Mitsubishi Electric CNC Meldas 60,60S Series Specifications Manual PDF

CNC

SPECIFICATIONS MANUAL

BNP-B2210F(ENG)

60/60S Series

MELDAS and MELSEC are registered trademarks of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective company.

Introduction

This manual describes the specifications of MELDAS 60/60S 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 : Option

: Selection : Special option

CAUTION The items that are not described in this manual must be interpreted as "not possible".

This manual is written on the assumption that all option functions are added. Some functions may differ or some functions may not be usable depending on the NC system (software) version.

General precautions

(1) When the contents of this manual is updated, the version (*, A, B, ) on the cover will be incremented.

Precautions for Safety

Always read the specifications issued by the machine maker, this manual, related manuals and attached documents before installation, operation, programming, maintenance or inspection to ensure correct use. Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".

DANGER

When there is a great risk that the user could be subject to fatalities or serious injuries if handling is mistaken.

WARNING

When the user could be subject to fatalities or serious injuries if handling is mistaken.

CAUTION

When the user could be subject to injuries or when physical damage could occur if handling is mistaken.

Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important information that must always be observed is described.

DANGER Not applicable in this manual.

WARNING Not applicable in this manual.

CAUTION

1. Items related to product and manual

The items that are not described in this manual must be interpreted as "not possible". This manual is written on the assumption that all option functions are added. Some functions may differ or some functions may not be usable depending on the NC

system (software) version.

2. Items related to start up and maintenance Follow the power specifications (input voltage range, frequency range, momentary

power failure time range) described in this manual. Follow the environment conditions (ambient temperature, humidity, vibration,

atmosphere) described in this manual.

! Follow the remote type machine contact input/output interface described in this manual. (Connect a diode in parallel with the inductive load or connect a protective resistor in serial with the capacitive load, etc.)

If the parameter is used to set the temperature rise detection function to invalid, overheating may occur, thereby disabling control and possibly resulting in the axes running out of control, which in turn may result in machine damage and/or bodily injury or destruction of the unit. It is for this reason that the detection function is normally left "valid" for operation.

i

CONTENTS 1 Control Axes ...................................................................................................................................... 1

1.1 Control Axes ................................................................................................................. 1 1.1.1 Number of Basic Control Axes (NC axes)............................................................ 1 1.1.2 Max. Number of Control Axes

(NC axes + Spindles + PLC axes + Auxiliary axes)............................................. 1 1.1.3 Number of Simultaneous Contouring Control Axes ............................................. 3 1.1.4 Max. Number of NC Axes in a Part System (Part System 1/Part System 2) ...... 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 Mode ....................................................................................................... 4 1.3.3 MDI Mode.............................................................................................................. 4 1.3.4 High-Speed Program Server Mode...................................................................... 4 1.3.5 IC Card Mode........................................................................................................ 4

1.3.5.1 IC Card in Control Unit............................................................................... 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 2.3.2.7 Special Format for MELDAS ..................................................................... 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 3.2.4 Spiral / Conical Interpolation................................................................................. 24 3.2.5 Cylindrical Interpolation......................................................................................... 26 3.2.6 Polar coordinate interpolation............................................................................... 27 3.2.7 Milling Interpolation ............................................................................................... 28

3.3 Curve Interpolation ....................................................................................................... 29 3.3.2 Exponential Interpolation ...................................................................................... 29 3.3.3 Spline Interpolation ............................................................................................... 30

ii

4 Feed...................................................................................................................................... 31

4.1 Feed Rate ..................................................................................................................... 31 4.1.1 Rapid Traverse Rate (m/min) ............................................................................... 31 4.1.2 Cutting Feed Rate (m/min) ................................................................................... 32 4.1.3 Manual Feed Rate (m/min)................................................................................... 33

4.2 Feed Rate Input Methods ............................................................................................. 34 4.2.1 Feed per Minute.................................................................................................... 34 4.2.2 Feed per Revolution.............................................................................................. 36 4.2.4 F 1-digit Feed........................................................................................................ 37

4.3 Override ........................................................................................................................ 38 4.3.1 Rapid Traverse Override ...................................................................................... 38 4.3.2 Cutting Feed Override .......................................................................................... 38 4.3.3 2nd Cutting Feed Override ................................................................................... 39 4.3.4 Override Cancel .................................................................................................... 39

4.4 Acceleration / Deceleration........................................................................................... 40 4.4.1 Automatic Acceleration / Deceleration after Interpolation .................................... 40 4.4.2 Rapid Traverse Constant Inclination Acceleration / Deceleration ....................... 41 4.4.3 Rapid Traverse Constant Inclination 3-step Acceleration / Deceleration ............ 44

4.5 Thread Cutting .............................................................................................................. 45 4.5.1 Thread Cutting (Lead/Thread Number Designation)............................................ 45 4.5.2 Variable Lead Thread Cutting............................................................................... 47 4.5.3 Synchronous Tapping........................................................................................... 48

4.5.3.1 Synchronous Tapping Cycle...................................................................... 48 4.5.3.2 Pecking Tapping Cycle.............................................................................. 50 4.5.3.3 Deep-hole Tapping Cycle .......................................................................... 51

4.5.4 Chamfering............................................................................................................ 52 4.5.6 Circular Thread Cutting......................................................................................... 53

4.6 Manual Feed................................................................................................................. 54 4.6.1 Manual Rapid Traverse ........................................................................................ 54 4.6.2 Jog Feed ............................................................................................................... 54 4.6.3 Incremental Feed.................................................................................................. 55 4.6.4 Handle Feed.......................................................................................................... 55 4.6.5 Manual Feed Rate B............................................................................................. 56

4.7 Dwell ............................................................................................................................. 57 4.7.1 Dwell (Time-based Designation) .......................................................................... 57

5 Program Memory / Editing................................................................................................. 58

5.1 Memory Capacity.......................................................................................................... 58 5.1.1 Memory Capacity (Number of Programs Stored)................................................. 58

5.2 Editing Method.............................................................................................................. 59 5.2.1 Program Editing .................................................................................................... 59 5.2.2 Background Editing............................................................................................... 60 5.2.3 Buffer Correction................................................................................................... 61 5.2.4 Word Editing.......................................................................................................... 62

6 Operation and Display ....................................................................................................... 63

6.1 Structure of Operation / Display Panel ......................................................................... 63 6.2 Operation Methods and Functions ............................................................................... 63

6.2.1 Memory Switch (PLC Switch) ............................................................................... 63 6.3 Display Methods and Contents .................................................................................... 64

6.3.1 Status Display ....................................................................................................... 64 6.3.2 Position Display .................................................................................................... 64 6.3.3 Program Running State Display ........................................................................... 66 6.3.4 Parameter Setting and Display............................................................................. 66 6.3.5 MDI Data Setting and Display .............................................................................. 66 6.3.6 Specification List Display ...................................................................................... 66

iii

6.3.7 Clock ..................................................................................................................... 66 6.3.8 Hardware / Software Configuration Display ......................................................... 67 6.3.9 Integrated Time Display........................................................................................ 67 6.3.10 Available Languages .......................................................................................... 67 6.3.11 Additional Languages ......................................................................................... 68

6.3.11.1 Japanese ................................................................................................. 68 6.3.11.2 English ..................................................................................................... 68 6.3.11.3 German .................................................................................................... 68 6.3.11.4 Italian........................................................................................................ 68 6.3.11.5 French...................................................................................................... 68 6.3.11.6 Spanish .................................................................................................... 68 6.3.11.7 Chinese.................................................................................................... 69 6.3.11.8 Korean...................................................................................................... 69 6.3.11.9 Portuguese............................................................................................... 69 6.3.11.10 Hungarian .............................................................................................. 69 6.3.11.11 Dutch...................................................................................................... 69 6.3.11.12 Swedish ................................................................................................. 69

6.3.12 Screen Saver, Backlight OFF............................................................................. 70 6.3.13 Screen Deletion .................................................................................................. 70

7 Input / Output Functions and Devices ............................................................................. 71

7.1 Input / Output Data ....................................................................................................... 71 7.2 Input / Output I/F ........................................................................................................... 72

7.2.1 RS-232C I/F .......................................................................................................... 72 7.2.2 IC Card I/F............................................................................................................. 72

7.2.2.1 I/F for IC Card in Control Unit .................................................................... 72 7.2.3 Data Server I/F...................................................................................................... 72 7.2.4 Ethernet I/F ........................................................................................................... 72

7.3 Computer Link............................................................................................................... 73 7.3.1 Computer Link B ................................................................................................... 73

8 Spindle, Tool and Miscellaneous Functions ................................................................... 74

8.1 Spindle Functions (S) ................................................................................................... 74 8.1.1 Command / Output ............................................................................................... 74

8.1.1.1 Spindle Functions ...................................................................................... 74 8.1.1.2 Spindle Serial I/F........................................................................................ 75 8.1.1.3 Spindle Analog I/F...................................................................................... 75 8.1.1.4 Coil Change ............................................................................................... 75 8.1.1.5 Automatic Coil Change.............................................................................. 75

8.1.2 Speed Control ....................................................................................................... 76 8.1.2.1 Constant Surface Speed Control............................................................... 76 8.1.2.2 Spindle Override ........................................................................................ 77 8.1.2.3 Multiple-spindle Control ............................................................................. 77

8.1.2.3.1 Multiple-spindle Control I .......................................................... 78 8.1.2.3.2 Multiple-spindle Control II............................................................. 78

8.1.3 Position Control..................................................................................................... 79 8.1.3.1 Spindle Orientation .................................................................................... 79 8.1.3.2 Spindle Position Control (Spindle / C Axis Control) .................................. 79 8.1.3.3 Spindle Synchronization ............................................................................ 80

8.1.3.3.1 Spindle Synchronization I............................................................. 80 8.1.3.3.2 Spindle Synchronization II............................................................ 81

8.1.3.4 Tool Spindle Synchronization I (Polygon) ................................................. 81 8.1.3.4.1 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)...... 81 8.1.3.4.2 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon)...... 82 8.1.3.4.3 Tool Spindle Synchronization IC (Spindle-NC axis, Polygon)..... 83

iv

8.2 Tool Functions (T)......................................................................................................... 84

8.2.1 Tool Functions....................................................................................................... 84 8.3 Miscellaneous Functions (M)........................................................................................ 85

8.3.1 Miscellaneous Functions ...................................................................................... 85 8.3.2 Multiple M Codes in 1 Block ................................................................................. 85 8.3.3 M Code Independent Output ................................................................................ 86 8.3.4 Miscellaneous Function Finish ............................................................................. 86 8.3.5 M Code Output during Axis Positioning................................................................ 87

8.4 2nd Miscellaneous Functions (B) ................................................................................. 88 8.4.1 2nd Miscellaneous Functions ............................................................................... 88

9 Tool Compensation ............................................................................................................ 89

9.1 Tool Length / Position Offset ........................................................................................ 89 9.1.1 Tool Length Offset ................................................................................................ 89 9.1.2 Tool Position Offset............................................................................................... 92 9.1.3 Tool Offset for Additional Axes ............................................................................. 92

9.2 Tool Radius................................................................................................................... 93 9.2.1 Tool radius Compensation.................................................................................... 93 9.2.2 3-dimensional Tool Radius Compensation .......................................................... 96 9.2.3 Tool Nose Radius Compensation (G40/41/42) .................................................... 97 9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40) ............. 98

9.3 Tool Offset Amount....................................................................................................... 99 9.3.1 Number of Tool Offset Sets .................................................................................. 99

9.3.1.1 20 .............................................................................................................. 99 9.3.1.2 40 .............................................................................................................. 99 9.3.1.3 80 .............................................................................................................. 99 9.3.1.5 200 ............................................................................................................ 99 9.3.1.6 400 ............................................................................................................ 99 9.3.1.7 999 ............................................................................................................ 99

9.3.2 Offset Memory ...................................................................................................... 100 9.3.2.1 Tool Shape/Wear Offset Amount .............................................................. 100

10 Coordinate System...................................................................................................... 103

10.1 Coordinate System Type and Setting ........................................................................ 103 10.1.1 Machine Coordinate System .............................................................................. 104 10.1.2 Coordinate System Setting................................................................................. 105 10.1.3 Automatic Coordinate System Setting................................................................ 106 10.1.4 Workpiece Coordinate System Selection (6 sets).............................................. 107 10.1.5 Extended Workpiece Coordinates System Selection ........................................ 108 10.1.6 Workpiece Coordinate System Preset (G92.1).................................................. 109 10.1.7 Local Coordinate System ................................................................................... 110 10.1.8 Coordinate System for Rotary Axis .................................................................... 111 10.1.9 Plane Selection ................................................................................................... 111 10.1.10 Origin Set .......................................................................................................... 112 10.1.11 Counter Set....................................................................................................... 112

10.2 Return ......................................................................................................................... 113 10.2.1 Manual Reference Position Return .................................................................... 113 10.2.2 Automatic 1st Reference Position Return .......................................................... 114 10.2.3 2nd, 3rd, 4th Reference Position Return............................................................ 116 10.2.4 Reference Position Verification .......................................................................... 117 10.2.5 Absolute position detection................................................................................. 118 10.2.6 Tool Exchange Position Return.......................................................................... 119 10.2.7 C Axis Reference Position Return...................................................................... 120

v

11 Operation Support Functions .................................................................................... 122

11.1 Program Control ......................................................................................................... 122 11.1.1 Optional Block Skip............................................................................................. 122 11.1.3 Single Block ........................................................................................................ 123

11.2 Program Test .............................................................................................................. 124 11.2.1 Dry Run ............................................................................................................... 124 11.2.2 Machine Lock...................................................................................................... 124 11.2.3 Miscellaneous Function Lock ............................................................................. 125 11.2.4 Graphic Check .................................................................................................... 125 11.2.5 Graphic Trace ..................................................................................................... 125

11.3 Program Search / Start / Stop .................................................................................... 126 11.3.1 Program Search.................................................................................................. 126 11.3.2 Sequence Number Search ................................................................................. 126 11.3.3 Collation Stop...................................................................................................... 127 11.3.4 Program Restart.................................................................................................. 128 11.3.5 Automatic Operation Start .................................................................................. 129 11.3.6 NC Reset............................................................................................................. 129 11.3.7 Feed Hold............................................................................................................ 130 11.3.8 Search & Start..................................................................................................... 130

11.4 Interrupt Operation...................................................................................................... 131 11.4.1 Manual Interruption............................................................................................. 131 11.4.2 Automatic Operation Handle Interruption........................................................... 132 11.4.3 Manual Absolute Mode ON / OFF...................................................................... 133 11.4.4 Thread Cutting Cycle Retract ............................................................................. 134 11.4.5 Tapping Retract .................................................................................................. 135 11.4.6 Manual Numerical value Command ................................................................... 136 11.4.8 MDI Interruption .................................................................................................. 136 11.4.9 Simultaneous Operation of Manual and Automatic Modes ............................... 137 11.4.10 Simultaneous Operation of Jog and Handle Modes ........................................ 137 11.4.11 Reference Position Retract............................................................................... 138 11.4.13 Tool Escape and Return................................................................................... 138 11.4.14 Skip Retract....................................................................................................... 138

12 Program Support Functions...................................................................................... 139

12.1 Machining Method Support Functions........................................................................ 139 12.1.1 Program .............................................................................................................. 139

12.1.1.1 Subprogram Control ................................................................................ 139 12.1.1.3 Scaling ..................................................................................................... 141

12.1.2 Macro Program ................................................................................................... 142 12.1.2.1 User Macro .............................................................................................. 142 12.1.2.2 Machine Tool Builder Macro.................................................................... 144

12.1.2.2.1 Machine Tool Builder Macro SRAM........................................... 144 12.1.2.3 Macro Interruption.................................................................................... 145 12.1.2.4 Variable Command.................................................................................. 146

12.1.2.4.1 100 sets ...................................................................................... 146 12.1.2.4.2 200 sets ...................................................................................... 146 12.1.2.4.3 300 sets ...................................................................................... 147 12.1.2.4.4 600 sets ...................................................................................... 147 12.1.2.4.5 700 sets ...................................................................................... 147 12.1.2.4.6 (50+50 x number of part systems) sets ..................................... 147 12.1.2.4.7 (100+100 x number of part systems) sets ................................. 147 12.1.2.4.8 (200+100 x number of part systems) sets ................................. 147 12.1.2.4.9 (400+100 x number of part systems) sets ................................. 147 12.1.2.4.10 (500+100 x number of part systems) sets ............................... 147

vi

12.1.3 Fixed Cycle ......................................................................................................... 148

12.1.3.1 Fixed Cycle for Drilling............................................................................. 149 12.1.3.2 Special Fixed Cycle ................................................................................. 155 12.1.3.3 Fixed Cycle for Turning Machining.......................................................... 159 12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining........................... 164 12.1.3.5 Multiple Repetitive Fixed Cycle for Turning Machining (Type II) ............ 172 12.1.3.6 Small-diameter Deep-Hole Drilling Cycle................................................ 173 12.1.3.7 Fixed Cycle for Drilling (Type II) .............................................................. 174

12.1.4 Mirror Image........................................................................................................ 175 12.1.4.1 Mirror Image by Parameter Setting ......................................................... 175 12.1.4.2 External Input Mirror Image ..................................................................... 175 12.1.4.3 G Code Mirror Image............................................................................... 176 12.1.4.4 Mirror Image for Facing Tool Posts ......................................................... 177 12.1.4.5 T Code Mirror Image for Facing Tool Posts............................................ 177

12.1.5 Coordinate System Operation ............................................................................ 178 12.1.5.1 Coordinate Rotation by Program............................................................. 178

12.1.6 Dimension Input .................................................................................................. 180 12.1.6.1 Corner Chamfering / Corner R ................................................................ 180 12.1.6.2 Linear Angle Command .......................................................................... 186 12.1.6.3 Geometric Command .............................................................................. 187 12.1.6.4 Polar Coordinate Command.................................................................... 191

12.1.7 Axis Control......................................................................................................... 192 12.1.7.1 High-speed Machining............................................................................. 192

12.1.7.1.3 High-speed Machining Mode III ................................................. 192 12.1.7.1.4 High-speed High-accuracy Control 1......................................... 193 12.1.7.1.5 High-speed High-accuracy Control 2......................................... 194 12.1.7.1.7 SSS Control................................................................................ 196

12.1.7.2 Chopping.................................................................................................. 197 12.1.7.2.1 Chopping .................................................................................... 197

12.1.7.4 Normal Line Control................................................................................. 199 12.1.7.5 Circular Cutting ........................................................................................ 200

12.1.8 Multi-part System Control ................................................................................... 201 12.1.8.1 Synchronization between Part Systems.................................................. 201 12.1.8.2 Start Point Designation Synchronization................................................. 202 12.1.8.3 Cross Machining Command ................................................................... 204 12.1.8.5 Control Axis Synchronization................................................................... 205 12.1.8.6 Balance Cut ............................................................................................. 206 12.1.8.7 Common Memory between Tool Posts................................................... 207 12.1.8.9 2-part System Program Management ..................................................... 207

12.1.9 Data Input by Program........................................................................................ 208 12.1.9.1 Parameter Input by Program ................................................................... 208 12.1.9.2 Compensation Data Input by Program.................................................... 209

12.1.10 Machining Modal............................................................................................... 211 12.1.10.1 Tapping Mode........................................................................................ 211 12.1.10.2 Cutting Mode.......................................................................................... 211

12.2 Machining Accuracy Support Functions..................................................................... 212 12.2.1 Automatic Corner Override................................................................................. 212 12.2.2 Deceleration Check ............................................................................................ 213

12.2.2.1 Exact Stop Mode ..................................................................................... 214 12.2.2.2 Exact Stop Check .................................................................................... 214 12.2.2.3 Error Detect.............................................................................................. 214 12.2.2.4 Programmable Inposition Check ............................................................. 215

12.2.3 High-Accuracy Control (G61.1) .......................................................................... 216 12.3 Programming Support Functions ............................................................................... 219

12.3.1 Playback.............................................................................................................. 219 12.3.2 Address Check.................................................................................................... 219

vii

13 Machine Accuracy Compensation............................................................................. 220

13.1 Static Accuracy Compensation .................................................................................. 220 13.1.1 Backlash Compensation..................................................................................... 220 13.1.2 Memory-type Pitch Error Compensation ............................................................ 221 13.1.3 Memory-type Relative Position Error Compensation......................................... 222 13.1.4 External Machine Coordinate System Compensation ....................................... 223 13.1.5 Circular Radius Error Compensation.................................................................. 223

13.2 Dynamic Accuracy Compensation ............................................................................. 224 13.2.1 Smooth High-gain Control (SHG Control) .......................................................... 224 13.2.2 Dual Feedback.................................................................................................... 225 13.2.3 Lost Motion Compensation................................................................................. 225

14 Automation Support Functions ...................................................................................... 226

14.1 External Data Input ..................................................................................................... 226 14.1.1 External Search .................................................................................................. 226 14.1.2 External Workpiece Coordinate Offset ............................................................... 227 14.1.3 External Tool Offset ............................................................................................ 228

14.2 Measurement.............................................................................................................. 229 14.2.1 Skip ..................................................................................................................... 229

14.2.1.1 Skip .......................................................................................................... 229 14.2.1.2 Multiple-step Skip .................................................................................... 230 14.2.1.4 PLC Skip .................................................................................................. 231 14.2.1.5 Speed Change Skip................................................................................. 232

14.2.5 Automatic Tool Length Measurement ................................................................ 233 14.2.6 Manual Tool Length Measurement 1.................................................................. 236 14.2.7 Manual Tool Length Measurement 2.................................................................. 237 14.2.8 Workpiece Coordinate Offset Measurement...................................................... 238 14.2.9 Workpiece Position Measurement...................................................................... 239

14.3 Monitoring ................................................................................................................... 241 14.3.1 Tool Life Management ........................................................................................ 241 14.3.2 Number of Tool Life Management Sets ............................................................. 242 14.3.3 Display of Integrated Time/Number of Parts ...................................................... 242 14.3.4 Load Meter .......................................................................................................... 242 14.3.5 Position Switch.................................................................................................... 243

14.5 Others ......................................................................................................................... 244 14.5.1 Programmable Current Limitation ...................................................................... 244

15 Safety and Maintenance .................................................................................................. 245

15.1 Safety Switches .......................................................................................................... 245 15.1.1 Emergency Stop ................................................................................................. 245 15.1.2 Data Protection Key............................................................................................ 245

15.2 Display for Ensuring Safety ........................................................................................ 246 15.2.1 NC Warning ........................................................................................................ 246 15.2.2 NC Alarm............................................................................................................. 246 15.2.3 Operation Stop Cause ........................................................................................ 247 15.2.4 Emergency Stop Cause...................................................................................... 247 15.2.5 Temperature Detection ....................................................................................... 248

15.3 Protection.................................................................................................................... 249 15.3.1 Stroke End (Over Travel).................................................................................... 249 15.3.2 Stored Stroke Limit ............................................................................................. 249

15.3.2.1 Stored Stroke Limit I/II ............................................................................ 250 15.3.2.2 Stored Stroke Limit IB............................................................................. 252 15.3.2.3 Stored Stroke Limit IIB............................................................................ 253 15.3.2.4 Stored Stroke Limit IC............................................................................. 253

15.3.4 Chuck/Tail Stock Barrier Check.......................................................................... 254 15.3.5 Interlock............................................................................................................... 255 15.3.6 External Deceleration ......................................................................................... 255

viii

15.3.8 Door Interlock..................................................................................................... 256

15.3.8.1 Door Interlock I........................................................................................ 256 15.3.8.2 Door Interlock II....................................................................................... 257

15.3.9 Parameter Lock.................................................................................................. 258 15.3.10 Program Protect (Edit Lock B, C) ..................................................................... 258 15.3.11 Program Display Lock....................................................................................... 259

15.4 Maintenance and Troubleshooting............................................................................. 260 15.4.1 History Diagnosis ................................................................................................ 260 15.4.2 Setup / Monitor for Servo and Spindle ............................................................... 260 15.4.3 Data Sampling .................................................................................................... 260 15.4.4 Waveform Display............................................................................................... 261 15.4.5 Machine Operation History Monitor.................................................................... 261 15.4.6 NC Data Backup ................................................................................................. 262 15.4.7 PLC I/F Diagnosis ............................................................................................... 263 15.4.8 MELDASNET...................................................................................................... 264

15.4.8.1 Machine Builder Network System .......................................................... 264 15.4.8.2 Anshin-net............................................................................................... 264

16 Cabinet and Installation................................................................................................... 265

16.1 Cabinet Construction .................................................................................................. 265 16.2 Power Supply, Environment and Installation Conditions ........................................... 269

17 Servo/Spindle System...................................................................................................... 272

17.1 Feed Axis .................................................................................................................... 272 17.1.1 MDS-C1-V1/C1-V2 (200V) ................................................................................. 272 17.1.2 MDS-B-V14L (200V)........................................................................................... 272 17.1.3 MDS-CH-V1/CH-V2 (400V)................................................................................ 272 17.1.4 MDS-B-SVJ2 (Compact and Small Capacity).................................................... 273

17.2 Spindle ........................................................................................................................ 274 17.2.1 MDS-C1-SP/C1-SPM/B-SP (200V).................................................................... 274 17.2.2 MDS-CH-SP/CH-SPH (400V) ............................................................................ 274 17.2.3 MDS-B-SPJ2 (Compact and Small Capacity).................................................... 274

17.3 Auxiliary Axis............................................................................................................... 274 17.3.1 Index/Positioning Servo: MR-J2-CT................................................................... 274

17.4 Power Supply.............................................................................................................. 275 17.4.1 Power Supply: MDS-C1-CV/B-CVE ................................................................... 275 17.4.2 AC Reactor for Power Supply............................................................................. 275 17.4.3 Ground plate ....................................................................................................... 275 17.4.4 Power Supply: MDS-A-CR (Resistance Regeneration)..................................... 275

18 Machine Support Functions............................................................................................ 276

18.1 PLC ............................................................................................................................. 276 18.1.1 PLC Basic Function ............................................................................................ 276

18.1.1.1 Built-in PLC Basic Function ..................................................................... 276 18.1.2 Built-in PLC Processing Mode............................................................................ 281

18.1.2.1 PLC4B I/F .............................................................................................. 281 18.1.2.2 MELSEC Development Tool I/F .............................................................. 281

18.1.3 Built-in PLC Capacity (Number of Steps)........................................................... 282 18.1.4 Machine Contact Input/Output I/F....................................................................... 282 18.1.5 Ladder Monitor.................................................................................................... 287 18.1.6 PLC Development............................................................................................... 287

18.1.6.1 On-board Development ........................................................................... 287 18.1.6.2 MELSEC Development Tool ................................................................... 287 18.1.6.3 PLC4B...................................................................................................... 287

18.1.7 C Language Function ......................................................................................... 287 18.1.8 PLC Protect......................................................................................................... 288 18.1.9 PLC Password Lock ........................................................................................... 289

ix

18.1.12 GOT Connection............................................................................................... 290

18.1.12.2 CC-Link Connection (Remote Device) .................................................. 290 18.1.13 PLC Message ................................................................................................... 291

18.1.13.1 Japanese ............................................................................................... 291 18.1.13.2 English ................................................................................................... 291 18.1.13.3 German .................................................................................................. 291 18.1.13.4 Italian...................................................................................................... 291 18.1.13.5 French.................................................................................................... 291 18.1.13.6 Spanish .................................................................................................. 291 18.1.13.9 Portuguese............................................................................................. 291 18.1.13.10 Hungarian ............................................................................................ 292 18.1.13.11 Dutch.................................................................................................... 292 18.1.13.12 Swedish ............................................................................................... 292

18.2 Machine Construction................................................................................................. 293 18.2.1 Servo OFF........................................................................................................... 293 18.2.2 Axis Detach......................................................................................................... 294 18.2.3 Synchronous Control .......................................................................................... 295

18.2.3.1 Position Tandem...................................................................................... 295 18.2.4 Inclined Axis Control ........................................................................................... 297 18.2.5 Index Table Indexing .......................................................................................... 298 18.2.6 NSK Table Connection Control .......................................................................... 299 18.2.7 Auxiliary Axis Control .......................................................................................... 300

18.3 PLC Operation ............................................................................................................ 301 18.3.1 Arbitrary Feed in Manual Mode .......................................................................... 301 18.3.3 PLC Axis Control................................................................................................. 302

18.4 PLC Interface.............................................................................................................. 303 18.4.1 CNC Control Signal ............................................................................................ 303 18.4.2 CNC Status Signal .............................................................................................. 304 18.4.5 DDB..................................................................................................................... 306

18.5 Machine Contact I / O................................................................................................. 307 18.6 External PLC Link ....................................................................................................... 308

18.6.1 External PLC link I (M-NET) ............................................................................... 308 18.6.2 External PLC Link II (Bus Connection)............................................................... 310

18.6.2.1 MELSEC-A, QnA Series.......................................................................... 310 18.6.3 IO Link................................................................................................................. 311 18.6.4 CC-Link ............................................................................................................... 312

18.7 Installing S/W for Machine Tools................................................................................ 316 18.7.1 APLC................................................................................................................... 316

Appendix 1 List of Specifications........................................................................................ 317 Appendix 2 Outline and installation dimension drawings of units ................................. 318

Appendix 2.1 Outline drawing of control unit...................................................................... 318 Appendix 2.1 Outline Drawing of Control Unit.................................................................... 318

Appendix 2.1.1 M64A/M64 Control Unit Outline Drawing............................................ 318 Appendix 2.1.2 M64AS/64S/65/65S/66/66S Control Unit Outline Drawing................. 319

Appendix 2.2 Communication Terminal Outline Drawing ................................................. 320 Appendix 2.2.1 FCUA-CT100/CT120........................................................................... 320 Appendix 2.2.2 FCUA-CR10......................................................................................... 321 Appendix 2.2.3 FCUA-LD100 ....................................................................................... 322 Appendix 2.2.4 FCUA-LD10 ......................................................................................... 323 Appendix 2.2.5 FCU6-DUT32....................................................................................... 324 Appendix 2.2.6 FCU6-DUT33....................................................................................... 325 Appendix 2.2.7 FCUA-KB20/KB30............................................................................... 326 Appendix 2.2.8 FCU6-KB021/KB031 ........................................................................... 327 Appendix 2.2.9 FCUA-KB10/KB12............................................................................... 328 Appendix 2.2.10 Key Arrangement .............................................................................. 329

Appendix 2.3 Base I/O Unit Outline Drawing .................................................................... 330 Appendix 2.4 Remote I/O Unit Outline Drawing................................................................ 331

1 Control Axes 1.1 Control Axes

- 1 -

1 Control Axes The NC axis, spindle, PLC axis are generically called the control axis. The NC axis is an axis that can be manually operated, or automatically operated with the machining program. The PLC axis is an axis that can be controlled from the PLC ladder.

