gsk GSK25i Programming Manual

This user manual describes all items concerning the operation of this CNC system in detail. However, it is impossible to give particular descriptions for all unnecessary or unallowable operations due to length limitation and products application conditions; Therefore, the items not presented herein should be considered impractical or unallowable.

Copyright is reserved to GSK CNC Equipment Co., Ltd. It is illegal for any organization or individual to publish or reprint this manual. GSK CNC Equipment Co., Ltd. reserves the right to ascertain their legal liability.

GSK 25i Milling CNC System User Manual

Preface

Your Excellency,

We are honored by your purchase of this GSK 25i Milling CNC System made by GSK CNC Equipment Co., Ltd.

This book is “Programming and Operation” section of the User Manual Volume I.

Special caution:

The power supply fixed on/in the cabinet is exclusively used for the CNC system made by GSK.

It can't be applied to other purposes, or else it may cause serious

danger.

II

Volume I Programming and Operation

Warning and Precaution

Accident may occur by improper connection and operation This system can only be operated by authorized and qualified personnel.

Please read this manual carefully before operation

Please read this manual and a manual from machine tool builder carefully before installation, programming and operation, and strictly observe the requirements.

This manual includes the precautions for protecting user and machine tool. The precautions are classified into Warning and Caution according to their bearing on safety, and supplementary information is described as Note. Read these Warnings, Cautions and Notes carefully before operation.

Warning

User may be injured or equipment be damaged if operation instructions and procedures are not observed.

Caution

Equipment may be damaged if operation instructions or procedures are not observed.

Note

It is used to indicate the supplementary information other than Warning and Caution.

III

GSK 25i Milling CNC System User Manual

Precautions

■Delivery and storage

●Packing box over 6 layers in pile is unallowed.

●Never climb the packing box, neither stand on it, nor place heavy objects on it.

●Do not move or drag the products by the cables connected to it.

●Forbid collision or scratch to the panel and display screen.

●Avoid dampness, insolation and drenching.

■Open-package inspection

●Confirm that the products are the required ones.

●Check that the products are not damaged in delivery.

●Confirm that the parts in packing box are in accordance with the packing list.

●Contact us in time if any inconsistence, shortage or damage is found.

■Connection

●Only qualified personnel can connect the system or check the connection.

●The system must be earthed, and the earth resistance must be less than 0.1Ω. The earth wire cannot be replaced by zero wire.

●The connection must be correct and firm to avoid any fault or unexpected consequence.

●Connect with surge diode in the specified direction to avoid damage to the system.

●Switch off power supply before plugging out or opening electric cabinet.

■Troubleshooting

●Only competent personnel are supposed to inspect the system or machine.

●Switch off power supply before troubleshooting or changing components.

●Check for fault when short circuit or overload occurs. Restart can only be done after troubleshooting.

●Frequent switching on/off of the power is forbidden, and the interval time should be at least 1 min.

IV

Volume I Programming and Operation

Announcement

●This manual describes various possibilities as much as possible. However, operations allowable or unallowable cannot be explained one by one due to so many possibilities that may involve with, so the contents that are not specially stated in this manual shall be considered as unallowable.

Caution

●Functions, technical indexes (such as precision and speed) described in this user manual are only for this system. Actual function deployment and technical performance of a machine tool with this CNC system are determined by machine tool builder’s design, so functions and technical indexes are subject to the user manual from machine tool builder.

●Refer to the user manual from machine tool builder for function and meaning of keys on control panel.

V

GSK 25i Milling CNC System User Manual

Safety Responsibility

Manufacturer’s Responsibility

——Be responsible for the danger which should be eliminated and/or controlled on design and configuration of the provided CNC systems and accessories.

——Be responsible for the safety of the provided CNC systems and accessories.

——Be responsible for the provided information and advice for the users.

User’s Responsibility

——Be trained with the safety operation of CNC system and familiar with the safety operation procedures.

——Be responsible for the dangers caused by adding, changing or altering to the original CNC systems and the accessories.

——Be responsible for the failure to observe the provisions for operation, adjustment, maintenance, installation and storage in the manual.

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

This manual is reserved by end user.

