gsk GSK983M Programming Manual

Download

GSK983M Milling CNC System

User Manual

(Volume I: Specifications and Programming)

This user manual describes all items concerning the operation of the

system in detail as much as possible. However, it is impractical to give

particular descriptions of all unnecessary and/or unavailable works of the

system due to the length limit of the manual, specific operations of the

product and other causes. Therefore, the operations not specified herein

may be considered impractical or unavailable.

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.

Company Profile

GSK, GSK CNC Equipment Co,. Ltd, is the largest CNC system production and

marketing enterprise in China at present. It is the Numerical Control industrial

base of South China, and the undertaking enterprise of the national 863 main

project Industrialization Support Technology for Medium Numerical Control

System. It is also one of the 20 basic equipment manufacture enterprises in

Guangdong province. It has been taking up the research and development,

design and the manufacture of machine CNC system (CNC device, drive unit and

servo motor) in recent 10 years. Now it has developed into a large high-tech

enterprise integrated with technology, education, industry and trade by enhancing

the popularization and trade of CNC machine tools. There are more than 1400

staffs in this company that involves 4 doctors, more than 50 graduate students

and 500 engineers; more than 50 among these staffs are qualified with senior

engineer post titles. The high performance-cost ratio products of GSK are

popularized in China and Southeast Asia. And the market occupation of GSK’s

product dominates the first and the turnout and sale ranks the top for successive

7 years in domestic market for the same product from the year 2000 to 2006,

which makes GSK the largest CNC manufacture base throughout China.

Field technical support services

Field support services are available when you encounter a problem insolvable

through telephone. GSK CNC Equipment Co. Ltd will designate a technical

support engineer to your place to solve technical problems for you.

Chinese version of all technical documents in Chinese and English languages is regarded as final.

Foreword

Dear user, We are really grateful for your patronage and purchase of GSK983M milling CNC

system made by GSK CNC Equipment Co., Ltd.

This manual consists of two volumes. Volume I mainly describes the

specifications and programming of the system while Volume II operations, all

codes, parameters, I/O interfaces and other appendices.

This system can only be operated by authorized and qualified personnel as

！

improper operations may cause accidents. Please carefully read this user

manual before usage.

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.

III

CONTENTS

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

1.1 Overview............................................................................................................................................1

1.2 Introduction to the Manual.............................................................................................................1

2. SPECIFICATIONS........................................................................................................................2

3. PROGRAMMING........................................................................................................................13

3.1 What Is Programming?.................................................................................................................13

3.2 Program Make-up ..........................................................................................................................13

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

3.2.2 Program word........................................................................................................................................14

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

3.2.4 Decimal programming .........................................................................................................................18

3.2.5 Maximum instruction value.................................................................................................................19

3.2.6 Program number...................................................................................................................................20

3.2.7 Sequence number ................................................................................................................................21

3.2.8 To skip over an optional block............................................................................................................21

3.3 Dimension Word............................................................................................................................23

3.3.1 Controllable axis ...................................................................................................................................23

3.3.2 Set unit....................................................................................................................................................25

3.3.2.1 Minimum set unit and minimum travel unit..............................................................................25

3.3.2.2 Input unit×10 ..................................................................................................................................26

3.3.3 Maximum travel.....................................................................................................................................26

3.3.4 Program origin and coordinate system............................................................................................26

3.3.5 Coordinate system and origin of processing ..................................................................................27

3.3.6 Workpiece coordinate system............................................................................................................27

3.3.7 Reference (position) point ..................................................................................................................28

3.3.8 Absolute value instruction and incremental value instruction .....................................................29

3.4 Feed Function (F function) ..........................................................................................................30

3.4.1 Rapid traverse (positioning) function ...............................................................................................30

3.4.2 Cutting feedrate ....................................................................................................................................30

3.4.3 To reduce feedrate to 1/10..................................................................................................................31

3.4.4 Synchronous feed (feed per rotation) ..............................................................................................31

3.4.5 F1 digit feed ...........................................................................................................................................32

3.4.6 Automatic acceleration and deceleration ........................................................................................33

3.4.7 Automatic angle adjustment...............................................................................................................34

3.4.7.1 Automatic adjustment of inner angle........................................................................................34

3.4.7.2 Switch of inner arc cutting feedrate ..........................................................................................37

3.5 Preparation Function (G function)..............................................................................................38

3.5.1 Selection of planes (G17, G18, G19)...............................................................................................40

3.5.2 Positioning (G00)..................................................................................................................................41

3.5.3 Unidirectional positioning (G60) ........................................................................................................42

3.5.4 Linear interpolation (G01)...................................................................................................................42

3.5.5 Arc interpolation (G02, G03) ..............................................................................................................44

3.5.5.1 Arc interpolation without any additional axis ...........................................................................44

3.5.5.2 Arc interpolation with an additional axis...................................................................................48

3.5.6 Sine-curve interpolation ......................................................................................................................48

3.5.7 Thread cutting (G33)............................................................................................................................49

3.5.8 Automatic return to reference point (reference positions G27～G30) ......................................51

3.5.8.1 Check of return to reference point (G27).................................................................................51

3.5.8.2 Automatic return to reference point (G28)...............................................................................52

3.5.8.3 Automatic return from reference point (G29)..........................................................................53

3.5.8.4 Return to the 2nd, 3rd or 4th reference point (G30) .............................................................55

3.5.9 Dwell (G04) ............................................................................................................................................55

3.5.10 Accurate stop detection (G09).........................................................................................................56

3.5.11 Accurate stop detecting mode (G61) and cutting mode (G64) ................................................56

3.5.12 Coordinate system setting (G92)....................................................................................................56

3.5.13 Workpiece coordinate system (G54～G59) .................................................................................57

3.5.14 To change workpiece coordinate system by program instruction ...........................................59

3.5.15 Automatic setting of a coordinate system .....................................................................................59

3.5.16 To switch between Inch and metric systems (G20, G21)..........................................................59

3.5.17 Storage travel limit (G22, G23) .......................................................................................................60

3.5.18 Skip function (G31) ............................................................................................................................63

3.6 Compensation................................................................................................................................65

3.6.1 Tool length compensation (G43, G44, G49)...................................................................................65

3.6.2 Tool offset (G45～G48) .......................................................................................................................67

3.6.3 Tool radius compensation (G40～G42) ...........................................................................................74

3.6.3.1 Tool radius compensation function............................................................................................74

3.6.3.2 Offset (D codes) ............................................................................................................................74

3.6.3.3 Offset vector...................................................................................................................................75

3.6.3.4 Plane selection and vector..........................................................................................................75

3.6.3.5 G40, G41 and G42 .......................................................................................................................75

3.6.3.6 Details about tool radius compensation C...............................................................................77

3.6.4 D and H functions ...............................................................................................................................109

3.6.5 External tool offset..............................................................................................................................110

3.6.6 To input offset through program (G10)...........................................................................................110

3.6.7 Zooming function (G50, G51) ..........................................................................................................110

3.7 Cycle Machining Function .........................................................................................................113

3.7.1 External moving function ..................................................................................................................113

3.7.2 Fixed cycles (G73, G74, G76 and G80～G89)............................................................................114

3.7.2.1 Repeating a fixed cycle .............................................................................................................126

3.7.3 Specifying an origin and Point R in a fixed cycle (G98, G99)...................................................132

3.8 Spindle Function (S function), Tool Function (T function), Miscellaneous Function (M function) and Secondary Miscellaneous Function (B function)

.........................133

3.8.1 Spindle function (S function) ............................................................................................................134

3.8.1.1 S 2 digits .......................................................................................................................................134

3.8.1.2 S 4 digits .......................................................................................................................................134

3.8.2 Constant surface speed control ......................................................................................................134

3.8.2.1 Instructed methods .....................................................................................................................135

3.8.2.2 Spindle speed ..............................................................................................................................135

3.8.2.3 Restraint of maximum rotational speed of spindle ..............................................................135

3.8.2.4 Rapid traverse (positioning) (G00)..........................................................................................136

3.8.3 Tool function (T function)...................................................................................................................137

3.8.4 Miscellaneous function (M function)...............................................................................................137

3.8.5 Secondary miscellaneous function (B function) ..........................................................................138

3.9 Subprogram......................................................................................................................................138

3.9.1 Creation of a subprogram.................................................................................................................139

3.9.2 Execution of a subprogram ..............................................................................................................139

3.9.3 Special methods of application........................................................................................................140

3.10 User Macro .....................................................................................................................................142

3.10.1 General...............................................................................................................................................142

3.10.2 Variables.............................................................................................................................................144

3.10.2.1 Indication of a variable ............................................................................................................144

3.10.2.2 Introduction of variables..........................................................................................................144

3.10.2.3 Undefined variables .................................................................................................................145

3.10.2.4 Display and setting of variable...............................................................................................146

3.10.3 Types of variables ............................................................................................................................146

3.10.3.1 Local variables # 1～# 33 .......................................................................................................147

3.10.3.2 Common variables #100～ #149 , #500～ #509 .............................................................147

3.10.3.3 System variables (for user Macro B)....................................................................................147

3.10.4 Operation instructions .....................................................................................................................160

3.10.4.1 Definition and substitution of variable ..................................................................................160

3.10.4.2 Additive operation.....................................................................................................................160

3.10.4.3 Multiply operation (Macro B option) .....................................................................................160

3.10.4.4 Function (Macro B option) ......................................................................................................160

3.10.4.5 Hybrid operation........................................................................................................................161

3.10.4.6 Changing operational order using [ ].................................................................................162

3.10.4.7 Accuracy .....................................................................................................................................162

3.10.4.8 Cautions regarding deterioration of precision ....................................................................162

3.10.5 Control instruction ............................................................................................................................163

3.10.5.1 Branch (GOTO).........................................................................................................................163

3.10.5.2 Repeat (how to select Macro B)............................................................................................165

3.10.6 Creation and storage of user macro body ..................................................................................169

3.10.6.1 Creation of user macro body..................................................................................................169

3.10.6.2 Storage of user macro body...................................................................................................170

3.10.6.3 Macro statement and NC statement ....................................................................................170

3.10.7 Macro call instruction.......................................................................................................................173

3.10.7.1 Simple calling ............................................................................................................................173

3.10.7.2 Modal calling..............................................................................................................................180

3.10.7.3 Multiple calling...........................................................................................................................181

3.10.7.4 Multiple modal calling ..............................................................................................................181

3.10.7.5 Calling a macro with G codes................................................................................................182

3.10.7.6 Calling a subprogram with an M code .................................................................................183

3.10.7.7 Calling macros with M codes .................................................................................................184

3.10.7.8 Calling a subprogram with a T code.....................................................................................185

3.10.7.9 The position of the decimal point of an independent variable........................................185

3.10.7.10 The difference between M98 (calling a subprogram) and G65 (calling a

macro body) ...............................................................................................................................................186

3.10.7.11 The nesting and local variables of user macro ................................................................186

3.10.8 The relationship with other functions ...........................................................................................187

3.10.9 Special codes and words used in user programs.....................................................................189

3.10.10 Restrictions......................................................................................................................................190

3.10.11 Descriptions for P/S alarm ...........................................................................................................191

3.10.12 Examples of user macros ............................................................................................................191

3.10.12.1 Groove machining ..................................................................................................................191

3.10.13 External output instructions .........................................................................................................193

3.10.13.1 OPEN instruction: POPEN...................................................................................................194

3.10.13.2 Data output instruction BPRNT DPRNT ...........................................................................194

3.10.13.3 Close instruction PCLOS......................................................................................................195

3.10.13.4 Necessary settings for using the function.........................................................................195

3.10.13.5 Cautions ...................................................................................................................................195

3.10.14 Macro interruption function (Macro B).......................................................................................196

3.11 Tool Life Management...............................................................................................................196

3.11.1 Setting of tool groups.......................................................................................................................196

3.11.2 Setting in machining processes ....................................................................................................198

3.11.3 Performance of tool life administration ........................................................................................200

3.11.3.1 Tool life calculation....................................................................................................................200

3.11.3.2 Tool change signal and tool change reset signal...............................................................200

3.11.3.3 New tool selection signal.........................................................................................................201

3.11.3.4 Tool skip signal ..........................................................................................................................201

3.11.4 The display and input of tool data.................................................................................................201

3.11.4.1 The display and modification of tool group number ..........................................................201

3.11.4.2 The display of tool life data during the execution of machine program ........................201

3.11.4.3 Presetting tool life counter ......................................................................................................202

3.11.5 Other cautions ...................................................................................................................................203

3.12 The Indexing Function of Indexing Worktable.....................................................................203

3.12.1 Instructing methods .........................................................................................................................203

3.12.1.1 Input unit.....................................................................................................................................203

3.12.1.2 Absolute / incremental instruction .........................................................................................203

3.12.1.3 Concurrently controlled axes .................................................................................................204

3.12.2 Minimum travel unit: 0.001 degree/pulse....................................................................................204

3.12.3 Feedrate .............................................................................................................................................204

3.12.4 The clamping and release of indexing worktable......................................................................204

3.12.5 Jog/step/handwheel.........................................................................................................................205

3.12.6 Other cautions...................................................................................................................................205

VII

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

1. GENERAL

1.1 Overview

As a high-accuracy and high-performance closed-loop CNC system with firmware, GSK983M

milling CNC system (hereinafter called “System”) was newly developed and launched by GSK

CNC Equipment Co., Ltd. to satisfy the demands of NC market and intended for CNC milling

machine and processing center. By employing a high-speed microprocessor, a general large scale

integrated circuit (LSI), a semiconductor memory and up-to-date storage elements, the reliability

as well as performance-to-price ratio of its control circuit are greatly improved, thereby facilitating

the reliability, functions/ performance to price ratio to a large extent.

With a widely applicable advanced servo, GSK983M milling CNC system uses a high-duty pulse

encoder as its detecting element, thereby composing a closed-loop CNC system.

This operating manual describes all available functions of the system. However, a real unit may not

necessarily be provided with all the optional functions. Should the specifications of the control panel

and operating mode of the machine change, the instruction manual supplied with the machine by the

manufacturer shall be referred to.

1.2 Introduction to the Manual

The functions of a NC machine system are not only dependent on its NC, but also on its mechanical

part. That is to say, its heavy current circuit, servo system, NC and mechanical operation panel

jointly determines its performance. The manual only gives a general account from the angle of NC as

it is difficult to describe all the functions of an NC machine and programming and operating

procedures in detail. As for a specific NC machine, please refer to the instruction manual supplied

with the machine by the manufacturer. The contents of the machine instruction manual are more

important than those herein.

The performance of a NC machine system is jointly determined by its NC system, mechanical

structure, heavy current control and servo system including its mechanical operation panel. The

operating manual only describes GSK983M CNC system. To know the performance, programming

and operating instructions of the entire NC machine system further, please refer to the machine

instruction manual supplied by the manufacturer.

The operating manual describes all matters in detail as much as possible. However, the listing of all

matters is unnecessary and impossible as this will complicate the contents of the manual. Therefore,

the functions that are not described in this manual may be considered impractical.

The functions that are not described in this manual may be deemed unavailable so far.

Some items are specifically explained in Note sections. Therefore, if any explanation is not available

in the current Note section, it is advisable to skip over it, thoroughly read the manual and then return

to the part.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

2. SPECIFICATIONS

Serial

No.

