transition arc and finish milling arc are different, while the interpolation direction in the instruction means the interpolation direction of the finish milling. Example: To finish mill a circular groove that has been rough milled as following by canned cycle G26 instruction:

Fig. 4-4-3-3

G90 G00 X50 Y50 Z50； (G00 rapid positioning) G99 G26 X25 Y25 Z-50 R5 I50 J30 F800； (Canned cycle starts, and goes down to the bottom

to perform the outer circle finish milling) G80 X50 Y50 Z50； (To cancel canned cycle and return from R level) M30；

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter NO: 48#0

is set to 1) and G26/G32 cannot be specified in a same block, or G26/G32 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

GSK218M CNC SYSTEM Programming and Operation Manual

4.4.4 Rectangular groove rough milling G33/G34

Format:

G33

G98/G99 X_ Y_ Z_ R_ I_ J_ L_ W_ Q_ V_ U_ D_ F_ K_

G34

Function: These instructions are used for linear cutting cycle from the rectangle center by the

parameter data specified till the rectangular groove programmed is machined.

Explanation:

G33： CCW rectangular groove rough milling

G34： CW rectangular groove rough milling

X、Y：The start point within X, Y plane

Z：Machining depth which is absolute position in G90 and position to R reference plane

in G91

R：R reference plane which is absolute position in G90 and position to start point of this

block in G91

I： Rectangular groove width in X axis, which should be over the tool radius and helical

feed radius should be less than half of it .

J： Rectangular groove width in Y axis, which should be over the tool radius

and helical feed radius should be less than half of it .

L：Cutting width increment within a specified plane, which should be less than the tool

diameter and over 0

W： Initial cut depth in Z axis, which is a downward distance from R level and is over 0

(if the initial cut exceeds the groove bottom, it will cut at the bottom position)

Q：Cut depth of each cutting feed

V：Distance to the end surface to be machined in rapid feed, which is over 0

U：Corner arc radius, no corner arc transition if omitted, U should be more than

or equal to the tool radius.

D：Tool diameter number, ranging within 0 ~ 256, D0 is defaulted for 0. The current tool

diameter value is given by the number specified.

K：Repetitions

Cycle process:

Rapid to a ⑴ start point within XY plane;

Rapid down to R level;⑵

⑶ The diameter helical feed W width can be gotten by radius compensation value

multiplying the parameter N0. 269 value

(4) Feed to the rectangle center X0 , Y0;

⑸ To mill a rectangular surface helically from center outward by L increment each

time;

⑹ Z axis rapids to R level; ⑺ X, Y axes rapidly locates to the rectangle center; ⑻ Z axis rapids down to a position that has a V distance to the end surface; ⑼ Z axis cuts downward for a（Q+V）depth; ⑽ Repeat the actions of（4）~（8）till the rectangular surface with the total depth is

machined;

⑾ Return to the initial level or R level according to G98 or G99 instruction.

Instruction path:

GSK218M CNC SYSTEM Programming and Operation Manual

G33 CCW rectangular groove rough milling

Note： is the helical radius coefficient

U-R

（U-R）/2

Feed

position

Programmed path

Start

position

Tool

Tool center path

groove border

Rectangular

G34 CW rectangular groove rough milling

U-R

（U-R）/2

Feed

position

Programmed path

Start

position

Tool

Tool center path

Rectangular

groove border

Fig. 4-4-4-1

Note: The NO:12#1 should be set to 1 when this instruction is used.

Example: To rough mill an inner rectangular groove as shown in the following by canned cycle G33 instruction:

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-4-4-2

G90 G00 X50 Y50 Z50； (G00 rapid positioning)

G99 G33 X25 Y25 Z-50 R5 I70 J50 L10 W20 Q10 V10 U5 F800；

(To run the inner rectangular groove rough milling cycle)

G80 X50 Y50 Z50； (To cancel canned cycle and return from R level)

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G33/G34 cannot be specified in a same block,

or G33/G34 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.5 Inner rectangular groove finish milling cycle G35/G36

Format:

G35

G98/G99 X_ Y_ Z_ R_ I_ J_ L_ U_ D_ F_ K_；

G36

Function: They are used for finish milling within a rectangle by the width and direction specified,

and the tool returns after finish milling.

