heidenhain TNC 620 Programming Manual

Download

TNC 620

User’s Manual Cycle Programming

NC Software 817600-02 817601-02 817605-02

English (en) 2/2015

Fundamentals

About this Manual

The symbols used in this manual are described below.

This symbol indicates that important information about the function described must be considered.

WARNING This symbol indicates a possibly

dangerous situation that may cause light injuries if not avoided.

This symbol indicates that there is one or more of the following risks when using the described function:

Danger to workpiece Danger to fixtures Danger to tool Danger to machine Danger to operator

This symbol indicates that the described function must be adapted by the machine tool builder. The function described may therefore vary depending on the machine.

This symbol indicates that you can find detailed information about a function in another manual.

Would you like any changes, or have you found any errors?

We are continuously striving to improve our documentation for you. Please help us by sending your requests to the following e-mail address: tnc-userdoc@heidenhain.de.

TNC 620 | User's Manual Cycle Programming | 2/2015

TNC model, software and features

This manual describes functions and features provided by TNCs as of the following NC software numbers.

TNC model NC software number

TNC 620 817600-02 TNC 620 E 817601-02 TNC 620 Programming Station 817605-02

The suffix E indicates the export version of the TNC. The export version of the TNC has the following limitations:

Simultaneous linear movement in up to 4 axes

The machine tool builder adapts the usable features of the TNC to his machine by setting machine parameters. Some of the functions described in this manual may therefore not be among the features provided by the TNC on your machine tool.

TNC functions that may not be available on your machine include:

Tool measurement with the TT

Please contact your machine tool builder to become familiar with the features of your machine.

Many machine manufacturers, as well as HEIDENHAIN, offer programming courses for the TNCs. We recommend these courses as an effective way of improving your programming skill and sharing information and ideas with other TNC users.

User's Manual:

All TNC functions that have no connection with cycles are described in the User's Manual of the TNC

620. Please contact HEIDENHAIN if you require a copy of this User's Manual.

ID of User's Manual for conversational programming: 1096884-xx.

ID of User’s Manual for DIN/ISO programming: 1096888-xx.

TNC 620 | User's Manual Cycle Programming | 2/2015

Fundamentals

TNC model, software and features

Software options

The TNC 620 features various software options that can be enabled by your machine tool builder. Each option is to be enabled separately and contains the following respective functions:

Additional Axis (option 0 and option 1) Additional axis

Advanced Function Set 1 (option 8) Expanded functions Group 1 Machining with rotary tables

Advanced Function Set 2 (option 9) Expanded functions Group 2 3-D machining:

Additional control loops 1 and 2

Cylindrical contours as if in two axes Feed rate in distance per minute

Coordinate transformations:

Tilting the working plane

Interpolation:

Circle in 3 axes with tilted working plane (spatial arc)

Motion control with minimum jerk 3-D tool compensation through surface normal vectors Using the electronic handwheel to change the angle of the swivel

head during program run without affecting the position of the tool point. (TCPM = Tool Center Point Management)

Keeping the tool normal to the contour Tool radius compensation perpendicular to traversing direction and

tool direction

Interpolation:

Linear in 5 axes (subject to export permit)

Touch Probe Functions (option 17) Touch probe functions

HEIDENHAIN DNC (option number 18)

Advanced Programming Features (option 19) Expanded programming functions FK free contour programming:

Touch probe cycles:

Compensation of tool misalignment in automatic mode Datum setting in the Manual Operation mode Datum setting in automatic mode Automatically measuring workpieces Tools can be measured automatically

Communication with external PC applications over COM component

Programming in HEIDENHAIN conversational format with graphic support for workpiece drawings not dimensioned for NC

TNC 620 | User's Manual Cycle Programming | 2/2015

Advanced Programming Features (option 19)

Fixed cycles:

Peck drilling, reaming, boring, counterboring, centering (cycles 201 to 205, 208, 240, 241)

Milling of internal and external threads (cycles 262 to 265, 267) Finishing of rectangular and circular pockets and studs (cycles 212 to

215, 251 to 257) Clearing level and oblique surfaces (cycles 230 to 233) Straight slots and circular slots (cycles 210, 211, 253, 254) Linear and circular point patterns (cycles 220, 221) Contour train, contour pocket—also with contour-parallel machining,

trochoidal slot (cycles 20 to 25, 275) Engraving (cycle 225) OEM cycles (special cycles developed by the machine tool builder)

can be integrated

TNC model, software and features

Advanced Graphic Features (option 20) Expanded graphic functions Program-verification graphics, program-run graphics

Plan view Projection in three planes 3-D view

Advanced Function Set 3 (option 21) Expanded functions Group 3 Tool compensation:

M120: Radius-compensated contour look-ahead for up to 99 blocks

3-D machining:

M118: Superimpose handwheel positioning during program run

Pallet Management (option 22) Pallet management

Display Step (option 23) Display step Input resolution:

Linear axes down to 0.01 µm Rotary axes to 0.00001°

DXF Converter (option 42) DXF converter

KinematicsOpt (option 48) Optimizing the machine

kinematics

TNC 620 | User's Manual Cycle Programming | 2/2015

Supported DXF format: AC1009 (AutoCAD R12) Adoption of contours and point patterns Simple and convenient specification of reference points Select graphical features of contour sections from conversational

programs

Backup/restore active kinematics Test active kinematics Optimize active kinematics

Fundamentals

Extended Tool Management (option 93) Extended tool management Python-based

Remote Desktop Manager (option 133)

TNC model, software and features

Remote operation of external computer units

Cross Talk Compensation – CTC (option 141) Compensation of axis couplings

Position Adaptive Control – PAC (option 142) Adaptive position control

Load Adaptive Control – LAC (option 143) Adaptive load control

Active Chatter Control – ACC (option 145) Active chatter control Fully automatic function for chatter control during machining

Windows on a separate computer unit Incorporated in the TNC interface

Determination of dynamically caused position deviation through axis acceleration

Compensation of TCP (Tool Center Point)

Changing of the control parameters depending on the position of the axes in the working space

Changing of the control parameters depending on the speed or acceleration of an axis

Automatic determination of workpiece weight and frictional forces Changing of control parameters depending on the actual mass of

the workpiece

TNC 620 | User's Manual Cycle Programming | 2/2015

TNC model, software and features

Feature Content Level (upgrade functions)

Along with software options, significant further improvements of the TNC software are managed via the Feature Content Level upgrade functions. Functions subject to the FCL are not available simply by updating the software on your TNC.

All upgrade functions are available to you without surcharge when you receive a new machine.

Upgrade functions are identified in the manual with FCL n, where n indicates the sequential number of the feature content level.

You can purchase a code number in order to permanently enable the FCL functions. For more information, contact your machine tool builder or HEIDENHAIN.

Intended place of operation

The TNC complies with the limits for a Class A device in accordance with the specifications in EN 55022, and is intended for use primarily in industrially-zoned areas.

Legal information

This product uses open source software. Further information is available on the control under

Programming and Editing operating mode MOD function LICENSE INFO softkey

TNC 620 | User's Manual Cycle Programming | 2/2015

Fundamentals

Optional parameters

The comprehensive cycle package is continuously further developed by HEIDENHAIN. Every new software version thus may also introduce new Q parameters for cycles. These new Q parameters are optional parameters, some of which have not been available in previous software versions. Within a cycle, they are always provided at the end of the cycle definition. You will find an overview of the optional Q parameters that have been added with this software version in the "New and changed cycle functions of software 81760x-02" section. You can choose whether to define optional Q parameters or delete them with the NO ENT key. You can also adopt the default value. If you have accidentally deleted an optional Q parameter or if you would like to extend cycles in your existing programs after a software update, you can include optional Q parameters in cycles when needed. The following steps describe how this is done:

To insert optional Q parameters in existing programs:

Call the cycle definition Press the right arrow key until the new Q parameters are

displayed Apply the default value or enter a value To transfer the new Q parameter, exit the menu by pressing

the right arrow key once again or by pressing END If you do not wish to apply the new Q parameter, press the

NO ENT key

Compatibility

The majority of part programs created on older HEIDENHAIN contouring controls (TNC 150 B and higher) can be executed with this new software version of the TNC 620. Even if new, optional parameters ("Optional parameters") have been added to existing cycles, you can normally continue running your programs as usual. This is achieved by using the stored default value. The other way round, if a program created with a new software version is to be run on an older control, you can delete the respective optional Q parameters from the cycle definition with the NO ENT key. In this way you can ensure that the program will be downward compatible. If NC blocks contain invalid elements, the TNC will mark them as ERROR blocks when the file is opened.

TNC 620 | User's Manual Cycle Programming | 2/2015

New cycle functions of software 81760x-01

The character set of the fixed cycle 225 Engraving was expanded by more characters and the diameter sign see "ENGRAVING (Cycle 225, DIN/ISO: G225)", page 280

New fixed cycle 275 Trochoidal Milling see "TROCHOIDAL SLOT (Cycle 275, DIN ISO G275, software option 19)", page 206

New fixed cycle 233 Face Milling see "FACE MILLING (Cycle 233, DIN/ISO: G233, software option 19)", page 161

In Cycle 205 Universal Pecking you can now use parameter Q208 to define a feed rate for retraction see "Cycle parameters", page 86

In the thread milling cycles 26x an approaching feed rate was introduced see "Cycle parameters", page 113

The parameter Q305 NUMBER IN TABLE was added to Cycle 404 see "Cycle parameters", page 316

In the drilling cycles 200, 203 and 205 the parameter Q395 DEPTH REFERENCE was introduced in order to evaluate the T ANGLE see "Cycle parameters", page 86

Cycle 241 SINGLE-LIP DEEP HOLE DRILLING was expanded by several input parameters see "SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241, software option 19)", page 91

The probing cycle 4 MEASURING IN 3-D was introduced see "MEASURING IN 3-D (Cycle 4, software option 17)", page 423

TNC 620 | User's Manual Cycle Programming | 2/2015

Fundamentals

New and changed cycle functions of software 81760x-02

New Load Adaptive Control (LAC) cycle for the load-dependent adaptation of control parameters (software option 143), see "ASCERTAIN THE LOAD (Cycle 239, DIN/ISO: G239, software option 143)", page 289

Cycle 270: CONTOUR TRAIN DATA was added to the cycle package (software option 19), see "CONTOUR TRAIN DATA (Cycle 270, DIN/ISO: G270, software option 19)", page 204

Cycle 39 CYLINDER SURFACE (software option 1) Contour was added to the cycle package, see "CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1)", page 226

The character set of the fixed cycle 225 Engraving was expanded by the CE, ß and @ characters and the system time, see "ENGRAVING (Cycle 225, DIN/ISO: G225)", page 280

Cycles 252 to 254 (software option 19) were expanded by the optional parameter Q439, see "Cycle parameters", page 142

Cycle 22 (software option 19) was expanded by the optional parameters Q401 and Q404, see "ROUGHING (Cycle 22, DIN/ ISO: G122, software option 19)", page 193

Cycle 484 (software option 17) was expanded by the optional parameter Q536, see "Calibrating the wireless TT 449 (Cycle 484, DIN/ISO: G484, DIN/ISO: G484, Option 17)", page 475

TNC 620 | User's Manual Cycle Programming | 2/2015

1 Fundamentals / Overviews............................................................................................................43

2 Using Fixed Cycles......................................................................................................................... 47

3 Fixed Cycles: Drilling......................................................................................................................67

4 Fixed Cycles: Tapping / Thread Milling........................................................................................ 97

5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling........................................................133

6 Fixed Cycles: Pattern Definitions................................................................................................ 171

7 Fixed Cycles: Contour Pocket......................................................................................................181

8 Fixed Cycles: Cylindrical Surface................................................................................................ 215

9 Fixed Cycles: Contour Pocket with Contour Formula...............................................................233

10 Cycles: Coordinate Transformations...........................................................................................247

11 Cycles: Special Functions............................................................................................................ 271

12 Using Touch Probe Cycles........................................................................................................... 291

13 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment.......................... 301

14 Touch Probe Cycles: Automatic Datum Setting........................................................................ 323

15 Touch Probe Cycles: Automatic Workpiece Inspection.............................................................377

16 Touch Probe Cycles: Special Functions......................................................................................419

17 Touch Probe Cycles: Automatic Kinematics Measurement......................................................435

18 Touch Probe Cycles: Automatic Tool Measurement..................................................................467

19 Tables of Cycles............................................................................................................................ 483

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

TNC 620 | User's Manual Cycle Programming | 2/2015

1 Fundamentals / Overviews............................................................................................................43

1.1 Introduction............................................................................................................................................44

1.2 Available Cycle Groups.........................................................................................................................45

Overview of fixed cycles........................................................................................................................ 45

Overview of touch probe cycles.............................................................................................................46

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

2 Using Fixed Cycles......................................................................................................................... 47

2.1 Working with fixed cycles....................................................................................................................48

Machine-specific cycles (software option19).......................................................................................... 48

Defining a cycle using soft keys.............................................................................................................49

Defining a cycle using the GOTO function............................................................................................. 49

Calling a cycle......................................................................................................................................... 50

2.2 Program defaults for cycles................................................................................................................. 52

Overview................................................................................................................................................. 52

Entering GLOBAL DEF............................................................................................................................52

Using GLOBAL DEF information............................................................................................................ 53

Global data valid everywhere..................................................................................................................54

Global data for drilling operations........................................................................................................... 54

Global data for milling operations with pocket cycles 25x..................................................................... 54

Global data for milling operations with contour cycles...........................................................................55

Global data for positioning behavior....................................................................................................... 55

Global data for probing functions........................................................................................................... 55

2.3 PATTERN DEF pattern definition......................................................................................................... 56

Application...............................................................................................................................................56

Entering PATTERN DEF.......................................................................................................................... 57

Using PATTERN DEF...............................................................................................................................57

Defining individual machining positions.................................................................................................. 58

Defining a single row..............................................................................................................................58

Defining a single pattern.........................................................................................................................59

Defining individual frames.......................................................................................................................60

Defining a full circle................................................................................................................................61

Defining a pitch circle............................................................................................................................. 62

2.4 Point tables............................................................................................................................................63

Application...............................................................................................................................................63

Creating a point table............................................................................................................................. 63

Hiding single points from the machining process.................................................................................. 64

Selecting a point table in the program................................................................................................... 64

Calling a cycle in connection with point tables...................................................................................... 65

TNC 620 | User's Manual Cycle Programming | 2/2015

3 Fixed Cycles: Drilling......................................................................................................................67

3.1 Fundamentals........................................................................................................................................ 68

Overview................................................................................................................................................. 68

3.2 CENTERING (Cycle 240, DIN/ISO: G240, software option 19)..........................................................69

Cycle run................................................................................................................................................. 69

Please note while programming:............................................................................................................69

Cycle parameters.................................................................................................................................... 70

3.3 DRILLING (Cycle 200)............................................................................................................................71

Cycle run................................................................................................................................................. 71

Please note while programming:............................................................................................................71

Cycle parameters.................................................................................................................................... 72

3.4 REAMING (Cycle 201, DIN/ISO: G201, software option 19).............................................................. 73

Cycle run................................................................................................................................................. 73

Please note while programming:............................................................................................................73

Cycle parameters.................................................................................................................................... 74

3.5 BORING (Cycle 202, DIN/ISO: G202, software option 19).................................................................75

Cycle run................................................................................................................................................. 75

Please note while programming:............................................................................................................76

Cycle parameters.................................................................................................................................... 77

3.6 UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203, software option 19).........................................78

Cycle run................................................................................................................................................. 78

Please note while programming:............................................................................................................78

Cycle parameters.................................................................................................................................... 79

3.7 BACK BORING (Cycle 204, DIN/ISO: G204, software option 19)......................................................81

Cycle run................................................................................................................................................. 81

Please note while programming:............................................................................................................82

Cycle parameters.................................................................................................................................... 83

3.8 UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205, software option 19)..........................................84

Cycle run................................................................................................................................................. 84

Please note while programming:............................................................................................................85

Cycle parameters.................................................................................................................................... 86

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

3.9 BORE MILLING (Cycle 208, software option 19)................................................................................88

Cycle run................................................................................................................................................. 88

Please note while programming:............................................................................................................89

Cycle parameters.................................................................................................................................... 90

3.10 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241, software option 19)......................91

Cycle run................................................................................................................................................. 91

Please note while programming:............................................................................................................91

Cycle parameters.................................................................................................................................... 92

3.11 Programming Examples....................................................................................................................... 94

Example: Drilling cycles.......................................................................................................................... 94

Example: Using drilling cycles in connection with PATTERN DEF..........................................................95

TNC 620 | User's Manual Cycle Programming | 2/2015

4 Fixed Cycles: Tapping / Thread Milling........................................................................................ 97

4.1 Fundamentals........................................................................................................................................ 98

Overview................................................................................................................................................. 98

4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206).....................................................99

Cycle run................................................................................................................................................. 99

Please note while programming:..........................................................................................................100

Cycle parameters.................................................................................................................................. 101

4.3 RIGID TAPPING without a floating tap holder (Cycle 207, DIN/ISO: G207)................................... 102

Cycle run............................................................................................................................................... 102

Please note while programming:..........................................................................................................103

Cycle parameters.................................................................................................................................. 104

Retracting after a program interruption................................................................................................ 104

4.4 TAPPING WITH CHIP BREAKING (Cycle 209, DIN/ISO: G209, software option 19).......................105

Cycle run............................................................................................................................................... 105

Please note while programming:..........................................................................................................106

Cycle parameters.................................................................................................................................. 107

4.5 Fundamentals of Thread Milling....................................................................................................... 109

Prerequisites..........................................................................................................................................109

4.6 THREAD MILLING (Cycle 262, DIN/ISO: G262, software option 19)...............................................111

Cycle run............................................................................................................................................... 111

Please note while programming:..........................................................................................................112

Cycle parameters.................................................................................................................................. 113

4.7 THREAD MILLING/COUNTERSINKING (Cycle 263, DIN/ISO:G263, software option 19)..............114

Cycle run............................................................................................................................................... 114

Please note while programming:..........................................................................................................115

Cycle parameters.................................................................................................................................. 116

4.8 THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264, software option 19).............................118

Cycle run............................................................................................................................................... 118

Please note while programming:..........................................................................................................119

Cycle parameters.................................................................................................................................. 120

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

4.9 HELICAL THREAD DRILLING/MILLING (Cycle 265, DIN/ISO: G265, software option 19)............. 122

Cycle run............................................................................................................................................... 122

Please note while programming:..........................................................................................................123

Cycle parameters.................................................................................................................................. 124

4.10 OUTSIDE THREAD MILLING (Cycle 267, DIN/ISO: G267, software option 19)...............................126

Cycle run............................................................................................................................................... 126

Please note while programming:..........................................................................................................127

Cycle parameters.................................................................................................................................. 128

4.11 Programming Examples..................................................................................................................... 130

Example: Thread milling........................................................................................................................130

TNC 620 | User's Manual Cycle Programming | 2/2015

5 Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling........................................................133

5.1 Fundamentals...................................................................................................................................... 134

Overview............................................................................................................................................... 134

5.2 RECTANGULAR POCKET (Cycle 251, DIN/ISO: G251, software option 19)................................... 135

Cycle run............................................................................................................................................... 135

Please note while programming:..........................................................................................................136

Cycle parameters.................................................................................................................................. 137

5.3 CIRCULAR POCKET (Cycle 252, DIN/ISO: G252, software option 19)............................................139

Cycle run............................................................................................................................................... 139

Please note while programming:..........................................................................................................141

Cycle parameters.................................................................................................................................. 142

5.4 SLOT MILLING (Cycle 253, DIN/ISO: G253), Software Option 19...................................................144

Cycle run............................................................................................................................................... 144

Please note while programming:..........................................................................................................145

Cycle parameters.................................................................................................................................. 146

5.5 CIRCULAR SLOT (Cycle 254, DIN/ISO: G254, software option 19).................................................148

Cycle run............................................................................................................................................... 148

Please note while programming:..........................................................................................................149

Cycle parameters.................................................................................................................................. 150

5.6 RECTANGULAR STUD (Cycle 256, DIN/ISO: G256, software option 19)....................................... 153

Cycle run............................................................................................................................................... 153

Please note while programming:..........................................................................................................154

Cycle parameters.................................................................................................................................. 155

5.7 CIRCULAR STUD (Cycle 257, DIN/ISO: G257, software option 19)................................................. 157

Cycle run............................................................................................................................................... 157

Please note while programming:..........................................................................................................157

Cycle parameters.................................................................................................................................. 159

5.8 FACE MILLING (Cycle 233, DIN/ISO: G233, software option 19)....................................................161

Cycle run............................................................................................................................................... 161

Please note while programming:..........................................................................................................164

Cycle parameters.................................................................................................................................. 165

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

5.9 Programming Examples..................................................................................................................... 168

Example: Milling pockets, studs and slots........................................................................................... 168

TNC 620 | User's Manual Cycle Programming | 2/2015

6 Fixed Cycles: Pattern Definitions................................................................................................ 171

6.1 Fundamentals...................................................................................................................................... 172

Overview............................................................................................................................................... 172

6.2 POLAR PATTERN (Cycle 220, DIN/ISO: G220, software option 19)................................................ 173

Cycle run............................................................................................................................................... 173

Please note while programming:..........................................................................................................173

Cycle parameters.................................................................................................................................. 174

6.3 LINEAR PATTERN (Cycle 221, DIN/ISO: G221, software option 19)............................................... 176

Cycle run............................................................................................................................................... 176

Please note while programming:..........................................................................................................176

Cycle parameters.................................................................................................................................. 177

6.4 Programming Examples..................................................................................................................... 178

Example: Polar hole patterns................................................................................................................ 178

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

7 Fixed Cycles: Contour Pocket......................................................................................................181

7.1 SL Cycles..............................................................................................................................................182

Fundamentals........................................................................................................................................182

Overview............................................................................................................................................... 183

7.2 CONTOUR (Cycle 14, DIN/ISO: G37).................................................................................................184

Please note while programming:..........................................................................................................184

Cycle parameters.................................................................................................................................. 184

7.3 Superimposed contours..................................................................................................................... 185

Fundamentals........................................................................................................................................185

Subprograms: overlapping pockets.......................................................................................................185

Area of inclusion................................................................................................................................... 186

Area of exclusion.................................................................................................................................. 187

Area of intersection.............................................................................................................................. 188

7.4 CONTOUR DATA (Cycle 20, DIN/ISO: G120, software option 19)...................................................189

Please note while programming:..........................................................................................................189

Cycle parameters.................................................................................................................................. 190

7.5 PILOT DRILLING (Cycle 21, DIN/ISO: G121, software option 19)................................................... 191

Cycle run............................................................................................................................................... 191

Please note while programming:..........................................................................................................192

Cycle parameters.................................................................................................................................. 192

7.6 ROUGHING (Cycle 22, DIN/ISO: G122, software option 19)........................................................... 193

Cycle run............................................................................................................................................... 193

Please note while programming:..........................................................................................................194

Cycle parameters.................................................................................................................................. 195

7.7 FLOOR FINISHING (Cycle 23, DIN/ISO: G123, software option 19)................................................197

Cycle run............................................................................................................................................... 197

Please note while programming:..........................................................................................................197

Cycle parameters.................................................................................................................................. 198

7.8 SIDE FINISHING (Cycle 24, DIN/ISO: G124, software option 19)................................................... 199

Cycle run............................................................................................................................................... 199

Please note while programming:..........................................................................................................200

Cycle parameters.................................................................................................................................. 201

TNC 620 | User's Manual Cycle Programming | 2/2015

7.9 CONTOUR TRAIN (Cycle 25, DIN/ISO: G125, software option 19)................................................. 202

Cycle run............................................................................................................................................... 202

Please note while programming:..........................................................................................................202

Cycle parameters.................................................................................................................................. 203

7.10 CONTOUR TRAIN DATA (Cycle 270, DIN/ISO: G270, software option 19).....................................204

Please note while programming:..........................................................................................................204

Cycle parameters.................................................................................................................................. 205

7.11 TROCHOIDAL SLOT (Cycle 275, DIN ISO G275, software option 19)............................................. 206

Cycle run............................................................................................................................................... 206

Please note while programming:..........................................................................................................207

Cycle parameters.................................................................................................................................. 208

7.12 Programming Examples..................................................................................................................... 210

Example: Roughing-out and fine-roughing a pocket............................................................................. 210

Example: Pilot drilling, roughing-out and finishing overlapping contours..............................................212

Example: Contour train......................................................................................................................... 214

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

8 Fixed Cycles: Cylindrical Surface................................................................................................ 215

8.1 Fundamentals...................................................................................................................................... 216

Overview of cylindrical surface cycles..................................................................................................216

8.2 CYLINDER SURFACE (Cycle 27, DIN/ISO: G127, software option 1)............................................... 217

Cycle run............................................................................................................................................... 217

Please note while programming:..........................................................................................................218

Cycle parameters.................................................................................................................................. 219

8.3 CYLINDER SURFACE Slot milling (Cycle 28, DIN/ISO: G128, software option 1)......................... 220

Cycle run............................................................................................................................................... 220

Please note while programming:..........................................................................................................221

Cycle parameters.................................................................................................................................. 222

8.4 CYLINDER SURFACE Ridge milling (Cycle 29, DIN/ISO: G129, software option 1).......................223

Cycle run............................................................................................................................................... 223

Please note while programming:..........................................................................................................224

Cycle parameters.................................................................................................................................. 225

8.5 CYLINDER SURFACE (Cycle 39, DIN/ISO: G139, software option 1)..............................................226

Cycle run............................................................................................................................................... 226

Please note while programming:..........................................................................................................227

Cycle parameters.................................................................................................................................. 228

8.6 Programming Examples..................................................................................................................... 229

Example: Cylinder surface with Cycle 27............................................................................................. 229

Example: Cylinder surface with Cycle 28............................................................................................. 231

TNC 620 | User's Manual Cycle Programming | 2/2015

9 Fixed Cycles: Contour Pocket with Contour Formula...............................................................233

9.1 SL cycles with complex contour formula.........................................................................................234

Fundamentals........................................................................................................................................234

Selecting a program with contour definitions.......................................................................................236

Defining contour descriptions............................................................................................................... 236

Entering a complex contour formula.................................................................................................... 237

Superimposed contours........................................................................................................................ 238

Contour machining with SL Cycles.......................................................................................................240

Example: Roughing and finishing superimposed contours with the contour formula...........................241

9.2 SL cycles with simple contour formula............................................................................................244

Fundamentals........................................................................................................................................244

Entering a simple contour formula....................................................................................................... 246

Contour machining with SL Cycles.......................................................................................................246

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

10 Cycles: Coordinate Transformations...........................................................................................247

10.1 Fundamentals...................................................................................................................................... 248

Overview............................................................................................................................................... 248

Effect of coordinate transformations.................................................................................................... 248

10.2 DATUM SHIFT (Cycle 7, DIN/ISO: G54)............................................................................................. 249

Effect..................................................................................................................................................... 249

Cycle parameters.................................................................................................................................. 249

10.3 DATUM SHIFT with datum tables (Cycle 7, DIN/ISO: G53)............................................................. 250

Effect..................................................................................................................................................... 250

Please note while programming:..........................................................................................................251

Cycle parameters.................................................................................................................................. 251

Selecting a datum table in the part program........................................................................................252

Edit the datum table in the Programming mode of operation..............................................................252

Configuring the datum table................................................................................................................. 254

To exit a datum table............................................................................................................................ 254

Status displays...................................................................................................................................... 254

10.4 DATUM SETTING (Cycle 247, DIN/ISO: G247)..................................................................................255

Effect..................................................................................................................................................... 255

Please note before programming:........................................................................................................ 255

Cycle parameters.................................................................................................................................. 255

Status displays...................................................................................................................................... 255

10.5 MIRRORING (Cycle 8, DIN/ISO: G28)................................................................................................ 256

Effect..................................................................................................................................................... 256

Please note while programming...........................................................................................................257

Cycle parameters.................................................................................................................................. 257

10.6 ROTATION (Cycle 10, DIN/ISO: G73)................................................................................................. 258

Effect..................................................................................................................................................... 258

Please note while programming:..........................................................................................................259

Cycle parameters.................................................................................................................................. 259

10.7 SCALING (Cycle 11, DIN/ISO: G72.................................................................................................... 260

Effect..................................................................................................................................................... 260

Cycle parameters.................................................................................................................................. 260

TNC 620 | User's Manual Cycle Programming | 2/2015

10.8 AXIS-SPECIFIC SCALING (Cycle 26).................................................................................................. 261

Effect..................................................................................................................................................... 261

Please note while programming:..........................................................................................................261

Cycle parameters.................................................................................................................................. 262

10.9 WORKING PLANE (Cycle 19, DIN/ISO: G80, software option 1).....................................................263

Effect..................................................................................................................................................... 263

Please note while programming:..........................................................................................................264

Cycle parameters.................................................................................................................................. 264

Resetting............................................................................................................................................... 265

Positioning the axes of rotation............................................................................................................ 265

Position display in the tilted system.....................................................................................................266

Workspace monitoring.......................................................................................................................... 266

Positioning in a tilted coordinate system..............................................................................................267

Combining coordinate transformation cycles........................................................................................267

Procedure for working with Cycle 19 WORKING PLANE..................................................................... 268

10.10 Programming Examples..................................................................................................................... 269

Example: Coordinate transformation cycles......................................................................................... 269

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

11 Cycles: Special Functions............................................................................................................ 271

11.1 Fundamentals...................................................................................................................................... 272

Overview............................................................................................................................................... 272

11.2 DWELL TIME (Cycle 9, DIN/ISO: G04)...............................................................................................273

Function.................................................................................................................................................273

Cycle parameters.................................................................................................................................. 273

11.3 PROGRAM CALL (Cycle 12, DIN/ISO: G39).......................................................................................274

Cycle function........................................................................................................................................274

Please note while programming:..........................................................................................................274

Cycle parameters.................................................................................................................................. 275

11.4 SPINDLE ORIENTATION (Cycle 13, DIN/ISO: G36)...........................................................................276

Cycle function........................................................................................................................................276

Please note while programming:..........................................................................................................276

Cycle parameters.................................................................................................................................. 276

11.5 TOLERANCE (Cycle 32, DIN/ISO: G62)..............................................................................................277

Cycle function........................................................................................................................................277

Influences of the geometry definition in the CAM system..................................................................277

Please note while programming:..........................................................................................................278

Cycle parameters.................................................................................................................................. 279

11.6 ENGRAVING (Cycle 225, DIN/ISO: G225)..........................................................................................280

Cycle run............................................................................................................................................... 280

Please note while programming:..........................................................................................................280

Cycle parameters.................................................................................................................................. 281

Allowed engraving characters............................................................................................................... 282

Characters that cannot be printed........................................................................................................ 282

Engraving system variables...................................................................................................................283

11.7 FACE MILLING (Cycle 232, DIN/ISO: G232, software option 19)....................................................284

Cycle run............................................................................................................................................... 284

Please note while programming:..........................................................................................................286

Cycle parameters.................................................................................................................................. 287

TNC 620 | User's Manual Cycle Programming | 2/2015

11.8 ASCERTAIN THE LOAD (Cycle 239, DIN/ISO: G239, software option 143).................................... 289

Cycle run............................................................................................................................................... 289

Please note while programming:..........................................................................................................289

Cycle parameters.................................................................................................................................. 290

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

12 Using Touch Probe Cycles........................................................................................................... 291

12.1 General information about touch probe cycles............................................................................... 292

Method of function............................................................................................................................... 292

Consideration of a basic rotation in the Manual Operation mode........................................................292

Touch probe cycles in the Manual Operation and Electronic Handwheel operating modes................. 292

Touch probe cycles for automatic operation.........................................................................................293

12.2 Before You Start Working with Touch Probe Cycles....................................................................... 295

Maximum traverse to touch point: DIST in touch probe table..............................................................295

Set-up clearance to touch point: SET_UP in touch probe table............................................................295

Orient the infrared touch probe to the programmed probe direction: TRACK in touch probe table...... 295

Touch trigger probe, probing feed rate: F in touch probe table............................................................ 296

Touch trigger probe, rapid traverse for positioning: FMAX................................................................... 296

Touch trigger probe, rapid traverse for positioning: F_PREPOS in touch probe table........................... 296

Multiple measurements........................................................................................................................ 297

Confidence interval of multiple measurements....................................................................................297

Executing touch probe cycles............................................................................................................... 298

12.3 Touch probe table............................................................................................................................... 299

General information...............................................................................................................................299

Editing touch probe tables....................................................................................................................299

Touch probe data...................................................................................................................................300

TNC 620 | User's Manual Cycle Programming | 2/2015

13 Touch Probe Cycles: Automatic Measurement of Workpiece Misalignment.......................... 301

13.1 Fundamentals...................................................................................................................................... 302

Overview............................................................................................................................................... 302

Characteristics common to all touch probe cycles for measuring workpiece misalignment.................303

13.2 BASIC ROTATION (Cycle 400, DIN/ISO: G400, software option 17)............................................... 304

Cycle run............................................................................................................................................... 304

Please note while programming:..........................................................................................................304

Cycle parameters.................................................................................................................................. 305

13.3 BASIC ROTATION over two holes (Cycle 401, DIN/ISO: G401, software option 17)......................307

Cycle run............................................................................................................................................... 307

Please note while programming:..........................................................................................................307

Cycle parameters.................................................................................................................................. 308

13.4 BASIC ROTATION over two studs (Cycle 402, DIN/ISO: G402, software option 17)..................... 310

Cycle run............................................................................................................................................... 310

Please note while programming:..........................................................................................................310

Cycle parameters.................................................................................................................................. 311

13.5 BASIC ROTATION compensation via rotary axis (Cycle 403, DIN/ISO: G403, software option

17)..........................................................................................................................................................313

Cycle run............................................................................................................................................... 313

Please note while programming:..........................................................................................................313

Cycle parameters.................................................................................................................................. 314

13.6 SET BASIC ROTATION (Cycle 404, DIN/ISO: G404, software option 17)........................................316

Cycle run............................................................................................................................................... 316

Cycle parameters.................................................................................................................................. 316

13.7 Compensating workpiece misalignment by rotating the C axis (Cycle 405, DIN/ISO: G405,

software option 17).............................................................................................................................317

Cycle run............................................................................................................................................... 317

Please note while programming:..........................................................................................................318

Cycle parameters.................................................................................................................................. 319

13.8 Example: Determining a basic rotation from two holes.................................................................321

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

14 Touch Probe Cycles: Automatic Datum Setting........................................................................ 323

14.1 Fundamentals...................................................................................................................................... 324

Overview............................................................................................................................................... 324

Characteristics common to all touch probe cycles for datum setting...................................................326

14.2 DATUM SLOT CENTER (Cycle 408, DIN/ISO: G408, software option 17).......................................328

Cycle run............................................................................................................................................... 328

Please note while programming:..........................................................................................................329

Cycle parameters.................................................................................................................................. 330

14.3 DATUM RIDGE CENTER (Cycle 409, DIN/ISO: G409, software option 17).....................................332

Cycle run............................................................................................................................................... 332

Please note while programming:..........................................................................................................332

Cycle parameters.................................................................................................................................. 333

14.4 DATUM FROM INSIDE OF RECTANGLE (Cycle 410, DIN/ISO: G410, software option 17).............335

Cycle run............................................................................................................................................... 335

Please note while programming:..........................................................................................................336

Cycle parameters.................................................................................................................................. 337

14.5 DATUM FROM OUTSIDE OF RECTANGLE (Cycle 411, DIN/ISO: G411, software option 17)......... 339

Cycle run............................................................................................................................................... 339

Please note while programming:..........................................................................................................339

Cycle parameters.................................................................................................................................. 340

14.6 DATUM FROM INSIDE OF CIRCLE (Cycle 412, DIN/ISO: G412, software option 17).....................342

Cycle run............................................................................................................................................... 342

Please note while programming:..........................................................................................................343

Cycle parameters.................................................................................................................................. 344

14.7 DATUM FROM OUTSIDE OF CIRCLE (Cycle 413, DIN/ISO: G413, software option 17).................347

Cycle run............................................................................................................................................... 347

Please note while programming:..........................................................................................................347

Cycle parameters.................................................................................................................................. 348

14.8 DATUM FROM OUTSIDE OF CORNER (Cycle 414, DIN/ISO: G414, software option 17).............. 351

Cycle run............................................................................................................................................... 351

Please note while programming:..........................................................................................................352

Cycle parameters.................................................................................................................................. 353

TNC 620 | User's Manual Cycle Programming | 2/2015

14.9 DATUM FROM INSIDE OF CORNER (Cycle 415, DIN/ISO: G415, software option 17).................. 356

Cycle run............................................................................................................................................... 356

Please note while programming:..........................................................................................................357

Cycle parameters.................................................................................................................................. 358

14.10DATUM CIRCLE CENTER (Cycle 416, DIN/ISO: G416, software option 17)....................................360

Cycle run............................................................................................................................................... 360

Please note while programming:..........................................................................................................361

Cycle parameters.................................................................................................................................. 362

14.11DATUM IN TOUCH PROBE AXIS (Cycle 417, DIN/ISO: G417, software option 17).........................364

Cycle run............................................................................................................................................... 364

Please note while programming:..........................................................................................................364

Cycle parameters.................................................................................................................................. 365

14.12DATUM AT CENTER OF 4 HOLES (Cycle 418, DIN/ISO: G418, software option 17)...................... 366

Cycle run............................................................................................................................................... 366

Please note while programming:..........................................................................................................367

Cycle parameters.................................................................................................................................. 368

14.13DATUM IN ONE AXIS (Cycle 419, DIN/ISO: G419, software option 17).........................................370

Cycle run............................................................................................................................................... 370

Please note while programming:..........................................................................................................370

Cycle parameters.................................................................................................................................. 371

14.14Example: Datum setting in center of a circular segment and on top surface of workpiece.........373

14.15Example: Datum setting on top surface of workpiece and in center of a bolt hole circle............374

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

15 Touch Probe Cycles: Automatic Workpiece Inspection.............................................................377

15.1 Fundamentals...................................................................................................................................... 378

Overview............................................................................................................................................... 378

Recording the results of measurement................................................................................................379

Measurement results in Q parameters................................................................................................ 381

Classification of results......................................................................................................................... 381

Tolerance monitoring.............................................................................................................................381

Tool monitoring......................................................................................................................................382

Reference system for measurement results........................................................................................ 383

15.2 DATUM PLANE (Cycle 0, DIN/ISO: G55, software option 17).........................................................384

Cycle run............................................................................................................................................... 384

Please note while programming:..........................................................................................................384

Cycle parameters.................................................................................................................................. 384

15.3 POLAR DATUM PLANE (Cycle 1, software option 17).....................................................................385

Cycle run............................................................................................................................................... 385

Please note while programming:..........................................................................................................385

Cycle parameters.................................................................................................................................. 385

15.4 MEASURE ANGLE (Cycle 420, DIN/ISO: G420, software option 17)..............................................386

Cycle run............................................................................................................................................... 386

Please note while programming:..........................................................................................................386

Cycle parameters.................................................................................................................................. 387

15.5 MEASURE HOLE (Cycle 421, DIN/ISO: G421, software option 17).................................................389

Cycle run............................................................................................................................................... 389

Please note while programming:..........................................................................................................389

Cycle parameters.................................................................................................................................. 390

15.6 MEASURE HOLE OUTSIDE (Cycle 422, DIN/ISO: G422, software option 17)................................392

Cycle run............................................................................................................................................... 392

Please note while programming:..........................................................................................................392

Cycle parameters.................................................................................................................................. 393

15.7 MEASURE RECTANGLE INSIDE (Cycle 423, DIN/ISO: G423, software option 17)........................ 395

Cycle run............................................................................................................................................... 395

Please note while programming:..........................................................................................................395

Cycle parameters.................................................................................................................................. 396

TNC 620 | User's Manual Cycle Programming | 2/2015

15.8 MEASURE RECTANGLE OUTSIDE (Cycle 424, DIN/ISO: G424, software option 17).....................398

Cycle run............................................................................................................................................... 398

Please note while programming:..........................................................................................................398

Cycle parameters.................................................................................................................................. 399

15.9 MEASURE INSIDE WIDTH (Cycle 425, DIN/ISO: G425, software option 17)................................. 401

Cycle run............................................................................................................................................... 401

Please note while programming:..........................................................................................................401

Cycle parameters.................................................................................................................................. 402

15.10MEASURE RIDGE WIDTH (Cycle 426, DIN/ISO: G426, software option 17).................................. 404

Cycle run............................................................................................................................................... 404

Please note while programming:..........................................................................................................404

Cycle parameters.................................................................................................................................. 405

15.11MEASURE COORDINATE (Cycle 427, DIN/ISO: G427, software option 17).................................... 407

Cycle run............................................................................................................................................... 407

Please note while programming:..........................................................................................................407

Cycle parameters.................................................................................................................................. 408

15.12MEASURE BOLT HOLE CIRCLE (Cycle 430, DIN/ISO: G430, software option 17)..........................410

Cycle run............................................................................................................................................... 410

Please note while programming:..........................................................................................................411

Cycle parameters.................................................................................................................................. 411

15.13MEASURE PLANE (Cycle 431, DIN/ISO: G431, software option 17).............................................. 413

Cycle run............................................................................................................................................... 413

Please note while programming:..........................................................................................................414

Cycle parameters.................................................................................................................................. 414

15.14Programming Examples..................................................................................................................... 416

Example: Measuring and reworking a rectangular stud....................................................................... 416

Example: Measuring a rectangular pocket and recording the results...................................................418

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

16 Touch Probe Cycles: Special Functions......................................................................................419

16.1 Fundamentals...................................................................................................................................... 420

Overview............................................................................................................................................... 420

16.2 MEASURE (Cycle 3, software option 17)..........................................................................................421

Cycle run............................................................................................................................................... 421

Please note while programming:..........................................................................................................421

Cycle parameters.................................................................................................................................. 422

16.3 MEASURING IN 3-D (Cycle 4, software option 17)..........................................................................423

Cycle run............................................................................................................................................... 423

Please note while programming:..........................................................................................................423

Cycle parameters.................................................................................................................................. 424

16.4 Calibrating a touch trigger probe......................................................................................................425

16.5 Displaying calibration values............................................................................................................. 426

16.6 CALIBRATE TS (Cycle 460, DIN/ISO: G460, software option 17)....................................................427

16.7 CALIBRATE TS LENGTH (Cycle 461, DIN/ISO: G461, software option 17).....................................429

16.8 CALIBRATE TS RADIUS INSIDE (Cycle 462, DIN/ISO: G462, software option 17).........................431

16.9 CALIBRATE TS RADIUS OUTSIDE (Cycle 463, DIN/ISO: G463, software option 17).....................433

TNC 620 | User's Manual Cycle Programming | 2/2015

17 Touch Probe Cycles: Automatic Kinematics Measurement......................................................435

17.1 Kinematics Measurement with TS Touch Probes (KinematicsOpt option)................................... 436

Fundamentals........................................................................................................................................436

Overview............................................................................................................................................... 437

17.2 Prerequisites.........................................................................................................................................438

Please note while programming:..........................................................................................................438

17.3 SAVE KINEMATICS (Cycle 450, DIN/ISO: G450, option)..................................................................439

Cycle run............................................................................................................................................... 439

Please note while programming:..........................................................................................................439

Cycle parameters.................................................................................................................................. 440

Logging function....................................................................................................................................440

Notes on data management................................................................................................................. 441

17.4 MEASURE KINEMATICS (Cycle 451, DIN/ISO: G451, option).........................................................442

Cycle run............................................................................................................................................... 442

Positioning direction.............................................................................................................................. 444

Machines with Hirth-coupled axes........................................................................................................445

Choice of number of measuring points................................................................................................446

Choice of the calibration sphere position on the machine table.......................................................... 447

Notes on the accuracy..........................................................................................................................447

Notes on various calibration methods.................................................................................................. 448

Backlash.................................................................................................................................................449

Please note while programming:..........................................................................................................450

Cycle parameters.................................................................................................................................. 451

Various modes (Q406).......................................................................................................................... 454

Logging function....................................................................................................................................455

17.5 PRESET COMPENSATION (Cycle 452, DIN/ISO: G452, option)...................................................... 456

Cycle run............................................................................................................................................... 456

Please note while programming:..........................................................................................................458

Cycle parameters.................................................................................................................................. 459

Adjustment of interchangeable heads.................................................................................................. 461

Drift compensation................................................................................................................................ 463

Logging function....................................................................................................................................465

TNC 620 | User's Manual Cycle Programming | 2/2015

Contents

18 Touch Probe Cycles: Automatic Tool Measurement..................................................................467

18.1 Fundamentals...................................................................................................................................... 468

Overview............................................................................................................................................... 468

Differences between Cycles 31 to 33 and Cycles 481 to 483............................................................. 469

Setting machine parameters................................................................................................................. 470

Entries in the tool table TOOL.T...........................................................................................................472

18.2 Calibrate the TT (Cycle 30 or 480, DIN/ISO: G480, Option 17 Option 17)......................................474

Cycle run............................................................................................................................................... 474

Please note while programming:..........................................................................................................474

Cycle parameters.................................................................................................................................. 474

18.3 Calibrating the wireless TT 449 (Cycle 484, DIN/ISO: G484, DIN/ISO: G484, Option 17)............. 475

Fundamentals........................................................................................................................................475

Cycle run............................................................................................................................................... 475

Please note while programming:..........................................................................................................476

Cycle parameters.................................................................................................................................. 476

18.4 Measuring tool length (Cycle 31 or 481, DIN/ISO: G481, Option 17).............................................477

Cycle run............................................................................................................................................... 477

Please note while programming:..........................................................................................................478

Cycle parameters.................................................................................................................................. 478

18.5 Measuring tool radius (Cycle 32 or 482, DIN/ISO: G482, Option 17)............................................. 479

Cycle run............................................................................................................................................... 479

Please note while programming:..........................................................................................................479

Cycle parameters.................................................................................................................................. 480

18.6 Measuring tool length and radius (Cycle 33 or 483, DIN/ISO: G483, Option 17).......................... 481

Cycle run............................................................................................................................................... 481

Please note while programming:..........................................................................................................481

Cycle parameters.................................................................................................................................. 482

TNC 620 | User's Manual Cycle Programming | 2/2015

19 Tables of Cycles............................................................................................................................ 483

19.1 Overview.............................................................................................................................................. 484

Fixed cycles...........................................................................................................................................484

Touch probe cycles................................................................................................................................486

TNC 620 | User's Manual Cycle Programming | 2/2015

Fundamentals /

Overviews

Fundamentals / Overviews

1.1 Introduction

Frequently recurring machining cycles that comprise several working steps are stored in the TNC memory as standard cycles. Coordinate transformations and several special functions are also available as cycles. Most cycles use Q parameters as transfer parameters.

Danger of collision!

Cycles sometimes execute extensive operations. For safety reasons, you should run a graphical program test before machining.

If you use indirect parameter assignments in cycles with numbers greater than 200 (e.g. Q210 = Q1), any change in the assigned parameter (e.g. Q1) will have no effect after the cycle definition. Define the cycle parameter (e.g. Q210) directly in such cases.

If you define a feed-rate parameter for fixed cycles greater than 200, then instead of entering a numerical value you can use soft keys to assign the feed rate defined in the TOOL CALL block (FAUTO soft key). You can also use the feed-rate alternatives FMAX (rapid traverse), FZ (feed per tooth) and FU (feed per rev), depending on the respective cycle and the function of the feed-rate parameter.

Note that, after a cycle definition, a change of the FAUTO feed rate has no effect, because internally the TNC assigns the feed rate from the TOOL CALL block when processing the cycle definition.

If you want to delete a block that is part of a cycle, the TNC asks you whether you want to delete the whole cycle.

TNC 620 | User's Manual Cycle Programming | 2/2015

Available Cycle Groups 1.2

1.2 Available Cycle Groups

Overview of fixed cycles

The soft-key row shows the available groups of cycles

Cycle group Soft key Page

Cycles for pecking, reaming, boring and counterboring 68

Cycles for tapping, thread cutting and thread milling 98

Cycles for milling pockets, studs and slots and for face milling 134

Coordinate transformation cycles which enable datum shift, rotation, mirror image, enlarging and reducing for various contours

Subcontour List (SL) cycles, which allow the machining of contours consisting of several overlapping subcontours, as well as cycles for cylinder surface machining and for trochoidal milling

Cycles for producing point patterns, such as circular or linear hole patterns 172

Special cycles such as dwell time, program call, oriented spindle stop, engraving, tolerance, ascertaining the load

If required, switch to machine-specific fixed cycles. These fixed cycles can be integrated by your machine tool builder.

248

216

272

TNC 620 | User's Manual Cycle Programming | 2/2015

Fundamentals / Overviews

1.2 Available Cycle Groups

Overview of touch probe cycles

The soft-key row shows the available groups of cycles

Cycle group Soft key Page

Cycles for automatic measurement and compensation of workpiece misalignment 302

Cycles for automatic workpiece presetting 324

Cycles for automatic workpiece inspection 378

Special cycles 420

Touch probe calibration 427

Cycles for automatic kinematics measurement 302

Cycles for automatic tool measurement (enabled by the machine tool builder) 468

If required, switch to machine-specific touch probe cycles. These touch probe cycles can be integrated by your machine tool builder.

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.1 Working with fixed cycles

Machine-specific cycles (software option19)

In addition to the HEIDENHAIN cycles, many machine tool builders offer their own cycles in the TNC. These cycles are available in a separate cycle-number range:

Cycles 300 to 399 Machine-specific cycles that are to be defined through the CYCLE DEF key

Cycles 500 to 599 Machine-specific touch probe cycles that are to be defined through the TOUCH PROBE key

Refer to your machine manual for a description of the specific function.

Sometimes machine-specific cycles use transfer parameters that HEIDENHAIN already uses in standard cycles. The TNC executes DEF-active cycles as soon as they are defined (see "Calling a cycle", page 50). It executes CALL-active cycles only after they have been called (see "Calling a cycle", page 50). When DEFactive cycles and CALL-active cycles are used simultaneously, it is important to prevent overwriting of transfer parameters already in use. Use the following procedure:

As a rule, always program DEF-active cycles before CALL-active cycles

If you do want to program a DEF-active cycle between the definition and call of a CALL-active cycle, do it only if there is no common use of specific transfer parameters

TNC 620 | User's Manual Cycle Programming | 2/2015

Defining a cycle using soft keys

The soft-key row shows the available groups of cycles

Press the soft key for the desired group of cycles, for example DRILLING for the drilling cycles

Select the cycle, e.g. THREAD MILLING. The TNC initiates the programming dialog and asks for all required input values. At the same time a graphic of the input parameters is displayed in the right screen window. The parameter that is asked for in the dialog prompt is highlighted.

Enter all parameters requested by the TNC and conclude each entry with the ENT key

The TNC ends the dialog when all required data has been entered

Working with fixed cycles 2.1

Defining a cycle using the GOTO function

The soft-key row shows the available groups of cycles

The TNC shows an overview of cycles in a pop-up window

Choose the desired cycle with the arrow keys, or Enter the cycle number and confirm it with the

ENT key. The TNC then initiates the cycle dialog as described above

Example NC blocks

7 CYCL DEF 200

Q200=2 ;

Q201=3 ;

Q206=150 ;FEED RATE FOR PLNGNG

Q202=5 ;

Q210=0 ;

Q203=+0 ;SURFACE COORDINATE

Q204=50 ;

Q211=0.25 ;

Q395=0 ;DEPTH REFERENCE

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.1 Working with fixed cycles

Calling a cycle

Prerequisites

The following data must always be programmed before a cycle call:

BLK FORM for graphic display (needed only for test graphics)

Tool call Direction of spindle rotation (M functions M3/M4) Cycle definition (CYCL DEF)

For some cycles, additional prerequisites must be observed. They are detailed in the descriptions for each cycle.

The following cycles become effective automatically as soon as they are defined in the part program. These cycles cannot and must not be called:

Cycle 220 for point patterns on circles and Cycle 221 for point patterns on lines

SL Cycle 14 CONTOUR GEOMETRY SL Cycle 20 CONTOUR DATA Cycle 32 TOLERANCE Coordinate transformation cycles Cycle 9 DWELL TIME All touch probe cycles

You can call all other cycles with the functions described as follows.

Calling a cycle with CYCL CALL

The CYCL CALL function calls the most recently defined fixed cycle once. The starting point of the cycle is the position that was programmed last before the CYCL CALL block.

To program the cycle call, press the CYCL CALL key

Press the CYCL CALL M soft key to enter a cycle call

If necessary, enter the miscellaneous function M (for example M3 to switch the spindle on), or end the dialog by pressing the END key

Calling a cycle with CYCL CALL PAT

The CYCL CALL PAT function calls the most recently defined fixed cycle at all positions that you defined in a PATTERN DEF pattern definition (see "PATTERN DEF pattern definition", page 56) or in a point table (see "Point tables", page 63).

TNC 620 | User's Manual Cycle Programming | 2/2015

Calling a cycle with CYCL CALL POS

The CYCL CALL POS function calls the most recently defined fixed cycle once. The starting point of the cycle is the position that you defined in the CYCL CALL POS block.

Using positioning logic the TNC moves to the position defined in the CYCL CALL POS block.

If the tool’s current position in the tool axis is greater than the top surface of the workpiece (Q203), the TNC moves the tool to the programmed position first in the machining plane and then in the tool axis.

If the tool’s current position in the tool axis is below the top surface of the workpiece (Q203), the TNC moves the tool to the programmed position first in the tool axis to the clearance height and then in the working plane to the programmed position.

Working with fixed cycles 2.1

Three coordinate axes must always be programmed in the CYCL CALL POS block. With the coordinate in the tool axis you can easily change the starting position. It serves as an additional datum shift.

The feed rate most recently defined in the CYCL CALL POS block applies only to traverse to the start position programmed in this block.

As a rule, the TNC moves without radius compensation (R0) to the position defined in the CYCL CALL POS block.

If you use CYCL CALL POS to call a cycle in which a start position is defined (for example Cycle 212), then the position defined in the cycle serves as an additional shift of the position defined in the CYCL CALL POS block. You should therefore always define the start position to be set in the cycle as 0.

Cycle call with M99/M89

The M99 function, which is active only in the block in which it is programmed, calls the last defined fixed cycle once. You can program M99 at the end of a positioning block. The TNC moves to this position and then calls the last defined fixed cycle.

If the TNC is to run the cycle automatically after every positioning block, program the first cycle call with M89.

To cancel the effect of M89, program:

M99 in the positioning block in which you move to the last starting point, or

Use CYCL DEF to define a new fixed cycle

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.2 Program defaults for cycles

Overview

All Cycles 20 to 25, as well as all of those with numbers 200 or higher, always use identical cycle parameters, such as the set-up clearance Q200, which you must enter for each cycle definition. The GLOBAL DEF function gives you the possibility of defining these cycle parameters once at the beginning of the program, so that they are effective globally for all fixed cycles used in the program. In the respective fixed cycle you then simply link to the value defined at the beginning of the program.

The following GLOBAL DEF functions are available:

Machining patterns Soft key Page

GLOBAL DEF COMMON Definition of generally valid cycle parameters

GLOBAL DEF DRILLING Definition of specific drilling cycle parameters

GLOBAL DEF POCKET MILLING Definition of specific pocket-milling cycle parameters

GLOBAL DEF CONTOUR MILLING Definition of specific contour milling cycle parameters

GLOBAL DEF POSITIONING Definition of the positioning behavior for CYCL CALL PAT

GLOBAL DEF PROBING Definition of specific touch probe cycle parameters

Entering GLOBAL DEF

Select the Programming and Editing operating mode

Press the special functions key

Select the functions for program defaults

Select GLOBAL DEF functions

Select the desired GLOBAL DEF function, e.g.

GLOBAL DEF COMMON

Enter the required definitions, and confirm each entry with the ENT key

TNC 620 | User's Manual Cycle Programming | 2/2015

Program defaults for cycles 2.2

Using GLOBAL DEF information

If you have entered the corresponding GLOBAL DEF functions at the beginning of the program, then you can link to these globally valid values when defining any fixed cycle.

Proceed as follows:

Select the Programming and Editing operating mode

Select fixed cycles

Select the desired group of cycles, for example: drilling cycles

Select the desired cycle, e.g. DRILLING The TNC displays the SET STANDARD VALUES soft

key, if there is a global parameter for it Press the SET STANDARD VALUES soft key. The

TNC enters the word PREDEF (predefined) in the cycle definition. You have now created a link to the corresponding GLOBAL DEF parameter that you defined at the beginning of the program

Danger of collision!

Please note that later changes to the program settings affect the entire machining program, and can therefore change the machining procedure significantly.

If you enter a fixed value in a fixed cycle, then this value will not be changed by the GLOBAL DEF functions.

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.2 Program defaults for cycles

Global data valid everywhere

Set-up clearance: Distance between tool tip and workpiece surface for automated approach of the cycle start position in the tool axis

2nd set-up clearance: Position to which the TNC positions the tool at the end of a machining step. The next machining position is approached at this height in the machining plane

F positioning: Feed rate at which the TNC traverses the tool within a cycle

F retraction: Feed rate at which the TNC retracts the tool

The parameters are valid for all fixed cycles with numbers greater than 2xx.

Global data for drilling operations

Retraction rate for chip breaking: Value by which the TNC retracts the tool during chip breaking

Dwell time at depth: Time in seconds that the tool remains at the hole bottom

Dwell time at top: Time in seconds that the tool remains at the set-up clearance

The parameters apply to the drilling, tapping and thread milling cycles 200 to 209, 240, and 262 to 267.

Global data for milling operations with pocket cycles 25x

Overlap factor: The tool radius multiplied by the overlap factor equals the lateral stepover

Climb or up-cut: Select the type of milling Plunging type: Plunge into the material helically, in a

reciprocating motion, or vertically

The parameters apply to milling cycles 251 to 257.

TNC 620 | User's Manual Cycle Programming | 2/2015

Global data for milling operations with contour cycles

Set-up clearance: Distance between tool tip and workpiece surface for automated approach of the cycle start position in the tool axis

Clearance height: Absolute height at which the tool cannot collide with the workpiece (for intermediate positioning and retraction at the end of the cycle)

Overlap factor: The tool radius multiplied by the overlap factor equals the lateral stepover

Climb or up-cut: Select the type of milling

The parameters apply to SL cycles 20, 22, 23, 24 and

25.

Program defaults for cycles 2.2

Global data for positioning behavior

Positioning behavior: Retraction in the tool axis at the end of the machining step: Return to the 2nd set-up clearance or to the position at the beginning of the unit

The parameters apply to each fixed cycle that you call with the CYCL CALL PAT function.

Global data for probing functions

Set-up clearance: Distance between stylus and workpiece surface for automated approach of the probing position

Clearance height: The coordinate in the touch probe axis to which the TNC traverses the touch probe between measuring points, if the Move to clearance height option is activated

Move to clearance height: Select whether the TNC moves the touch probe to the set-up clearance or clearance height between the measuring points

Applies to all Touch Probe Cycles 4xx.

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.3 PATTERN DEF pattern definition

Application

You use the PATTERN DEF function to easily define regular machining patterns, which you can call with the CYCL CALL PAT function. As with the cycle definitions, support graphics that illustrate the respective input parameter are also available for pattern definitions.

PATTERN DEF is to be used only in connection with the tool axis Z.

The following machining patterns are available:

Machining patterns Soft key Page

POINT Definition of up to any 9 machining positions

ROW Definition of a single row, straight or rotated

PATTERN Definition of a single pattern, straight, rotated or distorted

FRAME Definition of a single frame, straight, rotated or distorted

CIRCLE Definition of a full circle

PITCH CIRCLE Definition of a pitch circle

TNC 620 | User's Manual Cycle Programming | 2/2015

Entering PATTERN DEF

Select the Programming mode of operation

Press the special functions key

Select the functions for contour and point machining

Open a PATTERN DEF block

Select the desired machining pattern, e.g. a single row

Enter the required definitions, and confirm each entry with the ENT key

PATTERN DEF pattern definition 2.3

Using PATTERN DEF

As soon as you have entered a pattern definition, you can call it with the CYCL CALL PAT function "Calling a cycle", page 50. The TNC then performs the most recently defined machining cycle on the machining pattern you defined.

A machining pattern remains active until you define a new one, or select a point table with the SEL PATTERN function.

You can use the mid-program startup function to select any point at which you want to start or continue machining (see User's Manual, Test Run and Program Run sections).

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.3 PATTERN DEF pattern definition

Defining individual machining positions

You can enter up to 9 machining positions. Confirm each entry with the ENT key.

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

X coord. of machining position (absolute): Enter X coordinate

Y coord. of machining position (absolute): Enter Y coordinate

Coordinate of workpiece surface (absolute): Enter Z coordinate at which machining is to begin

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF POS1

(X+25 Y+33.5 Z+0) POS2 (X+50 Y +75 Z+0)

Defining a single row

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Starting point in X (absolute): Coordinate of the starting point of the row in the X axis

Starting point in Y (absolute): Coordinate of the starting point of the row in the Y axis

Spacing of machining positions (incremental): Distance between the machining positions. You can enter a positive or negative value

Number of repetitions: Total number of machining operations

Rot. position of entire pattern (absolute): Angle of rotation around the entered starting point. Reference axis: Reference axis of the active machining plane (e.g. X for tool axis Z). You can enter a positive or negative value

Coordinate of workpiece surface (absolute): Enter Z coordinate at which machining is to begin

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF ROW1

(X+25 Y+33.5 D+8 NUM5 ROT+0 Z +0)

TNC 620 | User's Manual Cycle Programming | 2/2015

Defining a single pattern

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

The Rotary pos. ref. ax. and Rotary pos. minor

ax. parameters are added to a previously performed rotated position of the entire pattern.

Starting point in X (absolute): Coordinate of the

starting point of the pattern in the X axis Starting point in Y (absolute): Coordinate of the

starting point of the pattern in the Y axis Spacing of machining positions X (incremental):

Distance between the machining positions in the X direction. You can enter a positive or negative value

Spacing of machining positions Y (incremental): Distance between the machining positions in the Y direction. You can enter a positive or negative value

Number of columns: Total number of columns in the pattern

Number of lines: Total number of rows in the pattern

Rot. position of entire pattern (absolute): Angle of rotation by which the entire pattern is rotated around the entered starting point. Reference axis: Reference axis of the active machining plane (e.g. X for tool axis Z). You can enter a positive or negative value

Rotary pos. ref. ax.: Angle of rotation around which only the reference axis of the machining plane is distorted with respect to the entered starting point. You can enter a positive or negative value.

Rotary pos. minor ax.: Angle of rotation around which only the minor axis of the machining plane is distorted with respect to the entered starting point. You can enter a positive or negative value.

Workpiece surface coordinate (absolute): Enter Z coordinate at which machining is to begin

PATTERN DEF pattern definition 2.3

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF PAT1 (X+25 Y+33.5

DX+8 DY+10 NUMX5 NUMY4 ROT+0 ROTX+0 ROTY+0 Z+0)

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.3 PATTERN DEF pattern definition

Defining individual frames

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

The Rotary pos. ref. ax. and Rotary pos. minor

ax. parameters are added to a previously performed rotated position of the entire pattern.

Starting point in X (absolute): Coordinate of the

starting point of the frame in the X axis Starting point in Y (absolute): Coordinate of the

starting point of the frame in the Y axis Spacing of machining positions X (incremental):

Distance between the machining positions in the X direction. You can enter a positive or negative value

Spacing of machining positions Y (incremental): Distance between the machining positions in the Y direction. You can enter a positive or negative value

Number of columns: Total number of columns in the pattern

Number of lines: Total number of rows in the pattern

Rotary pos. ref. ax.: Angle of rotation around which only the reference axis of the machining plane is distorted with respect to the entered starting point. You can enter a positive or negative value

Rotary pos. minor ax.: Angle of rotation around which only the minor axis of the machining plane is distorted with respect to the entered starting point. You can enter a positive or negative value.

Coordinate of workpiece surface (absolute): Enter Z coordinate at which machining is to begin

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF FRAME1

(X+25 Y+33.5 DX+8 DY+10 NUMX5 NUMY4 ROT+0 ROTX+0 ROTY+0 Z +0)

TNC 620 | User's Manual Cycle Programming | 2/2015

Defining a full circle

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Bolt-hole circle center X (absolute): Coordinate of the circle center in the X axis

Bolt-hole circle center Y (absolute): Coordinate of the circle center in the Y axis

Bolt-hole circle diameter: Diameter of the bolthole circle

Starting angle: Polar angle of the first machining position. Reference axis: Reference axis of the active machining plane (e.g. X for tool axis Z). You can enter a positive or negative value

Number of repetitions: Total number of machining positions on the circle

Coordinate of workpiece surface (absolute): Enter Z coordinate at which machining is to begin

PATTERN DEF pattern definition 2.3

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF CIRC1

(X+25 Y+33 D80 START+45 NUM8 Z +0)

TNC 620 | User's Manual Cycle Programming | 2/2015

Using Fixed Cycles

2.3 PATTERN DEF pattern definition

Defining a pitch circle

If you have defined a workpiece surface in Z not equal to 0, then this value is effective in addition to the workpiece surface Q203 that you defined in the machining cycle.

Bolt-hole circle center X (absolute): Coordinate of the circle center in the X axis

Bolt-hole circle center Y (absolute): Coordinate of the circle center in the Y axis

Bolt-hole circle diameter: Diameter of the bolthole circle

Starting angle: Polar angle of the first machining position. Reference axis: Major axis of the active machining plane (e.g. X for tool axis Z). You can enter a positive or negative value

Stepping angle/end angle: Incremental polar angle between two machining positions. You can enter a positive or negative value As an alternative you can enter the end angle (switch via soft key).

Number of repetitions: Total number of machining positions on the circle

Coordinate of workpiece surface (absolute): Enter Z coordinate at which machining is to begin

NC blocks

10 L Z+100 R0 FMAX

11 PATTERN DEF PITCHCIRC1

(X+25 Y+33 D80 START+45 STEP30 NUM8 Z+0)

TNC 620 | User's Manual Cycle Programming | 2/2015

2.4 Point tables

Application

You should create a point table whenever you want to run a cycle, or several cycles in sequence, on an irregular point pattern.

If you are using drilling cycles, the coordinates of the working plane in the point table represent the hole centers. If you are using milling cycles, the coordinates of the working plane in the point table represent the starting-point coordinates of the respective cycle (e.g. center-point coordinates of a circular pocket). Coordinates in the spindle axis correspond to the coordinate of the workpiece surface.

Creating a point table

Select the Programming mode of operation

Point tables 2.4

Call the file manager: Press the PGM MGT key.

FILE NAME?

Enter the name and file type of the point table and confirm your entry with the ENT key.

Select the unit of measure: Press the MM or INCH soft key. The TNC changes to the program blocks window and displays an empty point table.

With the INSERT LINE soft key, insert new lines and enter the coordinates of the desired machining position.

Repeat the process until all desired coordinates have been entered.

The name of the point table must begin with a letter. Use the soft keys X OFF/ON, Y OFF/ON, Z OFF/ON

(second soft-key row) to specify which coordinates you want to enter in the point table.

TNC 620 | User's Manual Cycle Programming | 2/2015

ENT

Using Fixed Cycles

2.4 Point tables

Hiding single points from the machining process

In the FADE column of the point table you can specify if the defined point is to be hidden during the machining process.

In the table, select the point to be hidden

Select the FADE column

Activate hiding, or

Deactivate hiding

Selecting a point table in the program

In the Programming mode of operation, select the program for which you want to activate the point table:

Press the PGM CALL key to call the function for selecting the point table

Press the POINT TABLE soft key

Enter the name of the point table and confirm your entry with the END key. If the point table is not stored in the same directory as the NC program, you must enter the complete path.

Example NC block

7 SEL PATTERN "TNC:\DIRKT5\NUST35.PNT"

TNC 620 | User's Manual Cycle Programming | 2/2015

Calling a cycle in connection with point tables

With CYCL CALL PAT the TNC runs the point table that you last defined (even if you defined the point table in a program that was nested with CALL PGM).

If you want the TNC to call the last defined fixed cycle at the points defined in a point table, then program the cycle call with CYCLE CALL PAT:

To program the cycle call, press the CYCL CALL key

Press the CYCL CALL PAT soft key to call a point table

Enter the feed rate at which the TNC is to move from point to point (if you make no entry the TNC will move at the last programmed feed rate; FMAX is not valid)

If required, enter a miscellaneous function M, then confirm with the END key

Point tables 2.4

The TNC retracts the tool to the clearance height between the starting points. Depending on which is greater, the TNC uses either the spindle axis coordinate from the cycle call or the value from cycle parameter Q204 as the clearance height.

If you want to move at reduced feed rate when pre-positioning in the spindle axis, use the miscellaneous function M103.

Effect of the point table with SL cycles and Cycle 12

The TNC interprets the points as an additional datum shift.

Effect of the point table with Cycles 200 to 208 and 262 to 267

The TNC interprets the points of the working plane as coordinates of the hole centers. If you want to use the coordinate defined in the point table for the spindle axis as the starting point coordinate, you must define the workpiece surface coordinate (Q203) as 0.

Effect of the point table with Cycles 251 to 254

The TNC interprets the points of the working plane as coordinates of the cycle starting point. If you want to use the coordinate defined in the point table for the spindle axis as the starting point coordinate, you must define the workpiece surface coordinate (Q203) as 0.

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles:

Drilling

Fixed Cycles: Drilling

3.1 Fundamentals

Overview

The TNC offers the following cycles for all types of drilling operations:

Cycle Soft key Page

240 CENTERING With automatic pre-positioning, 2nd set-up clearance, optional entry of the centering diameter or centering depth

200 DRILLING With automatic pre-positioning, 2nd set-up clearance

201 REAMING With automatic pre-positioning, 2nd set-up clearance

202 BORING With automatic pre-positioning, 2nd set-up clearance

203 UNIVERSAL DRILLING With automatic pre-positioning, 2nd set-up clearance, chip breaking, and decrementing

204 BACK BORING With automatic pre-positioning, 2nd set-up clearance

205 UNIVERSAL PECKING With automatic pre-positioning, 2nd set-up clearance, chip breaking, and advanced stop distance

208 BORE MILLING With automatic pre-positioning, 2nd set-up clearance

241 SINGLE-LIP D.H.DRLNG With automatic pre-positioning to deepened starting point, shaft speed and coolant definition

TNC 620 | User's Manual Cycle Programming | 2/2015

CENTERING (Cycle 240, DIN/ISO: G240, software option 19) 3.2

3.2 CENTERING (Cycle 240, DIN/ISO: G240, software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to set-up clearance above the workpiece surface.

The tool is centered at the programmed feed rate F to the

programmed centering diameter or centering depth. 3 If defined, the tool remains at the centering depth. 4 Finally, the tool path is retraced to setup clearance or—if

programmed—to the 2nd setup clearance at rapid traverse

FMAX.

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter Q344 (diameter) or Q201 (depth) determines the working direction. If you program the diameter or depth = 0, the cycle will not be executed.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive diameter or

depth is entered. This means that the tool moves

at rapid traverse in the tool axis to set-up clearance

below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.2 CENTERING (Cycle 240, DIN/ISO: G240, software option 19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Enter a positive value. Input range 0 to 99999.9999

Select depth/diameter (0/1) Q343: Select whether centering is based on the entered diameter or depth. If the TNC is to center based on the entered diameter, the point angle of the tool must be defined in the T ANGLE column of the tool table TOOL.T.

0: Centering based on the entered depth 1: Centering based on the entered diameter

Depth Q201 (incremental): Distance between workpiece surface and centering bottom (tip of centering taper). Only effective if Q343=0 is defined. Input range -99999.9999 to 99999.9999

Diameter (algebraic sign) Q344: Centering diameter. Only effective if Q343=1 is defined. Input range -99999.9999 to 99999.9999

Feed rate for plunging Q206: Traversing speed of the tool during centering in mm/min. Input range: 0 to 99999.999; alternatively FAUTO, FU

Dwell time at depth Q211: Time in seconds that the tool remains at the hole bottom. Input range 0 to

3600.0000 Coordinate of workpiece surface Q203 (absolute):

Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

NC blocks

10 L Z+100 R0 FMAX

11 CYCL DEF 240

Q200=2 ;

Q343=1 ;

Q201=+0 ;

Q344=-9 ;

Q206=250 ;FEED RATE FOR

PLNGNG

Q211=0.1 ;

Q203=+20 ;SURFACE COORDINATE

Q204=100 ;

12 L X+30 Y+20 R0 FMAX M3 M99

13 L X+80 Y+50 R0 FMAX M99

TNC 620 | User's Manual Cycle Programming | 2/2015

3.3 DRILLING (Cycle 200)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to set-up clearance above the workpiece surface. 2 The tool drills to the first plunging depth at the programmed

feed rate F. 3

The TNC returns the tool at FMAX to the set-up clearance,

dwells there (if a dwell time was entered), and then moves at

FMAX to the set-up clearance above the first plunging depth. 4 The tool then drills deeper by the plunging depth at the

programmed feed rate F. 5 The TNC repeats this process (2 to 4) until the programmed

total hole depth is reached. 6 Finally, the tool path is retraced to setup clearance from the

hole bottom or—if programmed—to the 2nd setup clearance at

FMAX.

DRILLING (Cycle 200) 3.3

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.3 DRILLING (Cycle 200)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Enter a positive value. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of

the tool in mm/min during drilling. Input range 0 to

99999.999, alternatively FAUTO, FU Plunging depth Q202 (incremental): Infeed per cut.

Input range 0 to 99999.9999. The depth does not have to be a multiple of the plunging depth. The TNC will go to depth in one movement if:

the plunging depth is equal to the depth the plunging depth is greater than the depth

Dwell time at top Q210: Time in seconds that the tool remains at set-up clearance after having been retracted from the hole for chip removal. Input range 0 to 3600.0000

Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Dwell time at depth Q211: Time in seconds that the tool remains at the hole bottom. Input range 0 to

3600.0000 Depth reference Q395: Select whether the entered

depth is referenced to the tool tip or the cylindrical part of the tool. If the TNC is to reference the depth to the cylindrical part of the tool, the point angle of the tool must be defined in the T ANGLE column of the tool table TOOL.T.

0 = Depth referenced to the tool tip 1 = Depth referenced to the cylindrical part of the

tool

NC blocks

11 CYCL DEF 200 DRILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-15 ;DEPTH

Q206=250 ;FEED RATE FOR

PLNGNG

Q202=5 ;PLUNGING DEPTH

Q211=0 ;DWELL TIME AT TOP

Q203=+20 ;SURFACE COORDINATE

Q204=100 ;2ND SET-UP

CLEARANCE

Q211=0.1 ;DWELL TIME AT

BOTTOM

Q395=0 ;DEPTH REFERENCE

12 L X+30 Y+20 FMAX M3

13 CYCL CALL

14 L X+80 Y+50 FMAX M99

TNC 620 | User's Manual Cycle Programming | 2/2015

REAMING (Cycle 201, DIN/ISO: G201, software option 19) 3.4

3.4 REAMING (Cycle 201, DIN/ISO: G201,

software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the entered set-up clearance above the workpiece

surface. 2 The tool reams to the entered depth at the programmed feed

rate F. 3 If programmed, the tool remains at the hole bottom for the

entered dwell time. 4 The tool then retracts to set-up clearance at the feed rate F, and

from there—if programmed—to the 2nd set-up clearance in

FMAX.

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.4 REAMING (Cycle 201, DIN/ISO: G201, software option 19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of

the tool during reaming in mm/min. Input range 0 to

99999.999; alternatively FAUTO, FU Dwell time at depth Q211: Time in seconds that

the tool remains at the hole bottom. Input range 0 to

3600.0000 Retraction feed rate Q208: Traversing speed of the

tool in mm/min when retracting from the hole. If you enter Q208 = 0, the tool retracts at the reaming feed rate. Input range 0 to 99999.999

Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range 0 to 99999.9999

2nd set-up clearance Q204 (incremental): Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

NC blocks

11 CYCL DEF 201 REAMING

Q200=2 ;SET-UP CLEARANCE

Q201=-15 ;DEPTH

Q206=100 ;FEED RATE FOR

PLNGNG

Q211=0.5 ;DWELL TIME AT

BOTTOM

Q208=250 ;RETRACTION FEED

RATE

Q203=+20 ;SURFACE COORDINATE

Q204=100 ;2ND SET-UP

CLEARANCE

12 L X+30 Y+20 FMAX M3

13 CYCL CALL

14 L X+80 Y+50 FMAX M9

15 L Z+100 FMAX M2

TNC 620 | User's Manual Cycle Programming | 2/2015

BORING (Cycle 202, DIN/ISO: G202, software option 19) 3.5

3.5 BORING (Cycle 202, DIN/ISO: G202,

software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to set-up clearance above the workpiece surface. 2 The tool drills to the programmed depth at the feed rate for

plunging. 3 If programmed, the tool remains at the hole bottom for the

entered dwell time with active spindle rotation for cutting free. 4 The TNC then orients the spindle to the position that is defined

in parameter Q336. 5 If retraction is selected, the tool retracts in the programmed

direction by 0.2 mm (fixed value). 6 The tool then retracts to set-up clearance at the retraction rate,

and from there—if programmed—to the 2nd set-up clearance at

FMAX. If Q214=0 the tool point remains on the wall of the hole.

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.5 BORING (Cycle 202, DIN/ISO: G202, software option 19)

Please note while programming:

Machine and TNC must be specially prepared by the machine tool builder for use of this cycle.

This cycle is effective only for machines with servocontrolled spindle.

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

After the cycle is completed, the TNC restores the coolant and spindle conditions that were active before the cycle call.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

Select a disengaging direction in which the tool moves away from the edge of the hole.

Check the position of the tool tip when you program a spindle orientation to the angle that you enter in Q336 (for example, in the Positioning with Manual Data Input mode of operation). Set the angle so that the tool tip is parallel to a coordinate axis.

During retraction the TNC automatically takes an active rotation of the coordinate system into account.

TNC 620 | User's Manual Cycle Programming | 2/2015

BORING (Cycle 202, DIN/ISO: G202, software option 19) 3.5

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of

the tool during boring at mm/min. Input range 0 to

99999.999; alternatively FAUTO, FU Dwell time at depth Q211: Time in seconds that

the tool remains at the hole bottom. Input range 0 to

3600.0000 Retraction feed rate Q208: Traversing speed of the

tool in mm/min when retracting from the hole. If you enter Q208 = 0, the tool retracts at feed rate for plunging. Input range 0 to 99999.999, alternatively

FMAX, FAUTO Coordinate of workpiece surface Q203 (absolute):

Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.999

Disengaging direction (0/1/2/3/4) Q214: Determine the direction in which the TNC retracts the tool on the hole bottom (after spindle orientation)

0: Do not retract the tool 1: Retract the tool in minus direction of the principle

axis

2: Retract the tool in minus direction of the minor

axis

3: Retract the tool in plus direction of the principle

axis

4: Retract the tool in plus direction of the minor axis

Angle for spindle orientation Q336 (absolute): Angle at which the TNC positions the tool before retracting it. Input range -360.000 to 360.000

10 L Z+100 R0 FMAX

11 CYCL DEF 202 BORING

Q200=2 ;SET-UP CLEARANCE

Q201=-15 ;DEPTH

Q206=100 ;FEED RATE FOR

PLNGNG

Q211=0.5 ;DWELL TIME AT

BOTTOM

Q208=250 ;RETRACTION FEED

RATE

Q203=+20 ;SURFACE COORDINATE

Q204=100 ;2ND SET-UP

CLEARANCE

Q214=1 ;DISENGAGING DIRECTN

Q336=0 ;ANGLE OF SPINDLE

12 L X+30 Y+20 FMAX M3

13 CYCL CALL

14 L X+80 Y+50 FMAX M99

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.6 UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203, software option

19)

3.6 UNIVERSAL DRILLING (Cycle 203,

DIN/ISO: G203, software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the entered set-up clearance above the workpiece

surface. 2 The tool drills to the first plunging depth at the entered feed rate

F. 3 If you have programmed chip breaking, the tool then retracts

by the entered retraction value. If you are working without chip

breaking, the tool retracts at the retraction feed rate to the set-

up clearance, remains there—if programmed—for the entered

dwell time, and advances again at FMAX to the set-up clearance

above the first PLUNGING DEPTH. 4 The tool then advances with another infeed at the programmed

feed rate. If programmed, the plunging depth is decreased after

each infeed by the decrement. 5 The TNC repeats this process (2 to 4) until the programmed

total hole depth is reached. 6 The tool remains at the hole bottom—if programmed—for

the entered dwell time to cut free, and then retracts to set-up

clearance at the retraction feed rate. If programmed, the tool

moves to the 2nd set-up clearance at FMAX.

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203, software option

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of

the tool during drilling in mm/min. Input range 0 to

99999.999; alternatively FAUTO, FU Plunging depth Q202 (incremental): Infeed per cut.

Input range 0 to 99999.9999. The depth does not have to be a multiple of the plunging depth. The TNC will go to depth in one movement if:

the plunging depth is equal to the depth the plunging depth is greater than the depth and

no chip breaking is defined

Dwell time at top Q210: Time in seconds that the tool remains at set-up clearance after having been retracted from the hole for chip removal. Input range 0 to 3600.0000

Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Decrement Q212 (incremental): Value by which the TNC decreases the plunging depth Q202 after each infeed. Input range 0 to 99999.9999

No. Breaks before retracting Q213: Number of chip breaks after which the TNC is to withdraw the tool from the hole for chip removal. For chip breaking, the TNC retracts the tool each time by the value in Q256. Input range 0 to 99999

Minimum plunging depth Q205 (incremental): If you have entered a decrement, the TNC limits the plunging depth to the value entered with Q205. Input range 0 to 99999.9999

NC blocks

11 CYCL DEF 203 UNIVERSAL DRILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-20 ;DEPTH

Q206=150 ;FEED RATE FOR

PLNGNG

Q202=5 ;PLUNGING DEPTH

Q211=0 ;DWELL TIME AT TOP

Q203=+20 ;SURFACE COORDINATE

Q204=50 ;2ND SET-UP

CLEARANCE

Q212=0.2 ;DECREMENT

Q213=3 ;CHIP BREAKING

Q205=3 ;MIN. PLUNGING DEPTH

Q211=0.25 ;DWELL TIME AT

BOTTOM

Q208=500 ;RETRACTION FEED

RATE

Q256=0.2 ;DIST. FOR CHIP BRKNG

Q395=0 ;DEPTH REFERENCE

3.6

19)

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.6 UNIVERSAL DRILLING (Cycle 203, DIN/ISO: G203, software option

19)

Dwell time at depth Q211: Time in seconds that the tool remains at the hole bottom. Input range 0 to

3600.0000 Feed rate for retraction Q208: Traversing speed of

the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the TNC retracts the tool at the feed rate Q206. Input range 0 to 99999.999, alternatively FMAX, FAUTO

Retraction rate for chip breaking Q256 (incremental): Value by which the TNC retracts the tool during chip breaking. Input range 0.000 to

99999.999 Depth reference Q395: Select whether the entered

0 = Depth referenced to the tool tip 1 = Depth referenced to the cylindrical part of the

tool

TNC 620 | User's Manual Cycle Programming | 2/2015

BACK BORING (Cycle 204, DIN/ISO: G204, software option 19) 3.7

3.7 BACK BORING (Cycle 204, DIN/ISO:

G204, software option 19)

Cycle run

This cycle allows holes to be bored from the underside of the workpiece.

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to set-up clearance above the workpiece surface. 2 The TNC then orients the spindle to the 0° position with an

oriented spindle stop and displaces the tool by the off-center

distance. 3 The tool is then plunged into the already bored hole at the

feed rate for pre-positioning until the tooth has reached set-up

clearance on the underside of the workpiece. 4 The TNC then centers the tool again over the bore hole,

switches on the spindle and the coolant and moves at the feed

rate for boring to the depth of bore. 5 If a dwell time is entered, the tool will pause at the top of the

bore hole and will then be retracted from the hole again. The

TNC carries out another oriented spindle stop and the tool is

once again displaced by the off-center distance. 6 The tool then retracts to set-up clearance at the feed rate for

pre-positioning, and from there—if programmed—to the 2nd

set-up clearance at FMAX.

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.7 BACK BORING (Cycle 204, DIN/ISO: G204, software option 19)

Please note while programming:

Machine and TNC must be specially prepared by the machine tool builder for use of this cycle.

This cycle is effective only for machines with servocontrolled spindle.

Special boring bars for upward cutting are required for this cycle.

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter depth determines the working direction. Note: A positive sign bores in the direction of the positive spindle axis.

The entered tool length is the total length to the underside of the boring bar and not just to the tooth.

When calculating the starting point for boring, the TNC considers the tooth length of the boring bar and the thickness of the material.

Danger of collision!

Check the position of the tool tip when you program a spindle orientation to the angle that you enter in

Q336 (for example, in the Positioning with Manual Data Input mode of operation). Set the angle so that

the tool tip is parallel to a coordinate axis. Select a disengaging direction in which the tool moves away from the edge of the hole.

TNC 620 | User's Manual Cycle Programming | 2/2015

BACK BORING (Cycle 204, DIN/ISO: G204, software option 19) 3.7

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth of counterbore Q249 (incremental): Distance between underside of workpiece and the top of the hole. A positive sign means the hole will be bored in the positive spindle axis direction. Input range -99999.9999 to 99999.9999

Material thickness Q250 (incremental): Thickness of the workpiece. Input range 0.0001 to 99999.9999

Off-center distance Q251 (incremental): Off-center distance for the boring bar; value from tool data sheet. Input range 0.0001 to 99999.9999

Tool edge height Q252 (incremental): Distance between the underside of the boring bar and the main cutting tooth; value from tool data sheet. Input range 0.0001 to 99999.9999

Feed rate for pre-positioning Q253: Traversing speed of the tool in mm/min when plunging into the workpiece, or when retracting from the workpiece. Input range 0 to 99999.999; alternatively FMAX,

FAUTO Feed rate for back boring Q254: Traversing speed

of the tool during back boring in mm/min. Input range 0 to 99999.999; alternatively FAUTO, FU

Dwell time Q255: Dwell time in seconds at the top of the bore hole. Input range 0 to 3600.000

Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Disengaging direction (1/2/3/4) Q214: Determine the direction in which the TNC displaces the tool by the off-center distance (after spindle orientation); programming 0 is not allowed

1: Retract the tool in minus direction of the principle

axis

2: Retract the tool in minus direction of the minor

axis

3: Retract the tool in plus direction of the principle

axis

4: Retract the tool in plus direction of the minor axis

Angle for spindle orientation Q336 (absolute): Angle at which the TNC positions the tool before it is plunged into or retracted from the bore hole. Input range -360.0000 to 360.0000

NC blocks

11 CYCL DEF 204 BACK BORING

Q200=2 ;SET-UP CLEARANCE

Q249=+5 ;DEPTH OF

COUNTERBORE

Q250=20 ;MATERIAL THICKNESS

Q251=3.5 ;OFF-CENTER DISTANCE

Q252=15 ;TOOL EDGE HEIGHT

Q253=750 ;F PRE-POSITIONING

Q254=200 ;F COUNTERBORING

Q255=0 ;DWELL TIME

Q203=+20 ;SURFACE COORDINATE

Q204=50 ;2ND SET-UP

CLEARANCE

Q214=1 ;DISENGAGING DIRECTN

Q336=0 ;ANGLE OF SPINDLE

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.8 UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205, software option

19)

3.8 UNIVERSAL PECKING (Cycle 205,

DIN/ISO: G205, software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the entered set-up clearance above the workpiece

surface. 2 If you enter a deepened starting point, the TNC move at the

defined positioning feed rate to the set-up clearance above the

deepened starting point. 3 The tool drills to the first plunging depth at the entered feed rate

F. 4 If you have programmed chip breaking, the tool then retracts

by the entered retraction value. If you are working without

chip breaking, the tool is moved at rapid traverse to the set-up

clearance, and then at FMAX to the entered starting position

above the first plunging depth. 5 The tool then advances with another infeed at the programmed

feed rate. If programmed, the plunging depth is decreased after

each infeed by the decrement. 6 The TNC repeats this process (2 to 4) until the programmed

total hole depth is reached. 7 The tool remains at the hole bottom—if programmed—for

the entered dwell time to cut free, and then retracts to set-up

clearance at the retraction feed rate. If programmed, the tool

moves to the 2nd set-up clearance at FMAX.

TNC 620 | User's Manual Cycle Programming | 2/2015

UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205, software option

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

If you enter different advance stop distances for Q258 and Q259, the TNC will change the advance stop distances between the first and last plunging depths at the same rate.

If you use Q379 to enter a deepened starting point, the TNC merely changes the starting point of the infeed movement. Retraction movements are not changed by the TNC, therefore they are calculated with respect to the coordinate of the workpiece surface.

3.8

19)

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.8 UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205, software option

19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole (tip of drill taper). Input range -99999.9999 to 99999.9999

Feed rate for plunging Q206: Traversing speed of the tool during drilling in mm/min. Input range 0 to

99999.999; alternatively FAUTO, FU Plunging depth Q202 (incremental): Infeed per cut.

Input range 0 to 99999.9999. The depth does not have to be a multiple of the plunging depth. The TNC will go to depth in one movement if:

the plunging depth is equal to the depth the plunging depth is greater than the depth

Coordinate of workpiece surface Q203 (absolute): Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Decrement Q212 (incremental): Value by which the TNC decreases the plunging depth Q202. Input range 0 to 99999.9999

Minimum plunging depth Q205 (incremental): If you have entered a decrement, the TNC limits the plunging depth to the value entered with Q205. Input range 0 to 99999.9999

Upper advanced stop distance Q258 (incremental): Set-up clearance for rapid traverse positioning when the TNC moves the tool again to the current plunging depth after retraction from the hole; value for the first plunging depth. Input range 0 to

99999.9999 Lower advanced stop distance Q259 (incremental):

Set-up clearance for rapid traverse positioning when the TNC moves the tool again to the current plunging depth after retraction from the hole; value for the last plunging depth. Input range 0 to

99999.9999 Infeed depth for chip breaking Q257

(incremental): Depth at which the TNC carries out chip breaking. No chip breaking if 0 is entered. Input range 0 to 99999.9999

Retraction rate for chip breaking Q256 (incremental): Value by which the TNC retracts the tool during chip breaking. Input range 0.000 to

99999.999 Dwell time at depth Q211: Time in seconds that

the tool remains at the hole bottom. Input range 0 to

3600.0000

NC blocks

11 CYCL DEF 205 UNIVERSAL PECKING

Q200=2 ;SET-UP CLEARANCE

Q201=-80 ;DEPTH

Q206=150 ;FEED RATE FOR

PLNGNG

Q202=15 ;PLUNGING DEPTH

Q203=+100;SURFACE COORDINATE

Q204=50 ;2ND SET-UP

CLEARANCE

Q212=0.5 ;DECREMENT

Q205=3 ;MIN. PLUNGING DEPTH

Q258=0.5 ;UPPER ADV. STOP

DIST.

Q259=1 ;LOWER ADV. STOP

DIST.

Q257=5 ;DEPTH FOR CHIP

BRKNG

Q256=0.2 ;DIST. FOR CHIP BRKNG

Q211=0.25 ;DWELL TIME AT

BOTTOM

Q379=7.5 ;START POINT

Q253=750 ;F PRE-POSITIONING

Q208=9999;RETRACTION FEED

RATE

Q395=0 ;DEPTH REFERENCE

TNC 620 | User's Manual Cycle Programming | 2/2015

UNIVERSAL PECKING (Cycle 205, DIN/ISO: G205, software option

19)

Deepened starting point Q379 (incremental with respect to the workpiece surface): Starting position for actual drilling operation. The TNC moves at the feed rate for pre-positioning from the set-up clearance above the workpiece surface to the set-up clearance above the deepened starting point. Input range 0 to 99999.9999

Feed rate for pre-positioning Q253: Defines the traversing speed of the tool when returning to the plunging depth after having retracted for chip breaking (Q256). This feed rate is also effective when the tool is positioned to a deepened starting point (Q379 not equal to 0). Entry in mm/min. Input range 0 to 99999.9999 alternatively FMAX, FAUTO

Feed rate for retraction Q208: Traversing speed of the tool in mm/min when retracting after the machining operation. If you enter Q208 = 0, the TNC retracts the tool at the feed rate Q206. Input range 0 to 99999.9999, alternatively FMAX,FAUTO

Depth reference Q395: Select whether the entered depth is referenced to the tool tip or the cylindrical part of the tool. If the TNC is to reference the depth to the cylindrical part of the tool, the point angle of the tool must be defined in the T ANGLE column of the tool table TOOL.T.

0 = Depth referenced to the tool tip 1 = Depth referenced to the cylindrical part of the

tool

3.8

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.9 BORE MILLING (Cycle 208, software option 19)

3.9 BORE MILLING (Cycle 208, software

option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the programmed set-up clearance above the workpiece

surface and then moves the tool to the bore hole circumference

on a rounded arc (if enough space is available). 2 The tool mills in a helix from the current position to the first

plunging depth at the programmed feed rate F. 3 When the drilling depth is reached, the TNC once again

traverses a full circle to remove the material remaining after the

initial plunge. 4 The TNC then positions the tool at the center of the hole again. 5

Finally the TNC returns to the setup clearance at FMAX. If

programmed, the tool moves to the 2nd set-up clearance at

FMAX.

TNC 620 | User's Manual Cycle Programming | 2/2015

BORE MILLING (Cycle 208, software option 19) 3.9

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

If you have entered the bore hole diameter to be the same as the tool diameter, the TNC will bore directly to the entered depth without any helical interpolation.

An active mirror function does not influence the type of milling defined in the cycle.

Note that if the infeed distance is too large, the tool or the workpiece may be damaged.

To prevent the infeeds from being too large, enter the maximum plunge angle of the tool in the ANGLE column of the tool table. The TNC then automatically calculates the max. infeed permitted and changes your entered value accordingly.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.9 BORE MILLING (Cycle 208, software option 19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool lower edge and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed

of the tool in mm/min during helical drilling. Input range 0 to 99999.999, alternatively FAUTO, FU, FZ

Infeed per helix Q334 (incremental): Depth of the tool plunge with each helix (=360°). Input range 0 to

99999.9999 Coordinate of workpiece surface Q203 (absolute):

Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Nominal diameter Q335 (absolute value): Bore-hole diameter. If you have entered the nominal diameter to be the same as the tool diameter, the TNC will bore directly to the entered depth without any helical interpolation. Input range 0 to 99999.9999

Roughing diameter Q342 (absolute): As soon as you enter a value greater than 0 in Q342, the TNC no longer checks the ratio between the nominal diameter and the tool diameter. This allows you to rough-mill holes whose diameter is more than twice as large as the tool diameter. Input range 0 to

99999.9999 Climb or up-cut Q351: Type of milling operation

with M3

+1 = Climb –1 = Up-cut

NC blocks

12 CYCL DEF 208 BORE MILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-80 ;DEPTH

Q206=150 ;FEED RATE FOR

PLNGNG

Q334=1.5 ;PLUNGING DEPTH

Q203=+100;SURFACE COORDINATE

Q204=50 ;2ND SET-UP

CLEARANCE

Q335=25 ;NOMINAL DIAMETER

Q342=0 ;ROUGHING DIAMETER

Q351=+1 ;CLIMB OR UP-CUT

TNC 620 | User's Manual Cycle Programming | 2/2015

SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241,

3.10 SINGLE-LIP DEEP-HOLE DRILLING

(Cycle 241, DIN/ISO: G241, software option 19)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the entered set-up clearance above the workpiece

surface. 2 Then the TNC moves the tool at the defined positioning feed

rate to the set-up clearance above the deepened starting point

and activates the drilling speed (M3) and the coolant. The TNC

executes the approach motion with the direction of rotation

defined in the cycle, with clockwise, counterclockwise or

stationary spindle. 3

The tool drills to the hole depth at the feed rate F, or to the

plunging depth if a smaller infeed value has been entered. The

plunging depth is decreased after each infeed by the decrement.

If you have entered a dwell depth, the TNC reduces the feed

rate by the feed rate factor after the dwell depth has been

reached. 4 If programmed, the tool remains at the hole bottom for chip

breaking. 5 The TNC repeats this process (3 to 4) until the programmed

total hole depth is reached. 6 After the TNC has reached the hole depth, the TNC switches off

the coolant and resets the drilling speed to the value defined for

retraction. 7 The tool is retracted to the set-up clearance at the retraction

feed rate. If programmed, the tool moves to the 2nd set-up

clearance at FMAX.

3.10

software option 19)

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.10 SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241, software option 19)

Cycle parameters

Set-up clearance Q200 (incremental): Distance between tool tip and workpiece surface. Input range 0 to 99999.9999

Depth Q201 (incremental): Distance between workpiece surface and bottom of hole. Input range

-99999.9999 to 99999.9999 Feed rate for plunging Q206: Traversing speed of

the tool during drilling in mm/min. Input range 0 to

99999.999; alternatively FAUTO, FU Dwell time at depth Q211: Time in seconds that

the tool remains at the hole bottom. Input range 0 to

3600.0000 Coordinate of workpiece surface Q203 (absolute):

Coordinate of the workpiece surface. Input range

-99999.9999 to 99999.9999 2nd set-up clearance Q204 (incremental):

Coordinate in the spindle axis at which no collision between tool and workpiece (fixtures) can occur. Input range 0 to 99999.9999

Retraction feed rate Q208: Traversing speed of the tool in mm/min when retracting from the hole. If you enter Q208 = 0, the TNC retracts the tool at the feed rate in Q206. Input range 0 to 99999.999, alternatively FMAX, FAUTO

Rotat. dir. of entry/exit (3/4/5) Q426: Desired direction of spindle rotation when tool moves into and retracts from the hole. Input:

3: Turn the spindle with M3 4: Turn the spindle with M4 5: Move with stationary spindle

Spindle speed of entry/exit Q427: Desired spindle speed when tool moves into and retracts from the hole. Input range 0 to 99999

Drilling speed Q428: Desired speed for drilling. Input range 0 to 99999

NC blocks

11 CYCL DEF 241 SINGLE-LIP

D.H.DRLNG

Q200=2 ;SET-UP CLEARANCE

Q201=-80 ;DEPTH

Q206=150 ;FEED RATE FOR

PLNGNG

Q211=0.25 ;DWELL TIME AT

BOTTOM

Q203=+100;SURFACE COORDINATE

Q204=50 ;2ND SET-UP

CLEARANCE

Q379=7.5 ;START POINT

Q253=750 ;F PRE-POSITIONING

Q208=1000;RETRACTION FEED

RATE

Q426=3 ;DIR. OF SPINDLE ROT.

Q427=25 ;ROT. SPEED INFEED/

OUT

Q428=500 ;DRILLING SPEED

Q429=8 ;COOLANT ON

Q430=9 ;COOLANT OFF

Q435=0 ;DWELL DEPTH

Q401=100 ;FEED RATE FACTOR

Q202=9999;MAX. PLUNGING

DEPTH PLUNGING DEPTH

Q212=0 ;DECREMENT

Q205=0 ;MIN. PLUNGING DEPTH

PLUNGING DEPTH

TNC 620 | User's Manual Cycle Programming | 2/2015

SINGLE-LIP DEEP-HOLE DRILLING (Cycle 241, DIN/ISO: G241,

software option 19)

M function for coolant on? Q429: M function for switching on the coolant. The TNC switches the coolant on if the tool is in the hole at the deepened starting point. Input range 0 to 999

M function for coolant off? Q430: M function for switching off the coolant. The TNC switches the coolant off if the tool is at the hole depth. Input range 0 to 999

Dwell depth Q435 (incremental): Coordinate in the spindle axis at which the tool is to dwell. If 0 is entered, the function is not active (standard setting). Application: During machining of throughholes some tools require a short dwell time before exiting the bottom of the hole in order to transport the chips to the top. Define a value smaller than the hole depth Q201; input range 0 to 99999.9999.

Feed rate factor Q401: Factor by which the TNC reduces the feed rate after the dwell depth has been reached. Input range 0 to 100

Plunging depth Q202 (incremental): Infeed per cut. The depth does not have to be a multiple of the plunging depth. Input range 0 to 99999.9999

Decrement Q212 (incremental): Value by which the TNC decreases the plunging depth Q202 after each infeed. Input range 0 to 99999.9999

Minimum plunging depth Q205 (incremental): If you have entered a decrement, the TNC limits the plunging depth to the value entered with Q205. Input range 0 to 99999.9999

3.10

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.11 Programming Examples

Example: Drilling cycles

0 BEGIN PGM C200 MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-20

2 BLK FORM 0.2 X+100 Y+100 Z+0

3 TOOL CALL 1 Z S4500

4 L Z+250 R0 FMAX

5 CYCL DEF 200 DRILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-15 ;DEPTH

Q206=250 ;FEED RATE FOR PLNGNG

Q202=5 ;PLUNGING DEPTH

Q210=0 ;DWELL TIME AT TOP

Q203=-10 ;SURFACE COORDINATE

Q204=20 ;2ND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT BOTTOM

Q395=0 ;DEPTH REFERENCE

6 L X+10 Y+10 R0 FMAX M3

7 CYCL CALL

8 L Y+90 R0 FMAX M99

9 L X+90 R0 FMAX M99

10 L Y+10 R0 FMAX M99

11 L Z+250 R0 FMAX M2

12 END PGM C200 MM

Definition of workpiece blank

Tool call (tool radius 3) Retract the tool Cycle definition

Approach hole 1, spindle ON Cycle call Approach hole 2, call cycle Approach hole 3, call cycle Approach hole 4, call cycle Retract the tool, end program

TNC 620 | User's Manual Cycle Programming | 2/2015

Example: Using drilling cycles in connection with PATTERN DEF

The drill hole coordinates are stored in the pattern definition PATTERN DEF POS and are called by the TNC with CYCL CALL PAT.

The tool radii are selected so that all work steps can be seen in the test graphics.

Program sequence

Centering (tool radius 4) Drilling (tool radius 2.4) Tapping (tool radius 3)

Programming Examples 3.11

0 BEGIN PGM 1 MM

1 BLK FORM 0.1 Z X+0 Y+0 Z-20

2 BLK FORM 0.2 X+100 Y+100 Y+0

3 TOOL CALL 1 Z S5000

4 L Z+10 R0 F5000

5 PATTERN DEF

POS1( X+10 Y+10 Z+0 )

POS2( X+40 Y+30 Z+0 )

POS3( X+20 Y+55 Z+0 )

POS4( X+10 Y+90 Z+0 )

POS5( X+90 Y+90 Z+0 )

POS6( X+80 Y+65 Z+0 )

POS7( X+80 Y+30 Z+0 )

POS8( X+90 Y+10 Z+0 )

6 CYCL DEF 240 CENTERING

Q200=2 ;SET-UP CLEARANCE

Q343=0 ;SELECT DEPTH/DIA.

Q201=-2 ;DEPTH

Q344=-10 ;DIAMETER

Q206=150 ;FEED RATE FOR PLNGNG

Q211=0 ;DWELL TIME AT BOTTOM

Q203=+0 ;SURFACE COORDINATE

Q204=50 ;2ND SET-UP CLEARANCE

7 CYCL CALL PAT F5000 M13

8 L Z+100 R0 FMAX

9 TOOL CALL 2 Z S5000

10 L Z+10 R0 F5000

Definition of workpiece blank

Call the centering tool (tool radius 4) Move tool to clearance height (enter a value for F): the TNC

positions to the clearance height after every cycle Define all drilling positions in the point pattern

Cycle definition: CENTERING

Call the cycle in connection with the hole pattern Retract the tool, change the tool Call the drilling tool (radius 2.4) Move tool to clearance height (enter a value for F)

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Drilling

3.11 Programming Examples

11 CYCL DEF 200 DRILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-25 ;DEPTH

Q206=150 ;FEED RATE FOR PLNGNG

Q202=5 ;PLUNGING DEPTH

Q211=0 ;DWELL TIME AT TOP

Q203=+0 ;SURFACE COORDINATE

Q204=50 ;2ND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT BOTTOM

Q395=0 ;DEPTH REFERENCE

12 CYCL CALL PAT F5000 M13

13 L Z+100 R0 FMAX

14 TOOL CALL 3 Z S200

15 L Z+50 R0 FMAX

16 CYCL DEF 206 TAPPING NEW

Q200=2 ;SET-UP CLEARANCE

Q201=-25 ;THREAD DEPTH

Q206=150 ;FEED RATE FOR PLNGNG

Q211=0 ;DWELL TIME AT BOTTOM

Q203=+0 ;SURFACE COORDINATE

Q204=50 ;2ND SET-UP CLEARANCE

17 CYCL CALL PAT F5000 M13

18 L Z+100 R0 FMAX M2

19 END PGM 1 MM

Cycle definition: drilling

Call the cycle in connection with the hole pattern Retract the tool Call the tapping tool (radius 3) Move tool to clearance height Cycle definition for tapping

Call the cycle in connection with the hole pattern Retract the tool, end program

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles:

Tapping / Thread

Milling

Fixed Cycles: Tapping / Thread Milling

4.1 Fundamentals

Overview

The TNC offers the following cycles for all types of threading operations:

Cycle Soft key Page

206 TAPPING NEW With a floating tap holder, with automatic pre-positioning, 2nd set-up clearance

207 TAPPING NEW Without a floating tap holder, with automatic pre-positioning, 2nd set-up clearance

209 TAPPING WITH CHIP BREAKING Without a floating tap holder, with automatic pre-positioning, 2nd set-up clearance, chip breaking

262 THREAD MILLING Cycle for milling a thread in pre-drilled material

263 THREAD MILLING/ COUNTERSINKING Cycle for milling a thread in pre-drilled material and machining a countersunk chamfer

264 THREAD DRILLING/MILLING Cycle for drilling into solid material with subsequent milling of the thread with a tool

265 HELICAL THREAD DRILLING/ MILLING Cycle for milling the thread into solid material

267 OUTSIDE THREAD MILLING Cycle for milling an external thread and machining a countersunk chamfer

102

105

111

114

118

122

126

TNC 620 | User's Manual Cycle Programming | 2/2015

TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206) 4.2

4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse

FMAX to the entered set-up clearance above the workpiece

surface. 2 The tool drills to the total hole depth in one movement. 3 Once the tool has reached the total hole depth, the direction of

spindle rotation is reversed and the tool is retracted to the set-

up clearance at the end of the dwell time. If programmed, the

tool moves to the 2nd set-up clearance at FMAX. 4 At the set-up clearance, the direction of spindle rotation

reverses once again.

TNC 620 | User's Manual Cycle Programming | 2/2015

Fixed Cycles: Tapping / Thread Milling

4.2 TAPPING with a floating tap holder (Cycle 206, DIN/ISO: G206)

Please note while programming:

Program a positioning block for the starting point (hole center) in the working plane with radius compensation R0.

The algebraic sign for the cycle parameter DEPTH determines the working direction. If you program DEPTH=0, the cycle will not be executed.

A floating tap holder is required for tapping. It must compensate the tolerances between feed rate and spindle speed during the tapping process.

When a cycle is being run, the spindle speed override knob is disabled. The feed-rate override knob is active only within a limited range, which is defined by the machine tool builder (refer to your machine manual).

For tapping right-hand threads activate the spindle with M3, for left-hand threads use M4.

If you enter the thread pitch of the tap in the Pitch column of the tool table, the TNC compares the thread pitch from the tool table with the thread pitch defined in the cycle. The TNC displays an error message if the values do not match. In Cycle 206 the TNC uses the programmed rotational speed and the feed rate defined in the cycle to calculate the thread pitch.

Danger of collision!

Use the machine parameter displayDepthErr to define whether, if a positive depth is entered, the TNC should output an error message (on) or not (off).

Keep in mind that the TNC reverses the calculation for pre-positioning when a positive depth is

entered. This means that the tool moves at rapid

traverse in the tool axis to set-up clearance below the workpiece surface!

100

TNC 620 | User's Manual Cycle Programming | 2/2015

heidenhain TNC 620 Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

TNC 620

Fundamentals

About this Manual

Would you like any changes, or have you found any errors?

TNC model, software and features

Software options

Feature Content Level (upgrade functions)

Intended place of operation

Legal information

Optional parameters

New cycle functions of software 81760x-01

New and changed cycle functions of software 81760x-02

Contents

1.1 Introduction

1.2 Available Cycle Groups

Overview of fixed cycles

Overview of touch probe cycles

Using Fixed Cycles

2.1 Working with fixed cycles

Machine-specific cycles (software option19)

Defining a cycle using soft keys

Defining a cycle using the GOTO function

Calling a cycle

2.2 Program defaults for cycles

Overview

Entering GLOBAL DEF

Using GLOBAL DEF information

Global data valid everywhere

Global data for drilling operations

Global data for milling operations with pocket cycles 25x

Global data for milling operations with contour cycles

Global data for positioning behavior

Global data for probing functions

2.3 PATTERN DEF pattern definition

Application

Entering PATTERN DEF

Using PATTERN DEF

Defining individual machining positions

Defining a single row

Defining a single pattern

Defining individual frames

Defining a full circle

Defining a pitch circle

2.4 Point tables

Application

Creating a point table

Hiding single points from the machining process

Selecting a point table in the program

Calling a cycle in connection with point tables

3.1 Fundamentals

Overview

3.2 CENTERING (Cycle 240, DIN/ISO: G240, software option 19)

Cycle run

Please note while programming:

Cycle parameters

3.3 DRILLING (Cycle 200)

Cycle run

Please note while programming:

Cycle parameters

REAMING (Cycle 201, DIN/ISO: G201, software option 19) 3.4

Cycle run

Please note while programming:

Cycle parameters

BORING (Cycle 202, DIN/ISO: G202, software option 19) 3.5

Cycle run

Please note while programming:

Cycle parameters

Cycle run

Please note while programming:

Cycle parameters

BACK BORING (Cycle 204, DIN/ISO: G204, software option 19) 3.7

Cycle run

Please note while programming:

Cycle parameters

Cycle run

Please note while programming: