gsk GSK980TDb User Manual

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 operations of

the system due to the manual content limit, product specific operations and

other causes. Therefore, the operations not specified herein shall be

considered impossible or unallowable.

This user manual is the property of GSK CNC Equipment Co., Ltd. All rights are reserved. It is against the law for any organization or

individual to publish or reprint this manual without the express written

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

liability.

GSK980TDb Turning CNC System User Manual

FOREWORD

Dear user,

We are really grateful for your patronage and purchase of this GSK980TDb Turning CNC system made by GSK CNC Equipment Co., Ltd.

The user manual describes the programming, operation, installation and connection of this GSK980TDb Turning CNC system. Please read it carefully before operation in order to get the safe and effective working.

Warning

This system can only be operated by authorized and qualified personnel as improper operations may cause accidents.

Please carefully read this user manual before use!

Note: The power supply installed on (in) the cabinet is exclusive to GSK’S CNC systems.

The power supply form is forbidden to be used for other purposes. Otherwise, there may be extreme danger!

This user manual shall be kept by final user.

II

Notes

Notes

■ Delivery and storage

zPacking box over 6 layers in pile is unallowed.

zNever climb the packing box, neither stand on it, nor place heavy objects on it.

zDo not move or drag the product by the cables connected with it.

zForbid collision or scratch to the panel and displayer.

zPacking box should be protected from damping, insolation and raining.

■Open packing box to check

zEnsure things in packing box are the required ones.

zEnsure the product is not damaged in delivery.

zEnsure the parts in packing box are in accordance to the order.

zContact us in time if the product type is inconsistent with the order, there is short of accessories, or product damage in delivery.

■Connection

zOnly qualified persons can connect the system or check the connection.

zThe system must be earthed, its resistance must be less than 4 Ω and the ground wire cannot be replaced by zero wire.

zConnection must be correct and firm to avoid the product to be damaged or other unexpected result.

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

zSwitch off power supply before pulling out plug or opening electric cabinet.

■Troubleshooting

zSwitch off power supply before troubleshooting or changing components.

zTroubleshoot and then startup the system when there is short circuit or overload.

zDo not switch on or off it frequently and an interval is 1 minute at least after the system is powered on again.

III

GSK980TDb Turning CNC System User Manual

Announcement

zThis manual describes various items as much as possible. However, operations allowable or unallowable cann’t 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 to be unavailable.

Warning

zPlease read this user manual and a manual from machine builder completely before installation, programming and operation; do operate the system and machine according to user manuals, otherwise it may damage the system, machine, workpiece and even injure the operator.

Cautions

z Functions, technical indexes described in this user manual are only for the system. Actual functions and technical performance of machine tool with this CNC system are determined by machine builder’s design, so refer to its user manual.

zThe system is employed with integrated machine control panel and the keys on machine control panel are defined by PLC program. Functions of keys in this user manual are for standard PLC program. Please notice it!

zRefer to user manual from machine manufacturer about functions and meanings of keys on machine control panel.

All specification and designs are subject to change without further notice.

IV

Summary

Volume Programming

GSK980TDb CNC Technical Specification, Product

Type, Command and Program Format

Volume Operation

GSK980TDb CNC Operation Use

Volume Installation and Connection

GSK980TDb CNC Installation, Connection and Setting

Appendix

CNC Ladder Function Allocation, Alarm Message Table

V

GSK980TDb Turning CNC System User Manual

Safety Responsibility

Manufacturer’s safety responsibility

——The manufacturer should be responsible for the cleared or the controlled safety in the design and the structure of the CNC system and the accessories.

——The manufacturer should be responsible for the CNC system and the accessories. ——The manufacturer should be responsible for the message and the suggestion for the user.

User’s safety responsibility

——The user should study and train the system safety operation, master the safety operation content.

——The user should be responsible for the danger caused by increasing, changing or modifying the CNC system, the accessories by itself.

——The user should be responsible for the danger because of the mistaken operation, regulation, maintenance, installation and storage.

VI

					Contents
					CONTENTS
				Volume Programming
CHAPTER 1		PROGRAMMING .........................................................................................................				3
1.1	GSK980TDb introduction .....................................................................................................					3
	1.1.1		Product introduction...................................................................................................			3
	1.1.2		Technical specification ...............................................................................................			4
	1.1.3		Environment and conditions.......................................................................................			6
	1.1.4		Power supply .............................................................................................................			7
	1.1.5		Guard.........................................................................................................................			7
1.2 CNC system of machine tools and CNC machine tools .......................................................						7
1.3	Programming fundamentals.................................................................................................					9
	1.3.1		Coordinates definition ................................................................................................			9
	1.3.2 Machine coordinate system, Machine Zero and machine reference point .................					9
	1.3.3 Workpiece coordinate system and Program Zero....................................................					10
	1.3.4		Interpolation function ...............................................................................................			11
	1.3.5 Absolute programming and incremental programming ............................................					12
	1.3.6 Diameter programming and radius programming ....................................................					12
1.4 Structure of an NC program ...............................................................................................						13
	1.4.1 General structure of a program................................................................................					14
	1.4.2 Main program and subprogram................................................................................					17
1.5	Program run.......................................................................................................................					18
	1.5.1 Sequence of program run ........................................................................................					18
	1.5.2 Execution sequence of word....................................................................................					19
1.6 Basic axis incremental system...........................................................................................						19
	1.6.1 Incremental system speed of basic axis ..................................................................					19
	1.6.2 Incremental system unit of basic axis ......................................................................					20
	1.6.3 Incremental system data range of basic axis ...........................................................					20
	1.6.4 Incremental system data range and unit of basic axis .............................................					21
	1.6.5 Program address value unit and range of incremental system of basic axis............					22
1.7 Additional axis incremental system ....................................................................................						23
	1.7.1 Additional axis being the current incremental system ..............................................					24
	1.7.2 Additional axis being IS-A incremental system ........................................................					24
CHAPTER 2		MSTF COMMAND		.....................................................................................................		25
2.1	M (miscellaneous function) ................................................................................................					25
	2.1.1		End of program	M02 .............................................................................................		25
	2.1.2		End of program run		M30 .......................................................................................	25
	2.1.3		Subprogram call	M98 ............................................................................................		26
	2.1.4		Return from subprogram M99 ...............................................................................			26
	2.1.5		Macro program call		M9000 M9999 .....................................................................	27
	2.1.6 M commands defined by standard PLC ladder diagram ..........................................					27
	2.1.7		Program stop M00.................................................................................................			28
	2.1.8 Program optional stop M01......................................................................................					28
	2.1.9 Spindle CW, CCW and stop control M03, M04, M05 ...............................................					29
	2.1.10		Cooling control	M08, M09 ...................................................................................		29
	2.1.11		Tailstock control	M10, M11 ..................................................................................		29
	2.1.12		Chuck control	M12, M13 .....................................................................................		29