Explanation:

G35： CCW inner rectangular groove finish milling cycle

G36： CW inner rectangular groove finish milling cycle

X、Y：The start point within X, Y plane

Z： Machining depth which is absolute position in G90 and position to R reference

plane in G91

R： R reference plane which is absolute position in G90 and position to start point of

this block in G91

I： Rectangular width in X axis, ranging within 0~9999.999mm

J： Rectangular width in Y axis, ranging within 0~9999.999mm

GSK218M CNC SYSTEM Programming and Operation Manual

L：Distance of start point to rectangular side in X axis, ranging within 0~9999.999mm;

U：Corner radius, no corner transition if omitted. Alarm is issued if U is omitted or equal

to 0 and the tool radius is over 0.

D：Tool diameter number, ranging within 0 ~ 256, D0 is defaulted for 0. The current tool

diameter value is given by the number specified.

K：Repetitions.

Cycle process:

Rapid to a location within XY plane;⑴

Rapid down to R level;⑵

Feed to the hole bottom;⑶ To position to th⑷ e start point from current position at the bottom; To make circular interpolation by the transition arc 1 from the start point; ⑸ To make linear and circular interpolation by the path 2⑹ -3-4-5-6; To make circular interpolation by the path of transi⑺ tion arc 7 and return to the start

point;

Return to the initial level or R level according to G98 or G99 instruction.⑻

Instruction path:

G35: CCW rectangular groove finish milling cycle

Tool center path

Rectangular

groove border

Tool

Start

position

G36: CW rectangular groove finish milling cycle

Tool

Start

position

Tool center path

Rectangular

groove border

Fig. 4-4-5-1

Note The NO:12#1 should be set to 1 when this instruction is used. Example: To finish mill a circular groove that has been rough milled as following by canned cycle

G35 instruction:

GSK218M CNC SYSTEM Programming and Operation Manual

Fig. 4-4-5-2

G90 G00 X50 Y50 Z50； (G00 rapid positioning)

G99 G35 X25 Y25 Z-50 R5 I80 J50 L30 U10 F800；(Canned cycle starts, and go down to

the bottom to perform the rectangular groove finish

milling)

G80 X50 Y50 Z50； (To cancel canned cycle and return from R level)

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G35/G36 cannot be specified in a same block,

or G35/G36 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.6 Rectangle outside finish milling cycle G35/G36

Format:

G37

G98/G99 X_ Y_ Z_ R_ I_ J_ L_ U_ D_ F_ K_

G38

Function: They are used for finish milling outside a rectangle by the width and direction

specified, and the tool returns after finish milling.

Explanation:

G37： CCW rectangle outside finish milling cycle

G38： CW rectangle outside finish milling cycle

X、Y：The start point within X, Y plane

Z：Machining depth which is absolute position in G90 and position to R reference plane

in G91

R：R reference plane which is absolute position in G90 and position to start point of this

block in G91

I： Rectangular width in X axis, ranging within 0 mm ~99999.999mm

GSK218M CNC SYSTEM Programming and Operation Manual

J： Rectangular width in Y axis, ranging within 0 mm ~99999.999mm L：Distance of start point to rectangular side in X axis, ranging within 0~9999.999mm U：Corner radius, no corner transition if omitted D：Tool diameter number, ranging within 0 ~ 256, D0 is defaulted for 0. The current tool

diameter value is given by the number specified

K：Repetitions

Cycle process:

Rapid to a location within XY plane;⑴

Rapid down to R level;⑵

Feed to the hole bottom;⑶ To position to the start point from current position at the bottom;⑷ To make circular interpolation by the transition arc 1 from the start poi⑸ nt; To make linear and circular interpolation by the path 2⑹ -3-4-5-6; To make circular interpolation by the path of transition arc 7 and return to the start ⑺

point;

Return to the initial level or R level according to G98 or G99 instruction.⑻

Instruction path:

G37 : C CW rec tangle o u t s id e finish milling cyc le

Tool

Tool center path

Rectangular

groove border

G38: C W rectangle ou t s ide finish milling cy c le

Tool

Rectangular

groove border

Fig. 4-4-6-1

Explanation:

For the rectangle outside finish milling, the interpolation direction of the transition arc is not

Tool center path

consistent with that of the finish milling arc, and the interpolation direction in explanation means that of the finish milling arc. Example: To finish mill a circular groove that has been rough milled as following by canned cycle G37 instruction: G90 G00 X50 Y50 Z50； (G00 rapid positioning)

G99 G37 X25 Y25 Z-50 R5 I80 J50 L30 U10 F800；

(Canned cycle starts, and go downward to the bottom to

GSK218M CNC SYSTEM Programming and Operation Manual

perform the rectangular groove finish milling)

G80 X50 Y50 Z50； (To cancel canned cycle and return from R level)

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G37/G38 cannot be specified in a same block,

or G37/G38 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.7 High-speed peck drilling cycle G73

Format: G73 X_Y_Z_R_Q_F_K_

Function: This cycle is especially defined for high-speed peck drilling, it performs intermittent

cutting feed to the bottom of a hole while removing chips from the hole by rapid retraction. The operation illustration is shown as Fig. 4-4-7-1.

Explanation:

X_Y_： Hole positioning data

Z_： In incremental programming it specifies the distance from point R level to

the bottom of the hole; in absolute programming it specifies the absolute

coordinate of the hole bottom.

R_： In incremental programming it specifies the distance from the initial level

to point R level; in absolute programming it specifies the absolute

coordinate of point R.

Q_： Depth of cut for each cutting feed

F_： Cutting feedrate

K_： Repetitions

GSK218M CNC SYSTEM Programming and Operation Manual

Point R

G73（G98）

Initial level

Point Z

Fig. 4-4-7-1

Point R

G73（G99）

Poin t R level

Point Z

Z, R： The hole bottom parameter Z and R must be correctly specified while performing the 1st

drilling operation (omitting unallowable) or the alarm is issued.

Q： If parameter Q is specified, the intermittent feed is performed as shown in above figure.

And the retraction is performed by the retraction value d (Fig.4-4-1-1) set in number parameter P270. The rapid tool retraction for a distance d is performed in each intermittent feeding.

If G73 and M codes are specified in a same block, M code is executed during the 1

hole positioning operation, then the system goes on the next drilling operation.

If the repetition K is specified, M code is only executed for the first hole.

Note 1 If parameter Q is not specified, alarm ”address Q not found(G73/G83)” will be

issued. If Q value is specified for a negative, the intermittent feed will be performed by the absolute value of Q.

Note2 In canned cycle, if the tool length compensation (G43，G44 or G49) is

specified, the offset value is either added or cancelled while positioning to point R level.

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G73 cannot be specified in a same block, otherwise G73 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

GSK218M CNC SYSTEM Programming and Operation Manual

Example 1

M3 S1500 Spindle running start

G90 G99 G73 X0 Y0 Z-15. R-10.Q5. F120. Positioning and drill hole 1 then return to point R

level Y-50; Positioning and drill hole 2 then return to point R level Y-80; Positioning and drill hole 3 then return to point R level X10; Positioning and drill hole 4 then return to point R level Y10; Positioning and drill hole 5 then return to point R level G98 Y75;Positioning and drill hole 6 then return to initial level G80； G28 G91 X0 Y0 Z0； Return to reference point M5； Spindle stop

M30；

Note The chip removal operation is still performed though Q is omitted in the machining

of the holes from 2

to 6.

4.4.8 Drilling cycle, spot drilling cycle G81

Format: G81 X_ Y_ Z_ R_ F_ K_ Function: It is used for normal drilling feed to the hole bottom, then the tool rapidly retracts from

the hole bottom.

Explanation:

X_Y_： Hole positioning data Z_： In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute coordinate of the hole bottom.

R_： In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R level. F_： Cutting feedrate K_： Repetitions (if necessary)

GSK218M CNC SYSTEM Programming and Operation Manual

G81（G98）

Initial level

Point R

Z点

G81（G99）

Point R level

Point R

Z点

Fig. 4-4-8-1

Z, R： The hole bottom parameter Z and R must be correctly specified while performing the

drilling operation(omitting unallowable) or the alarm occurs. If parameter P,Q are specified, they are ignored by system. After positioning along X and Z axes, the tool traverses to point R level to perform the drilling

from point R level to point Z level, then retracts rapidly.

The spindle is rotated by miscellaneous function M code before G81 is specified.

If G81 and M code are specified in a same block, M code is executed while the 1

hole

positioning operation is being performed, then the system goes on next drilling operation.

If number of repeats K is specified, M code is only executed for the 1st hole. If the tool length compensation G43, G44 or G49 is specified in canned cycle, the offset is

either added or cancelled while positioning to point R level.

Example

M3 S2000 Spindle running start G90 G99 G81 X300. Y-250. Z-150. R-10. F120. Positioning, drill hole 1, then return to point R level

Y-550.； Positioning, drilling hole 2, then return to point R level

Y-750.； Positioning, drill hole 3, then return to point R level

X1000.； Positioning, drill hole 4, then return to point R level

Y-550.； Positioning, drill hole 5, then return to point R level

G98 Y-750.； Positioning, drill hole 6, then return to initial level

G80；

G28 G91 X0 Y0 Z0 ； Return to reference point

M5； Spindle stops

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G81 cannot be specified in a same block,

GSK218M CNC SYSTEM Programming and Operation Manual

otherwise G81 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.9 Drilling cycle, counterboring G82

Format: G82 X_ Y_ Z_ R_ P_ F_ K_； Function: It is used for normal drilling to feed to the hole bottom and dwell, then retract the tool

rapidly from hole bottom.

Explanation:

X_Y_: Hole positioning data Z_: In incremental programming it specifies the distance from point R level to the bottom of

the hole; in absolute programming it specifies the absolute coordinate of the hole bottom.

R_: In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R. F_: Cutting feedrate P_: Dwell time K_: Repetitions

G82（G98）

Point R

Dwell

Initial level

Point Z

G82（G99）

Point R

P Dwell

Fig. 4-4-9-1

Point R level

Point Z

After positioning along X and Z axes, the tool traverses to point R level to perform the drilling from point R level to point Z level, then dwells and returns rapidly after the tool reaches the hole bottom.

The spindle is rotated by miscellaneous function M code before G82 is specified. If G82 and M code are specified in a same block, M code is executed while the 1 positioning operation is being performed, then the system goes on next drilling operation. If number of repeats K is specified, M code is only executed for the 1st hole.

hole

GSK218M CNC SYSTEM Programming and Operation Manual

If tool length compensation G43, G44 or G49 is specified in canned cycle, the offset value is

either added or cancelled while positioning to point R level.

P is a modal instruction, and the min. value of it is set by number parameter P281, the max.

value by P282. If P value is less than the setting by P281, the min. value is effective; if P value

is more than the setting by P282, the max. value is effective. If P is specified in a block

containing no drilling, it can’t be stored as a modal datum.

Example

M3 S2000 Spindle running start

G90 G99 G82 X300. Y-250. Z-150. R-100. P1000 F120 Positioning, drill hole 1 with 1s dwell at the

hole bottom, then return to point R level

Y-550； Positioning, drill hole 2 with 1s dwell at the hole bottom, then return to point R level

Y-750； Positioning, drill hole 3 with 1s dwell at the hole bottom, then return to point R level

X1000.； Positioning, drill hole 4 with 1s dwell at the hole bottom, then return to point R level

Y-550； Positioning, drill hole 5 with 1s dwell at the hole bottom, then return to point R level

G98 Y-750； Positioning, drill hole 6 with 1s dwell at the hole bottom, then return to initial level

G80； Cancel canned cycle

G28 G91 X0 Y0 Z0 ； Return to reference point

M5； Spindle stops

M30； Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G82 cannot be specified in a same block,

otherwise G82 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.10 Drilling cycle with chip removal G83

Format: G83 X_ Y_ Z_ R_ Q_ F_ K_

Function: It is used for peck drilling that the tool feeds to the hole bottom by intermittent feeding

with chips removed from hole during drilling.

Explanation:

X_Y_： Hole positioning data

Z_： In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute coordinate of

the hole bottom.

R_： In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R.

Q_： Depth of cut for each cutting feed

GSK218M CNC SYSTEM Programming and Operation Manual

F_： Cutting feedrate K_： Repetitions

G83（G98）

Initial level

Point R

Point Z

G83（G99）

Point R

Point Z

Fig. 4-4-10-1

Q： It specifies each cutting depth expressed by incremental value. In the second and the

following feeding, the tool rapidly traverse to the position which has a distance d to the end position of last drilling and still performs the feeding d that is set by parameter P270, as is shown in Fig. 4-4-10-1.

Only positive value can be specified for Q and the negative value is used as a positive one

with its negative sign ignored.

Q is specified in drilling block, it can’t be stored as a modal datum if it is specified in the block

containing no drilling.

The spindle is rotated by miscellaneous function(M code) before G83 is specified. If G83 and M code are specified in a same block, M code is executed while the 1st hole

positioning operation is being performed, then the system goes on next drilling operation.

If number of repeats K is specified, M code is only executed for the 1st hole. If tool length compensation G43,G44 or G49 is specified in canned cycle, the offset value is

either added or cancelled while positioning to point R level.

Example

M3 S2000 Spindle running start G90 G99 G83 X300. Y -250. Z-150. R-100. Q15 F120；Positioning, drill hole 1, then return to point R

level

GSK218M CNC SYSTEM Programming and Operation Manual

Y-550； Positioning, drill hole 2, then return to point R level Y-750； Positioning, drill hole 3, then return to point R level X1000； Positioning, drill hole 4, then return to point R level Y-550； Positioning, drill hole 5, then return to point R level G98 Y-750； Positioning, drill hole 6, then return to initial level G80； G28 G91 X0 Y0 Z0 ； Return to reference point M5； Spindle stops M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G83 cannot be specified in a same block, otherwise, G83 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.11 Right-handed tapping cycle G84

Format: G84 X_ Y_ Z_ R_ P_ F_ Function: It is used for tapping. In this tapping, when the tool reaches the hole bottom, the

spindle runs reversely.

Explanation:

X_Y_: Hole positioning data

Z_: In incremental programming it specifies the distance from point R level to the bottom

of the hole; in absolute programming it specifies the absolute coordinate of the hole bottom.

R_: In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R. P_: Dwell time. F_: Cutting feedrate.

GSK218M CNC SYSTEM Programming and Operation Manual

Point R

Spindle ccw

G84（G98）

Initial le vel

Spindle cw

Spindle ccw

Point Z

Point R

G84（G99）

Point R lev el

Spindle cw

Point Z

Fig. 4-4-11-1

Tapping is performed by rotating the spindle CW, when the tool reaches the hole bottom, the spindle is rotated reversely for retraction. This operation creates threads. Feedrate overrides are ignored during tapping. A feed hold does not stop the machine until the return operation is finished.

Before specifying G84, use a miscellaneous function (M code) to rotate the spindle. If the spindle CW rotation is not specified, it will be adjusted for CW rotation automatically in R level by the current spindle specification.

If G84 and M code are specified in a same block, M code is executed while the 1

hole

positioning operation is being performed, then the system goes on next drilling operation.

If number of repeats K is specified, M code is only executed for the 1

hole.

P is a modal instruction, and the min. value of it is set by number parameter P281, the max. value by P282. If P value is less than the setting by P281, the min. value is used; if P value is more than the setting by P282, the max. value is used. If P is specified in a block containing no drilling, it can’t be stored as a modal datum.

If tool length compensation G43, G44 or G49 is specified in canned cycle, the offset value is either added or cancelled while positioning to point R level.

In feeding per minute, the relation betwe en the thread lead and feedrate as well as spindle speed is as following:

Feedrate F=tap pitch×spindle speed S For example: for the M12×1.5 thread hole on the workpiece, the following parameter can be used: S500=500ｒ/min F=1.5×500=750mm/min For multi-start thread, F value can be gotten by multiplying the thread number.