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

VI

	Volume I Programming and Operation
	Contents
GENERAL ......................................................................................................................................		1
1 GENERAL ........................................................................................................................................		2
1.1	General...................................................................................................................................	2
1.2	Notes for Reading this Manual ...............................................................................................	2
PROGRAMMING ...........................................................................................................................		3
1 GENERAL ........................................................................................................................................		4
1.1	Definition ................................................................................................................................	4
1.2	Program Configuration ...........................................................................................................	4
	1.2.1 Program Name.............................................................................................................	4
	1.2.2 Sequence Number and Block.......................................................................................	5
	1.2.3 Word.............................................................................................................................	5
1.3	General Program Structure ....................................................................................................	6
	1.3.1 Subprogram Writing and Call .......................................................................................	7
	1.3.2 Program Inputting Format ............................................................................................	8
	1.3.3 Program End ................................................................................................................	9
	1.3.4 Optional Block Skip / ............................................................................................	9
2 PROGRAMMING FUNDAMENTALS...........................................................................................		11
2.1	Controlled Axes ....................................................................................................................	11
2.2	Axis Name............................................................................................................................	11
2.3	Coordinate system................................................................................................................	11
	2.3.1 Machine Coordinate System ......................................................................................	11
	2.3.2 Reference Point..........................................................................................................	12
	2.3.3 Workpiece Coordinate System...................................................................................	12
	2.3.4 Maximum Stroke ........................................................................................................	13
	2.3.5 Absolute and Incremental Programming ....................................................................	13
2.4	Modal and Non-Modal ..........................................................................................................	14
2.5	Decimal Point Programming.................................................................................................	15
2.6	Basic Functions ....................................................................................................................	15
	2.6.1 Tool Movement along Workpiece Parts Figure—Interpolation ...................................	15
	2.6.2 Feed—Feed Function.................................................................................................	16
	2.6.3 Cutting Speed, Spindle Speed Function.....................................................................	17
	2.6.4 Command for Machine Operations—Miscellaneous Function....................................	17
	2.6.5 Selection of Tool Used for Various Machining—Tool .................................................	17
	2.6.6 Tool Figure and Tool Motion by Program ...................................................................	18
3 PREPARATORY FUNCTION G CODES .......................................................................................		20
3.1	Types of G codes .................................................................................................................	20
3.2	Simple G Code .....................................................................................................................	23
	3.2.1 Positioning (G00)........................................................................................................	23
	3.2.2 Linear Interpolation G01.............................................................................................	24

VII

GSK 25i Milling CNC System	User Manual
3.2.3 Circular Interpolation (Helical Interpolation) G02/G03................................................	25
3.2.4 Cylindrical Interpolation (G07.1).................................................................................	30
3.2.5 NURBS Interpolation..................................................................................................	32
3.2.6 Dwell (G04) ................................................................................................................	37
3.2.7 Single Direction Positioning G60 ..........................................................................	38
3.2.8 Skip Function G31......................................................................................................	40
3.2.9 System Parameter Online Modification (G10)............................................................	42
3.2.10 Workpiece Coordinate System G54 G59...............................................................	43
3.2.11 Optional Angle Chamfering and Corner Rounding ...................................................	46
3.2.12 Selecting a Machine Coordinate System (G53) .......................................................	48
3.2.13 Floating Coordinate System (G92)...........................................................................	49
3.2.14 Local Coordinate System (G52)...............................................................................	50
3.2.15 Plane Selection G17/G18/G19.................................................................................	52
3.2.16 Starting/Canceling Polar Coordinate (G16/G15) ......................................................	52
3.2.17 Scaling in the Plane G51/G50..................................................................................	55
3.2.18 Coordinate System Rotation G68/G69.....................................................................	60
3.2.19 Inch/Metric Conversion (G20/G21)...........................................................................	64
3.2.20 Adding Workpiece Coordinate Systems G54.1Pn ..............................................	65
3.3 Reference Position G Codes .............................................................................................	66
3.3.1 Reference Point Return Check G27...........................................................................	66
3.3.2 Reference Point Return G28......................................................................................	67
3.3.3 Return from the Reference Position G29 ...................................................................	69
3.4 Canned Cycle G Codes .....................................................................................................	71
3.4.1 High-speed Peck Drilling Cycle G73 ..........................................................................	76
3.4.2 Left-handed Tapping Cycle G74 ................................................................................	77
3.4.3 Fine Boring Cycle G76 ...............................................................................................	79
3.4.4 Canned Cycle Cancel G80.........................................................................................	81
3.4.5 Drilling Cycle, Spot Drilling (G81)...............................................................................	82
3.4.6 Drilling Cycle, Counter Boring Cycle G82 ..................................................................	83
3.4.7 Peck Drilling Cycle (G83) ...........................................................................................	85
3.4.8 Right-handed Tapping Cycle G84..............................................................................	86
3.4.9 Boring Cycle G85 .......................................................................................................	88
3.4.10 Boring Cycle G86 .....................................................................................................	90
3.4.11 Boring Cycle, Back Boring Cycle (G87) ...................................................................	91
3.4.12 Boring Cycle (G88)...................................................................................................	93
3.4.13 Boring Cycle (G89)...................................................................................................	95
3.4.14 Left-handed Rigid Tapping Cycle G74 ...............................................................	97
3.4.15 Right-handed Rigid Tapping Cycle (G84).................................................................	99
3.4.16 Rough of the Groove in the Circle (G110/G111) ....................................................	103
3.4.17 Finishing the Whole Circle Cycle( G112/G113)......................................................	105
3.4.18 Protruding Roughing Outside of the Circle (G114/G115) .......................................	107
3.4.19 Outside of the Circle of External Circle (G116/G117).............................................	109
3.4.20 Roughing Rectangle Groove (G130/G131) ............................................................	111
3.4.21 Finishing Cycle in the Rectangular Groove (G132/G133) ......................................	113
3.4.22 Roughing Cycle Outside of the Rectangle (G134/G135)........................................	115
3.4.23 Finishing cycle outside of the Rectangle (G136/G137) ..........................................	116
3.5 Tool Compensation Function .............................................................................................	118