1.1 Control Axes

1.1.1 Number of Basic Control Axes (NC axes) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 3 3 3 3 3 3 3 3 L system 2 2 2 2 2 2 2 2

1.1.2 Max. Number of Control Axes (NC axes + Spindles + PLC axes + Auxiliary axes) Max. number of control axes (NC axes + spindles + PLC axes + auxiliary axes)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 9 11 11 11 9 11 11 11 L system 9 11 11 11 9 11 14 14

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 7 axes can be connected with each channel.

NC axis, PLC axis, spindle : They can be connected with the channel 1 and channel 2. The connection number of first axis to seventh axis 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 (J2-CT) : They can be connected with the channel 2. The connection order is the NC axis, PLC axis, spindle and auxiliary axis.

1 Control Axes 1.1 Control Axes

- 2 -

Max. number of axes (NC axes + spindles + PLC axes)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 5 7 7 7 5 7 7 7 L system 5 7 7 7 5 7 14 14

Max number of servo axes (NC axes + PLC axes)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 5 6 6 6 5 7 7 7 L system 5 6 6 6 5 7 14 14

Max. number of NC axes (in total for all the part systems)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 4 6 6 6 4 6 6 6 L system 4 6 6 6 4 7 12 12

Max. number of spindles

Includes analog spindles.

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 1 2 2 2 1 2 4 4 L system 1 2 2 2 1 2 4 4

Max. number of PLC axes

M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 2 2 2 2 2 2 2 2 L system 2 2 2 2 2 2 2 2

Max. number of auxiliary axes

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 4 4 4 4 4 4 4 4 L system 4 4 4 4 4 4 4 4

1 Control Axes 1.1 Control Axes

- 3 -

1.1.3 Number of Simultaneous Contouring Control Axes Simultaneous control of all axes is possible as a principle in the same part system. However, for actual use, the machine maker specification will apply.

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 4 4 4 6 4 4 4 6 L system 4 4 4 6 4 4 4 6

1.1.4 Max. Number of NC Axes in a Part System M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 4 6 6 6 4 6 6 6 L system 4 6 6 6 4 6 6 6

1.2 Control Part System

1.2.1 Standard Number of Part Systems M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 1 1 1 1 1 1 1 1 L system 1 1 1 1 1 1 1 1

1.2.2 Max. Number of Part Systems M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 1 2 2 2 1 1 1 1 L system 1 2 2 2 1 2 2 2

For actual use, the machine maker specification will apply.

1 Control Axes 1.3 Control Axes and Operation Modes

- 4 -

1.3 Control Axes and Operation Modes

1.3.1 Tape (RS-232C Input) Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The machining programs stored in the memory of the NC unit are run.

1.3.3 MDI Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The MDI data stored in the memory of the NC unit is executed. Once executed, the MDI data is set to the "setting incomplete" status, and the data will not be executed unless the "setting completed" status is established by performing screen operations.

1.3.4 High-Speed Program Server Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

In this mode, the NC unit is hooked up to a host computer using an Ethernet connection, and the programs are transferred to either the NC unit's memory or the IC card inside the NC unit. This function is executed with the transferred programs and memory operation (IC card operation) mode.

1.3.5 IC Card Mode

1.3.5.1 IC Card in Control Unit M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The machine programs stored in the IC card of the NC unit are run.

2 Input Command 2.1 Data Increment

- 5 -

2 Input Command 2.1 Data Increment

Least command increment: 1 m

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Least command increment: 0.1 m

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Least command increment: 0.01 m (10nm)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

(Note 1) The drive unit must be compatible to use the least command increment 0.01m (10nm). The relation of the control unit setting and usable drive unit compliance is shown below.

Last command increment MDS-B series MDS-C1 series 1 m/0.1 m 0.01 m (10nm)

(May be incompatible depending on servo drive unit version)

The data increment handled in the controller include the least input increment, least command increment and least detection increment. Each type is set with parameters. (1) The least input increment indicates the increment handled in the internal processing of the

controller. The counter and tool offset data, etc., input from the screen is handled with this increment. This increment is applied per part system (1st part system, 2nd part system).

(2) The least command increment indicates the command increment of the movement command in the machining program. This can be set per axis.

Metric unit system Inch unit system

Increment type Type Linear axis (Unit = mm)

Rotary axis (Unit = )

Linear axis (Unit = inch)

Rotary axis (Unit = )

B 0.001 0.001 0.0001 0.001 C 0.0001 0.0001 0.00001 0.0001 Least command increment D 0.00001 0.00001

(Note) The inch and metric systems cannot be used together.

(3) The least detection increment indicates the detection increment of the NC axis and PLC axis detectors. The increment is determined by the detector being used.

(4) If the least command increment is 0.1m/0.01m, the movement amount, movement range and command speed may be limited compared to the 1m.

2 Input Command 2.2 Unit System

- 6 -

2.2 Unit System

2.2.1 Inch/Metric Changeover M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 1.0 1.0 mm Inch unit system 1.0 1.0 inch

(Note) For the angle data, 1.0 means 1 degree () regardless of the unit system.

Data Parameter

Machining program Screen data

(Offset amount, etc.) Parameter

G20 Inch unit system 0 G21 Metric unit system Metric unit system

G20 Inch unit system I_inch 1 G21 Metric unit system Inch unit system

Not affected

0 Metric unit system M_inch 1 Not affected Not affected Inch unit system (Note 1) The parameter changeover is valid after the power is turned ON again. (Note 2) Even if parameter "I_inch" is changed, the screen data (offset amount, etc.) will not be

automatically converted. (Note 3) When the power is turned ON or resetting is performed, the status of the G20/G21 modal

depends on the "I_G20" parameter setting.

2 Input Command 2.3 Program Format

- 7 -

2.3 Program Format

2.3.1 Character Code M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Always significant . Always significant , Always significant / Always significant % Always significant CR Always significant LF/NL Always significant ( Always significant ) Always significant : Always significant # Always significant Always significant = Always significant [ Always significant ] Always significant SP Always significant ! Always significant $ Always significant BS An error results during operation (except when the character is part of a comment). HT An error results during operation (except when the character is part of a comment). & An error results during operation (except when the character is part of a comment). '(Apostrophe) An error results during operation (except when the character is part of a comment). ; An error results during operation (except when the character is part of a comment). < An error results during operation (except when the character is part of a comment). > An error results during operation (except when the character is part of a comment). ? An error results during operation (except when the character is part of a comment). @ An error results during operation (except when the character is part of a comment). " An error results during operation (except when the character is part of a comment). DEL Always ignored NULL Always ignored

2 Input Command 2.3 Program Format

- 8 -

2.3.2 Program Format

2.3.2.1 Format 1 for Lathe M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

2.3.2.4 Format 1 for Machining Center M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

2.3.2.7 Special Format for MELDAS M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The formats of the turning fixed cycles (G77 to G79), multiple repetitive turning fixed cycles (G71 to G76) and drilling fixed cycles (G80 to G89) can be switched to the MELDAS special formats.

2 Input Command 2.4 Command Value

- 9 -

2.4 Command Value

2.4.1 Decimal Point Input I, II M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 I Type II G00 X100. Y-200.5 X100mm, Y-200.5mm G1 X100 F20. X100m, F20mm/min X100mm, F20mm/min

Y200 F100 (*1) Y200m, F100mm/min Y200mm, F100mm/min G4 X1.5 Dwell 1.5 s

X2 2ms 2s (*1) The F unit is mm/min for either type (inch system : inch/min).

2 Input Command 2.4 Command Value

- 10 -

2.4.2 Absolute / Incremental Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) M system

When axis coordinate data is issued in a machining program command, either the incremental command method (G91) that commands a relative distance from the current position or the absolute command method (G90) that moves to a designated position in a predetermined coordinate system can be selected. The absolute and incremental commands can be both used in one block, and are switched with G90 or G91. However, the arc radius designation (R) and arc center designation (I, J, K) always use incremental designations.

G90 ... Absolute command (absolute value command) G91 ... Incremental command (incremental value command)

These G codes can be commanded multiple times in one block. Example G90 X100. G91 Y200. G90 Z300. ;

Absolute value Incremental value Absolute value

(Note 1) As with the memory command, if there is no G90/G91 designation in the MDI command, the previously executed modal will be followed.

(Incremental value command) (Absolute value command)

End pointY100.

(0, 0) X 100.

Current position

End point

G 91 X 100. Y100. ;

X 100.

G 90 X 100. Y100. ;

Y100. Y100.

X100. (0, 0)

Program coordinate

Current position

2 Input Command 2.4 Command Value

- 11 -

(2) L system When axis coordinate data is issued in a machining program command, either the incremental command method that commands a relative distance from the current position or the absolute command method that moves to a designated position in a predetermined coordinate system can be selected. When issuing an incremental value command, the axis address to be commanded as the incremental axis name is registered in the parameter. However, the arc radius designation (R) and arc center designation (I, J, K) always use incremental designations.

Absolute command (absolute value command) ... X, Z Incremental command (incremental value command) ... U, W

Example G00 X100. W200. ;

Absolute value Incremental value

End point

Current position

2

u1

The above drawing shows the case for the diameter command.

X X

Z

(Incremental value command) (Absolute value command)

G 00 U u1 W w1 ; G 00 X x1 Z z1 ;

The above drawing shows the case for the diameter command.

Z

w1

z1

End point

Current position

x1

(0,0)

(Note) In addition to the above command method using axis addresses, to switch the absolute

value command/incremental value command, the command method using G90/91 can also be selected using a parameter.

2 Input Command 2.4 Command Value

- 12 -

2.4.3 Diameter/Radius Designation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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.

x6 u4

x6

u4

Coordinate zero point

X-axis radius designation

Z Z

X X X-axis diameter designation

Coordinate zero point

The difference in the diameter designation and radius designation is shown below.

Absolute value command Incremental value command Radius designation Diameter designation Radius designation Diameter designation Actual movement amount = x1

Actual movement amount = 2 x1

Actual movement amount = u1

Actual movement amount = 2 u1

2 Input Command 2.5 Command Value and Setting Value Range

- 13 -

2.5 Command Value and Setting Value Range

2.5.1 Command Value and Setting Value Range M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

[M system] Metric command Inch command Rotary axis

(Metric command) Rotary axis

(Inch command) Program number 08 Sequence number N5 Preparatory function G3/G21

0.001() mm/ 0.0001 inch X+53 Y+53 Z+53 +53 X+44 Y+44 Z+44 +44 X+53 Y+53 Z+53 +53 X+53 Y+53 Z+53 +53Movement

axis 0.0001() mm/ 0.00001 inch X+44 Y+44 Z+44 +44 X+35 Y+35 Z+35 +35 X+44 Y+44 Z+44 +44 X+44 Y+44 Z+44 +44

0.001() mm/ 0.0001 inch I+53 J+53 K+53 R+53 I+44 J+44 K+44 R+44 I+53 J+53 K+53 R+53 I+44 J+44 K+44 R+44

(Note 5)Arc and cutter radius 0.0001() mm/

0.00001 inch I+44 J+44 K+44 R+44 I+35 J+35 K+35 R+35 I+44 J+44 K+44 R+44 I+35 J+35 K+35 R+35 (Note 5)

0.001() mm/ 0.0001 inch X+53/P+8

Dwell 0.0001() mm/ 0.00001 inch X+53/P+8

0.001() mm/ 0.0001 inch

F63(Feed per minute) F43(Feed per revolution)

F44(Feed per minute) F34(Feed per revolution)

F63(Feed per minute) F43(Feed per revolution)

F44(Feed per minute) F34(Feed per revolution)

(Note 6)Feed function 0.0001 () mm/

0.00001 inch F54(Feed per minute)

F34(Feed per revolution) F35(Feed per minute)

F25(Feed per revolution) F54(Feed per minute)

F34(Feed per revolution)

F35(Feed per minute) F25(Feed per revolution)

(Note 6) Tool offset H3 D3 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4

0.001() mm/ 0.0001 inch R+53 Q53 P8 L4 Fixed

cycle 0.0001() mm/ 0.00001 inch R+44 Q44 P8 L4

2 Input Command 2.5 Command Value and Setting Value Range

- 14 -

[L system] Metric command Inch command Rotary axis

(Metric command) Rotary axis

(Inch command) Program number 08 Sequence number N5 Preparatory function G3/G21

0.001() mm/ 0.0001 inch X+53 Z+53 +53 X+44 Z+44 +44 X+53 Z+53 +53 X+53 Z+53 +53

0.0001() mm/ 0.00001 inch X+44 Z+44 +44 X+35 Z+35 +35 X+44 Z+44 +44 X+44 Z+44 +44 Movement

axis 0.00001() mm/ 0.000001 inch X+35 Z+35 +35 X+35 Z+35 +35

0.001() mm/ 0.0001 inch I+53 K+53 R+53 I+44 K+44 R+44 I+53 K+53 R+53 I+44 K+44 R+44

(Note 5) 0.0001() mm/ 0.00001 inch I+44K+44 R+44 I+35 K+35 R+35 I+44 K+44 R+44 I+35 K+35 R+35

(Note 5)

Arc and cutter radius

0.0001() mm/ 0.00001 inch I+35 K+35 R+35 I+35 K+35 R+35

0.001() mm/ 0.0001 inch X+53/P+8

0.0001() mm/ 0.00001 inch X+53/P+8 Dwell

0.0001() mm/ 0.00001 inch X+53/P+8 X+53/P+8

0.001() mm/ 0.0001 inch

F63(Feed per minute) F43(Feed per revolution)

F44(Feed per minute) F34(Feed per revolution)

F63(Feed per minute) F44(Feed per revolution)

F44(Feed per minute) F34(Feed per revolution)

(Note 6)

0.0001() mm/ 0.00001 inch

F54(Feed per minute) F34(Feed per revolution)

F35(Feed per minute) F25(Feed per revolution)

F54(Feed per minute) F34(Feed per revolution)

F35(Feed per minute) F25(Feed per revolution)

(Note 6)

Feed function

0.00001() mm/ 0.000001 inch

F45(Feed per minute) F25(Feed per revolution)

F45(Feed per minute) F25(Feed per revolution)

Tool offset T1/T2 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4

0.001() mm/ 0.0001 inch R+53 Q53 P8 L4

0.0001() mm/ 0.00001 inch R+44 Q44 P8 L4 Fixed

cycle 0.00001() mm/ 0.000001 inch R+35 Q35 P8 L4 R+35 Q35 P8 L4

(Note 1) indicates the additional axis address, such as A, B or C. (Note 2) The No. of digits check for a word is carried out with the maximum number of digits of

that address.

(Note 3) Numerals can be used without the leading zeros. (Note 4) The meanings of the details are as follows :

Example 1 : 08 : 8-digit program number Example 2 : G21 : Dimension G is 2 digits to the left of the decimal point, and 1 digit to

the right. Example 3 : X+53 : Dimension X uses + or - sign and represents 5 digits to the left of the

decimal point and 3 digits to the right. For example, the case for when the X axis is positioned (G00) to the 45.123 mm position in the absolute value (G90) mode is as follows : G00 X45.123 ;

3 digits below the decimal point 5 digits above the decimal point, so it's +00045, but the leading zeros and the mark (+) have been omitted. G0 is possible, too.

2 Input Command 2.5 Command Value and Setting Value Range

- 15 -

(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the degrees will be converted into 0.1 inches for interpolation.

(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees. Example : With the F1. (per-minute-feed) command, this will become the 10

degrees/minute command.

(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command, with an invalid decimal point has been assigned with a decimal point.

(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit.

(Note 9) Command the program No. in an independent block. Command the program NO. in the head block of the program.

2 Input Command 2.5 Command Value and Setting Value Range

- 16 -

Linear axis Rotary axis Input unit: mm Input unit: inch Degree () Minimum input setting unit 0.001/0.0001/0.00001 0.0001/0.00001 0.001/0.0001/0.00001 Maximum stroke (Value on machine coordinate system)

99999.999 mm 9999.9999 mm 999.99999 mm

9999.9999 inch 999.99999 inch

99999.999 9999.9999 999.99999

Maximum command value 99999.999 mm 9999.9999 mm 999.99999 mm

9999.9999 inch 999.99999 inch

99999.999 9999.9999 999.99999

Rapid traverse rate (Including during dry run)

1 to 1000000 mm/min 1 to 100000 mm/min 1 to 10000 mm/min

1 to 39370 inch/min 1 to 3937 inch/min

1 to 1000000 /min 1 to 100000 /min 1 to 10000 /min

M system cutting feed rate (Including during dry run)

0.01 to 1000000 mm/min 0.001 to 100000 mm/min

0.001 to 100000 inch/min 0.0001 to 10000 inch/min

0.01 to 1000000 /min 0.001 to 100000 /min

L system cutting feed rate (Including during dry run)

0.001 to 1000000 mm/min 0.0001 to 100000 mm/min 0.00001 to 10000 mm/min

0.0001 to 39370.0787 inch/min 0.00001 to 3937.00787 inch/min

0.001 to 1000000 /min 0.0001 to 100000 /min 0.00001 to 10000 /min

M system synchronous feed 0.001 to 999.999 mm/rev 0.0001 to 99.9999 mm/rev

0.0001 to 999.9999 inch/rev 0.00001 to 99.99999 inch/rev

0.01 to 999.99 /rev 0.001 to 99.999 /rev

L system synchronous feed 0.0001 to 999.9999 mm/rev 0.00001 to 99.99999 mm/rev 0.000001 to 9.999999 mm/rev

0.000001 to 99.999999 inch/rev 0.0000001 to 9.9999999 inch/rev

0.0001 to 999.9999 /rev 0.00001 to 99.99999 /rev 0.000001 to 9.999999 /rev

2nd to 4th reference point offset (value on machine coordinate system)

99999.999 mm 9999.9999 mm 999.99999 mm

9999.9999 inch 999.99999 inch

99999.999 9999.9999 999.99999

Tool offset amount (shape) 999.999 mm 99.9999 mm 9.99999 mm

99.9999 inch 9.99999 inch

Tool offset amount (wear) 9999.999 mm 999.9999 mm 99.99999 mm

9.9999 inch 0.99999 inch

Incremental feed amount 0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse

0.0001 inch/pulse 0.00001 inch/pulse

0.001 /pulse 0.0001 /pulse 0.00001 /pulse

Handle feed amount 0.001 mm/pulse 0.0001 mm/pulse 0.00001 mm/pulse

0.0001 inch/pulse 0.00001 inch/pulse

0.001 /pulse 0.0001 /pulse 0.00001 /pulse

Soft limit range (value on machine coordinate system)

99999.999 mm to +99999.999 mm 9999.9999 mm to +9999.9999 mm 999.99999 mm to +999.99999 mm

9999.9999 inch to +9999.9999 inch 999.99999 inch to +999.99999 inch

1 to 359.999 1 to 359.9999 1 to 359.99999

Dwell time 0 to 99999.999 s 0 to 99999.999 s Backlash compensation amount

0 to 9999 pulse 0 to 9999 pulse 0 to 9999 pulse

Pitch error compensation 0 to 9999 pulse 0 to 9999 pulse 0 to 9999 pulse M system thread lead (F) 0.001 to 999.999 mm/rev

0.0001 to 99.9999 mm/rev

0.0001 to 99.9999 inch/rev 0.00001 to 9.99999 inch/rev

M system thread lead (Precise E)

0.00001 to 999.99999 mm/rev 0.000001 to 99.999999 mm/rev

0.000001 to 39.370078 inch/rev 0.000001 to 3.937007 inch/rev

L system thread lead (F) 0.0001 to 999.9999 mm/rev 0.00001 to 99.99999 mm/rev 0.000001 to 9.999999 mm/rev

0.000001 to 99.999999 inch/rev 0.0000001 to 9.9999999 inch/rev

L system thread lead (Precise E)

0.00001 to 999.99999 mm/rev 0.000001 to 99.999999 mm/rev 0.0000001 to 99.9999999 mm/rev

0.000010 to 9.9999999 inch/rev 0.0000010 to 0.99999999 inch/rev

(Note 1) The second line in the table applies when the least setting increment is 0.001, 0.0001 from the first line. The third line applies when the least setting increment is 0.001, 0.0001, 0.00001 from the first line.

3 Positioning / Interpolation 3.1 Positioning

- 17 -

3 Positioning / Interpolation 3.1 Positioning

3.1.1 Positioning M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function carries out positioning at high speed using rapid traverse with the movement command value given in the program.

G00 Xx1 Yy1 Zz1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)

(x1, y1, z1: numerical values denoting the position data)

The above command positions the tool by rapid traverse. The tool path takes the shortest distance to the end point in the form of a straight line. For details on the rapid traverse feed rate of the NC, refer to the section entitled "Rapid Traverse Rate". Since the actual rapid traverse feed rate depends on the machine, refer to the specifications of the machine concerned. (1) The rapid traverse feed rate for each axis can be set independently with parameters. (2) The number of axes which can be driven simultaneously depends on the specifications

(number of simultaneously controlled axes). The axes can be used in any combination within this range.

(3) The feed rate is controlled within the range that it does not exceed the rapid traverse rate of each axis and so that the shortest time is taken. (Linear type)

Parameter setting enables movement at the rapid traverse rates of the respective axes independently for each axis. In this case, the tool path does not take the form of a straight line to the end point. (Non-Linear type)

End pointY

X

G 00 G 91 X 100. Y 100. ;

Current position 100.

100.

(Example) Linear type (Moves lineary to the end point.)

(Example) Non-linear type (Each axis moves

with each parameter speed.)

Current position

X

Y

End point

100.

100.

G 00 G 91 X 100. Y 100. ;

(4) The tool is always accelerated at the start of the program command block and decelerated at the end of the block.

3 Positioning / Interpolation 3.1 Positioning

- 18 -

3.1.2 Unidirectional Positioning M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The G60 command always moves the tool to the final position in a direction determined with parameters. The tool can be positioned without backlash.

G60 Xx1 Yy1 Zz1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)

(x1, y1, z1: numerical values denoting the position data) With the above command, the tool is first moved to a position distanced from the end point position by an amount equivalent to the creep distance (parameter setting) and then moved to its final position. For details on the rapid traverse feed rate of the NC, refer to the section entitled "Rapid Traverse Rate". Since the actual rapid traverse feed rate depends on the machine, refer to the specifications of the machine concerned.

Positioning to the final point is shown below (when this positioning is in the "+" direction.)

+

(Example)

1. The rapid traverse rate for each axis is the value set with parameters as the G00 speed.

2. The vector speed to the interim point is the value produced by combining the distance and respective speeds.

Interim point G60 G91 X100. Y100. ;

Current position X100.

Y100.

End point

3. The creep distance of the distance between the interim and end points can be set independently for each axis by "parameters".

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 19 -

(Note 1) The processing of the above pattern will be followed even for the machine lock and Z- axis 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.

3.2 Linear/Circular Interpolation

3.2.1 Linear Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Ff1 ; (Also possible for additional axes A, B, C, U, V, W simultaneously)

(x1, y1, z1 : numerical values denoting the position data; f1 : numerical value denoting the feed rate data)

Linear interpolation is executed by the above command at the f1 feed rate. The tool path takes the shortest distance to the end point in the form of a straight line. For details on the f1 command values for NC, refer to the section entitled "Cutting Feed Rate". Since the actual cutting feed rate depends on the machine, refer to the specifications of the machine concerned. (Example)

Current position

100. (85mm/min)

Feed rate (120mm/min)

Y

G01 G91 X100. Y100. F120 ;

X

End point

100. (85mm/min)

1. The cutting feed rate command moves the tool in the vector direction.

2. The component speeds of each axis are determined by the proportion of respective command values to the actual movement distance with linear interpolation.

(1) The number of axes which can be driven simultaneously depends on the specifications

(number of simultaneously controlled axes). The axes can be used in any combination within this range.

(2) The feed rate is controlled so that it does not exceed the cutting feed rate clamp of each axis. (3) When a rotary axis has been commanded in the same block, it is treated as a linear axis in

degree() units (1 = 1mm), and linear interpolation is performed.

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 20 -

3.2.2 Circular Interpolation (Center / Radius Designation) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Circular interpolation with I, J, K commands

This function moves a tool along a circular arc on the plane selected by the plane selection G code with movement command value supplied in the program.

G02(G03) Xx1 Yy1 Ii1 Jj1 Ff1 ; (Also possible for additional axes A, B, C, U, V, W) G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values Ii1, Jj1 : Arc center values Ff1 : Feed rate

The above commands move the tool along the circular arc at the f1 feed rate. The tool moves along a circular path, whose center is the position from the start point designated by distance "i1" in the X- axis direction and distance "j1" in the Y-axis direction, toward the end point. The direction of the arc rotation is specified by G02 or G03.

G02: Clockwise (CW) G03: Counterclockwise (CCW)

The plane is selected by G17, G18 or G19. G17: XY plane G18: ZX plane G19: YZ plane

(Example) See below for examples of circular

commands.

Center

Start point

I, J

F

Y

X

End point

X

Y G17 X

Z

Y

Z

G18

G19

G02

G03

G02

G03

G02

G03

(a) The axes that can be commanded simultaneously are the two axes for the selected plane. (b) The feed rate is controlled so that the tool always moves at a speed along the circumference

of the circle. (c) Circular interpolation can be commanded within a range extending from 0 to 360. (d) The max. value of the radius can be set up to six digits above the decimal point.

(Note 1) The arc plane is always based on the G17, G18 or G19 command. If a command is issued with two addresses which do not match the plane, an alarm will occur.

(Note 2) The axes configuring a plane can be designated by parameters. Refer to the section entitled "Plane Selection".

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 21 -

(2) R-specified circular interpolation Besides the designation of the arc center coordinates using the above-mentioned I, J and K commands, arc commands can also be issued by designating the arc radius directly.

G02(G03) Xx1 Yy1 Rr1 Ff1 ; (Also possible for additional axes A, B, C, U, V, W ) G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values Rr1 : Arc radius Ff1 : Feed rate

G02 or G03 is used to designate the direction of the arc rotation. The arc plane is designated by G17, G18 or G19. The arc center is on the bisector which orthogonally intersects the segment connecting the start and end points, and the point of intersection with the circle, whose radius has been designated with the start point serving as the center, is the center coordinate of the arc command. When the sign of the value of R in the command program is positive, the command will be for an arc of 180 or less; when it is negative, it will be for an arc exceeding 180.

(Example)

Current position (arc start point)

Y

G02 G91 X100. Y100. R100. F120 ;

R100.

X

Feed rate: 120mm/min

Arc end point coordinates (X, Y)

(a) The axes that can be commanded simultaneously are the two axes for the selected plane. (b) The feed rate is controlled so that the tool always moves at a speed along the circumference

of the circle.

(Note 1) The arc plane is always based on the G17, G18 or G19 command. If a command is issued with two addresses which do not match the plane, an alarm will occur.

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 22 -

3.2.3 Helical Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With this function, any two of three axes intersecting orthogonally are made to perform circular interpolation while the third axis performs linear interpolation in synchronization with the arc rotation. This simultaneous 3-axis control can be exercised to machine large-diameter screws or 3- dimensional cams.

G17 G02(G03) Xx1 Yy1 Zz1 Ii1 Jj1 Pp1 Ff1 ; G17 : Arc plane G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate values for arc Zz1 : End point coordinate of linear axis Ii1, Jj1 : Arc center coordinates Pp1 : Pitch No. Ff1 : Feed rate (1) The arc plane is designated by G17, G18 or G19. (2) G02 or G03 is used to designate the direction of the arc rotation. (3) Absolute or incremental values can be assigned for the arc end point coordinates and the end

point 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 p1 + )/2) = e s = arctan (ye/xe) arctan (ys/xs) Where xs, ys are the start point coordinates (0 < 2)

xe, ye are the end point coordinates The combination of the axes which can be commanded simultaneously depends on the specifications. The axes can be used in any combination within this range. The feed rate is controlled so that the tool always moves at a speed along the circumference of the circle.

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 23 -

(Example)

I-100 W

J100

X

Start point

Command program path

X

Y

Z

Y

End point

XY plane projection path in command program

End point

Start point

G91 G17 G02 X0. Y200. Z100. I100. J100. F120 ;

(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.

End point

V Z

Y X

Start point

When a simultaneous 4-axis command is used with the V axis as the axis parallel to the Y axis, helical interpolation will result for a cylinder which is inclined as shown in the figure on the right. In other words, linear interpolation of the Z and V axes is carried out in synchronization with the circular interpolation on the XY plane.

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 24 -

3.2.4 Spiral / Conical Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function interpolates arcs where the start point and endpoint are not on the circumference of the same circle into spiral shapes. G17 G02.1(G03.1) Xx1 Yy1 Ii1 Jj1 Pp1 Ff1 ; G17 : Arc plane G02.1, G03.1 : Arc rotation direction Xx1, Yy1 : End point coordinate Ii1, Jj1 : Arc center value Pp1 : Pitch number Ff1 : Feed rate The circular interpolation operation is performed at the feed rate f1 by the commands listed above. The tool draws a spiral arc path whose center is at the position from the start point which is designated by distance i1 for the X-axis direction and distance j1 for the Y-axis direction as the tool moves toward the end point.

The arc plane is designated by G17, G18 or G19. G17: XY plane G18: ZX plane G19: YZ plane

The direction of the arc rotation is designated by G2.1 or G3.1. G2.1: Clockwise (CW) G3.1: Counterclockwise (CCW)

The pitch number (number of rotations) is designated by p1. By assigning zero to p1, the pitch number designation can be omitted in this case, the

interpolation is obtained as a spiral rotation of less than one full turn. Assigning 1 to p1 yields a spiral rotation of more than one full turn but less than two full turns.

Example: G91 G17 G01 X60. F500 ;

Y140. ; G2.1 X60. Y0 I100. P1 F300 ; G01 X-120 ; G90 G17 G01 X60. F500 ; Y140.; G2.1 X120. Y140. I100. P1 F300 ; G01 X0 ;

X

I100.

Y

140.

X60.

160.60.W

End point

Start point

Center

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 25 -

(1) The combination of the axes which can be commanded simultaneously depends on the specifications. Any combination can be used within the specified range.

(2) The feed rate is a constant tangential rate. (Note 1) This function cannot be used in combination with a tool radius compensation command

(G41, G42).

(Note 2) The arc plane is always based on the G17, G18 or G19 command. Arc control is performed on a plane by the G17, G18 or G19 command even when two addresses which are not on any one plane are designated.

Example: When an axis other than the ones for

the spiral interpolation plane has been designated at the same time, the other axis will also be interpolated in synchronization with the spiral interpolation.

G17 G91 G2.1 X100. Z150. I150. P3 F500 ;

In the example given above, truncated cone interpolation is performed.

W

Z

Y

X

X

W

Z

X

XY plane

XZ plane

In the case of command format type 2 Spiral interpolation

G17 G02(G03) Xx1 Yy1 Ii1 Jj1 Qq1/Ll1 Ff1 ; G17 : Arc plane G02, G03 : Arc rotation direction Xx1, Yy1 : End point coordinate Ii1, Jj1 : Arc center values Qq1 : Incremental/decremental amount of radius per spiral rotation Ll1 : Pitch number Ff1 : Feed rate Relation between Q and L

L = (arc end point radius arc start point radius) / Q Q takes precedence if both Q and L have been designated at the same time. Conical interpolation

G17 G02(G03) Xx1 Yy1 Zz1 Ii1 Jj1 Kk1 /Qq /Ll1 Ff1 ; Zz1 : End point coordinate in height direction Kk1 : Amount by which height is incremented or decremented per spiral rotation Qq1 : Amount by which radius is incremented or decremented per spiral rotation Ll1 : Pitch number Ff1 : Feed rate

Relation between L and (I, J) K L = | Height | / | Amount by which height is incremented or decremented (I, J, K) | Q takes precedence over K which in turn takes precedence over L if Q, K and L have been

designated at the same time.

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 26 -

3.2.5 Cylindrical Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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

Cylindrical interpolation machining

Cylinder radius value Z axis

X axis C axis

(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 ;

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 27 -

3.2.6 Polar Coordinate Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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.

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.

Polar coordinate interpolation plane (G17 plane)

Hypothetical axis

X axis

C axis

Z axis

3 Positioning/Interpolation 3.2 Linear/Circular Interpolation

- 28 -

3.2.7 Milling Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When a lathe with linear axes (X, Z axes) and rotary axis (C axis) serving as the control axes is to perform milling at a workpiece end face or in the longitudinal direction of the workpiece, this function uses the hypothetical axis Y which is at right angles to both the X and Z axes to enables the milling shape to be programmed as the X, Y and Z orthogonal coordinate system commands. With this function, the workpiece can be treated as a cylinder with radius X, and commands can be designated on the plane formed by transferring the cylinder side surface instead. With milling interpolation, the commands programmed by the orthogonal coordinate system are converted into linear axis and rotary axis movements (workpiece rotation) to control the contours.

Y (Hypothetical axis)

C

X

Z

G12.1 ; Milling mode ON G13.1 ; Milling mode OFF (Turning mode)

G16 (Y-Z cylindrical plane) G17 (X-Y plane) G19 (Y-Z plane)

Z

X

Y

Z

X

Y

Z

X

Y

Plane on which radius X cylinder is developed. Select to machine the cylindrical plane of a workpiece.

X-Y plane in XYZ orthogonal coordinate system. Use this to machine the workpiece end face.

Y-Z plane in XYZ orthogonal coordinate system. Select this to machine a plane of a cylinder cut in the longitudinal direction.

3 Positioning/Interpolation 3.3 Curve Interpolation

- 29 -

3.3 Curve Interpolation 3.3.2 Exponential Interpolation

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

With this function, the rotary axis is changed into exponential functions vis-a-vis the linear axis movements to achieve interpolation. When exponential function interpolation is performed, linear interpolation is performed between the other axes and the linear axis. This makes it possible to machine tapered grooves (equal helix machining of tapered shapes) whose helix angle is always constant. The function can be used for slotting and grinding end mills and other tools. [Equal helix machining of tapered shapes]

Helix angle : J1=J2=J3

A axis (rotary axis)

(linear axis)

Z axis

X axis J1 J2 J3

(G02.3/G03.3)

(G00)

(G01) (G01)

[Relationship between linear and rotary axes)

A axis (rotary axis)

X ax

is (l

in ea

r a xi

s)

X=B (eCA-1) {B, C = constants}

3 Positioning/Interpolation 3.3 Curve Interpolation

- 30 -

3.3.3 Spline Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function automatically generates spline curves that smoothly pass through rows of dots designated by a fine-segment machining program, and performs interpolation for the paths along the curves. This enables high-speed and high-accuracy machining to be achieved. To use this function, the high-accuracy control function (G08P1) is required.

4 Feed 4.1 Feed Rate

- 31 -

4 Feed 4.1 Feed Rate

4.1.1 Rapid Traverse Rate (m/min) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 1000 1000 1000 1000 1000 1000 1000 1000 L system 1000 1000 1000 1000 1000 1000 1000 1000

[M system]

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

Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)

Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)

[L system] The rapid traverse rate can be set independently for each axis. G00, G27, G28, G29, G30 and G53 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

Least input increment B C D

Metric input 1~1000000 (mm/min, /min)

1~100000 (mm/min, /min)

1~10000 (mm/min, /min)

Inch input 1~39370 (inch/min) 1~3937 (inch/min) Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch) Least input increment D : 0.00001 mm

4 Feed 4.1 Feed Rate

- 32 -

4.1.2 Cutting Feed Rate (m/min) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 1000 1000 1000 1000 1000 1000 1000 1000 L system 1000 1000 1000 1000 1000 1000 1000 1000

[M system]

This function specifies the feed rate of the cutting commands, and a feed amount per spindle rotation or feed amount per minute is commanded. Once commanded, it is stored in the memory as a modal value. The feed rate modal value is cleared to zero only when the power is turned ON. The maximum cutting feed rate is clamped by the cutting feed rate clamp parameter (whose setting range is the same as that for the cutting feed rate).

Cutting Feed Rate setting range

Least input increment B C Metric input 1~1000000 (mm/min, /min) 1~100000 (mm/min, /min) Inch input 1~39370 (inch/min) 1~3937 (inch/min)

Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch)

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.

[L system] This function specifies the feed rate of the cutting commands, and a feed amount per spindle rotation or feed amount per minute is commanded. Once commanded, it is stored in the memory as a modal value. The feed rate modal is cleared to zero only when the power is turned ON. The maximum cutting feed rate is clamped by the cutting feed rate clamp parameter (whose setting range is the same as that for the cutting feed rate).

Cutting Feed Rate setting range

Least input increment B C D

Metric input 1~1000000 (mm/min, /min)

1~100000 (mm/min, /min)

1~10000 (mm/min, /min)

Inch input 1~39370 (inch/min) 1~3937 (inch/min) Least input increment B : 0.001 mm (0.0001 inch) Least input increment C : 0.0001 mm (0.00001 inch) Least input increment D : 0.00001 mm

Effective G-code commands for the cutting feed

G01, G02, G03, G33, etc. As to others, refer to interpolation specifications.

4 Feed 4.1 Feed Rate

- 33 -

4.1.3 Manual Feed Rate (m/min) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 1000 1000 1000 1000 1000 1000 1000 1000 L system 1000 1000 1000 1000 1000 1000 1000 1000

The manual feed rates are designated as the feed rate in the jog mode or incremental feed mode for manual operation and the feed rate during dry run ON for automatic operation. The manual feed rates are set with external signals. The manual feed rate signals from the PLC includes two methods, the code method and numerical value method. Which method to be applied is determined with a signal common to the entire system. The signals used by these methods are common to all axes. Setting range under the code method

Metric input 0.00 to 14000.00 mm/min (31 steps) Inch input 0.000 to 551.000 inch/min (31 steps)

Setting range under the numerical value method

Metric input 0 to 1000000.00 mm/min in 0.01 mm/min increments Inch input 0 to 39370 inch/min in 0.001 inch/min increments

Multiplication factor PCF1 and PCF2 are available with the numerical value setting method.

4 Feed 4.2 Feed Rate Input Methods

- 34 -

4.2 Feed Rate Input Methods

4.2.1 Feed per Minute M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

[M system] By issuing the G94 command, the commands from that block are issued directly by the numerical value following F as the feed rate per minute (mm/min, inch/min).

Metric input (mm)

Least input increment (B) 0.001 mm (C) 0.0001 mm

F command increment (mm/min)

without decimal point with decimal point

F1 = 1 mm/min F1. = 1 mm/min

F1 = 1 mm/min F1. = 1 mm/min

Command range (mm/min) 0.01~1000000.000 0.001~100000.000

Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch

F command increment (inch/min)

without decimal point with decimal point

F1 = 1 inch/min F1. = 1 inch/min

F1 = 1 inch/min F1. = 1 inch/min

Command range (inch/min) 0.001~100000.0000 0.001~10000.0000

When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min). To assign commands under 1 mm/min (or 1 inch/min), ensure that commands are assigned with a decimal point.

The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter (I_Sync) to OFF.

The F command increments are common to the entire part system.

4 Feed 4.2 Feed Rate Input Methods

- 35 -

[L system] By issuing the G94 command, the commands from that block are issued directly by the numerical value following F as the feed rate per minute (mm/min, inch/min). Metric input (mm)

Least input increment (B) 0.001 mm (C) 0.0001 mm (D) 0.00001 mm F

command increment (mm/min)

without decimal point with decimal point

F1 = 1 mm/min F1. = 1 mm/min

F1 = 1 mm/min F1. = 1 mm/min

F1 = 1 mm/min F1. = 1 mm/min

Command range (mm/min) 0.001~1000000.000 0.0001

~100000.0000 0.00001

~10000.00000

Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch

F command increment (inch/min)

without decimal point with decimal point

F1 = 1 inch/min F1. = 1 inch/min

F1 = 1 inch/min F1. = 1 inch/min

Command range (inch/min) 0.0001~39370.0787 0.00001~3937.00787

When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min). To assign commands under 1 mm/min (or 1 inch/min), ensure that commands are assigned with a decimal point.

The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter (I_Sync) to OFF.

4 Feed 4.2 Feed Rate Input Methods

- 36 -

4.2.2 Feed per Revolution M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

By issuing the G95 command, the commands from that block are issued directly by the numerical value following F as the feed rate per spindle revolution (mm/revolution or inch/revolution). The least command increment and command range of the feed rate designation F are as follows.

[M system]

Metric input (mm) Least input increment (B) 0.001 mm (C) 0.0001 mm

F command increment (mm/rev)

without decimal point with decimal point

F1 = 0.01 F1. = 1

F1 = 0.01 F1. = 1

Command range (mm/rev) 0.001~999.999 0.0001~99.9999

Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch

F command increment (inch/rev)

without decimal point with decimal point

F1 = 0.001 F1. = 1

F1 = 0.001 F1. = 1

Command range (inch/rev) 0.0001~999.9999 0.00001~99.99999

When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min).

The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter (I_Sync) to OFF.

The F command increments are common to the entire part system.

[L system]

Metric input (mm) Least input increment (B) 0.001 mm (C) 0.0001 mm (D) 0.00001 mm

F command increment (mm/rev)

without decimal point with decimal point

F1 = 0.0001 F1. = 1

F1 = 0.0001 F1. = 1

F1 = 0.0001 F1. = 1

Command range (mm/rev) 0.0001~999.999 0.00001~99.99999 0.000001~9.999999

Inch input (inch) Least input increment (B) 0.0001 inch (C) 0.00001 inch

F command increment (inch/rev)

without decimal point with decimal point

F1 = 0.000001 F1. = 1

F1 = 0.000001 F1. = 1

Command range (inch/rev) 0.000001~99.999999 0.0000001~9.9999999

When commands without a decimal point have been assigned, it is not possible to assign commands under 1 mm/min (or 1 inch/min).

The initial status after power-ON can be set to asynchronous feed (per-minute-feed) by setting the "Initial synchronous feed" parameter (I_Sync) to OFF.

4 Feed 4.2 Feed Rate Input Methods

- 37 -

4.2.4 F 1-digit Feed M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When the "F1digt" parameter is ON, the feed rate registered by parameter in advance can be assigned by designating a single digit following address F. There are six F codes: F0 and F1 to F5. The rapid traverse rate is 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 direct command with feed rate value of 5 digits following address F. When an F 1-digit command has been designated, the "In F 1-digit" external output signal is output. When the programmed feed rate has been designated as an F 1-digit command, the feed rate can be increased or reduced by turning the manual handle. (Note) When using M64 and M64A, the feed rate cannot be increased or decreased using the

manual handle. (1) Amount by which speed is varied by manual handle Speed variation amount F is expressed by the equation below:

F = P K

FM

P : Handle pulses () FM : F1 to F5 upper limit (parameter setting) K : Speed variation constant (parameter setting)

Example: When the feed rate is to be increased or reduced by 10 mm/min per manual handle

scale increment

If Fmax is 3600 mm/min, then: F = 10 = 1 K

3600

Therefore, K = 360. (2) Conditions under which F1-digit feed is valid

(a) The automatic operation must be selected. (b) Automatic start must be underway. (c) Cutting feed must be underway, and the F 1-digit feed rate must be designated. (d) The F 1-digit valid parameter must be ON. (e) The F 1-digit feed rate change valid signal must be ON. (f) A dry run must not be in progress.

4 Feed 4.3 Override

- 38 -

4.3 Override

4.3.1 Rapid Traverse Override M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Type 1 (code method)

Four levels of override (1%, 25%, 50% and 100%) can be applied to manual or automatic rapid traverse using the external input signal supplied.

(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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Type 1 (code method)

Override can be applied in 10% steps from 0% to 300% to the feed rate command designated in the machining program using the external input signal supplied. Code method commands are assigned as combinations of Y 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 Feed 4.3 Override

- 39 -

4.3.3 2nd Cutting Feed Override M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Override can be further applied in 0.01% steps from 0% to 327.67% as a second stage override to the feed rate after the cutting feed override has been applied.

(Note 1) A PLC must be built into the unit for this function.

4.3.4 Override Cancel M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

By turning on the override cancel external signal, the override is automatically set to 100% for the cutting feed during an automatic operation mode (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.

4 Feed 4.4 Acceleration / Deceleration

- 40 -

4.4 Acceleration / Deceleration

4.4.1 Automatic Acceleration / Deceleration after Interpolation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

F F FC F

Tsr

Exponential acceleration / linear deceleration

Soft acceleration/deceleration

Exponential acceleration/deceleration

Tsr Tss Tss Tsc Tsc Tsc Tsr

(Note 1) The rapid traverse feed acceleration/deceleration patterns are 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).

4 Feed 4.4 Acceleration / Deceleration

- 41 -

Acceleration / Deceleration during Continuing Blocks (1) Continuous G1 blocks

T s c T sc

f 1

f 2

G 1 G 1

Tsc Tsc

f 1

f 2

G1

G10

0

The tool does not decelerate between blocks.

(2) Continuous G1-G0 blocks

Tsc

G1 G0

G1

G0Tsr

G1

Tsr

G0 G1

Tsc

Tsr

G0

Tsr

If the G0 command direction is the same as that for G1, whether G1 is to be decelerated is selected using a parameter. If no deceleration is set, superposition is performed even when G0 is in the constant inclination acceleration/deceleration state. If the G0 command direction is the opposite of that for G1, G0 will be executed after G1 has decelerated. (In the case of two or more simultaneous axes, G0 will also be executed after G1 has decelerated when the G0 command direction is the opposite of that for G1 for even one axis.)

4.4.2 Rapid Traverse Constant Inclination Acceleration / Deceleration M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

4 Feed 4.4 Acceleration / Deceleration

- 42 -

(1) When the interpolation distance is longer than the acceleration and deceleration distance

L

T s T s T d

T

Next block

rapid

rapid : Rapid traverse rate

Ts : Acceleration/deceleration time constant

Td : Command deceleration check time : Acceleration/deceleration inclination T : Interpolation time L : Interpolation distance

T = rapid

L +Ts

Td = Ts + (0~1.7 ms)

= tan-1 rapid

Ts ( )

(2) When the interpolation distance is shorter than the acceleration and deceleration distance

rapid: Rapid traverse rate

Ts: Acceleration/deceleration time constant Td: Command deceleration check time : Acceleration/deceleration inclination T: Interpolation time L: Interpolation distance

L

Ts Td

T

rapid

Next block

= tan-1 rapid

Ts ( )

Td = + (0 ~ 1.7 ms) T 2

T = 2 Ts L / rapid

The time required to perform a command deceleration check during rapid traverse constant inclination acceleration/deceleration is the longest value among the rapid traverse deceleration check times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration/deceleration time constant, and the interpolation distance, respectively.

4 Feed 4.4 Acceleration / Deceleration

- 43 -

(3) 2-axis simultaneous interpolation (When linear interpolation is used, Tsx < Tsz, and Lx Lz) When 2-axis simultaneous interpolation (linear interpolations) is performed during rapid traverse constant inclination acceleration and deceleration, the acceleration (deceleration) time is the longest value of the acceleration (deceleration) times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration and deceleration time constant, and the interpolation distance, respectively. Consequently, linear interpolation is performed even when the axes have different acceleration and deceleration time constants.

x Tsx Tsx

Tdx

Lx

Tx

Next block

X axis

Tsz

Lz

Tz

Z axis

rapid X

rapid Z

Z

Tsz Tdz

Next block

When Tsz is greater than Tsx, Tdz is also greater than Tdx, and Td = Tdz in this block.

The program format of G0 (rapid traverse command) when rapid traverse constant inclination acceleration/deceleration are executed is the same as when this function is invalid (time constant acceleration/deceleration). This function is valid only for G0 (rapid traverse).

4 Feed 4.4 Acceleration / Deceleration

- 44 -

4.4.3 Rapid Traverse Constant Inclination 3-Step Acceleration / Deceleration M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The acceleration is normally calculated on the basis of speed/time when acceleration or deceleration is to be performed. In actual fact, however, the time taken for the desired positioning may increase due to changes (such as a reduction in the acceleration capability due to reduced torque at high-speed rotation) in the acceleration caused by the characteristics of the motor. To offset this, the acceleration in the high rotation speed range is set separately from what is set for the low rotation speed range for a multi-step acceleration configuration. By so doing, the speed is controlled to match the characteristics of the motor so that acceleration can be performed up to the high rotation speed range while holding down the increase in the positioning time. This function is valid only during rapid traverse inclined constant linear acceleration/deceleration and G0 interpolation.

t

v

Com- mand

Motor operation

Case without 2- or 3-step acceleration/deceleration

(a) Case with 2-step acceleration/deceleration

t

v

t

v

Acceleration/decele ration that factors in the motor operation

Time which can be shortened

(b) Case with 3-step acceleration/deceleration

Time which can be shortened

4 Feed 4.5 Thread Cutting

- 45 -

4.5 Thread Cutting

4.5.1 Thread Cutting (Lead/Thread Number Designation) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Lead designation The thread cutting with designated lead are performed based on the synchronization signals from the spindle encoder.

G33 Zz1 Qq1 Ff1/Ee1 ;

G33 : Thread command Zz1 : Thread length Qq1 : Shift angle ("q1" is the shift angle at thread cutting start 0 to 360) Ff1 : Thread lead Ee1 : Thread lead (precise lead threads)

The tables below indicate the thread lead ranges. [M system]

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 ~999.999

0.00001 ~999.99999 0.0001 0.0001

~39.3700 0.000001

~39.370078

0.0001 0.0001 ~99.9999

0.000001 ~99.999999 0.00001 0.00001

~3.93700 0.000001

~3.937007

[L system]

Metric command Inch command Command increment

(mm) F (mm/rev) E (mm/rev)

Command increment

(inch) F (inch/rev) E (inch/rev)

0.001 0.0001 ~999.9999

0.00001 ~999.99999 0.0001 0.00001

~99.999999 0.000010

~9.9999999

0.0001 0.00001 ~99.99999

0.00001 ~99.99999 0.00001 0.000001

~9.9999999 0.0000010

~0.99999999 The axis direction characterized by a large movement serves as the reference for the lead.

4 Feed 4.5 Thread Cutting

- 46 -

(2) Thread number designation Inch threads are cut by designating the number of threads per inch with the E address. Whether the E command is a thread number designation or lead designation is selected with the parameters.

G33 Zz1 Qq1 Ee1 ;

G33 : Thread command Zz1 : Thread length Qq1 : Shift angle ("q1" is the shift angle at thread cutting start 0 to 360) Ee1 : Thread number per inch

The tables below indicate the thread leads. [M system]

Metric command Inch command Command increment

(mm)

Thread number command range

(thread/inch)

Command increment

(inch)

Thread number command range

(thread/inch) 0.001 0.03~999.99 0.0001 0.0255~9999.9999

0.0001 255~9999.999 0.00001 0.25401~999.9999

[L system]

Metric command Inch command Command increment

(mm)

Thread number command range

(thread/inch)

Command increment

(inch)

Thread number command range

(thread/inch) 0.001 0.03~999.99 0.0001 0.0101~9999.9999

0.0001 0.255~9999.999 0.00001 0.10001~999.99999 The number of thread per inch is commanded for both metric and inch systems, and the direction of the axis with a high movement serves as the reference.

4 Feed 4.5 Thread Cutting

- 47 -

4.5.2 Variable Lead Thread Cutting M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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__;

G34 X/U Z/W F/E K

: Variable lead thread cutting command : Thread end point X coordinate : Thread end point Z coordinate : Threads basic lead : Lead increment/decrement amount per thread rotation

F+3.5K

Non-lead axis

Lead axis

F+2.5K F+1.5K F+0.5K

Lead speed F+4K

F+3K F+2K F+K F

4 Feed 4.5 Thread Cutting

- 48 -

4.5.3 Synchronous Tapping

4.5.3.1 Synchronous Tapping Cycle M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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 , R1 ;

G84 G74 Xx1, Yy1 Zz1 Rr1 Pp1 Ff1 Ss1 ,R1

: Mode, forward tapping : Mode, reverse tapping : Hole position data, hole drilling coordinate position : Hole machining data, hole bottom position : Hole machining data, hole R position : Hole machining data, dwell time at hole bottom : Z-axis feed amount (tapping pitch) per spindle rotation : Spindle speed : Synchronous system selection

(2) Tapping thread number assignment

G84(G74) Xx1 Yy1 Zz1 Rr1 Pp1 Ee1 Ss1 , R1 ;

G84 G74 Xx1, Yy1 Zz1 Rr1 Pp1 Ee1 Ss1 ,R1

: Mode, forward tapping : Mode, reverse tapping : Hole position data, hole drilling coordinate position : Hole machining data, hole bottom position : Hole machining data, hole R position : Hole machining data, dwell time at hole bottom : Tap thread number per 1-inch feed of Z axis : Spindle speed : Synchronous system selection

4 Feed 4.5 Thread Cutting

- 49 -

The control state will be as described below when a tapping mode command (G74, G84) is commanded.

1. Cutting override Fixed to 100% 2. Feed hold invalid 3. "In tapping mode" signal is output 4. Deceleration command between blocks invalid 5. Single block invalid

The tapping mode will be canceled with the following G commands.

G61 ....... Exact stop check mode G61.1 .... High-accuracy control mode G62 ....... Automatic corner override G64 ....... Cutting mode

(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

Point R

(4)

G1 deceleration start with tap return

G0 feed start to point R

G1 decelera- tion start during tap cutting

In-position finish for G0 feed from point R

Feed rate

Hole bottom

Time T

(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)

4 Feed 4.5 Thread Cutting

- 50 -

4.5.3.2 Pecking Tapping Cycle M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

G84(G74) Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1 Ss1 ,Ss2 ,Ii1 ,Jj1 ,Rr2 ;

G X, Y Z R Q F P S , S , I , J , R

: G84 forward tapping cycle, G74 reverse tapping cycle : Hole drilling point position : Hole bottom position : Point R position : Depth of cut per pass (designated as an incremental value) : Cutting feed rate : 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 : r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode

G0 Xx1 Yy1 ,Ii1

G0 Zr1

G1 Zq1 Ff1

M4

G1 Z-m Ff1

M3

G1 Z(q1+m) Ff1

M4

G1 Z-m Ff1

M3

G1 Z(q1+m) Ff1

: :

G1 Z(z1-q1*n) Ff1

G4 Pp1

M4

G1 Z-z1 Ff1 Ss2

G4 Pp1

M3

G98G0 Z-r1 ,Ij1

G99

M3

M4

n7

q1

m

m q1

q1

x1,y1

r1

z1

G98 G99

n3n2

n1

n4 n4

n5 n6

n7

n3

n2 n1

n4

n5

n6

*1. m: "#8018 G84/G74 return" parameter 2. This program is for the G84 command. The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.

n5 n6

Adding this option, the deep-hole tapping cycle option is also added. Select either the pecking tapping cycle or the deep-hole tapping cycle with parameter. When the pecking tapping cycle is executed in the synchronous tapping mode, the synchronous tapping cycle option and pecking tapping cycle option are required.

(1)

(2)

(3) (6)

(4) (5) (7)

(10)

(9) (11)(8)

(n7)

(n5) (n6) (n5) (n6)

(n4) (n4)

(n1)

(n2) (n3) M98 mode

M99 mode

(1) Yy1 , Ii1 (2) 1 (3) Ff1 (4) 4 (5) - Ff1 (6) 3 (7) G1 Z(q1+m) Ff1 (8) M4 (9) G1 Z-m Ff1 (10) M3 (11) G1 Z(q1+m) Ff1 : : (n1) G1 Z(z1-q1*n) Ff1 (n2) G4 Pp1 (n3) M4 (n4) G1 Z-z1 Ff1 Ss2 (n5) G4 Pp1 (n6) M3 G98 mode G0 Z-r1 , Ij1 G99 mode No movement M3: Spindle forward rotation

4: Spindle reverse rotation

(n7)

* 1. m: "#8018 G84/G74 return" parameter 2. This program is for the G84 command. The spindle forward rotation (M3)

and reverse rotation (M4) are reversed with the G74 command.

4 Feed 4.5 Thread Cutting

- 51 -

4.5.3.3 Deep-hole Tapping Cycle M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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. Adding this option, the pecking tapping cycle option is also added. Select either the pecking tapping cycle or the deep-hole tapping cycle by parameter. When the deep-hole tapping cycle is executed in the synchronous tapping mode, the synchronous tapping cycle option and deep-hole tapping cycle option are required. When "depth of cut per pass Q" is designated in the block containing the G84 or G74 tapping cycle command in the state when the deep-hole tapping cycle is selected by parameter, the deep-hole tapping cycle is executed. In the following cases, the normal tapping cycle is established. When Q is not designated When the value of Q designated is zero

G84(G74) Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1 ,Rr2

G X,Y Z R Q F P ,R

: G84 forward tapping cycle, G74 reverse tapping cycle : Hole drilling point position : Hole bottom position : Point R position : Depth of cut per pass (designated as an incremental value) : Cutting feed rate : Dwell time at hole bottom and point R return : r2=1 synchronous tapping mode, r2=0 asynchronous tapping mode

(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G9 G1 Zq1 Ff1 (4) M4 (Spindle reverse rotaion) (5) G9 G1 Z-q1 Ff1 (6) G4 Pp1 (7) M3 (Spindle forward rotation) (8) G1 Z(q1-c) Ff1 (9) G9 G1 Z(q1+c) Ff1 (10) M4 (Spindle reverse rotaion) (11) G9 G1 Z-(2q1) Ff1 (12) G4 Pp1 (13) M3 (Spindle forward rotation) (14) G1 Z(2q1-c) Ff1 (15) G9 G1 Z(q1+c) Ff1 : (n1) G9 G1 Z(z1-q1*n+c) Ff1 (n2) G4 Pp1 (n3) M4 (Spindle reverse rotaion) (n4) G9 G1 Z-z1 Ff1 (n5) G4 Pp1 (n6) M3 (Spindle forward rotation) (n7) G98 modeG0 Z-r1 G99 modeNo movement

q1

c

c q1

q1

x1,y1

r1

z1

G98 mode

G99 mode

(1)

(2)

(3)

(4)

(5)

(6)(7)

(8)

(9)

(10)

(11)

*1. Clearance amount c : "#8010 G84/G74 return"parameter 2. This program is for the G84 command. The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.

R point (12)(13)

(14)

(15)

(n6)

(n2)

(n1)

(n4)

(n7)

(n5) (n6)(n5)

(n4)

(n3)

4 Feed 4.5 Thread Cutting

- 52 -

4.5.4 Chamfering M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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.

Chamfer amount

Thread cutting cycle

Chamfer angle

4 Feed 4.5 Thread Cutting

- 53 -

4.5.6 Circular Thread Cutting M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Circular threads in which the leads are in longitudinal direction can be cut. Command format

Ii Kk G35 (G36) Xx/Uu Zz/Ww

Rr Ff/Ee Qq

G35 : Clockwise (CW) G36 : Counterclockwise (CCW) Xx/Uu : X-axis arc end point coordinate (X: absolute value of workpiece coordinate

system, U: incremental value from present position) Zz/Ww : Z-axis arc end point coordinate (Z: absolute value of workpiece coordinate

system, W: incremental value from present position) Ii : X-axis arc center (incremental value of arc center as referenced from start

point) Kk : Z-axis arc center (incremental value of arc center as referenced from start

point) Rr : Arc radius Ff/Ee : Longitudinal axis (axis with most travel) direction lead (Ff: normal lead thread cutting, Ee: precision lead threads or inch threads) Qq : Thread cutting start shift angle

Center

Start point

X axis

Z axisR

WZ

I

K

End point

X

U/2

4 Feed 4.6 Manual Feed

- 54 -

4.6 Manual Feed

4.6.1 Manual Rapid Traverse M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 override is common to all part systems.

X

Rapid traverse override

Rapid traverse

Tool

Machine tool

CNC

PLC

Rapid traverse

100 1 50 25

Y Z Axis movement control

4.6.2 Jog Feed M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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. The jog feed rate is common to all part systems.

Manual cutting feed

Feed rate

Tool

Machine tool

CNC

PLC

Jog

30000

Z

Override

2000

Y X

Axis movement

control + + +

4 Feed 4.6 Manual Feed

- 55 -

4.6.3 Incremental Feed M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When the incremental feed mode is selected, the tool can be operated by an amount equivalent to the designated amount (incremental value) in the axis direction each time the jog switch is pressed. The incremental feed amount is the amount obtained by multiplying the least input increment that was set with the parameter by the incremental feed magnification rate. The incremental feed amount parameter and its magnification rate are common to all part systems.