Example:

M3 S100 Spindle running start

GSK218M CNC SYSTEM Programming and Operation Manual

G90 G99 G84 X300. Y-250. Z-150. R-120 P300 F120 Positioning, tap hole 1, then return to

point R level

Y-550.； Positioning, tap hole 2, then return to point R level Y-750.； Positioning, tap hole 3, then return to point R level X1000； Positioning, tap hole 4, then return to point R level Y-550.； Positioning, tap hole 5, then return to point R level G98 Y-750.； Positioning, tap hole 6, then return to initial level G80； G28 G91 X0 Y0 Z0 ； Return to reference point M5； Spindle stops M30

；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G84 cannot be specified in a same block,

otherwise G84 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.12 Left-handed tapping cycle G74

Format: G74 X_ Y_ Z_ R_ P_ F_

Function: It is used for tapping cycle. In this tapping cycle, when the hole bottom is reached,

the spindle rotates reversely.

Explanation:

X_Y_： Hole positioning data

Z_： In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute

coordinate of the hole bottom.

R_： In incremental programming it specifies the distance from the initial level to

point R level; in absolute programming it specifies the absolute coordinate of

point R.

P_： Dwell time.

F_： Cutting feedrate.

GSK218M CNC SYSTEM Programming and Operation Manual

Point R

Spindle cw

G74（G98）

Point Z

Initial level

Spindle ccw

Spindle cw

Point R

G74（G99）

Poin t R level

Spindle ccw

Point Z

Fig. 4-4-12-1

Tapping is performed by rotating the spindle CCW , when the tool reaches the hole bottom, the

spindle is rotated reversely for retraction. This operation creates threads.

Feedrate overrides are ignored during tapping. A feed hold does not stop the machine until

the retraction operation is finished.

Before specifying G74, use a miscellaneous function (M code) to rotate the spindle. If the spindle CCW rotation is not specified, it will be adjusted for CCW rotation in R level automatically by the current spindle speed specified.

If G74 and M code are specified in a same block, M code is executed while the 1

hole

positioning operation is being performed, then the system goes on next drilling operation.

If number of repeats K is specified, M code is only executed for the 1

hole.

If tool length compensation G43, G44 or G49 is specified in canned cycle, the offset value is either added or cancelled while positioning to point R level.

Example

M4 S100 Spindle running start G90 G99 G74 X300. Y-250. Z-150. R-120 P300 F120 Positioning, tap hole 1, then return to

point R level Y-550.； Positioning, tap hole 2, then return to point R level Y-750.； Positioning, tap hole 3, then return to point R level X1000； Positioning, tap hole 4, then return to point R level Y-550.； Positioning, tap hole 5, then return to point R level G98 Y-750.； Positioning, tap hole 6, then return to initial level G80； G28 G91 X0 Y0 Z0 ； Return to reference point

GSK218M CNC SYSTEM Programming and Operation Manual

M5； Spindle stops

M30

；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G74 cannot be specified in a same block,

otherwise G74 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.13 Fine boring cycle G76

Format: G76 X_Y_Z_Q_R_P_F_K_

Function: It is used for boring a hole precisely. When the tool reaches the hole bottom, the

spindle stops and the tool departs from the machined surface of the workpiece and

retracts. The retraction trail that affects machined surface finish and the tool damage

should be avoided in the operation.

Explanation:

X_Y_: Hole positioning data

Z_: In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute coordinate of

the hole bottom.

R_: In incremental programming it specifies the distance from the initial level to point

R level; in absolute programming it specifies the absolute coordinate of point R

level.

Q_: Offset of the hole bottom

P_: Dwell time.

F_: Cutting feedrate.

K_: Number of fine boring repeats

Fig. 4-4-13-1

GSK218M CNC SYSTEM Programming and Operation Manual

When the tool reaches the hole bottom, the spindle stops at a fixed rotation position and the tool is

moved in the direction opposite to the tool tip and retracted. This ensures that the machined

surface is not damaged and enables precise and efficient boring. The parameter Q specifies the

retraction distance and the retraction axis and direction are specified by bit parameter NO.42#4

and NO.42#5. And Q is a positive value, if Q is specified with a negative value, the sign is ignored.

