- Manuals
- Brands
- Mitsubishi
- Numerical Control
- C6
- Specification Manual
Mitsubishi C6 Numerical Control Specification Manual PDF
en
Summary of Content for Mitsubishi C6 Numerical Control Specification Manual PDF
CNC C6/C64
SPECIFICATIONS MANUAL
BNP-B2266C(ENG)
MELDAS and MELSEC are registered trademarks of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective company.
Introduction
This manual describes the specifications of MELDAS C6/C64. To safely use this CNC unit, thoroughly study the "Precautions for Safety" on the next page before use. Details described in this manual At the beginning of each item, a table indicating its specification according to the model.
: Standard : Option
: Selection : Special option
CAUTION The items that are not described in this manual must be interpreted as "not possible".
This manual is written on the assumption that all option functions are added. Some functions may differ or some functions may not be usable depending on the NC system (software) version.
General precautions
(1) When the contents of this manual is updated, the version (*, A, B, ) on the cover will be incremented.
Precautions for Safety
Always read the specifications issued by the machine maker, this manual, related manuals and attached documents before installation, operation, programming, maintenance or inspection to ensure correct use. Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".
DANGER
When there is a great risk that the user could be subject to fatalities or serious injuries if handling is mistaken.
WARNING
When the user could be subject to fatalities or serious injuries if handling is mistaken.
CAUTION
When the user could be subject to injuries or when physical damage could occur if handling is mistaken.
Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important information that must always be observed is described.
DANGER Not applicable in this manual.
WARNING Not applicable in this manual.
CAUTION
1. Items related to product and manual
The items that are not described in this manual must be interpreted as "not possible". This manual is written on the assumption that all option functions are added. Some functions may differ or some functions may not be usable depending on the NC
system (software) version.
2. Items related to start up and maintenance Follow the power specifications (input voltage range, frequency range, momentary
power failure time range) described in this manual. Follow the environment conditions (ambient temperature, humidity, vibration,
atmosphere) described in this manual.
! Follow the remote type machine contact input/output interface described in this manual. (Connect a diode in parallel with the inductive load or connect a protective resistor in serial with the capacitive load, etc.)
If the parameter is used to set the temperature rise detection function to invalid, overheating may occur, thereby disabling control and possibly resulting in the axes running out of control, which in turn may result in machine damage and/or bodily injury or destruction of the unit. It is for this reason that the detection function is normally left "valid" for operation.
i
CONTENTS 1. Control Axes....................................................................................................................... 1
1.1 Control Axes................................................................................................................. 1 1.1.1 Number of Basic Control Axes (NC axes) .......................................................... 1 1.1.2 Max. Number of Control Axes
(NC axes + Spindles + PLC axes + Auxiliary axes)........................................... 1 1.1.3 Number of Simultaneous Contouring Control Axes............................................ 2 1.1.4 Max. Number of NC Axes in a Part System ....................................................... 2
1.2 Control Part System..................................................................................................... 2 1.2.1 Standard Number of Part Systems..................................................................... 2 1.2.2 Max. Number of Part Systems............................................................................ 2
1.3 Control Axes and Operation Modes ............................................................................ 3 1.3.2 Memory Mode ..................................................................................................... 3 1.3.3 MDI Mode............................................................................................................ 3
2. Input Command ................................................................................................................. 4
2.1 Data Increment ............................................................................................................ 4 2.2 Unit System.................................................................................................................. 5
2.2.1 Inch/Metric Changeover; G20/G21..................................................................... 5 2.3 Program Format........................................................................................................... 6
2.3.1 Character Code................................................................................................... 6 2.3.2 Program Format .................................................................................................. 7
2.3.2.1 Format 1 for Lathe (G code list 2, 3) ...................................................... 7 2.3.2.4 Format 1 for Machining Center (G code list 1)....................................... 7
2.4 Command Value .......................................................................................................... 8 2.4.1 Decimal Point Input I, II ....................................................................................... 8 2.4.2 Absolute / Incremental Command; G90/G91 ..................................................... 9 2.4.3 Diameter/Radius Designation ............................................................................. 11
2.5 Command Value and Setting Value Range ................................................................ 12 2.5.1 Command Value and Setting Value Range........................................................ 12
3. Positioning/Interpolation .................................................................................................. 16
3.1 Positioning; G0, G60.................................................................................................... 16 3.1.1 Positioning; G0.................................................................................................... 16 3.1.2 Unidirectional Positioning; G60........................................................................... 17
3.2 Linear/Circular Interpolation; G1, G2/G3..................................................................... 18 3.2.1 Linear Interpolation; G1....................................................................................... 18 3.2.2 Circular Interpolation (Center/Radius Designation); G2/G3 ............................... 19 3.2.3 Helical Interpolation............................................................................................. 21
4. Feed..................................................................................................................................... 23
4.1 Feed Rate .................................................................................................................... 23 4.1.1 Rapid Traverse Rate (m/min).............................................................................. 23 4.1.2 Cutting Feed Rate (m/min).................................................................................. 24 4.1.3 Manual Feed Rate (m/min) ................................................................................. 25
4.2 Feed Rate Input Methods; G94/G95 ........................................................................... 26 4.2.1 Feed per Minute .................................................................................................. 26 4.2.2 Feed per Revolution............................................................................................ 28 4.2.4 F1-digit Feed ....................................................................................................... 29
4.3 Override ....................................................................................................................... 30 4.3.1 Rapid Traverse Override..................................................................................... 30 4.3.2 Cutting Feed Override......................................................................................... 30 4.3.3 2nd Cutting Feed Override.................................................................................. 30 4.3.4 Override Cancel .................................................................................................. 31
ii
4.4 Acceleration/Deceleration............................................................................................ 32 4.4.1 Automatic Acceleration/Deceleration after Interpolation .................................... 32 4.4.2 Rapid Traverse Constant Inclination Acceleration/Deceleration........................ 33
4.5 Thread Cutting ............................................................................................................. 36 4.5.1 Thread Cutting (Lead/Thread Number Designation); G33................................. 36 4.5.2 Variable Lead Thread Cutting; G34.................................................................... 38 4.5.3 Synchronous Tapping; G74, G84 ....................................................................... 39
4.5.3.1 Synchronous Tapping Cycle .................................................................. 39 4.5.4 Chamfering.......................................................................................................... 40
4.6 Manual Feed ................................................................................................................ 41 4.6.1 Manual Rapid Traverse....................................................................................... 41 4.6.2 Jog Feed ............................................................................................................. 41 4.6.3 Incremental Feed ................................................................................................ 42 4.6.4 Handle Feed........................................................................................................ 42
4.7 Dwell; G04.................................................................................................................... 43 4.7.1 Dwell (Time-based Designation)......................................................................... 43
5. Program Memory/Editing.................................................................................................. 44
5.1 Memory Capacity ......................................................................................................... 44 5.1.1 Memory Capacity (Number of Programs Stored) ............................................... 44
5.2 Editing Method ............................................................................................................. 45 5.2.1 Program Editing .................................................................................................. 45 5.2.2 Background Editing............................................................................................. 46
6. Operation and Display....................................................................................................... 47
6.1 Structure of Operation/Display Panel .......................................................................... 47 6.2 Operation Methods and Functions .............................................................................. 48
6.2.1 Memory Switch (PLC Switch) ............................................................................. 48 6.3 Display Methods and Contents.................................................................................... 48
6.3.1 Status Display ..................................................................................................... 48 6.3.2 Position Display................................................................................................... 49 6.3.3 Program Running Status Display........................................................................ 50 6.3.4 Setting and Display ............................................................................................. 50 6.3.5 MDI Data Setting and Display............................................................................. 50 6.3.7 Clock ................................................................................................................... 50 6.3.8 Hardware/Software Configuration Display.......................................................... 50 6.3.9 Integrated Time Display ...................................................................................... 51 6.3.10 Available Languages (Japanese/English) ........................................................ 52 6.3.11 Additional Languages (Japanese/English/Polish) ............................................ 52
6.3.11.1 Japanese.............................................................................................. 52 6.3.11.2 English.................................................................................................. 52 6.3.11.13 Polish.................................................................................................. 52
6.3.13 Screen Deletion................................................................................................. 52 6.4 Display Unit Switch ..................................................................................................... 53
6.4.1 Single-NC and Multi-Display Unit Switch........................................................... 53 6.4.2 Multi-NC and Common-Display Unit.................................................................. 53 6.4.4 Multi-NC and Common-external PC Display ..................................................... 53 6.4.5 Display Unit Detachable..................................................................................... 54
7. Input/Output Functions and Devices............................................................................... 55
7.1 Input/Output Data......................................................................................................... 55 7.2 Input/Output I/F ............................................................................................................ 56
7.2.1 RS-232C I/F ........................................................................................................ 56 7.2.2 IC Card I/F........................................................................................................... 56
7.2.2.1 I/F for IC Card in Control Unit................................................................. 56
iii
8. Spindle, Tool and Miscellaneous Functions .................................................................. 57 8.1 Spindle Functions (S)................................................................................................... 57
8.1.1 Command/Output................................................................................................ 57 8.1.1.1 Spindle Functions................................................................................... 57 8.1.1.2 Spindle Serial I/F .................................................................................... 58 8.1.1.3 Spindle Analog I/F .................................................................................. 58 8.1.1.4 Coil Change............................................................................................ 58 8.1.1.5 Automatic Coil Change........................................................................... 58
8.1.2 Speed Control ..................................................................................................... 59 8.1.2.1 Constant Surface Speed Control ........................................................... 59 8.1.2.2 Spindle Override..................................................................................... 60 8.1.2.3 Multiple-spindle Control.......................................................................... 60
8.1.2.3.1 Multiple-spindle Control I..................................................... 61 8.1.3 Position Control................................................................................................... 62
8.1.3.1 Spindle Orientation................................................................................. 62 8.1.3.3 Spindle Synchronization......................................................................... 63
8.1.3.3.1 Spindle Synchronization I ....................................................... 63 8.1.3.3.2 Spindle Synchronization II ...................................................... 64
8.2 Tool Functions (T)........................................................................................................ 65 8.2.1 Tool Functions..................................................................................................... 65
8.3 Miscellaneous Functions (M)....................................................................................... 66 8.3.1 Miscellaneous Functions..................................................................................... 66 8.3.2 Multiple M Codes in 1 Block................................................................................ 66 8.3.3 M Code Independent Output .............................................................................. 67 8.3.4 Miscellaneous Function Finish............................................................................ 67 8.3.5 M Code Output during Axis Positioning.............................................................. 68
8.4 2nd Miscellaneous Function (B) .................................................................................. 69 8.4.1 2nd Miscellaneous Function ............................................................................... 69
9. Tool Compensation ........................................................................................................... 70
9.1 Tool Length/Position Offset; G43 to G49 .................................................................... 70 9.1.1 Tool Length Offset............................................................................................... 70 9.1.3 Tool Offset for Additional Axes ........................................................................... 72
9.2 Tool Radius; G38 to G42, G46 .................................................................................... 73 9.2.1 Tool radius Compensation; G38 to G42 ............................................................. 73 9.2.3 Tool Nose Radius Compensation (G40/41/42) .................................................. 75 9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40)............ 76
9.3 Tool Offset Amount ...................................................................................................... 77 9.3.1 Number of Tool Offset Sets ................................................................................ 77
9.3.1.2 40 sets ................................................................................................... 77 9.3.1.3 80 sets ................................................................................................... 77 9.3.1.4 100 sets ................................................................................................. 77 9.3.1.5 200 sets ................................................................................................. 77
9.3.2 Offset Memory..................................................................................................... 78 9.3.2.1 Tool Shape/Wear Offset Amount ........................................................... 78
10. Coordinate System..................................................................................................... 81
10.1 Coordinate System Type and Setting; G52 to G59, G92.......................................... 81 10.1.1 Machine Coordinate System; G53.................................................................... 82 10.1.2 Coordinate System Setting; G92 ...................................................................... 83 10.1.3 Automatic Coordinate System Setting.............................................................. 84 10.1.4 Workpiece Coordinate System Selection (6 sets); G54 to G59 ....................... 85 10.1.5 Extended Workpiece Coordinates System Selection....................................... 86 10.1.7 Local Coordinate System; G54G52 to G59G52............................................... 87 10.1.8 Coordinate System for Rotary Axis................................................................... 88
iv
10.1.9 Plane Selection; G17 to G19 ............................................................................ 88 10.1.10 Origin Set ........................................................................................................ 89 10.1.11 Counter Set ..................................................................................................... 89
10.2 Return; G27 to G30.................................................................................................... 90 10.2.1 Manual Reference Point Return ....................................................................... 90 10.2.2 Automatic 1st Reference Point Return; G28, G29 ........................................... 91 10.2.3 2nd, 3rd, 4th Reference Point Return; G30...................................................... 93 10.2.4 Reference Point Verification; G27 .................................................................... 94 10.2.5 Absolute position detection............................................................................... 95 10.2.6 Tool Exchange Point Return; G30.1 to G30.6.................................................. 96
11. Operation Support Functions ................................................................................... 97
11.1 Program Control......................................................................................................... 97 11.1.1 Optional Block Skip........................................................................................... 97 11.1.3 Single Block ...................................................................................................... 98
11.2 Program Test ............................................................................................................. 99 11.2.1 Dry Run ............................................................................................................. 99 11.2.2 Machine Lock .................................................................................................... 99 11.2.3 Miscellaneous Function Lock............................................................................ 100
11.3 Program Search/Start/Stop........................................................................................ 101 11.3.1 Program Search................................................................................................ 101 11.3.2 Sequence Number Search ............................................................................... 101 11.3.5 Automatic Operation Start................................................................................. 102 11.3.6 NC Reset........................................................................................................... 102 11.3.7 Feed Hold.......................................................................................................... 103 11.3.8 Search & Start................................................................................................... 103
11.4 Interrupt Operation..................................................................................................... 104 11.4.1 Manual Interruption ........................................................................................... 104 11.4.2 Automatic Operation Handle Interruption ......................................................... 105 11.4.3 Manual Absolute Mode ON/OFF ...................................................................... 106 11.4.4 Thread Cutting Cycle Retract............................................................................ 107 11.4.5 Tapping Retract................................................................................................. 108 11.4.6 Manual Numerical value Command ................................................................. 109 11.4.8 MDI Interruption ................................................................................................ 109 11.4.9 Simultaneous Operation of Manual and Automatic Modes.............................. 110 11.4.10 Simultaneous Operation of Jog and Handle Modes....................................... 110 11.4.11 Reference Point Retract.................................................................................. 111
12. Program Support Functions...................................................................................... 112
12.1 Machining Method Support Functions....................................................................... 112 12.1.1 Program............................................................................................................. 112
12.1.1.1 Subprogram Control ............................................................................. 112 12.1.2 Macro Program ................................................................................................. 114
12.1.2.1 User Macro........................................................................................... 114 12.1.2.3 Macro Interruption ................................................................................ 117 12.1.2.4 Variable Command............................................................................... 118
12.1.2.4.6 (50+50 x number of part systems) sets................................ 118 12.1.2.4.7 (100+100 x number of part systems) sets............................ 118 12.1.2.4.8 (200+100 x number of part systems) sets............................ 118
12.1.3 Fixed Cycle........................................................................................................ 119 12.1.3.1 Fixed Cycle for Drilling ......................................................................... 120 12.1.3.2 Special Fixed Cycle; G34 to G37......................................................... 126 12.1.3.3 Fixed Cycle for Turning Machining; G77 to G79.................................. 130 12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining; G70 to G76... 135
v
12.1.4 Mirror Image...................................................................................................... 143
12.1.4.3 G Code Mirror Image............................................................................ 143 12.1.4.4 Mirror Image for Facing Tool Posts...................................................... 144
12.1.5 Coordinate System Operation .......................................................................... 145 12.1.5.1 Coordinate Rotation by Program ......................................................... 145
12.1.6 Dimension Input ................................................................................................ 147 12.1.6.1 Corner Chamfering / Corner R............................................................. 147 12.1.6.3 Geometric Command ........................................................................... 151
12.1.7 Axis Control ....................................................................................................... 155 12.1.7.5 Circular Cutting..................................................................................... 155
12.1.8 Multi-part System Control ................................................................................. 156 12.1.8.1 Synchronization between Part Systems .............................................. 156 12.1.8.2 Start Point Designation Synchronization.............................................. 158 12.1.8.6 Balance Cut (G14/G15)........................................................................ 160 12.1.8.8 2-part System Synchronous Thread Cutting (G76.1/G76.2) ............... 161
12.1.9 Data Input by Program...................................................................................... 163 12.1.9.1 Parameter Input by Program................................................................ 163 12.1.9.2 Compensation Data Input by Program................................................. 164
12.1.10 Machining Modal............................................................................................. 166 12.1.10.1 Tapping Mode; G63 ........................................................................... 166 12.1.10.2 Cutting Mode; G64 ............................................................................. 166
12.2 Machining Accuracy Support Functions.................................................................... 167 12.2.1 Automatic Corner Override; G62 ...................................................................... 167 12.2.2 Deceleration Check........................................................................................... 168
12.2.2.1 Exact Stop Mode; G61 ......................................................................... 169 12.2.2.2 Exact Stop Check; G09........................................................................ 169 12.2.2.3 Error Detect .......................................................................................... 169 12.2.2.4 Programmable In-position Check......................................................... 170
12.2.3 High-Accuracy Control; G61.1 .......................................................................... 171 12.3 Programming Support Functions............................................................................... 173
12.3.2 Address Check.................................................................................................. 173
13. Machine Accuracy Compensation............................................................................ 174 13.1 Static Accuracy Compensation.................................................................................. 174
13.1.1 Backlash Compensation ................................................................................... 174 13.1.2 Memory-type Pitch Error Compensation .......................................................... 175 13.1.3 Memory-type Relative Position Error Compensation ....................................... 176 13.1.4 External Machine Coordinate System Compensation...................................... 176 13.1.6 Ball Screw Thermal Expansion Compensation............................................... 177
13.2 Dynamic Accuracy Compensation ............................................................................ 178 13.2.1 Smooth High-gain Control (SHG Control) ........................................................ 178 13.2.2 Dual Feedback.................................................................................................. 179 13.2.3 Lost Motion Compensation ............................................................................... 179
14. Automation Support Functions ..................................................................................... 180
14.1 External Data Input .................................................................................................... 180 14.1.1 External Search................................................................................................. 180 14.1.2 External Workpiece Coordinate Offset ............................................................. 181
14.2 Measurement; G31, G37 ........................................................................................... 182 14.2.1 Skip ................................................................................................................... 182
14.2.1.1 Skip....................................................................................................... 182 14.2.1.2 Multiple-step Skip ................................................................................. 183
14.2.5 Automatic Tool Length Measurement............................................................... 185 14.2.6 Manual Tool Length Measurement 1................................................................ 188
14.3 Monitoring .................................................................................................................. 189 14.3.1 Tool Life Management ...................................................................................... 189
14.3.1.2 Tool Life Management II ...................................................................... 189
vi
14.3.2 Number of Tool Life Management Sets............................................................ 189 14.3.3 Display of Number of Parts ............................................................................... 189 14.3.4 Load Meter ........................................................................................................ 190 14.3.5 Position Switch.................................................................................................. 190
14.5 Others ........................................................................................................................ 191 14.5.1 Programmable Current Limitation..................................................................... 191 14.5.4 Automatic Restart.............................................................................................. 191
15. Safety and Maintenance.................................................................................................. 192
15.1 Safety Switches ......................................................................................................... 192 15.1.1 Emergency Stop................................................................................................ 192 15.1.2 Data Protection Key .......................................................................................... 192
15.2 Display for Ensuring Safety ....................................................................................... 193 15.2.1 NC Warning....................................................................................................... 193 15.2.2 NC Alarm........................................................................................................... 193 15.2.3 Operation Stop Cause ...................................................................................... 194 15.2.4 Emergency Stop Cause.................................................................................... 194 15.2.5 Temperature Detection ..................................................................................... 194
15.3 Protection................................................................................................................... 195 15.3.1 Stroke End (Over Travel) .................................................................................. 195 15.3.2 Stored Stroke Limit............................................................................................ 195
15.3.2.1 Stored Stroke Limit I/II......................................................................... 196 15.3.2.2 Stored Stroke Limit IB ......................................................................... 198 15.3.2.3 Stored Stroke Limit IIB ........................................................................ 199 15.3.2.4 Stored Stroke Limit IC ......................................................................... 199
15.3.3 Stroke Check Before Movement....................................................................... 199 15.3.4 Chuck/Tail Stock Barrier Check; G22/G23....................................................... 200 15.3.5 Interlock............................................................................................................. 201 15.3.6 External Deceleration........................................................................................ 201 15.3.8 Door Interlock................................................................................................... 202
15.3.8.1 Door Interlock I .................................................................................... 202 15.3.8.2 Door Interlock II ................................................................................... 203
15.3.9 Parameter Lock................................................................................................ 204 15.3.10 Program Protect (Edit Lock B, C) ................................................................... 204 15.3.11 Program Display Lock..................................................................................... 205
15.4 Maintenance and Troubleshooting ............................................................................ 206 15.4.1 History Diagnosis .............................................................................................. 206 15.4.2 Setup/Monitor for Servo and Spindle................................................................ 206 15.4.3 Data Sampling................................................................................................... 206 15.4.5 Machine Operation History Monitor .................................................................. 207 15.4.6 NC Data Backup ............................................................................................... 207 15.4.7 PLC I/F Diagnosis ............................................................................................. 207
16. Cabinet and Installation .................................................................................................. 208
16.1 Cabinet Construction ................................................................................................. 208 16.2 Power Supply, Environment and Installation Conditions .......................................... 211
17. Servo/Spindle System..................................................................................................... 213
17.1 Feed Axis ................................................................................................................... 213 17.1.1 MDS-C1-V1/C1-V2 (200V) ............................................................................... 213 17.1.4 MDS-B-SVJ2 (Compact and Small Capacity) .................................................. 213 17.1.6 MDS-R-V1/R-V2 (200V Compact and Small Capacity)................................ 213
17.2 Spindle ....................................................................................................................... 214 17.2.1 MDS-C1-SP/C1-SPM/B-SP (200V) .................................................................. 214 17.2.3 MDS-B-SPJ2 (Compact and Small Capacity) .................................................. 214
vii
17.3 Auxiliary Axis.............................................................................................................. 214 17.3.1 Index/Positioning Servo: MR-J2-CT ................................................................. 214
17.4 Power Supply............................................................................................................. 215 17.4.1 Power Supply: MDS-C1-CV/B-CVE ................................................................. 215 17.4.2 AC Reactor for Power Supply........................................................................... 215 17.4.3 Ground Plate ..................................................................................................... 215 17.4.4 Power Supply: MDS-A-CR (Resistance Regeneration) ................................... 215
18. Machine Support Functions ........................................................................................... 216
18.1 PLC ............................................................................................................................ 216 18.1.1 PLC Basic Function .......................................................................................... 216
18.1.1.1 Built-in PLC Basic Function.................................................................. 216 18.1.2 Built-in PLC Processing Mode .......................................................................... 220
18.1.2.2 MELSEC Development Tool I/F........................................................... 220 18.1.3 Built-in PLC Capacity (Number of Steps) ......................................................... 220 18.1.4 Machine Contact Input/Output I/F..................................................................... 221 18.1.6 PLC Development............................................................................................. 225
18.1.6.2 MELSEC Development Tool ................................................................ 225 18.1.7 C Language Function........................................................................................ 225 18.1.12 GOT Connection ............................................................................................. 226
18.1.12.1 CPU Direct Connection (RS-422/RS-232C)................................... 226 18.1.12.2 CC-Link Connection (Remote Device)............................................... 227 18.1.12.3 CC-Link Connection (Intelligent Terminal) ..................................... 227 18.1.12.5 Ethernet Connection ...................................................................... 228
18.1.13 PLC Message.................................................................................................. 229 18.1.13.1 Japanese............................................................................................ 229 18.1.13.2 English................................................................................................ 229 18.1.13.13 Polish................................................................................................ 229
18.2 Machine Construction ................................................................................................ 230 18.2.1 Servo OFF......................................................................................................... 230 18.2.2 Axis Detach ....................................................................................................... 231 18.2.3 Synchronous Control ........................................................................................ 232
18.2.3.1 Position Tandem .................................................................................. 232 18.2.3.2 Speed Tandem................................................................................. 234 18.2.3.3 Torque Tandem................................................................................ 234
18.2.7 Auxiliary Axis Control (J2-CT)........................................................................... 235 18.3 PLC Operation ........................................................................................................... 236
18.3.1 Arbitrary Feed in Manual Mode ........................................................................ 236 18.3.3 PLC Axis Control............................................................................................... 237
18.4 PLC Interface ............................................................................................................. 238 18.4.1 CNC Control Signal........................................................................................... 238 18.4.2 CNC Status Signal ............................................................................................ 239 18.4.5 DDB................................................................................................................... 241
18.5 Machine Contact I/O .................................................................................................. 242 18.6 External PLC Link ...................................................................................................... 243
18.6.4 CC-Link ............................................................................................................. 243 18.6.6 DeviceNet (Master/Slave) ................................................................................. 247 18.6.7 MELSEC-Q Series Input/Output/Intelligent Function Unit Connection ............ 248 18.6.9 MELSECNET/10 ............................................................................................... 250 18.6.10 Ethernet I/F (MELSEC Communication Protocol) .......................................... 254
18.7 Installing S/W for Machine Tools ............................................................................... 255 18.7.1 APLC................................................................................................................. 255 18.7.6 EzSocket I/F...................................................................................................... 255
viii
Appendix 1. List of Specifications....................................................................................... 256 Appendix 2. Outline and Installation Dimension Drawings of Units ............................... 257
Appendix 2.1 Outline Drawing of Control Unit.................................................................. 257 Appendix 2.2 Outline Drawing of Communication Terminal ............................................ 258
Appendix 2.2.1 FCUA-CT100 ..................................................................................... 258 Appendix 2.2.2 FCUA-CR10....................................................................................... 259 Appendix 2.2.3 FCUA-LD100 ..................................................................................... 260 Appendix 2.2.4 FCUA-LD10, KB20 ............................................................................ 261 Appendix 2.2.5 FCU6-DUT32, KB021........................................................................ 262 Appendix 2.2.6 Communication Terminal................................................................... 263
Appendix 2.3 Outline Drawing of Remote I/O Unit ........................................................... 264 Appendix 3. List of Specifications....................................................................................... 265
1. Control Axes 1.1 Control Axes
- 1 -
1. Control Axes The NC axis, spindle, PLC axis are generically called the control axis. The NC axis is an axis that can be manually operated, or automatically operated with the machining program. The PLC axis is an axis that can be controlled from the PLC ladder.
1.1 Control Axes
1.1.1 Number of Basic Control Axes (NC axes) C6 C64
T system L system M system L system T system 1 2 3 2 1
1.1.2 Max. Number of Control Axes (NC axes + Spindles + PLC axes + Auxiliary axes) A number of axes that are within the maximum number of control axes, and that does not exceed the maximum number given for the NC axis, spindle, PLC axis and auxiliary axis can be used. For example, if 14 NC axes are used, this alone is the maximum number of control axes, so a spindle, PLC axis and auxiliary axis cannot be connected. The connection order is the NC axis, PLC axis, spindle and auxiliary axis. Max. number of control axes (NC axes + spindles + PLC axes + auxiliary axes)
C6 C64 T system L system M system L system T system
7 7 14 14 14 Max. number of axes (NC axes + spindles + PLC axes)
C6 C64 T system L system M system L system T system
4 6 14 14 14
Max number of servo axes (NC axes + PLC axes)
C6 C64 T system L system M system L system T system
2 4 14 14 14 Max. number of NC axes (in total for all the part systems)
C6 C64 T system L system M system L system T system
2 4 14 12 14
1. Control Axes 1.1 Control Axes
- 2 -
Max. number of spindles Includes analog spindles.
C6 C64
T system L system M system L system T system 2 (1) 2 (1) 3 4 7 (1)
Values in parentheses indicate the maximum number of spindles per part system. Max. number of PLC axes
C6 C64 T system L system M system L system T system
7 7 7 Max. number of auxiliary axes (MR-J2-CT)
C6 C64 T system L system M system L system T system
5 5 7 7 7
1.1.3 Number of Simultaneous Contouring Control Axes Simultaneous control of all axes is possible as a principle in the same part system. However, for actual use, the machine tool builder specification will apply.
C6 C64 T system L system M system L system T system
2 2 4 4 2
1.1.4 Max. Number of NC Axes in a Part System C6 C64
T system L system M system L system T system 2 2 6 4 2
1.2 Control Part System
1.2.1 Standard Number of Part Systems C6 C64
T system L system M system L system T system 1 1 1 1 1
1.2.2 Max. Number of Part Systems C6 C64
T system L system M system L system T system 2 2 3 3 7
For actual use, the machine tool builder specification will apply.
1. Control Axes 1.3 Control Axes and Operation Modes
- 3 -
1.3 Control Axes and Operation Modes
1.3.2 Memory Mode C6 C64
T system L system M system L system T system
The machining programs stored in the memory of the NC unit are run.
1.3.3 MDI Mode C6 C64
T system L system M system L system T system
The MDI data stored in the memory of the NC unit is executed. Once executed, the MDI data is set to the "setting incomplete" status, and the data will not be executed unless the "setting completed" status is established by performing screen operations.
2. Input Command 2.1 Data Increment
- 4 -
2. Input Command 2.1 Data Increment
Least command increment: 1 m (Least input increment: 1 m)
C6 C64 T system L system M system L system T system
Least command increment: 0.1 m (Least input increment: 0.1 m)
C6 C64 T system L system M system L system T system
The data increment handled in the controller include the least input increment, least command increment and least detection increment. Each type is set with parameters. (1) The least input increment indicates the increment handled in the internal processing of the
controller. The counter and tool offset data, etc., input from the screen is handled with this increment. This increment is applied per part system (all part systems, PLC axis).
Metric unit system Inch unit system
Increment type Input
increment (parameter)
Linear axis (Unit = mm)
Rotary axis (Unit = )
Linear axis (Unit = inch)
Rotary axis (Unit = )
B 0.001 0.001 0.0001 0.001 Least input increment C 0.0001 0.0001 0.00001 0.0001
(Note) The inch and metric systems cannot be used together.
(2) The command increment indicates the command increment of the movement command in the machining program. This can be set per axis.
Metric unit system Inch unit system
Increment type Command increment
(parameter) Linear axis (Unit = mm)
Rotary axis (Unit = )
Linear axis (Unit = inch)
Rotary axis (Unit = )
10 0.001 0.001 0.0001 0.001 100 0.01 0.01 0.001 0.01
1000 0.1 0.1 0.01 0.1 Command increment
10000 1.0 1.0 0.1 1.0
(Note) The inch and metric systems cannot be used together.
(3) The least detection increment indicates the detection increment of the NC axis and PLC axis detectors. The increment is determined by the detector being used.
2. Input Command 2.2 Unit System
- 5 -
2.2 Unit System
2.2.1 Inch/Metric Changeover; G20/G21 C6 C64
T system L system M system L system T system
The unit systems of the data handled in the controller include the metric unit system and inch unit system. The type can be designated with the parameters and machining program. The unit system can be set independently for the (1) Program command, (2) Setting data such as offset amount and (3) Parameters.
Unit system Length data Meaning Metric unit system 1.0 1.0 mm Inch unit system 1.0 1.0 inch
(Note) For the angle data, 1.0 means 1 degree () regardless of the unit system.
Data Parameter
Machining program Screen data
(Offset amount, etc.) Parameter
G20 Inch unit system 0 G21 Metric unit system Metric unit system
G20 Inch unit system I_inch 1 G21 Metric unit system Inch unit system
Not affected
0 Metric unit system M_inch 1 Not affected Not affected Inch unit system (Note 1) The parameter changeover is valid after the power is turned ON again. (Note 2) Even if parameter "I_inch" is changed, the screen data (offset amount, etc.) will not be
automatically converted. (Note 3) When the power is turned ON or resetting is performed, the status of the G20/G21 modal
depends on the "I_G20" parameter setting.
2. Input Command 2.3 Program Format
- 6 -
2.3 Program Format
2.3.1 Character Code C6 C64
T system L system M system L system T system
The command information used in this CNC system consists of alphanumerics and symbols which are collectively known as characters. These characters are expressed as combinations of 8-bit data inside the NC unit. The expressions formed in this way are called codes, and this CNC system uses shift JIS codes. The characters which are valid in this CNC system are listed below.
Character Remarks 0 to 9 Always significant A to Z Always significant + Always significant Always significant . Always significant , Always significant / Always significant % Always significant CR Always significant LF/NL Always significant ( Always significant ) Always significant : Always significant # Always significant Always significant = Always significant [ Always significant ] Always significant SP Always significant ! Always significant $ Always significant BS An error results during operation (except when the character is part of a comment). HT An error results during operation (except when the character is part of a comment). & An error results during operation (except when the character is part of a comment). '(Apostrophe) An error results during operation (except when the character is part of a comment). ; An error results during operation (except when the character is part of a comment). < An error results during operation (except when the character is part of a comment). > An error results during operation (except when the character is part of a comment). ? An error results during operation (except when the character is part of a comment). @ An error results during operation (except when the character is part of a comment). " An error results during operation (except when the character is part of a comment). DEL Always ignored NULL Always ignored
2. Input Command 2.3 Program Format
- 7 -
2.3.2 Program Format
2.3.2.1 Format 1 for Lathe (G code list 2, 3) C6 C64
T system L system M system L system T system
The G-code of L system is selected by parameter. This specification manual explains the G function with G-code series 3 as standard.
2.3.2.4 Format 1 for Machining Center (G code list 1) C6 C64
T system L system M system L system T system
2. Input Command 2.4 Command Value
- 8 -
2.4 Command Value
2.4.1 Decimal Point Input I, II C6 C64
T system L system M system L system T system
There are two types of the decimal point input commands and they can be selected by parameter.
(1) Decimal point input type I (When parameter #1078 Decpt2 is 0.) When axis coordinates and other data are supplied in machining program commands, the assignment of the program data can be simplified by using the decimal point input. The minimum digit of a command not using a decimal point is the same as the least command increment. Usable addresses can be applied not only to axis coordinate values but also to speed commands and dwell commands. The decimal point position serves as the millimeter unit in the metric mode, as the inch unit in the inch mode and as the second unit in a time designation of dwell command.
(2) Decimal point input type II (When parameter #1078 Decpt2 is 1.)
As opposed to type I, when there is no decimal point, the final digit serves as the millimeter unit in the metric mode, as the inch unit in the inch mode and as the second unit in the time designation. The "." (point) must be added when commands below the decimal point are required.
Unit interpretation (for metric system)
Type I Type II G00 X100. Y-200.5 X100mm, Y-200.5mm G1 X100 F20. X100m, F20mm/min X100mm, F20mm/min G1 Y200 F100 (*1) Y200m, F100mm/min Y200mm, F100mm/min G4 X1.5 Dwell 1.5 s G4 X2 2ms 2s (*1) The F unit is mm/min for either type (inch system : inch/min).
2. Input Command 2.4 Command Value
- 9 -
2.4.2 Absolute/Incremental Command; G90/G91 C6 C64
T system L system M system L system T system
(1) T system, M system
When axis coordinate data is issued in a machining program command, either the incremental command method (G91) that commands a relative distance from the current position or the absolute command method (G90) that moves to a designated position in a predetermined coordinate system can be selected. The absolute and incremental commands can be both used in one block, and are switched with G90 or G91. However, the arc radius designation (R) and arc center designation (I, J, K) always use incremental designations.
G90 ... Absolute command (absolute value command) G91 ... Incremental command (incremental value command)
These G codes can be commanded multiple times in one block. Example G90 X100. G91 Y200. G90 Z300. ;
Absolute value Incremental value Absolute value
(Note 1) As with the memory command, if there is no G90/G91 designation in the MDI command, the previously executed modal will be followed.
(Incremental value command) (Absolute value command)
End pointY100.
(0, 0) X 100.
Current position
End point
G 91 X 100. Y100. ;
X 100.
G 90 X 100. Y100. ;
Y100. Y100.
X100. (0, 0)
Program coordinate
Current position
2. Input Command 2.4 Command Value
- 10 -
(2) L system When axis coordinate data is issued in a machining program command, either the incremental command method that commands a relative distance from the current position or the absolute command method that moves to a designated position in a predetermined coordinate system can be selected. When issuing an incremental value command, the axis address to be commanded as the incremental axis name is registered in the parameter. However, the arc radius designation (R) and arc center designation (I, J, K) always use incremental designations.
Absolute command (absolute value command) ... X, Z Incremental command (incremental value command) ... U, W
Example G00 X100. W200. ;
Absolute value Incremental value
End point
Current position
2
u1
The above drawing shows the case for the diameter command.
X X
Z
(Incremental value command) (Absolute value command)
G 00 U u1 W w1 ; G 00 X x1 Z z1 ;
The above drawing shows the case for the diameter command.
Z
w1
z1
End point
Current position
x1
(0,0)
(Note) In addition to the above command method using the above axis addresses, the absolute
value command and incremental value command can be switched by commanding the G code (G90/G91). (Select with the parameters.)
2. Input Command 2.4 Command Value
- 11 -
2.4.3 Diameter/Radius Designation C6 C64
T system L system M system L system T system
For axis command value, the radius designation or diameter designation can be changed over with parameters. When the diameter designation is selected, the scale of the length of the selected axis is doubled. (For instance, an actual length of 1 mm will be treated as 2 mm.) This function is used when programming the workpiece dimensions on a lathe as diameters. Changing over from the diameter designation to the radius designation or vice versa can be set separately for each axis.
x6 u4
x6
u4
Coordinate zero point
X-axis radius designation
Z Z
X X X-axis diameter designation
Coordinate zero point
The difference in the diameter designation and radius designation is shown below.
Absolute value command Incremental value command Radius designation Diameter designation Radius designation Diameter designation Actual movement amount = x1
Actual movement amount = 2 x1
Actual movement amount = u1
Actual movement amount = 2 u1
2. Input Command 2.5 Command Value and Setting Value Range
- 12 -
2.5 Command Value and Setting Value Range
2.5.1 Command Value and Setting Value Range C6 C64
T system L system M system L system T system
[T system, M system] Metric command Inch command Rotary axis
(Metric command) Rotary axis
(Inch command) Program number 08 Sequence number N5 Preparatory function G3/G21
0.001() mm/ 0.0001 inch X+53 Y+53 Z+53 +53 X+44 Y+44 Z+44 +44 X+53 Y+53 Z+53 +53 X+53 Y+53 Z+53 +53Movement
axis 0.0001() mm/ 0.00001 inch X+44 Y+44 Z+44 +44 X+35 Y+35 Z+35 +35 X+44 Y+44 Z+44 +44 X+44 Y+44 Z+44 +44
0.001() mm/ 0.0001 inch I+53 J+53 K+53 R+53 I+44 J+44 K+44 R+44 I+53 J+53 K+53 R+53 I+44 J+44 K+44 R+44
(Note 5)Arc and cutter radius 0.0001() mm/
0.00001 inch I+44 J+44 K+44 R+44 I+35 J+35 K+35 R+35 I+44 J+44 K+44 R+44 I+35 J+35 K+35 R+35 (Note 5)
0.001() mm/ 0.0001 inch X+53/P+8
Dwell 0.0001() mm/ 0.00001 inch X+44/P+8
0.001() mm/ 0.0001 inch
F63(Feed per minute) F43(Feed per revolution)
F44(Feed per minute) F34(Feed per revolution)
F63(Feed per minute) F43(Feed per revolution)
F44(Feed per minute) F34(Feed per revolution)
(Note 6)Feed function 0.0001 () mm/
0.00001 inch F54(Feed per minute)
F34(Feed per revolution) F35(Feed per minute)
F25(Feed per revolution) F54(Feed per minute)
F34(Feed per revolution)
F35(Feed per minute) F25(Feed per revolution)
(Note 6) Tool offset H3 D3 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4
0.001() mm/ 0.0001 inch R+53 Q53 P8 L4 Fixed
cycle 0.0001() mm/ 0.00001 inch R+44 Q44 P8 L4
2. Input Command 2.5 Command Value and Setting Value Range
- 13 -
[L system] Metric command Inch command Rotary axis
(Metric command) Rotary axis
(Inch command) Program number 08 Sequence number N5 Preparatory function G3/G21
0.001() mm/ 0.0001 inch X+53 Z+53 +53 X+44 Z+44 +44 X+53 Z+53 +53 X+53 Z+53 +53 Movement
axis 0.0001() mm/ 0.00001 inch X+44 Z+44 +44 X+35 Z+35 +35 X+44 Z+44 +44 X+44 Z+44 +44
0.001() mm/ 0.0001 inch I+53 K+53 R+53 I+44 K+44 R+44 I+53 K+53 R+53 I+44 K+44 R+44
(Note 5)Arc and cutter radius 0.0001() mm/
0.00001 inch I+44K+44 R+44 I+35 K+35 R+35 I+44 K+44 R+44 I+35 K+35 R+35 (Note 5)
0.001() mm/ 0.0001 inch X+53/P+8
Dwell 0.0001() mm/ 0.00001 inch X+44/P+8
0.001() mm/ 0.0001 inch
F63(Feed per minute) F43(Feed per revolution)
F44(Feed per minute) F34(Feed per revolution)
F63(Feed per minute) F43(Feed per revolution)
F44(Feed per minute) F34(Feed per revolution)
(Note 6)Feed function 0.0001() mm/
0.00001 inch F54(Feed per minute)
F34(Feed per revolution) F35(Feed per minute)
F25(Feed per revolution) F54(Feed per minute)
F34(Feed per revolution)
F35(Feed per minute) F25(Feed per revolution)
(Note 6) Tool offset T1/T2 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4
0.001() mm/ 0.0001 inch R+53 Q53 P8 L4 Fixed
cycle 0.0001() mm/ 0.00001 inch R+44 Q44 P8 L4
(Note 1) indicates the additional axis address, such as A, B or C. (Note 2) The No. of digits check for a word is carried out with the maximum number of digits of
that address.
(Note 3) Numerals can be used without the leading zeros. (Note 4) The meanings of the details are as follows :
Example 1 : 08 : 8-digit program number Example 2 : G21 : Dimension G is 2 digits to the left of the decimal point, and 1 digit to
the right. Example 3 : X+53 : Dimension X uses + or - sign and represents 5 digits to the left of the
decimal point and 3 digits to the right. For example, the case for when the X axis is positioned (G00) to the 45.123 mm position in the absolute value (G90) mode is as follows : G00 X45.123 ;
3 digits below the decimal point 5 digits above the decimal point, so it's +00045, but the leading zeros and the mark (+) have been omitted. G0 is possible, too.
2. Input Command 2.5 Command Value and Setting Value Range
- 14 -
(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the degrees will be converted into 0.1 inches for interpolation.
(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees. Example : With the F1. (per-minute-feed) command, this will become the 10
degrees/minute command.
(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command, with an invalid decimal point has been assigned with a decimal point.
(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit.
(Note 9) Command the program No. in an independent block. Command the program No. in the head block of the program.
2. Input Command 2.5 Command Value and Setting Value Range
- 15 -
Linear axis Rotary axis Input unit: mm Input unit: inch Degree () Least setting increment 0.001/0.0001 0.0001/0.00001 0.001/0.0001 Maximum stroke (Value on machine coordinate system)
99999.999 mm 9999.9999 mm
9999.9999 inch 999.99999 inch
99999.999 9999.9999
Maximum command value 99999.999 mm 9999.9999 mm
9999.9999 inch 999.99999 inch
99999.999 9999.9999
Rapid traverse rate (Including during dry run)
1 to 1000000 mm/min 1 to 100000 mm/min
1 to 39370 inch/min 1 to 3937 inch/min
1 to 1000000 /min 1 to 100000 /min
M system cutting feed rate (Including during dry run)
0.01 to 1000000 mm/min 0.001 to 100000 mm/min
0.001 to 100000 inch/min 0.0001 to 10000 inch/min
0.01 to 1000000 /min 0.001 to 100000 /min
L system cutting feed rate (Including during dry run)
0.001 to 1000000 mm/min 0.0001 to 100000 mm/min
0.0001 to 39370.0787 inch/min 0.00001 to 3937.00787 inch/min
0.001 to 1000000 /min 0.0001 to 100000 /min
M system synchronous feed 0.001 to 999.999 mm/rev 0.0001 to 99.9999 mm/rev
0.0001 to 999.9999 inch/rev 0.00001 to 99.99999 inch/rev
0.01 to 999.99 /rev 0.001 to 99.999 /rev
L system synchronous feed 0.0001 to 999.9999 mm/rev 0.00001 to 99.99999 mm/rev
0.000001 to 99.999999 inch/rev 0.0000001 to 9.9999999 inch/rev
0.0001 to 999.9999 /rev 0.00001 to 99.99999 /rev
2nd to 4th reference point offset (value on machine coordinate system)
99999.999 mm 9999.9999 mm
9999.9999 inch 999.99999 inch
99999.999 9999.9999
Tool offset amount (shape) 999.999 mm 99.9999 mm
99.9999 inch 9.99999 inch
Tool offset amount (wear) 9999.999 mm 999.9999 mm
9.9999 inch 0.99999 inch
Incremental feed amount 0.001 mm/pulse 0.0001 mm/pulse
0.0001 inch/pulse 0.00001 inch/pulse
0.001 /pulse 0.0001 /pulse
Handle feed amount 0.001 mm/pulse 0.0001 mm/pulse
0.0001 inch/pulse 0.00001 inch/pulse
0.001 /pulse 0.0001 /pulse
Soft limit range (value on machine coordinate system)
99999.999 mm to +99999.999 mm 9999.9999 mm to +9999.9999 mm
9999.9999 inch to +9999.9999 inch 999.99999 inch to +999.99999 inch
1 to 359.999 1 to 359.9999
Dwell time 0 to 99999.999 s 0 to 99999.999 s Backlash compensation amount
0 to 9999 pulse 0 to 9999 pulse 0 to 9999 pulse
Pitch error compensation 0 to 9999 pulse 0 to 9999 pulse 0 to 9999 pulse M system thread lead (F) 0.001 to 999.999 mm/rev
0.0001 to 99.9999 mm/rev 0.0001 to 99.9999 inch/rev 0.00001 to 9.99999 inch/rev
M system thread lead (Precise E)
0.00001 to 999.99999 mm/rev 0.000001 to 99.999999 mm/rev
0.000001 to 39.370078 inch/rev 0.000001 to 3.937007 inch/rev
L system thread lead (F) 0.0001 to 999.9999 mm/rev 0.00001 to 99.99999 mm/rev
0.000001 to 99.999999 inch/rev 0.0000001 to 9.9999999 inch/rev
L system thread lead (Precise E)
0.00001 to 999.99999 mm/rev 0.000001 to 99.999999 mm/rev
0.000010 to 9.9999999 inch/rev 0.0000010 to 0.99999999 inch/rev
(Note 1) The second line in the table applies when the least setting increment is 0.001, 0.0001 from the first line.
3. Positioning/Interpolation 3.1 Positioning
- 16 -
3. Positioning/Interpolation 3.1 Positioning; G0, G60
3.1.1 Positioning; G0 C6 C64
T system L system M system L system T system
This function carries out positioning at high speed using rapid traverse with the movement command value given in the program.
G00 Xx1 Yy1 Zz1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)
x1, y1, z1: numerical values denoting the position data
The above command positions the tool by rapid traverse. The tool path takes the shortest distance to the end point in the form of a straight line. For details on the rapid traverse feed rate of the NC, refer to the section entitled "Rapid Traverse Rate". Since the actual rapid traverse feed rate depends on the machine, refer to the specifications of the machine concerned. (1) The rapid traverse feed rate for each axis can be set independently with parameters. (2) The number of axes which can be driven simultaneously depends on the specifications
(number of simultaneously controlled axes). The axes can be used in any combination within this range.
(3) The feed rate is controlled within the range that it does not exceed the rapid traverse rate of each axis and so that the shortest time is taken. (Linear type)
Parameter setting enables movement at the rapid traverse rates of the respective axes independently for each axis. In this case, the tool path does not take the form of a straight line to the end point. (Non-Linear type)
End pointY
X
G 00 G 91 X 100. Y 100. ;
Current position 100.
100.
(Example) Linear type (Moves lineary to the end point.)
(Example) Non-linear type (Each axis moves at
each parameter speed.)
Current position
X
Y
End point
100.
100.
G 00 G 91 X 100. Y 100. ;
(Note) If the acceleration/deceleration conditions differ between the axes, the path will not be linear to the end point even when using the linear type.
(4) The tool is always accelerated at the start of the program command block and decelerated at
the end of the block.
3. Positioning/Interpolation 3.1 Positioning
- 17 -
3.1.2 Unidirectional Positioning; G60 C6 C64
T system L system M system L system T system
The G60 command always moves the tool to the final position in a direction determined with parameters. The tool can be positioned without backlash.
G60 Xx1 Yy1 Zz1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)
x1, y1, z1: numerical values denoting the position data With the above command, the tool is first moved to a position distanced from the end point position by an amount equivalent to the creep distance (parameter setting) and then moved to its final position. For details on the rapid traverse feed rate of the NC, refer to the section entitled "Rapid Traverse Rate". Since the actual rapid traverse feed rate depends on the machine, refer to the specifications of the machine concerned.
Positioning to the final point is shown below (when this positioning is in the "+" direction.)
+
(Example)
1. The rapid traverse rate for each axis is the value set with parameters as the G00 speed.
2. The vector speed to the interim point is the value produced by combining the distance and respective speeds.
Interim point G60 G91 X100. Y100. ;
Current position X100.
Y100.
End point
3. The creep distance of the distance between the interim and end points can be set independently for each axis by "parameters".
3. Positioning/Interpolation 3.2 Linear/Circular Interpolation
- 18 -
(Note 1) The processing of the above pattern will be followed even for the machine lock and Z- axis command cancel.
(Note 2) On the creep distance, the tool is moved with rapid traverse.
(Note 3) G60 is valid even for positioning in drilling in the fixed cycle.
(Note 4) When the mirror image function is on, the tool will be moved in the reverse direction by mirror image as far as the interim position, but operation over the creep distance with the final advance will not be affected by the mirror image.
3.2 Linear/Circular Interpolation; G1, G2/G3
3.2.1 Linear Interpolation; G1 C6 C64
T system L system M system L system T system
Linear interpolation is a function that moves a tool linearly by the movement command value supplied in the program at the cutting feed rate designated by the F code.
G01 Xx1 Yy1 Zz1 Ff1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)
x1, y1, z1 : numerical values denoting the position data f1 : numerical value denoting the feed rate data
Linear interpolation is executed by the above command at the f1 feed rate. The tool path takes the shortest distance to the end point in the form of a straight line. For details on the f1 command values for NC, refer to the section entitled "Cutting Feed Rate". Since the actual cutting feed rate depends on the machine, refer to the specifications of the machine concerned. (Example)
Current position
100. (85mm/min)
Feed rate (120mm/min)
Y
G01 G91 X100. Y100. F120 ;
X
End point
100. (85mm/min)
1. The cutting feed rate command moves the tool in the vector direction.
2. The component speeds of each axis are determined by the proportion of respective command values to the actual movement distance with linear interpolation.
(1) The number of axes which can be driven simultaneously depends on the specifications
(number of simultaneously controlled axes). The axes can be used in any combination within this range.
(2) The feed rate is controlled so that it does not exceed the cutting feed rate clamp of each axis. (3) When a rotary axis has been commanded in the same block, it is treated as a linear axis in
degree() units (1 = 1mm), and linear interpolation is performed.
3. Positioning/Interpolation 3.2 Linear/Circular Interpolation
- 19 -
3.2.2 Circular Interpolation (Center/Radius Designation); G2/G3 C6 C64
T system L system M system L system T system
(1) Circular interpolation with I, J, K commands
This function moves a tool along a circular arc on the plane selected by the plane selection G code with movement command value supplied in the program.
G02(G03) Xx1 Yy1 Ii1 Jj1 Ff1 ; (Also possible for additional axes A, B, C, U, V, W) G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values Ii1, Jj1 : Arc center coordinate values Ff1 : Feed rate
The above commands move the tool along the circular arc at the f1 feed rate. The tool moves along a circular path, whose center is the position from the start point designated by distance "i1" in the X- axis direction and distance "j1" in the Y-axis direction, toward the end point. The direction of the arc rotation is specified by G02 or G03.
G02: Clockwise (CW) G03: Counterclockwise (CCW)
The plane is selected by G17, G18 or G19. G17: XY plane G18: ZX plane G19: YZ plane
(Example) See below for examples of circular
commands.
Center
Start point
I, J
F
Y
X
End point
X
Y G17 X
Z
Y
Z
G18
G19
G02
G03
G02
G03
G02
G03
(a) The axes that can be commanded simultaneously are the two axes for the selected plane. (b) The feed rate is controlled so that the tool always moves at a speed along the circumference
of the circle. (c) Circular interpolation can be commanded within a range extending from 0 to 360. (d) The max. value of the radius can be set up to six digits above the decimal point.
(Note 1) The arc plane is always based on the G17, G18 or G19 command. If a command is issued with two addresses which do not match the plane, an alarm will occur.
(Note 2) The axes configuring a plane can be designated by parameters. Refer to the section entitled "Plane Selection".
3. Positioning/Interpolation 3.2 Linear/Circular Interpolation
- 20 -
(2) R-specified circular interpolation Besides the designation of the arc center coordinates using the above-mentioned I, J and K commands, arc commands can also be issued by designating the arc radius directly.
G02(G03) Xx1 Yy1 Rr1 Ff1 ; (Also possible for additional axes A, B, C, U, V, W ) G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values Rr1 : Arc radius Ff1 : Feed rate
G02 or G03 is used to designate the direction of the arc rotation. The arc plane is designated by G17, G18 or G19. The arc center is on the bisector which orthogonally intersects the segment connecting the start and end points, and the point of intersection with the circle, whose radius has been designated with the start point serving as the center, is the center coordinate of the arc command. When the sign of the value of R in the command program is positive, the command will be for an arc of 180 or less; when it is negative, it will be for an arc exceeding 180.
(Example)
Current position (arc start point)
Y
G02 G91 X100. Y100. R100. F120 ;
R100.
X
Feed rate: 120mm/min
Arc end point coordinates (X, Y)
(a) The axes that can be commanded simultaneously are the two axes for the selected plane. (b) The feed rate is controlled so that the tool always moves at a speed along the circumference
of the circle.
(Note 1) The arc plane is always based on the G17, G18 or G19 command. If a command is issued with two addresses which do not match the plane, an alarm will occur.
3. Positioning/Interpolation 3.2 Linear/Circular Interpolation
- 21 -
3.2.3 Helical Interpolation C6 C64
T system L system M system L system T system
With this function, any two of three axes intersecting orthogonally are made to perform circular interpolation while the third axis performs linear interpolation in synchronization with the arc rotation. This simultaneous 3-axis control can be exercised to machine large-diameter screws or 3- dimensional cams.
G17 G02(G03) Xx1 Yy1 Zz1 Ii1 Jj1 Pp1 Ff1 ; G17 : Arc plane G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values for arc Zz1 : End point coordinate value of linear axis Ii1, Jj1 : Arc center coordinate values Pp1 : Pitch No. Ff1 : Feed rate (1) The arc plane is designated by G17, G18 or G19. (2) G02 or G03 is used to designate the direction of the arc rotation. (3) Absolute or incremental values can be assigned for the arc end point coordinates and the end
point coordinate of the linear axis, but incremental values must be assigned for the arc center coordinates.
(4) The linear interpolation axis is the other axis which is not included in the plane selection. (5) Command the speed in the component direction that represents all the axes combined for the
feed rate.
Pitch l1 is obtained by the formula below. l1 = z1/((2 p1 + )/2) = e s = arctan (ye/xe) arctan (ys/xs) Where xs, ys are the start point coordinates (0 < 2)
xe, ye are the end point coordinates The combination of the axes which can be commanded simultaneously depends on the specifications. The axes can be used in any combination under the specifications. The feed rate is controlled so that the tool always moves at a speed along the circumference of the circle.
3. Positioning/Interpolation 3.2 Linear/Circular Interpolation
- 22 -
(Example)
I-100 W
J100
X
Start point
Command program path
X
Y
Z
Y
End point
XY plane projection path in command program
End point
Start point
G91 G17 G02 X0. Y200. Z100. I100. J100.
(Note 1) Helical shapes are machined by assigning linear commands for one axis which is not a circular interpolation axis using an orthogonal coordinate system. It is also possible to assign these commands to two or more axes which are not circular interpolation axes.
End point
V Z
Y X
Start point
When a simultaneous 4-axis command is used with the V axis as the axis parallel to the Y axis, helical interpolation will result for a cylinder which is inclined as shown in the figure on the right. In other words, linear interpolation of the Z and V axes is carried out in synchronization with the circular interpolation on the XY plane.
4. Feed 4.1 Feed Rate
- 23 -
4. Feed 4.1 Feed Rate
4.1.1 Rapid Traverse Rate (m/min) C6 C64
T system L system M system L system T system 1000 1000 1000 1000 1000
[T system, M system]
The rapid traverse rate can be set independently for each axis. The rapid traverse rate is effective for G00, G27, G28, G29, G30 and G60 commands. Override can be applied to the rapid traverse rate using the external signal supplied.
Rapid Traverse Rate setting range
Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)
Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)
[L system] The rapid traverse rate can be set independently for each axis. The rapid traverse rate is effective for G00, G27, G28, G29, G30 and G53 commands. Override can be applied to the rapid traverse rate using the external signal supplied. Rapid Traverse Rate setting range
Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)
Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)
4. Feed 4.1 Feed Rate
- 24 -
4.1.2 Cutting Feed Rate (m/min) C6 C64
T system L system M system L system T system 1000 1000 1000 1000 1000
[T system, M system]
This function specifies the feed rate of the cutting commands, and a feed amount per spindle rotation or feed amount per minute is commanded. Once commanded, it is stored in the memory as a modal value. The feed rate modal value is cleared to zero only when the power is turned ON. The maximum cutting feed rate is clamped by the cutting feed rate clamp parameter (whose setting range is the same as that for the cutting feed rate).
Cutting Feed Rate setting range
Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)
Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)
The cutting feed rate is effective for G01, G02, G03, G33 commands, etc. As to others, refer to
the interpolation specifications.
[L system] This function specifies the feed rate of the cutting commands, and a feed amount per spindle rotation or feed amount per minute is commanded. Once commanded, it is stored in the memory as a modal value. The feed rate modal is cleared to zero only when the power is turned ON. The maximum cutting feed rate is clamped by the cutting feed rate clamp parameter (whose setting range is the same as that for the cutting feed rate).
Cutting Feed Rate setting range
Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)
Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)
The cutting feed rate is effective for G01, G02, G03, G33 commands, etc. As to others, refer to
interpolation specifications.
4. Feed 4.1 Feed Rate
- 25 -
4.1.3 Manual Feed Rate (m/min) C6 C64
T system L system M system L system T system 1000 1000 1000 1000 1000
The manual feed rates are designated as the feed rate in the jog mode or incremental feed mode for manual operation and the feed rate during dry run ON for automatic operation. The manual feed rates are set with external signals. The manual feed rate signals from the PLC includes two methods, the code method and numerical value method. Which method to be applied is determined with a signal common to the entire system. The signals used by these methods are common to all axes. Setting range under the code method
Metric input 0.00 to 14000.00 mm/min (31 steps) Inch input 0.000 to 551.000 inch/min (31 steps)
Setting range under the value setting method
Metric input 0 to 1000000.00 mm/min in 0.01 mm/min increments Inch input 0 to 39370 inch/min in 0.001 inch/min increments
Multiplication factor PCF1 and PCF2 are available with the value setting method.
4. Feed 4.2 Feed Rate Input Methods
- 26 -
4.2 Feed Rate Input Methods; G94/G95
4.2.1 Feed per Minute C6 C64
T system L system M system L system T system
[T system, M system]
By issuing the G94 command, the commands from that block are issued directly by the numerical value following F as the feed rate per minute (mm/min, inch/min).
Metric input (mm)
Least input increment (B) 0.001 mm (C) 0.0001 mm
F command increment (mm/min)
without decimal point with decimal point
F1 = 1 mm/min F1. = 1 mm/min
F1 = 1 mm/min F1. = 1 mm/min
Command range (mm/min) 0.01~1000000.000 0.001~100000.000
Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch
F command increment (inch/min)
without decimal point with decimal point
F1 = 1 inch/min F1. = 1 inch/min
F1 = 1 inch/min F1. = 1 inch/min
Command range (inch/min) 0.001~100000.0000 0.001~10000.0000
When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min). To assign commands under 1 mm/min (or 1 inch/min), ensure that commands are assigned with a decimal point.
The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter to OFF.
The F command increments are common to all part systems.
4. Feed 4.2 Feed Rate Input Methods
- 27 -
[L system] By issuing the G94 command, the commands from that block are issued directly by the numerical value following F as the feed rate per minute (mm/min, inch/min). Metric input (mm)
Least input increment (B) 0.001 mm (C) 0.0001 mm
F command increment (mm/min)
without decimal point with decimal point
F1 = 1 mm/min F1. = 1 mm/min
F1 = 1 mm/min F1. = 1 mm/min
Command range (mm/min) 0.001~1000000.000 0.0001 ~100000.0000
Inch input (inch)
Least input increment (B) 0.0001 inch (C) 0.00001 inch
F command increment (inch/min)
without decimal point with decimal point
F1 = 1 inch/min F1. = 1 inch/min
F1 = 1 inch/min F1. = 1 inch/min
Command range (inch/min) 0.0001~39370.0787 0.00001~3937.00787
When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min). To assign commands under 1 mm/min (or 1 inch/min), ensure that commands are assigned with a decimal point.
The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter to OFF.
4. Feed 4.2 Feed Rate Input Methods
- 28 -
4.2.2 Feed per Revolution C6 C64
T system L system M system L system T system
By issuing the G95 command, the commands from that block are issued directly by the numerical value following F as the feed rate per spindle revolution (mm/revolution or inch/revolution). The F command increment and command range are as follows.
[T system, M system]
Metric input (mm) Least input increment (B) 0.001 mm (C) 0.0001 mm
F command increment (mm/rev)
without decimal point with decimal point
F1 = 0.01 F1. = 1
F1 = 0.01 F1. = 1
Command range (mm/rev) 0.001~999.999 0.0001~99.9999
Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch
F command increment (inch/rev)
without decimal point with decimal point
F1 = 0.001 F1. = 1
F1 = 0.001 F1. = 1
Command range (inch/rev) 0.0001~999.9999 0.00001~99.99999
When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min).
The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter to OFF.
The F command increments are common to all part systems.
[L system]
Metric input (mm) Least input increment (B) 0.001 mm (C) 0.0001 mm
F command increment (mm/rev)
without decimal point with decimal point
F1 = 0.0001 F1. = 1
F1 = 0.0001 F1. = 1
Command range (mm/rev) 0.0001~999.999 0.00001~99.99999
Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch
F command increment (inch/rev)
without decimal point with decimal point
F1 = 0.000001 F1. = 1
F1 = 0.000001 F1. = 1
Command range (inch/rev) 0.000001~99.999999 0.0000001~9.9999999
When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min).
The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter to OFF.
4. Feed 4.2 Feed Rate Input Methods
- 29 -
4.2.4 F1-digit Feed C6 C64
T system L system M system L system T system
When the "F1digt" parameter is ON, the feed rate registered by parameter in advance can be assigned by designating a single digit following address F. There are six F codes: F0 and F1 to F5. The rapid traverse rate is applied when F0 is issued which is the same as the G00 command. When one of the codes F1 to F5 is issued, the cutting feed rate set to support the code serves as the valid rate command. When a command higher than F5 is issued, it serves as a regular direct command with feed rate value of 5 digits following address F. When an F1-digit command has been issued, the "In F1-digit" external output signal is output.
4. Feed 4.3 Override
- 30 -
4.3 Override
4.3.1 Rapid Traverse Override C6 C64
T system L system M system L system T system
(1) Type 1 (code method)
Four levels of override (1%, 25%, 50% and 100%) can be applied to manual or automatic rapid traverse using the external input signal supplied.
Code method commands are assigned as combinations of Y device bit signals from the PLC.
(2) Type 2 (value setting method) Override can be applied in 1% steps from 0% to 100% to manual or automatic rapid traverse
using the external input signal supplied.
(Note 1) Type 1 and type 2 can be selected by PLC processing.
4.3.2 Cutting Feed Override C6 C64
T system L system M system L system T system
(1) Type 1 (code method)
Override can be applied in 10% steps from 0% to 300% to the feed rate command designated in the machining program using the external input signal supplied. Code method commands are assigned as combinations of Y device bit signals from the PLC.
(2) Type 2 (value setting method)
Override can be applied in 1% steps from 0% to 327% to the feed rate command designated in the machining program using the external input signal supplied.
4.3.3 2nd Cutting Feed Override C6 C64
T system L system M system L system T system
Override can be further applied in 0.01% steps from 0% to 327.67% as a second stage override to the feed rate after the cutting feed override has been applied.
4. Feed 4.3 Override
- 31 -
4.3.4 Override Cancel C6 C64
T system L system M system L system T system
By turning on the override cancel external signal, the override is automatically set to 100% for the cutting feed during an automatic operation mode (memory and MDI).
(Note 1) The override cancel signal is not valid for manual operation.
(Note 2) When the cutting feed override or second cutting feed override is 0%, the 0% override takes precedence and the override is not canceled.
(Note 3) The override cancel signal is not valid for rapid traverse.
4. Feed 4.4 Acceleration/Deceleration
- 32 -
4.4 Acceleration/Deceleration
4.4.1 Automatic Acceleration/Deceleration after Interpolation C6 C64
T system L system M system L system T system
Acceleration/deceleration is applied to all commands automatically. The acceleration/deceleration patterns are linear acceleration/deceleration, soft acceleration/deceleration, exponent function acceleration/deceleration, exponent function acceleration/linear deceleration and any of which can be selected by using a parameter. For rapid traverse feed or manual feed, acceleration/deceleration is always made for each block, and the time constant can be set for each axis separately. Linear acceleration/deceleration
F F FC F
Tsr
Exponential acceleration / linear deceleration
Soft acceleration/deceleration
Exponential acceleration/deceleration
Tsr Tss Tss Tsc Tsc Tsc Tsr
(Note 1) The rapid traverse feed acceleration/deceleration patterns are effective for the following:
G00, G27, G28, G29, G30, rapid traverse feed in manual run, JOG, incremental feed, return to reference position.
(Note 2) Acceleration/deceleration in handle feed mode is usually performed according to the acceleration/deceleration pattern for cutting feed. However, a parameter can be specified to select a pattern with no acceleration/deceleration (step).
4. Feed 4.4 Acceleration/Deceleration
- 33 -
Acceleration/Deceleration during Continuing Blocks (1) Continuous G1 blocks
T s c T sc
f 1
f 2
G 1 G 1
Tsc Tsc
f 1
f 2
G1
G10
0
The tool does not decelerate between blocks.
(2) Continuous G1-G0 blocks
Tsc
G1 G0
G1
G0Tsr
G1
Tsr
G0 G1
Tsc
Tsr
G0
Tsr
If the G0 command direction is the same as that for G1, whether G1 is to be decelerated is selected using a parameter. If no deceleration is set, superposition is performed even when G0 is in the constant inclination acceleration/deceleration state. If the G0 command direction is the opposite of that for G1, G0 will be executed after G1 has decelerated. (In the case of two or more simultaneous axes, G0 will also be executed after G1 has decelerated when the G0 command direction is the opposite of that for G1 for even one axis.)
4.4.2 Rapid Traverse Constant Inclination Acceleration / Deceleration C6 C64
T system L system M system L system T system
This function performs acceleration and deceleration at a constant inclination during linear acceleration/deceleration in the rapid traverse mode. Compared to the method of acceleration/ deceleration after interpolation, the constant inclination acceleration/deceleration method makes for improved cycle time. Rapid traverse constant inclination acceleration/deceleration are valid only for a rapid traverse command. Also, this function is effective only when the rapid traverse command acceleration/ deceleration mode is linear acceleration and linear deceleration. The acceleration/deceleration patterns in the case where rapid traverse constant inclination acceleration/deceleration are performed are as follows.
4. Feed 4.4 Acceleration/Deceleration
- 34 -
(1) When the interpolation distance is longer than the acceleration and deceleration distance
L
T s T s T d
T
Next block
rapid
rapid : Rapid traverse rate
Ts : Acceleration/deceleration time constant
Td : Command deceleration check time : Acceleration/deceleration inclination T : Interpolation time L : Interpolation distance
T = rapid
L +Ts
Td = Ts + (0~1.7 ms)
= tan-1 rapid
Ts ( )
(2) When the interpolation distance is shorter than the acceleration and deceleration distance
rapid: Rapid traverse rate
Ts: Acceleration/deceleration time constant Td: Command deceleration check time : Acceleration/deceleration inclination T: Interpolation time L: Interpolation distance
L
Ts Td
T
rapid
Next block
= tan-1 rapid
Ts ( )
Td = + (0 ~ 1.7 ms) T 2
T = 2 Ts L / rapid
The time required to perform a command deceleration check during rapid traverse constant inclination acceleration/deceleration is the longest value among the rapid traverse deceleration check times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration/deceleration time constant, and the interpolation distance, respectively.
4. Feed 4.4 Acceleration/Deceleration
- 35 -
(3) 2-axis simultaneous interpolation (When linear interpolation is used, Tsx < Tsz, and Lx Lz) When 2-axis simultaneous interpolation (linear interpolations) is performed during rapid traverse constant inclination acceleration and deceleration, the acceleration (deceleration) time is the longest value of the acceleration (deceleration) times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration and deceleration time constant, and the interpolation distance, respectively. Consequently, linear interpolation is performed even when the axes have different acceleration and deceleration time constants.
x Tsx Tsx
Tdx
Lx
Tx
Next block
X axis
Tsz
Lz
Tz
Z axis
rapid X
rapid Z
Z
Tsz Tdz
Next block
When Tsz is greater than Tsx, Tdz is also greater than Tdx, and Td = Tdz in this block.
The program format of G0 (rapid traverse command) when rapid traverse constant inclination acceleration/deceleration are executed is the same as when this function is invalid (time constant acceleration/deceleration). This function is valid only for G0 (rapid traverse).
4. Feed 4.5 Thread Cutting
- 36 -
4.5 Thread Cutting
4.5.1 Thread Cutting (Lead/Thread Number Designation); G33 C6 C64
T system L system M system L system T system
(1) Lead designation The thread cutting with designated lead are performed based on the synchronization signals from the spindle encoder.
G33 Zz1 Qq1 Ff1/Ee1 ;
G33 : Thread command Zz1 : Thread length Qq1 : Shift angle ("q1" is the shift angle at thread cutting start, within 0 to 360) Ff1 : Thread lead Ee1 : Thread lead (precise lead threads)
The tables below indicate the thread lead ranges. [T system, M system]
Metric command Inch command Least input increment
(mm) F (mm/rev) E (mm/rev)
Least input increment
(inch) F (inch/rev) E (inch/rev)
0.001 0.001 ~999.999
0.00001 ~999.99999 0.0001 0.0001
~39.3700 0.000001
~39.370078
0.0001 0.0001 ~99.9999
0.000001 ~99.999999 0.00001 0.00001
~3.93700 0.000001
~3.937007
[L system]
Metric command Inch command Least input increment
(mm) F (mm/rev) E (mm/rev)
Least input increment
(inch) F (inch/rev) E (inch/rev)
0.001 0.0001 ~999.9999
0.00001 ~999.99999 0.0001 0.00001
~99.999999 0.000010
~9.9999999
0.0001 0.00001 ~99.99999
0.00001 ~99.99999 0.00001 0.000001
~9.9999999 0.0000010
~0.99999999 The direction of the axis with a large movement serves as the reference for the lead.
4. Feed 4.5 Thread Cutting
- 37 -
(2) Thread number designation Inch threads are cut by designating the number of threads per inch with the E address. Whether the E command is a thread number designation or lead designation is selected with the parameters.
G33 Zz1 Qq1 Ee1 ;
G33 : Thread command Zz1 : Thread length Qq1 : Shift angle ("q1" is the shift angle at thread cutting start, within 0 to 360) Ee1 : Thread number per inch
The tables below indicate the thread leads. [T system, M system]
Metric command Inch command Least input increment
(mm)
Thread number command range
(thread/inch)
Least input increment
(inch)
Thread number command range
(thread/inch) 0.001 0.03~999.99 0.0001 0.0255~9999.9999
0.0001 255~9999.999 0.00001 0.25401~999.9999
[L system]
Metric command Inch command Least input increment
(mm)
Thread number command range
(thread/inch)
Least input increment
(inch)
Thread number command range
(thread/inch) 0.001 0.03~999.99 0.0001 0.0101~9999.9999
0.0001 0.255~9999.999 0.00001 0.10001~999.99999 The number of thread per inch is commanded for both metric and inch systems, and the direction of the axis with a large movement serves as the reference.
4. Feed 4.5 Thread Cutting
- 38 -
4.5.2 Variable Lead Thread Cutting; G34 C6 C64
T system L system M system L system T system
By commanding the lead increment/decrement amount per thread rotation, variable lead thread cutting can be done. The machining program is commanded in the following manner. G34 X/U__Z/W__F/E__K__;
G34 X/U Z/W F/E K
: Variable lead thread cutting command : Thread end point X coordinate : Thread end point Z coordinate : Threads basic lead : Lead increment/decrement amount per thread rotation
F+3.5K
Non-lead axis
Lead axis
F+2.5K F+1.5K F+0.5K
Lead speed F+4K
F+3K F+2K F+K F
4. Feed 4.5 Thread Cutting
- 39 -
4.5.3 Synchronous Tapping; G74, G84
4.5.3.1 Synchronous Tapping Cycle C6 C64
T system L system M system L system T system
This function performs tapping through the synchronized control of the spindle and servo axis. This eliminates the need for floating taps and enables tapping to be conducted at a highly precise tap depth.
(1) Tapping pitch assignment
G84(G74) Xx1 Yy1 Zz1 Rr1 Pp1 Ff1 Ss1 , R1 ;
G84 G74 Xx1, Yy1 Zz1 Rr1 Pp1 Ff1 Ss1 ,R1
: Synchronous tapping mode ON, forward tapping : Synchronous tapping mode ON, reverse tapping : Hole position data, hole drilling coordinate position : Hole machining data, hole bottom position : Hole machining data, hole R position : Hole machining data, dwell time at hole bottom : Z-axis feed amount (tapping pitch) per spindle rotation : Spindle speed : Synchronous system selection
(2) Tapping thread number assignment
G84(G74) Xx1 Yy1 Zz1 Rr1 Pp1 Ee1 Ss1 , R1 ;
G84 G74 Xx1, Yy1 Zz1 Rr1 Pp1 Ee1 Ss1 ,R1
: Synchronous tapping mode ON, forward tapping : Synchronous tapping mode ON, reverse tapping : Hole position data, hole drilling coordinate position : Hole machining data, hole bottom position : Hole machining data, hole R position : Hole machining data, dwell time at hole bottom : Tap thread number per 1-inch feed of Z axis : Spindle speed : Synchronous system selection
4. Feed 4.5 Thread Cutting
- 40 -
The control state will be as described below when a tapping mode command (G74, G84) is commanded.
1. Cutting override Fixed to 100% 2. Feed hold invalid 3. "In tapping mode" signal is output 4. Deceleration command between blocks invalid 5. Single block invalid
The tapping mode will be canceled with the following G commands.
G61 ....... Exact stop check mode G61.1 .... High-accuracy control mode G62 ....... Automatic corner override G64 ....... Cutting mode
4.5.4 Chamfering C6 C64
T system L system M system L system T system
Chamfering can be validated during the thread cutting cycle by using external signals. The chamfer amount and angle are designated with parameters.
Chamfer amount
Thread cutting cycle
Chamfer angle
4. Feed 4.6 Manual Feed
- 41 -
4.6 Manual Feed
4.6.1 Manual Rapid Traverse C6 C64
T system L system M system L system T system
When the manual rapid traverse mode is selected, the tool can be moved at the rapid traverse rate for each axis separately. Override can also be applied to the rapid traverse rate by means of the rapid traverse override function. Rapid traverse override is common to all part systems.
+ X
Rapid traverse override
Rapid traverse
Tool
Machine tool
CNC
PLC
Rapid traverse
100 1 50 25
Y Z Axis movement control
+ +
4.6.2 Jog Feed C6 C64
T system L system M system L system T system
When the jog feed mode is selected, the tool can be moved in the axis direction (+ or ) in which the machine is to be moved at the per-minute feed. The jog feed rate is common to all part systems.
Manual cutting feed
Feed rate
Tool
Machine tool
CNC
PLC
Jog
3000 0
Z
Override
2000
Y X
Axis movement
control + + +
4. Feed 4.6 Manual Feed
- 42 -
4.6.3 Incremental Feed C6 C64
T system L system M system L system T system
When the incremental feed mode is selected, the tool can be operated by an amount equivalent to the designated amount (incremental value) in the axis direction each time the jog switch is pressed. The incremental feed amount is the amount obtained by multiplying the least input increment that was set with the parameter by the incremental feed magnification rate. The incremental feed amount parameter and its magnification rate are common to all part systems.
Scale factor
Step feed
Tool
Machine tool
CNC
PLC
Incremental
1000
Z Axis
movement control
Y X + + +
4.6.4 Handle Feed C6 C64
T system L system M system L system T system
(1-axis) In the handle feed mode, the machine can be moved in very small amounts by rotating the manual pulse generator. The scale can be selected from X1, X10, X100, X1000 or arbitrary value.
(Note 1) The actual movement amount and scale may not match if the manual pulse generator is rotated quickly.
(3-axes) In the handle feed mode, individual axes can be moved in very small amounts either separately or simultaneously by rotating the manual pulse generators installed on each of the axes.
(Note 1) The actual movement amount and scale may not match if the manual pulse generator is rotated quickly.
4. Feed 4.7 Dwell
- 43 -
4.7 Dwell; G04
4.7.1 Dwell (Time-based Designation) C6 C64
T system L system M system L system T system
The G04 command temporarily stops the machine movement and sets the machine standby status for the time designated in the program.
(G94) G04 Xx1/Uu1 ; or (G94) G04 Pp1 ;
G94 : Asynchronous G04 : Dwell Xx1, Uu1, Pp1 : Time
"x1" of the time-based dwell can be designated in the range from 0.001 to 99999.999 seconds.
5. Program Memory/Editing 5.1 Memory Capacity
- 44 -
5. Program Memory/Editing 5.1 Memory Capacity
Machining programs are stored in the NC memory.
5.1.1 Memory Capacity (Number of Programs Stored) (Note) The tape length will be the total of two part systems when using the 2-part system
specifications. 40 m (64 programs)
C6 C64 T system L system M system L system T system
80 m (128 programs)
C6 C64 T system L system M system L system T system
160 m (200 programs)
C6 C64 T system L system M system L system T system
320 m (200 programs)
C6 C64 T system L system M system L system T system
600 m (400 programs)
C6 C64 T system L system M system L system T system
5. Program Memory / Editing 5.2 Editing
- 45 -
5.2 Editing Method
5.2.1 Program Editing C6 C64
T system L system M system L system T system
The following editing functions are possible.
(1) Program erasing (a) Machining programs can be erased individually or totally. (b) When all machining programs are to be erased, the programs are classified with their No. into
B: 8000 to 8999, C: 9000 to 9999, and A: all others.
(2) Program filing (a) This function displays a list of the machining programs stored (registered) in the controller
memory. (b) The programs are displayed in ascending order. (c) Comments can be added to corresponding program numbers.
(3) Program copying (a) Machining programs stored in the controller memory can be copied, condensed or merged. (b) The program No. of the machining programs in the memory can be changed.
(4) Program editing (a) Overwriting, inserting and erasing can be done per character.
5. Program Memory / Editing 5.2 Editing
- 46 -
5.2.2 Background Editing C6 C64
T system L system M system L system T system
This function enables one machining program to be created or editing while another program is being run.
Prohibited
Memory operation
Machining with memory operationProgram editing
Editing
O4000
O3000
O2000
O1000
Program registered in memory
(1) The data of the machining programs being used in memory operation can be displayed and
scrolled on the setting and display unit, but data cannot be added, revised or deleted. (2) The editing functions mentioned in the preceding section can be used at any time for machining
programs which are not being used for memory operation. This makes it possible to prepare and edit the next program for machining, and so the machining
preparations can be made more efficiently. (3) The machining program will not be searched as the operation target even when searched in the
edit screen.
6. Operation and Display 6.1 Structure of Operation/Display Panel
- 47 -
6. Operation and Display 6.1 Structure of Operation/Display Panel
The following display units can be used for the setting and display unit.
(1) 7.2-type monochrome LCD display unit
C6 C64 T system L system M system L system T system
(2) 10.4-type monochrome LCD display unit
C6 C64 T system L system M system L system T system
(3) 9-type monochrome CRT display unit
C6 C64 T system L system M system L system T system
(4) External personal computer display (Ethernet connection)
C6 C64 T system L system M system L system T system
(5) Graphic operation terminal (GOT)
C6 C64 T system L system M system L system T system
6. Operation and Display 6.2 Operation Methods and Functions
- 48 -
6.2 Operation Methods and Functions
6.2.1 Memory Switch (PLC Switch) C6 C64
T system L system M system L system T system
The toggle switches (PLC switches) can be defined on the screen. These switches can be turned ON/OFF on the screen, and the status can be read from the PLC ladder. This screen has been prepared in advance, so the switch names (display on screen) can be defined with the PLC ladder. There are a total of 32 switch points.
6.3 Display Methods and Contents
6.3.1 Status Display C6 C64
T system L system M system L system T system
The status of the program now being executed is indicated. (1) Display of G, S, T, M commands and 2nd miscellaneous command modal values (2) Feed rate display (3) Tool offset number and offset amount display (4) Real speed display (*)
(*) The feed rate of each axis is converted from the final speed output to the drive unit, and is
displayed. However, during follow up, the speed is converted and displayed with the signals from the detector installed on the servomotor.
6. Operation and Display 6.3 Display Methods and Contents
- 49 -
6.3.2 Position Display Position data such as present positions for tools, coordinate positions and workpiece coordinate positions can be displayed. (1) Present position counter
C6 C64 T system L system M system L system T system
Each axis present position including tool length offset amount, tool radius compensation amount and workpiece coordinate offset amount is indicated. (2) Workpiece coordinate counter
C6 C64 T system L system M system L system T system
The workpiece coordinate system modal number from G54 to G59 and the workpiece coordinate value in the workpiece coordinate system are indicated. (3) Remaining command counter
C6 C64 T system L system M system L system T system
The remaining distance of the movement command during the execution (incremental distance from the present position to the end point of the block) is indicated during the automatic start and automatic stop. (4) Machine position counter
C6 C64 T system L system M system L system T system
Each axis coordinate value in the basic machine coordinate system whose zero point is the characteristic position determined depending on the machine is indicated.
6. Operation and Display 6.3 Display Methods and Contents
- 50 -
6.3.3 Program Running Status Display C6 C64
T system L system M system L system T system
Program now being executed is displayed.
6.3.4 Setting and Display C6 C64
T system L system M system L system T system
The parameters used in controller operations can be set and displayed.
6.3.5 MDI Data Setting and Display C6 C64
T system L system M system L system T system
The MDI data having a multiple number of blocks can be set and displayed. As with the editing of machining programs, the MDI programs can be revised using the delete, change and add functions. Operation can be repeated using the programs which have been set.
6.3.7 Clock C6 C64
T system L system M system L system T system
The clock is built-in, and the date (year, month, date) and time (hour, minute, second) are displayed. Once the time is set, it can be seen as a clock on the screen. The clock time can be read/written (read/set) from PLC using the DDB function.
6.3.8 Hardware/Software Configuration Display C6 C64
T system L system M system L system T system
This function displays the configuration of the installed hardware and software.
6. Operation and Display 6.3 Display Methods and Contents
- 51 -
6.3.9 Integrated Time Display C6 C64
T system L system M system L system T system
The integrating run time count during each signal of power-ON, automatic operation, automatic start and external integrating run time is ON can be set and displayed. The maximum time displayed is 9999 hours 59 minutes 59 seconds. Power-ON: Total of all the integrated run times, each starting when the power of the
NC control unit is turned ON and ending when it is turned OFF. Automatic operation: Total of the integrated run times for all machining periods, each starting
when the auto start button is pressed in the memory mode and ending when the reset status is established (usually when the M02 / M30 command is designated or the reset button is pressed). (This differs according to PLC machining.)
Automatic start: Total of the integrated run times for all automatic start operations, each
starting when the auto start button is pressed in the memory or MDI mode and ending when the feed hold stop or block stop is established or the reset button is pressed.
External integration: Based on the PLC sequence, this is the integrated run time of the signal set
by the PLC, and it comes in two types, external integration 1 and external integration 2.
6. Operation and Display 6.3 Display Methods and Contents
- 52 -
6.3.10 Available Languages (Japanese, English) C6 C64
T system L system M system L system T system 2
languages 2
languages 2
languages 2
languages 2
languages This function makes it possible to switch between Japanese and English which are the standard languages used for the screen displays. The display can also be switched to Polish.
6.3.11 Additional Languages (Japanese, English, Polish)
6.3.11.1 Japanese C6 C64
T system L system M system L system T system
6.3.11.2 English C6 C64
T system L system M system L system T system
6.3.11.13 Polish C6 C64
T system L system M system L system T system
6.3.13 Screen Deletion C6 C64
T system L system M system L system T system
When there is no need to use a screen for extended periods, the entire screen can be cleared to prevent deterioration of the display unit by the following procedures.
6. Operation and Display 6.4 Display Unit Switch
- 53 -
6.4 Display Unit Switch
6.4.1 Single-NC and Multi-Display Unit Switch C6 C64
T system L system M system L system T system
When multiple display units are connected to one NC, the active display unit can be selected with the changeover switch. The functions that can be used with the display unit differ according to the functions and connection method. Change-
over target
Connection method Display Operation Reset input READY lamp Remote I/O
connection
Cascade connection
Displayed only on selected display unit
(No display on others)
Input not possible
Displayed only on selected display unit (Others are
OFF)
Single- NC and multi-
display unit
switch LAN connection Display on all display units
Only selected
display unit is valid
Cascade connection
Connection not possible
Daisy chain connection
Only selected NC is displayed
Input not possible
Only selected NC is displayed
Connectable with
restrictions Multi-NC
and common- display
unit LAN connection
Only selected NC is displayed
(Two NCs are simultaneously
displayed when using 2-screen display)
Only selected
NC is valid
Connection not possible
(Note) The new communication terminal (GOT) is required for the LAN connection. The
connection format may differ according to the LAN device being used.
6.4.2 Multi-NC and Common-Display Unit C6 C64
T system L system M system L system T system
When a multiple number of NC systems are to be used, this function enables a single display unit to be used as the display for all the systems. This function is useful when, for instance, the NC systems are used for dedicated machines on a line.
6.4.4 Multi-NC and Common-external PC Display C6 C64
T system L system M system L system T system
When a multiple number of NC systems are to be used, this function enables a single personal computer to be used as the display for all the systems. This function is useful when, for instance, the NC systems are used for dedicated machines on a line.
6. Operation and Display 6.4 Display Unit Switch
- 54 -
6.4.5 Display Unit Detachable C6 C64
T system L system M system L system T system
This function enables the displays to be connected or detached without turning OFF the NC system's power.
7. Input/Output Functions and Devices
7.1 Input/Output Data
- 55 -
7. Input/Output Functions and Devices
7.1 Input/Output Data Certain kinds of data handled by the NC system can be input and output between the NC system's memory and external devices.
Machining program input / output (including user macros and fixed cycle macros) C6 C64
T system L system M system L system T system
Tool offset data input / output
C6 C64 T system L system M system L system T system
Common variable input / output
C6 C64 T system L system M system L system T system
Parameter input / output
C6 C64 T system L system M system L system T system
History data output
C6 C64 T system L system M system L system T system
(Note) Options are required for the devices used for input and output.
7. Input/Output Functions and Devices
7.2 Input/Output I/F
- 56 -
7.2 Input/Output I/F
7.2.1 RS-232C I/F C6 C64
T system L system M system L system T system
Port 2 of the RS-232C interface can be used.
Port Port 2 Transmission speed ~ 19.2kbps Handshake method DC code method, RTS/CTS method possible
This port can be used for inputting/outputting data, and for printing, etc. (The application is designated with the parameters.)
7.2.2 IC Card I/F
7.2.2.1 I/F for IC Card in Control Unit C6 C64
T system L system M system L system T system
An IC card can be used as an NC data input/output device. A 2MB or larger, 2GB or smaller flash ATA card (commercially-available part) can be used for the IC card. The data backed up onto the flash ATA card is stored in DOS format. When using a personal computer compatible with the flash ATA card, the backed up data can be stored on a personal computer's hard disk, etc.
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 57 -
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
8.1.1 Command/Output 8.1.1.1 Spindle Functions
C6 C64 T system L system M system L system T system
The spindle rotation speed is determined in consideration of the override and gear ratio for the S command commanded in automatic operation or with manual numerical commands, and the spindle is rotated. The following diagram shows an outline of the spindle control. When an 8-digit number following address S (S00000000 to S99999999) is commanded, a signed 32-bit binary data or 8-digit BCD data and start signal will be output to the PLC. Up to seven sets of S commands can be commanded in one block. Processing and complete sequences must be incorporated on the PLC side for all S commands.
(1) The override can be designated as 50% to 120% in 10% increments or 0 to 200% in 1%
increments (with built-in PLC specifications). The override is not changed while the spindle stop input is ON, during the tapping mode, or
during the thread cutting mode. (2) The number of gear steps can be commanded up to four steps. (3) The max. spindle rotation speed can be set for each gear.
(Machining program, Manual numerical command)
Analog spindle
D/A converter
Changeover (Parameter)
Remote I/O unit
(Parameter)
6-digit
6-digit BIN
6-digit
BIN
PLC NC
S command value
Spindle output command creation
Gear ratio Max. rotation
speed
S command analysis
Spindle controller MDS-C1-SP series, etc.
S Command
Spindle rotation command
Start signal
Spindle rotation command
Override
Gear selection
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 58 -
8.1.1.2 Spindle Serial I/F C6 C64
T system L system M system L system T system
This I/F is used to connect the digital spindle (AC spindle motor and spindle drive unit (SP, SPJ2)).
8.1.1.3 Spindle Analog I/F C6 C64
T system L system M system L system T system
Spindle control can be executed using an analog spindle instead of the digital spindle. In this case, the remote I/O unit DX120/DX121 is required. The analog output voltage is calculated from the present rotation speed regarding the voltage at the max. rotation speed as the maximum analog voltage. The specifications of the analog voltage output are as follows. (1) Output voltage ... 0 to 10 V (2) Resolution ... 1/4095 (12 multiplier of 2) (3) Load conditions ... 10 k (4) Output impedance ... 220
8.1.1.4 Coil Change C6 C64
T system L system M system L system T system
Constant output characteristics can be achieved across a broad spectrum down to the low-speed range by switching the spindle motor connections. This is a system under which commands are assigned from the PLC.
8.1.1.5 Automatic Coil Change C6 C64
T system L system M system L system T system
Constant output characteristics can be achieved across a broad spectrum down to the low-speed range by switching the spindle motor connections. This is a system under which the NC unit switches the coils automatically in accordance with the motor speed.
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 59 -
8.1.2 Speed Control 8.1.2.1 Constant Surface Speed Control
C6 C64 T system L system M system L system T system
With radial direction cutting, this function enables the spindle speed to be changed in accordance with changes in the radial direction coordinate values and the workpiece to be cut with the cutting point always kept at a constant speed (constant surface speed). G code Function
G96 Constant surface speed G97 Constant surface speed cancel
The surface speed is commanded with an S code. For the metric designation, the speed is commanded with an m/min unit, and for the inch designation, the speed is commanded with a feet/min unit. In the constant surface speed cancel mode, the S code is a spindle rotation speed command. The axis for which constant surface speed is controlled is generally the X axis. However, this can be changed with the parameter settings or with address P in the G96 block.
(Note) If there is only one spindle, the spindle will not operate normally if the constant surface speed control command, S command or spindle related M command is commanded randomly from each part system. These commands must be commanded from only one certain part system, or commanded simultaneously with standby.
The controller will execute the following control for the constant surface speed control and S commands. The part system from which an S command was issued last will have the spindle control rights. That part system will judge whether the constant surface speed command mode is valid or canceled, and will execute spindle control.
Part system 1 Part system 2 Part system 1
Spindle control rights
S100 G96
1000 r/min S200 m/min S100 m/min S2000 r/min
S2000 G96 S200 G97 S1000
Spindle speed
Part system 2 program
Part system 1 program
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 60 -
8.1.2.2 Spindle Override C6 C64
T system L system M system L system T system
This function applies override to the rotation speed of a spindle or mill spindle assigned by the machining program command during automatic operation or by manual operation. There are two types of override. (1) Type 1 (code method)
Using an external signal, override can be applied to the commanded rotation speed of a spindle or mill spindle in 10% increments from 50% to 120%.
(2) Type 2 (value setting method)
Using an external signal, override can be applied to the commanded rotation speed of a spindle or mill spindle in 1% increments from 0% to 200%.
(Note 1) Selection between type 1 and type 2 can be designated by user PLC processing.
8.1.2.3 Multiple-spindle Control When using a machine tool equipped with several spindles (up to seven spindles), this function controls those spindles. Multiple-spindle control I: Control based on a spindle selection command (such as G43.1) and
spindle control command ([S******;] or [SO=******;]), etc. The figure below shows an example of the configuration for a machine which is equipped with second and third spindles.
Tool post 1
Fi rs
t s pi
nd le
S ec
on d
sp in
dl e
Tool spindle (third spindle)
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 61 -
8.1.2.3.1 Multiple-spindle Control I C6 C64
T system L system M system L system T system
(1) Spindle selection commands
Using the spindle selection command (such as G43.1 [G group 20]), this function makes it possible to switch the spindle among the first through seventh spindles to which the subsequent S command (S******) is to apply.
Command format
G43.1; Selected spindle control mode ON; the selected spindle number is set using a parameter.
G44.1; Second spindle control mode ON (2) Spindle control commands (using an extended word address (SO=******))
In addition to using the "S******" S commands, it is also possible to assign commands which differentiate the applicable spindle among the first through seventh spindles by using the SO=******. The S command can be issued from a machining program for any part system. The number of spindle axes differs according to the model, so check the specifications. The C6 T and L System and C64 T System cannot control multiple spindles in one part system.
Command format
SO=******; O : Number assigned as the spindle number (1: first spindle; 2: second spindle; 7: seventh
spindle); variables can be designated. ******: Rotational speed or surface speed value assigned by 6-digit analog command; variables
can be designated.
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 62 -
8.1.3 Position Control 8.1.3.1 Spindle Orientation
C6 C64 T system L system M system L system T system
(a) Orient This function stops the spindle rotation at a certain position when using the digital spindle. When the orient command is used, the spindle will rotate several times and then stop at the orient point. The orient point is the Z-phase position when using encoder orient (PLG and external encoder/ring sensor).
(b) Multi-point orient This function performs orientation to a position other than the Z-phase position by inputting a shift amount with the parameter or PLC. The shift amount is 0 to 4095. (Unit: 360/4096) (Note 1) Multi-point orient cannot be executed when using the magnetic sensor. (Note 2) Orient is possible only when the gear ratio is 1:1 for the PLG orient.
(The orient is completed at the PLG encoder's Z-phase, so when using reduction gears, the orient points will be generated at several points during one spindle rotation.)
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 63 -
8.1.3.3 Spindle Synchronization 8.1.3.3.1 Spindle Synchronization I
C6 C64 T system L system M system L system T system
In a machine with two or more spindles, this function controls the rotation speed and phase of one selected spindle (synchronized spindle) in synchronization with the rotation of the other selected spindle (basic spindle). It is used in cases where, for instance, workpiece clamped to the basic spindle is to be clamped to the synchronized spindle instead or where the spindle rotation speed is to be changed while one workpiece remains clamped to both spindles. The synchronous spindle is designated and the start/end of the synchronization are commanded with the G command in the machining program.
Command format Spindle synchronization control cancel (G113) This command releases the state of synchronization between two spindles whose rotation has been synchronized by the spindle synchronization command. G113;
Spindle synchronization control ON (G114.1) This command is used to designate the basic spindle and the spindle to be synchronized with the basic spindle, and it places the two designated spindles in the synchronized state. By designating the synchronized spindle phase shift amount, the phases of the basic spindle and synchronized spindle can be aligned.
G114.1 H__ D__ R__ A__ ;
H__ : Selects the basic spindle. D__ : Selects the spindle to be synchronized with the basic spindle. E__ : Designates the synchronized spindle phase shift amount. A__ : Designates the spindle synchronization acceleration/deceleration time constant.
8. Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)
- 64 -
8.1.3.3.2 Spindle Synchronization II C6 C64
T system L system M system L system T system
In a machine with two or more spindles, this function controls the rotation speed and phase of one selected spindle (synchronized spindle) in synchronization with the rotation of the other selected spindle (basic spindle). It is used in cases where, for instance, workpiece clamped to the basic spindle is to be clamped to the synchronized spindle instead or where the spindle rotation speed is to be changed while one workpiece remains clamped to both spindles. The selection of the spindles to be synchronized, the start of the synchronization and other settings are all designated from the PLC. The spindle synchronization control mode is established by inputting the spindle synchronization control signal. While this mode is established, the synchronized spindle is controlled in synchronization with the rotation speed assigned for the basic spindle.
8. Spindle, Tool and Miscellaneous Functions 8.2 Tool Functions (T)
- 65 -
8.2 Tool Functions (T)
8.2.1 Tool Functions C6 C64
T system L system M system L system T system
(1) T system, M system
When an 8-digit number following address T (T00000000 T99999999) is assigned, 8-digit code data and start signal will be output to PLC. Only one set of T commands can be commanded in a block. Processing and complete sequences must be incorporated on the PLC side for all T commands.
(Note 1) There are some screens in the setting and display unit that cannot display all eight digits.
(2) L system
The command is issued with an 8-digit number following address T (T0 T99999999).The high- order 6 digits or 7 digits are designated as the tool No., and the low-order 2 digits or 1 digit are designated as the offset No. Which method is to be used is designated with parameters.
The 6-digit (or 7-digit) tool No. code data and start signal will be output to the PLC. Processing and complete sequences must be incorporated on the PLC side for all T commands.
(Note 1) There are some screens in the setting and display unit that cannot display all eight digits.
Txxxxxxxx
Tool offset No.
Tool No.
Txxxxxxxx
Tool No.
Tool offset No.
8. Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)
- 66 -
8.3 Miscellaneous Functions (M)
8.3.1 Miscellaneous Functions C6 C64
T system L system M system L system T system
When an 8-digit number (M00000000~M99999999) is assigned following address M, the 8-digit code data and start signal are output to PLC. When a 2-digit number following address M (M00 M97) is assigned, the code data and start signal will be output to the PLC. Apart from the above signals, various special independent signals are also output for the following signals.
M00 : Program stop M01 : Optional stop M02 : Program end M30 : Program end
Respective processing and complete sequences must be incorporated on the PLC side for all M commands from M00000000 to M99999999. M98 and M99 have specific purposes and can not be used.
(Note 1) There are some screens in the setting and display unit that cannot display all eight digits.
8.3.2 Multiple M Codes in 1 Block C6 C64
T system L system M system L system T system
Four sets of M commands can be issued simultaneously in a block. Respective processing and completion sequences are required for all M commands included in a block (except M98 and M99).
(Note 1) The code data and start signals of all the M commands in the same block are transferred simultaneously from the controller to the PLC, and so high-speed machine control can be done by the PLC processing sequence.
8. Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)
- 67 -
8.3.3 M Code Independent Output C6 C64
T system L system M system L system T system
When the M00, M01, M02 or M30 command is assigned during an automatic operation (memory, MDI) or by a manual numerical command, the signal of this function is output. It is turned OFF after the miscellaneous function finishes or by the reset & rewind signal.
Machining program
M code independent output Response to controller
M00 M00 Fin1 or Fin2 M01 M01 Fin1 or Fin2 M02 M02 Reset & rewind M30 M30 Reset & rewind
If movement or dwell command exists in the same block as these M commands, this signal is output upon completion of the movement or dwell command.
8.3.4 Miscellaneous Function Finish C6 C64
T system L system M system L system T system
These signals inform the CNC system that a miscellaneous function (M), spindle function (S), tool function (T) or 2nd miscellaneous function (A, B, C) has been assigned and that the PLC which has received it has completed the required operation. They include miscellaneous function finish signal 1 (FIN1) and miscellaneous function finish signal 2 (FIN2). Miscellaneous function finish signal 1 (FIN1) When the controller checks that FIN1 is ON, it sets the function strobes OFF. Furthermore, when the PLC checks that the function strobes are OFF, it sets FIN1 OFF. The controller checks that FIN1 is OFF and advances to the next block. Below is an example of a time chart applying when a miscellaneous function has been assigned.
Miscellaneous function finish signal (FIN1)
Miscellaneous function strobe (MF)
Command Next block
8. Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)
- 68 -
Miscellaneous function finish signal 2 (FIN2) When the controller checks that FIN2 is ON, it sets the function strobes OFF and simultaneously advances to the next block. The PLC checks that the strobe signals are OFF and sets FIN2 OFF. Below is an example of a time chart applying when a miscellaneous function has been assigned.
8.3.5 M Code Output during Axis Positioning C6 C64
T system L system M system L system T system
This function controls the timing at which miscellaneous functions are output, and it outputs a miscellaneous function when axis reaches at the designated position movement. The command format is as follows.
G117 Xx1 Zz1 Cc1 ;
G117 : Command of M code output during axis positioning Xx1, Zz1, Cc1 : Movement start points
: Miscellaneous function The miscellaneous function can be commanded in the G117 block within the following range.
M command : Up to four sets S command : Up to two sets T command : Up to one set 2nd miscellaneous function command : Up to one set
The G117 command can be commanded in up to two continuous blocks. (Example) G117 Xx1 Zz1 Mm1 Mm2 Mm3 Mm4 ; G117 Xx2 Zz2 Mm5 Mm6 Mm7 Mm8 ; G01 X200 Z200 ;
Mm1
Mm2
Mm3
Mm4 Mm5
Mm6
Mm7
Mm8
End point (200, 200)
(x2, z2)
(x1, z1) Start point
Miscellaneous function finish signal (FIN2)
Miscellaneous function strobe (MF)
Command Next block
8. Spindle, Tool and Miscellaneous Functions 8.4 2nd Miscellaneous Function (B)
- 69 -
8.4 2nd Miscellaneous Function (B)
8.4.1 2nd Miscellaneous Function C6 C64
T system L system M system L system T system
The code data and start signals are output when an 8-digit number is assigned following the address code A, B or C whichever does not duplicate the axis name being used. Processing and complete sequences must be incorporated on the PLC side for all 2nd miscellaneous commands.
(Note 1) There are some screens in the setting and display unit that cannot display all eight digits.
9. Tool Compensation 9.1 Tool Length/Position Offset
- 70 -
9. Tool Compensation 9.1 Tool Length/Position Offset; G43 to G49
9.1.1 Tool Length Offset C6 C64
T system L system M system L system T system
These commands make it possible to control the axis movement by offsetting the position of the end point of the movement command by an offset amount set on the TOOL OFFSET screen. Using this function, it is possible to offset the difference in distance between the actual position of the machine's tool nose and the program coordinate position made by the tool length and to enhance both the programming and operational efficiency.
(1) T system, M system
G43 G44
Zz1 Zz1
Hh1 Hh1
Offset direction
Offset axis Offset No.
; ;
Tool length offset can be provided not only for the Z axis but for all other axes which can be controlled in the system (X, Y, etc.).
G49 ; Tool length offset cancel The offset direction is determined by the G command.
G43: Forward direction (z1 + h1) G44: Reverse direction (z1 h1)
Offset can be canceled by the following G commands. G49; G43 H0; G44 H0;
(Example) Example of tool length offset using a combination with tool length measurement type I
M
G28 X0 Y0 Z0 ; T01 ; T02 M06 ; G91 G00 G43 Z2.0 H01 ;
M
(Note) The tool length offset amount is set as a negative value such as H01 = 450.000.
Z + 2.0
H01 = 450.000
Z 2.0
H01 = 450.000
Z 0.0 Workpiece
Table Table
Workpiece
(Note) When the tool length offset axis is returned to the reference point, the offset of that axis is canceled.
9. Tool Compensation 9.1 Tool Length/Position Offset
- 71 -
(2) L system (a) Shape offset Tool length is offset in reference to the programmed base position. The programmed base position is usually the center of the tool rest or the nose position of the base tool.
Z-axis tool length offset
Tool used for machining
Base tool
X-axis tool length offset
Base position (base point)
Z-axis tool length offset
X-axis tool length offset
The programmed base position is the center of the tool rest:
The programmed base position is the nose of the base tool:
(b) Wear offset The wear of a tool nose can be offset.
Tool nose
Z-axis tool nose wear offset amount
X-axis tool nose wear offset amount
X
Z
9. Tool Compensation 9.1 Tool Length/Position Offset
- 72 -
(c) Command format Tool offset is performed by a T command. It is specified in eight digits following address T. Tool offset is divided into two types: tool length offset and tool nose wear offset. The Nos. of such two types of offsets are specified by a parameter. Also a parameter is used to specify whether the offset Nos. is specified by one or two low-order digits of a T command. 1. Specifying tool length and wear offset Nos. together using one or two low-order digits of the T
command
T********
T********
Tool length offset No. and tool nose wear offset No. Tool No.
Tool length offset No. and tool nose wear offset No. Tool No.
2. Specifying tool length and wear offset Nos. separately
T********
T********
Tool nose wear offset No. Tool length offset No. Tool No.
Tool nose wear offset No. Tool length offset No. Tool No.
The tool offset for the L system is valid only for the X and Z axes. If an additional axis (Y axis) is added, the tool offset will be validated for the additional axis. (Refer to 9.1.3.)
9.1.3 Tool Offset for Additional Axes C6 C64
T system L system M system L system T system
The tool offset for the L system is valid only for the X and Z axes. If an additional axis (Y axis) is added, the tool offset will be validated for the additional axis. The additional axis is the third or fourth axis which is selected using a parameter.
9. Tool Compensation 9.2 Tool Radius
- 73 -
9.2 Tool Radius; G38 to G42, G46
9.2.1 Tool Radius Compensation; G38 to G42 C6 C64
T system L system M system L system T system
These commands function to provide tool radius compensation. Through a combination with the G
command and D address assignment, they compensate for the actual tool center path either inside or outside the programmed path by an amount equivalent to the tool radius.
The tool path is calculated by the intersection point arithmetic system and, as a result, excessive cut amounts on the inside of corners are avoided.
G code Function G38 Vector change during tool radius compensation G39 Corner arc during tool radius compensation G40 Tool radius compensation cancel G41 Tool radius compensation left command G42 Tool radius compensation right command
r r
r: Tool radius compensation amount Programmed path
Tool center path
The tool radius compensation command controls the compensation from that block in which G41 or G42 is commanded. In the tool radius compensation mode, the program is read up to five blocks ahead including blocks with no movement, and interference check using tool radius is conducted up to three blocks ahead in any of those blocks with movement.
G17 G01 G41 Xx1 Yy1 Dd1 ;
G17 : Compensation plane G01 : Cutting command G41 : Left compensation Xx1,Yy1 : Movement axis Dd1 : Compensation No.
The compensation plane, movement axes and next advance direction vector are based on the plane selection command designated by G17 to G19.
G17: XY plane, X, Y, I, J G18: ZX plane, Z, X, K, I G19: YZ plane, Y, Z, J, K
9. Tool Compensation 9.2 Tool Radius
- 74 -
An arc is inserted at the corner by the following command during tool radius compensation.
G39 Xx1 Yy1 ;
Xx1, Yy1 : Movement amount
Tool center path Arc inserted at corner
Programmed path
The compensation vector can be changed in following two ways.
G38 Xx1 Yy1 ;
Xx1, Yy1 : Movement amount
The tool radius compensation vector amount and direction are retained. G38 Xx1 Yy1 Ii1 Jj1 Dd1 ;
Xx1, Yy1 : Movement amount Ii1, Jj1 : Compensation vector direction Dd1 : Compensation vector length
The tool radius compensation vector direction is updated by I and J.
N12 N11
N13 N14 N15
Tool center path Holding of previous intersection point vector Vector with length D (i14, j14)
Intersection point vector
N11G01Xx11; N12G38Xx12Yy12; N13G38Xx13Yy13; N14G38Xx14Ii14Jj14Dd14; N15G40Xx15Yy15;
The tool radius compensation is canceled by the following command. G40 Xx1 Yy1 Ii1 Jj1 ;
Xx1, Yy1 : Movement amount Ii1, Jj1 : Compensation vector direction
The vector prior to canceling is prepared by calculating the intersection point with the I and J direction.
When i and j commands are assigned to G40
N11 N12
N13
N14
(i14,J14)
N11G01Xx11; N12Xx12Yy12; N13Xx13Yy13; N14G40Xx14Ii14Jj14;
Tool center path
9. Tool Compensation 9.2 Tool Radius
- 75 -
9.2.3 Tool Nose Radius Compensation (G40/41/42) C6 C64
T system L system M system L system T system
Corresponding to the tool No., the tool nose is assumed to be a half circle of radius R, and compensation is made so that the half circle touches the programmed path. G code Function
G40 Nose R compensation cancel G41 Nose R compensation left command G42 Nose R compensation right command
R
Programmed path
Compensated path
Nose R interference check
In the nose radius compensation mode, the program is read up to five blocks ahead including blocks with no movement, and an interference check using the nose radius is conducted up to three blocks ahead in any of those blocks with movement.
9. Tool Compensation 9.2 Tool Radius
- 76 -
9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40) C6 C64
T system L system M system L system T system
The nose radius compensation direction is automatically determined from the tool nose point and the specified movement vector. G code Function
G40 Nose radius compensation cancel G46 Nose radius compensation ON
(Automatic decision of compensation direction) The compensation directions based on the movement vectors at the tool nose points are as follows:
Tool nose direction
Tool nose progress direction
1
R
2 3 4
LR L
R
RR
R
RR
R
RR
R L
L
LL
L
LL
L
LL
M ou
ve m
en t v
ec to
rs (to
ol n
os e
po in
ts 1
to 4
)
Tool nose point
Range of each tool nose point (1 to 4)
Tool nose progress direction
5
R
6 7 8
LR L
R
RR
R
RR
R
RR
R L
L
LL
L
LL
L
LL
Tool nose point Tool nose direction
M ou
ve m
en t v
ec to
rs (to
ol n
os e
po in
ts 5
to 8
)
Range of each tool nose point (5 to 8)
9. Tool Compensation 9.3 Tool Offset Amount
- 77 -
9.3 Tool Offset Amount
9.3.1 Number of Tool Offset Sets The number of tool offset sets is as follows.
9.3.1.2 40 sets C6 C64
T system L system M system L system T system
9.3.1.3 80 sets C6 C64
T system L system M system L system T system
9.3.1.4 100 sets C6 C64
T system L system M system L system T system
9.3.1.5 200 sets C6 C64
T system L system M system L system T system
9. Tool Compensation 9.3 Tool Offset Amount
- 78 -
9.3.2 Offset Memory
9.3.2.1 Tool Shape/Wear Offset Amount C6 C64
T system L system M system L system T system
This function registers the tool shape offset and wear offset amounts among the positions of the tools moving in the direction parallel to the control axis. Compensation may encompass two or more axes.
1. Shape offset amount The tool length offset amount, tool radius compensation amount, nose radius compensation amount, nose radius imaginary tool tip point or tool width can be set as the shape offset amount. The compensation amount that can be set and used differs depending on whether offset amount setting type 1, 2 or 3 is used.
2. Wear offset amount When the tip of the tool used has become worn, the wear offset amount is used to offset this wear. Types of wear offset amounts include the tool length wear offset amount, tool radius wear compensation amount, and nose radius wear compensation amount. The wear offset amount can be used with offset amount setting types 2 and 3, and it is added to the shape offset amount for compensation. (a) Type 1: 1-axis offset amount [T system, M system]
This is the value that is used by rotary tools. As the tool length offset amount, among the offset amounts for the position of the tool moving in the direction parallel to the control axis, the offset amount in the longitudinal direction of the rotary tool is registered. The tool length offset amount is set as a minus value. As the tool radius compensation amount, among the offset amounts for the position of the tool moving in the direction parallel to the control axis, the offset amount in the radial direction of the rotary tool is registered. The tool radius compensation amount is set as a plus value. One offset amount data is registered in one offset number, and the offset Nos. are assigned using the address D or H commands. When a No. is assigned by a D address command, offset is provided in the form of the tool radius; when it is assigned by an H address command, it is provided in the form of the tool length.
9. Tool Compensation 9.3 Tool Offset Amount
- 79 -
(b) Type 2: 1-axis offset amounts/with wear offset [T system, M system]
As with type 1, type 2 is for the offset amounts used by rotary tools. With type 2, four kinds of offset amount data are registered in one offset No.: the tool length offset amount, tool length wear offset amount, tool radius compensation amount, and tool radius wear compensation amount. When an offset No. is assigned by address D as the offset amount, the tool radius is compensated using the amount obtained by adding the tool radius compensation amount and tool radius wear compensation amount. Further, the tool length is offset using the amount obtained by adding the tool length offset amount and tool length wear offset amount.
Figure: Example of how the offset amount is handled when using the type 1 tool length offset amount (Offset types I and II are available for handling offset amounts.)
Wear offset amount when using type 2
M
Tool radius compensation amount
M
W
Offset type I Offset type II
Z0.0 Workpiece Workpiece
Table Table
Z0.0
Tool radius compensation amount
Tool length offset amount
Tool length offset amount
M
Tool length wear offset
t
Tool radius wear compensation amount
9. Tool Compensation 9.3 Tool Offset Amount
- 80 -
(c) Type 3: 2-axis offset amounts [L system]
Type 3 is for the offset amounts used by non-rotary tools. As the offset amounts, the tool length along the X, Y and Z axes and the wear amount along each of these axes, the nose radius and nose radius wear amount, tool tip point P and tool width can be registered. Offset is provided in the directions of the X, Y and Z axes from the base position in the program. Generally, the center of the tool rest or the tip of the base tool is used as the programmed base position.
1. The programmed base position 2. The programmed base position
is the center of the tool rest: is the tip of the base tool:
X-axis tool length offset
amount
Base position (base point)
Z-axis tool length offset amount
Base position (base point)
X-axis tool length offset amount
Tool used for machining
Base tool
Z-axis tool length offset amount
The tool tip contour arc radius (nose radius) of a non-rotary tool with an arc (nose radius) at its tip is registered as the nose radius offset amount.
Imaginary tool nose point
Tool nose center
Nose radius compensation amount
X-axis tool length wear offset
X
Z Z-axis tool length wear offset
Tool nose
The X-axis tool length offset amount, Z-axis tool length offset amount and nose radius compensation amount are set as plus amounts. The offset type (1, 2 or 3) is set using a parameter.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 81-
10. Coordinate System 10.1 Coordinate System Type and Setting; G52 to G59, G92
The coordinate system handled by the NC is shown below. The points that can be commanded with the movement command are points on the local coordinate system or machine coordinate system.
G52
G92
G55G54
L0
L0
W0-55
W0-54
EXT
ref
M0
G52
R
L0 Local coordinate system zero point Offset set with parameters G52 Local coordinate system offset *1) Offset set with program W0-54 Workpiece coordinate system zero point (G54) (0 when power is turned ON) W0-55 Workpiece coordinate system zero point (G55) G54 Workpiece coordinate system (G54) offset *1) G55 Workpiece coordinate system (G55) offset G92 G92 coordinate system shift EXT External workpiece coordinate offset M0 Machine coordinate system zero point ref Reference point *1)The G52 offset is available independently for G54 to G59.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 82-
10.1.1 Machine Coordinate System; G53 C6 C64
T system L system M system L system T system
The machine coordinate system is used to express the prescribed positions (such as the tool change position and stroke end position) characteristic to the machine, and it is automatically set immediately upon completion of the first dog-type reference point return after the power has been turned ON or immediately after the power has been turned ON if the absolute position specifications apply. The programming format for the commands to move the tool to the machine coordinate system is given below. G53 (G90) (G00) Xx1 Yy1 Zz1 ;
G53 : Coordinate system selection G90 : Incremental/absolute commands G00 : Movement mode [T system, M system] Xx1, Yy1, Zz1 : End point coordinate on the machine coordinate system
If the incremental or absolute commands and movement mode have been omitted, operation complies with the modal command that prevails at the time. G53 (movement on machine coordinate system) is an unmodal command which is effective only in the block where it is assigned. The workpiece coordinate system being selected is not changed by this command.
1st reference point
Workpiece coordinate system 1 (G54)
Machine coordinate system (G53)
G53 G90 G00 X0 Y0 ;
M
W1
10. Coordinate System 10.1 Coordinate System Type and Setting
- 83-
10.1.2 Coordinate System Setting; G92 C6 C64
T system L system M system L system T system
When a coordinate system setting is assigned using the G92 command, the G92 offset amount is applied so that the machine position in the current workpiece coordinate system is set to the coordinate values assigned by the G92 command, as shown in the figure below, and the workpiece coordinate systems are shifted accordingly. The machine does not run , and all the workpiece coordinate systems from G54 to G59 referenced to the machine coordinate system (or the external workpiece coordinate system if the external workpiece coordinate offset has been set) are shifted.
Machine position
Example where W1 is shifted to new W1 when the machine was at the position (x0, y0) above W1 and the G92 Xx1 Yy1; command was assigned when the workpiece coordinate system W1 is modal (external workpiece coordinate system offset = 0; interrupt amount offset = 0)
y0 W1
Machine coordinate system
M
G92 offset amount
Offset of coordinate system by G92 coordinate system setting
x1
y1
X : x0x1 Y : y0y1
x0
New W1
The shifted coordinate system is returned to its original position by dog-type reference point return or the program.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 84-
When the coordinate system setting is commanded by G92, all the workpiece coordinate systems from G54 through G59 referenced to the machine coordinate system undergo a shift.
Coordinate system created by automatic coordinate system setting
Coordinate system after coordinate system setting by G92
G92 Xx1 Yy1
Machine coordinate system
W1
M
x y'
G92 command position
Old W1
New W1
M
x1
Machine coordinate system
y1
Tool position
(1) All the workpiece coordinates from G54 to G59 move in parallel. (2) There are two ways to return a shifted coordinate system to its original position.
(a) Carry out dog-type reference point return (b) Move to machine coordinate system zero point and assign G92 and G53 commands in same block to set the machine coordinate system.
G90 G53 G00 X0 Y0 ; _____ Positioning at machine coordinate system zero point.
G92 G53 X0 Y0 ; __________ Coordinate system zero setting in machine coordinate system. This returns all the workpiece coordinates from G54 to G59 to their original positions.
10.1.3 Automatic Coordinate System Setting C6 C64
T system L system M system L system T system
When the tool has arrived at the reference point by means of the first manual or automatic dog-type reference point return after the controller power is turned ON, or immediately after the power is turned ON for the absolute position specifications, this function creates the coordinate systems in accordance with the parameters settings. The coordinate systems created are given below.
(1) Machine coordinate system corresponding to G53 (2) G54 to G59 workpiece coordinate system (3) Local coordinate systems created under G54 to G59 workpiece coordinate systems
The distances from the zero point of G53 machine coordinate system are set to the controller coordinate related parameters. Thus, where the No. 1 reference point is set in the machine is the base for the setting.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 85-
10.1.4 Workpiece Coordinate System Selection (6 sets); G54 to G59 C6 C64
T system L system M system L system T system
When a multiple number of workpieces with the same shape are to be machined, these commands enable the same shape to be machined by executing a single machining program in the coordinate system of each workpiece. Up to 6 workpiece coordinate systems can be selected. The G54 workpiece coordinate systems are selected when the power is turned ON or the reset signal which cancels the modal information is input.
G code Function G54 Workpiece coordinate system 1 (W1) G55 Workpiece coordinate system 2 (W2) G56 Workpiece coordinate system 3 (W3) G57 Workpiece coordinate system 4 (W4) G58 Workpiece coordinate system 5 (W5) G59 Workpiece coordinate system 6 (W6)
The command format to select the workpiece coordinate system and to move on the workpiece coordinate system are given below. (G90) G54 G00 Xx1 Yy1 Zz1 ;
(G90) : (Absolute value command) G54 : Coordinate system selection G00 : Movement mode Xx1, Yy1, Zz1 : Coordinate values of end point
The workpiece coordinate zero points are provided as distances from the zero point of the machine coordinate system. Settings can be performed in one of the following three ways:
(1) Setting using the setting and display unit (2) Setting using commands assigned from the machining program (3) Setting from the user PLC
W2
W3W4
Workpiece coordinate system 1 (G54)
Workpiece coordinate system 2 (G55)
Machine coordinate system (G53)
W1
M
Start
G90 G56 G00 X0 Y0 ;
Workpiece coordinate system 4 (G57)
Workpiece coordinate system 3 (G56)
10. Coordinate System 10.1 Coordinate System Type and Setting
- 86-
10.1.5 Extended Workpiece Coordinates System Selection Extended workpiece coordinate system selection (48 sets) G54.1P1 to P48
C6 C64 T system L system M system L system T system
In addition to the six workpiece coordinate systems G54 to G59, 48 workpiece coordinate systems can be used by assigning G54.1Pn command. The command format to select the workpiece coordinate system using the G54.1Pn command and to move on the workpiece coordinate system are given below. (G90) G54.1Pn G00 Xx1 Yy1 Zz1 ;
(G90) : (Absolute value command) G54.1Pn : Coordinate system selection G00 : Movement mode Xx1, Yy1, Zz1 : Coordinate values of end point
The numerical value n of P following G54.1 indicates each workpiece coordinate system. Specify a value between 1 and 48. The workpiece coordinate zero points are provided as distances from the zero point of the machine coordinate system. Settings can be performed in one of the following three ways:
(1) Setting using the setting and display unit (2) Setting using commands assigned from the machining program (3) Setting from the user PLC
(Note) While the G54.1Pn (extended workpiece coordinate system selection) is modal, the local coordinate offset is reduced to zero, and the G52 command cannot be used.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 87-
10.1.7 Local Coordinate System; G54G52 to G59G52 C6 C64
T system L system M system L system T system
This function is for assigning a coordinate system on the workpiece coordinate system now being selected. This enables the workpiece coordinate system to be changed temporarily. The local coordinate system can be selected independently on each workpiece coordinate system G54 to G59.
G code Function G54 G52 Local coordinate system on the workpiece coordinate system 1 G55 G52 Local coordinate system on the workpiece coordinate system 2 G56 G52 Local coordinate system on the workpiece coordinate system 3 G57 G52 Local coordinate system on the workpiece coordinate system 4 G58 G52 Local coordinate system on the workpiece coordinate system 5 G59 G52 Local coordinate system on the workpiece coordinate system 6
The command format of the local coordinate system is given below.
(G54) G52 Xx1 Yy1 Zz1 ;
(G54) : Workpiece coordinate system selection G52 : Local coordinate system setting Xx1, Yy1, Zz1 : Local coordinate offset amount
The local coordinate zero points are provided as distances from the zero point of the designated workpiece coordinate system (local coordinate offset). In the incremental value mode, the position obtained by adding the local coordinate offset amount to the previously specified offset amount serves as the new local coordinate zero point. If no workpiece coordinates are designated, the local coordinates will be created on the currently selected workpiece coordinates. This command is unmodal but the local coordinate system created by G52 is valid until the next G52 command is issued. The local coordinate system is canceled by the input of the reset signal or by manual or automatic dog-type reference point return.
W1
x1
L1
Workpiece coordinate 1 (G54)
Machine coordinate system (G53)
Local coordinate G54 G52
y1
M
10. Coordinate System 10.1 Coordinate System Type and Setting
- 88-
10.1.8 Coordinate System for Rotary Axis C6 C64
T system L system M system L system T system
The coordinate system of rotary axis ranges from 0 to 360. Note that, however, it can be displayed from 0 to 359.999. In absolute value command mode, the rotary axis can make a turn or less (not greater than 360). The turning direction depends on the specified sign. A negative sign () turns the axis in the negative direction and a positive sign (+) turns it in the positive (+) direction. Note that a parameter can be used to move the axis to the end point taking a short cut. In incremental value command mode, the rotary axis moves the specified distance only.
10.1.9 Plane Selection; G17 to G19 C6 C64
T system L system M system L system T system
These G codes are for specifying the planes for the arc, tool radius compensation, coordinate rotation and other such commands. G17 ; .................. Xp-Yp plane designation G18 ; .................. Zp-Xp plane designation G19 ; .................. Yp-Zp plane designation
(1) A parameter can be used to set either the X, Y or Z axis to which the additional axis is to be
parallel. (2) A parameter can be used to set the initialization status (when the power has been turned ON or
when the reset status has been entered) to G17, G18 or G19. (3) The movement commands have no connection with the plane selection.
Example
G19 X100. ; With these program commands, X100. is the axis which does not exist on the G19 (Yp, Zp) plane, Yp-Zp are selected by G19 and the X axis moves by 100. mm separately from the plane selection.
G17 X100. R50. ; With these program commands, the Xp-Yp plane is selected by G17 and the arc command is controlled on the X-Y plane by this command.
10. Coordinate System 10.1 Coordinate System Type and Setting
- 89-
10.1.10 Origin Set C6 C64
T system L system M system L system T system
Using the setting and display unit, the coordinate system (current position and workpiece coordinate position) can be set to "0" by operating the screen. This function is the same as the coordinate system setting command " G92 X0 (Y0 or Z0) ; ". [POSITION] [WORK(G54)]
[POSOTION] [WORK(G54)]
X -150.345 X -150.345 X 0.000 X 0.000 Y - 12.212 Y - 12.212 Y 0.000 Y 0.000 Z - 1.000 Z - 1.000 Z 0.000 Z 0.000 A - 0.000 A - 0.000 A 0.000 A 0.000
X
C.B CAN
Y
C.B CAN
Z
C.B CAN
When axes are set to "0" in order, the Y and Z axis can be set by pressing
C.B CAN key successively
without pressing
Y and
Z keys.
10.1.11 Counter Set C6 C64
T system L system M system L system T system
Using the setting and display unit, the position counter display can be change to "0" by operating the screen. (1) This operation is the same as the operation of "Origin Set", but press
INPUT key instead of
C.B CAN
key. (2) Only the [POSITION] counter display is changed to "0", and the other coordinate system counter
displays are not changed.
10. Coordinate System 10.2 Return
- 90-
10.2 Return; G27 to G30
10.2.1 Manual Reference Point Return C6 C64
T system L system M system L system T system
This function enables the tool to be returned manually to the position (reference point) which is characteristic to the machine.
(1) Return pattern to reference point
(a) Dog type
When starting in same direction When starting in opposite direction as final advance direction as final advance direction
(b) High-speed type
Reference position return speed
Dog Dog
R
1
R
Creep speed
Dog
Rapid traverse rate
R
(2) Differences according to detection method First return after power ON Second return and following Incremental position detection method Dog-type High-speed
Absolute position detection method High-speed High-speed
10. Coordinate System 10.2 Return
- 91-
10.2.2 Automatic 1st Reference Point Return; G28, G29 C6 C64
T system L system M system L system T system
The machine can be returned to the first reference point by assigning the G28 command during automatic operation. If the interim point is commanded, the machine is moved up to that point by rapid traverse so that it is positioned and then returned separately for each axis to the first reference point. Alternatively, by assigning the G29 command, the machine can be first positioned separately for each axis at the G28 or G30 interim point, and then positioned at the command position.
G code Function G28 Automatic 1st reference point return G29 Start position return (The tool first returns to the interim position of the 1st reference
point return start from the 1st reference point, and then is positioned at the position designated in the program.)
The G28 programming format is given below. G28 Xx1 Yy1 Zz1 ;
G28 : Return command Xx1, Yy1, Zz1 : Return control axes (interim point)
Each axis is first positioned by rapid traverse to the position (interim point) assigned for the assigned axis and then is returned independently to the 1st reference point. The G29 programming format is given below. G29 Xx1 Yy1 Zz1 ;
G29 : Return command Xx1, Yy1, Zz1 : Return control axes (assigned position)
The tool is first moved by rapid traverse to the interim position which is passed through with G28 or G30, and is then positioned by rapid traverse at the position assigned by the program.
Interim point
1st reference point R
Y
Non - interpolation movement
G29
G28
G28
G29
X
Interpolation or non - interpolation can be selected
Interpolation or non interpolation can be selected
10. Coordinate System 10.2 Return
- 92-
If the position detector is for the incremental detection system, the first reference point return for the first time after the NC power has been turned ON will be the dog-type. However, whether the second and subsequent returns are to be the dog type or the high-speed type can be selected by designating a parameter. The high-speed type is always used when the position detector is for the absolute position detection system. (Note 1) The automatic 1st reference point return pattern is the same as for manual reference
point return.
(Note 2) The number of axes for which reference point return can be performed simultaneously depends on the number of simultaneously controlled axes.
(Note 3) If, at the time of the first reference point return, the tool radius compensation or nose radius compensation has not been canceled, it will be temporarily canceled by the movement to the interim point. The compensation is restored by the next movement after the return.
(Note 4) If, at the time of the first reference point return, the tool length offset has not been canceled, the offset will be canceled by the movement from the interim point to the first reference point, and the offset amount will also be cleared. It is possible to cancel the tool length offset temporarily using a parameter instead. In this case, however, the offset is restored by the next movement command.
(Note 5) Interpolation or non-interpolation can be selected using a parameter for the movement up to the G28 interim point or for the movement from the G29 interim point to the command point. Non-interpolation applies for movement from the G28 interim point to the reference point and movement up to the G29 interim point.
(Note 6) The machine will not stop at the interim point even when a single block is selected.
10. Coordinate System 10.2 Return
- 93-
10.2.3 2nd, 3rd, 4th Reference Point Return; G30 C6 C64
T system L system M system L system T system
As with automatic 1st reference point return, commanding G30Pn during automatic operation enables the tool to be returned to the set points (2nd, 3rd or 4th reference points) characteristic to the machine. The 2nd, 3rd and 4th reference points can be set by parameters.
G code Function G30 P2 2nd reference point return G30 P3 3rd reference point return G30 P4 4th reference point return
The G30 programming format is given below. G30 Xx1 Yy1 Zz1 Pp1 ;
G30 : Return command Xx1, Yy1, Zz1 : Return control axes (interim point) Pp1 : Return position No.
The tool is first positioned by rapid traverse to the interim point commanded for the assigned axis and then is returned independently to the reference point.
G30 P2
Interim point
1st reference point 2nd reference point
Start point
4th reference point
3rd reference point
G30 P3
G30 P4
X
Y
(Note 1) The second reference point return is performed if the P address is omitted.
(Note 2) The number of axes for which reference point return can be performed simultaneously depends on the number of simultaneously controlled axes.
(Note 3) If, at the time of the reference point return, the tool radius compensation has not been canceled, it will be temporarily canceled by the movement up to the interim point. The compensation is restored by the next movement command after the return.
10. Coordinate System 10.2 Return
- 94-
(Note 4) If, at the time of the reference point return, the tool length offset has not been canceled, it will be canceled and the offset amount also cleared upon completion of reference point return. The tool length offset can also be canceled temporarily using a parameter. In this case, however, the tool offset is restored by the next movement command.
(Note 5) Whether interpolation or non-interpolation is to apply to the movement up to the interim point can be selected using a parameter. Non-interpolation applies for movement from the interim point to each of the reference points.
(Note 6) The machine will not stop at the interim point even when a single block is selected.
10.2.4 Reference Point Verification; G27 C6 C64
T system L system M system L system T system
By commanding G27, a machining program, which has been prepared so that the tool starts off from the reference point and returns to the reference point, can be checked to see whether the tool will return properly to the reference point. The G27 programming format is given below. G27 Xx1 Yy1 Zz1 Pp1 ;
G27 : Verification command Xx1, Yy1, Zz1 : Return control axes Pp1 : Verification No.
P1 : 1st reference point verification P2 : 2nd reference point verification P3 : 3rd reference point verification P4 : 4th reference point verification
The assigned axis is first positioned by rapid traverse to the commanded position and then, if this is the reference point, the reference point arrival signal is output. When the address P is omitted, the first reference point verification will be applied.
(Note 1) The number of axes for which reference point verification can be performed
simultaneously depends on the number of simultaneously controlled axes.
(Note 2) An alarm results unless the tool is positioned at the reference point upon completion of the command.
(Note 3) Whether interpolation or non-interpolation is to apply to the movement can be selected using a parameter.
10. Coordinate System 10.2 Return
- 95-
10.2.5 Absolute Position Detection C6 C64
T system L system M system L system T system
The absolute position detection function holds the relation of the actual machine position and the machine coordinates in the controller with a battery even when the power is turned OFF. When the power is turned ON again, automatic operation can be started without executing reference point return. (High-speed return will always be used for the reference point return command.) For the absolute position detection method, there are two method such as the dog-type and dog- less type according to how the zero point is established.
Method Details Establishment of zero point
Adjustment of zero point position
Dog-type Same method as incremental detection dog-type
Zero point is established with dog- type reference point return completion.
The data is set in the parameter of zero point shift amount.
Dog-less type
Marked point method
The zero point position is set from the screen.
The zero point is established by input from the zero point initialization screen.
The value equivalent to the shift amount is set in the zero point initialization screen.
Machine stopper method
The zero point is established by pressing the machine against a set point on the machine.
The zero point is established when a torque limit is applied on the servo and the torque limit is reached by pressing against the machine stopper.
The value equivalent to the shift amount is set in the zero point initialization screen.
Diagnosis during absolute position detection
(1) The machine position at power OFF and ON can be confirmed on the absolute position monitor screen.
(2) If the amount that the axis is moved during power OFF exceeds the tolerable value (parameter), a warning signal will be output.
(3) An alarm will be output if the absolute position information is lost. (4) An alarm will be output if the voltage of the battery for backing up the absolute position data
drops.
10. Coordinate System 10.2 Return
- 96-
10.2.6 Tool Change Position Return; G30.1 to G30.6 C6 C64
T system L system M system L system T system
By specifying the tool change position in a parameter and also assigning a tool change position return command in a machining program, the tool can be changed at the most appropriate position. The axes for which returning to the tool change position is performed and the order in which the axes begin to return can be changed by commands. G30.n ;
n = 1 to 6 : Specify the axes that return to the tool change position and the order in which they return. (For L system, n = 1 to 5)
Command and return order
[T system, M system] Command Return order
G30.1 Z axis X axis Y axis ( additional axis) G30.2 Z axis X axis Y axis ( additional axis) G30.3 Z axis Y axis X axis ( additional axis) G30.4 X axis Y axis Z axis ( additional axis) G30.5 Y axis X axis Z axis ( additional axis) G30.6 X axis Y axis Z axis ( additional axis)
[L system]
Command Return order G30.1 X axis only ( additional axis) G30.2 Z axis only ( additional axis) G30.3 X axis Z axis ( additional axis) G30.4 Z axis X axis ( additional axis) G30.5 X axis Z axis ( additional axis)
(Note 1) An arrow ( ) indicates the order of axes that begin to return. A period ( )
indicates that the axes begin to return simultaneously. Example: "Z axis X axis" indicate that the Z axis returns to the tool
change position, then the X axis does. (Note 2) G30.6 is only for the T system and M system.
The tool change position return ON/OFF for the additional axis can be set with parameter for the additional axis. For the order to return to the tool change position, the axes return after the standard axis completes the return to the tool change position (refer to above table). The additional axis cannot return to the tool change position alone.
11. Operation Support Functions 11.1 Program Control
- 97 -
11. Operation Support Functions 11.1 Program Control
11.1.1 Optional Block Skip C6 C64
T system L system M system L system T system
When "/" (slant code) is programmed at the head of a block, and the optional block skip input signal from the external source is turned ON for automatic operation, the block with the "/" code is skipped. If the optional block skip signal is turned OFF, the block with the "/" code will be executed without being skipped.
Optional block skip
Programming example
:
:
:
Switch ON Switch OFF
N7
N6
/N5
/N4
N3
N2
N1 N1
N2
N3
N4
N5
N6
N7
N1
N2
N3
N6
N7
11. Operation Support Functions 11.1 Program Control
- 98 -
11.1.3 Single Block C6 C64
T system L system M system L system T system
The commands for automatic operation can be executed one block at a time (block stop) by turning ON the single block input signal. When the single block input signal is turned ON temporarily during continuous operation, the machine will stop after that block has been executed. When operation is switched to another automatic operation mode (for example, memory operation mode to MDI operation mode) during continuous operation, the machine will stop after that block has been executed. Single block in the multi-part system also functions as the above single block in each independent part system.
G01 Z1000G01 Z100
SBK changeSBK ON at start
G01 X1000
INVALID
Single block (SBK)
Automatic operation
Movement block
start (ST)
during movement
VALID VALID
SBK ON after block completion
~ ~ ~ ~
~ ~
~ ~ ~ ~
11. Operation Support Functions 11.2 Program Test
- 99 -
11.2 Program Test
11.2.1 Dry Run C6 C64
T system L system M system L system T system
F code feed commands for automatic operation can be switched to the manual feed rate data of the machine operation board by turning ON the dry run input signal.
Dry run switch ON Command Rapid traverse
selector switch OFF Rapid traverse
selector switch ON G00, G27, G28, G29, G30, G60 Manual feed rate Rapid traverse rate G01, G02, G03 Manual feed rate Cutting clamp speed
11.2.2 Machine Lock C6 C64
T system L system M system L system T system
When the machine lock input signal is set to ON, the NC operations can be executed without assigning commands to the NC axes. Either the machine lock speed or command speed can be selected using a parameter as the feed rate during machine lock. The M, S, T and B commands are executed as usual, and so machine lock is completed by returning the FIN signal. (1) Reference point return (manual, G28, G29, G30) is controlled as far as the interim point in the
machine lock status but when the interim point is reached the counter is moved to the zero point and the block is completed.
(2) Machine lock is effective in the signal status applying when the axis has stopped. (3) Block stop will be applied if the machine lock signal is turned ON and OFF or OFF and ON
during automatic operation. (Using a parameter, the machine lock signal can be made to take effect immediately.)
(4) Whether the POSITION counter is to be held or the movement amount operated by machine lock is to be canceled when resetting is initiated during machine lock can be selected using a parameter.
11. Operation Support Functions 11.2 Program Test
- 100 -
11.2.3 Miscellaneous Function Lock C6 C64
T system L system M system L system T system
The M, S, T and B (2nd miscellaneous function) output signals are not output to the machine or PLC
when the miscellaneous function lock signal of external input is turned ON. This function can be used when checking only the movement commands in a program check.
The start signals of the M command are output for the M00, M01, M02 and M30 commands, and so a completion signal must be returned. (1) Fixed cycle spindle functions containing an S code and any M, S, T or B function assigned by
a manual numerical command or in automatic operation will not be executed. The code data and strobe (MF, SF, TF, BF) outputs are stopped.
(2) If this signal is set ON after the code data has already been output, the output is executed as it would normally be executed until the end (until FIN1 or FIN2 is received and the strobe is turned OFF).
(3) Even when this signal is ON, the M00, M01, M02 and M30 commands among the miscellaneous functions are executed, and the decode signal, code data and strobe signals are also output as they would be normally.
(4) Any miscellaneous functions which are executed only inside the controller and not output (M96, M97, M98, M99) are executed as they would be normally even if this signal is ON.
11. Operation Support Functions 11.3 Program Search/Start/Stop
- 101 -
11.3 Program Search/Start/Stop
11.3.1 Program Search C6 C64
T system L system M system L system T system
The program No. of the program to be operated automatically can be designated and called. Upon completion of search, the head of the program searched is displayed. Machining programs are stored in the memory inside the NC system.
11.3.2 Sequence Number Search C6 C64
T system L system M system L system T system
Blocks can be indexed by setting the program No., sequence No. and block No. of the program to be operated automatically. The searched program is displayed upon completion of the search. Machining programs are stored in the memory inside the NC system.
11. Operation Support Functions 11.3 Program Search/Start/Stop
- 102 -
11.3.5 Automatic Operation Start C6 C64
T system L system M system L system T system
With the input of the automatic operation start signal (change from ON to OFF), the automatic operation of the program that has been operation searched is started by the controller (or the halted program is restarted).
Automatic operation start (ST)
Movement block G01 X 100... G01 Z 100...
Automatic operation startup is performed on a part system by part system basis.
11.3.6 NC Reset C6 C64
T system L system M system L system T system
This function enables the controller to be reset.
PLC signal
name Target
Reset 1 Reset 2 Reset & Rewind
1 G command modals Retained Initialized Initialized
2 Tool compensation data Retained Canceled (no operations)
Canceled
3 Memory indexing Executed Not executed Executed 4 Errors/alarms Reset Reset Reset 5 M, S and T code outputs Retained Retained Retained
6 M code independent output
OFF OFF OFF
7 Control axis moving Decelerated and stopped
Decelerated and stopped
Decelerated and stopped
8 Output signals "In reset" signal "In reset" signal "In reset" signal "In rewind" signal
11. Operation Support Functions 11.3 Program Search/Start/Stop
- 103 -
11.3.7 Feed Hold C6 C64
T system L system M system L system T system
When the feed hold signal is set ON during automatic operation, the machine feed is immediately decelerated and stopped. The machine is started again by the "Automatic operation start (cycle start)" signal. (1) When the feed hold mode is entered during automatic start, the machine feed is stopped
immediately, but the M, S, T and B commands in the same block are still executed as programmed.
(2) When the mode is switched during automatic operation to manual operation (jog feed, handle feed or incremental feed), the feed hold stop mode is entered.
(3) An interrupt operation based on manual operation (jog feed, handle feed or incremental feed) can be executed during feed hold.
Atomatic operation start
Feed hold
Axis movement state
11.3.8 Search & Start C6 C64
T system L system M system L system T system
If the search & start signal is input in a status where the memory mode is selected, the designated machining program is searched and executed from its head. If the search & start signal has been input during automatic operation in the memory mode, search & start is executed after resetting.
11. Operation Support Functions 11.4 Interrupt Operation
- 104 -
11.4 Interrupt Operation
11.4.1 Manual Interruption C6 C64
T system L system M system L system T system
Manual interrupt is a function that enables manual operations to be performed during automatic operation. The systems used to select the operation mode are as follows: System which initiates the interrupt by switching from the automatic mode to manual mode System which initiates the interrupt by selecting the manual mode at the same time as the
automatic mode (Refer to "11.4.9 Simultaneous Operation of Manual and Automatic Modes".) Whether the manual interrupt amount is to be retained and automatic operation is to be continued is determined by setting manual absolute mode ON or OFF (refer to "11.4.3 Manual Absolute Mode ON/OFF").
11. Operation Support Functions 11.4 Interrupt Operation
- 105 -
11.4.2 Automatic Operation Handle Interruption C6 C64
T system L system M system L system T system
The handle command can interrupt and be superimposed onto a command without suspending automatic operation and the machine can be moved by rotating the manual pulse generator during automatic operation. If the spindle load is greatly exceeded when cutting a workpiece as per the machining program due to a high rough cutting amount in face machining, for instance, automatic handle interrupt makes it possible to raise the Z surface and reduce the load easily without suspending feed in the automatic operation mode. Automatic handle interrupt is conducted by setting the "automatic handle interrupt" valid switch which is provided separately from the "manual operation mode". The axis selection and pulse scale factor operation are conducted as for manual handle feed. Whether, after an interrupt, to return to the path of the machining program by automatic operation or remain offset by the amount equivalent to the interrupt amount is determined using a parameter.
Tool
Workpiece
Automatic feed
Handle feed
G01 Z _ F X _ Y _ ; X _ Y_ ; Z _ Y _ ;
Interrupt
100 10 1
Z Y X
~ ~
Feed path with automatic feed and handle feed superimposed
11. Operation Support Functions 11.4 Interrupt Operation
- 106 -
11.4.3 Manual Absolute Mode ON/OFF C6 C64
T system L system M system L system T system
The program absolute values are updated by an amount equivalent to the distance by which the tool is moved by hand when the manual absolute selection input signal is turned ON. In other words, the coordinate system based on the original program will not shift even if the tool (machine) is moved by hand. Thus, if automatic operation is started in this case, the tool will return to the path before manual movement.
W
Y
X
With manual absolute switch ON
Tool passes along same path as that programmed.
Path after manual interrupt
(Program absolute value is updated by an amount equivalent to traveled value.)
Manual interrupt
Feed hold stop Programmed path (absolute value command)
Path is shifted by an amount equivalent to manual interrupt value. (Zero point moves.)
(Program absolute value is not updated even when there is movement.)
Programmed path (absolute value command)
Manual interrupt
Path after manual interrupt
Feed hold stop
With manual absolute switch OFF
W
Y
X
The switch ON state will be entered when the power is turned ON.
11. Operation Support Functions 11.4 Interrupt Operation
- 107 -
11.4.4 Thread Cutting Cycle Retract C6 C64
T system L system M system L system T system
This function suspends the thread cutting cycle if a feed hold signal has been input during thread cutting in a thread cutting cycle. If a feed hold signal is input during chamfering or thread cutting without chamfering, operation stops at the position where the block following the thread cutting is completed.
Period when thread cutting is performed
Feed hold
Suspension position
Chamfering angle
Position where the block following the thread cutting is completed
11. Operation Support Functions 11.4 Interrupt Operation
- 108 -
11.4.5 Tapping Retract C6 C64
T system L system M system L system T system
If tapping is interrupted by a reset or emergency stop signal that is input during tapping and the tap is left engaged inside the workpiece, the tap tool engaged inside the workpiece can be rotated in the reverse direction so that it will be disengaged by inputting the tap retract signal.
Z axis (spindle)
Tap feed (spindle forward)
Tap retract (spindle reverse)
Retract signal
Tap bottom
This function can be used by an interruption initiated by reset or emergency stop. A return is made to the initial point by tap retract.
11. Operation Support Functions 11.4 Interrupt Operation
- 109 -
11.4.6 Manual Numerical Value Command C6 C64
T system L system M system L system T system
On the screen of the setting and display unit, the M, S and T (and B when 2nd miscellaneous function is valid) commands can be executed by setting numerical values and pressing [INPUT]. This enables operations such as spindle speed changing, starting, stopping, calling and selecting assigned tools and replacing of the spindle tools to be done easily without having to prepare or revise the machining program. Even in an automatic operation mode, these operations can be conducted with block stop. Furthermore, the M and T commands can be issued even on the tool offset amount setting and display screen, therefore at the manual tool length measurement, the tools can be called successively to the spindle and measured very simply without having to change the screen page.
T 12
S 3600
M 5
Manual numerical
value T command value
S command value
Input
3
6
0
2
5
9 8
1
4
7
T
S
M
M command value
PLC sequence processing
(Note) The input operation starts the execution of the M, S or T command.
11.4.8 MDI Interruption C6 C64
T system L system M system L system T system
This function enables MDI programs to be executed during automatic operation in the single block stop status. When the modal status is changed in the MDI program, the modal status in the automatic operation mode is also changed.
11. Operation Support Functions 11.4 Interrupt Operation
- 110 -
11.4.9 Simultaneous Operation of Manual and Automatic Modes C6 C64
T system L system M system L system T system
This function enables manual operations to be performed during automatic operation by selecting an automatic operation mode (MDI or memory) and manual mode (handle, step, jog or manual reference point return) simultaneously. (Arbitrary feed based on the PLC is also possible.)
Axis switching
Automatic operation
Axis control
X
Y
Z
Manual operation
Axis control
X
Y
Z
Memory
MDI
Jog
Handle
Return Manual mode
Automatic mode
Simultaneous manual and automatic operation
X-axis position control
Y-axis position control
Z-axis position control
The feed rates for the axes subject to automatic commands and the feed rates for axes subject to manual command are set separately. The acceleration/deceleration modes (rapid traverse, cutting feed) are also set separately. Rapid traverse override, cutting feed override and second cutting feed override are valid both for axes subject to automatic commands and axes subject to manual commands. Override cancel is valid for axes subject to automatic commands. Manual interlock is applied to axes subject to manual commands; automatic interlock is applies to axes subject to automatic commands.
11.4.10 Simultaneous Operation of JOG and Handle Modes C6 C64
T system L system M system L system T system
When executing the jog feed and handle feed, both these feeds are available without changing the mode each time by inputting the jog mode signal and simultaneous operation of jog and handle modes signal to the control unit. However, during moving in one of the two modes, the feed in the other mode is not valid.
11. Operation Support Functions 11.4 Interrupt Operation
- 111 -
11.4.11 Reference Point Retract C6 C64
T system L system M system L system T system
When the retract signal is turned ON during the automatic and manual operation, this function can retract the tool immediately to a set reference point. The reference point to be retracted to can be selected from the 1st reference point to 4th reference point with 2-bit input signal. Set the retracting order of axes with parameter (#2019 revnum). (1) Other operations
(a) When the retract signal is turned ON, the control unit is reset, the operation is interrupted, and the machining program is indexed.
(b) When the rapid traverse input signal is input, the rapid traverse rate is applied. When the rapid traverse input signal is not input, the manual feed rate is applied.
(c) If the retract signal is input during execution of a tapping cycle, the operation will be the tapping retract, and the normal reference point retract will be executed from the end point of tapping retract operation.
(d) Even if the retract signal is input during the thread cutting cycle, it will be invalid. However, if the retract signal is input in a block other than the thread cutting block, the retracting operation will be executed.
(e) If the retract signal is turned OFF midway during retracting, the operation will decelerate and stop. However, since the machining program is indexed, the block can not be resumed.
(f) The retract signal is invalid if the coordinate system is not established. An operation error will occur when the retract signal is input in such case.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 112 -
12. Program Support Functions 12.1 Machining Method Support Functions 12.1.1 Program
12.1.1.1 Subprogram Control C6 C64
T system L system M system L system T system
8 layers
8 layers
8 layers
8 layers
8 layers When the same pattern is repeated during machining, the machining pattern is registered as one subprogram and the subprogram is called from the main program as required, thereby realizing the same machining easily. Efficient use of program can be made. The call is designated with the program number and sequence number. M98 Pp1 Hh1 Ll1 ;
M98 : Call command Pp1 : Subprogram number Hh1 : Sequence number Ll1 : Number of repetitions
(Branch to subprogram) Op1 (Subprogram) : Nh1 : M99 ; (Return to main program)
Subprograms can be nested up to eight levels deep.
M99;
M98 P2
M99;
M98 P3; M99;
P1000 P2 P8
P1
Main program: Level 0 (P1000)
Main program: Level 1 (P1)
Main program: Level 2 (P2) Main program:
Level 8 (P8)
M02/M30 ;
M98 P1
8- le
ve l n
es tin
g
12. Programming Support Functions 12.1 Machining Method Support Functions
- 113 -
A subprogram branch destination or repetition of a subprogram can be specified.
Subprogram
Specifying a subprogram branch destination
Five repetitions
Return after five repetitions
Main program Main program Subprogram
Specifying repetition of a subprogram
P1000 P1 P1 P1000
M98 P1 H1;
M98 P1 H100;
M02/M30;
N1;
M99;
N100;
M99;
M98 P1 L5;
M02/M30;
M99;
12. Programming Support Functions 12.1 Machining Method Support Functions
- 114 -
12.1.2 Macro Program 12.1.2.1 User Macro
C6 C64 T system L system M system L system T system
4 layers
4 layers
4 layers
4 layers
4 layers
(1) Macro commands (1) ; G65 to G67 In order to carry through one integrated function, a group of control and arithmetic instructions
can be used and registered as a macro program. Furthermore, subprograms with a high degree of expandability can be configured by setting these macro programs as types which are capable of conducting control and arithmetic operations using variable commands.
G code Function
G65 Macro call (Sample call) G66 Macro modal call A G66.1 Macro modal call B G67 Macro modal call cancel
The program formats are given below.
G65 Pp1 Ll1 Argument ;
G65 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment
The macro program is called immediately by this command.
G66 Pp1 Ll1 Argument ;
G66 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment
The macro program is executed from the block with the axis command following this command.
G66.1 Pp1 Ll1 Argument ;
G66.1 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment
The macro program is executed with the word data of each block as the argument.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 115 -
The following macro command functions are available.
Arithmetic commands
#1 =
Assignment of priority of arithmetic operations
The portion in which the operator is to be given priority can be enclosed in [ ]. Up to five pairs of square parentheses [ ] including the function [ ] can be used. The normal priority of operation is functions and multiplication/division followed by addition/subtraction.
Control commands
(1) IF [
END m ;
The flow of the program can be controlled by these commands. "n" denotes the sequence numbers of the branching destination. "m" is an identification number, and 1 to 127 can be used. Note that only 27 nestings can be used.
(Note) The variable commands are provided under the optional specifications independently of the
user macros. If they are to be used, specify the optional specifications separately. (2) Macro commands (2) Specific G commands and the miscellaneous commands (M, S, T, B) can be used for macro
call.
(a) Macro call using G codes Simply by assigning a G code, it is possible to call user macro programs with the prescribed
program number.
Format GXX
GXX : G code for performing macro call
The correspondence between the G code which performs macro call and the program number for the macro to be called is set by a parameter.
1. Up to 10 codes from G00 to G255 can be used for this command. (Whether to use
codes such as G00, G01 or G02 which have already been clearly assigned for specific applications by the EIA standards as macro codes can be changed over using a parameter.)
12. Programming Support Functions 12.1 Machining Method Support Functions
- 116 -
(b) Macro call using miscellaneous commands (M, S, T, B code macro call) Simply by designating an M (or S, T, B) code, it is possible to call user macro programs with
the prescribed program number. (Entered M codes and all S, T and B codes can be used.)
Mm ; (or Ss;, Tt;, Bb;)
Mm (Ss, Tt, Bb) : M (or S, T, B) code for performing macro call
The correspondence between the Mm code which performs macro call and the program number for the macro to be called is set by a parameter. Up to 10 M codes from M00 to M95 can be entered.
Select codes to be entered which are not the codes basically required by the machine and which are not M codes M0, M1, M2, M30 and M96 through M99.
(Note 1) G commands in G code macro programs are not subject to macro calls but normal G
commands. M commands in M code macro programs are not subject to macro calls but normal M commands. (The same applies to S, T and B codes.)
(Note 2) The registration of the program number used for calling the G code macro or M code macro can be done independently for each system. [T system, M system]
12. Programming Support Functions 12.1 Machining Method Support Functions
- 117 -
12.1.2.3 Macro Interruption C6 C64
T system L system M system L system T system
By inputting a user macro interrupt signal from the PLC, the program being currently executed is interrupted and other programs can be called instead. Retract or return operations when tools have been damaged, for instance, and other kinds of restoration operations to be conducted when trouble has occurred are programmed in the interrupt programs. There are two types of interrupts, type 1 and type 2, as described below, and they are selected using a parameter.
[Interrupt type 1] The block being executed is immediately interrupted, and the interrupt program is run immediately.
[Interrupt type 2] After the block being executed is complete, the interrupt program is executed.
The command format is given below. M96 P__ H__ ; User macro interrupt valid M97 ; User macro interrupt invalid
P : Interrupt program No. H :Interrupt sequence No.
M02 ;
M97 ;
M96Ppi;
: :
: : : : : : :
: : : : : : : :
: : : : : : : :
The user macro interrupt signal is accepted during this period.
The user macro interrupt signal is not accepted during this period. The modal information is restored
to the status applying before interrupt.
Interrupt program Opi
Machining program Opm:
Interrupt signal
M99 ;
12. Programming Support Functions 12.1 Machining Method Support Functions
- 118 -
12.1.2.4 Variable Command Programming can be given flexible and general-purpose capabilities by designating variables instead of directly assigning numbers for addresses in programs and by supplying the values of those variables as required when running the programs. Arithmetic operations (adding, subtracting, multiplying and dividing) can also be conducted for the variables.
Number of variable sets specifications The numbers of common variable sets depend on the options, and are as follows.
Variable set option Variables common to all part systems
Variables for each part system
(50+50 number of part systems) sets #500 ~ #549 (50 sets) #100 ~ #149 (50 sets) (100+100 number of part systems) sets #500 ~ #599 (100 sets) #100 ~ #199 (100 sets) (200+100 number of part systems) sets #500 ~ #699 (200 sets) #100 ~ #199 (100 sets)
2. Variable names can be set for #500 ~ #519.
Variable expressions
Variable : # Numerical value #100 (Numerical value: 1, 2, 3, .....)
: # [Expression] #100 Expression :Numerical value
: Variable : Expression Operator Expression #100 + #101 : (minus) Expression #120 : [Expression] [#110] : Function [Expression] SIN [#110]
Variable definition Variable = expression (Note 1) Variables cannot be used with addresses "O" and "N".
12.1.2.4.6 (50+50 x number of part systems) sets C6 C64
T system L system M system L system T system
12.1.2.4.7 (100+100 x number of part systems) sets C6 C64
T system L system M system L system T system
12.1.2.4.8 (200+100 x number of part systems) sets C6 C64
T system L system M system L system T system
12. Programming Support Functions 12.1 Machining Method Support Functions
- 119 -
12.1.3 Fixed Cycle
List of fixed cycles
T system, M system L system Remarks
Type of fixed cycle G code system
1
G code system
2
G code system
3
G70 G80 G80 : : :
G89 G89 G89 G79 G83.2
G98 G98 G98
Fixed cycle for drilling
G99 G99 G99
Refer to 12.1.3.1. Refer to 4.5.3.
G34 G35 - -
Special fixed cycles
G36
Refer to 12.1.3.2.
G90 G77 - G92 G78
Fixed cycles for turning machining
G94 G79
Refer to 12.1.3.3.
G70 G70 : : - G76 G76 G76.1 G76.1
Multiple repetitive fixed cycles for turning machining
G76.2 G76.2
Refer to 12.1.3.4. Refer to 12.1.3.5.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 120 -
12.1.3.1 Fixed Cycle for Drilling C6 C64
T system L system M system L system T system
(1) T system, M system ; G70 to G89, G88, G99 These functions enable drilling, tapping and other hole machining cycles to be assigned in a
simple 1-block program.
G code Function
G70 G71 G72 G73 Step cycle G74 Reverse tapping cycle G75 G76 Fine boring G77 G78 G79 G80 Fixed cycle cancel G81 Drilling, spot drilling cycle G82 Drilling, counterboring cycle G83 Deep hole drilling cycle G84 Tapping cycle G85 Boring cycle G86 Boring cycle G87 Backboring cycle G88 Boring cycle G89 Boring cycle
There are two levels of hole machining axis return which apply upon completion of the fixed
cycle machining operation.
G code Function G98 Initial point level return G99 R point level return
12. Programming Support Functions 12.1 Machining Method Support Functions
- 121 -
The basic program format for the fixed cycle commands is shown below. G81 Xx1 Yy1 Zz1 Rr1 Qq1 Pp1 Ll1 Ff1 ;
G81 : Hole drilling mode Xx1, Yy1 : Hole position data; X-axis, Y-axis hole drilling position command
(rapid traverse) (incremental/absolute) Zz1 : Hole machining data; Hole bottom position designation (incremental/absolute) Rr1 : Hole machining data; Hole R point designation (incremental/absolute) Qq1 : Hole machining data; Depth of cut per pass in G73, G83 cycle
(incremental) Shift amount in G76, G87 cycle Depth of cut per pass in pecking tapping, deep hole tapping of G74, G84 cycle
Pp1 : Hole machining data; Dwell time at hole bottom Ll1 : Hole machining data; Number of fixed cycle repetitions Ff1 : Cutting feed rate
For details on the synchronous tapping cycle, refer to the section "4.5.3 Synchronous Tapping".
12. Programming Support Functions 12.1 Machining Method Support Functions
- 122 -
G73
Step cycle
nq
q
R point
G98 mode
Initial point
G99 mode
Z point
G74 Reverse tapping cycle
M03
M04
Initial point
R point
Z point
G98 mode
G76 Fine boring cycle
q
q
M19 Shift
qInitial point
R point
Z point
G98 mode
G99 mode
G81 Drilling, spot drilling cycle
Initial point
R point
Z point
G98 mode
G99 mode
G82 Drilling, counterboring
cycle
Dwell
Initial point
R point
Z point
G98 mode
G99 mode
G83 Deep hole drilling
cycle
Initial point
n
q
q R point
Z point
G98 mode
G99 mode
G84 Tapping cycle
Initial point
R point
Z point
G98 mode
M03
M04
G85 Boring cycle
Initial point
R point
Z point
G98 mode
G86 Boring cycle
Initial point
R point
Z point
G98 mode M03
M03
M05
G87 Back boring cycle
Initial point
R point M19
Z point M03
M19
G88 Boring cycle
Initial point
R point
Z point G98 mode
M03
M03
M05 Dwell
G89 Boring cycle
Dwell
Initial point
R point
Z point
G98 mode
12. Programming Support Functions 12.1 Machining Method Support Functions
- 123 -
(2) L system; G83 to G89, G80 In the fixed cycle for drilling, a machining program such as drilling, tapping, or boring and
positioning can be executed for a given machining sequence in 1-block commands.
G code Drilling axis
Drilling work start
Motion at hole bottom
Return motion Use
G80 ----- ----- ----- ----- Cancel
G83 Z Cutting feed Intermittent feed
In-position check Dwell
Rapid traverse feed
Deep-hole drilling cycle1
G84 Z Cutting feed In-position check Dwell Spindle CCW
Cutting feed Tapping cycle (Reverse tapping cycle)
G85 Z Cutting feed In-position check Dwell
Cutting feed Boring cycle
G87 X Cutting feed Intermittent feed
In-position check Dwell
Rapid traverse feed
Deep-hole drilling cycle1
G88 X Cutting feed In-position check Dwell Spindle CCW
Cutting feed Tapping cycle (Reverse tapping cycle)
G89 X Cutting feed In-position check Dwell
Cutting feed Boring cycle
G83.2 Z/X Cutting feed Intermittent feed
In-position check Dwell
Rapid traverse feed
Deep-hole drilling cycle2
The fixed cycle mode is canceled when a G command of the G80 or G01 group is specified. Data
is also cleared simultaneously.
Command format
G83/G84/G85 Xx1 Cc1 Zz1 Rr1 Qq11 Pp1 Ff1 Kk1 (Mm1) Ss1 ,Ss1 Dd1 ,Rr1 ; G87/G88/G89 Xx1 Cc1 Zz1 Rr1 Qq11 Pp1 Ff1 Kk1 (Mm1) Ss1 ,Ss1 Dd1 ,Rr1 ;
G83/G84/G85 : Fixed cycle mode of drilling (G83, G87), tapping (G84, G88), or boring (G85, G89)
G87/G88/G89 The drilling command is modal. Once it is given, it is effective until another drill command is given or drilling fixed cycle cancel command is given.
Xx1, Cc1 : Data for positioning X (Z) and C axes The data is unmodal. To execute the same hole machining mode
consecutively, specify the data for each block. Zz1, Rr1, Qq11, Pp1, Ff : Actual machining data in machining Only Q is unmodal. Specify Q in G83 or G87 for each block whenever
the data is required. Kk1 : To repeat in a single cycle for hole machining at equal intervals, specify
the number of repetitions in the range of 0 to 9999 (no decimal point can be used). It is unmodal and is effective only in the block in which the number of repetitions is specified.
If the number of repetitions is omitted, K1 is assumed to be specified. If K0 is specified, hole machining data is stored, but hole machining is
not performed. Hole machining data; R point position (incremental value from initial point) designation (sign ignored).
12. Programming Support Functions 12.1 Machining Method Support Functions
- 124 -
Mm1 : If axis C clamp M command (parameter setting) is given, the M code is
output at the initial point, and after return motion, C axis unclamp M code (clamp M code + 1) is output and the dwell time set in a given parameter is executed.
Ss1 : Designates spindle rotation speed ,Ss1 : Designates spindle rotation speed at retract Dd1 : Designates tap spindle No. for G84 (G88) ,Rr1 : Changes between synchronous/asynchronous in G84 (G88)
The drilling cycle motions generally are classified into the following seven.
Motion 1 Motion 1
Motion 4
Motion 3
Motion 5
Motion 6
Motion 7
R point
Initial point
Motion 1 : Rapid positioning up to the initial point of X (Z) and C axes. If the "positioning axis in-position width" is designated, the in-position check is
conducted upon completion of the block. Motion 2 : Output if the C axis clamp M code is given. Motion 3 : Rapid positioning up to the R point. Motion 4 : Hole machining at cutting feed. If the "drilling axis in-position width" is designated, the in-position check is conducted
upon completion of the block. However, in the case of deep-hole drilling cycles 1 and 2, the in-position check is not conducted with the drilling of any holes except the last one. The in-position check is conducted at the commanded hole bottom position (last hole drilling).
Motion 5 : Motion at the hole bottom position. It varies depending on the fixed cycle mode. Spindle CCW (M04), spindle CW (M03), dwell, etc., are included.
Motion 6: Return to the R point. Motion 7: Return to the initial point at rapid traverse feed. (Operations 6 and 5 may be conducted as a single operation depending on the fixed cycle mode. Note: With a synchronous tap command, the in-position check is conducted in accordance with the
parameters. Whether the fixed cycle is complete with motion 6 or 7 can be specified by using either of the following G commands: G98: Initial level return G99: R point level return These commands are modal. For example, once G98 is given, the G98 mode is entered until G99 is given. The G98 mode is entered in the initial state when the controller is ready.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 125 -
Deep-hole drilling cycle (G83, G87)
G83/G87 Deep-hole drilling cycle (G83: Z-axis direction, G87: X-axis direction)
When Q command is given When Q command is not given
Z / X point
G99 mode G98 mode
n
q q
R point Initial point
Z point / X point R point
Initial point
G99 mode G98 mode
G83.2 Deep-hole drilling cycle
Z / X point
Dwell
Dwell
Dwell
Dwell
Dwell
Dwell
Dwell
G84/88 Tapping cycle
Z / X point
R point Initial point
G98 mode
Reverse rotation of spindle/rotary tool
(C-axis clamp)
(C-axis unclamp) Forward rotation of spindle/rotary tool
Output or no output can be set using a parameter for the C-axis clamp/unclamp M code
G85/89 Boring cycle
f
2f
Z / X point
R point Initial point
G98 mode
(C-axis clamp)
(C-axis unclamp)
Dwell
Dwell
Output or no output can be set using a parameter for the C-axis clamp/unclamp M code
There are two levels of hole machining axis return which apply upon completion of the fixed cycle machining operation. (see the figure above)
G code Function G98 Initial point level return G99 R point level return
12. Programming Support Functions 12.1 Machining Method Support Functions
- 126 -
12.1.3.2 Special Fixed Cycle; G34 to G37 C6 C64
T system L system M system L system T system
Special fixed cycles must always be used in combination with fixed cycles.
(1) Bolt hole circle (G34) The tool starts at the point forming angle with the X axis on the circumference of a circle with radius R whose center is the coordinates designated by X and Y, and it drills "n" number of holes at "n" equal intervals along the circumference of that circle. The drilling data for the standard fixed cycle of the G81 or other such command is retained for the drilling operation at each hole position. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G34 command. G34 Xx Yy Ir J Kn ; Xx, Yy : Center position of bolt hole circle; this is affected by the G90/G91 commands. Ir : Radius "r" of circle; it is based on the least input increment and is provided using a
positive number. J : Angle at point to be drilled initially; the counterclockwise direction is taken to be
positive. Kn : Number "n" of holes to be drilled; any number of holes from 1 through 9999 can be
designated; 0 cannot be assigned. When 0 has been designated, the alarm will occur. A positive number provides
positioning in the counterclockwise direction; a negative number provides positioning in the clockwise direction.
(Example) With 0.001mm least input increment
Position prior to excution of G34 command
G0 command in N005
N001 G91 ; N002 G81 Z 10.000 R5.000 L0 F200 ; N003 G90 G34 X200.000 Y100.000 I100.000 J20.000 K6 ; N004 G80 ; .........................(G81 cancel) N005 G90 G0 X500.000 Y100.000 ;
(500 mm, 100 mm)
20
n = 6 holes
I = 100 mm
X1 = 200 mm
Y1 = 100 mm
W
As shown in the figure, the tool is positioned above the final hole upon completion of the G34 command. This means that when it is to be moved to the next position, it will be necessary to calculate the coordinates in order to issue the command or commands with incremental values, and so it is convenient to use the absolute value mode.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 127 -
(2) Line at angle (G35)
With the starting point at the position designated by X and Y, the tool drills "n" number of holes each at interval "d" in the direction forming angle with the X axis. A standard fixed cycle applies for the drilling operation at each of the hole positions and so there is a need to retain beforehand the drilling data (drilling mode and drilling data). All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G35 command.
G35 Xx Yy Id J Kn ; Xx, Yy : The starting point coordinates; they are affected by the G90/G91 commands. Id : Interval "d"; it is based on the least input increment and when "d" is negative, drilling
proceeds in the point symmetrical direction centered on the starting point. J : Angle ; the counterclockwise direction is taken to be positive. Kn : Number "n" of holes to be drilled including the starting point; any number of holes
from 1 through 9999 can be assigned. (Example)
X1=200mm
W
=30
N=5 holes
Y
X
With 0.001 mm least input increment
Position prior to execution of G35 command
d =100mm
y 1=100mm
G91 ; G81 Z 10.000 R5.000 L 0 F100 ; G35 X200.000 Y100.000 I100.000 J 30.000 K5;
12. Programming Support Functions 12.1 Machining Method Support Functions
- 128 -
(3) Arc (G36)
The tool starts at the point forming angle with the X axis on the circumference of a circle with radius "r" whose center is the coordinates designated by X and Y, and it drills "n" number of holes aligned at angle interval . As with the bolt hole circle function, the drilling operation at each of the hole positions is based on a hold drilling fixed cycle and so there is a need to retain the drilling data beforehand. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G36 command. G36 Xx Yy Ir J P Kn ; Xx, Yy : Center coordinates of arc; they are affected by the G90/G91 commands. Ir : Radius "r" of arc; it is based on the least input increment and is provided with a
positive number. J : Angle at the point to be drilled initially; the counterclockwise direction is taken to be
positive. P : Angle interval ; when it is positive, the tool drills in the counterclockwise direction
and when it is negative, it drills in the clockwise direction. Kn : Number "n" of holes to be drilled; any number of holes from 1 through 9999 can be
assigned.
(Example)
W
=15
With 0.001 mm least input increment
Position prior to execution of G36 command
n=6 holes
Y1=100mm
X1=300mm
=10
N001 G91; N002 G81 Z-10.000 R5.000 F100; N003 G36 X300.000 Y100.000 I300.000 J10.000 P 15.000 K6;
12. Programming Support Functions 12.1 Machining Method Support Functions
- 129 -
(4) Grid (G37.1)
With the starting point at on the position designated by X and Y, this function enables the tool to drill the holes on the lattice with "nx" number of holes at parallel intervals of x to the X axis. Drilling proceeds in the X-axis direction. The drilling operation at each of the hole positions is based on a standard fixed cycle and so there is a need to command the drilling data (drilling mode and drilling data) beforehand. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G37.1 command.
G37.1 Xx1 Yy1 Ix Pnx Jy Kny ;
Xx, Yy : The starting point coordinates; they are affected by the G90/G91 commands. Ix : X-axis interval x; it is based on the least input increment; when x is positive,
the intervals are provided in the positive direction as seen from the starting point and when it is negative, they are provided in the negative direction.
Pnx : Number of holes "nx" in the X-axis direction; any number of holes from 1 through 9999 can be assigned.
Jy : Y-axis interval y; it is based on the least input increment; when y is positive, the intervals are provided in the positive direction as seen from the starting point and when it is negative, they are provided in the negative direction.
Kny : Number of holes "ny" in the Y-axis direction; any number of holes from 1 through 9999 can be assigned.
(Example)
Position prior to execution of G37.1 command
With 0.001 mm least input increment G91 ; G81 ; Z 10.000 R5.000 F20 ; G37.1 X300.000 Y 100.000 I 50.000 P10 J 100.000 K8 ;
x=50mm
nx=10 holes
ny=8 holes
y= 100mm
W y1=100mm
x1=300mm
12. Programming Support Functions 12.1 Machining Method Support Functions
- 130 -
12.1.3.3 Fixed Cycle for Turning Machining; G77 to G79 C6 C64
T system L system M system L system T system
The shape normally programmed in several blocks for rough cutting, etc., in the turning machining can be commanded in one block. This function is useful for machining program simplification. The fixed cycles are as follows:
G code Function G77 Longitudinal cutting cycle G78 Thread cutting cycle G79 Face cutting cycle
Format:
G X/U_Z/W_I_K_R_F_(G18 plane)
Each fixed cycle command for turning machining is a modal G code and is effective until another command of the same modal group or a cancel command is given. The fixed cycle can be canceled by using any of the following G codes:
G00, G01, G02, G03 G09 G10, G11 G27, G28, G29, G30 G31 G33, G34 G37 G92 G52, G53 G65
12. Programming Support Functions 12.1 Machining Method Support Functions
- 131 -
(1) Longitudinal cutting cycle (G77) (a) Longitudinal cutting Straight cutting in the longitudinal direction can be performed consecutively by the following
block:
G77 X/U_ Z/W_ F_ ;
X axis
2 (F)
Z axis X
1 (R)
4 (R)
3 (F)
WZ
U 2
(R) : Rapid traverse feed (F) : Cutting feed
(b) Taper cutting Taper cutting in the longitudinal direction can be performed consecutively by the following
block: G77 X/U_ Z/W_ R_ F_ ;
(R) : Rapid traverse feed (F) : Cutting feed
X axis
Z axis
r
X
1 (R)
4 (R)
3 (F)
W Z
2 (F)
r: Taper part depth (radius designation, incremental value, sign is required)
U 2
12. Programming Support Functions 12.1 Machining Method Support Functions
- 132 -
(2) Thread cutting cycle (G78) (a) Straight thread cutting Straight thread cutting can be performed by the following block:
G78 X/U_ Z/W_ F/E_ ;
Z W
1 (R)2 (F)
4 (R)
3 (R)
X axis
Z axis
X
(R) : Rapid traverse feed (F) : F or E code designation
U 2
(b) Taper thread cutting Taper thread cutting can be performed by the following block:
G78 X/U_ Z/W_ R_ F/E_ ;
Z
r
W
1 (R) 2 (F)
4 (R)
3 (R)
X
(R) : Rapid traverse feed (F) : F or E code designation
X axis
Z axis
r: Taper part depth (radius designation, incremental value, sign is required)
U 2
12. Programming Support Functions 12.1 Machining Method Support Functions
- 133 -
Chamfering
: Thread cutting-up amount Assuming that thread lead is L, the thread cutting-up amount can be set in a given parameter in 0.1L steps in the range of 0 to 12.7L.
: Thread cutting-up angle
The thread cutting-up angle can be set in a given parameter in 1 steps in the range of 0 to 89.
(3) Face cutting cycle (G79) (a) Straight cutting Straight cutting in the end face direction can be performed consecutively by the following block:
G79 X/U_ Z/W_ F_ ;
X Z W
1(R)
2(F) 4(R)
3(F)
(R): Rapid traverse feed
(F): Cutting feed
X axis
Z axis
u / 2
12. Programming Support Functions 12.1 Machining Method Support Functions
- 134 -
(b) Taper cutting Taper cutting in the end face direction can be performed consecutively by the following block:
G79 X/U_ Z/W_ R_ F_ ;
X
r
Z W
1(R)
2(F) 4(R)
3(F)
Z axis
X axis
(R): Rapid traverse feed
(F): Cutting feed
r: Taper part depth (radius designation, incremental value, sign is required)
u / 2
12. Programming Support Functions 12.1 Machining Method Support Functions
- 135 -
12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining; G70 to G76 C6 C64
T system L system M system L system T system
(a) Longitudinal rough cutting cycle I (G71) The finish shape program is called, and straight rough cuttingis performed while intermediate
path is being calculated automatically. The machining program is commanded as follows.
G71 Ud Re ; G71 Aa Pp Qq Uu Ww Ff Ss Tt ; Ud : Cut depth d. (When P,Q command is not given). (Modal) Re : Retract amount e. (Modal) Aa : Finish shape program No. (If it is omitted, the program being executed is
assumed to be designated.) Pp : Finish shape start sequence No. (If it is omitted, the program top is
assumed to be designated.) Qq : Finish shape end sequence No. (If it is omitted, the program end is
assumed to be designated.) However, if M99 precedes the Q command, up to M99. Uu : Finishing allowance in the X axis direction. (When P, Q command is given).
(Diameter or radius designation) Ww : Finishing allowance in the Z axis direction. Ff : Cutting feed rate. Ss : Spindle speed. Tt : Tool command.
F, S, and T command in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.
(R)
(Cycle commanded point)
d Cut depth
Details of retract operation
(R) (F)
(F)
45 e
u / 2
W Finishing allowance
X
Z
12. Programming Support Functions 12.1 Machining Method Support Functions
- 136 -
(b) Face rough cutting cycle (G72) The finish shape program is called, and rough turning is performed in the end face direction
while intermediate path is being calculated automatically. The machining program is commanded as follows.
G72 Wd Re ; G72 Aa Pp Qq Uu Ww Ff Ss Tt ; Wd : Cut depth d. (When P,Q command is not given). (Modal) Re : Retract amount e. (Modal) Aa : Finish shape program No. (If it is omitted, the program being executed is
assumed to be designated.) Pp : Finish shape start sequence No. (If it is omitted, the program top is assumed
to be designated.) Qq : Finish shape end sequence No. (If it is omitted, the program end is assumed
to be designated.) However, if M99 precedes the Q command, up to M99. Uu : Finishing allowance in the X axis direction. Ww : Finishing allowance in the Z axis direction. (When P, Q command is given.) Ff : Cutting feed
rate. Ss : Spindle speed. Tt : Tool command.
F, S, and T command in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.
(Cycle commanded point)
d Cut depth
u / 2
W
Finishing allowance
(R)
Details of retrace operation
(F)
(F)
e
X
Z
45
S
E
12. Programming Support Functions 12.1 Machining Method Support Functions
- 137 -
(c) Molding material in rough cutting cycle (G73) The finish shape program is called. Intermediate path is automatically calculated and rough
cuttingis performed conforming to the finish shape. The machining program is commanded as follows.
G73 Ui Wk Rd ; G73 Aa Pp Qq Uu Ww Ff Ss Tt ; Ui : Cutting allowance in the X axis direction Wk : Cutting allowance in the Z axis direction Rd : Split count
i k d
Cutting allowance when P, Q command is not given.
Modal data Sign is ignored. Cutting allowance is given with a radius
designation.
Aa Finish shape program No. (If it is omitted, the present program is assumed to be designated.)
Pp Finish shape start sequence No. (If it is omitted, the program top is assumed to be designated.)
Qq Finish shape end sequence No. (If it is omitted, the program end is assumed to be designated.) However, if M99 precedes the Qq command, up to M99.
Uu : Finishing allowance in the X axis direction u Ww : Finishing allowance in the Z axis direction w
Finishing allowance when P, Q command is given.
Sign is ignored. Diameter or radius is designated according
to the parameter. The shift direction is determined by the
shape. Ff : Cutting feed rate (F function) Ss : Spindle speed (S function) Tt : Tool selection (T function)
The F, S, and T commands in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.
k + w
X
Z
S1 S2
S3
S
i + u/2
u/2 w A
E
2
3 4
5 6
7
8
9 10
11 12
13
14
15 16
17 18
19
1
12. Programming Support Functions 12.1 Machining Method Support Functions
- 138 -
(d) Finish cycle (G70) After rough cutting is performed by using G71 to G73, finish turning can be performed by using
the G70 command. The machining program is commanded as follows.
G70 A_ P_ Q_ ;
A : Finish shape program number. (If it is omitted, the program being executed is assumed to be designated.)
P : Finish shape start sequence number. (If it is omitted, the program top is assumed to be designated.)
Q : Finish shape end sequence number. (If it is omitted, the program end is assumed to be designated.) However, if M99 precedes the Q command, up to M99.
(1) The F, S, and T commands in the rough cutting cycle command G71 to G73 blocks are
ignored, and the F, S, and T commands in the finish shape program become effective. (2) The memory address of the finish shape program executed by G71 to G72 is not stored.
Whenever G70 is executed, a program search is made. (3) When the G70 cycle terminates, the tool returns to the start point at the rapid traverse feed
rate and the next block is read. (Example 1) Sequence No. designation
N200 ; N300 ;
N100 G70 P200 Q300 ;
N110
N120
N200
Finish shape program
N300
N310
:
:
:
:
:
(Example 2) Program No. designation
N100 G70 A100 ;
N110 ; N120 ;
:
O100
G01 X100 Z50 F0.5 ; M99 ;
: :
In either example 1 or 2, after the N100 cycle is executed, the N110 block is executed.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 139 -
(e) Face cutting-off cycle (G74) When the slotting end point coordinates, cut depth, cutting tool shift amount, and cutting tool
relief amount at the cut bottom are commanded, automatic slotting is performed in the end face direction of a given bar by G74 fixed cycle. The machining program is commanded as follows.
G74 Re ; G74 X/(U) Z/(W) Pi Qk Rd Ff ;
Re : Retract amount e (when X/U, Z/W command is not given) (Modal) X/U : B point coordinate (absolute/incremental) Z/W : B point coordinate (absolute/incremental) Pi : Tool shift amount (radius designation, incremental, sign not required) Qk : Cut depth k (radius designation, incremental, sign not required) Rd : Relief amount at cut bottom d (If sign is not provided, relief is made at the
first cut bottom. If minus sign is provided, relief is made not at the first cut bottom but at the second cut bottom and later.)
Ff : Feed rate
k k k k x
u/2
(1) (2)(3)(4)
(5) (6)(7)(8)
(9) (10)
(11)
(12) i
d
e
wz
B
S (start point)
(9) and (12) just before the last cycle are executed with the remaining distance.
(2), (4), (6), (8), (10), (11) and
(12) are executed at the rapid traverse feed rate.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 140 -
(f) Longitudinal cutting-off cycle (G75) When the slotting end point coordinates, cut depth, cutting tool shift amount, and cutting tool
relief amount at the cut bottom are commanded, automatic slotting is performed in the longitudinal direction of a given bar by G75 fixed cycle. The machining program is commanded as follows.
G75 Re ; G75 X/(U) Z/(W) Pi Qk Rd Ff ; Re : Retract amount e (when X/U, Z/W command is not given) (Modal) X/U : B point coordinate (absolute/incremental) Z/W : B point coordinate (absolute/incremental) Pi : Tool shift amount (radius designation, incremental, sign not required) Qk : Cut depth k (radius designation, incremental, sign not required) Rd : Relief amount at cut bottom d (If sign is not provided, relief is made at the
first cut bottom. If sign is provided, relief is made not at the first cut bottom but at the second cut bottom and later.)
Ff : Feed rate
k x
u / 2
(1)(2)
(3)
(4) (5)
(6) (7)
(8) (9)
(10)
(11)
(12)i
d
e
wz
B
S (start point)
i
i
i
(9) and (12) just before the last cycle are executed with the remaining distance.
(2), (4), (6), (8), (10), (11) and
(12) are executed at the rapid traverse feedrate.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 141 -
(g) Multiple repetitive thread cutting cycle (G76) When the thread cutting start and end points are commanded, cut at any desired angle can be
made by automatically cutting so that the cut section area (cutting torque) per time becomes constant in the G76 fixed cycle.
Various longitudinal threads can be cut by considering the thread cutting end point coordinate and taper height constituent command value.
Command Format
G76 Pmra Rd ; G76 X/U Z/W Ri Pk Qd Fl ; m : Cut count at finishing 01 to 99 (modal) r : Chamfering amount 00 to 99 (modal). Set in 0.1-lead increments. a : Nose angle (included angle of thread) 00 to 99 (modal) Set in 1-degree
increments. d : Finishing allowance (modal) X/U : X axis end point coordinate of thread part. Designate the X coordinate of the end point in the thread part in an
absolute or incremental value. Z/W : Z axis end point coordinate of thread part. Designate the Z coordinate of the end point in the thread part in an absolute
or incremental value. i : Taper height constituent in thread part (radius value). When i = 0 is set, straight
screw is made. k : Thread height. Designate the thread height in a positive radius value. d : Cut depth. Designate the first cut depth in a positive radius value. l : Thread lead
Configuration of one cycle In one cycle, (1), (2), (5), and (6) move at rapid traverse feed and (3) and (4) move at cutting
feed designated in F.
rx
(-i) k
z w
S
u/2
(1)
(2)
(3)
(4)
(5)
(6)
a/2When Ri is negative
12. Programming Support Functions 12.1 Machining Method Support Functions
- 142 -
r x
i
k
z w
S
u/2
(1)
(2)
(3)(4)
(5)
(6)
a/2
When Ri is positive
k
a
d x 2
d x n d (finishing allowance) (Cut "m" times at finishing)
nth time
Second time
First time
d
12. Programming Support Functions 12.1 Machining Method Support Functions
- 143 -
12.1.4 Mirror Image 12.1.4.3 G Code Mirror Image
C6 C64 T system L system M system L system T system
Using a program for the left or right side of an image, this function can machine the other side of the image when a left/right symmetrical shape is to be cut.
Mirror image can be applied directly by a G code when preparing a machining program.
The program format for the G code mirror image is shown below. G51.1 Xx1 Yy1 Zz1 ;
G51.1 : Mirror image on Xx1, Yy1, Zz1 : Command axes and command positions
With the local coordinate system, the mirror image is applied with the mirror positioned respectively at x1, y1 and z1. The program format for the G code mirror image cancel is shown below.
G50.1 Xx1 Yy1 Zz1 ; G50.1 : Mirror image cancel Xx1, Yy1, Zz1 : Command axes
The coordinate word indicates the axes for which the mirror image function is to be canceled and the coordinates are ignored. In the case of G51.1 Xx1
Y
X
Original shape (program)
Mirroring axis
Shape achieved when machining program for the left side has been executed after the mirror command
12. Programming Support Functions 12.1 Machining Method Support Functions
- 144 -
12.1.4.4 Mirror Image for Facing Tool Posts C6 C64
T system L system M system L system T system
With machines in which the base tool post and facing tool post are integrated, this function enables the programs prepared for cutting at the base side to be executed by the tools on the facing side. The distance between the two posts is set beforehand with the parameter.
The command format is given below. G68; Facing tool post mirror image ON G69; Facing tool post mirror image OFF
When the G68 command is issued, the subsequent program coordinate systems are shifted to the facing side and the movement direction of the X axis is made the opposite of that commanded by the program. When the G69 command is issued, the subsequent program coordinate systems are returned to the base side. The facing tool post mirror image function can be set to ON or OFF automatically by means of T (tool) commands without assigning the G68 command. A parameter is used to set ON or OFF for the facing tool post mirror image function corresponding to the T commands.
Programmed path
Facing side path (mirror image ON)
Z
X
Base post
Facing post
(G69)
Parameter for distance between posts (radial value, X axis only)
(G68)
12. Programming Support Functions 12.1 Machining Method Support Functions
- 145 -
12.1.5 Coordinate System Operation 12.1.5.1 Coordinate Rotation by Program
C6 C64 T system L system M system L system T system
When it is necessary to machine a complicated shape at a position that has been rotated with respect to the coordinate system, you can machine a rotated shape by programming the shape prior to rotation on the local coordinate system, then specifying the parallel shift amount and rotation angle by means of this coordinate rotation command. The program format for the coordinate rotation command is given below.
G68 Xx1 Yy1 Rr1 ; Coordinate rotation ON
G69 ; Coordinate rotation cancel
G68 : Call command Xx1, Yy1 : Rotation center coordinates Rr1 : Angle of rotation
(1) Angle of rotation "r1" can be set in least input increment from 360 to 360. (2) The coordinates are rotated counterclockwise by an amount equivalent to the angle which is
designated by angle of rotation "r1". (3) The counter is indicated as the point on the coordinate system prior to rotation. (4) The rotation center coordinates are assigned with absolute values.
(Original local coordinate system)
(Rotated local coordinate system)
r1 (Angle of rotation)
(x1, y1) (Center of rotation)
X
X
x1
W
W
Y
Y
y1
12. Programming Support Functions 12.1 Machining Method Support Functions
- 146 -
(Example) N01 G28 X Y Z ;
N02 G54 G52 X150. Y75. ; Local coordinate system assignment N03 G90 G01 G42 X0 Y0 ; Tool radius compensation ON N04 G68 X0 Y0 R30. ; Coordinate rotation ON N05 M98 H101 ; Subprogram execution N06 G69 ; Coordinate rotation cancel N07 G54 G52 X0 Y0 ; Local coordinate system cancel N08 G00 G40 X0 Y0 ; Tool radius compensation cancel N09 M02 ; Completion
Sub program (Shape programmed with original coordinate system)
N101 G90 G01 X50. F200 ; N102 G02 X100. R25. ; N103 G01 X125. ; N104 Y75. ; N105 G03 X100. Y100. R25. ; N106 G01 X50. ; N107 G02 X0 Y50. R50. ; N108 G01 X0 Y0 ; N109 M99 ;
100.
100. 300.200.
Y
X
200.
W
Actual machining shape
(Programmed coordinate)
12. Programming Support Functions 12.1 Machining Method Support Functions
- 147 -
12.1.6 Dimension Input 12.1.6.1 Corner Chamfering / Corner R
C6 C64 T system L system M system L system T system
This function executes corner processing by automatically inserting a straight line or arc in the commanded amount between two consecutive movement blocks (G01/G02/G03). The corner command is executed by assigning the ",C" or ",R" command for the block at whose end point the corner is inserted.
(1) Corner chamfering / Corner R I
When ",C" or ",R" is commanded for linear interpolation, corner chamfering or corner R can be inserted between linear blocks. Corner chamfering Corner R Example: Example:
N1 G01 Xx1 Zz1, Cc1 ; N2 Zz2 ;
N2 c 1
c 1
N1
N1 G01 Xx1 Zz1, Rr1 ; N2 Zz2 ;
N2
r 1 N1
(Note 1) If a corner chamfering or corner R command is issued specifying a length longer than the N1 or N2 block, a program error occurs.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 148 -
(2) Corner chamfering / corner R II (L system)
When ",C" or ",R" is command in a program between linear-circular, corner chamfering or corner R can be inserted between blocks.
(a) Corner chamfering II (Linear circular)
Cc1Hypothetical corner intersection
Cc1
Chamfering end point
Chamfering start point
Example: G01 X_Z_ ,Cc1 ;
(1)
(2)
G02 X_Z_ Ii1 Kki ;
(b) Corner chamfering II (Circular - linear)
Cc1
(1)
Cc1
Hypothetical corner intersection
Chamfering start point
Chamfering end point
Example: G03 X_Z_ Ii1 Kk1 ,Cc1 ;
(2)
G01 X_Z_ ;
(c) Corner chamfering II (Circular - circular)
(2)
Cc1
(1)
Cc1
Hypothetical corner intersection
Example: G02 X_Z_ Ii1 Kk1 ,Cc1 ; G02 X_Z_ Ii2 Kk2 ;
Chamfering start point
Chamfering end point
12. Programming Support Functions 12.1 Machining Method Support Functions
- 149 -
(d) Corner R II (Linear - circular)
(2)
(1)
Rr1
Hypothetical corner intersection
Corner R start point
Corner R end point
Example: G01 X_Z_ ,Rr1 ; G02 X_Z_ Ii1 Kk1 ;
(e) Corner R II (Circular linear)
(2)
(1)
Rr1
Hypothetical corner intersection
Example: G03 X_Z_ Ii1 Kk1 ,Rr1 ; G01 X_Z_ ;
Corner R start point
Corner R end point
(f) Corner R II (Circular circular)
(2)
(1)
Rr1
Hypothetical corner intersection
Corner R start point
Corner R start point
Example: G02 X_Z_ Ii1 Kk1 ,Rr1 ; G02 X_Z_ Ii2 Kk2 ;
12. Programming Support Functions 12.1 Machining Method Support Functions
- 150 -
(3) Specification of corner chamfering / corner R speed E
An E command can be used to specify the speed for corner chamfering or corner R. This enables a corner to be cut to a correct shape. (Example)
F
F
F
F
E
E
G01 X_Z_ ,Cc1 Ff1 Ee1 ; X_Z_ ;
G01 X_Z_ ,Rr1 Ff1 Ee1 ; X_Z_ ;
X
Z
An E command is a modal and remains effective for feeding in next corner chamfering or corner R. An E command has two separate modals: synchronous and asynchronous feed rate modals. The effective feed rate is determined by synchronous (G95) or asynchronous (G94) mode. If an E command is specified in 0 or no E command has been specified, the feed rate specified by an F command is assumed as the feed rate for corner chamfering or corner R. Hold or non-hold can be selected (M system only) using a parameter for the E command modal at the time of resetting. It is cleared when the power is turned OFF (as it is with an F command).
12. Programming Support Functions 12.1 Machining Method Support Functions
- 151 -
12.1.6.3 Geometric Command C6 C64
T system L system M system L system T system
When it is difficult to find the intersection point of two straight lines with a continuous linear interpolation command, this point can be calculated automatically by programming the command for the angle of the straight lines.
Example
N 1
a 2
X
Z W 1
N2
a1
N1 G01 Aa1 Ff1 ; N2 Xx1 Zz1 Aa2 ;
End point (X1, Z1)
Automatic intersection point calculation
Z1
x1 2
Start point
a: Angle () formed between straight line and horizontal axis on plane. The plane is the selected plane at this point.
(Note 1) This function cannot be used when using the A axis or 2nd miscellaneous function A.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 152 -
(1) Automatic calculation of two-arc contact
When two continuous circular arcs contact with each other and it is difficult to find the contact, the contact is automatically calculated by specifying the center coordinates or radius of the first circular arc and the end point absolute coordinates and center coordinates or radius of the second circular arc. Example
G18 G02 Ii1 Kk1 Ff1 ; G03 Xxc Zzx Ii2 Kk2 Ff2 ;
or G18 G02 Ii1 Kk1 Ff1 ;
G03 Xxc Zzc Rr2 Ff2 ; or G18 G02 Rr1 Ff1 ; G03 Xxc Zzc Ii2 Kk2 Ff2 ;
C(xc, zc)
r2
(p2,q2)
(p1,q1)
B(?,?) r1
A
I and K are circular center coordinate incremental values; distances from the start point in the first block or distances from the end point in the second block. P and Q commands (X, Z absolute center coordinates of circular arc) can be given instead of I and K commands.
(2) Automatic calculation of linear-arc intersection
When it is difficult to find the intersections of a given line and circular arc, the intersections are automatically calculated by programming the following blocks. Example
G18 G01 Aa1 Ff1 ; G02 Xxc Zzc Ii2 Kk2 Hh2 Ff2 ;
r1
(p2,q2)
B(?,?)
B(?,?) a1
A C(xc, zc)
I and K : Incrimental coordinates from circular end point P and Q : Absolute center coordinates of circular arc H = 0 : Intersection with shoter line H = 1 : Intersection with longer line
12. Programming Support Functions 12.1 Machining Method Support Functions
- 153 -
(3) Automatic calculation of arc-linear intersection
When it is difficult to find the intersections of a given circular arc and line, the intersections are automatically calculated by programming the following blocks. Example G18 G03 Ii1 Kk1 Hh1 Ff1 ; G01 Xxc Zzc Aa1 Ff2 ;
r1 a1
C(xc, zc)
B(?,?) B(?,?)
(p1,q1)
A
I and K : Incrimental coordinates from circular end point P and Q : Absolute center coordinates of circular arc (L3 only) H = 0 : Intersection with shoter line H = 1 : Intersection with longer line
(4) Automatic calculation of linear-arc contact
When it is difficult to find the contact of a given line and circular arc, the contact is automatically calculated by programming the following blocks. Example
G01 Aa1 Ff1 ; G03 Xxc Zzc Rr1 Ff2 ;
a1
A
B (?,?)
r1
C(xc, zc)
12. Programming Support Functions 12.1 Machining Method Support Functions
- 154 -
(5) Automatic calculation of arc-linear contact
When it is difficult to find the contact of a given circular arc and line, the contact is automatically calculated by programming the following blocks. Example
G02 Rr1 Ff1 ; G01 Xxc Zzc Aa1 Ff2 ;
a1 r1
A B (?,?)
C(xc, zc)
12. Programming Support Functions 12.1 Machining Method Support Functions
- 155 -
12.1.7 Axis Control 12.1.7.5 Circular Cutting
C6 C64 T system L system M system L system T system
In circular cutting, a system of cutting steps are performed: first, the tool departs from the center of the circle, and by cutting along the inside circumference of the circle, it draws a complete circle, then it returns to the center of the circle. The position at which G12 or G13 has been programmed serves as the center of the circle.
G code Function G12 G13
CW (clockwise) CCW (counterclockwise)
The program format is given below. G12/13 Ii Dd Ff ; G12/13 Ii Dd Ff
: Circular cutting command : Radius of complete circle : Compensation number : Feed rate
When the G12 command is used (path of tool center) 0 1 2 3 4 5 6 7 0 When the G13 command is used (path of tool center) 0 7 6 5 4 3 2 1 0 (Notes)
Circular cutting is undertaken on the plane which has been currently selected (G17, G18 or G19).
The (+) and () signs for the compensation amount denote reduction and expansion respectively.
Y
X
1
2
3
4
5
6
7
0
Radius of circle
Offset amount
12. Programming Support Functions 12.1 Machining Method Support Functions
- 156 -
12.1.8 Multi-part System Control 12.1.8.1 Synchronization between Part Systems
C6 C64 T system L system M system L system T system
The multi-axis, multi-part system compound control CNC system can simultaneously run multiple machining programs independently. This function is used in cases when, at some particular point during operation, the operations of different part systems are to be synchronized or in cases when the operation of only one part system is required.
! ;
! ;
! ;
%
Simultaneous and independent operation
Synchronized operation
Simultaneous and
i d d t ti
Part system 2 operation only;
part system 1 waits
Synchronized operation
Synchronized operation
Simultaneous and independent operation
! ;
%
No program
! ;
! ;
Part system 1 machining program Part system 2 machining program
12. Programming Support Functions 12.1 Machining Method Support Functions
- 157 -
Command format (1) Command for synchronizing with part system n
! n L 1 ; n : Part system number 1 : Synchronizing number 01 to 9999
$1
!2L1;
!3L2;
$2 $3
!1L1;
!1L2;
Synchro- nized operation
Synchronized operation
(2) Command for synchronizing among three part systems ! n ! m L 1 ;
n, m: Part system number n m 1 : Synchronizing number 01 to 9999
$1 $2 $3
!2!3L1 ;
!1!3L1 ;
!1!2L1 ;
Synchronized operation
Synchronized operation
12. Programming Support Functions 12.1 Machining Method Support Functions
- 158 -
12.1.8.2 Start Point Designation Synchronization C6 C64
T system L system M system L system T system
The synchronizing point can be placed in the middle of the block by designating the start point. (1) Start point designation synchronization Type 1 (G115) Command format
!Ll G115 X_ Z_ ; !Ll G115 X_, Z_
: Synchronizing command : G command : Own start point (designate other part system's coordinate value)
(a) The other part system starts first when synchronizing is executed. (b) The own part system waits for the other part system to move and reach the designated start
point, and then starts.
!G115
!G115
Own part system
Other part system
Designated start point
Designated start point
Synchronized operation
! Synchronized operation
!
Own part system
Other part system
(c) When the start point designated by G115 is not on the next block movement path of the
other part system, the own part system starts once the other part system has reached all of the start point axis coordinates.
: Movement : Command point : Actual start point
12. Programming Support Functions 12.1 Machining Method Support Functions
- 159 -
(2) Start point designation synchronization Type 2 (G116) Command format
!Ll G116 X_ Z_ ; !Ll G116 X_, Z_
: Synchronizing command : G command : Other start point (designate own part system's coordinate value)
(a) The own part system starts first when synchronizing is executed. (b) The other part system waits for the own part system to move and reach the designated start
point, and then starts.
Synchronized operation
Other part system !
Own part system !G116 Designated start point
Own part system
Synchronized operation Other part system !
Designated start point !G116
(c) When the start point designated by G116 is not on the next block movement path of the
own part system, the other part system starts once the own part system has reached all of the start point axis coordinates.
: Movement : Command point : Actual start point
12. Programming Support Functions 12.1 Machining Method Support Functions
- 160 -
12.1.8.6 Balance Cut; G14/G15 C6 C64
T system L system M system L system T system
When workpiece that is relatively long and thin is machined on a lathe, deflection may result, making it impossible for the workpiece to be machined with any accuracy. In cases like this, the deflection can be minimized by holding tools simultaneously from both sides of the workpiece and using them in synchronization to machine the workpiece (balance cutting). This method has an additional advantage: since the workpiece is machined by two tools, the machining time is reduced. The balance cutting function enables the movements of the tool rests belonging to part system 1 and part system 2 to be synchronized (at the block start timing) so that this kind of machining can easily be accomplished.
Part system 1
Part system 2
The command format is given below. G14 Balance cut command OFF (modal) G15 Balance cut command ON (modal)
G14 and G15 are modal commands. When the G15 command is assigned, the programmed operations of two part systems are synchronized (at the block start timing) for all blocks until the G14 command is assigned or until the modal information is cleared by the reset signal.
Part system 1 program Part system 2 program
T0101; G00 X_ Z_; G15; G01 Z_ F0.4;
T0102; G00 X_ Z_; G15; G01 Z_ F0.4;
... ...
.
... ...
.
Whereas synchronization is possible only with the next block when using the code ! of synchronization between part systems, the balance cutting function provides synchronization (at the block start timing) with multiple consecutive blocks.
12. Programming Support Functions 12.1 Machining Method Support Functions
- 161 -
12.1.8.8 2-part System Synchronous Thread Cutting; G76.1/G76.2 C6 C64
T system L system M system L system T system - - -
The 2-part system synchronous thread cutting cycle is the function which performs synchronous thread cutting for the same spindle by part systems 1 and 2. The 2-part system synchronous thread cutting cycle is "2-part system synchronous thread cutting cycle I" (G76.1) for synchronous thread cutting of two screws or "2-part system synchronous thread cutting cycle II" (G76.2) for thread cutting of one screw.
(1) 2-part system synchronous thread cutting cycle (I)
Command format
G76. 1 X/U_ Z/W_ Ri Pk Qd Fl ; X/U Z/W i k d l
: X axis end point coordinate of screw .... Designate the X coordinate of the end point at screw in an absolute or incremental value.
: Z axis end point coordinate of screw .... Designate the Z coordinate of the end point at screw in an absolute or incremental value.
: Height constituent of taper at screw (radius value) ... When i is 0, a straight screw is generated.
: Screw thread height .... Designate the thread height in a positive radius value. : Cut depth .... Designate the first cut depth in a positive radius value. : Thread lead
If G76.1 command is given in part system 1 or 2, a wait is made until G76.1 command is given in the other part system. Once the G76.1 command exists in both part systems, the thread cutting cycle is started.
G00 X_ Z_ ;
G76.1 . ; G00 X_ Z_ ;
G76.1 . ;
$ 2
Command for part system 1
Command for part system 2
$ 1
12. Programming Support Functions 12.1 Machining Method Support Functions
- 162 -
(2) 2-part system synchronous thread cutting cycle (II)
Command format
G76. 2 X/U_ Z/W_ Ri Pk Qd Aa Fl ; a : Thread cutting start shift angle
a
Thread cutting command waits for 1-revolution synchronizing signal of the spindle encoder and starts moving. The start point can be delayed by thread cutting start angle.
The address except A has the same meanings as those in 2-part system synchronous thread cutting cycle I. If G76.2 command is given in part system 1 or 2, a wait is made until G76.2 command is given in the other part system. Once the G76.2 command exists in both part systems, the thread cutting cycle is started.
G00 X_ Z_ ;
G76.2 . ; G00 X_ Z_ ;
G76.2 . ;
$ 2$ 1
In the G76.2 cycle, the same screw is assumed to be cut, and it is cut deeply according to alternate cut depth in part systems 1 and 2.
Command according to part system 1
(1): Cut by part system 1
(2): Cut by part system 2
Simultaneously machine on
screw with both part systems
Command according to part system 2
(1)
a
(2)
K
Finishing allowance d
1 d
(2) (2)
(1) (1) (2)(1) (2) (1)
2 d x 2 d x n
12. Programming Support Functions 12.1 Machining Method Support Functions
- 163 -
12.1.9 Data Input by Program 12.1.9.1 Parameter Input by Program
C6 C64 T system L system M system L system T system
The parameters set from the setting and display unit can be changed using the machining programs. The format used for the data setting is shown below.
G10 L50 ; ....... Data setting command
P Major classification No. A Axis No. N Data No. H Bit type data ; P Major classification No. A Axis No. N Data No. D Byte type data ; P Major classification No. A Axis No. N Data No. S Word type data ; P Major classification No. A Axis No. N Data No. L 2-word type data ;
G11 ; .. Data setting mode cancel (data setting completed)
The following types of data formats can be used according to the type of parameter (axis-common and axis-independent) and data type.
With axis-common data
Axis-common bit-type parameter -------------------- P N H ; Axis-common byte-type parameter------------------- P N D ; Axis-common word-type parameter ------------------ P N S ; Axis-common 2-word-type parameter --------------- P N L ;
With axis-independent data
Axis-independent bit-type parameter ---------------- P A N H ; Axis-independent byte-type parameter-------------- P A N D ; Axis-independent word-type parameter ------------- P A N S ; Axis-independent 2-word-type parameter ---------- P A N L ;
(Note 1) The order of addresses in a block must be as shown above. (Note 2) For a bit type parameter, the data type will be H ( is a value between 0 and 7). (Note 3) The axis number is set in the following manner: 1st axis is "1", 2nd axis is "2", and so forth.
When using the multi-part system, the 1st axis in each part system is set as "1", the 2nd axis is set as "2", and so forth.
(Note 4) Command G10L50 and G11 in independent blocks. A program error will occur if not commanded in independent blocks.
Depending on the G90/G91 modal status when the G10 command is assigned, the data is used to overwrite the existing data or added.
Parameter settings in data setting mode
12. Programming Support Functions 12.1 Machining Method Support Functions
- 164 -
12.1.9.2 Compensation Data Input by Program C6 C64
T system L system M system L system T system
(1) Workpiece coordinate system offset input The value of the workpiece coordinate systems selected by the G54 to G59 commands can be
set or changed by program commands.
G code Function G10 L2 P0 External workpiece coordinate system setting G10 L2 P1 Workpiece coordinate system 1 setting (G54) G10 L2 P2 Workpiece coordinate system 2 setting (G55) G10 L2 P3 Workpiece coordinate system 3 setting (G56) G10 L2 P4 Workpiece coordinate system 4 setting (G57) G10 L2 P5 Workpiece coordinate system 5 setting (G58) G10 L2 P6 Workpiece coordinate system 6 setting (G59)
The format for the workpiece coordinate system setting commands is shown below.
G10 L2 Pp1 Xx1 Yy1 Zz1 ; G10 L2 Pp1 Xx1, Yy1, Zz1
: Parameter change command : Workpiece coordinate No. : Settings
(Note) L2 can be omitted. Omitting Pp1 results in a program error. [T system, M system]
12. Programming Support Functions 12.1 Machining Method Support Functions
- 165 -
(2) Tool offset input The tool offset amounts, which have been set from the setting and display unit, can be input by
program commands. The command format differs between the [T system, M system] and the [L system]. The
respective command format must be set by a parameter. [T system, M system]
G code Function G10 L10 Tool length shape offset amount G10 L11 Tool length wear offset amount G10 L12 Tool radius shape offset amount G10 L13 Tool radius wear offset amount
The tool offset input format is as follows.
G10 Ll1 Pp1 Rr1 ; G10 Ll1 Pp1 Rr1
: Command for setting offset amount : Offset No. : Offset amount
(Note) When Ll1 has been omitted, the tool length shape offset amount is set. Omitting Pp1 results in a program error.
[L system]
G code Function G10 L10 Tool length offset amount G10 L11 Tool wear offset amount
The tool offset input format is as follows.
G10 L10(L11) Pp1 Xx1 Zz1 Rr1 Qq1 ; G10 L10(L11) Pp1 Xx1 Zz1 Rr1 Qq1
: Command for setting offset amount : Offset No. : X axis offset amount : Z axis offset amount : Nose R compensation amount : Hypothetical tool nose point
12. Programming Support Functions 12.1 Machining Method Support Functions
- 166 -
12.1.10 Machining Modal 12.1.10.1 Tapping Mode: G63
C6 C64 T system L system M system L system T system
When tapping mode commands are issued, the NC system is set to the following internal control modes required for tapping. 1. Cutting override is fixed at 100%. 2. Deceleration commands at joints between blocks are invalid. 3. Feed hold is invalid. 4. Single block is invalid. 5. "In tapping mode" signal is output.
G code Function
G63 Tapping mode ON
The tapping mode command will be canceled with the following commands: Exact stop check mode (G61) Automatic corner override (G62) Cutting mode (G64) High-accuracy control mode command (G61.1) [T system, M system]
The machine is in the cutting mode status when its power is turned on.
12.1.10.2 Cutting Mode; G64 C6 C64
T system L system M system L system T system
When a cutting mode command is issued, the NC system is set to the cutting mode that enables smooth cutting surface to be achieved. In this mode, the next block is executed continuously without the machine having to decelerate and stop between the cutting feed blocks: this is the opposite of what happens in the exact stop check mode (G61).
G code Function
G64 Cutting mode ON
The cutting mode command will be canceled with the following commands: Exact stop check mode (G61) Automatic corner override (G62) Tapping mode (G63) High-accuracy control mode command (G61.1) [T system, M system]
The machine is in the cutting mode status when its power is turned on.
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 167 -
12.2 Machining Accuracy Support Functions 12.2.1 Automatic Corner Override; G62
C6 C64 T system L system M system L system T system
To prevent machining surface distortion due to the increase in the cutting load during cutting of corners, this function automatically applies an override on the cutting feed rate so that the cutting amount is not increased for a set time at the corner. Automatic corner override is valid only during tool radius compensation. The automatic corner override mode is set to ON by the G62 command and it is canceled by any of the G commands below.
G40 ..... Tool radius compensation cancel G61 ..... Exact stop check mode G63 ..... Tapping mode G64 ..... Cutting mode G61.1.... High-accuracy control mode [T system, M system]
(1) (2) (3)
S
workpiece
Machining allowance
Machining allowance Programmed path (finished shape)
Workpiece surface shape
Tool center path
Tool
: Max. angle at inside corner Ci : Deceleration range (IN)
Ci Deceleration range
Operation (a) When automatic corner override is not to be applied : When the tool moves in the order of (1) (2) (3) in the figure above, the machining
allowance at (3) is larger than that at (2) by an amount equivalent to the area of shaded section S and so the tool load increases.
(b) When automatic corner override is to be applied : When the inside corner angle in the figure above is less than the angle set in the parameter,
the override set into the parameter is automatically applied in the deceleration range Ci.
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 168 -
12.2.2 Deceleration Check The deceleration check function leads the machine to decelerate and stop at the join between one block and another before executing the next block to alleviate the machine shock and to prevent the corner roundness that occurs when the feed rate of the control axis changes suddenly.
Without deceleration check With deceleration check
N010 G01 X100 ; N011 G01 Y-50 ;
Coner rounding occurs because the N011 block is started before the N010 command is completely finished.
N010 G09 G01 X100 ; N011 G01 Y-50 ;
A sharp edge is formed because the N011 block is started after the N010 remaining distance has reached the command deceleration check width or the in-position check width.
The conditions for executing deceleration check are described below. (1) Deceleration check in the rapid traverse mode In the rapid traverse mode, the deceleration check is always performed when block movement
is completed before executing the next block. (2) Deceleration check in the cutting feed mode
In the cutting feed mode, the deceleration check is performed at the end of block when any of the conditions below is applicable before executing the next block. (a) When G61 (exact stop check mode) is selected. (b) When the G09 (exact stop check) is issued in the same block. (c) when the error detect switch (external signal) is ON.
(3) Deceleration check system
Deceleration check is a system that executes the next block only after the command deceleration check is executed as shown below, and it has been confirmed that the position error amount, including the servo system, is less than the in-position check width (designated with parameter or with ",I" in same block).
Previous block
Servo
Command
In-position check widthBlock interpolation completion point
Next block
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 169 -
12.2.2.1 Exact Stop Check Mode; G61 C6 C64
T system L system M system L system T system
A deceleration check is performed when the G61 (exact stop check mode) command has been selected. G61 is a modal command. The modal command is released by the following commands.
G62.......Automatic corner override G63.......Tapping mode G64.......Cutting mode G61.1....High-accuracy control mode [T system, M system]
Refer to "12.2.2 Deceleration Check" for details on the deceleration check.
12.2.2.2 Exact Stop Check; G09
C6 C64 T system L system M system L system T system
A deceleration check is performed when the G09 (exact stop check) command has been designated in the same block. The G09 command is issued in the same block as the cutting command. It is an unmodal command. Refer to "12.2.2 Deceleration Check" for details on the deceleration check.
12.2.2.3 Error Detect C6 C64
T system L system M system L system T system
To prevent rounding of a corner during cutting feed, the operation can be changed by turning an external signal switch ON so that the axis decelerates and stops once at the end of the block and then the next block is executed. The deceleration stop at the end of the cutting feed block can also be commanded with a G code. Refer to "12.2.2 Deceleration Check" for details on the deceleration check.
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 170 -
12.2.2.4 Programmable In-position Check C6 C64
T system L system M system L system T system
This command is used to designate the in-position width, which is valid when a linear interpolation command is assigned, from the machining program. The in-position width designated with a linear interpolation command is valid only in cases when the deceleration check is performed, such as:
When the error detect switch is ON. When the G09 (exact stop check) command has been designated in the same block. When the G61 (exact stop check mode) command has been selected.
G01 X_ Z_ F_ ,I_; X_,Z_ F_ ,I_
: Linear interpolation coordinates of axes : Feed rate : In-position width
This command is used to designate the in-position width, which is valid when a positioning command is assigned, from the machining program. G00 X_ Z_ ,I_; X_,Z_ ,I_
: Positioning coordinates of axes : In-position width
In-position check operation After it has been verified that the position error between the block in which the positioning
command (G00: rapid traverse) is designated and the block in which the deceleration check is performed by the linear interpolation command (G01) is less than the in-position width of this command, the execution of the next block is commenced.
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 171 -
12.2.3 High-Accuracy Control; G61.1 C6 C64
T system L system M system L system T system
This function controls the operation so the lag will be eliminated in control systems and servo systems. With this function, improved machining accuracy can be realized, especially during high-speed machining, and machining time can be reduced.
The high-accuracy control is commanded with ;
G61.1 High-accuracy control ON
R
F
Machining path with a feed forward gain of 70% in high-accuracy control mode Commanded path
Machining path with a feed forward gain of 0% in high-accuracy control mode
Machining path when high-accuracy control mode is OFF
Neat machining of sharp corners without waste is realized with optimum linear acceleration/deceleration and corner judgement.
Effects in G02/G03 circular interpolation
Conventionally X
Y
F
T
Optimum corner deceleration
Conventionally
Optimum corner deceleration
R
R : Command radius (mm)
R: Radius error (mm)
F : Cutting feed rate (m/min)
(1) Acceleration / deceleration before interpolation [T system, M system] By accelerating /decelerating before interpolation, the machining shape error can be eliminated with smoothing, and a highly accurate path can be achieved. With the arc commands, the radius reduction error can be significantly minimized. Furthermore, since constant inclination acceleration/deceleration is performed, the time taken for positioning at microscopically small distances in the G00 command is reduced.
(Note 1) Whether acceleration/deceleration before interpolation in the rapid traverse command (G00) is to be performed always or not can be selected using a parameter setting independently from the high-accuracy control assignment.
(2) Optimum corner deceleration [T system, M system] By determining the command vector in the machining program and thereby performing corner deceleration, it is possible to machine workpiece with a high-edge accuracy. The figure below shows the pattern of the deceleration speed at the corners. (Optimum corner deceleration is a function of high-accuracy control mode.)
12. Programming Support Functions 12.2 Machining Accuracy Support Functions
- 172 -
The speed change can be smoothed by the S-shape filter, the machine vibration can be suppressed, and the surface accuracy improved. At the corner, the vector commanded in the machining program is automatically determined, and the speed is decelerated at the corner. A highly accurate edge can be machined by decelerating at the corner.
P
V0
F
Speed
F : Cutting feed rate V0 : Maximum allowable
deceleration speed Deccelerates as far as V0 Inclination of acceleration
/deceleration before interpolation (acceleration)
Time
N001
N002
N001 N002
(3) Feed forward control
A stable servo control with an extremely small servo error can be realized using the feed forward control characteristic to this CNC system.
Kp
Feed forward control
Kp : Position loop gain Kv : Speed loop gain M : Motor S : Differential
Detector
Kv
S
M
12. Programming Support Functions 12.3 Programming Support Functions
- 173 -
12.3 Programming Support Functions 12.3.2 Address Check
C6 C64 T system L system M system L system T system
When a machining program is to be run, it can be checked in 1-word units. A parameter is used to select whether or not to conduct an address check. Program address check operation In addition to the conventional program check, a simple check in 1-word units is conducted. If
letters of the alphabet follow successively, a program error results. (Word: Consists of one letter followed by a number composed of several digits.) With the conventional method, when a letter was not followed by a number, that the number
was assumed to be zero, however, now an error will result when this new check is performed. An error will not result in the following cases: (1) Machine language (2) Comment statements Example of a program address check Example 1: When the letter is not followed by a number G28X; Program should be reviewed and changed to G28X0; , etc. Example 2: When there is an illegal character string TEST; Program should be reviewed and changed to "(TEST);", etc.
13. Machine Accuracy Compensation 13.1 Static Accuracy Compensation
- 174 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13.1.1 Backlash Compensation C6 C64
T system L system M system L system T system
This function compensates for the error (backlash) produced when the direction of the machine system is reversed. The backlash compensation can be set in the cutting feed mode or rapid traverse mode. The amount of backlash compensation can be set separately for each axis. It is set using a number of pulses in increments of one-half of the least input unit. The output follows the output unit system. The "output unit system" is the unit system of the machine system (ball screw unit system). The amount of compensation for each axis ranges from 0 to 9999 (pulses).
13. Machine Accuracy Compensation 13.1 Static Accuracy Compensation
- 175 -
13.1.2 Memory-type Pitch Error Compensation C6 C64
T system L system M system L system T system
The machine accuracy can be improved by compensating for the errors in the screw pitch intervals among the mechanical errors (production errors, wear, etc.) of the feed screws. The compensation positions and amounts are stored in the memory by setting them beforehand for each axis, and this means that there is no need to attach dogs to the machine. The compensation points are divided into the desired equal intervals.
1. Division intervals of compensation points : 1 to 9999999 (m) 2. Number of compensation points : 1024 3. Compensation amount : 128 to 127 (output unit) 4. No. of compensated axes : 10 axes (including number of axes for relative position error compensation)
(1) The compensation position is set for the compensation axis whose reference point serves as
the zero (0) point. Thus, memory-type pitch error compensation is not performed if return to reference point is not made for the compensation base axis or compensation execution axis after the controller power is turned ON and the servo is turned ON.
(2) When the compensation base axis is a rotary axis, select the dividing intervals so that one rotation can be divided.
Compensation amount Compensation
base axis
Division interval
+
R#1
(3) As shown in the figure above, highly individualized compensation control is exercised using the minimum output units with linear approximation for the compensation intervals between the compensation points.
(Note 1) Compensation points 1,024 is a total including the points for memory-type relative position error compensation.
(Note 2) A scale of 0 to 99-fold is applied on the compensation amount.
13. Machine Accuracy Compensation 13.1 Static Accuracy Compensation
- 176 -
13.1.3 Memory-type Relative Position Error Compensation C6 C64
T system L system M system L system T system
Machine accuracy can be improved by compensating a relative error between machine axes, such as a production error or time aging. The compensation base axis and compensation execution axis are set by using parameters. The compensation points are divided at any desired equal intervals.
1. Compensation point dividing intervals : 1 to 9999999 (m) 2. Number of compensation points : 1024 3. Compensation amount : 128 to 127 (output unit) 4. No. of compensated axes : 10 axes (including number of axes for memory type pitch error compensation.)
(1) The compensation position is set for the compensation axis whose reference point serves as the zero (0) point. Thus, memory-type relative position error compensation is not performed if return to reference point is not made for the compensation base axis or compensation execution axis after the controller power is turned ON and the servo is turned ON.
(2) When the compensation base axis is a rotary axis, select the dividing intervals so that one rotation can be divided.
(3) Since all coordinate systems of compensation execution axes are shifted or displaced by the compensation amount when the relative position error compensation is made, the stroke check point and machine coordinate system are also shifted or displaced.
(Note 1) Compensation points 1,024 is a total including the points for memory-type pitch error compensation.
(Note 2) A scale of 0 to 99-fold is applied on the compensation amount.
13.1.4 External Machine Coordinate System Compensation C6 C64
T system L system M system L system T system
The coordinate system can be shifted by inputting a compensation amount from the PLC. This compensation amount will not appear on the counter (all counters including machine position). If the machine's displacement value caused by heat is input for example, this can be used for thermal displacement compensation.
Machine coordinate zero point when the external machine coordinate system offset amount is 0.
Mc:Compensation vector according to external machine coordinate system compensation
Machine coordinate zero point
13. Machine Accuracy Compensation 13.1 Static Accuracy Compensation
- 177 -
13.1.6 Ball Screw Thermal Expansion Compensation C6 C64
T system L system M system L system T system
(1) Outline The error in the axis feed caused by the thermal expansion of the ball screw is compensated with the value set in PLC I/F.
Compensation amount
Ball screw Machine coordinates
Offset compensation amount
Maximum compensation amount
X
Compensation amount at coordinate X
Thermal expansion compensation valid range Offset compensation
position
Compensation line
Zero point
Maximum compensation position
The offset compensation amount and maximum compensation amount are set from the PLC. The compensation amount based on the offset compensation amount is set as the maximum compensation amount. The offset compensation amount and maximum compensation amount are set beforehand in the parameters.
(2) Compensation operation
The offset compensation position and maximum compensation position are connected with a straight line following the designated compensation amount, and the compensation amount to the current coordinates is obtained and compensated. The compensation amount changes immediately when the offset compensation amount or maximum compensation amount changes. The thermal expansion compensation is valid only between the offset compensation amount and maximum compensation position, and is "0" outside of this range. The compensation amount is not included in the coordinate value display.
13. Machine Accuracy Compensation 13.2 Dynamic Accuracy Compensation
- 178 -
13.2 Dynamic Accuracy Compensation
13.2.1 Smooth High-gain Control (SHG Control) C6 C64
T system L system M system L system T system
This is a high-response and stable position control method using the servo system (MDS- - V /SVJ2). This SHG control realizes an approximately three-fold position loop gain equally compared to the conventional control method. The features of the SHG control are as follows. (1) The acceleration/deceleration becomes smoother, and the mechanical vibration can be
suppressed (approx. 1/2) during acceleration/deceleration. (In other words, the acceleration/ deceleration time constant can be shortened.)
6.0
3.0SHG control
Time
Speed
Machine vibration
Step response
SHG control (position loop gain = 50rad/S)
Conventional control (position loop gain = 33rad/S)
Current
Time
Conventional control
Machine vibration amount (m)
(2) The shape error is approx. 1/9 of the conventional control.
SHG control
1.0
Roundness error (m)
Y
X
SHG control + FF
Feed rate 3000mm/min. Radius 50mm 1. Conventional control 2. SHG control 3. SHG control + FF (Feed forward)
2
1
3 Conventional control
22.5
2.5
(3) The positioning time is approx. 1/3 of the conventional control.
200
60
Positioning time (ms)
1. Conventional control 2. SHG control 3. SHG control + FF (Feed forward)
3
Droop
Time
70SHG control
SHG control + FF
Conventional control2 1
Droop during rapid traverse deceleration
13. Machine Accuracy Compensation 13.2 Dynamic Accuracy Compensation
- 179 -
13.2.2 Dual Feedback C6 C64
T system L system M system L system T system
Depending on the frequency, the weight (gain) of the position feedback amount provided by the motor end detector and position feedback amount provided by the machine end detector stands in the correlation shown in the figure below. Semi-closed control is provided on a transient basis whereas positioning can be controlled by the closed status. This function is used to select the primary delay filter time constant during dual feedback control as a parameter setting.
Motor end
Weight (gain) of position feedback amounts
Machine end
0
db
rad/s
1 T
0
db
rad/s
1 T
Time constant T here is adjusted using a parameter.
13.2.3 Lost Motion Compensation C6 C64
T system L system M system L system T system
This function compensates the error in the protrusion shape caused by lost motion at the arc quadrant changeover section during circular cutting.
14. Automation Support Functions 14.1 External Data Input
- 180 -
14. Automation Support Functions
14.1 External Data Input
14.1.1 External Search C6 C64
T system L system M system L system T system
This function enables the program numbers, sequence numbers and block numbers of machining programs, which are to be used in automatic operation, to be searched from the memory using the user PLC. When a number is to be searched, the storage location of the program to be searched can be specified as the device number. The currently searched contents (device number, program number, sequence number, block number) can be read from the PLC.
14. Automation Support Functions 14.1 External Data Input
- 181 -
14.1.2 External Workpiece Coordinate Offset C6 C64
T system L system M system L system T system
External workpiece coordinate offset that serves as the reference for all the workpiece coordinate systems is available outside the workpiece coordinates. By setting the external workpiece coordinate offset, the external workpiece coordinate system can be shifted from the machine coordinate system, and all the workpiece coordinate systems can be simultaneously shifted by an amount equivalent to the offset. When the external workpiece coordinate offset is zero, the external workpiece coordinate systems coincide with the machine coordinate system. It is not possible to assign movement commands by selecting the external workpiece coordinates.
Machine coordinate system
External workpiece coordinate
External workpiece coordinate offset
Machine coordinate system (= External workpiece coordinate
Machine coordinate zero point
Workpiece coordinate 4 (G57)
Workpiece coordinate 5 (G58)
Workpiece coordinate 6 (G59)
Workpiece coordinate 1 (G54)
Workpiece coordinate 2 (G55)
Workpiece coordinate 3 (G56)
Workpiece coordinate 4 (G57)
Workpiece coordinate 5 (G58)
Workpiece coordinate 6 (G59)
Workpiece coordinate 1 (G54)
Workpiece coordinate 2 (G55)
Workpiece coordinate 3 (G56)
Machine coordinate zero point
14. Automation Support Functions 14.2 Measurement
- 182 -
14.2 Measurement; G31, G37
14.2.1 Skip
14.2.1.1 Skip C6 C64
T system L system M system L system T system
When the external skip signal is input during linear interpolation with the G31 command, the machine feed is stopped immediately, the remaining distance is discarded and the commands in the next block are executed. G31 Xx1 Yy1 Zz1 Ff1 ;
G31 : Measurement command Xx1, Yy1, Zz1 : Command values Ff1 : Feed rate
Feed rate
Command value
Actual movement distance
Programmed end point
Skip signal input
Remaining distance
Position
When the G31 command is issued, acceleration/deceleration is accomplished in steps (time constant = 0). There are two types of skip feed rate. (1) Feed rate based on program command when F command is present in program (2) Feed rate based on parameter setting when F command is not present in program
(Note 1) The approximate coasting distance up to feed stop based on the detection delay in the skip signal input is calculated as below.
= (Tp + t)
F 60
. .
: Coasting distance (mm) F : G31 rate (mm/min) Tp : Position loop time constant (s) = (position loop gain)1 T : Response delay time of 0.0035 (s)
(Note 2) Skipping during machine lock is not valid.
14. Automation Support Functions 14.2 Measurement
- 183 -
14.2.1.2 Multiple-step Skip C6 C64
T system L system M system L system T system
(1) G31.n method
This function realizes skipping by designating a combination of skip signals for each skip command (G31.1, G31.2, G31.3). The combination of the skip signals 1, 2 and 3 are designated with parameters for each G code (G31.1, 31.2, 31.3), and the skip operation is executed when all signals in the combination are input. G31.n Xx1 Yy1 Zz1 Ff1 ;
G31.n : Skip command (n=1, 2, 3) Xx1, Yy1, Zz1 : Command format axis coordinate word and target coordinates Ff1 : Feed rate (mm/min)
(2) G31Pn method
As with the G31.n method, the valid skip signal is designated and skip is executed. However, the method of designating the valid skip signal differs. The skip signals that can be used are 1 to 4. Which is to be used is designated with P in the program. Refer to Table 1 for the relation of the P values and valid signals. Skip can be executed on dwell, allowing the remaining dwell time to be canceled and the next block executed under the skip conditions (to distinguish external skip signals 1 to 4) set with the parameters during the dwell command (G04). G31 Xx1 Yy1 Zz1 Pp1 Ff1 ;
G31 : Skip command Xx1, Yy1, Zz1 : Command format axis coordinate word and target coordinates Pp1 : Skip signal command Ff1 : Feed rate (mm/min)
(a) Specify the skip rate in command feedrate F. However, F modal is not updated. (b) Specify skip signal command in skip signal command P. Specify the P value in the range
of 1 to 15. If it exceeds the specified range, a program error occurs. (c) When the skip signals are commanded in combination, the skip operation takes place with
OR result of those signals.
14. Automation Support Functions 14.2 Measurement
- 184 -
Table 1 Valid skip signals Valid skip signal
Skip signal command P 4 3 2 1 1
2
3
4
5
6
7
8
: : : : :
13
14
15
14. Automation Support Functions 14.2 Measurement
- 185 -
14.2.5 Automatic Tool Length Measurement C6 C64
T system L system M system L system T system
(1) Automatic Tool Length Measurement (T system, M system)
This function moves the tool in the direction of the tool measurement position by the commanded value between the measurement start position to the measurement position, it stops the tool as soon as it contacts the sensor and calculates the difference between the coordinates when the tool has stopped and commanded coordinates. It registers this difference as the tool length offset amount for that tool. If compensation has already been applied to the tool, it is moved in the direction of the measurement position with the compensation still applied, and when the measurement and calculation results are such that a further compensation amount is to be provided, the current compensation amount is further corrected. If the compensation amount at this time is one type, the compensation amount is automatically corrected; if there is a distinction between the tool length compensation amount and wear compensation amount, the wear amount is automatically corrected. G37 Z_R_D_F_ ;
Z : Measurement axis address and measurement position coordinate. ... X, Y, Z, (where is an optional axis)
R : The distance between the point at which tool movement is to start at the measurement speed and the measurement position.
D : The range in which the tool is to stop. F : The measurement rate. When R_, D_ and F_ have been omitted, the values set in the parameters are used.
Tool
Tool change point
Tool length measurement position (Za1)
Sensor
Amount of movement based on tool length measurement
Reference position (In case of machine coordinate system zero point.)
At this time, the tool length offset amount has a minus ("") value. Example of program G28 Z0 ; T01 ; M06 T02 ; G43 G00 Z0 H01 ; G37 Z300. R10.D2.F10 ; In this case, the distance (H01 = Za1 z0) from the tool T01 tip to the top of the measurement sensor is calculated as the tool length offset amount which is then registered in the tool offset table.
(Note 1) The measurement position arrival signal (sensor signal) is also used as the skip signal.
14. Automation Support Functions 14.2 Measurement
- 186 -
B2
B1 r1
d 1
d1 Measurement position (z 1)
Start point
A
Area A : Moves with rapid traverse feed rate. Areas B1, B2 : Moves with the measurement speed (f1 or parameter setting) If a sensor signal is input in area B1, an error will occur. If a sensor signal is not input in the area B2, an error will occur.
(2) Automatic tool length measurement (L series) This function moves the tool in the direction of the tool measurement position by the commanded value between the measurement start position to the measurement position, it stops the tool as soon as it contacts the sensor and calculates the difference between the coordinates when the tool has stopped and commanded coordinates. It registers this difference as the tool length offset amount for that tool. If compensation has already been applied to the tool, it is moved in the direction of the measurement position with the compensation still applied, and when the measurement and calculation results are such that a further compensation amount is to be provided, the current wear compensation amount is further corrected.
G37 _R_D_F_ ;
: Measurement axis address and measurement position coordinate. ... X, Z R : The distance between the point at which tool movement is to start at the
measurement speed and the measurement position. (Always a radial value: incremental value)
D : The range in which the tool is to stop. (Always a radial value: incremental value) F : The measurement rate. When R_, D_ and F_ have been omitted, the values set in the parameters are used.
14. Automation Support Functions 14.2 Measurement
- 187 -
F feed
Rapid traverse feed
Measuring instrument d1
d1
B
r1
Measurement position
A
Start position
r1, d1, and f1 can also be set in parameters.
When the tool moves from the start position to the measurement position specified in G37 x1 (z1), it passes through the A area at rapid traverse. Then, it moves at the measurement rate set in F command or parameter from the position specified in r1. If the measurement position arrival signal turns ON during the tool is moving in the B area, an error occurs. If the measurement position arrival signal does not turn ON although the tool passes through the measurement position x1 (z1) and moves d1, an error occurs.
(Note 1) The measurement position arrival signal (sensor signal) is also used as the skip signal. (Note 2) This is valid for the G code lists 2 and 3.
14. Automation Support Functions 14.2 Measurement
- 188 -
14.2.6 Manual Tool Length Measurement 1 C6 C64
T system L system M system L system T system
Simple measurement of the tool length is done without a sensor. (1) Manual tool length measurement I
[T system, M system] When the tool is at the reference point, this function enables the distance from the tool tip to the measurement position (top of workpiece) to be measured and registered as the tool length offset amount.
M
Table
Manual movement amount (tool length offset amount)
Workpiece
(2) Manual tool length
measurement I [L system] A measurement position (machine coordinates) to match the tool nose on the machine is preset and the tool nose is set to the measurement position by manual feed, then the operation key is pressed, thereby automatically calculating the tool offset amount and setting it as the tool length offset amount.
X axis tool length
Z axis tool length
X axis
Z axis
Measurement position
Parameter setting
Parameter setting
M
Measurement method (a) Preset the machine coordinates of the measurement position in a given parameter as the
measurement basic value. (b) Select a tool whose tool length offset amount is to be measured. (c) Set the tool nose to the measurement position by manual feed. (d) Press the input key. The tool length offset amount is calculated and displayed on the
setting area. Tool length offset amount = machine coordinates measurement basic value (e) Again press the input key to store the value in the memory as the tool length offset amount
of the tool.
14. Automation Support Functions 14.3 Monitoring
- 189 -
14.3 Monitoring
14.3.1 Tool Life Management
14.3.1.2 Tool Life Management II C6 C64
T system L system M system L system T system
(1) T system, M system A spare tool change function is added to tool life management I. This function selects a usable tool out of the spare tools of the group determined by the value specified by the user PLC, then outputs data of such usable spare tool. The spare tool can be selected in two ways: the tools are selected in order they were registered in the group or the tool whose remaining life is the longest of all in the group is selected.
(2) L system The life of each tool (time and frequency) is controlled, and when the life is reached, a spare tool that is the same type is selected from the group where the tool belongs and used. No. of groups: Max. 40 sets (each part system)/ For 1 part system: 80 sets No. of tools in group: Max. 16 tools
14.3.2 Number of Tool Life Management Sets The number of tools that can be managed for their lives are shown below. (These are fixed by the No. of part systems according to the model.) 20/40/80 sets
C6 C64 T system L system M system L system T system
80 80 100/200 sets
C6 C64 T system L system M system L system T system 100 100 100
14.3.3 Display of Number of Parts C6 C64
T system L system M system L system T system
The number of machined parts is counted up each time a part is machined, and displayed .
Maximum number of workpieces to be machined Number of workpieces machined
Number of workpieces machined
14. Automation Support Functions 14.3 Monitoring
- 190 -
14.3.4 Load Meter C6 C64
T system L system M system L system T system
Using the user PLC, this function displays the spindle load, Z-axis load, etc. in the form of bar graphs.
14.3.5 Position Switch C6 C64
T system L system M system L system T system 16 16 16 16 16
The position switch (PSW) function provides hypothetical dog switches in place of the dog switches provided on the machine axes by setting the axis names and coordinates indicating the hypothetical dog positions as parameters beforehand so that signals are output to the PLC interface when the machine has reached these hypothetical dog positions. The hypothetical dog switches are known as position switches (PSW). The coordinates indicating the hypothetical dog positions (dog1, dog2) on the coordinate axes whose names were set by parameters ahead of time in place of the dog switches provided on the machine axes are set using position switches. When the machine has reached the hypothetical dog positions, a signal is output to the device supported by the PLC interface. There can be a maximum of 16 switches for each part system.
Example of dog1, dog2 settings and execution dog1, dog2
settings dog1, dog2 positions Description
dog1 < dog2 dog1 dog2
Signal is output between dog1 and dog2
dog1 > dog2 dog2 dog1
Signal is output between dog2 and dog1
dog1 = dog2 dog1 = dog2
Signal is output at the dog1 (dog2) position
PSW width
Basic machine coordinate system zero point
Hypothetical dog
dog1
dog2
14. Automation Support Functions 14.5 Others
- 191 -
14.5 Others
14.5.1 Programmable Current Limitation C6 C64
T system L system M system L system T system
This function allows the current limit value of the servo axis to be changed to a desired value in the program, and is used for the workpiece stopper, etc. The commanded current limit value is designated with a ratio of the limit current to the rated current. The current limit value can also be set from the D.D.B. function and setting and display unit. The validity of the current limit can be selected with the external signal input. However, the current limit value of the PLC axis cannot be rewritten. G10 L14 X dn ;
L14 : Current limit value setting (+ side/ side) X : Axis address dn : Current limit value 1% to 300%
(1) If the current limit is reached when the current limit is valid, the current limit reached signal is
output. (2) The following two modes can be used with external signals as the operation after the current
limit is reached. Normal mode
The movement command is executed in the current state. During automatic operation, the movement command is executed to the end, and then the next block is moved to with the droops still accumulated.
Interlock mode The movement command is blocked (internal interlock). During automatic operation, the operation stops at the corresponding block, and the next block is not moved to. During manual operation, the following same direction commands are ignored.
(3) During the current limit, the droop generated by the current limit can be canceled with external signals. (Note that the axis must not be moving.)
(4) The setting range of the current limit value is 1% to 300%. Commands that exceed this range will cause a program error. "P35 CMD VALUE OVER" will be displayed.
(5) If a decimal point is designated with the G10 command, only the integer will be valid. (Example) G10 L14 X10.123 ; The current limit value will be set to 10%.
(6) For the axis name "C", the current limit value cannot be set from the program (G10 command). To set from the program, set the axis address with an incremental axis name, or set the axis name to one other than "C".
14.5.4 Automatic Restart
C6 C64 T system L system M system L system T system
The controller can be reset and the program started again from the head when the automatic restart signal is turned ON during program running.
15. Safety and Maintenance 15.1 Safety Switches
- 192 -
15. Safety and Maintenance 15.1 Safety Switches
15.1.1 Emergency Stop C6 C64
T system L system M system L system T system
All operations are stopped by the emergency stop signal input and, at the same time, the drive section is stopped using the dynamic brake and the movement of the machine is stopped. At this time, the READY lamp on the setting and display unit goes OFF and the servo ready signal is turned OFF.
15.1.2 Data Protection Key C6 C64
T system L system M system L system T system
With the input from the user PLC, it is possible to prohibit the setting and deletion of parameters and the editing of programs from the setting and display unit. Data protection is divided into the following groups. Group 1: For protecting the tool data and protecting the coordinate system presettings as based on origin setting (zero) Group 2: For protecting the user parameters and common variables Group 3: For protecting the machining programs
15. Safety and Maintenance 15.2 Display for Ensuring Safety
- 193 -
15.2 Display for Ensuring Safety
15.2.1 NC Warning C6 C64
T system L system M system L system T system
The warnings which are output by the NC system are listed below. When one of these warnings has occurred, a warning number is output to the PLC and a description of the warning appears on the screen. Operation can be continued without taking further action.
Type of warning Description Servo warning The servo warning is displayed. Spindle warning The spindle warning is displayed.
System warning The system warning is displayed. (State such as temperature rise, battery voltage low, etc.)
Absolute position warning A warning in the absolute position detection system is displayed. Auxiliary axis warning The auxiliary axis warning is displayed.
15.2.2 NC Alarm C6 C64
T system L system M system L system T system
The alarms which are output by the NC system are listed below. When one of these alarms has occurred, an alarm number is output to the PLC, and a description of the alarm appears on the screen. Operation cannot be continued without taking remedial action.
Type of warning Description
Operation alarm This alarm occurring due to incorrect operation by the operator during NC operation and that by machine trouble are displayed.
Servo alarm This alarm describes errors in the servo system such as the servo drive unit motor and encoder.
Spindle alarm This alarm describes errors in the spindle system such as the spindle drive unit motor and encoder.
MCP alarm An error has occurred in the drive unit and other interfaces. System alarm This alarm is displayed with the register at the time when the
error occurred on the screen if the system stops due to a system error.
Absolute position detection system alarm
An alarm in the absolute position detection system is displayed.
Auxiliary axis alarm The auxiliary axis alarm is displayed. User PLC alarm The user PLC alarm is displayed. Program error This alarm occur during automatic operation and the cause of
this alarm is mainly program errors which occur for instance when mistakes have been made in the preparation of the machining programs or when programs which conform to the specification have not been prepared.
15. Safety and Maintenance 15.2 Display for Ensuring Safety
- 194 -
15.2.3 Operation Stop Cause C6 C64
T system L system M system L system T system
The stop cause of automatic operation is displayed on the setting and display unit.
15.2.4 Emergency Stop Cause C6 C64
T system L system M system L system T system
When "EMG" (emergency stop) message is displayed in the operation status display area of the setting and display unit, the emergency stop cause can be confirmed.
15.2.5 Temperature Detection C6 C64
T system L system M system L system T system
When overheating is detected in the control unit or the communication terminal, an overheat signal is output at the same time as the alarm is displayed. If the system is in auto run at the time, run is continued, but it cannot be started after reset or M02/M30 run ends. (It can be started after block stop or feed hold.) When the temperature falls below the specified temperature, the alarm is released and the overheat signal is turned OFF. The overheat alarm occurs at 80C or more for the control unit or 70C or more for the communication terminal.
Overheat detection
Control unit
Communication terminal
Parameter Temperature alarm
User PLC
Message display
Cooling fan
Lamp alarm Emergency stop Others
Bit device
(70C)
(80C)
(Z53 TEMP. OVER) (Default valid)
Overheat detection
Parameter
(Default valid)
rotation
(Note 1) If the parameter is used to set the temperature rise detection function to invalid,
overheating may occur, thereby disabling control and possibly resulting in the axes running out of control, which in turn may result in machine damage and/or bodily injury or destruction of the unit. It is for this reason that the detection function is normally left "valid" for operation.
15. Safety and Maintenance 15.3 Protection
- 195 -
15.3 Protection
15.3.1 Stroke End (Over Travel) C6 C64
T system L system M system L system T system
When limit switches and dogs have been attached to the machine and a limit switch has kicked a dog, the movement of the machine is stopped by the signal input from the limit switch. At the same time, the alarm output is sent to the machine. The stroke end state is maintained and the alarm state is released by feeding the machine in the reverse direction in the manual mode to disengage the dog.
15.3.2 Stored Stroke Limit The stored stroke limits I, II, IIB, IB and IC are handled as follows.
Type Prohibited range Explanation
I Outside
Set by the machine maker. When used with II, the narrow range designated by the two types becomes the movement valid range. Can be rewritten with DDB.
II Outside
IIB Inside
Set by the user. The change or function of parameter can be turned OFF/ON with the program command. Select II or IIB with the parameters. Can be rewritten with DDB.
IB Inside Set by the machine maker.
IC Outside Set by the machine maker. Can be rewritten with DDB.
15. Safety and Maintenance 15.3 Protection
- 196 -
15.3.2.1 Stored Stroke Limit I/II C6 C64
T system L system M system L system T system
(1) Stored Stroke Limit I
This is the stroke limit function used by the machine maker, and the area outside the set limits is the entrance prohibited area. The maximum and minimum values for each axis can be set by parameters. The function itself is used together with the stored stroke limit II function described in the following section, and the tolerable area of both functions is the movement valid range. The setting range is 99999.999 to +99999.999mm. The stored stroke limit I function is made valid not immediately after the controller power is turned ON but after reference point return. The stored stroke limit I function will be invalidated if the maximum and minimum values are set to the same data.
M
"+" setting
Machine movement valid range
Point 1Prohibited area
Machine coordinate system
Feed rate
L
Pr oh
ib ite
d ar
ea
The values of points 1 and 2 are set using the coordinate values in the machine coordinate system.
Pr oh
ib ite
d ar
ea
Point 2 Prohibited area
"" setting
All axes will decelerate and stop if an alarm occurs even for a single axis during automatic operation. Only the axis for which the alarm occurs will decelerate and stop during manual operation. The stop position must be before the prohibited area. The value of distance "L" between the stop position and prohibited area differs according to the feed rate and other factors.
15. Safety and Maintenance 15.3 Protection
- 197 -
(2) Stored Stroke Limit II This is the stroke limit function which can be set by the user, and the area outside the set limits is the prohibited area. The maximum and minimum values for each axis can be set by parameters. The function itself is used together with the stored stroke limit I function described in the foregoing section, and the tolerable area of both functions is the movement valid range. The setting range is 99999.999 to +99999.999mm. The stored stroke limit II function will be invalidated if the maximum and minimum parameter values are set to the same data.
M
"+"
Area prohibited by stored stroke limit function II
setting
Prohibited area
L
Pr oh
ib ite
d ar
ea
Machine coordinate system
Machine movement valid range
Point 1
Point 3
Pr oh
ib ite
d ar
ea
Point 4
Point 2
Feed rate
"" setting
The values of points 3 and 4 are set with the coordinate values in the machine coordinate system. The area determined by points 1 and 2 is the prohibited area set with stored stroke limit I.
All axes will decelerate and stop if an alarm occurs even for a single axis during automatic operation. Only the axis for which the alarm occurs will decelerate and stop during manual operation. The stop position must be before the prohibited area. The value of distance "L" between the stop position and prohibited area differs according to the feed rate and other factors. The stored stroke limit II function can also be invalidated with the parameter settings.
15. Safety and Maintenance 15.3 Protection
- 198 -
15.3.2.2 Stored Stroke Limit IB C6 C64
T system L system M system L system T system
Three areas where tool entry is prohibited can be set using the stored stroke limit I, stored stroke limit II, IIB and stored stroke limit IB functions.
Stored Stroke Limit IB
Stored Stroke Limit I
Stored Stroke Limit IIB
When an attempt is made to move the tool beyond the set range, an alarm is displayed, and the tool decelerates and stops. If the tool has entered into the prohibited area and an alarm has occurred, it is possible to move the tool only in the opposite direction to the direction in which the tool has just moved. This function is an option. Precautions Bear in mind that the following will occur if the same data is set for the maximum and minimum
value of the tool entry prohibited area: 1. When zero has been set for the maximum and minimum values, tool entry will be
prohibited in the whole area. 2. If a value other than zero has been set for both the maximum and minimum values, it will
be possible for the tool to move in the whole area.
15. Safety and Maintenance 15.3 Protection
- 199 -
15.3.2.3 Stored Stroke Limit IIB C6 C64
T system L system M system L system T system
A parameter is used to switch between this function and stored stroke limit II. With stored stroke limit IIB, the range inside the boundaries which have been set serves as the tool entry prohibited area.
15.3.2.4 Stored Stroke Limit IC C6 C64
T system L system M system L system T system
The boundary is set for each axis with the parameters. The inside of the set boundary is the additional movement range. This cannot be used with soft limit IB.
Point 1
Machine coordinate system
P ro
hi bi
te d
ra ng
e
Machine movement valid range
Point 2
P ro
hi bi
te d
ra ng
e
Point 3
Point 4
Additional movement range
15.3.3 Stroke Check Before Movement C6 C64
T system L system M system L system T system
By assigning commands in the program to designate the boundaries beyond which machine entry is prohibited using the coordinate values in the machine coordinate system, this function ensures that machine entry inside these boundaries is prohibited. Whereas the regular stored stroke limit function stops the machine immediately in front of the set prohibited area, the stroke check before movement function raises a program alarm before the machine initiates the movement in a block containing a command which calls for the machine to move beyond the movement enabled range.
The values of points 3 and 4 are set with the coordinate values in the machine coordinate system. The area determined by points 1 and 2 is the prohibited area set with stored stroke limit I.
Pr oh
ib ite
d ar
ea
Pr oh
ib ite
d ar
ea
15. Safety and Maintenance 15.3 Protection
- 200 -
15.3.4 Chuck/Tail Stock Barrier Check; G22/G23 C6 C64
T system L system M system L system T system
By limiting the tool nose point move range, this function prevents the tool from colliding with the chuck or tail stock because of a programming error. When a move command exceeding the area set in a given parameter is programmed, the tool is stopped at the barrier boundaries. Program format
G22 ; ..... Barrier ON G23 ; ..... Barrier OFF (cancel)
(1) When the machine is about to exceed the area, the machine is stopped and an alarm is
displayed. To cancel the alarm, execute reset. (2) The function is also effective when the machine is locked. (3) This function is valid when all axes for which a barrier has been set have completed reference
point return. (4) The chuck barrier/tail stock barrier can be set independently for part system 1 and part system
2. (5) Chuck barrier/tail stock barrier setting
P 6
P 5
(Form 1)
Z axis
P 4 (P 0)
P 0
P 3
P 2
P 1
X axis
P 6
P 5
(Form 2)
Z axis
P 4
(P 0)
P 0
P 3
P 2
P 1 X axis
The chuck barrier and tail stock barrier are both set with the machine coordinate by inputting one set of three-point data in the parameter. Points P1, P2 and P3 are the chuck barrier, and points P4, P5 and P6 are the tail stock barrier. The X axis is set with the coordinate value (radius value) from the workpiece center, and the Z axis is set with the basic machine coordinate system coordinate. Point P0 is the chuck barrier and tail stock barrier's basic X coordinates, and the workpiece center coordinate in the basic machine coordinate system is set. The barrier area is assumed to be symmetrical for the Z axis, and if the X axis coordinate of barrier point P_ is minus, the sign is inverted to plus and the coordinate is converted for a check. Set the absolute values of the X axis coordinates of the barrier points as shown below: P1 >= P2 >= P3, P4 >= P5 >= P6 (However, this need not apply to the Z axis coordinates.)
15. Safety and Maintenance 15.3 Protection
- 201 -
15.3.5 Interlock C6 C64
T system L system M system L system T system
The machine movement will decelerate and stop as soon as the interlock signal, serving as the external input, is turned ON. When the interlock signal is turned OFF, the machine starts moving again.
(1) In the manual mode, only that axis for which the interlock signal is input will stop. (2) In the automatic mode, all axes will stop when the interlock signal is input to even one axis
which coincides with the moving axis. (3) Block start interlock While the block start interlock signal (*BSL) is OFF (valid), the execution of the next block
during automatic operation will not be started. The block whose execution has already commenced is executed until its end. Automatic operation is not suspended. The commands in the next block are placed on standby, and their execution is started as soon as the signal is turned ON.
(Note 1) This signal is valid for all blocks including internal operation blocks such as fixed cycles. (Note 2) This signal (*BSL) is set ON (invalid) when the power is turned ON. If it is not used, there
is no need to make a program with the PLC.
(4) Cutting start interlock While the cutting start interlock signal (*CSL) is OFF (valid), the execution of all movement
command blocks except positioning during automatic operation will not be started. The block whose execution has already commenced is executed until its end. Automatic operation is not suspended. The commands in the next block are placed on standby, and their execution is started as soon as the signal is turned ON.
(Note 1) The signal is valid for all blocks including internal operation block such as fixed cycles. (Note 2) This signal (*CSL) is set ON (invalid) when the power is turned ON. If it is not used, there
is no need to make a program with the PLC.
15.3.6 External Deceleration C6 C64
T system L system M system L system T system
This function reduces the feed rate to the deceleration speed set by the parameter when the external deceleration input signal, which is the external input from the user PLC, has been set to ON. External deceleration input signals are provided for each axis and for each movement direction ("+" and "-"), and a signal is valid when the signal in the direction coinciding with the direction of the current movement has been input. When an axis is to be returned in the opposite direction, its speed is returned immediately to the regular speed assigned by the command. When non-interpolation positioning is performed during manual operation or automatic operation, only the axis for which the signal that coincides with the direction of the current movement has been input will decelerate. However, with interpolation during automatic operation, the feed rate of the axis will be reduced to the deceleration rate if there is even one axis for which the signal that coincides with the direction of current movement has been input. The external deceleration input signal can be canceled using a parameter for the cutting feed only.
15. Safety and Maintenance 15.3 Protection
- 202 -
15.3.8 Door Interlock
15.3.8.1 Door Interlock I C6 C64
T system L system M system L system T system
Outline of function Under the CE marking scheme of the European safety standards (machine directive), the opening of any protection doors while a machine is actually moving is prohibited. When the door open signal is input from the PLC, this function first decelerates and stops all the control axes, establishes the ready OFF status, and then shuts off the drive power inside the servo drive units so that the motors are no longer driven. When the door open signal has been input during automatic operation, the suspended machining can be resumed by first closing the door concerned and then initiating cycle start again.
Description of operation When a door is open The NC system operates as follows when the door open signal is input:
(1) It stops operations. 1. When automatic operation was underway The machine is set to the feed hold mode, and all the axes decelerate and stop. The spindle also stops. 2. When manual operation was underway
All the axes decelerate and stop immediately. The spindle also stops.
(2) The complete standby status is established. (3) After all the servo axes and the spindle have stopped, the ready OFF status is
established. (4) The door open enable signal is output.
Release the door lock using this signals at the PLC.
When a door is closed After the PLC has confirmed that the door has been closed and locked, the NC system operates as follows when the door open signal is set to OFF. (5) All the axes are set to ready ON. (6) The door open enable signal is set to OFF.
Resuming operation
(7) When automatic operation was underway Press the AUTO START button. Operation now resumes from the block in which machining was suspended when the door open signal was input.
(8) When manual operation was underway Axis movement is commenced when the axis movement signals are input again.
(9) Spindle rotation Restore the spindle rotation by inputting the forward rotation or reverse rotation signal again: this can be done either by operations performed by the operator or by using the user PLC.
15. Safety and Maintenance 15.3 Protection
- 203 -
15.3.8.2 Door Interlock II C6 C64
T system L system M system L system T system
Outline of function Under the CE marking scheme of the European safety standards (machine directive), the opening of any protection doors while a machine is actually moving is prohibited. When the door open signal is input from the PLC, this function first decelerates and stops all the control axes, establishes the ready OFF status, and then shuts off the drive power inside the servo drive units so that the motors are no longer driven. With the door interlock function established by the door open II signal, automatic start can be enabled even when the door open signal has been input. However, the axes will be set to the interlock status.
Description of operation When a door is open
The NC system operates as follows when the door open II signal is input: (1) It stops operations.
All the axes decelerate and stop. The spindle also stops.
(2) The complete standby status is established. (3) After all the servo axes and the spindle have stopped, the ready OFF status is
established. However, the servo ready finish signal (SA) is not set to OFF.
When a door is closed After the PLC has confirmed that the door has been closed and locked, the NC system operates as follows when the door open signal is set to OFF. (4) All the axes are set to ready ON. (5) The door open enable signal is set to OFF.
Resuming operation
(6) When automatic operation was underway The door open signal is set to OFF, and after the ready ON status has been established for all the axes, operation is resumed.
(7) When manual operation was underway Axis movement is commenced when the axis movement signals are input again.
(8) Spindle rotation Restore the spindle rotation by inputting the forward rotation or reverse rotation signal again: this can be done either by operations performed by the operator or by using the user PLC.
(Note) Concerning the handling of an analog spindle
The signals described in this section are valid in a system with bus connections for the NC control unit and drive units. When an analog spindle is connected, the NC system cannot verify that the spindle has come to a complete stop. This means that the door should be opened after the PLC has verified that the spindle has come to a complete stop. Since the spindle may resume its rotation immediately after the door has been closed, set the forward and reverse rotation signals to OFF when opening the door so as to ensure safety.
15. Safety and Maintenance 15.3 Protection
- 204 -
Differences from door interlock I (1) The method used to stop the machine during automatic operation is the same as with the
axis interlock function. (2) The servo ready finish signal (SE) is not set to OFF. (3) Automatic start is valid during door interlock. However, the interlock takes effect for the
axis movements. (4) When this door interlock function (door open signal ON) is initiated during axis movement,
the axes decelerate and stop. (5) When this door interlock function (door open signal) is set to OFF, the axis movement
resumes.
15.3.9 Parameter Lock C6 C64
T system L system M system L system T system
This function is used to prohibit changing the setup parameter.
15.3.10 Program Protect (Edit Lock B, C)
C6 C64 T system L system M system L system T system
The edit lock function B or C inhibits machining program B or C (group with machining program numbers) from being edited or erased when these programs require to be protected.
Machining program A
1 ~ 7999
Machining program B (User-prepared standard subprogram)
8000 ~ 8999
Machining program C (Machine maker customized program)
9000 ~ 9999
Editing is inhibited by edit lock C.
Editing is inhibited by edit lock B.
Machining program A 10000 ~ 99999999
Editing is inhibited by data protect (KEY3).
15. Safety and Maintenance 15.3 Protection
- 205 -
15.3.11 Program Display Lock C6 C64
T system L system M system L system T system
This function allows the display of only a target program (label address 9000) to be invalidated for the program display in the monitor screen, etc. The operation search of a target program can also be invalidated. The validity of the display is selected with the parameters. The setting will be handled as follows according to the value. 0: Display and search are possible. 1: Display of the program details is prohibited. 2: Display and operation search of the program details are prohibited. The program details are not displayed in the prohibited state, but the program number and sequence number will be displayed.
15. Safety and Maintenance 15.4 Maintenance and Troubleshooting
- 206 -
15.4 Maintenance and Troubleshooting
15.4.1 History Diagnosis C6 C64
T system L system M system L system T system
This is a maintenance function which is useful for tracing down the history and NC operation information and analyzing trouble, etc. This information can be output as screen displays or as files.
(1) Screen display showing operation history and event occurrence times The times/dates (year/month/day and hour/minute/second) and messages are displayed as the operation history data. The key histories, alarm histories and input/output signal change histories are displayed as the messages. The part system information is displayed as the alarm histories. For instance, "$1" denotes the first part system, and "$2" the second part system. The history data containing the most recent operation history and event occurrence times (2,068 sets) are displayed on the "Operation history" screen. The most recent history data appears at the top of the screen, and the older data is displayed in sequence below.
(2) Outputting the data in the operation history memory Information on the alarms occurring during NC operation and stop codes, signal information on the changes in the PLC interface input signals and the key histories can be output through the RS- 232C interface.
15.4.2 Setup/Monitor for Servo and Spindle C6 C64
T system L system M system L system T system monitor monitor monitor monitor monitor
The information on the servos (NC axes), spindles, PLC axes and power supplies appears on the setting and display unit. Main information displayed on the monitor: Position loop tracking deviation, motor speeds, load current, detector feedback, absolute position detection information, drive unit alarm histories, operation times, drive unit software versions, etc.
15.4.3 Data Sampling C6 C64
T system L system M system L system T system
Sampling of the servo and spindle data for which an alarm occurrence is a stop condition is performed all the time.
15. Safety and Maintenance 15.4 Maintenance and Troubleshooting
- 207 -
15.4.5 Machine Operation History Monitor C6 C64
T system L system M system L system T system
Up to 256 past key inputs on the operation board and changes in the input signals are recorded. The history contents can be viewed on the history screen, and the data is retained even after the power has been turned OFF.
15.4.6 NC Data Backup This function serves to back up the parameters and other data of the NC control unit. The data can also be restored.
(1) RS-232C C6 C64
T system L system M system L system T system
[Backup target] Machining programs, parameters, workpiece offset data, common variables, tool compensation data, tool life control data Ladders (ladder, message)
(2) IC card C6 C64
T system L system M system L system T system
[Backup target] Machining programs, parameters, common variables, tool compensation data, tool life control data Ladders (ladder, message)
15.4.7 PLC I/F Diagnosis C6 C64
T system L system M system L system T system
When the I/F DIAGN menu key is pressed, the PLC interface diagnosis screen appears. The input and output signals for PLC control can be displayed and set on this screen. This function can be used to check the machine sequence operations for PLC development, check the input/output data between the control unit and PLC when trouble occurs in operation, initiate forced definitions, and so on.
16. Cabinet and Installation 16.1 Cabinet Construction
- 208 -
16. Cabinet and Installation 16.1 Cabinet Construction
The configuration of the unit used by the MELDAS C6/C64 series is shown below. Refer to the Connection / Maintenance Manual for details.
Manual pulse generator
Synchronous feed encoder
Machine control signal
C6/C64 Control unit
Servo drive unit MDS-B/C1-V1/ V2-
Spindle drive unit MDS-B/C1-SP- MDS-B-SPJ2-
Power supply unit MDS-B/C1-CV
Communication terminal
Remote I/O unit DX1
Operation panel, etc.
Sensor
Max. 4 channels Servo motor Spindle motor
Ethernet-connected device
Servo drive unit MDS-B-SVJ2- MR-J2-CT (auxiliary axis)
MITSUBISHI MDS-B-SVJ2
MDS-B-CVE-
D C 2 4 V I N
S E R V O 1
E N C
H A N D L E
S I O
T E R M I N A L
I C C A R D
S K I P
MITSUBISHI
M E L D A S C64S E R
V O 2
Other C6/C64 Control unit
Remote I/O unit DX1
RS-232 C unit
16. Cabinet and Installation 16.1 Cabinet Construction
- 209 -
List of configuration units
(1) Control unit Type Configuration element Details
HR851 card Main card HR891 card Back panel
FCU6-MU043 FCU6-MU042
C6 Control unit C64 Control unit
HR899 card IC card interface (2) Extension unit
Type Configuration element Details FCU6-EX871 DeviceNet (Master) HR871 card Expansion card FCU6-EX872 DeviceNet (Slave) HR872 card Expansion card FCU6-EX873 FL-net HR873 card Expansion card FCU6-EX875 Ethernet HR875/876 card Expansion card, Use as set FCU6-EX878 MELSECNET/10 (Coaxial interface) HR877/878 card Expansion card, Use as set FCU6-EX879 MELSECNET/10 (Optical interface) HR877/879 card Expansion card, Use as set FCU6-HR865 CC-Link HR865 card Expansion card
FCU6-EX871-40 DeviceNet HR871 card Expansion card FCU6-HR881 Extension DIO (Sink type) HR881 card Expansion card FCU6-HR882 Extension DIO
(Sink type, with AO) HR882 card Expansion card
FCU6-HR883 Extension DIO (Source type) HR883 card Expansion card FCU6-HR884 Extension DIO
(Source type, with AO) HR884 card Expansion card
FCU6-HR893 External extension unit HR893 card Extension back panel, a set of metal plates
(3) Communication terminal (Display unit/ NC keyboard)
Type Configuration element Details 7.2- type monochrome LCD RX213 card
FCUA-LD100 7.2-type monochrome LCD with integrated keyboard (Integrated type/machining system sheet) Key switch / escutcheon
Control card 24VDC input
7.2- type monochrome LCD Escutcheon
FCUA-LD10 7.2- type monochrome LCD with display unit (Keyboard separated type)
RX213 card
Use as set with FCUA-KB20 Control card 24VDC input
10.4- type monochrome LCD Escutcheon
FCU6-DUT32 10.4- type monochrome LCD with display unit (Keyboard separated type)
RX215 card
Use as set with FCUA-KB20 Control card 24VDC input
9- type CRT RX211 card
FCUA-CT100 Keyboard integrated type with 9- type CRT (Integrated type/machining system sheet) Key switch / escutcheon
Control card 24VDC input CRT 100VAC input
9- type CRT RX211 card
FCUA-CT120 Keyboard integrated type with 9- type CRT (Integrated type/lathe system sheet) Key switch / escutcheon
Control card 24VDC input CRT 100VAC input
9- type CRT Escutcheon
FCUA-CR10 Display unit with 9- type CRT (Keyboard separated type)
Use as set with FCUA-KB10 Control card 24VDC input CRT 100VAC input
Key switch FCUA-KB10 Keyboard (Separated type/machining system sheet)
RX211 card Use as set with FCUA-CR10
Key switch FCUA-KB20 Keyboard (Separated type/machining system sheet)
Use as set with FCUA-LD10 or FCU6-DUT32
Key switch FCU6-KB021 Keyboard (Separated type/machining system sheet)
Use as set with FCU6-DUT32 (FCUA-KB20 with changed outline dimensions)
Key switch FCUA-KB30 Keyboard (Separated type/lathe system sheet)
Use as set with FCUA-LD10 or FCU6-DUT32
FCU6-KB031 Keyboard (Separated type/lathe system sheet)
Key switch Use as set with FCU6-DUT32 (FCUA-KB30 with changed outline dimensions)
16. Cabinet and Installation 16.1 Cabinet Construction
- 210 -
(4) Peripheral device Type Configuration element Details HD60 Manual pulse generator Without MELDAS logo
HD60-1 Manual pulse generator With MELDAS logo Ground plate D Grounding plate D, one set Ground plate E Grounding plate E, one set
(5) Remote I/O unit Type Configuration element Details
RX311 Base PCB : DI (sink/source)/ DO (sink) = 32/32
FCUA-DX100 DI (sink/source)/DO (sink) = 32/32
Case RX311 Base PCB : DI (sink/source)/
DO (sink) = 32/32 RX321-1 Add-on PCB : DI (sink/source)/
DO (sink) = 32/16
FCUA-DX110 DI (sink/source)/DO (sink) = 64/48
Case RX311 Base PCB : DI (sink/source)/
DO (sink) = 32/32 RX321 Add-on PCB : DI (sink/source)/
DO (sink) = 32/16 analog output 1 point
FCUA-DX120 DI (sink/source)/DO (sink) = 64/48 Analog output 1 point
Case RX311 Base PCB : DI (sink/source)/
DO (sink) = 32/32 RX331 Add-on PCB : Manual pulse
generator 2ch
FCUA-DX130 DI (sink/source)/DO (sink) = 32/32 Manual pulse 2ch
Case RX311 Base PCB : DI (sink/source)/
DO (sink) = 32/32 RX341 Add-on PCB : Analog input 4
points, analog output 1 point
FCUA-DX140 DI (sink/source)/DO (sink) = 32/32 Analog input 4 points Analog output 1 point
Case RX312 Base PCB : DI (sink/source)/
DO (source) = 32/32
FCUA-DX101 DI (sink/source)/ DO (source) = 32/32
Case RX312 Base PCB : DI (sink/source)/
DO (source) = 32/32
RX322-1 Add-on PCB : DI (sink/source)/ DO (source) = 32/16
FCUA-DX111 DI (sink/source)/ DO (source) = 64/48
Case RX312 Base PCB : DI (sink/source)/
DO (source) = 32/32
RX322 Add-on PCB : DI (sink/source)/ DO (source) = 32/16 analog output 1 point
FCUA-DX121 DI (sink/source)/ DO (source) = 64/48 Analog output 1 point
Case RX312 Base PCB : DI (sink/source)/
DO (source) = 32/32
RX331 Add-on PCB : Manual pulse generator 2ch
FCUA-DX131 DI (sink/source)/ DO (source) = 32/32 Manual pulse 2ch
Case RX312 Base PCB : DI (sink/source)/
DO (source) = 32/32
RX341 Add-on PCB : Analog input 4 points, analog output 1 point
FCUA-DX141 DI (sink/source)/ DO (source) = 32/32 Analog input 4 points, analog output 1 point
Case
16. Cabinet and Installation 16.2 Power Supply, Environment and Installation Conditions
- 211 -
16.2 Power Supply, Environment and Installation Conditions
! Caution
! Follow the power supply specifications (input voltage range, frequency range, momentary power failure time range) described in this manual.
! Follow the environment conditions (ambient temperature, humidity, vibration, ambient atmosphere) described in this manual.
(1) Environment conditions in control part
Unit name Control unit Type FCU6-MU043/MU042/MU041
During operation 0 to 55C Ambient temperature During storage 20 to 60C
During operation Long term, Up to 75% RH (with no dew condensation) Short term (Within 1 month), Up to 95% RH (with no dew condensation)Ambient
humidity During storage Up to 75% RH (with no dew condensation)
Vibration resistance 4.9m/s2 or less (during operation) Shock resistance 29.4m/s2 or less (during operation) Working atmosphere No corrosive gases, dust or oil mist G
en er
al s
pe ci
fic at
io ns
Power noise 1kV (P-P) Power voltage 24VDC5% Ripple 5% (P-P) Instantaneous stop tolerance time 2.1ms (during 24VDC line cutting)
Po we
r sp
ec ific
at io
ns
Current consumption 3A (max.) Heating value 70W (during full option) Mass 1.6kg Unit size Refer to Appendix.
(2) Communication terminal
Unit name Communication terminal
Type FCUA-LD100/ FCUA-LD10+KB20
FCU6-DUT32 +KB021
FCUA-CT100/ FCUA-CR10+KB10
During operation 0 to 50C 0 to 55C Ambient temperature During storage 20 to 60C 20 to 65C
During operation Long term, Up to 75% RH (with no dew condensation)
Short term (Within 1 month), Up to 95% RH (with no dew condensation)Ambient humidity
During storage Up to 75% RH (with no dew condensation) Vibration resistance 4.9m/s2 or less (during operation) Shock resistance 29.4m/s2 or less (during operation) Working atmosphere No corrosive gases, dust or oil mist G
en er
al s
pe ci
fic at
io ns
Power noise 1kV (P-P) Single phase 100 to
115VAC 15%+10%
50/60Hz5% Power voltage 24VDC5% Ripple 5% (P-P)
24VDC5% Ripple 5% (P-P)
Instantaneous stop tolerance time Follows specifications of 24VDC power supply being used
P ow
er s
pe ci
fic at
io ns
Current consumption 24V, 0.9A 100V, 0.4A 24V, 0.6A
Heating value 20W 55W Mass 1600g 2200g 4800g Unit size Refer to Appendix.
16. Cabinet and Installation 16.2 Power Supply, Environment and Installation Conditions
- 212 -
(3) Remote I/O unit
Unit name Remote I/O unit
Type FCUA- DX10
FCUA- DX11
FCUA- DX12
FCUA- DX13
FCUA- DX14
During operation 0 to 55C Ambient
temperature During storage 20 to 65C During operation
Long term, Up to 75% RH (with no dew condensation) Short term (Within 1 month), Up to 95% RH (with no dew condensation)Ambient
humidity During storage Up to 75% RH (with no dew condensation)
Vibration resistance 4.9m/s2 or less (during operation) Shock resistance 29.4m/s2 or less (during operation) Working atmosphere No corrosive gases, dust or oil mist G
en er
al s
pe ci
fic at
io ns
Power noise 1kV (P-P) Power voltage 24VDC5% Ripple 5% (P-P) Instantaneous stop tolerance time
Po w
er
sp ec
ifi ca
tio ns
Current consumption 24V, 0.7A (Note 1) 24V, 1.5A (Note 1) 24V, 0.7A (Note 1)
Heating value 25W (Note 2) 30W (Note 2) 30W (Note 2)
Mass 470g 570g 590g 550g Unit size Refer to Appendix.
(Note 1) Only the amount consumed by the control circuit. (Note 2) When all points of the machine input/output interface circuit are operating.
(4) Servo / Spindle
Refer to the following manuals for details on the servo and spindle system. MDS-C1 Series Specification Manual (BNP-C3040) MDS-B-SVJ2 Series Specifications and Instruction Manual (BNP-B3937) MDS-B-SPJ2 Series Specification and Instruction Manual (BNP-B2164) MDS-J2-CT Series Specifications and Instruction Manual (BNP-B3944)
17. Servo/Spindle System 17.1 Feed Axis
- 213 -
17. Servo/Spindle System Refer to the following manuals for details on the servo and spindle system. MDS-C1 Series Specification Manual (BNP-C3040) MDS-B-SVJ2 Series Specifications and Instruction Manual (BNP-B3937) MDS-B-SPJ2 Series Specification and Instruction Manual (BNP-B2164) MDS-J2-CT Series Specifications and Instruction Manual (BNP-B3944)
17.1 Feed Axis
17.1.1 MDS-C1-V1/C1-V2 (200V)
(1) Servo motor: HC -A51/E51 (1000kp/rev) C6 C64
T system L system M system L system T system
(2) Servo motor: HC -A42/E42 (100kp/rev) C6 C64
T system L system M system L system T system
17.1.4 MDS-B-SVJ2 (Compact and Small Capacity)
(1) Servo motor: HC -A42/E42 (100kp/rev) C6 C64
T system L system M system L system T system
(2) Servo motor: HC -A47 (100kp/rev) C6 C64
T system L system M system L system T system
(3) Servo motor: HC -A33/E33 (25kp/rev) C6 C64
T system L system M system L system T system
17.1.6 MDS-R-V1/R-V2 (200V Compact and Small Capacity)
(1) Servo motor: HF -A51/E51 (1000kp/rev) C6 C64
T system L system M system L system T system
(2) Servo motor: HF -A42/E42 (100kp/rev) C6 C64
T system L system M system L system T system
(3) Servo motor: HF -A47 (100kp/rev) C6 C64
T system L system M system L system T system
17. Servo/Spindle System 17.2 Spindle
- 214 -
17.2 Spindle
17.2.1 MDS-C1-SP/C1-SPM/B-SP (200V)
(1) Spindle motor: SJ/SJ-V C6 C64
T system L system M system L system T system
17.2.3 MDS-B-SPJ2 (Compact and Small Capacity)
(1) Spindle motor: SJ-P/SJ-PF C6 C64
T system L system M system L system T system
17.3 Auxiliary Axis
17.3.1 Index/Positioning Servo: MR-J2-CT
(1) Servomotor: HC-SF/HC-RF (16kp/rev) C6 C64
T system L system M system L system T system
(2) Servomotor: HA-FF/HC-MF (8kp/rev) C6 C64
T system L system M system L system T system
17. Servo/Spindle System 17.4 Power Supply
- 215 -
17.4 Power Supply
17.4.1 Power Supply: MDS-C1-CV/B-CVE C6 C64
T system L system M system L system T system
17.4.2 AC Reactor for Power Supply C6 C64
T system L system M system L system T system
17.4.3 Ground Plate C6 C64
T system L system M system L system T system
17.4.4 Power Supply: MDS-A-CR (Resistance Regeneration) C6 C64
T system L system M system L system T system
18. Machine Support Functions 18.1 PLC
- 216 -
18. Machine Support Functions
18.1 PLC
18.1.1 PLC Basic Function
18.1.1.1 Built-in PLC Basic Function C6 C64
T system L system M system L system T system
(1) Ladder commands Basic commands (bit processing commands)
c LD, LDI, OR, ORI, AND, ANI, OUT, PLS, etc. Function commands
192 commands including data transfer, 4 basic arithmetic operations, logic arithmetic operations, large/small identification, binary/BCD conversion, branching, conditional branching, decoding, encoding, etc.
Exclusive commands 5 commands including ATC control Tool life management 12 types of network related commands
18. Machine Support Functions 18.1 PLC
- 217 -
(2) Devices The device number for devices X, Y, B, W and H are expressed with a hexadecimal. All other device numbers are expressed as decimals. Device Device range Units Details
X* X0 to XAFF 2816 points 1-bit Input signals to the PLC. Machine input, etc. Y* Y0 to YE7F 3712 points 1-bit Output signals from the PLC. Machine output, etc. M M0 to M8191 8192 points 1-bit For temporary memory L L0 to L255 256 points 1-bit Latch relay (Backup memory) F F0 to F127 128 points 1-bit For temporary memory. Alarm message interface
SB SB0 to SB1FF 512 points 1-bit Special relay for links B B0 to B1FFF 8192 points 1-bit Link relay
SM* SM0 to SM127 128 points 1-bit Special relay V V0 to V255 256 points 1-bit Edge relay
SW SW0 to SW1FF 512 points 16-bit Special register for links SD SD0 to SD127 128 points 16-bit Special register
T0 to T15 16 points 1-bit/16-bit 10ms unit timer T16 to T95 80 points 1-bit/16-bit 100ms unit timer T96 to T103 8 points 1-bit/16-bit 100ms incremented timer T104 to T143 40 points 1-bit/16-bit 10ms unit timer (Fixed timers) T144 to T239 96 points 1-bit/16-bit 100ms unit timer (Fixed timers) T240 to T255 16 points 1-bit/16-bit 100ms incremented timer (Fixed timers) T0000 to T0255 256 points 1-bit T1: Timer coil T1000 to T1255 256 points 1-bit T0: Timer contact T2000 to T2255 256 points 16-bit TS: Timer setting value
T
T3000 to T3255 256 points 16-bit TA: Timer current value C0 to C23 24 points 1-bit/16-bit Counter C24 to C127 104 points 1-bit/16-bit Counter (Fixed counters) C0000 to C0127 128 points 1-bit C1: Counter coil C1000 to C1127 128 points 1-bit C0: Counter contact C2000 to C2127 128 points 16-bit CS: Counter setting value
C
C3000 to C3127 128 points 16-bit CA: Counter current value D D0 to D8191 8192 points 16-bit/32-bit Data register R* R0 to R8191 8192 points 16-bit/32-bit File register. CNC word I/F W W0 to W1FFF 8192 points 16-bit/32-bit Link register Z Z0 to Z13 14 points 16-bit Address index N N0 to N7 Master control's nesting level
P* P0 to P255 P360 to P379 Conditional jump, subroutine call label
K-32768 to K32767 Decimal constant for 16-bit command K K-2147483647 to
K2147483647 Decimal constant for 32-bit command
H0 to HFFFF Hexadecimal constant for 16-bit command H H0 to HFFFFFFFF Hexadecimal constant for 32-bit command
(Note 1) Devices with an asterisk in the device field have sections with predetermined applications. Do not use these devices for other applications.
(Note 2) 8192 points of D device are available on the S/W version D or higher.
18. Machine Support Functions 18.1 PLC
- 218 -
(3) External alarm messages The contents of the alarms which have occurred during sequence (user PLC) processing can be displayed on the setting and display unit. Up to four alarm message displays can be displayed simultaneously on the alarm diagnosis screen. The maximum length of one message is 32 characters.
(4) External operator messages When a condition has arisen in which a message is to be relayed to the operator, an operator message can be displayed separately from the alarm message. The maximum length of an operator message on the alarm diagnosis screen is 60 characters. The number of messages displayed at the same time is one.
(5) PLC switches 32 points of PLC switches can be set on the setting and display unit screen, and the ON/OFF control executed. The switches can be used as part of the machine operation switches. The switch applications can be freely determined with the sequence program, and each switch name can be created with the PLC and displayed on the setting and display unit.
(6) Load meter display A load meter can be displayed on the setting and display unit. Up to two axes designated with the built-in PLC such as the spindle load and Z axis load can be displayed as bar graphs on the screen.
(7) Timer / counter setting display (a) PLC timer The setting value of the timer used by the built-in PLC can be set from the screen on the
setting and display unit. The timer types include the 10ms, 100ms and 100ms integral types. Whether to validate the timer in the PLC program or to validate the setting value from the
screen can be selected with the parameters. Whether to hold the integral timer when the power is turned OFF can also be selected. (b) PLC counter The setting value of the counter used by the built-in PLC can be set from this screen. Whether to validate the constants in the PLC program or to validate the setting value from
the screen can be selected with the parameters. Whether to hold the counter value when the power is turned OFF can also be selected.
(8) PLC parameter setting display The PLC constants set with the data type and the bit selection parameters set with bit types can be set from the screen as parameters used by the built-in PLC.
(a) PLC constants There are PLC constants that can be set with data types as parameters used by the built-in
PLC. The set data is set in the R register of the PLC and backed up. If data is set in the R register corresponding to the PLC constant with sequence program MOV commands, etc., the data will be backed up. However, the display will not change, so enter another screen, and then select this screen again.
Up to 48 items can be set, and the setting range is 8 digits. (b) Bit selection parameters There are bit selection parameters set with bit types as parameters used by the built-in PLC.
The set data is set in the R register of the PLC and backed up. When using bit operation in the sequence program, the details of the R register are
transferred to the temporary memory (M) with the MOV command. If the data is set in the R register corresponding to the bit selection with the MOV command, etc., the data will be backed up. However, the display will not change, so enter another screen and then select this screen again.
18. Machine Support Functions 18.1 PLC
- 219 -
(9) External key input By inputting the key data from the built-in PLC, the same operation as when the operator operates the operation board can be done.
(10) Real spindle speed output The real spindle speed is converted by the signals of the encoder installed on the spindle and is output to the PLC. The output increment is 0.001r/min.
(11) Workpiece counter display (parts counter) The number of parts can be set and displayed when continuously machining parts. The M code to be count, the current number of machined parts and the max. machining value is set with parameters. This data can be read by the user PLC (when built-in PLC specifications are used), and the number of machined parts can be controlled. A signal will be output to the PLC when the counted number reaches the set max. value.
(12) High speed input/output signal There are signals that can be input and output at a 7.1ms cycle for high-speed processing.
(a) Input signal ON time
tson tson 8ms
(b) After the signal output is set in the interface, it can be output to the machine side with a
max. 7.1ms delay. The input also appears on the interface with a 7.1ms delay. (c) The signals used for high-speed processing are assigned with the parameters.
Assignment is possible in a continuous 16-point unit.
(13) PLC analog voltage control (a) Analog output
When the specified data is put in the file register, the corresponding analog voltage is output from the analog output external connector.
Analog output (V)
Contents of file register
10V
4095
4095
0
10V
(Note) The remote I/O unit DX120/DX121 is required for analog output.
Output voltage 0 to 10V (5%) Resolution Full scale (10V)/4095 Load condition 10 k resistance load (standard) Output impedance 220
18. Machine Support Functions 18.1 PLC
- 220 -
18.1.2 Built-in PLC Processing Mode An exclusive sequence program that controls the various signals between the controller and machine to realize operation applicable to each machine must be created. The sequence execution modes include high-speed processing and main processing.
(1) High-speed processing
This mode provides repeated execution at 7.1ms cycles. It is used to process signals requiring high speeds.
The max. number of program steps for high-speed processing (1 period) is 150 steps when using basic commands.
(2) Main processing This mode provides normal sequence processing. The processing cycle depends on the number of sequence steps.
18.1.2.2 MELSEC Development Tool I/F C6 C64
T system L system M system L system T system
This function enables the data of the PLC contained inside the NC system to be developed and debugged using the GX Developer installed in a personal computer (OS: Windows). Many and varied functions of the GX Developer make it possible to reduce the PLC data development and debugging time.
18.1.3 Built-in PLC Capacity (Number of Steps) C6 C64
T system L system M system L system T system 32000 32000 32000 32000 32000
There are four bytes for each step.
18. Machine Support Functions 18.1 PLC
- 221 -
18.1.4 Machine Contact Input/Output I/F C6 C64
T system L system M system L system T system
! Caution
! Follow the remote type machine contact input/output interface described in this manual. (Connect a diode in parallel with the inductive load or connect a protective resistor in serial with the capacitive load, etc.)
Refer to the MELDAS C6/C64 Connection/Maintenance Manual for details. The machine contacts can be input or output using the internal DI/O and remote I/O, as shown in the figure below. There are two kinds of DI/O, the sink type and source type. A 24V power supply must be provided externally for this DI/O.
Manual pulse generator
Remote I/O unit DX1
Machine control signal
. . . . . . . . Max. 8 units
Max number of input: 256 points (X000 to X0FF) Max number of output: 256 points (Y000 to Y0FF)
RIO-M
Max. 4 channels (X418 to X41B)
Control unit
Built-in DI : 16 (X400 to X40F) Built-in DO : 1 (Y400)
DC2 4VINS ERVO1 S ERVO2
ENC HA NDLE
SIO TE RMI NAL
IC ARD
SKIP
RIO-M/S
Max. 2 additional DIO cards
Sensor
Remote I/O unit DX1
Machine control signal
. . . . . . . . Max. 8 units
Max. number of input: 256 points (X100 to X1FF) Max. number of output: 256 points (Y100 to Y1FF)
18. Machine Support Functions 18.1 PLC
- 222 -
Refer to the Connection Manual for details.
(1) Types of remote I/O units The remote I/O units (FCUA-DX ) are 10 shown in the remote I/O unit list according to the types of signals that can be input/output and the no. of contacts. There are 10 types, and are used as a control unit. Multiple remote I/O units can be combined for use if the total of possessed channel during the serial link connection is less than eight.
Remote I/O unit list
Unit model Compatible machine control signals
No. of channels
possessed by serial link
FCUA- DX100
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Sink type 1
FCUA- DX101
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Source type 1
FCUA- DX110
Digital input signal (DI) : 64 points (insulation) Common for sink/source
Digital output signal (DO): 48 points (non-insulated) Sink type 2
FCUA- DX111
Digital input signal (DI) : 64 points (insulation) Common for sink/source
Digital output signal (DO): 48 points (non-insulated) Source type 2
FCUA- DX120
Digital input signal (DI) : 64 points (insulation) Common for sink/source
Digital output signal (DO): 48 points (non-insulated) Sink type Analog output (AO) : 1 point
2
FCUA- DX121
Digital input signal (DI) : 64 points (insulation) Common for sink/source
Digital output signal (DO): 48 points (non-insulated) Source type Analog output (AO) : 1 point
2
FCUA- DX130
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Sink type Handle input : 2 handles
2
FCUA- DX131
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Source type Handle input : 2 handles
2
FCUA- DX140
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Sink type Analog input : 4 points Analog output : 1 point
2
FCUA- DX141
Digital input signal (DI) : 32 points (insulation) Common for sink/source
Digital output signal (DO): 32 points (non-insulated) Source type Analog input : 4 points Analog output : 1 point
2
(Note) The power for the input/output signal drive unit and receiver must be prepared by the machine maker.
18. Machine Support Functions 18.1 PLC
- 223 -
Interface specifications Input specifications
Sink type Source type Input voltage when ON 0 to 6V 18 to 24V Input voltage when OFF 20 to 24V 0 to 4V
Output specifications
Rated load voltage 24VDC Maximum output current 60mA
(2) Outline of digital signal input circuit
There is a sink type and source type digital signal input circuit. The type is selected with a card unit in each unit.
Input circuit
DI L / DI R
0V
24VDC(+)
Source type
(Machine side)
COM
2.2k
Control circuit
DI L / DI R
0V
Sink type
(Machine side)
24VDC(+) COM
2.2k
Control circuit
(3) Outline of digital signal output circuit
There is a sink type (DX1 0) and source type (DX1 1) digital signal output circuit. Use within the range of the specifications given below.
Output circuit
DO L / DO R
R
24VDC(+) (Machine side)
Source type (DX1 1)
Control circuit
RA
PL
R
24VDC(+) (Machine side)
Control circuit
RA
PL
Sink type (DX1 0)
DO L / DO R
Output conditions
Insulation method Non-insulated Rated load voltage +24VDC Max. output current 60mA Output delay time 40s
* When using an inductive load such as a relay, always connect a diode (withstand voltage 100V or more, 100mA or more) in parallel with the load. The diode should be inserted as close to the load (within 20cm) as possible.
* When using a capacitive load such as a lamp, connect a protective resistor (R=150 ) in serial with the load to limit the rush current. (Make sure that the current is lower than the above tolerable current, including momentary current.)
18. Machine Support Functions 18.1 PLC
- 224 -
(4) Outline of analog signal output circuit The analog signal output circuit can be used only with the FCUA-DX120/DX121.
Output circuit Output conditions
Output voltage 0V~ 10V (5%)
Resolution 12bit (10Vn/4095) (Note) Load conditions 10 k load resistance Output impedance 220
DAC R
R
220
A0 A0
(Note) n = (20 ~ 211)
(5) Input signal conditions The input signals must be used within the ranges of the following conditions.
Source type
Input voltage when external contact is ON 18V or more, 25.2V or less
Input current when external contact is ON 9mA or more Input voltage when external contact is OFF 4V or less Input current when external contact is OFF 2mA or less Tolerable chattering time 3ms or less (Refer to T1 below) Input signal hold time 40ms or more (Refer to T2 below) Input circuit operation delay time 3ms T3 T4 20ms Machine side contact capacity +30V or more, 16mA or more
Sink type
Input voltage when external contact is ON 6V or more
Input current when external contact is ON 9mA or more Input voltage when external contact is OFF 20V or less Input current when external contact is OFF 2mA or less Tolerable chattering time 3ms or less (Refer to T1 below) Input signal hold time 40ms or more (Refer to T2 below) Input circuit operation delay time 3ms T3 T4 20ms Machine side contact capacity DC30V or more, 16mA or more
T1 T1 T1T1
T2T2
Constantly open contact Constantly closed contact T4 T4 T3T3
18. Machine Support Functions 18.1 PLC
- 225 -
18.1.6 PLC Development
18.1.6.2 MELSEC Development Tool C6 C64
T system L system M system L system T system
The GX Developer installed in a personal computer (OS: Windows) can be used.
18.1.7 C Language Function C6 C64
T system L system M system L system T system
PLC subprograms prepared in C language can be called from PLC ladders.
18. Machine Support Functions 18.1 PLC
- 226 -
18.1.12 GOT Connection This function connects a Mitsubishi graphic operation terminal (GOT) with the C6/C64 so it can be used as a machine operation panel, etc. The information displayed on the GOT includes all of the PLC devices in the C6/C64, and the various monitor information. The C6/C64 dedicated setting and display screen and circuit monitor can also be displayed. The following methods can be used to connect the C6/C64 and GOT. A communication unit is required on each unit for either connection method. When using the CPU direct connection, an additional unit is not required on the C6/C64 side.
18.1.12.1 CPU Direct Connection (RS-422/RS-232C) C6 C64
T system L system M system L system T system
Connecting the C6/C64 and GOT with an RS-422 or RS-232C cable is the most cost efficient method. When connecting with RS-422, the GOT is connected to the GPP connector side of the F311 cable connected to the SIO connector on the G64 control unit. When connecting with RS-232C, the GOT is connected to the TERMINAL connector on the C64 control unit.
RS-232C/RS-422 (for GPP) relay
General-purpose RS-232C device connection connector
Cabinet side wall TERMINAL
F311 cable
SIO
LED1
Control unit
R S
-232C G
P P
RS-422 cable GOT
RS-232C cable
Only one method can be used.
GOT
18. Machine Support Functions 18.1 PLC
- 227 -
18.1.12.2 CC-Link Connection (Remote Device) C6 C64
T system L system M system L system T system
C6/C64 functions as the CC-Link system's intelligent device station and remote device station, and can be remotely operated over a network. To connect with CC-Link, the CC-Link unit (FCU6-HR865) must be mounted in the extension slot on the control unit. Use a dedicated cable for the CC-Link cable, and connect to the CC-Link unit (FCU6-HR865) terminal block. Always attach a resistor (enclosed) onto the unit which is the final station.
CC-Link
(Note 4)
(Note 1) With the CC-Link system, the performance will not be guaranteed if a cable other than the CC-Link dedicated cable is used. Refer to the CC-Link Association web site (http://cc-link.org) for information on the CC-Link dedicated cable specifications. (Information is given in the section "Partner Association".
(Note 2) Always use the enclosed terminator. The terminating resistance value differs according to the cable in use. The CC-Link dedicated cable is 110, and the CC-Link dedicated high-performance cable is 130.
(Note 3) Connect the FG wire from the FG terminal on the C64 control unit's CC-Link terminal block to the FG terminal at the bottom of the control unit.
(Note 4) For the C64 control unit's channel No. setting rotary switch and baud rate setting rotary switch, pull out the CC-Link unit from the control unit and set the switches.
Control unit
FG wire for CC-Link (Note 3)
LED1
GOT
Refer to section"18.6.4 CC-Link" for details on the CC-Link specifications for the MELDAS C6/C64. Refer to the "GOT-A900 Series User's Manual (GT Works2 Version1/GT Designer2 Version 1 compatible connection section) and other related documents for details on GOT.
18.1.12.3 CC-Link Connection (Intelligent Terminal) C6 C64
T system L system M system L system T system
Refer to section "18.1.12.2 CC-Link Connection (Remote Device)" for details.
18. Machine Support Functions 18.1 PLC
- 228 -
18.1.12.5 Ethernet Connection C6 C64
T system L system M system L system T system
When assembled in an Ethernet system, the C6/C64 can be remotely operated over a network. To connect with Ethernet, the Ethernet module (FCU6-EX875) must be mounted in the extension slot on the control unit. The Ethernet cable (10BASE-T cable) is connected to the Ethernet module's modular jack. The Ethernet cable is easily affected by noise, so separate it from the drive and power cables, and mount the ferrite core (enclosed) on the control unit side. Use of a shielded cable is recommended when using in a poor environment, or when compliance with EMC Directives is required.
LED1
(Note 1) Mount the ferrite core with the following procedures. (1) Turn the cable once. (2) Attach the case by pressing until a click is heard. (3) Fix with a binding band so that the position does not
deviate. (Note 2) When using a shielded cable, a separate FG cable must
be prepared to connect the shield the FG. Normally the cable is connected to the control unit's FG terminal, but if the position is near the grounding plate, connect directly to that plate.
(Note 3) To comply with the EMC Directives, a ferrite core must also be mounted on the GOT side.
GOT
One turn
(Note 1)
Ferrite core Ferrite core (Note 3) Ethernet
FG wire for Ethernet (Note 2)
Control unit
18. Machine Support Functions 18.1 PLC
- 229 -
18.1.13 PLC Message
18.1.13.1 Japanese C6 C64
T system L system M system L system T system
18.1.13.2 English C6 C64
T system L system M system L system T system
18.1.13.13 Polish C6 C64
T system L system M system L system T system
18. Machine Support Functions 18.2 Machine Construction
- 230 -
18.2 Machine Construction
18.2.1 Servo OFF C6 C64
T system L system M system L system T system
When the servo OFF signal (per axis) is input, the corresponding axis is set in the servo OFF state. When the moving axis is mechanically clamped, this function is designed to prevent the servomotor from being overloaded by the clamping force. Even if the motor shaft should move for some reason or other in the servo OFF state, the movement amount will be compensated in the next servo ON state by one of the following two methods. (You can select the compensation method using a parameter.) (1) The counter is corrected according to the movement amount (follow up function). (2) The motor is moved according to the counter and compensated. When follow up is designated, the movement amount will be compensated even in the emergency stop state. The axis is simultaneously set with servo OFF to the interlock state. Mechanical handle Even if the servo OFF axis is moved with the mechanical handle with the application of the servo OFF function and follow up function, the position data can be constantly read in and the machine position updated. Thus, even if the axis is moved with the mechanical handle, the coordinate value display will not deviate.
18. Machine Support Functions 18.2 Machine Construction
- 231 -
18.2.2 Axis Detach C6 C64
T system L system M system L system T system
This function enables the control axis to be freed from control. Conversely, an axis which has been freed from control can be returned to the control status. This function enables the rotary table or attachments to be removed and replaced. Automatic operation is disabled until the axis for which the axis detach command has been released completes its dog-type reference point return.
C-axis/turning table
Rotary magnetic scale
(OFF with C-axis control )
Spindle
motor (Coupled with C-axis control)
(Position feedback)
Spindle
amplifier
C-axis
amplifier
C-axis motor
This shows the configuration of a machine for which switching between the C axis and turning table is performed. When the spindle motor is connected, the C axis is placed in the detached status. As a result, the position feedback of the detector is ignored.
The detached status > < is indicated on the right of the current position display on the POSITION screen and at the same time the servo ready for the controller output signal is set to OFF. The current position counter retains the value applying when detach was assigned.
POSITION X 1 2 3 . 4 5 6 Z 0 . 0 0 0 #1 C 3 4 5 . 6 7 8 ><
(Note) Axis detach can be executed even for the absolute position detection specifications axis, but when the axis is reinstalled, the zero point must be set.
18. Machine Support Functions 18.2 Machine Construction
- 232 -
18.2.3 Synchronous Control
18.2.3.1 Position Tandem C6 C64
T system L system M system L system T system
The synchronous control is a control method that both master and slave axes are controlled with the same movement command by designated the movement command for the master axis also to the slave axis. This function is assumed to be used in the large machine tool, etc. which drives one axis with two servo motors. The axis for the base of the synchronization is called the master axis, and the axis according to the master axis is called the slave axis. The axis detach function cannot be added to the axes used in the synchronous control. The slave axis is controlled with the movement command for the master axis. One slave axis can be set to one master axis. Two sets are applied for the master and slave axes Synchronous control
Independent operation method
Synchronous operation method
Correction mode
Synchronous control mode
Y V
X
Z
(Master axis) (Slave axis)
18. Machine Support Functions 18.2 Machine Construction
- 233 -
(1) Synchronous control mode The following two operation methods are available in the synchronous control mode. (a) Synchronous operation
This is a method that both master and slave axes are moved simultaneously with the movement command for the master axis.
X
Y
V
Z
X
Y
V
Z M
S
Machining program
Axis motor
Servo control
Calculation of feed rate
Calculation of movement directions, movement amount
Position control section
Backlash compensation Reference position return
X axis control
CNC system
Y axis control
V axis control
Z axis control
Servo control
Servo control
Servo control
NC control section
There is a function that checks the correlation between the positions of the master axis and slave axis at all times while the synchronous operation method is selected to stop the feed as alarm when the allowable synchronization error value set in the parameter is exceeded. However, when the zero point is not established, the synchronous error is not checked.
(b) Independent operation
This is a method that either the master or slave axis is moved with the movement command for the master axis.
X
Y
V
Z
X
Y
V
Z M
S
Machining program
Axis motor
Servo control
Calculation of feed rate
Calculation of movement directions, movement amount
Position control section
Backlash compensation Reference position return
X axis control
CNC system
Y axis control
V axis control
Z axis control
Servo control
Servo control
Servo control
NC control section
(2) Correction mode The synchronization is temporary canceled to adjust the balance of the master and slave axes
during the synchronous control mode in the machine adjustment. Each axis can be moved separately with the manual handle feed or the arbitrary feed in manual mode. If the operation mode other than the manual handle feed and arbitrary feed in manual mode is applied during the correction mode, the operation error will occur.
18. Machine Support Functions 18.2 Machine Construction
- 234 -
18.2.3.2 Speed Tandem C6 C64
T system L system M system L system T system
This function is used to drive in parallel while matching the position and speed. In addition to the NC's synchronous control function, the master axis and slave axis speed command can be set to the same command by making the master axis and slave axis position feedback signal the same using the servo drive unit. The speed command synchronization control cannot be used unless the NC setting and servo drive unit settings are changed. The speed loop and current loop are controlled using the feedback signals for the respective axis.
18.2.3.3 Torque Tandem C6 C64
T system L system M system L system T system
This function is used to drive in parallel while matching the position, speed and current when the machine rigidity is high. In addition to the NC's synchronous control function, the master axis and slave axis speed command can be set to the same command by making the master axis and slave axis position feedback signal and the speed feedback signal the same using the servo drive unit. The current loop is controlled using the feedback signals for the respective axis.
18. Machine Support Functions 18.2 Machine Construction
- 235 -
18.2.7 Auxiliary Axis Control (J2-CT) C6 C64
T system L system M system L system T system
The MR-J2-CT drive unit for positioning and indexing can be connected for auxiliary axis control. The drive unit is a single-axis control unit, and the control is performed from the PLC. It comes with the following functions, and is suited to controlling a peripheral device of the machine. (1) Feed functions
(a) Four different feed rates can be set and selected using parameter settings. (b) Constant inclination acceleration/deceleration, linear acceleration/deceleration or soft
acceleration/deceleration can be selected. (c) When rotary axis is used, automatic short-cut discrimination and rotary direction can be
assigned by commands.
(2) Command methods (a) Station method Any point (station) obtained when the rotary axis has been divided into equal parts can be
selected by a command, and the axis can be positioned at that point. The maximum number of divisions is 360.
(b) Arbitrary coordinate designation method The arbitrary coordinates (absolute position as referenced to the zero point) can be
commanded from the PLC and the axis can be positioned at these coordinates. (3) Operation functions
(a) JOG mode In this mode, the axis is rotated at a constant speed in the designated direction while the
start signal is ON. (b) Automatic mode In this mode, the axis is positioned at the designated station number by the start signal. (c) Manual mode In this mode, the axis is rotated at a constant speed in the designated direction while the
start signal is ON. When the start signal is set to OFF, the axis is positioned at the nearest station position.
(d) Arbitrary coordinate mode In this mode, the axis is positioned at the arbitrary coordinates designated with the PLC by
the start signal. When the start signal is set to OFF prior to the completion of the positioning, the axis immediately decelerates and stops.
(e) Manual handle mode In this mode, axis travel is carried out by the pulse command (manual handle command)
sent from the PLC. (f) Reference point return mode In this mode, the axis is positioned at the coordinate reference point. Two methods are
used: one method is based on a dog switch and the other method is to carry out positioning to the reference point which is stored in the memory.
(g) Press-fit-and-positioning mode In this mode, the axis is positioned while it is pressed against the machine end, etc.
18. Machine Support Functions 18.3 PLC Operation
- 236 -
18.3 PLC Operation
18.3.1 Arbitrary Feed in Manual Mode C6 C64
T system L system M system L system T system
This function enables the feed directions and feed rates of the control axes to be controlled using commands from the user PLC. The arbitrary feed function controls the movement of the axes at the specified rates while the start signal is output from the PLC to the NC system. PLC operations can be performed even during manual operation or automatic operation, but they cannot be performed when an axis for which arbitrary feed has been assigned is executing a command from the NC system (that is, while the axis is moving).
18. Machine Support Functions 18.3 PLC Operation
- 237 -
18.3.3 PLC Axis Control C6 C64
T system L system M system L system T system
Over and above the NC control axes, this function enables axes to be controlled independently by commands based on the PLC.
PLC axis control ATC
DDB function
PLC
Item Description Number of control axes Max. 7 axes
Simultaneously controlled axes
PLC control axis is controlled independently from NC control axes. A multiple number of PLC axes can be started simultaneously.
Command increment Least command increment 0.001mm (0.0001 inch) 0.0001mm (0.00001 inch) (Same as command increment for NC control axes)
Feed rate Least command increment: 0.001mm Rapid traverse 0 to 1000000 mm/min (0 to 100000 inch/min) Cutting feed 0 to 1000000 mm/min (0 to 100000 inch/min) Least command increment: 0.0001mm Rapid traverse 0 to 100000 mm/min (0 to 10000 inch/min) Cutting feed 0 to 100000 mm/min (0 to 10000 inch/min)
Movement commands Incremental commands from current position Absolute commands for machine coordinate system 0 to 99999999 (0.001mm/0.0001 inch)
Operation modes Rapid traverse, cutting feed, jog feed (+) (), reference point return feed (+) (), handle feed
Acceleration/deceleration Rapid traverse, jog feed, reference point return feed ..... Linear acceleration/deceleration Cutting feed ..... Exponential function acceleration/deceleration Handle feed .......Step
Backlash compensation Available Stroke end None Soft limit Available Rotary axis command Available
For absolute commands: amount within 1 rotation (rotation by amount remaining after division into 360)
For incremental commands: rotation by assigned amount Inch/mm changeover None
Set to the command that corresponds to the feedback unit. Position detector Encoder (Absolute position can also be detected.)
18. Machine Support Functions 18.4 PLC Interface
- 238 -
18.4 PLC Interface
18.4.1 CNC Control Signal C6 C64
T system L system M system L system T system
Control commands to the CNC system are assigned from the PLC. Input signals with an A/D conversion function and skip inputs that respond at high speed can also be used.
(1) Control signals Control signals for operations in automatic operation mode Control signals for operations in manual operation mode Control signals for program execution Control signals for interrupt operations Control signals for servo Control signals for spindle Control signals for mode selection Control signals for axis selection Control signals for feed rates
(2) Analog voltage control [T system, M system] When an analog voltage is input to an external connector used to connect CNC analog inputs, the data corresponding to the input voltage can be read out in the prescribed file register. This data can be used for load meter displays, thermal deformation compensation, etc. (Maximum 8 points)
(3) Skip signals When signals are input to the skip input interface, they are processed by interrupt processing. This enables functions requiring a high response speed to be implemented. (Maximum 4 points) For further details, refer to the PLC Interface Manual.
18. Machine Support Functions 18.4 PLC Interface
- 239 -
18.4.2 CNC Status Signal C6 C64
T system L system M system L system T system
The status signals are output from the CNC system. They can be utilized by referencing them from the PLC. These signals can also be output as analog data by setting the data from the PLC in the R register.
Status output functions (1) Controller operation ready
When the controller power is turned ON and the controller enters the operation ready status, the "Ready" signal is output to the machine. Refer to the PLC Interface Manual for details of the sequences from when the controller power is supplied to when the controller ready status is entered.
(2) Servo operation ready When the controller power is turned ON and the servo system enters the operation ready status, the "Servo ready" signal is output to the machine. Refer to the PLC Interface Manual for details of the sequences from when the power is supplied to when the "Servo ready" signal is turned ON.
(3) In automatic operation Generally, if the "cycle start" switch is turned ON in the automatic operation mode (memory, MDI), this signal is output until the reset state or emergency stop state is entered by the M02, M30 execution or the reset & rewind input to the controller using the reset button.
(4) In automatic start The signal that denotes that the controller is operating in the automatic mode is output from the time when the cycle start button is pressed in the memory or MDI mode and the automatic start status has been entered until the time when the automatic operation is terminated in the automatic operation pause status entered by the "feed hold" function, block completion stop entered by the block stop function or resetting.
(5) In automatic pause An automatic operation pause occurs and this signal is output during automatic operation from when the automatic pause switch is pressed ON until the automatic start switch is pressed ON, or during automatic operation when the mode select switch is changed from the automatic mode to the manual mode.
(6) In rapid traverse The "In rapid traverse" signal is output when the command now being executed is moving an axis by rapid traverse during automatic operation.
(7) In cutting feed The "In cutting feed" signal is output when the command now being executed is moving an axis by cutting feed during automatic operation.
(8) In tapping The "In tapping" signal is output when the command now being executed is in a tap modal which means that one of the statuses below is entered during automatic operation.
(a) G84 (fixed cycle: tapping cycle) (b) G74 (fixed cycle: reverse tapping cycle) (c) G63 (tapping mode)
18. Machine Support Functions 18.4 PLC Interface
- 240 -
(9) In thread cutting The "In thread cutting" signal is output when the command now being executed is moving an axis by thread cutting feed during automatic operation.
(10) In rewinding The "In rewinding" signal is output when the reset & rewind signal is input by M02/M30, etc., during memory operation and the program currently being executed is being indexed. The rewinding time is short, so there may be cases when it cannot be confirmed with the sequence program (ladder).
(11) Axis selection output The "Axis selection output" signal for each axis is output to the machine during machine axis movement.
(a) Automatic mode The signal is output in the movement command of each axis. It is output until the machine
stops during stop based on feed hold or block stop. (b) Manual mode (including incremental feed) The signal is output while the axis is moving from the time when the jog feed signal is
turned ON until the time when it is turned OFF and the machine feed stops. (c) Handle feed mode The signal is output at all times when the axis selection input is on.
(12) Axis movement direction This output signal denotes the direction of the axis now moving, and for each axis a "+" (plus) signal and a "" (minus) signal are output respectively.
(13) Alarm This signal indicates the various alarm statuses that arise during controller operation. It is divided into the following types and output.
(a) System errors (b) Servo alarms (c) Program errors (d) Operation errors
(14) In resetting The "Reset" signal is output during the reset process when the reset & rewind command is input to the controller with the "reset" button on the setting and display unit is pressed or when the "Reset" signal is input from the machine operation panel, etc. This signal will also be output when the controller READY status is OFF, when the Emergency stop signal is input or when a servo alarm is occurring, etc.
(15) Movement command finish In the memory or MDI automatic operation, the "Movement command finish" signal is output when the command block in the machining program features a movement command and when that block command has been completed. When the movement command and M, S, T or B command have been assigned in the same block, then the movement command signal can be used as a sync signal for either executing the processing of the M, S, T or B command at the same time as the command or executing it upon completion of the movement command.
18. Machine Support Functions 18.4 PLC Interface
- 241 -
18.4.5 DDB C6 C64
T system L system M system L system T system
The DDB (direct data bus) provides the function for PLC to directly read/write controller data. PLC can read the specified data into a buffer and set (write) the specified data into the controller by setting information required for read/write in the buffer and calling the DDB function. Generally, data is read/written for each data piece, but data related to control axes is processed in batch for as many axes as the specified number of axes. The feature of the DDB function is the capability of referencing read data or write data in the next step just after a DDBA instruction is executed.
18. Machine Support Functions 18.5 Machine Contact I/O
- 242 -
18.5 Machine Contact I/O Standard DI/DO (DI:16/DO:1)
C6 C64 T system L system M system L system T system
Operation board IO DI:32/DO:32 C6 C64
T system L system M system L system T system
Operation board IO DI:64/DO:48
C6 C64 T system L system M system L system T system
Remote IO 32/32 C6 C64
T system L system M system L system T system
Remote IO 64/48
C6 C64 T system L system M system L system T system
Additional built-in DI/DO (DI:32/DO:32)
C6 C64 T system L system M system L system T system
18. Machine Support Functions 18.6 External PLC Link
- 243 -
18.6 External PLC Link
18.6.4 CC-Link C6 C64
T system L system M system L system T system
NC unit can be directly connected to the network to serve as the master/local station of the MELSEC CC-Link. To enable this connection, the CC-Link master/local units (HR865) must be installed in the expansion slots. Up to two communication units can be mounted. Refer to the "MELSEC CC-Link System Master/Local Unit User's Manual" for details on CC-Link.
18. Machine Support Functions 18.6 External PLC Link
- 244 -
(1) Performance specifications Item CC-Link master/local unit (HR865)
Baud rates 156kbps/625kbps/2.5Mbps/5Mbps/10Mbps can be selected.
Max. transmission distance The followings are obtained by the baud rate described above. 1200m/600m/200m/150m110m/100m80m50m
Max. number of connection units
64 units Note that the following conditions must be satisfied. {(1 a)+(2 b)+(3 c)+(4 d)} 64 a: Number of units that occupy station 1 b: Number of units that occupy station 2 c: Number of units that occupy station 3 d: Number of units that occupy station 4 {(16 A)+(54 B)+(88 C)} 2304 A: Number of remote I/O stations 64 units B: Number of remote device stations 42 units C: Local station, Standby master station, 26 units
Number of intelligent device stations Number of occupied stations (Number of local stations)
Station 1 to station 4 (Changing over with DIP switch)
Remote input/output (RX, RY) : Input/output each 2048 points
Remote register (RWw) : 256 points (Master station remote/local station)
(Note 1) Max. number of link points per one system
Remote register (RWw) : 256 points (Remote/local station master station)
Remote input/output (RX, RY) : 32points (Local station is 30 points)
Remote register (RWw) : 4 points (Mater station remote/local station)
Number of link points per one remote station/local station
Remote register (RWw) : 4 points (Remote/local station master station)
Communication method Polling method Synchronization method Flame synchronization method Encode method NRZI method Transmission path method Bus (RS485) Transmission format HDLC standard satisfied Illegal control method CRC (X16 + X12 +X5 + 1) Connection cable Twist pair cable with shield
RAS function Automatic link refresh function Sub-station isolation function Link special relay/error detection by register
Number of Input/output occupied points
32 points
(Note 1) When assigning the CC-Link master station to the C64, the maximum number of remote
input/output points may decrease depending on the number of device points that can be secured on the C64 side.
18. Machine Support Functions 18.6 External PLC Link
- 245 -
(2) Usable functions In the CC-Link functions, the ones listed in the table below can be used by the NC.
Function item MELSEC MELDAS C6/C64
Ver.1
M et
ho d
Ver.2
Communication between master station and remote I/O station
Communication between master station and remote device station
Communication between master station and local station
Mixed system communication Reserved station function Error cancel station function Setting of data link status when trouble occurs in CPU of master station
Registration of parameters in EEPROM Setting of input data status from data link trouble station
Unit resetting by sequence program Data link stop/restart Parameter registration function Automatic refresh function
Synchronous mode
M as
te r f
un ct
io n
Scan synchronization function Asynchronous
mode
Local station
LED diagnosis status 16-point display (A1SJ61QBT11)
16-point display
Station number setting
Baud rate setting Setting switches on card
Mode setting switch Se tti
ng a
nd
di sp
la y
fu nc
tio ns
Condition setting
Unit front panel switches Card front panel
switches
Automatic link refresh function Sub-station isolation function
Data link status check (SB/SW)
To SB/SW Automatic refresh
Off-line test On-line test Monitor diagnosis Standby master function
R A
S fu
nc tio
ns
Temporary error cancel station designation function
READ command/SREAD command
WRITE command/SWRITE command
D ed
ic at
ed
co m
m an
ds
RIRD command/RIWT command (Note 1)
(Note 1) Transient operation following these commands is applicable from software version D and
following.
18. Machine Support Functions 18.6 External PLC Link
- 246 -
(3) Connection The CC-Link unit (FCU6-HR865) must be mounted in the control unit's extension slot to connect IO devices using CC-Link. Connect a dedicated CC-Link cable to the CC-Link unit (FCU6-HR865) terminal block. Always install the enclosed terminator on the final station. This unit functions as the CC-Link system's master and local station. Refer to the MELSEC A1SJ61QBT11 type CC-Link System Master/Local Unit's User Manual, etc., for details on the CC- Link system.
CC-Link
Remote I/O station terminal block
Terminator (Note 2)
(Note 4)
(Note 1) The performance of the CC-Link system cannot be guaranteed when a cable other than the CC-Link dedicated cable is used. For details on the CC-Link dedicated cable, refer to the CC-Link Partner Association's web site (http://www.cc-link.org/). (Information is provided in the section "Introduction to Partner Makers".)
(Note 2) Use the enclosed terminator. The terminator value differs according to the cable being used. The CC-Link dedicated cable uses 110, and the CC-Link dedicated high-performance cable uses 130.
(Note 3) Connect the FG wire from the FG terminal on the C64 control unit's CC-Link terminal block to the FG terminal on the bottom of the control unit.
(Note 4) Pull out the CC-Link unit from the control unit and set the C64 control unit's station No. setting rotary switch and baud rate setting rotary switch.
Control unit
C64 control unit CC-Link terminal block
CC-Link FG wire (Note 3)
Shielded twisted pair cable (3-core type) (Note 1)
Shielded twisted pair cable (3-core type) (Note 1)
5 FG 4 SLD 3 DG 2 DB 1 DA
Terminator (Note 2)
Remote I/O station Remote I/O stationLED1
DA
FG
SLD
DG
DB
DA
FG
SLD
DG
DB
Remote I/O station terminal block
18. Machine Support Functions 18.6 External PLC Link
- 247 -
18.6.6 DeviceNet (Master/Slave) C6 C64
T system L system M system L system T system master master master master master
This function is for connecting MELDAS C6/C64 with DeviceNet as the master station. The HR871 dedicated interface card is required for this function.
Windows PC for setting the parameters +
SyCon2 made by Synergetic
C64
Network power supply (24VDC)
Terminator
HR871
Tap
RS-232C
Master + slaves = 64 units
Terminator
Features
DeviceNet complies with the revised version 2.0 of the written DeviceNet standards. C6/C64 operates as a Group2-only client of DeviceNet, and it communicates with the
Group2-only server. I/O communication involves 256 bytes (2048 points) each for the input and output.
Restrictions (1) The HR871 interface card enables C6/C64 to operate as the Group2-only client, but no
communication is performed with other masters. In other words, communication with the configurator in the network is not supported, and dynamic establishment of connections is not supported either.
(2) The communication circuit board is made by Hilsher of Germany and, as such, when the network analyzer is installed, it will appear to be a Hilsher product (since Hilsher's vendor ID is recognized).
(3) The DeviceNet communication parameters must be set (configured) using either the configurator SyCon Ver.2.0 made by Synergetic and running in Windows or the PLC program.
18. Machine Support Functions 18.6 External PLC Link
- 248 -
18.6.7 MELSEC-Q Series Input/Output/Intelligent Function Unit Connection C6 C64
T system L system M system L system T system
The MELSEC-Q Series input/output/intelligent function unit can be connected to the NC (MELDAS C6/C64). Connections with the following specifications are possible when the Q bus bridge card HR863 is added. Only one Q bus bridge card can be mounted, and the extension space for up to two stages can be connected to the Q bus bridge card. There is a maximum of 24 slots (number of units). Basic specifications for MELSEC I/O connection
Item Basic specifications Number of input/output points
Maximum input points: 512 points Maximum output points: 512 points
Access of intelligent unit's buffer memory
A maximum of 12k words can be accessed per scan of the intelligent unit's buffer memory using the FROM/TO commands issued from the C6/C64's built-in PLC.
Connectable MELSEC units I/O unit
Part Type Outline QX10 100 to 120VAC/7 to 8mA, 16 points, response time: 20ms, terminal block AD QX28 24VDC , 8 points, terminal block
QX40 240VDC/4mA, plus common, 16 points, response time: 1/5/10/20/70ms, terminal block
QX40-S1 24VDC plus common input, 16 points, terminal block, for high-speed input (response time can be designated as 0.1ms)
QX41 24VDC/4mA, plus common, 32 points, response time: 1/5/10/20/70ms, connector
QX42 24VDC/4mA, plus common, 64 points, response time: 1/5/10/20/70ms, connector
QX80 24VDC/4mA, minus common, 16 points, response time: 1/5/10/20/70ms, terminal block
Input unit DC
QX81 24VDC/4mA, minus common, 32 points, response time: 1/5/10/20/70ms, connector
QY10 240VAC/24VDC, 2A/point, 8A/common, 16 points (16 points/common), output delay: 12ms, no fuse, terminal block Contact
QY18A 240VAC/24VDC, 2A, 8-point independent contact output, terminal block, no fuse
AC Triac QY22 240VAC/0.6A, 16 points, terminal block, no fuse
QY40P 12/24VDC, 0.1A/point, 1.6A/common, 16 points (16 points/common), output delay: 1ms, terminal block, with short-circuit protection function
QY41P 12/24VDC, 0.1A/point, 2A/common, 32 points (32 points/common), output delay: 1ms, terminal block, with short-circuit protection function
QY42P 12/24VDC, 0.1A/point, 2A/common, 64 points (32 points/common), output delay: 1ms, connector, with short-circuit protection function
Transistor
QY50 12/24VDC, 0.5A/point, 4A/common, 16 points (16 points/common), output delay: 1ms, with fuse, terminal block
Transistor (sink) QY68A 5-24VDC, 2A/point, 8A/unit, 8 points, all points independent, sink/source,
terminal block, no fuse
QY70 5/12VDC, 16mA/point, 16 points (16 points/common), output delay: 0.3ms, with fuse, terminal block TTL CMOS
(sink) QY71 5/12VDC, 16mA/point, 32 points (32 points/common), output delay: 0.3ms, with fuse, connector
QY80 12/24VDC, 0.5A/point, 4A/common, 16 points (16 points/common), output delay: 1ms, with fuse, terminal block
Output unit
Transistor (source) QY81P 12/24VDC, 0.1A/point, 2A/common, 32points (32points/common), output
delay: 1ms, connector, with short-circuit protection function
18. Machine Support Functions 18.6 External PLC Link
- 249 -
Intelligent unit Part Type Outline
QJ71FL71-T-F01 QJ71FL71-B5-F01 FL-net (OPCN-2) unit QJ71FL71-B2-F01
AS-i master unit QJ71AS92 AS-i Standard Ver. 2.11 compatible master Others
Part Type Outline Q63B Power supply + 3-I/O slots, for mounting Q Series units Q65B Power supply + 5-I/O slots, for mounting Q Series units Q68B Power supply + 8-I/O slots, for mounting Q Series units
Extension base
Q612B Power supply + 12-I/O slots, for mounting Q Series units Q61P-A1 100-120VAC input/5VDC 6A output Q61P-A2 200-240VAC input/5VDC 6A output Q62P 100-240VAC input/5VDC 3A, 24VDC/0.6A output Q63P 24VDC input/5VDC 6A output
Power supply unit
Q64P 100-120/200-240VAC input, 5VDC 8.5A output
(Note 1) Up to two stages of extension bases can be connected. (Note 2) The extension base with no power supply cannot be used.
The MELSEC units are connected in the following manner.
MELSEC unit connection
QC B extension cable
C6/C64
Q bus bridge card HR863
Extension base
Extension base Maximum extension bases : 2 stages Maximum number of slots (number of units) : 24 (Including empty slots)
18. Machine Support Functions 18.6 External PLC Link
- 250 -
18.6.9 MELSECNET/10 C6 C64
T system L system M system L system T system
The coaxial bus type and optical loop type networks can be used between the controllers in the MELSECNET/10 data link system. When using the coaxial bus type, the FCU6-EX878 MELSECNET/10 unit must be mounted in the control unit's extension slot, and when using the optical loop type, the FCU6-EX879 MELSECNET/10 unit must be mounted. This unit functions as the control station and normal station of the MELSECNET/10 data link system. Refer to the AJ71QLP21 (S1)/AJ71QBR11 type MELSECNET/10 Network Unit User's Manual (Hardware Section) for details on MELSECNET/10.
(1) Performance specifications
Item Optical loop system (HR879) Coaxial bus system (HR878) LX/LY 8192 points LB 8192 points Maximum number of
links per network LW 8192 points
Maximum number of links per station
B 8192 points Maximum ring devices in NC W 8192 points
Communication speed 10MBPS (equivalent to 20MBPS during multiplex transmission) 10MBPS
Communication method Token ring method Token bus method Synchronization method Frame synchronization Coding method NRZI (Non Return to Zero Inverted) Manchester coding Transmission path format Double loop Single bus Transmission format HDLC compliant (frame type) Maximum number of networks 255 Maximum number of groups 9 Number of connected stations per network
64 stations (Control station 1, normal station: 63)
32 stations (Control station 1, normal station: 31)
3C-2V 5C-2V
Overall distance per network 30km (500mm between stations) 300m (300mm between
stations)
500m (500mm between
stations) Error control method Retry with CRC (X16+X12+X5+1) and overtime
RAS functions
Loop back at error detection and cable disconnection (only optical loop system) Diagnosis of local station's number of link check System down prevention with control station transfer Error detection with special relays and special registers, etc. Network monitor, various diagnosis functions
Transient transmission N:N communication (monitor, program upload, download, etc.) ZNRD/ZNWR (N:N)
Connection cable SI-200/250 3C-2V, 5C-2V or equivalent
Applicable connector 2-core connector plug CA7003
BNC-P-3-Ni-CAU, BNC-P-5-Ni-CAU (DDK) or equivalent
Cable transmission loss 12db/Km or less JIS C 3501 compliant
B + Y 8
+ (2 W) 2000 byte
18. Machine Support Functions 18.6 External PLC Link
- 251 -
(2) Usable functions The MELDAS C6/C64 can use the following MELSECNET/10 network functions.
Function item MELSEC MELDAS C6/C64 Control station function Control station transfer function
Communication with B/W (1:N)
Communication with X/Y (1:1)
Constant link scan function Data link stop/restart Transmission between data links
Cyclic transmission
Station parameters N:N communication Routing function Transient transmission Group function Automatic return function Loopback function Station cutoff function RAS function Data link status detection function
Remote I/O network
Multiple transmission function (only optical loop system)
(only optical loop system)
N et
w or
k fu
nc tio
n
Reserved station function
LED diagnosis function 22-point display 4-point (coaxial) or
7-point (optical loop) display
Network No. setting Group No. setting Station No. setting Condition setting
Setting switch on card
Mode setting switch Switch on front of cardSe tti
ng a
nd d
is pl
ay
fu nc
tio ns
Display changeover switch
Switch on front of unit
Hardware test Internal self-loopback test Self-loopback test Station-to-station test
Main/sub-loop test (only optical loop system)
Loop test Setting switch confirmation Station check order Line monitor Status monitor Error history monitor
Se lf-
di ag
no si
s fu
nc tio
n
Network test
READ/SREAD
D ed
ic at
ed
co m
m an
ds
WRITE/SWRITE
18. Machine Support Functions 18.6 External PLC Link
- 252 -
(3) Connecting the coaxial bus type MELSECNET/10 Connect a dedicated coaxial cable to the MELSECNET/10 unit (FCU6-EX878) connector. Use the enclosed F-shape connector, and always install the terminator A6RCON (optional) on the final unit.
Terminator
MELSEC NET/10
Control unit Control unit
MELSECNET/10 FG wire (Note 5)
F-shape connector
LED1 LED1
(Note 1) Use a high-frequency coaxial cable 3C-2V or 5C-
2V (compliant with JIS-C-3501). The BNC-P- -Ni-CAU (DDK) is recommended. (Note 2) Lay the coaxial cable at least 100mm away from
the other drive lines and control cables. When using in an adverse environment, or when
compliance to EMC Directives is required, use a double shielded coaxial cable (Mitsubishi Wire 5C- 2V-CCY, etc.). Connect the outer shield to the FG using the shield clamp fitting.
(Note 3) Use the following length of coaxial cable according to the total number of stations.
Total number of stations Distance between stations 1 to 9 stations 1 to 500m
10 to 32 stations
1 to 5m 13 to 17m
25 to 500m (Note 4) The BNC-TMP-05 (75) (Hirose Electric) terminator
can be used instead of the A6RCON-R75 (optional). (Note 5) Connect the FG wire from the FG terminal on the
front of the MELSECNET/10 unit (FCU6-EX878) to the FG terminal on the bottom of the control unit.
FG cable assembly diagram Protective tube or connector housing AMP: 171809-2 (black)
Recommended terminal type: AMP 250 Series 170232-2 (for AWG 20-14) 170234-2 (for AWG 12-10)
Select according to the terminal block being used.
Crimp terminal 2
Applicable tab shape 0.80.025
0.9
5.0
6.2
9.6
18. Machine Support Functions 18.6 External PLC Link
- 253 -
(4) Connecting the optical loop type MELSECNET/10 Connect a dedicated optical fiber cable to the optical connector on the MELSECNET/10 unit (FCU6-EX879).
(Note 1) An indoor standard cable AS-2P-5M-A, etc., is recommended for the optical fiber cable. Consult with Mitsubishi Electric System Service.
(Note 2) The optical loop system's optical module follows SI specifications. The total distance within one network is 30km, and the distance between stations is 500m.
(Note 3) The optical loop system is a double loop transmission path method. The following system is used to connect the optical fiber cables.
MELSEC NET/10
OUT T (F-SD) Main loop transmission (F) SD (OUT T (F-SD))
OUT R (R-RD) Sub-loop transmission (R) RD (OUT R (R-RD))
IN T (R-SD) Sub-loop transmission (R) SD (IN T (R-SD))
IN R (F-RD) Main loop transmission (F) RD (IN R (F-RD))
Control unit
LED1
Control unit
LED1
IN : Connect to OUT on previous station OUT : Connect to IN on next station
(Connection example) Station No.1
OUT IN OUT IN INOUT
Station No.2 Station No.3
18. Machine Support Functions 18.6 External PLC Link
- 254 -
18.6.10 Ethernet I/F (MELSEC Communication Protocol) C6 C64
T system L system M system L system T system
MELSEC communication protocol (hereinafter, MC protocol) is the name of the MELSEC communication method used to read/write the data in the MELSEC CPU. By using this protocol, the sequence programs and data in the C6/C64 can be accessed from an MELSEC peripheral device, etc., connected with Ethernet. In this explanation, the C6/C64 and MELSEC CPU are collectively called the "PLC CPU". On the PLC side, the Ethernet unit sends and receives data based on the instructions from the client device. Thus, a sequence program for exchanging data is not required on the PLC CPU side.
Can be connected to C6, C64, MELSEC 1 or 2.
C6, C64 or MELSEC 2 can be accessed.
C6, MELSEC 1 or 2 can be accessed.
C6, C64 or MELSEC 1 can be accessed.
C64, MELSEC 1 or 2 can be accessed.
GX Developer
MELSEC 2
MELSEC 1
Ethernet
C64
C6
MELSEC NET/10
18. Machine Support Functions 18.7 Installing S/W for Machine Tools
- 255 -
18.7 Installing S/W for Machine Tools Software other than the built-in PLC can be installed in order to implement the machine tool builder's own functions (customized release). The customized release function consists of the following items. (1) Screen release interface function : Change of CNC standard screen, preparation of
inherent screen (2) DDB interface function : Read/write CNC data (3) Machine control interface function : Set/reset PLC device (4) File release interface function : Preparation, modification, registration, etc. of user
files using file system of CNC system
18.7.1 APLC C6 C64
T system L system M system L system T system
The screens are released by pressing the "F0" function key (nothing is displayed on the screen of the NC unit). This enables the machine tool builder to display its own screens from its customized software. Using the APLC libraries, the customized software enables screen displays (characters, graphics), key loading, file read/write, NC unit internal information read/write, and exchanges of R register and other information with PLC ladders. Customized software is described using C language and developed using a commercial compiler.
18.7.6 EZSocket I/F C6 C64
T system L system M system L system T system
This middleware makes it easy to develop applications having a Windows interface. The various functions of the NC unit can be used from a Windows application using VC++ language, VB language and VBA macro language.
Appendix 1. List of Specifications
- 256 -
Appendix 1. List of Specifications
In te
rn al
N C
s ys
te m
fu nc
tio n
N um
er ic
al d
at a
A dd
re ss
es
S ig
n, v
ar ia
bl e
op er
at or
(+ )
S ig
n, v
ar ia
bl e
op er
at or
( )
D ec
im al
p oi
nt
Bl oc
k d ele
te (o
pti on
al blo
ck sk
ip) , v
ar iab
le op
er ato
r ( )
E nd
o f r
ec or
d (ta
pe st
or ag
e en
d) ,
re w
in d
st ar
t & s
to p
du rin
g ta
pe se
ar ch
E nd
o f b
lo ck
C on
tro l o
ut (c
om m
en t s
ta rt)
C on
tro l i
n (c
om m
en t e
nd )
P ro
gr am
n um
be r a
dd re
ss (i
ns te
ad o
f O , I
S O
o nl
y)
V ar
ia bl
e nu
m be
r
V ar
ia bl
e op
er at
or (
)
V ar
ia bl
e de
fin iti
on
V ar
ia bl
e op
er at
or
V ar
ia bl
e op
er at
or
SP s s
tar tin
g w ith
E OB
an d e
nd ing
w he
n f irs
t c ha
ra cte
r o r
nu mb
er co
de ap
pe ar
s a re
no t s
ub jec
t to pa
rity V
co un
t.
IS O
0 ~ 9
A ~ Z + . , / %
LF
( ) : # * = [ ]
SP (T
-V au
tom ati
c ad
jus tm
en t)
Pu nc
h- ou
t o ut
pu t
EI A
0 ~ 9
A ~ Z + . , /
E O
R
E O
B
2+ 4+
5
2+ 4+
7
SP (T
-V au
tom ati
c ad
jus tm
en t)
St or
ed
in
m em
or y
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
S to
re d
N ot
s to
re d
N ot
s to
re d
N ot
s to
re d
S to
re d
Se tti
ng a
nd
di sp
la y
un it
ke y-
in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
N o
ke y-
in
(a uto
ma tic
all y
ins er
ted )
K ey
-in , ;
/E O
B
K ey
-in , ;
/E O
B
K ey
-in , ;
/E O
B
N o
K ey
-in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
K ey
-in
N o
ke y-
in
N o
ke y-
in
K ey
-in
N o
ke y-
in
N o
ke y-
in
N o
ke y-
in
N o
ke y-
in
N o
ke y-
in
C R
T di
sp la
y
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
(% )
D is
pl ay
ed (;
)
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
D is
pl ay
ed
Bl an
k
Bl an
k
Bl an
k
Bl an
k
N ot
d is
pl ay
ed
N ot
d is
pl ay
ed
N ot
d is
pl ay
ed
(N ot
e 3)
Su bj
ec t
to p
ar ity
V
co un
t C
ou nt
ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
C ou
nt ed
N ot
c ou
nt ed
N ot
c ou
nt ed
N ot
c ou
nt ed
C ou
nt ed
C on
tr ol
u ni
t re
co gn
iti on
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
Y es
N o
N o
N o
N o
N o
N o
N o
N o
IS O
0 ~ 9
A ~ Z + . , / %
LF /N
L
( ) : # * = [ ] B S
H T
S P
C R
D E
L
N U
LL
(D E
L)
A ny
o th
er
Fu nc
tio n
co de
EI A
0 ~ 9
A ~ Z + . , /
E O
R
E O
B /C
R
2+ 4+
5
2+ 4+
7
B S
TA B
S P
D E
L
A ll
sp ac
e
A ll
m ar
k
A ny
o th
er
(N ot
e 1)
in
di ca
te s
th at
c or
re sp
on di
ng c
od e
pa tte
rn c
an b
e se
t b y
pa ra
m et
er .
(N ot
e 2)
C od
es n
ot li
st ed
a bo
ve a
re s
to re
d on
ta pe
b ut
a n
er ro
r w ill
re su
lt du
rin g
op er
at io
n if
th ey
a re
n ot
c om
m en
ts .
(N ot
e 3)
T hi
s de
no te
s ch
ar ac
te rs
(i nc
lu di
ng b
la nk
s) w
hi ch
a re
s to
re d
in si
de th
e co
nt ro
lle r a
nd w
hi ch
c or
re sp
on d
to th
e co
m m
an d
co de
s. @
is n
ot d
is pl
ay ed
.
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.1 Outline Drawing of Control Unit
- 257 -
Appendix 2. Outline and Installation Dimension Drawings of Units
Appendix 2.1 Outline Drawing of Control Unit
RI O- M RIO-M/S
30
60
2-M50.8 screw
80 180
Wiring allowance
Top
Bottom
6
15 15
10 10
H ea
t r ad
ia tio
n an
d w
ir in
g al
lo w
an ce
35 0
36 0
H ea
t r ad
ia tio
n al
lo w
an ce
11
38 0
50
D C 2 4 V I N
S E R V O 1
E N C
H A N D L E
S I O
T E R M I N A L
I C C A R D
S K I P
MITSUBISHI
M E L D A S C64
S E R V O 2
Top
Bottom
10 0
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 258 -
Appendix 2.2 Outline Drawing of Communication Terminal Appendix 2.2.1 FCUA-CT100
MITSUBISHI
382(Square hole)9 9
5 130 140
130130
260
8-4hole(For M3 screw) 5
18 0
9 9
250
382 (Square hole dimensions)
1300.2 1300.2 1300.2
18 2
(S qu
ar e
ho le
d im
en si
on s)
19 0
0. 2
8-M3screw
5 5
5 5
18 2(
S qu
ar e
ho le
)
Panel cut drawing
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 259 -
Appendix 2.2.2 FCUA-CR10
250
242 (Square hole dimensions)
1200.21300.2
6-M3 screw
19 0
0. 2
10
18 0
10
MITSUBISHI
242 (Square hole)9
120130
260
6-4 hole(for M3 screw) 5
18 0
9 9
20 0
5 5
5 5
9 18
2 (S
qu ar
e ho
le )
18 2
(S qu
ar e
ho le
d
im en
si on
s)
5
Panel cut drawing
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 260 -
Appendix 2.2.3 FCUA-LD100
MITSUBISHI
382 (Square hole)9 9
5 130 140
130130
260
8-4hole(for M3 screw) 5
5 18
0 10
9 9
19 0
5
10
70
1300.2 1300.2 1300.2
382 (Square hole dimensions) 44 8-M3 screw
4
18 2
(S qu
ar e
ho le
di
m en
si on
s)
4
19 0
0. 2
18 2
(S qu
ar e
ho le
)
Panel cut drawing
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 261 -
Appendix 2.2.4 FCUA-LD10, KB20
MITSUBISHI
120130
260
6-4 hole (for M3 screw) 5
5 18
0
6-M3 screw 248
(square hole dimensions)
1300.2 1200.2
19 0
0. 2
11 4-M3 screw 132 (square hole
dimensions)
1300.2
19 0
0. 2
5 130 140
18 0
5
19 0
20 0
10
5 10
5
30
19 0
20 0
10
5 10
5 70
4-4 hole (for M3 screw)
Panel cut drawing
18 2
(s qu
ar e
ho le
di
m en
si on
s)
4 4
18 2
(s qu
ar e
ho le
di
m en
si on
s)
4 4
11
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 262 -
Appendix 2.2.5 FCU6-DUT32, KB021
140
21 0
Menu keys 270
Escutcheon M3x8 screw
Protective cover
45
(50) 20
20 30
6-4 hole
18 2
0. 3
(S qu
ar e
ho le
d im
en si
on s)
19 0
0. 3
1
Square hole
4
132 (Square hole dimensions)
4- 4 hole
1 1
140(Keyboard outline) 1300.3
5
(9 ) (5 )
9
5 (1)
20 0
0. 3
18 2
(S qu
ar e
ho le
d im
en si
on s)
21 0
(K ey
bo ar
d ou
tli ne
)
21 0
1300.3
248 (Square hole dimensions)
1200.3
4
SFG EDIT MDI
MONI- TOR
TOOL PARAM
DIAGN IN/OUT
CB CAN
FO
9 N G
1 2 3
4 5 6
7 8
/
$
. ,
- +
* DELETE
INS
SHIFT
INPUT CALC
RESET
?
READY
O
Square hole
A
B
C
X U
Y V
Z W
F F
D L
D !
P I
Q J
R K
M (
S )
T [
EOB ]
0 SP
=
#
Panel cut drawing
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.2 Outline Drawing of Communication Terminal
- 263 -
Appendix 2.2.6 Communication Terminal (1) Appearance of CT100/LD100/separate type FCUA-CR10 + KB10, FCUA-EL10 + KB10
RESET
DELET INS
CB CA N
?
SHIFT
INPUT CALC
7 8 A O N
B G C
X U
READY
MONI- TOR
TOOL PARAM
EDIT MDI
DIAGN IN/OUT SFG F0
V W
E L
I
!
J K
( )
Y Z
F D
P Q R
M S T [ ]
EOB = / # *
H
-
+
0
1 2 3
4 5 6
9
SP ,
MITSUBISHI
Setting keys
READY LED
Function selection keys
Alphabetic character, numerical character, and symbol keys
Menu keys
Page keys
Reset key Cursor key
Input key (calculation)
Shif t key
Data correction keys
(Note) To input the alphabetic characters or symbols on the lower of the alphabetic character and symbol keys, press SHIFT key, then press the corresponding key.
(Example) "A" is input by pressing SHIFT , O A .
Appendix 2. Outline and Installation Dimension Drawings of units Appendix 2.3 Outline Drawing of Remote I/O Unit
- 264 -
Appendix 2.3 Outline Drawing of Remote I/O Unit
40
634
DX
2-M5-0.8 screw
70
6
135
16 8
13 5
15 6
6 6
Wiring allowance 15 0
10 0
Bottom
Top
H ea
t di
ss ip
at io
n al
lo w
an ce
H ea
t di
ss ip
at io
n, w
iri ng
a llo
w an
ce
Installation hole
Appendix 3. List of Specifications
- 265 -
Appendix 3. List of Specifications : Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 1 Control axes 1 Control axes 1 Number of basic control axes (NC axes) 1 2 3 2 1 2 Max. number of control axes (NC axes + Spindles +
PLC axes + Auxiliary axes) 7 7 14 14 14
Max. number of axes (NC axes + Spindles + PLC axes) 4 6 14 14 14 Max. number of servo axes (NC axes + PLC axes) 2 4 14 14 14 Max. number of NC axes (in total for all the part systems) 2 4 14 12 14 Max. number of spindles 2 (1)
(Note 1) 2 (1)
(Note 1) 3 4 7 (1) (Note 1)
Max. number of PLC axes 7 7 7 Max. number of auxiliary axes (MR-J2-CT) 5 5 7 7 7 3 Number of simultaneous contouring control axes 2 2 4 4 2 4 Max. number of NC axes in a part system 2 2 6 4 2 2 Control part system 1 Standard number of part systems 1 1 1 1 1 2 Max. number of part systems 2 2 3 3 7 3 Control axes and operation modes 2 Memory mode 3 MDI mode 2 Input command 1 Data increment 1 Data increment and parameter 2 Least input increment 3 Least command increment Least command increment 1m Least command increment 0.1m 4 Least detection increment 2 Unit system 1 Inch/Metric changeover 3 Program format 1 Character code 2 Program format 1 Format 1 for Lathe (G code series 2, 3) 4 Format 1 for Machining center (G code series 1) 4 Command value 1 Decimal point input I, II 2 Absolute/Incremental command 3 Diameter/Radius designation 5 Command value and setting value range 1 Command value and setting value range 3 Positioning/Interpolation 1 Positioning 1 Positioning 2 Unidirectional positioning 2 Linear/Circular interpolation 1 Linear interpolation 2 Circular interpolation (Center/Radius designation) 3 Helical interpolation
(Note 1) Values in parentheses indicate the maximum number of spindles per part system.
Appendix 3. List of Specifications
- 266 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 4 Feed 1 Feedrate 1 Rapid traverse rate (m/min) 1000 1000 1000 1000 1000 2 Cutting feed rate (m/min) 1000 1000 1000 1000 1000 3 Manual feed rate (m/min) 1000 1000 1000 1000 1000 2 Feed rate input methods 1 Feed per minute 2 Feed per revolution 4 F 1-digit feed 3 Overrite 1 Rapid traverse override 2 Cutting feed override 3 2nd cutting feed override 4 Override cancel 4 Acceleration/Deceleration 1 Automatic acceleration/deceleration after interpolation Linear acceleration/deceleration Soft acceleration/deceleration Exponential acceleration/deceleration Exponential acceleration/Linear deceleration 2 Rapid traverse constant inclination acceleration/
deceleration
5 Thread cutting 1 Thread cutting (Lead/Thread number designation) 2 Variable lead thread cutting 3 Synchronous tapping 1 Synchronous tapping cycle 4 Chamfering 6 Manual feed 1 Manual rapid traverse 2 Jog feed 3 Incremental feed 4 Handle feed 7 Dwell 1 Dwell (Time-based designation) 5 Program memory/editing 1 Memory capacity 1 Memory capacity (number of programs stored) 40m (64 programs) 80m (128 programs) 60m (200 programs) 320m (200 programs) 600m (400 programs) 2 Editing method 1 Program editing 2 Background editing
Appendix 3. List of Specifications
- 267 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 6 Operation and display 1 Structure of operation/display panel 7.2-type LCD monochrome display 10.4-type LCD monochrome display 9-type CRT monochrome display External PC display (connecting by Ethernet) Graphic operation terminal (GOT) 2 Operation methods and functions 1 Memory switch (PLC switch) 3 Display methods and contents 1 Status display 2 Position display 3 Program running status display 4 Setting and display 5 MDI data setting and display 7 Clock 8 Hardware/Software configuration display 9 Integrated time display 10 Available languages (Japanese/English) 2
languages 2
languages 2
languages 2
languages 2
languages 11 Additional languages (Japanese, English, Polish) 1 Japanese 2 English 13 Polish 13 Screen deletion 4 Display unit switch 1 Single-NC and multi-display unit switch 2 Multi-NC and common-display unit 4 Multi-NC and common-external PC display 5 Display unit detachable 7 Input/Output functions and devices 1 Input/Output data 1 Machining program input/output 2 Tool offset data input/output 3 Common variable input/output 4 Parameter input/output 5 History data output 2 Input/Output I/F 1 RS-232C I/F 2 IC card I/F 1 I/F for IC card in control unit
Appendix 3. List of Specifications
- 268 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 8 Spindle, Tool and Miscellaneous functions 1 Spindle functions (S) 1 Command/Output 1 Spindle functions 2 Spindle serial I/F 3 Spindle analog I/F 4 Coil change 5 Automatic coil change 2 Speed control 1 Constant surface speed control 2 Spindle override 3 Multiple-spindle control 1 Multiple-spindle control I 3 Position control 1 Spindle orientation 3 Spindle synchronization 1 Spindle synchronization I 2 Spindle synchronization II 2 Tool functions (T) 1 Tool functions 3 Miscellaneous functions (M) 1 Miscellaneous functions 2 Multiple M codes in 1 block 3 M code independent output 4 Miscellaneous function finish 5 M code output during axis positioning 4 2nd miscellaneous function (B) 1 2nd miscellaneous function 9 Tool compensation 1 Tool length/position offset 1 Tool length offset 3 Tool offset for additional axes 2 Tool radius 1 Tool radius compensation 3 Tool nose radius compensation (G40/41/42) 4 Automatic decision of nose radius compensation direction
(G46/40)
3 Tool offset amount 1 Number of tool offset sets 2 40 3 80 4 100 5 200 2 Offset memory 1 Tool shape/wear offset amount
Appendix 3. List of Specifications
- 269 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 10 Coordinate system 1 Coordinate system type and setting 1 Machine coordinate system 2 Coordinate system setting 3 Automatic coordinate system setting 4 Workpiece coordinate system selection (6 sets) 5 Extended workpiece coordinate system selection
(48 sets) G54.1P1 to P48
7 Local coordinate system 8 Coordinate system for rotary axis 9 Plane selection 10 Origin set 11 Counter set 2 Return 1 Manual reference point return 2 Automatic 1st reference point return 3 2nd, 3rd, 4th reference point return 4 Reference point verification 5 Absolute position detection 6 Tool exchange position return 11 Operation support functions 1 Program control 1 Optional block skip 3 Single block 2 Program test 1 Dry run 2 Machine lock 3 Miscellaneous function lock 3 Program search/start/stop 1 Program search 2 Sequence number search 5 Automatic operation start 6 NC reset 7 Feed hold 8 Search & Start 4 Interrupt operation 1 Manual interruption 2 Automatic operation handle interruption 3 Manual absolute mode ON/OFF 4 Thread cutting cycle retract 5 Tapping retract 6 Manual numerical value command 8 MDI interruption 9 Simultaneous operation of manual and automatic
modes
10 Simultaneous operation of JOG and handle modes 11 Reference point retract
Appendix 3. List of Specifications
- 270 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 12 Program support functions 1 Machining method support functions 1 Program 1 Subprogram control 8 layers 8 layers 8 layers 8 layers 8 layers 2 Macro program 1 User macro 4 layers 4 layers 4 layers 4 layers 4 layers 3 Macro interruption 4 Variable command 6 (50+50 number of part systems) sets 7 (100+100 number of part systems) sets 8 (200+100 number of part systems) sets 3 Fixed cycle 1 Fixed cycle for drilling 2 Special fixed cycle 3 Fixed cycle for turning machining 4 Multiple repetitive fixed cycle for turning machining 4 Mirror image 3 G code mirror image 4 Mirror image for facing tool posts 5 Coordinate system operation 1 Coordinate rotation by program 6 Dimension input 1 Corner chamfering/Corner R 3 Geometric command 7 Axis control 5 Circular cutting 8 Multi-part system control 1 Synchronization between part systems 2 Start point designation synchronization 6 Balance cut 8 2-part system synchronous thread cutting 9 Data input by program 1 Parameter input by program 2 Compensation data input by program 10 Machining modal 1 Tapping mode 2 Cutting mode 2 Machining accuracy support functions 1 Automatic corner override 2 Deceleration check 1 Exact stop check mode 2 Exact stop check 3 Error detect 4 Programmable inposition check 3 High-accuracy control (G61.1) 3 Programming support functions 2 Address check 13 Machine accuracy compensation 1 Static accuracy compensation 1 Backlash compensation 2 Memory-type pitch error compensation 3 Memory-type relative position error compensation 4 External machine coordinate system compensation 6 Ball screw thermal expansion compensation 2 Dynamic accuracy compensation 1 Smooth high-gain control (SHG control) 2 Dual feedback 3 Lost motion compensation
Appendix 3. List of Specifications
- 271 -
: Standard : Selection : No specification
: Optional : Special additional specifications C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 14 Automation support functions 1 External data input 1 External search 2 External workpiece coordinate offset 2 Measurement 1 Skip 1 Skip 2 Multiple-step skip 5 Automatic tool length measurement 6 Manual tool length measurement 1 3 Monitoring 1 Tool life management Tool life management II 2 Number of tool life management sets 20/40/80 sets 80 80 100/200 sets 100 100 100 3 Display of integrated time/number of parts 4 Load meter 5 Position switch 16 16 16 16 16 5 Others 1 Programmable current limitation 4 Automatic restart 15 Safety and maintenance 1 Safety switches 1 Emergency stop 2 Data protection key 2 Display for ensuring safety 1 NC warning display 2 NC alarm display 3 Operation stop cause 4 Emergency stop cause 5 Temperature detection 3 Protection 1 Stroke end (Over travel) 2 Stored stroke limit 1 Stored stroke limit I/II 2 Stored stroke limit IB 3 Stored stroke limit IIB 4 Stored stroke limit IC 3 Stroke check before movement 4 Chuck/Tailstock barrier check 5 Interlock 6 External deceleration 8 Door interlock 1 Door interlock I 2 Door interlock II 9 Parameter lock 10 Program protect (Edit lock B, C) 11 Program display lock 4 Maintenance and troubleshooting 1 History diagnosis 2 Setup/Monitor for servo and spindle Monitor Monitor Monitor Monitor Monitor 3 Data sampling 5 Machine operation history monitor 6 NC data backup RS-232C IC card 7 PLC I/F diagnosis
Appendix 3. List of Specifications
- 272 -
: Standard : Selection : No specification : Optional : Special additional specifications
C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 16 Cabinet and installation 1 Cabinet construction 1 Additional H/W I/F 2 slots 2 slots 2 slots 2 slots 2 slots 2 Power supply 1 Power supply specification 24V 24V 24V 24V 24V 3 Control power supply ON/OFF 1 Control power supply ON/OFF 4 Environment 2 Temperature 3 Humidity 4 Vibration 5 Ambient atmosphere 17 Servo/Spindle system 1 Feed axis 1 MDS-C1-V1/C1-V2 (200V) Servo motor: HC -A51/E51 (1000kp/rev) Servo motor: HC -A42/E42 (100kp/rev) 4 MDS-B-SVJ2 (Compact and small capacity) Servo motor: HC -A42/E42 (100kp/rev) Servo motor: HC -A47 (100kp/rev) Servo motor: HC -A33/E33 (25kp/rev) 6 MDS-R-V1/R-V2 (200V Compact and small capacity) Servo motor: HF -A51/E51 (1000kp/rev) Servo motor: HF -A42/E42 (100kp/rev) Servo motor: HF -A47 (100kp/rev) 2 Spindle 1 MDS-C1-SP/C1-SPM/B-SP (200V) Spindle motor: SJ/SJ-V 3 MDS-B-SPJ2 (Compact and small capacity) Spindle motor: SJ-P/SJ-PF 3 Auxiliary axis 1 Index/Positioning servo: MR-J2-CT Servo motor: HC-SF/HC-RF (16kp/rev) Servo motor: HA-FF/HC-MF (8kp/rev) 4 Power supply 1 Power supply: MDS-C1-CV/B-CVE 2 AC reactor for power supply 3 Ground plate 4 Power supply: MDS-A-CR (Resistance regeneration)
Appendix 3. List of Specifications
- 273 -
: Standard : Selection : No specification : Optional : Special additional specifications
C6 C64 for TRF for FTL for FTL for TRF
Pr im
ar y
cl
as s
Se co
nd ar
y
cl as
s
T system L system M system L system T system 18 Machine support functions 1 PLC 1 PLC basic function 1 Built-in PLC basic function 2 Built-in PLC processing mode 2 MELSEC development tool I/F 3 Built-in PLC capacity (Number of steps) 32000 32000 32000 32000 32000 4 Machine contact input/output I/F 6 PLC development 2 MELSEC development tool 7 C language function 12 GOT connection 1 CPU direct connection (RS-422/RS-232C) 2 CC-Link connection (Remote device) 3 CC-Link connection (Intelligent terminal) 5 Ethernet connection 13 PLC message 1 Japanese 2 English 13 Polish 2 Machine construction 1 Servo OFF 2 Axis detach 3 Synchronous control 1 Position tandem 2 Speed tandem 3 Torque tandem 7 Auxiliary axis control (J2-CT) 3 PLC operation 1 Arbitrary feed in manual mode 3 PLC axis control 4 PLC interface 1 CNC control signal 2 CNC status signal 5 DDB 5 Machine contact I/O Standard DI/DO (DI:16/DO:1) Operation board IO DI:32/DO:32 Operation board IO DI:64/DO:48 Remote IO 32/32 Remote IO 64/48 Additional built-in DI/DO (DI:32/DO:32) 6 External PLC link 4 CC-Link 6 DeviceNet (Master/Slave) Master Master Master Master Master 7 MELSEC Q series input/output/intelligent function
unit connection
9 MELSECNET/10 10 Ethernet I/F (MELSEC communication protocol) 7 Installing S/W for machine tools 1 APLC 6 EZSocket I/F
Revision History
Date of revision Manual No. Revision details
Mar. 2002 BNP-B2266A First edition created.
Jul. 2004 BNP-B2266C Due to changes in the List of Specifications (BNP-C3014-003), all items were generally reviewed, and order of listing was changed.
Details were revised to comply with software Version D. Mistakes, etc., were corrected.
Notice
Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible. Please contact your Mitsubishi Electric dealer with any questions or comments regarding the use of this product.
Duplication Prohibited This manual may not be reproduced in any form, in part or in whole, without written permission from Mitsubishi Electric Corporation.
2002-2004 MITSUBISHI ELECTRIC CORPORATION ALL RIGHTS RESERVED.
Related manuals for Mitsubishi C6 Numerical Control Specification Manual
en
Manualsnet FAQs
If you want to find out how the C6 Mitsubishi works, you can view and download the Mitsubishi C6 Numerical Control Specification Manual on the Manualsnet website.
Yes, we have the Specification Manual for Mitsubishi C6 as well as other Mitsubishi manuals. All you need to do is to use our search bar and find the user manual that you are looking for.
The Specification Manual should include all the details that are needed to use a Mitsubishi C6. Full manuals and user guide PDFs can be downloaded from Manualsnet.com.
The best way to navigate the Mitsubishi C6 Numerical Control Specification Manual is by checking the Table of Contents at the top of the page where available. This allows you to navigate a manual by jumping to the section you are looking for.
This Mitsubishi C6 Numerical Control Specification Manual consists of sections like Table of Contents, to name a few. For easier navigation, use the Table of Contents in the upper left corner.
You can download Mitsubishi C6 Numerical Control Specification Manual free of charge simply by clicking the “download” button in the upper right corner of any manuals page. This feature allows you to download any manual in a couple of seconds and is generally in PDF format. You can also save a manual for later by adding it to your saved documents in the user profile.
To be able to print Mitsubishi C6 Numerical Control Specification Manual, simply download the document to your computer. Once downloaded, open the PDF file and print the Mitsubishi C6 Numerical Control Specification Manual as you would any other document. This can usually be achieved by clicking on “File” and then “Print” from the menu bar.