HEIDENHAIN TNC 620 User Manual

TNC 620

User's Manual
HEIDENHAIN
Conversational Programming

NC Software
817600-01
817601-01
817605-01

English (en)
3/2014

Controls of the TNC

Controls of the TNC

Keys on visual display unit

Key Function

Select split screen layout

Toggle the display between
machining and programming
modes

Soft keys for selecting functions on
screen

Shifting between soft-key rows

Machine operating modes

Key Function

Manual operation

Electronic handwheel

Program/file management, TNC functions

Key Function

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, call TNCguide

Display all current error messages

Show calculator

Navigation keys

Key Function

Move highlight

Positioning with manual data input

Program run, single block

Program run, full sequence

Programming modes

Key Function

Programming

Test run

Go directly to blocks, cycles and
parameter functions

Potentiometer for feed rate and spindle speed

Feed rate Spindle speed

2

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

NO

ENT

Cycles, subprograms and program section repeats

Key Function

Define touch probe cycles

Define and call cycles

Enter and call labels for
subprogramming and program
section repeats

Enter program stop in a program

Tool functions

Key Function

Define tool data in the program

Call tool data

Special functions

Key Function

Show special functions

Select the next tab in forms

Up/down one dialog box or button

Entering and editing coordinate axes and numbers

Key Function

Select coordinate axes or enter

. . .

. . .

them in a program

Numbers

Decimal point / Reverse algebraic
sign

Programming path movements

Key Function

Approach/depart contour

FK free contour programming

Straight line

Circle center/pole for polar
coordinates

Circular arc with center

Circle with radius

Circular arc with tangential
connection

Chamfer/Corner rounding

Polar coordinate input /
Incremental values

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

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

3

Controls of the TNC

4

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Fundamentals

Fundamentals

About this manual

About this manual

The symbols used in this manual are described below.

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

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

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

This symbol indicates a possibly dangerous situation
that may cause light injuries if not avoided.

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

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

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

We are continuously striving to improve our documentation for you.
Please help us by sending your requests to the following e-mail
address: [e-mail].

6

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

TNC model, software and features

TNC model, software and features

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

TNC model NC software number

TNC 620 817600-01

TNC 620 E 817601-01

TNC 620 Programming Station 817605-01

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:

Tool measurement with the TT

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

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

User's Manual for Cycle Programming:

All of the cycle functions (touch probe cycles and
fixed cycles) are described in the Cycle Programming
User’s Manual. Please contact HEIDENHAIN if you
require a copy of this User's Manual. ID: 1096886-xx

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

7

Fundamentals

TNC model, software and features

Software options

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

Software option 1 (option number 08)

Rotary table machining

Coordinate transformation

Interpolation

Software option 2 (option number 09)

3-D machining

Interpolation

Touch probe function software option, (option number 17)

Touch probe cycles

■

Programming of cylindrical contours as if in two axes

■

Feed rate in distance per minute

■

Working plane, tilting the ...

■

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

Motion control with minimum jerk

■

3-D tool compensation through surface normal vectors

■

Using the electronic handwheel to change the angle of the swivel head

■

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

Keeping the tool normal to the contour

■

Tool radius compensation perpendicular to traversing and tool direction

■

Linear in 5 axes (subject to export permit)

■

Compensation of tool misalignment in automatic mode

■

Datum setting in manual mode

■

■

■

■

HEIDENHAIN DNC (option number 18)

■

Datum setting in automatic mode

Automatic workpiece measurement

Automatic tool measurement

Communication with external PC applications over COM component

8

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

TNC model, software and features

Advanced programming features software option (option number 19)

FK free contour
programming

Fixed cycles

Advanced graphic features software option (option number 20)

Program verification
graphics, program-run
graphics

Programming in HEIDENHAIN conversational format with graphic

■

support for workpiece drawings not dimensioned for NC

Peck drilling, reaming, boring, counterboring, centering (Cycles 201 to

■

205, 208, 240, 241)

Milling of internal and external threads (Cycles 262 to 265, 267)

■

Finishing of rectangular and circular pockets and studs (Cycles 212 to

■

215, 251 to 257)

Clearing level and oblique surfaces (Cycles 230 to 233)

■

Straight slots and circular slots (Cycles 210, 211, 253, 254)

■

Linear and circular point patterns (Cycles 220, 221)

■

Contour train, contour pocket—also with contour-parallel machining

■

(Cycles 20 to 25)

OEM cycles (special cycles developed by the machine tool builder) can

■

be integrated

Plan view

■

Projection in three planes

■

3-D view

■

Software option 3 (option number 21)

Tool compensation

3-D machining

Pallet management software option (option number 22)

Display step (Option number 23)

step

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

■

M118: Superimpose handwheel positioning during program run

■

Pallet management

■

Linear axes down to 0.01 µmInput resolution and display

■

Rotary axes to 0.00001°

■

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

9

Fundamentals

DXF Converter software option (option number 42)

TNC model, software and features

Extracting contour
programs and machining
positions from DXF data.
Extracting contour sections
from plain-language
programs.

KinematicsOpt software option (option number 48)

Touch-probe cycles for
automatic testing and
optimization of the machine
kinematics

Cross Talk Compensation (CTC) software option (option number 141)

Compensation of axis
couplings

Position Adaptive Control (PAC) software option (option number 142)

Changing control
parameters

Supported DXF format: AC1009 (AutoCAD R12)

■

For contours and point patterns

■

Simple and convenient specification of reference points

■

Select graphical features of contour sections from conversational

■

programs

Backup/restore active kinematics

■

Test active kinematics

■

Optimize active kinematics

■

Determination of dynamically caused position deviation through axis

■

acceleration

Compensation of the TCP

■

Changing of the control parameters depending on the position of the

■

axes in the working space

Changing of the control parameters depending on the speed or

■

acceleration of an axis

Load Adaptive Control (LAC) software option (option number 143)

Automatic determination of workpiece weight and frictional forcesDynamic changing of control

■

parameters

Active Chatter Control (ACC) software option (option number 145)

Fully automatic function for chatter control during machining

Continuous adaptation of the parameters of the adaptive precontrolling

■

to the actual weight of the workpiece during machining

10

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

TNC model, software and features

Feature Content Level (upgrade functions)

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

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

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

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

Intended place of operation

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

Legal information

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

Programming and Editing operating mode
MOD function
License Info soft key

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

11

Fundamentals

TNC model, software and features

New functions

New Functions 73498x-02

DXF files can be opened directly on the TNC in order to extract
contours and point patterns ("Programming: Data transfer from DXF
files or plain-language contours", page 237).

The active tool-axis direction can now be activated in manual
mode and during handwheel superimposition as a virtual tool axis
("Superimposing handwheel positioning during program run: M118
(Miscellaneous Functions software option)", page 354).

Writing and reading data in freely definable tables ("Freely definable
tables", page 379).

New touch probe cycle 484 for calibrating the wireless TT 449 tool
touch probe (see User's Manual for Cycles).

The new HR 520 and HR 550 FS handwheels are supported
("Traverse with electronic handwheels", page 440).

New machining cycle 225 ENGRAVING (see User’s Manual for
Cycle Programming)

New Active Chatter Control (ACC) software option ("Active Chatter
Control (ACC; software option)", page 365).

New manual probing cycle "Center line as datum" ("Setting a center
line as datum ", page 484).

New function for rounding corners ("Rounding corners: M197",
page 360).

External access to the TNC can now be blocked with a MOD
function ("External access", page 533).

12

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

TNC model, software and features

New Functions 73498x-02

The maximum number of characters for the NAME and DOC fields
in the tool table has been increased from 16 to 32 ("Enter tool data
into the table", page 162).

The columns ACC were added to the tool table ("Enter tool data
into the table", page 162).

Operation and position behavior of the manual probing cycles has
been improved ("Using 3-D touch probes (Touch Probe Function
software option)", page 464).

Predefined values can now be entered into a cycle parameter
with the PREDEF function in cycles (see User’s Manual for Cycle
Programming).

A new optimization algorithm is now used with the KinematicsOpt
cycles (see User’s Manual for Cycle Programming).

With Cycle 257, circular stud milling, a parameter is now available
with which you can determine the approach position on the stud
(see User's Manual for Cycle Programming)

With Cycle 256, rectangular stud, a parameter is now available with
which you can determine the approach position on the stud (see
User's Manual for Cycle Programming).

With the "Basic Rotation" probing cycle, workpiece misalignment
can now be compensated for via a table rotation ("Compensation of
workpiece misalignment by rotating the table", page 477)

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

13

Fundamentals

TNC model, software and features

New functions 81760x-01

New special operating mode Retraction ("Retraction after a power
interruption", page 520).

New graphic simulation ("Graphics (Advanced Graphic Features
software option)", page 502).

New MOD function "tool usage file" within the machine settings
group ("Tool usage file", page 533).

New MOD function "set system time" within the systems settings
group ("Set the system time", page 535).

New MOD group "graphic settings" ("Graphic settings",
page 532).

With the new cutting data calculator you can calculate the spindle
speed and the feed rate ("Cutting data calculator", page 138).

Now you can activate and deactivate the active chatter
compensation (ACC) by soft key ("Activating/deactivating ACC",
page 366).

New if/then decisions were introduced in the jump commands
("Programming if-then decisions", page 280).

The character set of the fixed cycle 225 Engraving was expanded
by more characters and the diameter sign (see User's Manual for
Cycle Programming).

New fixed cycle 275 trochoidal milling (see User’s Manual for Cycle
Programming)

New fixed cycle 233 ENGRAVING (see User’s Manual for Cycle
Programming)

In the drilling cycles 200, 203 and 205 the parameter Q395 BEZUG
DEPTH REFERENCE was introduced in order to evaluate the T
ANGLE (see User's Manual for Cycle Programming).

The probing cycle 4 MEASURING IN 3-D was introduced (see
User's Manual for Cycle Programming).

14

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

TNC model, software and features

Changed functions 81760x-01

Now up to 4 functions are allowed in an NC block ("Fundamentals",
page 342).

New soft keys for value transfer have been introduced in the pocket
calculator ("Operation", page 135).

The distance-to-go display can now also be displayed in the input
system ("Position Display Types", page 536).

Cycle 241 SINGLE-LIP DEEP HOLE DRILLING was expanded
by several input parameters (see User's Manual for Cycle
Programming).

Cycle 404 was expanded by the parameter Q305 NUMBER IN
TABLE (see User's Manual for Cycle Programming).

In the thread milling cycles 26x an approaching feed rate was
introduced (see User's Manual for Cycle Programming).

In Cycle 205 Universal Pecking you can now use parameter Q208
to define a feed rate for retraction (see User's Manual for Cycle
Programming).