Designation Descriptions

1 Controllable axes

Number of concurrently

controllable axes

Incremental system

Standard: 3 axes, namely axes X, Y and Z

(4 or 5 axes are also available upon customer’s request. The

address of the 4

That the 4

The address of the 5

or C. It is possible to specify whether the 5

axis can be selected from A, B, C, U, V or W.

axis is linear or rotary may be set by parameters.

axis can be designated as U, V, W, A, B

axis is linear or

rotary by parameters.)

Standard: 3, axis 3, link,

(The following configurations are also available upon customer’s

request: 4, axis 3, link; 4, axis 4, link; 5, axis 3, link; and 5, axis 4

and link.)

Min. set increment 0.001mm 0.0001 inch 0.001°

Min entered increment 0.001mm 0.0001 inch 0.001°

The minimal increment entered in accordance with parameter

setting metric system may be 0.01mm.

4 Bit detecting device Pulse encoder

±99999.999 mm

5 Max. instruction value

±9999.9999 inch

±99999.999°

6 Input format

Decimal point

programming

Changeable block, character and address formats are

employed.

It is possible to enter numerical values including a decimal point.

The addresses that may include a decimal point are X, Y, Z, A,

B, C, U, V, W, I, J, K, Q, R and F.

Axial speed can be up to 24,000m/min or 960 inch/min. In

8 Rapid traverse

addition, rapid traverse speed may be changed to FO，25，50 or

100% using rapid traverse override (optional).

Feedrate can be set within the following ranges: 1 mm/min～ 15,000mm/min and 0.01inch/min ～ 600.00 inch/min. It is

possible to set the upper speed limit of cutting feed by

parameters. A feedrate may be selected from 0 to 200% by

setting the override of feedrate to 10% as a step. The unit of

Miscellaneous function

(Bit M2)

feedrate may be changed to 0.01 mm/min, 0.001 mm/min or

0.001 inch/min according to parameter setting.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Both manual rapid traverse and automatic rapid traverse are

performed in linear acceleration/deceleration mode so as to

reduce positioning time.

Automatic

acceleration/deceleration

G codes may be used to select absolute or Incremental

Absolute/incremental

value instruction

programming.

G90: Absolute programming

G91: Incremental programming

When the instruction value for subsequent axes of G92 is used

to establish a coordinate system, the actual position of cutting

tool will become the instruction value for the coordinate system.

Coordinate system

setting (G92)

All axes individually move to the end point rapidly and

13 Positioning (G00)

decelerate until stop through instruction G00, and the machine

performs positioning (whether the machine reaches the

instructed position) detection by parameters setting.

Linear interpolation

(G01)

Linear interpolation may be conducted at the feedrate specified

by F codes using instruction G01.

When executing a block, the unit reads the next one in buffer

15 Buffer register

instruction operation caused by the time required for reading

may be avoided. While inputting data in buffer register, BUF will

appear on the lower right of LCD screen.

The operation of the next block can be delayed before execution

16 Dwell (G04)

using instruction G04. The delay time must be specified with

address P or X.

Accurate stop detection

(G09)

The block of instruction G09 decelerates and performs

positioning detection by the end of the block.

If G61 is instructed, the travel instructions following G61

decelerate from doubtful points of all blocks and continue to

execute the next block when it is positioned.

If G64 is instructed, the travel instructions following G64 rather

than positioning instruction do not decelerate but execute the

Accurate stop detecting

mode/cutting mode

(G61, G64)

following blocks. As a rule, they are applicable for cutting mode.

The instructions of M2 with 2 digits following may be used to

control the ON/OFF signal on machine side. Only one M code

can be instructed in one block.

Miscellaneous function

(Bit M2)

In dry running mode, feedrate becomes Jog (JOG) feedrate.

The rapid traverse speed keeps constant and rapid traverse

20 Dry run

override (option) is still valid in rapid traverse instruction (G00).

However, the dry running of instruction is available when it is set

to rapid traverse (positioning) according to parameters.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

It is possible for all axes to individually disable the feed of an

instructed axis. If any instructed axis in interlocked during

21 Interlock

traveling, all axes of the machine will decelerate until stop. Once

the interlock signal is cancelled, the machine will accelerate and

restart.

22 Single block A block instruction can be executed each time.

The block preceded by a “/” (slash) code may be ignored by

turning on the OPTIONAL BLOCK SKTP switch on the machine

side.

To skip over an optional

block

The switch may be used to reverse the program instructions of

24 External mirroring

axes X and the 4

to set mirroring with the MDI/LCD panel or the switch on the

machine side.

It is possible to determine whether to add the traveling amount

through the manual traveling tool to absolute coordinates by

switching the manual absolute value switch on the machine

side.

Manual Absolute Value

ON/OFF

Manual Absolute Value switch ON: To add; OFF: Not to add.

26 To lock auxiliary function

BCD code signal and strobe signal of M, S, T and B are sent to

the machine side.

The machine keeps still. However, position display is still valid

27 To lock the machine

as the machine is moving and machine locking is also valid even

in the execution of a block.

axis as well as the travel of MDI. It is possible

To cancel the instruction

for axis Z

The function is only equivalent to Z-axis locking. It is to be used

when NC program is checked by drawing a picture with a pen.

The function is used to temporarily stop the feed of all axes that

29 To feedrate feed

can be restarted by pressing Cycle Start button. Before the

restart of feed, it is possible to insert manual operation in

manual mode.

30 To cancel override

The function is used to fix the cutting feedrate at 100%

depending on the signals from the machine side.

By pressing the Emergent stop button all feed instructions stops

31 Emergent stop

(interrupt immediately) and the machine stops running at the

same time.

The function is used to reset NC from the outside of NC. The

signal stops all feed instruction and the machine decelerates

until stop by reset. Additionally, the Reset button on MDI/LCD

outputs reset signals to the machine side during emergent stop

External reset, reset

signal

and external reset.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The moving parts of the machine receives arriving signal when

33 Overtravel

they come to the end of travel. Then the movement of axis

decelerates until stop and overtravel warning is displayed at the

same time.

When the power supply is switched on, NC gives the signal in

34 NC Ready signal

controllable state. It stops sending signals to the machine side

once the power supply is cut off or the control unit overheats.

When the servo system is ready, the signal is sent to the

35 Servo Ready signal

machine side. For the axis to be braked, it is locked when the

signal has not been given off. LCD displays NO READY in the

absence of the signal.

36 NC warning signal The signal is sent out when NC is in warning state.

NC outputs the signal when the motion order ends up. If the

functions of M, S, T or B and motion instruction are active in a

block, the signal is given after the completion of the execution of

traveling instruction and the functions of M, S, T or B can be

Distribution Completed

signal

executed.

38 Cycle Operation signal NC gives the signal in cycle operation.

Cycle Operation Start

Indicator signal

Feed Hold Indicator

signal

NC sends out the signal at the start of cycle operation.

NC outputs the signal when it is in holding state through feed

hold.

(1) JOG feed: For JOG feedrate, the rotary switch may be used

for 24-step switching. The ratio of 24-step is geometric

progression.

41 Manual continuous feed

(2) Manual rapid traverse: Rapid traverse may also be achieved

by manual means. Rapid traverse override may be used for

the rapid traverse speed set by parameters. Rapid traverse

override is an optional function.

Manual continuous feed is available for 2 axes at one time.

Since the following increments may exert positioning control,

42 Incremental feed

manual positioning can be performed efficiently. Incremental

feed is available for 2 axes at one time (incremental feed

amount).

Sequence number

searching

Program number

searching

It is possible to search the sequence numbers in the currently

selected program with the MDI/LCD panel.

It is possible to search the program numbers of 4 digits following

O with the MDI/LCD panel.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

It is this function that compensates the lost amount of movement

45 Clearance compensation

of the machine. The amount of compensation is set in the

minimum amount of movement within 0 ~ 255 by parameters.

The function disables the display, setting and editing of the

46 Program key locking

program with a program number of 9000～9899 by means of

key locking.

(1) Ambient temperature

0℃～45 for operation and ℃ -20℃～55 for storage and ℃

shipment.

(2) Relative humidity

≤90%(without condensation), ≤95%(40 )℃

Environmental

conditions

(3) Vibration

Less than 0.5G for operation and 1G for storage and

shipment

(4) Ambient air

To install an NC in an environment with high density of dust,

machining fluid and organic solvent, contact the

manufacturer.

(1) Servo system

48 Self-diagnostics

(2) NC

(3) Status display

a. To give an alarm when the error of the error register

goes beyond the setting in halted state.

b. To give an alarm when the value of the error register

goes beyond the maximum setting.

c. To give an alarm in case of malfunction of positioning

detection system.

d. To give an alarm when the drift voltage is excessive.

e. To give an alarm in case of malfunction of speed control

unit.

a. To give an alarm in case of malfunction of the memory.

b. To give an alarm in case of malfunction of ROM and

RAM.

c. To give an alarm in case of malfunction of the

microprocessor.

a. To display the status of NC on LCD.

b. To display the status of I/O on LCD.

S function/T function

(BCD2 bit)

Once the instructions of 2 digits following S and T are instructed,

the code signal of BCD2 bit may be sent out while codes S and

T ad other codes are individually output. They are reserved until the following S and T are instructed.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The binary 12-bit or analog voltage corresponding to the speed

of principal axis is output to the machine side. The analog

voltage is up to ±10V, 2mA and the speed (r/min) of principal

axis is directly specified by S4 Bit. The speed of principal axis

may be regulated in the following range depending on the

contact signal on the machine side: 50, 60, 70, 80, 90, 100, 110

S4 Bit (binary 12-bit

output)

A/S4 Bit (analog output)

and 120%.

When the speed (r/min) of principal axis is directly specified, the

voltage for the current speed of principal axis is output by the

presently selected gear numbers 1 to 4.The switching of gear is

performed in a heavy-current circuit, resulting that the signal of

GRA or GRB is input in NC side. As the judging message for

switching gears on the heavy-current side, NC outputs the

S4 Bit (binary 12-bit

output)

A/S4 Bit (analog output)

higher 2 bits or lower 2 bits of S4 bit in BCD codes.

A position coder is installed on the principal axis. It is possible to

perform thread cutting using the pulse synchronous speed of the

position coder.

Thread cutting

/synchronous feeding

To achieve the feed that is in step with the rotation of the

principal axis, a device that may generate pulse voltage of which

53 Position coder

frequency is proportional to the number of revolutions of the

principal axis and generates 1024 pulses in each rotation shall

be directly connected.

Generally surface speed is instructed with B codes. In this way

Constant surface speed

control

the principal axis accordingly changes when the position of the

tool changes so that its surface cutting speed is always equal to

the linear speed set by S codes.

Address B is followed by three digits. Once it is instructed, a

BCD three-bit code signal will be sent out to position the index

table.

Second auxiliary function

(B3 bit)

Addresses S and T are followed by a 2-digit instruction. Once

they are instructed, the code signal of BCD2 bit will likely to be

56 T-function (BCD4 bit)

sent out and other codes of the addresses S and T are

individually sent out and held until the next S and T are

instructed.

ISO codes (ISO840) and EIA codes (EIA RS-244-A) can be

57 Code standards

used for program code. The identification of ISO codes and EIA

codes may be performed automatically.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The automatic or manual rapid traverse speed can be set in 4

58 Rapid traverse override

levels, i.e. FO, 25, 50 and 100% and FO is likely to be set to a

specific speed by parameters.

Return to reference point A consists the following procedures:

Return to reference point

(1) Manual return to the reference point;

(2) Examination of the return to the reference point (G27); (3) Automatic return to the reference point (G28).

Return to reference point

Return to the 3

and 4th

reference points

Storage travel limits 1

and 2

Memory type pitch error

compensation

Besides the functions of returning to reference point A, the

return to reference point B also includes the return to the 2

reference point (G30).

It is possible to set the 3

their distances from the 1

and 4th reference points by setting

reference point and return to these

reference points.

For storage travel limit 1, the area beyond those set by

parameters are exclusion areas. For storage travel limit 2, the

inside or outside of the area specified by parameters or

programs are exclusion areas. The validity or invalidity of

storage travel limit 2 is set by G codes.

G22: Valid G23: Invalid

The function is designed to compensate the pitch error caused

by the mechanical wear of the feed screw so as to maximize

processing accuracy and mechanical life. Compensation data is

saved in memory, thereby omitting the compensation

mechanism such as the stop and the relevant setting

operations.

The selection of a

workpiece coordinate

system

Tool offset (G45～G48)

It is possible to preset one of the 6 workpiece coordinate systems using six G codes, i.e. G54～G59 and subsequent

programming can be made in the selected coordinate system.

Tools can be offset using instructions G45～G48. Tool offset

refers to the side-play mount corresponding to a move

instruction’s elongation or reduction of an instruction of D or H codes in axial direction. D or H codes may instruct 1～32 and

the maximum offset shall be ±999.999mm or ±99.999 inches.

G45: To increase the set value;

G46: To reduce the set value;

G47: To increase the set value by twice;

G48: To reduce the set value by twice.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

To manually return to a reference point, parameters must be

Automatic setting of a

coordinate system

preset to establish a coordinate system, namely automatic

execution is similar to the condition that the instruction G92 is

used at the reference point.

Tool length offset (tool length compensation) is possible in the

Tool length offset (G43,

G44, G49)

direction of the axis Z using instructions G43 and G44. The offset number must be selected within 01～32 using H codes.

The offset shall fall within ±999.999mm or ±99.999 inches.

Tool radius compensation is possible using instructions G40～ G42. The offset number must be specified within 01～32 using

D codes. The offset shall fall within ±999.999mm or ±99.999

inches. Cutter compensation B is unavailable for a tool of a

medial angle less than 90°.

Tool radius

compensation B, C

(G40～G42)

Cutter compensation 0 can be used for the tool of a medial

angle less than 90°.

Manually position the standard tool to the fixed point of the

machine tool. Then manually position the machine tool to be

measured to the same mechanical point. The length

compensation of the tool will be input as offset once z INPUT

Tool length

measurement

is pressed.

Tool life management

function

Additional offset memory A The numbers of tool offset and tool radius compensation may be

Additional offset memory B The numbers of tool offset and tool radius compensation may be

Additional offset memory

74 F1- bit feed

Divide the tools in the cutting tool room into several groups and

specify service life for each group of cutting tools. Accumulate

the tool processing time or processing number that serves as

the evaluation standard for tool life whenever a tool in the

groups is used. The next cutting tool in the predetermined

sequence is automatically selected in the same group when the

tool reaches its service life.

increased to 64.

increased to 99.

The number of cutter compensation is increased to 200.

Once the number of F followed by one digit of 1~9 is instructed,

the feedrate corresponding to the number will be set. The

instruction FO is a rapid traverse speed. The feedrate of the

currently selected number can be increased or reduced by

turning the manual pulse generator when the machine side

gives a speed-changing signal.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

External moving function

(G80, G81)

Fixed cycle A (G80, G81,

G82, G84, G85, G86 and

G89)

Fixed cycle B (G73,

G74, G76,

G80～G89)

Switch between Inch and

metric systems (G20,

G21)

Arc interpolation (G02,

G03)

Instruction G81 is used to output external movement signals

after the positioning of X and Y axes and G80 to cancel it.

It is possible to perform 6 fixed cycles including drilling cycle,

tapping cycle and boring cycle.

It is possible to perform 12 fixed cycles including gun drilling

cycle, finish boring cycle, tapping cycle and reverse-tapping

cycle.

Input in Inch or metric system can be selected by switching G

codes.

G20: Input in Inch system G21: Input in metric system

Using G02 (or G03) may achieve any arc interpolation within 0～360° with the feedrate of F code instruction.