VII

GSK980TDb Turning CNC System User Manual

	2.1.13 Spindle position/speed control switch M14, M15 ...................................................							29
	2.1.14 Spindle clamped/released M20, M21.....................................................................							30
	2.1.15	The 2nd spindle position/speed switch					M24, M25................................................	30
	2.1.16 Lubricating control M32, M33 ................................................................................							30
	2.1.17 Spindle automatic gear change M41, M42, M43, M44...........................................							30
	2.1.18 Spindle 8-point orientation M50 M58...................................................................							30
	2.1.19 The 2nd spindle rotation CCW, rotation CW , stop M63, M64, M65........................							31
2.2	Spindle function .................................................................................................................							31
	2.2.1 Spindle speed switching value control .....................................................................							31
	2.2.2 Spindle speed analog voltage control ......................................................................							32
	2.2.3 Constant surface speed control G96, constant rotational speed control G97 ..........							32
	2.2.4	Spindle override.......................................................................................................						35
	2.2.5 Multiple spindle control function...............................................................................							35
	2.2.6 Cs contour control funciton......................................................................................							36
2.3	Tool function ......................................................................................................................							36
	2.3.1	Tool control ..............................................................................................................						36
	2.3.2	Tool life management ..............................................................................................						40
CHAPTER 3 G COMMANDS			..........................................................................................................					50
3.1	Commands ........................................................................................................................							50
	3.1.1 Modal, non-modal and initial mode..........................................................................							51
	3.1.2	Omitting words.........................................................................................................						51
	3.1.3	Related definitions ...................................................................................................						53
3.2	Rapid traverse movement				G00 .......................................................................................			53
3.3	Linear interpolation		G01..................................................................................................					54
3.4	Circular interpolation		G02, G03.......................................................................................					56
3.5	Three-point circular interpolation					G05 .............................................................................		59
3.6	Ellipse interpolation		G6.2, G6.3.......................................................................................					60
3.7	Parabola interpolation			G7.2, G7.3...................................................................................				63
3.8	Plane selection G17 G19 ................................................................................................							65
3.9	Polar coordinate interpolation G12.1, G13.1......................................................................							66
3.10	Cylindrical interpolation G7.1...........................................................................................							69
3.11	Chamfering function.........................................................................................................							72
	3.11.1	Linear chamfering..................................................................................................						72
	3.11.2	Circular chamfering................................................................................................						74
	3.11.3	Special cases.........................................................................................................						76
3.12	Dwell G04......................................................................................................................							78
3.13	Machine Zero function			.....................................................................................................				78
	3.13.1	Machine 1st reference point G28 ........................................................................						78
	3.13.2	Machine 2nd, 3rd, 4th reference point					G30.........................................................	79
3.14	Skip interpolation		G31...................................................................................................					81
3.15	Automatic tool offset			G36, G37 .....................................................................................				83
3.16	Workpiece coordinate system					G50 ...............................................................................		86
3.17	Fixed cycle command ......................................................................................................							87
	3.17.1	Axial cutting cycle			G90........................................................................................			87
	3.17.2	Radial cutting cycle			G94 .....................................................................................			90
	3.17.3 Caution of fixed cycle commands ..........................................................................							92
3.18	Multiple cycle commands.................................................................................................							93
	3.18.1 Axial roughing cycle G71.......................................................................................							93

VIII

				Contents
3.18.2 Radial roughing cycle G72.....................................................................................				99
3.18.3		Closed cutting cycle G73...................................................................................		103
3.18.4		Finishing cycle G70 .............................................................................................		107
3.18.5		Axial grooving multiple cycle G74 .....................................................................		108
3.18.6 Radial grooving multiple cycle G75......................................................................				111
3.19	Thread cutting commands .............................................................................................			114
3.19.1 Thread cutting with constant lead G32.................................................................				115
3.19.2 Rigid thread cutting G32.1 ...................................................................................				117
3.19.3		Thread cutting with variable lead	G34...............................................................	119
3.19.4		Z thread cutting G33 .........................................................................................		121
3.19.5 Rigid tapping G84, G88 .......................................................................................				122
3.19.6 Thread cutting cycle G92.....................................................................................				125
3.19.7 Multiple thread cutting cycle G76.........................................................................				128
3.20	Constant surface speed control G96, constant rotational speed control G97 ...........			132
3.21 Feedrate per minute G98, feedrate per rev G99............................................................				132
3.22.	Additional Axis Function................................................................................................			134
3.22.1		Additional axis start..............................................................................................		134
3.22.2 Motion of additional axis ......................................................................................				134
3.22.3 Additional axis coordinates display ......................................................................				135
3.23	Macro commands ..........................................................................................................			135
3.23.1		MACRO variables ................................................................................................		135
3.23.2		Operation and jump command	G65 ..................................................................	140
3.23.3 Program example with macro command .............................................................				143
3.24	Statement macro command ...........................................................................................			145
3.24.1 Arithmetic and logic operation..............................................................................				145
3.24.2		Transfer and cycle ...............................................................................................		147
3.25	Metric/Inch Switch..........................................................................................................			149
3.25.1		Functional summary ............................................................................................		149
3.25.2		Function command G20/G21...............................................................................		150
3.25.3		Notes ...................................................................................................................		150
CHAPTER 4 TOOL NOSE RADIUS COMPENSATION (G41, G42) .............................................				151
4.1	Application .......................................................................................................................			151
4.1.1		Overview................................................................................................................		151
4.1.2 Imaginary tool nose direction.................................................................................				152
4.1.3		Compensation value setting...................................................................................		155
4.1.4		Command format ...................................................................................................		156
4.1.5		Compensation direction .........................................................................................		156
4.1.6		Notes .....................................................................................................................		158
4.1.7		Application .............................................................................................................		159
4.2 Tool nose radius compensation offset path......................................................................				160
4.2.1 Inner and outer side...............................................................................................				160
4.2.2 Tool traversing when starting tool ..........................................................................				160
4.2.3 Tool traversing in Offset mode ...............................................................................				162
4.2.4 Tool traversing in Offset canceling mode ...............................................................				167
4.2.5		Tool interference check..........................................................................................		168
4.2.6 Commands for canceling compensation vector temporarily ..................................				170
4.2.7		Particulars..............................................................................................................		172