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

15

Fundamentals

TNC model, software and features

16

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Contents

1 First Steps with the TNC 620....................................................................................................... 47

2 Introduction.....................................................................................................................................67

3 Programming: Fundamentals, file management.........................................................................85

4 Programming: Programming aids.............................................................................................. 129

5 Programming: Tools..................................................................................................................... 157

6 Programming: Programming contours...................................................................................... 185

7 Programming: Data transfer from DXF files or plain-language contours............................... 237

8 Programming: Subprograms and program section repeats.................................................... 255

9 Programming: Q Parameters.......................................................................................................271

10 Programming: Miscellaneous functions.....................................................................................341

11 Programming: Special functions.................................................................................................361

12 Programming: Multiple Axis Machining.................................................................................... 385

13 Programming: Pallet editor......................................................................................................... 429

14 Manual operation and setup.......................................................................................................435

15 Positioning with Manual Data Input.......................................................................................... 495

16 Test run and program run........................................................................................................... 501

17 MOD functions..............................................................................................................................529

18 Tables and overviews...................................................................................................................557

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

17

Contents

18

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

1 First Steps with the TNC 620....................................................................................................... 47

1.1 Overview................................................................................................................................................ 48

1.2 Machine switch-on................................................................................................................................48

Acknowledging the power interruption and moving to the reference points..........................................48

1.3 Programming the first part..................................................................................................................49

Selecting the correct operating mode.................................................................................................... 49

The most important TNC keys................................................................................................................49

Creating a new program/file management............................................................................................. 50

Defining a workpiece blank.................................................................................................................... 51

Program layout........................................................................................................................................ 52

Programming a simple contour...............................................................................................................53

Creating a cycle program........................................................................................................................ 56

1.4 Graphically testing the first part (Advanced Graphic Features software option)........................... 58

Selecting the correct operating mode.................................................................................................... 58

Selecting the tool table for the test run.................................................................................................58

Choosing the program you want to test................................................................................................ 59

Selecting the screen layout and the view.............................................................................................. 59

Starting the test run................................................................................................................................60

1.5 Setting up tools.................................................................................................................................... 61

Selecting the correct operating mode.................................................................................................... 61

Preparing and measuring tools............................................................................................................... 61

The tool table TOOL.T............................................................................................................................ 62

The pocket table TOOL_P.TCH................................................................................................................63

1.6 Workpiece setup....................................................................................................................................64

Selecting the correct operating mode.................................................................................................... 64

Clamping the workpiece......................................................................................................................... 64

Datum setting with 3-D touch probe (software option: Touch probe function)....................................... 65

1.7 Running the first program................................................................................................................... 66

Selecting the correct operating mode.................................................................................................... 66

Choosing the program you want to run................................................................................................. 66

Start the program....................................................................................................................................66

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

19

Contents

2 Introduction.....................................................................................................................................67

2.1 The TNC 620.......................................................................................................................................... 68

Programming: HEIDENHAIN conversational and ISO formats............................................................... 68

Compatibility............................................................................................................................................68

2.2 Visual display unit and operating panel............................................................................................ 69

Display screen......................................................................................................................................... 69

Setting the screen layout........................................................................................................................70

Control Panel...........................................................................................................................................70

2.3 Modes of Operation..............................................................................................................................71

Manual Operation and El. Handwheel....................................................................................................71

Positioning with Manual Data Input........................................................................................................71

Programming........................................................................................................................................... 71

Test Run.................................................................................................................................................. 72

Program Run, Full Sequence and Program Run, Single Block................................................................72

2.4 Status displays...................................................................................................................................... 73

"General" status display...........................................................................................................................73

Additional status displays........................................................................................................................74

2.5 Window Manager..................................................................................................................................80

Task bar................................................................................................................................................... 81

2.6 SELinux security software....................................................................................................................82

2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels......................................83

3-D touch probes (Touch Probe Function software option).....................................................................83

HR electronic handwheels...................................................................................................................... 84

20

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

3 Programming: Fundamentals, file management.........................................................................85

3.1 Fundamentals........................................................................................................................................ 86

Position encoders and reference marks................................................................................................. 86

Reference system................................................................................................................................... 86

Reference system on milling machines..................................................................................................87

Designation of the axes on milling machines.........................................................................................87

Polar coordinates..................................................................................................................................... 88

Absolute and incremental workpiece positions...................................................................................... 89

Selecting the datum................................................................................................................................90

3.2 Opening programs and entering......................................................................................................... 91

Organization of an NC program in HEIDENHAIN Conversational format................................................91

Define the blank: BLK FORM................................................................................................................. 92

Opening a new part program................................................................................................................. 94

Programming tool movements in conversational................................................................................... 95

Actual position capture............................................................................................................................97

Editing a program....................................................................................................................................98

The TNC search function...................................................................................................................... 101

3.3 File manager: Fundamentals..............................................................................................................103

Files....................................................................................................................................................... 103

Displaying externally generated files on the TNC.................................................................................105

Data Backup.......................................................................................................................................... 105

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

21

Contents

3.4 Working with the file manager......................................................................................................... 106

Directories............................................................................................................................................. 106

Paths......................................................................................................................................................106

Overview: Functions of the file manager............................................................................................. 107

Calling the file manager........................................................................................................................ 108

Selecting drives, directories and files...................................................................................................109

Creating a new directory...................................................................................................................... 110

Creating a new file................................................................................................................................110

Copying a single file..............................................................................................................................110

Copying files into another directory......................................................................................................111

Copying a table..................................................................................................................................... 112

Copying a directory............................................................................................................................... 112

Choosing one of the last files selected................................................................................................113

Deleting a file........................................................................................................................................114

Deleting a directory...............................................................................................................................114

Tagging files.......................................................................................................................................... 115

Renaming a file..................................................................................................................................... 116

Sorting files........................................................................................................................................... 116

Additional functions...............................................................................................................................117

Additional tools for management of external file types........................................................................118

Data transfer to/from an external data medium................................................................................... 123

The TNC in a network.......................................................................................................................... 125

USB devices on the TNC......................................................................................................................126

22

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

4 Programming: Programming aids.............................................................................................. 129

4.1 Screen keyboard..................................................................................................................................130

Enter the text with the screen keyboard..............................................................................................130

4.2 Adding comments...............................................................................................................................131

Application............................................................................................................................................. 131

Entering comments during programming.............................................................................................131

Inserting comments after program entry............................................................................................. 131

Entering a comment in a separate block..............................................................................................131

Functions for editing of the comment..................................................................................................132

4.3 Display of NC Programs..................................................................................................................... 133

Syntax highlighting................................................................................................................................ 133

Scrollbar.................................................................................................................................................133

4.4 Structuring programs..........................................................................................................................134

Definition and applications.................................................................................................................... 134

Displaying the program structure window / Changing the active window............................................134

Inserting a structuring block in the (left) program window................................................................... 134

Selecting blocks in the program structure window.............................................................................. 134

4.5 Calculator............................................................................................................................................. 135

Operation...............................................................................................................................................135

4.6 Cutting data calculator.......................................................................................................................138

Application............................................................................................................................................. 138

4.7 Programming graphics....................................................................................................................... 141

Generate/do not generate graphics during programming.....................................................................141

Generating a graphic for an existing program...................................................................................... 141

Block number display ON/OFF..............................................................................................................142

Erasing the graphic............................................................................................................................... 142

Showing grid lines.................................................................................................................................142

Magnification or reduction of details.................................................................................................... 143

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

23

Contents

4.8 Error messages.................................................................................................................................... 144

Display of errors....................................................................................................................................144

Open the error window........................................................................................................................ 144

Closing the error window..................................................................................................................... 144

Detailed error messages.......................................................................................................................145

INTERNAL INFO soft key......................................................................................................................145

Clearing errors.......................................................................................................................................146

Error log.................................................................................................................................................146

Keystroke log.........................................................................................................................................147

Informational texts................................................................................................................................ 148

Saving service files............................................................................................................................... 148

Calling the TNCguide help system....................................................................................................... 149

4.9 TNCguide context-sensitive help system.........................................................................................150

Application............................................................................................................................................. 150

Working with the TNCguide................................................................................................................. 151

Downloading current help files............................................................................................................. 155

24

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

5 Programming: Tools..................................................................................................................... 157

5.1 Entering tool-related data.................................................................................................................. 158

Feed rate F............................................................................................................................................158

Spindle speed S.................................................................................................................................... 159

5.2 Tool data...............................................................................................................................................160

Requirements for tool compensation................................................................................................... 160

Tool number, tool name........................................................................................................................ 160

Tool length L......................................................................................................................................... 160

Tool radius R......................................................................................................................................... 160

Delta values for lengths and radii......................................................................................................... 161

Entering tool data into the program..................................................................................................... 161

Enter tool data into the table............................................................................................................... 162

Importing tool tables.............................................................................................................................170

Pocket table for tool changer................................................................................................................171

Call tool data......................................................................................................................................... 174

Tool change........................................................................................................................................... 176

Tool usage test......................................................................................................................................179

5.3 Tool compensation.............................................................................................................................. 181

Introduction........................................................................................................................................... 181

Tool length compensation..................................................................................................................... 181

Tool radius compensation..................................................................................................................... 182

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

25

Contents

6 Programming: Programming contours...................................................................................... 185

6.1 Tool movements.................................................................................................................................. 186

Path functions....................................................................................................................................... 186

FK free contour programming (Advanced programming features software option)..............................186

Miscellaneous functions M...................................................................................................................186

Subprograms and program section repeats......................................................................................... 187

Programming with Q parameters......................................................................................................... 187

6.2 Fundamentals of Path Functions.......................................................................................................188

Programming tool movements for workpiece machining.....................................................................188

6.3 Approaching and departing a contour............................................................................................. 192

Overview: Types of paths for contour approach and departure............................................................192

Important positions for approach and departure...................................................................................193

Approaching on a straight line with tangential connection: APPR LT................................................... 195

Approaching on a straight line perpendicular to the first contour point: APPR LN............................... 195

Approaching on a circular path with tangential connection: APPR CT..................................................196

Approaching on a circular path with tangential connection from a straight line to the contour:

APPR LCT.............................................................................................................................................. 197

Departing in a straight line with tangential connection: DEP LT.......................................................... 197

Departing in a straight line perpendicular to the last contour point: DEP LN....................................... 198

Departing on a circular path with tangential connection: DEP CT........................................................199

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT.............. 199

6.4 Path contours - Cartesian coordinates............................................................................................. 200

Overview of path functions.................................................................................................................. 200

Straight line L........................................................................................................................................201

Inserting a chamfer between two straight lines...................................................................................202

Corner rounding RND........................................................................................................................... 203

26

Circle center CC.................................................................................................................................... 204

Circular path C around circle center CC............................................................................................... 205

CircleCR with defined radius................................................................................................................ 206

Circle CT with tangential connection....................................................................................................208

Example: Linear movements and chamfers with Cartesian coordinates.............................................. 209

Example: Circular movements with Cartesian coordinates.................................................................. 210

Example: Full circle with Cartesian coordinates................................................................................... 211

TNC 620 | User's Manual

HEIDENHAIN Conversational Programming | 3/2014

6.5 Path contours – Polar coordinates.................................................................................................... 212

Overview............................................................................................................................................... 212

Zero point for polar coordinates: pole CC............................................................................................ 213

Straight line LP......................................................................................................................................213

Circular path CP around pole CC.......................................................................................................... 214

Circle CTP with tangential connection..................................................................................................214

Helix.......................................................................................................................................................215

Example: Linear movement with polar coordinates............................................................................. 217

Example: Helix...................................................................................................................................... 218

6.6 Path contours – FK free contour programming (Advanced Programming Features software

option).................................................................................................................................................. 219

Fundamentals........................................................................................................................................ 219

FK programming graphics..................................................................................................................... 221

Initiating the FK dialog.......................................................................................................................... 223

Pole for FK programming...................................................................................................................... 223

Free straight line programming.............................................................................................................224

Free circular path programming............................................................................................................ 225

Input options......................................................................................................................................... 226

Auxiliary points...................................................................................................................................... 229

Relative data..........................................................................................................................................230

Example: FK programming 1................................................................................................................ 232

Example: FK programming 2................................................................................................................ 233

Example: FK programming 3................................................................................................................ 234

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

27

Contents

7 Programming: Data transfer from DXF files or plain-language contours............................... 237

7.1 Processing DXF Files (Software Option).......................................................................................... 238

Application............................................................................................................................................. 238

Opening a DXF file............................................................................................................................... 239

Working with the DXF converter..........................................................................................................239

Basic settings........................................................................................................................................240

Setting layers.........................................................................................................................................242

Defining the datum............................................................................................................................... 243

Selecting and saving a contour.............................................................................................................245

Selecting and saving machining positions............................................................................................ 249

28

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

8 Programming: Subprograms and program section repeats.................................................... 255

8.1 Labeling Subprograms and Program Section Repeats................................................................... 256

Label...................................................................................................................................................... 256

8.2 Subprograms....................................................................................................................................... 257

Operating sequence..............................................................................................................................257

Programming notes...............................................................................................................................257

Programming a subprogram................................................................................................................. 257

Calling a subprogram............................................................................................................................ 258

8.3 Program-section repeats.................................................................................................................... 259

Label LBL.............................................................................................................................................. 259

Operating sequence..............................................................................................................................259

Programming notes...............................................................................................................................259

Programming a program section repeat............................................................................................... 259

Calling a program section repeat..........................................................................................................260

8.4 Any desired program as subprogram............................................................................................... 261

Operating sequence..............................................................................................................................261

Programming notes...............................................................................................................................261

Calling any program as a subprogram.................................................................................................. 262

8.5 Nesting................................................................................................................................................. 263

Types of nesting....................................................................................................................................263

Nesting depth........................................................................................................................................263

Subprogram within a subprogram........................................................................................................ 264

Repeating program section repeats......................................................................................................265

Repeating a subprogram.......................................................................................................................266

8.6 Programming examples..................................................................................................................... 267

Example: Milling a contour in several infeeds...................................................................................... 267

Example: Groups of holes.................................................................................................................... 268

Example: Group of holes with several tools.........................................................................................269

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

29

Contents

9 Programming: Q Parameters.......................................................................................................271

9.1 Principle and overview of functions................................................................................................. 272

Programming notes...............................................................................................................................273

Calling Q parameter functions.............................................................................................................. 274

9.2 Part families—Q parameters in place of numerical values............................................................. 275

Application............................................................................................................................................. 275

9.3 Describing contours with mathematical functions......................................................................... 276

Application............................................................................................................................................. 276

Overview............................................................................................................................................... 276

Programming fundamental operations..................................................................................................277

9.4 Angle functions (trigonometry).........................................................................................................278

Definitions............................................................................................................................................. 278

Programming trigonometric functions.................................................................................................. 278

9.5 Calculation of circles...........................................................................................................................279

Application............................................................................................................................................. 279

9.6 If-then decisions with Q parameters................................................................................................ 280

Application............................................................................................................................................. 280

Unconditional jumps..............................................................................................................................280

Programming if-then decisions............................................................................................................. 280

Abbreviations used:...............................................................................................................................281

9.7 Checking and changing Q parameters............................................................................................. 282

Procedure.............................................................................................................................................. 282

9.8 Additional functions............................................................................................................................284

Overview............................................................................................................................................... 284

FN 14: ERROR: Displaying error messages......................................................................................... 285

FN 16: F-PRINT: Output of formatted texts and Q parameter values....................................................289

FN 18: SYS-DATUM READ: Reading system data................................................................................ 293

FN 19: PLC: Transfer values to PLC..................................................................................................... 302

FN 20: WAIT FOR: NC and PLC synchronization................................................................................. 302

FN 29: PLC: Transfer values to the PLC...............................................................................................304

FN 37: EXPORT.....................................................................................................................................304

30

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

9.9 Accessing tables with SQL commands............................................................................................ 305

Introduction........................................................................................................................................... 305

A transaction......................................................................................................................................... 306

Programming SQL commands..............................................................................................................308

Overview of the soft keys.................................................................................................................... 308

SQL BIND..............................................................................................................................................309

SQL SELECT......................................................................................................................................... 310

SQL FETCH........................................................................................................................................... 312

SQL UPDATE.........................................................................................................................................313

SQL INSERT..........................................................................................................................................313

SQL COMMIT....................................................................................................................................... 314

SQL ROLLBACK.................................................................................................................................... 314

9.10 Entering formulas directly..................................................................................................................315

Entering formulas.................................................................................................................................. 315

Rules for formulas.................................................................................................................................317

Programming example.......................................................................................................................... 318

9.11 String parameters............................................................................................................................... 319

String processing functions.................................................................................................................. 319

Assigning string parameters................................................................................................................. 320

Chain-linking string parameters.............................................................................................................320

Converting a numerical value to a string parameter.............................................................................321

Copying a substring from a string parameter.......................................................................................322

Converting a string parameter to a numerical value.............................................................................323

Checking a string parameter.................................................................................................................324

Finding the length of a string parameter..............................................................................................325

Comparing alphabetic sequence...........................................................................................................326

Reading machine parameters............................................................................................................... 327

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

31

Contents

9.12 Preassigned Q parameters.................................................................................................................330

Values from the PLC: Q100 to Q107....................................................................................................330

Active tool radius: Q108........................................................................................................................330

Tool axis: Q109......................................................................................................................................330

Spindle status: Q110............................................................................................................................. 331

Coolant on/off: Q111............................................................................................................................. 331

Overlap factor: Q112............................................................................................................................. 331

Unit of measurement for dimensions in the program: Q113................................................................331

Tool length: Q114.................................................................................................................................. 331

Coordinates after probing during program run..................................................................................... 332

Deviation between actual value and nominal value during automatic tool measurement with the

TT 130....................................................................................................................................................332

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

TNC........................................................................................................................................................332

Measurement results from touch probe cycles (see also User’s Manual for Cycle Programming).......333

9.13 Programming examples..................................................................................................................... 335

Example: Ellipse.................................................................................................................................... 335

Example: Concave cylinder machined with spherical cutter.................................................................337

Example: Convex sphere machined with end mill................................................................................339

32

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

10 Programming: Miscellaneous functions.....................................................................................341

10.1 Entering miscellaneous functions M and STOP...............................................................................342

Fundamentals........................................................................................................................................ 342

10.2 M functions for program run inspection, spindle and coolant.......................................................343

Overview............................................................................................................................................... 343

10.3 Miscellaneous functions for coordinate data...................................................................................344

Programming machine-referenced coordinates: M91/M92.................................................................. 344

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130................... 346

10.4 Miscellaneous functions for path behavior......................................................................................347

Machining small contour steps: M97................................................................................................... 347

Machining open contour corners: M98................................................................................................ 348

Feed rate factor for plunging movements: M103.................................................................................349

Feed rate in millimeters per spindle revolution: M136.........................................................................350

Feed rate for circular arcs: M109/M110/M111.......................................................................................351

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 (Miscellaneous Functions

software option).................................................................................................................................... 352

Superimposing handwheel positioning during program run: M118 (Miscellaneous Functions software

option)....................................................................................................................................................354

Retraction from the contour in the tool-axis direction: M140...............................................................356

Suppressing touch probe monitoring: M141........................................................................................ 357

Deleting basic rotation: M143...............................................................................................................358

Automatically retract tool from the contour at an NC stop: M148....................................................... 359

Rounding corners: M197.......................................................................................................................360

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

33

Contents

11 Programming: Special functions.................................................................................................361

11.1 Overview of special functions........................................................................................................... 362

Main menu for SPEC FCT special functions........................................................................................ 362

Program defaults menu........................................................................................................................ 363

Functions for contour and point machining menu................................................................................ 363

Menu of various conversational functions............................................................................................ 364

11.2 Active Chatter Control (ACC; software option)................................................................................365

Application............................................................................................................................................. 365

Activating/deactivating ACC...................................................................................................................366

11.3 Working with the Parallel Axes U, V and W.................................................................................... 367

Overview............................................................................................................................................... 367

FUNCTION PARAXCOMP DISPLAY......................................................................................................368

FUNCTION PARAXCOMP MOVE..........................................................................................................368

FUNCTION PARAXCOMP OFF............................................................................................................. 369

FUNCTION PARAXMODE.....................................................................................................................369

FUNCTION PARAXMODE OFF............................................................................................................. 370

11.4 File functions....................................................................................................................................... 371

Application............................................................................................................................................. 371

Defining file functions........................................................................................................................... 371

11.5 Definition of a datum shift................................................................................................................ 372

Overview............................................................................................................................................... 372

TRANS DATUM AXIS............................................................................................................................ 372

TRANS DATUM TABLE......................................................................................................................... 373

TRANS DATUM RESET.........................................................................................................................374

11.6 Creating Text Files...............................................................................................................................375

34

Application............................................................................................................................................. 375

Opening and exiting text files...............................................................................................................375

Editing texts.......................................................................................................................................... 376

Deleting and re-inserting characters, words and lines..........................................................................376

Editing text blocks.................................................................................................................................377

Finding text sections.............................................................................................................................378

TNC 620 | User's Manual

HEIDENHAIN Conversational Programming | 3/2014

11.7 Freely definable tables....................................................................................................................... 379

Fundamentals........................................................................................................................................ 379

Creating a freely definable table...........................................................................................................379

Editing the table format........................................................................................................................380

Switching between table and form view..............................................................................................381

FN 26: TAPOPEN: Open a freely definable table................................................................................. 382

FN 27: TAPWRITE: Write to a freely definable table............................................................................383

FN 28: TAPREAD: Read from a freely definable table......................................................................... 384

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

35

Contents

12 Programming: Multiple Axis Machining.................................................................................... 385

12.1 Functions for multiple axis machining............................................................................................. 386

12.2 The PLANE Function: Tilting the Working Plane (Software Option 1)...........................................387

Introduction........................................................................................................................................... 387

Defining the PLANE function................................................................................................................389

Position display......................................................................................................................................389

Resetting the PLANE function.............................................................................................................. 390

Defining the working plane with the spatial angle: PLANE SPATIAL....................................................391

Defining the working plane with the projection angle: PLANE PROJECTED....................................... 393

Defining the working plane with the Euler angle: PLANE EULER........................................................394

Defining the working plane with two vectors: PLANE VECTOR.......................................................... 396

Defining the working plane via three points: PLANE POINTS..............................................................398

Defining the working plane via a single incremental spatial angle: PLANE SPATIAL............................400

Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)......................................401

Specifying the positioning behavior of the PLANE function.................................................................403

12.3 Inclined-tool machining in a tilted machining plane (software option 2)......................................408

Function.................................................................................................................................................408

Inclined-tool machining via incremental traverse of a rotary axis......................................................... 408

Inclined-tool machining via normal vectors...........................................................................................409

12.4 Miscellaneous functions for rotary axes.......................................................................................... 410

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1).............................................. 410

Shortest-path traverse of rotary axes: M126........................................................................................411

Reducing display of a rotary axis to a value less than 360°: M94........................................................412

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

option 2)................................................................................................................................................ 413

Selecting tilting axes: M138................................................................................................................. 416

Compensating the machine’s kinematics configuration for ACTUAL/NOMINAL positions at end of block:

M144 (software option 2)...................................................................................................................... 417

12.5 FUNCTION TCPM (software option 2).............................................................................................. 418

Function.................................................................................................................................................418

Defining the TCPM FUNCTION............................................................................................................ 418

Mode of action of the programmed feed rate..................................................................................... 419

Interpretation of the programmed rotary axis coordinates...................................................................419

Type of interpolation between the starting and end position............................................................... 421

Resetting the TCPM FUNCTION.......................................................................................................... 422

36

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

12.6 Three-dimensional tool compensation (software option 2)........................................................... 423

Introduction........................................................................................................................................... 423

Definition of a normalized vector..........................................................................................................424

Permitted tool shapes........................................................................................................................... 425

Using other tools: Delta values............................................................................................................ 425

3-D compensation without TCPM........................................................................................................ 425

Face Milling: 3D compensation with TCPM......................................................................................... 426

Peripheral Milling: 3-D radius compensation with TCPM and radius compensation (RL/RR)................ 427

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

37

Contents

13 Programming: Pallet editor......................................................................................................... 429

13.1 Pallet Management (software option).............................................................................................. 430

Application............................................................................................................................................. 430

Select pallet table................................................................................................................................. 432

Exiting the pallet file............................................................................................................................. 432

Run pallet file........................................................................................................................................ 432

38

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

14 Manual operation and setup.......................................................................................................435

14.1 Switch-on, switch-off..........................................................................................................................436

Switch-on...............................................................................................................................................436

Switch-off...............................................................................................................................................438

14.2 Moving the machine axes..................................................................................................................439

Note.......................................................................................................................................................439

Moving the axis with the machine axis direction buttons.................................................................... 439

Incremental jog positioning...................................................................................................................439

Traverse with electronic handwheels....................................................................................................440

14.3 Spindle speed S, feed rate F and miscellaneous function M......................................................... 450

Application............................................................................................................................................. 450

Entering values......................................................................................................................................450

Adjusting spindle speed and feed rate................................................................................................. 451

Activating feed-rate limitation............................................................................................................... 451

14.4 Functional safety FS (option)............................................................................................................ 452

Miscellaneous........................................................................................................................................452

Explanation of terms............................................................................................................................. 453

Checking the axis positions.................................................................................................................. 454

Activating feed-rate limitation............................................................................................................... 455

Additional status displays......................................................................................................................456

14.5 Datum setting without a 3-D touch probe.......................................................................................457

Note.......................................................................................................................................................457

Preparation.............................................................................................................................................457

Workpiece presetting with axis keys....................................................................................................457

Datum management with the preset table.......................................................................................... 458

14.6 Using 3-D touch probes (Touch Probe Function software option)................................................. 464

Overview............................................................................................................................................... 464

Functions in touch probe cycles........................................................................................................... 465

Selecting touch probe cycles................................................................................................................467

Recording measured values from the touch-probe cycles................................................................... 468

Writing measured values from the touch probe cycles in a datum table............................................. 469

Writing measured values from the touch probe cycles in the preset table.......................................... 470

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

39

Contents

14.7 Calibrating a 3-D touch trigger probe (software option Touch probe functions).......................... 471

Introduction........................................................................................................................................... 471

Calibrating the effective length............................................................................................................. 472

Calibrating the effective radius and compensating center misalignment............................................. 473

Displaying calibration values................................................................................................................. 475

14.8 Compensating workpiece misalignment with 3-D touch probe (Software-Option Touch probe

functions)............................................................................................................................................. 476

Introduction........................................................................................................................................... 476

Identifying basic rotation.......................................................................................................................477

Saving a basic rotation in the preset table...........................................................................................477

Compensation of workpiece misalignment by rotating the table.........................................................477

Displaying a basic rotation.................................................................................................................... 478

Canceling a basic rotation.....................................................................................................................478

14.9 Datum Setting with 3-D Touch Probe (Touch Probe Function Software Option).......................... 479

Overview............................................................................................................................................... 479

Datum setting in any axis..................................................................................................................... 479

Corner as datum................................................................................................................................... 480

Circle center as datum..........................................................................................................................482

Setting a center line as datum............................................................................................................. 484

Measuring workpieces with a 3-D touch probe................................................................................... 485

Using touch probe functions with mechanical probes or measuring dials............................................488

14.10Tilting the working plane (software option 1).................................................................................489

Application, function..............................................................................................................................489

Traversing reference points in tilted axes............................................................................................. 491

Position display in a tilted system........................................................................................................ 491

Limitations on working with the tilting function...................................................................................491

40

To activate manual tilting:..................................................................................................................... 492

Setting the current tool-axis direction as the active machining direction..............................................493

Setting the datum in a tilted coordinate system.................................................................................. 494

TNC 620 | User's Manual

HEIDENHAIN Conversational Programming | 3/2014

15 Positioning with Manual Data Input.......................................................................................... 495

15.1 Programming and executing simple machining operations...........................................................496

Positioning with manual data input (MDI)............................................................................................ 496

Protecting and erasing programs in $MDI............................................................................................499

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

41

Contents

16 Test run and program run........................................................................................................... 501

16.1 Graphics (Advanced Graphic Features software option)................................................................ 502

Application............................................................................................................................................. 502

Speed of the Setting test runs............................................................................................................. 503

Overview: Display modes..................................................................................................................... 504

Plan view...............................................................................................................................................505

Projection in three planes..................................................................................................................... 505

3-D view................................................................................................................................................ 506

Repeating graphic simulation................................................................................................................509

Tool display............................................................................................................................................509

Measurement of machining time......................................................................................................... 510

16.2 Showing the workpiece blank in the working space (Advanced Graphic Features software

option).................................................................................................................................................. 511

Application............................................................................................................................................. 511

16.3 Functions for program display.......................................................................................................... 512

Overview............................................................................................................................................... 512

16.4 Test Run................................................................................................................................................513

Application............................................................................................................................................. 513

16.5 Program run.........................................................................................................................................515

Application............................................................................................................................................. 515

Running a part program........................................................................................................................ 516

Interrupt machining............................................................................................................................... 517

Moving the machine axes during an interruption................................................................................. 518

Resuming program run after an interruption........................................................................................ 518

Retraction after a power interruption....................................................................................................520

Any entry into program (mid-program startup).....................................................................................523

Returning to the contour.......................................................................................................................525

16.6 Automatic program start....................................................................................................................526

Application............................................................................................................................................. 526

16.7 Optional block skip............................................................................................................................. 527

Application............................................................................................................................................. 527

Inserting the "/" character......................................................................................................................527

Erasing the "/" character........................................................................................................................ 527

42

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

16.8 Optional program-run interruption....................................................................................................528

Application............................................................................................................................................. 528

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

43

Contents

17 MOD functions..............................................................................................................................529

17.1 MOD function...................................................................................................................................... 530

Selecting MOD functions......................................................................................................................530

Changing the settings........................................................................................................................... 530

Exiting MOD functions..........................................................................................................................530

Overview of MOD functions................................................................................................................ 531

17.2 Graphic settings.................................................................................................................................. 532

17.3 Machine settings................................................................................................................................. 533

External access..................................................................................................................................... 533

Tool usage file....................................................................................................................................... 533

Select kinematics.................................................................................................................................. 534

17.4 System settings...................................................................................................................................535

Set the system time............................................................................................................................. 535

17.5 Position Display Types........................................................................................................................ 536

Application............................................................................................................................................. 536

17.6 Unit of Measurement......................................................................................................................... 537

Application............................................................................................................................................. 537

17.7 Displaying operating times................................................................................................................ 537

Application............................................................................................................................................. 537

17.8 Software numbers...............................................................................................................................538

Application............................................................................................................................................. 538

17.9 Entering the code number................................................................................................................. 538

Application............................................................................................................................................. 538

44

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

17.10 Setting up data interfaces..................................................................................................................539

Serial interfaces on the TNC 620......................................................................................................... 539

Application............................................................................................................................................. 539

Setting the RS-232 interface.................................................................................................................539

Setting the BAUD RATE (baudRate)..................................................................................................... 539

Setting the protocol (protocol).............................................................................................................. 540

Setting data bits (dataBits)....................................................................................................................540

Check parity (parity).............................................................................................................................. 540

Setting the stop bits (stopBits).............................................................................................................540

Setting handshaking (flowControl)........................................................................................................ 541

File system for file operations (fileSystem).......................................................................................... 541

Settings for data transfer with the TNCserver PC software.................................................................541

Setting the operating mode of the external device (fileSystem).......................................................... 542

Data transfer software.......................................................................................................................... 543

17.11 Ethernet interface................................................................................................................................545

Introduction........................................................................................................................................... 545

Connection options............................................................................................................................... 545

Configuring the TNC............................................................................................................................. 545

17.12 Firewall................................................................................................................................................. 551

Application............................................................................................................................................. 551

17.13 Configure HR 550 FS wireless handwheel....................................................................................... 554

Application............................................................................................................................................. 554

Assigning the handwheel to a specific handwheel holder................................................................... 554

Setting the transmission channel..........................................................................................................555

Selecting the transmitter power........................................................................................................... 555

Statistical data.......................................................................................................................................556

17.14 Load machine configuration.............................................................................................................. 556

Application............................................................................................................................................. 556

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

45

Contents

18 Tables and overviews...................................................................................................................557

18.1 Machine-specific user parameters.....................................................................................................558

Application............................................................................................................................................. 558

18.2 Connector pin layout and connection cables for data interfaces...................................................568

RS-232-C/V.24 interface for HEIDENHAIN devices...............................................................................568

Non-HEIDENHAIN devices....................................................................................................................570

Ethernet interface RJ45 socket............................................................................................................ 571

18.3 Technical Information..........................................................................................................................572

18.4 Overview tables...................................................................................................................................580

Fixed cycles...........................................................................................................................................580

Miscellaneous functions....................................................................................................................... 581

18.5 Functions of the TNC 620 and the iTNC 530 compared................................................................. 583

Comparison: Specifications................................................................................................................... 583

Comparison: Data interfaces.................................................................................................................583

Comparison: Accessories......................................................................................................................584

Comparison: PC software..................................................................................................................... 584

Comparison: Machine-specific functions.............................................................................................. 585

Comparison: User functions................................................................................................................. 585

Comparator: Cycles............................................................................................................................... 592

Comparison: Miscellaneous functions.................................................................................................. 595

Comparison: Touch probe cycles in the Manual Operation and El. Handwheel modes........................597

Comparison: Touch probe cycles for automatic workpiece inspection................................................. 597

Comparison: Differences in programming............................................................................................ 599

Comparison: Differences in Test Run, functionality.............................................................................. 603

Comparison: Differences in Test Run, operation.................................................................................. 603

46

Comparison: Differences in Manual Operation, functionality............................................................... 603

Comparison: Differences in Manual Operation, operation....................................................................605

Comparison: Differences in Program Run, operation........................................................................... 605

Comparison: Differences in Program Run, traverse movements..........................................................606

Comparison: Differences in MDI operation.......................................................................................... 610

Comparison: Differences in programming station................................................................................ 611

TNC 620 | User's Manual

HEIDENHAIN Conversational Programming | 3/2014

1

First Steps with

the TNC 620

1

First Steps with the TNC 620

1.1 Overview

1.1 Overview

This chapter is intended to help TNC beginners quickly learn to
handle the most important procedures. For more information on a
respective topic, see the section referred to in the text.