VIII

	Volume I Programming and Operation
	3.5.1 The Tool Length Compensation G43, G44 and G49................................................	118
	3.5.2 The Tool Radius Compensation C G40 G42 ...................................................	121
	3.5.3 The Detailed Introduction of the Tool Radius Compensation ...................................	127
	3.5.4 Corner Offset Arc Interpolation G39 .................................................................	154
	3.5.5 The Tool Compensation Value and Number Input the Compensation Value by the
	Program ............................................................................................................................	156
	3.5.6 Automatic Tool Length Measurement (G37) ............................................................	156
	3.5.7 Tool Position Offset (G45-G48)................................................................................	159
3.6 The Special Canned Cycle Commands ...........................................................................		162
	3.6.1 Circumference Holes Cycle(G120)...........................................................................	163
	3.6.2 The Angle Straight Hole Cycle G121 .................................................................	163
	3.6.3 Arc Hole Cycle G122 ........................................................................................	164
	3.6.4 The Chess Board Hole Cycle G123 ...................................................................	165
	3.6.5 Continuous Drilling in the Rectangle G124/G125 ...............................................	166
	3.6.6 Milling on the Plane G126/G127 .......................................................................	167
3.7	Macro Function ................................................................................................................	169
	3.7.1 The User Macro Program General Introduction........................................................	169
	3.7.2 The Variable.............................................................................................................	169
	3.7.3 Types of the Variable ...............................................................................................	172
	3.7.4 The Operational Commands ....................................................................................	181
	3.7.5 The Control Command .............................................................................................	184
	3.7.6 Macro Program Calling Commands .........................................................................	188
	3.7.7 Limitations ................................................................................................................	200
	3.7.8 Sample of Customer Macro Call...............................................................................	200
	3.7.9 Interruption Function of Macro Program...................................................................	202
3.8	Feed G Code ...................................................................................................................	202
	3.8.1 Feed Mode G64/G61/G63........................................................................................	202
	3.8.2 Automatic Corner Override G62 .......................................................................	203
3.9 Introduction of Five Axes Control .......................................................................................		205
	3.9.1 Tool Center Point (TCP) Control ..............................................................................	205
	3.9.2 Tilted Working Plane Command...............................................................................	213
4 AUXILIARY FUNCTION M FUNCTION .......................................................................................		221
4.1 M Command for Program Flow Controlling......................................................................		221
	4.1.1 M00 (Program Stop).................................................................................................	221
	4.1.2 M01 (Optional Stop) .................................................................................................	221
	4.1.3 End of Program M30,M02 ..................................................................................	221
	4.1.4 Subprogram Call M98 ........................................................................................	221
	4.1.5 End of Subprogram or Cycle M99 ......................................................................	222
4.2 M Commands Defined by Standard PLC.........................................................................		222
	4.2.1 Spindle CW/CCW Rotation and Stop Commands (M03, M04, and M05).................	222
	4.2.2 Cooling on/off Commands M08,M09 ..................................................................	222
	4.2.3 Spindle Directional Command (M19)........................................................................	222
	4.2.4 Rigid Tapping Commands (M29)..............................................................................	222
5 FEED FUNCTION......................................................................................................................		223