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

When an axis in the arc plane does not move (the axis is

80 Sine-curve interpolation

considered as an imaginary axis) in the spiral-curve

interpolation instruction, the other 2 axes may be used for

sine-curve interpolation.

The arc interpolation

using arc radius R for

programming

In arc interpolation, directly specifying radius with radius value R

rather than I, J and K simplifies programming. An arc over or

below 180° can be instructed.

The mechanical vibration at the end of travel can be minimized

82 External deceleration

and the range of effective travel maximized through the function.

External deceleration is not applicable for an additional axis.

The function is used to input any program number among 1～31

for NC from the outside such as machine side and to select

these programs from the memory of NC.

External workpiece

number search A

The function is used to transmit the following data from the

outside such as machine side:

84 External data input

(1) External workpiece number search C;

(2) External cutter compensation C;

(3) External warning message;

(4) External operation information.

Automatic acceleration/

deceleration of cutting

feed

Cutting feed and manual continuous feed can be set by

parameters to make power type acceleration/ deceleration in 8ms～4000ms time constant.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

9 switches for skipping over selected blocks can be set on

machine side by adding a digit (1~9) after the switching

instruction”/” of a block. When a switch n for skipping over

selected blocks is enabled, the blocks with “/n” will be skipped

Additional skipping over

selected blocks

over.

When G31 is followed by X, Y, Z, the 4

or 5th axis instruction as

same as G01, it is possible to make line interpolation. If skip

87 Skip function (G31)

signal is input from the outside during the execution of the

instruction, the remaining part of the instruction stops executing

and the blocks that follow will be executed.

88 Program restart

89 Unidirectional positioning

Addition of the number of

storable programs

91 Zoom

Insertion of a manual

tray

Automatic angle

adjustment

When the sequence number to be restarted is specified, the

program will restarts from here.

Positioning can only be performed in one direction in order to

eliminate clearance and achieve accurate positioning.

96 programs can be added to the standard programs to reach

191 programs in total.

The tool path instructed in a program can be zoomed in a range of 0.001～99.999x.

The tool movement overlapping an automatic running instruction

can be done only with the pulses of the manual pulse generator

without processing interruption.

When cutting the inner side of an angle in tool radius

compensation mode, adjustment can be automatically added in

the set area for processing at low speed.

The function is used to set the angle of the positive direction of

axis X on the dial gauge of the operation panel of the machine

and to make Jog feed in the set direction. In the XY plane, this function is only valid for the increment of 5° spacing within 0°～

Manual feed at any

angle

360° range.

Once the block with the same sequence number as the preset

Sequence number

comparison stop

one appears in the execution of a program, a single block will be

in stop status when the execution of the program ends. The

function is used to check a program.

96 Indication of running time

The NC automatic running time can be indicated on LCD in

seconds, minutes and hours.

The ON/OFF can be controlled by using the settings on

97 Menu switch

MDI/LCD rather than the switches on the operation panel on the

machine

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

User macros

A and B

These are the intrinsic functions available for manufacturer and

user and types A and B are provided due to functional limits.

99 Graphic display The tracks of cutting tools are traced out on LCD.

The manual pulse generator on the operation panel can be used

to perform Jog feed of the machine. The manual pulse

100 Manual pulse generator

generator sends out 100 pulses each turn. The travel of each

pulse can be switched between 1x, 10x and 100x depending on

the signals on the machine side.

PLC MODELS A and B are available.

101 PLC

Quantity of input

points

Quantity of output

points

Program step

PLC MODEL-A PLC MODEL-B

192 points 192 points

128 points 128 points

Up to 2,000

steps

Up to 5,000 steps

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3. PROGRAMMING

3.1 What Is Programming?

NC processing machine operates by developed programs. To process a part on the NC machine,

the route and other processing conditions of cutting feed shall be included in the program. The

program is called “part program”.

The following diagram indicates the processes from preparation of detail drawing to NC’s

execution of the processing program.

Detail drawing Processing plan Part programming NC’s execution of processing program

(1) Determine the NC processing range and select an NC machine to be used.

(2) Determine the assembling method of the workblank on the machine and select a

Part program is an NC instruction for controlling feed route and the auxiliary movement of a

machine written according to the rules for NC. The instructions are usually written in a program list.

necessary clamping device and a tool.

(3) Determine the cutting sequence (process type, home point of the cutting tool, the cut

depths of rough cutting and finish cutting and route of cutting feed).

(4) Select a cutting tool and a tool clamping device and determine the mounting position on

the machine.

(5) Set cutting conditions (spindle rotating speed, feed speed and whether to use cooling

fluid, etc).

This chapter will describe how to develop a part program.

3.2 Program Make-up

A program consists of main program and subprogram. As a rule, NC moves by the instructions of a

main program. When the main program gives an instruction to switch to a subprogram, NC moves

by the subprogram.

When there is an instruction to return to a main program in a subprogram, NC will return to the

main program and continue to move by the instructions of the main program.

NC memory can store 95 main programs and subprograms in total. When one of the main

programs is selected, NC machine can move by its instructions.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Main program Subprogram

[Instruction to switch to a subprogram]

Instruction 1

Instruction 2

┊

Instruction n

Instruction n+1

┊

Instruction 1

Instruction 2

┊

[Instruction to return to a main program]

Note: The number of programs that can be stored will be increased to 191 if the function

“Addition of the number of storable programs” (Optional) is selected.

Refer to Chapter 4: Operations for the storage method of program.

3.2.1 Block

A program is composed of a number of instructions. Each instruction unit in a program is called a block. Blocks are distinguished from each other by end code. As described below, end-of-block code is indicated with a “;”.

For example:

XXXX; XXXX; XXXX;

Note 1: The maximum number of characters a block is not limited in.

Note 2: End-of-block code: CR for EIA codes and LF for ISO codes.

3.2.2 Program word

The elements composing a block are program words. The program word below consists of an

address and a subsequent figure. A “+” and a “ –“ can also be added before the figure.

X - 1000

Address Figure

Program word

An address is indicated with a letter among A～Z. An address determines the meaning of its

subsequent figure. The addresses that can be used in an NC and their meanings are as follows.

An address may have different meanings depending on different instructions of preparation

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Sequenc No. eed

u c

d e

u c

function in a program.

Name Address Meaning

Program No. : (ISO) /O (EIA) Program number

Sequence No. N Sequence number

Preparatory

function

G Instructed move mode (linear, arc, etc)

X, Y, Z Move instruction of coordinate axis

A, B, C, U, V, W Move instruction of additional axis

Coordinate word

R Arc radius

I, J, K Coordinates of arc center

Feed function F Designation of feedrate

Spindle function S Designation of spindle rotational speed

Tool function T Designation of tool number and tool offset number

Auxiliary

function

M Designation of ON/OFF control on machine side

B Worktable indexing, etc.

Offset No. H, D Designation of offset number

Dwell P, X Designation of dwell time

Designation of

program No.

P Designation of subprogram number

Designation of

sequence No.

Number of

repetition

L Numbers of repetition of subprogram and fixed cycles

Designation of sequence number: Program is repeatedly

executed at this sequence number.

Parameter P, Q, R Parameters of fixed cycle

For example, these program words may compose the following block.

； N— G— X— Y— F— S— T— M— ；

Preparatory function

Coordinate No.

in f n ti n

l f n

ti n

Miscellaneous

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

In the following program list, a line indicates a block and a case in the block indicates a program word.

Name S57.10.10 Page/

Program No. 0 (: ) 2002

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

N20 G92 X

100.0 Y 200.0 Z 300

N21 G00 X

196.0 Y 315.0 Z 500

N22 G01 F10.0

(Note ) CR(EIA)，LF(ISO)

S400 T15 M03

；

3.2.3 Input format

All program words composing a block shall be instructed in the formats as specified below. The

input format of this system is a variable block format. Therefore, the number of the program

words in a block and the number of characters in a program word are variable, which makes

programming easier.

(1) Input in metric system

NO4·G02·XL+053·YL053·ZL+053·

RD053 D02

αL+053·βL+053· ·F050· ·

ID053·JD053·KD+053 H02

S02 T02

· ·B03·M02;

S04 T04

(2) Input in Inch system

NO4·G02·XL+044·YL+044·ZL+044·

RD044 D02

αL+053·βL+053· ·F032· ·

ID044·JD044·KD044 H02

S02 T02

· ·B03·M02；

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

S04 T04

Note 1: α and β are for any one of A, B, C, U, V and W.

Note 2: The address and digits in the above formats have the following meanings.

X L + 0 5 3

The three digits behind decimal point

The five digits before decimal point

Leading zero may be omitted.

With a symbol

Absolute value or incremental value

Address

J D 0 5 3

The three digits behind decimal point

The five digits before decimal point

Leading zero may be omitted.

Incremental value with a symbol

Address

For example: When a cutting tool moves to 50.123mm along X axis, its move instruction is as follows:

G00

X50 123

The three digits behind decimal point

The five digits before decimal point: 00050

The leading zero and T are omitted.

G00 must not be omitted even the leading zero may be

omitted. (G00 specifies rapid traverse (positioning)).

Note 3: When an address word in a block is instructed twice or more times, the last instruction will be

valid and not give any alarm in principle.

For example: G01 M03 S200 M08;

Now M08 is valid and M03 invalid. For G codes, the lastly specified one in each group of G

codes in a block is valid. However, G90/G91 is only valid at the specified location in a block

(see Section 3.3.8.).

Example G90 X10.0

G91 Y20.0 ；

Absolute Incremental

If R and I, J or K are concurrently instructed in an arc interpolation instruction, R is always valid

and this is not related to instruction sequence.

Note 4:F050 in Inch-system input format may also be changed into F051 through parameter switching.

Refer to Section 3.4.3 “To multiply feedrate by 1/10”.

Note 5: Since P and Q have a number of meanings, they are omitted in the above format.

Note 6: Refer to Section 3.2.4 ”Decimal entries”.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Note 7: Multiply the value input in metric system of X, Y, Z, A, B, C, U, V, W, I, J, K, Q and R by 10 by

means of parameter setting.

RD052

XL+052·YL+052·ZL+052·αL+052·βL+052· ID052·JD052·KD052

(α and β are A, B, C, U, V and W) (Input in metric system) Refer to Section 3.3.2.2 “To multiply

an input unit by 10”.

Note 8: Refer to Section 3.3.2.2 “To multiply an input unit by 10”.

3.2.4 Decimal programming

It is possible for this unit to input the numerical values with a decimal point. Decimal point is

used in the values in the unit of distance, time or speed. However, some addresses may not

use decimal for entry. The location of a decimal point indicates the position of mm, inch,

degree or second.

X15.0 X15mm or x15 inches

F10.0 10mm/min for 10 inch/min

G04×1 Feedrate for 1 second

B90.0 B90deg

The addresses that can be entered with decimal point are as follows:

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

Note 1: During the dwell of an instruction, X can be input with the decimal point but P cannot (because

P is also specified with a sequence number).

Note 2: When G codes are used to change the location of the decimal point, it is necessary to

predetermine G codes even in a block. G20; (specify in Inch system ) X1.0G04；X1.0 is

considered as a travel distance (in inch) because it does not indicate time. The result is held

for 10 seconds in relation to X10000G04.

When G04 is entered, its indication changes from 1.0 to 10.0.

G04X1.0 is treated as G04X1000 and the result is held for 1 second.

Note 3: Take note that the condition with or without a decimal point is quite different. Its programming

mode differs from an electronic computer.

G21; (specified in metric system)

X1……X1 mm

X1……X0.001 mm

G20; (specified in Inch system )

X1……X1 inch

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

X1……X0.0001 inch

Note 4: The numerical values with/without a decimal point can be mixed.

X1000 Y23.7；

X10 Y22359；

Note 5: If a specified value is less than the minimum setting, the value will be rounded down. The

instruction of X1.23456 is considered as X1.234 when it is entered in metric system and

1.2345 in Inch system . It has cumulative error for an incremental value instruction and has no

cumulative error but rounding error for an absolute value instruction. The instructed digits must

not exceed the allowable maximum digit.

X1.23456789……There is an error because it has more than 8 digits.

X1.2345678…… There is no error when it is up to 8 digits inclusive.

Note 6: When a figure with a decimal point is entered, the figure will be converted into the integer of the

minimum input increment.

(Example)X12.34 12340(entered in metric system)

In addition, it is necessary to perform digit number verification for the converted integer.

(Example)X1234567.8 X1234567800(entered in metric system). It gives an alarm

because the number of digits exceeds 8.

3.2.5 Maximum instruction value

The maximum instruction values of all addresses are as listed in the table below. Take note

that what the table lists are the ranges of the maximum specified values for the NC unit rather

than the mechanical moving ranges of the NC machine tool. For instance, the moving range of

X axis is about 100m (entered in metric system) for an NC unit while the travel distance of axis

X is likely to be limited to 2m for a machine tool and so is its feedrate. The cutting feedrate of

an NC unit is up to 15m/min while that of an NC machine tool is likely to be limited to 6m/min.

In actual programming, both this manual and the instruction manual supplied by machine

builder shall be referred to. Programming shall be performed on the basis of full knowledge

about the programming ranges of a specific machine tool.

Table 2.5: Basic addresses and ranges of instruction values (including additional options)

Name Address

Program No.

Sequence No. N

: (ISO)

O (EIA)

Input in mm

Output in mm

1～9999

Input in inch

Output in mm

See the left See the left See the left

″ ″ ″

Input in mm

Output in inch

Input in inch

Output in

inch

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Preparatory

function

Coordinate word

Feed per minute F

Feed per minute

(feedrate l/10)

(parameter

setting)

Spindle function S

Tool function T

Miscellaneous

function

Dwell X, P

Sequence No.

setting

X, Y, Z, I,

J, K, Q, R,

A, B, C,

U, V, W

0～99

±99999.999mm

±99999.999°

1～15000

mm/min

0.1～15000.0

mm/min

0～30000

0～9999

0～99

0s～99999.99s

1～9999

″ ″ ″

±3937.0078inch

±99999.999°

0.01～600.00

inch/min

See the above

See the left See the left See the left

″ ″ ″

±99999.999mm

±99999.999°

1～15000

mm/min

0.1～15000.0

mm/min

±937.0078inch

±9999.999°

0.01～600.00

inch/min

See the above

Repeated times L

Offset No. S, H

2nd auxiliary

function

1～9999

0～200

0～999

″ ″ ″

3.2.6 Program number

The control unit can store a number of programs in the memory of the NC. Program numbers

are added to all programs in order to distinguish them.

Program number

(From 1 to 9999.0 and preceding 0 may be omitted)

4 digits

The program starts from the program number and ends at M02, M30 or M99.

#1111 pr ogr am #2222 program

01111……………………M02； 02222………………………M30；

M02 and M30 indicate the end of a main program. M99 indicates the end of a subprogram.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

05555………………………M99；

#5555 subprogram

Note 1: For ISO codes, replace O with a “:”.

Note 2: The block with an optional block skip code such as /M02, /M30 and /M99 shall not be deemed

as the end of a program.

Note 3: When a program is not provided with a preceding program number, the first sequence number

(N…) other than NO of the program may be used to replace the program number.

Note 4: If a program is not provided with a preceding program number or sequence number, MDI/LCD

panel shall be used to specify a program number when storing the program into the memory.

Note 5: For several programs, the second program and the succeeding ones are not necessarily

provided with an EOB code skipped wit a mark. However, an EOB code shall be used before

the program when the foregoing program ends by ER (EIA) or %(ISO).

Note 6: It is possible to operate without a program number. Subprogram shall be provided with a

program number.