The following topics are included in this chapter:

Machine switch-on
Programming the first part
Graphically testing the first part
Setting up tools
Workpiece setup
Running the first program

1.2 Machine switch-on

Acknowledging the power interruption and moving to the reference points

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

Switch on the power supply for TNC and machine: The TNC
starts the operating system. This process may take several
minutes. Then the TNC will display the "Power interrupted"
message in the screen header.

Press the CE key: The TNC compiles the PLC
program.

Switch on the machine control voltage: The TNC
checks operation of the emergency stop circuit
and goes into the reference run mode

Cross the reference points manually in the
displayed sequence: For each external axis, press
the START key. If you have absolute linear and
angle encoders on your machine there is no need
for a reference run

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

Further information on this topic

Traversing the reference marks: See "Switch-on", page 436
Operating modes: See "Programming", page 71

48

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

NO

ENT

1.3 Programming the first part

Selecting the correct operating mode

You can write programs only in Programming mode:

Press the operating mode key: The TNC goes into
the Programming operating mode

Further information on this topic

Operating modes: See "Programming", page 71

The most important TNC keys

Functions for conversational guidance Key

Confirm entry and activate the next dialog
prompt

1

Programming the first part 1.3

Ignore the dialog question

End the dialog immediately

Abort dialog, discard entries

Soft keys on the screen with which you select
functions appropriate to the active state

Further information on this topic

Writing and editing programs: See "Editing a program",
page 98

Overview of keys: See "Controls of the TNC", page 2

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

49

1

First Steps with the TNC 620

1.3 Programming the first part

Creating a new program/file management

Press the PGM MGT key: The TNC opens the file
management. The file management of the TNC is
arranged much like the file management on a PC
with the Windows Explorer. The file management
enables you to manipulate data on the TNC hard
disk

Use the arrow keys to select the folder in which
you want to open the new file

Enter any desired file name with the extension .H:
The TNC then automatically opens a program and
asks for the unit of measure for the new program

Selecting the unit of measure: Press the MM or
INCH soft key

The TNC automatically generates the first and last blocks of the
program. Afterwards you can no longer change these blocks.

Further information on this topic

File management: See "Working with the file manager",
page 106

Creating a new program: See "Opening programs and entering",
page 91

50

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Programming the first part 1.3

Defining a workpiece blank

After you have created a new program you can define a workpiece
blank. For example, define a cuboid by entering the MIN and MAX
points, each with reference to the selected reference point.

After you have selected the desired blank form via soft key, the
TNC automatically initiates the workpiece blank definition and asks
for the required data:

Working plane in graphic: XY?: Enter the active spindle axis. Z
is saved as default setting. Accept with the ENT key

Workpiece blank def.: minimum X: Smallest X coordinate of
the workpiece blank with respect to the reference point, e.g. 0.
Confirm with the ENT key

Workpiece blank def.: minimum Y: Smallest Y coordinate of
the workpiece blank with respect to the reference point, e.g. 0.
Confirm with the ENT key

Workpiece blank def.: minimum Z: Smallest Z coordinate of
the workpiece blank with respect to the reference point, e.g.
–40. Confirm with the ENT key

Workpiece blank def.: maximum X: Largest X coordinate of
the workpiece blank with respect to the reference point, e.g.

100. Confirm with the ENT key
Workpiece blank def.: maximum Y: Largest Y coordinate of

the workpiece blank with respect to the reference point, e.g.

100. Confirm with the ENT key
Workpiece blank def.: maximum Z: Largest Z coordinate of

the workpiece blank with respect to the reference point, e.g. 0.
Confirm with the ENT key. The TNC concludes the dialog

1

Example NC blocks

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

Further information on this topic

Define the blank: page 94

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

51

1

First Steps with the TNC 620

1.3 Programming the first part

Program layout

NC programs should be arranged consistently in a similar manner.
This makes it easier to find your place, accelerates programming
and reduces errors.

Recommended program layout for simple, conventional contour
machining

1 Call tool, define tool axis
2 Retract the tool
3 Pre-position the tool in the working plane near the contour starting

point

4 In the tool axis, position the tool above the workpiece, or

preposition immediately to workpiece depth. If required, switch on

the spindle/coolant
5 Contour approach
6 Contour machining
7 Contour departure
8 Retract the tool, end program

Further information on this topic

Contour programming: See "Tool movements in the program"

Layout of contour machining
programs

0 BEGIN PGM BSPCONT MM

1 BLK FORM 0.1 Z X... Y... Z...

2 BLK FORM 0.2 X... Y... Z...

3 TOOL CALL 5 Z S5000

4 L Z+250 R0 FMAX

5 L X... Y... R0 FMAX

6 L Z+10 R0 F3000 M13

7 APPR ... RL F500

...

16 DEP ... X... Y... F3000 M9

17 L Z+250 R0 FMAX M2

18 END PGM BSPCONT MM

Recommended program layout for simple cycle programs

1 Call tool, define tool axis
2 Retract the tool
3 Define the machining positions
4 Define the fixed cycle
5 Call the cycle, switch on the spindle/coolant
6 Retract the tool, end program

Further information on this topic

Cycle programming: See User's Manual for Cycles

Cycle program layout

0 BEGIN PGM BSBCYC MM

1 BLK FORM 0.1 Z X... Y... Z...

2 BLK FORM 0.2 X... Y... Z...

3 TOOL CALL 5 Z S5000

4 L Z+250 R0 FMAX

5 PATTERN DEF POS1( X... Y... Z... ) ...

6 CYCL DEF...

7 CYCL CALL PAT FMAX M13

8 L Z+250 R0 FMAX M2

9 END PGM BSBCYC MM

52

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Programming a simple contour

The contour shown to the right is to be milled once to a depth of
5 mm. You have already defined the workpiece blank. After you
have initiated a dialog through a function key, enter all the data
requested by the TNC in the screen header.

Call the tool: Enter the tool data. Confirm each of
your entries with the ENT key. Do not forget the
tool axis

Retract the tool: Press the orange axis key Z in
order to get clear in the tool axis, and enter the
value for the position to be approached, e.g. 250.
Press the ENT key

Radius comp.: RL/RR/no comp.? confirm with the
ENT key: Activate no radius compensation

Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)

Confirm Miscellaneous function F=? with the END
key: The TNC stores the entered positioning block

Pre-position the tool in the working plane: Press
the orange axis key X and enter the value for the
position to be approached, e.g. -20.

Press the orange axis key Y and enter the value for
the position to be approached, e.g. -20. Confirm
your entry with the ENT key.

Radius comp.: RL/RR/no comp.? confirm with the
ENT key: Activate no radius compensation

Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)

Confirm Miscellaneous function F=? with the END
key: The TNC stores the entered positioning block

Move tool to depth: Press the orange axis key and
enter the value for the position to be approached,
e.g. -5. Press the ENT key

Radius comp.: RL/RR/no comp.? confirm with the
ENT key: Activate no radius compensation

Feed rate F=? Enter the positioning feed rate, e.g.
3000 mm/min and confirm with the ENT key

Miscellaneous function M? Switch on the spindle

and coolant, e.g. M13 and confirm with the END
key: The TNC stores the entered positioning block

To return to the contour, Press the APPR/DEP key.
The TNC displays a soft-key row with approach and
departure functions.

1

Programming the first part 1.3

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

53

1

First Steps with the TNC 620

1.3 Programming the first part

Select the approach function APPR CT: Enter the
coordinate of the contour starting point 1 in X and
Y, e.g. 5/5. Confirm with the ENT key

Center angle? Enter the approach angle, e.g. 90°,
and confirm with the ENT key

Circle radius? Enter the approach radius, e.g. 8
mm, and confirm with the ENT key

Radius comp.: Confirm RL/RR/no comp.? with
the ENT key: Activate radius compensation to the
left of the programmed contour

Feed rate F=? Enter the machining feed rate, e.g.
700 mm/min, and confirm your entry with the END
key

Machine the contour and move to the contour
point 2: You only need to enter the information
that changes. In other words, enter only the Y
coordinate 95 and save your entry with the END
key

Approach contour point 3: Enter the X coordinate
95 and save your entry with the END key

Define the chamfer at the contour point 3: Enter
the chamfer width 10 mm and confirm with the
END key

Approach contour point 4: Enter the Y coordinate 5
and save your entry with the END key

Define the chamfer at the contour point 4: Enter
the chamfer width 20 mm and confirm with the
END key

Approach contour point 1: Enter the X coordinate 5
and save your entry with the END key

Depart the contour

Select the departure function DEP CT
Center angle? Enter the departure angle, e.g. 90°,

and confirm with the ENT key
Circle radius? Enter the departure radius, e.g. 8

mm, and confirm with the ENT key
Feed rate F=? Enter the positioning feed rate, e.g.

3000 mm/min and confirm with the ENT key
Miscellaneous function M? Switch off the coolant,

e.g. M9, and confirm with the END key: The TNC
stores the entered positioning block

54

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Enter Retract tool: Press the orange axis key Z in
order to get clear in the tool axis, and enter the
value for the position to be approached, e.g. 250.
Press the ENT key

Radius comp.: RL/RR/no comp.? confirm with the
ENT key: Activate no radius compensation

Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)

MISCELLANEOUS FUNCTION M? Enter M2 to enter
end of program, then confirm with the END key.
The TNC saves the entered positioning block

Further information on this topic

Complete example with NC blocks: See "Example: Linear

movements and chamfers with Cartesian coordinates",

page 209

Creating a new program: See "Opening programs and entering",

page 91

Approaching/departing contours: See " Approaching and

departing a contour", page 192

Programming contours: See "Overview of path functions",

page 200

Programmable feed rates: See "Possible feed rate input",

page 96

Tool radius compensation: See "Tool radius compensation ",

page 182

Miscellaneous functions (M): See "M functions for program run

inspection, spindle and coolant ", page 343

1

Programming the first part 1.3

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

55

1

First Steps with the TNC 620

1.3 Programming the first part

Creating a cycle program

The holes (depth of 20 mm) shown in the figure at right are to be
drilled with a standard drilling cycle. You have already defined the
workpiece blank.

Call the tool: Enter the tool data. Confirm each of
your entries with the ENT key. Do not forget the

tool axis

Retract the tool: Press the orange Z axis key in
order to get clear in the tool axis, and enter the
value for the position to be approached, e.g. 250.
Press the ENT key

Radius comp.: Confirm RL/RR/no comp? with the
ENT key: Activate no radius compensation

Confirm feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)

Confirm Miscellaneous function F=? with the END
key: The TNC stores the entered positioning block

Call the cycle menu

Display the drilling cycles

Select standard drilling cycle 200: The TNC starts
the dialog for cycle definition. Enter all parameters
requested by the TNC step by step and conclude
each entry with the ENT key. In the screen to the
right, the TNC also displays a graphic showing the
respective cycle parameter

Call the menu for special functions

Display the functions for point machining

Select the pattern definition

Select point entry: Enter the coordinates of the 4
points and confirm each with the ENT key. After
entering the fourth point, save the block with the
END key

Display the menu for defining the cycle call

Run the drilling cycle on the defined pattern:
Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)
Miscellaneous function M? Switch on the spindle

and coolant, e.g. M13 and confirm with the END
key: The TNC stores the entered positioning block

56

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Enter Retract tool: Press the orange axis key Z in
order to get clear in the tool axis, and enter the
value for the position to be approached, e.g. 250.
Press the ENT key

Radius comp.: Confirm RL/RR/No comp.? with
the ENT key: Activate no radius compensation

Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)

Miscellaneous function M? Enter M2 to enter end
of program, then confirm with the END key. The
TNC stores the entered positioning block

Example NC blocks

0 BEGIN PGM C200 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 TOOL CALL 5 Z S4500

4 L Z+250 R0 FMAX

5 PATTERN DEF

POS1 (X+10 Y+10 Z+0)
POS2 (X+10 Y+90 Z+0)
POS3 (X+90 Y+90 Z+0)
POS4 (X+90 Y+10 Z+0)

6 CYCL DEF 200 DRILLING

Q200=2 ;SET-UP CLEARANCE

Q201=-20 ;DEPTH

Q206=250 ;FEED RATE FOR PLNGNG

Q202=5 ;INFEED DEPTH

Q210=0 ;DWELL TIME AT TOP

Q203=-10 ;SURFACE COORDINATE

Q204=20 ;SECOND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT DEPTH

7 CYCL CALL PAT FMAX M13

8 L Z+250 R0 FMAX M2

9 END PGM C200 MM

1

Programming the first part 1.3

Definition of workpiece blank

Tool call

Retract the tool

Define the machining positions

Define the cycle

Spindle and coolant on, call the cycle

Retract the tool, end program

Further information on this topic

Creating a new program: See "Opening programs and entering",

page 91

Cycle programming: See User's Manual for Cycles, "Cycle

fundamentals / Overviews"

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

57

1

First Steps with the TNC 620

1.4 Graphically testing the first part (Advanced Graphic Features

software option)

1.4 Graphically testing the first part

(Advanced Graphic Features software
option)

Selecting the correct operating mode

You can test programs only in the Test Run mode:

Press the operating-mode key: The TNC goes into
the Test Run operating mode

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 71

Testing programs: See "Test Run", page 513

Selecting the tool table for the test run

You only need to execute this step if you have not activated a tool
table in the Test Run mode.

Press the PGM MGT key: The TNC opens the file
management

Press the select type soft key: The TNC shows a
soft-key menu for selection of the file type to be
displayed

Press the DEFAULT soft key: The TNC shows all
saved files in the right window

Move the highlight to the left onto the directories

Move the highlight to the TNC:\ directory

Move the highlight to the right onto the files

Move the highlight to the file TOOL.T (active tool
table) and load with the ENT key: TOOL.T receives
the status S and is therefore active for the test run

Press the END key: Exit the file management

Further information on this topic

Tool management: See "Enter tool data into the table",

page 162

Testing programs: See "Test Run", page 513

58

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

1

Graphically testing the first part (Advanced Graphic Features

Choosing the program you want to test

Press the PGM MGT key: The TNC opens the file
management

Press the LAST FILES soft key: The TNC opens a
pop-up window with the most recently selected
files

Use the arrow keys to select the program that you
want to test. Load with the ENT key

Further information on this topic

Selecting a program: See "Working with the file manager",

page 106

Selecting the screen layout and the view

Press the key for selecting the screen layout: The
TNC displays all available alternatives in the soft­key row

Press the PROGRAM+GRAPHICS soft key: In
the left half of the screen the TNC shows the
program; in the right half it shows the workpiece
blank

Press the FURTHER VIEW OPTIONS soft key

1.4

software option)

Move the soft-key row further and select the
desired view by soft key

The TNC features the following views:

Soft key Function

Plan view

Projection in three planes

3-D view

Further information on this topic

Graphic functions: See "Graphics (Advanced Graphic Features

software option)", page 502

Running a test run: See "Test Run", page 513

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

59

1

First Steps with the TNC 620

1.4 Graphically testing the first part (Advanced Graphic Features

software option)

Starting the test run

Press the RESET + START soft key: The TNC
simulates the active program up to a programmed
break or to the program end

While the simulation is running, you can use the
soft keys to change views

Press the STOP soft key: The TNC interrupts the
test run

Press the START soft key: the TNC resumes the
test run after an interruption.

Further information on this topic

Running a test run: See "Test Run", page 513

Graphic functions: See "Graphics (Advanced Graphic Features

software option)", page 502

Adjust the simulation speed: See "Speed of the Setting test

runs", page 503

60

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

1.5 Setting up tools

Selecting the correct operating mode

Tools are set up in the Manual Operation mode:

Press the operating-mode key: The TNC switches
to the Manual mode of operation

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 71

1

Setting up tools 1.5

Preparing and measuring tools

Clamp the required tools in their chucks

When measuring with an external tool presetter: Measure the

tools, note down the length and radius, or transfer them directly

to the machine through a transfer program

When measuring on the machine: store the tools in the tool

changer page 63

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

61

1

First Steps with the TNC 620

1.5 Setting up tools

The tool table TOOL.T

In the tool table TOOL.T (permanently saved under TNC:\TABLE\),
save the tool data such as length and radius, but also further tool­specific information that the TNC needs to perform its functions.

To enter tool data in the tool table TOOL.T, proceed as follows:

Display the tool table

Edit the tool table: Set the EDITING soft key to ON
With the upward or downward arrow keys you can

select the tool number that you want to edit
With the rightward or leftward arrow keys you can

select the tool data that you want to edit
To exit the tool table, press the END key

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 71

Working with the tool table: See "Enter tool data into the table",

page 162

62

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

The pocket table TOOL_P.TCH

The function of the pocket table depends on the
machine. Refer to your machine manual.

In the pocket table TOOL_P.TCH (permanently saved under TNC:
\TABLE\) you specify which tools your tool magazine contains.

To enter data in the pocket table TOOL_P.TCH, proceed as follows:

Displaying the tool table: The TNC shows the tool
table

Display the pocket table: The TNC shows the
pocket table

Edit the pocket table: Set the EDIT soft key to ON
With the upward or downward arrow keys you can

select the pocket number that you want to edit
With the rightward or leftward arrow keys you can

select the data that you want to edit
Exit the pocket table: press the END key.

1

Setting up tools 1.5

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 71

Working with the pocket table: See "Pocket table for tool

changer", page 171

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

63

1

First Steps with the TNC 620

1.6 Workpiece setup

1.6 Workpiece setup

Selecting the correct operating mode

Workpieces are set up in the Manual Operation or Electronic
Handwheel mode

Press the operating-mode key: The TNC switches
to the Manual mode of operation

Further information on this topic

Manual Operation mode: See "Moving the machine axes",

page 439

Clamping the workpiece

Mount the workpiece with a fixture on the machine table. If you
have a 3-D touch probe on your machine, then you do not need to
clamp the workpiece parallel to the axes.

If you do not have a 3-D touch probe available, you have to align the
workpiece so that it is fixed with its edges parallel to the machine
axes.

64

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Datum setting with 3-D touch probe (software option: Touch probe function)

Insert a 3-D touch probe Insert the 3-D touch probe: In the MDI

mode, run a TOOL CALL block containing the tool axis and then

return to the Manual Operation mode

Select the probing functions: The TNC displays all
available functions in the soft-key row

Set the datum at a workpiece corner, for example
Position the touch probe near the first touch point

on the first workpiece edge
Select the probing direction via soft key
Press NC start Press NC start: The touch probe

moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the second touch
point on the first workpiece edge

Press NC start Press NC start: The touch probe
moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the first touch point
on the second workpiece edge

Select the probing direction via soft key
Press NC start Press NC start: The touch probe

moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the second touch
point on the second workpiece edge

Press NC start Press NC start: The touch probe
moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Then the TNC shows the coordinates of the
measured corner point

To set to 0: Press the SET DATUM soft key
Press the END soft key to close the menu

1

Workpiece setup 1.6

Further information on this topic

Datum setting: See "Datum Setting with 3-D Touch Probe (Touch

Probe Function Software Option)", page 479

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

65

1

First Steps with the TNC 620

1.7 Running the first program

1.7 Running the first program

Selecting the correct operating mode

You can run programs either in the Single Block or the Full
Sequence mode:

Press the operating-mode key: The TNC goes into
the Program Run, Single Block mode and the
TNC executes the program block by block. You
have to confirm each block with the NC start key

Press the operating-mode key: The switches
to the Program Run, Full Sequence operating
mode: The TNC switches to that mode and
runs the program after NC start up to a program
interruption or to the end of the program

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 71

Running programs: See "Program run", page 515

Choosing the program you want to run

Press the PGM MGT key: The TNC opens the file
management

Press the LAST FILES soft key: The TNC opens a
pop-up window with the most recently selected
files

If desired, use the arrow keys to select the
program that you want to run. Load with the ENT
key

Further information on this topic

File management: See "Working with the file manager",

page 106

Start the program

Press the NC start key: The TNC runs the active
program

Further information on this topic

Running programs: See "Program run", page 515

66

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

2

Introduction

2

Introduction

2.1 The TNC 620

2.1 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. They are designed for milling and drilling
machines, 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 functions are fast and easy to use.

Programming: HEIDENHAIN conversational and ISO formats

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 performs the necessary
calculations automatically. Workpiece machining can be graphically
simulated either during or before actual machining.

It is also possible to program the TNCs in ISO format or DNC
mode.

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

Compatibility

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 when the file is opened.

See "Functions of the TNC 620 and the iTNC 530
compared", page 583. Please also note the
detailed description of the differences between the
iTNC 530 and the TNC 620

68

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

2

3

4

5

8

9

6

7

1

4

2
3

4

5

8

9

6

7

1

4

Visual display unit and operating panel 2.2

2.2 Visual display unit and operating panel

Display screen

The TNC is available either as a compact version or with a separate
display unit and operating panel. Both TNC variants come with a 15­inch TFT color flat-panel display.

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 operating
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 soft­key row. You can select these functions by pressing the keys
immediately below them. The lines immediately above the
soft-key row indicate the number of soft-key rows that can be
called with the black arrow keys to the right and left. The bar
representing the active soft-key row is highlighted

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

modes

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

2

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

69

2

2

3

4

5

6

7

2

3

4

5

8

9

6

7

10

1

Introduction

2.2 Visual display unit and operating panel

Setting 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 the program
structure in the right window instead, 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 screen layout key: The soft-key row
shows the available layout options, see "Operating
modes", page 62

Select the desired screen layout

Control Panel

The TNC 620 is delivered with an integrated keyboard. As an
alternative, the TNC 620 is also available with a separate display
unit and an operating panel with alphabetic keyboard.

1 Alphabetic keyboard for entering texts and file names, and for

ISO programming.

2

3 Programming modes
4 Machine operating modes
5 Initiation of programming dialogs
6
7 Numerical input and axis selection
8 Touchpad
9 Mouse function keys
10 Machine operating panel (refer to your machine manual)

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

File management
Calculator
MOD function
HELP function

Navigation keys and GOTO jump command

Some machine manufacturers do not use the
standard operating panel from HEIDENHAIN. Refer
to your machine manual.

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

70

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

2.3 Modes of Operation

Manual Operation and El. Handwheel

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

The El. 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

Positions

2

Modes of Operation 2.3

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 prepositioning.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program blocks, right: status display

Programming

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 programmed paths of traverse.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program, right: program structure

Left: program, right: programming graphics

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

71

2

Introduction

2.3 Modes of Operation

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
working space. This simulation is supported graphically in different
display modes. (Software option Advanced Graphic Features)

Soft keys for selecting the screen layout: See "Program Run, Full
Sequence and Program Run, Single Block", page 72.

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

Left: program, right: program structure

Left: program, right: status

Left: program, right: graphics (Advanced

Graphic Features software option)

Graphics (Advanced Graphic Features
software option)

Soft keys for selecting the screen layout for pallet tables
(Software option Pallet management)

Window Soft key

Pallet table

Left: program, right: pallet table

Left: pallet table, right: status

72

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

2.4 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 Operation and El. Handwheel modes the status

display appears in the large window.

Information in the status display

Icon Meaning

ACTL. Position display: Actual, nominal or distance-to-go

coordinates mode

2

Status displays 2.4

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

Number of the active presets from the preset
table. If the datum was set manually, the TNC
displays the text MAN behind the symbol

F S M 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 is clamped

Axis can be moved with the handwheel

Axes are moving under a basic rotation

Axes are moving in a tilted working plane

The M128 function or TCPM FUNCTION is active

No active program

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

73

2

Introduction

2.4 Status displays

Icon Meaning

Program run has started

Program run is stopped

Program run is being aborted

The Active Chatter Control feature (ACC) is active
(software option)

The Cross Talk Compensation (CTC) is active
(software option)

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 of operation.

To switch on the additional status display:

Call the soft-key row for screen layout

Select the layout option for the additional status
display: In the right half of the screen, the TNC
shows the OVERVIEW status form

To select an additional status display:

Switch the soft-key rows until the STATUS soft
keys appear

Either select the additional status display directly
by soft key, e.g. positions and coordinates, or

use the switch-over soft keys to select the desired
view

The available status displays described below can be selected
either directly by soft key or with the switch-over soft keys.

74

Please note that some of the status information
described below is not available unless the
associated software option is enabled on your TNC.

TNC 620 | User's Manual

HEIDENHAIN Conversational Programming | 3/2014

Overview

After switch-on, the TNC displays the Overview status form,
provided that you have selected the PROGRAM+STATUS screen
layout (or POSITION + STATUS). The overview form contains a
summary of the most important status information, which you can
also find on the various detail forms.

Soft key Meaning

Position display

Tool information

Active M functions

Active coordinate transformations

Active subprogram

Active program section repeat

Program called with PGM CALL

Current machining time

Name of the active main program

2

Status displays 2.4

General program information (PGM tab)

Soft key Meaning

No direct
selection
possible

Name of the active main program

Circle center CC (pole)

Dwell time counter

Machining time when the program was
completely simulated in the Test Run operating
mode

Current machining time in percent

Current time

Active programs

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

75

2

Introduction

2.4 Status displays

Program section repeat/Subprograms (LBL tab)

Soft key Meaning

No direct
selection
possible

Information on standard cycles (CYC tab)

Soft key Meaning

No direct
selection
possible

Active program section repeats with block
number, label number, and number of
programmed repeats/repeats yet to be run

Active subprogram numbers with block number
in which the subprogram was called and the
label number that was called

Active machining cycle

Active values of Cycle 32 Tolerance

76

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Active miscellaneous functions M (M tab)

Soft key Meaning

2

Status displays 2.4

No direct
selection
possible

Positions and coordinates (POS tab)

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

Type of position display, e.g. actual position

Tilt angle of the working plane

Angle of a basic rotation

Active kinematics

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

77

2

Introduction

2.4 Status displays

Information on tools (TOOL tab)

Soft key Meaning

Display of active tool:

T: Tool number and name
RT: Number and name of a replacement tool

Tool axis

Tool length and radii

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

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

Display of programmed tool and replacement tool

Tool measurement (TT tab)

The TNC displays the TT tab only if the function is
active on your machine.

Soft key Meaning

No direct
selection
possible

Number of the tool to be measured

Display whether the tool radius or the tool
length is being measured

MIN and MAX values of the individual cutting
edges and the result of measuring the rotating
tool (DYN = dynamic measurement)

Cutting edge number with the corresponding
measured value. If the measured value is
followed by an asterisk, the permissible
tolerance in the tool table was exceeded

78

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Coordinate transformations (TRANS tab)

Soft key Meaning

Name of the active datum table

Active datum number (#), comment from the
active line of the active datum number (DOC)
from Cycle 7

Active datum shift (Cycle 7); The TNC displays
an active datum shift in up to 8 axes

Mirrored axes (Cycle 8)

Active basic rotation

Active rotation angle (Cycle 10)

Active scaling factor/factors (Cycles 11 / 26);
The TNC displays an active scaling factor in up
to 6 axes

Scaling datum

2

Status displays 2.4

For further information, refer to the User's Manual for Cycles,
"Coordinate Transformation Cycles."

Displaying Q parameters (QPARA tab)

Soft key Meaning

Display the current values of the defined Q
parameters

Display the character strings of the defined
string parameters

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

79

2

Introduction

2.5 Window Manager

2.5 Window Manager

The machine tool builder determines the scope of
function and behavior of the window manager. Refer
to your machine manual.

The TNC features the Xfce window manager. Xfce is a standard
application for UNIX-based operating systems, and is used to
manage graphical user interfaces. The following functions are
possible with the window manager:

Display a task bar for switching between various applications

(user interfaces).

Manage an additional desktop, on which special applications

from your machine tool builder can run.

Control the focus between NC-software applications and those

of the machine tool builder.

The size and position of pop-up windows can be changed.

It is also possible to close, minimize and restore the pop-up

windows.

The TNC shows a star in the upper left of the screen
if an application of the window manager or the
window manager itself has caused an error. In this
case, switch to the window manager and correct the
problem. If required, refer to your machine manual.

80

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Task bar

In the task bar you can choose different workspaces by mouse
click. The TNC provides the following workspaces:

Workspace 1: Active mode of operation

Workspace 2: Active programming mode

Workspace 3: Manufacturer's applications (optionally available)
In the task bar you can also select other applications that you have

started together with the TNC (switch for example to the PDF

viewer or TNCguide)

Click the green HEIDENHAIN symbol to open a menu in which
you can get information, make settings or start applications. The
following functions are available:

About Xfce: Information on the Windows manager Xfce

About HEROS: Information about the operating system of the

TNC

NC Control: Start and stop the TNC software. Only permitted

for diagnostic purposes

Web Browser: Start Mozilla Firefox

Diagnostics: Available only to authorized specialists to start

diagnostic functions

Settings: Configuration of miscellaneous settings

Date/Time: Set the date and time
Language: Language setting for the system dialogs. During

startup the TNC overwrites this setting with the language
setting of the machine parameter CfgLanguage

Network: Network setting
Reset WM-Conf: Restore basic settings of the Windows

Manager. May also reset settings implemented by your
machine manufacturer

Screensaver: Settings for the screen saver; several are
available

Shares: Configure network connections
Firewall: Configuring the Firewall See "Firewall", page 551

Tools: Only for authorized users. The applications available under

tools can be started directly by selecting the pertaining file

type in the file management of the TNC (See "File manager:

Fundamentals", page 103)

2

Window Manager 2.5

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

81

2

Introduction

2.6 SELinux security software

2.6 SELinux security software

SELinux is an extension for Linux-based operating systems.

SELinux is an additional security software package based on
Mandatory Access Control (MAC) and protects the system against
the running of unauthorized processes or functions and therefore
protects against viruses and other malware.

MAC means that each action must be specifically permitted
otherwise the TNC will not run it. The software is intended as
protection in addition to the normal access restriction in Linux.
Certain processes and actions can only be executed if the standard
functions and access control of SELinux permit it.

The SELinux installation of the TNC is prepared to
permit running of only those programs installed with
the HEIDENHAIN NC software. Other programs
cannot be run with the standard installation.

The access control of SELinux under HEROS 5 is regulated as
follows:

The TNC runs only those applications installed with the

HEIDENHAIN NC software.

Files in connection with the safety of the software (SELinux

system files, HEROS 5 boot files etc.) may only be changed by

programs that are selected explicitly.

New files generated by other programs must never be

executed.

There are only two processes that are permitted to execute new

files:

Starting a software update: A software update from
HEIDENHAIN can replace or change system files.

Starting the SELinux configuration: The configuration of
SELinux is usually password-protected by your machine tool
builder. Refer here to the relevant machine tool manual.

HEIDENHAIN generally recommends activating
SELinux because it provides additional protection
against attacks from outside.

82

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

2

Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

2.7 Accessories: HEIDENHAIN 3-D Touch

Probes and Electronic Handwheels

3-D touch probes (Touch Probe Function software option)

The various HEIDENHAIN 3-D touch probes enable you to:

Automatically align workpieces

Quickly and precisely set datums

Measure the workpiece during program run

Measure and inspect tools

All of the cycle functions (touch probe cycles and
fixed cycles) are described in the Cycle Programming
User’s Manual. Please contact HEIDENHAIN if you
require a copy of this User's Manual. ID: 1096886-xx

2.7

Handwheels

The TS 220, TS 440, TS 444, TS 640 and TS 740 triggering touch
probes edge finder

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 is a cost-effective alternative for applications where digitizing is
not frequently required.

The TS 640 (see figure) and the smaller TS 440 feature infrared
transmission of the triggering signal to the TNC. This makes
them highly convenient for use on machines with automatic tool
changers.

Principle of operation: HEIDENHAIN triggering touch probes feature
a wear resisting 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 the actual
value.

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.

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

83

2

Introduction

2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

Handwheels

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 panel-mounted
handwheels, HEIDENHAIN also offers the HR 410 portable
handwheel.

84

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

3

Programming:

Fundamentals, file

management

3

Programming: Fundamentals, file management

3.1 Fundamentals

3.1 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.

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.

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.

86

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

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.

The TNC 620 can control up to 5 axes. The axes U, V and W
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.

3

Fundamentals 3.1

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 secondary axis (2nd axis). The
assignment of the tool axis is decisive for the assignment of the
principal and secondary axes.

Tool axis Principal axis Secondary axis

X Y Z

Y Z X

Z X Y

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

87

3

Programming: Fundamentals, file management

3.1 Fundamentals

Polar coordinates

If the production drawing is dimensioned in Cartesian coordinates,
you also write the NC 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 two­dimensional 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, and the

Polar Angle, the value of the angle between the angle 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.

Coordinates of the pole
(plane)

X/Y +X

Y/Z +Y

Z/X +Z

Reference axis of the angle

88

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

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

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 an NC program in incremental
coordinates, you thus program the tool to move by the distance
between the previous and the subsequent nominal positions. This
is why they are also referred to as chain dimensions.

To program a position in incremental coordinates, enter the
function "I" before the axis.

Example 2: Holes dimensioned in incremental coordinates

3

Fundamentals 3.1

Absolute coordinates of hole 4

X = 10 mm

Y = 10 mm

Hole 5, with respect to 4 Hole 6, with respect 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 angle
reference axis.

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

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

89

3

Programming: Fundamentals, file management

3.1 Fundamentals

Selecting 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 User’s
Manual for Cycles, Cycles for Coordinate Transformation).

If the production drawing is not dimensioned for NC, set the
datum at a position or corner on the workpiece from which the
dimensions of the remaining workpiece positions can be most
easily measured.

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 Cycle Programming User’s
Manual.

Example

The workpiece drawing 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.

90

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Block number

Path functions

Words

Block

Opening programs and entering 3.2

3.2 Opening programs and entering

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 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.

3

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!

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

91

3

Programming: Fundamentals, file management

3.2 Opening programs and entering

Define the blank: BLK FORM

Immediately after initiating a new program, you define a cuboid,
unmachined workpiece blank. If you wish to define the blank at a
later stage, press the spec fct key, the PROGRAM DEFAULTS soft
key, and then the BLK FORM soft key. The TNC needs this definition
for graphic simulation.

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

The TNC can depict various types of blank forms.

Soft key Function

Define a workpiece blank

Define a cylindrical blank

Define a rotationally symmetric blank

Rectangular blank

The sides of the cuboid lie parallel to the X, Y and Z axes. This
blank 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

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

Program begin, name, unit of measure

Spindle axis, MIN point coordinates

MAX point coordinates

Program end, name, unit of measure

92

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Opening programs and entering 3.2

Cylindrical blank

The cylindrical blank form is defined by the dimensions of the
cylinder:

R: Radius of the cylinder

L: Length of the cylinder

DIST: Distance from datum to cylinder end

RI: Inside radius for a hollow cylinder

The DIST and RI parameters are optional and do not
need to be programmed.

Example: Display the BLK FORM CYLINDER in the NC program

0 BEGIN PGM NEW MM

1 BLK FORM CYLINDER Z R50 L105 DIST+5 RI10

2 END PGM NEW MM

Program begin, name, unit of measure

Spindle axis, radius, length, distance, inside radius

Program end, name, unit of measure

3

Rotationally symmetric blank of any shape

You define the contour of the rotationally symmetric blank in a
subprogram. In the workpiece blank definition you refer to the
contour description:

DIM_D, DIM_R: Diameter or radius of the rotationally

symmetrical blank form

LBL: Subprogram with the contour description

The subprogram can be designated with a number,
an alphanumeric name, or a QS parameter.

Example: Display the BLK FORM ROTATION in the NC program

0 BEGIN PGM NEW MM

1 BLK FORM ROTATION Z DIM_R LBL1

2 M30

3 LBL 1

4 L X+0 Z+1

5 L X+50

6 L Z-20

7 L X+70

8 L Z-100

9 L X+0

10 L Z+1

11 LBL 0

12 END PGM NEW MM

Program begin, name, unit of measure

Spindle axis, manner of interpretation, subprogram number

End of main program

Beginning of subprogram

Beginning of contour

End of contour

End of subprogram

Program end, name, unit of measure

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

93

3

Z

Programming: Fundamentals, file management

3.2 Opening programs and entering

Opening a new part program

You always enter a part program in the PROGRAMMING AND
EDITING mode of operation. An example of program initiation:

Select the PROGRAMMING mode of operation

To call the file manager, Press the PGM MGT key.

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

FILE NAME = ALT.H

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

Selecting 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 (workpiece blank)

Select a rectangular workpiece blank: Press the
soft key for a rectangular blank form

WORKING PLANE IN GRAPHIC: XY

Enter spindle axis, e.g. Z

WORKPIECE BLANK DEF.: MINIMUM

Enter in sequence the X, Y and Z coordinates of
the MIN point and confirm each of your entries
with the ENT key

WORKPIECE BLANK DEF.: MAXIMUM

Enter in sequence the X, Y and Z coordinates of
the MAX point and confirm each of your entries
with the ENT key

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.

Program begin, name, unit of measure

Spindle axis, MIN point coordinates

MAX point coordinates

Program end, name, unit of measure

If you do not wish to define a blank form, cancel the
dialog at Working plane in graphic: XY by pressing
the DEL key.

94

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Y

Opening programs and entering 3.2

Programming tool movements in conversational

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 positioning block

Open block

3

COORDINATES ?

10 (Enter the target coordinate for the X axis)

20 (Enter the target coordinate for the Y axis)

go to the next question with ENT.

RADIUS COMP.: RL/RR/NO COMP.?

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

FEED RATE F=? / F MAX = ENT

100 (Enter a feed rate of 100 mm/min for this path contour)

go to the next question with ENT.

MISCELLANEOUS FUNCTION M ?

Enter 3 (miscellaneous function M3 "Spindle ON").

With the END key, the TNC ends this dialog.

The program-block window displays the following line:

3 L X+10 Y+5 R0 F100 M3

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

95

3

NO

ENT

Programming: Fundamentals, file management

3.2 Opening programs and entering

Possible feed rate input

Functions for setting the feed rate Soft key

Rapid traverse, non-modal. Exception: If
defined before an APPR block, FMAX is also
in effect for moving to an auxiliary point
(See "Important positions for approach and
departure", page 193)

Traverse feed rate automatically calculated in

TOOL CALL

Move at the programmed feed rate (unit of
measure is mm/min or 1/10 inch/min). With
rotary axes, the TNC interprets the feed rate
in degrees/min, regardless of whether the
program is written in mm or inches

Define the feed per revolution (units in mm/
rev or inch/rev). Caution: In inch-programs, FU
cannot be combined with M136

Define the tooth feed (units in mm/tooth or
inch/tooth). The number of teeth must be
defined in the tool table in the CUT. column

Functions for conversational guidance Key

Ignore the dialog question

End the dialog immediately

Abort the dialog and erase the block

96

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

Opening programs and entering 3.2

Actual position capture

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

Positioning-block programming

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 actual-position capture: In the soft-key row
the TNC displays the axes whose positions can be
transferred

Select an axis: The TNC writes the current position
of the selected axis into the active input box

3

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 TNC keeps the soft-key row for axis selection
active until you deactivate it by pressing the actual­position-capture key again. This behavior remains in
effect even if you save the current block and open
a new one with a path function key. If you select a
block element in which you must choose an input
alternative via soft key (e.g. for radius compensation),
then the TNC also closes the soft-key row for axis
selection.

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

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

97

3

Programming: Fundamentals, file management

3.2 Opening programs and entering

Editing a program

You cannot edit a program while it is being run by the
TNC in a machine operating mode.

While you are creating or editing a part program, you can select any
desired line in the program or individual words in a block with the
arrow keys or the soft keys:

Function Soft key/Keys

Go to previous page

Go to next page

Go to beginning of program

Go to end of program

Change the position of the current block
on the screen. Press this soft key to
display additional program blocks that are
programmed before the current block

Change the position of the current block
on the screen. Press this soft key to
display additional program blocks that are
programmed after the current block

Move from one block to the next

Select individual words in a block

To select a certain block, press the GOTO
key, enter the desired block number, and
confirm with the ENT key. Or: Enter the
block number step and press the N LINES
soft key to jump over the entered number
of lines upward or downward

98

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual

NO

ENT

Opening programs and entering 3.2

Function Soft key/Key

Set the selected word to zero

Erase an incorrect number

Delete the (clearable) error message

Delete the selected word

Delete the selected block

Erase cycles and program sections

3

Insert the block that you last edited or
deleted

Inserting blocks at any desired location

Select the block after which you want to insert a new block and

initiate the dialog

Editing and inserting words

Select a word in a block and overwrite it with the new one. The

plain-language dialog is available while the word is highlighted

To accept the change, press the END key
If you want to insert a word, press the horizontal arrow key

repeatedly until the desired dialog appears. You can then enter the
desired value.

Looking for the same words in different blocks

Set the AUTO DRAW soft key to OFF.

To select a word in a block, press the arrow keys
repeatedly until the highlight is on the desired
word.

Select a block with the arrow keys

The word that is highlighted in the new block is the same as the
one you selected previously.

If you have started a search in a very long program,
the TNC shows a progress display window. You then
have the option of canceling the search via soft key.

TNC 620 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014

99

3

Programming: Fundamentals, file management

3.2 Opening programs and entering

Finding any text

Select the search function: Press the FIND soft key. The TNC

displays the Find text: dialog prompt

Enter the text that you wish to find

To find the text, Press the FINDRUN soft key

Marking, copying, deleting and inserting program sections

The TNC provides certain functions for copying program sections
within an NC program or into another NC program—see the table
below.

To copy a program section, proceed as follows:

Select the soft-key row containing the marking functions

Select the first (last) block of the section you wish to copy

To mark the first (last) block, press the SELECT BLOCK soft key.

The TNC then highlights the first character of the block and the

CANCEL SELECTION soft key appears

Move the highlight to the last (first) block of the program section

you wish to copy or delete. The TNC shows the marked blocks

in a different color. You can end the marking function at any time

by pressing the CANCEL SELECTION soft key

To copy the selected program section, press the COPY BLOCK

soft key. To delete the selected section, press the DELETE

BLOCK soft key. The TNC stores the selected block

Using the arrow keys, select the block after which you wish to

insert the copied (deleted) program section

To insert the section into another program, select the
corresponding program using the file manager and
then mark the block after which you wish to insert
the copied block.

To insert the block, press the INSERT BLOCK soft key

To end the marking function, press the Cancel selection soft

key

100

HEIDENHAIN Conversational Programming | 3/2014

TNC 620 | User's Manual