IX

	GSK 25i Milling CNC System	User Manual
5.1	Rapid Feed (Rapid Traverse).............................................................................................	223
5.2	Cutting Feed.......................................................................................................................	223
	5.2.1 Feed per Minute G94 .........................................................................................	223
	5.2.2 Feed per Revolution G95 ...................................................................................	224
5.3	Tangential Speed Control...................................................................................................	224
5.4	Acceleration/Deceleration Process on the Corner of Program ...........................................	225
6 SPINDLE FUNCTION ..................................................................................................................		226
6.1	Spindle Control...................................................................................................................	226
7 TOOL FUNCTION (T FUNCTION)...............................................................................................		227
7.1	Tool Selection Function......................................................................................................	227
OPERATION............................................................................................................................		229
1 OPERATION PANEL...................................................................................................................		230
1.1	Panel Division.....................................................................................................................	230
1.2	Panel Functions...............................................................................................................	230
	1.2.1 LCD (Liquid Crystal Display) ....................................................................................	230
	1.2.2 Edit Keypad..............................................................................................................	230
	1.2.3 Introduction of Screen Operation Keys ....................................................................	231
	1.2.4 Machine Control Panel.............................................................................................	232
2 SYSTEM POWER ON/OFF AND PROTECTION ........................................................................		235
2.1	System Power on ...............................................................................................................	235
2.2	Power off ............................................................................................................................	235
2.3	Safety Operation ................................................................................................................	236
	2.3.1 Reset........................................................................................................................	236
	2.3.2 Emergency Stop.......................................................................................................	236
	2.3.3 Feed Hold................................................................................................................	.237
2.4	Cycle Start and Feed Hold .................................................................................................	237
2.5	Overtravel Protection..........................................................................................................	237
	2.5.1 Hardware Overtravel Protection...............................................................................	237
	2.5.2 Software Overtravel Protection ................................................................................	238
	2.5.3 Eliminate Overtravel Alarm.......................................................................................	238
	2.5.4 Stored Stroke Check G22-G23 ..........................................................................	238
3 INTERFACE DISPLAY AND OPERATION .................................................................................		242
3.1	Position Interface................................................................................................................	242
	3.1.1 Five Ways for Interface Display................................................................................	242
3.2	Program Interface............................................................................................................	245
	3.2.1 Program Display.......................................................................................................	246
	3.2.2 Set up a program .....................................................................................................	246
	3.2.3 Edit program.............................................................................................................	248
	3.2.4 Cursor Positioning....................................................................................................	251
	3.2.5 MDI Input Display.....................................................................................................	251
	3.2.6 Data Display.............................................................................................................	253
	3.2.7 Detection Interface ...................................................................................................	254

X

		Volume I Programming and Operation
		3.2.8 File List Display ........................................................................................................	254
	3.3	Display Setting.................................................................................................................	256
		3.3.1 Page Setting.............................................................................................................	256
	3.4	Figure Display ....................................................................................................................	264
	3.5	Alarm Display .....................................................................................................................	268
	3.6	System Interface Display....................................................................................................	270
		3.6.1 System Interface Display..........................................................................................	270
	3.7	Help Interface Display ........................................................................................................	282
4	MANUAL OPERATION .............................................................................................................		289
	4.1	Coordinate Axis Move......................................................................................................	289
		4.1.1 Manual Feed ............................................................................................................	289
		4.1.2 Manual Rapid Traverse Move ..................................................................................	289
		4.1.3 Manual Feed and Manual Rapid Traverse Rate Selection .......................................	289
		4.1.4 Manual Intervention..................................................................................................	290
	4.2	Spindle Control ................................................................................................................	290
		4.2.1 Spindle Rotation CW................................................................................................	290
		4.2.2 Spindle Rotation CCW .............................................................................................	290
		4.2.3 Spindle Stop.............................................................................................................	290
		4.2.4 Spindle Exact Stop...................................................................................................	290
	4.3	Other Manual Operations.................................................................................................	291
		4.3.1 Coolant Control ........................................................................................................	291
		4.3.2 Lubricating Control ...................................................................................................	291
		4.3.3 Peck Control.............................................................................................................	291
5	SINGLE STEP OPERATION .....................................................................................................		292
	5.1	Single Step Feed .............................................................................................................	292
		5.1.1 The Selection of Movement Amount ........................................................................	292
		5.1.2 The Selection of Move Axis and Move Direction Key...............................................	292
	5.2	Single Step Interruption......................................................................................................	292
	5.3	Miscellaneous Control in Single Step Operation ................................................................	292
6	MPG OPERATION ....................................................................................................................		293
	6.1 MPG Feed ..........................................................................................................................		293
	6.2	Operation Control in MPG Interruption ...............................................................................	294
		6.2.1 The operation of MPG interruption ...........................................................................	294
	6.3	The Miscellaneous Control in MPG Operation ...................................................................	295
7	AUTOMATIC OPERATION .......................................................................................................		296
	7.1	Automatic Operation ......................................................................................................	296
		7.1.1 The Operation Procedure of Automatic Operation Program.....................................	296
		7.1.2 The Start of Automatic Operation.............................................................................	296
		7.1.3 Automatic Operation Stop ........................................................................................	296
		7.1.4 Spindle Control Speed in Automatic Operation ........................................................	297
		7.1.5 Speed Control in Automatic Operation.....................................................................	298
		7.1.6 Dry Run ....................................................................................................................	298
		7.1.7 Single Block Operation.............................................................................................	298
		7.1.8 All Axes Function Lock Operation ............................................................................	299