The hole bottom offset of Q is a modal value saved in canned cycle which should be specified

carefully as it is also used for the cutting depth for G73 and G83.

Before specifying G76, use a miscellaneous function (M code) to rotate the spindle.

If G76 and M code are specified in a same block, M code is executed while the 1

hole

positioning operation is being performed, then the system goes on next boring operation.

If number of repeats K is specified, M code is only executed for the 1st hole.

If tool length compensation G43,G44 or G49 is specified in canned cycle, the offset value is

either added or cancelled while positioning to point R level.

Axis switching: before the boring axis is changed, the canned cycle must be cancelled.

Boring: In a block that does not contain X , Y , Z, R or any additional axes, boring is not

performed.

Example

M3 S500 Spindle running start

G90 G99 G76 X300.Y-250. Positioning, bore hole 1, then return to point R level

Z-150. R-100.Q5. Orient at the hole bottom, then shift by 5mm

P1000 F120.; Stop at the hole bottom for 1s

Y-550.; Positioning, bore hole 2, then return to point R level

Y-750.; Positioning, bore hole 3, then return to point R level

X1000.; Positioning, bore hole 4, then return to point R level

Y-550.; Positioning, bore hole 5, then return to point R level

G98 Y-750.; Positioning, bore hole 6, then return to initial level

G80 G28 G91 X0 Y0 Z0 ; Return to reference point

M5; Spindle stops

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G76 cannot be specified in a same block,

otherwise G76 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.14 Boring cycle G85

Format: G85 X_ Y_ Z_ R_ F_ K_ Function: It is used to bore a hole.

Explanation:

GSK218M CNC SYSTEM Programming and Operation Manual

X_Y_： Hole positioning data

Z_： In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute coordinate of

the hole bottom.

R_： In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R.

F_： Cutting feedrate.

K_： Number of repeats

Fig. 4-4-14-1

After positioning along X and Y axis, traverse is performed to point R level, and boring is

performed from point R level to point Z level. As the tool reaches the hole bottom, cutting feed is

performed then return to point R level.

Before specifying G85, use a miscellaneous function (M code) to rotate the spindle.

If G85 and M code are specified in a same block, M code is executed while the 1

hole

positioning operation is being performed, then the system goes on next boring operation.

If number of repeats K is specified, M code is only executed for the 1

hole.

If the tool length compensation G43, G44 or G49 is specified in the canned cycle, the offset is

added while positioning to point R level.

Axis switching: Before the boring axis is changed, the canned cycle must be cancelled.

Boring: In a block that does not contain X , Y , Z, R or any additional axes, boring is not

performed.

Example

M3 S100 Spindle running start

G90 G99 G85 X300. Y-250. Z-150. R-120. F120. Positioning, bore hole 1, then return to

point R level

GSK218M CNC SYSTEM Programming and Operation Manual

Y-550.； Positioning, bore hole 2, then return to point R level

Y-750.； Positioning, bore hole 3, then return to point R level

X1000.； Positioning, bore hole 4, then return to point R level

Y-550.； Positioning, bore hole 5, then return to point R level

G98 Y-750.； Positioning, bore hole 6, then return to initial level

G80；

G28 G91 X0 Y0 Z0 ； Return to reference point

M5； Spindle stops

M30；

Restriction:

Cancellation：G codes in 01 group (G00 to G03), G60 modal G code (bit parameter

NO: 48#0 is set to 1) and G85 cannot be specified in a same block,

otherwise G85 will be cancelled.

Tool offset：The tool radius offset in canned cycle is ignored.

4.4.15 Boring cycle G86

Format: G86 X_ Y_ Z_ R_ F_ K_； Function: It is used to perform a boring cycle.

Explanation:

X_Y_： Hole positioning data

Z_： In incremental programming it specifies the distance from point R level to the

bottom of the hole; in absolute programming it specifies the absolute coordinate of

the hole bottom.

R_： In incremental programming it specifies the distance from the initial level to point R

level; in absolute programming it specifies the absolute coordinate of point R.

F_： Cutting feedrate

K_： Repetitions

gsk GSK218M Operation Manual

Specifications and Main Features

Frequently Asked Questions

User Manual