Note 7: In some cases, the program number from 9000 ～ 9899 can only used by machine

manufacturer rather than user.

Note 8: When it has a robot option, program numbers 9900～9999 are used as robot data.

Note 9: When there is no M02, M30 or M99 but ER (EIA)%(ISO) at the end of the program, or the next

program number is 0, the end of the program shall be set by parameter No.306 BIT3 (NEOP).

3.2.7 Sequence number

A sequence number may be specified with N followed by four or less digits (1~9999) at the

start of a block. The order of sequence numbers is random and discontinuous. It is likely that

all blocks are provided with sequence numbers or sequence numbers are only added at the

necessary locations of a program.

It is recommended to specify sequence number in succession at key locations, e.g. when

replacing new tools or change the worktable indexing to a new machined surface.

Note 1: The use of the sequence number NO. is not allowed for the purpose of compatibility with the

program formats of other NC units.

Note 2: Since 0 cannot be used as a program number, the sequence number treated as a program

number shall not be 0.

3.2.8 To skip over an optional block

When a slash followed by a digit /n(n=1～9) is specified at the beginning of a block and the

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

OPTIONAL BLOCK SKTP switch n is enabled on the operation panel , the block with a /n

corresponding to switch number n will be ignored.

When the OPTIONAL BLOCK SKTP switch n is disabled, the block with a /n is valid, namely

operator may choose to skip over the block with a /n. The 1 in /1 can be ignored. However, the

1 in /1 must not be ignored when two or more OPTIONAL BLOCK SKTP switches are used.

When an OPTIONAL BLOCK SKTP switch is enabled, the ignored area is as follows:

；/2N123G01X4……………………；N7856

Ignored area

Example: N100X100；

N101/2z100；

N102/2/3X200；

N103/3z200；

In the above example, blocks N101 and N102 will be skipped over when No. 2 switch is

enabled and N102 and N103 skipped over when No. 3 switch enabled.

Note 1:Slash (/) shall be specified at the beginning of a block. If it is specified at other places of a block,

the information from the slash (/) to EOB code will be ignored but the information before the

slash (/) will remain valid.

Note 2: When the OPTIONAL BLOCK SKTP switch is enabled, TH and TV checkouts shall be

performed for the skipped part as the switch is disabled.

Note 3: The block to be skipped over is identified when the memory sends information to the buffer

ignored even if the OPTIONAL BLOCK SKTP switch is enabled.

Note 4: The function remains available during sequence number searching.

Note 5: The function is invalid when saving a program in the memory. That is, the block preceded by a

slash (/) will be written in the memory regardless the state of OPTIONIAL BLOCK SKIP.

Note 6: The programs may be completely output from the memory regardless the state of OPTIONIAL

BLOCK SKIP.

Note 7: Some OPTIONIAL BLOCK SKIP switches are likely to be unavailable for some machines.

Therefore, it is necessary to consult the machine manufacturer for the number of usable

switches.

Note 8: For the system with additional function to skip over an optional block, the 1 in /1 must not be

omitted if there are two or more marks for skipping over an optional block in one block.

/1 shall be specified as per the above requirements.

Example: Incorrect: //3 G00 X10.0；

Correct: /1/3 G00 X10.0；

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.3 Dimension Word

A dimension word prescribes the movement of a tool. It composes a relevant instruction with

the address of a kinematical axis and a value indicating the direction and amount of travel. It

varies depending on the different absolute and incremental programming modes. (See Section

3.3.8.)

Address of dimension world Meaning

The addresses of all axes in a rectangular coordinate

Basic axes X, Y, Z

Additional axes A, B, C, U, V, W

R To specify the radius of an arc. Arc

interpolation

parameters

I, J, K

system: To indicate the location of the axis or the

distance in axial direction.

The addresses of the 4

angle of axis of rotation or the location and distance of

linear axis.

To indicate the distance from the home point to the arc

center along axis X, Y or Z or an axis parallel to them.

and 5th axes: To indicate the

3.3.1 Controllable axis

The kinematical axis of a machine under the control of the NC system is called controllable

axis.

Each control shaft is recalled with the dimension word address of the control unit.

The number of axes that can be controlled by the NC system may be 3 (axes X, Y and Z) and

can be added to 4 or 5.

An additional axis may use any address among A, B, C, U, V or W. A, B and C are

recommended for axis of rotation and U, V and W for linear axis.

2 standard axes can be controlled in a block at the same time. The number of concurrently

controllable may be increased to 3 or 4 by means of additional selection. Separate control of

additional axis is only used for 3-axis link. The selection of additional axis gang control function

enables the link of 2 or 3 additional axes. If 3-axis gang control function is selected, it is not

necessary to select additional axis gang control function any more.

Number of

controllable

axes

3 2

Number of

standard

axes

Number of concurrently controllable axes

Selection of

concurrently

controllable

additional axes

Concurrent

selection

of 3 axes

selection of 3 axes

control selection of

additional axes

Concurrent

+ Concurrent

Concurrent

selection of

4 axes

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

additional axes)

(Including

X, Y, Z 3

(Including

additional axes)

Note 1: The system gives #17 alarm if additional axes (A, B, C, U, V, W) are specified without

additional control function.

Note 2: The number of link axes is always 2 in manual operation.

Note 3: When the system has the 5

axis, the following function control shall be exerted.

① Thread cutting and synchronous feed cannot be performed.

② The capacity of part program is reduced to 75%.

③ Additional S4 digit analog output function is not available.

④ Additional constant surface speed control function is not available.

Coordinate axes and movement symbols

If the machine coordinate axes specified by the machine are not identical with the tool

movement symbols, programming is subject to serious disorder. The concerned basic

concepts are provided in EIA RS-267-A or ISO841.

However, the following points shall be observed during programming.

a) Program shall be developed on the basis of a standard coordinate system (right-manual

rectangular coordinate system).

b) When programming, assume that workpiece does not move and a cutting tool moves around

it.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.3.2 Set unit

3.3.2.1 Minimum set unit and minimum travel unit

1) Minimum set unit (input unit)

Minimum unit of tool travel is input by instruction. The minimum unit is given in mm, inch or

degree.

2) Minimum travel unit (output unit)

The minimum unit output to the machine is indicated in mm, inch or degree. Any one of the

following combinations may be employed.

Input/output Minimum set unit Minimum travel unit

Input in mm and output in mm 0.001mm 0.001mm

Linear axis

Note: The set unit of an axis of rotation cannot be converted between Inch and metric systems.

Whether the minimum travel unit is 0.001 mm or 0.0001inch shall be determined by the

machine and selected by presetting parameter No.006 BIT0 (SCW).

Whether the minimum travel unit is 0.001 mm or 0.0001inch shall be selected by G codes or by

setting parameter through MDI/LCD panel.

Input in inch and output in mm 0.0001inch 0.001mm

Input in mm and output in inch 0.001mm 0.0001inch

Input in inch and output in inch 0.0001inch 0.0001inch

Axis of rotation 0.001° 0.001°

G20……The minimum set unit of a linear axis is 0.0001inch.

G21……The minimum set unit of a linear axis is 0.001mm.

The state of G20 and G21 remains unchanged when the system is powered on/off.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.3.2.2 Input unit×10

The minimum set unit in mm may be changed to 0.01mm by parameter No.006 BIT1 setting.

The minimum set unit in inch cannot be changed.

setting.

Address

Dimension word X, Y, Z, Q, R, I, J, K, U, V, W 0.01mm 0.0001inch

Revolution axis A, B, C 0.01° 0.01°

Dwell time

It cannot be changed in the following cases:

a) Inputting differs from the above conditions

b) Display unit

c) Maximum range of instruction value

d) Units of step feed and manual feed

e) Offset input

f) Others

Note 1: In the following descriptions herein, input unit is either 0.0001inch or 0.001mm.

Note 2: Display unit may become 0.01mm or 0.01 degree by parameter No.006 BIT2 (MDL)

X 0.01s 0.001s

P 0.01s 0.001s

Input in mm Input in inch

Minimum set unit

3.3.3 Maximum travel

The maximum travels that can be instructed of the device are as listed in the table below:

Input in mm and

output in mm

±99999.999mm

±99999.999°

Note: The travels listed in the above table change depending on different machines.

Input in inch and

output in mm

±3937.0078inch

±99999.999°

3.3.4 Program origin and coordinate system

Program origin and coordinate system shall be determined during programming. Generally a

specific point on the workpiece is determined as the program origin.

Input in mm and

output in inch

±99999.999mm

±99999.999°

Input in inch and

output in inch

±9999.9999inch

±99999.999°

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

This coordinate system is a workpiece coordinate system.

3.3.5 Coordinate system and origin of processing

A workpiece coordinate system needs to be used when a program is sent to the NC. The

cutting tool starts motion from the origin and the program starts from the origin, but the NC

always need to know the coordinates of the cutting tool at the origin through G92 instruction

(coordinate system setting).

3.3.6 Workpiece coordinate system

Several workpiece coordinate systems are needed when the mounting positions of the several

trailing bars for the machine are different. In this case, the 6 coordinate systems preestablished on the machine may be selected with 6 G codes (G54～G59) and the following

programs are executed in the selected coordinate system. All coordinate systems shall be

determined with the set distance between a reference point (a fixed point on the machine) and

their respective origins of coordinate (workpiece origin offset). See the following diagram for

details.

Refer to Section 4.4.13 for the setting method of workpiece origin offset.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

It is not necessary to establish a coordinate system with G92 instruction when the above-mentioned workpiece coordinate system is used. Concurrent use of G54～G59 and G92 may substitute the coordinate system established by G54～G59. Therefore, usually G92 shall not be used in conjunction with G54～G59.

Note: When using the workpiece coordinate system established by G54～G59, make sure to

return to the first reference point after switching on so that G54 will automatically generate a

workpiece system. Hence it is not necessary to set an automatic coordinate system.

3.3.7 Reference (position) point

Reference point is a fixed point on the machine. Reference point return function allows the

cutting tool to return to the reference point. Therefore, a program is likely not to start from one

point on a workpiece coordinate system but from the reference point. In this case, the return of

the tool to the position of the reference point shall always be specified with G92 in the

workpiece coordinate system because the reference point is a specific point on the machine

and the program is developed on the basis of the workpiece coordinate system with a point on

the workpiece as its origin.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Note: G92 instruction is not necessary when the workpiece coordinate systems established

with G54～G59 are used.

3.3.8 Absolute value instruction and incremental value instruction

The distance that a cutting tool moves along all axes may be programmed with an incremental

instruction or absolute instruction.

It is possible to directly program a running distance in a block using an incremental instruction

(G91).

When using an absolute instruction (G90), the end position of the cutting tool is indicated with

a coordinates in the block.

In the above diagram, the program will give the following position when an incremental

instruction is employed:

G91 X-60.0 Y40.0；

In the above diagram, the program will give the following position when an absolute instruction

is employed:

G90 X40.0 Y70.0；

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The instruction mode of G90/G91 must not be changed for all addresses in a block so that the

program can be compatible with other NC.

3.4 Feed Function (F function)

3.4.1 Rapid traverse (positioning) function

All axes of the machine operate at the specified rapid traverse speed during rapid traverse.

As a rule, the rapid traverse speed has been set by manufacturer before shipment (set by

parameters RPDFX through RPDF4).

Since all axes of the machine moves individually, the times for all axes to move from their

home positions to end positions are different.

For example, when the rapid traverse speeds of axes X and Y reach 5m/min and 8m/min

respectively and movement program is as follows:

G91 X200.0 Y200.0；

The times for axes X and Y of the machine to run from the starting point to the end point are

24s and 15s respectively.

The locus of the cutting tool in the above example is as indicated in the figure below:

The control over the override of the rapid traverse speed can be achieved with the switch on

the operation panel of the machine. (FO, 25%, 50%, 100%) FO shall be determined by

setting parameter No.113 (SPDFL) and its unit shall not be indicated in percentage (%) but

mm/min or inch/min.

3.4.2 Cutting feedrate

The cutting feedrate shall be specified in the form of the distance per minute. The feedrate is

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

specified as follows with F codes:

F1 (1mm/min; 0.01inch/min)

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

The feedrate is restrained to the upper limit.

According to the upper limit, the manufacturer of the machine sets feedrate by parameter

No.106 (FEDMX) or exerts override restraint from 0 to 200% (10% each step) with the switch

on the operation panel. The control over upper limit speed is also effective for override feedrate.

The means of specifying feedrate with F codes is also applicable for the axis of rotation.

Example: To input in metric system F050

To input in Inch system F032

When inputting in metric and Inch system s, decimal point may be used for inputting

and it is located in the position of degree/min.

To input in metric system F12 0.12 degree/min

To input in Inch system F12 0.12 degree/min

To input in metric system F12.0 12 degree/min

To input in Inch system F12.0 12 degree/min

Note 1: Except the acceleration and deceleration processes in the row of NC, NC’s calculus error

regarding instructed feedrate is kept within ±2%. Moreover, the error is determined by

measuring a travel distance over 500mm when NC is in stable running state.

Note 2: The number of the digits of F codes is up to 7. Should the input feedrate is above the upper

limit, the feedrate is restrained to the upper limit.

3.4.3 To reduce feedrate to 1/10

The input speed in metric system can be changed to 1/10 of the original speed by parameter

No.006 BIT3 (FMIC) setting.

Item Minimum input unit Range

Feed per minute 0.1mm/min

F1 to F150,000 (0.1 mm/min to

15000.0mm/min)

3.4.4 Synchronous feed (feed per rotation)

It is possible to specify a feedrate in relation to the feed amount per minute of the spindle. G95

specifies synchronous feed while G94 feed per minute (with travel per minute as the feedrate).

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Meaning Address

G code

Input in

Range

Restraining

value

Override

A restraining value is set in mm/min or inch/min. Synchronous speed is converted to mm/min

or inch/min with the following formula:

fm=fr×R

Input in

inch

Both the feed per minute and synchronous feed at specific feedrate are

restrained. The restraining value is set by manufacturer (only the feedrate with

override is restrained).

The override from 0 to 200% (10% each step) is effective for both feed per

minute or synchronous feed.

Feed per minute Synchronous feed

Feed amount per minute of

cutting tool

F F

G94 G95

1mm/min～15000mm/min

(F1～F15000)

0.01inch/min～600.0inch/min (F1～F60000)

Feed amount of cutting tool per

rotation of spindle

0.01mm/r～500.00mm/r (F1～F50000)

0.0001inch/r～50.0000inch/r

Where fm: the feed per minute in mm/min or inch/min

fr: the synchronous feedrate in mm/r or inch/r

R: the rotational speed of the spindle in r/min

Note 1: Both G94 and G95 are modal. Once they are specified, they will be effective until other G

codes appear.

Note 2: The spindle shall be provided with a synchronous feed position coder.

Note 3: When the rotational speed of the position coder is as low as 1 rpm, the feedrate will become

irregular. The irregularity has no impact on the machining of the machine. Therefore it is still

usable when the rotational speed is as low as 1 rpm. However, the degree of irregularity must

not worsen more as the further reduction in rotational speed is subject to deterioration.

3.4.5 F1 digit feed

Specifying a digit (1～9) behind F sets the feedrate of the corresponding number. Feedrate is

preset for each number using parameter. Specify FO as the rapid traverse speed and set the

F1 digit feedrate switch on the machine panel to ON. Then rotate the manual pulse generator

to increase or reduce the feedrate of the currently selected number.

The increase or reduction in feedrate:

Fma

1×

F=△

100

Where: Fma×1 is used as the upper limit of feedrates of F1～F4 (set with a parameter).

