Advertisement
Advertisement
MELSEC is the registered trademark of Mitsubishi Electric Corporation.
Microsoft and Windows are the registered trademarks of Microsoft Corporation in the United States and/or other countries.
Other company and product names herein may be the trademarks or registered trademarks of their respective owners.
Introduction
This manual describes the specifications of EZMotion-NC E60/E68 series.
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
: Additional hardware is required separately.
: 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.
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............................................................... 3
1.1.4 Max. Number of NC Axes in a Part System .......................................................................... 3
1.2 Control Part System........................................................................................................................ 3
1.2.1 Standard Number of Part Systems ........................................................................................ 3
1.2.2 Max. Number of Part Systems............................................................................................... 3
1.3 Control Axes and Operation Modes ............................................................................................... 4
1.3.1 Tape (RS-232C Input) Mode ................................................................................................. 4
1.3.2 Memory .................................................................................................................................. 4
1.3.3 MDI......................................................................................................................................... 4
1.3.5 IC Card Mode......................................................................................................................... 4
1.3.5.2 Front IC Card Operation............................................................................................ 4
2. Input Command .................................................................................................................................... 5
2.1 Data Increment ............................................................................................................................... 5
2.2 Unit System..................................................................................................................................... 6
2.2.1 Inch/Metric Changeover......................................................................................................... 6
2.3 Program Format.............................................................................................................................. 7
2.3.1 Character Code...................................................................................................................... 7
2.3.2 Program Format ..................................................................................................................... 8
2.3.2.1 Format 1 for Lathe..................................................................................................... 8
2.3.2.3 Special Format for Lathe........................................................................................... 8
2.3.2.4 Format 1 for Machining Center ................................................................................. 8
2.4 Command Value ............................................................................................................................. 9
2.4.1 Decimal Point Input I, II .......................................................................................................... 9
2.4.2 Absolute / Incremental Command ....................................................................................... 10
2.4.3 Diameter/Radius Designation .............................................................................................. 12
2.5 Command Value and Setting Value Range ................................................................................. 13
2.5.1 Command Value and Setting Value Range......................................................................... 13
3. Positioning / Interpolation ................................................................................................................. 17
3.1 Positioning..................................................................................................................................... 17
3.1.1 Positioning............................................................................................................................ 17
3.1.2 Unidirectional Positioning..................................................................................................... 18
3.2 Linear / Circular Interpolation........................................................................................................ 19
3.2.1 Linear Interpolation .............................................................................................................. 19
3.2.2 Circular Interpolation (Center / Radius Designation)........................................................... 20
3.2.3 Helical Interpolation.............................................................................................................. 22
3.2.5 Cylindrical Interpolation........................................................................................................ 24
3.2.6 Polar Coordinate Interpolation ............................................................................................. 25
4. Feed...................................................................................................................................................... 26
4.1 Feed Rate ..................................................................................................................................... 26
4.1.1 Rapid Traverse Rate (m/min) ..............................................................................................26
4.1.2 Cutting Feed Rate (m/min)................................................................................................... 27
4.1.3 Manual Feed Rate (m/min) .................................................................................................. 28
4.2 Feed Rate Input Methods ............................................................................................................. 29
4.2.1 Feed per Minute ................................................................................................................... 29
4.2.2 Feed per Revolution............................................................................................................. 31
4.2.4 F1-Digit Feed ....................................................................................................................... 33
4.3 Override ........................................................................................................................................ 34
4.3.1 Rapid Traverse Override...................................................................................................... 34
4.3.2 Cutting Feed Override.......................................................................................................... 34
4.3.3 2nd Cutting Feed Override................................................................................................... 34
4.3.4 Override Cancel ................................................................................................................... 35
4.4 Acceleration / Deceleration........................................................................................................... 36
4.4.1 Automatic Acceleration / Deceleration after Interpolation ................................................... 36
4.4.2 Rapid Traverse Constant Inclination Acceleration / Deceleration....................................... 37
4.5 Thread Cutting .............................................................................................................................. 40
4.5.1 Thread Cutting (Lead/Thread Number Designation)........................................................... 40
4.5.2 Variable Lead Thread Cutting.............................................................................................. 43
4.5.3 Synchronous Tapping .......................................................................................................... 44
4.5.3.1 Synchronous Tapping Cycle ................................................................................... 44
4.5.3.2 Pecking Tapping Cycle ........................................................................................... 46
4.5.3.3 Deep-hole Tapping Cycle........................................................................................ 48
4.5.4 Chamfering........................................................................................................................... 50
4.6 Manual Feed ................................................................................................................................. 51
4.6.1 Manual Rapid Traverse........................................................................................................ 51
4.6.2 Jog Feed .............................................................................................................................. 51
4.6.3 Incremental Feed ................................................................................................................. 52
4.6.4 Handle Feed......................................................................................................................... 52
4.6.5 Manual Feed Rate B ............................................................................................................ 53
4.7 Dwell ............................................................................................................................................. 54
4.7.1 Dwell (Time-based Designation).......................................................................................... 54
5. Program Memory / Editing................................................................................................................. 55
5.1 Memory Capacity .......................................................................................................................... 55
5.1.1 Memory Capacity (Number of Programs Stored) ................................................................ 55
5.2 Editing ........................................................................................................................................... 55
5.2.1 Program Editing ................................................................................................................... 55
5.2.2 Background Editing.............................................................................................................. 56
5.2.3 Buffer Correction .................................................................................................................. 57
5.2.4 Word Editing......................................................................................................................... 58
6. Operation and Display........................................................................................................................ 59
6.1 Structure of Operation / Display Panel ......................................................................................... 59
6.2 Operation Methods and Functions ............................................................................................... 59
6.2.1 Memory Switch (PLC switch)............................................................................................... 59
6.3 Display Methods and Contents..................................................................................................... 60
6.3.1 Status Display ...................................................................................................................... 60
6.3.2 Position Display.................................................................................................................... 61
6.3.3 Program Running Status display ......................................................................................... 62
6.3.4 Setting and Display .............................................................................................................. 62
6.3.5 MDI Data Setting and Display.............................................................................................. 62
6.3.7 Clock .................................................................................................................................... 62
6.3.8 Hardware / Software Configuration Display......................................................................... 62
6.3.9 Integrated Time Display ....................................................................................................... 63
6.3.10 Standard Language ........................................................................................................... 63
6.3.11 Additional Languages ........................................................................................................ 63
6.3.12 Screen Saver, Backlight OFF ............................................................................................ 65
6.3.13 Screen Deletion.................................................................................................................. 65
7. Input / Output Functions and Devices ............................................................................................. 66
7.1 Input / Output Data........................................................................................................................ 66
7.2 Input / Output I/F ........................................................................................................................... 67
7.2.1 RS-232C I/F ......................................................................................................................... 67
7.2.2 IC Card I/F............................................................................................................................ 67
7.2.2.2 I/F for Front IC Card ................................................................................................ 67
7.3 Computer Link............................................................................................................................... 68
7.3.1 Computer Link B .................................................................................................................. 68
8. Spindle, Tool and Miscellaneous Functions ...................................................................................69
8.1 Spindle Functions (S) ................................................................................................................... 69
8.1.1 Command / Output............................................................................................................... 69
8.1.1.1 Spindle Functions.................................................................................................... 69
8.1.1.2 Spindle Serial I/F ..................................................................................................... 70
8.1.1.3 Spindle Analog I/F ................................................................................................... 70
8.1.1.4 Coil Change............................................................................................................. 70
8.1.1.5 Automatic Coil Change ........................................................................................... 70
8.1.2 Speed Control ...................................................................................................................... 71
8.1.2.1 Constant Surface Speed Control ............................................................................ 71
8.1.2.2 Spindle Override...................................................................................................... 71
8.1.2.3 Multiple-spindle Control........................................................................................... 72
8.1.2.3.1 Multiple-spindle Control I ......................................................................... 73
8.1.2.3.2 Multiple-spindle Control II ........................................................................ 73
8.1.3 Position Control.................................................................................................................... 74
8.1.3.1 Spindle Orientation.................................................................................................. 74
8.1.3.2 Spindle Position Control (Spindle / C Axis Control) ................................................ 74
8.1.3.3 Spindle Synchronization.......................................................................................... 75
8.1.3.3.1 Spindle Synchronization I ........................................................................ 75
8.1.3.3.2 Spindle Synchronization II ....................................................................... 76
8.1.3.11 Spindle Holding Power Improvement ................................................................... 76
8.2 Tool Functions (T)......................................................................................................................... 77
8.2.1 Tool Functions...................................................................................................................... 77
8.3 Miscellaneous Functions (M)........................................................................................................ 78
8.3.1 Miscellaneous Functions...................................................................................................... 78
8.3.2 Multiple M Codes in 1 Block................................................................................................. 78
8.3.3 M Code Independent Output ............................................................................................... 79
8.3.4 Miscellaneous Function Finish............................................................................................. 79
8.4 2nd Miscellaneous Functions (B) ................................................................................................. 80
8.4.1 2nd Miscellaneous Functions .............................................................................................. 80
9. Tool Compensation ............................................................................................................................ 81
9.1 Tool Length / Position Offset ........................................................................................................ 81
9.1.1 Tool Length Offset................................................................................................................ 81
9.1.2 Tool Position Offset.............................................................................................................. 84
9.1.3 Tool Offset for Additional Axes ............................................................................................ 84
9.2 Tool Radius................................................................................................................................... 85
9.2.1 Tool Radius Compensation .................................................................................................85
9.2.3 Tool Nose Radius Compensation (G40/41/42) ................................................................... 88
9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40)............................. 89
9.3 Tool Offset Amount ....................................................................................................................... 90
9.3.1 Number of Tool Offset Sets ................................................................................................. 90
9.3.2 Offset Memory...................................................................................................................... 91
9.3.2.1 Tool Shape/Wear Offset Amount ............................................................................ 91
10. Coordinate System ........................................................................................................................... 94
10.1 Coordinate System Type and Setting......................................................................................... 94
10.1.1 Machine Coordinate System.............................................................................................. 95
10.1.2 Coordinate System Setting ................................................................................................ 96
10.1.3 Automatic Coordinate System Setting............................................................................... 97
10.1.4 Workpiece Coordinate System Selection (6 sets) ............................................................. 98
10.1.5 Extended workpiece coordinate system selection (48 sets) G54.1P1 to P48 .................. 99
10.1.6 Workpiece Coordinate System Preset (G92.1) ............................................................... 100
10.1.7 Local Coordinate System.................................................................................................101
10.1.8 Coordinate System for Rotary Axis.................................................................................. 102
10.1.9 Plane Selection ................................................................................................................ 103
10.1.10 Origin Set ....................................................................................................................... 104
10.1.11 Counter Set .................................................................................................................... 104
10.2 Return ....................................................................................................................................... 105
10.2.1 Manual Reference Position Return.................................................................................. 105
10.2.2 Automatic 1st Reference Position Return........................................................................ 106
10.2.3 2nd, 3rd, 4th Reference Position Return ......................................................................... 108
10.2.4 Reference Position Verification........................................................................................ 109
10.2.5 Absolute Position Detection.............................................................................................110
10.2.6 Tool Exchange Position Return ....................................................................................... 111
10.2.7 C Axis Reference Position Return ................................................................................... 112
11. Operation Support Functions ....................................................................................................... 114
11.1 Program Control........................................................................................................................ 114
11.1.1 Optional Block Skip.......................................................................................................... 114
11.1.3 Single Block ..................................................................................................................... 115
11.2 Program Test ............................................................................................................................ 116
11.2.1 Dry Run ............................................................................................................................ 116
11.2.2 Machine Lock ................................................................................................................... 116
11.2.3 Miscellaneous Function Lock........................................................................................... 117
11.2.4 Graphic Check ................................................................................................................. 117
11.2.5 Graphic Trace .................................................................................................................. 117
11.3 Program Search / Start / Stop .................................................................................................. 118
11.3.1 Program Search ............................................................................................................... 118
11.3.2 Sequence Number Search .............................................................................................. 118
11.3.3 Collation Stop................................................................................................................... 119
11.3.4 Program Restart............................................................................................................... 120
11.3.5 Automatic Operation Start................................................................................................ 121
11.3.6 NC Reset.......................................................................................................................... 121
11.3.7 Feed Hold......................................................................................................................... 122
11.3.8 Search & Start.................................................................................................................. 122
11.4 Interrupt Operation.................................................................................................................... 123
11.4.1 Manual Interruption .......................................................................................................... 123
11.4.2 Automatic Operation Handle Interruption ........................................................................ 124
11.4.3 Manual Absolute Mode ON / OFF ................................................................................... 125
11.4.4 Thread Cutting Cycle Retract .......................................................................................... 126
11.4.5 Tapping Retract................................................................................................................ 127
11.4.6 Manual Numerical value Command ................................................................................ 128
11.4.8 MDI Interruption ............................................................................................................... 128
11.4.9 Simultaneous Operation of Manual and Automatic Modes............................................. 129
11.4.10 Simultaneous Operation of Jog and Handle Modes...................................................... 129
11.4.11 Reference Position Retract............................................................................................ 130
11.4.14 PLC Interruption ............................................................................................................. 130
12. Programming Support Functions................................................................................................. 131
12.1 Machining Method Support Functions...................................................................................... 131
12.1.1 Program............................................................................................................................ 131
12.1.1.1 Subprogram Control ............................................................................................ 131
12.1.1.3 Scaling................................................................................................................. 133
12.1.2 Macro Program ................................................................................................................ 134
12.1.2.1 User Macro .......................................................................................................... 134
12.1.2.2 Machine Tool Builder Macro ............................................................................... 136
12.1.2.2.1 Machine Tool Builder Macro SRAM................................................................. 136
12.1.2.3 Macro Interruption ............................................................................................... 137
12.1.2.4 Variable Command ............................................................................................. 138
12.1.3 Fixed Cycle ...................................................................................................................... 139
12.1.3.1 Fixed Cycle for Drilling ........................................................................................ 140
12.1.3.2 Special Fixed Cycle............................................................................................. 147
12.1.3.3 Fixed Cycle for Turning Machining ..................................................................... 151
12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining....................................... 156
12.1.3.5 Multiple Repetitive Fixed Cycle for Turning Machining (Type II) ........................ 164
12.1.3.7 Fixed Cycle for Drilling (Type II).......................................................................... 165
12.1.4 Mirror Image..................................................................................................................... 166
12.1.4.1 Mirror Image by Parameter Setting..................................................................... 166
12.1.4.2 External Input Mirror Image................................................................................. 166
12.1.4.3 G Code Mirror Image........................................................................................... 167
12.1.5 Coordinate System Operation ......................................................................................... 168
12.1.5.1 Coordinate Rotation by Program ........................................................................ 168
12.1.6 Dimension Input ............................................................................................................... 170
12.1.6.1 Corner Chamfering / Corner R............................................................................ 170
12.1.6.2 Linear Angle Command ...................................................................................... 176
12.1.6.3 Geometric Command .......................................................................................... 177
12.1.6.4 Polar Coordinate Command ............................................................................... 181
12.1.7 Axis Control...................................................................................................................... 182
12.1.7.1 High-speed Machining ........................................................................................ 182
12.1.7.1.3 High-speed Machining Mode III........................................................... 182
12.1.7.2 Chopping ............................................................................................................. 183
12.1.7.2.1 Chopping.............................................................................................. 183
12.1.7.5 Circular Cutting.................................................................................................... 185
12.1.9 Data Input by Program..................................................................................................... 186
12.1.9.1 Parameter Input by Program............................................................................... 186
12.1.9.2 Compensation Data Input by Program ............................................................... 187
12.1.10 Machining Modal............................................................................................................ 189
12.1.10.1 Tapping Mode ................................................................................................... 189
12.1.10.2 Cutting Mode ..................................................................................................... 189
12.2 Machining Accuracy Support Functions ................................................................................... 190
12.2.1 Automatic Corner Override .............................................................................................. 190
12.2.2 Deceleration Check.......................................................................................................... 191
12.2.2.1 Exact Stop Mode ................................................................................................. 192
12.2.2.2 Exact Stop Check................................................................................................ 192
12.2.2.3 Error Detect ......................................................................................................... 192
12.2.2.4 Programmable In-position Check........................................................................ 193
12.2.3 High-Accuracy Control ..................................................................................................... 194
12.2.3.1 High-accuracy Control (G61.1/G08P1)............................................................... 194
12.3 Programming Support Functions.............................................................................................. 199
12.3.1 Playback........................................................................................................................... 199
12.3.2 Address Check................................................................................................................. 199
13. Machine Accuracy Compensation................................................................................................ 200
13.1 Static Accuracy Compensation................................................................................................. 200
13.1.1 Backlash Compensation .................................................................................................. 200
13.1.2 Memory-type Pitch Error Compensation ......................................................................... 201
13.1.3 Memory-type Relative Position Error Compensation ...................................................... 202
13.1.4 External Machine Coordinate System Compensation..................................................... 202
13.1.9 Spindle Backlash Compensation..................................................................................... 203
13.2 Dynamic Accuracy Compensation ........................................................................................... 205
13.2.1 Smooth High-gain Control (SHG Control) ....................................................................... 205
13.2.2 Dual Feedback ................................................................................................................. 206
13.2.3 Lost Motion Compensation .............................................................................................. 206
14. Automation Support Functions .................................................................................................... 207
14.1 External Data Input ................................................................................................................... 207
14.1.1 External Search................................................................................................................ 207
14.1.2 External Workpiece Coordinate Offset ............................................................................ 208
14.1.3 External Tool Offset ......................................................................................................... 209
14.2 Measurement ............................................................................................................................ 210
14.2.1 Skip .................................................................................................................................. 210
14.2.1.1 Skip...................................................................................................................... 210
14.2.1.2 Multiple-step Skip ................................................................................................ 211
14.2.1.4 PLC Skip..............................................................................................................212
14.2.5 Automatic Tool Length Measurement.............................................................................. 213
14.2.6 Manual Tool Length Measurement 1............................................................................... 216
14.2.7 Manual Tool Length Measurement 2............................................................................... 217
14.2.8 Workpiece Coordinate Offset measurement ................................................................... 218
14.2.9 Workpiece Position Measurement................................................................................... 219
14.3 Monitoring ................................................................................................................................. 221
14.3.1 Tool Life Management ..................................................................................................... 221
14.3.1.1 Tool Life Management I ...................................................................................... 221
14.3.1.2 Tool Life Management II ..................................................................................... 221
14.3.2 Number of Tool Life Management Sets........................................................................... 222
14.3.3 Number of Parts ............................................................................................................... 222
14.3.4 Load Meter ....................................................................................................................... 223
14.3.5 Position Switch................................................................................................................. 223
14.3.12 Synchronous Error Observation .................................................................................... 223
14.5 Others ....................................................................................................................................... 224
14.5.1 Programmable Current Limitation.................................................................................... 224
15. Safety and Maintenance................................................................................................................. 225
15.1 Safety Switches ........................................................................................................................ 225
15.1.1 Emergency Stop .............................................................................................................. 225
15.1.2 Data Protection Key ......................................................................................................... 225
15.2 Display for Ensuring Safety ...................................................................................................... 226
15.2.1 NC Warning...................................................................................................................... 226
15.2.2 NC Alarm.......................................................................................................................... 226
15.2.3 Operation Stop Cause ..................................................................................................... 227
15.2.4 Emergency Stop Cause................................................................................................... 227
15.2.5 Temperature Detection .................................................................................................... 227
15.3 Protection .................................................................................................................................. 228
15.3.1 Stroke End (Over travel) .................................................................................................. 228
15.3.2 Stored Stroke Limit........................................................................................................... 228
15.3.2.1 Stored Stroke Limit I/II......................................................................................... 229
15.3.2.2 Stored Stroke Limit IB ......................................................................................... 231
15.3.2.3 Stored Stroke Limit IIB ........................................................................................ 232
15.3.2.4 Stored Stroke Limit IC ......................................................................................... 232
15.3.4 Chuck/Tailstock Barrier Check ........................................................................................ 233
15.3.5 Interlock............................................................................................................................ 234
15.3.6 External Deceleration....................................................................................................... 234
15.3.8 Door Interlock................................................................................................................... 235
15.3.8.1 Door Interlock I .................................................................................................... 235
15.3.8.2 Door Interlock II ................................................................................................... 236
15.3.9 Parameter Lock................................................................................................................ 237
15.3.10 Program Protect (Edit Lock B, C) .................................................................................. 237
15.3.11 Program Display Lock.................................................................................................... 238
15.4 Maintenance and Troubleshooting ...........................................................................................239
15.4.1 History Diagnosis ............................................................................................................. 239
15.4.2 Setup / Monitor for Servo and Spindle............................................................................. 239
15.4.3 Data Sampling.................................................................................................................. 239
15.4.4 Waveform Display............................................................................................................ 240
15.4.5 Machine Operation History Monitor ................................................................................. 240
15.4.6 NC Data Backup .............................................................................................................. 241
15.4.7 PLC I/F Diagnosis ............................................................................................................ 242
15.4.13 Signal Trace Function .................................................................................................... 242
16. Cabinet and Installation ................................................................................................................. 243
16.1 Cabinet Construction ................................................................................................................ 243
16.2 Power Supply............................................................................................................................ 248
17. Servo / Spindle System.................................................................................................................. 252
17.1 Feed Axis .................................................................................................................................. 252
17.1.1 MDS-C1-V1/C1-V2 (200V) .............................................................................................. 252
17.1.3 MDS-CH-V1/CH-V2 (400V) ............................................................................................. 252
17.1.4 MDS-B-SVJ2 (Compact and small capacity)................................................................... 253
17.1.6 MDS-R-V1/R-V2 (200V Compact and small capacity).................................................... 253
17.2 Spindle ...................................................................................................................................... 254
17.2.1 MDS-C1-SP/C1-SPH/C1-SPM/B-SP (200V)................................................................... 254
17.2.2 MDS-CH-SP/CH-SPH (400V).......................................................................................... 254
17.2.3 MDS-B-SPJ2 (Compact and small capacity)................................................................... 254
17.3 Auxiliary Axis............................................................................................................................. 255
17.3.1 Index/Positioning Servo: MR-J2-CT ................................................................................ 255
17.4 Power Supply............................................................................................................................ 255
17.4.1 Power Supply: MDS-C1-CV/B-CVE ................................................................................ 255
17.4.2 AC Reactor for Power Supply.......................................................................................... 255
17.4.3 Ground Plate .................................................................................................................... 255
18. Machine Support Functions .......................................................................................................... 256
18.1 PLC ........................................................................................................................................... 256
18.1.1 PLC Basic Function ......................................................................................................... 256
18.1.1.1 Built-in PLC Basic Function................................................................................. 256
18.1.2 Built-in PLC Processing Mode ......................................................................................... 260
18.1.2.2 MELSEC Development Tool I/F.......................................................................... 260
18.1.3 Built-in PLC Capacity (Number of steps)......................................................................... 261
18.1.4 Machine Contact Input/Output I/F.................................................................................... 261
18.1.5 Ladder Monitor ................................................................................................................. 268
18.1.6 PLC Development............................................................................................................ 268
18.1.6.1 On-board Development....................................................................................... 268
18.1.6.2 MELSEC Development Tool ............................................................................... 268
18.1.9 PLC Password Lock......................................................................................................... 269
18.1.13 PLC Message ................................................................................................................ 270
18.1.14 User PLC version up...................................................................................................... 271
18.2 Machine Construction ............................................................................................................... 272
18.2.1 Servo OFF........................................................................................................................ 272
18.2.2 Axis Detach ...................................................................................................................... 273
18.2.4 Inclined Axis Control ........................................................................................................ 274
18.2.5 Index Table Indexing........................................................................................................ 275
18.2.6 NSK Table Connection Control........................................................................................ 276
18.2.7 Auxiliary Axis Control (J2-CT)..........................................................................................277
18.3 PLC Operation .......................................................................................................................... 278
18.3.1 Arbitrary Feed In Manual Mode ....................................................................................... 278
18.3.3 PLC Axis Control.............................................................................................................. 279
18.4 PLC Interface ............................................................................................................................ 281
18.4.1 CNC Control Signal.......................................................................................................... 281
18.4.2 CNC Status Signal ........................................................................................................... 282
18.4.5 DDB.................................................................................................................................. 284
18.5 Machine Contact I / O ............................................................................................................... 285
18.7 Installing S/W for Machine Tools .............................................................................................. 287
18.7.3 Simple Customization ...................................................................................................... 287
Appendix 1 List of Specifications....................................................................................................... 288
Appendix 2. Format Details ................................................................................................................. 289
Appendix 3. Outline and Installation Dimension Drawings of Units .............................................. 291
Appendix 3.1 E60 Control Unit, Display Unit, Keyboard Unit Outline Drawing................................ 291
Appendix 3.1.1 Control unit, display unit (FCU6-MU071, FCU6-DUN26) outline drawing ........ 291
Appendix 3.1.2 Keyboard unit (FCU6-KB024) outline drawing .................................................. 292
Appendix 3.1.3 Control unit (FCU6-MU071, FCU6-KB071) outline drawing ............................. 293
Appendix 3.1.4 Display unit (FCU6-DUE71) outline drawing..................................................... 295
Appendix 3.1.5 Display unit (FCU6-DUT11) outline drawing ..................................................... 297
Appendix 3.2 E68 Control Unit, Display Unit, Keyboard Unit Outline Drawing................................ 299
Appendix 3.2.1 Control unit, display unit (FCU6-MU072,FCU6-DUN24) outline drawing ......... 299
Appendix 3.2.2 Keyboard unit (FCU6-KB024) outline drawing .................................................. 300
Appendix 3.2.3 Front IC card I/F unit (FCU6-EP105-1) outline drawing.................................... 301
Appendix 3.3 External Power Supply Unit (PD25) Outline Drawing ................................................ 302
Appendix 3.4 Base I/O Unit Outline Drawing ................................................................................... 303
Appendix 3.4.1 FCU6-HR341/HR351 outline drawing ............................................................... 303
Appendix 3.4.2 FCU6-DX220/DX221 outline drawing................................................................ 303
Appendix 3.5 Remote I/O Unit (FCUA-DX1xx) Outline Drawing...................................................... 304
EZMotion-NC E60/E68 Series Specifications List
1. Control Axes
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)
M system
L system
E60 E68
{3
{2
{3
{2
1.1.2 Max. Number of Control Axes (NC axes + Spindles + PLC axes + Auxiliary axes)
M system
E60 E68
5 8
L system 5 8
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.
Connection specifications of NC axis, PLC axis, spindle and auxiliary axis
There are two channels with which the servo and spindle are connected.
Maximum 5 axes (for E60) or 6 axes (for E68) can be connected with the channel 1.
NC axis, PLC axis, spindle : They can be connected with the channel 1. Connection Nos. for the 1st to 5th axis (for E60) or 1st to 6th axis (for E68) are assigned to each channel. Connect them from the first axis in order. More than one axis must be connected with the channel 1.
Auxiliary axis (J2CT) : They can be connected with the channel 2.
- 1 -
1. Control Axes
Max. number of axes (NC axes + spindles + PLC axes)
E60 E68
M system 5 6
L system 5 6
Max. number of servo axes (NC axes + PLC axes)
E60 E68
M system 4 6
L system 4 6
Max. number of NC axes (in total for all the part systems)
E60 E68
M system 3 4
L system 3 4
Max. number of spindles
Includes analog spindles.
E60 E68
M system
L system
Max. number of PLC axes
1
1
2
2
E60 E68
M system
L system
1
1
2
2
Max. number of auxiliary axes (MR-J2-CT)
E60 E68
M system
L system
1
1
4
4
- 2 -
1. Control Axes
1.1.3 Number of Simultaneous Contouring Control Axes
M system
L system
E60 E68
3 4
3 4
1.1.4 Max. Number of NC Axes in a Part System
M system
L system
1.2 Control Part System
E60 E68
3 4
3 4
1.2.1 Standard Number of Part Systems
M system
L system
1.2.2 Max. Number of Part Systems
E60 E68
1
1
1
1
M system
E60 E68
{1 {1
L system
{1 {1
For actual use, the machine maker specification will apply.
- 3 -
1. Control Axes
1.3 Control Axes and Operation Modes
1.3 Control Axes and Operation Modes
1.3.1 Tape (RS-232C Input) Mode
M system
E60 E68
{ {
{ {
L system
In this mode, operation is performed using the machining program data from the RS-232C interface built in the NC unit. A paper tape reader must be provided if machining programs on paper tape are to be run.
1.3.2 Memory
M system
L system
E60 E68
{ {
{ {
The machining programs stored in the memory of the NC unit are run.
1.3.3 MDI
M system
L system
E60 E68
{ {
{ {
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.
1.3.5 IC Card Mode
1.3.5.2 Front IC Card Operation
M system
E60 E68
–
{
L system – –
The IC card operation function enables a machining program registered in the IC card to be called and operated. With IC card, machining program can be edited on PC.
During IC card operation, a machining program in the NC memory can be called as the subprogram by M98 command. Also, a machining program in the IC card can be called from the main program in the memory as the sub-program by M198 command and operated.
It is recommended to use the SanDisk CF card.
(Note) When inserting/removing a commercially available CF card, preferably, turn the
MITSUBISHI device's power OFF to avoid any troubles. When inserting/removing a card while the power is ON, make sure to have sufficient time (approx. ten seconds or more) in between.
- 4 -
2. Input Command
2.1 Data Increment
Least command increment: 1
μm
E60 E68
M system
L system
{
{
{
{
Least command increment: 0.1
μm
M system
L system
E60 E68
–
{
–
{
The data increment handled in the controller include the least setting increment, least command increment and least detection increment. Each type is set with parameters.
(1) The least setting 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.
(2) The least command increment indicates the command increment of the movement command in the machining program. This can be set per axis.
(a) For E60
Increment type
Least command increment
Metric unit system
Type
Linear axis Rotary axis
(Unit = mm) (Unit =
°
)
B 0.001 0.001
Inch unit system
Linear axis
(Unit = inch)
Rotary axis
(Unit =
°
)
0.0001 0.001
(b) For E68
Increment type
Least command increment
Metric unit system
Type
Linear axis
(Unit = mm)
Rotary axis
(Unit =
°
)
B 0.001 0.001
Inch unit system
Linear axis
(Unit = inch)
0.0001
Rotary axis
(Unit =
0.001
°
)
(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.
(4) If the least command increment is 0.1
μm/0.01μm, the movement amount, movement range and command speed may be limited compared to the 1
μm.
- 5 -
2.2 Unit System
2.2.1 Inch/Metric Changeover
M system
E60 E68
{ {
{ {
L 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
Inch unit system
1.0
1.0
1.0 mm
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
I_inch
0
1
G20 Inch unit system
G21 Metric unit system
G20 Inch unit system
G21 Metric unit system
Metric unit system
Inch unit system
Not affected
M_inch
0
1
Not affected Not affected
Metric unit system
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.
- 6 -
2.3 Program Format
2.3.1 Character Code
M system
E60 E68
{ {
{ {
L 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
;
<
>
?
BS
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) .
& 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) .
- 7 -
2.3.2 Program Format
2.3.2.1 Format 1 for Lathe
E60 E68
M system
L 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.
2.3.2.3 Special Format for Lathe
M system
L system
E60 E68
–
{
–
{
2.3.2.4 Format 1 for Machining Center
M system
L system
E60 E68
{ {
– –
- 8 -
2.4 Command Value
2.4.1 Decimal Point Input I, II
M system
E60 E68
{ {
{ {
L 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 unit.
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 II
G00 X100. Y-200.5
G1 X100 F20.
Y200 F100
G4 X1.5
(*1)
X100mm, Y-200.5mm
←
X100µm, F20mm/min X100mm, F20mm/min
Y200µm, F100mm/min Y200mm, F100mm/min
Dwell 1.5 s
←
X2 2ms 2s
(*1) The F unit is mm/min for either type (inch system : inch/min).
- 9 -
2.4.2 Absolute / Incremental Command
M system
L system
(1) M system
E60 E68
{
{
{
{
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)
G 91 X 100. Y100. ;
(Absolute value command)
G 90 X 100. Y100. ;
End point
Y100.
Y100.
End point
Y100.
Current position
X 100.
(0, 0)
X 100.
Current position
Program coordinate
(0, 0)
X100.
- 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
;
(Incremental value command)
G 00 U
–
u1 W
–
w1 ;
X
Current position
(Absolute value command)
G 00 X x1 Z z1 ;
X
Current position
End point u1
2 x1
Z
End point w1 z1
Z
(0,0)
The above drawing shows the case for the diameter command.
The above drawing shows the case for the diameter command.
(Note) In addition to the above command method using axis addresses, to switch the absolute value command/incremental value command, the command method using G90/91 can also be selected using a parameter.
- 11 -
2.4.3 Diameter/Radius Designation
E60 E68
M system
L system
–
{
–
{
For 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 work 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.
X-axis radius designation
X-axis diameter designation
X X u4 x6 u4 x6
Z Z
Coordinate zero point
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
- 12 -
2.5 Command Value and Setting Value Range
2.5 Command Value and Setting Value Range
2.5.1 Command Value and Setting Value Range
M system
L system
E60 E68
{ {
{ {
<Brief summary of format details>
Program number
Sequence number
Preparatory function
Movement axis
0.001(°) mm/
0.0001 inch
Arc and cutter radius
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
Dwell
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
Metric command
08
N5
G3/G21
Inch command
←
←
←
M system
Rotary axis
(Metric command)
←
←
←
Rotary axis
(Inch command)
←
←
←
X+53 Y+53 Z+53
α+53
X+44 Y+44 Z+44
α+44
X+53 Y+53 Z+53
α+53
X+53 Y+53 Z+53
α+53
X+44 Y+44 Z+44
α+44
X+35 Y+35 Z+35
α+35
X+44 Y+44 Z+44
α+44
X+44 Y+44 Z+44
α+44
I+53 J+53 K+53 R+53
I+44 J+44 K+44 R+44
X+53 P+8
X+53/P+8
I+44 J+44 K+44 R+44
I+35 J+35 K+35 R+35
←
←
I+53 J+53 K+53 R+53
I+44 J+44 K+44 R+44
←
←
I+44 J+44 K+44 R+44
(Note 5)
I+35 J+35 K+35 R+35
(Note 5)
←
←
Feed function
0.001(°) mm/
0.0001 inch
0.0001 (°) mm/
0.00001 inch
Tool offset
Miscellaneous function (M)
Spindle function (S)
Tool function (T)
2nd miscellaneous function
Subprogram
F63(Feed per minute)
F43(Feed per revolution)
F54(Feed per minute)
F34(Feed per revolution)
H3 D3
M8
S8
T8
A8/B8/C8
P8 H5 L4
F44(Feed per minute)
F34(Feed per revolution)
F35(Feed per minute)
F25(Feed per revolution)
←
←
←
←
←
←
F63(Feed per minute)
F43(Feed per revolution)
F54(Feed per minute)
F34(Feed per revolution)
←
←
←
←
←
←
F44(Feed per minute)
F34(Feed per revolution)
(Note 6)
F35(Feed per minute)
F25(Feed per revolution)
(Note 6)
←
←
←
←
←
←
Fixed cycle
0.001(°) mm/
0.0001 inch
R+53 Q53 P8 L4
← ← ←
0.0001(°) mm/
0.00001 inch
R+44 Q44 P8 L4
← ← ←
- 13 -
2.5 Command Value and Setting Value Range
Program number
Sequence number
Preparatory function
Movement axis
Arc and cutter radius
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Dwell
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Feed function
0.0001(°) mm/
0.00001 inch
Tool offset
Miscellaneous function (M)
Spindle function (S)
Tool function (T)
2nd miscellaneous function
Subprogram
0.001(°) mm/
0.0001 inch
Fixed cycle
0.0001(°) mm/
0.00001 inch
Metric command
08
N5
G3/G21
Inch command
←
←
←
L system
Rotary axis
(Metric command)
←
←
←
Rotary axis
(Inch command)
←
←
←
X+53 Y+53 Z+53
α+53
X+44 Y+44 Z+44
α+44
X+53 Y+53 Z+53
α+53
X+53 Y+53 Z+53
α+53
X+44 Z+44
α+44 X+35
I+53 J+53 K+53 R+53
I+44 K+44 R+44
X+53 P+8
I+44 J+44 K+44 R+44
I+35 K+35 R+35
←
I+53 J+53 K+53 R+53
I+44 K+44 R+44
←
I+44 J+44 K+44 R+44
(Note 5)
I+35 K+35 R+35
(Note 5)
←
X+53/P+8
F54(Feed per minute)
F34(Feed per revolution)
T1/T2
M8
S8
T8
A8/B8/C8
P8 H5 L4
←
F63(Feed per minute)
F35(Feed per revolution)
F44(Feed per minute)
F26(Feed per revolution)
F35(Feed per minute)
F25(Feed per revolution)
←
←
←
←
←
←
← ←
F63(Feed per minute)
F34(Feed per revolution)
F44(Feed per minute)
F26(Feed per revolution)
(Note 6)
F54(Feed per minute)
F34(Feed per revolution)
←
←
←
←
←
←
F35(Feed per minute)
F25(Feed per revolution)
(Note 6)
←
←
←
←
←
←
R+53 Q53 P8 L4
← ← ←
R+44 Q44 P8 L4
← ← ←
- 14 -
2.5 Command Value and Setting Value Range
(Note 1)
α 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.
(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.
(Note 10) Least input setting increment "C" (0.0001(°)mm/0.00001inch) and dwell's U address are specifications for E68 system. These cannot be used with E60.
- 15 -
2.5 Command Value and Setting Value Range
<List of Command Value and Setting Value Ranges>
Linear axis Rotary axis
Input unit: mm
Minimum input setting unit 0.001
0.0001
Maximum stroke
(Value on machine coordinate system)
±99999.999 mm
±9999.9999 mm
Maximum command value ±99999.999 mm
±9999.9999 mm
Rapid traverse rate
(Including during dry run)
1 to 1000000 mm/min
1 to 100000 mm/min
M system cutting feed rate
(Including during dry run)
0.01 to 1000000 mm/min
0.001 to 100000 mm/min
L system cutting feed rate
(Including during dry run)
M system synchronous feed
0.001 to 1000000 mm/min
0.0001 to 100000 mm/min
0.001 to 999.999 mm/rev
0.0001 to 99.9999 mm/rev
L system synchronous feed 0.0001 to 999.9999 mm/rev
0.00001 to 99. 99999 mm/rev
2nd to 4th reference point offset (value on machine coordinate system)
±99999.999 mm
±9999.9999 mm
Tool offset amount (shape) ±999.999 mm
±99.9999 mm
Tool offset amount (wear) ±99.999 mm
±9.9999 mm
0.0001
0.00001
Input unit: inch
±9999.9999 inch
±999.99999 inch
±9999.9999 inch
±999.99999 inch
1 to 39370 inch/min
1 to 3937 inch/min
0.001 to 39370 inch/min
0.0001 to 3937 inch/min
0.0001 to 39370.0787 inch/min
0.00001 to 3937.00787 inch/min
0.0001 to 999.9999 inch/rev
0.00001 to 99.99999 inch/rev
0.000001 to 99.999999 inch/rev
0.0000001 to 9.9999999 inch/rev
±9999.9999 inch
±999.99999 inch
0.001
0.0001
Degree (°)
±99999.999 °
±9999.9999 °
±99999.999 °
±9999.9999 °
1 to 1000000 °/min
1 to 100000 °/min
0.01 to 1000000 °/min
0.001 to 100000 °/min
0.001 to 1000000 °/min
0.0001 to 100000 °/min
0.01 to 999.99 °/rev
0.001 to 99.999 °/rev
0.0001 to 999.9999 °/rev
0.00001 to 99.99999 °/rev
±99999.999 °
±9999.9999 °
Handle feed amount
0.0001 mm/pulse
0.001 mm/pulse
0.0001 mm/pulse
Soft limit range
(value on machine coordinate system)
–99999.999 to +99999.999 mm
–9999.9999 to +9999. 9999 mm
Dwell time
Backlash compensation amount
0 to 99999.999 s
0 to ±9999 pulse
Pitch error compensation 0 to ±9999 pulse
M system thread lead (F) 0.001 to 999.999 mm/rev
0.0001 to 99.9999 mm/rev
M system thread lead
(Precise E)
0.00001 to 999.99999 mm/rev
0.000001 to 99.999999 mm/rev
L system thread lead (F) 0.0001 to 999.9999 mm/rev
0.00001 to 99.99999 mm/rev
L system thread lead
(Precise E)
0.00001 to 999.99999 mm/rev
0.000001 to 99.999999 mm/rev
±99.9999 inch
±9.99999 inch
±9.9999 inch
±0.99999 inch
0.0001 inch/pulse
0.00001 inch/pulse
0.0001 inch/pulse
0.00001 inch/pulse
–9999.9999 to +9999.9999 inch
–999.99999 to +999.99999 inch
0 to 99999.999 s
0 to ±9999 pulse
0.001 °/pulse
0.0001 °/pulse
0.001 °/pulse
0.0001 °/pulse
1 to 359.999 °
1 to 359.9999 °
0 to ±9999 pulse
0 to ±9999 pulse
0.0001 to 39.3700 inch/rev
0.00001 to 3.93700 inch/rev
0.000001 to 39.370078 inch/rev
0.000001 to 3.937007 inch/rev
0.000001 to 99.999999 inch/rev
0.0000001 to 9.9999999 inch/rev
0.000010 to 9.9999999 inch/rev
0.0000010 to 0.99999999 inch/rev
0 to ±9999 pulse
(Note 1) The second line in the table applies when the least setting increment is 0.001, 0.0001 from the first line.
(Note 2) Least input setting increment "C" (0.0001(°)mm/0.00001inch) is a specification for E68 system. This cannot be used with E60.
- 16 -
3. Positioning / Interpolation
3.1 Positioning
3. Positioning / Interpolation
3.1 Positioning
3.1.1 Positioning
M system
L system
E60 E68
{ {
{ {
This function carries out positioning at high speed using rapid traverse with the movement command value given in the program.
G00 Xx1 Yy1 Zz1 … (NC axis) ;
(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 that 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(#1086 G00 non-interpolation) 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)
(Example) Linear type (Moves lineary to the end point.)
G 00 G 91 X 100. Y 100. ;
(
Example) Non-linear type (Each axis moves with each parameter speed.)
G 00 G 91 X 100. Y 100. ;
Y
End point
Y
End point
100.
100.
Current position
100.
Current position
100.
X
X
(4) The tool is always accelerated at the start of the program command block and decelerated at the end of the block.
- 17 -
3. Positioning / Interpolation
3.1 Positioning
3.1.2 Unidirectional Positioning
M system
L system
E60 E68
{
–
{
–
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 … (NC axis) ;
(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)
G60 G91 X100. Y100. ;
Interim point
End point
Y100.
Current position
X100.
–
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.
3. The creep distance of the distance between the interim and end points can be set independently for each axis by "parameters".
(Note 1) The processing of the above pattern will be followed even for the machine lock and Zaxis command cancel.
(Note 2) The creep distance 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.
- 18 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
3.2 Linear / Circular Interpolation
3.2.1 Linear Interpolation
M system
E60 E68
{
{
{
{
L 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 … (NC axis) Ff1 ;
(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)
G01 G91 X100. Y100. F120 ;
Y
End point
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
Feed rate
(120mm/min)
100.
(85mm/min) respective command values to the actual movement distance with linear interpolation.
Current position
100. (85mm/min)
X
(1) The number of axes that 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.
- 19 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
3.2.2 Circular Interpolation (Center / Radius Designation)
M system
L system
E60 E68
{
{
{
{
(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 (NC axis) Ii1 Jj1 Ff1 ;
G02, G03 : Arc rotation direction
Xx1, Yy1 : End point coordinate values
Ii1, Jj1 : Arc center 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 Xaxis 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.
Y
Y G17
G03
G02
X
X
G18
G03
G02
Z
Z
G19
Start point
F
G02
G03
I, J
End point
Y
Center
X
(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".
- 20 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
(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 (NC axis) Rr1 Ff1 ;
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)
G02 G91 X100. Y100. R100. F120 ;
Y
Feed rate:
120mm/min
Arc end point coordinates
(X, Y)
R100.
Current position
(arc start point)
X
(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.
- 21 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
3.2.3 Helical Interpolation
M system
L system
E60 E68
{
–
{
{
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 3dimensional cams.
G17 G02(G03) Xx1 Yy1 Zz1 Ii1 Jj1 Pp1 Ff1 ;
G17 : Arc plane
G02, G03
Xx1, Yy1
: Arc rotation direction
: End point coordinate values for arc
Zz1
Ii1, Jj1
Pp1
Ff1
: End point coordinate of linear axis
: Arc center coordinates
: Pitch No.
: 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 coordinates 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
π
• p1 +
θ)/2π)
θ = θe – θs = arctan (ye/xe) – arctan (ys/xs)
Where xs, ys are the start point coordinates (0
≤ θ < 2π) 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 within this range. The feed rate is controlled so that the tool always moves at a speed along the circumference of the circle.
- 22 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
(Example)
G91 G17 G02 X0. Y200. Z100. I–100. J100. F120 ;
Z
Command program path
Y
End point
End point
X
W
J100
I-100
Start point
Y
Start point
X
XY plane projection path in command program
(Note 1) Helical sharps 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.
Z
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.
V
●
End point
●
Start point
Y
X
- 23 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
3.2.5 Cylindrical Interpolation
M system
L system
E60 E68
–
–
{
{
This function transfers the shape that is on the cylinder's side surface (shape yielded by the cylindrical coordinate system) onto a plane, and when the transferred shape is designated in the program in the form of plane coordinates, the shape is converted into a movement along the linear and rotary axes of the original cylinder coordinates, and the contours are controlled by means of the CNC unit during machining.
Since the programming can be performed for the shapes produced by transferring the side surfaces of the cylinders, this function is useful when it comes to machining cylindrical cams and other such parts.
Program coordinate plane
Z axis
C axis
X axis
C axis
Cylindrical interpolation machining
Z axis
Cylinder radius value
(1) Cylindrical interpolation mode start
(G07.1 name of rotary axis cylinder radius value;)
Cylindrical interpolation is performed between the rotary axis designated in the G07.1 block and any other linear axis.
(a) Linear interpolation or circular interpolation can be designated in the cylindrical interpolation mode. However, assign the G19 command (plane selection command) immediately before the G07.1 block.
(b) The coordinates can be designated either in absolute values or incremental values.
(c) Tool radius compensation can be applied to the program commands. Cylindrical interpolation is performed for the path after tool radius compensation.
(d) For the feed rate, designate a tangential rate over the cylinder transfer surface using the F command.
The F rate is in either mm/min or inch/mm units.
(2) Cylindrical interpolation mode cancel
(G07.1 name of rotary axis 0;)
If "C" is the name of the rotary axis, the cylindrical interpolation cancel mode is established with the command below.
G07.1 C0 ;
- 24 -
3. Positioning / Interpolation
3.2 Linear / Circular Interpolation
3.2.6 Polar Coordinate Interpolation
E60 E68
M system
L system
–
–
–
{
This function converts the commands programmed by the orthogonal coordinate axes into rectilinear axis movements (tool movements) and rotary axis movements (workpiece rotation) to control the contours. It is useful for cutting linear cutouts on the outside diameter of the workpiece, grinding cam shafts, etc.
X axis
C axis
Z axis
Hypothetical axis
Polar coordinate interpolation plane (G17 plane)
Fig. 1 Diagram explaining polar coordinate interpolation axes
(1) Polar coordinate interpolation mode
(G12.1)
The polar coordinate interpolation mode is established by designating the G12.1 command.
The plane (hereafter referred to as the "polar coordinate interpolation plane"), for which the linear axis will be first orthogonal axis and the hypothetical axis at right angles to the linear axis will be the second axis, is selected.
Polar coordinate interpolation is performed on this plane.
(a) Linear interpolation and circular interpolation can be designated in the polar coordinate interpolation mode.
(b) Either absolute values or incremental values can be designated.
(c) Tool radius compensation can be applied to the program commands. Polar coordinate interpolation is performed for the path after tool radius compensation.
(d) For the feed rate, designate a tangential rate on the polar coordinate interpolation plane
(orthogonal coordinate system) using the F command.
The F rate is in either mm/min or inch/mm units.
(2) Polar coordinate interpolation cancel mode
(G13.1)
The polar coordinate interpolation cancel mode is established by designating the G13.1 command.
- 25 -
4. Feed
4. Feed
4.1 Feed Rate
4.1.1 Rapid Traverse Rate (m/min)
E60 E68
M system
L system
1000
1000
1000
1000
The rapid traverse rate can be set independently for each axis.
G00, G27, G28, G29, G30 and G60 are the effective commands for the rapid traverse rate.
Override can be applied to the rapid traverse rate using the external signal supplied.
• Rapid Traverse Rate setting range
(1) For E60
Least input increment
Metric input
Inch input
B
1 to 1000000 (mm/min,
°
/min)
1 to 39370 (inch/min)
Least input increment B: 0.001 mm (0.0001 inch)
(2) For E68
Least input increment
Metric input
Inch input
B
1 to 1000000 (mm/min,
°
/min) 1 to 100000 (mm/min,
°
/min)
1 to 39370 (inch/min)
C
1 to 3937 (inch/min)
Least input increment B: 0.001 mm (0.0001 inch)
Least input increment C: 0.0001 mm (0.00001 inch)
- 26 -
4. Feed
4.1.2 Cutting Feed Rate (m/min)
E60 E68
M system
L system
1000
1000
1000
1000
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
(1) For E60
Least input increment
Metric input
Inch input
B
1 to 1000000 (mm/min,
°
/min)
1 to 39370 (inch/min)
Least input increment B: 0.001 mm (0.0001 inch)
(2) For E68
Least input increment
Metric input
Inch input
B
1 to 1000000 (mm/min,
1 to 39370 (inch/min)
°
/min)
C
1 to 100000 (mm/min,
1 to 3937 (inch/min)
°
/min)
Least input increment B: 0.001 mm (0.0001 inch)
Least input increment C: 0.0001 mm (0.00001 inch)
• Effective G-code commands for the cutting feed
G01, G02, G03, G2.1 G3.1 G33, etc. As to others, refer to the interpolation specifications.
- 27 -
4. Feed
4.1.3 Manual Feed Rate (m/min)
E60 E68
M system
L system
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
Inch input
0.00 to 14000.00 mm/min (31 steps)
0.000 to 551.000 inch/min (31 steps)
• Setting range under the numerical value method
Metric input
Inch input
0 to 1000000.00 mm/min in 0.01 mm/min increments
0 to 39370 inch/min in 0.001 inch/min increments
Multiplication factor PCF1 and PCF2 are available with the numerical value setting method.
- 28 -
4.2 Feed Rate Input Methods
4. Feed
4.2 Feed Rate Input Methods
4.2.1 Feed per Minute
M system
L system
E60 E68
{
{
{
{
[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).
(1) For E60
Metric input (mm)
Least input increment
(B) 0.001 mm
F command increment
(mm/min) without decimal point with decimal point
Command range (mm/min)
F1 = 1 mm/min
F1. = 1 mm/min
0.01 to 1000000.000
Inch input (inch)
Least input increment
F command increment
(inch/min) without decimal point with decimal point
Command range (inch/min)
(B) 0.0001 inch
F1 = 1 inch/min
F1. = 1 inch/min
0.001 to 100000.0000
(2) For E68
Metric input (mm)
Least input increment
F command increment
(mm/min) without decimal point with decimal point
Command range (mm/min)
(B) 0.001 mm
F1 = 1 mm/min
F1. = 1 mm/min
0.01 to 1000000.000
(C) 0.0001 mm
F1 = 1 mm/min
F1. = 1 mm/min
0.001 to 100000.000
Inch input (inch)
Least input increment
F command increment
(inch/min) without decimal point with decimal point
Command range (inch/min)
(B) 0.0001 inch
F1 = 1 inch/min
F1. = 1 inch/min
0.001 to 100000.0000
(C) 0.00001 inch
F1 = 1 inch/min
F1. = 1 inch/min
0.001 to 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 (I_Sync) to OFF.
- 29 -
4. Feed
4.2 Feed Rate Input Methods
[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).
(1) For E60
Metric input (mm)
Least input increment
(B) 0.001 mm
F command increment
(mm/min) without decimal point with decimal point
Command range (mm/min)
F1 = 1 mm/min
F1. = 1 mm/min
0.001 to 1000000.000
Inch input (inch)
Least input increment
F command increment
(inch/min) without decimal point with decimal point
Command range (inch/min)
(2) For E68
Metric input (mm)
Least input increment
F command increment
(mm/min) without decimal point with decimal point
(B) 0.0001 inch
F1 = 1 inch/min
F1. = 1 inch/min
0.0001 to 39370.0787
(B) 0.001 mm
F1 = 1 mm/min
F1. = 1 mm/min
(C) 0.0001 mm
F1 = 1 mm/min
F1. = 1 mm/min
Command range (mm/min)
0.001 to 1000000.000
0.0001
to 100000.0000
Inch input (inch)
Least input increment
F command increment
(inch/min) without decimal point with decimal point
Command range (inch/min)
(B) 0.0001 inch
F1 = 1 inch/min
F1. = 1 inch/min
(C) 0.00001 inch
F1 = 1 inch/min
F1. = 1 inch/min
0.0001 to 39370.0787
0.00001 to 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 (I_Sync) to OFF.
- 30 -
4. Feed
4.2 Feed Rate Input Methods
4.2.2 Feed per Revolution
M system
L system
E60 E68
{
{
{
{
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 least command increment and command range of the feed rate designation F are as follows.
[M system]
(1) For E60
Metric input (mm)
Least input increment
(B) 0.001 mm
F command increment
(mm/rev)
F command increment
(inch/rev) without decimal point with decimal point
Command range (mm/rev)
Inch input (inch)
Least input increment without decimal point with decimal point
F1 = 0.01
F1. = 1
0.001 to 999.999
(B) 0.0001 inch
F1 = 0.001
F1. = 1
Command range (inch/rev)
(2) For E68
Metric input (mm)
Least input increment
F command increment
(mm/rev) without decimal point with decimal point
0.0001 to 999.9999
(B) 0.001 mm
F1 = 0.01
F1. = 1
(C) 0.0001 mm
F1 = 0.01
F1. = 1
Command range (mm/rev)
Inch input (inch)
Least input increment
F command increment
(inch/rev) without decimal point with decimal point
0.001 to 999.999
(B) 0.0001 inch
F1 = 0.001
F1. = 1
0.0001 to 99.9999
(C) 0.00001 inch
F1 = 0.001
F1. = 1
Command range (inch/rev)
0.0001 to 999.9999 0.00001 to 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 (I_Sync) to OFF.
- 31 -
4. Feed
4.2 Feed Rate Input Methods
[L system]
(1) For E60
Metric input (mm)
Least input increment
F command increment
(mm/rev) without decimal point with decimal point
Command range (mm/rev)
Inch input (inch)
Least input increment
F command increment
(inch/rev) without decimal point with decimal point
Command range (inch/rev)
(B) 0.001 mm
F1 = 0.0001
F1. = 1
0.0001 to 999.999
(B) 0.0001 inch
F1 = 0.000001
F1. = 1
0.000001 to 99.999999
(2) For E68
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
Command range (mm/rev)
Inch input (inch)
Least input increment
F1 = 0.0001
F1. = 1
0.0001 to 999.9999
F1 = 0.0001
F1. = 1
0.00001 to 99.99999
(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 to 99.999999
0.0000001 to 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 (I_Sync) to OFF.
- 32 -
4. Feed
4.2 Feed Rate Input Methods
4.2.4 F1-Digit Feed
M system
L system
E60 E68
{
{
{
{
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 established when F0 is designated which is the same as the G00 command. When one of the codes F1 to F5 is designated, the cutting feed rate set to support the code serves as the valid rate command. When a command higher than F5 is designated, it serves as a regular F command's direct command.
When an F 1-digit feed command has been designated, the "In F 1-digit" external output signal is output.
- 33 -
4. Feed
4.3 Override
4.3 Override
4.3.1 Rapid Traverse Override
M system
L system
(1) Type 1 (code method)
E60 E68
{
{
{
{
Four levels of override (1%, 25%, 50% and 100%) can be applied to manual or automatic rapid traverse using the external input signal supplied.
(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.
(Note 2) A PLC must be built into the unit for type 2.
4.3.2 Cutting Feed Override
M system
L system
(1) Type 1 (code method)
E60 E68
{
{
{
{
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 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.
(Note 1) A PLC must be built into the unit for type 2.
4.3.3 2nd Cutting Feed Override
M system
L system
E60 E68
{ {
{ {
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.
(Note 1) A PLC must be built into the unit for this function.
- 34 -
4. Feed
4.3 Override
4.3.4 Override Cancel
M system
L system
E60 E68
{
{
{
{
By turning on the override cancel external signal, the override is automatically set to 100% for the cutting feed during an automatic operation mode (tape, 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.
- 35 -
4. Feed
4.4 Acceleration / Deceleration
4.4 Acceleration / Deceleration
4.4.1 Automatic Acceleration / Deceleration after Interpolation
M system
E60 E68
{
{
{
{
L 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
Soft acceleration/deceleration
Exponential acceleration/deceleration
Exponential acceleration / linear deceleration
F F FC F
Tsr
Tsr
Tss
Tss Tsc
Tsc Tsc Tsr
(Note 1) The rapid traverse feed acceleration/deceleration patterns are also 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). f
2
Acceleration / Deceleration during Continuing Blocks
(1) Continuous G1 blocks
f
1
G1
0
f
1
Tsc
G1
Tsc
0
T s c f
2
The tool does not decelerate between blocks.
- 36 -
4. Feed
4.4 Acceleration / Deceleration
(2) Continuous G1-G0 blocks
Tsr
G1
Tsr
G0
G1
Tsc
G0
G1
Tsr
G0
Tsr
G1
Tsc
G0
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
M system
E60 E68
{ {
{ {
L 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.
- 37 -
4. Feed
4.4 Acceleration / Deceleration
(1) When the interpolation distance is longer than the acceleration and deceleration distance
rapid
L
Next block
θ
T s
T s
T d
T rapid : Rapid traverse rate
Ts : Acceleration/deceleration time constant
Td : Command deceleration check time
θ
: Acceleration/deceleration inclination
T : Interpolation time
L : Interpolation distance
T =
L rapid
+Ts
Td = Ts + (0~1.7 ms)
θ
= tan
-1
( rapid
Ts
)
(2) When the interpolation distance is shorter than the acceleration and deceleration distance
rapid
θ
Ts
L
T
Td
Next block rapid: Rapid traverse rate
Ts: Acceleration/deceleration time constant
Td: Command deceleration check time
θ
: Acceleration/deceleration inclination
T: Interpolation time
L: Interpolation distance
T = 2
×
√
Ts × L / rapid
T
Td =
2
+ (0
~
1.7 ms)
θ
= tan
-1
(
rapid
Ts
)
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.
- 38 -
4. Feed
4.4 Acceleration / Deceleration
(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. rapid X
Lx
Next block
X axis
θ x
Tsx
Tsx
Tdx
Tx rapid Z
Lz
Next block
θ
Z
Z axis
Tsz
Tsz
Tdz
Tz
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).
- 39 -
4. Feed
4.5 Thread Cutting
4.5.1 Thread Cutting (Lead/Thread Number Designation)
M system
L system
E60 E68
{
{
{
{
(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 : command
Zz1
Qq1
: Thread length
: Shift angle ("q1" is the shift angle at thread cutting start 0 to 360
°)
Ff1
Ee1
: Thread lead
: Thread lead (precise lead threads)
The tables below indicate the thread lead ranges.
[M system]
(a) For E60
Metric command Inch command
Command increment
(mm)
F (mm/rev) E (mm/rev)
Command increment
(inch)
F (inch/rev) E (inch/rev)
0.001
0.001
to 999.999
0.00001 to 999.99999
0.0001
0.0001 to 39.3700
0.000001 to 39.370078
(b) For E68
Metric command Inch command
Command increment
(mm)
F (mm/rev) E (mm/rev)
Command increment
(inch)
F (inch/rev) E (inch/rev)
0.001
0.0001
0.001 to 999.999
0.0001 to 99.9999
0.00001 to 999.99999
0.000001 to 99.999999
0.0001
0.00001
0.0001 to 39.3700
0.00001 to 3.93700
0.000001 to 39.370078
0.000001 to 3.937007
- 40 -
4. Feed
[L system]
(a) For E60
Metric command Inch command
Command increment
(mm)
F (mm/rev) E (mm/rev)
Command increment
(inch)
F (inch/rev) E (inch/rev)
0.001
0.0001 to 999.9999
0.00001 to 999.99999
0.0001
0.00001 to 99.999999
0.000010 to 9.9999999
(b) For E68
Metric command Inch command
Command increment
(mm)
F (mm/rev) E (mm/rev)
Command increment
(inch)
F (inch/rev) E (inch/rev)
0.001
0.0001
0.0001 to 999.9999
0.00001 to 99.99999
0.00001 to 999.99999
0.000001 to 99.999999
0.0001
0.00001
0.00001 to 99.999999
0.000001 to 9.9999999
0.000010 to 9.9999999
0.0000010 to 0.99999999
The axis direction characterized by a large movement serves as the reference for the lead.
- 41 -
4. Feed
(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 ;
Zz1
Qq1
Ee1
: Thread length
: Shift angle ("q1" is the shift angle at thread cutting start 0 to 360
°)
: Thread number per inch
The tables below indicate the thread leads.
[M system]
(a) For E60
Command increment
(mm)
0.001
Metric command
Thread number command range
(thread/inch)
0.03 to 999.99
Command increment
(inch)
0.0001
Inch command
Thread number command range
(thread/inch)
0.0255 to 9999.9999
(b) For E68
Command increment
(mm)
0.001
0.0001
Metric command
Thread number command range
(thread/inch)
0.03 to 999.99
255 to 9999.999
Command increment
(inch)
0.0001
0.00001
Inch command
Thread number command range
(thread/inch)
0.0255 to 9999.9999
0.25401 to 999.9999
[L system]
(a) For E60
Command increment
(mm)
0.001
Metric command
Thread number command range
(thread/inch)
0.03 to 999.99
(b) For E68
Command increment
(inch)
0.0001
Inch command
Thread number command range
(thread/inch)
0.0101 to 9999.9999
Command increment
(mm)
0.001
0.0001
Metric command
Thread number command range
(thread/inch)
0.03 to 999.99
0.255 to 9999.999
Command increment
(inch)
0.0001
0.00001
Inch command
Thread number command range
(thread/inch)
0.0101 to 9999.9999
0.1001 to 999.9999
The number of thread per inch is commanded for both metric and inch systems, and the direction of the axis with a high movement serves as the reference.
- 42 -
4. Feed
4.5.2 Variable Lead Thread Cutting
E60 E68
M system
L 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__;
X/U
Z/W
F/E
K
: Thread end point X coordinate
: Thread end point Z coordinate
: Thread’s basic lead
: Lead increment/decrement amount per thread rotation
Non-lead axis
Lead axis
F+3.5K
F+2.5K
F+1.5K
F+0.5K
Lead speed
F+4K
F+3K F+2K F+K F
- 43 -
4. Feed
4.5.3 Synchronous Tapping
4.5.3.1 Synchronous Tapping Cycle
M system
L system
E60 E68
Δ
Δ
{
{
This function performs tapping through the synchronized control of the spindle and servo. 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 ,Ss2 ,Ii1 ,Jj1 ,R2 ;
X, Y
Z
R
P
F
S
,S
,I
,J
,R
: 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
: Rotation speed of spindle during retract
: In-position width of positioning axis
: In-position width of hole drilling axis
: Synchronization method selection
(r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode)
(2) Tapping thread number assignment
G84(G74) Xx1 Yy1 Zz1 Rr1 Pp1 Ee1 Ss1 ,Ss2 ,Ii1 ,Jj1 ,R2 ;
S
,S
,I
,J
,R
X, Y
Z
R
P
E
: 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
: Rotation speed of spindle during retract
: In-position width of positioning axis
: In-position width of hole drilling axis
: Synchronization method selection
(r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode)
- 44 -
4. Feed
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 (E68)
G62 ....... Automatic corner override
G64 ....... Cutting mode
(Note)
The synchronous tapping cycle can be used for axes other than the Z axis with the plane selection.
Furthermore, in-position checks can be performed at the hole bottom or point R, etc. using the parameters. The figure below shows the correlation between the in-position width and the movement of the tapping axis of the synchronous tapping in-position check.
FIN
Hole bottom
Point R
→
Feed rate
Time T
→
G0 feed start to point R
→
In-position finish for G0 feed from point R
G1 deceleration start during tap cutting
G1 deceleration start with tap return
(4) (2) (3) (1)
(1) Section where in-position check is performed using servo in-position width
(2) Section where in-position check is performed using in-position width for tapping
(3) Section where in-position check is performed using in-position width for cutting feed (G1, G2, G3)
(4) Section where in-position check is performed using in-position width for rapid traverse (G0)
- 45 -
4. Feed
4.5.3.2 Pecking Tapping Cycle
M system
L system
E60 E68
–
–
{
–
The load applied to the tool can be reduced by designating the depth of cut per pass and cutting the workpiece to the hole bottom for a multiple number of passes.
The amount retracted from the hole bottom is set to the parameters.
Select either the pecking tapping cycle or the deep-hole tapping cycle by parameter.
When "depth of cut per pass Q" is designated in the block containing the G84 or G74 command in the state where the pecking tapping cycle is selected by parameter, the pecking tapping cycle is executed.
In the following cases, the normal tapping cycle is established.
• When Q is not designated
• When the command value of Q is "0"
G84(G74) Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1 Ss1 ,Ss2 ,Ii1 ,Jj1 ,Rr2 ；
F
P
S
,S
X,Y
Z
R
Q
,I
,J
,R
: Hole drilling point position
: Hole bottom position
: Point R position
: Depth of cut per pass (designated as an incremental value)
: Z-axis feed amount (tapping pitch) per spindle rotation
: Dwell time at hole bottom position
: Rotation speed of spindle
: Rotation speed of spindle during retract
: In-position width of positioning axis
: In-position width of hole drilling axis
: Synchronization method selection
(r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode)
(Note) When ",R0" is commanded, F address is regarded as cutting feed rate.
- 46 -
4. Feed
(1) x
1
,y
1
(2) q
1 q
1 q
1
(3)
(4)
(6) m
(5)
(7)
(10) m
(9)
(8)
(11)
(n5)(n6)
(n1)
(n7)
(n5)(n6) r
1
(n4) (n4) z
1
(9)
(10)
(11)
:
(n1)
(n2)
(n3)
(n4)
(n5)
(n6)
(5)
(6)
(7)
(8)
(1)
(2)
(3)
(4)
(n2)(n3) G98 mode
G99 mode
(n7)
G0 Xx1 Yy1 ,Ii1
G0 Zr1
G1 Zq1 Ff1
M4 (Spindle reverse rotation)
G1 Z-m Ff1
M3 (Spindle forward rotation)
G1 Z(q1+m) Ff1
M4 (Spindle reverse rotation)
G1 Z-m Ff1
M3 (Spindle forward rotation)
G1 Z(q1+m) Ff1
:
G1 Z(z1-q1*n) Ff1
G4 Pp1
M4 (Spindle reverse rotation)
G1 Z-z1 Ff1 Ss2
G4 Pp1
M3 (Spindle forward rotation)
G98 mode G0 Z-r1 ,Ij1
G99 mode No movement
*1. m : Parameter
2. This program is for the G84 command. The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the
G74 command.
- 47 -
4. Feed
4.5.3.3 Deep-hole Tapping Cycle
M system
L system
E60 E68
–
–
{
–
In the deep-hole tapping, the load applied to the tool can be reduced by designating the depth of cut per pass and cutting the workpiece to the hole bottom for a multiple number of passes.
Under the deep-hole tapping cycle, the tool is retracted to the R-point every time.
Select either the pecking tapping cycle or the deep-hole tapping cycle by parameter.
When "depth of cut per pass Q" is designated in the block containing the G84 or G74 tapping cycle command in the state where the deep-hole tapping cycle is selected, the deep-hole tapping cycle is executed.
In the following cases, the normal tapping cycle is established.
• When Q is not designated
• When the command value of Q is "0"
G84(G74) Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1 Ss1 ,Ss2 ,Ii1 ,Jj1 ,Rr2 ；
F
P
S
,S
X,Y
Z
R
Q
,I
,J
,R
: Hole drilling point position
: Hole bottom position
: Point R position
: Depth of cut per pass (designated as an incremental value)
: Z-axis feed amount (tapping pitch) per spindle rotation
: Dwell time at hole bottom and point R return
: Rotation speed of spindle
: Rotation speed of spindle during retract
: In-position width of positioning axis
: In-position width of hole drilling axis
: Synchronization method selection
(r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode)
(Note) When ",R0" is commanded, F address is regarded as cutting feed rate.
- 48 -
4. Feed
(1)
R point q
1 q
1 q
1 x
1
,y
1
(2)
(3)
(4)
(6)(7) (12)(13)
(8)
(5) c
(9)
(11)
(10)
(14) c
(15)
(n5)(n6)
(n1)
(n7)
(n2)(n3) G98 mode
(n5)(n6)
G99 mode r
1
(n4) (n4) z
1
*1. Clearance amount c : Parameter
2. This program is for the G84 command. The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.
(n6)
(n7)
(9)
(10)
(11)
(12)
(13)
(14)
(15)
:
(n1)
(n2)
(n3)
(n4)
(n5)
(5)
(6)
(7)
(8)
(1)
(2)
(3)
(4)
G0 Xx1 Yy1
G0 Zr1
G9 G1 Zq1 Ff1
M4
(Spindle reverse rotation)
G9 G1 Z-q1 Ff1
G4 Pp1
M3
(Spindle forward rotation)
G1 Z(q1-c) Ff1
G9 G1 Z(q1+c) Ff1
M4
(Spindle reverse rotation)
G9 G1 Z-(2･q1) Ff1
G4 Pp1
M3
(Spindle forward rotation)
G1 Z(2･q1-c) Ff1
G9 G1 Z(q1+c) Ff1
:
G9 G1 Z(z1-q1*n+c) Ff1
G4 Pp1
M4 (Spindle reverse rotation)
G9 G1 Z-z1 Ff1
G4 Pp1
M3 (Spindle forward rotation)
G98 mode G0 Z-r1
G99 mode No movement
- 49 -
4. Feed
4.5.4 Chamfering
E60 E68
M system
L system
–
{
–
{
Chamfering can be validated during the thread cutting cycle by using external signals.
The chamfer amount and angle are designated with parameters.
Thread cutting cycle
Chamfer angle
Chamfer amount
- 50 -
4. Feed
4.6 Manual Feed
4.6.1 Manual Rapid Traverse
M system
E60 E68
{
{
{
{
L 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
×
Rapid traverse override
25
×
1
×
50
×
100
CNC
Tool
Machine tool
X
– –
Y Z
–
PLC
Axis movement control
Rapid traverse
4.6.2 Jog Feed
M system
E60 E68
{ {
{ {
L 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.
Jog
Feed rate Override
Machine tool
CNC
Tool
X
–
0
3000
Y
–
0
200
Z
–
PLC
Axis movement control
Manual cutting feed
- 51 -
4. Feed
4.6.3 Incremental Feed
M system
L system
E60 E68
{
{
{
{
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.
Incremental
Scale factor
Machine tool
1000
CNC
Tool
X
–
Y
–
Z
–
PLC
Axis movement control
Step feed
4.6.4 Handle Feed
M system
E60 E68
{(2)
{(2)
{(2)
{(2)
L 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 random.
(Note 1) The actual movement amount and scale may not match if the manual pulse generator is rotated quickly.
(2 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.
- 52 -
4. Feed
4.6.5 Manual Feed Rate B
M system
L system
E60 E68
{
{
{
{
"Manual feed rate B" is a function that sets a random axis feed rate from the user PLC separately from the "manual feed rate". The "manual feed rate B" feed rate setting can be selected from the feed rate common for all axes and the feed rate independent of reach axis. By combining the
"manual feed rate B" function with the manual/automatic simultaneous function, a random axis can be moved at the "manual feed rate B" independently of the machining program operation even during automatic operation. Similarly, if the jog mode and other manual operation mode are set simultaneously, a random axis can be moved at a speed independent from the "manual feed rate" even during the manual operation mode.
The "manual feed rate B" function can move an axis at a speed different from the "manual feed rate". This is not affected by dry run, or by manual or cutting override, so a random axis can be moved independently even in operations during automatic operation or override during manual axis movement.
The relation of the "manual feed rate B" and "manual feed rate" is shown below.
Manual override validity
Y229=0
Cutting override
Manual feed rate
Dry run validity
Y21D=0
Dry run speed
Y260=0
Y2BC=1
Each axis manual feed rate B speed 1st axis
R400
R401
X axis speed
Y261=0
Each axis manual feed rate B speed 2nd axis
R402
R403
Y axis speed
Y262=0
Each axis manual feed rate B speed 3rd axis
R404
R405
Z axis speed
Y263=1
R138
R139
Each axis manual feed rate B speed 4th axis
R406
R407
B axis speed
Manual feed rate B valid n-th axis
Validity
Each axis manual feed rate B valid
Validity
- 53 -
4. Feed
4.7 Dwell
4.7 Dwell
4.7.1 Dwell (Time-based Designation)
M system
E60 E68
{
{
{
{
L 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 ;
Xx1, Uu1, Pp1 : Time (For U, E68 L system only.)
(1) When designating the dwell time with X or U, the decimal point command is valid.
(2) When designating the dwell time with P, the availability of the decimal point command can be selected with the parameter. When the decimal point command is invalid in the parameter setting, the command below the decimal point issued with P is ignored.
(3) When the decimal point command is valid or invalid, the dwell time command range is as follows.
Command range when the decimal point command is valid
0.001 to 99999.999 (s)
Command range when the decimal point command is invalid
1 to 99999999 (ms)
- 54 -
5. Program Memory / Editing
5.1 Memory Capacity
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)
600 m (400 programs)
E60 E68
M system
L system
{
{
{
{
5.2 Editing
5.2.1 Program Editing
M system
E60 E68
{ {
{ {
L 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.
- 55 -
5. Program Memory / Editing
5.2 Editing
5.2.2 Background Editing
M system
E60 E68
{
{
{
{
L system
This function enables one machining program to be created or editing while another program is being run.
Prohibited
Program registered in memory
O1000
Editing
O2000
O3000
O4000
Memory operation
Program editing Machining with memory operation
(1) The machining programs being used in memory operation cannot be edited, but can be displayed.
(2) The editing functions such as adding, revising or deleting data 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.
- 56 -
5. Program Memory / Editing
5.2 Editing
5.2.3 Buffer Correction
M system
E60 E68
{
{
{
{
L system
During automatic operation (memory, tape or IC card) or MDI operation, this function initiates single block stop and enables the next command to be corrected or changed.
Only memory operation allows the changes with buffer corrections to be updated in the machining program.
When a program error has occurred, the function enables the block in which the error occurred to be corrected and operation to be resumed without having to perform NC resetting.
Tape mode
Tape or IC card
Memory
Memory mode
Pre-read block
Execution block
NC opera- tion
MDI
MDI mode
Setting and display unit
Buffer correction
- 57 -
5. Program Memory / Editing
5.2 Editing
5.2.4 Word Editing
M system
E60 E68
{
{
{
{
L system
In addition to the conventional editing function, this function enables programs to be edited in word increments.
It is also possible to create programs by deleting, replacing and inserting in word increments.
<List of function>
012345678 TEST CUT PROGRAM
EDIT
N1 G28 X0 Y0 Z0 ;
N2 G00 X100.0 ;
N3 Z100.0 ;
N4 G01 X200.0 Z200.0 F500 ;
N5 X300.0 ;
N6 Z300.0 ;
N7 ;
N8 ;
N9 ;
<SEARCH DATA>
<EDIT BUFFER>
>
N10 ;
N11 ;
N12 ;
SEARCH DELETE REPLACE INSERT MENU
Menu Function
Delete The word on which the cursor is positioned can be deleted. (A deleted word can also be un-deleted.)
Replace The word on which the cursor is positioned can be replaced with editing buffer data. (The same word can also be repeatedly replaced.)
Insert
Copy
The editing buffer data can be inserted after the word on which the cursor is positioned. (The same word can also be repeatedly inserted.)
The word on which the cursor is positioned can be copied into the editing buffer. (The copied word can be used for replacement or insertion.)
Program A list of the programs is displayed.
Operation search Program numbers, sequence numbers and block numbers in the foreground can be searched.
Background search Program numbers, sequence numbers and block numbers for background editing can be searched. New machining programs can be registered as well.
Background exit Background editing is exited.
Comment
Word
↓
Comments can be set in machining programs.
A downward search for a word is conducted, and the cursor is moved to the word in question. (The same word can be repeatedly searched.)
Word
↑
String
↓
An upward search for a word is conducted, and the cursor is moved to the word in question. (The same word can be repeatedly searched.)
A downward search for a character string is conducted, and the cursor is moved to the words in question. (The same character string can be repeatedly searched.)
String
↑
An upward search for a character string is conducted, and the cursor is moved to the words in question. (The same character string can be repeatedly searched.)
Running program display
Program operation start position setting
The program being run is displayed when the program running display request (PLC) is ON.
The start block can be designated by moving the cursor on the editing screen.
- 58 -
6.2 Operation Methods and Functions
6. Operation and Display
6.1 Structure of Operation / Display Panel
The setting and display unit is configured of the display unit and keyboard unit. When the key switches are pressed, a buzzer sounds allowing the operation to be confirmed visually and audibly.
(1) 7.2-type monochrome LCD display
M system
E60 E68
–
L system
–
(2) 9-type monochrome CRT display
M system
E60 E68
–
L system
–
(3) 8.4-type color LCD(TFT) display
E60 E68
M system
L system
6.2 Operation Methods and Functions
6.2.1 Memory Switch (PLC switch)
M system
E60 E68
{ {
{ {
L system
The toggle switches (PLC switches) can be defined on the screen.
The screen can be operated by turning the switches ON/OFF, 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.
- 59 -
6.3 Display Methods and Contents
6.3 Display Methods and Contents
6.3.1 Status Display
M system
E60 E68
{
{
{
{
L 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 amplifier, and is displayed. However, during follow up, the speed is converted and displayed with the signals from the detector installed on the servomotor.
- 60 -
6.3 Display Methods and Contents
6.3.2 Position Display
M system
L system
E60 E68
{
{
{
{
Position data such as present positions for tools, coordinate positions and workpiece coordinate positions can be displayed.
(1) Present position counter
Each axis’ present value including tool length offset amount, tool radius compensation amount and workpiece coordinate offset amount is indicated.
Whether the tool reference position (figure below (a)) or the present position of the tool nose position (figure below (b)) that considers offset, such as tool length offset amount or tool diameter compensation amount, in the tool reference position is applied to the display of the relative value can be selected with the parameter.
Tool
Relative value (a)
(Machine position)
Displayed by tool reference position
Workpiece coordinate
Present value B
Relative value (b)
Displayed by tool nose position
Workpiece zero point
Workpiece offset
Machine zero point
Tool reference position
Tool nose position
(2) Workpiece coordinate counter
The workpiece coordinate system modal number from G54 to G59 and the workpiece coordinate value in the workpiece coordinate system are indicated.
The remaining distance of the movement command during the execution (incremental distance from the present value to the end point of the block) is indicated during the automatic start and automatic stop.
(4) Machine position counter
Each axis’s coordinate value in the basic machine coordinate system whose zero point is the characteristic position determined depending on the machine is indicated.
(5) Present value B
Each axis’ value not including tool length offset amount, tool radius compensation amount and workpiece coordinate offset amount is indicated.
Whether the counter value on the Position screen is expressed with the Present or with the present value B can be selected using parameter.
The present value B can be selected for the counter value indicated on the coordinate value screen using parameter.
(6) Manual interrupt amount counter
The amount moved with the manual mode while the manual absolute switch was OFF is indicated.
On the coordinate value screen, in addition to the manual interrupt amount, the MST display, next command counter and present value B can be selected for the indicated counter using parameter.
- 61 -
6.3 Display Methods and Contents
6.3.3 Program Running Status display
M system
L system
E60 E68
{
{
{
{
Program now being executed is displayed.
6.3.4 Setting and Display
M system
E60 E68
{
{
{
{
L system
The parameters used in controller operations can be set and displayed.
6.3.5 MDI Data Setting and Display
M system
E60 E68
{
{
{
{
L 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
M system
E60 E68
{ {
{ {
L system
The clock is built-in, and the date and time 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
M system
E60 E68
{ {
{ {
L system
This function displays the configuration of the installed hardware and software.
- 62 -
6.3 Display Methods and Contents
6.3.9 Integrated Time Display
M system
L system
E60 E68
{
{
{
{
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
Automatic start: 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.)
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.
6.3.10 Standard Language
M system
L system
6.3.11 Additional Languages
Japanese
M system
English
L system
M system
L system
German
M system
L system
E60 E68
{13 languages {13 languages
{13 languages {13 languages
E60 E68
{
{
{
{
{
{
E60 E68
{
{
E60 E68
{*
{*
{*
{*
- 63 -
6.3 Display Methods and Contents
Italian
M system
L system
E60 E68
{* {*
{* {*
French
M system
L system
E60 E68
{* {*
{* {*
Spanish
M system
E60 E68
{*
{*
{*
{*
L system
Chinese
(1) Chinese (Traditional Chinese characters)
M system
L system
E60 E68
{*
{*
(2) Chinese (Simplified Chinese characters)
{*
{*
M system
E60 E68
{
{
{
{
Korean
L system
M system
E60 E68
{* {*
{* {*
L system
Portuguese
M system
E60 E68
{* {*
{* {*
L system
Hungarian
M system
L system
E60 E68
{* {*
{* {*
- 64 -
6.3 Display Methods and Contents
Dutch
M system
L system
E60 E68
{* {*
{* {*
Swedish
M system
L system
E60 E68
{* {*
{* {*
* : Display only, Manual for each language will be provided from next version.
6.3.12 Screen Saver, Backlight OFF
M system
E60 E68
{
{
{
{
L system
The screen saver and backlight OFF functions turn off the displays when there is no need to view the screen.
<Screen saver>
This function protects the screen display unit by blanking the screen after the time set in the parameter has elapsed.
Inputting any key causes the screen to reappear.
<Backlight OFF>
This function turns off the backlight in order to extend the service life of the LCD screen's backlight.
6.3.13 Screen Deletion
M system
E60 E68
{
{
{
{
L 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.
- 65 -
7. Input / Output Functions and Devices
7.1 Input / Output Data
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)
M system
L system
Tool offset data input / output
M system
L system
E60 E68
{
{
{
{
E60 E68
{ {
{ {
Common variable input / output
M system
L system
E60 E68
{ {
{ {
Parameter input / output
M system
E60 E68
{ {
{ {
L system
History data output
M system
L system
E60 E68
{ {
{ {
Remote program input
M system
L system
E60 E68
–
–
{
{
System configuration data output
E60 E68
M system
L system
{
{
{
{
With this function, NC hardware/software configuration and version information can be output to outside the NC.
- 66 -
7. Input / Output Functions and Devices
7.2 Input / Output I/F
7.2 Input / Output I/F
7.2.1 RS-232C I/F
M system
E60 E68
{ {
{ {
L system
Port 2 of the RS-232C interface can be used. (Port 1 is used for the maintenance.)
Port
Port 2
Transmission speed to 19.2kbps
Bandshake method
DC code method, RTS/CTS method
It can be used for tape operation, data input/output and printing, etc.
(The application is designated with parameters.)
7.2.2 IC Card I/F
7.2.2.2 I/F for Front IC Card
M system
E60 E68
–
–
{
{
L system
I/F card to use IC card can be attached in front of the display unit and used.
A SanDisk CF card is recommended.
- 67 -
7. Input / Output Functions and Devices
7.3 Computer Link
7.3 Computer Link
7.3.1 Computer Link B
M system
E60 E68
–
{
–
{
L system
This function sends DC1 to the host computer (hereafter abbreviated to "HOST") at the CNC cycle start, and it enables operation to be performed while the machining programs are received from the
HOST.
The computer link has a 32-kbyte reception buffer so that operation will be less susceptible to the effects of the data transfer status at the HOST end. This means that when the machine is connected to a HOST capable of transferring data at a high speed (of 38,400 bps), it is possible to perform high-speed machining based on fine-segment data.
The high-speed machining mode option is required for high-speed fine-segment machining.
CNC
HOST
Operation
Com- mands
CNC
Machining programs
Com- munication software
32-kbyte reception buffer
RS-232C
Machining programs
BTR operation
- 68 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.1 Command / Output
8.1.1.1 Spindle Functions
M system
E60 E68
{
{
{
{
L 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 a 8-digit number following address S (S00000000 to S±99999999) is commanded, a signed
32-bit binary data or 8-digit BCD data and start signal will be output to the PLC.
Only one set of S commands can be commanded in one block.
Processing and complete sequences must be incorporated on the PLC side for all S commands.
NC PLC
S Command
8-digit
(Machining program,
Manual numerical command)
S command analysis
S command value
Start signal
Spindle rotation command
8-digit
BIN
Changeover
(Parameter)
Spindle controller
Spindle output command creation
Spindle rotation command
8-digit BIN
Gear selection
Override
Remote I/O unit
D/A converter
Analog spindle
Gear ratio
Max. rotation speed
(Parameter)
(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.
- 69 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.1.2 Spindle Serial I/F
M system
E60 E68
Δ
Δ
{
{
L system
Digital spindle
This interface is used to connect the spindle driver (SP, SPJ2) with the AC spindle motor.
8.1.1.3 Spindle Analog I/F
M system
E60 E68
{
{
L system
Spindle control can be executed using an analog spindle instead of the digital spindle.
In this case, the remote I/O unit DX12x/DX14x and the base I/O unit HR341/HR351 are 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 ±10V (±5%)
(2) Resolution ... 1/4095 (–12 multiplier of 2)
(3) Load conditions ... 10 k
Ω
(4) Output impedance ... 220
Ω
8.1.1.4 Coil Change
M system
L system
E60 E68
{ {
{ {
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
M system
E60 E68
{ {
{ {
L 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.
- 70 -
8.1.2 Speed Control
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.2.1 Constant Surface Speed Control
M system
E60 E68
{
{
{
{
L 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
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.
8.1.2.2 Spindle Override
M system
E60 E68
{
{
{
{
L 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 (number 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.
- 71 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.2.3 Multiple-spindle Control
Multi-spindle control is a function that controls the sub-spindle for a machine tool equipped with the second spindle (sub-spindle) in addition to the first spindle (main spindle).
Multi-spindle control I can be switched to multi-spindle control II or vice versa using a parameter and, by so doing, the spindle control method changes.
Multi-spindle control I: Control based on a spindle selection command (such as G43.1) and spindle control command ([S*****;] or [SO=*****;]), etc.
Multi-spindle control II: Control based on an external signal (spindle command selection signal, spindle selection signal) and spindle control command ([S*****;] only), etc.
Spindle selection commands [SO=*****;] cannot be used for this control.
Tool post 1
- 72 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.2.3.1 Multiple-spindle Control I
M system
E60 E68
–
–
{
{
L system
(1) Spindle selection command
With the spindle selection command (such as G43.1 [G group 20]), it is possible to switch the spindles between 1st spindle and 2nd spindle and determine as to which one of the two axes the subsequent S command (S*****) is applied to.
Command format
G43.1; First spindle control mode ON
G44.1; Selected spindle control mode ON; the selected spindle number is set using a parameter.
G47.1; All spindles simultaneous control mode ON
(2) Spindle control command (Using extended word address (S
{=****))
In addition to using the "S*****" S commands, it is also possible to assign commands in which the
1st spindle and 2nd spindle are differentiated by using the S○=*****.
Command format
S
{=*****;
{
: Number assigned as the spindle number (1: first spindle; 2: second spindle); variables can be designated.
***** : Rotational speed or surface speed value assigned by 5-digit analog command; variables can be designated.
8.1.2.3.2 Multiple-spindle Control II
M system
L system
E60 E68
–
{
–
{
With this function, one S command is used to command to the spindle, and which spindle is selected is decided depending on a signal from the PLC.
A parameter is used to switch between multi-spindle control II and the conventional multi-spindle control I function.
Spindle command selection, spindle selection
The S command for the spindle is output as the rotation speed command to the spindle which has been selected by the spindle selection signal ON from the PLC. The selected spindle rotates at the rotation speed that was output. The spindles that were de-selected by spindle selection signal
OFF continue to rotate at the same rotation speed as the speed immediately before their deselection. As a result, each of the spindles can be made to rotate simultaneously at a different rotation speed.
- 73 -
8.1.3 Position Control
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.3.1 Spindle Orientation
M system
E60 E68
Δ
Δ
{
{
L 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.)
(c) Pre-positioning orient (spindle orient 2)
When the in-position pre-positioning parameter is valid and the second in-position is valid, this function turns ON the orient finish signal as soon as the spindle reaches within the prepositioning in-position width. It also turns ON the second in-position signal as soon as the spindle reaches within the orient in-position width. (OINP) actually.
Since orient completion can be predicted using this function, it is possible to eliminate the sequence delay time, etc. for tool changes and other such operations, thereby achieving a faster tact time.
8.1.3.2 Spindle Position Control (Spindle / C Axis Control)
M system
E60 E68
Δ
Δ
{
{
L system
This function enables one digital spindle (SP) to be used also as the C axis (rotary axis) using an external signal.
The C axis servo ON signal is used to switch between the spindle and C axis.
Spindle C axis
Spindle
Servo ON
At servo OFF: ---------- Spindle (C axis cannot be controlled).
C axis is in the reference position return incomplete status.
At servo ON: ----------- C axis (spindle cannot be controlled).
C axis is in the reference position return incomplete status.
A parameter is used to initiate reference position return (orient) when servo ON is started
.
- 74 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.3.3 Spindle Synchronization
8.1.3.3.1 Spindle Synchronization I
E60 E68
M system
L system
–
–
–
{
In a machine with two spindles, this function controls the rotation speed and phase of one spindle
(synchronized spindle) in synchronization with the rotation of the other 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 Hh1 Dd1 Rr1 Aa1 ;
Hh1
Dd1
Rr1
Aa1
: Selects the basic spindle.
: Selects the spindle to be synchronized with the basic spindle.
: Designates the synchronized spindle phase shift amount.
: Designates the spindle synchronization acceleration/deceleration time constant.
- 75 -
8. Spindle, Tool and Miscellaneous Functions
8.1 Spindle Functions (S)
8.1.3.3.2 Spindle Synchronization II
M system
E60 E68
–
–
{
{
L system
In a machine with two spindles, this function controls the rotation speed and phase of one spindle
(synchronized spindle) in synchronization with the rotation of the other 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.
8.1.3.11 Spindle Holding Power Improvement
M system
E60 E68
Δ {
Δ {
L system
Spindle holding force can be increased when the spindle holding force up request signal is turned
ON by ladders while the spindle is stopped for orientation function or spindle/C-axis selected, etc.
When the spindle holding force up request signal is turned ON, the system changes the gain and validates disturbance observer. As a result, the spindle holding force is increased.
Lathe milling, such as D cutting and eccentric drilling, is possible by the spindle holding force up.
For inquiries about spindle drive unit compatible with this function, contact MITSUBISHI.
(Note 1) Depending on the size of load applied to the spindle during machining, a mechanism in which the spindle is mechanically locked may be required. In such a case, consider mounting a mechanical lock on the spindle in advance when designed.
- 76 -
8. Spindle, Tool and Miscellaneous Functions
8.2 Tool Functions (T)
8.2 Tool Functions (T)
8.2.1 Tool Functions
M system
L system
(1) M system
E60 E68
{
{
{
{
When an 8-digit number following address T (T00000000 to 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) This function requires a built-in PLC.
(Note 2) There are some screens that cannot display all eight digits.
(2) L system
The command is issued with an 8-digit number following address T (T0 to T99999999).The highorder 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.
Txxxxxxxx
Tool offset No.
Tool No.
Txxxxxxxx
Tool offset No.
Tool No.
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) This function requires a built-in PLC.
(Note 2) There are some screens that cannot display all eight digits.
- 77 -
8. Spindle, Tool and Miscellaneous Functions
8.3 Miscellaneous Functions (M)
8.3 Miscellaneous Functions (M)
8.3.1 Miscellaneous Functions
M system
E60 E68
{ {
{ {
L system
When an 8-digit number (M00000000 to M99999999) is assigned following address M, the 8-digit code data and start signal are output to PLC.
M2-digit BCD output is used for the standard PLC specifications.
When a 2-digit number following address M (M00 to 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 M00 to M97.
M98 and M99 have specific purposes and can not be used.
8.3.2 Multiple M Codes in 1 Block
M system
E60 E68
{
{
{
{
L system
Four sets of M commands can be issued simultaneously in a block.
Apart from the above signals, various special independent signals are also output for the following signals.
Respective processing and completion sequences are required for all M commands included in a block (except M98 and M99). transferred simultaneously as the M command in the same block from the controller to the
PLC, and so high-speed machine control can be done by the PLC processing sequence.
- 78 -
8. Spindle, Tool and Miscellaneous Functions
8.3 Miscellaneous Functions (M)
8.3.3 M Code Independent Output
M system
E60 E68
{
{
{
{
L system
When the M00, M01, M02 or M30 command is assigned during an automatic operation (tape, 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
M00
M01
M02
M30
M code output
Independent
M00
M01
M02
M30
Response to controller
Fin1 or Fin2
Fin1 or Fin2
Reset & rewind
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
M system
E60 E68
{ {
{ {
L 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.
Command
Next block
Miscellaneous function strobe (MF)
Miscellaneous function finish signal
(FIN1)
- 79 -
8. Spindle, Tool and Miscellaneous Functions
8.4 2nd Miscellaneous Functions (B)
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.
Command
Next block
Miscellaneous function strobe (MF)
Miscellaneous function finish signal
(FIN2)
8.4 2nd Miscellaneous Functions (B)
8.4.1 2nd Miscellaneous Functions
M system
L system
E60 E68
{ {
{ {
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) This function requires a built-in PLC.
(Note 2) There are some screens that cannot display all eight digits.
- 80 -
9. Tool Compensation
9. Tool Compensation
9.1 Tool Length / Position Offset
9.1.1 Tool Length Offset
M system
L system
E60 E68
{ {
{ {
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) M system
G43
G44
Zz1
Zz1
Hh1
Hh1
Offset direction
G49 ;
Offset axis
No.
;
;
The offset direction is determined by the G command.
G43: Forward direction (z1 + h1)
G44: Reverse direction (z1 – h1)
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.).
Tool length offset cancel
Offset can be canceled by the following G commands.
G49;
G43 H0;
G44 H0;
(Note) When the tool length offset axis is returned to the reference position, the offset of that axis is canceled.
(Example) Example of tool length offset using a combination with tool length measurement type I
G28 X0 Y0 Z0 ;
T01 ;
T02 M06 ;
G91 G00 G43
Z2.0 H01 ;
(Note) The tool length offset amount is set as a negative value such as
H01 = –450.000.
M
H01 =
– 450.000
Workpiece
Table
Z 0.0
Z + 2.0
M
H01 =
– 450.000
Z 2.0
Workpiece
Table
- 81 -
9. Tool Compensation
(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.
The programmed base position is the center of the tool rest:
The programmed base position is the nose of the base tool:
Base position
(base point)
Base tool
X-axis tool length offset
Tool used for machining
X-axis tool length offset
Z-axis tool length offset
Z-axis tool length offset
(b) Wear offset
The wear of a tool nose can be offset.
X
Tool nose
X-axis tool nose wear offset amount
Z-axis tool nose wear offset amount
Z
- 82 -
9. Tool Compensation
(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* * * * * * * *
Tool length offset No. and tool nose wear offset No.
Tool No.
T* * * * * * * *
Tool length offset No. and tool nose wear offset No.
Tool No.
2. Specifying tool length and wear offset Nos. separately
T* * * * * * * *
Tool nose wear offset No.
Tool length offset No.
Tool No.
T
* * * * * * * *
Tool nose wear offset No.
Tool length offset No.
Tool No.
The tool offset for the lathe is valid only for the X and Z axes. If the 3rd axis (Y axis) is added, the tool offset will be validated for the 3rd axis.
With E68, whether to set the additional axis tool offset for the 3rd axis or 4th axis can be changed by the parameter.
- 83 -
9. Tool Compensation
9.1.2 Tool Position Offset
M system
L system
E60 E68
–
–
{
–
This function uses commands to control the movement by changing the positions of the end points of the movement commands to positions which have been extended or reduced by an amount equivalent to the tool compensation amount.
This function can be used to compensate for the difference in distance between the position where the tool on the machine is actually mounted and the programmed coordinate position based on the tool position and thereby improve the efficiency of both machining and operation.
G45 G00 Xx1 Yy1 Dd1 ;
G45
Xx1, Yy1
Dd1
: Tool position offset command
: Movement axes
: Offset No.
With tool position offset, the offset operation is performed only for blocks containing a G45 to G48 command.
G45 command
Extension by amount equivalent to offset amount
G46 command
Reduction by amount equivalent to offset amount
G47 command G48 command
Extension by twice the offset Reduction by twice the offset amount amount
Program command
Program command
Program command
Program command
Actual movement amount
Actual movement amount
Actual movement amount
Actual movement amount
(1) If the start and end points are on an axis, the radius can be extended or reduced only for onequarter, one-half and three-quarter arcs.
(2) In the case of absolute commands, the position is extended or reduced in each axial direction from the end point of the previous block along the line of the movement toward the position commanded in the block containing the G45 (or G46, G47 or G48) command.
(3) In the case of simultaneous n axes command, the same amount of offset is applied to all the axes that have the command within the range of the number of the axes which can be simultaneously controlled. Tool position offset is also valid for additional axes.
9.1.3 Tool Offset for Additional Axes
E60 E68
M system
L system
–
{
–
{
Tool compensation for the L series is valid for the X and Z axes. If an additional axis (such as the Y axis) has been added to these axes, tool compensation is valid for the additional axis.
- 84 -
9. Tool Compensation
9.2 Tool Radius
9.2.1 Tool Radius Compensation
M system
E60 E68
{ {
L 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
Tool center path r r r: Tool radius compensation amount
Programmed 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 G00 G41 Xx1 Yy1 Dd1 ;
G17 : Compensation plane
G41
Xx1.Yy1
Dd1
: Left compensation
: Movement axis
: Offset 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
- 85 -
9. Tool Compensation
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
Ii1, Jj1
Dd1
: Movement amount
: Compensation vector direction
: Compensation vector length
The tool radius compensation vector direction is updated by I and J.
Tool center path
Holding of previous intersection point vector
N12
N13
N11
Intersection point vector
Vector with length D (i14, j14)
N14
N15
N11G01Xx11;
N12G38Xx12Yy12;
N13G38Xx13Yy13;
N14G38Xx14Ii14Jj14Dd14;
N15G40Xx15Yy15;
The tool radius compensation is canceled by the following command.
G40 Xx1 Yy1 Ii1 Jj1 ;
Xx1, Yy1
Ii1, Jj1
: Movement amount
: Compensation vector direction
- 86 -
9. Tool Compensation
The vector prior to canceling is prepared by calculating the intersection point with the I and J direction.
Tool center path
When i and j commands are assigned to G40
N14
N11
N12
N13
N11G01Xx11;
N12Xx12Yy12;
N13Xx13Yy13;
N14G40Xx14Ii14Jj14;
(i14,J14)
- 87 -
9. Tool Compensation
9.2.3 Tool Nose Radius Compensation (G40/41/42)
E60 E68
M system
L 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
Compensated path
Programmed 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.
- 88 -
9. Tool Compensation
9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40)
E60 E68
M system
L 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 point
Tool nose direction
Tool nose point
Tool nose progress direction
1 2
3
4
Tool nose progress direction
5
6
7 8
R R
L L
R L
R
L L
R L
L R R L
L
R
R
R L
R R
L
L
R
L
L L
L
R
R
R
L
R
R
R
R
L
L
L
R
R
R
R
L
L
L L
Range of each tool nose point
(1 to 4)
Range of each tool nose point
(5 to 8)
- 89 -
9. Tool Compensation
9.3 Tool Offset Amount
9.3.1 Number of Tool Offset Sets
The number of tool offset sets is as follows.
80 sets
E60 E68
M system –
{
–
{
L system
200 sets
M system
E60 E68
{
–
– – L system
400 sets
M system
L system
E60 E68
–
–
{
–
- 90 -
9. Tool Compensation
9.3.2 Offset Memory
9.3.2.1 Tool Shape/Wear Offset Amount
M system
L system
E60 E68
{
{
{
{
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 [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.
- 91 -
9. Tool Compensation
(b) Type 2: 1-axis offset amounts/with wear offset [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 Wear offset amount when the type 1 tool length offset amount (Offset types I and II are available for handling offset amounts.)
Offset type I Offset type II using type 2
M
M
M
Tool radius compensation amount
Tool radius compensation amount
Tool length wear offset t
Tool length offset amount
Z0.0
Tool length offset amount
Z0.0
Workpiece
W
Workpiece
Table
Table
Tool radius wear compensation amount
(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)
Base position
(base point)
Base tool
Tool used for machining
Z-axis tool length offset amount
X-axis tool length offset amount
Z-axis tool length offset amount
- 92 -
9. Tool Compensation
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.
X
Tool nose center
Tool nose
Nose radius compensation amount
Imaginary tool nose point
X-axis tool length wear offset
Z-axis tool length wear offset
Z
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.
- 93 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10. Coordinate System
10.1 Coordinate System Type and Setting
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.
L
0
G52
L
0
G52
W
0
－
54
G54
G55
W
0
－
55
G92
M
0
EXT
R ref
Offset set with parameters L
0
G52
Local coordinate system zero point
Local coordinate system offset
*1)
Offset set with program
W
0-54
Workpiece coordinate system zero point (G54) (0 when power is turned ON)
W
0-55
Workpiece coordinate system zero point (G55)
G54 Workpiece coordinate system (G54) offset
*1)
G55 Workpiece coordinate system (G55) offset
G92
EXT
M
0
G92 coordinate system shift
External workpiece coordinate offset
Machine coordinate system zero point
*1)The G52 offset is available independently for G54 to G59.
- 94 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.1 Machine Coordinate System
M system
E60 E68
{
{
{
{
L 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 position 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
G90
: Coordinate system selection
: Incremental/absolute commands
G00 : Movement mode [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 that is effective only in the block where it is assigned. The workpiece coordinate system being selected is not changed by this command.
Machine coordinate system (G53)
M
1st reference position
Workpiece coordinate system 1
W1
G53 G90 G00 X0 Y0 ;
- 95 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.2 Coordinate System Setting
M system
E60 E68
{
{
{
{
L 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 move, 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.
Offset of coordinate system by G92 coordinate system setting
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)
G92 offset amount
Machine coordinate system
X : x0–x1
Y : y0–y1
M
New W1 y1
W1 y0 x1 x0
Machine position
The shifted coordinate system is returned to its original position by dog-type reference position return or the program.
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
M
M
Machine coordinate system
New W1
Machine coordinate system
y'
x’
Tool position
W1
G92
Xx1
Yy1 y1
x1
G92 command position
Old W1
- 96 -
10. Coordinate System
10.1 Coordinate System Type and Setting
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) Dog-type reference position 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
M system
E60 E68
{
{
{
{
L system
When the tool has arrived at the reference position by means of the first manual or automatic dog type reference position 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 points
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.
- 97 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.4 Workpiece Coordinate System Selection (6 sets)
M system
E60 E68
{
{
{
{
L 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)
G54
: (Absolute value command)
: Coordinate system selection
G00 : Movement mode
Xx1, Yy1, Zz1 : Coordinate positions of movement destination
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 from the screen
2.Setting using commands assigned from the machining program
3.Setting from the user PLC
Machine coordinate system (G53)
M
W2
Workpiece coordinate system 2
(G55)
W1
Workpiece coordinate system 1 (G54)
Start
G90 G56 G00 X0 Y0 ;
Workpiece coordinate system 4
(G57)
W4
W3
Workpiece coordinate system 3 (G56)
- 98 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.5 Extended workpiece coordinate system selection (48 sets) G54.1P1 to P48
M system
E60 E68
{
{
{
{
L 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 ;
G54.1Pn
G00
: Coordinate system selection
: Movement mode
Xx1, Yy1, Zz1 : Coordinate position 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.
- 99 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.6 Workpiece Coordinate System Preset (G92.1)
E60 E68
M system
L system
–
–
–
{
This function presets the workpiece coordinate system, which has been shifted by the programmed command or the manual operation, as the workpiece coordinate system which has been offset by the programmed command (G92.1) from the machine zero point by an amount equivalent to the workpiece coordinate offset amount.
The workpiece coordinate system is shifted from the machine coordinate system when such operations or programmed commands as below have been performed.
• When manual intervention has occurred in the manual absolute OFF status
• When a movement command was performed in the machine lock status
• When movement was initiated by handle interrupt
• When a movement command was performed in the mirror image mode
• When a local coordinate system was set using the G52 command
• When a workpiece coordinate system was shifted using the G92 command
Just as when manual reference position return has been performed, this function presets the workpiece coordinate system that has been shifted once to the workpiece coordinate system that has been offset from the machine zero point by an amount equivalent to the workpiece coordinate offset amount.
Furthermore, whether to preset relative coordinates as well is selected with a parameter.
Command format
G92.1 (G50.3) X0 Y0 Z0
α0 ; (where α is an additional axis)
Designate the addresses of the axes to be preset.
Axes whose addresses have not designated will not be preset.
Depending on the command type, G50.3 command is used in stead.
A program error results when a value other than 0 is commanded.
- 100 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.7 Local Coordinate System
M system
E60 E68
{
{
{
{
L 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.
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
G52
: Workpiece coordinate selection
: Local coordinate 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 position return.
Machine coordinate system (G53)
M
L1
Local coordinate
G54 G52 y1 x1
Workpiece coordinate 1
(G54)
W1
- 101 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.8 Coordinate System for Rotary Axis
M system
E60 E68
{
{
{
{
L system
The axis designated as the rotary axis with the parameters is controlled with the rotary axis' coordinate system.
The rotary axis includes the rotating type (short-cut valid/invalid) and linear type.
The display range is 0 to 359.999° for the rotating type and 0 to ±99999.999° for the linear type.
The range of each coordinate system is 0 to ±359.999° for the rotating type and 0 to ±99999.999° for the linear type.
The rotary axis is commanded with a degree (°) unit regardless of the inch or metric designation.
The rotary axis type is common for all rotary axes and can be set with the parameters.
Rotary axis
Rotating type rotary axis
Linear axis
Short-cut invalid Short-cut valid
Linear type rotary axis
Workpiece coordinate position
Machine coordinate position
/relative position
Displayed in the range of 0° to 359.999°.
Displayed in the range of 0° to 359.999°.
Displayed in the range of 0° to
±99999.999°.
Displayed in the range of 0° to
±99999.999°.
ABS command
INC command
The incremental amount from the end point to the current position is divided by 360°, and the axis moves by the remainder amount according to the sign.
The incremental amount from the end point to the current position is divided by 360°, and the axis takes a shortcut to moves by the remainder amount.
In the same manner as the normal linear axis, moves according to the sign by the amount obtained by subtracting the current position from the end point (without rounding up to 360°.).
Moves in the direction of the commanded sign by the commanded incremental amount starting at the current position.
Reference position return
Follows the absolute/relative command for a movement to the interim position.
Returns to the reference position from the
Moves and returns in the reference interim position within a 360° movement. position direction for the difference from the interim position to the reference position.
- 102 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.9 Plane Selection
M system
E60 E68
{
{
{
{
L 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. ;
G17 X100. R50. ;
With these program commands, X100. is the axis which does not exist on the G19 (Yp, Zp) plane, YpZp are selected by G19 and the X axis moves by 100. mm separately from the plane selection.
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.
- 103 -
10. Coordinate System
10.1 Coordinate System Type and Setting
10.1.10 Origin Set
M system
E60 E68
{
{
{
{
L system
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)]
X -150.345 X -150.345
Y - 12.212
Z - 1.000
A - 0.000
Y - 12.212
Z - 1.000
A - 0.000
X
Y
C.B
CAN
C.B
CAN
Z
C.B
CAN
[POSOTION]
X 0.000
Y 0.000
Z 0.000
A 0.000
[WORK(G54)]
X 0.000
Y 0.000
Z 0.000
A 0.000
When axes are set to "0" in order, the Y and Z axis can be set by pressing without pressing
Y
and
Z
keys.
C.B
CAN
key successively
10.1.11 Counter Set
M system
L system
E60 E68
{ {
{ {
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.
- 104 -
10. Coordinate System
10.2 Return
10.2 Return
10.2.1 Manual Reference Position Return
M system
E60 E68
{ {
{ {
L system
This function enables the tool to be returned manually to the position (reference position) that is characteristic to the machine.
(1) Return pattern to reference position
(a) Dog type
Creep speed
Reference position return speed
Dog
R
Dog
R
1
When starting in same direction as final advance direction
(b) High-speed type
When starting in opposite direction
as final advance direction
Rapid traverse rate
Dog
R
(2) Differences according to detection method
Incremental position detection method
Absolute position detection method
First return after power ON Second return and following
Dog-type High-speed
High-speed High-speed
- 105 -
10. Coordinate System
10.2 Return
10.2.2 Automatic 1st Reference Position Return
M system
E60 E68
{
{
{
{
L system
The machine can be returned to the first reference position 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 position.
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
G28
G29
Function
Automatic 1st reference position return
Start position return (The tool first returns to the interim position of the 1st reference position return start from the 1st reference position, and then is positioned at the position designated in the program.)
The G28 programming format is given below.
G28 Xx1 Yy1 Zz1 ;
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 position.
The G29 programming format is given below.
G29 Xx1 Yy1 Zz1 ;
Xx1, Yy1, Zz1 : Return control axes (assigned position)
The tool is first moved by rapid traverse to the interim position that is passed through with G28 or
G30, and is then positioned by rapid traverse at the position assigned by the program.
1st reference point
R
–X
G28
Non - interpolation movement
G28
Interpolation or non - interpolation can be selected
Interim point
G29
G29
Interpolation or non – interpolation can be selected
–Y
- 106 -
10. Coordinate System
10.2 Return
If the position detector is for the incremental detection system, the first reference position 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 position return pattern is the same as for manual reference position return.
(Note 2) The number of axes for which reference position return can be performed simultaneously depends on the number of simultaneously controlled axes.
(Note 3) If, at the time of the first reference position 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 position 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 position, 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 position 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.
- 107 -
10. Coordinate System
10.2 Return
10.2.3 2nd, 3rd, 4th Reference Position Return
M system
E60 E68
{
{
{
{
L system
As with automatic 1st reference position return, commanding G30Pn during automatic operation enables the tool to be returned to the set points (2nd, 3rd or 4th reference positions) characteristic to the machine. The 2nd, 3rd and 4th reference positions can be set by parameters.
G code
G30 P2
G30 P3
G30 P4
Function
2nd reference position return
3rd reference position return
4th reference position return
The G30 programming format is given below.
G30 Xx1 Yy1 Zz1 Pp1 ;
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 position.
2nd reference point
1st reference point
–X
G30 P2
Start point
Interim point
G30 P3
G30 P4
3rd reference point
–Y
4th reference point
(Note 1) The second reference position return is performed if the P command is omitted.
(Note 2) The number of axes for which reference position return can be performed simultaneously depends on the number of simultaneously controlled axes.
(Note 3) If, at the time of the reference position 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.
- 108 -
10. Coordinate System
10.2 Return
(Note 4) If, at the time of the reference position return, the tool length offset has not been canceled, it will be canceled and the offset amount also cleared upon completion of reference position 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 positions.
(Note 6) The machine will not stop at the interim point even when a single block is selected.
10.2.4 Reference Position Verification
M system
E60 E68
{
{
{
{
L system
By commanding G27, a machining program, which has been prepared so that the tool starts off from the reference position and returns to the reference position, can be checked to see whether the tool will return properly to the reference position.
The G27 programming format is given below.
G27 Xx1 Yy1 Zz1 Pp1 ;
Xx1, Yy1, Zz1 : Return control axes
Pp1 : No.
P1 : 1st reference position verification
P2 : 2nd reference position verification
P3 : 3rd reference position verification
P4 : 4th reference position verification
The assigned axis is first positioned by rapid traverse to the commanded position and then, if this is the reference position, the reference position arrival signal is output.
When the address P is omitted, the first reference position verification will be applied.
(Note 1) The number of axes for which reference position 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 position upon completion of the command.
(Note 3) Whether interpolation or non-interpolation is to apply to the movement can be selected using a parameter.
- 109 -
10. Coordinate System
10.2 Return
10.2.5 Absolute Position Detection
M system
L system
E60 E68
Δ Δ
Δ Δ
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 position return. (High-speed return will always be used for the reference position return command.)
For the absolute position detection method, there are two methods such as the dog-type and dogless type according to how the zero point is established.
Method
Dog-type
Dog-less type
Marked point method stopper method
Details
Same method as incremental detection dog-type
The zero point position is set from the screen. established by pressing the machine against a set point on the machine.
Establishment of zero point
Zero point is established with dogtype reference position return completion.
The zero point is established by input from the zero point initialization screen.
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.
Adjustment of zero point position
The data is set in the parameter of zero point shift amount.
The value equivalent to the shift amount is set in the zero point initialization screen.
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.
- 110 -
10.2.6 Tool Exchange Position Return
10. Coordinate System
10.2 Return
M system
E60 E68
{
{
{
{
L 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
[M system]
G30.1
G30.2
G30.3
G30.4
G30.5
G30.6
Z axis
→ X axis • Y axis
(
→ additional axis)
Z axis
→ X axis → Y axis ( → additional axis)
Z axis
→ Y axis→ X axis
(
→ additional axis)
X axis
→ Y axis • Z axis
(
→ additional axis)
Y axis
→ X axis • Z axis
(
→ additional axis)
X axis
• Y axis • Z axis
(
→ additional axis)
[L system]
G30.1
G30.2
G30.3
G30.4
G30.5
X axis only
Z axis only
(
→ additional axis)
(
→ additional axis)
X axis
→ Z axis
(
→ additional axis)
Z axis
→ X axis
(
→ additional axis)
X axis
• Z axis
(
→ additional axis)
(Note1) 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" indicates that the Z axis returns to the tool change position, then the X axis does.
(Note2) G30.6 is only for the 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.
- 111 -
10. Coordinate System
10.2 Return
10.2.7 C Axis Reference Position Return
E60 E68
M system
L system
–
Δ
–
{
This function is used to carry out the position control for the spindle with the axis motor, and applied to the machine that can switch the spindle motor connected with the spindle to the axis motor.
The C axis (rotation axis) is generally used for the axis motor, and the specification will be the same as the normal C axis control after switching.
As for the reference position return during the C axis connection, either the normal dog-type reference position return with the C axis or the Z-phase pulse type reference position return with the spindle encoder can be selected with parameter.
Dog type (with C axis detector)
Reference position return met hod
Z-phase pulse type
(with spindle encoder)
(Supplements)
(1) Reference position return method
The Z-phase pulse type is applied in the first reference position return after the servo OFF for the C axis (generally means changing to the spindle). The high-speed type is applied in the
(second or later) reference position return after the Z-phase pulse type reference position return.
(2) Z-phase pulse type reference position return
When there is the reference position return command, the spindle is rotated until the Z-phase pulse of the spindle encoder is detected, and then stopped. (Figure 1 (1))
Encoder gear ratio 1:1 The Z-pulse is detected within one rotation.
Encoder gear ratio 1:2 The Z-pulse is detected within two rotations.
Next, in order to catch the change of the pulse position and improve the accuracy of the remaining distance, the spindle is rotated with G28crp (approach speed) and then stopped again. (Figure 1 (2))
Set as follows: Standard value G28crp = 8 (°/min) (Encoder gear ratio 1:1)
For the spindle, one rotation to the point where the Z-pulse is detected is made with G28rap
(G28 rapid traverse rate). (Figure 1 (3)) This point is applied to the reference position. If the reference position shift amount is included, the spindle is rotated to the point of the figure 1 (4) and then stopped.
Spindle encoder Z-phase pulse
G28crp
G28rap
G28rap
(1) (2) (3) (4)
Base shift amount
(one rotation of spindle)
G28sft
Figure 1 Z-phase pulse type reference position return
- 112 -
(1)
Spindle
10. Coordinate System
10.2 Return
(3)
(2)
(2)
Spindle
(1)
(3)
(1) G28rap
(2) G28crp
(3) G28rap
(a) (b)
Figure 2 Operation of spindle
With the figure 2 (a), the rotation of the spindle that the G28 rapid traverse is performed in the forward direction (the same direction as the parameter #2030) is looked from the front. With the figure 2 (b), the rotation of the spindle that the G28 rapid traverse is performed in the opposite direction (the opposite direction to the parameter #2030) is looked from the front.
(3) High-speed type reference position return
After the Z-phase pulse type reference position return, the high-speed type reference position return is applied in the second or later reference position return.
G28rap
Figure 3 High-speed type reference position return
- 113 -
11. Operation Support Functions
11.1 Program Control
11. Operation Support Functions
11.1 Program Control
11.1.1 Optional Block Skip
M system
E60 E68
{
{
{
{
L 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 OFF Switch ON
N1
N2
N3
/N4
/N5
N6
N7
N1
N2
N3
N4
N5
N6
N7
N1
N2
N3
N6
N7
: : :
- 114 -
11. Operation Support Functions
11.1 Program Control
11.1.3 Single Block
M system
E60 E68
{
{
{
{
L 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 (SBK)
~ ~
Automatic operation start
(ST)
G01 X1000…
~ ~
G01 Z100…
~ ~
G01 Z1000…
Movement block
~ ~
SBK ON at start
INVALID
SBK change during movement
VALID
SBK ON after block completion
VALID
- 115 -
11. Operation Support Functions
11.2 Program Test
11.2 Program Test
11.2.1 Dry Run
M system
E60 E68
{ {
{ {
L 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
G00, G27, G28, G29, G30, G60
G01, G02, G03
Rapid traverse selection switch OFF
Manual feed rate
Manual feed rate
Rapid traverse selection switch ON
Rapid traverse rate
Cutting clamp speed
11.2.2 Machine Lock
M system
E60 E68
{
{
{
{
L system
Operation can be executed with the machine in the servo lock status for that axis when the machine lock input signal is turned ON.
The feed rate in the machine lock status is the command speed.
The M, S, T and B commands are executed as usual and operation is completed by returning the
FIN signal.
(1) Reference position return (manual, G28, G29, G30) is controlled as far as the interim point in the machine lock status but the block is completed when the interim point is reached.
(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.
All axes will be simultaneous with the standard PLC.
- 116 -
11. Operation Support Functions
11.2 Program Test
11.2.3 Miscellaneous Function Lock
M system
E60 E68
{
{
{
{
L 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 that 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.
11.2.4 Graphic Check
M system
E60 E68
{ {
{ {
L system
The movement path of the machine tool can be monitored and traced, and the path of machining programs can be traced and checked using the check and tracing functions based on processing inside the controller.
This function enables the tool path of machining programs to be traced without operating any functions.
For the display mode, 1-plane, 2-plane and 3-dimensional display are provided. In the 3dimensional display mode, cubic shapes can be rotated and tracing of the figure seen from the desired direction can be assigned.
11.2.5 Graphic Trace
M system
L system
E60 E68
{ {
{ {
The machine position of the machine tool is traced. By this operation, the actual movement path in automatic operation or manual operation is traced.
For the display mode, 1-plane, 2-plane and 3-dimensional display are provided. In the 3dimensional display mode, cubic shapes can be rotated and tracing of the figure seen from the desired direction can be assigned.
- 117 -
11. Operation Support Functions
11.3 Program Search / Start / Stop
11.3 Program Search / Start / Stop
11.3.1 Program Search
M system
E60 E68
{ {
{ {
L 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
M system
E60 E68
{ {
{ {
L 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.
- 118 -
11. Operation Support Functions
11.3 Program Search / Start / Stop
11.3.3 Collation Stop
M system
L system
E60 E68
–
{
– {
This function enables the single block stop status to be established at any block without having to set the SINGLE BLOCK switch to ON.
It can be used to readily check the machining shape up to the designated block and resume machining.
(Example)
O100:
G91;
……
G00 Z-150.;
N100 G81 X-100. Z-100. R-50. F100;
N101 X-100.
N102 X-100.
N103 Y100.
N104 X100.
N105 X100.
……
……
4 5 6
3 2 1
Yes
する
Check subsequent machining shapes?
加工条件（工具長補正量等）修正 length offset amount, etc.). previous collation stop position.
照合停止設定ブロックで照合停止
Collation stop at block in which
Measure and check the machining shape?
前回照合停止位置から加工再開 previous collation stop position.
しない
1個目の加工形状から加工開始 machining shape of the first work.
する
- 119 -
11. Operation Support Functions
11.3 Program Search / Start / Stop
11.3.4 Program Restart
M system
E60 E68
{
{
{
{
L system
When a machining program is to be resumed after it has been suspended midway due to tool damage or for some other reason, this function searches the program and the block to be resumed and enables machining to be resumed from the block. When multiple part systems are used, only for 1-part system, the program can be resumed.
There are two resumption methods, type 1 and type 2.
Resumption type 1
Machining is resumed by type 1 if feed hold has been performed due to tool damage, etc. or if resetting has been performed.
(a) Type A (standard specification)
The designated sequence No. and block No. are searched only in the designated program No..
In case of the standard specification, the program No. cannot be omitted.
The program No. cannot be input since the main program which has been searched itself serves as the target. (A setting error results if the program No. is input.)
The designated sequence No. and block No. are searched in all the programs (including subprograms) among the searched programs.
Resumption type 2
(a) Type A (standard specification)
If, before a resume search is initiated for the machining program to be resumed, a machining program differing from that program was run in the tape or memory mode, the machining program to be resumed will be resumed using type 2. It is also resumed using type 2 in cases where the coordinate system to be used when machining is resumed is to be changed from the coordinate system used during the previous automatic operation.
The operation sequence for type 2 is the same as for type 1. However, the coordinate system settings and other operations that must be performed before running the machining program must all be performed before initiating the resume search. The main program to be resumed should be searched at any time up to the moment immediately prior to starting the resumption of the machining.
The designated sequence No. and block No. are searched only in the designated program No..
In case of the standard specification, the program No. cannot be omitted.
If, before a resume search is initiated for the machining program to be resumed, a machining program differing from that program was run in the tape or memory mode, the machining program to be resumed will be resumed using type 2. It is also resumed using type 2 in cases where the coordinate system to be used when machining is resumed is to be changed from the coordinate system used during the previous automatic operation.
The operation sequence for type 2 is the same as for type 1. However, the coordinate system settings and other operations that must be performed before running the machining program must all be performed before initiating the resume search.
The program No. cannot be input since the main program which has been searched itself serves as the target. (A setting error results if the program No. is input.)
Therefore, the main program to be resumed must be searched before the resume search is initiated. The designated sequence No. and block No. are searched in all the programs
(including sub-programs) among the searched programs.
- 120 -
11. Operation Support Functions
11.3 Program Search / Start / Stop
11.3.5 Automatic Operation Start
M system
E60 E68
{
{
{
{
L system
With the input of the automatic operation start signal (change from ON to OFF), the automatic operation of the program, which has been operation searched, is started by the controller (or the halted program is restarted).
Automatic operation start (ST)
G01 X 100...
G01 Z 100...
Movement block
11.3.6 NC Reset
M system
E60 E68
{ {
{ {
L system
This function enables the controller to be reset.
2
Reset 1
Retained
Tool compensation data Retained
Reset 2
Initialized
Canceled
(no operations)
Reset & Rewind
Initialized
Canceled
4 Errors/alarms Reset Reset Reset
5 M, S and T code outputs Retained Retained Retained
OFF OFF OFF
6
M code independent output
Control axis moving
7
Decelerated and stopped
Decelerated and stopped
Decelerated and stopped
8
Output signals "In reset" signal "In reset" signal "In reset" signal
"In rewind" signal
- 121 -
11. Operation Support Functions
11.3 Program Search / Start / Stop
11.3.7 Feed Hold
M system
E60 E68
{
{
{
{
L 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
M system
E60 E68
{ {
{ {
L 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.
- 122 -
11.4 Interrupt Operation
11. Operation Support Functions
11.4 Interrupt Operation
11.4.1 Manual Interruption
M system
E60 E68
{ {
{ {
L system
Manual interrupt is a function that enables manual operations to be performed during the 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 simultaneous operation of manual and automatic modes in section 11.4.9.)
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 manual absolute mode
ON/OFF in section 11.4.3).
- 123 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.2 Automatic Operation Handle Interruption
M system
E60 E68
{
{
{
{
L 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 the 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 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
X
Y
Z
1
10
100
Interrupt
Workpiece
Handle feed
Automatic feed
X
_
Y
_
;
X
_
Y
_
;
Z
_
Y
_
;
Feed path with automatic feed and handle feed superimposed
- 124 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.3 Manual Absolute Mode ON / OFF
M system
E60 E68
{
{
{
{
L system
The program absolute positions 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.
X
W
Feed hold stop
Programmed path
(absolute command)
Manual interrupt
(Program absolute position is updated by an amount equivalent to traveled value.)
Path after manual interrupt
Tool passes along same path as that programmed.
–Y
With manual absolute switch ON
W
Feed hold stop
X
Programmed path
(absolute command)
Manual interrupt
(Program absolute position is not updated even if axis moves)
Path after manual interrupt
–Y
Path is shifted by an amount equivalent to manual interrupt value.
(Zero point moves.)
With manual absolute switch OFF
The switch ON state will be entered when the power is turned ON.
- 125 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.4 Thread Cutting Cycle Retract
M system
L system
E60 E68
– –
– {
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.
Position where the block following the thread cutting is completed
Suspension position
Chamfering angle
θ
Feed hold
Period when thread cutting is performed
- 126 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.5 Tapping Retract
M system
E60 E68
{
{
{
{
L 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.
- 127 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.6 Manual Numerical value Command
M system
E60 E68
{
{
{
{
L system
On the screen, 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.
S command value
S 3600
T 12
M 5
Manual numerical value
T command value
M command value
PLC sequence processing
S
T
M
7
4
1
–
8
5
2
0
9
6
3
•
Input
(Note) The input operation starts the execution of the M, S or T command.
11.4.8 MDI Interruption
M system
E60 E68
{
{
{
{
L 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.
- 128 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.9 Simultaneous Operation of Manual and Automatic Modes
M system
E60 E68
{
{
{
{
L system
This function enables manual operations to be performed during automatic operation by selecting an automatic operation mode (tape, MDI or memory) and manual mode (handle, step, jog or manual reference position return) simultaneously.
(Arbitrary feed based on the PLC is also possible.)
Axis switching
Tape
Automatic mode
Memory
MDI
Automatic operation
X
Y
Axis control
Z
X-axis posi-tion control
Simultaneous manual and automatic operation Y-axis posi-tion control
Manual mode
Jog
Handle
Return
Manual operation
X
Y
Axis control
Z
Z-axis posi-tion 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
M system
L system
E60 E68
{ {
{ {
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.
- 129 -
11. Operation Support Functions
11.4 Interrupt Operation
11.4.11 Reference Position Retract
M system
E60 E68
{
{
{
{
L 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 position.
The reference position to be retracted to can be selected from the 1st reference position to 4th reference position with 2-bit input signal.
Set the retracting order of axes with parameter (#2019 revnum).
(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 position 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 cannot be resumed.
(f) The retract signal is invalid the coordinate system is not established. An operation error will occur when the retract signal is input in such case.
11.4.14 PLC Interruption
M system
L system
E60 E68
–
{
– {
The interrupt program set with the R register is executed with the signals from the PLC during single block stop in program operation or during the manual mode.
- 130 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.1 Program
12.1.1.1 Subprogram Control
E60 E68
M system
L system
{
{
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
Pp1
Hh1
Ll1
: Call command
: Subprogram number
: Sequence number
: Number of repetitions
(Branch to subprogram)
Op1 (Subprogram)
:
Nh1
:
M99 ; (Return to main program)
Subprograms can be nested up to eight levels deep.
Main program:
Level 0 (P1000)
Main program:
Level 1 (P1)
Main program:
Level 2 (P2)
…
Main program:
Level 8 (P8)
P8
M98 P1
M98 P3;
M99;
•
•
•
M99;
M02/M30 ;
M98 P2
M99;
- 131 -
12. Programming Support Functions
12.1 Machining Method Support Functions
A subprogram branch destination or repetition of a subprogram can be specified.
Specifying a subprogram branch destination
Main program
Subprogram
P1000 P1
N1;
M98 P1 H1;
M99;
N100;
Specifying repetition of a subprogram
P1000
Main program
Five repetitions
M98 P1 L5;
M98 P1 H100;
M02/M30;
M99;
M02/M30;
M99;
Return after five repetitions
- 132 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.1.3 Scaling
M system
E60 E68
{ {
L system – –
The shape commanded by the program can be extended or reduced to the desired size by applying a scale factor to the movement axis command position.
G code
G50
G51
Function
Scaling cancel
Scaling ON
The program format is given below.
G51 Xx1 Yy1 Zz1 Pp1 ;
G51 : Call command
Xx1, Yy1, Zz1 : Scaling center coordinate position
Pp1 : Scale factor
The scale factor ranges from 0.000001 to 99.999999 times. y1
Y sc s1 p1 s1,s2,s3 : Shape after scaling s3 s2 p2 p3 x1
X
(Note 1)
Scaling cannot be applied to compensation amount for tool radius compensation, tool position offset, or tool length compensation, etc. (The compensation and offset are calculated for the scaled shape.)
(Note 2)
Scaling applies only to the axes commanded with G51 block; it does not apply to axes that have not been commanded.
When the scale factor is not assigned, the parameter setting applies instead.
- 133 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.2 Macro Program
12.1.2.1 User Macro
E60 E68
M system { 4 layers { 4 layers
L system { 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 that 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
Ll1
Argument
: No. of repetitions
: Variable data assignment
The macro program is called immediately by this command.
G66 Pp1 Ll1 Argument ;
G66 : Call command
Ll1
Argument
: No. of repetitions
: 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
Ll1
Argument
: No. of repetitions
: Variable data assignment
The macro program is executed with the word data of each block as the argument.
- 134 -
12. Programming Support Functions
12.1 Machining Method Support Functions
The following macro command functions are available.
Arithmetic commands
Assignment of priority of arithmetic operations
Control commands
#1 = <Expression> ;
Various arithmetic operations can be conducted between variables by the above.
"<Expression>" is a combination of constants, variables, functions and operators.
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.
(1) IF [<Conditional expression>] GOTO n ;
(2) WHILE [<Conditional expression>] DO m ;
⋅ ⋅ ⋅
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 <Argument> ;
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.
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. [M system].)
Up to 800 codes from G200 to G999 can be used in this command. [L system]
- 135 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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.
Neither the codes basically required by the machine nor M codes M0, M1, M2, M30, M96 to M99 are to be entered.
(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.)
12.1.2.2 Machine Tool Builder Macro
12.1.2.2.1 Machine Tool Builder Macro SRAM
M system
E60 E68
– {
L system – {
This function enables macro programs exclusively designed for use by the machine builders to be registered in addition to the regular macro programs. These macros can be called from user programs using the same method as the one used for regular macros. Machine builder macros can be locked, preventing them from being viewed unless the key word is input.
Machine builder macro programs are stored in a dedicated area which means that the user program registration area is not reduced in the process.
Call format 1
G65 Pp1 Ll ;
P l
: Machine builder macro program number (0100001000 – 0199999998)
: Number of repetitions
Note:
Machine builder macros cannot be called using the G66, G66.1 or M98 command.
Call format 2
G*** ;
*** : G code defined in macro definition program
- 136 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.2.3 Macro Interruption
M system
E60 E68
{ {
L 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.
Machining program Opm:
The user macro interrupt signal is accepted during this period.
The user macro interrupt signal is not accepted during this period.
Interrupt signal
:
:
M96Ppi;
:
:
:
:
:
:
:
M97 ;
:
:
:
:
:
:
:
:
M02 ;
Interrupt program Opi
:
:
:
:
:
:
:
:
M99 ;
The modal information is restored to the status applying before interrupt.
- 137 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.2.4 Variable Command
E60 E68
M system { 200 { 300
L system { 200 { 300
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.
200 sets #100 ~ #199, #500 ~ #599
• Variable names can be set for #500 ~ #519.
Variable expressions
Variable : # Numerical value
(Numerical value: 1, 2, 3, .....)
: # [Expression]
#100
#100
: Variable
: Expression Operator Expression
: – (minus) Expression
: [Expression]
: Function [Expression]
Variable definition
#100 + #101
–#120
[#110]
SIN [#110]
Variable = expression
(Note 1)
Variables cannot be used with addresses "O" and "N".
- 138 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3 Fixed Cycle
List of fixed cycles
Type of fixed cycle
Fixed cycle for drilling
M system L system
G code G code system
2
G code system
3
G code system
6
G code system
7
Remarks system
1
G70 G80 G80 G80 G80
: : : : :
Refer to 4.5.3.
G89 G89 G89 G89 G89
G79 G83.2
G79 G83.2
G98 G98 G98 G98 G98
G99 G99 G99 G99 G99
Special fixed cycles
Fixed cycles for turning machining
Multiple repetitive fixed cycles for turning machining
G35
― ― ― ―
G36
―
G92 G78 G92 G78
G94 G79 G94 G79
G70 G70 G70 G70
: : : :
―
G76 G76 G76 G76
G76.1
G76.1
G76.1
G76.1
G76.2
G76.2
G76.2
G76.2
- 139 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.1 Fixed Cycle for Drilling
M system
E60 E68
{ {
L system { {
(1) M series ; 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
G74 Reverse tapping cycle
G75
G76 Fine
G77
G78
G79
G80 Fixed cycle cancel
G81 Drilling, spot drilling cycle
G82 Drilling, counterboring cycle
G83 Deep hole drilling cycle
G84 Tapping
G85 Boring
G86 Boring
G87 Backboring
G88 Boring
G89 Boring
There are two levels of hole machining axis return which apply upon completion of the fixed cycle machining operation.
G code
G98
Function
Initial point level return
G99 R point level return
- 140 -
12. Programming Support Functions
12.1 Machining Method Support Functions
The basic program format for the fixed cycle commands is shown below.
G81 Xx1 Yy1 Zz1 Rr1 Qq1 Pp1 Ll1 Ff1 ;
G81
Xx1, Yy1
Zz1
Rr1
Qq1
Pp1
Ll1
: Hole drilling mode
: Hole position data; X-axis, Y-axis hole drilling position command
(rapid traverse) (incremental/absolute)
: Hole machining data; Hole bottom position designation (incremental/absolute)
: Hole machining data; Hole R point designation (incremental/absolute)
: 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
: Hole machining data; Dwell time at hole bottom
: Hole machining data; Number of fixed cycle repetitions
For details on the synchronous tapping cycle (including pecking tapping cycle and deep-hole tapping cycle), refer to the section "4.5.3 Synchronous tapping".
- 141 -
Initial point
G73
Step cycle
G98 mode
R point q q n
G99 mode
12. Programming Support Functions
12.1 Machining Method Support Functions
G74
Reverse tapping cycle
G98 mode
Initial point
M04
R point
G76
Fine boring cycle
G98 mode
Initial point
R point q q
Z point
M03
Z point q
M19 Shift
G99 mode
G81
Drilling, spot drilling cycle
Initial point
R point
Z point
G98 mode
G99 mode
Initial point
R point
G82
Z point
Dwell
Z point
Drilling, counterboring cycle
G98 mode
G99 mode
G83
Deep hole drilling cycle
G98 mode
Initial point
R point q n q
G99 mode
G84
Tapping cycle
G98 mode
Initial point
R point
M03
Z point
M04
G85
Boring cycle
G98 mode
Initial point
R point
Z point
Initial point
R point
G86
Boring cycle
Z point
M05
M03
G98 mode
M03
Z point
G87
Back boring cycle
M19
Initial point
R point
M19
Z point
M03
G88
Boring cycle
Initial point
R point
M03
M03
Z point
M05
Dwell
G98 mode
G89
Boring cycle
Initial point
R point
Z point
Dwell
G98 mode
- 142 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(2) L series ; 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
In-position check
Dwell
Rapid traverse feed
Deep-hole drilling cycle1
G84 Z Cutting
In-position check
Dwell
Spindle CCW
In-position check
Dwell
In-position check
Dwell
Cutting feed
Cutting feed
Rapid traverse feed
Tapping cycle
(Reverse tapping cycle)
Boring cycle
Deep-hole drilling cycle1
G88 X Cutting
In-position check
Dwell
Spindle CCW
Cutting feed Tapping cycle
(Reverse tapping cycle)
In-position check
Dwell
Cutting feed Boring cycle
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.
- 143 -
12. Programming Support Functions
12.1 Machining Method Support Functions
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
G87/G88/G89
Xx1, Cc1
: Fixed cycle mode of drilling (G83, G87), tapping (G84, G88), or boring
(G85, 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.
: 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
Kk1 the data is required.
: 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)
Mm1
Ss1
,Ss1
Dd1
,Rr1
: 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.
: Designates spindle rotation speed (When the spindle that is not analog is mounted)
: Designates spindle rotation speed of return speed (When the spindle that is not analog is mounted)
: Designates tap spindle NO. for G84 (G88) speed (When the spindle that is not analog is mounted)
: Changes between synchronous/asynchronous in G84 (G88) speed
(When the spindle that is not analog is mounted)
- 144 -
12. Programming Support Functions
12.1 Machining Method Support Functions
The drilling cycle motions generally are classified into the following seven.
Motion 1
Motion 1
Initial point
Motion 3
R point
Motion 7
Motion 4
Motion 6
Motion 5
If the "positioning axis in-position width" is designated, the in-position check is conducted upon completion of the block.
Motion 1 : Rapid positioning up to the initial point of X (Z) and C axes.
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.
- 145 -
12. Programming Support Functions
12.1 Machining Method Support Functions
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 q q n
Z point / X point
R point
G99 mode
Initial point
G98 mode
Z / X point
G99 mode
G83.2
Deep-hole drilling cycle
G98 mode
Initial point
R point
G84/88
Tapping cycle
(C-axis clamp)
Reverse rotation of spindle/rotary tool
G85/89
Boring cycle
Dwell
Dwell
Dwell
(C-axis clamp) f
2f
Dwell
Dwell
Dwell
Z / X point
Dwell
Dwell
Z / X point
R point
Initial point
G98 mode
(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
Z / X point
R point
Initial point
G 98 mode
(C-axis unclamp)
Dwell
O utput 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
- 146 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.2 Special Fixed Cycle
M system
E60 E68
{ {
L 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
θ 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
θ Kn ;
Xx, Yy
Ir
J
θ
Kn
: Center position of bolt hole circle; this is affected by the G90/G91 commands.
: Radius "r" of circle; it is based on the least input increment and is provided using a positive number.
: Angle
θ at point to be drilled initially; the counterclockwise direction is taken to be positive.
: 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
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 ;
X1 = 200 mm n = 6 holes
20
°
I = 100 mm
Y1 = 100 mm
Position prior to excution of G34 command
W
(500 mm, 100 mm)
G0 command in
N005
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.
- 147 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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
θ 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
θ Kn ;
Xx, Yy
Id
J θ
Kn
: The starting point coordinates; they are affected by the G90/G91 commands.
: 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.
: Angle θ; the counterclockwise direction is taken to be positive.
: Number "n" of holes to be drilled including the starting point; any number of holes from 1 through 9999 can be assigned.
(Example)
Y d =100mm
With 0.001 mm least input increment
G91 ;
G81 Z – 10.000 R5.000 L 0 F100 ;
G35 X200.000 Y100.000 I100.000
J 30.000 K5;
θ
=30°
N=5 holes
X y
1
=100mm
W
Position prior to execution of G35 command
X
1
=200mm
- 148 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(3) Arc (G36)
The tool starts at the point forming angle θ 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 Δ
θ. 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
θ PΔθ Kn ;
Xx, Yy
Ir
: Center coordinates of arc; they are affected by the G90/G91 commands.
: Radius "r" of arc; it is based on the least input increment and is provided with a
Kn positive number.
J
θ : be positive.
PΔ θ :
Δθ; when it is positive, the tool drills in the counterclockwise direction and when it is negative, it drills in the clockwise direction.
: Number "n" of holes to be drilled; any number of holes from 1 through 9999 can be assigned.
(Example)
With 0.001 mm least input increment
N001 G91;
N002 G81 Z-10.000 R5.000 F100;
N003 G36 X300.000 Y100.000 I300.000 J10.000
P 15.000 K6;
Position prior to execution of G36 command n=6 holes
Δθ
=15°
θ
=10°
Y
1
=100mm
W
X
1
=300mm
- 149 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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 Δx 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 IΔx Pnx JΔy Kny ;
Xx, Yy
IΔx
Pnx
JΔy
Kny
: The starting point coordinates; they are affected by the G90/G91 commands.
: X-axis interval Δx; it is based on the least input increment; when Δx 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.
: Number of holes "nx" in the X-axis direction; any number of holes from 1 through
9999 can be assigned.
: Y-axis interval Δy; it is based on the least input increment; when Δy 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.
: Number of holes "ny" in the Y-axis direction; any number of holes from 1 through
9999 can be assigned.
(Example)
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 ;
Position prior to execution of
G37.1 command ny=8 holes
W y1=100mm
Δy=
100mm x1=300mm
Δx=50mm nx=10 holes
- 150 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.3 Fixed Cycle for Turning Machining
E60 E68
M system – –
L 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
G78 Thread cutting cycle cutting
Format:
GΔΔ 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
- 151 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(1) Longitudinal cutting cycle (G77)
Straight cutting in the longitudinal direction can be performed consecutively by the following block:
G77X/U_Z/W_F_ ;
X axis
4 (R)
3 (F)
1 (R)
U
2
(R) : Rapid traverse feed
(F) : Cutting feed
Z
2 (F)
W
X
Z axis
Taper cutting in the longitudinal direction can be performed consecutively by the following block:
G77X/U_Z/W_R_F_ ;
X axis
4 (R)
3 (F)
2 (F)
1 (R)
U
2
(R) : Rapid traverse feed
(F) : Cutting feed r
Z W
X
Z axis r: Taper part depth (radius designation, incremental value, sign is required)
- 152 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(2) Thread cutting cycle (G78)
Straight thread cutting can be performed by the following block:
G78X/U_Z/W_F/E_ ;
X axis
(R) : Rapid traverse feed
(F) : F or E code designation
Z
4 (R)
3 (R)
2 (F)
W
1 (R) U
2
X
Z axis
(b) Taper thread cutting
Taper thread cutting can be performed by the following block:
G78X/U_Z/W_R_F/E_ ;
X axis (R) : Rapid traverse feed
(F) : F or E code designation
4 (R)
3 (R)
1 (R)
2 (F)
U
2 r
Z
W
X
Z axis r: Taper part depth (radius designation, incremental value, sign is required)
- 153 -
12. Programming Support Functions
12.1 Machining Method Support Functions
Chamfering
θ
α : 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.
θ : 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
°.
α
(3) Face cutting cycle (G79)
Straight cutting in the end face direction can be performed consecutively by the following block:
G79X/U_Z/W_F_ ;
X axis
1(R)
2(F)
4(R) u / 2
(R): Rapid traverse feed
(F): Cutting feed
3(F)
Z
W
X
Z axis r: Taper part depth (radius designation, incremental value, sign is required)
- 154 -
12. Programming Support Functions
12.1 Machining Method Support Functions
Taper cutting in the end face direction can be performed consecutively by the following block:
G79X/U_Z/W_R_F_ ;
X axis
Z r
2(F)
1(R)
3(F)
W
4(R) u / 2
(R): Rapid traverse feed
(F): Cutting feed
X
Z axis r: Taper part depth (radius designation, incremental value, sign is required)
- 155 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining
E60 E68
M system – –
L system { {
(a) Longitudinal rough cutting cycle I (G71)
The finish shape program is called, and straight rough cutting is 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
Re
Aa
Pp
Uu
Ww
: Cut depth d. (When P,Q command is not given). (Modal)
: Retract amount e. (Modal)
: Finish shape program No. (If it is omitted, the program being executed is assumed to be designated.)
: Finish shape start sequence No. (If it is omitted, the program top is assumed to be designated.)
: 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.
: Finishing allowance in the X axis direction. (When P, Q command is given).
(Diameter or radius designation)
: Finishing allowance in the Z axis direction.
Ss : speed.
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)
(R) d Cut depth
X
Details of retract operation
(R)
(F)
45
° e
(F)
Z
W u / 2
Finishing allowance
- 156 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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
Re
Aa
Pp
: Cut depth d. (When P,Q command is not given). (Modal)
: Retract amount e. (Modal)
: Finish shape program No. (If it is omitted, the program being executed is assumed to be designated.)
: Finish shape start sequence No. (If it is omitted, the program top is assumed to be designated.)
: Finish shape end sequence No. (If it is omitted, the program end is assumed to be designated.)
Uu
However, if M99 precedes the Q command, up to M99.
: Finishing allowance in the X axis direction.
Ww : Finishing allowance in the Z axis direction. (When P, Q command is given.)
Ss :
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. d
Cut depth
S
(Cycle commanded point)
Details of retrace operation
(F) e
(R)
X
45
°
(F)
Z
E
W u / 2
Finishing allowance
- 157 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(c) Molding material in rough cutting cycle (G73)
The finish shape program is called. Intermediate path is automatically calculated and rough cutting is 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 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.
Pp : Finish shape start sequence No.
Qq : Finish shape end sequence No.
Uu : Finishing allowance in the X axis direction u
Ww : Finishing allowance in the Z axis direction w
Ff : Cutting feed rate (F function)
Ss : Spindle speed (S function)
Tt : Tool selection (T function)
(If it is omitted, the present program is assumed to be designated.)
(If it is omitted, the program top is assumed to be designated.)
(If it is omitted, the program end is assumed to be designated.)
However, if M99 precedes the Qq command, up to M99.
• 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.
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.
X
E
Z
13
19
6
18
12
17
11
5
16
10
4
7
3
15
9
A w k + w
S
2
S
1
S
S
3
1
2
14
8 i + u/2 u/2
- 158 -
12. Programming Support Functions
12.1 Machining Method Support Functions
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
P
Q
: Finish shape program number. (If it is omitted, the program being executed is assumed to be designated.)
: Finish shape start sequence number. (If it is omitted, the program top is assumed to be designated.)
: 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
:
N100 G70 P200 Q300 ;
N110
N120
:
N200
:
N300
N310
:
Finish shape program
N200 … ;
:
N300 ･･ ;
(Example 2)
Program No. designation
:
N100 G70
A100 ;
N110 ･････ ;
:
O100
G01 X100 Z50 F0.5 ;
M99 ;
:
In either example 1 or 2, after the N100 cycle is executed, the N110 block is executed.
- 159 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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
X/U
Z/W
Pi
Qk
Rd
Ff
: Retract amount e (when X/U, Z/W command is not given) (Modal)
: B point coordinate (absolute/incremental)
: B point coordinate (absolute/incremental)
: Tool shift amount (radius designation, incremental, sign not required)
: Cut depth k (radius designation, incremental, sign not required)
: 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.)
: Feed rate z w
(11) i
(10)
(9)
(8) d
(7)
(6)
(5)
(4)
(3)
(2)
(1)
S (start point)
(12) u/2
• (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. e
B x k k k k
- 160 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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
X/U
Z/W
Pi
Qk
Rd
Ff
: Retract amount e (when X/U, Z/W command is not given) (Modal)
: B point coordinate (absolute/incremental)
: B point coordinate (absolute/incremental)
: Tool shift amount (radius designation, incremental, sign not required)
: Cut depth k (radius designation, incremental, sign not required)
: 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.)
: Feed rate z w i i i i
B e d
S (start point)
(12)
(2)
(4)
(3)
(1)
(5)
(11)
(6)
(7)
(8)
(9) u / 2 k
(10) x
- 161 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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 QΔd Fl ;
m r a
: Cut count at finishing 01 to 99 (modal)
: Chamfering amount 00 to 99 (modal). Set in 0.1-lead increments.
: Nose angle (included angle of thread) 00 to 99 (modal) Set in 1-degree increments. d : (modal)
X/U
Z/W
: 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 axis end point coordinate of thread part. i
Designate the Z coordinate of the end point in the thread part in an absolute or incremental value.
: Taper height constituent in thread part (radius value). When i = 0 is set, straight screw is made. k
Δd
: Thread height. Designate the thread height in a positive radius value.
: Cut depth. Designate the first cut depth in a positive radius value.
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. z w
S
(6) (1)
(5) u/2
(4)
(2)
(3)
(i) k x r
When Ri is negative a°/2
- 162 -
12. Programming Support Functions
12.1 Machining Method Support Functions
z w
S
(6)
(1) k u/2 x
(5) r
(4)
(2)
(3) k i a°/2
When Ri is positive a°
Δ d
First time
Second time
Δ
√
Δ
√
nth time d (finishing allowance)
(Cut "m" times at finishing)
- 163 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.5 Multiple Repetitive Fixed Cycle for Turning Machining (Type II)
E60 E68
M system – –
L system – {
Pocket shapes can be machined in the longitudinal rough cutting cycle (G71) and face rough cutting cycle (G72).
Command format (This is a command format when the G71 is commanded. The G72 command is based on the G71 command.)
G71 Ud Re Hh ;
← (can be omitted when values set in parameters are used)
G71 Aa Pp Qq Uu Ww Ff Ss Tt ;
<H0: Used for finished shapes without pockets> <H1: Mainly used for finished shapes with pockets>
G71 Ud Re H0;
G71 Pp Qq . .; q
(R)
Rough cutting start point
(f)
(R)
(R/f) d
G71 Ud Re H1;
G71 Pp Qq . .; q
(f)
(R)
Rough cutting start point
(R)
(R/f) d
X
(f)
(R)
45 °
(f) e
Z p u/2 w
X
(f)
(R) e
Hole bottom
Z p u/2 w
Hh : Pocket machining (modal) ... reversible parameter ("G71 pocket machining")
0: Select this only for finished shapes without hollow areas (pockets).
* With the beginning of the pockets, the tool is pulled up in the 45-degree direction with each cycle until the finished shape is finally traced.
1: This can be selected regardless of whether the finished shape has hollow (pocket) parts or not.
* A method that traces the finished shape with each cycle is used for the beginning of the pockets.
- 164 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.3.7 Fixed Cycle for Drilling (Type II)
E60 E68
M system – –
L system { {
In the longitudinal hole drilling fixed cycle, the X axis is designated as the hole drilling axis.
However, in the longitudinal hole drilling fixed cycle (type II), the Y axis can be designated as the hole drilling axis with the longitudinal hole drilling axis selection function.
The relationship between the longitudinal hole drilling axis selection signal’s ON/OFF state and the hole drilling axis of the fixed cycle for drilling is shown below.
G87
G code Details
G80 Cancel
G83
G84 (G84.1)
G88 (G88.1)
G83.2
Deep hole drilling cycle 1
Tapping cycle
Deep hole drilling cycle 1
Tapping cycle
Deep hole drilling cycle 2
Y axis cross tap function selection signal state
-
ON
Hole drilling axis
-
Z
OFF
ON
OFF
ON
Z
Z
OFF
ON Y
OFF X
ON Y
OFF X
ON Y
OFF X
ON Z/X
OFF
- 165 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.4 Mirror Image
12.1.4.1 Mirror Image by Parameter Setting
M system
E60 E68
– {
L system – {
A parameter is used to designate the axis for which the mirror image function is to be executed before the machining program is run. When mirror image is set to ON by the parameter, an operation that is symmetrical on the left and right or at the top or bottom is performed. Each axis has its own parameter.
12.1.4.2 External Input Mirror Image
M system
E60 E68
– {
L system – {
Signals from an external device (PLC) to request the mirror image operation either while a machining program is running or before it is run. When ON has been set for mirror image from an external device, an operation that is symmetrical on the left and right or at the top or bottom is performed. Each axis has its own request signal.
- 166 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.4.3 G Code Mirror Image
M system
E60 E68
{ {
L 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.
G code Function
G50.1 G code mirror image cancel
G51.1 G code mirror image ON
The program format for the G code mirror image is shown below.
G51.1 Xx1 Yy1 Zz1 ;
G51.1 : 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 : 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
Original shape (program)
Shape achieved when machining program for the left side has been executed after the mirror command
Mirroring axis
X
- 167 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.5 Coordinate System Operation
12.1.5.1 Coordinate Rotation by Program
M system
E60 E68
{ {
L 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
Xx1, Yy1
Rr1
: Rotation center coordinates
: Angle of rotation
(元のローカル
座標系)
(Rotated local coordinate system)
(回転したローカル座標系)
(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.
- 168 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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 ;
Y
200.
100.
Actual machining shape
(Programmed coordinate)
W
100.
200.
X
300.
- 169 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.6 Dimension Input
12.1.6.1 Corner Chamfering / Corner R
M system
E60 E68
{ {
L 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 rounding I
When ",C" or ",R" is commanded for linear interpolation, corner chamfering or corner rounding can be inserted between linear blocks.
• Corner chamfering
Example:
• Corner rounding
Example:
N1 G01 Xx1 Zz1, Cc1 ;
N2 Zz2 ;
N1 G01 Xx1 Zz1, Rr1 ;
N2 Zz2 ;
N2 c 1 c 1
N1
N2 r 1
N1
(Note 1)
If a corner chamfering or corner rounding command is issued specifying a length longer than the N1 or N2 block, a program error occurs.
- 170 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(2) Corner chamfering / corner rounding II (L system)
When ",C" or ",R" is command in a program between linear-circular, corner chamfering or corner rounding can be inserted between blocks.
(a) Corner chamfering II (Linear – circular)
Example:
G01 X_Z_ ,Cc1 ;
G02 X_Z_ Ii1 Kki ;
Hypothetical corner intersection
Cc1
Cc1
Chamfering end point
(2)
(1)
Chamfering start point
(b) Corner chamfering II (Circular - linear)
Example:
G03 X_Z_ Ii1 Kk1 ,Cc1 ;
G01 X_Z_ ;
Hypothetical corner intersection
Cc1
Cc1
Chamfering start point
(1)
(2)
Chamfering end point
(c) Corner chamfering II (Circular - circular)
Example:
G02 X_Z_ Ii1 Kk1 ,Cc1 ;
G02 X_Z_ Ii2 Kk2 ;
Hypothetical corner intersection
Cc1
Chamfering end point
(2)
(1)
Cc1
Chamfering start point
- 171 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(3) Corner rounding
(a) Corner R II (Linear - circular)
Example:
G01 X_Z_ ,Rr1 ;
G02 X_Z_ Ii1 Kk1 ;
Corner rounding start point
Hypothetical corner
intersection
(1)
Corner rounding end point
Rr1
(2)
(b) Corner R II (Circular – linear)
Example:
G03 X_Z_ Ii1 Kk1 ,Rr1 ;
G01 X_Z_ ;
Corner rounding end point
Hypothetical corner intersection
(2)
Rr1
Corner rounding start point
(1)
(c) Corner R II (Circular – circular)
Example:
G02 X_Z_ Ii1 Kk1 ,Rr1 ;
G02 X_Z_ Ii2 Kk2 ;
Hypothetical corner intersection
(1)
Corner rounding start point
Rr1
Corner rounding start point
(2)
- 172 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(4) Specification of corner chamfering / corner rounding speed E
An E command can be used to specify the speed for corner chamfering or rounding.
This enables a corner to be cut to a correct shape.
(Example)
F
E
G01 X_Z_ ,Cc1 Ff1 Ee1 ;
X_Z_ ;
F
F
E
G01 X_Z_ ,Rr1 Ff1 Ee1 ;
X_Z_ ;
X
F
Z
An E command is a modal and remains effective for feeding in next corner chamfering or rounding.
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 rounding.
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).
- 173 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(5) Corner chamfering / corner rounding (I, K designation) (L system)
With this command format, by means of parameter settings, corners are chamfered using the "I",
"K" or "C" address without a comma, and corners are rounded using the "R" address.
The ",C" and ",R" commands with commas can also be used.
(a) Corner chamfering (I, K designation)
Corners are chamfered using the "I_", "K_" or "C_" address with no comma. Corners can be chamfered to any angle. Signs, if they are provided for the corner chamfering commands, are ignored.
Command format
N100 Xx/Uu Zz/Ww Ii/Kk/Cc ;
N200 Xx/Uu Zz/Ww ;
X/u
Z/w i/k/c
: X-axis end point coordinate
: Z-axis end point coordinate
: The length from the hypothetical corner intersection to the chamfering start point or chamfering end point is designated using the I, K or C address.
X axis
N200
Chamfering end point
Chamfering start point
N100 i, k, c
Hypothetical corner intersection i, k, c
0 Z axis
• If multiple "I", "K" or "C" addresses or duplicated addresses have been designated in the same block, the last command will take effect.
• If both corner chamfering and corner rounding commands are present in the same block, the last command will take effect.
• If "C" is used as the name of an axis, corner chamfering commands cannot be designated using the "C" address.
• If "C" is used as a 2nd miscellaneous function, corner chamfering commands cannot be designated using the "C" address.
• Corner chamfering commands using the "I" or "K" address cannot be designated in an arc command block. "I" and "K" are the arc center commands.
- 174 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(b) Corner rounding (I, K designation)
Corners are rounded using the "R_" address with no comma. Corners can be rounded to any angle. Signs, if they are provided for the corner rounding commands, are ignored.
N100 Xx/Uu Zz/Ww Rr ;
N200 Xx/Uu Zz/Ww ;
x/u z/w r
: X-axis end point coordinate
: Z-axis end point coordinate
: Radius of corner rounding arc
X axis
Corner rounding end point
N200 r
N100
Hypothetical corner intersection
Corner rounding start point
0
Z axis
• If both corner chamfering and corner rounding commands are present in the same block, the last command will take effect.
• Corner rounding commands using the "R" address cannot be designated in an arc command block. "R" is the arc radius command.
- 175 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.6.2 Linear Angle Command
M system
E60 E68
{ {
L system { {
The end point coordinates are automatically calculated by assigning one element (one component of the selected plane) of the end point coordinates and the linear angle.
G17 Xx1 Aa1 ; or G17 Yy1 Aa1 ;
Xx1, Yy1 : 1 element of the end point coordinate
Example
G17 G91 X100. A60. ;
Y
Start point
60°
X100.
End point
(Automatically calculated with operation)
Y
X
(Note 1)
If the axis "A" or 2nd miscellaneous function "A" is used, address "A" is treated as the axis "A" command or the 2nd miscellaneous function, respectively.
- 176 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.6.3 Geometric Command
M system
E60 E68
{ {
L 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
x1
2
X
N1 G01 Aa1 Ff1 ;
N2 Xx1 Zz1 Aa2 ;
End point (X1, Z1) a: Angle (
°) formed between straight line and horizontal axis on plane.
The plane is the selected plane at this point.
N2 a 2
Automatic intersection N 1 point calculation a1
Start point
W 1
Z1
Z
(Note 1)
This function cannot be used when using the A axis or 2nd miscellaneous function A.
- 177 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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)
A r1
(p1,q1)
B’(?,?)
(p2,q2) r2
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
B(?,?)
B(?,?) a1
(p2,q2)
I and K
P and Q
H = 0
H = 1
:
:
:
A
Incrimental coordinates from circular end point
Absolute center coordinates of circular arc
Intersection with shoter line
:
Intersection with longer line
C(xc, zc)
- 178 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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 ;
B’(?,?)
A
(p1,q1) r1
B(?,?) a1
C(xc, zc)
I and K
P and Q
:
Incrimental coordinates from circular end point
:
Absolute center coordinates of circular arc (L3 only)
H = 0
H = 1
:
Intersection with shoter line
:
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 ;
C(xc, zc) r1
B (?,?) a1
A
- 179 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(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 ;
B (?,?)
A r1 a1
C(xc, zc)
- 180 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.6.4 Polar Coordinate Command
M system
E60 E68
– {
L system – –
With this function, the end point position is commanded with the radius and angle.
Command format
G16 ;
Polar coordinate command mode ON
G15 ;
Polar coordinate command mode OFF
Example of program
G1x ;
G16 ;
G9x G01 Xx1 Yy1 F2000 ;
:
Plane selection for polar coordinate command (G17/G18/G19)
Polar coordinate command mode ON
Polar coordinate command
G9x : Center selection for polar coordinate command (G90/G91)
G90
…
G91
…
The workpiece coordinate system zero point is the polar coordinate center.
The present position is the polar coordinate center. x1 : 1st axis for the plane
…
The radius commanded y1 : 2nd axis for the plane
…
The angle commanded
Y
G15 ;
Commanded position (end point) x1 y1
Plus
Minus
Present position
X
For G90/G17(X-Y plane)
Polar coordinate command mode OFF
- 181 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.7 Axis Control
12.1.7.1 High-speed Machining
12.1.7.1.3 High-speed Machining Mode III
E60 E68
M system – Δ
L system – –
This function runs machining programs, in which free-form curved surfaces have been approximated by fine-segments, at high speed.
It is effective in increasing the speed at which dies with free-form curved surfaces are machined.
High-accuracy machining can be achieved by using this function in combination with the highaccuracy control function.
Command format
G05 P3 ;
High-speed machining mode III ON
G05 P0 ;
High-speed machining mode III OFF
Example of program
G28 X0. Y0. Z0. ;
G91 G00 X-100. Y-100. ;
G01 F3000 ;
G05 P3 ; …. High-speed machining mode III ON
X0.1 ;
X0.1 Y0.001 ;
X0.1 Y0.002 ;
G90 G00 X0 Y0 Z0 ;
G02 X__Y__R__F__ ;
Rapid traverse
Absolute modal R-designated arc
G03 X__Y__I__J__F__ ; y
Incremental modal linear cutting
Arc y y
G05 P0 ;
M02;
…. High-speed machining mode III OFF
(1) The following G codes can be used in the high-speed machining mode III:
G00, G01, G02, G03, G90, G91, G17, G18 and G19.
(2) In the high-speed machining mode III, only the axis names, movement amounts (no variables or arithmetic operations), F commands and I/J/K/R/P commands can be designated.
(Comments can be used.)
(3) The machining speed may be compromised depending on the number of characters in a block.
- 182 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.7.2 Chopping
12.1.7.2.1 Chopping
M system
E60 E68
– {
L system – {
This function continuously raises and lowers the chopping axis independently of the program operation when workpiece profiles are to be cut. It can be used for grinding operations using machining centers, for instance.
Which of the axes is to serve as the chopping axis is set by a parameter ahead of time.
(1) Chopping action
Wheel
Chopping action
Workpiece
- 183 -
12. Programming Support Functions
12.1 Machining Method Support Functions
The chopping operation is initiated by setting the upper dead point position, lower dead point position and number of cycles (number of up/down movements per minute) and pressing the chopping start switch.
Note 1:
The upper dead point position, lower dead point position and number of cycles are set and the start and stop commands are designated by input signals from the user PLC.
Note 2:
The setting for the number of cycles differs according to the motor, inertia and other factors.
The chopping operation is performed as follows.
Base position
Upper dead point
Lower dead point
Start
Rapid traverse
Stop
Rapid traverse
(a) The axis moves from the base position to the upper dead point by rapid traverse.
(b) Next, the axis moves repeatedly from the upper dead point to the lower dead point and then from the lower dead point to the upper dead point. (Sinusoidal waveforms)
The feed rate is tailored to achieve the number of cycles set for the up/down motion.
Chopping override
Override in 1% increments from 0% to 100% can be applied to the chopping operation.
Note:
Bear in mind that the override increment differs according to the machine specifications.
- 184 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.7.5 Circular Cutting
M system
E60 E68
{
Function
CW
( clockwise
)
CCW (counterclockwise)
{
L 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
G12
G13
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
4
Radius of circle
5
Y
0
3
7
1
X
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)
1.Circular cutting is undertaken on the plane which has been currently selected (G17, G18 or
G19).
2.The (+) and (–) signs for the compensation amount denote reduction and expansion respectively.
3.When [radius (I) – compensation amount] is zero or negative, the alarm results to indicate an error in the circular cutting radius.
Offset amount
2
6
- 185 -
12.1.9 Data Input by Program
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.9.1 Parameter Input by Program
M system
E60 E68
{ {
L system { {
The parameters set from the screen 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
N Data No.
H Bit type data ;
P Major classification No. A Axis N Data No.
D Byte type data ;
P Major classification No. A Axis N Data No.
S Word type data ;
P Major classification No. A Axis 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 (axiscommon 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.
(Note 4)
Command G10L50 and G11 in independent blocks. A program error will occur if not commanded in independent blocks.
(Note 5)
Depending on the G90/G91 modal status when the G10 command is assigned, the data is used to overwrite the existing data or added.
- 186 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.9.2 Compensation Data Input by Program
M system
E60 E68
{ {
L 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)
G10 L20 Pn Extended workpiece coordinate system setting (G54.1 Pn) (n = 1 to 48)
The format for the workpiece coordinate system setting commands is shown below.
G10 L2 Pp1 Xx1 Yy1 Zz1 ;
G10 L2
Pp1
: Parameter change command
: Workpiece coordinate No.
Xx1, Yy1, Zz1 : Settings
(Note)
L2 can be omitted. Omitting Pp1 results in a program error. [M system]
- 187 -
12. Programming Support Functions
12.1 Machining Method Support Functions
(2) Tool offset input
The tool offset amounts, which have been set from the screen, can be input by program commands.
The command format differs between the [M system] and the [L system]. The respective command format must be set by a parameter.
G code
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
Function
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.
G code
G10 L10 Tool length offset amount
G10 L11 Tool wear offset amount
Function
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
- 188 -
12. Programming Support Functions
12.1 Machining Method Support Functions
12.1.10 Machining Modal
12.1.10.1 Tapping Mode
M system
E60 E68
{ {
L 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
G63
Function
Tapping mode ON
The tapping mode command will be canceled with the following commands:
• Exact stop check mode (G61)
• Automatic corner override (G62) [M system]
• Cutting mode (G64)
• High-accuracy control mode command (G61.1) [M system]
12.1.10.2 Cutting Mode
M system
E60 E68
{ {
L 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) [M system]
• Tapping mode (G63) [M system]
• High-accuracy control mode command (G61.1) [M system]
The machine is in the cutting mode status when its power is turned on.
- 189 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
12.2 Machining Accuracy Support Functions
12.2.1 Automatic Corner Override
M system
E60 E68
{ {
L 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 workpiece
θ
(1)
S
Machining allowance
(2)
(3)
Machining
allowance
Ci
Deceleration range
Tool
Programmed path
(finished shape)
Workpiece surface shape
Tool center path
θ : Max. angle at inside corner
Ci : Deceleration range (IN)
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
θ 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.
- 190 -
12.2.2 Deceleration Check
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
The deceleration check function leads the machine to decelerate and stop at the join between one block and another before executing the next block. This is effective to alleviate the machine shock and prevent the corner rounding when the feed rate of the control axis changes suddenly.
Without deceleration check With deceleration check
N010 G01 X100 ;
N011 G01 Y-50 ;
N010 G09 G01 X100 ;
N011 G01 Y-50 ;
Coner rounding occurs because the N011 block is started before the N010 command is completely finished.
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).
Servo
Previous block
Command
Block interpolation completion point
Next block
In-position check width
- 191 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
12.2.2.1 Exact Stop Mode
M system
E60 E68
{ {
L 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/G08P1 ..... High-accuracy control mode [M system]
Refer to "12.2.2 Deceleration Check" for details on the deceleration check.
12.2.2.2 Exact Stop Check
M system
E60 E68
{ {
L 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
M system
E60 E68
{ {
L 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.
- 192 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
12.2.2.4 Programmable In-position Check
M system
E60 E68
{ {
L 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.
- 193 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
12.2.3 High-Accuracy Control
12.2.3.1 High-accuracy Control (G61.1/G08P1)
M system
E60 E68
– {
L system – –
With this function, the error caused by the accuracy in control system during machining is to be improved. There are parameter (of turning initial high-accuracy ON) method and G code command method available in order to achieve the high-accuracy control mode.
With the normal control method, there are problems as indicated below.
(1) Corner rounding occurs at the corner where two lines are connected because the next command movement starts before the previous command finishes. (Refer to Fig. 1)
(2) When cutting with the circle command, an error occurs further inside the commanded path, resulting in a smaller finish. (Refer to Fig. 2)
Commanded path
Commanded path
Actual path
Actual path
Fig.1 Roundness at linear corner
Fig.2 Error by radius reduction with arc command
This function uses the following six functions to reduce the shape error while minimizing the extension of machining time.
(1) Acceleration/deceleration before interpolation (Linear acceleration/deceleration)
(2) Optimum speed control
(3) Vector accuracy interpolation
(4) Feed forward control
(5) Arc entrance/exit speed control
(6) S-pattern filter control
- 194 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
The high-accuracy control is commanded as follows.
G61.1 or G08 can be selected by the parameter.
G61.1 Ff1 ;
G61.1 : High-accuracy control ON
Ff1 : Feed rate command
High-accuracy control mode is validated from the block containing the G61.1 command.
"G61.1" high-accuracy control mode is canceled with one of the G code group 13's functions.
G08 P1(P0) ;
G08
P1
: High-accuracy control mode
: High-accuracy control mode start
P0 : High-accuracy control mode end
"G08P1" high-accuracy control mode is canceled with P0 in G08.
Command G08P_ in can independent block.
The decimal places below the decimal point are ignored for P address.
(Note)
G code group in G08 is "0"; the priority is given to the function of the G code group 0 over that of the G code group 13. After "G08 P1" is commanded, G code group 13 is changed automatically to G64 (cutting) mode. Other command of "13" results in error. Even if highaccuracy control mode is canceled by "G08 P0" command, G64 (cutting) mode will not be changed. If you want to return to the function of the G code group "13" when "G08 P1" has been commanded, command again after high-accuracy control mode is canceled.
- 195 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
(1) Acceleration / deceleration before interpolation
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 speed control
(a) Optimum corner deceleration
By calculating the angle of the seam between blocks, and carrying out acceleration/deceleration control in which the corner is passed at the optimum speed, highly accurate edge machining can be realized. When the corner is entered, that corners optimum speed (optimum corner speed) is calculated from the angle with the next block.
The machine decelerates to that speed in advance, and then accelerates back to the command speed after the corner is passed.
(b) Arc speed clamp
During circular interpolation, even when moving at a constant speed, acceleration is generated as the advance direction constantly changes. When the arc radius is large enough compared to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration does not exceed the tolerable acceleration/deceleration speed before interpolation calculated with the parameters.
This allows arc cutting to be carried out at an optimum speed for the arc radius.
- 196 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
(3) Feed forward control
With this function, the constant speed error caused by the position loop control of the servo system can be greatly reduced. However, if machine vibration occurs as the feed forward coefficient is increased, use this function together with the smooth high gain (SHG) and more stably compensate the delay by the servo system's position loop so that a high accuracy control is realized. As the response is smoother during acceleration/deceleration, the position loop gain can be increased.
Command during acceleration/deceleration before interpolation
Command during acceleration/deceleration after interpolation
+
+
Feed forward control
-
Kp
+
-
Kv
Kp
: Position loop gain
Kv
: Speed loop gain
M : Motor
S : Differential
M
Detector
Machine error compensation amount
S
- 197 -
12. Programming Support Functions
12.2 Machining Accuracy Support Functions
(4) Vector accuracy interpolation
When a fine segment is commanded and the angle between the blocks is extremely small (when not using optimum corner deceleration), interpolation can be carried out more smoothly using the vector accuracy interpolation.
Vector accuracy interpolation
Commanded path
(5) Arc entrance/exit speed control
There are cases where the speed fluctuates and the machine vibrates at the joint from the straight line to arc or from the arc to straight line.
This function decelerates to the deceleration speed before entering the arc and after exiting the arc to reduce the machine vibration. If this is overlapped with corner deceleration, the function with the slower deceleration speed is valid.
(6) S-pattern filter control
This control interpolates while smoothing the changes in the segments distributed to each axis element with vector accuracy interpolation. With this, the fluctuation amplified by feed forward control is reduced and the effect onto the machine is reduced.
- 198 -
12. Programming Support Functions
12.3 Programming Support Functions
12.3 Programming Support Functions
12.3.1 Playback
M system
E60 E68
{ {
L system { {
By repeatedly operating the controls on the panel, the amounts by which the machine is to move by jog feed, rapid traverse and handle feed can be converted into the command format of the control unit, and by repeatedly writing this data into the memory, machining programs for all the steps can be prepared.
12.3.2 Address Check
M system
E60 E68
{ {
L 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.
- 199 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13.1.1 Backlash Compensation
M system
E60 E68
{ {
L 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).
- 200 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13.1.2 Memory-type Pitch Error Compensation
M system
E60 E68
{ {
L 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 (µm)
2. Number of compensation points
3. Compensation amount
4. No. of compensated axes
: 1024
: –128 to 127 (output unit)
: 10 axes (including number of axes for relative
position error compensation)
(1) The compensation position is set for the compensation axis whose reference position serves as the zero (0) point. Thus, memory-type pitch error compensation is not performed if return to reference position 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
R#1
Compensation base axis
Division interval
(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.
- 201 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13.1.3 Memory-type Relative Position Error Compensation
M system
E60 E68
{ {
L 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 (µm)
2. Number of compensation points : 1024
3. Compensation amount
4. No. of compensated axes
: –128 to 127 (detection unit)
: 10 axes (including number of axes for memory
type pitch error compensation.)
(1) The compensation position is set for the compensation axis whose reference position serves as the zero (0) point. Thus, memory-type relative position error compensation is not performed if return to reference position 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
E60 E68
M system { {
L 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
- 202 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
13.1.9 Spindle Backlash Compensation
M system
L system
E60 E68
– {
– {
This function compensates for the backlash produced when the spindle is reversed in tapping. This is effective in improving the accuracy of tapping.
The amount of spindle backlash compensation is set by parameter.
(1) Synchronous tapping cycle
Backlash compensation is only performed in the tapping retract operation after the machine has reached the hole bottom position ((3) in the figure below).
Rapid traverse
Cutting feed
Tap spindle cutting operation
(Spindle rotates)
(1) (2)
(1) (4)
(Spindle stops)
Tap spindle retract operation
(Spindle rotates)
(2) (3)
Hole bottom position
(Spindle temporarily stops)
State of the tap spindle gear spback
(3) (4)
Compensation executed spback : spindle backlash compensation amount
- 203 -
13. Machine Accuracy Compensation
13.1 Static Accuracy Compensation
(2) Pecking tapping cycle / deep-hole tapping cycle
Backlash compensation is performed at three times as follows.
(a) In the retract operation after the tap spindle cutting operation ((3) and (n3) in the figure below).
(b) In the tap spindle cutting operation for the second time or later ((n1) and (n5) in the figure below).
(c) In the tapping retract operation after reaching the hole bottom point ((n7) in the figure below).
Compensation frequency at (a) and (b) is changed according to the number of cuttings at each time.
Rapid traverse
Cutting feed
Tap spindle cutting operation
(spindle rotates)
(1)
(2)
(4) (n1)
(3)
(n4) (n5)
(n8)
Point R position
(spindle stops)
Tap spindle retract operation
(spindle rotates)
(n2) (n3)
(n6) (n7)
State of the tap spindle gear hole bottom position
(spindle temporarily stops)
(1) (2) (3) spback
Compensation executed
(4)
(n1)
(n5)
Compensation executed spback
(n3)
(n7) spback
Compensation executed
(n4)
(n8) spback : spindle backlash compensation amount
(Note) In the deep-hole tapping cycle, point R position is set at (4), (n1), (n4), and (n5) in the figure above.
- 204 -
13. Machine Accuracy Compensation
13.2 Dynamic Accuracy Compensation
13.2 Dynamic Accuracy Compensation
13.2.1 Smooth High-gain Control (SHG Control)
E60 E68
M system
L system
{
{
{
{
This is a high-response and stable position control method using the servo system (MDS- -
V /SVJ2). This SHG control realizes an approximately two-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.)
Conventional control
(position loop gain = 33rad/S)
SHG control
(position loop gain = 50rad/S)
Step response
Speed
Conventional control
6.0
Current
SHG control
3.0
Machine vibration
Time
Time
Machine vibration amount (µm)
(2) The shape error is approx. 1/9 of the conventional control.
Y
3
2
1
X
Feed rate 3000mm/min.
Radius 50mm
1. Conventional control
2. SHG control
3. SHG control + FF (Feed forward)
Conventional control
SHG control
2.5
22.5
SHG control + FF
1.0
Roundness error (µm)
(3) The positioning time is approx. 1/3 of the conventional control.
Droop
Droop during rapid traverse deceleration
3
2 1
Time
Conventional control
SHG control
70
SHG control + FF
60
200
Positioning time (ms)
1. Conventional control
2. SHG control
3. SHG control + FF (Feed forward)
- 205 -
13. Machine Accuracy Compensation
13.2 Dynamic Accuracy Compensation
13.2.2 Dual Feedback
M system
E60 E68
– Δ
L system – Δ
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.
Weight (gain) of position feedback amounts db
0
Motor end
1
T db rad/s
0
Machine end
1
T rad/s
Time constant T here is adjusted using a parameter.
13.2.3 Lost Motion Compensation
M system
E60 E68
{ {
L system { {
This function compensates the error in the protrusion shape caused by lost motion at the arc quadrant changeover section during circular cutting.
- 206 -
14. Automation Support Functions
14.1 External Data Input
14. Automation Support Functions
14.1 External Data Input
By using the DDB interface, the following functions can be realized from the PLC ladder.
14.1.1 External Search
M system
E60 E68
{ {
{ {
L system
The program No. and sequence No. to be automatically started in the memory or tape mode, ladder can be searched from the PLC ladder. The currently searched details can be read.
- 207 -
14. Automation Support Functions
14.1 External Data Input
14.1.2 External Workpiece Coordinate Offset
M system
L system
E60 E68
{ {
{ {
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.
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 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)
External workpiece coordinate
External workpiece coordinate offset
Machine coordinate zero point
Machine coordinate system
- 208 -
14. Automation Support Functions
14.1 External Data Input
14.1.3 External Tool Offset
M system
L system
E60 E68
{ {
{ {
The tool offset amount can be referred and updated from the PLC ladder.
- 209 -
14. Automation Support Functions
14.2 Measurement
14.2 Measurement
14.2.1 Skip
14.2.1.1 Skip
M system
E60 E68
{
{
{
{
L 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 ;
M31 : Measurement command
Xx1, Yy1, Zz1 : Command values
Ff1 : Feed rate
Skip signal input
Feed rate
Programmed end point
Actual movement distance
Remaining distance
Position
Command value
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.
δ •
F
=
× (Tp + t)
•
60
δ : 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.
- 210 -
14. Automation Support Functions
14.2 Measurement
14.2.1.2 Multiple-step Skip
M system
L system
E60 E68
{ {
{ {
(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 ;
M31.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
Ff1
: Skip signal command
: Feed rate (mm/min)
(a) Specify the skip rate in command feed rate 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.
- 211 -
14. Automation Support Functions
14.2 Measurement
Table 1 Valid skip signals
Valid skip signal
Skip signal command P
4 3 2 1
1 {
3
{
{
8
7
{
{
:
13
14
15
: : : :
{ { {
{ { {
{ { { {
14.2.1.4 PLC Skip
M system
E60 E68
–
{
–
{
L system
This function enables skip operations to be performed by signals that are input from the user PLC.
- 212 -
14. Automation Support Functions
14.2 Measurement
14.2.5 Automatic Tool Length Measurement
M system
L system
E60 E68
{ {
{ {
(1) Automatic Tool Length Measurement; G37 (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
R
: Measurement axis address and measurement position coordinate. X, Z ...(NC axis)
: The distance between the point at which tool movement is to start at the
D
F
: measurement speed and the measurement position.
The range in which the tool is to stop.
: The measurement rate.
When R_, D_ and F_ have been omitted, the values set in the parameters are used.
Tool change position
Tool
Sensor
Reference position
(In case of machine coordinate system zero point.)
Amount of movement based on tool length measurement
Tool length measurement position (Za1)
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 Z–300. 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 that is then registered in the tool offset table.
- 213 -
14. Automation Support Functions
14.2 Measurement
A
B
1 r
1
Start point
Area A : Moves with rapid traverse
feed rate.
Areas B
1
, B
2
: Moves with the
measurement speed (f
1
or
parameter setting)
If a sensor signal is input in area
B
1
, an error will occur.
If a sensor signal is not input in
the area B
2
, an error will occur.
B
2 d
1 d
1
Measurement position (z
1
)
(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
α_R_D_F_ ;
α
R
: Measurement axis address and measurement position coordinate. ... X, Z
: 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
F
:
:
The range in which the tool is to stop. (Always a radial value: incremental value)
The measurement rate.
When R_, D_ and F_ have been omitted, the values set in the parameters are used.
- 214 -
14. Automation Support Functions
14.2 Measurement
r1, d1, and f1 can also be set in parameters.
Start position
A Rapid traverse feed r1
B d1 F feed
Measuring instrument d1
Measurement position
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.
- 215 -
14. Automation Support Functions
14.2 Measurement
14.2.6 Manual Tool Length Measurement 1
M system
L system
E60 E68
{ {
{ {
Simple measurement of the tool length is done without a sensor.
(1) Manual tool length measurement 1
[M system]
When the tool is at the reference position, 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
Manual movement amount (tool length offset amount)
Workpiece
Table
(2) Manual tool length 1 measurement
[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
Parameter setting
X axis tool length
Z axis tool length
Measurement position
Parameter setting
Z axis
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.
- 216 -
14. Automation Support Functions
14.2 Measurement
14.2.7 Manual Tool Length Measurement 2
M system
L system
E60 E68
–
{
{ {
(1) Manual tool length measurement 2
[M system]
When the tool is positioned at the reference position, this function enables the distance from the reference position to the tool tip to be measured and registered as the tool length offset amount. In this case, the position of the gauge block used as a reference must be set as the basic height.
M
TLM basic length (setup parameter)
Gauge block
Table
Tool length offset amount
Manual movement amount
Basic height
If the height axis designation parameter is ON, the axis designated for plane selection basic axis K is the axis targeted for measurement as the height axis.
Furthermore, if the tool length measurement check parameter is ON, an input OK/cancel confirmation message appears after input key has been pressed.
(2) Manual tool length 2 measurement II [L system]
A device in which a touch sensor is built is used. Simply by causing the tool nose to touch the touch sensor in manual feed, the tool offset amount can be calculated and stored in tool offset amount memory.
X axis
– touch face
X axis tool length
Z axis tool length
Z axis + touch face
Z axis – touch face
X axis + touch face
M
Measurement method
(a) Preset the machine coordinates of the touch sensor touch face in parameter as the measurement basic value.
(b) Select the tool whose tool length offset amount is to be measured.
(c) Cause the tool nose to touch the touch sensor in manual feed.
The tool length offset amount is automatically calculated from the machine coordinates when the tool nose touches the touch sensor and the measurement basic value. It is stored in memory as tool length offset amount.
Tool length offset amount
= machine coordinates – measurement basic value (sensor position)
- 217 -
14. Automation Support Functions
14.2 Measurement
14.2.8 Workpiece Coordinate Offset Measurement
M system
E60 E68
–
–
{(*)
{
L system
The external workpiece coordinate offset data for the Z axis can be set by cutting the workpiece face by means of manual operations and inputting the workpiece measurement signal.
Measurement of external workpiece coordinate offset data for Z axis
X axis
Tool post
Machine zero point
Workpiece
Z axis
Workpiece coordinate zero point
Setting method
(1) Select the tool, and cut the workpiece face.
(2) When the workpiece measurement signal is input, the external workpiece coordinate offset data for the Z axis is calculated from the machine coordinate values, length of the tool used and tool nose wear offset amount, and stored in the memory.
(Note) The (*) mark is the simple workpiece coordinate offset input.
With this function, the workpiece coordinate system offset data automatic calculation value and machine position for corresponding axes are displayed in the setting part on the workpiece coordinate offset screen.
- 218 -
14. Automation Support Functions
14.2 Measurement
14.2.9 Workpiece Position Measurement
M system
E60 E68
–
–
{
–
L system
The workpiece position measurement function is used to measure each axis’ coordinate point by installing a sensor on the spindle and the sensor contacting the workpiece with the manual feed or handle feed.
The surface, hole center and width center coordinates are calculated from the measured coordinates, and those calculated results are set in the workpiece coordinate offset.
Only 1st part system is available for the workpiece position measurement.
(1) Surface workpiece offset measurement
The workpiece position measurement coordinates are calculated from the skip machine position of the X, Y and Z axes.
Measurement position coordinate X = X axis’ skip machine position + Sensor diameter/2
+ Center compensation amount (Horizontal)
Measurement position coordinate Y = Y axis’ skip machine position + Sensor diameter/2
+ Center compensation amount (Vertical)
Measurement position coordinate Z = Z axis’ skip machine position - Sensor length
The sensor diameter/2 changes between +/- with the last tool movement direction during the measurement.
The sensor diameter and center compensation amount are applied to the X axis or Y axis.
The sensor length is applied to the Z axis.
The measurement position coordinate of the X axis, Y axis or Z axis is set in the specified workpiece coordinate offset.
To set the workpiece coordinate offset, the X axis is measured and the X axis’
X
Workpiece coordinate zero point offset coordinate is set. Then, the Y axis’ offset is measured and set. Finally, the Z axis’ offset is measured and set.
Y axis measurement constant position
Y
X axis measuremen
- 219 -
14. Automation Support Functions
14.2 Measurement
(2) Hole center workpiece offset measurement
The measurement position coordinates of two axes (X, Y) are measured at three points, and the hole center is calculated. The calculated result is set in the specified workpiece coordinate offset.
The workpiece position measurement coordinates are calculated from the skip machine position of the X, Y and Z axes.
Measurement position coordinate X = X axis’ skip machine position + Center compensation amount
(Horizontal)
Measurement position coordinate Y = Y axis’ skip machine position + Center compensation amount
(Vertical)
X
Measuement B point
Workpiece coordinate zero point
Y
To set the workpiece coordinate offset, the position X and Y of the measurement A point are measured, and the measured values are set in the measurement
A point. In the same manner as the measurement A point, the measurement B point and then C point are measured and set.
The hole center coordinate is calculated by setting the workpiece coordinate system after setting three points, and the calculated result is set in the workpiece coordinate offset.
(3) Width center workpiece offset measurement
The measurement position coordinate of the X axis or Y axis is measured at two points, and each axis’ groove center is calculated. The calculated result is set in the specified workpiece coordinate offset.
The workpiece position measurement coordinates are calculated from the skip machine position of the X, Y and Z axes.
Measurement position coordinate X = X axis’ skip machine position + Center compensation amount
(Horizontal)
Measurement position coordinate Y = Y axis’ skip machine position + Center compensation amount
(Vertical)
X
Measurement B point
Measurement
A point
To set the workpiece coordinate offset, the position X (position Y) of the measurement A point is measured, and the measured value is set in the measurement A point.
In the same manner as the measurement A point, the measurement B point is measured and set.
The groove width center coordinate of the X axis (Y axis) is calculated by setting the workpiece coordinate
Y system after setting two points, and the calculated result is set in the workpiece coordinate offset.
- 220 -
14. Automation Support Functions
14.3 Monitoring
14.3 Monitoring
14.3.1 Tool Life Management
14.3.1.1 Tool Life Management I
M system
L system
(1) M series
E60 E68
{
{
{
{
The time (0 to 4000 hours) and frequency (0 to 65000 times) of use of the user PLC specified tool are accumulated. Tool data including the time and frequency of use of the PLC specified tool is output.
(2) L series
Tool life management is performed using the time and frequency of use of a tool.
(a) Management by the time of use
The cutting time after specification of a tool selection (T) command (G01, G02, and G33) is added to the tool use time for the specified tool.
If the use time reaches the life time when a tool selection command is specified, an alarm is given.
(b) Management by the frequency of use
The tool use counter corresponding to the number of the specified tool is incremented each time a tool selection (T) command is specified for the tool.
If the counter reaches the life time when a tool selection command is specified, an alarm is given.
14.3.1.2 Tool Life Management II
M system
L system
(1) M series
E60 E68
{
{
{
{
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 series
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. y No. of groups: 80 sets y No. of tools in group: Max. 16 tools
- 221 -
14. Automation Support Functions
14.3 Monitoring
14.3.2 Number of Tool Life Management Sets
20/40/80 sets
M system
L system
100/200 sets
M system
L system
14.3.3 Number of Parts
E60 E68
–
{80
–
{80
E60 E68
{100
–
{200
–
M system
E60 E68
{ {
{ {
L system
Part count display
The number of machined parts is counted up each time a part is machined, and displayed .
Number of workpieces machined
Maximum number of workpieces to be machined
Number of workpieces machined
- 222 -
14. Automation Support Functions
14.3 Monitoring
14.3.4 Load Meter
M system
E60 E68
{
{
{
{
L 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
M system
E60 E68
{24
{24
{24
{24
L system
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.
Example of dog1, dog2 settings and execution dog1, dog2 settings
dog1 < dog2
dog1, dog2 positions
dog1 dog2
Description
Signal is output between dog1 and dog2 dog1 > dog2 Signal is output between dog2 and dog1 dog1 = dog2 dog1 ＝ dog2
Signal is output at the dog1
(dog2) position
14.3.12 Synchronous Error Observation
Basic machine coordinate system zero point
Hypothetical dog dog1
PSW width dog2
M system
E60 E68
–
–
{
{
L system
With this function, synchronous tapping error (screw pitch error) generated during synchronous tapping cycle operation is monitored and a warning is output when the error exceeds a certain value.
- 223 -
14. Automation Support Functions
14.5 Others
14.5 Others
14.5.1 Programmable Current Limitation
M system
L system
E60 E68
–
{
–
{
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) 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".
- 224 -
15. Safety and Maintenance
15.1 Safety Switches
15. Safety and Maintenance
15.1 Safety Switches
15.1.1 Emergency Stop
M system
E60 E68
{
{
{
{
L 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 goes OFF and the servo ready signal is turned OFF.
15.1.2 Data Protection Key
M system
E60 E68
{
{
{
{
L 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 screen.
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
- 225 -
15. Safety and Maintenance
15.2 Display for Ensuring Safety
15.2 Display for Ensuring Safety
15.2.1 NC Warning
M system
E60 E68
{ {
{ {
L system
The warnings that 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
Servo warning
Spindle warning
System warning
Absolute position warning
Auxiliary axis warning
Description
The servo warning is displayed.
The spindle warning is displayed.
The system warning is displayed. (State such as temperature rise, battery voltage low, etc.)
A warning in the absolute position detection system is displayed.
The auxiliary axis warning is displayed.
15.2.2 NC Alarm
M system
E60 E68
{ {
{ {
L system
The alarms that 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
Operation alarm
Servo alarm
Spindle alarm
MCP alarm
System alarm
Description
This alarm occurring due to incorrect operation by the operator during NC operation and that by machine trouble are displayed.
This alarm describes errors in the servo system such as the servo drive unit‚ motor and encoder.
This alarm describes errors in the spindle system such as the spindle drive unit‚ motor and encoder.
An error has occurred in the drive unit and other interfaces.
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.
An alarm in the absolute position detection system is displayed. Absolute position detection system alarm
Auxiliary axis alarm
Computer link error
User PLC alarm
Program error
The auxiliary axis alarm is displayed.
The computer link alarm is displayed.
The user PLC alarm is displayed.
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.
- 226 -
15. Safety and Maintenance
15.2 Display for Ensuring Safety
15.2.3 Operation Stop Cause
M system
E60 E68
{
{
{
{
L system
The stop cause of automatic operation is displayed on the screen.
15.2.4 Emergency Stop Cause
M system
E60 E68
{ {
{ {
L system
When "EMG" (emergency stop) message is displayed in the operation status display area of the screen, the emergency stop cause can be confirmed.
15.2.5 Temperature Detection
M system
E60 E68
{ {
{ {
L system
When overheating is detected in the control unit, an overheat signal is output at the same time as the alarm is displayed. If the system is in automatic run at the time, run is continued, but it cannot be started after reset or completion by M02/M30. (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 80
°C or more in the control unit.
Control unit
Overheat detection
Parameter
Temperature alarm
Message display
(Default: valid)
(80°)
Bit device
User PLC
Cooling fan rotation
Lamp alarm
Emergency stop
Others
(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.
- 227 -
15. Safety and Maintenance
15.3 Protection
15.3 Protection
15.3.1 Stroke End (Over travel)
M system
E60 E68
{ {
{ {
L 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
•Set by the machine maker.
I Outside designated by the two types becomes the movement valid range.
•The change or function of parameter
IIB Inside can be turned OFF/ON with the program command.
•Select II or IIB with the parameters.
•Set by the machine maker.
IC Outside
•Can be rewritten with DDB.
- 228 -
15. Safety and Maintenance
15.3 Protection
15.3.2.1 Stored Stroke Limit I/II
M system
E60 E68
{
{
{
{
L 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 position return.
The stored stroke limit I function will be invalidated if the maximum and minimum values are set to the same data.
Prohibited area Point 1
Machine coordinate system
M
The values of points 1 and 2 are set using the coordinate values in the machine coordinate system.
Machine movement valid range
Point 2
Prohibited area
"
–
"
setting
Feed rate
"+" setting
L
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.
- 229 -
15. Safety and Maintenance
15.3 Protection
(2) Stored Stroke Limit II
This is the stroke limit function that 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.
Prohibited area Point 1
Point 3
Area prohibited by stored stroke limit function II
Machine coordinate system
Machine movement valid range
M
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.
Point 4
Point 2
"
–
"
setting
"
+
" setting
Feed rate
L
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.
- 230 -
15. Safety and Maintenance
15.3 Protection
15.3.2.2 Stored Stroke Limit IB
M system
L system
E60 E68
–
{
– {
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.
: Prohibited area
Stored Stroke Limit IB
Stored Stroke Limit IIB
Stored Stroke Limit I
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.
(Note 1) 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.
- 231 -
15. Safety and Maintenance
15.3 Protection
15.3.2.3 Stored Stroke Limit IIB
M system
L system
E60 E68
–
{
– {
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
M system
E60 E68
–
–
{
{
L 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 stored stroke limit IB.
Machine coordinate system
M
Point 1
The position of points 3 and 4 are set with the machine coordinate.
The area determined by points
1 and 2 is the prohibited area set with stored stroke limit I.
Machine movement valid range
: Prohibited area
Point 2
Point 3
Additional movement range
Point 4
- 232 -
15. Safety and Maintenance
15.3 Protection
15.3.4 Chuck/Tailstock Barrier Check
M system
E60 E68
– –
{ {
L 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 position return.
(4) Chuck barrier/tail stock barrier setting
X axis
P 4
X axis
P 4
P 1
P 1
(P 0)
P 5
(P 0)
P 5
P 2
P 2
P 6
P 6
P 3 P 3
P 0
Z axis
P 0
Z axis
(Form 1) (Form 2)
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.)
- 233 -
15. Safety and Maintenance
15.3 Protection
15.3.5 Interlock
M system
E60 E68
{
{
{
{
L 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
M system
E60 E68
{ {
{ {
L 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.
- 234 -
15. Safety and Maintenance
15.3 Protection
15.3.8 Door Interlock
15.3.8.1 Door Interlock I
M system
L system
E60 E68
{
{
{
{
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 amplifiers 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.
- 235 -
15. Safety and Maintenance
15.3 Protection
15.3.8.2 Door Interlock II
M system
L system
E60 E68
{
{
{
{
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 amplifiers 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.
- 236 -
15. Safety and Maintenance
15.3 Protection
Appendix 1. 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
M system
E60 E68
{
{
{
{
L system
This function is used to prohibit changing the setup parameter.
15.3.10 Program Protect (Edit Lock B, C)
M system
E60 E68
{ {
{ {
L system
The edit lock function B or C inhibits machining program B or C (group with 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
Machining program A
10000 ～99999999
Editing is inhibited by edit lock C.
Editing is inhibited by edit lock B.
Editing is inhibited by data protect (KEY3).
- 237 -
15. Safety and Maintenance
15.3 Protection
15.3.11 Program Display Lock
M system
E60 E68
{
{
{
{
L 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.
- 238 -
15. Safety and Maintenance
15.4 Maintenance and Troubleshooting
15.4 Maintenance and Troubleshooting
15.4.1 History Diagnosis
M system
E60 E68
{ {
{ {
L 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.
(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
M system
L system
E60 E68
{ {
{ {
The information on the servos (NC axes), spindles, PLC axes and power supplies appears on the screen.
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
M system
L system
E60 E68
{ {
{ {
• Sampling of the servo and spindle data for which an alarm occurrence is a stop condition is performed all the time. By using the waveform display function, this sampling data can be displayed in the waveforms.
• The data currently displayed can be stored on a memory card, and read out when required.
- 239 -
15. Safety and Maintenance
15.4 Maintenance and Troubleshooting
15.4.4 Waveform Display
M system
E60 E68
{
{
{
{
L system
The following servo data and spindle data can be displayed as waveforms. Data can be displayed for two channels simultaneously in 1-hour increments on a continuous basis or on a one-shot basis.
Servo data
Current feedback
Current command
Position deviation
Position command
Speed feedback
Motor load
Spindle data
Motor rotation speed (speed command value)
Position deviation
Position command
Speed feedback (r/min)
Synchronous tap error width (
μm)
Synchronous tap error angle (0.001 degree)
15.4.5 Machine Operation History Monitor
M system
E60 E68
{
{
{
{
L 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.
- 240 -
15. Safety and Maintenance
15.4 Maintenance and Troubleshooting
15.4.6 NC Data Backup
With this function, the parameters and other data of the NC control unit can be backed up in the memory cassette.
The data can also be restored.
(1) RS-232C
M system
L system
E60 E68
{
{
{
{
[Backup target]
Machining programs, parameters, workpiece offset data, common variables, tool compensation data, tool life control data
Ladders (ladder, message)
SRAM data
(2) Cassette memory
M system
E60 E68
{ {
{ {
L system
The memory cassette for maintenance is used to back up and restore the NC data.
Model Compatible memory cassette for maintenance
E60/E68 HR410/HR450
[Backup targets ... The following data is backed up in a batch.]
Ladders (ladder, message)
SRAM data
(3) IC card
M system
L system
E60 E68
–
{
–
{
[Backup target]
Machining programs, parameters, common variables, tool compensation data, tool life control data
Ladders (ladder, message)
SRAM data
- 241 -
15. Safety and Maintenance
15.4 Maintenance and Troubleshooting
15.4.7 PLC I/F Diagnosis
M system
E60 E68
{
{
{
{
L 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.
15.4.13 Signal Trace Function
M system
E60 E68
–
{
–
{
L system
With this function, status of various devices to be used for the external signals and user ladders can be traced, and ladder program can be monitored.
Set the <BITDEVICE> (max. 8 points) and <WORDDEVICE> (max. 2 points) to be traced on the
"DEVICE SET" screen and also set the <MONI SELECT>. Once trace is started, tracing status of the set device can be monitored in the "DEVICE MONITOR" screen. The latest 256 sampling data can be monitored for each device.
Trace can be stopped at the specific conditions by setting the trigger.
Trace is continued until it is stopped manually or by trigger. So, trace is automatically started when the power is turned OFF and ON during trace execution.
- 242 -
16. Cabinet and Installation
16.1 Cabinet Construction
16. Cabinet and Installation
16.1 Cabinet Construction
The configuration of the unit used by the EZMotion-NC E60/E68 series is shown below.
Refer to the Connection / Maintenance Manual for details.
Display unit / NC unit
NC unit
Remote I/O unit
FCUA-DX1xx
MC link B
Base I/O unit
Manual pulse generator
Servo drive unit
MDS-B-SVJ2 series
MDS-R series
MR-J2-CT series
RS-232C device
Spindle drive unit
MDS-x-SPx series
MDS-B-SPJ2 series
Power supply unit
MDS-x-CV series
MC link A
MITSUBISHI
MC link B
Sensor
Sensor
Remote I/O unit
FCUA-DX1xx
Max. 4 points h l
Synchronous feed encoder
- 243 -
Refer to connection manuals of servo.
Servo motor Spindle motor
16. Cabinet and Installation
16.1 Cabinet Construction
List of configuration units
(1) NC unit
Model Configuration module model Function
FCU6-MU071
(E60)
FCU6-MU072
(E68)
HR761/HR763 card Main card
HR741 card Memory card
Q6-BAT Battery
Base plate
Cover
HR761/HR763 card Main card
HR742 card Memory card
Q6-BAT Battery
Base plate
Cover
(2) Option for NC unit
Configuration module model Function
HR753 card (E60)
HR751 card (E68)
E60 spindle connection option
PLC accelerator card
(3) Option for front IC card I/F unit
Model Configuration Function
FCU6-EP105-1
(E68)
HR253 Front IC card
F161 cable
Installation plate
Bus cable
- 244 -
16. Cabinet and Installation
16.1 Cabinet Construction
(4) Display unit
Model
FCU6-DUE71
/FCU6-DUE71-1
(Note 1)
(E60)
FCU6-DUT11
/FCU6-DUT11-1
(Note 1)
(E60)
Configuration module model Function
MDT962B-4A
FCUA-R100 cable
F590 cable
9-type monochrome CRT
CRT power supply cable
Between HR761 and CRT
Menu key
Escutcheon
Base plate
LTBLDT168G6C
HR721 card
F090 cable
NZ24-4 cable
Menu key
7.2-type monochrome LCD
Power supply for backlight
Between HR761 and HR721
Between HR721 and LCD
Escutcheon
Base plate
AA084VC06
HR722 card
8.4-type color LCD
LCD relay card
FCU6-DUN24
(Note 2)
(E68)
FCU6-DUN26
(E60)
(Note 3)
F090 L0.1M cable
F098 cable
F484 L0.25M cable
Menu key
Between HR761 and HR722
Between HR722 and LCD
Inverter cable
Escutcheon
Base plate
(Note 1) The units with the name FCU6-xxxxx-1 are provided with an adapter for mounting on the front of the units.
(Note 2) With E68 standard, the display unit is mounted from the front.
(Note 3) Escutcheon of FCU6-DUN26 differs from that of FCU6-DUN24.
(5) Keyboard unit
Model
FCU6-KB071
/FCU6-KB071-1
(Note 1)
(E60)
FCU6-KB024
(Note 2)
(E60/E68)
Configuration module model Function
Housing Sheet attached for machining center
F053 cable
Base plate
Housing
F054 cable
Base plate
Between HR761 and keyboard
Sheet attached for machining center
Between HR761 and keyboard
- 245 -
(6) Base I/O unit
Model
FCU6-HR341 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
I/O share line (Note 5)
FCU6-HR351 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
I/O share line (Note 5)
FCU6-DX220
(E68)
FCU6-DX221
(E68)
16. Cabinet and Installation
16.1 Cabinet Construction
Sink/Source input 64 points
Sink output 64 points
I/O share line (Note 3)(Note 4)
Sink/Source input 64 points
Source output 64 points
I/O share line (Note 3)(Note 4)
Configuration module model Function
HR341 card DI64/DO48/AO1
Aluminum die-cast
HR351 card
Aluminum die-cast
HR327 card
Aluminum die-cast
HR337 card
DI64/DO48/AO1
DI64/DO64
DI64/DO64
Aluminum die-cast
(Note 1) The units with the name FCU6-xxxxx-1 are provided with an adapter for mounting on the front of the units.
(Note 2) With E68 standard, the keyboard unit is mounted from the front.
(Note 3) DI/O is a cable with no strain relief.
(Note 4) The 5th to 8th channels of SKIP and 2nd channel of RIO cannot be used.
(Note 5) I/O share line is the interface with servo drive unit, remote I/O, skip signal input and synchronous feed encoder.
(7) Remote I/O unit
Model
FCUA-DX100 Sink/Source input 32 points
Sink output 32 points
FCUA-DX101 Sink/Source input 32 points
Sink output 32 points
FUCA-DX110 Sink/Source input 64 points
Sink output 48 points
FCUA-DX111 Sink/Source input 64 points
Sink output 48 points
FUCA-DX120 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
FUCA-DX121 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
FCUA-DX140 Sink/Source input 32 points
Sink output 32 points
Analog input 4 points
Analog output 1 point
FCUA-DX141 Sink/Source input 32 points
Sink output 32 points
Analog input 4 points
Analog output 1 point
Component module model Function
RX311 card DI32/DO32
Case
RX312 card DI32/DO32
Case
RX311 card
RX321-1 card
DI32/DO32
DI32/DO16
Case
RX312 card
RX322-1 card
DI32/DO32
DI32/DO16
Case
RX311 card
RX321 card
DI32/DO32
DI32/DO16/AO1
Case
RX312 card
RX322 card
DI32/DO32
DI32/DO16/AO1
Case
RX311 card
RX341 card
DI32/DO32
AI4/AO1
Case
RX312 card
RX341 card
DI32/DO32
AI4/AO1
Case
- 246 -
16. Cabinet and Installation
16.1 Cabinet Construction
(8)Peripheral devices
Model
PD25 Input:
Output: 24VDC generator generator generator
FCUA-R-TM Terminal
FCUA-A-TM
Ground plate D
Terminal connector
Component module model Function
With the power supply ON/OFF function
Manual pulse generator for
12VDC
(25pulse/rev)
Use F320/F321 cable.
Without MELDAS logo.
Manual pulse generator for
12VDC
(25pulse/rev)
Use F320/F321 cable.
With MELDAS logo.
Manual pulse generator for 5VDC
(100pulse/rev)
Use F023/F024 cable.
Without MELDAS logo.
Terminal for remote I/O communication
Terminal for drive part communication
Appendix 1.9
Ground plate E
A complete set of ground plate D
A complete set of ground plate E
Appendix 1.9 encoder
- 247 -
16. Cabinet and Installation
16.2 Power Supply
16.2 Power Supply
!
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
(a) E60: Color display
Unit name NC unit Display unit Keyboard unit
Ambient
During operation temperature
During
Ambient
0 to 55°C
-20 to 60°C storage
Long term 10 to 75% RH (With no dew condensation) humidity
Short term 10 to 95% RH (With no dew condensation) (Note 1)
Vibration resistance 4.9m/s
2
or less
Shock resistance 29.4m/s
2
or less
Working atmosphere
Power supply voltage
No corrosive gas, dust or oil mist
24VDC ±5%
Ripple 200mV max.
Instantaneous stop tolerance time
Current consumption
(max.)
Heating value (max.)
Mass
Outline dimension
Depends on the specifications of 24VDC power supply unit used.
(Use more than 20ms)
2A
(NC unit + display unit + keyboard unit)
50W
3.2kg (with FUC6-DUN26)
Refer to Appendix 3.1
1.0kg
(Note 1) Short term refers to within one month.
(b) E60: Monochrome display
Unit name NC unit Display unit
Ambient temperature
During operation
0 to 55°C
During storage
-20 to 60°C
Ambient Long term 10 to 75% RH (With no dew condensation) humidity
Short term 10 to 95% RH (With no dew condensation) (Note 2)
Vibration resistance 4.9m/s
2
or less
Shock resistance 29.4m/s
2
or less
Working atmosphere No corrosive gas, dust or oil mist
Power supply voltage
24VDC ±5%
Ripple 200mV max.
Single phase 100VAC
-15% to +10%
50/60Hz
Instantaneous stop tolerance time
20ms (with an external power supply unit PD25)
Current consumption (max.)
Heating value (max.)
Mass
Outline dimension
2A
(NC unit + display unit)
100VAC 0.4A
80W (with FCU6-DUE71), 50W (with FCU6-DUT11)
5.5kg (with FCU6-DUE71), 2.5 kg (with FCU6-DUT11)
Refer to Appendix 3.1
(Note 1) If it is hotter than 45°C, the quality of the LCD (contrast ratio) deteriorates.
(Note 2) Short term refers to within one month.
Surface temperature of LCD display unit:
0 to 50°C (Note 1)
－
－
- 248 -
16. Cabinet and Installation
16.2 Power Supply
(c) E68
Unit name NC unit Display unit Keyboard unit
During
Ambient operation temperature During storage
Power supply voltage
0 to 55°C
-20 to 60°C
Ambient Long term 10 to 75% RH (With no dew condensation) humidity
Short term 10 to 95% RH (With no dew condensation) (Note 1)
Vibration resistance 4.9m/s
2
or less
Shock resistance 29.4m/s
2
or less
Working atmosphere No corrosive gas, dust or oil mist
24VDC ±5%
Ripple 200mV max.
Heating value (max.)
Mass
Instantaneous stop tolerance time
Current consumption
(max.)
Outline dimension
Depends on the specifications of 24VDC power supply unit used.
(Use more than 20ms)
2A
(NC unit + display unit + keyboard unit)
50W
3.2kg (with FCU6-DUN24)
Refer to Appendix 3.2
1.0kg
(Note 1) Short term refers to within one month.
- 249 -
16. Cabinet and Installation
16.2 Power Supply
(2) Environment conditions in electric cabinet
Unit name Base I/O unit
During
Ambient operation temperature During storage
0 to 55°C
-20 to 60°C
Ambient Long term 10 to 75% RH (With no dew condensation) humidity
Short term 10 to 95% RH (With no dew condensation) (Note 1)
Vibration resistance 4.9m/s
2
or less
Shock resistance 29.4m/s
2
or less
Working atmosphere No corrosive gas, dust or oil mist
Power supply voltage
24VDC ±5%
Ripple 200mV max.
Instantaneous stop tolerance time
Depends on the external power supply used.
(Use more than 20ms)
Current consumption
(max.)
Heating value (max.)
0.8A (Note 2)
40W (Note 3)
Mass 0.6kg
Outline dimension Refer to Appendix 3.4.
(Note 1) Short term refers to within one month.
(Note 2) This value is only of the control circuit part (DCIN connector). For the current value of the I/O circuit, calculate with the number of points used and load.
(Note 3) When all DI/DO points are ON.
(3) Remote I/O unit
Unit name Remote I/O unit
Ambient temperatur e
During operation
During storage
Ambient humidity
Long term
Short term
Vibration resistance
Shock resistance
Working atmosphere
Power supply voltage
Instantaneous stop tolerance time
Current consumption
(max.)
Heating value (max.)
0 to 55°C
-20 to 60°C
10 to 75% RH (With no dew condensation)
10 to 95% RH (With no dew condensation) (Note 1)
4.9m/s
2
or less
29.4m/s
2
or less
No corrosive gas, dust or oil mist
24VDC ±5%
Ripple 200mV max.
Depends on the external power supply used.
(Use more than 20ms)
Outline dimension Refer to Appendix 3.5.
(Note 1) Short term refers to within one month.
(Note 2) This value is only of the control circuit part (DCIN connector). For the current value of the I/O circuit, calculate with the number of points used and load.
(Note 3) When all DI/DO points are ON.
- 250 -
16. Cabinet and Installation
16.2 Power Supply
(4) Servo / Spindle
Refer to the following manuals for details on the servo and spindle system.
MDS-C1 Series SPECIFICATIONS MANUAL (BNP-C3040)
MDS-CH Series SPECIFICATIONS MANUAL (BNP-C3016)
MDS-R Series SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-C3045)
MDS-B-SVJ2 Series SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-B3937)
MDS-B-SPJ2 Series SPECIFICATIONS MANUAL (BNP-B2164)
MR-J2-CT Series SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-B3944)
- 251 -
17. Servo / Spindle System
17.1 Feed Axis
17. Servo / Spindle System
Refer to the following manuals for details on the servo and spindle system.
MDS-C1 Series
MDS-CH Series
MDS-R Series
MDS-B-SVJ2 Series
SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-C3045)
SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-B3937)
MR-J2-CT Series
17.1 Feed Axis
SPECIFICATIONS AND INSTRUCTION MANUAL (BNP-B3944)
17.1.1 MDS-C1-V1/C1-V2 (200V)
(1) Servo motor: HCxx-A51/E51(1000kp/rev)
E60 E68
M system
L system
–
–
(2) Servo motor: HCxx-A42/E42 (100kp/rev)
E60 E68
M system
L system
–
–
17.1.3 MDS-CH-V1/CH-V2 (400V)
(1) Servo motor: HCxx-A51/E51 (1000kp/rev)
E60 E68
M system –
L system –
(2) Servo motor: HCxx-A42/E42 (100kp/rev)
E60 E68
M system
L system
–
–
- 252 -
17. Servo / Spindle System
17.1 Feed Axis
17.1.4 MDS-B-SVJ2 (Compact and small capacity)
(1) Servo motor: HCxx-A42/E42 (100kp/rev)
E60 E68
M system
L system
(2) Servo motor: HCxx-A47 (100kp/rev)
E60 E68
M system
L system
(3) Servo motor: HCxx-A33/E33(25kp/rev)
E60 E68
M system
L system
(4) Servo motor: HC-SF/HC-RF (16kp/rev)
M system
E60 E68
L system
(5) Servo motor: HC-MF (8kp/rev)
E60 E68
M system
L system
17.1.6 MDS-R-V1/R-V2 (200V Compact and small capacity)
(1) Servo motor: HFxx-A48 (260kp/rev)
E60 E68
M system
L system
(2) Servo motor: HFxx-A47 (130kp/rev)
E60 E68
M system
L system
- 253 -
17. Servo / Spindle System
17.2 Spindle
17.2 Spindle
17.2.1
MDS-C1-SP/C1-SPH/C1-SPM/B-SP (200V)
(1) Spindle motor: SJ/SJ-V
M system
E60 E68
–
L system
(2) IPM spindle motor: SJ-PMF
–
M system
E60 E68
–
L system –
17.2.2 MDS-CH-SP/CH-SPH (400V)
M system
L system
E60 E68
–
–
17.2.3 MDS-B-SPJ2 (Compact and small capacity)
(1) Spindle motor: SJ-P/SJ-PF
E60 E68
M system
L system
Δ
Δ
- 254 -
17. Servo / Spindle System
17.3 Auxiliary Axis
17.3 Auxiliary Axis
17.3.1 Index/Positioning Servo: MR-J2-CT
(1) Servo motor: HC-SF/HC-RF(16kp/rev)
E60 E68
M system
L system
(2) Servo motor: HC-MF(8kp/rev)
M system
E60 E68
L system
17.4 Power Supply
17.4.1 Power Supply: MDS-C1-CV/B-CVE
M system
L system
17.4.2 AC Reactor for Power Supply
E60 E68
–
–
M system
L system
E60 E68
–
–
17.4.3 Ground Plate
M system
L system
E60 E68
Δ Δ
Δ Δ
- 255 -
18. Machine Support Functions
18.1 PLC
18. Machine Support Functions
18.1 PLC
18.1.1 PLC Basic Function
18.1.1.1 Built-in PLC Basic Function
M system
E60 E68
{
{
{
{
L system
(1) Ladder commands
Basic commands (bit processing commands)
20 commands including LD, LDI, OR, ORI, AND, ANI, OUT, PLS, etc.
Function commands
76 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
ATC control commands, and 14 others
Tool life management
Processing speed 2µs/step
- 256 -
18. Machine Support Functions
18.1 PLC
(2) Devices
The table below lists the devices that can be used by the PLC. (GX Developer)
X
Y
M
X0 to X4BF
Y0 to Y53F
M0 to M8191
Device Details Remarks
(1216 points)
(1344 points)
(8192 points)
1 bit
1 bit
1 bit
Input signal to PLC
Machine input, etc.
Output signal from PLC
Machine output, etc.
Temporary memory
F
L
F0 to F127
L0 to L255
(128 points) 1 bit
(256 points) 1 bit
Temporary memory,
Alarm message interface
Latch relay (backup memory)
SM
T
C
D
R
Z
N
P
K
H
SM0 to SM127
T0 to T15
T16 to T55
T56 to T135
T136 to T231
T232 to T239
T240 to T255
C0 to C23
C24 to C127
D0 to D1023
R0 to R8191
Z0 to Z1
N0 to N7
P0 to P255
K-32768 to K32767
K-2147483648
H0 to HFFFF
H0 to HFFFFFFFF
(128 points) 1 bit
(16 points) 1 bit/16 bits
Special relay
10 ms unit timer
(40 points)
(80 points)
1 bit/16 bits
1 bit/16 bits
10 ms unit timer (fixed timer)
100 ms unit timer
(96 points)
(8 points)
(16 points)
(24 points)
1 bit/16 bits
1 bit/16 bits
1 bit/16 bits
1 bit/16 bits
100 ms unit timer (fixed timer)
100 ms integral timer
100 ms integral timer (fixed timer)
Counter
(104 points) 1 bit/16 bits Counter (fixed counter)
(1024 points)
(8192 points)
(2 point)
16 bits/
32 bits
16 bits/
32 bits
16 bits
Data register
Register for arithmetic operations
File register. R500 to R549 and R1900 to
R2799 are released to the user for interface between the PLC and controller. R1900 to R2799 are backed up by the battery.
For D or R address indexing (for
±n)
(8 points) –––
(256 points) –––
–––
Master controller nesting level
Label for conditional jump and subroutine call commands
Decimal constant for 16-bit command
–––
–––
–––
Decimal constant for 32-bit command
Hexadecimal constant for 16-bit command
Hexadecimal constant for 32-bit command
(Note) The maximum number of part systems for E60/E68 is 1. Therefore, 2nd part system cannot be used.
- 257 -
18. Machine Support Functions
18.1 PLC
(3) External alarm messages
The contents of the alarms that have occurred during sequence (user PLC) processing can be displayed on the screen.
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 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 screen.
(6) Load meter display
A load meter can be displayed on the screen.
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 screen.
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.
- 258 -
18. Machine Support Functions
18.1 PLC
(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
The number of workpieces can be set and displayed when continuously machining workpieces.
The M code to be count, the current number of machined workpieces 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 workpieces 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.
<Relationship between file register contents and analog output voltage>
Analog output (V)
10V
–4095
0
Contents of file register
4095
–10V
Output voltage
Resolution
Load condition
Output impedance
0 to ±10V (±5%)
Full scale (10V)/4095
10 k
Ω resistance load (standard)
220
Ω
(Note) The remote I/O unit DX12x/DX14x and the base I/O unit HR341/HR351 are required for analog output.
- 259 -
18. Machine Support Functions
18.1 PLC
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
M system
E60 E68
{ {
{ {
L 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.
- 260 -
18. Machine Support Functions
18.1 PLC
18.1.3 Built-in PLC Capacity (Number of steps)
4000(PLC Emulation)
M system
L system
10000(PLC Emulation)
M system
L system
32000
M system
L system
E60 E68
{
{
–
–
–
–
E60 E68
{
{
E60 E68
–
–
Δ
Δ
18.1.4 Machine Contact Input/Output I/F
M system
L system
E60 E68
{ {
{ {
!
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 "EZMotion-NC E60/E68 Series CONNECTION AND MAINTENANCE MANUAL" for details.
- 261 -
18. Machine Support Functions
18.1 PLC
(1) Types of remote I/O units
Remote I/O unit list
Model
FCUA-DX100 Sink/Source input 32 points
Sink output 32 points
FCUA-DX101 Sink/Source input 32 points
Sink output 32 points
FUCA-DX110 Sink/Source input 64 points
Sink output 48 points
FCUA-DX111 Sink/Source input 64 points
Sink output 48 points
FUCA-DX120 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
FUCA-DX121 Sink/Source input 64 points
Sink output 48 points
Analog output 1 point
FCUA-DX140 Sink/Source input 32 points
Sink output 32 points
Analog input 4 points
Analog output 1 point
FCUA-DX141 Sink/Source input 32 points
Sink output 32 points
Analog input 4 points
Analog output 1 point
Component module model
RX311 card
Function
DI32/DO32
Case
RX312 card DI32/DO32
Case
RX311 card DI32/DO32
RX321-1 card DI32/DO16
Case
RX312 card DI32/DO32
RX322-1 card DI32/DO16
Case
RX311 card DI32/DO32
RX321 card DI32/DO16/AO1
Case
RX312 card DI32/DO32
RX322 card DI32/DO16/AO1
Case
RX311 card DI32/DO32
RX341 card AI4/AO1
Case
RX312 card DI32/DO32
RX341 card AI4/AO1
Case
- 262 -
18. Machine Support Functions
18.1 PLC
(2) Operation board remote I/O unit
With this function, the assignment of the operation board remote I/O directly connected with the control unit to the PLC device can be switched by the parameter. Depending on the parameter settings, the operation board remote I/O can be used as the remote I/O channel #2 equivalent.
Control unit
Remote I/O unit
RIO
FCUA-R211 cable
Assignment of the operation board remote I/O unit to the PLC device includes the following two patterns and can be switched.
(a) Standard (M50 compatible) assignment method (Pattern 1)
PLC devices are assigned by the M50 compatible assignment method. That means that the input device Nos. are assigned to X100 and after, and the output device Nos. are assigned to Y100 and after.
Up to 4 stations can be used for the remote I/O units. Set the rotary switch within the range
0 to 3.
(b) Remote I/O channel #2 equivalent assignment method (Pattern 2)
PLC devices are assigned by the remote I/O channel #2 equivalent method. That means that the input device Nos. are assigned to X640 and after, and the output device Nos. are assigned to Y740 and after.
Up to 8 stations can be used for the remote I/O units. Set the rotary switch within the range
0 to 7.
Remote I/O unit
Rotary switch No.
Device No. to be input Device No. to be output
0
1
2
3
4
5
6
7
Pattern 1 Pattern 2 Pattern 1 Pattern 2
X100 to X11F X640 to X65F Y100 to Y11F Y740 to Y75F
X120 to X13F X660 to X67F Y120 to Y13F Y760 to Y77F
R80, R81 X680 to X69F R180, R181 Y780 to Y79F
R82, R83
-
X6A0 to X6BF
X6C0 to X6DF
R182, R183 Y7A0 to Y7BF
- Y7C0 to Y7DF
-
-
-
X6E0 to X6FF
X700 to X71F
X720 to X73F
-
-
-
Y7E0 to Y7FF
Y800 to Y81F
Y820 to Y83F
(Note 1) X108 is assigned for an operation board reset signal and cannot be used for the other applications.
(Note 2) Analog output is not possible even if DX12x or DX14x is connected.
- 263 -
18. Machine Support Functions
18.1 PLC
(3) 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.
DI – L / DI – R
(Machine side)
DC24V(+)
2.2k
DI – L / DI – R
(Machine side)
Control circuit
0V
2.2k
Control circuit
DC24V(+)
COM
COM
0V
Source type Sink type
- 264 -
18. Machine Support Functions
18.1 PLC
(4) Outline of digital signal input circuit
The digital signal input circuit can be selected from the sink type or source type for each connector of each unit.
(a) Input circuit
Source type
(Machine side)
CF31(DI1) / CF32(DI2)
3.3kΩ
0V
3.3kΩ
0V
3.3kΩ
0V
3.3k
Ω
0V
3.3k
Ω
0V
Control circuit
24VDC
Sink type
(Machine side)
CF31 (DI1) / CF32 (DI2)
24VDC
3.3kΩ
A3, B3 COM
24VDC
3.3kΩ
24VDC
3.3kΩ
24VDC
3.3kΩ
24VDC
3.3kΩ
Control circuit
: 2.2k
Ω for
FCU6-DX220/DX221
A3, B3 COM
0V
- 265 -
18. Machine Support Functions
18.1 PLC
(b) Conditions for input
The input signals must be used within the following condition ranges.
Sink type
Input voltage at external contact ON 6V or less
Input current at external contact ON
Input voltage at external contact OFF
Input current at external contact OFF
Tolerable chattering time
Input signal holding time
Input circuit operation delay time
9mA or more
20V or more, 25.2V or less
2mA or less
3ms or less (Refer to T1 below)
40ms or more (Refer to T2 below) (Note 1)
3ms≦T3≒T4≦16ms
Machine side contact capacity 30V or more, 16mA or more
(Note 1) "40ms or more" is a rough standard. An input signal cannot be recognized unless it lasts longer than the period of the process cycle of the ladder.
Source type
Input voltage at external contact ON
Input current at external contact ON
18V to 25.2V
9mA or more
Input voltage at external contact OFF
Input current at external contact OFF
Tolerable chattering time
Input signal holding time
Input circuit operation delay time
4V or less
2mA or less
3ms or less (Refer to T1 below)
40ms or more (Refer to T2 below) (Note 1)
Machine side contact capacity
3ms≦T3≒T4≦16ms
30V or more, 16mA or more
(Note 1) "40ms or more" is a rough standard. An input signal cannot be recognized unless it lasts longer than the period of the process cycle of the ladder.
Sink type Source type
T2 T2
T1
T1
T1
T1
T3
T4
T3 T4
- 266 -
18. Machine Support Functions
18.1 PLC
(5) Outline of digital signal output circuit
The digital signal output circuit has the sink type and source type
(a) Output circuit
(Machine side)
(Machine side)
24VDC
CF33 (DO1) / CF34 (DO2) 24VDC
CF33 (DO1) / CF34 (DO2)
RA
RA
PL
R
Control circuit
R
Control circuit
PL
Sink type
Source type
(b) Conditions for output
Insulation method
Rated load voltage
Max. output current
Output delay time
Non-insulation
24VDC
60mA/Point
40
μs
(6) Outline of analog signal output circuit (Only FCU6-HR341/HR351)
Analog signals are output to the CF34 connector or AO connector, so connect either of the connectors which is easier to connect.
(a) Output circuit
CF34 (DO2)
AO
B4
A4
AO*
AO
AO
7
AO*
220Ω
1, 5, 11, 15
Ｒ
Ｒ
ＤＡＣ
(b) Conditions for output
Output voltage
Resolution
Load condition
Output impedance
0V to ±10V(±5%)
12bits (±10V×n/4096) (n=2
0
to 2
11
)
10k
Ω load resistance
220
Ω
- 267 -
18. Machine Support Functions
18.1 PLC
18.1.5 Ladder Monitor
M system
E60 E68
{
{
{
{
L system
This function enables the operating status of the sequence circuit to be checked on the screen.
The monitor functions include the following.
(2) Screen stop by monitor stop trigger point
(4) Decimal-hexadecimal conversion present value monitoring
18.1.6 PLC Development
18.1.6.1 On-board Development
M system
E60 E68
{ {
{ {
L system
PLC ladders can be developed on the control unit.
PLC ladder circuits can be created, edited, etc.
18.1.6.2 MELSEC Development Tool
M system
E60 E68
{ {
{ {
L system
The GX Developer installed in a personal computer (OS: Windows) can be used.
- 268 -
18. Machine Support Functions
18.1 PLC
18.1.9 PLC Password Lock
M system
E60 E68
{
{
{
{
L system
This function makes it possible to use a code number to prohibit user PLC editing and input/output in order to prevent the illegal writing by the end users of the user PLC data prepared by the machine tool builder.
User PLC protection using code number
On-board PLC file writing, editing operations (write, insert, delete, change) for PLC circuits and PLC file input/output operations are enabled by inputting the code number.
The operations that are prohibited during user PLC protection by the code number are listed in the table below.
List of operations
Operation
Ladder circuits Readout
Code number input
Possible
No code number input
Possible
Remarks
PLC files
External alarm messages
RUN/STOP Possible Possible
Input/output Possible Impossible
- 269 -
18. Machine Support Functions
18.1 PLC
18.1.13 PLC Message
Japanese
M system
E60 E68
{
{
{
{
English
L system
M system
E60 E68
{ {
{ {
L system
German
M system
L system
E60 E68
{ {
{ {
Italian
M system
L system
E60 E68
{ {
{ {
French
M system
L system
E60 E68
{ {
{ {
Spanish
M system
L system
E60 E68
{
{
{
{
Chinese (Simplified Chinese characters)
E60 E68
M system
L system
{
{
{
{
Portuguese
M system
L system
E60 E68
{ {
{ {
- 270 -
18. Machine Support Functions
18.1 PLC
Hungarian
M system
L system
Dutch
M system
L system
Swedish
M system
L system
E60 E68
{
{
{
{
E60 E68
{
{
{
{
E60 E68
{ {
{ {
18.1.14 User PLC version up
M system
E60 E68
–
–
{
{
L system
With this function, version upgrade is available by using the ROM cassette in which PLC program is written.
- 271 -
18.2 Machine Construction
18. Machine Support Functions
18.2 Machine Construction
18.2.1 Servo OFF
M system
E60 E68
{ {
{ {
L 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.
- 272 -
18. Machine Support Functions
18.2 Machine Construction
18.2.2 Axis Detach
M system
E60 E68
{
{
{
{
L system
This function enables the control axis to be freed from control. Conversely, an axis that 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 control axis detach command has been released completes its dog-type reference position return.
C-axis/turning table
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.
Rotary magnetic scale
(Position feedback)
(OFF with C-axis control )
Spindle
motor
C-axis motor
(Coupled with C-axis control)
Spindle amplifier
C-axis amplifier
POSITION
X 1 2 3 . 4 5 6
Z 0 . 0 0 0 #1
C 3 4 5 . 6 7 8 ><
The detached status > < is indicated on the right of the current value 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.
(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.
- 273 -
18. Machine Support Functions
18.2 Machine Construction
18.2.4 Inclined Axis Control
M system
E60 E68
– –
{ {
L system
Even when the control axes configuring that machine are mounted at an angle other than 90 degrees, this function enables it to be programmed and controlled in the same way as with an orthogonal axis.
The inclination angle is set using a parameter, and axes are controlled using the movement amounts of the axes that are obtained through conversion and offset using this angle.
<Example of use> When the X axis serves as the basic axis and the Y axis serves as the inclined axis
X
Yp*tan
θ
Xa
X: Actual X axis
Y: Actual Y axis y: Programmed Y axis
θ: Inclination angle
θ
θ
Yp/cos
θ
Ya
Yp
Y y
The Y-axis position and Yp on the programmed coordinates (on the orthogonal coordinates) are respectively the Xa and Ya positions produced by combining the X axis and Y axis along which the machine actually moves.
Therefore, the Y-axis (inclined axis) movement amount is expressed by the following formula:
Ya = Yp/cos (1)
The X-axis (basic axis) movement amount is offset by the inclined movement of the Y axis, and it is expressed as follows:
Xa = Xp - Yp x tan
θ (2)
The Y-axis (inclined axis) speed is as follows:
Fa = Fp/cos
θ
Xa, Ya and Fa are the actual movement amounts and speed.
Xp, Yp and Fp are the movement amounts and speed on the program coordinates.
- 274 -
18. Machine Support Functions
18.2 Machine Construction
18.2.5 Index Table Indexing
M system
L system
E60 E68
–
{
– {
The indexing of the index table can be performed by setting the index axes. Programming is facilitated because, in terms of the index commands, only the indexing angle need to be designated using the address of the programmed axis serving as the index setting axis, and there is no need to designate special M codes for clamping and unclamping the table.
The following operations are performed for the index table indexing function.
(1) Set "1" to the "index axis selection" parameter for the axis along which the indexing table is to be indexed.
(2) Designate the movement commands (absolute or incremental) for the selected axis using a program.
(3) The unclamp command signal is now output prior to the axis movement.
(4) When the axes are unclamped, the unclamp finish signal is set (ladder used for processing).
(5) After checking the unclamp finish signal, the designated axis starts moving.
(6) Upon completion of the movement, the unclamp command signal is set to OFF.
(7) Clamp the axes and set the unclamp finish signal to OFF (ladder used for processing).
(8) After checking that the unclamp finish signal is OFF, processing of the next block is initiated.
Operation timing chart
Programmed command
G0 B90.;
Unclamp command
Unclamp finish
B-axis movement
T10 Standing by for completion 0800 T10 Standing by for completion 0800
- 275 -
18. Machine Support Functions
18.2 Machine Construction
18.2.6 NSK Table Connection Control
M system
L system
E60 E68
–
{
– {
By assigning commands to the control unit from the 2nd miscellaneous function and the PLC and pulse train input, this function transmits commands by serial communication (RS-232C specification) to the dedicated drive unit of the NSK mega-torque motor.
Command designation method
By setting the command for the prescribed R register and the numerical value command following address B designated by the 2nd miscellaneous function as signed binary numbers using the PLC, the control unit prepares the positioning commands from this command and numerical value command, and it sends them to the drive unit by serial communication (RS-232C specification).
Furthermore, by setting ON the handle mode of the prescribed R register using the PLC, the pulse train input based on the handle is sent as the movement command to the drive unit.
Designate the commands with the number of mega-torque motor axes connected already set in the parameter and with the settings for the input/output basic parameters used for communication already set. Up to 16 axes can be connected as the mega-torque motor axes.
The numerical value command in angle increments is prepared by setting the numerical value following address B of the 2nd miscellaneous function as a signed binary number in the prescribed
R register using the PLC.
- 276 -
18. Machine Support Functions
18.2 Machine Construction
18.2.7 Auxiliary Axis Control (J2-CT)
M system
L system
E60 E68
Δ Δ
Δ Δ
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.
(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.
(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.
(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 position return mode
In this mode, the axis is positioned at the coordinate reference position. Two methods are used: one method is based on a dog switch and the other method is to carry out positioning to the reference position that 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.
- 277 -
18. Machine Support Functions
18.3 PLC Operation
18.3 PLC Operation
18.3.1 Arbitrary Feed In Manual Mode
M system
E60 E68
{ {
{ {
L 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).
- 278 -
18. Machine Support Functions
18.3 PLC Operation
18.3.3 PLC Axis Control
M system
L system
E60 E68
Δ Δ
Δ Δ
Over and above the NC control axes, this function enables axes to be controlled independently by commands based on the PLC.
PLC
ATC
PLC axis control
DDB function
- 279 -
18. Machine Support Functions
18.3 PLC Operation
Item Description
E60 E68
Max. 2 axes Number of control axes Max. 1 axes
Simultaneously controlled axes
Least command increment
Feed rate
PLC control axis is controlled independently from NC control axes.
A multiple number of PLC axes can be started simultaneously.
Least command increment Least command increment inch) (0.0001
0.0001mm (0.00001 inch)
(Least command increment: (Least command increment:
0.001mm)
Rapid traverse
0 to 240000 mm/min
(0 to 9448.8 inch/min)
Cutting feed
0 to 240000 mm/min
(0 to 9448.8 inch/min)
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 to ±99999999
(0.001mm/0.0001 inch) (0.001mm/0.0001 inch)
0 to ±9999999
(0.0001mm/0.00001 inch)
Operation modes Rapid traverse, cutting feed, jog feed (+) (–), reference position return feed (+) (–), handle feed
Acceleration/deceleration Rapid traverse, jog feed, reference position return feed
..... Linear acceleration/deceleration
Cutting feed ..... Exponential function acceleration/deceleration
Handle feed .......Step
Backlash compensation Available
Stroke end None
Soft limit
Rotary axis command
Available
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
Position detector
None
Set to the command that corresponds to the feedback unit.
Encoder (Absolute position can also be detected.)
(Note) Least input setting increment "C" (0.0001(°)mm/0.00001inch) is a specification for E68 system. This cannot be used with E60
- 280 -
18. Machine Support Functions
18.4 PLC Interface
18.4 PLC Interface
18.4.1 CNC Control Signal
M system
E60 E68
{ {
{ {
L 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 [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.
- 281 -
18. Machine Support Functions
18.4 PLC Interface
18.4.2 CNC Status Signal
M system
E60 E68
{
{
{
{
L 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)
- 282 -
18. Machine Support Functions
18.4 PLC Interface
(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 (including the control 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.
- 283 -
18. Machine Support Functions
18.4 PLC Interface
18.4.5 DDB
M system
E60 E68
{
{
{
{
L 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 capabilities of referencing read data or write data in the next step just after a DDBA instruction is executed.
- 284 -
18. Machine Support Functions
18.5 Machine Contact I / O
18.5 Machine Contact I / O
DI:64/DO:64
M system
E60 E68
–
–
L system
DI:64/DO:48/A0:1
M system
L system
E60 E68
{
{
DI:96/DO:80
M system
E60 E68
–
–
L system
DI:96/DO:80/A0:1
M system
L system
E60 E68
–
–
Additional DI/DO (DI:64/DO:48)
E60 E68
M system
L system
Additional DI/DO(DI:32/DO:32)
M system
L system
E60 E68
Operation board IO (DI:32/DO:32)
M system
L system
E60 E68
Operation board IO DI:64/DO:48
M system
L system
E60 E68
- 285 -
Remote IO 32/32
M system
L system
Remote IO 64/48
M system
L system
18. Machine Support Functions
18.5 Machine Contact I / O
E60 E68
Δ Δ
Δ Δ
E60 E68
Δ
Δ
Δ
Δ
- 286 -
18. Machine Support Functions
18.7 Installing S/W for Machine Tools
18.7 Installing S/W for Machine Tools
18.7.3 Simple Customization
M system
E60 E68
{ {
{ {
L system
Some messages can be displayed on the initial screen that appears when NC power is turned ON.
The total messages can include up to 40 characters in a line and up to 10 lines.
- 287 -
Appendix 1. List of Specifications
Appendix 1. List of Specifications
- 288 -
Appendix 2. Format Details
Appendix 2. Format Details
Program number
Sequence number
Preparatory function
Movement axis
Arc and cutter radius
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Dwell
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Feed function
0.0001 (°) mm/
0.00001 inch
Tool offset
Miscellaneous function (M)
Spindle function (S)
Tool function (T)
2nd miscellaneous function
Subprogram
Fixed cycle
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
Metric command
08
N5
G3/G21
Inch command
←
←
←
M system
Rotary axis
(Metric command)
←
←
←
Rotary axis
(Inch command)
←
←
←
X+53 Y+53 Z+53
α+53
X+44 Y+44 Z+44
α+44
X+53 Y+53 Z+53
α+53 X+53 Y+53 Z+53 α+53
X+44 Y+44 Z+44
α+44
X+35 Y+35 Z+35
α+35
X+44 Y+44 Z+44
α+44 X+44 Y+44 Z+44 α+44
I+53 J+53 K+53 R+53
I+44 J+44 K+44 R+44
I+44 J+44 K+44 R+44
I+35 J+35 K+35 R+35
I+53 J+53 K+53 R+53
I+44 J+44 K+44 R+44
I+44 J+44 K+44 R+44
(Note 5)
I+35 J+35 K+35 R+35
(Note 5)
X+53 P+8
← ← ←
X+53/P+8
F63(Feed per minute)
F43(Feed per revolution)
F44(Feed per minute)
F34(Feed per revolution)
F54(Feed per minute)
F34(Feed per revolution)
F35(Feed per minute)
F25(Feed per revolution)
H3 D3
M8
S8
T8
A8/B8/C8
P8 H5 L4
R+53 Q53 P8 L4
←
←
←
←
←
←
←
←
← ←
F63(Feed per minute)
F43(Feed per revolution)
F44(Feed per minute)
F34(Feed per revolution)
(Note 6)
F54(Feed per minute)
F34(Feed per revolution)
←
←
←
←
←
←
F35(Feed per minute)
F25(Feed per revolution)
(Note 6)
←
←
←
←
←
←
← ←
R+44 Q44 P8 L4
← ← ←
Program number
Sequence number
Preparatory function
Movement axis
0.001(°) mm/
0.0001 inch
Arc and cutter radius
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Dwell
0.0001(°) mm/
0.00001 inch
0.001(°) mm/
0.0001 inch
Feed function
0.0001(°) mm/
0.00001 inch
Tool offset
Miscellaneous function (M)
Spindle function (S)
Tool function (T)
2nd miscellaneous function
Subprogram
0.001(°) mm/
0.0001 inch
Fixed cycle
0.0001(°) mm/
0.00001 inch
Metric command
08
N5
G3/G21
Inch command
←
←
←
L system
Rotary axis
(Metric command)
←
←
←
Rotary axis
(Inch command)
←
←
←
X+53 Y+53 Z+53
α+53
X+44 Y+44 Z+44
α+44
X+53 Y+53 Z+53
α+53 X+53 Y+53 Z+53 α+53
X+44 Z+44
α+44 X+35
I+53 J+53 K+53 R+53
I+44 K+44 R+44
X+53 P+8
I+44 J+44 K+44 R+44
I+35 K+35 R+35
←
I+53 J+53 K+53 R+53
I+44 K+44 R+44
←
I+44 J+44 K+44 R+44
(Note 5)
I+35 K+35 R+35
(Note 5)
←
X+53/P+8
F63(Feed per minute)
F35(Feed per revolution)
F54(Feed per minute)
F34(Feed per revolution)
T1/T2
M8
S8
T8
A8/B8/C8
P8 H5 L4
R+53 Q53 P8 L4
← ← ←
F44(Feed per minute)
F26(Feed per revolution)
F35(Feed per minute)
F25(Feed per revolution)
←
←
←
←
←
←
F63(Feed per minute)
F34(Feed per revolution)
F54(Feed per minute)
F34(Feed per revolution)
←
←
←
←
←
←
F44(Feed per minute)
F26(Feed per revolution)
(Note 6)
F35(Feed per minute)
F25(Feed per revolution)
(Note 6)
←
←
←
←
←
←
← ← ←
R+44 Q44 P8 L4
← ← ←
- 289 -
Appendix 2. Format Details
(Note 1)
α 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.
(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.
(Note 10) Least input setting increment "C" (0.0001(°)mm/0.00001inch) and dwell's U address are specifications for E68 system. These cannot be used with E60.
- 290 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3. Outline and Installation Dimension Drawings of Units
Appendix 3.1 E60 Control Unit, Display Unit, Keyboard Unit Outline Drawing
Appendix 3.1.1 Control unit, display unit (FCU6-MU071, FCU6-DUN26) outline drawing
Panel-cut drawing
260
260(Unit outline)
250
±
0.3
20 120
(Space required for wiring: with expansion PCB)
How to fix with screws from the front of the unit (Reference)
251
4-M3 screw
4-C10
- 291 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.1.2 Keyboard unit (FCU6-KB024) outline drawing
140
Panel-cut drawing
140 (Keyboard outline)
130
±0.3
122
20 110
Space required for wiring
How to fix with screws from the front of the unit (Reference)
4-M3 screw
- 292 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.1.3 Control unit (FCU6-MU071, FCU6-KB071) outline drawing
(1) In the case of FCU6-KB071 (Fix with screws from the back of the unit)
140
Panel-cut drawing
20 80
Wiring space
(60)
How to fix with screws from the back of the unit (Reference)
Square hole
(Keyboard outline) hole
Machine side mounting plate
- 293 -
Appendix 3. Outline and installation dimension drawings of units
(2) In the case of FCU6-KB071-1 (Fix with screws from the front of the unit)
140 24 76
W iring space
(60)
Panel-cut drawing
(Keyboard outline)
How to fix with screws from the front of the unit
(Reference)
Square hole
- 294 -
Machine side mounting plate
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.1.4 Display unit (FCU6-DUE71) outline drawing
(1) In the case of FCU6-DUE71 (Fix with screws from the back of the unit)
Panel-cut drawing
260 20
Wiring space
(50)
230
How to fix with screws from the back of the unit (Reference)
Square hole
(Display unit outline) hole
Machine side mounting plate
- 295 -
Appendix 3. Outline and installation dimension drawings of units
(2) In the case of FCU6-DUE071-1 (Fix with screws from the front of the unit)
260
Panel-cut drawing
24 226
Wiring space
(50)
How to fix with screws form the front of the unit (Reference)
Square hole
(Display unit outline)
Machine side mounting plate
- 296 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.1.5 Display unit (FCU6-DUT11) outline drawing
(1) In the case of FCU6-DUT11 (Fix with screws from the back of the unit)
Panel-cut drawing
260
20 22
Wiring space
(50)
How to fix with screws from the back of the unit (Reference)
Square hole
(Display unit outline)
Machine side mounting plate
hole
- 297 -
Appendix 3. Outline and installation dimension drawings of units
(2) In the case of FCU6-DUT11-1 (Fix with screws from the back of the unit)
Panel-cut drawing
260
24 18
Wiring space
(50)
How to fix with screws from the front of the unit (Reference)
Square hole
(Display unit outline)
Machine side mounting plate
- 298 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.2 E68 Control Unit, Display Unit, Keyboard Unit Outline Drawing
Appendix 3.2.1 Control unit, display unit (FCU6-MU072,FCU6-DUN24) outline drawing
Panel-cut drawing
260
260 (Unit outline)
250
±0.3
4-M3 screw
4-C10
251
- 299 -
20 120
(Space required for wiring: with expansion PCB)
How to fix with screws from the front of the unit (Reference)
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.2.2 Keyboard unit (FCU6-KB024) outline drawing
140
Panel-cut drawing
140 (Keyboard outline)
130
±0.3
122
20 110
Space required for wiring
How to fix with screws from the front of the unit (Reference)
4-M3 screw
- 300 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.2.3 Front IC card I/F unit (FCU6-EP105-1) outline drawing
(1)
Explanation of the front IC card I/F unit/connector functions
No. Connector
(1) Memory
Card I/F
Function
PC Card Standard
ATA-compliant CF card
TYPEI, TYPEII only
(5VDC : max 220mA)
- 301 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.3 External Power Supply Unit (PD25) Outline Drawing
65
φ6
AC IN
6
ON/OFF SW
ON/OFF
POWER
DC OUT
2-
R
3
6
30
130
- 302 -
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.4 Base I/O Unit Outline Drawing
Appendix 3.4.1 FCU6-HR341/HR351 outline drawing
Wiring space
(100)
6
Appendix 3.4.2 FCU6-DX220/DX221 outline drawing
Wiring space
(100)
208
220
6
6 208
220
- 303 -
6
Appendix 3. Outline and installation dimension drawings of units
Appendix 3.5 Remote I/O Unit (FCUA-DX1xx) Outline Drawing
- 304 -
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
1 Control axes
1 Control axes
1 Number of basic control axes (NC axes)
2 Max. number of control axes (NC axes + Spindles + PLC axes + Auxiliary axes)
Max. number of axes (NC axes + Spindles + PLC axes)
Max. number of servo axes (NC axes + PLC axes)
Max. number of NC axes (in total for all the part systems)
Max. number of spindles (parenthesis means max. number in a part system)
Max. number of PLC axes
Max. number of auxiliary axes (MR-J2-CT)
3 Number of simultaneous contouring control axes
4 Max. number of NC axes in a part system
2 Control part system
1 Standard number of part systems
2 Max. number of part systems
3 Control axes and operation modes
1 Tape (RS-232C input) mode
2 Memory mode
3 MDI mode
5 IC card mode
2 Front IC card
2 Input command
1 Data increment
1 Data increment and parameter
2 Least input increment
3 Least command increment
Least command increment 1um
2 Unit system
Least command increment 0.1um
1 Inch/Metric changeover
3 Program format
1 Character code
2 Program format
1 Format 1 for Lathe
3 Special format for Lathe
4 Format 1 for Machining center
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
5 Cylindrical interpolation
6 Polar coordinate interpolation
○
○
○
○
○
○
-
-
-
○
○
○
○
○
○
○
○
-
○
-
○
○
○
○
-
-
-
○
○
○
○
-
-
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
-
○
○
○
○
○
M
E68
L
1
○1
○
○
○
2
4
4
2
○ 2
8
6
6
4
4
-
1
○1
○
○
○
○
2
4
4
2
○ 3
8
6
6
4
4
M
E60
L
1
○1
○
○
○
1
1
3
1
○ 3
5
5
4
3
3
-
1
○1
○
○
○
1
1
3
1
○ 2
5
5
4
3
3
-
○
○
○
-
○
-
○
○
○
○
○
○
－
-
-
○
○
－
1 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
4 Feed
1 Feed rate
1 Rapid traverse rate (m/min)
2 Cutting feed rate (m/min)
3 Manual feed rate (m/min)
2 Feed rate input methods
1 Feed per minute
2 Feed per revolution
4 F 1-digit feed
3 Override
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
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
2 Pecking tapping cycle
3 Deep-hole tapping cycle
4 Chamfering
6 Manual feed
1 Manual rapid traverse
7 Dwell
2 Jog feed
3 Incremental feed
4 Handle feed
5 Manual feed rate B
1 Dwell (Time-based designation)
5 Program memory/editing
1 Memory capacity
1 Memory capacity (number of programs stored)
600m (400 programs)
2 Editing method
1
Program editing
2 Background editing
3 Buffer correction
4 Word editing
○
○
○
○
○
M
E68
L
1000
1000
1000
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○(2)
○
○
-
-
○
○
1000
1000
1000
○
○
○
○
○
○
○
○
○
○
-
○
○
○
-
○
○
○
○(2)
○
○
M
E60
L
1000
1000
1000
○
○
○
○
○
○
○
○
○
○
○
△
-
-
○
○
○
○
○(2)
○
○
1000
1000
1000
○
○
○
○
○
○
○
○
○
○
-
-
-
△
-
○
○
○
○(2)
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
2 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
6 Operation and display
1 Structure of operation/display panel
7.2-type LCD monochrome display
9-type CRT monochrome display
8.4-type LCD (TFT) color display
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
11 Additional languages
1 Japanese
2 English
3 German
4 Italian
5 French
6 Spanish
7 Chinese
Traditional Chinese characters
Simplified Chinese characters
8 Korean
9 Portuguese
10 Hungarian
11 Dutch
12 Swedish
12 Screen saver, backlight OFF
13 Screen deletion
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
6 Remote program input
7
System configuration data output
2 Input/Output I/F
1 RS-232C I/F
2 IC card I/F
2 I/F for front IC card
3 Computer link
1 Computer link B
M
E68
L
-
-
○
○
○
○
○*
○*
○*
○*
○*
○
○*
○*
○*
○*
○*
○
○
○
○
○
○
○
○
○
○
○13
○
○
○
○
○
○
○
○
○
○
-
-
○
○
○
○
○*
○*
○*
○*
○*
○
○*
○*
○*
○*
○*
○
○
○
○
○
○
○
○
○
○
○13
○
○
○
○
○
○
○
○
○
○
M
E60
L
-
-
○
○
○
○
○
-
○
○
□
□
□
○
○
○
○*
○*
○*
○*
○*
○
○*
○*
○*
○*
○*
○
○
○
○
○
○
○
○
○
○
○13
-
-
○
○
○
○
○
-
○
○
□
□
□
○
○
○
○*
○*
○*
○*
○*
○
○*
○*
○*
○*
○*
○
○
○
○
○
○
○
○
○
○
○13
3 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
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
2 Multiple-spindle control II
3 Position control
1 Spindle orientation
2 Spindle position control (Spindle/C axis control)
3 Spindle synchronization
1 Spindle synchronization I
2 Spindle synchronization II
11 Spindle holding power improvement
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
4 2nd miscellaneous function (B)
1 2nd miscellaneous function
9 Tool compensation
1 Tool length/poistion offset
1 Tool length offset
2 Tool position 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
3 80
5 200
6 400
2 Offset memory
1 Tool shape/wear offset amount
M
E68
L
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
□
○
○
○
○
○
-
-
○
○
-
-
-
○
○
M
E60
L
○
○
○
○
○
○
-
-
△
-
-
△
△
○
△
○
○
○
○
○
○
-
-
○
-
-
-
○
-
○
○
-
○
-
○
○
○
-
-
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
□
○
○
○
-
○
-
○
○
○
-
-
○
○
○
○
○
○
○
-
-
△
-
-
△
△
○
△
○
○
○
○
○
4 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
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
6 Workpiece coordinate system preset (G92.1)
7 Local coordinate system
8 Coordinate system for rotary axis
9 Plane selection
10 Origin set
11 Counter set
2 Return
1 Manual reference position return
2 Automatic 1st reference position return
3 2nd, 3rd, 4th reference position return
4 Reference position verification
5 Absolute position detection
6 Tool exchange position return
7 C axis reference 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
4 Graphic check
5 Graphic trace
3 Program search/start/stop
1 Program search
2 Sequence number search
3 Collation stop
4 Program restart
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 position retract
14 PLC interruption
M
E60
L
○
○
○
-
○
○
○
-
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
△
○
-
-
○
○
○
○
○
○
○
○
○
○
○
○
○
-
○
○
○
-
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
△
○
△
○
○
○
○
M
E68
L
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
△
○
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
△
○
-
-
○
○
○
○
○
○
○
○
○
○
5 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
12 Program support functions
1 Machining method support functions
1 Program
1 Subprogram control
3 Scaling
2 Macro program
1 User macro
2 Machine tool builder macro
1 Machine tool builder macro SRAM
3 Macro interruption
4 Variable command
2 200 sets
3 300 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
5 Multiple repetitive fixed cycle for turning machining (Type II)
6 Small-diameter deep-hole drilling cycle
7 Fixed cycle for drilling (Type II)
4 Mirror image
1 Mirror image by parameter setting
2 External input mirror image
3 G code mirror image
4 Mirror image for facing tool posts
5 T code mirror image for facing tool posts
5 Coordinate system operation
1 Coordinate rotation by program
6 Dimension input
1 Corner chamfering/Corner R
2 Linear angle command
3 Geometric command
4 Polar coordinate command
7 Axis control
1 High-speed machining
3 High-speed machining mode III
2 Chopping
1 Chopping
5 Circular 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
High-accuracy control (G61.1)
High-accuracy control (G08)
3 Programming support functions
1 Playback
2 Address check
M
E68
L M
E60
L
○
○
○
○
○
○
○
○
○
-
○
-
-
-
○
○
○
○
○
○
○
○
○
○
○
△
○
○
○
○
○
○
○8 layers ○8 layers ○8 layers ○8 layers
○
-
○
-
-
-
○
○
○
○
○
○
○
○
-
-
-
-
-
○
○
○4 layers ○4 layers ○4 layers ○4 layers
○
○
○
○
-
○
-
○
-
○
-
○
○
-
○
○
○
-
○
○
-
-
-
-
-
-
○
○
○
-
○
-
○
○
-
-
○
-
-
○
○
-
-
○
○
○
-
-
-
○
-
-
○
○
○
○
-
○
○
○
-
-
-
-
-
-
-
-
-
○
○
○
○
○
○
○
○
○
○
-
-
○
○
-
○
○
○
○
-
-
○
○
○
○
○
-
-
○
○
6 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
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
9 Spindle backlash compensation
2 Dynamic accuracy compensation
1 Smooth high-gain control (SHG control)
2 Dual feedback
3 Lost motion compensation
14 Automation support functions
1 External data input
1 External search
2 External workpiece coordinate offset
3 External tool offset
2 Measurement
1 Skip
1 Skip
2 Multiple-step skip
4 PLC skip
5 Automatic tool length measurement
6 Manual tool length measurement 1
7 Manual tool length measurement 2
8 Workpiece coordinate offset measurement
9 Workpiece position measurement
3 Monitoring
1 Tool life management
Tool life management I
Tool life management II
2 Number of tool life management sets
20/40/80 sets
100/200 sets
3 Display of integrated time/number of parts
4 Load meter
5 Position switch
12 Synchronous error observation
5 Others
1 Programmable current limitation
M
E68
L
○
○
○
○
○
○
△
○
○
○
○
○
○
○
○
○
○
△
○
○
○
○
M
○
○
○
○
-
○
-
○
○
○
○
○
○
-
○200
○
○
○24
○
○
○
○
○
○
○
○
○*
○
○
○
-
○100
○
○
○24
-
-
-
-
-
○
○
-
○
○
○
○
○80
-
○
○
○24
○
○
○
○
○
○
○
○
○
-
E60
L
○
○
○80
-
○
○
○24
-
-
○
○
-
○
○
○
-
-
○
○
○
○
-
○
-
○
○
○
○
7 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
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
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
3 Data sampling
4 Waveform display
5 Machine operation history monitor
6 NC data backup
RS-232C
Cassette memory
IC card
7 PLC I/F diagnosis
6 Signal tracing
M
E68
L
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
○
M
E60
L
○
○
○
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
-
-
○
-
-
○
○
○
○
○
○
○
○
○
○
○
○
○
○
-
○
○
○
○
○
○
○
○
○
○
○
-
-
-
○
○
○
8 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
16 Cabinet and installation
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)
3 MDS-CH-V1/CH-V2 (400V)
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)
Servo motor: HC-SF/HC-RF (16kp/rev)
Servo motor: HA-FF/HC-MF (8kp/rev)
6 MDS-R-V1/R-V2 (200V Compact and small capacity)
Servo motor: HF**-A48 (260kp/rev)
Servo motor: HF**-A47 (100kp/rev)
2 Spindle
1 MDS-C1-SP/C1-SPM/B-SP (200V)
Spindle motor: SJ/SJ-V
IPM spindle motor: SJ-PMF
2 MDS-CH-SP/CH-SPH (400V)
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
M
E68
L M
E60
L
□
□
□
□
△
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
-
-
△
-
-
-
△
-
-
□
□
□
□
□
□
□
-
-
□
□
□
□
△
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
□
-
-
△
-
-
-
△
-
-
□
□
□
□
□
□
□
-
-
9 / 10
EZMotion-NC E60/E68 Series Specifications List
○:Standard, ○*:Display only, △:Optional, ☆:Planning, □:Selection
Class
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)
4000(PLCemulation)
6000(PLCemulation)
32000
4 Machine contact input/output I/F
5 Ladder monitor
6 PLC development
1 On-board development
2 MELSEC development tool
9 PLC password lock
13 PLC message
1 Japanese
2 English
3 German
4 Italian
5 French
6 Spanish
7 Chinese
Simplified Chinese characters
9 Portuguese
10 Hungarian
11 Dutch
12 Swedish
14 User PLC version up
2 Machine construction
1 Servo OFF
2 Axis detach
4 Inclined axis control
5 Index table indexing
6 NSK table connection control
7 Auxiliary axis control
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
DI:64/DO:64
DI:64/DO:48/AO:1
DI:96/DO:80
DI96/DO:80/AO:1
Additional DI/DO (DI:64/DO:48)
Additional DI/DO (DI:32/DO:32)
Operation board IO DI:32/DO:32
Operation board IO DI:64/DO:48
Remote IO 32/32
Remote IO 64/48
7 Installing S/W for machine tools
3 Simple customization
M
E68
L
○
△
○
○
○
○
○
-
○
○
△
□
□
□
□
□
□
□
□
△
△
○
○
○
○
○
○
○
○
○
○
○
○
○
-
○
△
○
○
○
○
○
○
○
M
E60
L
○
○
○
-
-
○
○
○
○
○
○
○
○
○
○
○
○
△
○
○
○
○
○
○
○
○
-
-
-
○
○
-
△
-
○
□
□
△
△
-
-
□
□
○
○
△
○
○
○
○
○
○
○
○
△
□
□
□
□
□
□
□
□
△
△
○
○
○
○
○
○
○
○
○
○
○
○
○
-
○
△
○
○
○
○
○
○
○
○
○
○
-
-
○
○
○
○
○
○
○
○
○
○
○
○
△
○
○
○
○
○
○
○
○
-
-
-
△
○
○
○
-
○
□
□
△
△
□
□
-
-
○
10 / 10
Revision History
Date of revision
Mar. 2006
Manual No.
IB(NA)1500171-A First edition created.
Aug. 2006
Revision details
IB(NA)1500171-B • Contents were revised to correspond to E60 system S/W version C.
• FCU6-DUN26, color display for E60 was added.
• Mistakes were corrected.
Global service network
NORTH AMERICA FA Center
EUROPEAN FA Center
CHINA FA Center
KOREAN FA Center
North America FA Center (MITSUBISHI ELECTRIC AUTOMATION INC.)
Illinois CNC Service Center
500 CORPORATE WOODS PARKWAY, VERNON HILLS, IL. 60061, U.S.A.
TEL: +1-847-478-2500 (Se FAX: +1-847-478-2650 (Se
California CNC Service Center
5665 PLAZA DRIVE, CYPRESS, CA. 90630, U.S.A.
TEL: +1-714-220-4796
Georgia CNC Service Center
FAX: +1-714-229-3818
2810 PREMIERE PARKWAY SUITE 400, DULUTH, GA., 30097, U.S.A.
TEL: +1-678-258-4500 FAX: +1-678-258-4519
New Jersey CNC Service Center
200 COTTONTAIL LANE SOMERSET, NJ. 08873, U.S.A.
TEL: +1-732-560-4500 FAX: +1-732-560-4531
Michigan CNC Service Satellite
2545 38TH STREET, ALLEGAN, MI., 49010, U.S.A.
TEL: +1-847-478-2500
Ohio CNC Service Satellite
FAX: +1-269-673-4092
62 W. 500 S., ANDERSON, IN., 46013, U.S.A.
TEL: +1-847-478-2608 FAX: +1-847-478-2690
Texas CNC Service Satellite
1000, NOLEN DRIVE SUITE 200, GRAPEVINE, TX. 76051, U.S.A.
TEL: +1-817-251-7468
Canada CNC Service Center
FAX: +1-817-416-1439
4299 14TH AVENUE MARKHAM, ON. L3R OJ2, CANADA
TEL: +1-905-475-7728 FAX: +1-905-475-7935
Mexico CNC Service Center
MARIANO ESCOBEDO 69 TLALNEPANTLA, 54030 EDO. DE MEXICO
TEL: +52-55-9171-7662 FAX: +52-55-9171-7698
Monterrey CNC Service Satellite
ARGENTINA 3900, FRACC. LAS TORRES, MONTERREY, N.L., 64720, MEXICO
TEL: +52-81-8365-4171 FAX: +52-81-8365-4171
Brazil MITSUBISHI CNC Agent Service Center
(AUTOMOTION IND. COM. IMP. E EXP. LTDA.)
ACESSO JOSE SARTORELLI, KM 2.1 18550-000 BOITUVA – SP, BRAZIL
TEL: +55-15-3363-9900 FAX: +55-15-3363-9911
European FA Center (MITSUBISHI ELECTRIC EUROPE B.V.)
Germany CNC Service Center
GOTHAER STRASSE 8, 40880 RATINGEN, GERMANY
TEL: +49-2102-486-0
South Germany CNC Service Center
FAX:+49-2102486-591
KURZE STRASSE. 40, 70794 FILDERSTADT-BONLANDEN, GERMANY
TEL: +49-711-3270-010 FAX: +49-711-3270-0141
France CNC Service Center
25, BOULEVARD DES BOUVETS, 92741 NANTERRE CEDEX FRANCE
TEL: +33-1-41-02-83-13
Lyon CNC Service Satellite
FAX: +33-1-49-01-07-25
U.K CNC Service Center
TRAVELLERS LANE, HATFIELD, HERTFORDSHIRE, AL10 8XB, U.K.
TEL: +44-1707-282-846 FAX:-44-1707-278-992
Italy CNC Service Center
ZONA INDUSTRIALE VIA ARCHIMEDE 35 20041 AGRATE BRIANZA, MILANO ITALY
TEL: +39-039-60531-342
Spain CNC Service Satellite
FAX: +39-039-6053-206
CTRA. DE RUBI, 76-80 -APDO.420 08190 SAINT CUGAT DEL VALLES, BARCELONA SPAIN
TEL: +34-935-65-2236 FAX:
Turkey MITSUBISHI CNC Agent Service Center
(GENEL TEKNIK SISTEMLER LTD. STI.)
DARULACEZE CAD. FAMAS IS MERKEZI A BLOCK NO.43 KAT2 80270 OKMEYDANI ISTANBUL,
TURKEY
TEL: +90-212-320-1640 FAX: +90-212-320-1649
Poland MITSUBISHI CNC Agent Service Center (MPL Technology Sp. z. o. o)
UL SLICZNA 34, 31-444 KRAKOW, POLAND
TEL: +48-12-632-28-85 FAX:
Wroclaw MITSUBISHI CNC Agent Service Satellite (MPL Technology Sp. z. o. o)
UL KOBIERZYCKA 23, 52-315 WROCLAW, POLAND
TEL: +48-71-333-77-53 FAX: +48-71-333-77-53
Czech MITSUBISHI CNC Agent Service Center
(AUTOCONT CONTROL SYSTEM S.R.O. )
NEMOCNICNI 12, 702 00 OSTRAVA 2 CZECH REPUBLIC
TEL: +420-596-152-426 FAX: +420-596-152-112
ASEAN FA Center
HONG KONG FA Center
TAIWAN FA Center
ASEAN FA Center (MITSUBISHI ELECTRIC ASIA PTE. LTD.)
Singapore CNC Service Center
307 ALEXANDRA ROAD #05-01/02 MITSUBISHI ELECTRIC BUILDING SINGAPORE 159943
TEL: +65-6473-2308 FAX: +65-6476-7439
Thailand MITSUBISHI CNC Agent Service Center (F. A. TECH CO., LTD)
898/19,20,21,22 S.V. CITY BUILDING OFFICE TOWER 1 FLOOR 12,14 RAMA III RD BANGPONGPANG,
YANNAWA, BANGKOK 10120. THAILAND
TEL: +66-2-682-6522 FAX: +66-2-682-6020
Malaysia MITSUBISHI CNC Agent Service Center
(FLEXIBLE AUTOMATION SYSTEM SDN. BHD.)
60, JALAN USJ 10/1B 47620 UEP SUBANG JAYA SELANGOR DARUL EHSAN MALAYSIA
TEL: +60-3-5631-7605 FAX: +60-3-5631-7636
JOHOR MITSUBISHI CNC Agent Service Satellite
(FLEXIBLE AUTOMATION SYSTEM SDN. BHD.)
NO. 16, JALAN SHAHBANDAR 1, TAMAN UNGKU TUN AMINAH, 81300 SKUDAI, JOHOR MALAYSIA
TEL: +60-7-557-8218 FAX: +60-7-557-3404
Indonesia MITSUBISHI CNC Agent Service Center
(PT. AUTOTEKNINDO SUMBER MAKMUR)
WISMA NUSANTARA 14TH FLOOR JL. M.H. THAMRIN 59, JAKARTA 10350 INDONESIA
TEL: +62-21-3917-144 FAX: +62-21-3917-164
India MITSUBISHI CNC Agent Service Center (MESSUNG SALES & SERVICES PVT. LTD.)
B-36FF, PAVANA INDUSTRIAL PREMISES M.I.D.C., BHOASRI PUNE 411026, INDIA
TEL: +91-20-2711-9484 FAX: +91-20-2712-8115
BANGALORE MITSUBISHI CNC Agent Service Satellite
(MESSUNG SALES & SERVICES PVT. LTD.)
S 615, 6TH FLOOR, MANIPAL CENTER, BANGALORE 560001, INDIA
TEL: +91-80-509-2119 FAX: +91-80-532-0480
Delhi MITSUBISHI CNC Agent Parts Center (MESSUNG SALES & SERVICES PVT. LTD.)
1197, SECTOR 15 PART-2, OFF DELHI-JAIPUR HIGHWAY BEHIND 32ND MILESTONE GURGAON
122001, INDIA
TEL: +91-98-1024-8895 FAX:
Philippines MITSUBISHI CNC Agent Service Center
(FLEXIBLE AUTOMATION SYSTEM CORPORATION)
UNIT No.411, ALABAMG CORPORATE CENTER KM 25. WEST SERVICE ROAD SOUTH SUPERHIGHWAY,
ALABAMG MUNTINLUPA METRO MANILA, PHILIPPINES 1771
TEL: +63-2-807-2416 FAX: +63-2-807-2417
Vietnam MITSUBISHI CNC Agent Service Center (SA GIANG TECHNO CO., LTD)
47-49 HOANG SA ST. DAKAO WARD, DIST.1 HO CHI MINH CITY, VIETNAM
TEL: +84-8-910-4763 FAX: +84-8-910-2593
China FA Center (MITSUBISHI ELECTRIC AUTOMATION (SHANGHAI) LTD.)
China CNC Service Center
2/F., BLOCK 5 BLDG.AUTOMATION INSTRUMENTATION PLAZA, 103 CAOBAO RD. SHANGHAI 200233,
CHINA
TEL: +86-21-6120-0808 FAX: +86-21-6494-0178
Shenyang CNC Service Center
TEL: +86-24-2397-0184 FAX: +86-24-2397-0185
Beijing CNC Service Satellite
9/F, OFFICE TOWER1, HENDERSON CENTER, 18 JIANGUOMENNEI DAJIE, DONGCHENG DISTRICT,
BEIJING 100005, CHINA
TEL: +86-10-6518-8830 FAX: +86-10-6518-8030
China MITSUBISHI CNC Agent Service Center
(BEIJING JIAYOU HIGHTECH TECHNOLOGY DEVELOPMENT CO.)
RM 709, HIGH TECHNOLOGY BUILDING NO.229 NORTH SI HUAN ZHONG ROAD, HAIDIAN DISTRICT ,
BEIJING 100083, CHINA
TEL: +86-10-8288-3030 FAX: +86-10-6518-8030
Tianjin CNC Service Satellite
RM909, TAIHONG TOWER, NO220 SHIZILIN STREET, HEBEI DISTRICT, TIANJIN, CHINA 300143
TEL: -86-22-2653-9090 FAX: +86-22-2635-9050
Shenzhen CNC Service Satellite
RM02, UNIT A, 13/F, TIANAN NATIONAL TOWER, RENMING SOUTH ROAD, SHENZHEN, CHINA 518005
TEL: +86-755-2515-6691
Changchun Service Satellite
FAX: +86-755-8218-4776
TEL: +86-431-50214546
Hong Kong CNC Service Center
FAX: +86-431-5021690
UNIT A, 25/F RYODEN INDUSTRIAL CENTRE, 26-38 TA CHUEN PING STREET, KWAI CHUNG, NEW
TERRITORIES, HONG KONG
TEL: +852-2619-8588 FAX: +852-2784-1323
Taiwan FA Center (MITSUBISHI ELECTRIC TAIWAN CO., LTD.)
Taichung CNC Service Center
NO.8-1, GONG YEH 16TH RD., TAICHUNG INDUSTIAL PARK TAICHUNG CITY, TAIWAN R.O.C.
TEL: +886-4-2359-0688
Taipei CNC Service Satellite
FAX: +886-4-2359-0689
FAX: +886-4-2359-0689 TEL: +886-4-2359-0688
Tainan CNC Service Satellite
TEL: +886-4-2359-0688 FAX: +886-4-2359-0689
Korean FA Center (MITSUBISHI ELECTRIC AUTOMATION KOREA CO., LTD.)
Korea CNC Service Center
DONGSEO GAME CHANNEL BLDG. 2F. 660-11, DEUNGCHON-DONG KANGSEO-KU SEOUL, 157-030
KOREA
TEL: +82-2-3660-9607 FAX: +82-2-3663-0475
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.
© 2006 MITSUBISHI ELECTRIC CORPORATION
ALL RIGHTS RESERVED.
Advertisement