XI

		GSK 25i Milling CNC System	User Manual
		7.1.9 Miscellaneous Function Lock Operation ..................................................................	299
	7.2	MDI Operation .................................................................................................................	299
		7.2.1 MDI Program Edit.....................................................................................................	299
		7.2.2 MDI Command Operation and Stop .........................................................................	300
	7.3 Conversion of Operation Modes.........................................................................................		300
8	ZERO RETURN OPERATION...................................................................................................		301
	8.1	Machine Zero Return.......................................................................................................	301
		8.1.1 Machine Zero Point Concept....................................................................................	301
		8.1.2 The Operation Procedures of Machine Zero Return ................................................	301
9	SYSTEM COMMUNICATION....................................................................................................		304
	9.1	Series Terminal Port Communication ..............................................................................	304
		9.1.1 Program Start...........................................................................................................	304
		9.1.2 Function Introduction................................................................................................	304
		9.1.3 Software Usage........................................................................................................	305
	9.2	Network Communication..................................................................................................	305
		9.2.1 Program Start...........................................................................................................	306
		9.2.2 Software Usage........................................................................................................	306
	Appendix Alarm List...............................................................................................................		309

XII

Volume I Programming and Operation

GENERAL

1

GSK 25i Milling CNC System User Manual

1 GENERAL

About this manual

This manual consists of the following parts: 1. GENERAL

Describes chapter organization, related manuals, and notes for reading this manual.

2. PROGRAMMING

Describes each function: format used to program functions in the NC language, characteristics, and restrictions.

3. OPERATION

Describes the manual operation and automatic operation of a machine, procedures for MDI and editing a program.

APPENDIX

Lists alarm codes.

1.1 General

GSK 25i Milling Machining CNC system (hereinafter referred to as the system) is a new generation of CNC device, developing by our company with full heart. It is featured by high precision, great performance, 5 axes simultaneous control and closed-loop control (half closed-loop control and full closed-loop control) and can be widely applied in CNC milling machine and machining center.

This manual detailedly describes procedures for programming, operation of a machine, and introduction for parameter, and inputting and outputting data.

Optional functions are also described in this manual, but not all of them are involved in the actual device. Look up the optional functions incorporated into your system in the manual written by the machine tool builder.

1.2 Notes for Reading this Manual

The performance of a machine tool not only depends on the CNC system, but also the strong current circuit of machine tool, the servo device, the CNC controller and the machine operation control. However, it’s impossible for us to describe all of the functions and procedures of programming and operation in this manual, only the functions of CNC system is presented in it. For various machining functions of a machine tool, refer to the manual provided by the machine tool builder.

All the items described in this manual are prior to that of the manual written by the machine tool builder.

This manual describes items concerning the operation of the system as much as possible. However, it is impractical and unnecessary to present all the descriptions, and the undescribed ones are explained in this manual accordingly.

This manual makes explanations for some special items in notes.

2

Volume I Programming and Operation

PROGRAMMING

3

GSK 25i Milling CNC System User Manual

1 GENERAL

1.1 Definition

To a CNC machine tool, a written program is needed to operate the machine. For example, when machining a part, the tool path and other machining conditions should be programmed in advance, this program is called part program.

1.2 Program Configuration

Program consists of a group of blocks while a block consists of several words. Each block is separated by end-of-block code “; ”(LF in the ISO code and CR in the EIA code).

	PROGRAM	WORD	O00002 N00180
PROGRAM	O00002;
NAME	N60 X100 Y0
			EOB CODE
	N120 X0
	N180 G01 X50 Y50 F2000
	N240 G41 X100 D1
SEQUENCE	N300 G01 Y100		BLOCK
	N360 G02 X200 R50
NO.	N420 G01 Y0 F2500		PROGRAM
	N480 X0
	N540 M30		END
ADD:		Ln 2	S0000 T0100
	EDIT
	PRG MDI CUR/MOD CUR/NXT DIR

Fig. 1-1 Program configuration

The assembly of commands to complete machining is called program. After a program is input to CNC system, commands such as linear/circular movement of tool, spindle rotation/stop can be performed. The program should be written in accordance with the actual move sequence of a machine tool. Program configuration is shown in Fig. 1-1.

1.2.1 Program Name

This system is able to store several different programs. A program name consisting of the address O followed by four-digit number is assigned to each program at the beginning to identify them. Shown in Fig. 1-2.

4

Volume I Programming and Operation

Fig. 1-2 Block configuration

1.2.2 Sequence Number and Block

A program consists of several commands. One command unit is called a block (see Fig. 1-1). One block is separated from another with “; ” as the end of block code. (See Fig. 1-1)

At the head of a block, a sequence number consisting of address N followed by six-digit numbers can be placed (see Fig. 1-1). The leading zero can be omitted. Sequence number can be specified in a random order, and any number can be skipped. Sequence number may be specified for all blocks or only for important blocks of a program. In general, however, it is convenient to assign sequence numbers in ascending order in phase with the machining steps. (For example, when a new tool is used by tool replacement and machining proceeds to a new surface with table indexing.)

1.2.3 Word

Word is an essential for a block. A word consists of an address followed by a number some digit long. (The plus sign (+) or minus sign (-) may be prefixed to a number.)

Fig. 1-3 Word configuration

For an address, one of the letters (A to Z) is used. An address defines the meaning of a number that follows the address. Table1-1 indicates the usable address and their meanings.

The same address may have different meanings, depending on the preparatory function specification.

5

GSK 25i Milling CNC System User Manual

Table 1-1

	Address	Ranges	Function and Meaning
	O	0 99999	Program name
	N	0 999999	Sequence number
	G	000 999	Preparatory function
	X	-999999.9999 999999.9999 mm	X-coordinate address
		0 9999.9999 s	Dwell time
	Y	-999999.9999 999999.9999 mm	X-coordinate address
	Z	-999999.9999 999999.9999 mm	X-coordinate address
	R	-999999.9999 999999.9999 mm	Shift amount of circular radius/angle
		-999999.9999 999999.9999 mm	R surface of canned cycle
	I	-999999.9999 999999.9999 mm	X vector between arc center and starting point
	J	-999999.9999 999999.9999 mm	Y vector between arc center and starting point
	K	-999999.9999 999999.9999 mm	Z vector between arc center and starting point
	F	0.1 1000000 mm/min	Feedrate per minute
		0.001 10000(mm/r)	Feedrate per revolution
	S	0 50000 r/min	Specifying spindle speed
		00 06	Multi-gear spindle output
	T	0 999	Tool function
	M	00 999	Miscellaneous function output, program
			executed flow, subprogram call
	P	0 9999 s	Dwell time
		1 99999	Call subprogram number
	Q	-999999.999 999999.999 mm	Cutting depth or offset amount for low hole in
			canned cycle
	H	00 256	Length offset number
	D	00 256	Radius offset number

Please note that Table 1-1 shows the restriction only for CNC device, the restrictions for machine tool are not included. Reading this manual as well as the one provided by machine tool builder before programming enables better understanding to the restriction.

1.3 General Program Structure

A program contains main program and subprogram. Usually, the CNC system performs according to main program, unless there is a subprogram call in the main program. The main program will be executed again after a returning command is performed. The sequence is shown in Fig. 1-4.

6

Volume I Programming and Operation

Fig. 1-4 Program run sequence

The structure of a main program is consistent with that of the subprogram.

If a program contains a fixed sequence and frequently repeated pattern, such a sequence or pattern can be stored as subprogram in memory to simplify the program. A subprogram can be called in auto mode by command M98. A called subprogram can also call another subprogram. The subprogram calls can be nested up to four levels (shown in Fig. 1-5). The last block of the main program should be the return command M99 which enables the next subprogram to be executed. The program can be repeated when M99 is executed at the end of main program.

Fig. 1-5 Two-level nesting subprogram

A single call command can repetitively and continually call a subprogram up to 999 times.

1.3.1Subprogram Writing and Call

1.3.1.1Subprogram Writing

Write a subprogram as following format:

7

GSK 25i Milling CNC System User Manual

Fig. 1-6

At the beginning of a subprogram, the address O and subprogram number is placed. The end of the subprogram is command M99 (writing format is shown as above).

A subprogram is called by a call command whose format is shown as follows:

● If the repetition number is omitted, it is assumed to be 1.

(e.g.) M98 P51002 ; indicates that subprogram number 1002 is called continually 5 times

●M98 P__ should not coexist with move command in the same block.

●The sequence of subprogram call in a subprogram is the same with that in main program.

Note: CNC enters the alarm state, if a subprogram number specified by address P can not be found.

1.3.2 Program Inputting Format

Words that constitute a block should be input with following format. When the format is variable, the word quantity in a block and the letter quantity in a word can be changed, it is convenient for programming.

E.g. with following command, the tool can be positioned to 50.123mm along X axis:

Note: If two commands are assigned by one address in the same block, the later command is valid in principle. No alarm will occur.

8

Volume I Programming and Operation

e.g.:

G00 G01 X100. Y200.;

G01 is valid, G00 is invalid.

1 G code is valid in the last command of the same block.

2 If there are R, I and K codes in the same arc command, R code is valid regardless of the sequence.

1.3.3 Program End

A Program starts from the program name and ends with command M02, M30 or M99. M02 and M30 enables the system enter into a reset state at the end of a program; the program can be repeated with command M99; if M99 is executed at the end of a subprogram, system returns to the program that call the subprogram. By using parameter N0:1803#5 and N0:1803#4 respectively, M30 and M02 determine whether the system returns to the beginning of the program or not.

Warning!

If the optional block skip switch on the machine operation panel is ON, the block with “/” will be skipped, e.g., command /M02; , /M30; , or /M99; do not indicate the program end.

1.3.4 Optional Block Skip /

When a slash followed by a number n(n=1~9) is specified at the head of a block, and optional block skip switch n on the machine operator panel is set to on, the information contained in the block for which /n corresponding to switch number n is specified is ignored in DNC operation or memory operation. When the optional block skip switch n is set to off, the information contained in the block specified by /n is valid. This means the operator can decide whether to skip blocks contain /n or not. Number 1 of /1 can be omitted. However, when more than two optional block skip switches are used

in one block, number 1 of /1 cannot be omitted.
Example)	(incorrect)	(correct)
	//3 G00X10.0;	/1/3 G00X10.0;

When a program is loaded into memory, this function is ignored. The blocks containing /n are also stored into memory regardless of how the optional block skip is set. Programs held in memory can be output regardless of how the optional block skip is set.

The optional block skip is valid even when sequence number is being searched. Different machine tool has different amount of optional block skip switches (1-9), refer to the manual from machine tool builder for specific details.

Note:

1. The position of the slash

The slash (/) should be at the head of a block. Otherwise, information between the slash and

9

GSK 25i Milling CNC System User Manual

EOB code is ignored.

2. Disabling of optional block skip switch

When a block is read into buffer from memory or tape, the optional block skip operation is processed. After blocks read into a buffer, the already read blocks are not ignored even if the optional block skip switch is set to on.

3. TV and TH check

When the optional block skip switch is set to on, the TH and TV check is performed for the skipped blocks in the same way as when the optional block skip switch is off.

10

Volume I Programming and Operation

2 PROGRAMMING FUNDAMENTALS

2.1 Controlled Axes

Table 2-1

Item	GSK25i
Number of basic controlled axes	5 axes X,Y,Z,4TH,5TH
Simultaneously controlled axes in total	6 axes at most

2.2 Axis Name

The names of 5 basic axes are always X,Y,Z, 4TH,5TH. Parameter No. 9101 sets the number of controlled axes and NO.1020 assigns name for each.

2.3Coordinate system

2.3.1Machine Coordinate System

The point that is specific to a machine and serves as the reference of the machine is referred to as the machine zero point. A machine tool builder sets a machine zero point for each machine. A coordinate system with a machine zero point set as its origin is referred to as a machine coordinate system. A machine coordinate system is set by performing manual reference position return after power-on. A machine coordinate system, once set, remains unchanged until the power is turned off, the system is restart or emergency stop is employed.

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

11

GSK 25i Milling CNC System User Manual

2.3.2 Reference Point

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

Fig.2-1

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

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

2.Auto reference point return

2.3.3 Workpiece Coordinate System

The coordinate system used for workpiece machining is called workpiece coordinate system (or part coordinate system), which is preset by CNC system to set workpiece coordinate system .

The tool machines workpiece into desired shape on the drawing according to program, so it is necessary to set relationship between machine coordinate system and workpiece coordinate system.

The method to determine the relationship between these two coordinate systems is called alignment. It can be done by different methods according to part shape or workpiece quantity.

12

Volume I Programming and Operation

) By workpiece base point	) When part is fixed on jig
To align the tool center to the workpiece	Because the tool center can’t be located at
base point, specify the workpiece coordinate	the workpiece base point, locate the tool to a
system by CNC instructions at this position, and the	position (or reference point) that has a distance
workpiece coordinate system coincides with the	to the base point, set the workpiece coordinate
programming coordinate system.	system by this distance(e.g. G92)

Workpiece coordinate system can be set by one program and can be altered by moving its origin. There are two methods to set the workpiece coordinate system:

1.By G92, see 3.2.11 for details.

2.By G54 to G59, see 3.2.8 for details.

2.3.4Maximum Stroke

Maximum stroke= least command increment×99999999

Table 2-2 Maximum strokes

Increment system	Maximum stroke
Metric machine system	±999999.9999mm
	±999999.9999degree
Inch machine system	±99999.9999inch
	±999999.9999degree

Note:

1 A command exceeding the maximum stroke cannot be specified. 2 The actual stroke depends on the machine tool.

Fig.2-3

2.3.5 Absolute and Incremental Programming

There are two ways to command travels of the tool: the absolute command and the incremental command. In the absolute command, coordinate value of the end position is programmed; in the

13

GSK 25i Milling CNC System User Manual

incremental command, move distance of the position itself is programmed.

Incremental value command is a method based on the move distance. Regardless of the coordinate, it just needs the move direction and distance of end position relative to the start position.

G90 and G91 are used to instruct absolute and incremental command.

In Fig. 2-3, moving from the start position to end position involves the following two commands (G90 and G91) respectively:

G90 G0 X40 Y70;

or G91 G0 X 60 Y40 ;

Either of two methods produces the same motion, and is available for operator to select.

Explanation:

¾G90 and G91 are the modal value of the same group, i.e. G90 mode is defaulted before G91 is specified; G91 is valid till G90 is specified.

System parameter

Parameter N0:1801#3 determines whether G90 (when parameter is 0) or G91 (when parameter is 1) is employed as default mode.

2.4 Modal and Non-modal

Modal means that the number followed an address is valid till it is reset. Another function of modal is that after a word being set, it is not necessary to re-input the word when the same function is used.

¾For example:

G0 X100 Y100; positioning to X100 Y100

X20 Y30; positioning to X20 Y30, G0 is modal and can be omitted.

G1 X50 Y50 F300 linear interpolation to X50 Y50, at a feedrate of 300mm/min G0→G1

X100; linear interpolation to X100 Y50, at a feedrate of 300mm/min, G1,Y50 and F300 are all modal and can be omitted.

Initial mode is the default mode after power-on. See Table 3-1 for details.

¾For example:

¾O00001

¾X100 Y100; positioning to X100 Y100, G0 is initial mode

¾G1 X0 Y0 F100; linear interpolation to X0 Y0, at a feedrate of 100mm/min, G98 is initial mode

Non-mode means that the numbers after an address is valid in only in the current block and should be re-specified in next block. As G command of group 00 shown in table 3-1.

Table 2-3 describes the modal and non-modal of commands.

14

Volume I Programming and Operation

Table 2-3 modal and non-modal of commands

		Modal G function	G commands are being executed till they are
			invalidated by another G commands.
	Modal
		Modal M function	M commands is being executed till they are
			invalidated by another M commands.
		Non-modal G function	Only valid in specified blocks and to be cancelled
	Non-modal		at the end of a program
		Non-modal M function	Only valid in the current block

2.5 Decimal Point Programming

Numerical value can be entered with a decimal point. A decimal point can be used when entering a distance, time, or speed. Decimal points can be specified with the following addresses:

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

Explanation:

1.Parameter N0:1800#5 determines the employment of decimal point programming. When N0:1800#5=1, the unit of programming value is mm, inch or degree; when N0:1800#5=0, the unit is the least movement unit, determining by parameter N0:1000#1.

2.Fractions less than the least input increment are truncated.

For example:

X9.87654; when the least input increment is 0.001mm, truncated to X 9.876. when the least input increment is 0.0001mm, processed as X 9.8765.

2.6Basic Functions

2.6.1Tool Movement along Workpiece Parts Figure—Interpolation

1 The tool moves along straight lines

15

GSK 25i Milling CNC System User Manual

2 The tool moves along arcs

The function of moving the tool along straight lines and arcs is called the interpolation.

Symbols of the programmed commands G01, G02…are called the preparatory function and specify the type of interpolation conducted in the control unit.

a) Movement along				straight line
G01 Y		;
X	Y	;
b) Movement along				arc
G03 X		Y	R	;
				Interpolation		X axis (M otor)
						Y axis (M otor)
			a) Movement along straight line
			b) Movement along		arc	Tool m ovement

Note: Some machines move tables instead of tools but this manual assumes that tools are moved against workpiece. Refer to the actual move direction to avoid danger and damages.

2.6.2 Feed—Feed Function

The function of specifying a feedrate is called feed function.

Feed is to move the tool with a specified rate. The feedrate is indicated by numeric command. For example, command F200 means the tool infeeds at a speed of 200mm/min.

16

Volume I Programming and Operation

2.6.3 Cutting Speed, Spindle Speed Function

	Tool
r/min	Tool diameter
RPM	V: Cutting speed
	(m/min
	workpiece

The speed of the tool with respect to the workpiece when the workpiece is cut is called the cutting speed. For CNC, it can be specified by the spindle speed RPM r/min .

For example, when a workpiece is machined with a tool 100mm in diameter at a cutting speed of 80m/min, the spindle speed is about 250r/min, which is obtained from N=1000V/πD. The command is S250.

Commands related to the spindle speed are called the spindle function.

2.6.4 Command for Machine Operations—Miscellaneous Function

When machining is actually started, it’s necessary to rotate the spindle, and feed coolant accordingly. Thus, the on-off switch for spindle motor and coolant valve should be controlled.

The function of specifying the on-off operations of the machine or program through NC system is called the miscellaneous function, which is specified by M mode.

For example, when M03 is specified, the spindle rotates clockwise at the specified speed. (Clockwise means operator views over the spindle along the negative direction of Z axis.)

2.6.5 Selection of Tool Used for Various Machining—Tool

When drilling, tapping, boring, milling or the like, is performed, it is necessary to select a suitable tool. When a number is assigned to each tool and the number is specified in the program. The corresponding tool is selected.

17