/Manual pulse generator per case

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Fma×2: is used as the upper limit of feedrates of F5～F9 (set with a parameter).

X: Any figure between 1 and 127 (set with a parameter).

Set or modified feedrate can be saved even in case of power failure. The current feedrate is

displayed on the LCD.

3.4.6 Automatic acceleration and deceleration

During the start or stop of feed, acceleration or deceleration is performed at some time

constant so as to prevent the mechanical system from shock. Hence it is possible to consider

the problem of acceleration and deceleration during programming.

It is impossible to machine a sharp angle under the influence of automatic acceleration and

deceleration. To machine a sharp angle, dwell instruction (G04) must be added between two

blocks.

Once the dwell instruction is inserted, the actual tool path tallies with the programmed path.

The rapider feedrate is, the greater time constant of acceleration and deceleration and angle

error will be.

Note 1: The changes of feedrate between the blocks that have specified different moving modes are

as listed in the table below.

Foregoing blocks

New blocks

Positioning × × ×

Cutting feed ×

Not to move × × ×

×: The next block will be executed when the instruction speed is reduced to zero.

○: Continue to execute the next block so that the feedrate will not change excessively.

Note 2: Acceleration/deceleration is independently performed on both axes (axes X and Z) and their

feedrates changes between blocks, resulting in the discrepancy between the actual path of the

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

along axis Z in the next block, the movement in the direction of axis X starts to decelerate near

the angle. Meanwhile, it starts accelerated movement in the direction of axis Z. The actual path

Positioning Cutting feed Not to move

○

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

of the tool is as indicated in the figure below.

In arc interpolation, the actual arc radius is less than the programmed on (see the Appendix).

The deviation may be increased by minimizing the time constant of acceleration and

deceleration.

3.4.7 Automatic angle adjustment

Tool cutting is subject to overload if the tool performs the rough machining with tool

compensation in inner angle and inner arc area at programmed feedrate. The function

automatically reduces feedrate so as to lower the tool’s overload in the above machining areas,

thereby obtaining a smooth machining surface.

3.4.7.1 Automatic adjustment of inner angle

1) Working conditions

Feedrate can be automatically regulated provided that both the two blocks in succession

passing the angle satisfy the following requirements.

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

b. The offset is not 0 in offset mode.

c. Offsetting shall be performed inside the angle to be processed.

d. The axis moves along the offset surface.

e. Instructions G41 and G42 do not exit in the succeeding block.

f. Instructions G41 and G42 do not exist in the preceding block or the block is not started

though it has the two instructions.

g. The inner angle is less than the θ preset by parameter.

The angle judgment with regard to programmed path:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(I) Straight line Straight line

(II) Straight line Arc

(III) Arc Straight line

(IV) Arc Arc

The angle may be considered as an inner angle when θ≤θP. The value of θP shall be set by parameter (NO·335) (1°≤θP≤179°). It is subject to error in judgment less than 0.001° provided that θ is nearly equal to θP.

Operation range

When an angle is determined as an inner angle, feedrate is regulated from the range specified by the Lθ in the block on one side of the intersection point of the angle to the range specified by the Ls in the block one the other side of the intersection point. Ls and Lθ are the straight distances from one point on the path of the tool center to the intersection point. Lθand Ls are

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

set by different parameters (N0·355 and 356).

Feedrate is regulated in the range from point a to point b.

Feedrate is regulated within the range from Point a to Point b.

For an arc, the adjustment function is effective for the end point of a block provided that the

following requirements are fulfilled.

① Within the range of Lθ;

② The origin and end point of the arc are in the same quadrant or the origin is in the quadrant

adjacent to the one in which the end point is. Similarly, the adjustment of the origin of the

block is effective when the following conditions are met.

① Within the range of Ls;

② The origin and end point of the arc are in the same quadrant or the origin is in the quadrant

adjacent to the one in which the end point is.

(Example) For a disc:

For the program for an② arc, feedrate is regulated from point a to point b and from point c to

point d.

Amount of adjustment

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Amount of adjustment is set by No. 335 parameter.

1≤amount of adjustment (1% each step) ≤100 (%)

This is effective for commissioning and F1 digit instruction. For F4 digit instruction, the actual

feedrate will become:

Fx (inner angle adjustment) × (feedrate adjustment)

Whether inner angle adjustment is effective

Whether to adjust an inner angle or not may be selected with G codes. The inclusion of G62 in

the group 15 in which G61 and G64 are is as shown in the table below. These G codes are

related to accurate stop checking mode.

Accurate stop detecting mode Inner angle adjustment

G61 Valid Invalid

G62 Invalid Valid

G64 Invalid Invalid

Note 1: It is in G64 mode when powered on or cleared.

Note 2: It is necessary to specify G09 when you plan to perform accurate stop detection in G62 mode.

Note 3: The switch of inner arc cutting feedrate is always valid as described in Section 4.7.2 and is not

subject to the influence of G codes.

3.4.7.2 Switch of inner arc cutting feedrate

For inner arc offset cutting, the feedrate of programmed path shall be specified by F codes

while its actual feedrate F×R

radius of program path.

The switch is also effective for commissioning and F1 digit instruction.

(Example 1)

(where RC is the radius of the path of tool center and RP the

C/RP

However, if RC is much less than RP, i.e. RC/RP=0, the tool will stop. Therefore, when

≤MDR after the minimum reduction ratio (MDR) is set, the actual feedrate will be FX

C/RP

(MDR).

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

MDR is set by N0·333 parameter. When 1≤MDR (1% each step)≤100, it is applicable for F1

digit and commissioning. The reduction ratio of automatic inner angle adjustment is not under

the influence of MDR.

Note: If inner arc cutting is overlapped on automatic inner angle adjustment, now the actual

feedrate will be F×

× (angle adjustment)× (feedrate override).

3.5 Preparation Function (G function)

The two digits following address G determine the meaning that the concerned block involves.

G codes may be divided into the following two types:

Type Meaning

Primary valid G codes It is only valid in its instructed block.

Modal G codes

(Example) G01 and G00 are modal G codes.

G01 X ;

Y ; G01 is valid in this range.

After being instructed to be valid, the G codes become invalid only

when another G code in the same group is instructed.

X ;

G00 Y ;

Table 5.1: G codes list

G codes Group Function

G00 Positioning (rapid traverse)

G01 Linear interpolation (feed)

G02 Arc interpolation CW (clockwise)

G03

G04 Hold

G07 Speed sine-curve control (specified imaginary axis)

G09 Accurate stop detection

G10

G17 To select XY plane

G18 To select ZX plane

G19

G20 Input in inch

G21

G22 04 Storage travel limit ON

Arc interpolation CCW (counterclockwise)

Offset setting, workpiece zero offset setting

To select YZ plane

Input in mm

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G23 Storage travel limit OFF

G27 Reference point return check

G28 To return to reference point

G29 To return from reference point

G30 To return to the 2nd, 3rd and 4th reference points

G31

To skip over cutting

G33 01 Thread cutting

G40 To cancel tool compensation

G41 Tool compensation – left side

G42

Tool compensation – right side

G43 Forward compensation of tool length

G44 Reverse compensation of tool length

G49

To cancel tool length compensation

G45 To increase tool offset

G46 To reduce tool offset

G47 To increase tool offset by twice

G48

G50 Zooming OFF

G51

To reduce tool offset by twice

Zooming ON

G54 14 To select workpiece coordinate system 1

G55 To select workpiece coordinate system 2

G56 To select workpiece coordinate system 3

G57 To select workpiece coordinate system 4

G58 To select workpiece coordinate system 5

G59

To select workpiece coordinate system 6

G60 00 unidirectional positioning

G61 Accurate stop detecting mode

G62 To enable automatic angle adjustment

G64

Cutting mode

G65 00 Simple recall of a microinstruction

G66 Modal recall of microinstruction

G67

To cancel modal recall of microinstruction

G73 Gun drilling cycle

G74 Reverse-tapping cycle

G76 Finish boring

G80 To disable fixed cycle

G81 Drilling cycle, spotter

G82 Drilling cycle, counterboring

G83 Peck drilling cycle

G84 Tapping cycle

G85 Boring cycle

G86 Boring cycle

G87 Reverse boring cycle

G88 Boring cycle

G89

Boring cycle

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G90 Absolute value programming

G91

G92 Absolute zero programming

G94 Feed per minute

G95

G98 To return fixed cycle to the initial point

G99

G96

G97

(Note 1) The G codes marked with ^ are the initial G codes of all groups. That is, these G codes are

established when the system parameters specifying initial G codes are validated by

powering on or pressing the RESET key. For G22 and G23, G22 is selected when power is

switched on and G22 or G23 (one of them is valid before reset) is established after reset.

The selection of the state of the initial G codes such as G00, G01, G43, G44, G49, G90, G91

or G94 and G95 shall be set by parameters ((G00, G43, G44, G90 and G95).

For G20 or G21, the valid one is selected before powering off or pressing the RESET key.

Incremental value programming

Feed per rotation

To return fixed cycle to point R

(Note 2) The G codes in group 00 are modal and are only valid in the blocks they belong to.

(Note 3) When a G code not listed in the above table is specified or an optional G code not defined by

control unit is specified, (N0.0/0) will give an alarm. (N0.0/0) But G38 and G39 are ignored.

(Note 4) Some G codes may be specified in the same block even they do not belong to the same

group. When 2 or more G codes than belong to the same group are specified in a block, the

lastly specified G code will be valid.

(Note 5) If any G code in group 01 in fixed cycle mode, the fixed cycle will be automatically disabled

and the system will be in G80 state. However, the G codes in group 01 are not subject to the

influence of the G codes of fixed cycle.

(Note 6) G70 and G71 replaces G20 and G21 (special G codes) by parameter No.008 BIT5 (GSP)

setting.

(Note 7) The G codes of all groups are displayed.

3.5.1 Selection of planes (G17, G18, G19)

A plane is selected with the instruction for arc interpolation and tool compensation.

G17……XY plane

G18……ZX plane

G19……YZ plane

Travel instruction is not related to the selection of planes G17/G18/G19. For example, when

G17Z—— is specified, Z will move.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.5.2 Positioning (G00)

Using this code positions the tool at the points programmed by addresses X, Y and Z or A, B,

C, U, V and W. Coordinates shall be always specified in absolute instructions while the

distance from the origin to the end point in incremental instructions. All axes move the tool at

rapid traverse (positioning) rates individually and the tool path is not always straight line

during positioning.

2 axes (2 addresses) can be programmed concurrently in a block. But only one can be

programmed for the 4

G00 specifies a position.

G00α——β——:

(α·β=X, Y or Z)

Example: The program shall be as follows when the rapid traverse (positioning)rate is

9.600mm/min in the direction of axis X and 9.600mm/min in the direction of axis Y:

axis.

G00 X25.0 Y-10.0

Note 1: The rapid traverse (positioning) rate in G00 instruction is set for all axes respectively by

manufacturer. Therefore rapid traverse (positioning) rate can not be specified through

program.

In the positioning mode of G00, the tool start speeding up until it reaches the predetermined

speed. Then it rapidly travels and finally slows down to the end point. When it comes to the

“proper position”, the next block is executed in sequence (Note 2).

Note 2: The so-called “proper position” means motor feed is within the specified range (The range is

determined by manufacturer). The travel instruction in the following format may be specified

provided that the system selects three-axis link function.

G00 X——Y——Z——:

In this example, axes X, Y and Z move the tool to designated position in specified rapid

traverse.

When the system selects the linked control function with additional axes, not only addresses X,

Y and Z, but also the addresses of additional axes may be instructed. If they are instructed in

this way, 3 or 4 axes can move at the same time.

Example: X500.0 Y300.0 Z25.0 B20.0:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.5.3 Unidirectional positioning (G60)

For the accurate positioning without offset, final positioning can be achieved in only one

direction.

Origin

End point

(The direction for final positioning is from right to left.)

The condition that replaces G00 with G60 is as follows:

G60 α——β——γ——δ——:

(α, β and γ= X, Y and Z or additional axes A, B, C, U, V or W. This is the case of concurrent

control of 3 or 4 axes. The situation of concurrent control of 2 or 3 axes includes the selection

of one additional axis.

Overshoot and positioning direction are set by parameter. The tool stops once before the end

point even the positioning direction of instruction is identical with parameter setting.

Note 1: G60 is an one-off valid G code.

Note 2: Axis Z must not be positioned in a single direction in fixed drilling cycle.

Note 3: The axis whose overshoot has not been set by parameter shall not be positioned in a single

direction.

Note 4: When the travel distance instruction is O, unidirectional positioning will not be performed.

Note 5: When mirroring function is used, it is invalid to set its direction by parameter.

Note 6: Unidirectional position does not apply to fixed cycles G76 and G87.

3.5.4 Linear interpolation (G01)

G01α——β——F——:

(α, β and γ=X, Y, Z, A, B, C, U, V and W. Gang control is exerted for 4

This actually specifies linear interpolation mode. α and β defines the travel distance of the tool.

Whether the distance is in absolute or incremental mode depends on the current state of

G90/G91. Feedrate shall be specified by F codes, which are modal.

and other axes.)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Example of program: (G91) G01 X200.0 Y100.0 F200.0

Y End point

0 Origin 200.0 X

The feedrate instructed by F codes is the traveling speed of the tool. If F codes are not

specified, the feedrate is considered as 0.

The travel instruction (linear interpolation) with 3-axis gang control function is as follows:

G01 X——Y——Z——F——:

It is possible for the instruction to perform linear interpolation for 3 axes at one time.

When additional gang control function is selected, the addresses (A, B or C) of the fourth axis

may be used to replace X, Y or Z. In this way the 3-axis gang control involving the 4

axis can

be exerted.

Example: G01 X500.0 Y300.0 B20.0 F10.0:

When the system is provided with optional 4-axis gang control functio0n, the use of the

following instruction is allowed.

G01α——β——γ——δ——F——:

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

Note 1: Axial feedrates are as follows: G01αα

The feedrate in the direction of axis α: Fα=

ββ F f:

·f

The feedrate in the direction of axis β: Fβ=

·f

Note 2: The feedrate of an axis of rotation shall be instructed in degree/min (input in metric system:

F050; input in inch system: F032).

Example: G91 G01 B90.0 F300:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Note 3: In the linear interpolation involving the 4

axis (axis of rotation A, B or C), the unit of cutting

feed is changed from degree to inch (or mm) and the cutting feedrate in α—β rectangular

coordinate system is controlled so that it keeps identical with the speed specified by F codes.

The feedrate of an axis of rotation is determined with the formulas in Note 1 and its unit is

changed into degree/min.

E: G91 G01 X20.0 B40.0 F300.0:

When the unit (degree) of B-axis movement instruction is changed into mm or inch, machining

time shall be determined as follows:

4020

300

=0.014907 (min)

The feedrate of axis B is:

=268.3 °/min

14907.0

Note 4: For 3- or 4-axis link, the method for calculating the feedrate in rectangular coordinate system is

the same as 2-axis control.

Note 5: For inputting in Inch system and inputting in metric system, the upper limit of the feedrate of an

axis of rotation is approximately 6000°/min. The speed is fixed at the upper limit even the

feedrate of an instruction exceeds the upper limit.

3.5.5 Arc interpolation (G02, G03)

3.5.5.1 Arc interpolation without any additional axis

The instruction below moves the tool along the arc.

The arc in the X——Y plane:

G02 R——

G17 X——Y—— F——;

G03 I——J——

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The arc in the Z——X plane:

G02 R——

G18 X——Z—— F——:

G03 I——K——

The arc in the Y——Z plane:

G02 R——

G19 X——Z—— F——:

G03 J——K——

Item Instruction Meaning

G17 The arc in the plane of XY

1 Plane selection

G18 The arc in the plane of ZX

G19 The arc in the plane of YZ

G02 Clockwise (CW)

2 Rotating direction

G03 Counterclockwise (CCW)

The position of the end point in the

workspace coordinate system

The distance from the origin to the

end point

The distance from the origin to the

center

The position

of end point

The distance from the

starting point to the center

G90 mode 2 of axes X, Y and Z

G91 mode 2 of axes X, Y and Z

2 of axes I, J and K

Arc radius R Arc radius

Once the unit is switched on, G17 is enabled as the initial code for plane selection.

Whether it is in clockwise or counterclockwise direction depends on the left-manual or

right-manual coordinate system.

The end point of the arc is determined by address X, Y or Z and its indication in absolute or

incremental value by G90 or G91. In incremental indication, the coordinate of the end point is

specified from the origin of the arc.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The center of the arc is determined by the addresses I, J and K corresponding to axes X, Y and Z.

The digit following I, J or K is a coordinate component from the origin to the center of the arc and

they are always specified as an incremental value. The provision has no bearing upon G90 and

G91.

The marks of I, J and K correspond to the specified directions.

Arc interpolation may substitute I and J with R or gives an instruction with K. The instruction is

given in the following format:

G02

X——Y——R——:

G03

There are two types of arc in the arc interpolation with R (specified by radius) – the arc less

than 180° and more than 180°. Its analysis is as indicated in the diagram below.

Example of Instruction:

1． The arc less than 180°:

G02 X6.0 Y2.0 R5.0:

2． The arc over 180°:

G02 X6.0 Y2.0 R-5.0:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

a) Absolute programming

(1) G92 Ｘ200.0 Y40.0 Z0;

G90 G03 X140.0 Y100.0 I-60.0 F300.0;

G02 X120.0 Y60.0 I-50.0;

(2) G92 X200.0 Y40.0 Z0;

G90 G03 X140.0 Y100.0 R60.0 F300;

G01 X120.0 Y60.0 R50.0;

b) Increment programming

(I) G91 G03 X-60.0 Y60.0 I-60.0 F300;

G02 X-20.0 Y-40.0 I-50.0;

(II) G91 G03 X-60.0 Y60.0 R60.0 F300;

G02 X-20.0 Y-40.0 R50.0;

The tangential feedrate of arc interpolation is equal to the cutting feedrate specified by F codes.

However, the arc interpolation involving the fourth axis is not allowed.

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

Note 2: When the end point of an arc coincides with its origin, I, J and K are used to instruct a center of

a circle for programming a 360° arc (full circle) and X, Y and Z may be omitted.

Note 3: It will give No. 023 alarm if an arc of radius of 0 is programmed.

Note 4: The deviation of instruction feedrate from actual tool feedrate is less than or equal to ±2%. In

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

Note 5: If the addresses I, J, K and R are assigned to the same block, the arc specified by address R is

valid and other I, J and K are ignored.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.5.5.2 Arc interpolation with an additional axis

The arc interpolation with an additional axis is allowable. An axis (X, Y or Z) shall be set to

parallel with the additional axis by parameter setting. If the additional axis does not parallel with

any axis, arc interpolation will be impractical. G code for plane selection shall be specified for

arc interpolation. An address of an axis is specified with the G code for plane selection so as to

determine the axes performing arc interpolation.

Example: Assuming that additional axes U and W parallel with axes X and Y respectively.

a) G17X-Y-…………………XY plane

b) G17U-Y-…………………UY plane (U parallels with X)

c) G17Y-……………………XY plane

d) G17………………………XY plane

e) G17 X-Y-U-……… …Alarm

f) G18X-W-………………XW plane (W parallels with Z)

Addresses I, J and K may also be used to specify the center of the arc. This is similar to the arc

interpolation without any additional axis. The addresses I, J and K are used for the axes

parallel to axes X, Y and Z.

The arc interpolation specified with R is also valid.

3.5.6 Sine-curve interpolation

In spiral cutting instruction, sinusoidal interpolation is realized by specifying an arc instruction

axis not to move during arc interpolation. The imaginary axis is specified as follows:

G07α0: (Specify α as the imaginary axis)

G07α1: (Specify α as the real axis)

(α= X, Y, Z or additional axes A, B, C, U, V and W)

After instruction G07α0, axis α is deemed as an imaginary axis until G07α1 instruction is given.

For the single-period sine interpolation in Y-Z plane, axis X serves as an imaginary axis.

2+Y2

= r2 (r: arc radius)

Y = rsin(

)Z( l : the travel distance along axis Z in a single period)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

N001 G07 X0:

N002 G91 G17 G03 X-200 Y0.0 I-10.0 Z20.0 F100:

N003 G01 X10.0:

N004 G07 X1:

Axis X is deemed as an imaginary axis during N002～N003 blocks.

In the N003 block, spiral-curve cutting instruction is given in this way when axis Z is used a

linear axis. However, axis Y moves only when axis Z is performing sine interpolation since axis

X does not move.

In N003 block, the machine is in suspended state after interpolation because axis X does not

move.

Note 1: Imaginary axis is only available for automatic operation but not for manual operation.

Note 2: Interlock, travel limit and external deceleration are also available for imaginary axis.

Note 3: Manual insertion is also valid for imaginary axis. That is, the axis moves by manual insertion.

3.5.7 Thread cutting (G33)

The possibility of cutting determines the threads of screw pitch.

G33Z Z

Where Z is the length of thread (incremental instruction) or end point of thread (absolute

instruction)

F: f:

f: screw pitch

Input in mm

Input in inch

Minimum input increment Range

0.01mm F1 to F50000 (0.01mm to 500.00mm)

0.0001inch F1 to 500000 (0.0001inch to 50.0000inch)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Spindle axis is restricted as follows:

1≤R≤(Maximum feedrate/screw pitch) or allowable rotational speed of the position coder)

Where:

R: Spindle speed (r/min)

Screw pitch: mm or inch

Maximum feedrate: mm/min or inch/min

The instruction signal of maximum feed per minute or the maximum feedrate due to the

restriction of motor or machine, whichever is lower;

Allowable rotational speed of position coder: 4,000r/min (position coder A)

6, 000r/min (position coder B)

Note 1: Spindle speed may be read continuously through the position coder installed on the spindle.

The coder converts the spindle speed into the cutting feed per minute for purposes of feed.

Note 2: The converted cutting feedrate is not overridden but fixed at 100%.

Note 3: The converted cutting feedrate shall be fixed.

Note 4: Feed hold is invalid during thread cutting.

Example:

N20 G90 G00 X100.0 Y… S45 M03;

N21 Z200.0 ;

N22 G33 Z120.0 F5.0 ;

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

N23 M19;

N24 G00 X105.0 M03;

N25 Z200.0 M00;

N26 X100.0 M03;

N27 G04 X2.0 ;

N28 G33 Z120.0 F5.0 ;

Notes:

N20, N21: To locate the tool at the center of the hole and to clockwise (CW) rotate the spindle.

N22: To perform thread cutting for the first time with screw pitch specified by address F.

N23: M19 orders the spindle to stop in a fixed position on the circumference (M19: Spindle

stops in a fixed position).

N24: To withdraw the cutting tool in the direction of axis X.

N25: To move the cutting tool above the hole: M00 orders the program to stop and allows

operator to adjust the tool for the thread cutting for the second time.

N26: To align the cutting tool with the center of the hole and to start forward rotation of the

spindle.

N27: When the travel instruction in the N26 block is relatively short, it is necessary to add

another dwell instruction so that the spindle has adequate time to reach the rated

rotational speed.

N28: To perform thread cutting for the second time.

3.5.8 Automatic return to reference point (reference positions G27～G30)

3.5.8.1 Check of return to reference point (G27)

A point fixed on a machined plane is called reference point (reference position). Once a tool is

manually returned to a reference point, it is positioned at the point.

G27 instruction function is used to check that the tool is positioned at the reference point.

G27α—β—:

(α, β are selected from address X, Y and Z and additional axes A, B, C, U, V and W) The

instruction is used to rapidly position the tool at the reference point.

Once the tool reaches the reference point, the indicator indicating controllable axis’s return to

the reference point is lit.

After returning to the reference point, the next block will be executed if M00 or M01 does not

exist in M00 or M01. If the return to the reference point is not required in all cycles, optional

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

program skip function can be used.

If the system is provided with 3-axis gang control function, the G27 instruction may be

expressed in the following format:

G27α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and

W. However, only one axis can be controlled at one time if concurrent control of additional axes

is not selected.)

The use of the following instruction is allowable when 4-axis gang control is selected:

G27α—β—r—δ—:

Where α, β, r, δ= X, Y, Z, A, B, C, U, V or W

Note 1: In tool compensation mode, the position that the tool reaches with G27 is the position with

offset. In this case, the tool is also not at the reference point and the indicator for return to the

reference point does not illuminate. As a rule, G27 is only used for compensation cancellation

mode.

Note 2: In a inch mechanical system that inputs in metric system, the indicator illuminates even the

programmed position of the tool offsets from the reference point by 1μ as a result of that the

minimum input increment is less than the minimum traveling increment of the mechanical

system.

3.5.8.2 Automatic return to reference point (G28)

G28 α—β—:

(The addresses α and β shall be selected from X, Y, Z and additional axes A, B, C, U, V and W.

However, additional axes can only be individually controlled without additional axis gang

control function.)

The axis specified by the instruction can be automatically positioned at the reference point. As move instructions, α and β shall be specified in absolute/incremental value in G90/G91 mode.

The end point of the instruction is called “intermediate point” and the coordinates specified by

this instruction are saved to the NC.

The procedures in the G28 block are as follows:

First all controlled axes are positioned at intermediate points rapidly. Then they move from the

intermediate points to the reference points. If now the machine is not locked, the indicator for

return to the reference point is lit.

The positioning at the intermediate point and reference point in this way is equivalent to the

positioning of G00.

The instruction for 3-axis link is as follows:

G28α—β— r —:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and

W.) The following instruction is allowed for 4-axis link function.

G28α—β— r —δ—:

Where α, β, r, δ= X, Y, Z, A, B, C, U, V or W

Generally the G28 instruction is used for automatic tool change (ATC). In principle, tool radius

compensation, tool offset compensation and tool length compensation shall be cancelled

before executing the instruction.

Note 1: Not only the coordinates of move instruction, but also the coordinates of intermediate point is

saved to memory in the blocks of G28. This is, for the axes without instruction in the blocks of

G28, the foregoing coordinates in G28 serves as the coordinates of the intermediate point of

the axis.

Example: N1 G90 X100.0 Y200.0 Z300.0:

N2 G28 X400.0 Y500.0:

N3 G28 Z600.0:

Remarks:

N2: Intermediate point - 400.0, 500.0

N3: Intermediate point - 400.0, 500.0, 600.0

Note 2: After the system is switched on without manual return to the reference point, it moves from the

intermediate point when G28 is specified. This is similar to the manual return to the reference

point. Now the moving direction from the intermediate point has become the direction of return

to the reference point set by parameter.

Note 3: If G28 is instructed for an axis of rotation, the moving direction from the intermediate point to

the reference point has become the direction of return to the reference point. Furthermore, the

travel is within 360°.

3.5.8.3 Automatic return from reference point (G29)

G29α—β—:

(The addresses α and β shall be selected from X, Y, Z and additional axes A, B, C, U, V and W.

However, additional axes can not be interlocked with one the three basic axes if additional axis

gang control function is not selected.)

The tool may be positioned at the specified point through an intermediate point using this

function. As a rule, the instruction is used after a G28 instruction.

Α and β are specified in absolute/incremental value depending on the current G90/G91 state.

In an incremental instruction, an incremental value relative to the intermediate value shall be

specified.

Using the movement of the blocks of G29 allows all instructed axes to pass through the

intermediate point previously defined by G28 instruction and to reach the specified point at

rapid traverse (positioning) rate.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

The procedures for positioning at the intermediate point and then the specified point are similar

to the positioning with G00.

Example of G28 and G29 application:

For G91:

G28 X1000.0 Y200.0: (From A to B)

M06:

G29 X500.0 Y-400.0: (From B to C)

The example shows that programmer needs not to calculate the actual travel distance from the

intermediate point to the reference point. The G29 instruction for a system with 3-axis

concurrent control function is as follows:

G29α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and

W. However, additional axes can not be interlocked with one the three basic axes if additional

axis concurrent control function is not selected.)

The following instruction is allowed for the system with 4-axis link function:

G29α—β— r —δ—:

Where α, β, r, δ = X, Y, Z, A, B, C, U, V and W

Note: After the tool passes through the intermediate point and reaches the reference point

under the instruction of G29/30, the intermediate point shall move to a new coordinate system

in case of change in the position of workpiece coordinate system. Thereafter the tool shall pass

through the intermediate point that has moved to the new coordinate system and reach the

specified point when G29 is instructed.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.5.8.4 Return to the 2nd, 3rd or 4th reference point (G30)

The following instruction moves the specified axis to the 2nd, 3rd or 4th reference points (G30).

G30 P3 α—β—; (P2 may be omitted)

P2: The 2nd reference point

P3: The 3rd reference point

P4: The 4th reference point

Determining the positions of the 2

between the 1

reference point but to the 2nd, 3rd and 4th reference points, the function is similar to G28’s

reference points for field adjustment. Except that the tool does not return to the

instructions of return to reference point. After the G30 instruction, G29 instruction positions the

cutting tool to the specified position through the intermediated established by G30 instruction.

Its movement is the same as the situation of specifying G29 instruction after G28 instruction.

When the G30 instruction’s normal position of automatic tool change (ATC) varies from the

reference point, the G30 instruction is as follows if 3-axis link function is provided:

, 3rd and 4th reference points is to preset the distance

G30α—β— r —:

(The addresses α, β and r shall be selected from X, Y, Z and additional axes A, B, C, U, V and

W. However, additional axes can not be concurrently controlled along with one the three basic

axes if additional axis concurrent control function is not selected.)

The following instruction may be used when 4-axis gang control function is selected.

G30 P3 α—β— r —δ—;

Where α, β, r, δ = X, Y, Z, A, B, C, U, V or W

Note: After switching on, it is necessary to manually or automatically return to the reference

point once (G28) before executing the G30 instruction.

3.5.9 Dwell (G04)

G04X (t): or

G04P (t

Either of the above methods may be used for hold. After executing the previous block, It is

necessary to wait for (t) seconds before executing the next block.

The maximum instruction time is 99999.999s and time error is about 16ms.

Example: To suspend for 2.5s

G04 X2.5 or G04 P2500:

Note 1: Address P does not program with a decimal point.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Note 2: Dwell and time delay are applicable for the two conditions below and are enabled by

parameter setting.

1. After the speed of the foregoing block drops to 0

2. After the tool reaches the instruction value (after the inspection of locating point)

3.5.10 Accurate stop detection (G09)

A block involving G09 reduces its feedrate to 0 at the end point and affirms the state of locating

point (Note 2). Then the next block is executed. The function is used to machine a sharp edge

or corner. G09 is only valid in its specified block.

Note 1: Locating point detection is automatically performed in the locate modes (G00, G60) without

G09.

Note 2 Locating point means that a feed motor is within the range of the specified end point.

3.5.11 Accurate stop detecting mode (G61) and cutting mode (G64)

(1) Accurate stop detecting mode (G61)

The move instructions of all blocks following G61 decelerate to 0 at its end point until G64

instruction. They are determined as being in positioned state and then the next block is

executed.

(2) Cutting mode (G64)

The blocks following G64 do not accelerate until the end point of the move instruction of G61

but immediately go to the next block. Even in the G64 mode, feedrate is reduced to 0 and

positioning detection is performed under a positioning instruction (G00 or G60) or in the blocks

that has determined (G09) accurate stop detection.

3.5.12 Coordinate system setting (G92)

To move the cutting tool to a specific point with absolute instruction, make sure to preset the

coordinate system, which is established with the following instruction.

G92X (X) Y (Y) Z (Z) r (r) δ (δ):

(r, δ= A, B, C, U, V, W)

The instruction establishes a coordinate system whose origin is located at a point keeping a

specified distance from the tool. The following absolute instruction will refer to the coordinates

in the workpiece coordinate system.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G92 X25.0 Z23.0:

As shown in the above program, G92 is used at the beginning of the block to ensure the nose

of the tool coincides with the origin of the program.

G92 X600.0 Z1200.0:

As shown in the above diagram, G92 will confirm that the tool point coincides with the origin of

the program and execute an absolute instruction. The standard point is positioned at the

specified point. To position the nose of the tool to the specified point, the deviation of the nose

of the point from the reference point shall be corrected by tool length compensation.

Note 1: In the coordinate system established with G92 instruction in offset mode, the coordinates of

the tool in specified position does not include offset.

Note 2: Tool radius compensation is temporarily disabled by G92 instruction.

3.5.13 Workpiece coordinate system (G54～G59)

G92 instruction is not used to establish a workpiece coordinate system. However, the

machine’s six exclusive coordinate systems may be preset and selected with G54 and G59.

G54…………………Workpiece coordinate system 1

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

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

The six coordinate systems are determined by setting all axes’ distances (the offset of the zero

point of workpiece) from the reference point to their respective points.

Example: G55 G00 X100.0 Z20.0:

X15.5 Z25.5:

In the above example, it is positioned in the workpiece coordinate system 2 (X =100.0, Z =20.0)

and (X =15.5, Z =25.5).

Workpiece coordinate systems 1 to 6 are established after switching on and returning from the

reference point. G54 coordinate system is enabled upon switching on.

Note 1: When the range of the workpiece zero point offset of all axes compensated by external data

inputting (optional) is 0～±0.7999mm or 0～±0.7999mm, check the machine instruction

manual for the function.

Note 2:When G54～G59 are used, the coordinate system is not set with G92 but established with G92.

G54～G59 are used to move the coordinate system. G54～G59 must not be incorporated with

G92 except the special situation that G54～G59 are used to move the coordinate system.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

When the tool is positioned at (200, 160) in G54 mode, G92 X10 Y100; The specified

workpiece coordinate system 1 (X’, Y’) is moved by vector A. However, all other workpiece

coordinate systems shall concurrently offset vector A.

Note 3: When automatic coordinate system setting is not selected, proper parameter values shall be

set (309 APX～AP4).

3.5.14 To change workpiece coordinate system by program instruction

When the number of workpiece coordinate system becomes inadequate (although 6 are ready)

or when they are to be moved as required, we move them through programming instructions.

G10L2P P

Where P=1～6: the 1～6 X, Y, Z, r, δ (r, δ= one of A, B, C, U, V and W) of the corresponding

coordinate system: the workpiece zero offsets of all axes.

Note: External workpiece origin offset may be changed by setting P= 0.

X—Y—Z— r —δ:

3.5.15 Automatic setting of a coordinate system

A coordinate system may be set in the preset parameter number (375PPRTMX～441PPRTI5)

when returning to the reference point for the first time after switching on, namely it functions as

that G92 automatically sets a coordinate system at the reference point.

Note: If workpiece coordinate system setting function is enabled, it is necessary to set No.

375～378 and 400 parameters to 0 or No. 379～382 and 441 parameters to 0. If they are not

set to 0, the workpiece coordinate system

(1～6) will offset.

3.5.16 To switch between Inch and metric systems (G20, G21)

Inputting in metric or Inch system may be selected using G codes.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

System of units G codes Minimum input unit

Inch (Inch system ) G20 0.0001inch

mm (metric system) G21 0.001mm

Both the G codes must be instructed with a single block before the start of the program and

setting of the workpiece coordinate system.

N10 G20:

N20 G92 X—Y—:

The following items changes with the G codes:

(1) The feedrate instructed by F;

(2) Position indication;

(3) Offset

(4) The unit of the scale of the manual pulse generator;

(5) The travel of incremental feed;

(6) A part of parameters

Note 1: Once it is switched on, it enters into the state before power off.

Note 2: Switching between G20 and G21 in the midway of a program is not allowed.

Note 3: When the system of the units of the machine differs from that of the program, the maximum

deviation is 1/2 of the minimum traveling unit. The deviation value does not accumulate.

3.5.17 Storage travel limit (G22, G23)

The movable range of the tool may be restricted by the two means below.

(The tool does not enter the shadow area.)

Storage travel limit 1:

The outside of the boundary set by parameter is an exclusion area. As a rule, it shall not

change once it is set by manufacturer. Therefore it is set at the maximum travel of the machine

and is equivalent to the current so-called software limit.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Storage travel limit 2:

The outside or inside of the boundary set by parameter or instruction is an exclusion area.

Whether it is inside or outside is determined by parameter No.009 BIT6(RWL).

G22 instruction is used to stop the tool from entering the exclusion area and G23 to cancel the

restriction.

The instruction below is used to establish or change an exclusion area.

G22 X—Y—Z—I—J—K—:

X＞I, Y＞J, Z＞K

X－I＞2000 (Minimum instruction increment)

Y－J＞2000 (Minimum instruction increment)

Z－K＞2000 (Minimum instruction increment)

The points A and B in the figure below shall be involved during parameter setting.

, Y1＞Y2, Z1＞Z2

1＞X2

＞2000 (Minimum instruction increment)

1－X2

＞2000 (Minimum instruction increment)

1－Y2

＞2000 (Minimum instruction increment)

1－Z2

If the exclusion area is set by parameter, X, Y, Z, I, J and K shall be set by the minimum travel

unit (input unit) of the mechanical system with the reference as its origin.

If the exclusion area is set by G22 instruction, X, Y, Z, I, J and K shall be set by the minimum

travel unit (input unit) of the mechanical system with the reference as its origin. Then the

programming data is changed into the numerical value in the minimum traveling unit and the

value is set a parameter.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Since it is necessary to detect which part of the tool nose or clamp has entered the exclusion

area, the computing methods for X, Y, Z, I, J and K are different.

If point A is detected to enter into the exclusion area, a shall be set. If point B is detected to

enter into the exclusion area, b shall be set.

When point A is used to detect the nose of the tool, it is safe without changing the settings of

the tool each time if the tool of varied lengths are set to the required length.

Overlapped setting is possible for the area.

Note 1: All limits will become effective after power on and manual return from the reference point or

G28 completes automatic return from the reference point.

Note 2: If the reference point is within the exclusion area of all limits, the system immediately gives an

alarm when the storage travel limits are valid after power on and manual return from the

reference point. (For storage limit 2, only G22 mode is applicable.)

When G23 is changed to G22 and the tool is in the exclusion area, the system will give an

alarm in the next block.

Note 3: Pressing the emergent stop switch to cancel the restrictions and move the tool out of the

exclusion area in G23 mode when the tool remains still in the exclusion area under the

conditions of Note 2. The settings shall be changed if they are set incorrectly. Then the tool

returns from the reference point.

Note 4: Since the axis without the function of returning from the reference point, the axis does not give

an alarm in the exclusion area.

Note 5: For the setting of the exclusion area, the area is described as follows:

When the exclusion area is beyond the specified area, all the areas are movable.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

When the exclusion area is within the specified area, all the areas are restricted for movement

(in G22 mode).

Note 6: The settings beyond the travel of the machine are not necessary.

Note 7: The tool may reversely move provided that the tool is in the exclusion are and an alarm is

given.

Note 8: Even the sequence of the coordinates of the two points In the set area are set incorrectly, the

rectangle with the two points as its acmes can also be created into a limit area.

Note 9: G22 and G23 shall be instructed in single blocks.

Note 10: Storage travel limit 2 cannot be used for additional axes.

3.5.18 Skip function (G31)

The G31 followed by a move instruction is capable of instructing linear interpolation as G01. If

skip signal is input form the outside in the midway of the instruction, the remaining part of the

instruction will be interrupted and the next block will be executed.

G31 instruction is one-off and only valid in the instructed block.

The movement after skip signal depends on whether the next block is incremental or absolute.

1) The next block is an incremental instruction.

To make incremental movement from the break point:

Example: G31 G91 X100.0:

Y50.0:

The next block is an absolute instruction (only one axis)

The axis instructed in one block moves to the instructed position while those not instructed

remain in the positions input by skip signal.

Example: G31 G90 X200.0:

Y100.0:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

2) The next block is an absolute instruction (to instruct 2 axes)

The next block moves to the instructed position wherever skip signal is input.

Example: G31 G90 X200.0:

X300.0 Y100.0:

The feedrate of a block is specified （G31）with No. 306 (SKPF) parameter in the following two

ways:

a) Feedrate is specified with F codes (may be specified in the foregoing blocks or G31 block)

b) No. 342 parameter is set by No. 342 parameter.

The coordinates when skip signal is switched on are stored in the system variables #5061 to

#5065 of the user macro. Therefore they may be used in macros.

#5061………………………X coordinates

#5062………………………Y coordinates

#5063………………………Z coordinates

#5064………………………The 4

#5065………………………The 5

coordinates

The skip function may be used to the situation with unknown travel. Therefore, it is applicable

in the following conditions.

a) For the standard-dimension feed of the milling machine;

b) To enable tool contact pick-off to measure

Note 1: Once G31 instruction is performed in the active state of tool compensation C, No. 035 alarm

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

will be given. Tool compensation shall be canceled with G40 before G31 instruction.

Note 2: If the feedrate instructed by G31 is related to the speed set by parameter, it will have a bearing

upon parameter setting in no-load operation.

Note 3: If the feedrate instructed by G31 is related to the speed set by parameter, the automatic

acceleration/deceleration will be invalid. In this way the accuracy of automatic measurement in

skip function applications is improved.

3.6 Compensation

3.6.1 Tool length compensation (G43, G44, G49)

Using G43

Z—H—; or

G44

G43

H—;

G44

The end position of the axis Z move instruction is moved forward or reversely by setting the

offset set in the offset storage. Using this function may set the difference between the tool

length estimated in programming and the actual one in service into the offset storage to

achieve compensation without changing the program. H instructs the offset set into the offset

storage by instructing the offsetting direction with G43 and G44.

Offsetting direction

G43 Offset in + direction

G44 Offset in - direction

Whether in the situation of absolute or incremental instruction, the offset specified by H codes

and saved in the offset storage is added to the coordinates of the end point of the spindle move

instruction for G43 and detracted from it for G44. The calculated coordinates become the end

point of the coordinates. It may be illustrated in the same way when axis Z move instruction is

ignored as follows:

G43 G91 ZOH——; G44

The offset is positive for G43 and negative for G44.

G43 and G44 are modal G codes and, when instructed, are always valid if no G codes in the

same group are coded. G 43 or G44 code is valid upon power on depends on parameter setting.

Offset specification

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Offset number is specified with H codes. The offset set in the offset storage of the number is

added to or detracted from the programming value of axis Z. Offset number may be specified

with H00 or H200. The number of the D codes using tool radius compensation hits 32 (It is also

possible to choose 64, 99 or 200).

Offset corresponds to offset number and may be preset in the offset storage through MDI/LCD

or communicating operations. The setting range of the offset is as follows:

Input in mm Input in inch

Offset

0mm～±999.999mm 0 inch～±999.999inch

The offset of the corresponding offset No.00, i.e. H00 is generally 0. The offset corresponding

to H00 shall not be set.

Cancellation of tool length compensation

To cancel tool length compensation, G49 or H00 shall be instructed. Once H00 or G49 is

instructed, canceling operation will be performed.

(1) Example of tool length compensation (machining of #1, #2 and #3 holes)

H01= －4.0 (Offset)

N1 G91 G00 X120.0 Y80.0 ; ……………①

N2 G43 Z-32.0 H01 ; ……………②

N3 G01 Z-21.0 F1000 ; ……………③

N4 G04 P2000 ; ……………④

N5 G00 Z21.0 ; ……………⑤

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

N6 X30.0 Y-50.0 ; ……………⑥

N7 G01 Z-41.0 ; ……………⑦

N8 G00 Z41.0 ; ……………⑧

N9 X50.0 Y30.0 ; ……………⑨

N10 G01 Z-25.0 ; ……………⑩

N11 G04 P2000 ; ……………⑪

N12 G00 Z57.0 H00 ; ……………⑫

N13 X-200.0 Y-60.0 ; ……………⑬

Note 1: When offset is changed due to the change of the offset number, the new offset will not be

added to the original offset.

H01…………Offset 20.0

H02…………Offset 30.0

G90 G43 Z100.0 H01: ……Z will hit 120.0

G90 G43 Z100.0 H02: ……Z will hit 130.0

Note 2: D codes cannot be used for tool length compensation. Other axes except axis Z may employ

tool length compensation.

Which axis will be added with tool length compensation is instructed with axis address α in the

same block with G43 and G44

G43

α＿H＿: (α: any axis)

G44

Tool length compensation can only be added to an axis at one time. Therefore the system

gives an alarm in the following instructions. To switch an axis for tool length compensation, it is

necessary to cancel the one-off tool length compensation.

G43 Z＿H＿:

G43 X＿H＿: (Alarm)

3.6.2 Tool offset (G45～G48)

The moving distance of the specified axis may be zoomed in or zoomed out by the numerical values set in the offset storage through instructions G45～G48. G codes and their functions

are listed in Table 6.2.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Table 6.2: Tool offset and G codes

G codes Function

G45 To zoom in an offset

G46 To zoom out an offset

G47 To zoom in an offset by twice

G48 To zoom out an offset by twice

These G codes are modal and only valid in instructed blocks.

These amounts of compensation are instructed by D or H codes and remain unchanged once

they selected before selecting other amounts of compensation.

Whether tool offset compensation uses H or D codes is set by parameter No.010 BIT3

(OFSD).

In offset storage, the shape of the workpiece serves as the path of the tool for programming

during the setting of the radius of the tool.

Range of offset

Input in metric system Input in Inch system

Offset value

0mm～±999.999mm 0”～±99.9999”

～±999.9990 0

The offset function is valid for an additional axis (the 4

When the offset number is 00 (H00 or D00), the offset will also be 0.

Zooming is made in the moving direction of the tool of the axis. When the absolute value

instructs, the tool starts to move to the position instructed by the instructions in the blocks of

G45～G48 and makes zooming compensation.

1) G45 instruction (only to lengthen the offset)

axis).

～±999.9990

～～～～～～～ Move instruction value

Offset

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Actual travel

a) Move instruction +12.34 offset +5.67 b) Move instruction+12.34 offset

c) Move instruction offset +5.67 d) Move instruction -12.34 offset -5.67

2) G46 instruction (only to reduce by one offset)

If the sign of the offset is reversed in G45 instruction, it will be identical with G46.

a) Move instruction+12.34 offset+5.67(b)～(d) (omitted)

3) G47 instruction (lengthen the offset by twice)

a) Move instruction+12.34 offset+1.23 b) Move instruction+12.34 offset-1.23

c) Move instruction-12.34 offset+1.23 d) Move instruction-12.34 offset-1.23

4) G48 instruction (to reduce the offset by twice)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

If the sign of the offset is reversed in G47 instruction, it will be identical with G48.

a) Move instruction+12.34 offset +1.23(b)～(d) (omitted)

When offset is moved in the mode of incremental instruction (G91), the instruction for travel will

be 0. No movement will be performed if the travel instructed in the mode of absolute instruction

(G90).

Offset +12.34 (offset No. 01)

NC instruction G91 G45 X0 D01: G91 G46 X0 D01: G91 G45 X-0 D01 G91 G46 X-0 D01:

Equivalent

instructions

X12.34 X-12.34 X-12.34 X12.34:

Note 1: If one of G45～G48 is specified for 2-axis gang control, the tool offset is valid for both axes.

For G45

Move instruction X1000.0 Y5000.0

Offset +200.0 Offset No. 02

Programming instruction G45 G01 X1000.0 Y500.0 D02:

Note 2: During bevel machining, it is subject to overcutting or under-cutting if tool offsetting is

performed.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G01 X

G47 X

F ； Y ；

Y ；

G01 G45 X

G45 Y ；

F D ；

Y ；

Note 3: When the offset is higher than the move instruction value, the actual moving direction of the

tool will be contrary to the programmed direction.

Example: G46 X2.50;

(Incremental instruction) Equivalent to X-1.20:

Offset+3.70

Note 4: For arc interpolation (G02, G03), only the tool offset under the conditions of 1/4 and 3/4 circles

may be resulted by G45 to G48 instructions. That is, tool compensation is only available for 1/4

and 3/4 arc instructions.

Example 6.21: Offset +20.0, Offset No. 01

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Example of programming:

(G91)

G45 G03 X-70.0 Y70.0 I-70.0 D01:

Example 6.22: The tool position offset during arc interpolation

N1 G46 G00 X—Y—D—;

N2 G45 G01 Y—F—;

N3 G45 G03 X—Y—I—;

N4 G01 X—;

Example 6.23: The program with tool offset

Tool radius compensation

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

1. G91 G46 G00 X80.0 Y50.0 D01;

2. G47 G01 X50.0 F120;

3. Y40.0;

4. G48 X40.0;

5. Y-40.0;

6. G45 X30.0;

7. G45 G03 X30.0 Y30.0 J30.0;

8. G45 G01 Y20.0;

9. G46 X0; …… Only to move the offset in the direction of -X

10. G46 G02 X-30.0 Y30.0 J30.0;

11. G45 G01 Y0; …………Only to move the offset in the direction of -Y

12. G47 X-12.0;

13. G47 Y-80.0;

14. G46 G00 X-80.0 Y-50.0;

Note 5: Only axis Z moves an offset if H codes are used in G43 or G44 mode. Therefore, it is

recommended not to use H codes but D codes in the offsets of G45～G48 as much as

possible.

Note 6: G45～G48 modes are ignored in fixed cycles. Hence G45～G48 shall be programmed before

instructing fixed cycles and they must always be cancelled after fixed cycles.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Note 7: Tool offset modes (G45 ～ G48) are not allowed in the modes of G41 or G42 (tool

compensation); otherwise P/S alarm will be given (alarm no. 36).

3.6.3 Tool radius compensation (G40～G42)

3.6.3.1 Tool radius compensation function

As shown in the figure below, to machine the workpiece indicated by A in the figure with a tool

of radius R, the corresponding tool center must always be B path keeping a distance of R away

from A. Moving the tool from the workpiece by one distance in this way is called offsetting. The

tool compensating function is used to determine the path (i.e. offset) of the tool that has moved

for a distance.

Therefore, programmer may use the tool offset mode to program the outline of a workpiece.

Furthermore, if tool radius (offset) is measured and set in the NC during machining, the tool

path will be offset (path B) regardless the programmed path.

Two types of tool compensation (B and C) are available. This section only describes type C.

The difference between B and C is as follows:

In the mode of type B tool compensation, inward offsetting cannot be performed for angles

equal to or less than 90°. In this condition, make sure to program it into a proper inward arc.

3.6.3.2 Offset (D codes)

At most 32 amounts of offset may be set in the offset storage (64, 99 and 200 are optional)

(including 32 amounts of offset for tool length compensation and tool position offsetting). The

offset depends upon the D instructed in program and the number of digits is set with MDI/LCD.

The range of programmable offsets is as follows:

Input in mm Input in inch

Offset

The offset corresponding to No. 00 or D00 is always 0.

0mm ~

999.999mm 0inch ~ ± 99.9999inch

So the offset corresponding to D00 need not be set.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

3.6.3.3 Offset vector

Two-dimensional offset vector is equal to the vector of the offset specified by D codes. It is

determined in the control unit and its direction is duly corrected in accordance with tool feed of

all axes. The offset vector (hereafter called “vector”) is generated in the control unit so as to

determine the amount of tool offsetting movement and calculate the actual path that the tool

radius offsets from the programmed path. The offset vector will be cleared away by reset.

The vector changes with the movement of the tool. It is very important to know the status of the

vector during developing a program. Please read the following sections and carefully make

certain how the vector is generated.

3.6.3.4 Plane selection and vector

The calculation of offset is performed in the plane established by G17, G18 and G19, which is

called offset plane. For instance, (X, Y) or (I, J) is used to calculate the offset as well as vector

when XY plane is selected. The coordinates of the axes beyond the offset plane are not under

the influence of offset but follows instructed value in the instruction.

In 3-axis gang control, the tool path projected on the offset plane is compensated.

Plane selection switching shall be performed in the mode of offset cancellation. No. 027 alarm

will be given if plane selection switching is performed in offset mode.

G codes Offset plane

G17

G18

G19

To set an offset plane with an additional axis, it is necessary to preset which one in axes X, Y

and Z that the additional axis parallels with by parameter. When none axis it parallels with, the

offset plane cannot be defined.

While setting the offset plane with an additional axis, the additional axis shall be instructed at

the same time with the G codes, i.e. G17, G18 and G19.

a) G17 X_Y_; ……XY plane

b) G17 U_Y_; ……UY plane (U parallels with axis X)

X－Y plane Z－X plane Y－Z plane

c) G17 Y_; ………XY plane

d) G17; …………XY plane

e) G17 X_Y_U_; ……Alarm

f) G18 X_W_; ……XW plane (W parallels with axis Z)

3.6.3.5 G40, G41 and G42

G40, G41 and G42 are used to specify the cancellation and generation of a tool radius

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

compensation vector. To determine the direction of an offset vector and the moving direction of

the tool, G40, G41 and G42 may be instructed concurrently with G00, G01, G02 or G03.

G codes Function

G40 To cancel tool compensation

G41 Tool compensation, left

G42 Tool compensation, left

G41 or G42 instruction allows the system to enter into offset mode.

G40 instruction allows the system to enter into cancellation mode.

An example of offsetting course will be illustrated in the following figure.

Start-up block ①: Offset cancellation mode becomes offset mode (G41) in this block. The tool

center is offset at the end point (P

section of program path (from P

) of the block by the radius perpendicular to the lower

). The tool compensating value is specified by D07, i.e.

1~P2

offset No.7. G41 means that the tool offsets to the left.

After workpiece shape P

——→P8→P9→P1 programming and starting, the system

1→P2

automatically performs tool compensation.

In block ①, the tool returns to the point of origin (offset cancellation) through G40. The tool

center moves (from P

) normal to the programmed path at the end point of the 10th block.

9～P1

G 40 instruction (program cancellation) shall be instructed at the end point of the program.

Example of program for tool compensation C:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G92 X0 Y0 Z0

① N1 G90 G17 G00 G41 D07 X250.0 Y550.0: (The offset is preset in D07 by MDI)

② N2 G01 Y900.0 F150:

③ N3 X450.0:

④ N4 G03 X500.0 Y1150.0 I-600.0 J250.0:

⑤ N5 G02 X900.0 I200.0 J150.0:

⑥ N6 G03 X950.0 Y900.0 I250.0 J0:

⑦ N7 G01 X1150.0:

⑧ N8 Y550.0:

⑨ N9 X700.0 Y650.0:

⑩ N10 X250.0 Y550.0:

⑪ N11 G00 G40 X0 Y0:

3.6.3.6 Details about tool radius compensation C

The tool radius compensation C is described in detail as follows.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(1) Cancellation mode

The system will be in offset cancellation mode after power on, reset or completion of the

program by executing M02 and M03.

In cancellation mode, the vector is always 0 and the tool center path coincides with the

programmed path. It shall be ended up by means of cancellation at the end of the program.

When the program ends in offset mode, positioning the tool at the end point of the program

cannot be performed and the position of the tool will offset from the end position by a vector.

(2) Start-up

When a block satisfying all the following requirements is executed in cancellation mode, the

system will be in offset mode. This block is called start-up block.

a) G41or G42 has been instructed and the system is in the state of G41 or G42.

b) Tool compensation number is not D00.

c) Axes (other than axes I, J and K) (even one axis is acceptable) in the offset plane is

allowable and their travel is not 0.

In a start-up block, arc instructions (G02, G03) shall not be used; otherwise the NC will gives

No. 34 alarm and stops operation. The NC reads in two blocks. The next block enters into the

tool compensation buffer register (the contents of the register cannot be displayed) once the

first block is read in and executed.

In addition, two blocks in succession are read in when the system is in single block mode. The

block is firstly read in stops after execution. As a rule, two blocks are normally read in after that.

Hence there are three blocks in the NC, namely the executing block and the next two blocks.

Note: The meaning of the so-called interior angle and other terms are as indicated in the

following figure. The intersection angle of the move instructions of two blocks is called “interior

angle” when its angular degree on the workpiece side is above 180° and “exterior angle” when it falls within 0°～180°.

(i) To machine along the interior side

Straight line → Straight line

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Where:

S indicates the dwell point of single block.

L indicates line motion.

C indicates arc motion.

Straight line → Arc

(ii) When the tool machines one side of an obtuse angle, the start-up and cancellation of a

(90°≤α≤180°) tool path have the noses A and B and they are selected by parameter No.011

BIT1 (SUPM).

Type A: (Straight line → Straight line)

(Straight line → Arc)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Type B: (Straight line → Straight line)

Intersection point is a point at which the offset paths determined by two blocks in

succession intersect.

(Straight line → Arc)

The intersection point in the above diagram is a point where the offset paths of the r length

of two blocks.

(iii) To machine an acute angle (α＜90°＝exterior)

Type A (Straight line → Straight line)

(Straight line → Arc)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Type B (Straight line→ Straight line)

(Straight line→ Arc)

Note: For Type B, compensation shall be performed as follows when the tool moves on one

side of a sharp angle less than 1

(3) Offset mode

In offset mode, arc interpolation may offset even linear interpolation is instructed.

In offset mode, the blocks without move instruction but miscellaneous function, hold, etc

cannot be instructed in two blocks in succession; otherwise it is subject to undercutting or

overcutting.

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Offset plane cannot be changed in offset mode; otherwise the system will stop after No. 37

alarm.

(i) Situations of interior angle (180°≤α)

Straight line→ Straight line

Straight line→ Arc

Arc→ Straight line

Arc→ Arc

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

For the condition of straight line to straight line, a narrow and closed angle less than 1° is

machined. Now its offset vector becomes extremely big.

User may follow the above procedures for the conditions of arc to straight line, straight line

to arc and arc to arc.

(ii) To machine an obtuse angle along the exterior side (90°≤α＜180°)

Straight line →Straight line

Straight line →Arc

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Arc→ Straight line

Arc→ Arc

(iii) To machine an acute angle along the exterior side

Straight line →Straight line

Straight line →Arc

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Arc→ Straight line

Arc→ Arc

Note 1: Special cases

When the end point of an arc is not on it

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

If there is a lead on the arc as shown in the diagram, use the arc center connecting to the

end point of the arc as the center of a circle to make a imaginary arc. Make a vector for

compensation by using the imaginary arc as the arc of tool compensation. Its result varies

from the tool center path that uses the arc lead a lead for tool compensation.

Follow the same procedures for the situation of arc → arc.

The situation without an internal intersection point

As shown in the diagram below, arc intersection point exists on compensation path when

the offset is small. Increase in the offset eliminates the intersection point. Now the system

gives No. 33 alarm and stops at the end point of the previous block.

As shown in the diagram below, arc intersection point P exists on compensation paths of arc A

and arc B when the offset is small. Increase in the offset eliminates the intersection point. For

that center coincides with the origin or end point, the system gives No. 38 alarm and stops

program execution at the end point of the previous block.

(4) Offset cancellation

When executing a block satisfying one of the following requirements in offset mode, the

system enters into tool cancellation mode. The function of the block is called offset

cancellation.

（G41 mode）

N5 G01 X1000;

N6 G02 X1000 I0 J0;

N7 G03 Y-1000 J-1000;

(a) G40 is instructed (b) D00 is instructed as a tool compensation number.

(G02) and (G03) cannot be instructed when offset cancellation is performed. If they are

instructed, No. 34 alarm will be sent out and NC will stop.

When a block is read in offset cancellation mode, two blocks including that stored in the buffer

(not display) for tool compensation will be executed. In single block mode, a block is read in

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

and executed before stop. The next block is read in and executed by pressing the START

button.

After the control system enters into cancellation mode, the next executed block will be normally

saved in the buffer register rather than typed in the tool compensation buffer register.

(a) To machine an interior angle (α≥180°)

Straight line →Straight line

Arc→ Straight line

(b) To machine an exterior angle (90°≤α＜180°, obtuse angle)

(i) Type A

Straight line →Straight line

Straight line →Arc

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(ii) Type B

Straight line →Straight line

Arc→ Straight line

(i) Type A

Straight line →Straight line

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

Arc→ Straight line

(ii) Type B

Straight line →Straight line

Arc→ Straight line

Note: For the situation of type B, compensation is performed as follows when the tool machine

an acute angle below 1

by means of straight line to straight line from the exterior side:

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(5) G codes for tool compensation in offset mode

It is possible set an offset vector in relation to the direction of the foregoing block by individually

instructing G codes (G41, G42) for tool compensation in offset mode so as to create a correct

angle. It is independent of the inner wall or outer wall to be processed.

Correct arc motion cannot be performed provided that the codes (G41, G42) are included in an

arc instruction.

To reverse the direction of compensation through the G codes (G41, G42) for tool

compensation, refer to Note 2: To change offsetting direction in offset mode.

Straight line →Straight line

Arc→ Straight line

Note 2: Change offsetting direction in offset mode.

Offsetting direction is identified with the G codes (G41 and G42) for tool compensation and

offset signs as follows:

Offset signs

＋－

G codes

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

G41 Offsetting to the left Offsetting to the right

G42 Offsetting to the right Offsetting to the left

In special cases, offsetting direction can be changed by switching between G41 and G42 in

offset mode. However, it cannot be changed for the start-up block and the block that follows. In

the situation of changing offsetting direction, the concepts of interior side and exterior side are

canceled to adapt to all conditions. The amounts of offset are assumed to be positive in all the

following examples.

(Straight line →Straight line)

(Straight line →Arc)

(Arc→ Straight line)

GSK983M Milling CNC System Operation Manual (Volume I: Specifications and Programming)

(Arc→ Arc)

When a path with offset has not intersection point:

If the switch between G41 and G42 is performed and there is no intersection point of offset

path from block A to block B, a vector perpendicular to the programmed direction will be

established at the point of origin of block B.

gsk GSK983M Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual