heidenhain TNC 620 Users Manual

User’s Manual
HEIDENHAIN
Conversational Format

TNC 620

NC Software
340 560-01
340 561-01
340 564-01

English (en)
9/2008

Controls on the visual display unit

Split screen layout
Switch between machining or

programming modes
Soft keys for selecting functions on

screen
Shift between soft-key rows

Machine operating modes

Manual Operation

Electronic Handwheel

Positioning with Manual Data Input

Program Run, Single Block

Program Run, Full Sequence

Programming modes

Programming and Editing

Test Run

Program/file management, TNC functions

Select or delete programs and files
External data transfer

Define program call, select datum and point tables

Select MOD functions

Display help text for NC error messages

Display all current error messages

Show pocket calculator

Moving the cursor, going directly to blocks, cycles and
parameter functions

Go directly to blocks, cycles and parameter functions

Move highlight

Override control knobs for feed rate/spindle speed

100

0

1

S %

50

50

100

0

1

F %

50

50

Programming path movements

Approach/depart contour

FK free contour programming

Straight line

Circle center/pole for polar coordinates

Circle with center

Circle with radius

Circular arc with tangential connection

Chamfering/Corner rounding

Tool functions

Enter and call tool length and radius

Cycles, subprograms and program section repeats

Define and call cycles
Enter and call labels for subprogramming and

program section repeats

Program stop in a program

Define touch probe cycles

Coordinate axes and numbers: Entering and editing

. . .

. . .

Decimal point / Reverse algebraic sign
Polar coordinate input/

Select coordinate axes or
enter them into the program

Numbers

Incremental dimensions

Q parameter programming/Q parameter status

Save actual position or values from calculator

Skip dialog questions, delete words

Confirm entry and resume dialog

Conclude block and exit entry

Clear numerical entry or TNC error message

Abort dialog, delete program section

Delete individual characters

Special functions / smarT.NC

Show special functions

No function

Up/down one dialog box or button

HEIDENHAIN TNC 620 3

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 620 340 560-01

TNC 620 E 340 561-01

TNC 620 programming station 340 564-01

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:

 Probing function for the 3-D touch probe
 Rigid tapping
 Returning to the contour after an interruption

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.

Touch Probe Cycles User’s Manual:

All of the touch probe functions are described in a separate
manual. Please contact HEIDENHAIN if you need a copy of
this User’s Manual. ID: 661 891-20

HEIDENHAIN TNC 620 5

Software options

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

Hardware options

Additional axis for 4 axes and closed-loop spindle

Additional axis for 5 axes and closed-loop spindle

Software option 1 (option number #08)
Cylinder surface interpolation (Cycles 27, 28 and 29)

Feed rate in mm/min on rotary axes: M116

Tilting the machining plane (Cycle 19 and 3-D ROT soft key in the
manual operating mode)

Circle in 3 axes with tilted working plane

Software option 2 (option number #09)
Block processing time 1.5 ms instead of 6 ms

5-axis interpolation

3-D machining:

 M128: Maintaining the position of the tool tip when positioning

with tilted axes (TCPM)

 M144: Compensating the machine’s kinematics configuration for

ACTUAL/NOMINAL positions at end of block

 Additional finishing/roughing and tolerance for rotary axes

parameters in Cycle 32 (G62)

 LN blocks (3-D compensation)

Touch probe function (option number #17)
Touch probe cycles

 Compensation of tool misalignment in manual mode
 Compensation of tool misalignment in automatic mode

 Datum setting in manual mode
 Datum setting in automatic mode

 Automatic workpiece measurement
 Automatic tool measurement

6

Advanced programming features (option number #19)
FK free contour programming

 Programming in HEIDENHAIN conversational format with

graphic support for workpiece drawings not dimensioned for NC

Machining cycles

 Peck drilling, reaming, boring, counterboring, centering

(Cycles 201 to 205, 208, 240)

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

(Cycles 212 to 215)

 Clearing level and oblique surfaces (Cycles 230 to 232)
 Straight slots and circular slots (Cycles 210, 211)
 Linear and circular point patterns (Cycles 220, 221)
 Contour train, contour pocket—also with contour-parallel

machining (Cycles 20 to 25)

 OEM cycles (special cycles developed by the machine tool

builder) can be integrated

Advanced graphic features (option number #20)
Verification graphics, machining graphics

 Plan view
 Projection in three planes
 3-D view

Software option 3(option number #21)
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 number #22)
Pallet management

HEIDENHAIN DNC (option number #18)
Communication with external PC applications over COM

component

HEIDENHAIN TNC 620 7

Display step (option number #23)
Input resolution and display step:

 For linear axes to 0.01 µm
 Angular axes to 0.000 01°

Double speed (option number #49)
Double-speed control loops are used primarily for high-speed

spindles as well as linear motors and torque motors

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 soft key

8

Contents

Introduction

1

Manual Operation and Setup

Positioning with Manual Data Input

Programming: Fundamentals of File
Management, Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Cycles

Programming: Subprograms and
Program Section Repeats

Programming: Q Parameters

Test Run and Program Run

MOD Functions

Technical Information

2
3
4
5
6
7
8
9

10

11
12
13

HEIDENHAIN TNC 620 9

1 Introduction ..... 29

1.1 The TNC 620 ..... 30

Programming: HEIDENHAIN conversational format ..... 30

Compatibility ..... 30

1.2 Visual Display Unit and Keyboard ..... 31

Visual display unit ..... 31

Sets the screen layout ..... 32

Operating panel ..... 33

1.3 Operating Modes ..... 34

Manual Operation and Electronic Handwheel ..... 34

Positioning with Manual Data Input ..... 34

Programming and Editing ..... 35

Test Run ..... 35

Program Run, Full Sequence and Program Run, Single Block ..... 36

1.4 Status Displays ..... 37

“General” status display ..... 37

Additional status displays ..... 39

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels ..... 42

3-D touch probes ..... 42

TT 140 tool touch probe for tool measurement ..... 43

HR electronic handwheels ..... 43

HEIDENHAIN TNC 620 11

2 Manual Operation and Setup ..... 45

2.1 Switch-On, Switch-Off ..... 46

Switch-on ..... 46

Switch-off ..... 48

2.2 Traversing the Machine Axes ..... 49

Note ..... 49

To traverse with the machine axis direction buttons: ..... 49

Incremental jog positioning ..... 50

Traversing with the HR 410 electronic handwheel ..... 51

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 52

Function ..... 52

Entering values ..... 52

Changing the spindle speed and feed rate ..... 53

2.4 Datum Setting (Without a 3-D Touch Probe) ..... 54

Note ..... 54

Preparation ..... 54

Datum setting with axis keys ..... 55

Datum management with the preset table ..... 56

2.5 Tilting the Working Plane (Software Option 1) ..... 62

Application, function ..... 62

Traversing the reference points in tilted axes ..... 64

Position display in a tilted system ..... 64

Limitations on working with the tilting function ..... 64

Activating manual tilting ..... 65

12

3 Positioning with Manual Data Input (MDI) ..... 67

3.1 Programming and Executing Simple Machining Operations ..... 68

Positioning with Manual Data Input (MDI) ..... 68

Protecting and erasing programs in $MDI ..... 71

HEIDENHAIN TNC 620 13

4 Programming: Fundamentals of NC, File Management, Programming Aids ..... 73

4.1 Fundamentals ..... 74

Position encoders and reference marks ..... 74

Reference system ..... 74

Reference system on milling machines ..... 75

Designation of the axes on milling machines ..... 75

Polar coordinates ..... 76

Absolute and incremental workpiece positions ..... 77

Setting the datum ..... 78

4.2 File Management: Fundamentals ..... 79

Files ..... 79

Screen keypad ..... 81

Data backup ..... 81

4.3 Working with the File Manager ..... 82

Directories ..... 82

Paths ..... 82

Overview: Functions of the file manager ..... 83

Calling the file manager ..... 84

Selecting drives, directories and files ..... 85

Creating a new directory ..... 86

Copying a single file ..... 87

Copying a directory ..... 87

Choosing one of the last 10 files selected ..... 88

Deleting a file ..... 88

Deleting a directory ..... 88

Marking files ..... 89

Renaming a file ..... 90

File sorting ..... 90

Additional functions ..... 90

Data transfer to or from an external data medium ..... 91

Copying files into another directory ..... 93

The TNC in a network ..... 94

USB devices on the TNC ..... 95

4.4 Creating and Writing Programs ..... 96

Organization of an NC program in HEIDENHAIN conversational format ..... 96

Define the blank: BLK FORM ..... 96

Creating a new part program ..... 97

Programming tool movements in conversational format ..... 99

Actual position capture ..... 100

Editing a program ..... 101

The TNC search function ..... 105

14

4.5 Interactive Programming Graphics ..... 107

Generating / Not generating graphics during programming ..... 107

Generating a graphic for an existing program ..... 107

Block number display ON/OFF ..... 108

Erasing the graphic ..... 108

Magnifying or reducing a detail ..... 108

4.6 Structuring Programs ..... 109

Definition and applications ..... 109

Displaying the program structure window / Changing the active window ..... 109

Inserting a structuring block in the (left) program window ..... 109

Selecting blocks in the program structure window ..... 109

4.7 Adding Comments ..... 110

Function ..... 110

Adding a comment line ..... 110

Functions for editing of the comment ..... 110

4.8 Integrated Pocket Calculator ..... 111

Operation ..... 111

4.9 Error Messages ..... 113

Display of errors ..... 113

Open the error window ..... 113

Close the error window ..... 113

Detailed error messages ..... 114

INTERNAL INFO soft key ..... 114

Clearing errors ..... 115

Error log ..... 115

Keystroke log ..... 116

Informational texts ..... 117

Saving service files ..... 117

HEIDENHAIN TNC 620 15

5 Programming: Tools ..... 119

5.1 Entering Tool-Related Data ..... 120

Feed rate F ..... 120

Spindle speed S ..... 121

5.2 Tool Data ..... 122

Requirements for tool compensation ..... 122

Tool numbers and tool names ..... 122

Tool length L ..... 122

Tool radius R ..... 123

Delta values for lengths and radii ..... 123

Entering tool data into the program ..... 123

Entering tool data in the table ..... 124

Pocket table for tool changer ..... 130

Calling tool data ..... 133

5.3 Tool Compensation ..... 134

Introduction ..... 134

Tool length compensation ..... 134

Tool radius compensation ..... 135

5.4 Three-Dimensional Tool Compensation (Software Option 2) ..... 138

Introduction ..... 138

Definition of a normalized vector ..... 139

Permissible tool forms ..... 140

Using other tools: Delta values ..... 140

3-D compensation without tool orientation ..... 140

Face milling: 3-D compensation with and without tool orientation ..... 141

Peripheral milling: 3-D radius compensation with workpiece orientation ..... 142

16

6 Programming: Programming Contours ..... 145

6.1 Tool Movements ..... 146

Path functions ..... 146

FK free contour programming (Advanced programming features software option) ..... 146

Miscellaneous functions M ..... 146

Subprograms and program section repeats ..... 146

Programming with Q parameters ..... 146

6.2 Fundamentals of Path Functions ..... 147

Programming tool movements for workpiece machining ..... 147

6.3 Contour Approach and Departure ..... 150

Overview: Types of paths for contour approach and departure ..... 150

Important positions for approach and departure ..... 151

Approaching on a straight line with tangential connection: APPR LT ..... 153

Approaching on a straight line perpendicular to the first contour point: APPR LN ..... 153

Approaching on a circular path with tangential connection: APPR CT ..... 154

Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT ..... 155

Departing on a straight line with tangential connection: DEP LT ..... 156

Departing on a straight line perpendicular to the last contour point: DEP LN ..... 156

Departure on a circular path with tangential connection: DEP CT ..... 157

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT ..... 157

6.4 Path Contours—Cartesian Coordinates ..... 158

Overview of path functions ..... 158

Straight line L ..... 159

Inserting a chamfer CHF between two straight lines ..... 160

Corner rounding RND ..... 161

Circle center CC ..... 162

Circular path C around circle center CC ..... 163

Circular path CR with defined radius ..... 164

Circular path CT with tangential connection ..... 166

6.5 Path Contours—Polar Coordinates ..... 171

Overview ..... 171

Polar coordinate origin: Pole CC ..... 172

Straight line LP ..... 172

Circular path CP around pole CC ..... 173

Circular path CTP with tangential connection ..... 173

Helical interpolation ..... 174

HEIDENHAIN TNC 620 17

6.6 Path Contours—FK Free Contour Programming (Software Option) ..... 178

Fundamentals ..... 178

Graphics during FK programming ..... 180

Initiating the FK dialog ..... 181

Pole for FK programming ..... 181

Free programming of straight lines ..... 182

Free programming of circular arcs ..... 182

Input possibilities ..... 183

Auxiliary points ..... 186

Relative data ..... 187

18

7 Programming: Miscellaneous Functions ..... 195

7.1 Entering Miscellaneous Functions M and STOP ..... 196

Fundamentals ..... 196

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 198

Overview ..... 198

7.3 Miscellaneous Functions for Coordinate Data ..... 199

Programming machine-referenced coordinates: M91/M92 ..... 199

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130 ..... 201

7.4 Miscellaneous Functions for Contouring Behavior ..... 202

Machining small contour steps: M97 ..... 202

Machining open contours: M98 ..... 204

Feed rate for circular arcs: M109/M110/M111 ..... 205

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 (software option 3) ..... 206

Superimposing handwheel positioning during program run: M118 (software option 3) ..... 208

Retraction from the contour in the tool-axis direction: M140 ..... 209

Suppressing touch probe monitoring: M141 ..... 210

Delete basic rotation: M143 ..... 210

Automatically retract tool from the contour at an NC stop: M148 ..... 211

7.5 Miscellaneous Functions for Rotary Axes ..... 212

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1) ..... 212

Shorter-path traverse of rotary axes: M126 ..... 213

Reducing display of a rotary axis to a value less than 360°: M94 ..... 214

Maintaining the position of the tool tip when positioning with tilted axes (TCPM): M128 (software

option 2) ..... 215

HEIDENHAIN TNC 620 19

8 Programming: Cycles ..... 217

8.1 Working with Cycles ..... 218

Machine-specific cycles (Advanced programming features software option) ..... 218

Defining a cycle using soft keys ..... 219

Defining a cycle using the GOTO function ..... 219

Cycles Overview ..... 220

Calling cycles ..... 221

8.2 Cycles for Drilling, Tapping and Thread Milling ..... 223

Overview ..... 223

CENTERING (Cycle 240, Advanced programming features software option) ..... 225

DRILLING (Cycle 200) ..... 227

REAMING (Cycle 201, Advanced programming features software option) ..... 229

BORING (Cycle 202, Advanced programming features software option) ..... 231

UNIVERSAL DRILLING (Cycle 203, Advanced programming features software option) ..... 233

BACK BORING (Cycle 204, Advanced programming features software option) ..... 235

UNIVERSAL PECKING (Cycle 205, Advanced programming features software option) ..... 237

BORE MILLING (Cycle 208, Advanced programming features software option) ..... 240

TAPPING NEW with floating tap holder (Cycle 206) ..... 242

RIGID TAPPING without a floating tap holder NEW (Cycle 207) ..... 244

TAPPING WITH CHIP BREAKING (Cycle 209, Advanced programming features software option) ..... 246

Fundamentals of thread milling ..... 249

THREAD MILLING (Cycle 262, Advanced programming features software option) ..... 251

THREAD MILLING/COUNTERSINKING (Cycle 263, Advanced programming features software option) ..... 253

THREAD DRILLING/MILLING (Cycle 264, Advanced programming features software option) ..... 257

HELICAL THREAD DRILLING AND MILLING (Cycle 265, Advanced programming features software

option) ..... 261

OUTSIDE THREAD MILLING (Cycle 267, Advanced programming features software option) ..... 265

8.3 Cycles for Milling Pockets, Studs and Slots ..... 271

Overview ..... 271

POCKET MILLING (Cycle 4) ..... 272

POCKET FINISHING (Cycle 212, Advanced programming features software option) ..... 274

STUD FINISHING (Cycle 213, Advanced programming features software option) ..... 276

CIRCULAR POCKET (Cycle 5) ..... 278

CIRCULAR POCKET FINISHING (Cycle 214, Advanced programming features software option) ..... 280

CIRCULAR STUD FINISHING (Cycle 215, Advanced programming features software option) ..... 282

SLOT (oblong hole) with reciprocating plunge-cut (Cycle 210, Advanced programming features software

option) ..... 284

CIRCULAR SLOT (oblong hole) with reciprocating plunge-cut (Cycle 211, Advanced programming features

software option) ..... 287

8.4 Cycles for Machining Point Patterns ..... 293

Overview ..... 293

CIRCULAR PATTERN (Cycle 220, Advanced programming features software option) ..... 294

LINEAR PATTERN (Cycle 221, Advanced programming features software option) ..... 296

20

8.5 SL Cycles ..... 300

Fundamentals ..... 300

Overview of SL cycles ..... 302

CONTOUR GEOMETRY (Cycle 14) ..... 303

Overlapping contours ..... 304

CONTOUR DATA (Cycle 20, Advanced programming features software option) ..... 307

PILOT DRILLING (Cycle 21, Advanced programming features software option) ..... 308

ROUGH-OUT (Cycle 22, Advanced programming features software option) ..... 309

FLOOR FINISHING (Cycle 23, Advanced programming features software option) ..... 311

SIDE FINISHING (Cycle 24, Advanced programming features software option) ..... 312

CONTOUR TRAIN (Cycle 25, Advanced programming features software option) ..... 313

Program defaults for cylindrical surface machining cycles (software option 1!) ..... 315

CYLINDER SURFACE (Cycle 27, software option 1) ..... 316

CYLINDER SURFACE slot milling (Cycle 28, software option 1) ..... 318

CYLINDER SURFACE ridge milling (Cycle 29, software option 1) ..... 320

8.6 Cycles for Multipass Milling ..... 331

Overview ..... 331

MULTIPASS MILLING (Cycle 230, Advanced programming features software option) ..... 332

RULED SURFACE (Cycle 231, Advanced programming features software option) ..... 334

FACE MILLING (Cycle 232, Advanced programming features software option) ..... 337

8.7 Coordinate Transformation Cycles ..... 344

Overview ..... 344

Effect of coordinate transformations ..... 344

DATUM SHIFT (Cycle 7) ..... 345

DATUM SHIFT with datum tables (Cycle 7) ..... 346

DATUM SETTING (Cycle 247) ..... 349

MIRROR IMAGE (Cycle 8) ..... 350

ROTATION (Cycle 10) ..... 352

SCALING FACTOR (Cycle 11) ..... 353

AXIS-SPECIFIC SCALING (Cycle 26) ..... 354

WORKING PLANE (Cycle 19, software option 1) ..... 355

8.8 Special Cycles ..... 363

DWELL TIME (Cycle 9) ..... 363

PROGRAM CALL (Cycle 12) ..... 364

ORIENTED SPINDLE STOP (Cycle 13) ..... 365

TOLERANCE (Cycle 32) ..... 366

HEIDENHAIN TNC 620 21

9 Programming: Subprograms and Program Section Repeats ..... 369

9.1 Labeling Subprograms and Program Section Repeats ..... 370

Labels ..... 370

9.2 Subprograms ..... 371

Actions ..... 371

Programming notes ..... 371

Programming a subprogram ..... 371

Calling a subprogram ..... 371

9.3 Program Section Repeats ..... 372

Label LBL ..... 372

Actions ..... 372

Programming notes ..... 372

Programming a program section repeat ..... 372

Calling a program section repeat ..... 372

9.4 Separate Program as Subprogram ..... 373

Actions ..... 373

Programming notes ..... 373

Calling any program as a subprogram ..... 373

9.5 Nesting ..... 374

Types of nesting ..... 374

Nesting depth ..... 374

Subprogram within a subprogram ..... 374

Repeating program section repeats ..... 376

Repeating a subprogram ..... 377

9.6 Programming Examples ..... 378

22

10 Programming: Q Parameters ..... 385

10.1 Principle and Overview ..... 386

Programming notes ..... 387

Calling Q-parameter functions ..... 387

10.2 Part Families—Q Parameters in Place of Numerical Values ..... 388

Example NC blocks ..... 388

Example ..... 388

10.3 Describing Contours through Mathematical Operations ..... 389

Function ..... 389

Overview ..... 389

Programming fundamental operations ..... 390

10.4 Trigonometric Functions ..... 391

Definitions ..... 391

Programming trigonometric functions ..... 392

10.5 Calculating Circles ..... 393

Function ..... 393

10.6 If-Then Decisions with Q Parameters ..... 394

Function ..... 394

Unconditional jumps ..... 394

Programming If-Then decisions ..... 394

Abbreviations used: ..... 395

10.7 Checking and Changing Q Parameters ..... 396

Procedure ..... 396

10.8 Additional Functions ..... 397

Overview ..... 397

FN14: ERROR: Displaying error messages ..... 398

FN 16: F-PRINT: Formatted output of text and Q parameter values ..... 402

FN18: SYS-DATUM READ Read system data ..... 407

FN19: PLC: Transferring values to the PLC ..... 415

FN20: WAIT FOR: NC and PLC synchronization ..... 416

FN29: PLC: Transferring values to the PLC ..... 418

FN37:EXPORT ..... 418

10.9 Accessing Tables with SQL Commands ..... 419

Introduction ..... 419

A Transaction ..... 420

Programming SQL commands ..... 422

Overview of the soft keys ..... 422

SQL BIND ..... 423

SQL SELECT ..... 424

SQL FETCH ..... 427

SQL UPDATE ..... 428

SQL INSERT ..... 428

SQL COMMIT ..... 429

SQL ROLLBACK ..... 429

HEIDENHAIN TNC 620 23

10.10 Entering Formulas Directly ..... 430

Entering formulas ..... 430

Rules for formulas ..... 432

Programming example ..... 433

10.11 String Parameters ..... 434

String processing functions ..... 434

Assigning string parameters ..... 435

Chain-linking string parameters ..... 435

Converting a numerical value to a string parameter ..... 436

Copying a substring from a string parameter ..... 437

Converting a string parameter to a numerical value ..... 438

Checking a string parameter ..... 439

Finding the length of a string parameter ..... 440

Comparing alphabetic priority ..... 441

10.12 Preassigned Q Parameters ..... 442

Values from the PLC: Q100 to Q107 ..... 442

Active tool radius: Q108 ..... 442

Tool axis: Q109 ..... 442

Spindle status: Q110 ..... 443

Coolant on/off: Q111 ..... 443

Overlap factor: Q112 ..... 443

Unit of measurement for dimensions in the program: Q113 ..... 443

Tool length: Q114 ..... 443

Coordinates after probing during program run ..... 444

Deviation between actual value and nominal value during automatic tool measurement with the TT 130 ..... 445

Tilting the working plane with mathematical angles: rotary axis coordinates calculated by the TNC ..... 445

Measurement results from touch probe cycles (see also User’s Manual for Touch Probe Cycles) ..... 446

10.13 Programming Examples ..... 448

24

11 Test Run and Program Run ..... 455

11.1 Graphics (Advanced Graphic Features Software Option) ..... 456

Function ..... 456

Overview of display modes ..... 457

Plan view ..... 457

Projection in 3 planes ..... 458

3-D view ..... 459

Magnifying details ..... 460

Repeating graphic simulation ..... 462

Measuring the machining time ..... 462

11.2 Show the Workpiece in the Working Space (Advanced Graphic Features Software Option) ..... 463

Function ..... 463

11.3 Functions for Program Display ..... 464

Overview ..... 464

11.4 Test Run ..... 465

Function ..... 465

11.5 Program Run ..... 467

Function ..... 467

Running a part program ..... 468

Interrupting machining ..... 468

Moving the machine axes during an interruption ..... 469

Resuming program run after an interruption ..... 470

Mid-program startup (block scan) ..... 471

Returning to the contour ..... 472

11.6 Automatic Program Start ..... 473

Function ..... 473

11.7 Optional Block Skip ..... 474

Function ..... 474

Inserting the “/” character ..... 474

Erasing the “/” character ..... 474

11.8 Optional Program-Run Interruption ..... 475

Function ..... 475

HEIDENHAIN TNC 620 25

12 MOD Functions ..... 477

12.1 Selecting MOD Functions ..... 478

Selecting the MOD functions ..... 478

Changing the settings ..... 478

Exiting the MOD functions ..... 478

Overview of MOD functions ..... 479

12.2 Software Numbers ..... 480

Function ..... 480

12.3 Position Display Types ..... 481

Function ..... 481

12.4 Unit of Measurement ..... 482

Function ..... 482

12.5 Displaying Operating Times ..... 483

Function ..... 483

12.6 Entering Code Numbers ..... 484

Function ..... 484

12.7 Setting the Data Interfaces ..... 485

Serial interface on the TNC 620 ..... 485

Function ..... 485

Setting the RS-232 interface ..... 485

Setting the baud rate (baudRate) ..... 485

Set the protocol (protocol) ..... 485

Set the data bits (dataBits) ..... 486

Parity check (parity) ..... 486

Setting the stop bits (stopBits) ..... 486

Setting the handshake (flowControl) ..... 486

Settings for data transfer with the TNCserver PC software ..... 487

Setting the mode of the external device (fileSystem) ..... 487

Software for data transfer ..... 488

12.8 Ethernet Interface ..... 490

Introduction ..... 490

Connection possibilities ..... 490

Connecting the control to the network ..... 491

26

13 Tables and Overviews ..... 497

13.1 Machine-Specific User Parameters ..... 498

Function ..... 498

13.2 Pin Layout and Connecting Cables for Data Interfaces ..... 506

RS-232-C/V.24 interface for HEIDEHAIN devices ..... 506

Non-HEIDENHAIN devices ..... 507

Ethernet interface RJ45 socket ..... 507

13.3 Technical Information ..... 508

13.4 Exchanging the Buffer Battery ..... 515

HEIDENHAIN TNC 620 27

Introduction

1.1 The TNC 620

HEIDENHAIN TNC controls are workshop-oriented contouring
controls that enable you to program conventional machining
operations right at the machine in an easy-to-use conversational
programming language. The TNC 620 is designed for milling and
drilling machine tools, as well as machining centers, with up to 5 axes.
You can also change the angular position of the spindle under program
control.

Keyboard and screen layout are clearly arranged in such a way that the

1.1 The TNC 620

functions are fast and easy to use.

Programming: HEIDENHAIN conversational format

The HEIDENHAIN conversational programming format is an especially
easy method of writing programs. Interactive graphics illustrate the
individual machining steps for programming the contour. If a
production drawing is not dimensioned for NC, the FK free contour
programming feature (Advanced programming features software
option), performs the necessary calculations automatically. Workpiece
machining can be graphically simulated either during or before actual
machining (Advanced graphic features software option).

You can also enter and test one program while the control is running
another.

Compatibility

The scope of functions of the TNC 620 does not correspond to that of
the TNC 4xx and iTNC 530 series of controls. Therefore, machining
programs created on HEIDENHAIN contouring controls (starting from
the TNC 150 B) may not always run on the TNC 620. If NC blocks
contain invalid elements, the TNC will mark them as ERROR blocks
during download.

30

1.2 Visual Display Unit and
Keyboard

Visual display unit

The TNC is delivered with a 15-inch TFT color flat-panel display (see
figure at top right).

1 Header

When the TNC is on, the selected operating modes are shown in
the screen header: the machining mode at the left and the
programming mode at right. The currently active mode is
displayed in the larger box, where the dialog prompts and TNC
messages also appear (unless the TNC is showing only graphics).

2 Soft keys

In the footer the TNC indicates additional functions in a soft-key
row. You can select these functions by pressing the keys
immediately below them. The lines immediately above the soft­key row indicate the number of soft-key rows that can be called
with the black arrow keys to the right and left. The active soft-key
row is indicated by brightened bar.

3 Soft-key selection keys
4 Shift between soft-key rows
5 Selecting the screen layout
6 Shift key for switchover between machining and programming

modes

7 Soft-key selection keys for machine tool builders
8 Switches soft-key rows for machine tool builders
9 USB connection

1

1

9

1

5 1

4

2

3

1

8

7

6

4

1.2 Visual Display Unit and Keyboard

HEIDENHAIN TNC 620 31

Sets the screen layout

You select the screen layout yourself: In the programming mode of
operation, for example, you can have the TNC show program blocks in
the left window while the right window displays programming
graphics. You could also display status information in the right window
instead of the graphics, or display only program blocks in one large
window. The available screen windows depend on the selected
operating mode.

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row
shows the available layout options (see “Operating
Modes,” page 34).

Select the desired screen layout.

1.2 Visual Display Unit and Keyboard

32

Operating panel

The TNC 620 is delivered with an integrated keyboard. The figure at
right shows the controls and displays of the keyboard:

1  File management

 Online calculator
 MOD function
 HELP function

2 Programming modes
3 Machine operating modes
4 Initiation of programming dialog
5 Arrow keys and GOTO jump command
6 Numerical input and axis selection
7 Navigation keys

The functions of the individual keys are described on the inside front
cover.

Machine panel buttons, e.g. NC START or NC STOP, are
described in the manual for your machine tool.

1

3

4

1

6

2

1

5

77

1.2 Visual Display Unit and Keyboard

HEIDENHAIN TNC 620 33

1.3 Operating Modes

Manual Operation and Electronic Handwheel

The Manual Operation mode is required for setting up the machine
tool. In this operating mode, you can position the machine axes
manually or by increments and set the datums.

The Electronic Handwheel mode of operation allows you to move the
machine axes manually with the HR electronic handwheel.

Soft keys for selecting the screen layout (select as described
previously)

Window Soft key

1.3 Operating Modes

Positions

Left: positions, right: status display

Positioning with Manual Data Input

This mode of operation is used for programming simple traversing
movements, such as for face milling or pre-positioning.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program blocks, right: status display

34

Programming and Editing

In this mode of operation you can write your part programs. The FK
free programming feature, the various cycles and the Q parameter
functions help you with programming and add necessary information.
If desired, you can have the programming graphics show the individual
steps.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program blocks, right: program structure

Left: program blocks, right: graphics

Test Run

In the Test Run mode of operation, the TNC checks programs and
program sections for errors, such as geometrical incompatibilities,
missing or incorrect data within the program or violations of the work
space. This simulation is supported graphically in different display
modes (Advanced graphic features software option).

Soft keys for selecting the screen layout: see “Program Run, Full
Sequence and Program Run, Single Block,” page 36.

1.3 Operating Modes

HEIDENHAIN TNC 620 35

Program Run, Full Sequence and Program Run, Single Block

In the Program Run, Full Sequence mode of operation the TNC
executes a part program continuously to its end or to a manual or
programmed stop. You can resume program run after an interruption.

In the Program Run, Single Block mode of operation you execute each
block separately by pressing the machine START button.

Soft keys for selecting the screen layout

Window Soft key

Program

1.3 Operating Modes

Left: program blocks, right: status

Left: program blocks, right: graphics
(Advanced graphic features software option)

Graphics

36

1.4 Status Displays

“General” status display

The status display in the lower part of the screen informs you of the
current state of the machine tool. It is displayed automatically in the
following modes of operation:

 Program Run, Single Block and Program Run, Full Sequence, except

if the screen layout is set to display graphics only, and

 Positioning with Manual Data Input (MDI).

In the Manual mode and Electronic Handwheel mode the status
display appears in the large window.

1.4 Status Displays

HEIDENHAIN TNC 620 37

Information in the status display

ACTL

C

Symbol Meaning

.

Actual or nominal coordinates of the current position.

1.4 Status Displays

X Y Z

F S M

T
PM

Machine axes; the TNC displays auxiliary axes in
lower-case letters. The sequence and quantity of
displayed axes is determined by the machine tool
builder. Refer to your machine manual for more
information.

Tool number T

The displayed feed rate in inches corresponds to one
tenth of the effective value. Spindle speed S, feed
rate F and active M functions.

Axis locked.

Override setting in percent.

Axis can be moved with the handwheel.

Axes are moving under a basic rotation.

Axes are moving in a tilted working plane.

The function M128 (TCPM) is active.

No active program.

Program run started.

Stops the program run.

Program run is being aborted.

38

Additional status displays

The additional status displays contain detailed information on the
program run. They can be called in all operating modes except for the
Programming mode.

To switch on the additional status display:

Call the soft-key row for screen layout.

Select the layout option for the additional status
display.

To select an additional status display:

Shift the soft-key rows until the STATUS soft keys
appear.

Select the desired additional status display, e.g.
general program information.

You can choose between several additional status displays with the
following soft keys:

1.4 Status Displays

HEIDENHAIN TNC 620 39

General program information

Soft key Meaning

Name of the active main program

Active programs

Active machining cycle

Circle center CC (pole)

Machining time

1.4 Status Displays

Positions and coordinates

Soft key Meaning

Dwell time counter

Type of position display, e.g. actual position

Number of the active datum from the preset table.

Tilt angle of the working plane

Angle of a basic rotation

Information on tools

Soft key Meaning

 Display of tool: Tool number

Tool axis

Tool lengths and radii

Oversizes (delta values) from TOOL CALL (PGM) and
the tool table (TAB)

Tool life, maximum tool life (TIME 1) and maximum
tool life for TOOL CALL (TIME 2)

Display of the active tool and the (next) replacement
tool

40

Coordinate transformation

Soft key Meaning

Program name

Active datum shift (Cycle 7)

Mirrored axes (Cycle 8)

Active rotation angle (Cycle 10)

Active scaling factor(s) (Cycles 11 / 26)

See “Coordinate Transformation Cycles” on page 344.

Active miscellaneous functions M

Soft key Meaning

List of the active M functions with fixed meaning

List of the active M functions that are adapted by your
machine manufacturer

Status of Q parameters

1.4 Status Displays

Soft key Meaning

List of Q parameters defined with the Q PARAM LIST
soft key

HEIDENHAIN TNC 620 41

1.5 Accessories: HEIDENHAIN 3-D
Touch Probes and Electronic
Handwheels

3-D touch probes

If the Touch probe function software option is active, you can use
the various HEIDENHAIN 3-D touch probe systems to:

 Automatically align workpieces
 Quickly and precisely set datums
 Measure the workpiece during program run
 Measure and inspect tools

All of the touch probe functions are described in a
separate manual. Please contact HEIDENHAIN if you
require a copy of this User’s Manual. ID 661 891-10.

TS 220, TS 440 and TS 640 touch trigger probes

These touch probes are particularly effective for automatic workpiece
alignment, datum setting and workpiece measurement. The TS 220
transmits the triggering signals to the TNC via cable and may be a
more economical alternative.

The TS 440, TS 444, TS 640 and TS 740 (see figure at right) feature
infrared transmission of the triggering signal. This makes them highly
convenient for use on machines with automatic tool changers.

Principle of operation: HEIDENHAIN triggering touch probes feature a
wear-resistant optical switch that generates an electrical signal as
soon as the stylus is deflected. This signal is transmitted to the
control, which stores the current position of the stylus as an actual
value.

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels

42

TT 140 tool touch probe for tool measurement

The TT 140 is a triggering 3-D touch probe for tool measurement and
inspection. Your TNC provides three cycles for this touch probe with
which you can measure the tool length and radius automatically either
with the spindle rotating or stopped. The TT 140 features a particularly
rugged design and a high degree of protection, which make it
insensitive to coolants and swarf. The triggering signal is generated by
a wear-resistant and highly reliable optical switch.

HR electronic handwheels

Electronic handwheels facilitate moving the axis slides precisely by
hand. A wide range of traverses per handwheel revolution is available.
Apart from the HR 130 and HR 150 integral handwheels,
HEIDENHAIN also offers the HR 410 portable handwheel.

HEIDENHAIN TNC 620 43

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels

Manual Operation and Setup

2.1 Switch-On, Switch-Off

Switch-on

Switch-on and crossing of the reference points can vary
depending on the machine tool. Refer to your machine
manual.

Switch on the power supply for control and machine. The TNC then
displays the following dialog:

SYSTEM STARTUP

TNC is started

POWER INTERRUPTED

2.1 Switch-On, Switch-Off

TNC message that the power was interrupted—clear
the message.

CONVERT PLC PROGRAM

The PLC program of the TNC is automatically compiled.

RELAY EXT. DC VOLTAGE MISSING

Switch on external dc voltage. The TNC checks the
functioning of the EMERGENCY STOP circuit.

MANUAL OPERATION
TRAVERSE REFERENCE POINTS

Cross the reference points manually in the displayed
sequence: For each axis press the machine START
button, or

Cross the reference points in any sequence: Press
and hold the machine axis direction button for each
axis until the reference point has been traversed.

If your machine is equipped with absolute encoders, you
can leave out crossing the reference marks. In such a
case, the TNC is ready for operation immediately after the
machine control voltage is switched on.

46

The TNC is now ready for operation in the Manual Operation mode.

The reference points need only be crossed if the machine
axes are to be moved. If you intend only to write, edit or
test programs, you can select the Programming or Test
Run modes of operation immediately after switching on
the control voltage.

You can cross the reference points later by pressing the
PASS OVER REFERENCE soft key in the Manual
Operation mode.

Crossing the reference point in a tilted working plane

The TNC automatically activates the tilted working plane if this
function was enabled when the control was switched off. Then the
TNC moves the axes in the tilted coordinate system when an axis­direction key is pressed. Position the tool in such a way that a collision
is excluded during the subsequent crossing of the reference points. To
cross the reference points you have to deactivate the "Tilt Working
Plane" function, see “Activating manual tilting,” page 65.

Make sure that the angle values entered in the menu for
tilting the working plane match the actual angles of the
tilted axis.

Deactivate the "Tilt Working Plane" function before you
cross the reference points. Take care that there is no
collision. Retract the tool from the current position first, if
necessary.

2.1 Switch-On, Switch-Off

If you use this function, then for non-absolute encoders
you must confirm the positions of the rotary axes, which
the TNC displays in a pop-up window. The position
displayed is the last active position of the rotary axes
before switch-off.

HEIDENHAIN TNC 620 47

Switch-off

To prevent data from being lost at switch-off, you need to shut down
the operating system of the TNC as follows:

 Select the Manual Operation mode.

 Select the function for shutting down, confirm again

with the YES soft key.

 When the TNC displays the message NOW IT IS SAFE

TO TURN POWER OFF in a superimposed window, you

may cut off the power supply to the TNC.

Inappropriate switch-off of the TNC can lead to data loss.
Remember that pressing the END key after the control

has been shut down restarts the control. Switch-off
during a restart can also result in data loss!

2.1 Switch-On, Switch-Off

48

2.2 Traversing the Machine Axes

Note

Traversing with the machine axis direction buttons can
vary depending on the machine tool. The machine tool
manual provides further information.

To traverse with the machine axis direction buttons:

Select the Manual Operation mode.

Press the machine axis direction button and hold it as
long as you wish the axis to move, or

Move the axis continuously: Press and hold the
machine axis direction button, then press the

and

You can move several axes at a time with these two methods. You can
change the feed rate at which the axes are traversed with the F soft
key (see “Spindle Speed S, Feed Rate F and Miscellaneous Functions
M,” page 52).

machine START button.

To stop the axis, press the machine STOP button.

2.2 Traversing the Machine Axes

HEIDENHAIN TNC 620 49

Incremental jog positioning

With incremental jog positioning you can move a machine axis by a
preset distance.

Select the Manual Operation or Electronic Handwheel
mode.

Z

Select incremental jog positioning: Switch the
INCREMENT soft key to ON.

LINEAR AXES:

Enter the jog increment in mm, e.g. 8 mm, and press
the CONFIRM VALUE soft key.

Finish the entry with the OK soft key.

2.2 Traversing the Machine Axes

Press the machine axis direction button as often as
desired

To deactivate the function, press the Switch off soft key.

8

8

8

X

16

50

Traversing with the HR 410 electronic handwheel

The portable HR 410 handwheel is equipped with two permissive
buttons. The permissive buttons are located below the star grip.

You can only move the machine axes when a permissive button is
depressed (machine-dependent function).

The HR 410 handwheel features the following operating elements:

1 EMERGENCY STOP button
2 Handwheel
3 Permissive buttons
4 Axis address keys
5 Actual-position-capture key
6 Keys for defining the feed rate (slow, medium, fast; the feed rates

are set by the machine tool builder)

7 Direction in which the TNC moves the selected axis
8 Machine function (set by the machine tool builder)

The red indicator lights show the axis and feed rate you have selected.
It is also possible to move the machine axes with the handwheel

during program run if M118 is active (software option 3).

Procedure for traversing

Select the Electronic Handwheel operating mode.

1

2

3

4

6

8

4
5

7

2.2 Traversing the Machine Axes

Press and hold a permissive button.

Select the axis.

Select the feed rate.

Move the active axis in the positive or negative

or

HEIDENHAIN TNC 620 51

direction.

2.3 Spindle Speed S, Feed Rate F
and Miscellaneous Functions M

Function

In the Manual Operation and Electronic Handwheel operating modes,
you can enter the spindle speed S, feed rate F and the miscellaneous
functions M with soft keys. The miscellaneous functions are
described in Chapter 7 “Programming: Miscellaneous Functions.”

The machine tool builder determines which
miscellaneous functions M are available on your control
and what effects they have.

Entering values

Spindle speed S, miscellaneous function M

To enter the spindle speed, press the S soft key.

SPINDLE SPEED S =

1000

The spindle speed S with the entered rpm is started with a
miscellaneous function M. Proceed in the same way to enter a
miscellaneous function M.

Feed rate F

After entering a feed rate F, you must confirm your entry with the OK
key instead of the machine START button.

The following is valid for feed rate F:

 If you enter F=0, then the lowest feed rate from the machine

parameter minFeed is effective

 If the feed rate entered exceeds the value defined in the machine

parameter maxFeed, then the parameter value is effective.

 F is not lost during a power interruption

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M

Enter the desired spindle speed and confirm your
entry with the machine START button.

52

Changing the spindle speed and feed rate

With the override knobs you can vary the spindle speed S and feed
rate F from 0% to 150% of the set value.

The override knob for spindle speed is only functional on
machines with infinitely variable spindle drive.

HEIDENHAIN TNC 620 53

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M

2.4 Datum Setting (Without a 3-D
Touch Probe)

Note

For datum setting with a 3-D touch probe, refer to the
Touch Probe Cycles Manual.

You fix a datum by setting the TNC position display to the coordinates
of a known position on the workpiece.

Preparation

 Clamp and align the workpiece.
 Insert the zero tool with known radius into the spindle.
 Ensure that the TNC is showing the actual position values.

2.4 Datum Setting (Without a 3-D Touch Probe)

54

Datum setting with axis keys

Fragile workpiece?

If the workpiece surface must not be scratched, you can
lay a metal shim of known thickness d on it. Then enter a
tool axis datum value that is larger than the desired datum
by the value d.

Select the Manual Operation mode.

Move the tool slowly until it touches (scratches) the
workpiece surface.

Select the axis.

DATUM SET Z=

Zero tool in spindle axis: Set the display to a known
workpiece position (here, 0) or enter the thickness d
of the shim. In the tool axis, offset the tool radius.

Repeat the process for the remaining axes.
If you are using a preset tool, set the display of the tool axis to the

length L of the tool or enter the sum Z=L+d

The TNC automatically saves the datum set with the axis
keys in line 0 of the preset table.

Y

Z

Y

-R

-R

X

X

2.4 Datum Setting (Without a 3-D Touch Probe)

HEIDENHAIN TNC 620 55

Datum management with the preset table

You should definitely use the preset table if:

 Your machine is equipped with rotary axes (tilting table

or swivel head) and you work with the function for tilting
the working plane

 Up to now you have been working with older

TNC controls with REF-based datum tables

 You wish to machine identical workpieces that are

differently aligned

The preset table can contain any number of lines (datums).
To optimize the file size and the processing speed, you
should use only as many lines as you need for datum
management.

For safety reasons, new lines can be inserted only at the
end of the preset table.

Saving the datums in the preset table

The preset table has the name PRESET.PR, and is saved in the directory
TNC:\table. PRESET.PR is editable only in the Manual Operation and
Electronic Handwheel modes. In the Programming mode you can only

read the table, not edit it.
It is permitted to copy the preset table into another directory (for data

backup).
Never change the number of lines in the copied tables! That could

cause problems when you want to reactivate the table.
To activate the preset table copied to another directory you have to

copy it back to the directory TNC:\table.

2.4 Datum Setting (Without a 3-D Touch Probe)

56

There are several methods for saving datums and/or basic rotations in
the preset table:

 Through probing cycles in the Manual Operation or Electronic

Handwheel modes (see User’s Manual, Touch Probe Cycles,
Chapter 2)

 Through the Probing Cycles 400 to 419 (see User’s Manual, Touch

Probe Cycles, Chapter 3)

 Manual entry (see description below)

Basic rotations from the preset table rotate the coordinate
system about the preset, which is shown in the same line
as the basic rotation.

When setting a preset, take care that the position of the
tilting axes matches the corresponding values of the 3-D
ROT menu. Therefore:

 If the “Tilt working plane” function is not active, the

position displays for the rotary axes must = 0° (zero the
rotary axes if necessary).

 If the “Tilt working plane” function is active, the position

displays for the rotary axes must match the angles
entered in the 3-D ROT menu.

Line 0 in the preset table is write protected. In line 0, the
TNC always saves the datum that you most recently set
manually via the axis keys or via soft key.

HEIDENHAIN TNC 620 57

2.4 Datum Setting (Without a 3-D Touch Probe)

Manually saving the datums in the preset table

In order to set datums in the preset table, proceed as follows:

Select the Manual Operation mode.

Move the tool slowly until it touches (scratches) the
workpiece surface, or position the measuring dial
correspondingly.

Display the preset table: The TNC opens the preset
table

Select functions for entering the presets: The TNC
displays the available possibilities for entry in the soft­key row. See the table below for a description of the
entry possibilities.

Select the line in the preset table that you want to
change (the line number is the preset number).

2.4 Datum Setting (Without a 3-D Touch Probe)

If needed, select the column (axis) in the preset table
that you want to change.

Use the soft keys to select one of the available entry
possibilities (see the following table).

58

Function Soft key

Directly transfer the actual position of the tool
(the measuring dial) as the new datum: This
function only saves the datum in the axis which
is currently highlighted.

Assign any value to the actual position of the tool
(the measuring dial): This function only saves the
datum in the axis which is currently highlighted.
Enter the desired value in the pop-up window.

Incrementally shift a datum already stored in the
table: This function only saves the datum in the
axis which is currently highlighted. Enter the
desired corrective value with the correct sign in
the pop-up window. If inch display is active: Enter
the value in inches, and the TNC will internally
convert the entered values to mm.

Directly enter the new datum without calculation
of the kinematics (axis-specific). Only use this
function if your machine has a rotary table, and
you want to set the datum to the center of the
rotary table by entering 0. This function only
saves the datum in the axis which is currently
highlighted. Enter the desired value in the pop-up
window. If inch display is active: Enter the value
in inches, and the TNC will internally convert the
entered values to mm.

Select the BASIC TRANSFORMATION/AXIS
OFFSET view. The BASIC TRANSFORMATION
view shows the X, Y and Z columns. Depending
on the machine, the SPA, SPB and SPC columns
are displayed additionally. Here, the TNC saves
the basic rotation (for the Z tool axis, the TNC
uses the SPC column). The OFFSET view shows
the offset values to the preset.

Write the currently active datum to a selectable
line in the table: This function saves the datum in
all axes, and then activates the appropriate row in
the table automatically. If inch display is active:
enter the value in inches, and the TNC will
internally convert the entered values to mm.

HEIDENHAIN TNC 620 59

2.4 Datum Setting (Without a 3-D Touch Probe)

Editing the preset table

Editing function in table mode Soft key

Select beginning of table

Select end of table

Select previous page in table

Select next page in table

Select the functions for preset entry

Display Basic Transformation/Axis Offset
selection

Activate the datum of the selected line of the
preset table

Add the entered number of lines to the end of the
table (2nd soft-key row)

Copy the highlighted field (2nd soft-key row)

Insert the copied field (2nd soft-key row)

Reset the selected line: The TNC enters – in all
columns (2nd soft-key row)

2.4 Datum Setting (Without a 3-D Touch Probe)

Insert a single line at the end of the table
(2nd soft-key row)

Delete a single line at the end of the table
(2nd soft-key row)

60

Activating a datum from the preset table in the Manual Operation
mode

When activating a datum from the preset table, the TNC
resets the active datum shift, mirroring, rotation and
scaling factor.

However, a coordinate transformation that was
programmed in Cycle 19 Tilted Working Plane, remains
active.

Select the Manual Operation mode.

Display the preset table.

Select the datum number that you want to activate, or

Activate the preset.

Confirm activation of the datum. The TNC sets the
display and—if defined—the basic rotation.

Leave the preset table.

Activating a datum from the preset table in an NC program

To activate datums from the preset table during program run, use
Cycle 247. In Cycle 247 you define only the number of the datum that
you want to activate (see “DATUM SETTING (Cycle 247)” on page

349).

HEIDENHAIN TNC 620 61

2.4 Datum Setting (Without a 3-D Touch Probe)

2.5 Tilting the Working Plane
(Software Option 1)

Application, function

The functions for tilting the working plane are interfaced to
the TNC and the machine tool by the machine tool builder.
With some swivel heads and tilting tables, the machine tool
builder determines whether the entered angles are
interpreted as coordinates of the rotary axes or as angular
components of a tilted plane. Refer to your machine
manual.

The TNC supports the tilting functions on machine tools with swivel
heads and/or tilting tables. Typical applications are, for example,
oblique holes or contours in an oblique plane. The working plane is
always tilted around the active datum. The program is written as usual
in a main plane, such as the X/Y plane, but is executed in a plane that
is tilted relative to the main plane.

There are two functions available for tilting the working plane:

 3-D ROT soft key in the Manual Operation mode and Electronic

Handwheel mode (see “Activating manual tilting,” page 65).

 Tilting under program control, Cycle 19 WORKING PLANE, in the part

program (see “WORKING PLANE (Cycle 19, software option 1)” on
page 355).

The TNC functions for "tilting the working plane" are coordinate
transformations. The working plane is always perpendicular to the
direction of the tool axis.

Z

Y

B

10°

X

2.5 Tilting the Working Plane (Software Option 1)

62

When tilting the working plane, the TNC differentiates between two
machine types:

 Machine with tilting tables

 You must tilt the workpiece into the desired position for

machining by positioning the tilting table, for example with an
L block.

 The position of the transformed tool axis does not change in

relation to the machine-based coordinate system. Thus if you
rotate the table—and therefore the workpiece—by 90° for
example, the coordinate system does not rotate. If you press the
Z+ axis direction button in the Manual Operation mode, the tool
moves in Z+ direction.

 In calculating the transformed coordinate system, the TNC

considers only the mechanically influenced offsets of the
particular tilting table (the so-called “translational” components).

 Machine with swivel head

 You must bring the tool into the desired position for machining by

positioning the swivel head, for example with an L block.

 The position of the transformed tool axis changes in relation to the

machine-based coordinate system. Thus if you rotate the swivel
head of your machine—and therefore the tool—in the B axis by
90° for example, the coordinate system rotates also. If you press
the Z+ axis direction button in the Manual Operation mode, the
tool moves in X+ direction of the machine-based coordinate
system.

 In calculating the transformed coordinate system, the TNC

considers both the mechanically influenced offsets of the
particular swivel head (the so-called “translational” components)
and offsets caused by tilting of the tool (3-D tool length
compensation).

HEIDENHAIN TNC 620 63

2.5 Tilting the Working Plane (Software Option 1)

Traversing the reference points in tilted axes

The TNC automatically activates the tilted working plane if this
function was enabled when the control was switched off. Then the
TNC moves the axes in the tilted coordinate system when an axis­direction key is pressed. Position the tool in such a way that a collision
is excluded during the subsequent crossing of the reference points.
To cross the reference points you have to deactivate the "Tilt Working
Plane" function!

Position display in a tilted system

The positions displayed in the status window (ACTL. and NOML.) are
referenced to the tilted coordinate system.

Limitations on working with the tilting function

 PLC positioning (determined by the machine tool builder) is not

possible.

2.5 Tilting the Working Plane (Software Option 1)

64

Activating manual tilting

To select manual tilting, press the 3-D ROT soft key.

Use the arrow keys to move the highlight to the
Manual Operation menu item.

Open the selection menu with the GOTO key and use
the arrow key to select the Active menu item;
confirm with the ENT key.

Use the arrow keys to position the highlight on the
desired rotary axis.

Enter the tilt angle or

Press the CONFIRM VALUE soft key to confirm the
current REF position of the active rotary axes.

To conclude entry, press the OK soft key.

To cancel the entry, press the CANCEL soft key.

To reset the tilting function, set the desired operating modes in the
menu “Tilt working plane” to inactive.

If the tilted working plane function is active and the TNC moves the
machine axes in accordance with the tilted axes, the status display
shows the symbol.

If you activate the “Tilt working plane” function for the Program Run
operating mode, the tilt angle entered in the menu becomes active in
the first block of the part program. If you use Cycle 19 WORKING PLANE
in the machining program, the angle values defined there are in effect.
The TNC will then overwrite the angle values entered in the menu with
the values from Cycle 19.

2.5 Tilting the Working Plane (Software Option 1)

HEIDENHAIN TNC 620 65

Positioning with Manual Data Input (MDI)

3.1 Programming and Executing
Simple Machining Operations

The Positioning with Manual Data Input mode of operation is
particularly convenient for simple machining operations or pre­positioning of the tool. You can write a short program in HEIDENHAIN
conversational programming and execute it immediately. You can also
call TNC cycles. The program is stored in the file $MDI. In the
Positioning with MDI mode of operation, the additional status displays
can also be activated.

Positioning with Manual Data Input (MDI)

Select the Positioning with MDI mode of operation.
Program the file $MDI as you wish.

To start program run, press the machine START key.

Constraints:
The following functions are not available in the MDI mode:

 FK free contour programming
 Program section repeats
 Subprogramming
 Path compensation
 The programming graphics
 Program call PGM CALL
 The program-run graphics

3.1 Programming and Executing Simple Machining Operations

68

Example 1

A hole with a depth of 20 mm is to be drilled into a single workpiece.
After clamping and aligning the workpiece and setting the datum, you
can program and execute the drilling operation in a few lines.

First you pre-position the tool in L blocks (straight-line blocks) to the
hole center coordinates at a setup clearance of 5 mm above the
workpiece surface. Then drill the hole with Cycle 200 DRILLING.

0 BEGIN PGM $MDI MM
1 TOOL CALL 1 Z S1860

2 L Z+200 R0 FMAX
3 L X+50 Y+50 R0 FMAX M3

4 CYCL DEF 200 DRILLING

Q200=5 ;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 DEPTH
5 CYCL CALL
6 L Z+200 R0 FMAX M2
7 END PGM $MDI MM

Z

Y

50

50

Call tool: tool axis Z
Spindle speed 1860 rpm
Retract tool (F MAX = rapid traverse)
Move the tool at F MAX to a position above the

hole,
Spindle on
Define DRILLING cycle
Set-up clearance of the tool above the hole
Total hole depth (algebraic sign=working direction)
Feed rate for drilling
Depth of each plunge before retraction
Dwell time after every retraction in seconds
Coordinate of the workpiece surface
Set-up clearance of the tool above the hole
Dwell time in seconds at the hole bottom
Call DRILLING cycle
Retract the tool
End of program

X

Straight line function L, (see “Straight line L” on page 159) DRILLING
cycle. (see “DRILLING (Cycle 200)” on page 227).

HEIDENHAIN TNC 620 69

3.1 Programming and Executing Simple Machining Operations

Example 2: Correcting workpiece misalignment on machines
with rotary tables

Use the 3-D touch probe to rotate the coordinate system
(Touch probe function software option). See “Touch Probe Cycles in
the Manual and Electronic Handwheel Operating Modes,” section
“Compensating workpiece misalignment,” in the Touch Probe Cycles
User’s Manual.

Write down the rotation angle and cancel the basic rotation.

Select operating mode: Positioning with MDI.

Select the axis of the rotary table, enter the rotation
angle you wrote down previously and set the feed
rate. For example: L C+2.561 F50

Conclude entry.

Press the machine START button: The rotation of the
table corrects the misalignment.

3.1 Programming and Executing Simple Machining Operations

70

Protecting and erasing programs in $MDI

The $MDI file is generally intended for short programs that are only
needed temporarily. Nevertheless, you can store a program, if
necessary, by proceeding as described below:

Select the Programming and Editing mode of
operation.

Press the PGM MGT key (program management) to
call the file manager.

Move the highlight to the $MDI file.

To select the file copying function, press the COPY
soft key.

TARGET FILE =

BOREHOLE

For more information, see “Copying a single file,” page 87.

Enter the name under which you want to save the
current contents of the $MDI file.

Copy the file.

Press the END soft key to close the file manager.

3.1 Programming and Executing Simple Machining Operations

HEIDENHAIN TNC 620 71

Programming: Fundamentals of NC, File Management, Programming Aids

4.1 Fundamentals

Position encoders and reference marks

The machine axes are equipped with position encoders that register
the positions of the machine table or tool. Linear axes are usually
equipped with linear encoders, rotary tables and tilting axes with angle
encoders.

When a machine axis moves, the corresponding position encoder
generates an electrical signal. The TNC evaluates this signal and
calculates the precise actual position of the machine axis.

4.1 Fundamentals

If there is a power interruption, the calculated position will no longer
correspond to the actual position of the machine slide. To recover this
association, incremental position encoders are provided with
reference marks. The scales of the position encoders contain one or
more reference marks that transmit a signal to the TNC when they are
crossed over. From that signal the TNC can re-establish the
assignment of displayed positions to machine positions. For linear
encoders with distance-coded reference marks the machine axes
need to move by no more than 20 mm, for angle encoders by no more
than 20°.

With absolute encoders, an absolute position value is transmitted to
the control immediately upon switch-on. In this way the assignment
of the actual position to the machine slide position is re-established
directly after switch-on.

X

MP

X (Z,Y)

Z

Y

X

Reference system

A reference system is required to define positions in a plane or in
space. The position data are always referenced to a predetermined
point and are described through coordinates.

The Cartesian coordinate system (a rectangular coordinate system) is
based on the three coordinate axes X, Y and Z. The axes are mutually
perpendicular and intersect at one point called the datum. A
coordinate identifies the distance from the datum in one of these
directions. A position in a plane is thus described through two
coordinates, and a position in space through three coordinates.

Coordinates that are referenced to the datum are referred to as
absolute coordinates. Relative coordinates are referenced to any other
known position (reference point) you define within the coordinate
system. Relative coordinate values are also referred to as incremental
coordinate values.

Z

Y

X

74

Reference system on milling machines

When using a milling machine, you orient tool movements to the
Cartesian coordinate system. The illustration at right shows how the
Cartesian coordinate system describes the machine axes. The figure
illustrates the right-hand rule for remembering the three axis
directions: the middle finger points in the positive direction of the tool
axis from the workpiece toward the tool (the Z axis), the thumb points
in the positive X direction, and the index finger in the positive Y
direction.

As an option, the TNC 620 can control up to 5 axes. The axes U, V and
W (which are not presently supported by the TNC 620) are secondary
linear axes parallel to the main axes X, Y and Z, respectively. Rotary
axes are designated as A, B and C. The illustration at lower right shows
the assignment of secondary axes and rotary axes to the main axes.

Designation of the axes on milling machines

The X, Y and Z axes on your milling machine are also referred to as tool
axis, principal axis (1st axis) and minor axis (2nd axis). The assignment
of the tool axis is decisive for the assignment of the principal and
minor axes.

Tool axis Principal axis Minor axis

XYZ

YZX

+Y

+Z

+Y

+X

+Z

+X

4.1 Fundamentals

Z

Y

W+

ZXY

V+

B+

C+

A+

X

U+

HEIDENHAIN TNC 620 75

Polar coordinates

If the production drawing is dimensioned in Cartesian coordinates, you
also write the part program using Cartesian coordinates. For parts
containing circular arcs or angles it is often simpler to give the
dimensions in polar coordinates.

While the Cartesian coordinates X, Y and Z are three-dimensional and
can describe points in space, polar coordinates are two-dimensional
and describe points in a plane. Polar coordinates have their datum at a
circle center (CC), or pole. A position in a plane can be clearly defined
by the:

 Polar Radius, the distance from the circle center CC to the position,

4.1 Fundamentals

and the

 Polar Angle, the value of the angle between the reference axis and

the line that connects the circle center CC with the position.

Setting the pole and the angle reference axis

The pole is set by entering two Cartesian coordinates in one of the
three planes. These coordinates also set the reference axis for the
polar angle PA.

Y

PR

PA

2

PA

3

10

PR

CC

PA

PR

1

0°

X

30

Coordinates of the pole
(plane)

X/Y +X

Y/Z +Y

Z/X +Z

Reference axis for the angle

Z

Y

Z

Y

X

Z

Y

X

X

76

Absolute and incremental workpiece positions

Absolute workpiece positions

Absolute coordinates are position coordinates that are referenced to
the datum of the coordinate system (origin). Each position on the
workpiece is uniquely defined by its absolute coordinates.

Example 1: Holes dimensioned in absolute coordinates

Hole 1 Hole 2 Hole 3
X = 10 mm X = 30 mm X = 50 mm
Y = 10 mm Y = 20 mm Y = 30 mm

Y

3

30

2

20

1

10

4.1 Fundamentals

Incremental workpiece positions

Incremental coordinates are referenced to the last programmed
nominal position of the tool, which serves as the relative (imaginary)
datum. When you write a part program in incremental coordinates,
you thus program the tool to move by the distance between the
previous and the subsequent nominal positions. Incremental
coordinates are therefore also referred to as chain dimensions.

To program a position in incremental coordinates, enter the prefix “I”
before the axis.

Example 2: Holes dimensioned in incremental coordinates
Absolute coordinates of hole 4
X = 10 mm

Y = 10 mm
Hole 5, relative to 4 Hole 6, relative to 5

X = 20 mm X = 20 mm
Y = 10 mm Y = 10 mm

Absolute and incremental polar coordinates

Absolute polar coordinates always refer to the pole and the reference
axis.

Incremental polar coordinates always refer to the last programmed
nominal position of the tool.

X

10 30 50

Y

6

5

4

10 10

10

10

20

20

X

Y

+IPR

PR

PA

PR

0°

+IPA

PR

10

+IPA

CC

X

30

HEIDENHAIN TNC 620 77

Setting the datum

A production drawing identifies a certain form element of the
workpiece, usually a corner, as the absolute datum. When setting the
datum, you first align the workpiece along the machine axes, and then
move the tool in each axis to a defined position relative to the
workpiece. Set the display of the TNC either to zero or to a known
position value for each position. This establishes the reference system
for the workpiece, which will be used for the TNC display and your part
program.

If the production drawing is dimensioned in relative coordinates,
simply use the coordinate transformation cycles (see “Coordinate

4.1 Fundamentals

Transformation Cycles” on page 344).
If the production drawing is not dimensioned for NC, set the datum at

a position or corner on the workpiece which is suitable for deducing
the dimensions of the remaining workpiece positions.

The fastest, easiest and most accurate way of setting the datum is by
using a 3-D touch probe from HEIDENHAIN. See “Setting the Datum
with a 3-D Touch Probe” in the Touch Probe Cycles User’s Manual.

Example

The workpiece drawing at right shows holes (1 to 4) whose
dimensions are shown with respect to an absolute datum with the
coordinates X=0, Y=0. Holes 5 to 7 are dimensioned with respect to a
relative datum with the absolute coordinates X=450, Y=750. With the
DATUM SHIFT cycle you can temporarily set the datum to the position
X=450, Y=750, to be able to program holes 5 to 7 without further
calculations.

750

320

Z

Y

MAX

X

MIN

Y

150

7

0

6
5

-150

0,1
±

300

3 4

0

21

325

450 900

950

78

X

4.2 File Management:
Fundamentals

Files

Files in the TNC Ty p e
Programs

In HEIDENHAIN format
In DIN/ISO format

.H
.I

Tables for

Tools
Tool changers
Datums
Presets
Touch probes
Backup files

Texts as

ASCII files
Log files

When you write a part program on the TNC, you must first enter a file
name. The TNC saves the program as a file with the same name. The
TNC can also save texts and tables as files.

The TNC provides a special file management window in which you can
easily find and manage your files. Here you can call, copy, rename and
erase files.

With the TNC you can manage and save files up to a total size of
300 MB.

Depending on the setting, the TNC generates a backup file
(*.bak) after editing and saving of NC programs. This can
reduce the memory space available to you.

.T
.TCH
.D
.PR
.TP
.BAK

.A
.TXT

4.2 File Management: Fundamentals

HEIDENHAIN TNC 620 79

File names

When you store programs, tables and texts as files, the TNC adds an
extension to the file name, separated by a point. This extension
indicates the file type.

PROG20 .H
File name File type

File names should not exceed 25 characters, otherwise the TNC
cannot display the entire file name. The following characters are not
permitted in file names:

! “ ’ ( ) * + / ; < = > ? [ ] ^ ` { | } ~

The space (HEX 20) and delete (HEX 7F) characters are not
permitted in file names, either.

The maximum limit for the path and file name together is
256 characters (see “Paths” on page 82).

4.2 File Management: Fundamentals

80

Screen keypad

You can enter letters and special characters with the screen keypad or
(if available) with a PC keyboard connected over the USB port.

Enter the text with the screen keypad

 Press the GOTO key if you want to enter a text, for example a

program name or directory name, using the screen keypad

 The TNC opens a window in which the numeric entry field of the

TNC is displayed with the corresponding letters assigned

 You can move the cursor to the desired character by repeatedly

pressing the respective key

 Wait until the selected character is transferred to the entry field

before you enter the next character

 Use the OK soft key to load the text into the open dialog field

Use the abc/ABC soft key to select upper or lower case. If your
machine tool builder has defined additional special characters, you can
call them with the SPECIAL CHARACTER soft key and insert them.
To delete individual characters, use the Backspace soft key.

Data backup

We recommend saving newly written programs and files on a PC at
regular intervals.

HEIDENHAIN provides a backup function for this purpose in the data
transfer software TNCremoNT. Your machine tool builder can provide
you with a copy of TNCBACK.EXE.

You additionally need a data medium on which all machine-specific
data, such as the PLC program, machine parameters, etc., are stored.
Please contact your machine tool builder for more information on both
the backup program and the floppy disk.

4.2 File Management: Fundamentals

Take the time occasionally to delete any unneeded files so
that the TNC always has enough memory space for
system files (such as the tool table).

HEIDENHAIN TNC 620 81

4.3 Working with the File Manager

Directories

If you save many programs in the TNC, we recommend that you save
your files in directories (folders) so that you can easily find your data.
You can divide a directory into further directories, which are called
subdirectories. With the –/+ key or ENT you can show or hide the
subdirectories.

Paths

A path indicates the drive and all directories and subdirectories under
which a file is saved. The individual names are separated by a
backslash “\”.

Example

The directory AUFTR1 was created on the TNC:\ drive. Then, in the
AUFTR1 directory, the directory NCPROG was created and the part

program PROG1.H was copied into it. The part program now has the
following path:

TNC:\AUFTR1\NCPROG\PROG1.H

4.3 Working with the File Manager

The chart at right illustrates an example of a directory display with
different paths.

TNC:\

AUFTR1

NCPROG

WZTAB

A35K941

ZYLM

TESTPROG
HUBER

KAR25T

82

Overview: Functions of the file manager

Function Soft key

Copying a file

Display a specific file type

Display the last 10 files that were selected

Delete a file or directory

Mark a file

Rename a file

Manage network drives

Select the editor

Protect a file against editing and erasure

Cancel file protection

Create new file

Sort files by properties

Copy a directory

Delete directory with all its subdirectories

Display all the directories of a particular drive

Rename directory

Create a new directory

4.3 Working with the File Manager

HEIDENHAIN TNC 620 83

Calling the file manager

Press the PGM MGT key: the TNC displays the file
management window (The figure at right shows the
factory default setting. If the TNC displays a different
screen layout, press the WINDOW soft key.)

The narrow window on the left shows the available drives and
directories. Drives designate devices with which data are stored or
transferred. One drive is the internal memory of the TNC. Other drives
are the RS232, RS422, Ethernet and USB interfaces, which you can
used, for example, to connect a personal computer or other storage
device. A directory is always identified by a folder symbol to the left
and the directory name to the right. A subdirectory is displayed to the
right of and below its parent directory. A box with the + symbol in front
of the folder symbol indicates that there are further subdirectories,
which can be shown with the –/+ key or ENT.

The wide window on the right shows you all files that are stored in the
selected directory. Each file is shown with additional information,
illustrated in the table below.

Column Meaning

4.3 Working with the File Manager

FILE NAME Name with an extension, separated by a dot

(file type)

BYTE File size in bytes

STATUS

E

S

M

DATE Date on which file was last changed

TIME Time at which file was last changed

84

File properties:

Program is selected in the Programming
mode of operation.

Program is selected in the Test Run mode of
operation.

Program is selected in a Program Run mode
of operation.

File is protected against editing and erasure.

Selecting drives, directories and files

Call the file manager

Use the arrow keys or the soft keys to move the highlight to the
desired position on the screen:

Moves the highlight from the left to the right window,
and vice versa.

Moves the highlight up and down within a window.

Moves the highlight one page up or down within a
window.

Step 1: Select drive

Move the highlight to the desired drive in the left window:

4.3 Working with the File Manager

Select a drive: Press the SELECT soft key or the ENT

or

Step 2: Select a directory

Move the highlight to the desired directory in the left-hand window—
the right-hand window automatically shows all files stored in the
highlighted directory.

key.

HEIDENHAIN TNC 620 85

Step 3: Select a file

Press the SELECT TYPE soft key.

Press the soft key for the desired file type, or

Press the SHOW ALL soft key to display all files, or

Move the highlight to the desired file in the right window

The selected file is opened in the operating mode
from which you have called the File Manager. Now

or

Creating a new directory

4.3 Working with the File Manager

Move the highlight in the left window to the directory in which you
want to create a subdirectory.

press the SELECT soft key or the ENT key.

NEW

DIRECTORY NAME?

86

Enter the new file name, and confirm with ENT.

Press the OK soft key to confirm, or

abort with the CANCEL soft key.

Copying a single file

 Move the highlight to the file you wish to copy.

 Press the COPY soft key to select the copy function.

The TNC opens a pop-up window

 Enter the name of the destination file and confirm your

entry with the ENT key or OK soft key. The TNC
copies the file to the active directory or to the
corresponding destination directory. The original file
is retained.

Copying a directory

Move the highlight in the left window onto the directory you want to
copy. Then press the COPY DIR soft key instead of the COPY soft key.
Subdirectories can be copied by the TNC at the same time.

Making a setting in a selection box

In various dialogs, the TNC opens a pop-up window in which you can
make settings in selection boxes.

 Move the cursor into the desired selection box and press the GOTO

key

 Use the arrow keys to position the cursor to the required setting
 With the OK soft key you confirm the value, and with the CANCEL

soft key you discard the selection

4.3 Working with the File Manager

HEIDENHAIN TNC 620 87

Choosing one of the last 10 files selected

Call the file manager

Display the last 10 files selected: Press the LAST
FILES soft key.

Use the arrow keys to move the highlight to the file you wish to select:

Moves the highlight up and down within a window.

Select a file: Press the OK soft key or ENT

or

4.3 Working with the File Manager

Deleting a file

 Move the highlight to the file you want to delete

 To select the erasing function, press the DELETE soft

key.

 To confirm, press the OK soft key or
 To cancel deletion, press the CANCEL soft key

Deleting a directory

 Delete all files and subdirectories stored in the directory that you

want to delete

 Move the highlight to the directory you want to delete.

 To select the erasing function, press the DELETE ALL

soft key. The TNC asks whether you really want to
erase the subdirectories and files.

 To confirm, press the OK soft key or
 To cancel deletion, press the CANCEL soft key

88

Marking files

Tagging functions Soft key

Tag a single file

Tag all files in the directory

Untag a single file

Untag all files

Some functions, such as copying or erasing files, can not only be used
for individual files, but also for several files at once. To tag several files,
proceed as follows:

Move the highlight to the first file.

To display the tagging functions, press the TAG soft
key.

Tag a file by pressing the TAG FILE soft key.

Move the highlight to the next file you wish to mark:

To tag more files, press the TAG FILE soft key.

To copy the marked files, with the back soft key,
leave the TAG function

To copy the marked files, select the COPY soft key

To delete the marked files, press the back soft key to
exit the marking function and then press the DELETE
soft key

4.3 Working with the File Manager

HEIDENHAIN TNC 620 89

Renaming a file

 Move the highlight to the file you wish to rename.

 Select the renaming function.
 Enter the new file name; the file type cannot be

changed.

 To rename: Press the OK soft key or the ENT key

File sorting

 Select the folder in which you wish to sort the files

 Select the SORT soft key
 Select the soft key with the corresponding display

criterion

Additional functions

Protecting a file / Canceling file protection

 Move the highlight to the file you want to protect.

 To select the additional functions, press the MORE

4.3 Working with the File Manager

FUNCTIONS soft key.

 To enable file protection, press the PROTECT soft

key. The file is distinguished by a symbol.

 To cancel file protection, proceed in the same way

using the UNPROTECT soft key.

Select the editor

 Move the highlight in the right window onto the file you want to

open.

 To select the additional functions, press the MORE

FUNCTIONS soft key.

 To select the editor with which to open the selected

file, press the SELECT EDITOR soft key.

 Mark the desired editor.
 Press the OK soft key to open the file.

Activate or deactivate USB devices.

 To select the additional functions, press the MORE

FUNCTIONS soft key.

 Shift the soft-key row.
 Select the soft key for activating or deactivating.

90

Data transfer to or from an external data medium

You might have to set up the data interface before you
can transfer data to an external data medium (see
“Setting the Data Interfaces” on page 485).

Depending on the data transfer software you use,
problems can occur occasionally when you transmit data
over a serial interface. They can be overcome by repeating
the transmission.

Call the file manager

Select the screen layout for data transfer: press the
WINDOW soft key. Select the desired directory in
both halves of the screen. In the left half of the screen
the TNC shows, for example, all files saved on its hard
disk. In the right half of the screen it shows all files
saved on the external data medium. Use the SHOW
FILES and SHOW TREE soft keys to switch between
the folder view and file view.

4.3 Working with the File Manager

Use the arrow keys to highlight the file(s) that you want to transfer:

Moves the highlight up and down within a window.

Moves the highlight from the left to the right window,
and vice versa.

If you wish to copy from the TNC to the external data medium, move
the highlight in the left window to the file to be transferred.

HEIDENHAIN TNC 620 91

To transfer a single file, position the highlight on the desired file, or

To transfer several files: Press the TAG soft key (in
the second soft-key row, see “Marking files,” page

89) and mark the corresponding files. With the back

soft key, exit the TAG function again.

Press the COPY soft key

Confirm with the OK soft key or with the ENT key. For long programs,
a status window appears on the TNC informing you of the copying
progress.

To end data transfer, move the highlight into the left
window and then press the WINDOW soft key. The
standard file manager window is displayed again.

4.3 Working with the File Manager

To select another directory in the split-screen display,
press the SHOW TREE soft key. If you press the SHOW
FILES soft key, the TNC shows the content of the
selected directory!

92

Copying files into another directory

 Select a screen layout with two equally sized windows.
 To display directories in both windows, press the SHOW TREE soft

key.

In the right window

 Move the highlight to the directory to copy the files to and display

the files in this directory with the SHOW FILES soft key.

In the left window

 Select the directory with the files to copy and press the SHOW

FILES soft key to display them.

 Call the file tagging functions.

 Move the highlight to the files to be copied and mark

them. You can tag several files in this way, if desired.

 Copy the tagged files into the target directory.

Additional marking functions: see “Marking files,” page 89.
If you have tagged files in both the left and right windows, the TNC

copies from the directory in which the highlight is located.

Overwriting files

If you copy files into a directory in which other files are stored under
the same name, the TNC will reply with a “protected file” error
message. Use the TAG function to overwrite the file anyway:

 To overwrite two or more files, mark them in the “existing files”

pop-up window and press the OK soft key

 To leave the files as they are, press the CANCEL soft key

4.3 Working with the File Manager

HEIDENHAIN TNC 620 93

The TNC in a network

To connect the Ethernet card to your network, see
“Ethernet Interface,” page 490.

The TNC logs error messages during network operation
(see “Ethernet Interface” on page 490).

If the TNC is connected to a network, it also displays the connected
network drives in the directory window (left half of the screen). All the
functions described above (selecting a drive, copying files, etc.) also
apply to network drives, provided that you have been granted the
corresponding rights.

Connecting and disconnecting a network drive

 To select the program management: Press the PGM

MGT key. If necessary, press the WINDOW soft key
to set up the screen as it is shown at the upper right.

 To manage the network drives: Press the NETWORK

soft key (second soft-key row). In the right-hand
window the TNC shows the network drives available
for access. With the soft keys described below you
can define the connection for each drive.

4.3 Working with the File Manager

Function Soft key

Establish the network connection. If the
connection is active, the TNC marks the Mnt
column.

Delete network connection.

Automatically establish network connection
whenever the TNC is switched on. The TNC
marks the Auto column if the connection is
established automatically

Use the PING function to test your network
connection

If you press the NETWORK INFO soft key, the
TNC displays the current network settings

94

USB devices on the TNC

Backing up data from or loading onto the TNC is especially easy with
USB devices. The TNC supports the following USB block devices:

 Floppy disk drives with FAT/VFAT file system
 Memory sticks with the FAT/VFAT file system
 Hard disks with the FAT/VFAT file system
 CD-ROM drives with the Joliet (ISO 9660) file system

The TNC automatically detects these types of USB devices when
connected. The TNC does not support USB devices with other file
systems (such as NTFS). After connection, the TNC displays an error
message.

The TNC also displays an error message if you connect a
USB hub. In this case simply acknowledge the message
with the CE key.

In theory, you should be able to connect all USB devices
with the file systems mentioned above to the TNC. If
problems occur nevertheless, please contact
HEIDENHAIN.

The USB devices appear as separate drives in the directory tree, so
you can use the file-management functions described in the earlier
chapters correspondingly.

In order to remove a USB device, you must proceed as follows:

 Press the PGM MGT soft key to call the file manager.

 Select the left window with the arrow key.

 Use the arrow keys to select the USB device to be

removed.

 Scroll through the soft-key row.

 Select additional functions.

 Select the function for removing USB devices. The

TNC removes the USB device from the directory tree.

 Exit the file manager.

In order to re-establish a connection with a USB device that has been
removed, press the following soft key:

 Select the function for reconnection of USB devices.

4.3 Working with the File Manager

HEIDENHAIN TNC 620 95

4.4 Creating and Writing Programs

Organization of an NC program in HEIDENHAIN conversational format

A part program consists of a series of program blocks. The figure at
right illustrates the elements of a block.

The TNC numbers the blocks in ascending sequence.
The first block of a program is identified by BEGIN PGM, the program

name and the active unit of measure.
The subsequent blocks contain information on:

 The workpiece blank
 Tool definitions, tool calls
 Approaching a safe position
 Feed rates and spindle speeds, as well as
 Path contours, cycles and other functions

The last block of a program is identified by END PGM, the program name
and the active unit of measure.

Block

10 L X+10 Y+5 R0 F100 M3

Path function

Block number

Words

4.4 Creating and Writing Programs

After each tool call, HEIDENHAIN recommends always
traversing to a safe position, from which the TNC can
position the tool for machining without causing a collision!

Define the blank: BLK FORM

After initiating a new program, you define a cuboid workpiece blank.
To define the workpiece blank, press the SPEC FCT soft key and then
the BLK FORM soft key. This definition is needed for the TNC’s
graphic simulation feature. The sides of the workpiece blank lie parallel
to the X, Y and Z axes and can be up to 100 000 mm long. The blank
form is defined by two of its corner points:

 MIN point: the smallest X, Y and Z coordinates of the blank form,

entered as absolute values.

 MAX point: the largest X, Y and Z coordinates of the blank form,

entered as absolute or incremental values.

You only need to define the blank form if you wish to run
a graphic test for the program!

96

Creating a new part program

0

0

0

You always enter a part program in the Programming and Editing
mode of operation. An example of program initiation:

Select the Programming and Editing mode of
operation.

Press the PGM MGT key to call the file manager.

Select the directory in which you wish to store the new program:

FILE NAME = 123.H

Enter the new program name and confirm your entry
with the ENT key.

To select the unit of measure, press the MM or INCH
soft key. The TNC switches the screen layout and
initiates the dialog for defining the BLK FORM.

WORKING SPINDLE AXIS X/Y/Z?

Enter the spindle axis.

DEF BLK FORM: MIN CORNER?

Enter in sequence the X, Y and Z coordinates of the
MIN point.

-40

DEF BLK FORM: MAX CORNER?

100

100

Enter in sequence the X, Y and Z coordinates of the
MAX point.

4.4 Creating and Writing Programs

HEIDENHAIN TNC 620 97

Example: Display the BLK form in the NC program

0 BEGIN PGM NEW MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 END PGM NEW MM

The TNC automatically generates the block numbers as well as the
BEGIN and END blocks.

If you do not wish to define a blank form, cancel the dialog
at Working spindle axis X/Y/Z by pressing the DEL key!

The TNC can display the graphics only if the shortest side
is at least 50 µm long and the longest side is no longer
than 99 999.999 mm.

4.4 Creating and Writing Programs

Program begin, name, unit of measure
Spindle axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure

98

Programming tool movements in conversational format

To program a block, initiate the dialog by pressing a function key. In the
screen headline, the TNC then asks you for all the information
necessary to program the desired function.

Example of a dialog

Dialog initiation

COORDINATES?

10

5

RADIUS COMP. RL/RR/NO COMP. ?

FEED RATE F=? / F MAX = ENT

00

MISCELLANEOUS FUNCTION M?

The program-block window displays the following line:

3 L X+10 Y+5 R0 F100 M3

Enter the target coordinate for the X axis.

Enter the target coordinate for the Y axis, and go to
the next question with ENT

Enter “No radius compensation” and go to the next
question with ENT.

Enter a feed rate of 100 mm/min for this path contour;
go to the next question with ENT.

Enter the miscellaneous function M3 “spindle ON.”
Pressing the ENT key terminates this dialog.

4.4 Creating and Writing Programs

HEIDENHAIN TNC 620 99

Possible feed rate input

Functions for setting the feed rate Soft key

Rapid traverse

Traverse feed rate automatically calculated in

TOOL CALL

Move at the programmed feed rate (unit of
measure is mm/min)

Functions for conversational guidance Key

Ignore the dialog question

End the dialog immediately

Abort the dialog and erase the block

Actual position capture

4.4 Creating and Writing Programs

The TNC enables you to transfer the current tool position into the
program, for example during

 Positioning-block programming and
 Cycle programming

To transfer the correct position values, proceed as follows:

 Place the input box at the position in the block where you want to

insert a position value.

 Select the actual-position-capture function. In the soft-

key row the TNC displays the axes whose positions
can be transferred.

 Select the axis. The TNC writes the current position of

the selected axis into the active input box.

In the working plane the TNC always captures the
coordinates of the tool center, even though tool radius
compensation is active.

In the tool axis the TNC always captures the coordinates
of the tool tip and thus always takes the active tool length
compensation into account.

The actual-position-capture function is not allowed if the
tilted working plane function is active.

100