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
Ⅰ GENERAL ......................................................................................................................................1
1 GENERAL ........................................................................................................................................2
1.1 General...................................................................................................................................2
1.2 Notes for Reading this Manual ...............................................................................................2
Ⅱ 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
Ⅲ 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
Ⅰ 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
Ⅱ 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).
O00002 N00180
EOB CODE
BLOCK
PROGRAM
END
S0000 T0100
PROGRAM
NAME
SEQUENCE
NO.
ADD: Ln：2
PROGRAM
O00002;
N60 X100 Y0；
N120 X0；
N180 G01 X50 Y50 F2000 ；
N240 G41 X100 D1；
N300 G01 Y100；
N360 G02 X200 R50；
N420 G01 Y0 F2500；
N480 X0；
N540 M30；
WORD
EDIT
【◆PRG】
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.
【CUR
/
MOD】 【DIR】【MDI】
【CUR/NXT】
Fig. 1-1 Program configuration
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
N
G
X
Y
Z
R
I
J
K
F
S
T
M
P
Q
H
D
0～99999
0～999999
000～999
-999999.9999～999999.9999（mm）
0～9999.9999（s）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
-999999.9999～999999.9999（mm）
0.1～1000000（mm/min）
0.001～10000(mm/r)
0～50000（r/min）
00～06
0～999
00～999
0～9999（s）
1～99999
-999999.999～999999.999（mm）
00～256
00～256
Shift amount of circular radius/angle
X vector between arc center and starting point
Y vector between arc center and starting point
Z vector between arc center and starting point
Miscellaneous function output, program
executed flow, subprogram call
Cutting depth or offset amount for low hole in
Program name
Sequence number
Preparatory function
X-coordinate address
Dwell time
X-coordinate address
X-coordinate address
R surface of canned cycle
Feedrate per minute
Feedrate per revolution
Specifying spindle speed
Multi-gear spindle output
Tool function
Dwell time
Call subprogram number
canned cycle
Length offset number
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.
1.3.1 Subprogram Writing and Call
1.3.1.1 Subprogram 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
Simultaneously controlled axes（in total
）
5 axes（X,Y,Z,4TH,5TH）
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.
2.3 Coordinate system
2.3.1 Machine 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
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.
GSK 25i Milling CNC System User Manual
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 Ⅰ workpiece base point ) When part is fixed on jigⅡ
To align the tool center to the workpiece
base point, specify the workpiece coordinate
system by CNC instructions at this position, and the
workpiece coordinate system coincides with the
programming coordinate system.
Workpiece coordinate system 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.
Because the tool center can’t be located at
the workpiece base point, locate the tool to a
position (or reference point) that has a distance
to the base point, set the workpiece coordinate
system by this distance(e.g. G92)
2.3.4 Maximum 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:
¾ G90 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.
¾ For 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.
¾ For example:
¾ O00001
¾ X100 Y100; （positioning to X100 Y100, G0 is initial mode）
¾ G1 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
Modal
Modal M function
Non-modal G function
Non-modal M function Only valid in the current block
G commands are being executed till they are
invalidated by another G commands.
M commands is being executed till they are
invalidated by another M commands.
Only valid in specified blocks and to be cancelled
at the end of a program Non-modal
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.
2.6 Basic Functions
2.6.1 Tool 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
Note:
Some machines move tables instead of tools but this manual assumes that tools are
Y R ;
Interpolation
a) Movement along straight line
b) Movement along arc
moved against workpiece. Refer to the actual move direction to avoid danger and damages.
2.6.2 Feed—Feed Function
X axis (Motor)
Y axis (Motor)
Tool movement
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
工 件
Tool diameter
V: Cutting speed
(m/min）
r/min
RPM
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
Loading...