Scale factor

Step feed

Tool

Machine tool

CNC

PLC

Incremental

1000

Z Axis

movement control

Y X + + +

4.6.4 Handle Feed M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

(3 axes) In the handle feed mode, individual axes can be moved in very small amounts either separately or simultaneously by rotating the manual pulse generators installed on each of the axes.

(Note 1) The actual movement amount and scale may not match if the manual pulse generator is rotated quickly.

4 Feed 4.6 Manual Feed

- 56 -

4.6.5 Manual Feed Rate B M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

"Manual feedrate B" is a function that sets a random axis feedrate from the user PLC separately from the "manual feedrate". The "manual feedrate B" feedrate setting can be selected from the feedrate common for all axes and the feedrate independent of reach axis. By combining the "manual feedrate B" function with the manual/automatic simultaneous function, a random axis can be moved at the "manual feedrate 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 feedrate" even during the manual operation mode. The "manual feedrate B" function can move an axis at a speed different from the "manual feedrate". 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 feedrate B" and "manual feedrate" is shown below.

B axis speed

Z axis speed

Y axis speed

X axis speed

Manual federate Cutting override

Dry run speed

M an

ua l f

ee dr

at e

B s

pe ed

Manual override validity

Dry run validity

Manual feedrate B valid n-th axis Validity

Each axis manual feedrate B speed 1st axis

Each axis manual feedrate B speed 2nd axis

Each axis manual feedrate B speed 3rd axis

Each axis manual feedrate B speed 4th axis

Each axis manual feedrate B valid Validity

Y260=0

Y261=0

Y262=0

Y263=1

Y2BC=1

Y21D=0

Y229=0

R138 R139

R400 R401

R402 R403

R406 R407

R404 R405

4 Feed 4.7 Dwell

- 57 -

4.7 Dwell

4.7.1 Dwell (Time-based Designation) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 ;

G94 : Asynchronous G04 : Dwell Xx1, Uu1, Pp1 : Time

"x1" of the time-based dwell can be designated in the range from 0.001 to 99999.999 seconds.

5 Program Memory / Editing 5.1 Memory Capacity

- 58 -

5 Program Memory / Editing 5.1 Memory Capacity

Machining programs are stored in the NC memory.

5.1.1 Memory Capacity (Number of Programs Stored) (Note) The tape length will be the total of two part systems when using the 2-part system

specifications. 40 m (64 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

80 m (128 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

160 m (200 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

320 m (200 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

600 m (400 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

1280 m (1000 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

2560 m (1000 programs)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

5120 m (1000 programs) M65S, M66S: When APLC is added, up to 2560m.

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

5 Program Memory / Editing 5.2 Editing

- 59 -

5.2 Editing Method

5.2.1 Program Editing M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

5 Program Memory / Editing 5.2 Editing

- 60 -

5.2.2 Background Editing M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables one machining program to be created or editing while another program is being run.

Prohibited

Memory operation

Machining with memory operationProgram editing

Editing

O4000

O3000

O2000

O1000

Program registered in memory

(1) The data of the machining programs being used in memory operation can be displayed and

scrolled on the setting and display unit, but data cannot be added, revised or deleted. (2) The editing functions mentioned in the preceding section can be used at any time for machining

programs which are not being used for memory operation. This makes it possible to prepare and edit the next program for machining, and so the machining

preparations can be made more efficiently. (3) The machining program will not be searched as the operation target even when searched in the

edit screen.

5 Program Memory / Editing 5.2 Editing

- 61 -

5.2.3 Buffer Correction M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

During automatic operation (memory or tape operation) or MDI operation, this function initiates single block stop and enables the next command to be corrected or changed. 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.

Pre-read block

Execution block

Setting and display unit

NC opera-

tion

Buffer correction

Memory mode

MDI mode

Memory

MDI

Tape or IC card

Tape mode

5 Program Memory / Editing 5.2 Editing

- 62 -

012345678 TEST CUT PROGRAM EDIT BACKGROUND EDITING 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 ; > N10 ; N11 ; N12 ;

SEARCH DELETE REPLACE INSERT MENU

5.2.4 Word Editing M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

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 The editing buffer data can be inserted after the word on which the cursor is

positioned. (The same word can also be repeatedly inserted.) Copy 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 Comments can be set in machining programs. Word 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 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.) String 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

The program being run is displayed when the program running display request (PLC) is ON.

Program operation start position setting

The start block can be designated by moving the cursor on the editing screen.

6 Operation and Display 6.1 Structure of Operation / Display Panel

- 63 -

6 Operation and Display 6.1 Structure of Operation / Display Panel

The setting and display unit is configured of the setting section and keyboard section. When the key switches are pressed, a buzzer sounds allowing the operation to be confirmed visually and audibly. The following display units can be used for the setting and display unit.

Type Function Configuration element Details

FCU6-DUT32 10.4-type monochrome LCD display unit (separated type)

10.4-type LCD, Escutcheon Control card (RX215)

Used as a set with FCUA-KB20. Control card 24VDC input

FCU6-DUN33 10.4-type color LCD display unit (separated type)

10.4-type LCD, Escutcheon Control card (RX215)

Used as a set with FCUA-KB20. Control card 24VDC input

FCUA-LD100 7.2-type monochrome LCD liquid crystal (integrated type)

7.2-type LCD, Escutcheon Control card (RX213) Key switches

Control card 24VDC input

FCUA-LD10 7.2-type monochrome LCD display unit (separated type)

7.2-type LCD, Escutcheon Control card (RX213)

Used as a set with FCUA-KB20. Control card 24VDC input

FCUA-CT100 9-type monochrome CRT + communication terminal (integrated type, machining center system sheet)

9-type monochrome CRT, Escutcheon Control card (RX211) Key switches

Control card 24VDC input CRT section 100VAC input

FCUA-CT120 9-type monochrome CRT + communication terminal (integrated type, lathe system sheet)

9-type monochrome CRT, Escutcheon Control card (RX211) Key switches

Control card 24VDC input CRT section 100VAC input

FCUA-CR10 9-type monochrome CRT communication terminal (separated type)

9-type monochrome CRT, Escutcheon Used as a set with FCUA-KB10/KB12. Control card 24VDC input CRT section 100VAC input

FCUA-KB10 Communication terminal (separated type, machining center system sheet)

Key switch Control card

Used as a set with FCUA-CR10.

FCUA-KB12 Communication terminal (separated type, lathe system sheet)

Key switch Control card

Used as a set with FCUA-CR10.

FCUA-KB20 Communication terminal (separated type, machining center system sheet)

Key switch Use as a set with FCU6-DUT32/ DUN33 or FCUA-LD10

FCUA-KB021 Communication terminal (separated type, machining center system sheet)

Key switch Use as a set with FCU6-DUT32/ DUN33 KB20 with changed outline dimensions

FCUA-KB30 Communication terminal (separated type, lathe system sheet)

Key switch Use as a set with FCU6-DUT32/ DUN33 or FCUA-LD10

FCU6-KB031 Communication terminal (separated type, lathe system sheet)

Key switch Use as a set with FCU6-DUT32/ DUN33 KB30 with changed outline dimensions

6.2 Operation Methods and Functions

6.2.1 Memory Switch (PLC Switch) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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. There are a total of 32 switch points.

6 Operation and Display 6.3 Display Methods and Contents

- 64 -

6.3 Display Methods and Contents

6.3.1 Status Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

6.3.2 Position Display Position data such as present positions for tools, coordinate positions and workpiece coordinate positions can be displayed. (1) Present position counter

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

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.

Workpiece offset Machine zero point

Workpiece zero point

Relative value (a) (Machine position) Displayed by tool reference position

Workpiece coordinate

Present value B

Tool reference position Tool nose position

Relative value (b) Displayed by tool nose position

Tool

6 Operation and Display 6.3 Display Methods and Contents

- 65 -

(2) Workpiece coordinate counter

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

The workpiece coordinate system modal number from G54 to G59 and the workpiece coordinate value in the workpiece coordinate system are indicated. (3) Remaining command counter

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

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

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Each axis coordinate value in the basic machine coordinate system whose zero point is the characteristic position determined depending on the machine is indicated. (5) Present value B

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

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

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

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.

6 Operation and Display 6.3 Display Methods and Contents

- 66 -

6.3.3 Program Running Status display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Program now being executed is displayed.

6.3.4 Setting and Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The parameters used in controller operations can be set and displayed.

6.3.5 MDI Data Setting and Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

6.3.6 Specification List Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function displays a list of the specifications which are currently valid.

6.3.7 Clock M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Operation and Display 6.3 Display Methods and Contents

- 67 -

6.3.8 Hardware / Software Configuration Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function displays the configuration of the installed hardware and software.

6.3.9 Integrated Time Display M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The integrating run time count during each signal of power-ON, automatic operation, automatic start and external integrating run time is ON can be set and displayed. The maximum time displayed is 9999 hours 59 minutes 59 seconds. Power-ON: Total of all the integrated run times, each starting when the power of the

NC control unit is turned ON and ending when it is turned OFF. Automatic operation: Total of the integrated run times for all machining periods, each starting

when the auto start button is pressed in the memory mode and ending when the reset status is established (usually when the M02 / M30 command is designated or the reset button is pressed). (This differs according to PLC machining.)

Automatic start: Total of the integrated run times for all automatic start operations, each starting when the auto start button is pressed in the memory or MDI mode and ending when the feed hold stop or block stop is established or the reset button is pressed.

External integration: Based on the PLC sequence, this is the integrated run time of the signal set by the PLC, and it comes in two types, external integration 1 and external integration 2.

6.3.10 Available Languages M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 12 languages

12 languages

12 languages

12 languages

13 languages

13 languages

13 languages

13 languages

L system 12 languages

12 languages

12 languages

12 languages

13 languages

13 languages

13 languages

13 languages

This function makes it possible to switch between Japanese and English which are the standard languages used for the screen displays. Furthermore, under the optional specifications, the display language can be switched to German, Italian, French, Spanish, Chinese (Traditional Chinese characters, simplified Chinese characters), Korean, Portuguese, Hungarian, Dutch or Swedish.

6 Operation and Display 6.3 Display Methods and Contents

- 68 -

6.3.11 Additional Languages (Japanese, English, German, Italian, French, Spanish, Chinese, Korean, Portuguese, Hungarian, Dutch, Swedish)

6.3.11.1 Japanese M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.2 English M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.3 German M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.4 Italian M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.5 French M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.6 Spanish M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6 Operation and Display 6.3 Display Methods and Contents

- 69 -

6.3.11.7 Chinese (1) Chinese (Traditional Chinese characters)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

(2) Chinese (Simplified Chinese characters)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

6.3.11.8 Korean M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.9 Portuguese M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.10 Hungarian M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.11 Dutch M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6.3.11.12 Swedish M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

6 Operation and Display 6.3 Display Methods and Contents

- 70 -

6.3.12 Screen Saver, Backlight OFF M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The screen saver and backlight OFF functions turn off the displays when there is no need to view the screen. This function is available only on the LCD.

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.

This function turns off the backlight in order to extend the service life of the LCD screen's backlight.

6.3.13 Screen Deletion M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

7 Input / Output Functions and Devices

7.1 Input / Output Data

- 71 -

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) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Tool offset data input / output

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Common variable input / output

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Parameter input / output

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

History data output

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

Remote program input

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

7 Input / Output Functions and Devices

7.2 Input / Output I/F

- 72 -

7.2 Input / Output I/F

7.2.1 RS-232C I/F M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Port 1 and 2 of the RS-232C interface can be used.

Port Port 1/2 Transmission speed ~ 19.2kbps Handshake method DC code method, RTS/CTS method possible

Each port can be used for the following application.

Port 1: Input/output, tape operation, Anshin-net Port 2: Input/output, tape operation, GX Developer communication, computer link, Anshin-net

7.2.2 IC Card I/F

7.2.2.1 I/F for IC card in Control Unit M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

IC cards can be attached inside the NC unit and used.

7.2.3 Data Server I/F M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Ethernet I/F cards can be attached onto the NC unit and used. (The Ethernet for the data server interface is the same as that for the Ethernet interface described in section 7.2.4.)

7.2.4 Ethernet I/F M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Ethernet I/F card can be attached onto the NC unit and used.

7 Input / Output Functions and Devices

7.3 Computer Link

- 73 -

7.3 Computer Link

7.3.1 Computer Link B M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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. When using the 2-part system, this function cannot be operated in the 2nd part system.

CNC Com-

munication software

CNC HOST

RS-232C Com- mands

Machining programs

Machining programs 32-kbyte reception buffer

BTR operation

Operation

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 74 -

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

8.1.1 Command / Output 8.1.1.1 Spindle Functions

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 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 an 8-digit number following address S (S00000000 to S99999999) is commanded, a signed 32-bit binary data or 8-digit BCD data and start signal will be output to the PLC. 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.

(Machining program, Manual numerical command)

Analog spindle

D/A converter

Changeover (Parameter)

Remote I/O unit

(Parameter)

6-digit

6-digit BIN

6-digit

BIN

PLC NC

S command value

Spindle output command creation

Gear ratio Max. rotation

speed

S command analysis

Spindle controller MDS-C1-SP series, etc.

S Command

Spindle rotation command

Start signal

Spindle rotation command

Override

Gear selection

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 75 -

(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.

8.1.1.2 Spindle Serial I/F M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This I/F is used to connect the digital spindle (AC spindle motor and spindle driver (SP, SPJ2)).

8.1.1.3 Spindle Analog I/F M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Spindle control can be executed using an analog spindle instead of the digital spindle. In this case, the remote I/O unit DX120/DX121 is required. The analog output voltage is calculated from the present rotation speed regarding the voltage at the max. rotation speed as the maximum analog voltage. The specifications of the analog voltage output are as follows. (1) Output voltage ... 0 to 10 V (2) Resolution ... 1/4095 (12 multiplier of 2) (3) Load conditions ... 10 k (4) Output impedance ... 220

8.1.1.4 Coil Change M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 commands are assigned from the PLC.

8.1.1.5 Automatic Coil Change M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 76 -

8.1.2 Speed Control 8.1.2.1 Constant Surface Speed Control

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 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

G96 Constant surface speed G97 Constant surface speed cancel

The surface speed is commanded with an S code. For the metric designation, the speed is commanded with an m/min unit, and for the inch designation, the speed is commanded with a feet/min unit. In the constant surface speed cancel mode, the S code is a spindle rotation speed command. The axis for which constant surface speed is controlled is generally the X axis. However, this can be changed with the parameter settings or with address P in the G96 block.

(Note) If there is only one spindle, the spindle will not operate normally if the constant surface speed control command, S command or spindle related M command is commanded randomly from each part system. These commands must be commanded from only one certain part system, or commanded simultaneously with standby.

The controller will execute the following control for the constant surface speed control and S commands. The part system from which an S command was issued last will have the spindle control rights. That part system will judge whether the constant surface speed command mode is valid or canceled, and will execute spindle control.

Part system 1 Part system 2 Part system 1

Spindle control rights

S100 G96

1000 r/min S200 m/min S100 m/min S2000 r/min

S2000 G96 S200 G97 S1000

Spindle speed

Part system 2 program

Part system 1 program

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 77 -

8.1.2.2 Spindle Override M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

8.1.2.3 Multiple-spindle Control Multi-spindle control is a function that controls all the spindles except for the first spindle for a machine tool equipped with second, third and fourth spindles (sub-spindles) 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. The figure below shows an example of the configuration for a machine which is equipped with second and third spindles.

Tool post 1

Fi rs

t s pi

nd le

S ec

on d

sp in

dl e

Tool spindle (third spindle)

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 78 -

8.1.2.3.1 Multiple-spindle Control I M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Spindle selection function

Using the spindle selection command (such as G43.1 [G group 20]), this function makes it possible to switch the spindle among the first through fourth spindles to which the subsequent S command (S*****) is to apply.

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

Spindle control commands using an extended word address (SO=*****) In addition to using the "S*****" S commands, it is also possible to assign commands which differentiate the applicable spindle among the first through fourth spindles by using the SO=*****. Command format

SO=*****; O : Number assigned as the spindle number (1: first spindle; 2: second spindle; 3: third

spindle; 4: fourth 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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 (SWS) ON from the PLC. The selected spindle rotates at the rotation speed which was output. The spindles which were de-selected by spindle selection signal (SWS) OFF continue to rotate at the same rotation speed as the speed immediately before their de-selection. As a result, each of the spindles can be made to rotate simultaneously at a different rotation speed. The spindle command selection signal is used to select which of the spindles is to receive the S command from which system.

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 79 -

8.1.3 Position Control 8.1.3.1 Spindle Orientation

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 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 pre- positioning 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) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

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.

C axis Spindle Spindle

Servo ON

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 80 -

8.1.3.3 Spindle Synchronization 8.1.3.3.1 Spindle Synchronization I

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

In a machine with two or more spindles, this function controls the rotation speed and phase of one selected spindle (synchronized spindle) in synchronization with the rotation of the other selected spindle (basic spindle). It is used in cases where, for instance, workpiece clamped to the basic spindle is to be clamped to the synchronized spindle instead or where the spindle rotation speed is to be changed while one workpiece remains clamped to both spindles. The synchronous spindle is designated and the start/end of the synchronization are commanded with the G command in the machining program.

Command format Spindle synchronization control cancel (G113) This command releases the state of synchronization between two spindles whose rotation has been synchronized by the spindle synchronization command. G113;

Spindle synchronization control ON (G114.1) This command is used to designate the basic spindle and the spindle to be synchronized with the basic spindle, and it places the two designated spindles in the synchronized state. By designating the synchronized spindle phase shift amount, the phases of the basic spindle and synchronized spindle can be aligned.

G114.1 H__ D__ R__ A__ ;

H__ : Selects the basic spindle. D__ : Selects the spindle to be synchronized with the basic spindle. E__ : Designates the synchronized spindle phase shift amount. A__ : Designates the spindle synchronization acceleration/deceleration time constant.

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 81 -

8.1.3.3.2 Spindle Synchronization II M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

In a machine with two or more spindles, this function controls the rotation speed and phase of one selected spindle (synchronized spindle) in synchronization with the rotation of the other selected spindle (basic spindle). It is used in cases where, for instance, workpiece clamped to the basic spindle is to be clamped to the synchronized spindle instead or where the spindle rotation speed is to be changed while one workpiece remains clamped to both spindles. The selection of the spindles to be synchronized, the start of the synchronization and other settings are all designated from the PLC. The spindle synchronization control mode is established by inputting the spindle synchronization control signal. While this mode is established, the synchronized spindle is controlled in synchronization with the rotation speed assigned for the basic spindle.

8.1.3.4 Tool Spindle Synchronization I (Polygon) 8.1.3.4.1 Tool Spindle Synchronization IA (Spindle-Spindle, Polygon)

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

With a machine equipped with two or more spindles under serial connection control, this function enables spindle-spindle polygonal machining (IA) by controlling the workpiece spindle rotation in synchronization with the rotary tool spindle rotation. The rotary tool spindle and workpiece spindle are designated among the spindles subject to serial connection control. Serial connection control for the workpiece spindle and rotary tool spindle can be performed by MDS-*-SP or MDS-*-SPJ2. Command format Spindle-spindle polygonal machining mode command (G114.2) This command establishes the spindle-spindle polygonal machining mode in which two spindles are rotated in synchronization at two different speeds by designating the rotary tool spindle and workpiece spindle and by designating the rotational ratios (number of rotary tool teeth and number of work angles) of the two designated spindles. G114.2 H__ D__ E__ L__ R__ ;

H__ : Selects the rotary tool spindle. D__ : Selects the workpiece spindle. E__ : Designates the rotary tool spindle rotational ratio. L__ : Designates the workpiece spindle rotational ratio. R__ : Synchronized spindle phase shift amount

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 82 -

Spindle-spindle polygonal machining mode cancel command (G113) This command releases the state of synchronization between two spindles whose rotation has been synchronized by the spindle synchronization command. G113;

8.1.3.4.2 Tool Spindle Synchronization IB (Spindle-Spindle, Polygon) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With a machine equipped with two or more spindles under serial connection control, this function enables spindle-spindle polygonal machining (IB) by controlling the rotary tool spindle rotation in synchronization with the workpiece spindle rotation. The rotary tool spindle and workpiece spindle are designated among the spindles subject to serial connection control. A parameter is used to switch from spindle-spindle polygonal machining (IB) to spindle-NC axis polygonal machining (IC) or vice versa. Serial connection control for the workpiece spindle and rotary tool spindle can be performed by MDS-*-SP or MDS-*-SPJ2.

Command format Spindle-spindle polygonal machining mode ON (G51.2 or G251) This command establishes the spindle-spindle the polygonal machining mode in which two spindles are rotated in synchronization at two different speeds by designating the rotary tool spindle and workpiece spindle and by designating the rotational ratios (number of work angles and number of rotary tool teeth) of the two designated spindles. G51.2 H__ D__ P__ Q__ R__ ;

H__ : Selects the workpiece spindle (spindle). D__ : Selects the rotary tool spindle (spindle). P__ : Designates the workpiece spindle rotational ratio. Q__ : Designates the rotary tool spindle rotational ratio. R__ : Synchronized spindle phase shift amount

Spindle-spindle polygonal machining cancel command (G50.2) G50.2:

8 Spindle, Tool and Miscellaneous Functions 8.1 Spindle Functions (S)

- 83 -

8.1.3.4.3 Tool Spindle Synchronization IC (Spindle-NC axis, Polygon) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With a machine equipped with a workpiece spindle subject to serial connection control and also an NC axis serving as the rotary tool axis, this function enables spindle-NC axis polygonal machining (IC) by controlling the rotary tool axis rotation in synchronization with the workpiece spindle rotation. A parameter is used to switch from spindle-spindle polygonal machining (IB) to spindle-NC axis polygonal machining (IC) or vice versa. Serial connection control for the workpiece spindle can be performed by MDS-*-SP or MDS-*- SPJ2.The rotary tool axis can be performed by MDS-*-V1/V2. Command format G51.2 P__ Q__ ;

P__ : Selects the workpiece spindle (spindle). Q__ : Selects the rotary tool axis (NC axis).

Spindle-spindle polygonal machining cancel command (G50.2) G50.2:

8 Spindle, Tool and Miscellaneous Functions 8.2 Tool Functions (T)

- 84 -

8.2 Tool Functions (T)

8.2.1 Tool Functions M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) M system

When an 8-digit number following address T (T00000000 T99999999) is assigned, 8-digit code data and start signal will be output to PLC. Only one set of T commands can be commanded in a block. Processing and complete sequences must be incorporated on the PLC side for all T commands.

(Note 1) This function requires a built-in PLC.

(Note 2) There are some screens in the setting and display unit that cannot display all eight digits.

(2) L system

The command is issued with an 8-digit number following address T (T0 T99999999).The high- order 6 digits or 7 digits are designated as the tool No., and the low-order 2 digits or 1 digit are designated as the offset No. Which method is to be used is designated with parameters.

The 6-digit (or 7-digit) tool No. code data and start signal will be output to the PLC. Processing and complete sequences must be incorporated on the PLC side for all T commands.

(Note 1) This function requires a built-in PLC.

(Note 2) There are some screens in the setting and display unit that cannot display all eight digits.

Txxxxxxxx

Tool offset No.

Tool No.

Txxxxxxxx

Tool No.

Tool offset No.

8 Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)

- 85 -

8.3 Miscellaneous Functions (M)

8.3.1 Miscellaneous Functions M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When an 8-digit number (M00000000~M99999999) is assigned following address M, the 8-digit code data and start signal are output to PLC. M2-digit BCD output is used for the standard PLC specifications. When a 2-digit number following address M (M00 M97) is assigned, the code data and start signal will be output to the PLC. Apart from the above signals, various special independent signals are also output for the following signals.

M00 : Program stop M01 : Optional stop M02 : Program end M30 : Program end

Respective processing and complete sequences must be incorporated on the PLC side for all M commands from M00 to M97. M98 and M99 have specific purposes and can not be used.

(Note 1) There are some screens in the setting and display unit that cannot display all eight digits.

8.3.2 Multiple M Codes in 1 Block

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 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).

(Note 1) This function requires a built-in PLC. In this case, the code data and start signal are 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.

8 Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)

- 86 -

8.3.3 M Code Independent Output M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

M code output Independent Response to controller

M00 M00 Fin1 or Fin2 M01 M01 Fin1 or Fin2 M02 M02 Reset & rewind M30 M30 Reset & rewind

If movement or dwell command exists in the same block as these M commands, this signal is output upon completion of the movement or dwell command.

8.3.4 Miscellaneous Function Finish M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

Miscellaneous function finish signal (FIN1)

Miscellaneous function strobe (MF)

Command Next block

8 Spindle, Tool and Miscellaneous Functions 8.3 Miscellaneous Functions (M)

- 87 -

Miscellaneous function finish signal 2 (FIN2) When the controller checks that FIN2 is ON, it sets the function strobes OFF and simultaneously advances to the next block. The PLC checks that the strobe signals are OFF and sets FIN2 OFF. Below is an example of a time chart applying when a miscellaneous function has been assigned.

8.3.5 M Code Output during Axis Positioning M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function controls the timing at which miscellaneous functions are output, and it outputs a miscellaneous function when axis reaches at the designated position movement. The command format is as follows. G117 Xx1 Zz1 Cc1 ;

G117 : In-axis-movement miscellaneous function output command Xx1, Zz1, Cc1 : Movement start points

: Miscellaneous function

(Example) G117 Xx1 Zz1 Mm1 Mm2 Mm3 Mm4 ; G117 Xx2 Zz2 Mm5 Mm6 Mm7 Mm8 ; G01 X200 Z200 ;

Mm1

Mm2

Mm3

Mm4 Mm5

Mm6

Mm7

Mm8

End point (200, 200)

(x2, z2)

(x1, z1) Start point

Miscellaneous function finish signal (FIN2)

Miscellaneous function strobe (MF)

Command Next block

8 Spindle, Tool and Miscellaneous Functions 8.4 2nd Miscellaneous Functions (B)

- 88 -

8.4 2nd Miscellaneous Function (B)

8.4.1 2nd Miscellaneous Function M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The code data and start signals are output when an 8-digit number is assigned following the address code A, B or C whichever does not duplicate the axis name being used. Processing and complete sequences must be incorporated on the PLC side for all 2nd miscellaneous commands.

(Note 1) This function requires a built-in PLC.

(Note 2) There are some screens in the setting and display unit that cannot display all eight digits.

9 Tool Compensation 9.1 Tool Length / Position Offset

- 89 -

9 Tool Compensation 9.1 Tool Length / Position Offset

9.1.1 Tool Length Offset M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

These commands make it possible to control the axis movement by offsetting the position of the end point of the movement command by an offset amount set on the TOOL OFFSET screen. Using this function, it is possible to offset the difference in distance between the actual position of the machine's tool nose and the program coordinate position made by the tool length and to enhance both the programming and operational efficiency.

(1) M system

G43 G44

Zz1 Zz1

Hh1 Hh1

Offset direction

Offset axis Offset No.

; ;

Tool length offset can be provided not only for the Z axis but for all other axes which can be controlled in the system (X, Y, etc.).

G49 ; Tool length offset cancel The offset direction is determined by the G command.

G43: Forward direction (z1 + h1) G44: Reverse direction (z1 h1)

Offset can be canceled by the following G commands. G49; G43 H0; G44 H0;

(Example) Example of tool length offset using a combination with tool length measurement type I

M

G28 X0 Y0 Z0 ; T01 ; T02 M06 ; G91 G00 G43 Z2.0 H01 ;

M

(Note) The tool length offset amount is set as a negative value such as H01 = 450.000.

Z + 2.0

H01 = 450.000

Z 2.0

H01 = 450.000

Z 0.0 Workpiece

Table Table

Workpiece

(Note) When the tool length offset axis is returned to the reference position, the offset of that axis is canceled.

9 Tool Compensation 9.1 Tool Length / Position Offset

- 90 -

(2) L system (a) Shape offset Tool length is offset in reference to the programmed base position. The programmed base position is usually the center of the tool rest or the nose position of the base tool.

Z-axis tool length offset

Tool used for machining

Base tool

X-axis tool length offset

Base position (base point)

Z-axis tool length offset

X-axis tool length offset

The programmed base position is the center of the tool rest:

The programmed base position is the nose of the base tool:

(b) Wear offset The wear of a tool nose can be offset.

Tool nose

Z-axis tool nose wear offset amount

X-axis tool nose wear offset amount

X

Z

9 Tool Compensation 9.1 Tool Length / Position Offset

- 91 -

(c) Command format Tool offset is performed by a T command. It is specified in eight digits following address T. Tool offset is divided into two types: tool length offset and tool nose wear offset. The Nos. of such two types of offsets are specified by a parameter. Also a parameter is used to specify whether the offset Nos. is specified by one or two low-order digits of a T command. 1. Specifying tool length and wear offset Nos. together using one or two low-order digits of the T

command

T********

T********

Tool length offset No. and tool nose wear offset No. Tool No.

Tool length offset No. and tool nose wear offset No. Tool No.

2. Specifying tool length and wear offset Nos. separately

T********

T********

Tool nose wear offset No. Tool length offset No. Tool No.

Tool nose wear offset No. Tool length offset No. Tool No.

The tool offset for the lathe is valid only for the X and Z axes. If an additional axis (Y axis) is added, the tool offset will be validated for the additional axis. The additional axis is the third or fourth axis which is selected using a parameter.

9 Tool Compensation 9.1 Tool Length / Position Offset

- 92 -

9.1.2 Tool Position Offset M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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 radius 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 : Offset Xx1, Yy1 : Movement axes Dd1 : Offset No.

With tool position offset, the compensation operation is performed only for blocks containing a G45 to G48 command

G45 command G46 command G47 command G48 command Extension by amount equivalent to offset amount

Reduction by amount equivalent to offset amount

Extension by twice the offset amount

Reduction by twice the offset amount

Program command

Actual move- ment amount

Program command

Actual move- ment amount

Program command

Actual move- ment amount

Program command

Actual move- ment amount

(1) If the start and end points are on an axis, the radius can be extended or reduced only for one- quarter, one-half and three-quarter arcs.

(2) In the case of absolute value 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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.

9 Tool Compensation 9.2 Tool Radius

- 93 -

9.2 Tool Radius

9.2.1 Tool Radius Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

r r

r: Tool radius compensation amount Programmed path

Tool center path

The tool radius compensation command controls the compensation from that block in which G41 or G42 is commanded. In the tool radius compensation mode, the program is read up to five blocks ahead including blocks with no movement, and interference check using tool radius is conducted up to three blocks ahead in any of those blocks with movement.

9 Tool Compensation 9.2 Tool Radius

- 94 -

G17 G01 G41 Xx1 Yy1 Dd1 ;

G17 : Compensation plane G01 : Cutting G41 : Left compensation Xx1.Yy1 : Movement axis Dd1 : 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

An arc is inserted at the corner by the following command during tool radius compensation.

G39 Xx1 Yy1 ;

Xx1, Yy1 : Movement amount

Tool center path Arc inserted at corner

Programmed path

The compensation vector can be changed in following two ways.

G38 Xx1 Yy1 ;

Xx1, Yy1 : Movement amount

The tool radius compensation vector amount and direction are retained. G38 Xx1 Yy1 Ii1 Jj1 Dd1 ;

Xx1, Yy1 : Movement amount Ii1, Jj1 : Compensation vector direction Dd1 : Compensation vector length

The tool radius compensation vector direction is updated by I and J.

N12 N11

N13 N14 N15

Tool center path Holding of previous intersection point vector Vector with length D (i14, j14)

Intersection point vector

N11G01Xx11; N12G38Xx12Yy12; N13G38Xx13Yy13; N14G38Xx14Ii14Jj14Dd14; N15G40Xx15Yy15;

9 Tool Compensation 9.2 Tool Radius

- 95 -

The tool radius compensation is canceled by the following command. G40 Xx1 Yy1 Ii1 Jj1 ;

Xx1, Yy1 : Movement amount Ii1, Jj1 : Compensation vector direction

The vector prior to canceling is prepared by calculating the intersection point with the I and J direction.

When i and j commands are assigned to G40

N11 N12

N13

N14

(i14,J14)

N11G01Xx11; N12Xx12Yy12; N13Xx13Yy13; N14G40Xx14Ii14Jj14;

Tool center path

9 Tool Compensation 9.2 Tool Radius

- 96 -

9.2.2 3-dimensional Tool Radius Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This command serves the function of compensating for the spherical radius of ball end mills. It corrects the actual tool center path to be either more outside or inside the programmed path by an amount equivalent to the tool radius amount in accordance with the 3-dimensional vectors.

G code Function G40 Tool radius compensation cancel G41 Tool radius compensation left command (compensation in the direction toward

IJK) G42 Tool radius compensation right command (compensation in the direction away

from IJK) With 3-dimensional tool radius compensation, the compensation is controlled from the block in which the block containing the G41 or G42 command has been designated. G01 G41 Xx1 Yy1 Zz1 Ii1 Jj1 Kk1 Dd1 ;

G01 : Cutting G41 : Left compensation Xx1, Yy1, Zz1 : Movement axis Ii1, Jj1, Kk1 : Tool sphere center vectors Dd1 : Offset No.

The radius from the tool spherical center to the end nose serves as the compensation amount that corresponds to the tool offset No. designated by d1. The offset Nos. that can be used are limited by the "number of tool compensation amount sets." If the compensation vectors (tool spherical center vectors) are to be changed, the G41 and I, J and K commands must be assigned.

3-dimensional compensation vector

Tool

Tool center coordinates

(x, y, z) (I, J, K) Normal line vector

r: Tool radius

Work

Programmed coordinates (x, y, z)

Z (K)

X (I)Y (J)

9 Tool Compensation 9.2 Tool Radius

- 97 -

9.2.3 Tool Nose Radius Compensation (G40/41/42) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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

Programmed path

Compensated path

Nose R interference check

In the nose radius compensation mode, the program is read up to five blocks ahead including blocks with no movement, and an interference check using the nose radius is conducted up to three blocks ahead in any of those blocks with movement.

9 Tool Compensation 9.2 Tool Radius

- 98 -

9.2.4 Automatic Decision of Nose Radius Compensation Direction (G46/40) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 progress direction

1

R

2 3 4

LR L

R

RR

R

RR

R

RR

R L

L

LL

L

LL

L

LL

M ou

ve m

en t v

ec to

rs (to

ol n

os e

po in

ts 1

to 4

)

Tool nose point

Range of each tool nose point (1 to 4)

Tool nose progress direction

5

R

6 7 8

LR L

R

RR

R

RR

R

RR

R L

L

LL

L

LL

L

LL

Tool nose point Tool nose direction

M ou

ve m

en t v

ec to

rs (to

ol n

os e

po in

ts 5

to 8

)

Range of each tool nose point (5 to 8)

9 Tool Compensation 9.3 Tool Offset Amount

- 99 -

9.3 Tool Offset Amount

9.3.1 Number of Tool Offset Sets The number of tool offset sets is as follows.

9.3.1.1 20 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9.3.1.2 40 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9.3.1.3 80 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9.3.1.5 200 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9.3.1.6 400 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9.3.1.7 999 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

9 Tool Compensation 9.3 Tool Offset Amount

- 100 -

9.3.2 Offset Memory

9.3.2.1 Tool Shape/Wear Offset Amount M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function registers the tool shape offset and wear offset amounts among the positions of the tools moving in the direction parallel to the control axis. Compensation may encompass two or more axes.

1. Shape offset amount The tool length offset amount, tool radius compensation amount, nose radius compensation amount, nose radius imaginary tool tip point or tool width can be set as the shape offset amount. The compensation amount that can be set and used differs depending on whether offset amount setting type 1, 2 or 3 is used.

2. Wear offset amount When the tip of the tool used has become worn, the wear offset amount is used to offset this wear. Types of wear offset amounts include the tool length wear offset amount, tool radius wear compensation amount, and nose radius wear compensation amount. The wear offset amount can be used with offset amount setting types 2 and 3, and it is added to the shape offset amount for compensation. (a) Type 1: 1-axis offset amount [M system]

This is the value that is used by rotary tools. As the tool length offset amount, among the offset amounts for the position of the tool moving in the direction parallel to the control axis, the offset amount in the longitudinal direction of the rotary tool is registered. The tool length offset amount is set as a minus value. As the tool radius compensation amount, among the offset amounts for the position of the tool moving in the direction parallel to the control axis, the offset amount in the radial direction of the rotary tool is registered. The tool radius compensation amount is set as a plus value. One offset amount data is registered in one offset number, and the offset Nos. are assigned using the address D or H commands. When a No. is assigned by a D address command, offset is provided in the form of the tool radius; when it is assigned by an H address command, it is provided in the form of the tool length.

9 Tool Compensation 9.3 Tool Offset Amount

- 101 -

(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 the type 1 tool length offset amount (Offset types I and II are available for handling offset amounts.)

Wear offset amount when using type 2

M

Tool radius compensation amount

M

W

Offset type I Offset type II

Z0.0 Workpiece Workpiece

Table Table

Z0.0

Tool radius compensation amount

Tool length offset amount

Tool length offset amount

M

Tool length wear offset

t

Tool radius wear compensation amount

(c) Type 3: 2-axis offset amounts [L system]

Type 3 is for the offset amounts used by non-rotary tools. As the offset amounts, the tool length along the X, Y and Z axes and the wear amount along each of these axes, the nose radius and nose radius wear amount, tool tip point P and tool width can be registered. Offset is provided in the directions of the X, Y and Z axes from the base position in the program. Generally, the center of the tool rest or the tip of the base tool is used as the programmed base position.

1. The programmed base position 2. The programmed base position

is the center of the tool rest: is the tip of the base tool:

X-axis tool length offset

amount

Base position (base point)

Z-axis tool length offset amount

Base position (base point)

X-axis tool length offset amount

Tool used for machining

Base tool

Z-axis tool length offset amount

9 Tool Compensation 9.3 Tool Offset Amount

- 102 -

The tool tip contour arc radius (nose radius) of a non-rotary tool with an arc (nose radius) at its tip is registered as the nose radius offset amount.

Imaginary tool nose point

Tool nose center

Nose radius compensation amount

X-axis tool length wear offset

X

Z Z-axis tool length wear offset

Tool nose

The X-axis tool length offset amount, Z-axis tool length offset amount and nose radius compensation amount are set as plus amounts. The offset type (1, 2 or 3) is set using a parameter.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 103 -

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.

G52

G92

G55G54

L0

L0

W055

W054

EXT

ref

M0

G52

R

L0 Local coordinate system zero point Offset set with parameters G52 Local coordinate system offset *1) Offset set with program W0-54 Workpiece coordinate system zero point (G54) (0 when power is turned ON) W0-55 Workpiece coordinate system zero point (G55) G54 Workpiece coordinate system (G54) offset *1) G55 Workpiece coordinate system (G55) offset G92 G92 coordinate system shift EXT External workpiece coordinate offset M0 Machine coordinate system zero point ref Reference position *1)The G52 offset is available independently for G54 to G59.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 104 -

10.1.1 Machine Coordinate System M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 : Coordinate system selection G90 : 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 which is effective only in the block where it is assigned. The workpiece coordinate system being selected is not changed by this command.

1st reference position

Workpiece coordinate system 1

Machine coordinate system (G53)

G53 G90 G00 X0 Y0 ;

M

W1

10 Coordinate System 10.1 Coordinate System Type and Setting

- 105 -

10.1.2 Coordinate System Setting M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

Machine position

Example where W1 is shifted to new W1 when the machine was at the position (x0, y0) above W1 and the G92 Xx1 Yy1; command was assigned when the workpiece coordinate system W1 is modal (external workpiece coordinate system offset = 0; interrupt amount offset = 0)

y0 W1

Machine coordinate system

M

G92 offset amount

Offset of coordinate system by G92 coordinate system setting

x1

y1

X : x0x1 Y : y0y1

x0

New W1

The shifted coordinate system is returned to its original position by dog-type reference position return or the program.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 106 -

When the coordinate system setting is commanded by G92, all the workpiece coordinate systems from G54 through G59 referenced to the machine coordinate system undergo a shift.

Coordinate system created by automatic coordinate system setting

Coordinate system after coordinate system setting by G92

G92 Xx1 Yy1

Machine coordinate system

W1

M

x y'

G92 command position

Old W1

New W1

M

x1

Machine coordinate system

y1

Tool position

1. All the workpiece coordinates from G54 to G59 move in parallel. 2. There are two ways to return a shifted coordinate system to its original position.

a) 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 system 3. Local coordinate systems created under G54 to G59 workpiece coordinate systems

The distances from the zero point of G53 machine coordinate system are set to the controller coordinate related parameters.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 107 -

10.1.4 Workpiece Coordinate System Selection (6 sets) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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) : (Absolute value command) G54 : 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 using the setting and display unit 2.Setting using commands assigned from the machining program 3.Setting from the user PLC

W2

W3W4

Workpiece coordinate system 1 (G54)

Workpiece coordinate system 2 (G55)

Machine coordinate system (G53)

W1

M

Start

G90 G56 G00 X0 Y0 ;

Workpiece coordinate system 4 (G57)

Workpiece coordinate system 3 (G56)

10 Coordinate System 10.1 Coordinate System Type and Setting

- 108 -

10.1.5 Extended Workpiece Coordinates System Selection (48 Sets) G54 1P1 to P48 Extended workpiece coordinate system selection (48 sets) G54. 1P1 to P48

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 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 ;

(G90) : (Absolute value command) G54.1Pn : Coordinate system selection G00 : Movement mode Xx1, Yy1, Zz1 : Coordinate positions of movement destination

The numerical value n of P following G54.1 indicates each workpiece coordinate system. Specify a value between 1 and 48. The workpiece coordinate zero points are provided as distances from the zero point of the machine coordinate system. Settings can be performed in one of the following three ways:

1.Setting using the setting and display unit 2.Setting using commands assigned from the machining program 3.Setting from the user PLC

(Note) While the G54.1Pn (extended workpiece coordinate system selection) is modal, the local coordinate offset is reduced to zero, and the G52 command cannot be used.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 109 -

10.1.6 Workpiece Coordinate System Preset (G92.1) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 the such operations or the 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 which has been shifted once to the workpiece coordinate system which 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 0 ; (where 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.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 110 -

10.1.7 Local Coordinate System M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

G code Function G54 G52 Local coordinate system on the workpiece coordinate system 1 G55 G52 Local coordinate system on the workpiece coordinate system 2 G56 G52 Local coordinate system on the workpiece coordinate system 3 G57 G52 Local coordinate system on the workpiece coordinate system 4 G58 G52 Local coordinate system on the workpiece coordinate system 5 G59 G52 Local coordinate system on the workpiece coordinate system 6

The command format of the local coordinate system is given below.

(G54) G52 Xx1 Yy1 Zz1 ;

(G54) : Workpiece coordinate system selection G52 : Local coordinate system setting Xx1, Yy1, Zz1 : Local coordinate offset amount

The local coordinate zero points are provided as distances from the zero point of the designated workpiece coordinate system (local coordinate offset). In the incremental value mode, the position obtained by adding the local coordinate offset amount to the previously specified offset amount serves as the new local coordinate zero point. If no workpiece coordinates are designated, the local coordinates will be created on the currently selected workpiece coordinates. This command is unmodal but the local coordinate system created by G52 is valid until the next G52 command is issued. The local coordinate system is canceled by the input of the reset signal or by manual or automatic dog-type reference position return.

W1

x1

L1

Workpiece coordinate 1 (G54)

Machine coordinate system (G53)

Local coordinate G54 G52

y1

M

10 Coordinate System 10.1 Coordinate System Type and Setting

- 111 -

10.1.8 Coordinate System for Rotary Axis M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The coordinate system of rotary axis ranges from 0 to 360. Note that, however, it can be displayed from 0 to 359.999. In absolute value command mode, the rotary axis can make a turn or less (not greater than 360). The turning direction depends on the specified sign. A negative sign () turns the axis in the negative direction and a positive sign (+) turns it in the positive (+) direction. Note that a parameter can be used to move the axis to the end point taking a short cut. In incremental value command mode, the rotary axis moves the specified distance only.

10.1.9 Plane Selection M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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. ; With these program commands, X100. is the axis which does not exist on the G19 (Yp, Zp) plane, Yp-Zp are selected by G19 and the X axis moves by 100. mm separately from the plane selection.

G17 X100. R50. ; With these program commands, the Xp-Yp plane is selected by G17 and the arc command is controlled on the X-Y plane by this command.

10 Coordinate System 10.1 Coordinate System Type and Setting

- 112 -

10.1.10 Origin Set M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Using the setting and display unit, the coordinate system (current position and workpiece coordinate position) can be set to "0" by operating the screen. This function is the same as the coordinate system setting command " G92 X0 (Y0 or Z0) ; ".

[POSITION] [WORK(G54)]

[POSOTION] [WORK(G54)] X -150.345 X -150.345 X 0.000 X 0.000 Y - 12.212 Y - 12.212 Y 0.000 Y 0.000 Z - 1.000 Z - 1.000 Z 0.000 Z 0.000 A - 0.000 A - 0.000 A 0.000 A 0.000

X

C.B CAN

Y

C.B CAN

Z

C.B CAN

When axes are set to "0" in order, the Y and Z axis can be set by pressing

C.B CAN key successively

without pressing

Y and

Z keys.

10.1.11 Counter Set M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Using the setting and display unit, the position counter display can be change to "0" by operating the screen. (1) This operation is the same as the operation of "Origin Set", but press

INPUT key instead of

C.B CAN

key. (2) Only the [POSITION] counter display is changed to "0", and the other coordinate system counter

displays are not changed.

10 Coordinate System 10.2 Return

- 113 -

10.2 Return

10.2.1 Manual Reference Position Return M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables the tool to be returned manually to the position (reference position) which is characteristic to the machine.

(1) Return pattern to reference position

(a) Dog type

When starting in same direction When starting in opposite direction as final advance direction as final advance direction

(b) High-speed type

Reference position return speed

Dog Dog

R

1

R

Creep speed

Dog

Rapid traverse rate

R

(2) Differences according to detection method First return after power ON Second return and following Incremental position detection method Dog-type High-speed

Absolute position detection method High-speed High-speed

10 Coordinate System 10.2 Return

- 114 -

10.2.2 Automatic 1st Reference Position Return M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Function G28 Automatic 1st reference position return G29 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 ;

G28 : Return command Xx1, Yy1, Zz1 : Return control axes (interim point)

Each axis is first positioned by rapid traverse to the position (interim point) assigned for the assigned axis and then is returned independently to the 1st reference position. The G29 programming format is given below. G29 Xx1 Yy1 Zz1 ;

G29 : Return command Xx1, Yy1, Zz1 : Return control axes (assigned position)

The tool is first moved by rapid traverse to the interim position which is passed through with G28 or G30, and is then positioned by rapid traverse at the position assigned by the program.

Interim point

1st reference point R

Y

Non - interpolation movement

G29

G28

G28

G29

X

Interpolation or non - interpolation can be selected

Interpolation or non interpolation can be selected

10 Coordinate System 10.2 Return

- 115 -

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.

10 Coordinate System 10.2 Return

- 116 -

10.2.3 2nd, 3rd, 4th Reference Position Return M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Function G30 P2 2nd reference position return G30 P3 3rd reference position return G30 P4 4th reference position return

The G30 programming format is given below. G30 Xx1 Yy1 Zz1 Pp1 ;

G30 : Return command Xx1, Yy1, Zz1 : Return control axes (interim point) Pp1 : Return position No.

The tool is first positioned by rapid traverse to the interim point commanded for the assigned axis and then is returned independently to the reference position.

G30 P2

Interim point

1st reference point 2nd reference point

Start point

4th reference point

3rd reference point

G30 P3

G30 P4

X

Y

(Note 1) The second reference position return is performed if the P address 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.

10 Coordinate System 10.2 Return

- 117 -

(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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 ;

G27 : Verification command Xx1, Yy1, Zz1 : Return control axes Pp1 : Verification 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.

10 Coordinate System 10.2 Return

- 118 -

10.2.5 Absolute Position Detection M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The absolute position detection function holds the relation of the actual machine position and the machine coordinates in the controller with a battery even when the power is turned OFF. When the power is turned ON again, automatic operation can be started without executing reference position return. (High-speed return will always be used for the reference position return command.) For the absolute position detection method, there are two method such as the dog-type and dog- less type according to how the zero point is established.

Method Details Establishment of zero point

Adjustment of zero point position

Dog-type Same method as incremental detection dog-type

Zero point is established with dog- type reference position return completion.

The data is set in the parameter of zero point shift amount.

Dog-less type

Marked point method

The zero point position is set from the screen.

The zero point is established by input from the zero point initialization screen.

The value equivalent to the shift amount is set in the zero point initialization screen.

Machine stopper method

The zero point is established by pressing the machine against a set point on the machine.

The zero point is established when a torque limit is applied on the servo and the torque limit is reached by pressing against the machine stopper.

The value equivalent to the shift amount is set in the zero point initialization screen.

Diagnosis during absolute position detection (1) The machine position at power OFF and ON can be confirmed on the absolute position monitor

screen. (2) If the amount that the axis is moved during power OFF exceeds the tolerable value (parameter),

a warning signal will be output. (3) An alarm will be output if the absolute position information is lost. (4) An alarm will be output if the voltage of the battery for backing up the absolute position data

drops.

10 Coordinate System 10.2 Return

- 119 -

10.2.6 Tool Exchange Position Return M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

By specifying the tool change position in a parameter and also assigning a tool exchange 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] Command Return order

G30.1 Z axis X axis Y axis ( additional axis) G30.2 Z axis X axis Y axis ( additional axis) G30.3 Z axis Y axis X axis ( additional axis) G30.4 X axis Y axis Z axis ( additional axis) G30.5 Y axis X axis Z axis ( additional axis) G30.6 X axis Y axis Z axis ( additional axis)

[L system]

Command Return order G30.1 X axis only ( additional axis) G30.2 Z axis only ( additional axis) G30.3 X axis Z axis ( additional axis) G30.4 Z axis X axis ( additional axis) G30.5 X axis Z axis ( additional axis)

(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" indicate 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 exchange 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.

10 Coordinate System 10.2 Return

- 120 -

10.2.7 C Axis Reference Position Return M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function is used to carry out the position control for the spindle with the axis motor, and applied to the machine which 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.

Reference position return method Dog type (with C axis detector)

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.

(1) (2) (3) (4)

Base shift amount (one rotation of spindle)

G28sft

G28rap G28rap

Spindle encoder Z-phase pulse

G28crp

Figure 1 Z-phase pulse type reference position return

10 Coordinate System 10.2 Return

- 121 -

Spindle

(1)

(2)

(3)

Spindle

(1)(2)

(3)

(a) (b)

(1) G28rap (2) G28crp (3) G28rap

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

11 Operation Support Functions 11.1 Program Control

- 122 -

11 Operation Support Functions 11.1 Program Control

11.1.1 Optional Block Skip M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 ON Switch OFF

N7

N6

/N5

/N4

N3

N2

N1 N1

N2

N3

N4

N5

N6

N7

N1

N2

N3

N6

N7

11 Operation Support Functions 11.1 Program Control

- 123 -

11.1.3 Single Block M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

G01 Z1000G01 Z100

SBK changeSBK ON at start

G01 X1000

INVALID

Single block (SBK)

Automatic operation

Movement block

start (ST)

during movement

VALID VALID

SBK ON after block completion

~ ~ ~ ~

~ ~

~ ~ ~ ~

As with the multi-part system specification, the following function can be selected instead. Multi-part system single block (L system) This function is for executing single block operation while maintaining the synchronization

between the part systems when two or more part systems are operated. When one part system has been stopped by single block stop, the other part systems are stopped by feed hold.

11 Operation Support Functions 11.2 Program Test

- 124 -

11.2 Program Test

11.2.1 Dry Run M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

Command Manual rapid traverse selector switch OFF

Manual rapid traverse selector switch ON

G00, G27, G28, G29, G30, G60 Manual feed rate Rapid traverse rate G01, G02, G03 Manual feed rate Cutting clamp speed

11.2.2 Machine Lock M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When the machine lock input signal is set to ON, the NC operations can be executed without assigning commands to the NC axes. 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.

11 Operation Support Functions 11.2 Program Test

- 125 -

11.2.3 Miscellaneous Function Lock M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 which are executed only inside the controller and not output (M96, M97, M98, M99) are executed as they would be normally even if this signal is ON.

11.2.4 Graphic Check M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 3- dimensional 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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 3- dimensional display mode, cubic shapes can be rotated and tracing of the figure seen from the desired direction can be assigned.

11 Operation Support Functions 11.3 Program Search / Start / Stop

- 126 -

11.3 Program Search / Start / Stop

11.3.1 Program Search M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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. Machining programs are stored in the memory inside the NC system.

11 Operation Support Functions 11.3 Program Search / Start / Stop

- 127 -

11.3.3 Collation Stop M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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.

O100 N101

O100 N102

1

1

123

654

Start Operation procedure

Set collation stop in O100 N101.

Auto start

Collation stop upon completion of O100 N102 positioning

Measure and check the machining shape of the first

Machining OK? OK NG

Yes

Set collation stop again.

Restart

Machining resumes from previous collation stop position.

Collation stop at block in which collation stop has been set.

Measure and check the machining shape?

No

Check subsequent machining shapes?

Restart

Machining resumes from previous collation stop position.

Reset

Modify machining conditions (tool length offset amount, etc.).

Re-check machining shape?

Auto start

Machining starts from the machining shape of the first work.

End

11 Operation Support Functions 11.3 Program Search / Start / Stop

- 128 -

11.3.4 Program Restart M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 the case of the standard specification, the program No. cannot be omitted.

(b) Type B 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 sub-

programs) 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 which 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 the case of the standard specification, the program No. cannot be omitted.

(b) Type B 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 which 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.

11 Operation Support Functions 11.3 Program Search / Start / Stop

- 129 -

11.3.5 Automatic Operation Start M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With the input of the automatic operation start signal (change from ON to OFF), the automatic operation of the program that has been operation searched is started by the controller (or the halted program is restarted).

Automatic operation start (ST)

Movement block G01 X 100... G01 Z 100...

Automatic operation startup is performed on a part system by part system basis.

11.3.6 NC Reset M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables the controller to be reset. Reset 1 Reset 2 Reset & Rewind 1 G command modals Retained Initialized Initialized

2 Tool compensation data Retained Canceled (no operations)

Canceled

3 Memory indexing Executed Not executed Executed 4 Errors/alarms Reset Reset Reset 5 M, S and T code outputs Retained Retained Retained

6 M code independent output

OFF OFF OFF

7 Control axis moving Decelerated and stopped

Decelerated and stopped

Decelerated and stopped

8 Output signals "In reset" signal "In reset" signal "In reset" signal "In rewind" signal

11 Operation Support Functions 11.3 Program Search / Start / Stop

- 130 -

11.3.7 Feed Hold M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

11 Operation Support Functions 11.4 Interrupt Operation

- 131 -

11.4 Interrupt Operation

11.4.1 Manual Interruption M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Manual interrupt is a function that enables manual operations to be performed during automatic operation. The systems used to select the operation mode are as follows: System which initiates the interrupt by switching from the automatic mode to manual mode System which initiates the interrupt by selecting the manual mode at the same time as the

automatic mode (Refer to "11.4.9 Simultaneous Operation of Manual and Automatic Modes".) Whether the manual interrupt amount is to be retained and automatic operation is to be continued is determined by setting manual absolute mode ON or OFF (refer to "11.4.3 Manual Absolute Mode ON/OFF").

11 Operation Support Functions 11.4 Interrupt Operation

- 132 -

11.4.2 Automatic Operation Handle Interruption M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 automatic operation. If the spindle load is greatly exceeded when cutting a workpiece as per the machining program due to a high rough cutting amount in face machining, for instance, automatic handle interrupt makes it possible to raise the Z surface and reduce the load easily without suspending feed in the automatic operation mode. Automatic handle interrupt is conducted by setting the "automatic handle interrupt" valid switch which is provided separately from the "manual operation mode". The axis selection and pulse scale factor operation are conducted as for manual handle feed. Whether, after an interrupt, to return to the path of the machining program by automatic operation or remain offset by the amount equivalent to the interrupt amount is determined using a parameter.

Tool

Workpiece

Automatic feed

Handle feed

G01 Z _ F X _ Y _ ; X _ Y_ ; Z _ Y _ ;

Interrupt

100 10 1

Z Y X

~ ~

Feed path with automatic feed and handle feed superimposed

11 Operation Support Functions 11.4 Interrupt Operation

- 133 -

11.4.3 Manual Absolute Mode ON / OFF M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The program absolute values are updated by an amount equivalent to the distance by which the tool is moved by hand when the manual absolute selection input signal is turned ON. In other words, the coordinate system based on the original program will not shift even if the tool (machine) is moved by hand. Thus, if automatic operation is started in this case, the tool will return to the path before manual movement.

W

Y

X

With manual absolute switch ON

Tool passes along same path as that programmed.

Path after manual interrupt

(Program absolute value is updated by an amount equivalent to traveled value.)

Manual interrupt

Feed hold stop Programmed path (absolute value command)

Path is shifted by an amount equivalent to manual interrupt value. (Zero point moves.)

(Program absolute value is not updated by an amount equivalent to traveled value.)

Programmed path (absolute value command)

Manual interrupt

Path after manual interrupt

Feed hold stop

With manual absolute switch OFF

W

Y

X

The switch ON state will be entered when the power is turned ON.

11 Operation Support Functions 11.4 Interrupt Operation

- 134 -

11.4.4 Thread Cutting Cycle Retract M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function suspends the thread cutting cycle if a feed hold signal has been input during thread cutting in a thread cutting cycle. If a feed hold signal is input during chamfering or thread cutting without chamfering, operation stops at the position where the block following the thread cutting is completed.

Period when thread cutting is performed

Feed hold

Suspension position

Chamfering angle

Position where the block following the thread cutting is completed

11 Operation Support Functions 11.4 Interrupt Operation

- 135 -

11.4.5 Tapping Retract M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

11 Operation Support Functions 11.4 Interrupt Operation

- 136 -

11.4.6 Manual Numerical Value Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

On the screen of the setting and display unit, the M, S and T (and B when 2nd miscellaneous function is valid) commands can be executed by setting numerical values and pressing [INPUT]. This enables operations such as spindle speed changing, starting, stopping, calling and selecting assigned tools and replacing of the spindle tools to be done easily without having to prepare or revise the machining program. Even in an automatic operation mode, these operations can be conducted with block stop. Furthermore, the M and T commands can be issued even on the tool offset amount setting and display screen, therefore at the manual tool length measurement, the tools can be called successively to the spindle and measured very simply without having to change the screen page.

T 12

S 3600

M 5

Manual numerical

value T command value

S command value

Input

3

6

0

2

5

9 8

1

4

7

T

S

M

M command value

PLC sequence processing

(Note) The input operation starts the execution of the M, S or T command.

11.4.8 MDI Interruption M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

11 Operation Support Functions 11.4 Interrupt Operation

- 137 -

11.4.9 Simultaneous Operation of Manual and Automatic Modes M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

Automatic operation

X

Y

Z

X-axis posi-tion control

X

Y

Z

Tape

Memory

MDI

Jog

Handle

Return Manual mode

Automatic mode

Simultaneous manual and automatic operation

Axis control

Manual operation

Axis control

Y-axis posi-tion control

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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When executing the jog feed and handle feed, both these feeds are available without changing the mode each time by inputting the jog mode signal and simultaneous operation of jog and handle modes signal to the control unit. However, during moving in one of the two modes, the feed in the other mode is not valid.

11 Operation Support Functions 11.4 Interrupt Operation

- 138 -

11.4.11 Reference Position Retract M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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). (1) Other operations

(a) When the retract signal is turned ON, the control unit is reset, the operation is interrupted, and the machining program is indexed.

(b) When the rapid traverse input signal is input, the rapid traverse rate is applied. When the rapid traverse input signal is not input, the manual feed rate is applied.

(c) If the retract signal is input during execution of a tapping cycle, the operation will be the tapping retract, and the normal reference 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 can not be resumed.

(f) The retract signal is invalid if the coordinate system is not established. An operation error will occur when the retract signal is input in such case.

11.4.13 Skip Retract M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function is used to return to the opposite advance direction when the skip signal is input during G31 command.

11.4.14 PLC Interruption M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

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.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 139 -

12 Program Support Functions 12.1 Machining Method Support Functions

12.1.1 Program

12.1.1.1 Subprogram Control M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

L system 8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

8 layers

When the same pattern is repeated during machining, the machining pattern is registered as one subprogram and the subprogram is called from the main program as required, thereby realizing the same machining easily. Efficient use of program can be made. The call is designated with the program number and sequence number. M98 Pp1 Hh1 Ll1 ;

M98 : Call command Pp1 : Subprogram number Hh1 : Sequence number Ll1 : Number of repetitions

(Branch to subprogram) Op1 (Subprogram) : Nh1 : M99 ; (Return to main program)

Subprograms can be nested up to eight levels deep.

M99;

M98 P2

M99;

M98 P3; M99;

P1000 P2 P8

P1

Main program: Level 0 (P1000)

Main program: Level 1 (P1)

Main program: Level 2 (P2) Main program:

Level 8 (P8)

M02/M30 ;

M98 P1

8- le

ve l n

es tin

g

12 Programming Support Functions 12.1 Machining Method Support Functions

- 140 -

A subprogram branch destination or repetition of a subprogram can be specified.

Subprogram

Specifying a subprogram branch destination

Five repetitions

Return after five repetitions

Main program Main program Subprogram

Specifying repetition of a subprogram

P1000 P1 P1 P1000

M98 P1 H1;

M98 P1 H100;

M02/M30;

N1;

M99;

N100;

M99;

M98 P1 L5;

M02/M30;

M99;

12 Programming Support Functions 12.1 Machining Method Support Functions

- 141 -

12.1.1.3 Scaling M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 value within the range assigned by the scaling command.

G code Function

G50 G51

Scaling cancel Scaling ON

The program format is given below. G51 Xx1 Yy1 Zz1 Pp1 ;

G51 : Call command Xx1, Yy1, Zz1 : Scaling center coordinates Pp1 : Scale factor

The scale factor ranges from 0.000001 to 99.999999 times.

sc s1

s3 s2

p2

p1

p3

Y

Xx1

y1 sc : Scaling center p1,p2,p3 : Programmed shape s1,s2,s3 : Shape after scaling

(Note 1) Scaling cannot be applied to tool radius compensation, tool position offset, tool length offset or to other such offset amounts.

(Note 2) Scaling applies only to those axes among X, Y and Z which have been commanded; it does not apply to axes which have not been commanded. When the scale factor is not assigned, the parameter setting applies instead.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 142 -

12.1.2 Macro Program

12.1.2.1 User Macro M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

L system 4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

4 layers

(1) Macro commands (1) ; G65 to G67 In order to carry through one integrated function, a group of control and arithmetic instructions

can be used and registered as a macro program. Furthermore, subprograms with a high degree of expandability can be configured by setting these macro programs as types which are capable of conducting control and arithmetic operations using variable commands.

G code Function

G65 Macro call (Sample call) G66 Macro modal call A

G66.1 Macro modal call B G67 Macro modal call cancel

The program formats are given below.

G65 Pp1 Ll1 Argument ;

G65 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment

The macro program is called immediately by this command.

G66 Pp1 Ll1 Argument ;

G66 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment

The macro program is executed from the block with the axis command following this command.

G66.1 Pp1 Ll1 Argument ;

G66.1 : Call command Pp1 : Program No. Ll1 : No. of repetitions Argument : Variable data assignment

The macro program is executed with the word data of each block as the argument.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 143 -

The following macro command functions are available.

Arithmetic commands

#1 = ; Various arithmetic operations can be conducted between variables by the above. " " is a combination of constants, variables, functions and operators.

Assignment of priority of arithmetic operations

The portion in which the operator is to be given priority can be enclosed in [ ]. Up to five pairs of square parentheses [ ] including the function [ ] can be used. The normal priority of operation is functions and multiplication/division followed by addition/subtraction.

Control commands

(1) IF [ ] GOTO n ; (2) WHILE [ ] 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 ;

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]

12 Programming Support Functions 12.1 Machining Method Support Functions

- 144 -

(b) Macro call using miscellaneous commands (M, S, T, B code macro call) Simply by designating an M (or S, T, B) code, it is possible to call user macro programs

with the prescribed program number. (Entered M codes and all S, T and B codes can be used.)

Mm ; (or Ss;, Tt;, Bb;)

Mm (Ss, Tt, Bb) : M (or S, T, B) code for performing macro call

The correspondence between the Mm code which performs macro call and the program number for the macro to be called is set by a parameter. Up to 10 M codes from M00 to M95 can be entered.

Select codes to be entered which are not the codes basically required by the machine and which are not M codes M0, M1, M2, M30 and M96 through M99.

(Note 1) G commands in G code macro programs are not subject to macro calls but normal G

commands. M commands in M code macro programs are not subject to macro calls but normal M commands. (The same applies to S, T and B codes.)

(Note 2) The registration of the program number used for calling the G code macro or M code macro can be done independently for each system. [M system]

12.1.2.2 Machine Tool Builder Macro

12.1.2.2.1 Machine Tool Builder Macro SRAM M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 : Machine builder macro program number (0100001000 0199999998) l : 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

12 Programming Support Functions 12.1 Machining Method Support Functions

- 145 -

12.1.2.3 Macro Interruption M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

M02 ;

M97 ;

M96Ppi;

: :

: : : : : : :

: : : : : : : :

: : : : : : : :

The user macro interrupt signal is accepted during this period.

The user macro interrupt signal is not accepted during this period. The modal information is restored

to the status applying before interrupt.

Interrupt program Opi

Machining program Opm:

Interrupt signal

M99 ;

12 Programming Support Functions 12.1 Machining Method Support Functions

- 146 -

12.1.2.4 Variable Command Programming can be given flexible and general-purpose capabilities by designating variables instead of directly assigning numbers for addresses in programs and by supplying the values of those variables as required when running the programs. Arithmetic operations (adding, subtracting, multiplying and dividing) can also be conducted for the variables.

Number of variable sets specifications The numbers of common variable sets depend on the options, and are as follows.

Number of variable sets specifications

100 sets #100 ~ #149, #500 ~ #549 200 sets #100 ~ #199, #500 ~ #599 300 sets #100 ~ #199, #500 ~ #699 600 sets #100 ~ #199, #500 ~ #999 S

ys te

m 1

700 sets #100 ~ #199, #400 ~ #999 50 + 50 sets #100 ~ #149 (per part system), #500 ~ #549 (common to part system) 100 + 100 sets #100 ~ #199 (per part system), #500 ~ #599 (common to part system) 100 + 400 sets #100 ~ #199 (per part system), #500 ~ #899 (common to part system)

S ys

te m

2

100 + 500 sets #100 ~ #199 (per part system), #500 ~ #999 (common to part system)

Variable names can be set for #500 ~ #519.

Variable expressions Variable : # Numerical value #100 (Numerical value: 1, 2, 3, .....)

: # [Expression] #100 Expression :Numerical value

: Variable : Expression Operator Expression #100 + #101 : (minus) Expression #120 : [Expression] [#110] : Function [Expression] SIN [#110]

Variable definition Variable = expression (Note 1) Variables cannot be used with addresses "O" and "N".

12.1.2.4.1 100 sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.2 200 sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12 Programming Support Functions 12.1 Machining Method Support Functions

- 147 -

12.1.2.4.3 300 sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.4 600 sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.5 700 sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.6 (50+50 x number of part systems) sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.7 (100+100 x number of part systems) sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.8 (200+100 x number of part systems) sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.9 (400+100 x number of part systems) sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12.1.2.4.10 (500+100 x number of part systems) sets M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

12 Programming Support Functions 12.1 Machining Method Support Functions

- 148 -

12.1.3 Fixed Cycle

List of fixed cycles M system L system

Type of fixed cycle G code system

1

G code system

2

G code system

3

G code system

6

G code system

7

Remarks

G70 G80 G80 G80 G80 : : : : :

G89 G89 G89 G89 G89 G79 G83.2 G79 G83.2

G98 G98 G98 G98 G98

Fixed cycle for drilling

G99 G99 G99 G99 G99

Refer to 12.1.3.1. Refer to 4.5.3.

G34 G35

Special fixed cycles

G36

Refer to 12.1.3.2.

G90 G77 G90 G77 G92 G78 G92 G78

Fixed cycles for turning machining

G94 G79 G94 G79

Refer to 12.1.3.3.

G70 G70 G70 G70 : : : : G76 G76 G76 G76 G76.1 G76.1 G76.1 G76.1

Multiple repetitive fixed cycles for turning machining

G76.2 G76.2 G76.2 G76.2

Refer to 12.1.3.4. Refer to 12.1.3.5. Refer to 4.5.8.

Small-diameter deep- hole drilling cycle

G83 Refer to 12.1.3.6.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 149 -

12.1.3.1 Fixed Cycle for Drilling M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 cycle G74 Reverse tapping cycle G75 G76 Fine boring G77 G78 G79 G80 Fixed cycle cancel G81 Drilling, spot drilling cycle G82 Drilling, counterboring cycle G83 Deep hole drilling cycle G84 Tapping cycle G85 Boring cycle G86 Boring cycle G87 Backboring cycle G88 Boring cycle G89 Boring cycle

There are two levels of hole machining axis return which apply upon completion of the fixed

cycle machining operation.

G code Function

G98 Initial point level return G99 R point level return

12 Programming Support Functions 12.1 Machining Method Support Functions

- 150 -

The basic program format for the fixed cycle commands is shown below. G81 Xx1 Yy1 Zz1 Rr1 Qq1 Pp1 Ll1 Ff1 ;

G81 : Hole drilling mode Xx1, Yy1 : Hole position data; X-axis, Y-axis hole drilling position command

(rapid traverse) (incremental/absolute) Zz1 : Hole machining data; Hole bottom position designation (incremental/absolute) Rr1 : Hole machining data; Hole R point designation (incremental/absolute) Qq1 : Hole machining data; Depth of cut per pass in G73, G83 cycle (incremental)

Shift amount in G76, G87 cycle Depth of cut per pass in pecking tapping, deep hole tapping of G74, G84 cycle

Pp1 : Hole machining data; Dwell time at hole bottom Ll1 : Hole machining data; Number of fixed cycle repetitions Ff1 : Cutting feed rate

For details on the synchronous tapping cycle (including pecking tapping cycle and deep-hole tapping cycle), refer to the section "4.5.3 Synchronous Tapping".

12 Programming Support Functions 12.1 Machining Method Support Functions

- 151 -

G73

Step cycle

nq

q

R point

G98 mode

Initial point

G99 mode

Z point

G74 Reverse tapping cycle

M03

M04

Initial point

R point

Z point

G98 mode

G76 Fine boring cycle

q

q

M19 Shift

qInitial point

R point

Z point

G98 mode

G99 mode

G81 Drilling, spot drilling cycle

Initial point

R point

Z point

G98 mode

G99 mode

G82 Drilling, counterboring

cycle

Dwell

Initial point

R point

Z point

G98 mode

G99 mode

G83 Deep hole drilling

cycle

Initial point

n

q

q R point

Z point

G98 mode

G99 mode

G84 Tapping cycle

Initial point

R point

Z point

G98 mode

M03

M04

G85 Boring cycle

Initial point

R point

Z point

G98 mode

G86 Boring cycle

Initial point

R point

Z point

G98 mode M03

M03

M05

G87 Back boring cycle

Initial point

R point M19

Z point M03

M19

G88 Boring cycle

Initial point

R point

Z point G98 mode

M03

M03

M05 Dwell

G89 Boring cycle

Dwell

Initial point

R point

Z point

G98 mode

12 Programming Support Functions 12.1 Machining Method Support Functions

- 152 -

(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

G83 Z Cutting feed Intermittent feed

In-position check Dwell

Rapid traverse feed

Deep-hole drilling cycle1

G84 Z Cutting feed In-position check Dwell Spindle CCW

Cutting feed Tapping cycle (Reverse tapping cycle)

G85 Z Cutting feed In-position check Dwell

Cutting feed Boring cycle

G87 X Cutting feed Intermittent feed

In-position check Dwell

Rapid traverse feed

Deep-hole drilling cycle1

G88 X Cutting feed In-position check Dwell Spindle CCW

Cutting feed Tapping cycle (Reverse tapping cycle)

G89 X Cutting feed In-position check Dwell

Cutting feed Boring cycle

G83.2 Z/X Cutting feed Intermittent feed

In-position check Dwell

Rapid traverse feed

Deep-hole drilling cycle2

The fixed cycle mode is canceled when a G command of the G80 or G01 group is specified. Data is

also cleared simultaneously.

Command format

G83/G84/G85 Xx1 Cc1 Zz1 Rr1 Qq11 Pp1 Ff1 Kk1 (Mm1) Ss1 ,Ss1 Dd1 ,Rr1 ; G87/G88/G89 Xx1 Cc1 Zz1 Rr1 Qq11 Pp1 Ff1 Kk1 (Mm1) Ss1 ,Ss1 Dd1 ,Rr1 ;

G83/G84/G85 : Fixed cycle mode of drilling (G83, G87), tapping (G84, G88), or boring (G85, G89)

G87/G88/G89 The drilling command is modal. Once it is given, it is effective until another drill command is given or drilling fixed cycle cancel command is given.

Xx1, Cc1 : Data for positioning X (Z) and C axes The data is unmodal. To execute the same hole machining mode

consecutively, specify the data for each block. Zz1, Rr1, Qq11, Pp1, Ff : Actual machining data in machining Only Q is unmodal. Specify Q in G83 or G87 for each block whenever

the data is required. Kk1 : To repeat in a single cycle for hole machining at equal intervals, specify

the number of repetitions in the range of 0 to 9999 (no decimal point can be used). It is unmodal and is effective only in the block in which the number of repetitions is specified.

If the number of repetitions is omitted, K1 is assumed to be specified. If K0 is specified, hole machining data is stored, but hole machining is

not performed. Hole machining data; R point position (incremental value from initial point) designation (sign ignored)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 153 -

Mm1 : If axis C clamp M command (parameter setting) is given, the M code is

output at the initial point, and after return motion, C axis unclamp M code (clamp M code + 1) is output and the dwell time set in a given parameter is executed.

Ss1 : Designates spindle rotation speed ,Ss1 : Designates spindle rotation speed of return Dd1 : Designates tap spindle NO. for G84 (G88) ,Rr1 : Changes between synchronous/asynchronous in G84 (G88)

The drilling cycle motions generally are classified into the following seven.

Motion 1 Motion 1

Motion 4

Motion 3

Motion 5

Motion 6

Motion 7

R point

Initial point

Motion 1 : Rapid positioning up to the initial point of X (Z) and C axes. If the "positioning axis in-position width" is designated, the in-position check is

conducted upon completion of the block. Motion 2 : Output if the C axis clamp M code is given. Motion 3 : Rapid positioning up to the R point. Motion 4 : Hole machining at cutting feed. If the "drilling axis in-position width" is designated, the in-position check is conducted

upon completion of the block. However, in the case of deep-hole drilling cycles 1 and 2, the in-position check is not conducted with the drilling of any holes except the last one. The in-position check is conducted at the commanded hole bottom position (last hole drilling).

Motion 5 : Motion at the hole bottom position. It varies depending on the fixed cycle mode. Spindle CCW (M04), spindle CW (M03), dwell, etc., are included.

Motion 6: Return to the R point. Motion 7: Return to the initial point at rapid traverse feed. (Operations 6 and 5 may be conducted as a single operation depending on the fixed cycle mode. Note: With a synchronous tap command, the in-position check is conducted in accordance with the

parameters. Whether the fixed cycle is complete with motion 6 or 7 can be specified by using either of the following G commands: G98: Initial level return G99: R point level return These commands are modal. For example, once G98 is given, the G98 mode is entered until G99 is given. The G98 mode is entered in the initial state when the controller is ready.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 154 -

Deep-hole drilling cycle (G83, G87)

G83/G87 Deep-hole drilling cycle (G83: Z-axis direction, G87: X-axis direction)

When Q command is given When Q command is not given

Z / X point

G99 mode G98 mode

n

q q

R point Initial point

Z point / X point R point

Initial point

G99 mode G98 mode

G83.2 Deep-hole drilling cycle

Z / X point

Dwell

Dwell

Dwell

Dwell

Dwell

Dwell

Dwell

G84/88 Tapping cycle

Z / X point

R point Initial point

G98 mode

Reverse rotation of spindle/rotary tool

(C-axis clamp)

(C-axis unclamp) Forward rotation of spindle/rotary tool

Output or no output can be set using a parameter for the C-axis clamp/unclamp M code

G85/89 Boring cycle

f

2f

Z / X point

R point Initial point

G98 mode

(C-axis clamp)

(C-axis unclamp)

Dwell

Dwell

Output or no output can be set using a parameter for the C-axis clamp/unclamp M code

There are two levels of hole machining axis return which apply upon completion of the fixed cycle machining operation. (see the figure above)

G code Function G98 Initial point level return G99 R point level return

12 Programming Support Functions 12.1 Machining Method Support Functions

- 155 -

12.1.3.2 Special Fixed Cycle M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 with the X axis on the circumference of a circle with radius R whose center is the coordinates designated by X and Y, and it drills "n" number of holes at "n" equal intervals along the circumference of that circle. The drilling data for the standard fixed cycle of the G81 or other such command is retained for the drilling operation at each hole position. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G34 command. G34 Xx Yy Ir J Kn ; Xx, Yy : Center position of bolt hole circle; this is affected by the G90/G91 commands. Ir : Radius "r" of circle; it is based on the least input increment and is provided using a

positive number. J : Angle at point to be drilled initially; the counterclockwise direction is taken to be

positive. Kn : Number "n" of holes to be drilled; any number of holes from 1 through 9999 can be

designated; 0 cannot be assigned. When 0 has been designated, the alarm will occur. A positive number provides

positioning in the counterclockwise direction; a negative number provides positioning in the clockwise direction.

(Example) With 0.001mm least input increment

Position prior to excution of G34 command

G0 command in N005

N001 G91 ; N002 G81 Z 10.000 R5.000 L0 F200 ; N003 G90 G34 X200.000 Y100.000 I100.000 J20.000 K6 ; N004 G80 ; .........................(G81 cancel) N005 G90 G0 X500.000 Y100.000 ;

(500 mm, 100 mm)

20

n = 6 holes

I = 100 mm

X1 = 200 mm

Y1 = 100 mm

W

As shown in the figure, the tool is positioned above the final hole upon completion of the G34 command. This means that when it is to be moved to the next position, it will be necessary to calculate the coordinates in order to issue the command or commands with incremental values, and so it is convenient to use the absolute value mode.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 156 -

(2) Line at angle (G35)

With the starting point at the position designated by X and Y, the tool drills "n" number of holes each at interval "d" in the direction forming angle with the X axis. A standard fixed cycle applies for the drilling operation at each of the hole positions and so there is a need to retain beforehand the drilling data (drilling mode and drilling data). All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G35 command.

G35 Xx Yy Id J Kn ; Xx, Yy : The starting point coordinates; they are affected by the G90/G91 commands. Id : Interval "d"; it is based on the least input increment and when "d" is negative, drilling

proceeds in the point symmetrical direction centered on the starting point. J : Angle ; the counterclockwise direction is taken to be positive. Kn : Number "n" of holes to be drilled including the starting point; any number of holes

from 1 through 9999 can be assigned. (Example)

X1=200mm

W

=30

N=5 holes

Y

X

With 0.001 mm least input increment

Position prior to execution of G35 command

d =100mm

y 1=100mm

G91 ; G81 Z 10.000 R5.000 L 0 F100 ; G35 X200.000 Y100.000 I100.000 J 30.000 K5;

12 Programming Support Functions 12.1 Machining Method Support Functions

- 157 -

(3) Arc (G36)

The tool starts at the point forming angle with the X axis on the circumference of a circle with radius "r" whose center is the coordinates designated by X and Y, and it drills "n" number of holes aligned at angle interval . As with the bolt hole circle function, the drilling operation at each of the hole positions is based on a hold drilling fixed cycle and so there is a need to retain the drilling data beforehand. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G36 command. G36 Xx Yy Ir J P Kn ; Xx, Yy : Center coordinates of arc; they are affected by the G90/G91 commands. Ir : Radius "r" of arc; it is based on the least input increment and is provided with a

positive number. J : Angle at the point to be drilled initially; the counterclockwise direction is taken to

be positive. P : Angle interval ; when it is positive, the tool drills in the counterclockwise direction

and when it is negative, it drills in the clockwise direction. Kn : Number "n" of holes to be drilled; any number of holes from 1 through 9999 can be

assigned.

(Example)

W

=15

With 0.001 mm least input increment

Position prior to execution of G36 command

n=6 holes

Y1=100mm

X1=300mm

=10

N001 G91; N002 G81 Z-10.000 R5.000 F100; N003 G36 X300.000 Y100.000 I300.000 J10.000 P 15.000 K6;

12 Programming Support Functions 12.1 Machining Method Support Functions

- 158 -

(4) Grid (G37.1)

With the starting point at on the position designated by X and Y, this function enables the tool to drill the holes on the lattice with "nx" number of holes at parallel intervals of x to the X axis. Drilling proceeds in the X-axis direction. The drilling operation at each of the hole positions is based on a standard fixed cycle and so there is a need to command the drilling data (drilling mode and drilling data) beforehand. All movements between the hole positions are conducted in the G00 mode. The data is not retained upon completion of the G37.1 command.

G37.1 Xx1 Yy1 Ix Pnx Jy Kny ; Xx, Yy : The starting point coordinates; they are affected by the G90/G91 commands. Ix : X-axis interval x; it is based on the least input increment; when x is positive,

the intervals are provided in the positive direction as seen from the starting point and when it is negative, they are provided in the negative direction.

Pnx : Number of holes "nx" in the X-axis direction; any number of holes from 1 through 9999 can be assigned.

Jy : Y-axis interval y; it is based on the least input increment; when y is positive, the intervals are provided in the positive direction as seen from the starting point and when it is negative, they are provided in the negative direction.

Kny : Number of holes "ny" in the Y-axis direction; any number of holes from 1 through 9999 can be assigned.

(Example)

Position prior to execution of G37.1 command

With 0.001 mm least input increment G91 ; G81 ; Z 10.000 R5.000 F20 ; G37.1 X300.000 Y 100.000 I 50.000 P10 J 100.000 K8 ;

x=50mm

nx=10 holes

ny=8 holes

y= 100mm

W y1=100mm

x1=300mm

12 Programming Support Functions 12.1 Machining Method Support Functions

- 159 -

12.1.3.3 Fixed Cycle for Turning Machining M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 G77 Longitudinal cutting cycle G78 Thread cutting cycle G79 Face cutting cycle

Format:

G X/U_Z/W_I_K_R_F_(G18 plane)

Each fixed cycle command for turning machining is a modal G code and is effective until another command of the same modal group or a cancel command is given. The fixed cycle can be canceled by using any of the following G codes:

G00, G01, G02, G03 G09 G10, G11 G27, G28, G29, G30 G31 G33, G34 G37 G92 G52, G53 G65

12 Programming Support Functions 12.1 Machining Method Support Functions

- 160 -

(1) Longitudinal cutting cycle (G77) (a) Longitudinal cutting Straight cutting in the longitudinal direction can be performed consecutively by the following

block:

G77 X/U_ Z/W_ F_ ;

X axis

2 (F)

Z axis X

1 (R)

4 (R)

3 (F)

WZ

U 2

(R) : Rapid traverse feed (F) : Cutting feed

(b) Taper cutting Taper cutting in the longitudinal direction can be performed consecutively by the following

block: G77 X/U_ Z/W_ R_ F_ ;

(R) : Rapid traverse feed (F) : Cutting feed

X axis

Z axis

r

X

1 (R)

4 (R)

3 (F)

W Z

2 (F)

r: Taper part depth (radius designation, incremental value, sign is required)

U 2

12 Programming Support Functions 12.1 Machining Method Support Functions

- 161 -

(2) Thread cutting cycle (G78) (a) Straight thread cutting Straight thread cutting can be performed by the following block:

G78 X/U_ Z/W_ F/E_ ;

Z W

1 (R)2 (F)

4 (R)

3 (R)

X axis

Z axis

X

(R) : Rapid traverse feed (F) : F or E code designation

U 2

(b) Taper thread cutting Taper thread cutting can be performed by the following block:

G78 X/U_ Z/W_ R_ F/E_ ;

Z

r

W

1 (R) 2 (F)

4 (R)

3 (R)

X

(R) : Rapid traverse feed (F) : F or E code designation

X axis

Z axis

r: Taper part depth (radius designation, incremental value, sign is required)

U 2

12 Programming Support Functions 12.1 Machining Method Support Functions

- 162 -

Chamfering

: Thread cutting-up amount Assuming that thread lead is L, the thread cutting-up amount can be set in a given parameter in 0.1L steps in the range of 0 to 12.7L.

: Thread cutting-up angle

The thread cutting-up angle can be set in a given parameter in 1 steps in the range of 0 to 89.

(3) Face cutting cycle (G79) (a) Straight cutting Straight cutting in the end face direction can be performed consecutively by the following

block: G79 X/U_ Z/W_ F_ ;

X Z W

1(R)

2(F) 4(R)

3(F)

(R): Rapid traverse feed

(F): Cutting feed

X axis

Z axis

u / 2

r: Taper part depth (radius designation, incremental value, sign is required)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 163 -

(b) Taper cutting Taper cutting in the end face direction can be performed consecutively by the following block:

G79 X/U_ Z/W_ R_ F_ ;

X

r

Z W

1(R)

2(F) 4(R)

3(F)

Z axis

X axis

(R): Rapid traverse feed

(F): Cutting feed

r: Taper part depth (radius designation, incremental value, sign is required)

u / 2

12 Programming Support Functions 12.1 Machining Method Support Functions

- 164 -

12.1.3.4 Multiple Repetitive Fixed Cycle for Turning Machining M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(a) Longitudinal rough cutting cycle I (G71) The finish shape program is called, and straight rough cuttingis performed while intermediate

path is being calculated automatically. The machining program is commanded as follows.

G71 Ud Re ; G71 Aa Pp Qq Uu Ww Ff Ss Tt ; Ud : Cut depth d. (When P,Q command is not given). (Modal) Re : Retract amount e. (Modal) Aa : Finish shape program No. (If it is omitted, the program being executed is

assumed to be designated.) Pp : Finish shape start sequence No. (If it is omitted, the program top is assumed

to be designated.) Qq : Finish shape end sequence No. (If it is omitted, the program end is assumed

to be designated.) However, if M99 precedes the Q command, up to M99. Uu : Finishing allowance in the X axis direction. (When P, Q command is given).

(Diameter or radius designation) Ww : Finishing allowance in the Z axis direction. Ff : Cutting feed rate. Ss : Spindle speed. Tt : Tool command.

F, S, and T command in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.

(R)

(Cycle commanded point)

d Cut depth

Details of retract operation

(R) (F)

(F)

45 e

u / 2

W Finishing allowance

X

Z

12 Programming Support Functions 12.1 Machining Method Support Functions

- 165 -

(b) Face rough cutting cycle (G72) The finish shape program is called, and rough turning is performed in the end face direction

while intermediate path is being calculated automatically. The machining program is commanded as follows.

G72 Wd Re ; G72 Aa Pp Qq Uu Ww Ff Ss Tt ; Wd : Cut depth d. (When P,Q command is not given). (Modal) Re : Retract amount e. (Modal) Aa : Finish shape program No. (If it is omitted, the program being executed is

assumed to be designated.) Pp : Finish shape start sequence No. (If it is omitted, the program top is assumed to

be designated.) Qq : Finish shape end sequence No. (If it is omitted, the program end is assumed to

be designated.) However, if M99 precedes the Q command, up to M99. Uu : Finishing allowance in the X axis direction. Ww : Finishing allowance in the Z axis direction. (When P, Q command is given.) Ff : Cutting feed rate. Ss : Spindle speed. Tt : Tool command.

F, S, and T command in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.

(Cycle commanded point)

d Cut depth

u / 2

W

Finishing allowance

(R)

Details of retrace operation

(F)

(F)

e

X

Z

45

S

E

12 Programming Support Functions 12.1 Machining Method Support Functions

- 166 -

(c) Molding material in rough cutting cycle (G73) The finish shape program is called. Intermediate path is automatically calculated and rough

cuttingis performed conforming to the finish shape. The machining program is commanded as follows.

G73 Ui Wk Rd ; G73 Aa Pp Qq Uu Ww Ff Ss Tt ; Ui : Cutting allowance in the X axis direction Wk : Cutting allowance in the Z axis direction Rd : Split count

i k d

Cutting allowance when P, Q command is not given.

Modal data Sign is ignored. Cutting allowance is given with a radius

designation.

Aa : Finish shape program No. (If it is omitted, the present program is assumed to be designated.)

Pp : Finish shape start sequence No. (If it is omitted, the program top is assumed to be designated.)

Qq : Finish shape end sequence No. (If it is omitted, the program end is assumed to be designated.) However, if M99 precedes the Qq command, up to M99.

Uu : Finishing allowance in the X axis direction u Ww : Finishing allowance in the Z axis direction w

Finishing allowance when P, Q command is given.

Sign is ignored. Diameter or radius is designated

according to the parameter. The shift direction is determined by the

shape. Ff : Cutting feed rate (F function) Ss : Spindle speed (S function) Tt : Tool selection (T function)

The F, S, and T commands in the finish shape program are ignored, and the value in the rough cutting command or the preceding value becomes effective.

k + w

X

Z

S1 S2

S3

S

i + u/2

u/2 w A

E

2

3 4

5 6

7

8

9 10

11 12

13

14

15 16

17 18

19

1

12 Programming Support Functions 12.1 Machining Method Support Functions

- 167 -

(d) Finish cycle (G70) After rough cutting is performed by using G71 to G73, finish turning can be performed by using

the G70 command. The machining program is commanded as follows.

G70 A_ P_ Q_ ;

A : Finish shape program number. (If it is omitted, the program being executed is assumed to be designated.)

P : Finish shape start sequence number. (If it is omitted, the program top is assumed to be designated.)

Q : Finish shape end sequence number. (If it is omitted, the program end is assumed to be designated.) However, if M99 precedes the Q command, up to M99.

(1) The F, S, and T commands in the rough cutting cycle command G71 to G73 blocks are

ignored, and the F, S, and T commands in the finish shape program become effective. (2) The memory address of the finish shape program executed by G71 to G72 is not stored.

Whenever G70 is executed, a program search is made. (3) When the G70 cycle terminates, the tool returns to the start point at the rapid traverse feed

rate and the next block is read. (Example 1) Sequence No. designation

N200 ;

N300 ;

N100 G70 P200 Q300 ;

N110

N120

N200

Finish shape program

N300

N310

:

:

:

:

:

(Example 2) Program No. designation

N100 G70

A100 ; N110 ;

:

O100

G01 X100 Z50 F0.5 ; M99 ;

: :

In either example 1 or 2, after the N100 cycle is executed, the N110 block is executed.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 168 -

(e) Face cutting-off cycle (G74) When the slotting end point coordinates, cut depth, cutting tool shift amount, and cutting tool

relief amount at the cut bottom are commanded, automatic slotting is performed in the end face direction of a given bar by G74 fixed cycle. The machining program is commanded as follows.

G74 Re ; G74 X/(U) Z/(W) Pi Qk Rd Ff ;

Re : Retract amount e (when X/U, Z/W command is not given) (Modal) X/U : B point coordinate (absolute/incremental) Z/W : B point coordinate (absolute/incremental) Pi : Tool shift amount (radius designation, incremental, sign not required) Qk : Cut depth k (radius designation, incremental, sign not required) Rd : Relief amount at cut bottom d (If sign is not provided, relief is made at the first

cut bottom. If minus sign is provided, relief is made not at the first cut bottom but at the second cut bottom and later.)

Ff : Feed rate

k k k k x

u/2

(1) (2)(3)(4)

(5) (6)(7)(8)

(9) (10)

(11)

(12) i

d

e

wz

B

S (start point)

(9) and (12) just before the last cycle are executed with the remaining distance.

(2), (4), (6), (8), (10), (11) and

(12) are executed at the rapid traverse feed rate.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 169 -

(f) Longitudinal cutting-off cycle (G75) When the slotting end point coordinates, cut depth, cutting tool shift amount, and cutting tool

relief amount at the cut bottom are commanded, automatic slotting is performed in the longitudinal direction of a given bar by G75 fixed cycle. The machining program is commanded as follows.

G75 Re ; G75 X/(U) Z/(W) Pi Qk Rd Ff ; Re : Retract amount e (when X/U, Z/W command is not given) (Modal) X/U : B point coordinate (absolute/incremental) Z/W : B point coordinate (absolute/incremental) Pi : Tool shift amount (radius designation, incremental, sign not required) Qk : Cut depth k (radius designation, incremental, sign not required) Rd : Relief amount at cut bottom d (If sign is not provided, relief is made at the first

cut bottom. If sign is provided, relief is made not at the first cut bottom but at the second cut bottom and later.)

Ff : Feed rate

k x

u / 2

(1)(2)

(3)

(4) (5)

(6) (7)

(8) (9)

(10)

(11)

(12)i

d

e

wz

B

S (start point)

i

i

i

(9) and (12) just before the last cycle are executed with the remaining distance.

(2), (4), (6), (8), (10), (11) and

(12) are executed at the rapid traverse feedrate.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 170 -

(g) Multiple repetitive thread cutting cycle (G76) When the thread cutting start and end points are commanded, cut at any desired angle can be

made by automatically cutting so that the cut section area (cutting torque) per time becomes constant in the G76 fixed cycle.

Various longitudinal threads can be cut by considering the thread cutting end point coordinate and taper height constituent command value.

Command Format

G76 Pmra Rd ; G76 X/U Z/W Ri Pk Qd Fl ; m : Cut count at finishing 01 to 99 (modal) r : Chamfering amount 00 to 99 (modal). Set in 0.1-lead increments. a : Nose angle (included angle of thread) 00 to 99 (modal) Set in 1-degree

increments. d : Finishing allowance (modal) X/U : X axis end point coordinate of thread part. Designate the X coordinate of the end point in the thread part in an absolute or

incremental value. Z/W : Z axis end point coordinate of thread part. Designate the Z coordinate of the end point in the thread part in an absolute or

incremental value. i : Taper height constituent in thread part (radius value). When i = 0 is set,

straight screw is made. k : Thread height. Designate the thread height in a positive radius value. d : Cut depth. Designate the first cut depth in a positive radius value. l : Thread lead

Configuration of one cycle In one cycle, (1), (2), (5), and (6) move at rapid traverse feed and (3) and (4) move at cutting

feed designated in F.

rx

(-i) k

z w

S

u/2

(1)

(2)

(3)

(4)

(5)

(6)

a/2When Ri is negative

12 Programming Support Functions 12.1 Machining Method Support Functions

- 171 -

r x

i

k

z w

S

u/2

(1)

(2)

(3)(4)

(5)

(6)

a/2

When Ri is positive

k

a

d 2 d n

d (finishing allowance) (Cut "m" times at finishing)

nth time

Second time

First time

d

12 Programming Support Functions 12.1 Machining Method Support Functions

- 172 -

12.1.3.5 Multiple Repetitive Fixed Cycle for Turning Machining (Type II) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 ;

G71 Ud Re H0; G71 Pp Qq . .;

Rough cutting start point q

(R) (R)

(R/f)

d

u/2 p

w

(f)

(R) (f)

(f) e

Z

X

45

G71 Ud Re H1; G71 Pp Qq . .;

q

(R) (R)

(R/f)

d

u/2p

w

(f)

(R)(f)

e Z

X

Hole bottom

Rough cutting start point

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.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 173 -

12.1.3.6 Small-diameter Deep-hole Drilling Cycle M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

In deep hole drilling, cutting and retract are repeated and the workpiece is machined multiple times. In addition, when PLC signals are input during cutting, the cutting for the time concerned is skipped. In this way, this cycle reduces the load applied to the tool. Command format The small-diameter deep hole drilling cycle mode is established by designating the M code command which was set in the parameter. If the G83 command is designated in this mode, the small-diameter deep hole drilling cycle is executed. The mode is canceled by the following conditions. Designation of a fixed cycle cancel command (G80, G commands in Group 1) Resetting The small-diameter deep hole drilling mode M command does not output MF or wait for FIN. G83 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Pp1 ;

X, Y : Hole drilling point position Z : Hole bottom position R : R point position Q : Depth of cut in each pass (designated as incremental value) F : Cutting feed rate P : Dwell time at hole bottom position

12 Programming Support Functions 12.1 Machining Method Support Functions

- 174 -

12.1.3.7 Fixed Cycle for Drilling (Type II) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 signals ON/OFF state and the hole drilling axis of the fixed cycle for drilling is shown below.

G code Details Y axis cross tap function selection signal state Hole drilling axis

G80 Cancel ON G83 Deep hole drilling cycle 1 OFF

Z

ON G84 Tap cycle OFF

Z

ON G85 Boring cycle OFF

Z

ON Y G87 Deep hole drilling cycle 1 OFF X ON Y G88 (G88.1) Tap cycle OFF X ON Y G89 Boring cycle OFF X ON G83.2 Deep hole drilling cycle 2 OFF

Z/X

12 Programming Support Functions 12.1 Machining Method Support Functions

- 175 -

12.1.4 Mirror Image

12.1.4.1 Mirror Image by Parameter Setting M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 which 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 which is symmetrical on the left and right or at the top or bottom is performed. Each axis has its own request signal.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 176 -

12.1.4.3 G Code Mirror Image M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 : Mirror image on Xx1, Yy1, Zz1 : Command axes and command positions

With the local coordinate system, the mirror image is applied with the mirror positioned respectively at x1, y1 and z1. The program format for the G code mirror image cancel is shown below. G50.1 Xx1 Yy1 Zz1 ;

G50.1 : Mirror image cancel Xx1, Yy1, Zz1 : Command axes

The coordinate word indicates the axes for which the mirror image function is to be canceled and the coordinates are ignored. In the case of G51.1 Xx1

Y

X

Original shape (program)

Mirroring axis

Shape achieved when machining program for the left side has been executed after the mirror command

12 Programming Support Functions 12.1 Machining Method Support Functions

- 177 -

12.1.4.4 Mirror Image for Facing Tool Posts M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With machines in which the base tool post and facing tool post are integrated, this function enables the programs prepared for cutting at the base side to be executed by the tools on the facing side. The distance between the two posts is set beforehand with the parameter.

The command format is given below.

G code Function G68 G69

Facing tool post mirror image ON Facing tool post mirror image OFF

When the G68 command is issued, the subsequent program coordinate systems are shifted to the facing side and the movement direction of the X axis is made the opposite of that commanded by the program. When the G69 command is issued, the subsequent program coordinate systems are returned to the base side. The facing tool post mirror image function can be set to ON or OFF automatically by means of T (tool) commands without assigning the G68 command. A parameter is used to set ON or OFF for the facing tool post mirror image function corresponding to the T commands.

Programmed path

Facing side path (mirror image ON)

Z

X

Base post

Facing post

(G69)

Parameter for distance between posts (radial value, X axis only)

(G68)

12.1.4.5 T Code Mirror Image for Facing Tool Posts M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

If, when tools that correspond to tool Nos. 1 to 64 are selected (T commands), these are tool Nos. for which the facing tool post mirror image function has already been designated with a parameter, the status equivalent to G68 (facing tool post mirror image ON) is established. When the commands apply to tool Nos. for which the facing tool post mirror image function is not designated, the status equivalent to G69 (facing tool post mirror image OFF) is established.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 178 -

12.1.5 Coordinate System Operation

12.1.5.1 Coordinate Rotation by Program M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

G68 : Call command Xx1, Yy1 : Rotation center cordinates Rr1 : Angle of rotation

r1()y1

x1

(x1,y1)()

W

'

'

W'

( )

() (1) Angle of rotation "r1" can be set in least input increment from 360 to 360 . (2) The coordinates are rotated counterclockwise by an amount equivalent to the angle which is

designated by angle of rotation "r1". (3) The counter is indicated as the point on the coordinate system prior to rotation. (4) The rotation center coordinates are assigned with absolute values.

(Original local coordinate system)

(Rotated local coordinate system)

r1 (Angle of rotation)

(x1, y1) (Center of rotation)

X

X

x1

W

Y

Y

y1

12 Programming Support Functions 12.1 Machining Method Support Functions

- 179 -

(Example) N01 G28 X Y Z ;

N02 G54 G52 X150. Y75. ; Local coordinate system assignment N03 G90 G01 G42 X0 Y0 ; Tool radius compensation ON N04 G68 X0 Y0 R30. ; Coordinate rotation ON N05 M98 H101 ; Subprogram execution N06 G69 ; Coordinate rotation cancel N07 G54 G52 X0 Y0 ; Local coordinate system cancel N08 G00 G40 X0 Y0 ; Tool radius compensation cancel N09 M02 ; Completion

Sub program (Shape programmed with original coordinate system)

N101 G90 G01 X50. F200 ; N102 G02 X100. R25. ; N103 G01 X125. ; N104 Y75. ; N105 G03 X100. Y100. R25. ; N106 G01 X50. ; N107 G02 X0 Y50. R50. ; N108 G01 X0 Y0 ; N109 M99 ;

100.

100. 300.200.

Y

X

200.

W

Actual machining shape

(Programmed coordinate)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 180 -

12.1.6 Dimension Input

12.1.6.1 Corner Chamfering / Corner R M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 R I When ",C" or ",R" is commanded for linear interpolation, corner chamfering or corner R can be inserted between linear blocks. Corner chamfering Corner R Example: Example:

N1 G01 Xx1 Zz1, Cc1 ; N2 Zz2 ;

N2 c 1

c 1

N1

N1 G01 Xx1 Zz1, Rr1 ; N2 Zz2 ;

N2

r 1 N1

(Note 1) If a corner chamfering or corner R command is issued specifying a length longer than the N1 or N2 block, a program error occurs.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 181 -

(2) Corner chamfering / corner R II (L system) When ",C" or ",R" is command in a program between linear-circular, corner chamfering or corner R can be inserted between blocks.

(a) Corner chamfering II (Linear circular)

Cc1Hypothetical corner intersection

Cc1

Chamfering end point

Chamfering start point

Example: G01 X_Z_ ,Cc1 ;

(1)

(2)

G02 X_Z_ Ii1 Kki ;

(b) Corner chamfering II (Circular - linear)

Cc1

(1)

Cc1

Hypothetical corner intersection

Chamfering start point

Chamfering end point

Example: G03 X_Z_ Ii1 Kk1 ,Cc1 ;

(2)

G01 X_Z_ ;

(c) Corner chamfering II (Circular - circular)

(2)

Cc1

(1)

Cc1

Hypothetical corner intersection

Example: G02 X_Z_ Ii1 Kk1 ,Cc1 ; G02 X_Z_ Ii2 Kk2 ;

Chamfering start point

Chamfering end point

12 Programming Support Functions 12.1 Machining Method Support Functions

- 182 -

(d) Corner R II (Linear - circular)

(2)

(1)

Rr1

Hypothetical corner intersection

Corner R start point

Corner R end point

Example: G01 X_Z_ ,Rr1 ; G02 X_Z_ Ii1 Kk1 ;

(e) Corner R II (Circular linear)

(2)

(1)

Rr1

Hypothetical corner intersection

Example: G03 X_Z_ Ii1 Kk1 ,Rr1 ; G01 X_Z_ ;

Corner R start point

Corner R end point

(f) Corner R II (Circular circular)

(2)

(1)

Rr1

Hypothetical corner intersection

Corner R start point

Corner R start point

Example: G02 X_Z_ Ii1 Kk1 ,Rr1 ; G02 X_Z_ Ii2 Kk2 ;

12 Programming Support Functions 12.1 Machining Method Support Functions

- 183 -

(3) Specification of corner chamfering / corner R speed E

An E command can be used to specify the speed for corner chamfering or corner R. This enables a corner to be cut to a correct shape. (Example)

F

F

F

F

E

E

G01 X_Z_ ,Cc1 Ff1 Ee1 ; X_Z_ ;

G01 X_Z_ ,Rr1 Ff1 Ee1 ; X_Z_ ;

X

Z

An E command is a modal and remains effective for feeding in next corner chamfering or corner R. An E command has two separate modals: synchronous and asynchronous feed rate modals. The effective feed rate is determined by synchronous (G95) or asynchronous (G94) mode. If an E command is specified in 0 or no E command has been specified, the feed rate specified by an F command is assumed as the feed rate for corner chamfering or corner R. Hold or non-hold can be selected (M system only) using a parameter for the E command modal at the time of resetting. It is cleared when the power is turned OFF (as it is with an F command).

12 Programming Support Functions 12.1 Machining Method Support Functions

- 184 -

(4) Corner chamfering / corner R (I, K designation) 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. This command format is valid for the L system of M64AS, M64S, M65S, and M66S only. (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 : X-axis end point coordinate Z/w : Z-axis end point coordinate i/k/c : 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.

N100

0 Z axis

X axis

N200

i, k, c

i, k, c Hypothetical corner intersection

Chamfering end point

Chamfering start point

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 R 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.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 185 -

(b) Corner R (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 R commands, are ignored. Command format

N100 Xx/Uu Zz/Ww Rr ;

N200 Xx/Uu Zz/Ww ;

x/u : X-axis end point coordinate z/w : Z-axis end point coordinate r : Radius of corner R arc

N100

0 Z axis

X axis

N200

r

Corner R start point

Corner R end point

Hypothetical corner intersection

If both corner chamfering and corner R commands are present in the same block, the last

command will take effect. Corner R commands using the "R" address cannot be designated in an arc command

block. "R" is the arc radius command.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 186 -

12.1.6.2 Linear Angle Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 ;

G17 : Plane selection Xx1, Yy1 : 1 element Aa1 : Angle

Example

Note 1: If both the axis "A" or 2nd miscellaneous function "A" are used, address "A" is treated as

the axis "A" command and or the 2nd miscellaneous function, respectively.

G17 G91 X100. A60. ; End point

Start point

(Automatically calculated with operation)

X100.

Y

Y

X

60

12 Programming Support Functions 12.1 Machining Method Support Functions

- 187 -

12.1.6.3 Geometric Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

N 1

a 2

X

Z W 1

N2

a1

N1 G01 Aa1 Ff1 ; N2 Xx1 Zz1 Aa2 ;

End point (X1, Z1)

Automatic intersection point calculation

Z1

x1 2

Start point

a: Angle () formed between straight line and horizontal axis on plane. The plane is the selected plane at this point.

(Note 1) This function cannot be used when using the A axis or 2nd miscellaneous function A.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 188 -

(1) Automatic calculation of two-arc contact

When two continuous circular arcs contact with each other and it is difficult to find the contact, the contact is automatically calculated by specifying the center coordinates or radius of the first circular arc and the end point absolute coordinates and center coordinates or radius of the second circular arc. Example

G18 G02 Ii1 Kk1 Ff1 ; G03 Xxc Zzx Ii2 Kk2 Ff2 ;

or G18 G02 Ii1 Kk1 Ff1 ;

G03 Xxc Zzc Rr2 Ff2 ; or G18 G02 Rr1 Ff1 ; G03 Xxc Zzc Ii2 Kk2 Ff2 ;

C(xc, zc)

r2

(p2,q2)

(p1,q1)

B(?,?) r1

A

I and K are circular center coordinate incremental values; distances from the start point in the first block or distances from the end point in the second block. P and Q commands (X, Z absolute center coordinates of circular arc) can be given instead of I and K commands.

(2) Automatic calculation of linear-arc intersection

When it is difficult to find the intersections of a given line and circular arc, the intersections are automatically calculated by programming the following blocks. Example

G18 G01 Aa1 Ff1 ; G02 Xxc Zzc Ii2 Kk2 Hh2 Ff2 ;

r1

(p2,q2)

B(?,?)

B(?,?) a1

A C(xc, zc)

I and K : Incrimental coordinates from circular end point P and Q : Absolute center coordinates of circular arc H = 0 : Intersection with shoter line H = 1 : Intersection with longer line

12 Programming Support Functions 12.1 Machining Method Support Functions

- 189 -

(3) Automatic calculation of arc-linear intersection

When it is difficult to find the intersections of a given circular arc and line, the intersections are automatically calculated by programming the following blocks. Example G18 G03 Ii1 Kk1 Hh1 Ff1 ; G01 Xxc Zzc Aa1 Ff2 ;

r1 a1

C(xc, zc)

B(?,?) B(?,?)

(p1,q1)

A

I and K : Incrimental coordinates from circular end point P and Q : Absolute center coordinates of circular arc (L3 only) H = 0 : Intersection with shoter line H = 1 : Intersection with longer line

(4) Automatic calculation of linear-arc contact

When it is difficult to find the contact of a given line and circular arc, the contact is automatically calculated by programming the following blocks. Example

G01 Aa1 Ff1 ; G03 Xxc Zzc Rr1 Ff2 ;

a1

A

B (?,?)

r1

C(xc, zc)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 190 -

(5) Automatic calculation of arc-linear contact

When it is difficult to find the contact of a given circular arc and line, the contact is automatically calculated by programming the following blocks. Example

G02 Rr1 Ff1 ; G01 Xxc Zzc Aa1 Ff2 ;

a1 r1

A B (?,?)

C(xc, zc)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 191 -

12.1.6.4 Polar Coordinate Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With this function, the end point coordinate value 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 ;

Plane selection for polar coordinate command (G17/G18/G19) Polar coordinate command mode ON

G9x G01 Xx1 Yy1 F2000 ; :

Polar coordinate command G9x : Center selection for polar coordinate command (G90/G91)

G90The workpiece coordinate system zero point is the polar coordinate center.

G91The present position is the polar coordinate center. x1 : 1st axis for the planeThe radius commanded y1 : 2nd axis for the planeThe angle commanded

For G90/G17(X-Y plane)

Commanded position (end point)

Present position y1

x1

X

Y

Plus

Minus

G15 ;

Polar coordinate command mode OFF

12 Programming Support Functions 12.1 Machining Method Support Functions

- 192 -

12.1.7 Axis Control

12.1.7.1 High-speed Machining

12.1.7.1.3 High-speed Machining Mode III M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 16m 16m 16m 16m 16m 16m 16m 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 high- accuracy 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 ; Incremental modal linear cutting X0.1 Y0.002 ; G90 G00 X0 Y0 Z0 ; Rapid traverse G02 X__Y__R__F__ ; Absolute modal R-designated arc G03 X__Y__I__J__F__ ; Arc

G05 P0 ; . High-speed machining mode III OFF M02;

(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.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 193 -

12.1.7.1.4 High-speed High-accuracy Control 1

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 16m 16m 16m 16m 16m L system

This function runs machining programs, in which free-form curved surfaces have been approximated by fine-segments, at high speed and with a high accuracy. It is effective in increasing the speed at which dies with free-form curved surfaces are machined. Command format G05.1 Q1 ; High-speed high-accuracy control I ON G05.1 Q0 ; High-speed high-accuracy control I OFF

The performance of simultaneous 3 axis and 1mm-length fine-segment is as follows.

Performance of fine-segment length High-accuracy control I mode No radius compensation Radius compensation Program restriction

Invalid 8.4m/min 8.4m/min None Valid 16.8m/min 16.8m/min Available

Program restrictions The machining speed may drop depending on the number of characters in one block. During high-speed high-accuracy control I operation using tape operation, the machining speed may be suppressed depending on the program transmission speed and the number of characters in one block. Modes which can be designated by commands The modal statuses when the G05.1 Q1 command is assigned must be as shown in the table below. If the conditions listed are not satisfied, a program error will result.

Function G code modal

Tool radius compensation mode G40 Tool length compensation G49 G code mirror image G50.1 Mirror image by parameter setting Cancel External signal mirror image Cancel Cutting mode G64 Macro modal call mode G67 Coordinate conversion mode G69 Fixed cycle mode G80 Per-revolution feed G94 Constant surface speed control mode G97 Interrupt-type macro mode M97

12 Programming Support Functions 12.1 Machining Method Support Functions

- 194 -

12.1.7.1.5 High-speed High-accuracy Control 2 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 33m 67m(*) 33m 67m(*) 67m(*) L system

(Note) (*) changes depending on the axis configuration and operation condition. This function runs machining programs, in which free-form curved surfaces have been approximated by fine-segments, at high speed and with a high accuracy. It is effective in increasing the speed at which dies with free-form curved surfaces are machined. Command format

G05 P10000 ; High-speed high-accuracy control II ON

G05 P0 ; High-speed high-accuracy control II OFF

The performance of fine-segment execution when 3 axes are moved simultaneously is as follows.

Performance of fine segment execution (1mm-length) (No radius compensation) High-accuracy

control II mode Fairing invalid Fairing valid Program restriction

Invalid 8.4m/min 8.4m/min None Valid

(Number of NC axes 1 to 4)

67.5m/min 50.6m/min

Valid (Number of NC axes 5 and 6)

50.6m/min 42.1m/min

Available

Program restrictions The machining speed may drop depending on the number of characters in one block. During high-speed high-accuracy control II operation using tape operation, the machining speed may be suppressed depending on the program transmission speed and the number of characters in one block. When the fairing is valid (#8033 is set to 1), if the successive fairing is executed in the machining program, the performance of fine-segment execution may decelerate less than the value described in the above table. In the network connection, the value described in the above table may not be guaranteed depending on the state. Modes which can be designated by commands The modal statuses when the G05 P10000 command is assigned must be as shown in the table below. If the conditions listed are not satisfied, a program error will result.

Function G code modal Tool radius compensation mode G40 Tool length compensation G49 G code mirror image G50.1 Mirror image by parameter setting Cancel External signal mirror image Cancel Cutting mode G64 Macro modal call mode G67 Coordinate conversion mode G69 Fixed cycle mode G80 Per-revolution feed G94 Constant surface speed control mode G97 Interrupt-type macro mode M97

12 Programming Support Functions 12.1 Machining Method Support Functions

- 195 -

Additional functions when high-speed high-accuracy control 2 mode is ON (1) Fairing

If the protruding path (zigzagging path) is shorter than the parameter setting values in the machining program generated with a CAM, etc., this function can be used to eliminate the protruding paths smaller than the setting value so that the front and back paths are smoothly connected. This function is valid only for continuous linear commands (G1).

After fairing Before fairing

G1 G1G1

If there is any protruding path after fairing, fairing is repeated.

Before fairing After first fairing After final faring

(2) Acceleration clamp speed Parameter settings are used to clamp the speed so that the acceleration occurring due to movement of each block does not exceed the tolerable value. This function clamps the speed optimally even at a section where" angle change at each block is small but entire curvature is large" such as shown below. The tolerable acceleration value is calculated from the parameter setting values.

If the tool moves along the large curvature section without deceleration, a large acceleration is generated resulting in a path error from the inner route.

R

(3) High-speed mode corner deceleration During high-accuracy control, if the angle is large between adjacent blocks in the machining program, this function automatically decelerates so that the acceleration generated when passing through the corner is within the tolerable value. If a small block is inserted at the corner section with the machining program generated with the CAM, etc., the corner passing speed will not match the periphery. This can affect the machining surface. If this type of small block is inserted while this function is valid, the corner will be largely judged by the parameter settings. The small block is excluded when the angle is judged, but it not excluded from the actual movement command.

If this function is valid, the axis decelerates at the corner without being affected by the small block.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 196 -

12.1.7.1.7 SSS Control M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(Note) The "12.1.7.1.5 High-speed high-accuracy control 2" option is required to use this function. With normal high-accuracy control, the angle between two blocks is compared with the corner deceleration angle to determine whether to execute corner deceleration between the blocks. This can cause the speed to suddenly change between the blocks with an angle close to the corner deceleration angle, or can cause scratches or streaks to form. With SSS (Super Smooth Surface) control, the large area path information is used instead of just the angle between the blocks. Thus, optimum speed control that is not adversely affected by minute steps or waviness is possible. This enables machining with fewer scratches and streaks on the cutting surface compared to the normal high-accuracy control function.

Conventional optimum corner deceleration

Feedrate

Time

Do not decelerate

Feedrate

Time

SSS control

Decelerate according to angle When smaller than corner deceleration angle

Feedrate

Time

When larger than corner deceleration angle

Feedrate

Time

Gradually speed deceleration

[Features of SSS control]

(1) Speed fluctuation, caused by the effect of the blocks (minute stepping or waviness) and resulting in disturbed machining, is suppressed, and scratches caused by these blocks is reduced.

(2) This speed control is not easily affected by the steps found in the path. (3) If adjacent paths are similar in terms of shape accuracy, the acceleration/deceleration pattern

is also similar, and the fluctuation of accuracy caused by a difference in speed is suppressed. (4) Even if corner deceleration is not required, the speed is clamped if the predicted acceleration

is high. (5) The machining time can be reduced in machining applications having many corners.

The length of the path direction recognized with SSS control can be adjusted with the machining parameter "reference length". The range is increased as the setting value increases, and the effect of the error is reduced. (Note) The high-speed high-accuracy control 2 option is required to use this function.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 197 -

12.1.7.2 Chopping

12.1.7.2.1 Chopping M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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

Workpiece

Wheel Chopping action

12 Programming Support Functions 12.1 Machining Method Support Functions

- 198 -

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

Rapid traverse

Start 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.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 199 -

12.1.7.4 Normal Line Control M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function controls the swiveling of the C axis (rotary axis) so that the tool is always pointing in the normal line direction for the X and Y axes movement commands during program operation. It can be used for machining springs, for sewing operations involving sewing machines, carpets, etc. It is valid for only one C axis (rotary axis).

C-axis center (rotary axis)

Tool tip position C axis swiveling

G code Function G40.1 G41.1 G42.1

Normal line direction control cancel Normal line direction control left ON Normal line direction control right ON

12 Programming Support Functions 12.1 Machining Method Support Functions

- 200 -

12.1.7.5 Circular Cutting M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Function G12 G13

CW (clockwise) CCW (counterclockwise)

The program format is given below. G12/13 Ii Dd Ff ; G12/13 Ii Dd Ff

: Circular cutting command : Radius of complete circle : Compensation number : Feed rate

When the G12 command is used (path of tool center) 0 1 2 3 4 5 6 7 0 When the G13 command is used (path of tool center) 0 7 6 5 4 3 2 1 0

(Notes) Circular cutting is undertaken on the plane

which has been currently selected (G17, G18 or G19).

The (+) and () signs for the compensation amount denote reduction and expansion respectively.

Y

X

1

2

3

4

5

6

7

0

Radius of circle

Offset amount

12 Programming Support Functions 12.1 Machining Method Support Functions

- 201 -

12.1.8 Multi-part System Control

12.1.8.1 Synchronization between Part Systems M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables part systems to be synchronized (block start synchronization) using the program. ! ; Part system 1 and part system 2 are synchronized. When the part system number is

to be omitted This synchronization command makes it possible to control the simultaneous operation of two part systems and the independent operation of part systems.

Pi1

Pi2

Pn1

Synchronized operation

Part system 1

Part system 2 program

Pi1 Pn1

! ;

Part system 1 program Part

system 2

Simultaneously start

! ;

Pn2Pn2 Pi2

(Note 1) When the part system with which the operation is to be synchronized is not operating, the

other part system moves on to the next block. This function is useful when conducting program checks on a part system by part system basis.

(Note 2) The synchronization command is normally assigned as a separate command. However, if a movement command and M, S or T command have been assigned in the same block, a parameter is set to decide whether the operations are to be synchronized after the movement command and M, S or T command have been executed or the movement command and M, S or T command are to be executed upon completion of the synchronization.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 202 -

12.1.8.2 Start Point Designation Synchronization M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The synchronizing point can be placed in the middle of the block by designating the start point. (1) Start point designation synchronization Type 1 (G115) Command format

!Ll G115 X_ Z_ C_ ; !Ll G115 X_,Z_,C_

: Synchronizing command : G command : Own start point (designate other part system's coordinate value)

(a) The other part system starts first when synchronizing is executed. (b) The own part system waits for the other part system to move and reach the designated

start point, and then starts.

!G115

!G115

Own part system

Other part system

Designated start point

Designated start point

Synchronized operation

! Synchronized operation

!

Own part system

Other part system

(c) When the start point designated by G115 is not on the next block movement path of the

other part system, the own part system starts once the other part system has reached all of the start point axis coordinates.

: Movement : Command point : Actual start point

12 Programming Support Functions 12.1 Machining Method Support Functions

- 203 -

(2) Start point designation synchronization Type 2 (G116) Command format

!Ll G116 X_ Z_ C_ ; !Ll G116 X_,Z_,C_

: Synchronizing command : G command : Other start point (designate own part system's coordinate value)

(a) The own part system starts first when synchronizing is executed. (b) The other part system waits for the own part system to move and reach the designated

start point, and then starts.

Synchronized operation

Other part system !

Own part system !G116 Designated start point

Own part system

Synchronized operation Other part system !

Designated start point !G116

(c) When the start point designated by G116 is not on the next block movement path of the

own part system, the other part system starts once the other part system has reached all of the start point axis coordinates.

: Movement : Command point : Actual start point

12 Programming Support Functions 12.1 Machining Method Support Functions

- 204 -

12.1.8.3 Cross Machining Command M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables any axis to be replaced by another axis between part systems. This makes it possible to perform operations which are not possible with regular axis configurations: for instance, tools which are provided only on part system 1 can be used for machining on part system 2. This manual contains descriptions where part system numbers have been added after the axis names in order to identify which part system the axes belong to (such as X1). In terms of designating the program commands, however, a single letter is used to designate the axis address just as before.

X1

Z1

Z2

X2

X1

Z1

X2

Z2

Axis X1 and axis X2 are exchanged.

Part system 1 (X1, Z1) Part system 2 (X2, Z2) Part System 1 (X2, Z1) Part system 2 (X1, Z2)

Cross machining control is switched from ON to OFF and vice versa using a PLC signal. Parameters are used to set what axis is to be placed in the cross machining control status in response to which PLC signal.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 205 -

12.1.8.5 Control Axis Synchronization M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Synchronization control enables an arbitrary control axis in the other part system to move in synchronization with the movement command assigned to an arbitrary control axis. The direction in which the axis is to move synchronously can also be reversed using a parameter.

Base axis :Axis to which movement command to synchronize axes is assigned. Synchronized axis :Axis whose movement is synchronized with base axis.

X1

Part system 1 (X1, Z1) Part system 2 (Z2)

Z2

(synchronized axis)

Z1 (base axis)

12 Programming Support Functions 12.1 Machining Method Support Functions

- 206 -

12.1.8.6 Balance Cut M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

When workpiece that is relatively long and thin is machined on a lathe, deflection may result, making it impossible for the workpiece to be machined with any accuracy. In cases like this, the deflection can be minimized by holding tools simultaneously from both sides of the workpiece and using them in synchronization to machine the workpiece (balance cutting). This method has an additional advantage: since the workpiece is machined by two tools, the machining time is reduced. The balance cutting function enables the movements of the tool rests belonging to part system 1 and part system 2 to be synchronized (at the block start timing) so that this kind of machining can easily be accomplished.

Part system 1

Part system 2

The command format is given below. G14 Balance cut command OFF (modal) G15 Balance cut command ON (modal)

G14 and G15 are modal commands. When the G15 command is assigned, the programmed operations of two part systems are synchronized (at the block start timing) for all blocks until the G14 command is assigned or until the modal information is cleared by the reset signal.

T0101; G00 X_ Z_; G15; G01 Z_ F0.4;

: :

T0102; G00 X_ Z_; G15; G01 Z_ F0.4;

: :

Part system 1 program Part system 2 program

T0101; G00 X_ Z_; G15; G01 Z_ F0.4;

T0102; G00 X_ Z_; G15; G01 Z_ F0.4;

... ...

.

... ...

.

Whereas synchronization is possible only with the next block using the inter-part system synchronization code "!", the balance cutting function provides synchronization (at the block start timing) with multiple consecutive blocks.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 207 -

12.1.8.7 Common Memory between Tool Posts M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

For the machine with two part systems, the common variables and tool compensation memory which exist in 1-part system and 2-part system respectively can be made common in those systems by the parameter setting.

(1) Common variables

For 2-part system, normally, common variables #100 to #199 are provided per part system, and common variables #500 to #999 are common for part systems. However, when this function is valid, common variables #500 to #999 are also provided per part system. To make a part or all of common variables #100 to #199 and #500 to #999 to be used commonly between part systems, set parameters to designate the number of variables to be used commonly for #100 to #199 and #500 to #999 respectively. As for the variables designated to be common to part systems, the data for part system 1 is used.

(2) Tool compensation memory When the common tool compensation memory between part systems is valid, the tool compensation memory used during operation in part system 2 is changed so that part system 1 data is used. Therefore, part system 2 data is not used because part systems are made common. This function is only for the lathe system and supported up to 2 part systems.

(Note) The setting (such as number of axes and axis names) for the tool offset amount of part

system 1 and part system 2 must be the same. If the settings differ, the setting of part system 1 will be applied.

12.1.8.9 2-part System Program Management M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Using parameter (#1050 MemPrg) the machining program can be created for each system, and can be input/output for each system.

12 Programming Support Functions 12.1 Machining Method Support Functions

- 208 -

12.1.9 Data Input by Program

12.1.9.1 Parameter Input by Program M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The parameters set from the setting and display unit can be changed using the machining programs. The format used for the data setting is shown below.

G10 L50 ; ....... Data setting command

P Major classification No. A Axis No. N Data No. H Bit type data ; P Major classification No. A Axis No. N Data No. D Byte type data ; P Major classification No. A Axis No. N Data No. S Word type data ; P Major classification No. A Axis No. N Data No. L 2-word type data ;

G11 ; .. Data setting mode cancel (data setting completed)

The following types of data formats can be used according to the type of parameter (axis- common and axis-independent) and data type.

With axis-common data

Axis-common bit-type parameter --------------------- P N H ; Axis-common byte-type parameter ------------------- P N D ; Axis-common word-type parameter ------------------ P N S ; Axis-common 2-word-type parameter --------------- P N L ;

With axis-independent data

Axis-independent bit-type parameter ---------------- P A N H ; Axis-independent byte-type parameter -------------- P A N D ; Axis-independent word-type parameter ------------- P A N S ; Axis-independent 2-word-type parameter ---------- P A N L ;

(Note 1) The order of addresses in a block must be as shown above. (Note 2) For a bit type parameter, the data type will be H ( is a value between 0 and 7). (Note 3) The axis number is set in the following manner: 1st axis is "1", 2nd axis is "2", and so

forth. When using the 2-part system, the 1st axis in each part system is set as "1", the 2nd axis is set as "2", and so forth.

(Note 4) Command G10L50 and G11 in independent blocks. A program error will occur if not commanded in independent blocks.

Depending on the G90/G91 modal status when the G10 command is assigned, the data is used to overwrite the existing data or added.

Parameter settings in data setting mode

12 Programming Support Functions 12.1 Machining Method Support Functions

- 209 -

12.1.9.2 Compensation Data Input by Program M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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)

The format for the workpiece coordinate system setting commands is shown below.

G10 L2 Pp1 Xx1 Yy1 Zz1 ; G10 L2 Pp1 Xx1, Yy1, Zz1

: Parameter change command : Workpiece coordinate No. : Settings

(Note) L2 can be omitted. Omitting Pp1 results in a program error. [M system]

12 Programming Support Functions 12.1 Machining Method Support Functions

- 210 -

(2) Tool offset input The tool offset amounts, which have been set from the setting and display unit, can be input by

program commands. The command format differs between the [M system] and the [L system]. The respective

command format must be set by a parameter. [M system]

G code Function G10 L10 Tool length shape offset amount G10 L11 Tool length wear offset amount G10 L12 Tool radius shape offset amount G10 L13 Tool radius wear offset amount

The tool offset input format is as follows.

G10 Ll1 Pp1 Rr1 ; G10 Ll1 Pp1 Rr1

: Command for setting offset amount : Offset No. : Offset amount

(Note) When Ll1 has been omitted, the tool length shape offset amount is set. Omitting Pp1 results in a program error.

[L system]

G code Function G10 L10 Tool length offset amount G10 L11 Tool wear offset amount

The tool offset input format is as follows.

G10 L10(L11) Pp1 Xx1 Zz1 Rr1 Qq1 ; G10 L10(L11) Pp1 Xx1 Zz1 Rr1 Qq1

: Command for setting offset amount : Offset No. : X axis offset amount : Z axis offset amount : Nose R compensation amount : Hypothetical tool nose point

12 Programming Support Functions 12.1 Machining Method Support Functions

- 211 -

12.1.10 Machining Modal

12.1.10.1 Tapping Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 Function

G63 Tapping mode ON

The tapping mode command will be canceled with the following commands: Exact stop check mode (G61) Automatic corner override (G62) Cutting mode (G64) High-accuracy control mode command (G61.1) [M system]

The machine is in the cutting mode status when its power is turned on.

12.1.10.2 Cutting Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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) Tapping mode (G63) High-accuracy control mode command (G61.1) [M system]

The machine is in the cutting mode status when its power is turned on.

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 212 -

12.2 Machining Accuracy Support Functions

12.2.1 Automatic Corner Override M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 [M system]

(1) (2) (3)

S

workpiece

Machining allowance

Machining allowance Programmed path (finished shape)

Workpiece surface shape

Tool center path

Tool

: Max. angle at inside corner Ci : Deceleration range (IN)

Ci Deceleration range

Operation (a) When automatic corner override is not to be applied : When the tool moves in the order of (1) (2) (3) in the figure above, the machining

allowance at (3) is larger than that at (2) by an amount equivalent to the area of shaded section S and so the tool load increases.

(b) When automatic corner override is to be applied : When the inside corner angle in the figure above is less than the angle set in the parameter,

the override set into the parameter is automatically applied in the deceleration range Ci.

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 213 -

12.2.2 Deceleration Check The deceleration check function leads the machine to decelerate and stop at the join between one block and another before executing the next block to alleviate the machine shock and to prevent the corner roundness that occurs when the feed rate of the control axis changes suddenly.

Without deceleration check With deceleration check

N010 G01 X100 ; N011 G01 Y-50 ;

Coner rounding occurs because the N011 block is started before the N010 command is completely finished.

N010 G09 G01 X100 ; N011 G01 Y-50 ;

A sharp edge is formed because the N011 block is started after the N010 remaining distance has reached the command deceleration check width or the in-position check width.

The conditions for executing deceleration check are described below. (1) Deceleration check in the rapid traverse mode In the rapid traverse mode, the deceleration check is always performed when block movement

is completed before executing the next block. (2) Deceleration check in the cutting feed mode

In the cutting feed mode, the deceleration check is performed at the end of block when any of the conditions below is applicable before executing the next block. (a) When G61 (exact stop check mode) is selected. (b) When the G09 (exact stop check) is issued in the same block. (c) when the error detect switch (external signal) is ON.

(3) Deceleration check system

Deceleration check is a system that executes the next block only after the command deceleration check is executed as shown below, and it has been confirmed that the position error amount, including the servo system, is less than the in-position check width (designated with parameter or with ",I" in same block).

Previous block

Servo

Command

In-position check widthBlock interpolation completion point

Next block

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 214 -

12.2.2.1 Exact Stop Mode M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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....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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 215 -

12.2.2.4 Programmable Inposition Check M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 216 -

12.2.3 High-Accuracy Control (G61.1) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function controls the operation so the lag will be eliminated in control systems and servo systems. With this function, improved machining accuracy can be realized, especially during high- speed machining, and machining time can be reduced. The high-accuracy control function is a combination of the following element functions.

The high-accuracy control is commanded with ;

G61.1 High-accuracy control ON

R

F

Machining path with a feed forward gain of 70% in high-accuracy control mode Commanded path

Machining path with a feed forward gain of 0% in high-accuracy control mode

Machining path when high-accuracy control mode is OFF

Neat machining of sharp corners without waste is realized with optimum linear acceleration/deceleration and corner judgement.

Effects in G02/G03 circular interpolation

Conventionally X

Y

F

T

Optimum corner deceleration

Conventionally

Optimum corner deceleration

R

R : Command radius (mm)

R: Radius error (mm)

F : Cutting feed rate (m/min)

(1) Acceleration / deceleration before interpolation By accelerating /decelerating before interpolation, the machining shape error can be eliminated with smoothing, and a highly accurate path can be achieved. With the arc commands, the radius reduction error can be significantly minimized. Furthermore, since constant inclination acceleration/deceleration is performed, the time taken for positioning at microscopically small distances in the G00 command is reduced.

(Note 1) Whether acceleration/deceleration before interpolation in the rapid traverse command (G00) is to be performed always or not can be selected using a parameter setting independently from the high-accuracy control assignment.

(2) Optimum corner deceleration By determining the command vector in the machining program and thereby performing corner deceleration, it is possible to machine workpiece with a high-edge accuracy. The figure below shows the pattern of the deceleration speed at the corners. (Optimum corner deceleration is a function of high-accuracy control mode.)

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 217 -

The speed change can be smoothed by the S-shape filter, the machine vibration can be suppressed, and the surface accuracy improved. At the corner, the vector commanded in the machining program is automatically determined, and the speed is decelerated at the corner. A highly accurate edge can be machined by decelerating at the corner.

P

V0

F

Speed

F : Cutting feed rate V0 : Maximum allowable

deceleration speed Deccelerates as far as V0 Inclination of acceleration

/deceleration before interpolation (acceleration)

Time

N001

N002

N001 N002

(3) Feed forward control

Kp

A stable servo contorol with an extremely small servo error can be realized using the feed forward control charactaristic to this CNC system.

Feed forward control

Kp : Position loop gain Kv : Speed loop gain M : Motor S : Differential

Detector

Kv

S

M

(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.

Commanded path

Vector accuracy interpolation

12 Programming Support Functions 12.2 Machining Accuracy Support Functions

- 218 -

(5) Arc entrance/exit speed control There are cases when 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.

12 Programming Support Functions 12.3 Programming Support Functions

- 219 -

12.3 Programming Support Functions

12.3.1 Playback M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

13 Machine Accuracy Compensation 13.1 Static Accuracy Compensation

- 220 -

13 Machine Accuracy Compensation

13.1 Static Accuracy Compensation

13.1.1 Backlash Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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).

13 Machine Accuracy Compensation 13.1 Static Accuracy Compensation

- 221 -

13.1.2 Memory-type Pitch Error Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 (output unit) 2. Number of compensation points : 1024 3. Compensation amount : 128 to 127 pulses (output unit) 4. No. of compensated axes : 10 axes (including number of axes for relative position error compensation)

(1) The compensation position is set for the compensation axis whose reference 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 Compensation

base axis

Division interval

+

R#1

(3) As shown in the figure above, highly individualized compensation control is exercised using the minimum output units with linear approximation for the compensation intervals between the compensation points.

(Note 1) Compensation points 1,024 is a total including the points for memory-type relative position error compensation.

(Note 2) A scale of 0 to 99-fold is applied on the compensation amount.

13 Machine Accuracy Compensation 13.1 Static Accuracy Compensation

- 222 -

13.1.3 Memory-type Relative Position Error Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 (output unit) 2. Number of compensation points : 1024 3. Compensation amount : 128 to 127 pulses (detection unit) 4. No. of compensated axes : 10 axes (including number of axes for memory type pitch error compensation.)

(1) The compensation position is set for the compensation axis whose reference 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 Machine Accuracy Compensation 13.1 Static Accuracy Compensation

- 223 -

13.1.4 External Machine Coordinate System Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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

13.1.5 Circular Radius Error Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

With commands designated during arc cutting, this function compensates for movement toward the inside of the arcs caused by a factor such as servo delay.

13 Machine Accuracy Compensation 13.2 Dynamic Accuracy Compensation

- 224 -

13.2 Dynamic Accuracy Compensation

13.2.1 Smooth High-gain Control (SHG Control) M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S 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 three-fold position loop gain equally compared to the conventional control method. The features of the SHG control are as follows. (1) The acceleration/deceleration becomes smoother, and the mechanical vibration can be

suppressed (approx. 1/2) during acceleration/deceleration. (In other words, the acceleration/deceleration time constant can be shortened.)

6.0

3.0SHG control

Time

Speed

Machine vibration

Step response

SHG control (position loop gain = 50rad/S)

Conventional control (position loop gain = 33rad/S)

Current

Time

Conventional control

Machine vibration amount (m)

(2) The shape error is approx. 1/9 of the conventional control.

SHG control

1.0

Roundness error (m)

Y

X

SHG control + FF

Feed rate 3000mm/min. Radius 50mm 1. Conventional control 2. SHG control 3. SHG control + FF (Feed forward)

2

1

3 Conventional control

22.5

2.5

(3) The positioning time is approx. 1/3 of the conventional control.

200

60

Positioning time (ms)

1. Conventional control 2. SHG control 3. SHG control + FF (Feed forward)

3

Droop

Time

70SHG control

SHG control + FF

Conventional control2 1

Droop during rapid traverse deceleration

13 Machine Accuracy Compensation 13.2 Dynamic Accuracy Compensation

- 225 -

13.2.2 Dual Feedback M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Depending on the frequency, the weight (gain) of the position feedback amount provided by the motor end detector and position feedback amount provided by the machine end detector stands in the correlation shown in the figure below. Semi-closed control is provided on a transient basis whereas positioning can be controlled by the closed status. This function is used to select the primary delay filter time constant during dual feedback control as a parameter setting.

Motor end

Weight (gain) of position feedback amounts

Machine end

0

db

rad/s

1 T

0

db

rad/s

1 T

Time constant T here is adjusted using a parameter.

13.2.3 Lost Motion Compensation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function compensates the error in the protrusion shape caused by lost motion at the arc quadrant changeover section during circular cutting.

14 Automation Support Functions 14.1 External Data Input

- 226 -

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 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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.

14 Automation Support Functions 14.1 External Data Input

- 227 -

14.1.2 External Workpiece Coordinate Offset M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

External workpiece coordinate offset that serves as the reference for all the workpiece coordinate systems is available outside the workpiece coordinates. By setting the external workpiece coordinate offset, the external workpiece coordinate system can be shifted from the machine coordinate system, and all the workpiece coordinate systems can be simultaneously shifted by an amount equivalent to the offset. When the external workpiece coordinate offset is zero, the external workpiece coordinate systems coincide with the machine coordinate system. It is not possible to assign movement commands by selecting the external workpiece coordinates.

Machine coordinate system

External workpiece coordinate

External workpiece coordinate offset

Machine coordinate system (= External workpiece coordinate

Machine coordinate zero point

Workpiece coordinate 4 (G57)

Workpiece coordinate 5 (G58)

Workpiece coordinate 6 (G59)

Workpiece coordinate 1 (G54)

Workpiece coordinate 2 (G55)

Workpiece coordinate 3 (G56)

Workpiece coordinate 4 (G57)

Workpiece coordinate 5 (G58)

Workpiece coordinate 6 (G59)

Workpiece coordinate 1 (G54)

Workpiece coordinate 2 (G55)

Workpiece coordinate 3 (G56)

Machine coordinate zero point

14 Automation Support Functions 14.1 External Data Input

- 228 -

14.1.3 External Tool Offset M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The tool offset amount can be referred and updated from the PLC ladder.

14 Automation Support Functions 14.2 Measurement

- 229 -

14.2 Measurement

14.2.1 Skip

14.2.1.1 Skip M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 ;

G31 : Measurement command Xx1, Yy1, Zz1 : Command values Ff1 : Feed rate

Feed rate

Command value

Actual movement distance

Programmed end point

Skip signal input

Remaining distance

Position

When the G31 command is issued, acceleration/deceleration is accomplished in steps (time constant = 0). There are two types of skip feed rate. 1. Feed rate based on program command when F command is present in program 2. Feed rate based on parameter setting when F command is not present in program

(Note 1) The approximate coasting distance up to feed stop based on the detection delay in the skip signal input is calculated as below.

= (Tp + t) F

60

: Coasting distance (mm) F : G31 rate (mm/min) Tp : Position loop time constant (s) = (position loop gain)1 T : Response delay time of 0.0035 (s)

(Note 2) Skipping during machine lock is not valid.

14 Automation Support Functions 14.2 Measurement

- 230 -

14.2.1.2 Multiple-step Skip M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) G31.n method

This function realizes skipping by designating a combination of skip signals for each skip command (G31.1, G31.2, G31.3). The combination of the skip signals 1, 2 and 3 are designated with parameters for each G code (G31.1, 31.2, 31.3), and the skip operation is executed when all signals in the combination are input. G31.n Xx1 Yy1 Zz1 Ff1 ;

G31.n : Skip command (n=1, 2, 3) Xx1, Yy1, Zz1 : Command format axis coordinate word and target coordinates Ff1 : Feed rate (mm/min)

(2) G31Pn method

As with the G31.n method, the valid skip signal is designated and skip is executed. However, the method of designating the valid skip signal differs. The skip signals that can be used are 1 to 7. 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 7) set with the parameters during the dwell command (G04). G31 Xx1 Yy1 Zz1 Pp1 Ff1 ;

G31 : Skip command Xx1, Yy1, Zz1 : Command format axis coordinate word and target coordinates Pp1 : Skip signal command Ff1 : Feed rate (mm/min)

(a) Specify the skip rate in command feedrate F. However, F modal is not updated. (b) Specify skip signal command in skip signal command P. Specify the P value in the range

of 1 to 127. If it exceeds the specified range, a program error occurs.

14 Automation Support Functions 14.2 Measurement

- 231 -

Table 1 Valid skip signals Valid skip signal

Skip signal command P 7 6 5 4 3 2 1 1

2

3

4

5

6

7

8

: : : : : : : :

125

126

127

14.2.1.4 PLC Skip M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function enables skip operations to be performed by signals which are input from the user PLC.

14 Automation Support Functions 14.2 Measurement

- 232 -

14.2.1.5 Speed Change Skip M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function is used to change the feed rate or to stop the movement by inputting the skip signal during the linear interpolation. After stopping the movement with skipping, the remaining movement command is canceled and the next block is executed. G31 Xx Yy Zz Ff F1 = f1 ... Fn = fn ;

(n is the skip signal 1 to 8.) Xx, Yy, Zz : Command value Ff : Feed rate when starting the cutting feed (mm/min) fn : Feed rate after detecting the skip signal (mm/min)

fn=0: Movement stop fn0: Changing the feed rate to fn

F1=Feed rate after inputting the skip signal 1 ...

F8=Feed rate after inputting the skip signal 8 Operation example

G31 X100. Ff F1=0 F2 = f2 F3 = f3 F4 = f4;

f4

f

Time

f3

f2

0

Skip time constant

Skip signal 4

Skip signal 3

Skip signal 2

Skip signal 1

f1

Position loop time constant (position loop gain1)

Speed

14 Automation Support Functions 14.2 Measurement

- 233 -

14.2.5 Automatic Tool Length Measurement M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Automatic Tool Length Measurement (M system)

This function moves the tool in the direction of the tool measurement position by the commanded value between the measurement start position to the measurement position, it stops the tool as soon as it contacts the sensor and calculates the difference between the coordinates when the tool has stopped and commanded coordinates. It registers this difference as the tool length offset amount for that tool. If compensation has already been applied to the tool, it is moved in the direction of the measurement position with the compensation still applied, and when the measurement and calculation results are such that a further compensation amount is to be provided, the current compensation amount is further corrected. If the compensation amount at this time is one type, the compensation amount is automatically corrected; if there is a distinction between the tool length compensation amount and wear compensation amount, the wear amount is automatically corrected. G37 Z_R_D_F_ ;

Z : Measurement axis address and measurement position coordinate. ... X, Y, Z, (where is an optional axis)

R : The distance between the point at which tool movement is to start at the measurement speed and the measurement position.

D : The range in which the tool is to stop. F : The measurement rate. When R_, D_ and F_ have been omitted, the values set in the parameters are used.

Tool

Tool change position

Tool length measurement position (Za1)

Sensor

Amount of movement based on tool length measurement

Reference position (In case of machine coordinate system zero point.)

At this time, the tool length offset amount has a minus ("") value. Example of program G28 Z0 ; T01 ; M06 T02 ; G43 G00 Z0 H01 ; G37 Z300. R10.D2.F10 ; In this case, the distance (H01 = Za1 z0) from the tool T01 tip to the top of the measurement sensor is calculated as the tool length offset amount which is then registered in the tool offset table.

14 Automation Support Functions 14.2 Measurement

- 234 -

B2

B1 r1

d 1

d1 Measurement position (z 1)

Start point

A

Area A : Moves with rapid traverse feed rate. Areas B1, B2 : Moves with the measurement speed (f1 or parameter setting) If a sensor signal is input in area B1, an error will occur. If a sensor signal is not input in the area B2, an error will occur.

(2) Automatic tool length measurement (L series) This function moves the tool in the direction of the tool measurement position by the commanded value between the measurement start position to the measurement position, it stops the tool as soon as it contacts the sensor and calculates the difference between the coordinates when the tool has stopped and commanded coordinates. It registers this difference as the tool length offset amount for that tool. If compensation has already been applied to the tool, it is moved in the direction of the measurement position with the compensation still applied, and when the measurement and calculation results are such that a further compensation amount is to be provided, the current wear compensation amount is further corrected.

G37 _R_D_F_ ;

: Measurement axis address and measurement position coordinate. ... X, Z R : The distance between the point at which tool movement is to start at the

measurement speed and the measurement position. (Always a radial value: incremental value)

D : The range in which the tool is to stop. (Always a radial value: incremental value) F : The measurement rate. When R_, D_ and F_ have been omitted, the values set in the parameters are used.

14 Automation Support Functions 14.2 Measurement

- 235 -

F feed

Rapid traverse feed

Measuring instrument d1

d1

B

r1

Measurement position

A

Start position

r1, d1, and f1 can also be set in parameters.

When the tool moves from the start position to the measurement position specified in G37 x1 (z1), it passes through the A area at rapid traverse. Then, it moves at the measurement rate set in F command or parameter from the position specified in r1. If the measurement position arrival signal turns ON during the tool is moving in the B area, an error occurs. If the measurement position arrival signal does not turn ON although the tool passes through the measurement position x1 (z1) and moves d1, an error occurs.

14 Automation Support Functions 14.2 Measurement

- 236 -

14.2.6 Manual Tool Length Measurement 1 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Simple measurement of the tool length is done without a sensor. (1) Manual tool length measurement I

[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

Table

Manual movement amount (tool length offset amount)

Workpiece

(2) Manual tool length

measurement I [L system] A measurement position (machine coordinates) to match the tool nose on the machine is preset and the tool nose is set to the measurement position by manual feed, then the operation key is pressed, thereby automatically calculating the tool offset amount and setting it as the tool length offset amount.

X axis tool length

Z axis tool length

X axis

Z axis

Measurement position

Parameter setting

Parameter setting

M

Measurement method (a) Preset the machine coordinates of the measurement position in a given parameter as the

measurement basic value. (b) Select a tool whose tool length offset amount is to be measured. (c) Set the tool nose to the measurement position by manual feed. (d) Press the input key. The tool length offset amount is calculated and displayed on the

setting area. Tool length offset amount = machine coordinates measurement basic value (e) Again press the input key to store the value in the memory as the tool length offset amount

of the tool.

14 Automation Support Functions 14.2 Measurement

- 237 -

14.2.7 Manual Tool Length Measurement 2 M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) Manual tool length measurement II

[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

Gauge block

Table

Basic height

Manual movement amount

Tool length offset amount

TLM basic length (setup parameter)

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

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 tool length

Z axis tool length X axis

touch face

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)

14 Automation Support Functions 14.2 Measurement

- 238 -

14.2.8 Workpiece Coordinate Offset Measurement M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system (*) (*) (*) (*) 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

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.

X axis

Workpiece

Tool post Machine zero point

Z axis

Workpiece coordinate zero point

14 Automation Support Functions 14.2 Measurement

- 239 -

14.2.9 Workpiece Position Measurement M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 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 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.

X

Y

X axis measuremen

X axis measurement constant position

Workpiece coordinate zero point

Y axis measurement constant position

To set the workpiece coordinate offset, the X axis is measured and the X axis offset coordinate is set. Then, the Y axis offset is measured and set. Finally, the Z axis offset is measured and set.

14 Automation Support Functions 14.2 Measurement

- 240 -

(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

Y

Workpiece coordinate zero point

Measurement A point

Measuement B point

Measurement C point

Measurement A point

Measurement C point

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 A point

Measurement B point

Y

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 system after setting two points, and the calculated result is set in the workpiece coordinate offset.

14 Automation Support Functions 14.3 Monitoring

- 241 -

14.3 Monitoring

14.3.1 Tool Life Management Tool Life Management I

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system

(1) M series

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.

Tool Life Management II M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

(1) M series 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. No. of groups: Max. 40 sets (each part system)/ For 1 part system: 80 sets No. of tools in group: Max. 16 tools

14 Automation Support Functions 14.3 Monitoring

- 242 -

14.3.2 Number of Tool Life Management Sets The number of tools that can be managed for their lives are shown below. (These are fixed by the No. of systems according to the model.) 20/40/80 sets

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system L system 80 80 80 80 80 80 80 80

100/200 sets

M64/65/66 M64/65/66S Model M/L system M64A M64 M65 M66 M64AS M64S M65S M66S

M system 100 100 100 100 200 200 200 200 L system

14.3.3 Display of Integrated Time/Number of Parts M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

The number of machined parts is counted up each time a part is machined, and displayed .

Maximum number of workpieces to be machined Number of workpieces machined

Number of workpieces machined

14.3.4 Load Meter M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

Using the user PLC, this function displays the spindle load, Z-axis load, etc. in the form of bar graphs.

14 Automation Support Functions 14.3 Monitoring

- 243 -

14.3.5 Position Switch M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system 8 8 8 8 24 24 24 24 L system 8 8 8 8 24 24 24 24

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 (M60: PSW1 to PSW8, M60S: PSW1 to PSW24). 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 positions Description

dog1 < dog2 dog1 dog2

Signal is output between dog1 and dog2

dog1 > dog2 dog2 dog1

Signal is output between dog2 and dog1

dog1 = dog2 dog1 dog2

Signal is output at the dog1 (dog2) position

PSW width

Basic machine coordinate system zero point

Hypothetical dog

dog1

dog2

14 Automation Support Functions 14.5 Others

- 244 -

14.5 Others

14.5.1 Programmable Current Limitation M64/65/66 M64/65/66S Model

M/L system M64A M64 M65 M66 M64AS M64S M65S M66S M system L system

This function allows the current limit value of the servo axis to be changed to a desired value in the program, and is used for the workpiece stopper, etc. The commanded current limit value is designated with a ratio of the limit current to the rated current. The current limit value can also be set from the D.D.B. function and setting and display unit. The validity of the current limit can be selected with the external signal input. However, the current limit value of the PLC axis cannot be rewritten. G10 L14 X dn ;

L14 : Current limit value setting (+ side/ side) X : Axis address dn : Current limit value 1% to 300%

(1) If the current limit is reached when the current limit is valid, the current limit reached signal is

output. (2) The following two modes can be used with external signals as the operation after the current

limit is reached. Normal mode

The movement command is executed in the current state. During automatic operation, the movement command is executed to the end, and then the next block is moved to with the droops still accumulated.

Interlock mode The movement command is blocked (internal interlock). During automatic operation, the operation stops at the corresponding block, and the next block is not moved to. During manual operation, the following same direction commands are ignored.

(3) During the current limit, the droop generated by the current limit can be canceled with external signals. (Note that the axis must not be moving.)

(4) The setting range of the current limit value is 1% to 300%. Commands that exceed this range will cause a program error. "P35 CMD VALUE OVER" will be displayed.

(5) If a decimal point is designated with the G10 command, only the integer will be valid. (Example) G10 L14 X10.123 ; The current limit value will be set to 10%.

(6) For the axis name "C", the current limit value cannot be set from the program (G10 command). To set from the program, set the axis address with an incremental axis name, or set the axis name to one other than "C".