www.teknikokul.net
SAFETY PRECAUTIONS When using a machine equipped with the MANUAL GUIDE, be sure to observe the following safety precautions.
s-1
www.teknikokul.net
SAFETY PRECAUTIONS
B-63424EN/03
DEFINITION OF WARNING, CAUTION, AND NOTE This manual includes safety precautions for protecting the user and preventing damage to the machine. Precautions are classified into Warning and Caution according to their bearing safety. Also, supplementary information id described as a Note. Read the Warning, Caution, and Note thoroughly before attempting to use the machine.
! WARNING Applied when there is a danger of the user being injured or when there is a danger of both the user being injured and the equipment being damaged if the approved procedure is not observed.
! CAUTION Applied when there is a danger of the equipment being damaged, if the approved procedure is not observed.
NOTE The Note is used to indicate supplementary information other than Warning and Caution. Read this manual carefully, and store it in a safe place.
s-2
www.teknikokul.net
SAFETY PRECAUTIONS
B-63424EN/03
FOR SAFETY DURING OPERATION To ensure safety while using a machine featuring the MANUAL GUIDE function, observe the following precautions:
! WARNING 1. Confirm, on the screen, that the data has been entered correctly before proceeding to the next operation. Attempting operation with incorrect data may cause the tool to strike the work-piece or machine, possibly breaking the tool or machine or injuring the operator. 2. Before starting the machine using the tool compensation function, carefully determine the direction of compensation and the compensation value, and ensure that the tool will not strike the work-piece or machine. Otherwise the tool or machine may be damaged or the operator may injured. 3. Before playing back an operation after teaching it, check the tool paths on the confirmation screen to ensure that the tool will not strike the work-piece or machine. Otherwise, the tool or machine may be damaged or the operator may be injured. 4. Set all necessary parameters and data items before starting MANUAL GUIDE operations. Note that if the cutting conditions are not suitable for the work-piece, the tool may be damaged or the operator may be injured. 5. After teaching a machining program created using MANUAL GUIDE functions, do no run the machine on that program immediately. Instead, confirm every step of the resultant program, and make sure that the tool path and machining operation are correct and that the tool will not strike the work-piece or machine. Before starting production machining, run the machine with no work-piece attached to the machine to make sure that the tool will not strike a work-piece or the machine. If the tool strikes the machine and/or work-piece, the tool and/or machine may be damaged, and even injuries the operator.
! CAUTION 1. After pressing the power-on button, do not touch any keys on the keyboard until the initial screen appears. Some keys are used for maintenance or special operations such that pressing such a key may cause an unexpected operation.
s-3
www.teknikokul.net
Table of Contents
B-63424EN/03
SAFETY PRECAUTIONS ............................................................................ s-1 I. GENERAL 1. OVERVIEW ........................................................................................................... 3 2. GUIDANCE HANDWHEEL ................................................................................ 4 3. ALL-IN-ONE SCREEN......................................................................................... 6 4. SYMBOLS USED................................................................................................... 8 5. PARAMETERS...................................................................................................... 9
II. OPERATION 1. OVERVIEW OF THE PROCEDURE............................................................... 13 1.1
MAIN FEATURES OF MANUAL GUIDE ........................................................................... 14
1.2
FLOWCHART OF OPERATIONS ........................................................................................ 15
2. PRE-SETTING OF THE OPERATIONS ......................................................... 17 2.1
SETTING OF WORK COORDINATE SYSTEM ................................................................. 18
2.2
SETTING OF TOOL OFFSET VALUES .............................................................................. 19
2.3
SETTING OF DISPLAYING WINDOW .............................................................................. 20
3. PROGRAMMING OPERATIONS .................................................................... 21 3.1
3.2
OVERVIEW OF PROGRAMMING OPERATION .............................................................. 22 3.1.1
Inputting of Program Number / Program Name.......................................................... 22
3.1.2
Selecting of Soft-key Menus....................................................................................... 24
3.1.3
Program Window........................................................................................................ 25
3.1.4
Pop-up Window.......................................................................................................... 26
3.1.5
Graphic Window......................................................................................................... 27
DETAIL OF EACH MENUS ................................................................................................. 28 3.2.1
Initial Setting .............................................................................................................. 28
3.2.2
Tool Setting ................................................................................................................ 31
3.2.3
MSF code ................................................................................................................... 34
3.2.4
Compensation ............................................................................................................. 35
3.2.5
Positioning.................................................................................................................. 37
3.2.6
Contour ....................................................................................................................... 38
3.2.7
Cycles ......................................................................................................................... 48
3.2.8
Teaching ..................................................................................................................... 48
3.3
EDITING OPERATION......................................................................................................... 49
3.4
CONTOUR PROGRAMMING OPERATION....................................................................... 52 3.4.1
Overview of Contour Programming............................................................................ 52
c-1
www.teknikokul.net
Table of Contents
B-63424EN/03
3.4.2
Contour Repetition ..................................................................................................... 53
3.4.3
Detail of Contour Calculation..................................................................................... 56
4. GUIDANCE CUTTING OPERATIONS (OPTIONAL FUNCTION)............ 67 4.1
SELECTING THE GUIDANCE CUTTING.......................................................................... 68
4.2
INPUTTING COMMON DATA............................................................................................ 68
4.3
TEACH-IN CUTTING MOTIONS ........................................................................................ 69
4.4
4.3.1
Program Window........................................................................................................ 69
4.3.2
Operation of Teach-in Auxiliary Function Blocks...................................................... 70
4.3.3
Operation of Teach-in a Rapid Traverse Motion Block ............................................. 70
4.3.4
Operation of Teach-in a Simple Linear Cutting Motion Block................................... 71
4.3.5
Operation of Guidance Cutting (Line) ........................................................................ 72
4.3.6
Operation of Guidance Cutting (Circle)...................................................................... 75
4.3.7
Operation of Teach-in a Cutting Block....................................................................... 78
EDITING TAUGHT-IN BLOCKS......................................................................................... 79 4.4.1
Program Window........................................................................................................ 79
4.4.2
Operations for Program Editing.................................................................................. 80
4.5
CHECKING CUTTING MOTIONS ON A GRAPHIC WINDOW ....................................... 81
4.6
PLAYBACK MACHINING ................................................................................................... 82 4.6.1
Execution of Playback Machining Program ............................................................... 82
4.6.2
Checking of Playback Machining Program ................................................................ 82
5. PROGRAM CHECKING.................................................................................... 84 5.1
5.2
TOOL PATH DRAWING ...................................................................................................... 85 5.1.1
Enlarge / Reduce......................................................................................................... 85
5.1.2
Tool Position .............................................................................................................. 86
5.1.3
Parameters of Tool Path Drawing............................................................................... 86
ANIMATED SIMULATION.................................................................................................. 88 5.2.1
Rotation ...................................................................................................................... 88
5.2.2
3-Plan View ................................................................................................................ 89
5.2.3
Cross Sectional View.................................................................................................. 89
5.2.4
Plan View ................................................................................................................... 90
5.2.5
Parameters of Animated Simulation ........................................................................... 90
5.3
FULL SCREEN GRAPHIC DISPLAY FUNCTION ............................................................. 92
5.4
BACKGROUND DRAWING (OPTION FUNCTION) ......................................................... 94 5.4.1
Selection of the Program with Which Drawing Is to Be Executed ............................. 94
5.4.2
Display and Cancellation of Alarms That May Be Generated During the Execution of Drawing................................................................................................. 95
5.4.3
Screen Switching Using a Function Key..................................................................... 95
c-2
www.teknikokul.net
Table of Contents
B-63424EN/03
5.5
5.4.4
Display of the Operation Status on the Drawing Screen............................................. 95
5.4.5
Handling of Various Data Items ................................................................................. 95
NOTES ON DRAWING......................................................................................................... 97
6. MACHINING OPERATION .............................................................................. 99 6.1
MEMORY OPERATION ..................................................................................................... 100
6.2
BACKGROUND EDITING ................................................................................................. 101
7. MDI / MANUAL OPERATION ....................................................................... 102 7.1
MDI OPERATION ............................................................................................................... 103
7.2
MANUAL OPERATION...................................................................................................... 104
8. OTHER FUNCTIONS....................................................................................... 105 8.1
CALCULATOR FUNCTION............................................................................................... 105
8.2
NC FORMAT OUTPUT FUNCTION ................................................................................. 107 8.2.1
Operation .................................................................................................................. 107
8.2.2
Window of Output NC Statements ........................................................................... 108
8.2.3
System variable for distinguishing the executing state (#3010)................................ 108
8.2.4
Parameter.................................................................................................................. 109
III. TYPES OF CYCLE MOTIONS 1. HOLE MACHINING......................................................................................... 113 1.1
1.2
1.3
1.4
DRILLING............................................................................................................................ 114 1.1.1
Drilling Cycle (Without Dwell) (G81)................................................................... 114
1.1.2
Drilling Cycle (With Dwell) (G82)........................................................................ 116
1.1.3
Drilling Cycle (Peck) (G83) .................................................................................. 119
1.1.4
Drilling Cycle (High-speed Peck) (G73) ............................................................... 122
BORING ............................................................................................................................... 124 1.2.1
Boring Cycle (Feed Retraction) (G85) .................................................................. 125
1.2.2
Boring Cycle (Rapid Retraction) (G86)................................................................. 127
1.2.3
Boring Cycle (Manual Retraction) (G88) .............................................................. 129
1.2.4
Boring Cycle (With Dwell) (G89) ......................................................................... 131
1.2.5
Boring Cycle (Fine Boring) (G76)......................................................................... 133
1.2.6
Boring Cycle (Back Boring) (G87) ....................................................................... 136
TAPPING ............................................................................................................................. 139 1.3.1
Tapping Cycle (G84) ............................................................................................... 140
1.3.2
Left-handed Tapping Cycle (G74)........................................................................... 142
RIGID TAPPING (G243) ................................................................................................... 144
2. HOLE PATTERN .............................................................................................. 147 2.1
POINTS (G200).................................................................................................................. 148
c-3
www.teknikokul.net
Table of Contents
B-63424EN/03
2.2
LINE (G201)........................................................................................................................ 149
2.3
GRID (G202) ...................................................................................................................... 151
2.4
SQUARE (G203) ................................................................................................................ 153
2.5
CIRCLE (G204)................................................................................................................... 155
2.6
ARC (G205)......................................................................................................................... 157
3. FACING .............................................................................................................. 159 3.1
SQUARE SURFACE (G210) .............................................................................................. 160
3.2
CIRCLE SURFACE (G211) ................................................................................................ 166
4. SIDE CUTTING................................................................................................. 169 4.1
SQUARE SIDE (G220) ....................................................................................................... 170
4.2
CIRCLE SIDE (G221) ......................................................................................................... 177
4.3
TRACK SIDE (G222).......................................................................................................... 180
4.4
ONE SIDE (G223)............................................................................................................... 183
4.5
CONTOUR SIDE (G224).................................................................................................... 187
5. POCKETING ..................................................................................................... 193 5.1
SQUARE POCKET (G230) ................................................................................................ 194
5.2
CIRCLE POCKET (G231) .................................................................................................. 200
5.3
TRACK POCKET (G232)................................................................................................... 203
5.4
GROOVE (G233) ................................................................................................................ 206
5.5
CONTOUR POCKET (G234) ............................................................................................. 212
5.6
CONTOUR GROOVE (G235) ............................................................................................ 219
6. OVERVIEW OF MEASURING CYCLES FUNCTION ............................... 226 6.1
PARAMETERS FOR MEASUREMENT ............................................................................ 227
6.2
MACRO VARIABLE FOR CALIBRATION CYCLES ...................................................... 228
6.3
MACRO VARIABLE FOR MEASURING CYCLES.......................................................... 229
6.4
DISPLAY THE MEASUREMENT RESULT...................................................................... 230
7. CALIBRATION CYCLES (OPTIONAL FUNCYION) ................................ 233 7.1
PROBE LENGTH CALIBRATION (G170) ........................................................................ 234
7.2
STYLUS BALL DIAMETER CALIBRATION (G171) ...................................................... 236
7.3
STYLUS X AND Y OFFSETS CALIBRATION- A (G172) ............................................... 238
7.4
STYLUS X AND Y OFFSETS CALIBRATION- B (G173) ............................................... 240
8. MEASURING CYCLES (OPTIONAL FUNCYION) .................................... 242 8.1
X/Y/Z SINGLE SURFACE MEASUREMENT (G180)....................................................... 243
8.2
WEB WIDTH MEASUREMENT (G181) ........................................................................... 246
8.3
GROOVE WIDTH MEASUREMENT (G182).................................................................... 248
8.4
OUTSIDE CIRCLE MEASUREMENT (G183)................................................................... 250
8.5
OUTSIDE CIRCLE MEASUREMENT (G183)................................................................... 253
c-4
www.teknikokul.net
Table of Contents
B-63424EN/03
8.6
OUTSIDE RECTANGULAR MEASUREMENT (G185) ................................................... 256
8.7
INSIDE RECTANGULAR MEASUREMENT (G186) ....................................................... 259
8.8
OUTSIDE CORNER MEASUREMENT (G187)................................................................. 262
8.9
INSIDE CORNER MEASUREMENT (G188)..................................................................... 264
8.10 BOLT-HOLE-CIRCLE MEASUREMENT (G189) ............................................................. 266 8.11 4- HOLES CENTER MEASUREMENT (G190) ................................................................. 269 8.12 WORK PIECE ANGLE MEASUREMENT (G191) ............................................................ 272 8.13 2-HOLES ANGLE MEASUREMENT (G192) .................................................................... 274
IV. SAMPLE OF PROGRAMMING 1. EXAMPLE OF INPUTTING PROGRAM...................................................... 279
APPENDIX A. PARAMETERS.................................................................................................. 295 A.1 GRAPHIC DISPLAY PARAMETERS ................................................................................ 296 A.2 MACRO EXECUTOR PARAMETERS............................................................................... 298 A.3 PARAMETERS FOR PROGRAMMING ............................................................................ 300 A.4 PARAMETERS FOR CYCLE MACHINING ..................................................................... 304 A.5 USER PARAMETERS ......................................................................................................... 308 A.6 COLOR PALLET SETTING PARAMETERS .................................................................... 309
B. ALARMS............................................................................................................. 312
c-5
www.teknikokul.net
I. GENERAL
www.teknikokul.net
GENERAL
B-63424EN/03
1
1. OVERVIEW
OVERVIEW
Overview of the manual This manual describes the functions related to MANUAL GUIDE for Milling of Series 16i/18i/21i-MA/MB. For other functions, refer to the operator’s manual for the Series 16i/18i/21i-MA/MB. The specifications and usage of the MANUAL GUIDE may vary according to the specifications of the operator’s panel of a machine tool. Be sure to read the manual provided by the machine tool builder. The functions of the CNC machine tool system are determined not only by the CNC, but by the combination of the machine tool, the power magnetic circuit in the machine tool, the servo system, the CNC and the operator’s panel. It is impossible to cover all possible combinations of all functions, programming methods, and operations in a single manual. This manual explains only the MANUAL GUIDE operations provided for the CNC. For individual CNC machine tools refer to applicable manuals from the machine tool builders. The manuals from machine tool builders take precedence over this manual. This manual explains as many detailed functions as possible. However, it is not possible to describe all of the items which cannot be done or which the operator must not do. Therefore, please assume that functions other than those described in this manual cannot be performed. Detailed information and special conditions are explained in notes. The readers may encounter new technical terms in the notes not previously defined or described. In this case, read this manual through first, then review the details.
-3-
www.teknikokul.net
2. GUIDANCE HANDWHEEL
2
GENERAL
B-63424EN/03
GUIDANCE HANDWHEEL
Guidance Cutting and Guidance Handwheel When a handwheel of a milling machine is rotated, the tool moves along only one axis. To carry out machining along a tapered or arc figure, an operator must rotate two handwheels simultaneously in synchronization. It is almost impossible to ensure accurate machining with this method.
Machining with a Milling Machine The Guidance Cutting eliminates the limitation of the milling machine and enables sophisticated machining. A guidance handwheel is provided so that an operator of the milling machine can easily implement the function. When the MANUAL GUIDE is used, just a few turns of the single guidance handle are required to carry out machining along a tapered or arc figure.
-4-
www.teknikokul.net
B-63424EN/03
GENERAL
2. GUIDANCE HANDWHEEL
Rotating the Guidance Handwheel for Machining After cutting a work-piece by using the above guidance cutting, this cutting motion can be taught into a machining program as an one block motion command, and these taught-in motion command can be used for playback machining.
Synchronous Feed and Guidance Handwheel During running a machining program under automatic executing mode, an operator can control a tool motion by using guidance handwheel. By selecting a synchronous feed mode on guidance handwheel, an operator can make a tool moved by the feedrate which is synchronized with handwheel rotating instead of inputted feedrate in the machining program.
NOTE This Guidance Cutting is the optional function of MANUAL GUIDE.
-5-
www.teknikokul.net
3. ALL-IN-ONE SCREEN
3
GENERAL
B-63424EN/03
ALL-IN-ONE SCREEN In MANUAL GUIDE, basically, only one screen called All-in-one Screen is used for all the operations for it.
Title area
CNC status area
FANUC MANUAL GUIDE Distance to go
Spindle speed & Spindle mode
Next block motion
Feedrate & Handwheel mode
Actual Position
Status indicator window
Program & Sequence Number & Others
Program (ISO code)
Graphic window
Key-in buffer
<
+
Soft-keys
Pop-up window
Program window
Title area : The title of MANUAL GUIDE is displayed always. CNC status area : Following CNC status information are displayed always. • Mode • Alarm status • Reset or Emergency stop status • Actual time Status indicator window : Following CNC status information are displayed always. • Actual machine position ( Max. 5 axes ) • Moving distance of actual and next block • Feedrate and Guidance handwheel mode • Spindle rotating speed and mode • Actual program and sequence number • Actual command by machining program (M, S, T, F) -6-
www.teknikokul.net
B-63424EN/03
GENERAL
3. ALL-IN-ONE SCREEN
Graphic window: Following graphical drawing are displayed as occasion demands. • Tool path of inputted ISO code program • Taught-in tool path of guidance cutting • Animated drawing of machining simulation • Tool path of machining simulation Program window : Following program information are displayed as occasion demands. • ISO code program Pop-up window : Following supplemental screens are displayed as occasion demands. • Work coordinate system • Tool Offset value • Program list • Detailed program data and illustration • Supplemental program data and illustration Key-in buffer : Inputting numerical data and its comment are displayed as occasion demands. Soft-keys : Following soft-keys comment for indicating its contents are displayed as occasion demands. • Machining type menu • Data item menu • Teach-in type menu • Operating key • Pop-up window menu There are the following soft-keys which means a special use. • Left end soft-key [<] : Return to the first soft-key. • Right end soft-key [+] : Display the next soft-key.
-7-
www.teknikokul.net
4. SYMBOLS USED
4
GENERAL
B-63424EN/03
SYMBOLS USED The following explains how keys and buttons are indicated in this manual. (1) Functions buttons are indicated in bold type : Example) PROG, OFFSET (2) The numeric key to be pushed is represented by underlining the corresponding number. Example) 12.345 (3) The input key is indicated in bold type in the same way as the function buttons. Generally, the input key follows numeric key input : Example) 12.345 INPUT (4) Soft-keys are enclosed in brackets [ ] : Example) [ LIST ], [LINE ] (5) The cursor keys are indicated by the following symbols : Example) ↑, ↓, ←, → (6) The page keys are indicated by the following symbols : Example) ↑, ↓
-8-
www.teknikokul.net
B-63424EN/03
5
GENERAL
5. PARAMETERS
PARAMETERS To use the MANUAL GUIDE, set the following parameter bits: (1) SGD (bit 0 of parameter No. 3112) = 0 SGD: Normal graphic display (0)/servo waveform display (1) (2) OIM (bit 0 of parameter No. 5006) = 0 OIM: Automatically converts the tool compensation during inch/metric conversion (1)/does not converts it(0).
-9-
www.teknikokul.net
II. OPERATION
www.teknikokul.net
B-63424EN/03
1
OPERATION
1. OVERVIEW OF THE PROCEDURE
OVERVIEW OF THE PROCEDURE
-13-
www.teknikokul.net
1. OVERVIEW OF THE PROCEDURE
1.1
OPERATION
B-63424EN/03
MAIN FEATURES OF MANUAL GUIDE By using MANUAL GUIDE, an operator can handle a milling machine from simple cutting using a handwheel to complicated machining. I. Guidance Cutting (Optional Function) By inputting target line or circle figure data, an operator can carry out an approach cutting or along cutting by using a guidance handwheel. Still more, by teaching these cutting motion blocks into CNC memory, an operator can carry out a playback machining repeatedly by using them, and at this time, he can control a tool motion by using a guidance handwheel in synchronous mode. II. Cycle Cutting By specifying the following canned cycles, an operator can carry out a complicated machining. • Hole machining • Hole position pattern • Facing • Side cutting ( included contour geometry ) • Pocketing ( included contour geometry ) Still more, an operator can create an ISO code program easily because of the following features. 1). Programming by selecting menu soft-keys MANUAL GUIDE classified the complicated ISO codes into several menus. Therefore, by selecting menu soft-keys, an operator can create an ISO code program easily. 2). Guidance window to illustrate required parameter Guidance window is displayed when it necessary, and support an operator to enter the data. 3). Inputted program checking Tool path and animated simulation are displayed on the graphic window. Therefore, an operator can confirm both the program and tool path easily at the same time. 4). Graphical Icon menu soft-keys All the menu soft-keys are prepared with graphical Icon. Therefore, an operator can understand the content of the menu easily. 5). Advanced canned cycles A lot of advanced canned cycles are prepared such as Drilling, Facing, Side cutting, Pocketing. Therefore, an operator can carry out the complicated machining automatically by specifying the canned cycles. -14-
www.teknikokul.net
1.2
1. OVERVIEW OF THE PROCEDURE
OPERATION
B-63424EN/03
FLOWCHART OF OPERATIONS After power ON, the following initial soft-keys are displayed. All necessary operations were arranged in the initial soft-keys. By pushing each soft-keys, each operation soft-keys are displayed. EDIT
MEM
MDI
HANDLE
CHECK
LIST
WRK-CO
OFFSET
SETING
The general of each soft-keys are as follows. • EDIT : Making or editing a program • MEM : Machining operation • MDI : MDI operation • HANDLE : Manual operation with JOG or HANDLE • CHECK : Checking a program with the graphic function • LIST : Program list for selecting, copying or deleting a program • WRK-CO : Setting of the work coordinate system • OFFSET : Setting of the tool offset value • SETING : Setting of the graphic window There are the following soft-keys, which means a special use. • Left end soft-key [<] : Return to the initial soft-keys • Right end soft-key [+] : Display the next page of soft-keys
-15-
www.teknikokul.net
1. OVERVIEW OF THE PROCEDURE
OPERATION
B-63424EN/03
The following flow chart shows the general procedure from preparing to start making a machining program to executing a machining by using MANUAL GUIDE. < Reference & Softkey > Set parameters
Set tool offset data
APPENDX
II.2 PRE-SETTING OF THE OPERATION WRK-CO
ISO code programming start
OFFSET
SETING
II.3 PROGRAMMING OPERATIONS EDIT
Input program No.
II.3.1.1 INPUTTING OF O NO. / NAME LIST
Which menu ?
Guidance cutting
Line, Arc, MSF code etc.
II.3.2 DETAIL OF EACH MENUS II.3.3 EDITING OPERATIONS Canned cycles III. TYPES OF CYCLE MOTIONS
Programming end ? No Yes Check by animated drawing
II.5 PROGRAM CHECKING CHECK
Execute a machining program
II.6 MACHINING OPERATION MEM
MDI operation / Manual operation
II.7 MDI / MANUAL OPERATION MDI
-16-
www.teknikokul.net
HANDLE
B-63424EN/03
2
OPERATION
2. PRE-SETTING OF THE OPERATIONS
PRE-SETTING OF THE OPERATIONS An operator have to set the work coordinate system and tool offset before the operation of programming or machining.
-17-
www.teknikokul.net
2. PRE-SETTING OF THE OPERATIONS
2.1
OPERATION
B-63424EN/03
SETTING OF WORK COORDINATE SYSTEM By pushing the soft-key [WRK CO], the following soft-keys are displayed. These soft-keys are the menu for setting the work coordinate system. INPUT
+INPUT
RETURN
The general of each soft-keys are as follows. • INPUT/ +INPUT : Set the work coordinate system to the inputted data • RETURN : Return to the former soft-keys At same time, the following pop-up window of the work coordinate system is displayed on the screen. This window consists of two or more pages. Therefore, by pushing ↑, ↓ page key, the desired page is displayed. An operator sets the offset values for the work-piece zero point by pushing ↑, ↓, ←, → cursor key and inputting the data. WORK CO. NO.
DATA
NO.
DATA
0.000 0.000 0.000
02 X (G55) Y Z
152.580 56.284 0.000
01 X 100.000 (G54) Y 50.000 Z 50.000
03 X (G56) Y Z
300.000 200.000 0.000
00 X (EXT) Y Z
NOTE 1 In the case that the machine has one work coordinate system only, please set the work coordinate system by using G92 command at the first of program. 2 This window does not support workpiece coordinate system 48 or 300.
-18-
www.teknikokul.net
2.2
2. PRE-SETTING OF THE OPERATIONS
OPERATION
B-63424EN/03
SETTING OF TOOL OFFSET VALUES By pushing the soft-key [OFFSET], the following soft-keys are displayed. These soft-keys are the menu for setting the tool offset. INPUT
+INPUT
RETURN
The general of each soft-keys are as follows. • INPUT/ +INPUT : Set the work coordinate system to the inputted data • RETURN : Return to the former soft-keys At same time, the following pop-up window for setting tool offset values is displayed on the screen. This window consists of two or more pages. Therefore, by pushing ↑, ↓ page key, the desired page is displayed. In MANUAL GUIDE, the offset code for cutter compensation and tool length compensation are specified as D code and H code. An operator sets the offset values by pushing ↑, ↓, ←, → cursor key and inputting the data. OFFSET
001/25
LENGTH
RADIUS
NO. GEOMETRY WEAR GEOMETRY WEAR 1 2 3 4 5 6
100.0 200.0 300.0 400.0 500.0 600.0
0.1 0.2 0.3 0.4 0.5 0.6
-19-
www.teknikokul.net
10.0 20.0 30.0 40.0 50.0 60.0
0.1 0.2 0.3 0.4 0.5 0.6
2. PRE-SETTING OF THE OPERATIONS
2.3
OPERATION
B-63424EN/03
SETTING OF DISPLAYING WINDOW By pushing a [SETTNG], the following pop-up window for displaying the work figure is displayed on the screen. These data are defining automatically by setting the INITIAL SET menu. So, in ordinary case, an operator needs not to set or refer to it. When more detailed control for display, set to these data if necessary.
PROGRAMING FIGURE SETTING WORK FIGURE COORDINATE SCALE MAX X AXIS Y AXIS Z AXIS SCALE MIN X AXIS Y AXIS Z AXIS COLOR PATH WORK
= = = = = = = = = =
ON XY 0.000 0.000 0.000 0.000 0.000 0.000 WHITE WHITE
The meanings of each parameter are described below. 1)
WORK FIGURE Select whether a work figure is displayed or not.
2)
COORDINATE This parameter specifies a type of drawing screens. ( Only X-Y plane is available at present. )
3)
SCALE MAX. / MIN. The maximum drawing coordinates (X, Y, Z) / minimum drawing coordinates (I, J, K) are set. ( Usually these scale factors are automatically determined so that this parameter need not be set. )
4)
COLOR Seven colors (white, red, green, yellow, blue, purple, and light blue) are available for selection. - PATH : Specify the color for drawing the tool path. ( It is not available at present. ) - WORK : Specify the color for drawing the work figure.
-20-
www.teknikokul.net
B-63424EN/03
3
OPERATION
3. PROGRAMMING OPERATIONS
PROGRAMMING OPERATIONS
-21-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
3.1
OPERATION
B-63424EN/03
OVERVIEW OF PROGRAMMING OPERATION ISO code program consists of G-code and the attached parameters. Therefore, an operator has to grasp the meaning of the G-code and parameters. But, it is very difficult for an inexperienced operator to do it. MANUAL GUIDE makes an operator to create ISO code program easily by conversational methods.
3.1.1
Inputting of Program Number / Program Name By pushing the soft-key [LIST], the following soft-keys are displayed. These soft-keys are the menu for selecting, copying or deleting a program. SELECT
COPY
DELETE
O
RETURN
SEARCH
The general of each soft-keys are as follows. • • • • •
SELECT COPY DELETE O-SEARCH RETURN
: Select a program or insert new program : Copy a program : Delete a program : Search program number (O) : Return to the former soft-keys
At the same time, the following pop-up window of program list is displayed on the screen. PROGRAM LIST PROGRAM NO. USED / FREE 3 / 122 MEMORY AREA USED / FREE 900 / 3000 NO. NAME DATE O0010: CIRCLE MACHINING 1999/01/12 10:12 O0020: LINE MACHINING 1999/02/10 11:21 O0020
SIZE 380 520
Cursor
Program Number Program Name (Max 12ch.)
-22-
www.teknikokul.net
Lastly modified date and time
Program size
OPERATION
B-63424EN/03
3. PROGRAMMING OPERATIONS
The displayed items of this window are as follows. • The number of Used / Free program • The size of Used / Free memory area • Program number • Program name (Max. 12ch./ Character except “(“, ” )”, “;”, “,” ) • Lastly modified date and time • Program size The operation of each menu is as follows. l Insert a new program 1) In the pop-up window of program list, input a new program number to the key-in buffer. 2)
Push INSERT or soft-key [SELECT]. After that, the new program is inserted in program memory.
l Select a program 1) In the pop-up window of program list, place the cursor at the program to select. 2)
By pushing [SELECT], the program is selected.
l Input a name of program 1) In the pop-up window of program list, place the cursor to the program name field. 2)
Input program name through key-board, and push INPUT. The maximum character number of it is 12.
l Copy a program 1) In the pop-up window of program list, place the cursor at the program to be copied. 2)
Push [COPY] and input the new program number to the key-in buffer with LCD/MDI key.
3)
By pushing [EXEC], the program is copied to new program. When new program number already exists, push [OVER WRITE] if not care.
l Delete a program 1) In the pop-up window of program list, place the cursor at the program to be deleted. 2)
Push [DELETE] and push [EXEC]. After that, the program is deleted.
-23-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
l Search a program 1) Input the program number, which you want to search, to the key-in buffer 2)
3.1.2
By pushing [SEARCH], the program is searched.
Selecting of Soft-key Menus MANUAL GUIDE classified the complicated ISO codes into several menus. Therefore, by selecting Icon menu soft-keys, an operator can create ISO code program easily. After inputting program number and name, by pushing [EDIT] of the initial soft-keys, The following soft-keys of Editing menu are displayed. INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
In MANUAL GUIDE, this menu is called “ Editing menu ”. The general of Editing menu are as follows. • INIT • • • • • • • •
TOOL MSF COMP POSTIN CONTUR CYCLE TEACH RETURN
:
Definition of work coordinate system, blank form data : Definition of tool data : Instruction of M, S, F code except G code : Instruction of cutter or tool length compensation : Instruction of Line figure : Instruction of Contour figure ( Line + Circle ) : Definition of canned cycles such as drilling, milling : Guidance cutting operation and teaching : Return to the former soft-keys
NOTE As to [TEACH] menu, please refer to “4. GUIDANCE CUTTING OPERATIONS (OPTION)”.
-24-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
The input sequence of machining program is basically as follows. (1). INIT → Definition of initial data (2). TOOL → Definition of tool data (3). POSTIN → Move tool to a start point by positioning command (4). CYCLE → Definition of canned cycles for milling (5). POSTIN → Retract tool at the safety point by postioning command (6). Repeating (2), (3), (4), (5) (7). MSF → Instruction of program end such as M30, M02
NOTE In each CYCLE machining, the tool is moved from the present position to cutting start point (R point). Therefore, be sure to move the tool to the safety point which do not interfere with work-piece and jig. After that, please define each CYCLE machining. In the case that the tool is at the safety position, the above block of (3) and (5) are not necessary.
3.1.3
Program Window The inputted ISO code program is displayed in a program window. The number of the end-left side is block sequence number and the number is corresponded to the number which is indicated as tool path number on a graphic window. An operator can create a ISO code program by selecting Editing menu soft-key and inputting the data of pop-up window. ( Refer to the next paragraph.) And an operator can create a program by inputting directly the data without displaying a pop-up window, too.
1 2 3 4 5 6 7 8
Sequence Number
G17 G90 G54 ; G00 X0. Y0. Z100. ; M6 T1; S4240 M7 G43 H1 ; G0 X10. Y10. Z0. ; G1 X30. Y10. F500. ; G1 X30. Y20. ; G2 X60. Y50. R20. ;
Program Window
-25-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
3.1.4
OPERATION
B-63424EN/03
Pop-up Window When the operator selects each menu soft-keys, the soft-keys [ON/OFF (WINDOW)] and [DETAIL] (if a detail menu exists) are displayed. After that, soft-key [ON/OFF] is described as [WINDOW] in this manual. • [WINDOW] soft-key By pushing [WINDOW] soft-key, the following pop-up window in which is displayed the necessary item and illustration. And this window is available from now on. In the case of no pop-up window display, push [WINDOW] again. The data is entered by pushing INPUT key. After inputting the whole necessary data, by pushing a INSERT key, a pop-up window is closed and inputted data are displayed in a program window. The displaying maximum item number of a pop-up window is 8. If the number is beyond, by pushing a page key ↑ and ↓, the item more than 8 are displayed in a pop-up window. TOOL SET
1/1
TOOL NO. CUTTER OFFSET NO. LENGTH OFFSET NO. ANIMATION T RADIUS
T= D= H= R=
T
R
[TOOL] Pop-up Window
• [DETAIL] soft-key By pushing [DETAIL] soft-key, the following pop-up window in which is displayed the supplemental item and illustration. In ordinary case, an operator needs not to call this detail data window excepting the case of checking these data. When more detailed control for machining motions is necessary, check and change these data if necessary. TOOL SET (DETAIL) NEXT TOOL NO.
N= T
[TOOL] Pop-up Window of Detailed Data
-26-
www.teknikokul.net
N
3.1.5
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
Graphic Window In the contour programming, inputted G code blocks are displayed on the graphic window with a tool path as the same time of inputting G code block. The number of tool path is corresponded to the number which is indicated as the block sequence number on a program window.
8 7 5 6 Graphic Window
NOTE The tool path of Cycle motion such as Hole machining, Facing or Pocketing is not displayed.
-27-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
3.2
OPERATION
B-63424EN/03
DETAIL OF EACH MENU MANUAL GUIDE has the following Editing menus.
NOTE On any menu, pushing the MDI keys [CAN] + [INPUT] causes blank data to be entered.
3.2.1
Initial Setting This is the menu which is defined the necessary initial data before programming such as a work coordinate system, blank form data and son on. An operator basically sets this menu at first. • In the case of [WINDOW] ON By pushing [INIT], the following pop-up window is displayed. INITIAL SET WORK CO-ORD. WORK SHAPE WORK X CO-ORD. WORK Y CO-ORD. WORK Z CO-ORD. WORK X WIDTH WORK Y WIDTH WORK THICKNESS
WORK CO-ORD.
1/1 G= NO OUT P= RECT. X= Y= Z= I= J= K=
: Select the standard coordinate system (G54, G55, , , G59, NO OUT) from soft-keys.
NOTE Workpiece coordinate systems 48 and 300 are not supported. WORK SHAPE
: Select the work shape from the following soft-keys.
[RECT: rectangular], [CYLIN: cylinder] [NO OUT: no instruction] WORK X, Y, Z CO-ORD. WORK X,Y WIDTH THICKNESS
: Input coordinates (X,Y,Z) of blank origin. : Input a blank dimension.
Rect. : length along X-axis(I), Y-axis(J), Zaxis(K) Cyl. : out radius(I), inside radius(J), blank length(K)
-28-
www.teknikokul.net
B-63424EN/03
3. PROGRAMMING OPERATIONS
OPERATION
By pushing [DETAIL], the following pop-up window is displayed. INITIAL SET (DETAIL) ABS / INC PLANE SELECTION ORIGIN POINT
A= NO OUT S= NO OUT B= CENTER
: Select the command travels from the following soft-keys. [ABS: G90], [INC: G91], [NO OUT: no instruction] : Select the used plane from the following softkeys. [XY-PLANE: G17], [ZX-PLANE: G18], [YZ-PLANE: G19], [NO OUT: no instruction] : Select the blank origin point from the following soft-keys. [CENTER], [DOWN-LEFT] : (if the inch/metric conversion option is enabled) Select the input unit (inch: G20, millimeter: G21, or no output).
ABS / INC
PLANE SELECTION
ORIGIN POINT
INPUT UNIT
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G300 W
P X Y Z I
J
K (A S
B M );
← Setting of Initial Data
• In the case of [WINDOW] OFF In case that a pop-up window is closed, G code or the addresses is display in a key-in buffer field automatically as the above ISO code program is created. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
-29-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
NOTE If ISM (bit 6 of parameter No. 9105) is 1, the detailed input items, travel distance specification, plane selection, and input unit, are displayed in the normal window. INITIAL SET WORK CO-ORD. ABS / INC PLANE SELECTION INPUT UNIT WORK X CO-ORD. WORK Y CO-ORD. WORK Z CO-ORD. WORK SHAPE
-30-
www.teknikokul.net
G= NO OUT A= NO OUT S= NO OUT M= NO OUT X= Y= Z= P=RECT.
3.2.2
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
Tool Setting This is the menu which is defined the data of used tool for a machining. An operator basically sets this menu before each machining. • In the case of [WINDOW] ON By pushing [TOOL], the following pop-up window is displayed. TOOL SET
1/1
TOOL NO. CUTTER OFFSET NO LENGTH OFFSET NO ANIMATION T RADIUS
TOOL NO. CUTTER OFFSET NO LENGTH OFFSET NO ANIMATION T RADIUS
T= D= H= R=
: Input the used tool number (T code). : Input the used offset number (D code) for cutter compensation. : Input the used offset number (H code) for tool length compensation. : Input the radius of used tool for animated simulation.
By pushing [DETAIL], the following pop-up window is displayed. TOOL SET (DETAIL) NEXT TOOL NO.
NEXT TOOL NO.
N=
: When a machine with an automatic tool changer (ATC) is used, input the next used tool number so that the tool can be selected from the tool magazine used to set the tool in standby position.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G301 T
D
H
(R N ) ;
-31-
www.teknikokul.net
← Setting of Tool Data (Tool Change Motion )
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
• In the case of [WINDOW] OFF In case that a pop-up window is closed, G code or the addresses is display in a key-in buffer field automatically as the above ISO code program is created. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
NOTE 1) In the case of the parameter No.9105 #1(DCD) = 0 & No.9105 #2(ATR) = 0 TOOL SET TOOL NO. CUTTER OFFSET NO LENGTH OFFSET NO
1/1 T= D= H=
The offset data (D) is used for animation. The operator has to input (D) in spite of the drilling tool. 2) In the case of the parameter No.9105 #1(DCD) = 0 & No.9105 #2(ATR) = 1 TOOL SET TOOL NO. CUTTER OFFSET NO LENGTH OFFSET NO ANIMATION T RADIUS
1/1 T= D= H= R=
The offset data of (D) is displayed as the default data of (R), and the data of (R) is used for animation. 3) In the case of the parameter No.9105 #1(DCD) = 1 & No.9105 #2(ATR) = 1 TOOL SET
1/1
TOOL NO. T= ANIMATION T RADIUS R=
The data (R) is used for animation. The operator has to input (D) in COMP menu in order to calculate the tool path automatically in the cycle machining.
-32-
www.teknikokul.net
B-63424EN/03
3. PROGRAMMING OPERATIONS
OPERATION
NOTE 4) This menu is supposed as the following tool change sequence. In this sequence, the tool length compensation function is not instructed. So, when the operator wants to use it, please instruct it in COMP menu. The specifications of tool change is different for each machine. Therefore, please refer to the manual prepared by machine tool builder. TOOL CHANGE MACRO PROGRAM O9301 ; G91 ; G28 Z0 ; G28 X0 Y0 ; G90 ; T M6 ; D ; H ; T ; G10 L91 R ; M99 ;
( Change tool ) ( Set cutter offset No. ) ( Set length offset No. ) ( Set tool in stand by position ) ( Set radius for simulation )
By setting the parameter No.9106 to the sub program number, the program is called instead of M6 only.
-33-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
3.2.3
OPERATION
B-63424EN/03
MSF code This is the menu which is instructed M code (auxiliary function), S code (spindle speed function) and F code (feed function) except G code.
NOTE The specifications of M code is different for each machine. So, please refer to the manual prepared by machine tool builder. • In the case of [WINDOW] ON By pushing [MSF], the following pop-up window is displayed. MSF CODE
1/1
M CODE SPINDLE SPEED FEED RATE
M CODE SUBPROGRAM SPINDLE SPEED FEED RATE
M= S= F=
: Input the M code number of the auxiliary function. : Input the program number of subprogram ( In the case of M98) : Input the speed of the tool. : Input the tool feed rate.
In this menu, there is no detail data window. Therefore, when an operator pushes [DETAIL], the detail data window remained closing. After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
M (S F P ) ;
← Instructing of MSF code
-34-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
• In the case of [WINDOW] OFF In case that a pop-up window is closed, G code or the addresses is display in a key-in buffer field automatically as the above ISO code program is created. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
3.2.4
Compensation This is the menu which is instructed the cutter compensation and tool length offset such as G40, G41, G43, G44 and G49. • In the case of [WINDOW] ON By pushing [COMP], the following pop-up window is displayed. COMPENSATION CUTTER COMP. CUTTER OFFSET NO LENGTH COMP. LENGTH OFFSET NO RAPID / CUT. END POINT X END POINT Y END POINT Z
1/2 G= D= G= H= G= X= Y= Z=
CUTTER COMP.
CUTTER OFFSET NO LENGTH COMP.
LENGTH OFFSET NO RAPID / CUT. END POINT X, Y, Z FEED RATE
COMPENSATION FEED RATE
2/2 F=
: Select the cutter compensation from the following soft-keys. [G41], [G42], [G40], [NO OUT] : Input the offset number for cutter compensation. : Select the tool length compensation from the following soft-keys. [G43], [G44], [G49], [NO OUT] : Input the offset number for tool length compensation. : Select the motion from the following soft-keys. [RAPID: G00], [CUT: G01] : Input the coordinate (X, Y, Z) of the end point in the work coordinate system. : Input the tool feed rate.
-35-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G40/G41/G42 D
G43/G44/G49 H
G00/G01 X
Y Z F ;
← Instructing of Compensation function • In the case of [WINDOW] OFF In case that a pop-up window is closed, G code or the addresses is display in a key-in buffer field automatically as the above ISO code program is created. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
-36-
www.teknikokul.net
OPERATION
B-63424EN/03
3.2.5
3. PROGRAMMING OPERATIONS
Positioning This is the menu which is instructed the positioning such as G0, G60, G28 and G30. • In the case of [WINDOW] ON By pushing a [POSTIN], the following pop-up window is displayed. POSITIONING ABS / INC POSITIONIING REF POST RETURN END POINT X END POINT Y END POINT Z
ABS / INC
POSITIONING
REF POST RETURN REFERENCE POSITION END POINT X, Y, Z INTERMED POINT X, Y, Z
FEED RATE
1/1 G= NO OUT G= NO OUT G= NO OUT X= Y= Z=
: Select the travel ways from the following softkeys. [G90], [G91], [NO-OUT] : Select the positioning from the following softkeys. [G00], [G01], [G60], [NO-OUT] : Select the reference position return from the following soft-keys. [G28], [G30], [NO-OUT] : Select the reference position from the following soft-keys. [2ND], [3RD], [4TH] : Input the coordinate (X, Y, Z) of the end point in the work coordinate system. ( in the case of G00, G01 or G60 ) : Input the coordinate (X, Y, Z) of the intermediate point in the work coordinate system. ( in the case of G28 or G30 ) : Input the tool feed rate. ( in the case of G01)
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
(G90/G91) G0/G60/G28/G30 (P ) X ← Instructing of Positioning command -37-
www.teknikokul.net
Y Z ;
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
• In the case of [WINDOW] OFF In case that a pop-up window is closed, G code or the addresses is display in a key-in buffer field automatically as the above ISO code program is created. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
3.2.6
Contour This is the menu which is instructed the contour figure by selecting the figure type menu. By pushing a [CONTR] soft-key, the following menu soft-keys are displayed. START
LINE
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT
RECALC
RETURN
The general of each menus are as follows. • START : Instructing the start point • LINE : Instructing the line figure • CW ARC : Instructing the clockwise arc figure • CCW AR : Instructing the counterclockwise arc figure • CHAMF : Instructing the chamfer figure • ROUND : Instructing the round figure • END : Instructing the end of figure • TANGNT : Instructing the tangent • RECALC : Executing the calculation of intersection After this, the manual is described only the case that a pop-up window is opened. Select a figure type by pushing the corresponding soft-key. When a figure has been selected, a pop-up window for inputting contour figure data appears. Enter the data that is designated on the plan. As to the case that a pop-up window is closed, G code or the addresses correspond to the above figure type menus is display in a key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next addresses is displayed. After repeating this operations, by pushing INSERT key, and inputted data are decided. ( “;” is inserted.)
-38-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
1) START POINT By pushing [START], the following pop-up window is displayed. Usually, pushing [CONTOUR] on an Editing menu first causes the following [START POINT] window to be automatically displayed. START POINT START POINT X START POINT Y START POINT TYPE
START POINT X, Y START POINT TYPE
1/1 X= Y= E= START
: Input the coordinate (X, Y) of the start point in the contour figure : Select the start point type from the following soft-keys. [START] : Start point of external figure [ISLAND] : Start point of island figure
NOTE The maximum number of island is 6. [NXT MVE]: Start point of next groove figure [DIRECT] : Start point of single cut or positioning
NOTE In the case of DIRECT, please be sure to select the soft-key [END] in the END menu. ISLAND Z CO-ORD. GROOVE Z CO-ORD. MOV TYPE TO ST. PT.
FEED RATE TO ST. PT. FEED RATE FROM ST. PT. CUTTER
: In the case of ISLAND, input the Z coordinate of the top island. : In the case of NXT MVE, input the Z coordinate of the escape for moving the next groove. : In the case of DIRECT, select the moving type from the following soft-keys. [RAPID] : Rapid traverse to start point [CUT] : Cutting motion to start point : In the case of DIRECT + CUT, input the feed rate from the present point to the start point. : In the case of DIRECT, input the feed rate from the start point. : (in the case of [DIRECT])
-39-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
Select from among cutting on the left side as the cutter faces the shape, cutting on the right side, and no output.
COMPENSATION DIRECTION
Right side
Left side
NOTE On the END (G106) menu, cutter compensation cancel (G40) is output. After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G100 X Y E
(Z R P F D U ) ; Inputted data Start point type End point (X, Y) G code for start point
2) LINE By pushing [LINE], the following pop-up window is displayed. LINE
1/1
DIRECTION END POINT X END POINT Y LENGTH ANGLE
B= M= N= L= K=
DIRECTION
: Select the direction of the line from the following soft-keys.
END POINT X, Y
: Input the coordinate (X, Y) of the end point in the line. : Input the length of the line. : Input the angle of the line.
LENGTH ANGLE
-40-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
An angle is specified as a displacement from the X axis. ( CCW : +, CW : - ) By pushing [DETAIL], the following pop-up window is displayed. LINE (DETAIL) COMPONENT ANG-X COMPONENT ANG-Y AUX. POINT X AUX. POINT Y AUX. DISTANCE PAR. / VERT. REF. BLOCK NO.
COMPONENT ANGL – X, Y AUX. POINT X, Y AUX. DISTANCE PAR. / VERT.
REF. BLOCK NO
I= J= U= V= D= E= A=
: Input the X and Y component of the angle.
: Input the coordinate (X, Y) of an auxiliary point : Input the distance between the auxiliary point and oblique line. : Specify whether the line to be defined is parallel or vertical to a line defined in a previous block. : To define the line, parallel or vertical to a line defined in a previous block, specify the number of that block.
After inputting the necessary data, by pushing INSERT, pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G101 X Y B
M N L K Q
(I J
U V D E
A );
Inputted data End point (X, Y) G code for contour line
NOTE After calculating intersections, the address only is displayed in the case that the data is not defined.
-41-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
3) CW ARC By pushing [CW ARC], the following pop-up window is displayed. CW ARC
1/1
RADIUS CENTER POINT X CENTER POINT Y END POINT X END POINT Y ANGLE
E= V= W= M= N= K=
: Input the radius of the arc. : Input the coordinate (X, Y) of the center of the arc. : Input the coordinate (X, Y) of the end point of the arc. : Input the center angle of the arc.
RADIUS CENTER POINT X, Y END POINT X, Y ANGLE
By pushing displayed.
[DETAIL], the following pop-up window is
CW ARC (DETAIL) CHORD LENGTH TANGENT ANGLE
L= A=
: Input the chord length of an arc. Straight-line distance from the start point of an arc to its end point : Input the angle of an inclination of the straight line which is tangent to the circle to be defined, at the start point of the arc.
CHORD LENGTH TANGENT ANGLE
-42-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G102 X Y R I
J
B
E
V W
M N K Q
(L
A );
Inputted data Center point (X, Y) Radius of arc End point (X, Y) G code for contour CW arc
NOTE After calculating intersections, the address only is displayed in the case that the data is not defined. 4) CCW ARC By pushing [CCW ARC], the following pop-up window is displayed. CCW ARC
1/1
RADIUS CENTER POINT X CENTER POINT Y END POINT X END POINT Y ANGLE
E= V= W= M= N= K=
: Input the radius of the arc. : Input the coordinate (X, Y) of the center of the arc. : Input the coordinate (X, Y) of the end point of the arc. : Input the center angle of the arc.
RADIUS CENTER POINT X, Y END POINT X, Y ANGLE
-43-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
By pushing displayed.
B-63424EN/03
[DETAIL], the following pop-up window is
CCW ARC (DETAIL) CHORD LENGTH TANGENT ANGLE
L= A=
: Input the chord length of an arc. Straight-line distance from the start point of an arc to its end point : Input the angle of an inclination of the straight line which is tangent to the circle to be defined, at the start point of the arc.
CHORD LENGTH TANGENT ANGLE
After inputting the necessary data, by pushing a INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G103 X Y R I
J
B
E
V W
M N K Q
(L
A );
Inputted data Center point (X, Y) Radius of arc End point (X, Y) G code for contour CCW arc
NOTE After calculating intersections, the address only is displayed in the case that the data is not defined.
-44-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
5) CHAMFER By pushing [CHAMFER], the following pop-up window is displayed. CHAMFER CHAMFER
1/1 I=
: Input the chamfer amount.
CHAMFER
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G104 X Y I
; Inputted data End point (X, Y) G code for contour chamfer
NOTE After calculating intersections, the address only is displayed in the case that the data is not defined. 6) ROUND By pushing [ROUND], the following pop-up window is displayed. ROUND
1/1
RADIUS
R=
: Input the radius of Corner-C.
RADIUS
-45-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G105 X Y R I
J
; Center point (X, Y) Radius of an arc End point (X, Y) G code for contour chamfer
NOTE After calculating intersections, the address only is displayed in the case that the data is not defined.
7) END By pushing a [END], the following pop-up window is displayed. END
1/1
CONTINUE
P= END
: Specify whether an island or a groove will be defined or not from soft-keys [END] and [CONT].
CONTINUE
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G106 P
; Inputted data G code for contour end
-46-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
8) TANGENT Pushing [TANGNT] specifies that the next figure form a tangent to the previous figure ( either figure must be a arc). For next figure, arc or line must be entered. Address Q of G101,G102 and G103 are used to this data. When [TANGNT] is selected, “TANGNT” is displayed on a screen. 9) RECAL When a new contour figure is added at the end of a series of previously inputted figures, contour calculating is automatically done after pushing INSERT. On the other hand, when some figures are changed after inputted and contour calculated, during data changing, there may be a case that some contradiction between changing figures. By this reason, contour calculation at figure editing is done only at [RECALC] is pushed by an operator. 10) CONTACT SELECTION When there are some points of contact as a result of calculation, the following message is displayed in a key-in buffer field automatically. P
SELECT POINT OF CONTACT
At the same time, the figure with a number of the point is displayed in graphic window. An operator can select the point to be defined by inputting the number. By pushing INSERT, inputted data are inserted into the selected block as the following ISO code program.
(G101,,,,105) X Y • • • • P
;
Number of a contact point
11) INTERSECT SELECTION When there are some points of intersection as a result of calculation, the following message is displayed in a key-in buffer field automatically. P
SELECT POINT OF INTERSECTION
At the same time, the figure with a number of the point is displayed in graphic window.
-47-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
An operator can select the point to be defined by inputting the number. By pushing INSERT, inputted data are inserted into the selected block as the following ISO code program.
(G101,,,,105) X Y • • • • P
;
Number of a intersect point
3.2.7
Cycles This is the menu which is defined milling cycle machining. By pushing [CYCLE] soft-key, the following menu soft-keys are displayed. HOLE
PATTER
FACE
SIDE
POCKET
RETURN
The general of each menus are as follows. • HOLE : Defining the cycle machining of hole • PATTERN : Defining the hole pattern • FACE : Defining the cycle machining of facing • SIDE : Defining the cycle machining of side cutting • POCKET : Defining the cycle machining of pocketing For details, refer to “III. TYPES OF CYCLE MOTIONS”.
NOTE In these cycle motions, please be sure not to use the cutter compensation function such as G41 or G42.
3.2.8
Teaching This is the menu which an operator executes the guidance cutting. For details, refer to “II. OPERATION - 4. GUIDANCE CUTTING OPERATIONS (OPTION)”.
-48-
www.teknikokul.net
OPERATION
B-63424EN/03
3.3
3. PROGRAMMING OPERATIONS
EDITING OPERATION By pushing soft-key [EDIT], the following Editing soft-keys will be displayed. INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE
TEACH
RETURN
Next, by pushing right end soft-key [+], the following edit soft-keys will be displayed. MOVE
COPY
DELETE
ALTER
O SEARCH
↑
↓
SEARCH SEARCH
RETURN
The general of each soft-keys are as follows. • MOVE : Move the blocks with some range to a desired position • COPY : Copy the blocks with some range to a desired position • DELETE : Delete the blocks with some range • ALTER : Alter the data correspond to the position of a cursor • O-SEARCH : Search a program with O number • ↑-SEARCH : Search an address to the upper direction • ↓-SEARCH : Search an address to the lower direction • RETURN : Return to the former soft-keys The operation of each menu is as follows. l Move of block This function can move the blocks with some range to a desired position. 1) In a program window, place the cursor at the beginning of the block to be moved. 2)
Push soft-key [MOVE] and place the cursor at the end of the block to be moved.
3)
Push soft-key [DECIDE]. The range of blocks to be moved is selected.
4)
Move the cursor to the specified position and push [EXEC]. The blocks are moved.
l Copy of block This function can copy the blocks with some range to a desired position. 1) In a program window, place the cursor at the beginning of the block to be copied.
-49-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
2)
Push soft-key [COPY] and place the cursor at the end of the block to be copied.
3)
Push soft-key [DECIDE]. The range of blocks to be copied is selected.
4)
Move the cursor to the specified position and push [EXEC]. The blocks are copied.
l Delete of block This function can delete the blocks with some range. 1) In a program window, place the cursor at the beginning of the block to be deleted. 2)
Push soft-key [DELETE] and place the cursor at the end of the block to be deleted.
3)
Push soft-key [DECIDE]. The range of blocks to be copied is selected.
4)
Push [EXEC]. The blocks are deleted.
l Alter of block 1) In a program window, place the cursor at the block to be altered. 2)
By pushing soft-key [ALTER] or ALTER, the pop-up window which corresponds to the block is displayed.
3)
Change the data of the pop-up window and push INSERT. The block is altered.
In the case of [WINDOW] OFF, the pop-up window is closed in spite of pushing [ALTER]. The operation is as follows. 1)
In a program window, place the cursor at the data which to be altered.
2)
The item which corresponds to the data is displayed on Key-in buffer. Modify the data of the program window directly and push INPUT. The block is altered.
l Insert of block 1) By pushing soft-key [+] twice, the following Editing softkeys will be displayed. INIT
TOOL
2)
MSF
COMP POSTIN
CONTR
CYCLE
TEACH
RETURN
Push the above Editing menu to be inserted and input the necessary data. -50-
www.teknikokul.net
OPERATION
B-63424EN/03
3)
3. PROGRAMMING OPERATIONS
By pushing INSERT, the block is inserted after the block which a cursor exists.
l Search of program 1) Input the O number to the key-in buffer. 2)
By pushing soft-key [O SEARCH], the program will be searched.
l Search of address 1) Input the address to the key-in buffer. 2)
By pushing soft-key [↑ / ↓ SEARCH], the address will be searched.
-51-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
3.4
CONTOUR PROGRAMMING OPERATION
3.4.1
Overview of Contour Programming
B-63424EN/03
The soft-key [CONTUR] of Editing menu is used to the definition of the shape of contour side cutting(G224), contour pocketing (G234) and contour grooving (G235). Therefore, G224 or G234 or G235 is not worked by oneself and is constituted with G100,,,G106 as a cycle machining.
NOTE 1) After specified contour side cutting (G224) or contour pocketing (G234) or contour grooving (G235), be sure to specify the contour shape by using contour menu (G100,,,G106). 2) By setting of the parameter No.9125, 9126, 9127, the soft-keys are automatically changed from each contour cycles (G224, G234, G235) to contour shape (G100,,,G106). The format of contour programming are as follows. a) Format of contour side cutting program G224 P G100 X G101 X G106 X
L Z S B F E ; Y E ; Y M N L K ;
Prepare G code
Shape G code Y P ;
b) Format of contour pocketing program G234 P G100 X G101 X G106 X
L Z S B J F E ; Y E ; Y M N L K ;
Prepare G code
Shape G code Y P ;
-52-
www.teknikokul.net
3.4.2
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
Contour Repetition In contour program by using [CONTUR] in the Editing menu, a series of figures can be automatically repeated several times. There are three repetition types. This function helps the operator to program even complicated figures easily. By pushing [CONTUR], the following soft-keys are displayed. START
CW ARC
LINE
POINT
CCW ARC
CHAMF
ROUND
END
TANGNT
RECAL. RETURN
Push the right-end soft-key [+] and the following second soft-keys is displayed. TRANS ROTATE MIRROR COPY COPY COPY
RETURN
Three repetition types [TRANS], [ROTATE] and [MIRROR] can be done. l Translate copy The linear movement can be repeated a specified number of times, with the end point of a specified figure used as the start point. By pushing [TRANS], the following pop-up window is displayed. TRANSLATE COPY NO. OF REPEAT
1/1
R=
: Specify the repetition count.
NO. OF REPEAT
-53-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
The operation of repetition is as follows. 1) 2) 3) 4)
Create a figure to be repeated at first. Then, push [TRANS] and input the necessary data. After that push INSERT. In a program window, place the cursor at the first block of the figure to be repeated, then push [START]. Move the cursor at the last block of the figure to be repeated, then push [END]. In a graphic window, repeated figures is displayed. Push [EXEC] and the specified blocks of figure is copied.
Linear movement is performed a specified number of times, using the end point of a specified figure as the start point. l Rotation copy The rotation can be repeated a specified number of times, with specified coordinates used as the rotation center. By pushing [ROTATE], the following pop-up window is displayed. ROTATION COPY NO. OF REPEAT CENTER X COORD CENTER Y COORD
1/1 R= X= Y=
NO. OF REPEAT CENTER X, Y COORD ANGLE
ROTATION COPY (DETAIL) ANGLE
K=
: Specify the repetition count. : Specify the X and Y coordinates of the rotation center. : Specify the angle of rotation, in degree. Specify a negative of clockwise rotation, and a positive value for counterclockwise rotation. It is not necessary to specify it ordinarily.
The operation of repetition is the same as translate copy. Rotation is performed about a specified rotation center, through a specified angle, a specified number of times, where the end point of a specified figure is used as the start point.
-54-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
NOTE As the rotation angle, the angle between the line connecting the start point of a specified figure and the rotation center, and the line connecting the end point and the rotation center, is normally specified. If a different angle is specified, movement from the end point of the specified figure to the end point specified in the first block of the rotated figure is assumed to be specified for the block. l Mirror copy The mirror transformed can be copied about a specified linear axis. By pushing [MIRROR], the following pop-up window is displayed. MIRROR COPY BASE POINT X BASE POINT Y ANGLE
1/1 X= Y= K=
: Specify the X and Y coordinates through which the symmetry axis for mirror transformation passes. The symmetry axis connects the point at the specified X and Y coordinate with the end point of specified figure. : Specify the angle between the symmetry axis and the +X axis, in degrees. With the +X direction assumed to be 0, a negative value indicates a clockwise displacement, while a positive value indicates a counterclockwise displacement.
SYMMETRY AXIS X, Y
ANGLE
NOTE Specify “SYMMETRY AXIS X,Y” or “ANGLE”. If both items are specified at the same time, “SYMMETRY AXIS X,Y” is used. The operation of repetition is the same as translate copy.
-55-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
3.4.3
OPERATION
B-63424EN/03
Detail of Contour Calculation A figure block, a part of a contour, with its end point not determined is said to be in the pending state. A pending figure block is drawn by dotted line. In the pop-up window for inputting contour figure data, more data input items than required are provided. These data items are used to calculate the cross point with the immediately preceding pending figure block, and also calculate the end point. The pending state is then released.
NOTE 10 successive figure blocks can be specified as pending blocks. 1) LINE a) When the preceding figure block is not pending i) Only X is inputted -> This line is determined as a vertical line. ii) Only Y is inputted -> This line is determined as a horizontal line. iii) A and either X or Y are inputted -> The end point which is not inputted is calculated. X or Y end point
A
b) When the preceding figure block specifying an arc is not pending, and TANGNT is specified. i) Either X or Y is inputted -> The angle A is calculated automatically, and an end point is determined. If neither X nor Y is inputted, this line will be pending. X or Y end point
Arc end point
-56-
www.teknikokul.net
A (This angle is calculated automatically)
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
c) When the preceding figure block is pending, and TANGNT is not specified. i) Both X and Y, and A are inputted -> The cross point between the preceding figure block is calculated. X and Y end point
A Cross point
When the preceding figure is an arc, the cross point selection request window is displayed. Input number data 1 or 2, then push INSERT. d) When the preceding figure block is pending arc, and TANGNT is specified. It is assumed that the radius and the center point coordinate (I,K) of arc have already inputted. i)
Only A is inputted -> The tangential point selection request window is displayed. Input number data 1 or 2, then push INSERT This line will be pending.
Tangential point
Tangential point
ii)
Both X and Y are inputted -> The tangential point selection request window is displayed. Input number data 1 or 2, then push INSERT The end point of this line will be determined. Tangential point
Tangential point
-57-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
iii) A and either X or Y are inputted -> The tangential point selection request window is displayed. Input number data 1 or 2, then push INSERT The end point of this line will be determined. X or Y Tangential point
A
Tangential point
If the positional relationship between the tangential point and the line is such that an inputted A conflicts with the inputted X or Y, a warning message is displayed to indicate that invalid data has been inputted. iv) A and both X and Y are inputted -> The end point of the arc and line will be determined. The tangential point selection request window is not displayed. (X, Y) Tangential point
Start point
-58-
www.teknikokul.net
B-63424EN/03
OPERATION
3. PROGRAMMING OPERATIONS
2) ARC a) When the preceding figure block is not pending, and TANGNT is not specified i) I and K are inputted -> This arc will be pending. ii) X, Y and R are inputted, or iii) X, Y, I and K are inputted -> A minor arc will be determined. End point (X, Y)
R Center (I, K) Start point
NOTE In the distance (radius) between the start point and center differs from the one between the end point and center, the figure displayed in a graphic window will differ from the actual form, and machining will not be performed correctly. iv) Only R is inputted -> By specifying TANGNT and inputting a line with A = 180 degree and X coordinate as an immediately after figure, this arc can be determined. However, there are two possible tangential points, so one of them must be selected by inputting number data 1 or 2. Tangential point R
-59-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
b) When the preceding figure block is not pending, and TANGNT is specified i) X and Y are inputted -> The radius is automatically calculated and this arc will be determined. End point (X,Y)
Tangential point
c) When the preceding figure block is pending (for which the start point has been determined), and TANGNT is not specified i) R, I and K are inputted -> The cross point selection request window is displayed. Input number data 1 or 2, then push INSERT. This arc will be pending.
Cross point Cross point
R Center(I,K)
ii)
X, Y, I and K are inputted -> The cross point selection request window is displayed. Input number data 1 or 2, then push INSERT. This arc will be determined.
Cross point End point (X,Y)
Cross point Center(I,K)
-60-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
d) When the preceding figure block is pending (for which the start point has been determined), and TANGNT is specified i) R, I and K are inputted -> The tangential point is calculated, and this arc will be pending.
Tangential point R Center(I,K)
ii)
X, Y, I and K are inputted -> The tangential point is calculated, and this arc will be determined.
Center (I,K)
End point (X,Y)
Tangential point
iii) R and X, Y are inputted -> The tangential selection request window is displayed. Input number data 1 or 2, but in this case, select a tangential point to define a minor arc.
End point (X,Y) R
R
Minor arc Tangential point
-61-
www.teknikokul.net
Tangential point
Major arc
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
e) When the preceding figure block “arc” is pending (for which the start point has been determined and only the R is to be inputted), and TANGNT is specified In this case, the directions of two arcs must be the same. i) R, X and Y are inputted -> The tangential selection request window is displayed. Input number data 1 or 2, but in this case, select a tangential point to define a minor arc. This arc will be determined. Major arc
End point (X,Y)
R2
Minor arc Tangential point
Tangential point
R1
ii)
R, I and K are inputted -> A tangential point is calculated. This arc will be pending.
Center (I,K)
R2
Tangential point
R1
-62-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
3)
Line tangential to two arcs
(2) (2) Center of (1) Start point (I1,K1) of (1)
(2)
Center of (3) (I3,K3) R3
(2)
By inputting 3 successive figure as follows, Line (2) tangential to 2 arcs can be specified as the above drawing. The end points of (1) and (2) will be determined, and (3) will be pending. Among the above 4 lines possibility, depending on the directions of 2 arcs, the line that makes a smooth connection to the arcs will be automatically selected. 1st figure ARC(1) : I and K are inputted. (A start point is determined. This arc is pending.) 2nd figure LINE(2) : No data. 3rd figure ARC(3) : R, I and K are inputted.
-63-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
4)
B-63424EN/03
Arc that contacts to both crossing lines and arcs (3) (3)
R Tangential point
R
(2) (1)
(2) (1)
Tangential point
Tangentia l point R
(3) Tangential point
Tangential (2) point (1)
By inputting 3 successive figure as follows, Arc (2) tangential to 2 lines or arcs can be specified as the above drawing. The end points of (1) and (2) will be determined, and (3) will be pending. 1st figure LINE(1) or ARC(1) : Line that is pending (for which the start point has been determined), or Arc that is pending (for which the start point has been determined) 2nd figure ARC(2) : Only R is inputted. 3rd figure LINE(3) or ARC(3) : Line with A, X and Y, or Arc with R, I and K
-64-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
B-63424EN/03
5)
Arc that contacts to uncrossing line and arc
(2)
Tangential point
(1)
R
Tangentia l point
(3)
By inputting 3 successive figure as follows, Arc (2) tangential to line and arc , these 2 figures (1) and (3) do not cross, can be specified as the above drawing. The end points of (1) and (2) will be determined, and (3) will be pending. Among the above 2 arcs possibility, the arc that makes a smooth connection to the line (1) and arc (3) will be automatically selected. 1st figure LINE(1) : Line that is pending (for which the start point has been determined) 2nd figure ARC(2) : Only R is inputted. 3rd figure ARC(3) : Arc with R, I and K
-65-
www.teknikokul.net
3. PROGRAMMING OPERATIONS
OPERATION
6)
B-63424EN/03
Arc that contacts to uncrossing 2 arcs
Start point
(3)
(1)
R3 Center point (I1,K1)
Tangential point
Tangential point
R (2)
Center point (I3,K3)
By inputting 3 successive figure as follows, Arc (2) tangential to 2 arcs , these 2 figures (1) and (3) do not cross, can be specified as the above drawing. The end points of (1) and (2) will be determined, and (3) will be pending. Among 8 arcs possibility, depending on the directions of 2 arcs, the line that makes a smooth connection to the arcs will be automatically selected. 1st figure ARC(1) : Arc with I and K, and it is pending (for which the start point has been determined) 2nd figure ARC(2) : No data. 3rd figure ARC(3) : Arc with R, I and K
-66-
www.teknikokul.net
B-63424EN/03
4
OPERATION
4. GUIDANCE CUTTING OPERATIONS
GUIDANCE CUTTING OPERATIONS (OPTIONAL FUNCTION) As described in Chapter “I.2 GUIDANCE HANDWHEEL”, an operator can carry out machining along a tapered or arc figure by using a guidance handwheel. And also, he can enter the motion block into program memory, this entering operation is called “Teaching-in”. And the program is called “Playback Machining Program”. By using this playback machining program, an operator can carry out same machining motions repeatedly later on.
NOTE 1) Before selecting the guidance cutting, be sure to set the work coordinate system of INITIAL SET menu. Because, the guidance cutting or teaching will be done on the work coordinate system which is selected at present. 2) Be sure to set the blank form data of INITIAL SET menu. Because, the tool path of teaching is drawn on the scale of the blank form data.
-67-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.1
OPERATION
B-63424EN/03
SELECTING THE GUIDANCE CUTTING By pushing the soft-key [TEACH] of the following Editing menu, an operator can select a Guidance Cutting mode. INIT
4.2
TOOL
MSF
COMP POSTIN
CONTR
CYCLE
TEACH
RETURN
INPUTTING COMMON DATA By selecting Guidance Cutting, the following Common Data items are displayed in a Pop-up Window. GUIDANCE CUTTING TOOL NO. D CODE NO. FEED RATE SPINDLE SPEED
: : : :
TOOL NO. D CODE NO. FEED RATE SPINDLE SPEED
T= D= F= S=
Number of tool used for guidance cutting Number of tool used D code for guidance cutting Feedrate at playback machining Spindle speed of tool used for guidance cutting
By pushing [INPEND], the common data is defined. When an operator wants to set or refer to the common data again, he can do it by pushing the soft-key [COMMON].
-68-
www.teknikokul.net
4.3
4. GUIDANCE CUTTING OPERATIONS
OPERATION
B-63424EN/03
TEACH-IN CUTTING MOTIONS After inputting the common data and pushing [INPEND], a cursor moves into Program Window automatically, and then, an operator can begin guidance cutting and teach-in operation. This status is called ‘Teach-in mode’.
4.3.1
Program Window As described above, at the time that a cursor is in a program window, an operator can carry out a guidance cutting using guidance handwheel, and teach-in these cutting motions into program memory for later playback machining. In this program window, taught-in cutting motion blocks are displayed, and an operator can edit the contents of them. Program Window
M06 T101 ; S3000 ; M03 ; G0 X200. Y50. ; G0 X100. Y20. ; G01 X90. F30. ;
During Teach-in mode, the following soft-keys are displayed and they are used for teach-in operations. LINE
SAVE
CIRCLE
AUX
RAPID
CUT
COMMON
RETURN
The general of each soft-keys are as follows. • LINE : Guidance cutting of Line • CIRCLE : Guidance cutting of Circle • SAVE : Save the feed rate (F) and spindle speed (S) for Teaching • AUX : Teach-in the auxiliary function command to program memory • RAPID : Teach-in the rapid traverse motion command to program memory • CUT : Teach-in the cutting motion command to program memory • COMMON : Setting of the common data • RETURN : Return to the former soft-keys
-69-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.3.2
OPERATION
B-63424EN/03
Operation of Teach-in Auxiliary Function Blocks On a machine operator’s panel, the following auxiliary function switches are prepared. • • • • • • • •
Tool select ( T-code + M6 ) Spindle CW Spindle CCW Spindle Stop Coolant ON Coolant OFF Return to Tool Change Position ( G30 ) Return to Machine Reference Position ( G28 )
By pushing a necessary switch among these switches, corresponding auxiliary function is carried out. During Teach-in mode, these carried out auxiliary functions can be taught-in into program memory for later playback machining. After pushing one or continuously several ones, maximum 10 blocks, of the above auxiliary function switches, by pushing [AUX], an operator can teach-in these commands into program memory for later playback. By pushing [SAVE] during guidance cutting, the feed rate (F) and spindle speed (S) are recorded into temporary memory. The feed rate is used for playback machining and the spindle speed is used for execution of auxiliary function such as [Spindle CW] or [Spindle CCW].
4.3.3
Operation of Teach-in a Rapid Traverse Motion Block During Teach-in mode, an operator can move a tool by handwheel or JOG stick on a machine operator’s panel. After moving a tool toward a proper position, by pushing [RAPID], an operator can teach-in this tool motion into CNC as a rapid traverse block for later playback. This taught-in block is displayed in a figure data window as following sample.
G00 X78.010 Y10.053 ;
Work coordinate of actual position G-code of rapid traverse motion
-70-
www.teknikokul.net
B-63424EN/03
4.3.4
OPERATION
4. GUIDANCE CUTTING OPERATIONS
Operation of Teach-in a Simple Linear Cutting Motion Block During Teach-in mode, an operator can cut a work-piece in direction of only X-axis or Y-axis by using a normal handwheel on a machine operator’s panel. By pushing [SAVE] during guidance cutting, the feed rate (F) at the time is recorded into temporary memory. This value is used for playback machining. When no pushing [SAVE], the value inputted in common data is used. After moving a tool toward a proper position, by pushing [CUT], an operator can teach-in this tool motion into CNC as a linear cutting block for later playback. This taught-in block is displayed in a program window as following sample.
G01 X78.010 Y10.053 F0.5 ; Feedrate inputted in common window or recorded by [SAVE] Work coordinate of actual position G-code of linear cutting motion
-71-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.3.5
OPERATION
B-63424EN/03
Operation of Guidance Cutting (Line) By using a guidance handwheel on a machine operator’s panel, an operator can carry out the following 2 types of linear cutting in simultaneous X and Y-axis direction. • Approach Cutting to an inputted Target Line • Along Cutting to an inputted Target Line In order to input a target line, the following data input window is displayed in a pop-up window, and it can be called by pushing a [LINE]. X1 POS. Y1 POS. X2 POS. Y2 POS. ANGLE
= = = = =
(X2,Y2) A (X1,Y1)
: Absolute coordinate of separated 2 points on a line. : Angle of line from +X-axis. A positive angle is clockwise direction from +Y-axis, and minus angle is counter clockwise direction. If this data is inputted, only 1 point coordinate data is necessary among the above 2 points.
X1/Y1/X2/Y2 POS. ANGLE
After inputting necessary data in the above window, by pushing [INPEND], an operator can begin guidance cutting. Besides inputting data for target line, the following distance data are displayed in a pop-up window. An operator can move the tool while checking the distance to the target line. : Distance between the current tool position and the target line. : Distance between the current tool position and the target line along X or Y-axis.
D DX/DY
DY D DX
-72-
www.teknikokul.net
OPERATION
B-63424EN/03
4. GUIDANCE CUTTING OPERATIONS
NOTE At guidance cutting, the tool radius value is used for the tool offset data of inputted T code number in a common data window. 1)
Approach Cutting By switching the guidance handwheel mode on a machine operator’s panel, an operator can select an Approaching Cutting mode. In an approach cutting mode, a tool moves along a line perpendicular to the target line according as an operator rotates a guidance handwheel. During approach cutting mode, the following guidance is displayed in a pop-up window. X1 POS. Y1 POS. X2 POS. Y2 POS. ANGLE
= 10.000 = -10.000 = 80.000 =-100.000 =
D DX
3.679 7.893 DY
10.148
In the guidance displayed in a pop-up window, pink and green arrows indicate the direction in which the tool is moved. The direction in which the handwheel is rotated determines the direction of approach. At the end of hollow arrow, the handwheel and the direction of its rotation are displayed. The feedrate of the tool motion depends on the speed at which the guidance handwheel is rotated. 2)
Along Cutting By switching the guidance handwheel mode on a machine operator’s panel, an operator can select an Along Cutting mode. In an along cutting mode, a tool moves along a line parallel to the target line according as an operator rotates a guidance handwheel. During along cutting mode, similar to the former approach cutting mode, the guidance for handwheel rotation is displayed in a popup window. In the guidance, blue arrows indicate the direction of along cutting. The direction in which the handwheel is rotated determines the direction of along cutting. At the end of solid arrow, the handwheel and the direction of its rotation are displayed. The feedrate of the tool motion depends on the speed at which the guidance handwheel is rotated.
-73-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
OPERATION
3)
B-63424EN/03
Limit Setting Normally, a limit is set such that a tool does not exceed the target line. When the target line is inputted, an opposite area of target line from the tool position is set to the limit area. By pushing a [LMTOFF], this soft-key display is changed to [LMT ON] and limit becomes unavailable. In order to make this limit be valid, push [LMT ON]. During this limit is valid, a black line is displayed at the top of the approaching arrow in a guidance drawing.
-74-
www.teknikokul.net
OPERATION
B-63424EN/03
4.3.6
4. GUIDANCE CUTTING OPERATIONS
Operation of Guidance Cutting (Circle) By using a guidance handwheel on a machine operator’s panel, an operator can carry out the following 2 types of circular cutting in simultaneous X and Y-axis direction. • Approach Cutting to an inputted Target Circle • Along Cutting to an inputted Target Circle In order to input a target circle, the following data input window is displayed in a pop-up window, and it can be called by pushing a [CIRCLE]. CENTER X = CENTER Y = RADIUS =
R (X,Y)
: Absolute coordinate of circle center. : Radius of circle. After inputting necessary data in the above window, by pushing [INPEND], an operator can begin guidance cutting. CENTER X/Y RADIUS
Similar to the guidance cutting for line, besides inputting data for target circle, the following distance data are displayed in a pop-up window. An operator can move the tool while checking the distance to the target circle. : Distance between the current tool position and the target circle.
D
D
NOTE Similar to line cutting, the tool radius value is used for the tool offset data of inputted T code number in a common data window. After inputting necessary data in the above window, by pushing [INPUT END], an operator can begin guidance cutting. By switching the guidance handwheel mode on a machine operator’s panel, an operator can select one of Approaching Cutting or Along Cutting. -75-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
OPERATION
1)
B-63424EN/03
Approach Cutting By switching the guidance handwheel mode on a machine operator’s panel, an operator can select an Approaching Cutting mode. In an approach cutting mode, a tool moves along a line connecting the center of the tool nose and the center of the target circle according as an operator rotates a guidance handwheel. During approach cutting mode, the following guidance is displayed in a pop-up window.
CENTER X = 50.000 CENTER Y =-100.000 RADIUS = 50.000
D
6.576
In the guidance displayed in a pop-up window, pink and green arrows indicate the direction in which the tool is moved. The direction in which the handwheel is rotated determines the direction of approach. At the end of hollow arrow, the handwheel and the direction of its rotation are displayed. The feedrate of the tool motion depends on the speed at which the guidance handwheel is rotated.
-76-
www.teknikokul.net
OPERATION
B-63424EN/03
4. GUIDANCE CUTTING OPERATIONS
2)
Along Cutting By switching the guidance handwheel mode on a machine operator’s panel, an operator can select an Along Cutting mode. In an along cutting mode, a tool moves along a circle having the same center as the target line according as an operator rotates a guidance handwheel. During along cutting mode, similar to the former approach cutting mode, the guidance for handwheel rotation is displayed in a popup window. In the guidance, blue arrows indicate the direction of along cutting. The direction in which the handwheel is rotated determines the direction of along cutting. At the end of solid arrow, the handwheel and the direction of its rotation are displayed. The feedrate of the tool motion depends on the speed at which the guidance handwheel is rotated.
3)
Limit Setting Similar to the former line guidance cutting, normally, a limit is set such that a tool does not exceed the target line. When the target line is inputted, an opposite area of target line from the tool position is set to the limit area. By pushing a [LMTOFF], this soft-key display is changed to [LMT ON] and limit becomes unavailable. In order to make this limit be valid, push [LMT ON]. During this limit is valid, a black line is displayed at the top of the approaching arrow in a guidance drawing.
-77-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.3.7
OPERATION
B-63424EN/03
Operation of Teach-in a Cutting Block As described in former description, during Teach-in mode, an operator can cut a work-piece by using a normal handwheel or guidance handwheel. After cutting a work-piece toward a proper position, by pushing [CUT], an operator can teach-in this tool motion into CNC as a cutting block for later playback. This taught-in block is displayed in a figure data window as following sample. Sample of Linear Cutting)
G01 X78.010 Y10.053 F0.25 ; Feedrate inputted in common data window or recorded by [SAVE] Work coordinate of actual position G-code of linear cutting
Sample of Circular Cutting)
G02 X78.010 Y10.053 R20.0 F0.25 ; Feedrate inputted in common data window or recorded by [SAVE] Radius of cutting arc path Work coordinate of actual position G-code of circular cutting
NOTE In the case that Along Circular Cutting block is over an angle of 180 degrees, please make sure to divide the angle within 180 degrees before Teach-in operation.
-78-
www.teknikokul.net
OPERATION
B-63424EN/03
4.4
4. GUIDANCE CUTTING OPERATIONS
EDITING TAUGHT-IN BLOCKS Taught-in “Auxiliary Function Block”, “Rapid Traverse Block” and “Cutting Motion Block” can be displayed in a program window. And an operator can edit these blocks by pushing [EDIT] of the initial softkeys or changing the mode to EDIT mode on the operator’s panel.
4.4.1
Program Window By using 4-directional cursor keys ↑ ↓ → ← on a LCD/MDI unit, a cursor in a program data window can be moved for pointing the data word of taught-in blocks. In this program window, taught-in cutting motion blocks are displayed, and an operator can edit the contents of them. By pushing a cursor key ↑ or ↓, the contents of program window are shifted up and down, and an operator can see the whole blocks. Program Window
M06 S300 ; M03 ;
T101 M06;
Cursor
G1 X100. Y20. F30. ; G1 X90, Y25. F30. ;
-79-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.4.2
OPERATION
B-63424EN/03
Operations for Program Editing 1)
2)
3)
4)
5)
6)
Alteration of numeric value After pointing the objective word (=Address + Numeric data) by cursor, input only new numeric data through numeric keys on LCD/MDI unit, and push ALTER key. By these operations, only numeric value can be altered. Alteration of Address and numeric value After pointing the objective word (=Address + Numeric data) by cursor, input new address and numeric data through address and numeric keys on LCD/MDI unit, and push ALTER key. By these operations, address and numeric value can be altered. Insertion of a new word After pointing the word after that a new word should be inserted, input new word (=Address + Numeric data) through address and numeric keys , and push INSERT. By these operations, a new word can be inserted after the pointed word. Insertion of a new motion block After pointing the character “;”, end of the motion block after that a new motion block should be inserted, input necessary word address data such as G-code, axis motion word (X_____ Y_____) etc. After inputting whole necessary word address data, lastly, push INSERT. By these operations, a new motion block word can be inserted after the pointed word. Deletion of a word After pointing the objective word (=Address + Numeric data), push DELETE. By these operations, this objective word can be deleted. Deletion of a motion block After pointing a block which must be deleted, push DELETE. Prompting message for confirmation of deleting will be displayed, so push DELETE again. By these operations, this objective motion block can be deleted.
-80-
www.teknikokul.net
B-63424EN/03
4.5
OPERATION
4. GUIDANCE CUTTING OPERATIONS
CHECKING CUTTING MOTIONS ON A GRAPHIC WINDOW By pushing the soft-key [RAPID] or [CUT], taught-in “Rapid Traverse Block” and “Cutting Motion Block” can be displayed graphically in a graphic window. In a graphic window, drawing of taught-in motion blocks are displayed in line form. Cutting motion blocks are displayed by solid lines, and rapid traverse blocks are displayed by dotted line. Figure which is specified by the operation described in Chapter 4.3.5 and 4.3.6 is displayed by solid line with red color.
NOTE The 1st block, since its starting point is not clear, is not displayed as a line drawing.
-81-
www.teknikokul.net
4. GUIDANCE CUTTING OPERATIONS
4.6
OPERATION
B-63424EN/03
PLAYBACK MACHINING Taught-in “Auxiliary Block”, “Rapid Traverse Block” and “Cutting Motion Block” can be executed in the form of ISO code program (Gcode etc.), and it is called Playback Machining.
4.6.1
Execution of Playback Machining Program The operation of playback machining is the same as one of the usual ISO code program.
4.6.2
1)
Push a [MEM] of the initial soft-key.
2)
By pushing [EXEC] or Cycle Start switch on machine’s operators panel, playback machining of the taught-in blocks can be started.
Checking of Playback Machining Program Taught-in “Auxiliary Block”, “Rapid Traverse Block” and “Cutting Motion Block”, can be checked by a playback machining simulation. And this machining simulation is done with tool path drawing only. The checking operation is the same as one of the usual ISO code program. By pushing a [CHECK] of the initial soft-keys, the following soft-keys are displayed. ANIME
SCAL ING
[ANIME] [SCALING]
SINGLE START
ERASE SCALE
TOOL POS.
PARAM
RETURN
: Switch to the animated simulation screen. : Indicate whether to use scaling or not before drawing. : Cause a single block stop while continuous simulation is being executed. Or, starts single block simulation : Start the continuous simulation drawing. : Erase all drawn tool path. : Enlarge or reduces a part of the drawn tool path. : Display the current tool center position with a mark. : Change the drawing parameters.
[SINGLE] [START] [ERASE] [SCALE] [POS.] [PARAM]
-82-
www.teknikokul.net
B-63424EN/03
OPERATION
4. GUIDANCE CUTTING OPERATIONS
NOTE Unless the initial setting menu is specified in advance, [ANIME] is not effective. (The shape, origin, size, and tool radius of the material must be specified.) For details, see the subsequent chapter, Chapter 5, "Program Checking."
-83-
www.teknikokul.net
5. PROGRAM CHECKING
5
OPERATION
B-63424EN/03
PROGRAM CHECKING This function is used to check a created machining program by drawing it. The following two functions are available. 1) Tool Path Drawing (wire-frame) The tool path is drawn with lines in three dimensions. The machining program can be checked closely using this drawing. 2)
Animated Simulation (solid) A three dimensional profile subject to machining is drawn using surfaces. The machining program can be easily understood by viewing this simulation.
-84-
www.teknikokul.net
5.1
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
TOOL PATH DRAWING By pushing [CHECK], the following soft-keys are displayed. ANIME
SCAL ING
SINGLE START
ERASE SCALE
TOOL POS.
PARAM
RETURN
The meaning of each soft-key are as follows. : Switch to the animated simulation screen. : Indicate whether to use scaling or not before drawing. : Cause a single block stop while continuous simulation is being executed. Or, starts single block simulation : Start the continuous simulation drawing. : Erase all drawn tool path. : Enlarge or reduces a part of the drawn tool path. : Display the current tool center position with a mark. : Change the drawing parameters.
[ANIME] [SCALING] [SINGLE]
[START] [ERASE] [SCALE] [POS.] [PARAM]
5.1.1
Enlarge / Reduce A part of a drawing can be enlarged or reduced. By pushing a [SCALE], the following soft-keys are displayed. SCALE UP
SCALE DOWN
SET END
The meaning of each soft-key are as follows. : Increase or decrease the drawing scale factor.
[SCALE UP / DOWN] [SET END]
: Push when setting is completed.
Select the center of a section to be enlarged or reduced, by using MDI keys ← → ↑ ↓. Then, set a relative scale factor by pushing [UP] or [SDOWN]. The scale factor can be set to as large as 100 times the actual size.
-85-
www.teknikokul.net
5. PROGRAM CHECKING
5.1.2
OPERATION
B-63424EN/03
Tool Position On the tool path drawing execution of the graphic window, push [POS.]. The current tool center position is displayed with a blinking marked on the tool path drawing already generated. This mark blinks at shorter time intervals when the tool is stopped, and blinks at longer time intervals when the tool is moving. On a bi-plane drawing, the tool position mark is displayed on the X-Y plane.
5.1.3
Parameters of Tool Path Drawing By pushing [PARAM], the following pop-up window is displayed. PATH GRAPHIC PARAMETER AXES = ROTATION ANGLE = TITLTING ANGLE = SCALE = MAX.(CENTER) X = Y= Z= MIN. I= J= K= START SEQ. NO. = END SEQ. NO. = TOOL RAD. COMP = COLOR : PATH = AUTO = TOOL POS =
The meanings of each parameter are described below. 1)
AXES Seven types of drawing screens are available for selection as follows. [X-Y (plane)], [Y-Z (plane)], [Z-Y (plane)], [X-Z (plane)], [XYZ (Isometric projection)], [ZXY(Isometric projection)], [X-Y, Y-Z (Bi-plane)]
2)
ROTATION ANNGLE This parameter specifies an angle of rotation (-180 to +180) around the vertical axis in degrees.
3)
TILTING ANNGLE This parameter specifies a tilt angle (-180 to +180) with respect to the vertical axis in degrees.
-86-
www.teknikokul.net
OPERATION
B-63424EN/03
5. PROGRAM CHECKING
4)
SCALE A value from 0.01 to 100.0 can be specified. When 1.0 is set, an actual size drawing is generated. When 0 is set, a scale factor is automatically determined. ( Usually the scale factor is automatically determined so that this parameter need not be set. )
5)
MAX. CENTER / MIN. The coordinates (X, Y, Z) of a drawing center, or maximum drawing coordinates (X, Y, Z) / minimum drawing coordinates (I, J, K) are set. ( Usually these scale factors are automatically determined so that this parameter need not be set. )
6)
START SEQ. NO. This parameter set the sequence number of a drawing start block with a four digit number. When 0 is set, drawing starts at the beginning of the program. A sequence number check is made with the main program and subprograms as well. In the case of including cycle motion, please make sure to set 0.
7)
END SEQ. NO. This parameter set the sequence number of a drawing end block with a four digit number. When 0 is set, drawing is performed until the end of the program. A sequence number check is made with the main program and subprograms as well. In the case of including cycle motion, please make sure to set 0.
8)
TOOL RADIUS COMP. This parameter specifies whether to use the cutter compensation in tool path drawing.
9)
COLOR Seven colors (white, red, green, yellow, blue, purple, and light blue) are available for selection. - PATH : Specify the color for drawing the tool path. - AUTO : Specify this item when the color of the tool path is to be automatically changed by T command. - TOOL POS : Specify the color of the mark used to indicate the current tool position.
-87-
www.teknikokul.net
5. PROGRAM CHECKING
5.2
OPERATION
B-63424EN/03
ANIMATED SIMULATION By pushing [CHECK], the following soft-keys are displayed. PATH
PLAN
START
ROTATE
CROSS 3-PLAN PARAM
RETURN
The meaning of each soft-key are as follows. : Switch to the tool path drawing screen. : Display a plan view of a work-piece. : Start drawing after drawing a blank and performing the head search operation. : Rotate a generated drawing. : Display a cross-sectional view of a work-piece. : Display a tri-plane view from a drawn machining profile. : Change the drawing parameters.
[PATH] [PLAN] [START] [ROTATE] [CROSS] [3-PLAN] [PARAM]
5.2.1
Rotation A drawing can be rotated. By pushing a [ROTATE], the following soft-keys are displayed. CW
CCW
ROTATE ROTATE
SET END
The meaning of each soft-key are as follows. [CW ROTATE] [CCW ROTATE] [END]
: Rotate a blank in the + direction around the vertical axis. : Rotate a blank in the - direction around the vertical axis. : Push when setting is completed.
A rotated blank is drawn when [START] is pressed after [END].
-88-
www.teknikokul.net
5.2.2
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
3-Plan View A tri-plane drawing can be generated from a drawn machining profile. By pushing a [3-PLAN], the following soft-keys are displayed. ROTATE
SET END
The meaning of each soft-key are as follows. : Move the cross section position of a left or right side face by pushing ← → of LCD/MDI key. : Move the cross section position of a top or bottom side face by pushing ↑ ↓ of LCD/MDI key. : Select a side view of a drawing. : Push when setting is completed.
[← ← , →] [↑ ↑ , ↓] [ROTATE] [END]
To move the cross section position of a side face, move mark ▲,▼,►,◄ by pushing ←, →, ↑, ↓ of LCD/MDI key. Push [SET END] to return to the original screen.
5.2.3
Cross Sectional View Cross sections of the drawn figure can be displayed based on the XY, YZ, ZX plane. By pushing a [CROSS], the following soft-keys are displayed. +SIDE +
+SIDE -
-SIDE +
-SIDE -
SECT PLAN
SET END
The meaning of each soft-key are as follows. : Move a plane in the positive / negative direction when it is on the positive side of selected plane. : Move a plane in the positive / negative direction when it is on the negative side of selected plane : Select a plane perpendicular to X, Y, Z-axis. : Push when setting is completed.
[+ SIDE+, -] [- SIDE+, -] [SECT X/Y/Z] [END]
By pushing [SECT X/Y/Z], the cross-sectional plane can be selected. By pushing [+SIDE+,-] and [-SIDE+,-], the cross-section can be moved. The unit in which the cross-section is moved can be specified with parameter No. 6515. Push [END] to return to the original screen.
-89-
www.teknikokul.net
5. PROGRAM CHECKING
5.2.4
OPERATION
B-63424EN/03
Plan View A plan view (viewed from the –Z direction) of the drawn figure can be displayed. By pushing a [PLAN], the following soft-keys are displayed. SOLID
PATH
START
PARAM
FIGURE
RETURN
The meaning of each soft-key are as follows. : Start plane view drawing from a blank. : Return the display to a solid figure.
[START] [SOLID FIGURE]
A plan view is displayed in 16 tones of the color specified with “PLANE COLOR” on the parameter.
5.2.5
Parameters of Animated Simulation By pushing [PARAM], the following pop-up window is displayed. ANIMATE GRAPHIC PARAMETER BLANK FORM = BLANK POSITION X= Y= Z= BLANK DIMENSN I = J= K= TOOL RADIUS = TOOL LENGTH START SEQ. NO. END SEQ. NO. ANIME SPEED PLANE COLOR
= = = = =
The meanings of each parameter are described below. 1)
BLANK FORM Specify the blank figure types from the following types. [RECTANGULAR SOLID], [COLUM]
-90-
www.teknikokul.net
OPERATION
B-63424EN/03
5. PROGRAM CHECKING
2)
BLANK POSITION (X, Y, Z) This parameter sets the coordinates (X, Y, Z) of the reference position of a blank in the work-piece coordinate system. When the blank is a rectangular solid, its reference position is the corner facing the negative direction along each axis. When the blank is a column or cylinder, its reference position is the center of the base.
3)
BLANK DIMENSION (I, J, K) This parameter sets the dimensions of a blank.
4)
TOOL RADIUS This parameter sets the tool radius. This one applies only when the tool figure is a cylinder.
5)
TOOL LENGTH This parameter sets the distance (usually 0) between the programmed point and the tool chip.
6)
START SEQ. NO. This parameter set the sequence number of a drawing start block with a four digit number. When 0 is set, drawing starts at the beginning of the program. A sequence number check is made with the main program and subprograms as well. In the case of including cycle motion, please make sure to set 0.
7)
END SEQ. NO. This parameter set the sequence number of a drawing end block with a four digit number. When 0 is set, drawing is performed until the end of the program. A sequence number check is made with the main program and subprograms as well. In the case of including cycle motion, please make sure to set 0.
8)
ANIME SPEED This parameter sets the interval (0 to 255) used in animated simulation drawing. A new drawing is displayed each time the machining of specified number of blocks has been completed. When 0 is specified, a drawing is generated for each block.
9)
PLANE COLOR Specify the color for a plan and 3 plan view from Seven colors (white, red, green, yellow, blue, purple, and light blue).
-91-
www.teknikokul.net
5. PROGRAM CHECKING
5.3
OPERATION
B-63424EN/03
FULL SCREEN GRAPHIC DISPLAY FUNCTION Setting WDS (bit 2 of parameter No. 9107) to 1 causes the graphic window to fill the entire screen. Setting the above parameter bit to 1 and selecting the soft-key "DRAW" causes the following soft-keys to be displayed, with the soft-key [FUL ON/OF] added. FUL ON/OF
ANIME
SBK SCAL ON/OF ON/OF
START
ERASE
SCALE
POS.
PARAM RETURN
Selecting the soft-key [ANIME] causes the following soft-keys to be displayed, with the new [FUL ON/OF] soft-key added. FUL ON/OF
PATH
PLAN
START
ROTATE
CROSS 3-PLAN PARAM RETURN
Pushing the soft-key [FUL ON/OF] causes switching between the full screen mode and the conventional graphic window display mode.
NOTE In the full screen mode, the above soft-keys are available as the same of the usual screen mode. • Screen constitution in [FUL OF] mode
• Screen constitution in [FUL ON] mode
1.1.1.1.1
Actual position
Distance Spindle speed to go
Next block Graphic window
<
Graphic window
Modal inf.
FUL ON/OF
Feed-rate
次ﾌﾞﾛｯ ｸ
実速度
Program window
+
<
-92-
www.teknikokul.net
+
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
The parameters related to full screen drawing and display are as follows: 9107
WDS NCD
NCD
WDS
0 : The soft-key [FUL ON/OF] is not displayed on Graphic simulation. 1 : The soft-key [FUL ON/OF] is displayed on Graphic simulation. 0 : The NC program is not displayed with Tool path in the full screen mode. (In the case of WDS = 1 only) 1 : The NC program is displayed with Tool path in the full screen mode. (In the case of WDS = 1 only)
-93-
www.teknikokul.net
5. PROGRAM CHECKING
5.4
OPERATION
B-63424EN/03
BACKGROUND DRAWING (OPTION FUNCTION) This function is a function by which, while machining is in progress, tool path drawing and animated simulation can be executed concurrently using another program.
NOTE This function requires the option function for NC background drawing. The operating instructions are the same as those of the conventional tool path drawing and animated simulation functions, except the following: 1. Selection of the program with which drawing is to be executed 2. Display and cancellation of alarms that may be generated during the execution of drawing 3. Screen switching using a function key 4. Display of the operation status on the drawing screen
5.4.1
Selection of the Program with Which Drawing Is to Be Executed To select a program, first push the soft-key [DIR] and then select the desired one from the program directory window. Pushing the soft-key [DIR] causes the following soft-keys to be displayed. Position the cursor on the desired program No. and push the soft-key [CHECK], and the program No. is selected and the system switches to the drawing screen. EDIT
CHECK
COPY
DELETE
CNY NC
O-
RETURN
SEARCH
If the soft-key [CHECK] is pushed in a window other than the program directory window, which is displayed by pushing the soft-key [DIR], the program No. currently selected in the foreground is assumed the desired program No. and the system switches to the drawing screen. If the function key GRAPH is pushed, no new program No. is selected, but the program No. currently selected in the background is assumed and the system switches to the drawing screen.
-94-
www.teknikokul.net
OPERATION
B-63424EN/03
5.4.2
5. PROGRAM CHECKING
Display and Cancellation of Alarms That May Be Generated During the Execution of Drawing If an alarm is generated due to the execution of drawing by this function, drawing temporarily stops and, at the same time, the alarm No. is displayed in the message bar. This disables the setting of bit 7 of parameter No. 3111 (NPA). To cancel the alarm, either use the softkey [STOP] or the CAN key on the MDI. Pushing the RESET key also cancels the alarm. Use caution, however, because this causes machining to stop if machining is in progress in the foreground. Bit 0 of parameter No. 8100 (RST) may be set so that pushing the RESET key during drawing does not affect the foreground. If an alarm is generated in the foreground during background drawing, "ALM" is displayed in the status display area.
5.4.3
Screen Switching Using a Function Key If screen switching is performed using a function key during the execution of drawing, the execution of drawing stops.
5.4.4
Display of the Operation Status on the Drawing Screen The various items that may be displayed in the status display window always indicate the status of the program running in the foreground. The operating status (mode, operation, alarm, etc.) of the machine that is displayed in the title bar is always that of the program in the foreground.
5.4.5
Handling of Various Data Items During the execution of this function, various data items are handled as described below. l
Tool offset value Separate values, one for machining (foreground) and one for drawing (background), must be prepared. During program selection, the value for machining is copied as that for drawing. These two values will never affect each other even if they are changed with the G10 command during machining and drawing.
l
Parameters The parameters used during machining are also used during drawing.
-95-
www.teknikokul.net
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
l
Workpiece origin offset This data item is a parameter. Separate values, one for machining and one for drawing, must be prepared. During program selection, the value for machining is copied as that for drawing. These two values will never affect each other even if they are changed with the G10 command during machining or drawing.
l
Macro variable Separate values, one for machining and one for drawing, must be prepared. During program selection, the value for machining is copied as that for drawing. These two values will never affect each other even if they are changed during machining or drawing.
-96-
www.teknikokul.net
5.5
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
NOTES ON DRAWING 1). The program with which drawing is to be executed must have already been registered with memory. Drawing is not possible with programs not registered with memory. Either M02 or M30 must be specified at the end of that program. 2). Drawing is not possible unless the machine is operable. Nor it is possible during the operation of the machine. The main settings and switches necessary for drawing are as follows: Setting/switch Tool compensation Single block Optional block skip Feed hold Dry run
State Correctly set if drawing is performed by enabling tool compensation. Off Correctly set. Off Off
CAUTION Background drawing is possible even during the operation of the machine. 3). During the execution of drawing, no machine control signals are output by auxiliary and other functions, but control signals such as "OP," "STL," "SPL," "RST," and "AL" may be output. During the execution of drawing, the drawing-in-progress signal "CKGRP," shown below, is output. F062
CKGRP
If the control signals that may be output during the execution of drawing affect machine control, the PMC Ladder program must be modified so that these signals are ignored, by using the drawing-in-progress signal. 4). During the execution of drawing, the system is automatically placed in the machine locked state. Those move commands that are affected by the machine position at the time of program execution (such as G28, G30, and G31) cause the same movement as that in the machine locked state. 5). Drawing is possible only on linear movement axes deriving from the X-, Y-, and Z-axes. Drawing is not possible on rotation, additional, PMC, and other axes. 6). For details of parameters Nos. 6500 to 6515 related to drawing, see the parameter table.
-97-
www.teknikokul.net
5. PROGRAM CHECKING
OPERATION
B-63424EN/03
7). The drawing function requires that the X-, Y,- and Z-axes be the first, second, and third axes. Otherwise, drawing is not performed correctly.
-98-
www.teknikokul.net
B-63424EN/03
6
OPERATION
MACHINING OPERATION
-99-
www.teknikokul.net
6. MACHINING OPERATION
6. MACHINING OPERATION
6.1
OPERATION
B-63424EN/03
MEMORY OPERATION The machining program can be executed by using this menu. By pushing [MEM], the following soft-keys are displayed. These softkeys are the menu for memory operation. EXEC
O
N
SEARCH
SEARCH
REWIND
CHECK
BGEDIT RETURN
The general of each soft-keys is as follows. • EXEC : Execute a program ( equal to Cycle Start switch of machine’s panel ) • O-SEARCH : Search program number (O) • N-SEARCH : Search sequence number (N) • REWIND : Rewind the pointer of a program • CHECK : Check a program with graphic function • BGEDIT : Background edit operation • RETURN : Return to the former soft-keys
NOTE By setting the parameter No.9104 NST (#0) to 1, it is available not to display soft-key [EXEC].
By pushing the righ end soft-key [+], it is available to display the following soft-keys. LIST
-100-
www.teknikokul.net
WRK-CO
OFFSET RETURN
6.2
6. MACHINING OPERATION
OPERATION
B-63424EN/03
BACKGROUND EDITING An operator can edit a program during memory operation by using this menu. By pushing [BGEDIT], the following soft-keys are displayed. And the pop-up window of Program List is displayed on the screen at the same time. These soft-keys are the menu for a background edit operation. SELECT
COPY DELETE
O SEARCH
RETURN
The general of each soft-keys is as follows. • SELECT : Select a program or insert a new program for Background edit • COPY : Copy a program • DELETE : Delete a program • O-SEARCH : Search program number (O) • RETURN : Return to the former soft-keys
NOTE 1) By pushing the soft-key [RETURN] or left end soft-key [<], Background edit operation is finished. 2) In Background edit operation, it is not possible to select a program which was selected on Foreground.
-101-
www.teknikokul.net
7. MDI / MANUAL OPERATION
7
OPERATION
MDI / MANUAL OPERATION
-102-
www.teknikokul.net
B-63424EN/03
7.1
7. MDI / MANUAL OPERATION
OPERATION
B-63424EN/03
MDI OPERATION By pushing [MDI], the following soft-keys are displayed. These softkeys are the menu for MDI operation. EXEC
REWIND
RETURN
The general of each soft-keys is as follows. • EXEC : Execute a program which was inputted by MDI key ( equal to Cycle Start switch of machine’s panel ) • REWIND : Rewind the pointer of a program • RETURN : Return to the former soft-keys
NOTE By setting the parameter No.9104 NST (#0) to 1, it is available not to display soft-key [EXEC].
By pushing the righ end soft-key [+], it is available to display the following soft-keys. LIST
-103-
www.teknikokul.net
WRK-CO
OFFSET RETURN
7. MDI / MANUAL OPERATION
7.2
OPERATION
B-63424EN/03
MANUAL OPERATION By pushing [HANDLE], the following soft-keys are displayed. These soft-keys are the menu for Manual operation with JOG or HANDLE mode. LINE
CIRCLE
RETURN
The general of each soft-keys is as follows. • LINE : Guidance cutting of Line • CIRCLE : Guidance cutting of Circle • RETURN : Return to the former soft-keys
NOTE 1) These soft-keys [LINE] and [CIRCLE] needs the optional function of Guidance Cutting function. 2) Nothing is displayed on the graphic window because of no teaching block.
By pushing the righ end soft-key [+], it is available to display the following soft-keys. LIST
-104-
www.teknikokul.net
WRK-CO
OFFSET RETURN
OPERATION
B-63424EN/03
8 8.1
8. OTHER FUNCTIONS
OTHER FUNCTIONS CALCULATOR FUNCTION Expressions can be entered on the data input window to perform calculations using entered numeric data such as the arithmetic operations ( +, -, *, / ), the trigonometric function ( sin, cos, tan ) and the square root. l
Arithmetic operations In one operation, any binomial arithmetical operation ( addition, subtraction, multiplication or division ) can be performed. However, the result of each operation can be used in succession as the first term of the next operation. Thus, any number of operations can be performed in one numeric data input item. Use the following key operations for the arithmetic operations : (1) Addition : 100.+200.[INPUT] → The result is displayed where the cursor is placed in the input data. (2) Subtraction : 100.-200.[INPUT] → Same as above (3) Multiplication : 100.*20.[INPUT] → Same as above (4) Division : 100./10.[INPUT] → Same as above
Example of entering data for an arithmetic operation (subtraction) in TRACK POCKET
The displayed result of an operation is not directly entered in the numeric data item. The operator must check the displayed result of an operation, then press [INPUT] to enter the result in the input data item. -105-
www.teknikokul.net
8. OTHER FUNCTIONS
OPERATION
B-63424EN/03
Example) To calculate and enter the result of the operation 210.65.3+1.25, press the following keys. 210.-65.3[INPUT] +1.25[INPUT][INPUT] l
Trigonometric function ( SIN, COS, TAN ) SIN, COS and TAN are available. Use the following key operations for the trigonometric function : (1) SIN : 45S[INPUT] → The result is displayed where the cursor is placed in the input data. (2) COS : 45C[INPUT] → Same as above (3) TAN : 45T[INPUT] → Same as above The displayed result of an operation is not directly entered in the numeric data item. The operator must check the displayed result of an operation, then press [INPUT] to enter the result in the input data item.
l
Square root Square root is available. Use the following key operations for the square root: (1) Square root : 45R[INPUT] → The result is displayed where the cursor is placed in the input data.
-106-
www.teknikokul.net
8.2
8. OTHER FUNCTIONS
OPERATION
B-63424EN/03
NC FORMAT OUTPUT FUNCTION By using this function, it is available to convert the machining program to normal NC format, which was created with Cycle Cutting for Manual Guide such like G210.
NOTE 1) This is the basic function. 2) It is impossible to output the converted NC program into an external storage unit.
8.2.1
Operation 1). In initial soft-keys or other one, push a soft-key [LIST]. 2). Since the following soft-keys will be displayed, move the cursor to the program which you want to convert in NC format and push a soft-key [CNV NC]. COPY DELETE
SELECT
CNV NC
RETURN
3). Since the following soft-keys will be displayed, input the outputted program number and push a soft-key [SELECT]. SELECT CENCEL
4). Since the following soft-keys will be displayed, push a soft-key [EXEC]. After that, the conversion will be done from the original program to the new objective program. SBK OFF
SCL ON
EXEC
ERASE
ON/OFF PARAM RETURN
In the state of the soft-key [SCL ON], a scaling is done before drawing. In the state of the soft-key [SBK ON], a single block is converted one by one. In the state of the concave soft-key [ON/OFF], the window of Output NC statements is displaying during conversion. 5).
During conversion, the following soft-keys will be displayed. It is available to stop the conversion by pushing a soft-key [STOP]. SBK OFF
6).
STOP
ON/OFF
During a single block conversion, the following soft-keys will be displayed. It is available to restart the next block conversion by pushing a soft-key [1BLOCK]. SBK ON
STOP
1BLOCK
-107-
www.teknikokul.net
ON/OFF
8. OTHER FUNCTIONS
OPERATION
7).
B-63424EN/03
After the end of conversion, the following soft-keys will be displayed. By pushing a soft-key [RETURN], it is returned to the former soft-keys. RETURN
8.2.2
Window of Output NC Statements Before conversion or during conversion, by pushing a soft-key [ON/OFF], it is available to display the window on which the converted NC program is displayed
The status of a soft-key [ON/OFF] is retained after conversion. That is, the status of it will be retained in next conversion.
8.2.3
System variable for distinguishing the executing state (#3010) In order to distinguish the executing state of the program, machining custom macro program can refer to the following system variable #3010. System Variable #3010
Value =1 =2 =4 =12
Executing State Under machining Under tool path drawing Under animated simulation Under tool path drawing with conversion
Example) In the tool setting menu (G301), tool setting program would call the tool change macro under normal simulation, and execute “M6” only under conversion. -108-
www.teknikokul.net
8. OTHER FUNCTIONS
OPERATION
B-63424EN/03
/* Tool Setting(G301) */ O9301 call_canned_cycle_cancel G91 ; G28 Z0 ; G28 X0 Y0 ; G90 ; ****** ****** ****** if[#3010le10] then T[tool_no] ; call_tool_change [call_tool_macro] ; else T[tool_no] M6 ; Endif ****** ******
8.2.4
Parameter This function refers the following parameter. 9108
OPO
GRO
Standard 00000000 GRO OPO
1 : No G10 command is outputted in the NC format conversion 0 : G10 command is outputted in the NC format conversion 1 : Optional Block Delete (/) is outputted in the NC format conversion. 0 : No Optional Block Delete (/) is outputted in the NC format conversion.
-109-
www.teknikokul.net
III. TYPES OF CYCLE MOTIONS
www.teknikokul.net
B-63424EN/03
1
TYPES OF CYCLE MOTIONS
1. HOLE MACHINING
HOLE MACHINING By pushing [HOLE], the hole machining menu are displayed as follows. DRILL
BORE
TAP
RGTAP
RETURN
After this, we will explain the case of [WINDOW] ON. As to the case of [WINDOW] OFF, the address which corresponds to the item of each menu is displayed in key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next address is displayed. After repeating this operations, by pushing INSERT key, inputted data are decided. ( “;” is inserted.)
NOTE 1) As to the detailed specifications such as the restriction, refer to the operator’s manual describing the NC of the FANUC Series 16/18/21i –MA/MB. 2) After pushing INSERT key, the soft-keys of Hole Pattern menu are displayed automatically.
-113-
www.teknikokul.net
1. HOLE MACHINING
1.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
DRILLING By pushing [DRILL], the following pop-up window is displayed. The all items are changed according to “MACHINE PATTERN” DRILLING CYCLE MACHINE PATTERN Z POINT R POINT FEED RATE
MACHINE PATTERN
1.1.1
1/1
G= Z= R= F=
: Specify the machining pattern from the following soft-keys. [NO DWL] : Drilling cycle without a dwell (G81) [DWELL] : Drilling cycle with a dwell (G82) [PECK] : Drilling cycle with a peck (G83) [S-PECK] : Drilling cycle with a high-speed peck
Drilling Cycle (Without Dwell) (G81) This cycle is used for normal drilling. Cutting feed is performed to the bottom of the hole. The tool is then retracted from the bottom of the hole in rapid traverse. By pushing [NO DWL], the following items are displayed. DRILLING CYCLE MACHINE PATTERN Z POINT R POINT FEED RATE
1/1
G= NO DWL Z= R= F=
-114-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
1. HOLE MACHINING
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level
Z POINT
R POINT
G90
G91 Initial level
Initial level R Point R
R
Point R Z=0 Z
Z Point Z
Point Z
: Cutting feed rate
FEED RATE
By pushing [DETAIL], the following pop-up window is displayed. DRILLING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-115-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: Rapid traverse Feed traverse
G81 (G98)
G81 (G99)
Initial level Point R level Point R
Point R
Point Z
Point Z
After positioning along the X and Y axes, rapid traverse is performed to point R. Drilling is performed from point R to point Z. The tool is then retracted in rapid traverse. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G81 (X Y ) Z R F (K ) ;
1.1.2
Drilling Cycle (With Dwell) (G82) This cycle is used for normal drilling. Cutting feed is performed to the bottom of the hole. At the bottom, a dwell is performed, then the tool is retracted in rapid traverse. This cycle is used to drill holes more accurately with respect to depth. By pushing [DWELL], the following items are displayed. DRILLING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
1/1
G= DWELL Z= R= P= F=
-116-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
Z POINT
R POINT
DWELL TIME FEED RATE
1. HOLE MACHINING
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time at the bottom of a hole : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. DRILLING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-117-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
:
P
Rapid traverse Feed traverse Dwell
G82 (G98)
G82 (G99)
Initial level Point R level Point R
Point R
Point Z P
Point Z P
After positioning along the X and Y axes, rapid traverse is performed to point R. Drilling is performed from point R to point Z. The tool is then retracted in rapid traverse. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G82 (X Y ) Z R P F (K ) ;
-118-
www.teknikokul.net
B-63424EN/03
1.1.3
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Drilling Cycle (Peck) (G83) This cycle performs peck drilling. It performs intermittent cutting feed to the bottom of a hole while removing shavings from the hole. And an arbor with the overload torque detection function is used to retract the tool when the overload torque detection signal is detected during drilling. Drilling is resumed after the spindle speed and cutting feed-rate are changed. By pushing [PECK], the following items are displayed. DRILLING CYCLE MACHINE PATTERN Z POINT R POINT PITCH DEPTH FEED RATE
Z POINT
R POINT
PITCH DEPTH FEED RATE
1/1
G= PECK Z= R= Q= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Depth of cut for each cutting feed : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. DRILLING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y TRAVEL SPEED DWELL TIME REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= I= P= K= 0
-119-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
B-63424EN/03
REPEAT NUMBER
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental) ], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Forward or backward traveling speed ( only for small-hole peck cycle) : Dwell time at the bottom of the hole ( only for small-hole peck cycle) : Number of repeat. It is used in the case of no using Hole Pattern menu.
MOVEMENTS
:
ABS / INC
RETURN POINT HOLE POINT X, Y TRAVEL SPEED DWELL TIME
Rapid traverse Feed traverse Dwell
P • Peck Drilling Cycle G83 (G98)
G83 (G99)
Initial level Point R
Point R Q
d
Q
Point R level
d
Q
Q d
d Q
Q Point Z
Point Z
“Q” represents the depth of cut for each cutting feed. It must always be specified as an incremental value. In the second and subsequent cutting feeds, rapid traverse is performed up to a “d” point just before where the last drilling ended, and cutting feed is performed again. “d” is set in parameter (No.5115).
-120-
www.teknikokul.net
B-63424EN/03
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
• Small-hole Peck Drilling Cycle G83 (G98)
G83 (G99)
Initial level
Point R
Point R level
Point R
Q
Q ∆
∆
∆
∆ Overload torque Point Z
∆ P
Overload torque Point Z
∆ P
“∆” is an initial clearance when the tool is retracted to point R and the clearance from the bottom of the hole in the second or subsequent drilling (parameter No.5174). After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G83 (X Y ) Z R Q
-121-
www.teknikokul.net
F (I P K ) ;
1. HOLE MACHINING
1.1.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
Drilling Cycle (High-speed Peck) (G73) This cycle performs high-speed peck drilling. It performs intermittent cutting feed to the bottom of a hole while removing shavings from the hole. By pushing [S-PECK], the following items are displayed. DRILLING CYCLE MACHINE PATTERN Z POINT R POINT PITCH DEPTH FEED RATE
Z POINT
R POINT
PITCH DEPTH FEED RATE
1/1
G= S-PECK Z= R= Q= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Depth of cut for each cutting feed : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. DRILLING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
-122-
www.teknikokul.net
B-63424EN/03
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
HOLE POINT X, Y REPEAT NUMBER
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
MOVEMENTS
:
ABS / INC
RETURN POINT
Rapid traverse Feed traverse G73 (G98)
G73 (G99)
Initial level Point R
Point R Q
Q
d
Q
d
Q
Point R level d
d
Q
Q Point Z
Point Z
The high-speed peck drilling cycle performs intermittent feeding along the Z axis. When this cycle is used, chips can be removed from the hole easily, and a smaller value can be set for retraction. This allow, drilling to be performed efficiently. Set the clearance “d” in parameter No.5114. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G73 (X Y ) Z R Q
-123-
www.teknikokul.net
F (K ) ;
1. HOLE MACHINING
1.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
BORING By pushing [BORE], the following pop-up window is displayed. The all items are changed according to “MACHINE PATTERN” BORING CYCLE MACHINE PATTERN Z POINT R POINT FEED RATE
MACHINE PATTERN
1/1 G= Z= R= F=
: Specify the machining pattern from the following soft-keys. [FEED] : Boring cycle with a feed retraction (G85) [RAPID] : Boring cycle with a feed retraction (G86) [MANUAL] : Boring cycle with a manual retraction (G88) [DWELL] : Boring cycle with a dwell (G89) [FINE] : Fine boring cycle (G76) [BACK] : Back boring cycle (G87)
-124-
www.teknikokul.net
B-63424EN/03
1.2.1
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Boring Cycle (Feed Retraction) (G85) This cycle is used to bore a hole with feed retraction. By pushing [FEED], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT FEED RATE
1/1 G= FEED Z= R= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Cutting feed rate
Z POINT
R POINT
FEED RATE
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following softkeys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-125-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: Rapid traverse Feed traverse
G85 (G98)
G85 (G99)
Initial level Point R level Point R
Point R
Point Z
Point Z
After positioning along the X and Y axes, rapid traverse is performed to point R. Boring is performed from point R to point Z. When point Z has been reached, cutting feed is performed to return to point R. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G85 (X Y ) Z R F (K ) ;
-126-
www.teknikokul.net
B-63424EN/03
1.2.2
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Boring Cycle (Rapid Retraction) (G86) This cycle is used to bore a hole with rapid retraction. By pushing [RAPID], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT FEED RATE
1/1 G= RAPID Z= R= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Cutting feed rate
Z POINT
R POINT
FEED RATE
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-127-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: Rapid traverse Feed traverse
G86 (G98)
G86 (G99)
Spindle CW Initial level
Point R
Spindle CW Point R
Point R level
Point Z
Point Z
Spindle stop
Spindle stop
After positioning along the X and Y axes, rapid traverse is performed to point R. Boring is performed from point R to point Z. When the spindle is stopped at the bottom of the hole, the tool is retracted in rapid traverse. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G86 (X Y ) Z R F (K ) ;
-128-
www.teknikokul.net
B-63424EN/03
1.2.3
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Boring Cycle (Manual Retraction) (G88) This cycle is used to bore a hole with manual retraction. By pushing [MANUAL], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
Z POINT
R POINT
DWELL TIME FEED RATE
1/1 G= MANUAL Z= R= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time at the bottom of a hole : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-129-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
:
P
Rapid traverse Feed traverse Manual traverse Dwell
G88 (G98)
G88 (G99)
Spindle CW Initial level
Spindle CW
Point R
Point R
Point Z
Point Z P
Spindle stop after dwell
Point R level
Spindle stop after dwell
After positioning along the X and Y axes, rapid traverse is performed to point R. Boring is performed from point R to point Z. When boring is completed, a dwell is performed, then the spindle is stopped. The tool is manually retracted from the bottom of the hole (point Z) to point R. At point R, the spindle is rotated clockwise, and rapid traverse is performed to the initial level. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G88 (X Y ) Z R P F (K ) ;
-130-
www.teknikokul.net
B-63424EN/03
1.2.4
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Boring Cycle (With Dwell) (G89) This cycle is used to bore a hole with dwell. By pushing [DWELL], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
Z POINT
R POINT
DWELL TIME FEED RATE
1/1 G= DWELL Z= R= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time at the bottom of a hole : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER MOVEMENTS
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu. :
-131-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
B-63424EN/03
Rapid traverse Feed traverse Dwell
P G85 (G98)
G85 (G99)
Initial level Point R level Point R
Point R
Point Z P
Point Z P
This cycle is almost the same as G85. The difference is that this cycle performs a dwell at the bottom of the hole. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G89 (X Y ) Z R P F (K ) ;
-132-
www.teknikokul.net
B-63424EN/03
1.2.5
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
Boring Cycle (Fine Boring) (G76) The fine boring cycle bores a hole precisely. When the bottom of the hole has been reached, the spindle stops, and the tool is moved away from the machined surface of the work-piece and retraced. By pushing [FINE], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT TOOL SHIFT AMOUT DWELL TIME FEED RATE
Z POINT
R POINT
TOOL SHIFT AMOUNT
1/1 G= FINE Z= R= Q= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Shift amount at the bottom of a hole
NOTE Q (shift at the bottom of a hole) is a modal value retained within canned cycles. It must be specified carefully because it is also used as the depth of cut for G73 and G83. DWELL TIME FEED RATE
: Dwell time at the bottom of a hole : Cutting feed rate
-133-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
B-63424EN/03
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
MOVEMENTS
:
OSS
Rapid traverse Feed traverse Oriented spindle stop Shift (rapid traverse)
P
Dwell
G76 (G98)
G76 (G99)
Spindle CW Initial level Point R
Spindle CW Point R level
Point R
P OSS
Point Z Q
P OSS
Point Z Q
When the bottom of the hole has been reached, the spindle is stopped at the fixed rotation position, and the tool is moved in the direction opposite to the tool tip and retraced. This ensures that the machined surface is not damaged and enables precise and efficient boring to be performed. -134-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
1. HOLE MACHINING
After inputting the necessary data, by pushing INSERT, pop-up window closed and inputted data are displayed in a program window as the following ISO code program.
G76 (X Y ) Z R Q
-135-
www.teknikokul.net
P F (K ) ;
1. HOLE MACHINING
1.2.6
TYPES OF CYCLE MOTIONS
B-63424EN/03
Boring Cycle (Back Boring) (G87) This cycle performs accurate boring. By pushing [BACK], the following items are displayed. BORING CYCLE MACHINE PATTERN Z POINT R POINT TOOL SHIFT AMOUT DWELL TIME FEED RATE
Z POINT
R POINT
TOOL SHIFT AMOUNT DWELL TIME FEED RATE
1/1 G= BACK Z= R= Q= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Shift amount at the bottom of a hole : Dwell time at the bottom of a hole : Cutting feed rate
NOTE Q (shift at the bottom of a hole) is a modal value retained within canned cycles. It must be specified carefully because it is also used as the depth of cut for G73 and G83.
-136-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
1. HOLE MACHINING
By pushing [DETAIL], the following pop-up window is displayed. BORING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
MOVEMENTS
:
OSS
Rapid traverse Feed traverse Oriented spindle stop Shift (rapid traverse)
P
Dwell
G87 (G98)
G87 (G99)
Q OSS
Not use
Spindle CW OSS Point Z
P Spindle CW
Point R
-137-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
B-63424EN/03
After positioning along the X and Y axes, the spindle is stopped at the fixed rotation position. The tool is moved in the direction opposite to the tool tip, positioning (rapid traverse) is performed to the bottom of the hole (point R). The tool is then shifted in the direction of the tool tip and the spindle is rotated clockwise. Boring is performed in the positive direction along the Z axis until point Z is reached. At point Z, the spindle is stopped at the fixed rotation position again, the tool is shifted in the direction opposite to the tool tip, then the tool is returned to the initial level. The tool is then shifted in the direction of the tool tip and the spindle is rotated clockwise to proceed to the next block operation. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G87 (X Y ) Z R Q
-138-
www.teknikokul.net
P F (K ) ;
1.3
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
B-63424EN/03
TAPPING By pushing [TAP], the following pop-up window is displayed. TAPPING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
MACHINE PATTERN
1/1 G= 84 Z= R= P= F=
: Specify the machining pattern from the following soft-keys. [TAP] : Tapping cycle (G84) [REV TAP] : Left-handed tapping cycle (G74)
-139-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
1.3.1
(G84)
Tapping Cycle
B-63424EN/03
This cycle performs tapping. In this tapping cycle, when the bottom of the hole has been reached, the spindle is rotated in the reverse direction. By pushing [TAP], the following items are displayed. TAPPING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
Z POINT
R POINT
DWELL TIME FEED RATE
1/1 G= TAP Z= R= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. TAPPING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following softkeys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-140-
www.teknikokul.net
B-63424EN/03
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
:
P
Rapid traverse Feed traverse Dwell
• Tapping Cycle G84 (G98)
G84 (G99)
1.1
Initial level Spindle CW Point R
P
P
Spindle CW Point R
Point Z Spindle CCW
Point R level
Point Z P
Spindle CCW
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G84 (X Y ) Z R P F (K ) ;
-141-
www.teknikokul.net
1. HOLE MACHINING
1.3.2
TYPES OF CYCLE MOTIONS
Left-handed Tapping Cycle
B-63424EN/03
(G74)
This cycle performs left-handed tapping. In the left-handed tapping cycle, when the bottom of the hole has been reached, the spindle rotates clockwise. By pushing [REVTAP], the following items are displayed. TAPPING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE
Z POINT
R POINT
DWELL TIME FEED RATE
1/1 G= REVTAP Z= R= P= F=
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time : Cutting feed rate
By pushing [DETAIL], the following pop-up window is displayed. TAPPING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y REPEAT NUMBER
G= NO-OUT G= NO-OUT X= Y= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99l)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-142-
www.teknikokul.net
B-63424EN/03
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
:
P
Rapid traverse Feed traverse Dwell
• Left-handed Tapping Cycle G74 (G98)
G74 (G99)
1.3
Initial level Spindle CCW Point R
P
P
Spindle CCW P
Point R
Point Z Spindle CW
Point R level
Point Z P
Spindle CW
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G74 (X Y ) Z R P F (K ) ;
-143-
www.teknikokul.net
1. HOLE MACHINING
1.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
RIGID TAPPING (G243) When the spindle motor is controlled in rigid mode as if it were a servo motor, a tapping cycle can be sped up. And the peck rigid tapping cycle is useful. By pushing [RGTAP], the following pop-up window is displayed. TAPPING CYCLE MACHINE PATTERN Z POINT R POINT DWELL TIME FEED RATE SPINDLE SPEED
1/1 M= RGTAP Z= R= P= F= S=
MACHINE PATTERN
: Specify the machining pattern from the following soft-keys. [RGTAP] : Rigit tapping cycle [RGRTAP] : Left-handed rigid tapping cycle
Z POINT
: In the case G90 - the Z axis position of the bottom of the hole In the case G91 - the distance from point R to the bottom of the hole : In the case G90 - the Z axis position of point R level In the case G91 - the distance from the initial level to point R level : Dwell time (Unit is ordinarily 1 msec, but it is 0.1 msec in IS-C nuit) : Cutting feed rate : Spindle speed
R POINT
DWELL TIME FEED RATE SPINDLE SPEED
-144-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
1. HOLE MACHINING
By pushing [DETAIL], the following pop-up window is displayed. TAPPING CYCLE (DETAIL) ABS / INC RETURN POINT HOLE POINT X HOLE POINT Y PITCH DEPTH REPEAT NUMBER
ABS / INC
RETURN POINT HOLE POINT X, Y PITCH DEPTH REPEAT NUMBER
A= NO-OUT I= NO-OUT X= Y= Q= K= 0
: Specify travel ways from the following soft-keys. [G90ABS (absolute)], [G91INC (incremental)], [NO-OUT] : Specify return point level from the following soft-keys. [I-LVL (G98)], [R-LVL (G99)], [NO-OUT] : Hole position data. It is used in the case of no using Hole Pattern menu. : Depth of cut for each cutting feed. : Number of repeat. It is used in the case of no using Hole Pattern menu.
-145-
www.teknikokul.net
1. HOLE MACHINING
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: Rapid traverse Feed traverse Dwell
P
• Rigid Tapping Cycle G84 (G98)
G84 (G99)
Spindle stop Initial level Spindle stop P
Point R
Spindle stop Spindle stop
Spindle CW
P Point R level
Point R
Point Z
Point Z Spindle stop
P
Spindle CCW
Spindle stop
P Spindle CCW
• Left-handed Peck Rigid Tapping Cycle G74 (G98)
G74 (G99)
Spindle stop Initial level Spindle CCW
Spindle stop P
Point R
Spindle stop Spindle stop Spindle CCW Point R
Spindle CW
Point R level
Point Z
Point Z Spindle stop
P
Spindle stop
P Spindle CW
• Peck Rigid Tapping Cycle G74 (G98)
G74 (G99)
Initial level Point R
Point R level
Q
Q
d
Q
Point R
d
Q
Q
Point R level d d
Q Point Z
Point Z
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G243 M Z R S
K (P F A I
-146-
www.teknikokul.net
X Y Q
) ;
B-63424EN/03
2
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
HOLE PATTERN By pushing [PATTRN], the hole pattern menu are displayed as follows. POINTS
LINE
GRID
SQUARE
CIRCLE
ARC
RETURN
After this, we will explain the case of [WINDOW] ON. As to the case of [WINDOW] OFF, the address which corresponds to the item of each menu is displayed in key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next address is displayed. After repeating this operations, by INSERT key, inputted data are decided. (“;” is inserted.)
-147-
www.teknikokul.net
2. HOLE PATTERN
2.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
POINTS (G200) This is a menu for specifying the arbitrary hole positions. By pushing [POINTS], the following pop-up window is displayed. POINTS
1/1
POINT X POINT Y PATTERN CONT.
POINT X / Y POINT-2 X / Y PATTERN CONT.
X= Y= Q= END
: X and Y coordinate of the position of each hole. : If the above items is inputted, display the next X and Y point automatically. (Max.: 8 holes points ) : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G200 X Y Q (A B C D E F
-148-
www.teknikokul.net
• • • • ) ;
2.2
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
LINE
(G201) This is a menu for specifying the pattern of hole positions at same or different spaces on arbitrary line. By pushing [LINE], the following pop-up window is displayed. LINE
1/1
SPACE START POINT X START POINT Y LINE ANGLE HOLES NUMBER PITCH SPACE PATTERN CONT.
W= SAME X= Y= A= 0.000 N= P= Q= END
• In the case of W = SAME SPACE START POINT X/Y LINE ANGLE HOLES NUMBER PITCH SPACE PITCH SPACE -1 / -2 / -3 PATTERN CONT.
LINE SPACE START POINT X START POINT Y LINE ANGLE PITCH SPACE-1 PITCH SPACE-2 PITCH SPACE-3 PATTERN CONT.
1/1 W= DIFFER X= Y= A= 0.000 B= C= D= Q= END
• In the case of W = DIFFER
: Select the space from the following soft-keys. [SAME (space)], [DIFFER (space)] : X and Y coordinate of the position of the 1st hole. : The angle between the X axis and the straight line. If there is no input, 0 is regarded. : The total number of holes, including the number of the points to be omitted. : The space in the hole position. : Each space in the hole position. : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
-149-
www.teknikokul.net
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
By pushing [DETAIL], the following pop-up window is displayed. LINE (DETAIL)
LINE (DETAIL)
LINE LENGTH OMIT POINT-1 OMIT POINT-2 OMIT POINT-3 OMIT POINT-4
L= B= C= D= E=
PITCH SPACE-4 PITCH SPACE-5 PITCH SPACE-6 PITCH SPACE-7 PITCH SPACE-8 PITCH SPACE-9 PITCH SPACE-10
• In the case of W = SAME LINE LENGTH OMIT POINT -1 / -2 / -3 / -4 PITCH SPACE -4/-5/-6/-7/-8/ -9/-10
E= F= H= I= J= K= L=
• In the case of W = DIFFER
: The length of the straight. Input either PITCH SPACE (P) or LINE LENGTH (L). : To designate the point to be omitted, input the hole drilling sequence number including its point. : Each space in the hole position. (Max.: 8 points)
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G201 W X Y A N P Q
-150-
www.teknikokul.net
(L
B
C
• • • • ) ;
2.3
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
GRID (G202) This is a menu for specifying the holes positions of a grid. By pushing [GRID], the following pop-up window is displayed. GRID
1/1
SRART POINT X SRART POINT Y U-LENGTH V-LENGTH U-NUMBER V-NUMBER PATTERN CONT.
START POINT X/Y U / V -LENGTH U / V -NUMBER PATTERN CONT.
X= Y= U= V= I= J= Q= END
: X / Y coordinates of the position of the hole of the 1st point respectively. The 1st point is at the lower left position of the grid. : The length in the horizontal and vertical direction. : The number of the holes in the horizontal and vertical direction respectively. : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
By pushing [DETAIL], the following pop-up window is displayed. GRID (DETAIL) X-U ANGLE U-V ANGLE OMIT POINT-1 OMIT POINT-2 OMIT POINT-3 OMIT POINT-4
-151-
www.teknikokul.net
K= 0.000 L= 90.000 B= C= D= E=
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
X-U ANGLE
U-V ANGLE
OMIT POINT -1 / -2 / -3 / -4
B-63424EN/03
: The angle between the line in the horizontal direction and the X axis. It is considered to be 0 if not input. : The acute angle between the line defined by the points and the horizontal direction and vertical direction. It is considered to be 0 if not input : To designate the point to be omitted, input the hole drilling sequence number including its point.
Hole Machining Sequence
1
2
3
GRID
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G202 X Y U V I
-152-
www.teknikokul.net
J
K L
Q
(B
C D E
) ;
B-63424EN/03
2.4
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
SQUARE (G203) This is a menu for specifying the holes positions of a square. By pushing [SQUARE], the following pop-up window is displayed. SQUARE SRART POINT X SRART POINT Y U-LENGTH V-LENGTH U-NUMBER V-NUMBER PATTERN CONT.
START POINT X/Y U / V -LENGTH U / V -NUMBER PATTERN CONT.
1/1 X= Y= U= V= I= J= Q= END
: X / Y coordinates of the position of the hole of the 1st point respectively. The 1st point is at the lower left position of the square. : The length in the horizontal and vertical direction. : The number of the holes in the horizontal and vertical direction respectively. : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
By pushing [DETAIL], the following pop-up window is displayed. SQUARE (DETAIL) X-U ANGLE U-V ANGLE OMIT POINT-1 OMIT POINT-2 OMIT POINT-3 OMIT POINT-4
-153-
www.teknikokul.net
K= 0.000 L= 90.000 A= B= C= D=
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
X-U ANGLE
U-V ANGLE
OMIT POINT -1 / -2 / -3 / -4
B-63424EN/03
: The angle between the line in the horizontal direction and the X axis. It is considered to be 0 if not input. : The acute angle between the line defined by the points and the horizontal direction and vertical direction. It is considered to be 0 if not input : To designate the point to be omitted, input the hole drilling sequence number including its point.
Hole Machining Sequence
1
2
3
SQUARE
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G203 X Y U V I
-154-
www.teknikokul.net
J
K L
Q
(B
C D E
) ;
2.5
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
CIRCLE
(G204) This is a menu for specifying the holes positions of a circle in a same space. By pushing [CIRCLE], the following pop-up window is displayed. CIRCLE CENTER POINT X CENTER POINT Y RADIUS START ANGLE HOLE NUMBER PATTERN CONT.
CENTER POINT X/Y RADIUS START ANGLE
HOLE NUMBER PATTERN CONT.
1/1 X= Y= R= A= 0.000 N= Q= END
: X and Y coordinate of the center of the circle. : The radius of the circle : The angle between the segment from the center of the circle to starting point and the X axis. If there is no input, 0 is regarded and the starting point is considered to be on the X axis. : The total number of holes, including the number of the points to be omitted. : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
-155-
www.teknikokul.net
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
By pushing [DETAIL], the following pop-up window is displayed. CIRCLE (DETAIL) OMIT POINT-1 OMIT POINT-2 OMIT POINT-3 OMIT POINT-4
OMIT POINT -1 / -2 / -3 / -4
B= C= D= E=
: To designate the point to be omitted, input the hole drilling sequence number including its point. Hole Machining Sequence 2 3
1
CIRCLE
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G204 X Y R A N Q
-156-
www.teknikokul.net
(B
C
• • • • ) ;
2.6
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
ARC
(G205) This is a menu for specifying the holes positions of a same space arc or a differ space arc. By pushing [ARC], the following pop-up window is displayed. ARC
1/1
SPACE CENTER POINT X CENTER POINT Y RADIUS START ANGLE PITCH ANGLE HOLE NUMBER PATTERN CONT.
W= SAME X= Y= R= A= 0.000 P= N= Q= END
• In the case of W = SAME
ARC SPACE CENTER POINT X CENTER POINT Y RADIUS START ANGLE PITCH ANGLE-1 PITCH ANGLE-2 PATTERN CONT.
1/1 W= DIFFER X= Y= R= A= 0.000 B= C= Q= END
• In the case of W = DIFFER
: Select the space from the following soft-keys. [SAME (space arc)], [DIFFER (space arc)] CENTER POINT : X and Y coordinate of the center of the circle. SPACE
X/Y RADIUS START ANGLE
PITCH ANGLE HOLE NUMBER PITCH SPACE -1 / -2 PATTERN CONT.
: The radius of the circle : The angle between the segment from the center of the circle to starting point and the X axis. If there is no input, 0 is regarded and the starting point is considered to be on the X axis. : The angle between the segments from the center of the circle to each point only for same space arc. : The total number of holes, including the number of the points to be omitted. : The angle between the segments from the center of the circle to each point. Input the angles one by one starting from angle1. : Select whether to continue entering another hole pattern from the following soft-keys. [END (end)], [CONT (continue)]
-157-
www.teknikokul.net
2. HOLE PATTERN
TYPES OF CYCLE MOTIONS
B-63424EN/03
By pushing [DETAIL], the following pop-up window is displayed. ARC (DETAIL) OMIT POINT-1 OMIT POINT-2 OMIT POINT-3 OMIT POINT-4
ARC (DETAIL) B= C= D= E=
PITCH SPACE-3 PITCH SPACE-4 PITCH SPACE-5 PITCH SPACE-6 PITCH SPACE-7 PITCH SPACE-8 PITCH SPACE-9 PITCH SPACE-10
• In the case of W = SAME OMIT POINT -1 / -2 / -3 / -4
D= E= F= H= I= J= K= L=
• In the case of W = DIFFER
: To designate the point to be omitted, input the hole drilling sequence number including its point. Hole Machining Sequence 3
2 1
ARC PITCH SPACE -3/-4/-5/-6/-7/-8/9/-10
: Each space in the hole position. (Max.: 8 points)
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G205 W X Y R A N P Q (B C
-158-
www.teknikokul.net
• • • • ) ;
TYPES OF CYCLE MOTIONS
B-63424EN/03
3
3. FACING
FACING By pushing [FACE], the facing menus are displayed as follows. SQUARE
CIRCLE
RETURN
After this, we will explain the case of [WINDOW] ON. As to the case of [WINDOW] OFF, the address which corresponds to the item of each menu is displayed in key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next address is displayed. After repeating this operations, by INSERT key, inputted data are decided. (“;” is inserted.)
-159-
www.teknikokul.net
3. FACING
3.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
SQUARE SURFACE (G210) This is a menu for facing the surface on a square shape plane. By pushing [SQUARE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. SQUARE FACE MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH FINISHING ALW. FEED RATE CUTTING WITDH
1/2 P= ROUGH Z= B= J= H= 0.000 F= C= 70.000
• First page
SQUARE FACE CENTER POINT X CENTER POINT Y U-LENGTH V-LENGTH
2/2 X= Y= U= V=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (cutting)], [FINISH (cutting)] END POINT Z : Z coordinate of the final machined surface. REMOVAL : The machining allowance in the Z direction of the DEPTH cutting surface. ( For ROUGH only ) REMOVAL : The machining allowance of one pass for rough PITCH cutting in the Z direction. Rough cutting is done in one pass if no input. ( For ROUGH only ) FINISHING : The machining allowance in the Z direction for ALW. finish cutting. This is cut in one pass. Finish cutting is not done if no input. ( For ROUGH only ) FEED RATE : The feed rate of the tool. CUTTING : The machining allowance of one pass in the XY WITDH direction. It is specified a rate (%) of the tool. (less than 70%) CENTER POINT : X and Y coordinate of the center of the square. MACH. PROCESS
X/Y U / V - LENGTH
: The horizontal and vertical length of the square.
-160-
www.teknikokul.net
B-63424EN/03
3. FACING
TYPES OF CYCLE MOTIONS
By pushing [DETAIL], the following pop-up window is displayed. SQUARE FACE (DETAIL) CLEARANCE CUT DIRECTION INCLINE ANGLE START POINT SEL. APPROACH GAP ESCAPE GAP
CLEARANCE
CUT DIRECTION
L= 3.000 W= UNIDIR A= 0.000 E= [1] M= 5.000 N= 5.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [UNIDIR (uni-direction)], [BIDIR (bi-direction)], [RING (Ring-direction)]
Uni-direction
Bi-direction
Ring-direction
: The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input.
INCLINE ANGLE
A Workpiece
-161-
www.teknikokul.net
X axis
3. FACING
TYPES OF CYCLE MOTIONS
START POINT SEL.
APPROACH GAP ESCAPE GAP
U-SIDE WIDTH V-SIDE WIDTH
MOVEMENTS
B-63424EN/03
: Select the starting position of the machining from the following soft-keys. [1], [2], [3], [4] [4]
[2]
[3]
[1]
: The gap between the tool edge in the cutting feed start point and the work. If there is no input, 5mm is regarded. : The gap between the tool edge and the workpiece when the tool moves away from the work. If there is no input, 5mm is regarded. : The width of the frame corresponding to side U. ( For RING only ) : The width of the frame corresponding to side V. ( For RING only ) : Rapid Traverse (G00) Feed Traverse (G01)
• Uni-direction Pitch
Clearance Depth Finish ALW.
Z X D Y
C X
A Approach Gap
-162-
www.teknikokul.net
Cutting Width B Escape Gap
3. FACING
TYPES OF CYCLE MOTIONS
B-63424EN/03
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the point equal to (END POINT Z + REMOVAL DEPTH – REMOVAL PITCH) 3. Cutting feed to the opposite side (B) of the starting point. 4. Rise along the Z axis in rapid traverse by an amount of (CLEARANCE + REMOVAL PITCH). 5. Rapid traverse along the X-Y axis up to the next starting point (C). 6. Descent along the Z axis in rapid traverse by an amount of (CLEARANCE + REMOVAL PITCH). 7. 3.- 6. is repeated up to the ending point (D). 8. Rise along the Z axis in rapid traverse by an amount of (CLEARANCE + REMOVAL PITCH). 9. Repeat steps 1. to 8. advancing in the –Z direction, pitch by pitch, up to the point (END POINT Z + FINISHING ALW.). 10. Rise along the Z axis up to the point (END POINT Z + CLEARANCE). In the case of finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the point equal to END POINT Z. 3. Cutting feed to the opposite side (B) of the starting point. 4. Rise along the Z axis in rapid traverse by an amount of CLEARANCE. 5. Rapid traverse along the X-Y axis up to the next starting point (B). 6. Descent along the Z axis in rapid traverse up to END POINT Z. 7. 3.- 6. is repeated up to the ending point (D). 8. Rise along the Z axis in rapid traverse by an amount of CLEARANCE.
b)
• Bi-direction Pitch
Clearance Depth Finish ALW.
Z X
Y
C
D X
Cutting Width
A Approach Gap
a)
B Escape Gap
In the case of rough cutting 1. Rapid traverse up to the starting point (A). -163-
www.teknikokul.net
3. FACING
TYPES OF CYCLE MOTIONS
2.
b)
B-63424EN/03
Rapid traverse along the Z axis up to the point equal to (END POINT Z + REMOVAL DEPTH – REMOVAL PITCH) 3. Cutting feed to the other side (B) in the X axis (U direction). 4. Rapid traverse in the Y axis (V direction) to next starting point (C) according to CUTTING WITDH. 5. Cutting feed to the other side (D) in the X axis (U direction). 6. Rapid traverse in the Y axis (V direction) to next starting point according to CUTTING WITDH. 7. 3.- 6. is repeated up to the ending point (D). 8. Rise along the Z axis in rapid traverse by an amount of CLEARANCE. 9. Repeat steps 1. to 8. advancing in the –Z direction, pitch by pitch, up to the point (END POINT Z + FINISHING ALW.). 10. Rise along the Z axis up to the point (END POINT Z + FINISHING ALW. + CLEARANCE). In the case of finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the point equal to END POINT Z. 3. Cutting feed to the other side (B) in the X axis (U direction). 4. Rapid traverse in the Y axis (V direction) to next starting point (C) according to CUTTING WITDH. 5. Cutting feed to the other side (D) in the X axis (U direction). 6. Rapid traverse in the Y axis (V direction) to next starting point according to CUTTING WITDH. 7. 3.- 6. is repeated up to the ending point (D). 8. Rise along the Z axis in rapid traverse by an amount of CLEARANCE.
-164-
www.teknikokul.net
3. FACING
TYPES OF CYCLE MOTIONS
B-63424EN/03
• Ring-direction Pitch Z
Clearance Depth Finish ALW.
X
Y X
Cutting Width A Approach Gap
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the point equal to (END POINT Z + REMOVAL DEPTH – REMOVAL PITCH) 3. Cut spirally and finally move in cutting feed by an amount equal to ESCAPE GAP. 4. Rise along the Z axis in rapid traverse by an amount equal to CLEARANCE. 5. Repeat steps 1. to 4. advancing in the –Z direction, pitch by pitch, up to the point (END POINT Z + FINISHING ALW.). 6. Rise along the Z axis up to the point (END POINT Z + FINISHING ALW. + CLEARANCE).
b)
In the case of finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the point equal to END POINT Z. 3. Cut spirally and finally move in cutting feed by an amount equal to ESCAPE GAP. 4. Rise along the Z axis in rapid traverse by an amount equal to CLEARANCE.
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G210 P L Z B J H F C W X Y
-165-
www.teknikokul.net
• • • • ;
3. FACING
3.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
CIRCLE SURFACE (G211) This is a menu for facing the surface on a circle shape plane. By pushing [CIRCLE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CIRCLE FACE MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH FINISHING ALW. FEED RATE CUTTING WITDH
1/2 P= ROUGH Z= B= J= H= 0.000 F= C= 70.000
• First page
CIRCLE FACE CENTER POINT X CENTER POINT Y RADIUS
2/2 X= Y= R=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (cutting)], [FINISH (cutting)] END POINT Z : Z coordinate of the final machined surface. REMOVAL : The machining allowance in the Z direction of the DEPTH cutting surface. ( For ROUGH only ) REMOVAL : The machining allowance of one pass for rough PITCH cutting in the Z direction. Rough cutting is done in one pass if no input. ( For ROUGH only ) FINISHING : The machining allowance in the Z direction for ALW. finish cutting. This is cut in one pass. Finish cutting is not done if no input. ( For ROUGH only ) FEED RATE : The feed rate of the tool. CUTTING : The machining allowance of one pass in the XY WITDH direction. It is specified a rate (%) of the tool. (less than 70%) CENTER POINT : X and Y coordinate of the center of the circular X/Y surface. RADIUS : The radius of the circular surface. MACH. PROCESS
-166-
www.teknikokul.net
B-63424EN/03
3. FACING
TYPES OF CYCLE MOTIONS
By pushing [DETAIL], the following pop-up window is displayed. CIRCLE FACE (DETAIL) CLEARANCE CUT DIRECTION START POINT SEL. APPROACH GAP ESCAPE GAP
CLEARANCE
CUT DIRECTION
L= 3.000 W= UNIDIR E= [1] M= 5.000 N= 5.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [UNIDIR (uni-direction)], [BIDIR (bi-direction)], [RING (Ring-direction)]
Uni-direction START POINT SEL.
Bi-direction
Ring-direction
: Select the starting position of the machining from the following soft-keys. [1], [2], [3], [4]
-167-
www.teknikokul.net
[4]
[2]
[3]
[1]
3. FACING
TYPES OF CYCLE MOTIONS
APPROACH GAP ESCAPE GAP
RING WIDTH MOVEMENTS
B-63424EN/03
: The gap between the tool edge in the cutting feed start point and the work. If there is no input, 5mm is regarded. : The gap between the tool edge and the workpiece when the tool moves away from the work. If there is no input, 5mm is regarded. : The width of the ring. ( For RING only ) : Except for the shape of the circle surface, the machining movements are the same the one for a square surface.
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G211 P L Z B J H F C W X Y
-168-
www.teknikokul.net
• • • • ;
B-63424EN/03
4
TYPES OF CYCLE MOTIONS
4. SIDE CUTTING
SIDE CUTTING By pushing [SIDE], the side cutting menus are displayed as follows. SQUARE
CIRCLE
TRACK
1-SIDE
CONTUR
RETURN
After this, we will explain the case of [WINDOW] ON. As to the case of [WINDOW] OFF, the address which corresponds to the item of each menu is displayed in key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next address is displayed. After repeating this operations, by INSERT key, inputted data are decided. (“;” is inserted.)
-169-
www.teknikokul.net
4. SIDE CUTTING
4.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
SQUARE SIDE (G220) This is a menu for cutting the square shape side. By pushing [SQUARE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. SQUARE SIDE MACH. PROCESS END POINT Z SIDE REMOVAL SIDE PITCH SIDE FINISH BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
1/2 P= ROUGH Z= S= I= D= 0.000 B= J= H= 0.000
• First page MACH. PROCESS
END POINT Z SIDE REMOVAL SIDE PITCH
SIDE FINISH
BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
CHAMFER REMOVAL
SQUARE SIDE FEED RATE Z-CUT FEED RATE MACH. SHAPE CENTER POINT X CENTER POINT Y U-LENGTH V-LENGTH
2/2 F= E= M= X= Y= U= V=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)] : Z coordinate of the final machined surface. : The side machining allowance. ( For ROUGH and B-FIN only ) : The side machining allowance of one pass for rough cutting. Rough cutting is done in one pass if no input. ( For ROUGH and B-FIN only ) : The machining allowance of the side finish cutting. This is cut in one pass. Side finish cutting is not done if no input. ( For ROUGH only ) : The machining allowance in the Z direction of the cutting surface. : The machining allowance of one pass in the Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN only ) : The machining allowance of the bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( For ROUGH only ) : The amount of chamfering. ( For CHAMF only )
-170-
www.teknikokul.net
B-63424EN/03
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
TOOL SMALL DIA.
: The small diameter of chamfer tool. ( For CHAMF only ) Tool Diameter
Small Diameter
: The tool edge angle of a chamfering tool. ( For CHAMF only )
CHAMFER ANGLE
Tool Angle
: The thrust depth of a chamfering tool. ( For CHAMF only )
TOOL OUT DEPTH
Tool Depth Workpiece
FEED RATE Z-CUT FEED RATE
MACH. SHAPE
: The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + BOTTOM REMOVAL + CLEARANCE) : Select the machining shape from the following soft-keys. [OUTSID], [INSIDE]
Out-side
-171-
www.teknikokul.net
In-side
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
CENTER POINT X/Y U/V–LENGTH
B-63424EN/03
: X and Y coordinate of the center of the square. : The horizontal and vertical length of the square. In the case of INSIDE, be sure that U > V or U=V. If not, input INCLINE ANGLE of detail to 90.
By pushing [DETAIL], the following pop-up window is displayed. SQUARE SIDE (DETAIL) CLEARANCE CUT DIRECTION CORNER TYPE CORNER R / C INCLINE ANGLE APPROACH GAP START POINT SEL.
L= 3.000 W= DOWNCT Q= R M= 0.000 A= 0.000 K= 5.000 N= [1]
CLEARANCE
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
CUT DIRECTION
: Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction.
End-mill Down-cut
-172-
www.teknikokul.net
Up-cut
B-63424EN/03
TYPES OF CYCLE MOTIONS
CORNER TYPE
CORNER R / C
4. SIDE CUTTING
: Select the corner type of the outside square shape from the following soft-keys. (For outside only) [R (corner R)], [C (corner C)] : The amount of radius or chamfer at a corner.
C R Corner R
Corner C
: The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input.
INCLINE ANGLE
A X axis Workpiece
: The gap between the tool edge in the cutting feed start point and the workpiece. The default data is 5mm. ( For ROUGH or B-FIN only )
APPROACH GAP
K APPROACH / ESCAPE
: The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only )
K
-173-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
B-63424EN/03
: Select the starting position of the machining from the following soft-keys. [1], [2]
START POINT SEL.
[2]
[2]
[1] Out-side
MOVEMENTS
[1]
In-side
: Rapid Traverse (G00) Feed Traverse (G01)
• Out-side
Z
Point R
Bottom Pitch
X
Clearance Bottom Removal Bottom Finish Side Removal Side Finish
Y X
A B
Side Pitch
Approach/Escape Gap
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (BOTTOM PITCH). 4. Cutting movement (FEED RATE) toward the center by the pitch (SIDE PITCH) . 5. Side cutting with the cutting width of the pitch (SIDE PITCH). 6. 4.-5. are repeated up to the point of the distance (SIDE FINISH). 7. Move away the amount (CLEARANCE) along the Z axis. 8. Rapid traverse back to the starting point (A). 9. 3.-8. are repeated up to the point of the distance (BOTTOM FINISH).
-174-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
4. SIDE CUTTING
10. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE). b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the point (END POINT Z). 4. Cutting movement (FEED RATE) toward the center by the pitch (SIDE PITCH) . 5. Side cutting with the cutting width of the pitch (SIDE PITCH). 6. 4.-5. are repeated up to the point of the distance (SIDE FINISH). 7. Move away the amount (CLEARANCE) along the Z axis.
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point (B). 2. Rapid traverse along the Z axis up to the cutting point + CLEARANCE. (Cutting point : It is calculated by END POINT Z, BOTTOM REMOVAL, BOTTOM PITCH, CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the cutting point. 4. Cut into the workpiece following a circular path. 5. Cutting of the side finish allowance (SIDE FINISH). 6. Move away from the workpiece following a circular path after cutting. 7. Move away the amount (CLEARANCE) along the Z axis. 8. Rapid traverse back to the starting point (B). 9. 2.-8. are repeated up to the point (END POINT Z). 10. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
d)
In the case of chamfering 1. Rapid traverse up to the starting point (B). 2. Rapid traverse along the Z axis up to the cutting point. (Cutting point : It is calculated by END POINT Z, BOTTOM REMOVAL, CHAMFER REMOVAL, TOOL SMALL DIA. CHAMFER ANGLE, TOOL OUT DEPTH, CLEARANCE) 3. Cut into the workpiece following a circular path. 4. Cutting of the chamfering allowance (CHAMFER REMOVAL). 5. Move away from the workpiece following a circular path after cutting. 6. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
-175-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
B-63424EN/03
• In-side
Z
Point R
Bottom Pitch
Clearance Bottom Removal Bottom Finish
X
Side Removal Side Finish
A B
Y
Side Pitch
X Approach/Escape Gap
: Except for cutting inside, the basic movements are similar to those of the Out-side cutting
MOVEMENTS
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G220 P L
Z S
I
D B
-176-
www.teknikokul.net
J
H
F E
• • • • ;
B-63424EN/03
4.2
TYPES OF CYCLE MOTIONS
4. SIDE CUTTING
CIRCLE SIDE (G221) This is a menu for cutting the circle shape side. By pushing [CIRCLE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CIRCLE SIDE MACH. PROCESS END POINT Z SIDE REMOVAL SIDE PITCH SIDE FINISH BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
1/2 P= ROUGH Z= S= I= D= 0.000 B= J= H= 0.000
• First page MACH. PROCESS
END POINT Z SIDE REMOVAL SIDE PITCH
SIDE FINISH
BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
CHAMFER REMOVAL TOOL SMALL DIA.
CIRCLE SIDE FEED RATE Z-CUT FEED RATE MACH. SHAPE CENTER POINT X CENTER POINT Y RADIUS
2/2 F= E= M= X= Y= R=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)] : Z coordinate of the final machined surface. : The side machining allowance. ( For ROUGH and B-FIN only ) : The side machining allowance of one pass for rough cutting. Rough cutting is done in one pass if no input. ( For ROUGH and B-FIN only ) : The machining allowance of the side finish cutting. This is cut in one pass. Side finish cutting is not done if no input. ( For ROUGH only ) : The machining allowance in the Z direction of the cutting surface. : The machining allowance of one pass for rough cutting in the Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN only ) : The machining allowance of the bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( For ROUGH only ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only )
-177-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
CHAMFER ANGLE TOOL OUT DEPTH FEED RATE Z-CUT FEED RATE
MACH. SHAPE
B-63424EN/03
: The tool edge angle of a chamfering tool. ( For CHAMF only ) : The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + BOTTOM REMOVAL + CLEARANCE) : Select the machining shape from the following soft-keys. [OUTSID], [INSIDE]
Out-side CENTER POINT X/Y RADIUS
In-side
: X and Y coordinate of the center of the circle. : The radius of a circle.
By pushing [DETAIL], the following pop-up window is displayed. CIRCLE SIDE (DETAIL) CLEARANCE CUT DIRECTION APPROACH GAP START POINT SEL.
CLEARANCE
L= 3.000 W= DOWNCT K= 5.000 N= [1]
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
-178-
www.teknikokul.net
B-63424EN/03
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
: Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction. : The gap between the tool edge in the cutting feed start point and the workpiece. The default data is 5mm. ( For ROUGH or B-FIN only ) : The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only ) : Select the starting position of the machining from the following soft-keys. [1], [2]
CUT DIRECTION
APPROACH GAP
APPROACH / ESCAPE
START POINT SEL.
[2] [2]
[1] Out-side
MOVEMENTS
[1] In-side
: Except for the shape of the circle, the basic movements are similar to those of Square Side.
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G221 P L Z S I D B J H F E
-179-
www.teknikokul.net
• • • • ;
4. SIDE CUTTING
4.3
TYPES OF CYCLE MOTIONS
B-63424EN/03
TRACK SIDE (G222) This is a menu for cutting the track shape side. By pushing [TRACK], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. TRACK SIDE MACH. PROCESS END POINT Z SIDE REMOVAL SIDE PITCH SIDE FINISH BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
1/2 P= ROUGH Z= S= I= D= 0.000 B= J= H= 0.000
• First page MACH. PROCESS
END POINT Z SIDE REMOVAL SIDE PITCH
SIDE FINISH
BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
CHAMFER REMOVAL TOOL SMALL DIA.
TRACK SIDE FEED RATE Z-CUT FEED RATE MACH. SHAPE CENTER POINT X CENTER POINT Y CENTER DISTANCE RADIUS
2/2 F= E= M= X= Y= U= R=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)] : Z coordinate of the final machined surface. : The side machining allowance. ( For ROUGH and B-FIN only ) : The side machining allowance of one pass for rough cutting. Rough cutting is done in one pass if no input. ( For ROUGH and B-FIN only ) : The machining allowance of the side finish cutting. This is cut in one pass. Side finish cutting is not done if no input. ( For ROUGH only ) : The machining allowance in the Z direction of the cutting surface. : The machining allowance of one pass for rough cutting in the Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN only ) : The machining allowance of the bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( For ROUGH only ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only )
-180-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
CHAMFER ANGLE TOOL OUT DEPTH FEED RATE Z-CUT FEED RATE
MACH. SHAPE
: The tool edge angle of a chamfering tool. ( For CHAMF only ) : The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + BOTTOM REMOVAL + CLEARANCE) : Select the machining shape from the following soft-keys. [OUTSID], [INSIDE]
Out-side CENTER POINT X/Y CENTER DISTANCE RADIUS
4. SIDE CUTTING
In-side
: X and Y coordinate of the center of the left arc. : The distance between the centers of the two arcs. : The radius of a circle.
By pushing [DETAIL], the following pop-up window is displayed. TRACK SIDE (DETAIL) CLEARANCE CUT DIRECTION INCLINE ANGLE APPROACH GAP START POINT SEL.
CLEARANCE
L= 3.000 W= DOWNCT A= 0.000 K= 5.000 N= [1]
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
-181-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
CUT DIRECTION
INCLINE ANGLE APPROACH GAP
APPROACH / ESCAPE
START POINT SEL.
B-63424EN/03
: Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction. : The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input. : The gap between the tool edge in the cutting feed start point and the workpiece. The default data is 5mm. ( For ROUGH or B-FIN only ) : The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only ) : Select the starting position of the machining from the following soft-keys. [1], [2]
[2]
[1]
[2] Out-side
[1]
In-side
: Except for the shape of the track, the basic movements are similar to those of Square Side.
MOVEMENTS
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G222 P L
Z S
I
D B
-182-
www.teknikokul.net
J
H
F E
• • • • ;
B-63424EN/03
4.4
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
ONE SIDE (G223) This is a menu for cutting the one side only. By pushing [1-SIDE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. ONE SIDE
1/2
MACH. PROCESS END POINT Z SIDE REMOVAL SIDE PITCH SIDE FINISH BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
P= ROUGH Z= S= I= D= 0.000 B= J= H= 0.000
• First page MACH. PROCESS
END POINT Z SIDE REMOVAL SIDE PITCH
SIDE FINISH
BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
CHAMFER REMOVAL TOOL SMALL DIA.
ONE SIDE FEED RATE CENTER POINT X CENTER POINT Y U-LENGTH
2/2 F= X= Y= U=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)] : Z coordinate of the final machined surface. : The side machining allowance. ( For ROUGH and B-FIN only ) : The side machining allowance of one pass for rough cutting. Rough cutting is done in one pass if no input. ( For ROUGH and B-FIN only ) : The machining allowance of the side finish cutting. This is cut in one pass. Side finish cutting is not done if no input. ( For ROUGH only ) : The machining allowance in the Z direction of the cutting surface. : The machining allowance of one pass for rough cutting in the Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN only ) : The machining allowance of the bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( For ROUGH only ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only )
-183-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
CHAMFER ANGLE TOOL OUT DEPTH FEED RATE CENTER POINT X/Y U – LENGTH
B-63424EN/03
: The tool edge angle of a chamfering tool. ( For CHAMF only ) : The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : X and Y coordinate of the center of the cutting surface after cutting. : The length of the workpiece in the cutting surface.
By pushing [DETAIL], the following pop-up window is displayed. ONE SIDE (DETAIL) CLEARANCE CUT DIRECTION INCLINE ANGLE APPROACH GAP ESCAPE GAP
L= W= A= M= N=
3.000 1:DOWN 0.000 5.000 5.000
CLEARANCE
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
CUT DIRECTION
: Select the cutting direction from the following soft-keys. [1-DOWN], [2-UP], [3-DOWN], [4-UP] [4: Down-cut]
[2: Up-cut] (X, Y) Approach / Escape gap (X, Y)
[3: Up-cut]
[1: Down-cut]
: The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input. : The gap between the tool edge in the machining start point and the workpiece edge. The default data is 5mm. : The gap between the tool edge when the tool
INCLINE ANGLE APPROACH GAP ESCAPE GAP
-184-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
4. SIDE CUTTING
moves away from the workpiece after cutting and the workpiece edge. The default data is 5mm. MOVEMENTS
: Rapid Traverse (G00) Feed Traverse (G01)
Z
Bottom Pitch
Point R X
Clearance Bottom Removal Bottom Finish
Y X A
Side Pitch Approach/Escape Gap
Side Removal Side Finish Clearance
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Rapid traverse toward one side by the pitch (SIDE PITCH). 4. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (BOTTOM PITCH). 5. Side cutting with the cutting width of the pitch (SIDE PITCH). 6. Rise to point R in rapid traverse along the Z axis. 7. Rapid traverse back to the starting point (A). 8. 3.-7. are repeated up to the point of the distance (SIDE FINISH). 9. 3.-8. are repeated up to the point of the distance (BOTTOM FINISH). 10. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Rapid traverse toward one side by the pitch (SIDE PITCH). 4. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the end point (END POINT Z). 5. Side cutting with the cutting width of the pitch (SIDE PITCH). -185-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
6. 7. 8.
B-63424EN/03
4.-5. are repeated up to the point of the distance (SIDE FINISH). Move away from the workpiece after cutting in Z axis by a clearance. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE). 3. Rapid traverse toward one side by the allowance (SIDE FINISH). 4. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) with the pitch (BOTTOM PITCH). 5. Side cutting with the cutting width of the allowance (SIDE FINISH). 6. Move away from the workpiece after cutting 7. 3.-6. are repeated up to the point (END POINT Z). 8. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
d)
In the case of chamfering 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to the cutting point. (Cutting point : It is calculated by END POINT Z, BOTTOM REMOVAL, CHAMFER REMOVAL, TOOL SMALL DIA. CHAMFER ANGLE, TOOL OUT DEPTH, CLEARANCE) 3. Cut into the workpiece following a circular path. 4. Cutting of the chamfering allowance (CHAMFER REMOVAL). 5. Move away from the workpiece following a circular path after cutting. 6. Rapid traverse along Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE).
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G223 P L
Z S
I
D B
-186-
www.teknikokul.net
J
H
F
• • • • ;
B-63424EN/03
4.5
TYPES OF CYCLE MOTIONS
4. SIDE CUTTING
CONTOUR SIDE (G224) This is a menu for cutting the arbitrary shape side. By pushing [CONTUR] on the Editing menu, the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CONTOUR SIDE MACH. PROCESS END POINT Z SIDE REMOVAL SIDE FINISH BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
1/2 P= ROUGH Z= S= D= 0.000 B= J= H= 0.000
• First page MACH. PROCESS
END POINT Z SIDE REMOVAL SIDE FINISH
BOTTOM REMOVAL BOTTOM PITCH BOTTOM FINISH
CONTOUR SIDE FEED RATE CUTTING WIDTH% Z-CUT FEED RATE COMP. DIRECTION
2/2 F= C= 70.000 E= U=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)] : Z coordinate of the final machined surface. : The side machining allowance. ( For ROUGH and B-FIN only ) : The machining allowance of the side finish cutting. This is cut in one pass. Side finish cutting is not done if no input. ( For ROUGH only ) : The machining allowance in the Z direction of the cutting surface. : The machining allowance of one pass for rough cutting in the Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN only ) : The machining allowance of the bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( For ROUGH only )
-187-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
FEED RATE CUTTING WIDTH% Z-CUT FEED RATE
COMP. DIRECTION
B-63424EN/03
: The feed rate of the tool. : The machining allowance of one path in the XY direction. It is specified a rate (5) of the tool. (less than 70%) ( For ROUGH, B-FIN) : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + BOTTOM REMOVAL + CLEARANCE) : Select the direction of compensation from the following soft-keys. [LEFT (side)], [RIGHT (side)]
LEFT
RIGHT
By pushing [DETAIL], the following pop-up window is displayed. CONTOUR SIDE (DETAIL) CLEARANCE CUT DIRECTION APPROACH TYPE APPROACH RADIUS APPROACH ANGLE ESCAPE TYPE ESCAPE RADIUS ESCAPE ANGLE
CLEARANCE
CUT DIRECTION
L= 3.000 U= DOWNCT A= CIRCLE M= 5.000 N= 90.000 R= CIRCLE W= 5.000 X= 90.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction.
-188-
www.teknikokul.net
B-63424EN/03
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
: Select the approach type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)]
APPROACH TYPE
Tangent Circle
Tangent Line
Vertical Line
: The radius and angle of tangent circle approach.
APPROACH RADIUS / ANGLE
Angle Radius
: The distance of tangent line or vertical line approach.
APPROACH DIST.
Distance Tangent Line
ESCAPE TYPE
Distance Vertical Line
: Select the escape type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)]
Tangent Circle
-189-
www.teknikokul.net
Tangent Line
Vertical Line
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
B-63424EN/03
: The radius and angle of tangent circle escape.
ESCAPE RADIUS / ANGLE
Angle Radius
ESCAPE DIST.
: The distance of tangent line or vertical line escape. Distance
Tangent Line
Distance Vertical Line
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G224 P L
Z S
D B
J
H
F C E
U • • • • ;
l Definition of arbitrary shape Arbitrary shape is defined by using [CONTUR] of G code menu. In detail, refer to “II. OPERATION, 3.2.8 Contour”. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G100 X Y ; G101 X Y M N L G106 X Y P ;
-190-
www.teknikokul.net
K ;
TYPES OF CYCLE MOTIONS
B-63424EN/03
4. SIDE CUTTING
NOTE 1) G224 is not worked independently. Therefore, after specified G224, be sure to specify the contour shape by using contour menu (G100,,,G106). 2) By setting the parameter No.9125 to 224, the softkeys are automatically changed to contour shape (G100,,,G106). MOVEMENTS
: Rapid Traverse (G00) Feed Traverse (G01, G02, G03)
Z
Point R
Bottom Pitch
Clearance Bottom Removal Bottom Finish
X
Tool Diameter × Cutting Width Y
A Side Removal Side Finish
X A
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (BOTTOM PITCH). 4. Cut into the workpiece in cutting feed following approach type (CIRCLE, TANGNT or VERTCL) 5. Side cutting with the cutting width (Tool Diameter × CUTTING WIDTH) along the contour shape. 6. Move away from the workpiece following escape type (CIRCLE, TANGNT or VERTCL) 7. Move away along the Z axis up to point R in cutting feed. 8. Rapid traverse up to the next starting point. 9. 3.-8. are repeated up to the point of the distance (SIDE FINISH). 10. 3.-9. are repeated up to the point of the distance (BOTTOM FINISH). 11. Rise in cutting feed along Z axis up to point R.
-191-
www.teknikokul.net
4. SIDE CUTTING
TYPES OF CYCLE MOTIONS
B-63424EN/03
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the point (END POINT Z). 4. Cut into the workpiece in cutting feed following approach type (CIRCLE, TANGNT or VERTCL) 5. Side cutting with the cutting width (Tool Diameter × CUTTING WIDTH) along the contour shape. 6. Move away from the workpiece following escape type (CIRCLE, TANGNT or VERTCL) 7. Move away up to R point in cutting feed. 8. Rapid traverse up to the next starting point. 9. 3.-8. are repeated up to the point of the distance (SIDE FINISH 10. Rise in cutting feed along Z axis up to point R.
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + BOTTOM REMOVAL + CLEARANCE) 3. Descent along the lower Z axis up to the end point (END POINT Z) in cutting feed (Z-CUT FEED RATE). 4. Cut into the workpiece in cutting feed following approach type (CIRCLE, TANGNT or VERTCL) 5. Side cutting with the cutting width of the pitch (SIDE FINISH) along the contour shape. 6. Move away from the workpiece following escape type (CIRCLE, TANGNT or VERTCL) 7. Rise in cutting feed along Z axis up to point R.
NOTE The alarm may occur owing to the restriction of contour figure number or work memory size for calculation. In this case, please divide the contour figure into some group.
-192-
www.teknikokul.net
B-63424EN/03
5
5. POCKETING
TYPES OF CYCLE MOTIONS
POCKETING By pushing [POCKET], the side cutting menus are displayed as follows. SQUARE
CIRCLE
TRACK
GROOVE
CONTUR
C-GROV
RETURN
After this, we will explain the case of [WINDOW] ON. As to the case of [WINDOW] OFF, the address which corresponds to the item of each menu is displayed in key-in buffer field automatically. When the data is not necessary, by pushing INPUT key, the data becomes invalid and the next address is displayed. After repeating this operations, by INSERT key, inputted data are decided. (“;” is inserted.)
-193-
www.teknikokul.net
5. POCKETING
5.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
SQUARE POCKET (G230) This is a menu for pocketing the square shape. By pushing [SQUARE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. SQUARE POCKET MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
1/2 P= ROUGH Z= B= J= H= 0.000 D= 0.000
SQUARE POCKET FEED RATE Z-CUT FEED RATE CUTTING WIDTH% CENTER POINT X CENTER POINT Y U-LENGTH V-LENGTH
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
CHAMFER REMOVAL TOOL SMALL DIA.
2/2 F= E= C= 70.000 X= Y= U= V=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)], [HOLE (Drilling)] : Z coordinate of the final machined surface. : The depth of the pocket. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except CHAMF and HOLE ) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( For ROUGH, B-FIN ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only ) Tool Diameter
Small Diameter
-194-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
: The tool edge angle of a chamfering tool. ( For CHAMF only )
CHAMFER ANGLE
Tool Angle
: The thrust depth of a chamfering tool. ( For CHAMF only )
TOOL OUT DEPTH
Tool Depth Workpiece
: The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + REMOVAL DEPTH + CLEARANCE) ( Except HOLE ) CUTTING : The machining allowance of one path in the XY WIDTH % direction. It is specified a rate (%) of the tool. ( less than 70% ) ( For ROUGH, B-FIN ) CENTER POINT : X and Y coordinate of the center of the square. FEED RATE Z-CUT FEED RATE
X/Y U/V – LENGTH CYCLE SELECT
PITCH DEPTH
: The horizontal and vertical length of the square. : Select the drilling cycle for pre-hole from the following soft-keys. [G81 (Normal drilling)], [G83 (Peck drilling)] ( For HOLE only ) : The depth of cut for each cutting cycle. It is used for G83 only. ( For HOLE only )
-195-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
By pushing [DETAIL], the following pop-up window is displayed. SQUARE POCKET (DETAIL) CLEARANCE CUT DIRECTION CORNER R INCLINE ANGLE
CLEARANCE
CUT DIRECTION
L= 3.000 W= DOWNCT R= 0.000 A= 0.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction.
End-mill Down-cut
Up-cut
: The amount of radius at a corner.
CORNER R
R Corner R
-196-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
: The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input.
INCLINE ANGLE
Angle X axis Workpiece
APPROACH / ESCAPE
: The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only )
K
-197-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
:
MOVEMENTS
Rapid Traverse (G00) Feed Traverse (G01)
Point R
Removal Pitch
Z X
Y
Clearance Removal Depth Bottom Finish
Side Finish Cutting Width
X
a)
In the case of rough cutting 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Cutting from the inside to the outside using the same cutting width (CUTTING WIDTH) in cutting feed (FEED RATE). 5. After cutting, side finish allowance (SIDE FINISH) remains. 6. Rapid traverse along Z axis up to point R 7. Rapid traverse back to the starting point (A). 8. Rapid traverse down to the cutting surface + clearance (CLEARANCE) along Z axis. 9. Advance in –Z axis by the pitch (REMOVAL PITCH) and repeat steps 3. to 8. up to the point of the distance (SIDE FINISH). 10. Rapid traverse along Z axis up to point R.
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the end point (END POINT Z). 4. Cutting from the inside to the outside using the same cutting width (CUTTING WIDTH) in cutting feed (FEED RATE). 5. After cutting, side finish allowance (SIDE FINISH) remains. 6. Rapid traverse along Z axis up to point R In the case of side finish cutting 1. Rapid traverse up to the starting point.
c)
-198-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
2. 3. 4. 5. 6. 7.
Rapid traverse along the Z axis up to the cutting point. (Cutting point : It is calculated by END POINT Z, REMOVAL DEPTH, REMOVAL PITCH, CLEARANCE) Cut into the workpiece following a circular path. Cutting of the side finish allowance (SIDE FINISH). Move away from the workpiece following a circular path after cutting. 3.-5. are repeated up to the point (END POINT Z) by the pitch (REMOVAL PITCH). Rapid traverse along Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE).
d)
In the case of chamfering 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to the cutting point. (Cutting point : It is calculated by END POINT Z, REMOVAL DEPTH, CHAMFER REMOVAL, TOOL SMALL DIA., CHAMFER ANGLE, TOOL OUT DEPTH, CLEARANCE) 3. Cut into the workpiece following a circular path. 4. Cutting of the chamfering allowance (CHAMFER REMOVAL). 5. Move away from the workpiece following a circular path after cutting. 6. Rapid traverse along Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE).
e)
In the case of drilling for pre-hole 1. Rapid traverse up to the starting point. 2. Rapid traverse along the lower Z axis up to the point R. 3. Drilling along Z axis up to the point Z (END POINT Z). 4. Rapid traverse along Z axis up to point R level (END POINT Z + REMOVAL DEPTH + CLEARANCE).
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G230 P L
Z B
J
-199-
www.teknikokul.net
H
D F C E
• • • • ;
5. POCKETING
5.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
CIRCLE POCKET (G231) This is a menu for pocketing the circle shape side. By pushing [CIRCLE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CIRCLE POCKET MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
1/2 P= ROUGH Z= B= J= H= 0.000 D= 0.000
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
CHAMFER REMOVAL TOOL SMALL DIA. CHAMFER ANGLE
CIRCLE POCKET FEED RATE Z-CUT FEED RATE CUTTING WIDTH% CENTER POINT X CENTER POINT Y RADIUS
2/2 F= E= C= 70.000 X= Y= R=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)], [HOLE (Drilling)] : Z coordinate of the final machined surface. : The depth of the pocket. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except CHAMF and HOLE ) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( For ROUGH and B-FIN ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only ) : The tool edge angle of a chamfering tool. ( For CHAMF only )
-200-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
5. POCKETING
: The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + REMOVAL DEPTH + CLEARANCE) ( Except HOLE ) CUTTING : The machining allowance of one path in the XY WIDTH % direction. It is specified a rate (%) of the tool. ( less than 70% ) ( For ROUGH and B-FIN ) CENTER POINT : X and Y coordinate of the center of the circle. TOOL OUT DEPTH FEED RATE Z-CUT FEED RATE
X/Y RADIUS CYCLE SELECT
PITCH DEPTH
: The radius of a circle. : Select the drilling cycle for pre-hole from the following soft-keys. [G81 (Normal drilling)], [G83 (Peck drilling)] ( For HOLE only ) : The depth of cut for each cutting cycle. It is used for G83 only. ( For HOLE only )
By pushing [DETAIL], the following pop-up window is displayed. CIRCLE POCKET (DETAIL) CLEARANCE CUT DIRECTION
CLEARANCE
L= 3.000 W= DOWNCT
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
-201-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
: Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction. : The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only ) : Except for the shape of the circle, the basic movements are similar to those of Square Pocket.
CUT DIRECTION
APPROACH / ESCAPE
MOVEMENTS
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G231 P L
Z B
J
-202-
www.teknikokul.net
H
D F C E
• • • • ;
B-63424EN/03
5.3
TYPES OF CYCLE MOTIONS
5. POCKETING
TRACK POCKET (G232) This is a menu for pocketing the track shape side. By pushing [TRACK], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. TRACK POCKET MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
1/2 P= ROUGH Z= B= J= H= 0.000 D= 0.000
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
CHAMFER REMOVAL TOOL SMALL DIA. CHAMFER ANGLE
TRACK POCKET FEED RATE Z-CUT FEED RATE CUTTING WIDTH% CENTER POINT X CENTER POINT Y CENTER DISTANCE RADIUS
2/2 F= E= C= 70.000 X= Y= U= R=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)], [HOLE (Drilling)] : Z coordinate of the final machined surface. : The depth of the pocket. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except CHAMF and HOLE) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( For ROUGH, B-FIN ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only ) : The tool edge angle of a chamfering tool. ( For CHAMF only )
-203-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
: The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + REMOVAL DEPTH + CLEARANCE) CUTTING : The machining allowance of one path in the XY WIDTH % direction. It is specified a rate (%) of the tool. ( less than 70% ) ( For ROUGH and B-FIN ) CENTER POINT : X and Y coordinate of the center of the left arc. TOOL OUT DEPTH FEED RATE Z-CUT FEED RATE
X/Y CENTER DISTANCE RADIUS CYCLE SELECT
PITCH DEPTH
: The distance between the centers of the two arcs. : The radius of a circle. : Select the drilling cycle for pre-hole from the following soft-keys. [G81 (Normal drilling)], [G83 (Peck drilling)] ( For HOLE only ) : The depth of cut for each cutting cycle. It is used for G83 only. ( For HOLE only )
By pushing [DETAIL], the following pop-up window is displayed. TRACK POCKET (DETAIL) CLEARANCE CUT DIRECTION INCLINE ANGLE
CLEARANCE
L= 3.000 W= DOWNCT A= 0.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm.
-204-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
: Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction. : The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input. : The radius of approach or escape. The movement is performed as a quarter arc. It is calculated automatically if not input. ( For S-FIN or CHAMF only ) : Except for the shape of the track, the basic movements are similar to those of Square Pocket.
CUT DIRECTION
INCLINE ANGLE APPROACH / ESCAPE
MOVEMENTS
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G232 P L
Z B
J
-205-
www.teknikokul.net
H
D F C E
• • • • ;
5. POCKETING
5.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
GROOVE (G233) This is a menu for machining the liner groove. By pushing [GROOVE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. GROOVE
1/2
MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
P= ROUGH Z= B= J= H= 0.000 D= 0.000
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
CHAMFER REMOVAL TOOL SMALL DIA. CHAMFER ANGLE
GROOVE FEED RATE CUTTING WIDTH% CENTER POINT X CENTER POINT Y U-LENGTH GROOVE WIDTH
2/2 F= C= 70.000 X= Y= U= V=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [CHAMF (chamfering)] : Z coordinate of the final machined surface. : The depth of the groove. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except CHAMF and HOLE) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( For ROUGH, B-FIN ) : The amount of chamfering. ( For CHAMF only ) : The small diameter of chamfer tool. ( For CHAMF only ) : The tool edge angle of a chamfering tool. ( For CHAMF only )
-206-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
5. POCKETING
: The thrust depth of a chamfering tool. ( For CHAMF only ) : The feed rate of the tool. : The machining allowance of one path in the XY direction. It is specified a rate (%) of the tool. ( less than 70% ) ( For ROUGH and B-FIN ) CENTER POINT : X and Y coordinate of the center of the groove. TOOL OUT DEPTH FEED RATE CUTTING WIDTH %
X/Y U – LENGTH GROOVE WIDTH
: The length of the groove. : The width of the groove.
By pushing [DETAIL], the following pop-up window is displayed. GROOVE (DETAIL) CLEARANCE CUT DIRECTION INCLINE ANGLE START POINT SEL. APPROACH GAP ESCAPE GAP
CLEARANCE
CUT DIRECTION
L= 3.000 W= DOWNCT A= 0.000 N= [1] K= 5.000 M= 5.000
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction.
-207-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
INCLINE ANGLE ATART POINT SEL.
B-63424EN/03
: The angle between the U side and the X axis, when the work is inclined with respect to the X axis. It is considered to be 0 if not input. : Select the starting point from the following softkeys. [1], [2]
[1]
APPROACH GAP ESCAPE GAP
[2]
: The gap between the tool edge in the cutting feed start point and the workpiece. If there is no input, 5mm is regards. : The gap between the tool edge and the workpiece when the tool moves away from the work. If there is no input, 5mm is regards.
-208-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: Rapid Traverse (G00) Feed Traverse (G01)
Removal Pitch
Point R
Clearance
Z
Removal Depth Bottom Finish
X
Y X
A
(X,Y)
Approach/Escape Gap
a)
B
Side Finish Groove Width
Cutting Width
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Cutting the opposite side of the starting point in cutting feed (FEED RATE). 5. Widening of the groove on the right and left sides symmetrically using the cutting width (CUTTING WIDTH). 6. The side finish allowance (SIDE FINISH) is left and the groove is cut. 7. Move up along Z axis to point R 8. 3.–7. are repeated until reaching the point of the distance (BOTTOM FINISH). 9. Rapid traverse along Z axis up to point R.
-209-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the end point (END POINT Z). 4. Cutting the opposite side of the starting point in cutting feed (FEED RATE). 5. Widening of the groove on the right and left sides symmetrically using the cutting width (CUTTING WIDTH). 6. The groove bottom side is cut leaving the side finish allowance (SIDE FINISH). 7. Rapid traverse along Z axis up to point R
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point (B). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Move down along Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Both sides groove are cut by the allowance (SIDE FINISH). 5. Move away from the workpiece after cutting. 6. 3.-5. are repeated up to the point (END POINT Z) by the pitch (REMOVAL PITCH). 7. Rapid traverse along Z axis up to point R.
d)
In the case of chamfering 1. Rapid traverse up to the starting point (B). 2. Rapid traverse along the Z axis up to the cutting point + CLEARANCE. (Cutting point : It is calculated by END POINT Z, REMOVAL DEPTH, CHAMFER REMOVAL, TOOL SMALL DIA., CHAMFER ANGLE, TOOL OUT DEPTH) 3. Move down along Z axis to the cutting point in cutting feed (Z-CUT FEED RATE). 4. Cut into the workpiece following a circular path. 5. Cutting of the chamfering allowance (CHAMFER REMOVAL). 6. Move away from the workpiece following a circular path after cutting. 7. Rapid traverse along Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE).
-210-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G233 P L
Z B
J
-211-
www.teknikokul.net
H
D F C
• • • • ;
5. POCKETING
5.5
TYPES OF CYCLE MOTIONS
B-63424EN/03
CONTOUR POCKET (G234) This is a menu for pocketing the arbitrary shape. By pushing [CIRCLE], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CONTOUR POCKET MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
1/2
P= ROUGH Z= B= J= H= 0.000 D= 0.000
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
FEED RATE CUTTING WIDTH % Z-CUT FEED RATE
CONTOUR POCKET FEED RATE CUTTING WIDTH% Z-CUT FEED RATE
2/2
F= C= 70.000 E=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [HOLE (Drilling)] : Z coordinate of the final machined surface. : The depth of the pocket. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH and S-FIN ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except HOLE ) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( Except S-FIN ) : The feed rate of the tool. : The machining allowance of one path in the XY direction. It is specified a rate (%) of the tool. ( less than 70% ) ( Except S-FIN ) : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + REMOVAL DEPTH + CLEARANCE) ( Except HOLE ) : D code number of milling tool for rough machining. It needs to calculate the pre-hole position. ( For HOLE only )
ROUGH D-CODE
-212-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
CYCLE SELECT
PITCH DEPTH
: Select the drilling cycle for pre-hole from the following soft-keys. [G81 (Normal drilling)], [G83 (Peck drilling)] ( For HOLE only ) : The depth of cut for each cutting cycle. It is used for G83 only. ( For HOLE only )
By pushing [DETAIL], the following pop-up window is displayed. CONTOUR POCKET (DETAIL) CLEARANCE CUT DIRECTION CUT METHOD CUT ANGLE
CLEARANCE
CUT DIRECTION
CUT METHOD
L= 3.000 U= DOWNCT K= INSIDE A= 0
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction. : Select the cutting method from the following soft-keys. [INSIDE (in-side)], [OUTSID (out-side)] In-side : Cutting from inside to outside Out-side : Cutting from outside to inside
In-side
Out-side
: The data of the cutting angle for tool-axis in-feed of pocketing. In the case of 0, it is regards 90. ( range : 0 to 90 degree )
CUT ANGLE
-213-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
A
: Select the approach type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)] ( For S-FIN only )
APPROACH TYPE
Tangent Circle
Tangent Line
Vertical Line
: The radius and angle of tangent circle approach. ( For S-FIN and CIRCLE type )
APPROACH RADIUS / ANGLE
Angle Radius
: The distance of tangent line or vertical line approach. ( For S-FIN and TANGNT / VERTCL type )
APPROACH DIST.
Distance Tangent Line
-214-
www.teknikokul.net
Distance Vertical Line
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
: Select the escape type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)] ( For S-FIN only )
ESCAPE TYPE
Tangent Circle
Tangent Line
Vertical Line
: The radius and angle of tangent circle escape. ( For S-FIN and CIRCLE type )
ESCAPE RADIUS / ANGLE
Angle Radius
: The distance of tangent line or vertical line escape. ( For S-FIN and TANGNT / VERTCL type )
ESCAPE DIST.
Distance
Distance
Tangent Line
Vertical Line
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G234 P L
Z B
J
-215-
www.teknikokul.net
H
D F C E
• • • • ;
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
l Definition of arbitrary shape Arbitrary shape is defined by using [CONTUR] of G code menu. In detail, refer to “II. OPERATION, 3.2.8 Contour”. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G100 X Y ; G101 X Y M N L
K ;
G106 X Y P ;
NOTE 1) G234 is not worked independently. Therefore, after specified G234, be sure to specify the contour shape by using contour menu (G100,,,G106). 2) By setting the parameter No.9126 to 234, the softkeys are automatically changed to contour shape (G100,,,G106).
-216-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
5. POCKETING
: Rapid Traverse (G00) Feed Traverse (G01, G02, G03)
Point R
Removal Pitch Clearance Removal Depth Bottom Finish
Z X
Y
Cutting Width X Side Finish
a)
In the case of rough cutting 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Cutting from the inside to the outside using the same cutting width (CUTTING WIDTH) in cutting feed (FEED RATE). • Tool path will be created like setting cutter compensation forward inside in order to be high efficiency. • Tool will turns around the island without jumping it. • Tool will not be interfere with a pocket figure or island figure. 5. After cutting, side finish allowance (SIDE FINISH) remains. 6. Rapid traverse along Z axis up to point R 7. Rapid traverse back to the starting point. 8. Rapid traverse down to the cutting surface + clearance (CLEARANCE) along Z axis. 9. Advance in –Z axis by the pitch (REMOVAL PITCH) and repeat steps 3. to 8. up to the point of the distance (SIDE FINISH). 10. Rapid traverse along Z axis up to point R.
-217-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the end point (END POINT Z). • Tool path will be created like setting cutter compensation forward inside in order to be high efficiency. • Tool will turns around the island without jumping it. • Tool will not be interfere with a pocket figure or island figure. 4. Cutting from the inside to the outside using the same cutting width (CUTTING WIDTH) in cutting feed (FEED RATE). 5. After cutting, side finish allowance (SIDE FINISH) remains. 6. Rise along Z axis in cutting feed by a clearance (CLEARANCE). 7. Rapid traverse along Z axis up to point R
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point. 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent up to the end point (END POINT Z) in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Cut into the workpiece in cutting feed following approach type (CIRCLE, TANGENT and VERTCL). 5. Side cutting with the side finish allowance (SIDE FINISH). 6. Move away from the workpiece following escape type (CIRCLE, TANGENT and VERTCL). 7. Rise in cutting feed along Z axis up to point R.
d)
In the case of drilling for pre-hole 1. Rapid traverse up to the starting point. 2. Rapid traverse along the lower Z axis up to the point R. 3. Drilling along Z axis up to the point Z (END POINT Z). 4. Rapid traverse along Z axis up to point R level (END POINT Z + REMOVAL DEPTH + CLEARANCE).
NOTE The alarm may occur owing to the restriction of contour figure number or work memory size for calculation. In this case, please divide the contour figure into some group.
-218-
www.teknikokul.net
B-63424EN/03
5.6
TYPES OF CYCLE MOTIONS
5. POCKETING
CONTOUR GROOVE (G235) This is a menu for machining the arbitrary groove. By pushing [C-GROV], the following pop-up window is displayed. The all items are changed according to “MACH. PROCESS”. CONTOUR GROOVE MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
1/2
P= ROUGH Z= B= J= H= 0.000 D= 0.000
• First page MACH. PROCESS
END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH
SIDE FINISH
FEED RATE CUTTING WIDTH % Z-CUT FEED RATE
CONTOUR GROOVE FEED RATE CUTTING WIDTH% Z-CUT FEED RATE GROOVE WIDTH
2/2
F= C= 70.000 E= V=
• Second page
: Select the machining process from the following soft-keys. [ROUGH (roughing)], [B-FIN (bottom finishing)], [S-FIN (side finishing)], [HOLE (Drilling)] : Z coordinate of the final machined surface. : The depth of the pocket. : The machining allowance of one pass for rough cutting, in Z direction. Cutting is done in one pass if no input. ( For ROUGH ) : The bottom machining allowance for bottom finish cutting. This is cut in one pass. Bottom finish cutting is not done if no input. ( Except CHAMF ) : The side machining allowance for side finish cutting. Side finish cutting is not done if no input. ( Except S-FIN ) : The feed rate of the tool. : The machining allowance of one path in the XY direction. It is specified a rate (%) of the tool. ( less than 70% ) ( Except S-FIN ) : The cutting feed rate in Z axis direction from point R. (Point R = END POINT Z + REMOVAL DEPTH + CLEARANCE) ( Except HOLE ) : D code number of milling tool for rough machining. It needs to calculate the pre-hole position. ( For HOLE only )
ROUGH D-CODE
-219-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
CYCLE SELECT
: Select the drilling cycle for pre-hole from the following soft-keys. [G81 (Normal drilling)], [G83 (Peck drilling)]
PITCH DEPTH
: The depth of cut for each cutting cycle. It is used for G83 only. ( For HOLE only ) : The width of the groove.
( For HOLE only )
GROOVE WIDTH
By pushing [DETAIL], the following pop-up window is displayed. CONTOUR GROOVE (DETAIL) CLEARANCE CUT DIRECTION
CLEARANCE
CUT DIRECTION
L= 3.000 U= DOWNCT
: The amount of clearance for cutting feed in the Z axis at the approach or escape movement. The default data is 3mm. : Select the cutting direction from the following soft-keys. [DOWNCT (down-cut)], [UPCUT (up-cut)] Down-cut : Rotation of the cutting tool in the forward direction. Up-cut : Rotation of the cutting tool in the reverse direction.
-220-
www.teknikokul.net
B-63424EN/03
5. POCKETING
TYPES OF CYCLE MOTIONS
: Select the approach type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)] ( For S-FIN only )
APPROACH TYPE
Tangent Circle
Tangent Line
Vertical Line
: The radius and angle of tangent circle approach. ( For S-FIN and CIRCLE type )
APPROACH RADIUS / ANGLE
Angle Radius
: The distance of tangent line or vertical line approach. ( For S-FIN and TANGNT / VERTCL type )
APPROACH DIST.
Distance
Distance
Tangent Line
ESCAPE TYPE
Vertical Line
: Select the escape type from the following softkeys. [CIRCLE (Tangent Circle)], [TANGNT (Tangent Line)], [VERTCL (Vertical Line)] ( For S-FIN only )
Tangent Circle
-221-
www.teknikokul.net
Tangent Line
Vertical Line
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
: The radius and angle of tangent circle escape. ( For S-FIN and CIRCLE type )
ESCAPE RADIUS / ANGLE
Angle Radius
ESCAPE DIST.
: The distance of tangent line or vertical line escape. ( For S-FIN and TANGNT / VERTCL type ) Distance
Distance
Tangent Line
Vertical Line
After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G235 P L
Z B
J
-222-
www.teknikokul.net
H
D V F C E
• • • • ;
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
●
Definition of arbitrary shape Arbitrary shape is defined by using [CONTUR] of G code menu. In detail, refer to “II. OPERATION, 3.2.8 Contour”. After inputting the necessary data, by pushing INSERT, pop-up window is closed and inputted data are displayed in a program window as the following ISO code program.
G100 X Y ; G101 X Y M N L
K ;
G106 X Y P ;
NOTE 1) G235 is not worked independently. Therefore, after specified G235, be sure to specify the contour shape by using contour menu (G100 to G106). 2) By setting the parameter No.9127 to 235, the softkeys are automatically changed to contour shape.
-223-
www.teknikokul.net
5. POCKETING
TYPES OF CYCLE MOTIONS
B-63424EN/03
:
MOVEMENTS
Rapid Traverse (G00) Feed Traverse (G01, G02, G03)
Z
Removal Pitch
Point R
Clearance Removal Depth Bottom Finish
X
Y X
Side Finish Groove Width
A Cutting Width
a)
In the case of rough cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) by the pitch (REMOVAL PITCH). 4. Cutting to the opposite side of the starting point along the center line of the groove in cutting feed (FEED RATE). 5. Widening of the groove on the right and left sides symmetrically using the specified cutting width (CUTTING WIDTH). 6. The side finish cutting allowance (SIDE FINISH) and groove is cut. 7. Rise in cutting feed along Z axis up to point R 8. 3.-7. are repeated up to the point of the depth (BOTTOM FINISH) in Z axis. 9. Rise in cutting feed along Z axis up to point R.
b)
In the case of bottom finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent along the lower Z axis in cutting feed (Z-CUT FEED RATE) up to the end point (END POINT Z). 4. Cutting to the opposite side of the starting point along the center line of the groove in cutting feed (FEED RATE). 5. Widening of the groove on the right and left sides symmetrically using the specified cutting width (CUTTING WIDTH).
-224-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
6. 7.
5. POCKETING
The groove bottom side is cut leaving the side finish allowance (SIDE FINISH). Rise in cutting feed along Z axis up to point R
c)
In the case of side finish cutting 1. Rapid traverse up to the starting point (A). 2. Rapid traverse along the Z axis up to point R (END POINT Z + REMOVAL DEPTH + CLEARANCE) 3. Descent up to the end point (END POINT Z) along the lower Z axis in cutting feed (Z-CUT FEED RATE). 4. Cut into the workpiece in cutting feed following approach type (CIRCLE, TANGENT and VERTCL). 5. Groove side cutting with the side finish allowance (SIDE FINISH). 6. Move away from the workpiece following escape type (CIRCLE, TANGENT and VERTCL). 7. 3.-6. are repeated up to the point (END POINT Z) by the pitch (REMOVAL PITCH). 8. Rise in cutting feed along Z axis up to point R.
d)
In the case of drilling for pre-hole 1. Rapid traverse up to the starting point. 2. Rapid traverse along the lower Z axis up to the point R. 3. Drilling along Z axis up to the point Z (END POINT Z). 4. Rapid traverse along Z axis up to point R level (END POINT Z + REMOVAL DEPTH + CLEARANCE).
NOTE The alarm may occur owing to the restriction of contour figure number or work memory size for calculation. In this case, please divide the contour figure into some group.
-225-
www.teknikokul.net
6. OVERVIEW OF MEASURING CYCLES FUNCTION
6
TYPES OF CYCLE MOTIONS
B-63424EN/03
OVERVIEW OF MEASURING CYCLES FUNCTION When optional functions of CYCLE are added, clicking soft key [CYCLE] brings up the following cycle menu: This time, the soft-key [CARIB] and [MEASUR] were added newly. HOLE
PATTER
FACE
SIDE
POCKET
CARIB
MEASUR
RETURN
The general of the new menus are as follows. l l
CARIB
: Calibrating a spindle probe in order to ensure the length of probe, the size and center position of the stylus ball MEASURE : Measuring the size and position of work-piece and setting it to the work-piece origin offset number or macro variables
The following paragraphs describe the parameters and macro variables the user needs to set before using measurement cycles.
-226-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
6.1
6. OVERVIEW OF MEASURING CYCLES FUNCTION
PARAMETERS FOR MEASUREMENT The operator needs to set the common data for the measurement to the some macro variables. And it is possible to change the number of the variables by set the following parameter. 9150
MESRNO
FANUC setting MESRNO
800
Starting variable number of which is used to the measurement
NOTE If the above data is empty or zero, the alarm is occurred. This measuring cycles has the specifications to rotate prove at a special position, too. When the machine has the spindle orientation function, please set the following parameter to M code number for Spindle Orientation. 12050
SPNORM
SPNORM
M code number for Spindle Orientation
-227-
www.teknikokul.net
6. OVERVIEW OF MEASURING CYCLES FUNCTION
6.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
MACRO VARIABLE FOR CALIBRATION CYCLES The following variables are necessary to calibrate probe equipment. Executing the calibration cycles automatically sets the following macro variables. Therefore, in ordinary case, the operator needs not to set to the following variables. But, depending on circumstances, a probe might not always need to be calibrated precisely. Instead, experience value can be used. To calibrate using experience values, the operator needs to enter the values to the following variables.
●
# (MESRNO + 0) : Probe Length → Automatic set by G170
The length from the spindle gauge to the top of the stylus
● ● ● ●
# (MESRNO + 1) : Stylus Ball Diameter for X axis → Automatic set by G171 # (MESRNO + 2) : Stylus Ball Diameter for Y axis → Automatic set by G171 # (MESRNO + 3) : Stylus Ball Offset for X axis → Automatic set by G172, G173 # (MESRNO + 4) : Stylus Ball Offset for Y axis → Automatic set by G172, G173 The offset amounts between stylus ball center and spindle center
-228-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
6.3
6. OVERVIEW OF MEASURING CYCLES FUNCTION
MACRO VARIABLE FOR MEASURING CYCLES The following variables are necessary to control the movement of a probe. Please be sure to enter the data to them before using measuring cycles.
NOTE If the following data is empty or zero, the alarm is occurred. ● ●
# (MESRNO + 10) : Feed-rate for First Measurement (f) # (MESRNO + 11) : Approach Distance for First Measurement (α) # (MESRNO + 12) : Escaping Distance for First Measurement (β) = Approach Distance for Second Measurement # (MESRNO + 13) : Overlap Distance for Measurement (γ) # (MESRNO + 14) : Feed-rate for Approaching Start Point (fa) If the probe collide with work-piece with (fa), the alarm will occur and stop immediately. # (MESRNO + 15) : Escaping Distance for Second Measurement (ε)
●
● ●
●
1st Measure
2nd Measure
Measuring surface
Measuring start point
fa
f α
Measuring surface
Measuring start point
F γ
β
β
ε
-229-
www.teknikokul.net
γ
6. OVERVIEW OF MEASURING CYCLES FUNCTION
6.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
DISPLAY THE MEASUREMENT RESULT By setting the following parameters, Macro variables and the result for a measurement can be displayed on the user window. 9110
-
-
-
-
-
FANUC setting UWN MWN
0: 1: 0: 1:
UWN
EDTUSR
FANUC setting
6690
Macro program number of user window for editing operation screen
9113
MCHUSR
FANUC setting MCHUSR
MWN
00000011
User window is not available on the editing operation screen. User window is available on the editing operation screen. User window is not available on the machining operation screen. User window is available on the machining operation screen.
9111
EDTUSR
-
6690
Macro program number of user window for machining operation screen When the above parameters are set, the following soft-keys [USER] are displayed on the each screen.
INIT
TOOL
MSF
COMP
POSTIN
CONTR CYCLE TEACH
USER
RETURN
( Editing operation screen )
EXEC
O
N
SEARCH
SEARCH
REWIND
CHECK
USER
BGEDIT
RETURN
( Machining operation screen )
-230-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
6. OVERVIEW OF MEASURING CYCLES FUNCTION
By pushing the soft-key [USER], the following user window for setting data is displayed. The operator can set or refer to the data of macro variables for measurement on this window. MEASURING CYCLE - DATA SET PROBE LENGTH STYLUS BALL DIAMETER FOR X AXIS STYLUS BALL DIAMETER FOR Y AXIS STYLUS BALL OFFSET FOR X AXIS STYLUS BALL OFFSET FOR Y AXIS
= = = = =
MEASURING FEEDRATE OF 1ST APPROACH DISTANCE OF 1ST ESCAPING DISTANCE OF 1ST MEASURING OVERLAP DISTANCE APPROACH FEEDRATE TO START PT ESCAPE DISTANCE OF 2ND
= = = = = =
The soft-key [MEASURE RESULT] is displayed on the above screen. So, by pushing the soft-key [RESULT], the following user window for referring to the result of measurement is displayed. MEASURING CYCLE - RESULT X/Y/Z SINGLE SURFACE COD. (M) = COD. (W) = WEB WIDTH CNT X COD.(M) = CNT X COD.(W) = WIDTH = GROOVE WIDTH CNT X COD.(M) = CNT X COD.(W) = WIDTH = OUTSIDE CIRCLE CNT X COD.(M) = CNT X COD.(W) = RADIUS =
1/3
CNT Y COD.(M) = CNT Y COD.(W) =
CNT Y COD.(M) = CNT Y COD.(W) =
CNT Y COD.(M) = CNT Y COD.(W) =
By pushing MDI key âá, the next or previous window can be displayed. And by pushing the soft-key [DATA SET], the former window for setting data can be displayed.
-231-
www.teknikokul.net
6. OVERVIEW OF MEASURING CYCLES FUNCTION
TYPES OF CYCLE MOTIONS
MEASURING CYCLE - RESULT INSIDE CIRCLE CNT X COD.(M) = CNT X COD.(W) = RADIUS = OUTSIDE RECTANGULAR CNT X COD.(M) = CNT X COD.(W) = LENGTH X AXIS = INSIDE RECTANGULAR CNT X COD.(M) = CNT X COD.(W) = LENGTH X AXIS = OUTSIDE CORNER COR X COD.(M) = COR X COD.(W) =
2/3
CNT Y COD.(M) = CNT Y COD.(W) =
CNT Y COD.(M) = CNT Y COD.(W) = LENGTH Y AXIS = CNT Y COD.(M) = CNT Y COD.(W) = LENGTH Y AXIS = COR Y COD.(M) = COR Y COD.(W) =
MEASURING CYCLE - RESULT INSIDE CORNER COR X COD.(M) = COR X COD.(W) = BOLT HOLE CIRCLE CNT X COD.(M) = CNT X COD.(W) = RADIUS = 4-HOLES CENTER CNT X COD.(M) = CNT X COD.(W) = WORK PIECE ANGLE ANGLE = 2-HOLES ANGLE ANGLE =
B-63424EN/03
3/3
COR Y COD.(M) = COR Y COD.(W) = CNT Y COD.(M) = CNT Y COD.(W) =
CNT Y COD.(M) = CNT Y COD.(W) =
NOTE (M) and (W) of the result means Machine coordinate system and Work-piece coordinate system.
-232-
www.teknikokul.net
B-63424EN/03
7
TYPES OF CYCLE MOTIONS
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
CALIBRATION CYCLES (OPTIONAL FUNCTION) By pushing the soft-key [CARIB], the following menus soft-keys are displayed. PROBE
DIA.
OFFSET
OFFSET
A
B
RETURN
These calibration cycles measure and calculate the correct data for a probe by using the ring gauge, and output them to some macro variables. The measuring cycles do a measurement by using them. Calibration Cycles do a measurement two times per one measuring point. One is for confirming the position of a measuring point, the other is for measuring the correct position that was confirmed by first measurement. The following description applies when soft key WINDOW is valid. When WINDOW is invalid, the argument address equivalent to the item of each menu is automatically displayed. If there is nothing to enter, just press the INPUT key. The data will be invalidated, displaying the next argument address. Repeat this operation. To have the block accepted (to have it stored in CNC memory), press the INSERT key.
-233-
www.teknikokul.net
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
7.1
TYPES OF CYCLE MOTIONS
B-63424EN/03
PROBE LENGTH CALIBRATION (G170) This is a menu for calibrating a probe length. By pushing the soft-key [PROBE], the following pop-up window is displayed. PROBE LENGTH DISTANCE FOR MOV DIST. GAUGE-TABLE RING GAUGE HEIGHT FEEDRATE FOR MOV
1/1 Z= D= H= F=
: Input the distance from the measuring start point to the ring gauge. DIST. GAUGE : Input the distance from the spindle gauge line to -TABLE the machine table. RING GAUGE : Input the height of the ring gauge. DISTANCE FOR MOV
HEIGHT FEEDRATE FOR MOV MOVEMENTS
: Input the feed-rate for movement on measuring. : The movement on the calibration is as follows 1st Measure 2nd Measure
Probe
Probe length
Measuring start point
D
Z
Z γ
β
Measuring surface
H
Ring gauge
1. 2.
3.
At first, please set the ring gauge on the machine table and move the probe right over the ring gauge. When this cycle is executed, it does a measurement from start point within the distance (Z + γ) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with a rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement
-234-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G170 Z D H F ; When G170 is executed, the system will calculate the length of the probe from measurement position and output it to the following variable. •
# (MESRNO + 0) : Probe Length
-235-
www.teknikokul.net
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
7.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
STYLUS BALL DIAMETER CALIBRATION (G171) This is a menu for calibrating the diameter of a stylus ball for X axis and Y axis. By pushing the soft-key [DIA.], the following pop-up window is displayed. STYLUS BALL DIAMETER DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV
DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV MOVEMENTS
1/1
Z= R= F=
: Input the distance from the measuring start point to the ring gauge. : Input the radius of the ring gauge. : Input the feed-rate for movement on measuring. : The movement on the calibration is as follows Ring gauge
α
γ
R
Probe
1st Measure Measuring start point Ring gauge
2nd Measure
Z
β
-236-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
1. 2.
3. 4.
5.
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
At first, please set the ring gauge on the machine table and move the probe right over the ring gauge. When this cycle is executed, the probe moves the distance (Z) along the –Z axis with feed-rate (fa). After that, it moves the distance (R - α) with feed-rate (fa) and does a measurement from the point within the distance (R + γ) with the feed-rate (f). → First measurement Next, the probe returns the measuring start point and does a measurement as the same one in the direction –X axis and ±Y axis. After the first measurement, the probe moves the point (1st measuring position - β) with feed-rate (fa), and do a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement The probe does a measurement as the same one in the direction – X axis and ±Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G171 Z R F ; When G171 is executed, the system will calculate the diameter of the stylus ball for X, Y axis from measurement position and output it to the following variables. • •
# (MESRNO + 1) : Stylus Ball Diameter for X axis # (MESRNO + 2) : Stylus Ball Diameter for Y axis
-237-
www.teknikokul.net
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
7.3
TYPES OF CYCLE MOTIONS
B-63424EN/03
STYLUS X AND Y OFFSETS CALIBRATION- A (G172) This is a menu for calibrating X and Y offset of a stylus ball. By pushing the soft-key [OFFSET], the following pop-up window is displayed. STYLUS X/Y OFFSETS – A DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV
DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV MOVEMENTS
1/1
Z= R= F=
: Input the distance from the measuring start point to the ring gauge. : Input the radius of the ring gauge. : Input the feed-rate for movement on measuring. : The movement on the calibration is as follows Ring gauge
R
Probe Measuring start point Ring gauge
Stylus radius α γ
1st Measure 2nd Measure
Z
β
-238-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
1. 2.
3. 4.
5. 6.
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
At first, please set the ring gauge on the machine table and move the probe right over the ring gauge. When this cycle is executed, the probe moves the distance (Z) along the –Z axis with feed-rate (fa). After that, it moves the distance (R - α - stylus radius) with feed-rate (fa) and does a measurement from the point within the distance (R + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the measuring start point and does a measurement as the same one in the direction –X axis and ±Y axis. After the first measurement, the probe moves the point (1st measuring position - β) with feed-rate (fa), and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement The probe does a measurement as the same one in the direction – X axis and ±Y axis. After executing 180° Spindle Orientation, the probe does a measurement as the same one in the direction –X axis and ±Y axis again.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G172 Z R F ; When G172 is executed, the system will calculate the stylus ball offset for X, Y axis from measurement position and output it to the following variables. • •
# (MESRNO + 3) : Stylus Ball Offset for X axis # (MESRNO + 4) : Stylus Ball Offset for Y axis
-239-
www.teknikokul.net
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
7.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
STYLUS X AND Y OFFSETS CALIBRATION- B (G173) This is a menu for calibrating X and Y offset of a stylus ball. By pushing the soft-key [OFFSET], the following pop-up window is displayed. STYLUS X/Y OFFSETS – B CENTER POINT X CENTER POINT Y DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV
CENTER POINT X / Y DISTANCE FOR MOV RING GAUGE RADIUS FEEDRATE FOR MOV MOVEMENTS
1. 2.
3. 4.
5.
1/1
Y= Y= Z= R= F=
: Input the X and Y coordinate of center of the ring gauge. : Input the distance from the measuring start point to the ring gauge. : Input the radius of the ring gauge. : Input the feed-rate for movement on measuring. : The movement on the calibration is as follows
At first, please set the ring gauge on the machine table and move the probe right over the ring gauge. When this cycle is executed, the probe moves the distance (Z) along the –Z axis with feed-rate (fa). After that, it moves the distance (R - α - stylus radius) with feed-rate (fa) and does a measurement from the point within the distance (R + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the measuring start point and does a measurement as the same one in the direction –X axis and ±Y axis. After the first measurement, the probe moves the point (1st measuring position - β) with feed-rate (fa), and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement The probe does a measurement as the same one in the direction – X axis and ±Y axis.
-240-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
7. CALIBRATION CYCLES (OPTIONAL FUNCYION)
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G173 X Y Z R F ; When G173 is executed, the system will calculate the stylus ball offset for X, Y axis from measurement position and output it to the following variables. • •
# (MESRNO + 1) : Stylus Ball Diameter for X axis # (MESRNO + 2) : Stylus Ball Diameter for Y axis
-241-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8
TYPES OF CYCLE MOTIONS
MEASURING FUNCTION)
B-63424EN/03
CYCLES
(OPTIONAL
By pushing the soft-key [MEASURE], the following menus soft-keys are displayed. FACE
WEB
GROOVE
4-HOLE
ANGLE
ANGLE
CIRCLE CIRCLE
RECT
RECT
CORNER
3-HOLE
RETURN
RETURN
+
Measuring Cycles do a measurement two times per one measuring point. One is for confirming the position of a measuring point, the other is for measuring the correct position that was confirmed by first measurement. These cycles measure the position and size of work-piece and output them to the work-piece origin offset value and macro variables.
NOTE 1) Please be sure to execute the calibration cycles before using the measuring cycles. 2) Please be sure to move the probe to the measuring start point before executing the measuring cycles.
-242-
www.teknikokul.net
B-63424EN/03
8.1
TYPES OF CYCLE MOTIONS
8. MEASURING CYCLES (OPTIONAL FUNCYION)
X/Y/Z SINGLE SURFACE MEASUREMENT (G180) This is a menu for measuring a single surface for X, Y and Z axis. By pushing the soft-key [FACE], the following pop-up window is displayed. X/Y/Z SINGLE SURFACE MEASURE POSITION WORK CO-ORD. VALU DISTANCE FOR MOV FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1
A= V= D= F= W=
: Select the single surface from the following softkeys. [X AXIS], [Y AXIS], [Z-AXIS] : Input the work-piece origin offset value which would like to set.
MEASURE POSITION WORK COORD. VALUE DISTANCE FOR MOV
: Input the distance from the measuring start point to the single surface. In the case of X or Y axis, + and - represents the direction. The other hand, in Z axis, - only is allowed. : Input the feed-rate for movement on measuring.
FEEDRATE FOR MOV WORK COORD. SYST.
: Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
MOVEMENTS
: The movement on the measurement is as follows
-243-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
•
B-63424EN/03
X and Y single surface 1st Measure 2nd Measure
Measuring start point
1. 2.
3.
•
D
β
γ
Measuring surface
At first, please move the probe to the measuring start point. When this cycle is executed, it does a measurement from start point within the distance (D + γ) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with a rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement Z single surface 1st Measure Measuring start point
D γ
1. 2.
3.
2nd Measure
β Measuring surface
At first, please move the probe to the measuring start point. When this cycle is executed, it does a measurement from start point within the distance (D + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the position (1st measuring point + β) with a rapid traverse and does a measurement from the position to the position (1st measuring point - γ) with the feed-rate (F). → Second measurement
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G180 A V D F W ;
-244-
www.teknikokul.net
TYPES OF CYCLE MOTIONS
B-63424EN/03
8. MEASURING CYCLES (OPTIONAL FUNCYION)
When G180 is executed, the system will output a measurement position to the work-piece origin offset value and the following variables. • •
# (MESRNO + 50) : Single surface position (Machine coordinate system) # (MESRNO + 51) : Single surface position (Work-piece coordinate system)
-245-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.2
TYPES OF CYCLE MOTIONS
B-63424EN/03
WEB WIDTH MEASUREMENT (G181) This is a menu for measuring the center position and width of a web By pushing the soft-key [WEB], the following pop-up window is displayed. WEB WIDTH
1/1
HEIGHT FOR Z AXIS MEASURE DIRECTION WEB WIDTH FEEDRATE FOR MOV WORK CO-ORD. SYST.
Z= D= V= F= W=
MEASURE POSITION
: Select the single surface from the following softkeys. [X AXIS], [Y AXIS], [Z-AXIS]
HEIGHT FOR Z AXIS
: Input the height from the measuring start point to the point which will be measured. : Select the measuring direction from the following soft-keys. [X AXIS], [Y AXIS] : Input the approximate width of the web. : Input the feed-rate for movement on measuring.
MEASURE DIRECTION WEB WIDTH FEEDRATE FOR MOV WORK CO-ORD. SYST.
: Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-246-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows
Measuring start point
β 2nd Measure
Z
1st Measure γ
α
D Stylus radius
1. 2.
3.
4.
At first, please move the probe right over the web center. When this cycle is executed, the probe moves the distance (V/2 + α + stylus radius) along the X or Y axis with feed-rate (fa). After that, it moves the distance (Z) along –Z axis with feed-rate (fa), and does a measurement from the point within the distance (V/2 γ + stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse, and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement After that, the probe does a measurement as the same one in the direction –X axis and –Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G181 Z D V F W ; When G181 is executed, the system will calculate the center position and width of the web from measurement position and output it to the work-piece origin offset value and the following variables. • • • • •
# (MESRNO + 50) : X coordinate of web center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of web center (Machine coordinate system) # (MESRNO + 52) : X coordinate of web center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of web center (Work-piece coordinate system) # (MESRNO + 54) : Width of web
-247-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.3
TYPES OF CYCLE MOTIONS
B-63424EN/03
GROOVE WIDTH MEASUREMENT (G182) This is a menu for measuring the center position and width of a groove. By pushing the soft-key [GROOVE], the following pop-up window is displayed. GROOVE WIDTH HEIGHT FOR Z AXIS MEASURE DIRECTION GROOVE WIDTH FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS MEASURE DIRECTION GROOVE WIDTH FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1 Z= D= V= F= W=
: Input the height from the measuring start point to the point which will be measured. : Select the measuring direction from the following soft-keys. [X AXIS], [Y AXIS] : Input the approximate width of the groove. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-248-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows
Measuring start point
β 2nd Measure
Z
1st Measure
α γ D
1. 2.
3.
4.
Stylus radius
At first, please move the probe right over the groove center. When this cycle is executed, the probe moves the distance (Z) along –Z axis with feed-rate (fa), and moves the distance (V/2 + α + stylus radius) along the X or Y axis with feed-rate (fa). After that, and does a measurement from the point within the distance (V/2 + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse, and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement After that, the probe does a measurement as the same one in the direction –X axis and –Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G182 Z D V F W ; When G182 is executed, the system will calculate the center position and width of groove from measurement position and output it to the work-piece origin offset value and the following variables. • • • • •
# (MESRNO + 50) : X coordinate of groove center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of groove center (Machine coordinate system) # (MESRNO + 52) : X coordinate of groove center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of groove center (Work-piece coordinate system) # (MESRNO + 54) : Groove of web
-249-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.4
TYPES OF CYCLE MOTIONS
B-63424EN/03
OUTSIDE CIRCLE MEASUREMENT (G183) This is a menu for measuring the center position and radius of an outside circle. By pushing the soft-key [CIRCLE], the following pop-up window is displayed. OUTSIDE CIRCLE HEIGHT FOR Z AXIS OUTSIDE RADIUS FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS OUTSIDE RADIUS FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1 Z= R= F= W=
: Input the height from the measuring start point to the point which will be measured. : Input the approximate radius of the outside circle. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-250-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows Stylus radius γ α
Measuring start point R
1st Measure
Z
2nd Measure
β
1. 2.
3. 4. 5.
6. 7.
At first, please move the probe right over the center of outside circle. When this cycle is executed, the probe moves the distance (R + α + stylus radius) along the X axis with feed-rate (fa). After that, it moves the distance (Z) along –Z axis with feed-rate (fa), and does a measurement from the point within the distance (R - γ + stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (ε) and returns the measuring start point with rapid traverse. The probe does a measurement as the same one in the direction – X axis and ±Y axis. After the first measurement, the probe moves to the position (1st measuring position - β) along the X axis with feed-rate (fa) and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement Next, the probe returns the distance (ε) and returns the measuring start point with rapid traverse The probe does a measurement as the same one in the direction – X axis and ±Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G183 Z R F W ;
-251-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
When G183 is executed, the system will calculate the center position and radius of circle from measurement position and output it to the work-piece origin offset value and the following variables. • • • • •
# (MESRNO + 50) : X coordinate of circle center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of circle center (Machine coordinate system) # (MESRNO + 52) : X coordinate of circle center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of circle center (Work-piece coordinate system) # (MESRNO + 54) : Radius of circle
-252-
www.teknikokul.net
B-63424EN/03
8.5
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
OUTSIDE CIRCLE MEASUREMENT (G183) This is a menu for measuring the center position and radius of an inside circle. By pushing the soft-key [CIRCLE], the following pop-up window is displayed. INSIDE CIRCLE
1/1
HEIGHT FOR Z AXIS INSIDE RADIUS FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS INSIDE RADIUS FEEDRATE FOR MOV WORK CO-ORD. SYST.
Z= D= F= W=
: Input the height from the measuring start point to the point which will be measured. : Input the approximate radius of the inside circle. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-253-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: The movement on the measurement is as follows Stylus radius
α
Measuring start point
γ
R
Z
1st Measure 2nd Measure
β
1. 2.
3. 4.
5.
At first, please move the probe right over the center of inside circle. When this cycle is executed, the probe moves the distance (Z) along the –Z axis with feed-rate (fa), and moves the distance (R α - stylus radius) along the +X axis with feed-rate (fa). After that, it does a measurement from the point within the distance (R + γ stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the measuring start point with rapid traverse. The probe does a measurement as the same one in the direction –X axis and ±Y axis. After the first measurement, the probe moves to the position (1st measuring position - β) along the +X axis with feed-rate (fa) and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement Next, the probe does a measurement as the same one in the direction –X axis and ±Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G184 Z R F W ;
-254-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
8. MEASURING CYCLES (OPTIONAL FUNCYION)
When G184 is executed, the system will calculate the center position and radius of circle from measurement position and output it to the work-piece origin offset value and the following variables. • • • • •
# (MESRNO + 50) : X coordinate of circle center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of circle center (Machine coordinate system) # (MESRNO + 52) : X coordinate of circle center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of circle center (Work-piece coordinate system) # (MESRNO + 54) : Radius of circle
-255-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.6
TYPES OF CYCLE MOTIONS
B-63424EN/03
OUTSIDE RECTANGULAR MEASUREMENT (G185) This is a menu for measuring the center position and length of an outside rectangular. By pushing the soft-key [RECT.], the following pop-up window is displayed. OUTSIDE RECTANGULAR HEIGHT FOR Z AXIS LENGTH FOR X AXIS LENGTH FOR Y AXIS FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS HEIGHT FOR Z AXIS LENGTH FOR X AXIS LENGTH FOR Y AXIS FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1
Z= U= V= F= W=
: Input the height from the measuring start point to the point which will be measured. : Input the height from the measuring start point to the point which will be measured. : Input the approximate length of outside rectangular for X axis. : Input the approximate length of outside rectangular for Y axis. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-256-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
: The movement on the measurement is as follows
MOVEMENTS
Stylus radius Measuring start point
γ α 1st Measure
Z
V 2nd Measure
β U
1. 2.
3.
4. 5.
At first, please move the probe right over the center of outside rectangular. When this cycle is executed, the probe moves the distance (U/2 + α + stylus radius) along the X axis with feed-rate (fa). After that, it moves the distance (Z) along –Z axis with feed-rate (fa), and does a measurement from the point within the distance (U/2 - γ + stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement After the second measurement, the probe returns the distance (ε) and returns the measuring start point with rapid traverse. After that, the probe does a measurement as the same one in the direction –X axis and ±Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G185 Z U V F W ;
-257-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
When G185 is executed, the system will calculate the center position and length of rectangular from measurement position and output it to the work-piece origin offset value and the following variables. • • • • • •
# (MESRNO + 50) : X coordinate of rectangular center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of rectangular center (Machine coordinate system) # (MESRNO + 52) : X coordinate of rectangular center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of rectangular center (Work-piece coordinate system) # (MESRNO + 54) : Length of rectangular for X axis # (MESRNO + 55) : Length of rectangular for Y axis
-258-
www.teknikokul.net
B-63424EN/03
8.7
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
INSIDE RECTANGULAR MEASUREMENT (G186) This is a menu for measuring the center position and length of an inside rectangular By pushing the soft-key [RECT.], the following pop-up window is displayed. INSIDE RECTANGULAR HEIGHT FOR Z AXIS LENGTH FOR X AXIS LENGTH FOR Y AXIS FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS LENGTH FOR X AXIS LENGTH FOR Y AXIS FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1
Z= U= V= F= W=
: Input the height from the measuring start point to the point which will be measured. : Input the approximate length of inside rectangular for X axis. : Input the approximate length of inside rectangular for Y axis. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-259-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
: The movement on the measurement is as follows
MOVEMENTS
Stylus radius
α γ
Measuring start point
Z
V
1st Measure 2nd Measure
β U
1. 2.
3.
4.
At first, please move the probe right over the center of inside rectangular. When this cycle is executed, the probe moves the distance (Z) along –Z axis with feed-rate (fa) and moves the distance (U/2 - α stylus radius) along the X axis with feed-rate (fa). After that, it does a measurement from the point within the distance (U/2 + γ stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement After the second measurement, the probe returns to the measuring start point with rapid traverse, and it does a measurement as the same one in the direction –X axis and ±Y axis.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G186 Z U V F W ;
-260-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
8. MEASURING CYCLES (OPTIONAL FUNCYION)
When G186 is executed, the system will calculate the center position and length of rectangular from measurement position and output it to the work-piece origin offset value and the following variables. • • • • • •
# (MESRNO + 50) : X coordinate of rectangular center (Machine coordinate system) # (MESRNO + 51) : Y coordinate of rectangular center (Machine coordinate system) # (MESRNO + 52) : X coordinate of rectangular center (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of rectangular center (Work-piece coordinate system) # (MESRNO + 54) : Length of rectangular for X axis # (MESRNO + 55) : Length of rectangular for Y axis
-261-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.8
TYPES OF CYCLE MOTIONS
B-63424EN/03
OUTSIDE CORNER MEASUREMENT (G187) This is a menu for measuring an outside corner position. By pushing the soft-key [CORNER], the following pop-up window is displayed. OUTSIDE CORNER
1/2
1ST MEASURE POINT X 1ST MEASURE POINT Y 3RD MEASURE POINT X 3RD MEASURE POINT Y DISTANCE FOR X AXIS
A= B= C= D= U=
DISTANCE FOR Y AXIS
V=
INCREMENT FOR X AXIS INCREMENT FOR Y AXIS
I= J=
1ST MEASURE POINT X / Y 3RD MEASURE POINT X / Y DISTANCE FOR X AXIS DISTANCE FOR Y AXIS INCREMENT FOR X AXIS INCREMENT FOR Y AXIS FEEDRATE FOR MOV WORK CO-ORD. SYST.
OUTSIDE CORNER FEEDRATE FOR MOV WORK CO-ORD. SYST.
2/2 F= W=
: Input the approximate X and Y coordinate of 1st measuring point. : Input the approximate X and Y coordinate of 3rd measuring point. : Input the distance from measuring start point to single surface of X axis. : Input the distance from measuring start point to single surface of Y axis. : Input the increment from 1st point from 2nd point for X axis. : Input the increment from 3rd point from 4th point for Y axis. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-262-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows
V
4 J
3 (C,D) 1 (A,B) I
2 U
Measuring start point
1. 2.
3.
4. 5.
At first, please move the probe to the measuring start point. When this cycle is executed, the probe moves the distance (U - α stylus radius) with feed-rate (fa), and it does a measurement from the point within the distance (U + γ - stylus radius) with the feedrate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement After the second measurement, the probe returns the distance (ε) with rapid traverse. The probe does a measurement as the same one in the 2nd, 3rd and 4th measuring point.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G187 A B C D U I J F W ; When G187 is executed, the system will calculate the corner position from measurement position and output it to the work-piece origin offset value and the following variables. • • • •
# (MESRNO + 50) : X coordinate of corner (Machine coordinate system) # (MESRNO + 51) : Y coordinate of corner (Machine coordinate system) # (MESRNO + 52) : X coordinate of corner (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of corner (Work-piece coordinate system) -263-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.9
TYPES OF CYCLE MOTIONS
B-63424EN/03
INSIDE CORNER MEASUREMENT (G188) This is a menu for measuring an inside corner position By pushing the soft-key [CORNER], the following pop-up window is displayed. INSIDE CORNER CORNER POSITION 1ST MEASURE POINT X 1ST MEASURE POINT Y DISTANCE FOR X AXIS DISTANCE FOR Y AXIS INCREASE FOR X AXIS INCREASE FOR Y AXIS FEEDRATE FOR MOV
1/2 C= A= B= U= V= I= J= F=
INSIDE CORNER WORK CO-ORD. SYST.
2/2 W=
: Select the corner position from the following softkeys. [1], [2], [3], [4] 1ST MEASURE : Input the approximate X and Y coordinate of 1st POINT X / Y measuring point. DISTANCE : Input the distance from measuring start point to FOR X AXIS single surface of X axis. DISTANCE : Input the distance from measuring start point to FOR Y AXIS single surface of Y axis. INCREASE : Input the increment from 1st point from 2nd point FOR X AXIS for X axis. INCREASE : Input the increment from 3rd point from 4th point FOR Y AXIS for Y axis. FEEDRATE : Input the feed-rate for movement on measuring. CORNER POSITION
FOR MOV WORK CO-ORD. SYST.
: Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-264-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows V
4
Measuring start point
J
3
I U
1 (A,B)
1. 2.
3.
4.
2
At first, please move the probe to the measuring start point. When this cycle is executed, the probe moves the distance (U + α + stylus radius) with feed-rate (fa), and it does a measurement from the point within the distance (U - γ + stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the distance (β) with rapid traverse and does a measurement from the position within the distance (β + γ) with the feed-rate (F). → Second measurement The probe does a measurement as the same one in the 2nd, 3rd and 4th measuring point.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G188 C A B U V I J F W ; When G188 is executed, the system will calculate the corner position from measurement position and output it to the work-piece origin offset value and the following variables. • • • •
# (MESRNO + 50) : X coordinate of corner (Machine coordinate system) # (MESRNO + 51) : Y coordinate of corner (Machine coordinate system) # (MESRNO + 52) : X coordinate of corner (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of corner (Work-piece coordinate system)
-265-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.10
TYPES OF CYCLE MOTIONS
B-63424EN/03
BOLT-HOLE-CIRCLE MEASUREMENT (G189) This is a menu for measuring a center position and radius of a bolthole-circle by using 3 holes. By pushing the soft-key [3 HOLE], the following pop-up window is displayed. BOLT HOLE CIRCLE HEIGHT FOR Z AXIS RADIUS HOLE NOMINAL DIA. 1ST HOLE ANGLE 2ND HOLE ANGLE 3RD HOLE ANGLE FEEDRATE FOR MOV WORK CO-ORD. SYST.
HEIGHT FOR Z AXIS RADIUS HOLE NOMINAL DIA. 1ST / 2ND / 3RD HOLE ANGLE FEEDRATE FOR MOV WORK CO-ORD. SYST.
1/1 Z= R= D= A= B= C= F= W=
: Input the height from the measuring start point to the point which will be measured. : Input the approximate radius of the bolt-holecircle. : Input the nominal diameter of the hole. : Input the angle of each hole center position from X axis. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-266-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
MOVEMENTS
: The movement on the measurement is as follows
1st Hole
Measuring start point B
2nd Hole
Z
A
D R
C 3rd Hole
1. 2. 3.
4. 5.
6. 7. 8.
At first, please move the probe right over the approximate center position of a bolt-hole-circle. When this cycle is executed, the probe moves to the center position of the 1st measuring hole with feed-rate (fa), and it moves the distance (Z) along –Z axis with feed-rate (fa). After that, the probe moves the distance (D/2 - α - stylus radius) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (D/2 + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the center position of the hole with rapid traverse, and it does a measurement as the same one in the –X axis and ±Y axis. After the first measurement, the probe moves to the position (1st measuring position - β) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (β + γ) with the feed-rate (f). → Second measurement The probe does a measurement as the same one in the –X axis and ±Y axis, and find the correct center position of 1st hole. The probe does a measurement as the same one in the 2nd hole and finds the correct center position of it. The probe does a measurement as the same one in the 3rd hole and finds the correct center position of it
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G189 Z R D A B C F W ;
-267-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
B-63424EN/03
When G189 is executed, the system will calculate the center position of Bolt-Hole-Circle from measurement position and output it to the work-piece origin offset value and the following variables. • • • • •
# (MESRNO + 50) : X coordinate of Bolt-Hole-Circle (Machine coordinate system) # (MESRNO + 51) : Y coordinate of Bolt-Hole-Circle (Machine coordinate system) # (MESRNO + 52) : X coordinate of Bolt-Hole-Circle (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of Bolt-Hole-Circle (Work-piece coordinate system) # (MESRNO + 54) : Radius of Bolt-Hole-Circle
-268-
www.teknikokul.net
B-63424EN/03
8.11
TYPES OF CYCLE MOTIONS
8. MEASURING CYCLES (OPTIONAL FUNCYION)
4- HOLES CENTER MEASUREMENT (G190) This is a menu for measuring a center position and radius of 4 holes. By pushing the soft-key [4-HOLE], the following pop-up window is displayed. 4 HOLES CENTER HEIGHT FOR Z AXIS HOLE NOMINAL DIA. 1ST HOLE POINT X 1ST HOLE POINT Y 2ND HOLE POINT X 2ND HOLE POINT Y 3RD HOLE POINT X 3RD HOLE POINT Y
1/2 Z= D= A= B= C= E= H= I=
4 HOLES CENTER 4TH HOLE POINT X 4TH HOLE POINT Y FEEDRATE FOR MOV WORK CO-ORD. SYST.
2/2 J= K= F= W=
MOVEMENTS
: The movement on the measurement is as follows
HEIGHT FOR Z AXIS
: Input the height from the measuring start point to the point which will be measured. : Input the nominal diameter of the hole.
HOLE NOMINAL DIA. 1ST HOLE POINT X / Y 2ND HOLE POINT X / Y 3RD HOLE POINT X / Y 4TH HOLE POINT X / Y FEEDRATE FOR MOV WORK CO-ORD. SYST.
: Input the approximate X and Y coordinate of 1st measuring hole center. : Input the approximate X and Y coordinate of 2nd measuring hole center. : Input the approximate X and Y coordinate of 3rd measuring hole center. : Input the approximate X and Y coordinate of 4th measuring hole center. : Input the feed-rate for movement on measuring. : Select the work-piece coordinate system from the soft-keys. [G54],[G55],[G56],[G57],[G58],[G59] If Work-piece Coordinate System 48-pairs is available, input the number which will be set as follows. G54.1P1 ↔ P48 : 1001 ↔ 1048
-269-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
TYPES OF CYCLE MOTIONS
MOVEMENTS
B-63424EN/03
: The movement on the measurement is as follows
Measuring start point
Z
4th Hole
3rd Hole
(J,K)
(H,I)
st
2nd Hole
1 Hole
D (A,B)
1. 2. 3.
4. 5.
6. 7. 8. 9.
(C,E)
At first, please move the probe over the center position of the 1st measuring hole. When this cycle is executed, the probe moves to the center position of the 1st measuring hole with feed-rate (fa), and it moves the distance (Z) along –Z axis with feed-rate (fa). After that, the probe moves the distance (D/2 - α - stylus radius) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (D/2 + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the center position of the hole with rapid traverse, and it does a measurement as the same one in the –X axis and ±Y axis. After the first measurement, the probe moves to the position (1st measuring position - β) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (β + γ) with the feed-rate (f). → Second measurement The probe does a measurement as the same one in the –X axis and ±Y axis, and find the correct center position of 1st hole. The probe does a measurement as the same one in the 2nd hole and finds the correct center position of it. The probe does a measurement as the same one in the 3rd hole and finds the correct center position of it. The probe does a measurement as the same one in the 4th hole and finds the correct center position of it.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G190 Z D A B C E H I J K F W ;
-270-
www.teknikokul.net
B-63424EN/03
TYPES OF CYCLE MOTIONS
8. MEASURING CYCLES (OPTIONAL FUNCYION)
When G190 is executed, the system will calculate the center position of 4-Hole from measurement position and output it to the work-piece origin offset value and the following variables. • • • •
# (MESRNO + 50) : X coordinate of 4-Hole (Machine coordinate system) # (MESRNO + 51) : Y coordinate of 4-Hole (Machine coordinate system) # (MESRNO + 52) : X coordinate of 4-Hole (Work-piece coordinate system) # (MESRNO + 53) : Y coordinate of 4-Hole (Work-piece coordinate system)
-271-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.12
TYPES OF CYCLE MOTIONS
B-63424EN/03
WORK PIECE ANGLE MEASUREMENT (G191) This is a menu for measuring an inclined angle of single surface in the work-piece. By pushing the soft-key [ANGLE], the following pop-up window is displayed. WORK PIECE ANGLE
1/1
1ST MEASURE POINT X 1ST MEASURE POINT Y 2ND MEASURE POINT X 2ND MEASURE POINT Y DISTANCE FOR MOV PROBE AXIS FOR MOV FEEDRATE FOR MOV
1ST MEASURE POINT X / Y 2ND MEASURE POINT X / Y DISTANCE FOR MOV PROBE AXIS FOR MOV FEEDRATE FOR MOV MOVEMENTS
A= B= C= I= D= J= F=
: Input the approximate X and Y coordinate of 1st measuring point. : Input the approximate X and Y coordinate of 2nd measuring point. : Input the distance from the measuring start point to the single surface. : Select the probe moving axis and direction from the following the soft-keys. [+X], [-X], [+Y], [-Y] : Input the feed-rate for movement on measuring. : The movement on the measurement is as follows
Y (C,I) (A,B)
2
1
Measuring start point
-272-
www.teknikokul.net
J D
X
TYPES OF CYCLE MOTIONS
B-63424EN/03
1. 2.
3. 4.
8. MEASURING CYCLES (OPTIONAL FUNCYION)
At first, please move the probe to the 1st measuring point. When this cycle is executed, the probe moves the distance (D - α stylus radius) with feed-rate (fa), and it does a measurement from the point within the distance (D + γ - stylus radius) with the feedrate (f). → First measurement After the 1st measurement, the probe returns the distance (ε) with rapid traverse, and it does a measurement from the point within the distance (β + γ) with the feed-rate (f). → Second measurement The probe does a measurement as the same one in the second measuring point.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G191 A B C I D J F ; When G191 is executed, the system will calculate the angle of X axis from measurement position and output it to the following variables. •
# (MESRNO + 50) : Angle between X-axis and Workpiece
-273-
www.teknikokul.net
8. MEASURING CYCLES (OPTIONAL FUNCYION)
8.13
TYPES OF CYCLE MOTIONS
B-63424EN/03
2-HOLES ANGLE MEASUREMENT (G192) This is a menu for measuring an inclined angle of 2 holes center line. By pushing the soft-key [ANGLE], the following pop-up window is displayed. 2 HOLES ANGLE HEIGHT FOR Z AXIS HOLE NOMINAL DIA. 1ST MEASURE POINT X 1ST MEASURE POINT Y 2ND MEASURE POINT X 2ND MEASURE POINT Y I= FEEDRATE FOR MOV F=
1/1 Z= D= A= B= C=
: Input the height from the measuring start point to the point which will be measured. HOLE NOMINAL : Input the nominal diameter of the hole. HEIGHT FOR Z AXIS
DIA. 1ST MEASURE POINT X / Y
2ND MEASURE POINT X / Y FEEDRATE FOR MOV MOVEMENTS
: Input the approximate X and Y coordinate of 1st measuring hole center. : Input the approximate X and Y coordinate of 2nd measuring hole center. : Input the feed-rate for movement on measuring. : The movement on the measurement is as follows
Measuring start point
Y 2nd Hole
D
1st Hole
Z
(C,I)
(A,B)
-274-
www.teknikokul.net
X
TYPES OF CYCLE MOTIONS
B-63424EN/03
1. 2. 3.
4. 5.
6. 7.
8. MEASURING CYCLES (OPTIONAL FUNCYION)
At first, please move the probe over the center position of the 1st measuring hole. When this cycle is executed, the probe moves to the center position of the 1st measuring hole with feed-rate (fa), and it moves the distance (Z) along –Z axis with feed-rate (fa). After that, the probe moves the distance (D/2 - α - stylus radius) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (D/2 + γ - stylus radius) with the feed-rate (f). → First measurement Next, the probe returns the center position of the hole with rapid traverse, and it does a measurement as the same one in the –X axis and ±Y axis. After the first measurement, the probe moves to the position (1st measuring position - β) along +X axis with feed-rate (fa), and it does a measurement from the point within the distance (β + γ) with the feed-rate (f). → Second measurement The probe does a measurement as the same one in the –X axis and ±Y axis, and find the correct center position of 1st hole. The probe does a measurement as the same one in the 2nd hole and finds the correct center position of it.
After inputting the necessary data, by pushing INSERT, a pop-up windows is closed and inputted data are displayed in a program window as the following ISO code program.
G192 Z D A B C I F ; When G192 is executed, the system will calculate the angle of X axis from measurement position and output it to the following variables. •
# (MESRNO + 50) : Angle between X-axis and Line through 2-Hole center
-275-
www.teknikokul.net
IV. SAMPLE OF PROGRAMMING
www.teknikokul.net
B-63424EN/03
1
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
EXAMPLE OF INPUTTING PROGRAM !
WARNING
The following example of entering data is intend only to illustrate how to operate to make a program. The inputting data given in the example may not be able to used in actual machining. If the machine is forced to run according to a program like the one shown above, the tool may bump against the work-piece, and the machine may be forced to perform unnatural machining, possibly causing damage to the tool and/or machine, and even injuries. l Sample plan φ 4- 8
R30 70
R15
80
20 30
35
35 55
110 120 10
-279-
www.teknikokul.net
20
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
1.
B-63424EN/03
Setting of Tool Offset
EDIT
MEM
MDI
HANDLE
LIST
CHECK
WRK-CO
OFFSET SETING
Input the data of the tool length and radius by MDI key. [OFFSET]
001/25
TOOL LENGTH
CUTTER COMP.
NO. GEOM(H) WEAR(H) GEOM(D) WEAR(D) 1 2 3 4 5 6
2. EDIT
100.000 120.000 110.000 000.000 000.000 000.000
0.000 0.000 0.000 0.000 0.000 0.000
30.000 4.000 5.000 0.000 0.000 0.000
SAMPLE
0.000 0.000 0.000 0.000 0.000 0.000
Face Mill Drill End Mill
Inputting of Program Number MEM
MDI
HANDLE
LIST
CHECK
WRK-CO
OFFSET SETING
Input the program number and name by MDI key. PROGRAM LIST PROGRAM NO. USED / FREE 3 / 122 MEMORY AREA USED / FREE 900 / 3000 NO NAME DATE O0010: CIRCLE MACHINING 1999/01/12 10:12 O0020 LINE MACHINING O0020: 1999/02/10 11:21
SIZE 380 520
Cursor Program Number Program Name (Max 12ch.)
3.
Lastly modified date and time
Program size
Selecting of G code menus
EDIT
MEM
MDI
HANDLE
INIT
TOOL
MSF
COMP POSTIN
LIST
CHECK
-280-
www.teknikokul.net
CONTR
WRK-CO
OFFSET SETING
CYCLE TEACH
RETURN
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
4. INIT
Initial Setting TOOL
MSF
COMP POSTIN
INITIAL SET WORK CO-ORD. WORK SHAPE WORK X CO-ORD. WORK Y CO-ORD. WORK Z CO-ORD. WORK X WIDTH WORK Y WIDTH WORK THICKNESS
INIT
CYCLE TEACH
RETURN
1/1 G= G54 P= RECT. X= 0.000 Y= 0.000 Z= 5.000 I= 120.000 J= 80.000 K= 25.000
G300 W1 P1 X0 Y0 Z5. I120. J80. K25. A3 S4 B1;
INSERT
5.
CONTR
Tool Setting ( Tool = Face Mill for facing ) TOOL
MSF
COMP POSTIN
TOOL SET
CONTR
CYCLE TEACH
RETURN
1/1
TOOL NO T= 1 CUTTER OFFSET NO D= 1 LENGTH OFFSET NO H= 1 ANIMATION T RADIUS R= 30.000
G301 T1 D1 H1 R30. ;
INSERT
6. INIT
Instruction of M / S code ( Spindle speed ) TOOL
MSF
COMP POSTIN
-281-
www.teknikokul.net
CONTR
CYCLE TEACH
RETURN
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
MSF CODE M CODE SPINDLE SPEED FEED RATE
1/1 M= 3 S= 3000. F=
M3 S3000 ;
INSERT
7.
Instruction of Facing
INIT
TOOL
MSF
HOLE
PATTER
FACE
SQUARE
CIRCLE
SIDE
CONTR
CYCLE TEACH
RETURN
RETURN
POCKET
RETURN
SQUARE FACE MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH FINISHING ALW. FEED RATE CUTTING WITDH
COMP POSTIN
1/2 P= ROUGH Z= 0.000 B= 5.000 J= 5.000 H= 0.000 F= 500.000 C= 70.000
SQUARE FACE CENTER POINT X CENTER POINT Y U-LENGTH V-LENGTH
2/2 X= Y= U= V=
0.000 0.000 120.000 80.000
G210 P1. L3. Z0 B5. J5. H0 F500. C70. W1 X0 Y0 U120. V80. A0 E1. M5. N5. ;
INSERT
-282-
www.teknikokul.net
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
8. INIT
Instruction of M / S code ( Spindle Stop ) TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) M5 ;
INSERT
9. INIT
Tool Setting ( Tool = Drill for Hole Machining ) TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G301 T2 D2 H2 R4. ;
INSERT
10. Instruction of M / S code ( Spindle speed ) INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) M3 S5000 ;
INSERT
11. Instruction of Hole Machining HOLE
PATTER
FACE
SIDE
DRILL
BORE
TAP
RGTAP
RETURN
DRILLING CYCLE MACHINE PATTERN Z POINT DISTANCE R POINT DISTANCE PITCH DEPTH FEED RATE
RETURN
POCKET
G= Z= R= Q= F=
INSERT
-283-
www.teknikokul.net
1/1 S-PECK -20.000 2.000 5.000 50.000
G73 Z-20. R2. Q5. F50. K0 ;
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
12. Instruction of Hole Pattern POINTS
LINE
GRID
SQUARE
ARC
CIRCLE
SQUARE SRART POINT X SRART POINT Y U-LENGTH V-LENGTH U-NUMBER V-NUMBER PATTERN CONT.
RETURN
1/1 X= -55.000 Y= -35.000 U= 110.000 V= 70.000 I= 3 J= 3 Q= END
G203 X-55. Y-35. U110. V70. I3 J3 K0 L90. Q1 ;
INSERT
13. Instruction of M / S code ( Spindle Stop ) INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) M5 ;
INSERT
14. Tool Setting ( Tool = End Mill for Contour Pocketing ) INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) INSERT
-284-
www.teknikokul.net
G301 T3 D3 H3 R5. ;
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
15. Instruction of M / S code ( Spindle speed ) INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) M3 S1200 ;
INSERT
16. Instruction of Contour Pocketing HOLE
PATTER
FACE
SIDE
POCKET
SQUARE
CIRCLE
TRACK
GROOVE
CONTUR
CONTOUR POCKET MACH. PROCESS END POINT Z REMOVAL DEPTH REMOVAL PITCH BOTTOM FINISH SIDE FINISH
P= Z= B= J= H= D=
1/2 ROUGH -10.000 10.000 5.000 0 0
RETURN
C-GROV
RETURN
CONTOUR POCKET
2/2
FEED RATE Z-CUT FEED RATE CUTTING WIDTH%
F= 80.000 E= 30.000 C= 70.000
G234 P1. L3. Z-10. B10. J5. H0 D0 F80. C70. E30. W1. K1. ;
INSERT
17. Definition of Contour Pocket shape
(6) (5) (4)
(7) (15) (14) (11) (16) (13) (17)
(3)
(9)
(12) (10)
(2) (1)
-285-
www.teknikokul.net
(8)
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
(1). Definition of Start Point INIT
TOOL
MSF
COMP POSTIN
CONTR
START
LINE
CW ARC
CCW ARC
ROUND
POINT
CHAMF
START POINT
CYCLE TEACH
END
RETURN
TANGNT RECALC. RETURN
1/1
START POINT X START POINT Y START POINT TYPE
X= 0.000 Y= -30.000 E= START
G100 X0 Y-30. E1 ;
INSERT
(2). Definition of Clockwise Arc START
POINT
LINE
CW ARC
CCW ARC
CHAMF
ROUND
CW ARC RADIUS CENTER POINT X CENTER POINT Y END POINT X END POINT Y ANGLE
INSERT
-286-
www.teknikokul.net
END
TANGNT RECALC. RETURN
1/1 E= 30.000 V= 0.000 W= 0.000 M= N= K=
G102 X Y R I J Q0 E30. V0 W0 ;
B-63424EN/03
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
(3). Definition of Tangent Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
LINE
ROUND
END
TANGNT RECALC. RETURN
1/1
DIRECTION END POINT X END POINT Y LENGTH ANGLE
B= M= N= L= K=
G101 X Y Q1 B4 ;
INSERT
(4). Definition of Tangent Clockwise Arc START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G102 X Y R I J Q1 E15. V-35. W0. ;
INSERT
(5). Definition of Tangent Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q1 B2 ;
INSERT
(6). Definition of Tangent Clockwise Arc START
POINT
LINE
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) INSERT
-287-
www.teknikokul.net
G102 X Y R I J Q1 E30. V0. W0. ;
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
(7). Definition of Tangent Line START
LINE
POINT
CW ARC
CCW ARC
ROUND
CHAMF
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q1 B8 ;
INSERT
(8). Definition of Tangent Clockwise Arc START
LINE
POINT
CW ARC
CCW ARC
ROUND
CHAMF
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G102 X Y R I J Q1 E15. V35. W0 ;
INSERT
(9). Definition of Tangent Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q1 B6 ;
INSERT
(10). Definition of Tangent Clockwise Arc START
POINT
LINE
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) INSERT
-288-
www.teknikokul.net
G102 X0 Y-30. R30. I0 J0 Q1 E30. V0 W0 M0 N-30.;
B-63424EN/03
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
(11). Definition of Island START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
END
TANGNT RECALC. RETURN
1/1
CONTINUE
P= CONT
G106 P2 ;
INSERT
(12). Definition of Start Point for Island START
LINE
POINT
CW ARC
CCW ARC
CHAMF
START POINT
ROUND
END
TANGNT RECALC. RETURN
1/1
START POINT X START POINT Y START POINT TYPE ISLAND Z CO-ORD.
X= Y= E= Z=
0.000 -10.000 ISLAND 0.000
G100 X0. Y-10. E2 Z0 ;
INSERT
(13). Definition of Line START
POINT
LINE
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q2 B5 M-15. N-10. ;
INSERT
-289-
www.teknikokul.net
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
(14). Definition of Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q2 B3 M-15. N10. ;
INSERT
(15). Definition of Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q2 B1 M15. N10. ;
INSERT
(16). Definition of Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q2 B7 M15. N-10. ;
INSERT
(17). Definition of Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G101 X Y Q2 B5 M0 N-10. ;
INSERT
(18). Definition of Line START
LINE
POINT
CW ARC
CCW ARC
CHAMF
ROUND
END
TANGNT RECALC. RETURN
Input the necessary data by MDI key. ( Omission of the detail ) G106 P1 ;
INSERT
-290-
www.teknikokul.net
1. EXAMPLE OF INPUTTING PROGRAM
SAMPLE OF PROGRAMMING
B-63424EN/03
18. Instruction of M / S code ( Program End ) INIT
TOOL
MSF
COMP POSTIN
CONTR
CYCLE TEACH
RETURN
Input the necessary data by MDI key. ( Omission of the detail ) INSERT
-291-
www.teknikokul.net
M2 ;
APPENDIX
www.teknikokul.net
APPENDIX
B-63424EN/03
A
A. PARAMETERS
PARAMETERS !
WARNING
Be sure to use the parameters set by the machine builder. If you change the setting of a parameter, the machining program may not work correctly. If the machining program does not work correctly, the tool may bump against the work-piece, and the machine may be forced to perform unnatural machining, possibly causing damage to the tool and/or machine, and even injuries.
-295-
www.teknikokul.net
A. PARAMETERS
A.1
APPENDIX
B-63424EN/03
GRAPHIC DISPLAY PARAMETERS 6500
DPO
FANUC standard settings 00100000 DPO
1: 0:
6501
The current position of the tool is displayed on the machining profile and tool path drawing display screens. The current position of the tool is not displayed on the machining profile or tool path drawing display screen.
CSR
FIM
RID
3PL
TLC
ORG
FANUC standard settings 00000000 ORG
1: 0:
TLC
1: 0:
3PL
1: 0:
RID
1: 0:
FIM CSR
1: 0: 1: 0:
If the coordinate system is updated during a drawing operation, the drawing operation is continued in the same coordinate system. If the coordinate system is updated during a drawing operation, the drawing operation is performed by assuming that the current position of the tool is set in the new coordinate system. Tool length compensation is made on the machining profile drawing. Tool length compensation is not made on the machining profile drawing. The triplane machining profile drawing is created using thirdangle projection. The triplane machining profile drawing is created using firstangle projection. On the machining profile drawing, the plan view is drawn using edge lines. On the machining profile drawing, the plan view is drawn without using edge lines. The machining profile drawing is displayed in the detail mode. The machining profile drawing is displayed in the coarse mode. On the tool path drawing, the graphic cursor is represented with X when the drawing is enlarged. On the tool path drawing, the graphic cursor is represented with n when the drawing is enlarged.
6511
RGTBLK Valid data range Units FANUC standard settings
RGTBLK
Amount of the right-side margin on the machining profile drawing (On the machining profile drawing, the position of an element to be drawn is set up using an amount of blank on the CRT screen.) 0 to 100 1 (point) 0
6512
LFTBLK
-296-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
LFTBLK Valid data range Units FANUC standard settings
Amount of the left-side margin on the machining profile drawing 0 to 100 1 (point) 0
6513
UPBLK Valid data range Units FANUC standard settings
UPBLK
Amount of the upper-side margin on the machining profile drawing 0 to 100 1 (point) 0
6514
DWNBLK Valid data range Units FANUC standard settings
DWNBLK
Amount of the lower-side margin on the machining profile drawing 0 to 100 1 (point) 0
6515
CRSSCT
Valid data range Units FANUC standard settings
CRSSCT
Amount of change to the cross-section position (For the triplane and cross-section drawing displays, the amount of a change to the cross-section position that occurs when a soft key is kept pressed is set up.) 0 to 100 1 (point) 10
-297-
www.teknikokul.net
A. PARAMETERS
A.2
APPENDIX
B-63424EN/03
MACRO EXECUTOR PARAMETERS 9000
L2R
MKG
RSC
EXS
STP
NDP
SQN
FANUC standard settings 00001000 SQN
1: 0:
NDP
1: 0:
STP
1: 0:
EXS
1: 0:
RSC
1: 0:
MKG L2R
1: 0: 1: 0:
When a registered program is being executed, the program and sequence numbers in the program are displayed. When a registered program is being executed, the program and sequence numbers in a called user program are displayed. The local and common variables for the P-CODE program are displayed. The local and common variables for the P-CODE program are not displayed. The conversational macro program is stopped. (This parameter is set to "1" automatically by the break function.) Neither local nor common variables for the P-CODE program are displayed. If macros are being executed on the execution level, their execution is not stopped before the next NC statement appears even when a feed hold is put in effect. If macros are being executed on the execution level, their execution is stopped the moment a feed hold is put in effect. When the NC is reset, common variables #100 to #149 are cleared to
. When the NC is reset, none of common variables #100 to #149 is cleared to . No graphic screen is displayed. A graphic screen is displayed. Neither conversational auxiliary macro execution nor screen display is performed during an execution macro-based operation. Both conversational auxiliary macro execution and screen displays are performed during an execution macro-based operation.
9002
BLKNO1 Valid data range Units FANUC standard settings
BLKNO1
Conversational macro break program number 0 to 9999 1 0
-298-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
9003
BLKNO2 Valid data range Units FANUC standard settings
BLKNO2
Conversational macro break program number 0 to 9999 1 0
-299-
www.teknikokul.net
A. PARAMETERS
A.3
APPENDIX
B-63424EN/03
PARAMETERS FOR PROGRAMMING 9100
STAMAC Valid data range Units FANUC standard settings
STAMAC
Start up macro program number for MANUAL GUIDE screen 0 to 9999 1 8000
9101
EDTTBL Valid data range Units FANUC standard settings
EDTTBL
Starting variable number for a edit macro definition table It is not necessary for the operator to set this parameter. 0 to 9999 1 0
9102
DATVAL Valid data range Units FANUC standard settings
DATVAL
Starting variable number for a process data It is not necessary for the operator to set this parameter. 0 to 9999 1 0
NOTE When these parameters 9100, 9101 and 9102 are changed or set, please power OFF and ON.
9104
DMA
CGO
LDM
SLM
MOD
NST
FANUC standard settings 00000000 NST
1:
MOD
0: 1: 0:
Soft-key [EXEC] is not displayed on the machining operation screen. Soft-key [EXEC] is displayed on the machining operation screen. PMC software changes the mode by checking the mode changing signals. The operator changes the mode by setting the operator’s panel of the machine.
-300-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
NOTE 1). In the case of MOD = 0, the screen is automatically changed according to the mode. • EDIT mode • MEM mode • MDI mode • JOG mode
→ → → →
Program edit screen Machining operation screen MDI operation screen Manual operation screen
2). In the case of MOD = 1, the mode is automatically changed according to the screen. • Program edit screen • Machining operation screen • MDI operation screen • Manual operation screen SLM LDM CGO
DMA
→ → → →
EDIT mode MEM mode MDI mode JOG mode
1: 0: 1: 0: 1:
Spindle load meter is not displayed on the CNC status area. Spindle load meter is displayed on the CNC status area. Servo load meter is not displayed on the CNC status area. Servo load meter is displayed on the CNC status area. When the cursor is placed at a contour figure block on program window, the contour figure is not displayed on the graphic window. 0 : When the cursor is placed at a contour figure block on program window, the contour figure is displayed on the graphic window. Specifies how the distance yet to go and the next block are displayed in the status display window, as follows: 1 : Only the axis along which the tool is currently moving is displayed. 0 : The first to third axes are displayed.
9105
ISM
G68
G41
ATR
DCD
SUR
FANUC standard settings 00000000 SUR
1: 0:
DCD
1: 0:
The item of WORK SURFACE Z (B) is displayed on the screen of each cycle menus. It means the workpiece coordinate of the top surface. The item of REMOVAL DEPTH (B) is displayed on the screen of each cycle menus. It means the depth of the bottom surface. The item of CUTTER OFFSET NO (D) and LENGTH OFFSET NO (H) are not displayed on the screen of TOOL SET menus. ( The operator has to set it to COMP menu. ) The item of CUTTER OFFSET NO (D) and LENGTH OFFSET NO (H) are displayed on the screen of TOOL SET menus.
-301-
www.teknikokul.net
A. PARAMETERS
APPENDIX
ATR
G41
G68
ISM
B-63424EN/03
1:
The item of ANIMATION T RADIUS (R) is displayed on the screen of TOOL SET menus. 0 : The item of ANIMATION T RADIUS (R) is not displayed on the screen of TOOL SET menus. Specifies which tool path is output during side-facing and pocket side-facing as follows: 1 : A tool path with cutter compensation used is output. 0 : A tool path with no cutter compensation used is output. Caution) If G41 = 1, the cutter compensation C optional function is necessary. 1 : The message of the mode for 3-dimensional coordinate conversion is displayed on the CNC status area. 0 : The message of the mode for 3-dimensional coordinate conversion is not displayed on the CNC status area Specifies how to display input items in the initial setting menu, as follows: 1 : The "travel distance command," "plane selection," and "unit of inputs" are displayed in the first section of the window. 0 : The "travel distance command," "plane selection," and "unit of inputs" are displayed in the detail window.
9106
TOLCHG Valid data range Units FANUC standard settings
TOLCHG
Sub program number called tool change sequence instead of M6 0 to 9999 1 0
9107
NCD
WDS
WGP
FANUC standard settings 00000000 WGP
WDS
NCD
Specifies axis movement on the boring machine as follows: 1 : W-axis movement (parallel to the Z-axis) as well as Z-axis movement is taken into account for drawing. 0 : W-axis movement (parallel to the Z-axis) is not taken into account for drawing. Specifies whether to enable the [FULL ON/OFF] soft key for tool path and animated simulation drawings, as follows: 1 : The [FULL ON/OFF] soft key is enabled. 0 : The [FULL ON/OFF] soft key is disabled. Specifies whether to display NC statements if the [FULL ON/OFF] soft key is enabled (WDS = 1), as follows: 1 : NC statements are displayed on the drawing screen. 0 : NC statements are not displayed on the drawing screen.
-302-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
9108
OPO
GRO
FANUC standard settings 00000000 GRO
OPO
Specifies whether to output the G10 command when NC statements are output, as follows: 1 : The G10 command is output. 0 : The G10 command is not output. Specifies whether to add an optional block delete (/) symbol when NC statements are output, as follows: 1 : An optional block delete (/) symbol is added. 0 : An optional block delete (/) symbol is not added.
9110
MUW
UWN
FANUC standard settings 00000000 UWN MUW
1: 0: 1: 0:
User window display is enabled on the editing screen. User window display is disabled on the editing screen User window display is enabled on the operation screen. User window display is disabled on the operation screen.
9111
EDTUWN Valid data range Units FANUC standard settings
EDTUWN
Macro program number for the user window on the editing screen 0 to 9999 1 0
9112
EDTGNO Valid data range Units FANUC standard settings
EDTGNO
G code number used in the user window on the editing screen 100 to 999 (3-digit) 1 0
9113
MCHUWN Valid data range Units FANUC standard settings
MCHUWN
Macro program number for the user window on the operation screen 0 to 9999 1 0
-303-
www.teknikokul.net
A. PARAMETERS
A.4
APPENDIX
B-63424EN/03
PARAMETERS FOR CYCLE MACHINING 9120
TOLANG Valid data range Units FANUC standard settings
TOLANG (A)
Default data of cutting angle for tool-axis in-feed of Pocketing. 0 to 90 ( In the case of 0, it is regards 90. ) 1 degree 0 A
9121
FEEDRM (Frm)
9122
FEEDTM (Ftm)
FEEDRM FFEDTM Valid data range Units FANUC standard settings
Feedrate used for in-feed tool movement vertical to the tool axis. If 0 input, movement is rapid traverse. ( In the case of ESC = 1 only ) Feedrate used for tool movement along the tool axis. If 0 input, movement is rapid traverse. 0 to 65535 1mm/min 0 Frm Ftm
9123
CHK
CNR
ESC
ILA
FANUC standard settings 00000000 ILA
1: 0:
The top of a island is not cut. The top of a island is cut by controlling the cut depth ILA= 0
ILA = 1
-304-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
ESC
1: 0:
Retract the tool to the point ( surface + clearance ). Retract the tool to the point ( cutting plane + clearance ).
ESC = 1
ESC = 0
clearance
clearance
NOTE In ESC = 1, the tool may interfere with the workpiece. if the tool is not lifted to a safe position depending on the clearance for in-feed. Therefore, be particularly careful to avoid interference between the tool and work-piece. CNR
1: 0:
Cut corners using circular interpolation. Cut corners using linear interpolation.
CNR = 1
CHK
1:
0:
There is a check cut leaving. If there is a portion left uncut at a corner in pocketing, it is identified automatically and cut off. This function may decrease the processing speed for tool path preparation. There is no check cut leaving.
9125
CONSID Valid data range Units FANUC standard settings
CNR = 0
CONSID
G-code number of Contour Side Cutting for automatic changing softkeys 0 to 999 1 224
-305-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
9126
CNTPOK Valid data range Units FANUC standard settings
CNTPOK
G-code number of Contour Pocketing for automatic changing soft-keys 0 to 999 1 234
9127
CNTGRV Valid data range Units FANUC standard settings
CNTGRV
G-code number of Contour Grooving for automatic changing soft-keys 0 to 999 1 235
NOTE When the above parameters No.9125, 9126 or 9127 are set, the soft-keys are automatically changed from each contour cycle to contour profile menu. 9140
RESTZ Valid data range Units FANUC standard settings
RESTZ
Allowable amount of remainder during driving in Z direction in roughing. 0 to 9999 1% 20
9141
RESTXY Valid data range Units FANUC standard settings
RESTXY
Allowable amount of remainder during driving in XY direction in roughing and bottom finishing. 0 to 9999 1% 20
9150
MESRNO Valid data range Units FANUC standard settings
MESRNO
Variable start number to be used in measurement cycle 0 to 99999 1 800
-306-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
12050
SPNORM Valid data range Units
SPNORM
M code for orientation to be used in measurement cycle 0 to 99 1
-307-
www.teknikokul.net
A. PARAMETERS
A.5
APPENDIX
B-63424EN/03
USER PARAMETERS 9200 ... ...
Bit Parameters
9250 9251 ... ...
Word Parameters
9299
NOTE For details of parameter Nos.9200 to 9299, refer to the manual supplied by the machine tool builder.
-308-
www.teknikokul.net
A.6
A. PARAMETERS
APPENDIX
B-63424EN/03
COLOR PALLET SETTING PARAMETERS Setting the following parameters can change the color of characters and graphic elements displayed on the manual guide screen. 9701
GRPNO1
9702
GRPNO2
9703
GRPNO3
to 9714
GRPNO14
9715
GRPNO15
FANUC standard settings GRPNO*
0 (No.9701 to 9715) Color setting data for graphic color number * (1 to 15) The graphic color numbers correspond to portions on the guide drawing. The color numbers listed below especially are associated with the color of the workpiece on the machining profile drawing.
Color number 7 13 14
Color of the corresponding portion Top surface of the workpiece on the machining profile drawing Front surface of the workpiece on the machining profile drawing Front surface of the workpiece on the machining profile drawing
-309-
www.teknikokul.net
Standard color setting White Light gray Rather dark gray
A. PARAMETERS
APPENDIX
B-63424EN/03
9716
CHRNO1
9717
CHRNO2
9718
CHRNO3
to 9729
CHRNO14
9730
CHRNO15
FANUC standard settings CHRNO*
0 (No.9716 to 9730) Color setting data for character color number * (1 to 15) The character color numbers correspond to portions on the screen as listed below.
Color number 1 2 3
4 5 6 7 8 9 10 11 12 13 14 15
Color of the corresponding portion Alarm message Mode display background color Title bar and cursor display on the uppermost section of the conversational screen Window title background color and soft key character Icon display Icon display Title character, soft key frame, and cursor display Load meter display (Not used) Icon and load meter display Status display section background color and window background color Icon display (Not used) Window and soft key shade Program display area background color and soft key background color
Standard color setting Red Green Yellow
Blue Purple Light blue White Yellow Blue Bright green Light gray Dark turquoise White Rather dark gray Gray
The graphic and character color numbers are set as follows: •
Unit of data
: cc××ρρ (6-digit number) (cc: Value for red, ××: Value for green, ρρ: Value for blue) If the specified number is smaller than 6 digits, it is assumed that leading zeros are omitted.
-310-
www.teknikokul.net
A. PARAMETERS
APPENDIX
B-63424EN/03
•
Valid data range : 0 to 15 for each color If a value greater than 15 is specified, 15 is assumed.
If parameter Nos. 9701 to 9730 are all zeros, the same color scheme as for when the following data is specified is used. No.9701 = 150000 No.9702 = 800 No.9703 = 131200 No.9704 = 30311 No.9705 = 120010 No.9706 = 1515 No.9707 = 141414 No.9708 = 131200 No.9709 = 30311 No.9710 = 41004 No.9711 = 121209 No.9712 = 30311 No.9713 = 121212 No.9714 = 60606 No.9715 = 40404
Red Green Yellow Blue Purple Light blue White Yellow Blue Yellowish green Yellowish gray Blue Light gray Rather dark gray Dark gray
No.9716 = 150000 No.9717 = 800 No.9718 = 131200 No.9719 = 30311 No.9720 = 120010 No.9721 = 1515 No.9722 = 141414 No.9723 = 131200 No.9724 = 30311 No.9725 = 41004 No.9726 = 121209 No.9727 = 30311 No.9728 = 121212 No.9729 = 60606 No.9730 = 40404
Red Green Yellow Blue Purple Light blue White Yellow Blue Bright green Dark gray Dark turquoise White Rather dark gray Gray
-311-
www.teknikokul.net
B. ALARMS
B
APPENDIX
B-63424EN/03
ALARMS If one or more of the set of the parameters or inputted programs are not correct when an attempt is made to execute that program, the following P/S alarms are raised. When an alarm other than the following P/S alarms is raised, refer to the relevant NC operator’s manual. Alarm 3001
Cause Action
Reference 3002
Cause Action Reference
3003
Cause Action Reference
3004
Cause Action Reference
3005
Cause Action Reference
Description Necessary data is not entered. Or entered data is invalid. Display the block data of pop-up window, at which is occurred the alarm, and enter the correct data after confirming it. III. Types of Cycle Motions. All cycle machining except for hole machining The offset data corresponding to the specified D code is 0 or less. Confirm the D code, at which is occurred the alarm and enter the correct data to the offset table. III. Types of Cycle Motions. All cycle machining except for hole machining The tool interferes with the opposite surface. Confirm the tool, at which is occurred the alarm and select the tool of smaller radius than the last time. III. Types of Cycle Motions. Facing in the cased of CUT DIRECTION = RING. Machining is impossible because the cutter diameter is too large. Confirm the tool, at which is occurred the alarm and select the tool of smaller radius than the last time. III. Types of Cycle Motions. Side cutting and Pocketing The tool interferes with the opposite edge because the length of approach is too long. Confirm the approach data, at which is occurred the alarm and enter the correct data to the approach. III. Types of Cycle Motions. Side cutting and Pocketing
-312-
www.teknikokul.net
B. ALARMS
APPENDIX
B-63424EN/03
Alarm 3006
Cause Action Reference
3007
Cause Action
Reference 3008
Cause Action Reference
3012
Cause Action Reference
3013
Cause Action Reference
3014
Cause Action Reference
3015
Cause Action Reference
Description Corner R interferes with the opposite one because the radius of corner R is too large. Confirm the radius of corner R, at which is occurred the alarm and enter the correct data to the radius. III. Types of Cycle Motions. Side cutting and Pocketing in the cased of Corner R Corner C interferes with the opposite one because the chamfer amount is too large. Confirm the chamfer amount of corner C, at which is occurred the alarm and enter the correct data to the chamfer. III. Types of Cycle Motions. Side cutting in the cased of Corner C Corner R machining can not be performed because the cutter diameter is larger than corner R. Confirm the tool, at which is occurred the alarm and select the tool of smaller radius than the last time. III. Types of Cycle Motions. Side cutting and Pocketing in the cased of Corner R The chamfering tool interferes with the bottom surface (Z point) in chamfering. Confirm the block data related to chamfer tool, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Chamfering in Side cutting and Pocketing The angle at which the chamfering tool is placed is not specified. Confirm the block data related to chamfer tool, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Chamfering in Side cutting and Pocketing The tool path can not create because the memory for the calculation is over the limitation. Divide the entered contour figure block or machining area. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing The tool path can not create because the contour shape is not correct. Confirm the block data of the contour shape, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing
-313-
www.teknikokul.net
B. ALARMS
APPENDIX Alarm 3016
Cause Action
Reference 3017
Cause Action
Reference 3018
Cause Action
Reference 3020
Cause Action
Reference 3022
Cause Action Reference
B-63424EN/03
Description The tool path can not create because the data of cutting condition is not correct. Confirm the block data related to the cutting condition, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing The machining can not be performed because the cutting start point positions at the outer machining field. Confirm the block data related to the cutting condition and contour shape, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing The cutting start point can not be calculated because the data is not correct. Confirm the block data related to the cutting condition and contour shape, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing The tool interferes with the machining shape. Confirm the block data related to the cutting condition and contour shape, at which is occurred the alarm and enter the correct data to it. III. Types of Cycle Motions. Contour shape of Side cutting and Pocketing D code is not specified. Before the block at which is occurred the alarm, specify D code by using Tool Setting menu. II. Operation. 3.2.2 Tool Setting menu
-314-
www.teknikokul.net
INDEX
B-63424EN/03
CONTOUR GROOVE (G235), 219
p
CONTOUR POCKET (G234), 212 CONTOUR PROGRAMMING OPERATION, 52
2-HOLES ANGLE MEASUREMENT (G192), 274
Contour Repetition, 53
3-Plan View, 89
CONTOUR SIDE (G224), 187
4- HOLES CENTER MEASUREMENT (G190), 269
Cross Sectional View, 89 Cycles, 48
ALARMS, 312
ALL-IN-ONE SCREEN, 6
Detail of Contour Calculation, 56
ANIMATED SIMULATION, 88
DETAIL OF EACH MENUS, 28
ARC (G205), 157
Display and Cancellation of Alarms That May Be Generated During the Execution of Drawing, 95
Display of the Operation Status on the Drawing Screen, 95
BACKGROUND DRAWING (OPTION FUNCTION), 94
DISPLAY THE MEASUREMENT RESULT, 230
BACKGROUND EDITING, 101
Drilling Cycle (High-speed Peck) (G73), 122
BOLT-HOLE-CIRCLE MEASUREMENT (G189), 266
Drilling Cycle (Peck) (G83), 119 Drilling Cycle (With Dwell) (G82), 116
BORING, 124
Drilling Cycle (Without Dwell) (G81), 114
Boring Cycle (Back Boring) (G87), 136
DRILLING, 114
Boring Cycle (Feed Retraction) (G85), 125 Boring Cycle (Fine Boring) (G76), 133
Boring Cycle (Manual Retraction) (G88), 129
EDITING OPERATION, 49
Boring Cycle (Rapid Retraction) (G86), 127
EDITING TAUGHT-IN BLOCKS, 79
Boring Cycle (With Dwell) (G89), 131
Enlarge / Reduce, 85 EXAMPLE OF INPUTTING PROGRAM, 279
Execution of Playback Machining Program, 82
CALCULATOR FUNCTION, 105 CALIBRATION CYCLES (OPTIONAL FUNCYION), 233
CHECKING CUTTING MOTIONS ON A GRAPHIC WINDOW, 81
FACING, 159
Checking of Playback Machining Program, 82
FULL SCREEN GRAPHIC DISPLAY FUNCTION, 92
FLOWCHART OF OPERATIONS, 15
CIRCLE (G204), 155 CIRCLE POCKET (G231), 200
CIRCLE SIDE (G221), 177 CIRCLE SURFACE (G211), 166
GRAPHIC DISPLAY PARAMETERS, 296
COLOR PALLET SETTING PARAMETERS, 309
Graphic Window, 27
Compensation, 35
GRID (G202), 151
Contour, 38
GROOVE (G233), 206
i-1
www.teknikokul.net
INDEX
B-63424EN/03
GROOVE WIDTH MEASUREMENT (G182), 248
GUIDANCE CUTTING OPERATIONS (OPTIONAL FUNCTION), 67
ONE SIDE (G223), 183
GUIDANCE HANDWHEEL, 4
Operation, 107 Operation of Guidance Cutting (Circle), 75
Operation of Guidance Cutting (Line), 72
Handling of Various Data Items, 95
Operation of Teach-in a Cutting Block, 78
HOLE MACHINING, 113
Operation of Teach-in a Rapid Traverse Motion Block, 70
HOLE PATTERN, 147
Operation of Teach-in a Simple Linear Cutting Motion Block, 71
Operation of Teach-in Auxiliary Function Blocks, 70
Initial Setting, 28
Operations for Program Editing, 80
INPUTTING COMMON DATA, 68
OTHER FUNCTIONS, 105
Inputting of Program Number / Program Name, 22
OUTSIDE CIRCLE MEASUREMENT (G183), 250, 253
INSIDE CORNER MEASUREMENT (G188), 264
OUTSIDE CORNER MEASUREMENT (G187), 262
INSIDE RECTANGULAR MEASUREMENT (G186), 259
OUTSIDE RECTANGULAR MEASUREMENT (G185), 256 OVERVIEW, 3
Overview of Contour Programming, 52
Left-handed Tapping Cycle (G74), 142
OVERVIEW OF MEASURING CYCLES FUNCTION, 226
LINE (G201), 149
OVERVIEW OF PROGRAMMING OPERATION, 22
OVERVIEW OF THE PROCEDURE, 13
MACHINING OPERATION, 99
MACRO EXECUTOR PARAMETERS, 298 MACRO VARIABLE FOR CALIBRATION CYCLES, 228
Parameter, 109
MACRO VARIABLE FOR MEASURING CYCLES, 229
PARAMETERS FOR CYCLE MACHINING, 304
PARAMETERS, 9, 295
MAIN FEATURES OF MANUAL GUIDE, 14
PARAMETERS FOR MEASUREMENT, 227
MANUAL OPERATION, 104
PARAMETERS FOR PROGRAMMING, 300
MDI / MANUAL OPERATION, 102
Parameters of Animated Simulation, 90
MDI OPERATION, 103
Parameters of Tool Path Drawing, 86
MEASURING CYCLES (OPTIONAL FUNCYION), 242
Plan View, 90
MEMORY OPERATION, 100
POCKETING, 193
MSF code, 34
POINTS (G200), 148
PLAYBACK MACHINING, 82
Pop-up Window, 26
Positioning, 37
NC FORMAT OUTPUT FUNCTION, 107
PRE-SETTING OF THE OPERATIONS, 17
NOTES ON DRAWING, 97
PROBE LENGTH CALIBRATION (G170), 234
i-2
www.teknikokul.net
INDEX
B-63424EN/03
PROGRAM CHECKING, 84
TRACK POCKET (G232), 203
Program Window, 25, 69, 79
TRACK SIDE (G222), 180
PROGRAMMING OPERATIONS, 21
USER PARAMETERS, 308
RIGID TAPPING (G243), 144
Rotation, 88
WEB WIDTH MEASUREMENT (G181), 246
Window of Output NC Statements, 108 WORK PIECE ANGLE MEASUREMENT (G191), 272
SAFETY PRECAUTIONS, s-1 Screen Switching Using a Function Key, 95 Selecting of Soft-key Menus, 24
SELECTING THE GUIDANCE CUTTING, 68
X/Y/Z SINGLE SURFACE MEASUREMENT (G180), 243
Selection of the Program with Which Drawing Is to Be Executed, 94 SETTING OF DISPLAYING WINDOW, 20 SETTING OF TOOL OFFSET VALUES, 19 SETTING OF WORK COORDINATE SYSTEM, 18 SIDE CUTTING, 169 SQUARE (G203), 153 SQUARE POCKET (G230), 194 SQUARE SIDE (G220), 170 SQUARE SURFACE (G210), 160 STYLUS BALL DIAMETER CALIBRATION (G171), 236 STYLUS X AND Y OFFSETS CALIBRATION- A (G172), 238 STYLUS X AND Y OFFSETS CALIBRATION- B (G173), 240 SYMBOLS USED, 8 System variable for distinguishing the executing state (#3010), 108
TAPPING, 139 Tapping Cycle (G84), 140 TEACH-IN CUTTING MOTIONS, 69 Teaching, 48 TOOL PATH DRAWING, 85 Tool Position, 86 Tool Setting, 31
i-3
www.teknikokul.net
www.teknikokul.net
Jun.,2000 Improvement for easy operation
Nov., 1999
Date
02
01
Edition
Contents
May, 2001
03
Addition of new functions Applied to Series 16i/18i/21i-B
Edition
Date
Contents
FANUC MANUAL GUIDE (For Milling) OPERATOR’S MANUAL (B-63424EN)
Revision Record
·
No part of this manual may be reproduced in any form.
·
All specifications and designs are subject to change without notice.
www.teknikokul.net