IX

GSK980TDb Turning CNC System User Manual

Volume Operation

CHAPTER 1 OPERATION MODE AND DISPLAY INTERFACE ...................................................			175
1.1	Panel division...................................................................................................................		175
	1.1.1	State indication ......................................................................................................	176
	1.1.2	Edit keypad............................................................................................................	176
	1.1.3	Menu display .........................................................................................................	177
	1.1.4	Machine panel .......................................................................................................	177
1.2	Summary of operation mode ...........................................................................................		180
1.3	Display interface ..............................................................................................................		181
	1.3.1	POS interface ........................................................................................................	183
	1.3.2	PRG interface ........................................................................................................	186
	1.3.3 TOOL OFFSET&WEAR, MACRO, TOOL-LIFE MANAGEMENT interfaces ..........		188
	1.3.4	ALARM interface ...................................................................................................	190
	1.3.5	Setting interface.....................................................................................................	191
	1.3.6 BIT PARAMETER, DATA PARAMETER, SCREW-PITCH COMP interfaces .........		194

1.3.7CNC DIAGNOSIS, PLC STATE, PLC VALUE, TOOL PANEL, VERSION MESSAGE

	interfaces ..........................................................................................................................		195
CHAPTER 2 POWER ON/OFF AND PROTECTION....................................................................			199
2.1	System power on .............................................................................................................		199
2.2	System power off .............................................................................................................		199
2.3	Overtravel protection .......................................................................................................		199
	2.3.1	Hardware overtravel protection..............................................................................	200
	2.3.2	Software Overtravel Protection..............................................................................	200
2.4	Emergency operation.......................................................................................................		201
	2.4.1	Reset .....................................................................................................................	201
	2.4.2	Emergency stop.....................................................................................................	201
	2.4.3	Feed hold...............................................................................................................	201
	2.4.4	Power-off ...............................................................................................................	201
CHAPTER 3		MANUAL OPERATION ............................................................................................	202
3.1	Coordinate axis move ......................................................................................................		202
	3.1.1	Manual feed...........................................................................................................	202
	3.1.2	Manual rapid traverse............................................................................................	203
	3.1.3	Speed tune ............................................................................................................	203
3.2	Other manual operations .................................................................................................		204
	3.2.1 Spindle CCW, CW, stop control .............................................................................		204
	3.2.2	Spindle jog .............................................................................................................	204
	3.2.3	Cooling control.......................................................................................................	205
	3.2.4	Lubricating control .................................................................................................	205
	3.2.5	Chuck control.........................................................................................................	206
	3.2.6	Tailstock control .....................................................................................................	206
	3.2.7	Hydraulic control....................................................................................................	206
	3.2.8	Manual tool change ...............................................................................................	207
	3.2.9	Spindle override.....................................................................................................	207

X

			Contents
CHAPTER 4		MPG/STEP OPERATION.........................................................................................	208
4.1	Step feed..........................................................................................................................		208
	4.1.1	Increment selection................................................................................................	208
	4.1.2	Moving direction selection .....................................................................................	209
4.2	MPG(handwheel) feed .....................................................................................................		209
	4.2.1	Increment selection................................................................................................	209
	4.2.2 Moving axis and direction selection .......................................................................		210
	4.2.3	Other operations ....................................................................................................	210
	4.2.4	Explanation items ..................................................................................................	211
CHAPTER 5		MDI OPERATION ....................................................................................................	212
5.1	Code words input.............................................................................................................		212
5.2	Code words execution .....................................................................................................		213
5.3	Parameter setting.............................................................................................................		213
5.4	Data alteration..................................................................................................................		213
5.5	Other operations ..............................................................................................................		214
CHAPTER 6 PROGRAM EDIT AND MANAGEMENT ..................................................................			215
6.1	Program creation .............................................................................................................		215
	6.1.1 Creating a block number........................................................................................		215
	6.1.2	Inputting a program................................................................................................	215
	6.1.3	Searching a character............................................................................................	216
	6.1.4	Inserting a character ..............................................................................................	218
	6.1.5	Deleting a character...............................................................................................	219
	6.1.6	Altering a character................................................................................................	219
	6.1.7 Deleting a single block...........................................................................................		220
	6.1.8	Deleting blocks ......................................................................................................	220
	6.1.9	Deleting a segment................................................................................................	221
	6.1.10 Macro program edit..............................................................................................		222
6.2	Program annotation .........................................................................................................		222
	6.2.1 Creating a program annotation ..............................................................................		222
	6.2.2 Altering a program annotation................................................................................		224
6.3	Deleting program .............................................................................................................		224
	6.3.1	Deleting a program ................................................................................................	224
	6.3.2	Deleting all programs.............................................................................................	224
	6.3.3 Initiation of program area.......................................................................................		224
6.4	Selecting a program.........................................................................................................		224
	6.4.1	Search ...................................................................................................................	224
	6.4.2	Scanning................................................................................................................	225
	6.4.3	Cursor....................................................................................................................	225
6.5	Execution of the program.................................................................................................		226
6.6	Renaming a program .......................................................................................................		226
6.7	Copy a program ...............................................................................................................		226
6.8	Program management .....................................................................................................		226
	6.8.1	Program list............................................................................................................	226
	6.8.2	Part-Prg number ....................................................................................................	226
	6.8.3 Memory size and used capacity.............................................................................		227

XI

		GSK980TDb Turning CNC System	User Manual
6.9	Other operations available in Edit mode ..........................................................................		227
CHAPTER 7 TOOL OFFSET AND SETTING ...............................................................................			228
7.1	Tool positioning setting ....................................................................................................		228
7.2	Trial toolsetting ................................................................................................................		229
7.3	Toolsetting by machine zero return ..................................................................................		230
7.4	Setting and altering the offset value.................................................................................		232
	7.4.1	Offset setting .........................................................................................................	233
	7.4.2	Offset alteration .....................................................................................................	234
	7.4.3 Offset alteration in communication mode...............................................................		234
	7.4.4 Clearing the offset values ......................................................................................		235
	7.4.5 Setting and altering the tool wear ..........................................................................		235
	7.4.6 Locking and unlocking the offset value ..................................................................		235
	7.4.7 No.0 tool offset moving workpiece coordinate system...........................................		236
CHAPTER 8 AUTO OPERATION .................................................................................................			238
8.1	Automatic run...................................................................................................................		238
	8.1.1 Selection of the program to be run ........................................................................		238
	8.1.2 Start of the automatic run.......................................................................................		239
	8.1.3 Stop of the automatic run.......................................................................................		239
	8.1.4 Automatic run from an arbitrary block....................................................................		240
	8.1.5 Adjustment of the feedrate, rapid rate ...................................................................		240
	8.1.6	Spindle speed adjustment......................................................................................	241
8.2	Running state...................................................................................................................		241
	8.2.1	Single block execution...........................................................................................	241
	8.2.2	Dry run...................................................................................................................	242
	8.2.3	Machine lock..........................................................................................................	243
	8.2.4	MST lock................................................................................................................	244
	8.2.5	Block skip ..............................................................................................................	244
8.3	Other operations ..............................................................................................................		245
CHAPTER 9 ZERO RETURN OPERATION .................................................................................			246
9.1	Program zero return.........................................................................................................		246
	9.1.1	Program Zero ........................................................................................................	246
	9.1.2 Program zero return steps .....................................................................................		246
9.2	Machine Zero return ........................................................................................................		247
	9.2.1 Machine Zero (machine reference point)...............................................................		247
	9.2.2 Machine Zero return steps.....................................................................................		247
9.3	Other operations in zero return ........................................................................................		248
CHAPTER 10 DATA SETTING, BACKUP and RESTORE ............................................................			249
10.1	Data setting....................................................................................................................		249
	10.1.1	Switch setting ......................................................................................................	249
	10.1.2	Graphic display....................................................................................................	249
	10.1.3	Parameter setting ................................................................................................	251
10.2 Data recovery and backup.............................................................................................			256
10.3 Password setting and alteration.....................................................................................			257
	10.3.1	Operation level entry ...........................................................................................	258

XII

			Contents
	10.3.2	Altering the password ..........................................................................................	259
	10.3.3 Setting the lower password level .........................................................................		260
CHAPTER 11 U OPERATION FUNCTION ...................................................................................			262
11.1	File catalog window........................................................................................................		262
11.2 Commonly use file operation function introduction.........................................................			262
	11.2.1 File extension and return......................................................................................		262
	11.2.2	File copy...............................................................................................................	263
	11.2.3	Open CNC file......................................................................................................	263
CHAPTER 12 ADVANCED OPERATION USB FUNCTION ....................................................			264
12.1	Entering the advanced operation window ......................................................................		264
12.2	Operation path ...............................................................................................................		264
12.3	Operation explanation....................................................................................................		265
12.4	Note	...............................................................................................................................	266
CHAPTER 13		COMMUNICATION ................................................................................................	267
13.1	TDComm2a communication software introduction of GSK980TDb ...............................		267
	13.1.1	Files download (PC→CNC) .................................................................................	268
	13.1.2	Uploading files (CNC→PC)..................................................................................	273
	13.1.3	Setting option.......................................................................................................	275
13.2	Preparation before communication ................................................................................		275
13.3	Data input (PC→CNC)...................................................................................................		276
	13.3.1	Inputting a program..............................................................................................	276
	13.3.2 Inputting a tool offset............................................................................................		278
	13.3.3 Input of the parameter..........................................................................................		279
13.4	Data output(CNC→PC)..................................................................................................		280
	13.4.1	Output a program.................................................................................................	280
	13.4.2	Outputting all programs .......................................................................................	283
	13.4.3 Outputting a tool offset.........................................................................................		284
	13.4.4	Outputting a parameter........................................................................................	285
13.5	Communication between CNC and CNC .......................................................................		286
CHAPTER 14		MACHINING EXAMPLES ......................................................................................	288
14.1	Programming .................................................................................................................		289
14.2	Program input ................................................................................................................		290
	14.2.1 View a saved program .........................................................................................		290
	14.2.2 Creating a new program ......................................................................................		291
14.3 Checkout a program .........................................................................................................			292
	14.3.1	Graphic setting.....................................................................................................	292
	14.3.2	Program check.....................................................................................................	292
14.4	Toolsetting and running..................................................................................................		293

XIII

		GSK980TDb Turning CNC System	User Manual
		Volume Connection
CHAPTER 1		INSTALLATION LAYOUT.........................................................................................	299
1.1	GSK980TDb system connection......................................................................................		299
	1.1.1 GSK980TDb, GSK980TDb-V back cover interface layout.....................................		299
	1.1.2	Interface explanation .............................................................................................	300
1.2	GSK980TDb installation ..................................................................................................		300
	1.2.1	GSK980TDb external dimensions .........................................................................	300
	1.2.2 Preconditions of the cabinet installation.................................................................		300
	1.2.3	Measures against interference ..............................................................................	300
CHAPTER 2 DEFINITION & CONNECTION OF INTERFACE SIGNALS.....................................			302
2.1	Connection to drive unit ...................................................................................................		302
	2.1.1	Drive interface definition ........................................................................................	302
	2.1.2 Code pulse and direction signals...........................................................................		302
	2.1.3 Drive unit alarm signal nALM.................................................................................		302
	2.1.4 Axis enable signal nEN..........................................................................................		303
	2.1.5 Pulse disable signal nSET.....................................................................................		303
	2.1.6	Zero signal nPC.....................................................................................................	303
	2.1.7 Connection to a drive unit......................................................................................		305
2.2	Being connected with spindle encoder ............................................................................		306
	2.2.1 Spindle encoder interface definition.......................................................................		306
	2.2.2	Signal explanation .................................................................................................	306
	2.2.3 Being connected with spindle encoder interface....................................................		306
2.3	Being connected with MPG (Manual Pulse Generator) ...................................................		307
	2.3.1	MPG interface definition ........................................................................................	307
	2.3.2	Signal explanation .................................................................................................	307
2.4	Spindle interface ..............................................................................................................		308
	2.4.1	Spindle interface definition.....................................................................................	308
	2.4.2 Connection to inverter ..............................................................................................		308
2.5	GSK980TDb GSK980TDb-V being connected with PC ................................................		309
	2.5.1	Communication interface definition........................................................................	309
	2.5.2	Communication interface connection.....................................................................	309
2.6	Power interface connection .............................................................................................		310
2.7	I/O interface definition......................................................................................................		310
	2.7.1	Input signal ............................................................................................................	312
	2.7.2	Output signal .........................................................................................................	313
2.8	I/O function and connection .............................................................................................		315
	2.8.1 Stroke limit and emergency stop............................................................................		315
	2.8.2	Tool change control ...............................................................................................	317
	2.8.3	Machine zero return...............................................................................................	323
	2.8.4	Spindle control .......................................................................................................	330
	2.8.5 Spindle switching volume control...........................................................................		333
	2.8.6 Spindle automatic gearing control..........................................................................		333
	2.8.7	Spindle eight-point orientation function..................................................................	335
	2.8.8 Spindle Cs axis control function.............................................................................		338

XIV

		Contents
2.8.9	Multiple spindle function ........................................................................................	340
2.8.10	Rigid tapping function ..........................................................................................	343
2.8.11 External cycle start and feed hold ........................................................................		344
2.8.12	Cooling control.....................................................................................................	345
2.8.13	Lubricating control ...............................................................................................	345
2.8.14	Chuck control.......................................................................................................	347
2.8.15	Tailstock control ...................................................................................................	349
2.8.16	Low pressure detection........................................................................................	350
2.8.17 Hydraulic control (only applied to 980TDb-V) ......................................................		351
2.8.18	Safety door detection...........................................................................................	352
2.8.19	Block skip.............................................................................................................	352
2.8.20	CNC macro variables...........................................................................................	353
2.8.21	Tri-colour indicator ...............................................................................................	353
2.8.22	External override..................................................................................................	354
2.8.23	External MPG ......................................................................................................	354
2.8.24 Gear/tool number display (only applied to 980TDb-V) .........................................		355
2.9 Commonly use symbol of electricity drawing ...................................................................		356
CHAPTER 3 PARAMETERS ........................................................................................................		357
3.1 Parameter description (by sequence) ..............................................................................		357
3.1.1	Bit parameter .........................................................................................................	357
3.1.2	Data parameter......................................................................................................	366
3.1.3 PLC K parameter standard PLC definition .......................................................		386
3.2 Parameter description (by function sequence).................................................................		388
3.2.1 X, Z, Y, 4th,5th axis control logic..............................................................................		388
3.2.2	Acceleration&deceleration control .........................................................................	390
3.2.3	Precision compensation.........................................................................................	392
3.2.4	Machine protection ................................................................................................	395
3.2.5	Machine zero return...............................................................................................	395
3.2.6	Threading function .................................................................................................	400
3.2.7	Spindle control .......................................................................................................	401
3.2.8	Tool compensation.................................................................................................	404
3.2.9 Tool life management function ...............................................................................		404
3.2.10	Tool wear parameter ............................................................................................	405
3.2.11	Edit and display....................................................................................................	405
3.2.12	Communication setting ........................................................................................	405
3.2.13	MPG Parameters .................................................................................................	406
3.2.14 PLC axis control function .....................................................................................		406
3.2.15	Skip function ........................................................................................................	406
3.2.16	Automatic toolsetting function..............................................................................	407
3.2.17 Input and output function in metric and inch system ............................................		407
3.2.18 Parameters related to arc turning ........................................................................		408
3.2.19 Parameters related to the additional ....................................................................		408
CHAPTER 4 MACHINE DEBUGGING METHODS AND MODES ................................................		411
4.1 Emergency stop and limit.................................................................................................		411
4.2 Drive unit configuration ....................................................................................................		411

XV

GSK980TDb Turning CNC System User Manual

4.3	Gear ratio adjustment ......................................................................................................		411
4.4	ACC&DEC characteristic adjustment...............................................................................		412
4.5	Mechanical (machine) zero adjustment ...........................................................................		413
4.6	Spindle adjustment ..........................................................................................................		415
	4.6.1	Spindle encoder.....................................................................................................	415
	4.6.2	Spindle brake.........................................................................................................	415
	4.6.3	Switch volume control of spindle speed.................................................................	416
	4.6.4	Analog voltage control of spindle speed ................................................................	416
4.7	Backlash Offset................................................................................................................		416
4.8	Tool Post Debugging........................................................................................................		417
4.9	Step/MPG Adjustment......................................................................................................		418
4.10	Other adjustment ...........................................................................................................		418
CHAPTER 5		DIAGNOSIS MESSAGE ..........................................................................................	420
5.1	CNC diagnosis.................................................................................................................		420
	5.1.1 I/O status and data diagnosis message.................................................................		420
	5.1.2 CNC motion state and data diagnosis message....................................................		420
	5.1.3	Diagnosis keys ......................................................................................................	421
	5.1.4	Others....................................................................................................................	422
5.2	PLC state.........................................................................................................................		422
	5.2.1 X address (machine→PLC , defined by standard PLC ladders) ............................		422
	5.2.2 Y address (PLC→machine, defined by standard PLC ladders) .............................		424
	5.2.3	Machine panel .......................................................................................................	426
	5.2.4	F address(CNC→PLC)..........................................................................................	428
	5.2.5	G address(PLC→CNC) .........................................................................................	435
	5.2.6 Address A (message display requiery signal, defined by standard PLC ladders) ..		440
	5.2.7 K address K parameter, standard PLC definition .............................................		441
5.3	PLC data..........................................................................................................................		444
	5.3.1 Timer address T(defined by standard PLC ladders) ..............................................		444
	5.3.2 Counter address C(Defined by standard PLC Ladders) ........................................		445
	5.3.3 Timer presetting address DT(Defined by standard PLC ladders) ..........................		445
	5.3.4 Counter presetting address DC .............................................................................		445
CHAPTER 6 MEMORIZING PITCH ERROR COMPENSATION ..................................................			446
6.1	Function description.........................................................................................................		446
6.2	Specification ....................................................................................................................		446
6.3	Parameter setting ............................................................................................................		446
	6.3.1	Pitch compensation ...............................................................................................	446
	6.3.2	Pitch error origin ....................................................................................................	446
	6.3.3	Offset interval ........................................................................................................	447
	6.3.4	Offset value ...........................................................................................................	447
6.4	Notes of offset setting ......................................................................................................		447
6.5	Setting examples of offset parameters.............................................................................		447

XVI

		Contents
	Appendix
Appendix 1 GSK980TDb, GSK980TDb-V contour dimension.............................................................		453
Appendix 2 GSK980TDb-B outline dimension .......................................................................................		454
Appendix 3 Outline Dimension of Accessional Panel AP01.................................................................		454
Appendix 4 Outline Dimension of Accessional Panel AP02.................................................................		455
Appendix 5 Outline Dimension of Accessional Panel AP03.................................................................		455
Appendix 6	Outline Dimension of I/O deconcentrator MCT01A ..........................................................	456
Appendix 7	Outline Dimension of I/O deconcentrator MCT02.............................................................	456
Appendix 8	Delivery standard parameter................................................................................................	457
Appendix 9	Alarm list .................................................................................................................................	463
Appendix 10 Operation list ........................................................................................................................		471

XVII

GSK980TDb Turning CNC System User Manual

XVIII

Chapter 1 Programming

Volume Programming

1

GSK980TDb Turning CNC System User Manual

2

Chapter 1 Programming

CHAPTER 1 PROGRAMMING

1.1GSK980TDb introduction

1.1.1Product introduction

GSK980TDb is a new upgraded software, hardware product based of GSK980TDa, with 5 feed axes(including C axis), 2 analog spindles, 2ms high-speed interpolation, 0.1μm control precision, which can obviously improve the machining efficiency, precision and surface quality. It adds the USB interface, U disc file operation and program run. As the upgrade product of GSK980TDa, GSK980TDb (GSK980TDb-V) is the best choice of economic CNC turning machine.

Programming Volume

GSK980TDb

GSK980TDb-V

X, Z, Y, 4th, 5th ; axis name and axis type of Y, 4th, 5th can be defined

2ms interpolation period, control precision 1μm, 0.1μm

Max. speed 60m/min up to 24m/min in 0.1μm

Adapting to the servo spindle to realize the spindle continuously positioning, rigid tapping, and the rigid thread machining

Built-in multi PLC programs, and the PLC program currently running can be selected

G71 supporting flute contour cycle cutting

Statement macro command programming, macro program call with parameter

Metric/inch programming, automatic toolsetting, automatic chamfer, tool life management function

Chinese, English, Spanish, Russian display can be selected by parameters.

USB interface, U disc file operation, system configuration and software

2-channel 0V 10V analog voltage output, two-spindle control

1-channel MPG input, MPG function

41 input signals and 36 output signals

Appearance installation dimension, and command system are compatible with GSK980TDa

3

			GSK980TDb Turning CNC System	User Manual
		1.1.2	Technical specification
			Controllable axes
			Controllable axes: 5 X, Z, Y , 4th,5th
			Link axes 3
Volume
			PLC controllable axes 3 X, Z, Y
			Feed axis function
			Least input unit: 0.001mm 0.0001inch and 0.0001mm 0.00001inch
Programming			Least command unit 0.001mm 0.0001inch and 0.0001mm 0.00001inch
			Position command range: ±99999999× least command unit
			Rapid traverse speed max. speed 60m/min in 0.001mm command unit, max. speed
			24m/min in 0.0001mm command unit
			Rapid override: F0, 25%, 50%, 100%
			Feedrate override: 0 150% 16 grades to tune
			Interpolation mode: linear interpolation, arc interpolation(three-point arc interpolation),
			thread interpolation, ellipse interpolation, parabola interpolation and rigid tapping
			Automatic chamfer function
			Thread function
			General thread(following spindle)/rigid thread
			Single/multi metric, inch straight thread, taper thread, end face thread, constant pitch
			thread and variable pitch thread
			Thread run-out length, angle, speed characteristics can be set
			Thread pitch: 0.01mm 500mm or 0.06 tooth/inch 2540 tooth/inch
			Acceleration/deceleration function
			Cutting feed: linear
			Rapid traverse: linear, S
			Thread cutting: linear, exponential
			Initial speed, termination speed, time of acceleration/deceleration	can be set by
			parameters.
			Spindle function
			2-channel 0V 10V analog voltage output, two-spindle control
			1-channel spindle encoder feedback, spindle encoder line can be set 100p/r 5000p/r
			Transmission ratio between encoder and spindle: 1 255 : 1 255
			Spindle speed: it is set by S or PLC, and speed range: 0r/min 9999r/min
			Spindle override: 50% 120% 8 grades tune
			Spindle constant surface speed control
			Rigid tapping
			Tool function
			Tool length compensation
			Tool nose radius compensation C

Tool wear compensationTool life management

Toolsetting mode: fixed-point toolsetting, trial-cut toolsetting, reference point return toolsetting, automatic toolsetting

4

Chapter 1 Programming

	Tool offset execution mode: modifying coordinate mode, tool traverse mode
	Precision compensation
	Backlash compensation
	Memory pitch error compensation
	PLC function	Volume
	Two-level PLC program up to 5000 steps the 1st program refresh period 8ms
	PLC program communication download
	PLC warning and PLC alarm
		Programming
	Many PLC programs up to 16PCS , the PLC program currently running can be
	selected
	Basic I/O 41 input signals /36 output signals
Man-machine interface
	7.4″ wide screen LCD resolution: 234×480
	Chinese, English, Spanish, Russian display
	Planar tool path display
	Real-time clock
	Operation management
	Operation mode: edit, auto, MDI, machine zero return, MPG/single, manual, program
	zero return
	Multi-level operation privilege management
	Alarm record
	Program edit
	Program capacity: 40MB 10000 programs including subprograms and macro
	programs
	Edit function: program/block word search, modification, deletion
	Program format: ISO command, statement macro command programming, relative
	coordinate, absolute coordinate and compound coordinate programming
	Program call: macro program call with parameter, 4-level program built-in
	Communication function
	RS232 two-way transmitting part programs and parameters, PLC program, system
	software serial upgrade
	USB U file operation, U file directly machining, PLC program, system software U
	upgrade
	Safety function
	Emergency stop
	Hardware travel limit

Software travel check

Data backup and recovery

5

Programming Volume

GSK980TDb Turning CNC System User Manual

G command table

Table 1-1

Command Function

G00	Rapid traverse
	(positioning)
G01	Linear interpolation
G02	CW arc interpolation
G03	CCW arc interpolation
G04	Dwell, exact stop
G05	Three-point	arc
	interpolation
G6.2	Ellipse interpolation
	(CW)
G6.3	Ellipse
	interpolation(CCW)
G7.2	Parabola
	interpolation(CW)
G7.3	Parabola
	interpolation(CCW)
G12.1	Polar coordinate
	interpolation
G7.1	Cylinder interpolation
G15	Polar coordinate
	command cancel
G16	Polar coordinate
	command
G17	Plane selection
	command
G18	Plane selection
	command
G19	Plane selection
	command
G10	Data input ON
G11	Data input OFF

Command			Function
G20	Input in inch
G21	Input in metric
G28	Reference point return
G30	2nd, 3rd,		4th reference		point
	return
G31	Skip function
G32	Constant pitch thread cutting
G32.1	Rigid thread cutting
G33	Z tapping cycle
G34	Thread	cutting		with variable
	lead
G36	Automatic tool compensation X
G37	Automatic tool compensation Z
G40	Tool nose radius compensation
	cancel
G41	Tool nose radius compensation
	left
G42	Tool nose radius compensation
	right
G50	Workpiece		coordinate system
	setting
G65	Macro command non-modal
	call
G66	Macro program modal call
G67	Macro	program		modal	call
	cancel
G71	Axial roughing cycle(flute cycle)

Command

G72

G73

G70

G74

G75

G76

G80

G84

G88

G90

G92

G94

G96

G97

G98

G99

Function

Radial roughing cycle

Closed cutting cycle

Finishing cycle

Axial grooving cycle

Radial grooving cycle Multiple thread cutting cycle

Rigid tapping state cancel

Axial rigid tapping

Radial rigid tapping

Axial cutting cycle

Thread cutting cycle

Radial cutting cycle

Constant surface speed control

Constant surface speed control cancel

Feed per minute

Feed per revolution

1.1.3Environment and conditions

GSK980TDb storage delivery, working environment as follows:

Table 1-2

Item	Working conditions	Storage delivery conditions
Ambient temperature	0 45	-40 +70
Ambient humidity	≤90%(no freezing)	≤95%(40 )
Atmosphere pressure	86 kPa 106 kPa	86 kPa 106 kPa
Altitude	≤1000m	≤1000m

6

Chapter 1 Programming

1.1.4Power supply

GSK980TDb can normally run in the following AC input power supply.

Voltage: within(0.85 1.1)×rated AC input voltage (AC 220V);

Frequency: 49Hz 51Hz continuously changing

1.1.5Guard

GSK980TDb guard level is not less than IP20.

1.2CNC system of machine tools and CNC machine tools

CNC machine tool is an electro-mechanical integrated product, composed of Numerical Control Systems of Machine Tools, machines, electric control components, hydraulic components, pneumatic components, lubricant, cooling and other subsystems (components), and CNC systems of machine tools are control cores of CNC machine tools. CNC systems of machine tools are made up of computerized numerical control(CNC), servo (stepper) motor drive devices, servo (or stepper) motor etc.

Operational principles of CNC machine tools: according to requirements of machining technology, edit user programs and input them to CNC, then CNC outputs motion control commands to the servo (stepper) motor drive devices, and last the servo (or stepper) motor completes the cutting feed of machine tool by mechanical driving device; logic control commands in user programs to control spindle start/stop, tool selections, cooling ON/OFF, lubricant ON/OFF are output to electric control systems of machine tools from CNC, and then the electric control systems control output components including buttons, switches, indicators, relays, contactors and so on. Presently, the electric control systems are employed with Programmable Logic Controller (PLC) with characteristics of compact, convenience and high reliance. Thereof, the motion control systems and logic control systems are the main of CNC machine tools.

GSK980TDb Turning Machine CNC system has simultaneously motion control and logic control function to control two axes of CNC machine tool to move, and has nested PLC function. Edit PLC programs (ladder diagram) according to requirements of input and output control of machine tool and then download them to GSK980TDb Turning Machine CNC system, which realizes the required electric control requirements of machine tool, is convenient to electric design of machine tool and reduces cost of CNC machine tool.

Software used to control GSK980TDb Turning Machine CNC system are divided into system software (NC for short) and PLC software (PLC for short). NC system is used to control the display, communication, edit, decoding, interpolation and acceleration/deceleration, and PLC system for controlling explanations, executions, inputs and outputs of ladder diagrams.

Standard PLC programs are loaded (except for the special order) when GSK980TDb Turning Machine CNC System is delivered, concerned PLC control functions in following functions and operations are described according to control logics of standard PLC programs, marking with “Standard PLC functions” in GSK980TDb Turning CNC System User Manual. Refer to Operation Manual of machine manufacturer about functions and operations of PLC control because the machine manufacturer may modify or edit PLC programs again.

Programming Volume

7

Programming Volume

GSK980TDb Turning CNC System User Manual

Fig. 1-1

Programming is a course of workpiece contours, machining technologies, technology parameters and tool parameters being edit into part programs according to special CNC programming G codes. CNC machining is a course of CNC controlling a machine tool to complete machining of workpiece according requirements of part programs.

Technical flow of CNC machining is as following Fig. 1-2.

Analyse workpiece drawings and confirm machining processing

Edit part programs and record into CNC

Test part programs and execute trial run

Execute toolsetting and set tool offsets and coordinates

Run part programs and machine workpiece

Check part dimension and modify part programs and compensations

O0001

G00 X3.76 Z0

G01 Z-1.28 F50

…

M30

The machining ends and the workpiece is formed

Fig. 1-2

8

1.3Programming fundamentals

1.3.1Coordinates definition

Sketch map of CNC turning machine is as follows:

Chapter 1 Programming

Programming Volume

Fig. 1-3

GSK980TDb uses a rectangular coordinate system composed of X, Z axis. X axis is perpendicular with axes of spindle and Z axis is parallel with axes of spindle; negative directions of them approach to the workpiece and positive ones are away from it.

There is a front tool post and a rear tool post of NC turning machine according to their relative position between the tool post and the spindle, Fig. 1-5 is a coordinate system of the front tool post and Fig. 1-6 is a rear tool post one. It shows exactly the opposite of X axes, but the same of Z axes from figures. In the manual, it will introduce programming application with the front tool post coordinate system in the following figures and examples.

Z

X

Fig.1-4 Front tool post coordinate system

X

Z

Fig.1-5 Rear tool post coordinate system

1.3.2 Machine coordinate system, Machine Zero and machine reference point

Machine tool coordinate system is a benchmark one used for CNC counting coordinates and a fixed one on the machine tool. Machine tool zero is a fixed point which position is specified by zero switch or zero return switch on the machine tool. Usually, the zero return switch is installed on max. stroke in X, Z positive direction. Machine reference point is located at the position at which the

9

Programming Volume

GSK980TDb Turning CNC System User Manual

machine zero value adding the data parameter No.114/No.115 value. When No.114/No.115 value is 0, the machine reference point coincides with the machine zero. The coordinates of machine reference point is the No.120/No.121 value. Machine zero return/G28 zero return is to execute the machine reference point return. After the machine zero return/machine reference point return is completed, GSK980TDb machine coordinate system which takes No.120/No.121 value as the reference point.

Note: Do not execute the machine reference point return without the reference point switch installed on the machine tool, otherwise, the motion exceeds the travel limit and the machine to be damaged.

1.3.3Workpiece coordinate system and Program Zero

The workpiece coordinate system is a rectangular coordinate system based on the part drawing, also called floating coordinate system. After the workpiece is installed on the machine, the absolute coordinates of tool’s current position is set by G50 according to the workpiece’s measure, and so the workpiece coordinate system is established in CNC. Generally, Z axis of the workpiece coordinate system coincides with the spindle axis. The established workpiece is valid till it is replaced by a new one.

The current position of workpiece coordinate system set by G50 is the program zero.

Note: Do not execute the machine reference point return without using G50 to set the workpiece coordinate system after power on, otherwise, the alarm occurs.

Workpiece Rod

Z1 (Z2)

O2

O1

x1/2 (x2/2)

z1

z2

(x,z)

(x1,z1)

X/2

X2

X1

(x2,z2)

Z

(0,0)

Z

Fig. 1-6

X

In the above figure, XOZ is the coordinate system of machine tool, X1O1Z1 is the workpiece coordinate system of X axis located at the heading of workpiece, X2O2Z2 is the one of X axis located at the ending of workpiece, O point is the machine reference point, A point is the tool nose and coordinates of A point in the above-mentioned coordinate systems is as follows:

A point in the machine tool coordinate system: (x,z); A point in X1O1Z1 coordinate system: (x1,z1);

A point in X2O2Z2 coordinate system: (x2,z2).

10

Chapter 1 Programming

1.3.4Interpolation function

Interpolation is defined as a planar or three dimensional contour formed by path of 2 or multiple axes moving at the same time, also called Contour control. The controlled moving axis is called link axis when the interpolation is executed. The moving distance, direction and speed of it are controlled synchronously in the course of running to form the required Composite motion path. Positioning control is defined that motion end point of one axis or multiple axes instead of the motion path in the course of running is controlled.

GSK980TDb X and Z axis are link axes and 2 axes link CNC system. The system possesses linear, circular and thread interpolation function.

Linear interpolation: Composite motion path of X, Z axis is a straight line from starting point to end point.

Circular interpolation: Composite motion path of X, Z axis is arc radius defined by R or the circle center (I, K) from starting point to end point.

Thread interpolation: Moving distance of X or Z axis or X and Z axis is defined by rotation angle of spindle to form spiral cutting path on the workpiece surface to realize the thread cutting. For thread interpolation, the feed axis rotates along with the spindle, the long axis moves one pitch when the spindle rotates one rev, and the short axis and the long axis directly interpolate.

Example:

			Fig. 1-7
…
G32 W-27 F3;			(B→C; thread interpolation)
G1	X50	Z-30 F100;
G1	X80	Z-50;	(D→E; linear interpolation)
G3	X100 W-10 R10; (E→F; circular interpolation)

…

M30;

Programming Volume

11