HEIDENHAIN TNC 640 User Manual

TNC 640

User's Manual

HEIDENHAIN
Conversational Programming

NC Software
340590-02
340591-02
340594-02

English (en)
5/2013

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

Alphanumeric keyboard

Key Function

File names, comments

DIN/ISO programming

Programming modes

Key Function

Programming

Test run

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

Machine operating modes

Key Function

Manual operation

Electronic handwheel

Positioning with manual data input

Program run, single block

Program run, full sequence

Show calculator

Navigation keys

Key Function

Move highlight

Go directly to blocks, cycles and
parameter functions

Potentiometer for feed rate and spindle speed

Feed rate Spindle speed

2

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

3

Controls of the TNC

4

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 notes about the
function described must be regarded.

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 | 5/2013

TNC 640 | 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 640 340590-02
TNC 640 E 340591-02
TNC 640 Programming Station 340594-02

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

Simultaneous linear movement in up to 4 axes

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

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

Tool measurement with the TT

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

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

User's Manual 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: 892905-xx

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

7

Fundamentals

TNC model, software and features

Software options

The TNC 640 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:

Hardware, options

■

1st additional axis for 4 axes plus spindle

■

2nd additional axis for 5 axes plus spindle

Software option 1 (option number 08)
Rotary table machining

Coordinate transformation
Interpolation

Software option 2 (option number 09)
3-D machining

Interpolation

HEIDENHAIN DNC (option number 18)

Display step (Option number 23)

step

■

■

■

■

■

■

■

■

■

■

■

■

■

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)

Communication with external PC applications over COM component

Linear axes to 0.01 µmInput resolution and display
Rotary axes to 0.00001°

Dynamic Collision Monitoring (DCM) software option (option number 40)
Collision monitoring in all

machine operating modes

Software option for additional conversational languages (option number 41)
Additional conversational

languages

8

The machine manufacturer defines objects to be monitored

■

Three warning levels in manual operation

■

Program interrupt during automatic operation

■

Includes monitoring of 5-axis movements

■

Slovenian

■

Norwegian

■

Slovak

■

Latvian

■

Korean

■

Estonian

■

Turkish

■

Romanian

■

Lithuanian

■

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

TNC model, software and features

DXF Converter software option (option number 42)
Extracting contour

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

Adaptive Feed Control (AFC) software option (option number 45)
Function for adaptive feed-

rate control for optimizing
the machining conditions
during series production

KinematicsOpt software option (option number 48)
Touch-probe cycles for

automatic testing and
optimization of the machine
kinematics

Mill-Turning software option (option number 50)
Functions for milling/turning

mode

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

Recording the actual spindle power by means of a teach-in cut

■

Defining the limits of automatic feed rate control

■

Fully automatic feed control during program run

■

Backup/restore active kinematics

■

Test active kinematics

■

Optimize active kinematics

■

Switching between Milling/Turning mode of operation

■

Constant cutting speed

■

Tool-tip radius compensation

■

Turning cycles

■

Extended Tool Managment software option (option number 93)

Extended tool management, python-based

■

Remote Desktop Manager software option (option number 133)

Windows on a separate computer unitRemote operation of

■

external computer units
(e.g. Windows PC) via the
TNC user interface

Incorporated in the TNC interface

■

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

9

Fundamentals

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

TNC model, software and features

Compensation of axis
couplings

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

parameters

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

parameters

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

Fully automatic function for chatter control during machining

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

Automatic determination of workpiece weight and frictional forcesDynamic changing of control

■

Continuous adaptation of the parameters of the adaptive precontrolling

■

to the actual weight of the workpiece during machining

10

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

11

Fundamentals

TNC model, software and features

New functions

New functions 34059x-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 243).

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 ,
page 360).

The machine manufacturer can now define any areas on the
machine for collision monitoring (Dynamic Collision Monitoring
(software option), page 371).

Writing and reading data in freely definable tables (Freely definable
tables, page 402).

The Adaptive Feed Control (AFC) function has been integrated
(Adaptive Feed Control Software Option (AFC), page 377)

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 490).

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 389).

New manual probing cycle "Center line as datum" (Setting a center
line as datum , page 535).

New function for rounding corners (Rounding corners: M197,
page 366).

External access to the TNC can now be blocked with a MOD
function (External access, page 584).

12

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

TNC model, software and features

Modified functions 34059x-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 160).

The columns AFC and ACC were added to the tool table (Enter tool
data into the table, page 160).

Operation and position behavior of the manual probing cycles has
been improved (Using 3-D touch probes , page 514).

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

The status display has been expanded with the AFC tab (Additional
status displays, page 76).

The FUNCTION TURNDATA SPIN rotational function has been
expanded with an input option for maximum speed (Program
spindle speed, page 464).

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 528)

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

13

Fundamentals

TNC model, software and features

14

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

Contents

1 First Steps with the TNC 640......................................................................................................... 47

2 Introduction.......................................................................................................................................69

3 Programming: Fundamentals, file management...........................................................................89

4 Programming: Programming aids................................................................................................ 131

5 Programming: Tools....................................................................................................................... 155

6 Programming: Programming contours........................................................................................ 191

7 Programming: Data transfer from DXF files or plain-language contours................................. 243

8 Programming: Subprograms and program section repeats...................................................... 261

9 Programming: Q Parameters.........................................................................................................277

10 Programming: Miscellaneous functions.......................................................................................347

11 Programming: Special functions.................................................................................................. 367

12 Programming: Multiple Axis Machining...................................................................................... 409

13 Programming: Pallet editor........................................................................................................... 453

14 Programming: Turning Operations............................................................................................... 459

15 Manual operation and setup.........................................................................................................485

16 Positioning with Manual Data Input............................................................................................ 547

17 Test run and program run............................................................................................................. 553

18 MOD functions................................................................................................................................581

19 Tables and overviews.....................................................................................................................605

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

15

Contents

16

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

1 First Steps with the TNC 640......................................................................................................... 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..........................................................................................................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

Workpiece alignment with 3-D touch probe............................................................................................ 65

Datum setting with 3-D touch probe....................................................................................................... 66

1.7 Running the first program.................................................................................................................... 67

Selecting the correct operating mode..................................................................................................... 67

Choosing the program you want to run.................................................................................................. 67

Start the program.....................................................................................................................................67

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

17

Contents

2 Introduction.......................................................................................................................................69

2.1 The TNC 640........................................................................................................................................... 70

Programming: HEIDENHAIN conversational and ISO formats.................................................................70

Compatibility.............................................................................................................................................70

2.2 Visual display unit and operating panel..............................................................................................71

Display screen..........................................................................................................................................71

Setting the screen layout.........................................................................................................................71

Control Panel............................................................................................................................................72

2.3 Modes of Operation...............................................................................................................................73

Manual Operation and El. Handwheel.....................................................................................................73

Positioning with Manual Data Input.........................................................................................................73

Programming............................................................................................................................................ 73

Test Run................................................................................................................................................... 74

Program Run, Full Sequence and Program Run, Single Block.................................................................74

2.4 Status displays....................................................................................................................................... 75

"General" status display............................................................................................................................75

Additional status displays.........................................................................................................................76

2.5 Window Manager...................................................................................................................................83

Task bar.................................................................................................................................................... 84

2.6 SELinux security software.....................................................................................................................85

2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels.......................................86

3-D touch probes..................................................................................................................................... 86

HR electronic handwheels....................................................................................................................... 87

18

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

3 Programming: Fundamentals, file management...........................................................................89

3.1 Fundamentals......................................................................................................................................... 90

Position encoders and reference marks.................................................................................................. 90

Reference system.................................................................................................................................... 90

Reference system on milling machines...................................................................................................91

Designation of the axes on milling machines..........................................................................................91

Polar coordinates...................................................................................................................................... 92

Absolute and incremental workpiece positions....................................................................................... 93

Selecting the datum.................................................................................................................................94

3.2 Opening programs and entering.......................................................................................................... 95

Organization of an NC program in HEIDENHAIN Conversational format.................................................95

Define the blank: BLK FORM.................................................................................................................. 95

Opening a new part program.................................................................................................................. 96

Programming tool movements in conversational.....................................................................................97

Actual position capture.............................................................................................................................99

Editing a program...................................................................................................................................100

The TNC search function....................................................................................................................... 103

3.3 File manager: Fundamentals...............................................................................................................105

Files........................................................................................................................................................ 105

Displaying externally generated files on the TNC..................................................................................107

Data Backup........................................................................................................................................... 107

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

19

Contents

3.4 Working with the file manager.......................................................................................................... 108

Directories.............................................................................................................................................. 108

Paths.......................................................................................................................................................108

Overview: Functions of the file manager.............................................................................................. 109

Calling the file manager......................................................................................................................... 110

Selecting drives, directories and files....................................................................................................111

Creating a new directory....................................................................................................................... 112

Creating a new file.................................................................................................................................112

Copying a single file...............................................................................................................................112

Copying files into another directory.......................................................................................................113

Copying a table...................................................................................................................................... 114

Copying a directory................................................................................................................................ 115

Choosing one of the last files selected.................................................................................................115

Deleting a file.........................................................................................................................................116

Deleting a directory................................................................................................................................116

Tagging files........................................................................................................................................... 117

Renaming a file...................................................................................................................................... 118

Sorting files............................................................................................................................................ 118

Additional functions................................................................................................................................119

Additional tools for management of external file types.........................................................................120

Data transfer to/from an external data medium.................................................................................... 125

The TNC in a network............................................................................................................................127

USB devices on the TNC.......................................................................................................................128

20

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

4 Programming: Programming aids................................................................................................ 131

4.1 Adding comments................................................................................................................................132

Application.............................................................................................................................................. 132

Entering comments during programming..............................................................................................132

Inserting comments after program entry.............................................................................................. 132

Entering a comment in a separate block...............................................................................................132

Functions for editing of the comment...................................................................................................133

4.2 Display of NC Programs...................................................................................................................... 134

Syntax highlighting................................................................................................................................. 134

Scrollbar..................................................................................................................................................134

4.3 Structuring programs...........................................................................................................................135

Definition and applications..................................................................................................................... 135

Displaying the program structure window / Changing the active window.............................................135

Inserting a structuring block in the (left) program window.................................................................... 135

Selecting blocks in the program structure window............................................................................... 135

4.4 Calculator.............................................................................................................................................. 136

Operation................................................................................................................................................136

4.5 Programming graphics........................................................................................................................ 138

Generating / not generating graphics during programming................................................................... 138

Generating a graphic for an existing program....................................................................................... 138

Block number display ON/OFF...............................................................................................................139

Erasing the graphic................................................................................................................................ 139

Showing grid lines..................................................................................................................................139

Magnification or reduction of details..................................................................................................... 140

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

21

Contents

4.6 Error messages..................................................................................................................................... 141

Display of errors.....................................................................................................................................141

Open the error window......................................................................................................................... 141

Closing the error window...................................................................................................................... 141

Detailed error messages........................................................................................................................142

INTERNAL INFO soft key.......................................................................................................................142

Clearing errors........................................................................................................................................143

Error log..................................................................................................................................................143

Keystroke log..........................................................................................................................................144

Informational texts................................................................................................................................. 145

Saving service files................................................................................................................................ 145

Calling the TNCguide help system........................................................................................................ 146

4.7 TNCguide context-sensitive help system..........................................................................................147

Application.............................................................................................................................................. 147

Working with the TNCguide.................................................................................................................. 148

Downloading current help files.............................................................................................................. 152

22

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

5 Programming: Tools....................................................................................................................... 155

5.1 Entering tool-related data................................................................................................................... 156

Feed rate F.............................................................................................................................................156

Spindle speed S..................................................................................................................................... 157

5.2 Tool data................................................................................................................................................158

Requirements for tool compensation.................................................................................................... 158

Tool number, tool name......................................................................................................................... 158

Tool length L.......................................................................................................................................... 158

Tool radius R.......................................................................................................................................... 158

Delta values for lengths and radii.......................................................................................................... 159

Entering tool data into the program...................................................................................................... 159

Enter tool data into the table.................................................................................................................160

Importing tool tables..............................................................................................................................169

Pocket table for tool changer.................................................................................................................170

Call tool data.......................................................................................................................................... 173

Tool change............................................................................................................................................ 175

Tool usage test.......................................................................................................................................178

Tool management (software option)...................................................................................................... 180

5.3 Tool compensation............................................................................................................................... 187

Introduction.............................................................................................................................................187

Tool length compensation...................................................................................................................... 187

Tool radius compensation...................................................................................................................... 188

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

23

Contents

6 Programming: Programming contours........................................................................................ 191

6.1 Tool movements................................................................................................................................... 192

Path functions........................................................................................................................................ 192

FK free contour programming................................................................................................................192

Miscellaneous functions M....................................................................................................................192

Subprograms and program section repeats.......................................................................................... 193

Programming with Q parameters.......................................................................................................... 193

6.2 Fundamentals of Path Functions........................................................................................................194

Programming tool movements for workpiece machining......................................................................194

6.3 Approaching and departing a contour...............................................................................................198

Overview: Types of paths for contour approach and departure.............................................................198

Important positions for approach and departure....................................................................................199

Approaching on a straight line with tangential connection: APPR LT.................................................... 201

Approaching on a straight line perpendicular to the first contour point: APPR LN................................ 201

Approaching on a circular path with tangential connection: APPR CT...................................................202

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

LCT......................................................................................................................................................... 203

Departing in a straight line with tangential connection: DEP LT........................................................... 204

Departing in a straight line perpendicular to the last contour point: DEP LN........................................ 204

Departing on a circular path with tangential connection: DEP CT.........................................................205

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT...............205

6.4 Path contours - Cartesian coordinates...............................................................................................206

Overview of path functions................................................................................................................... 206

Straight line L.........................................................................................................................................207

Inserting a chamfer between two straight lines....................................................................................208

Corner rounding RND.............................................................................................................................209

24

Circle center CC..................................................................................................................................... 210

Circular path C around circle center CC................................................................................................ 211

Circle CR with defined radius................................................................................................................ 212

Circle CT with tangential connection.....................................................................................................214

Example: Linear movements and chamfers with Cartesian coordinates............................................... 215

Example: Circular movements with Cartesian coordinates................................................................... 216

Example: Full circle with Cartesian coordinates.................................................................................... 217

TNC 640 | User's Manual

HEIDENHAIN Conversational Programming | 5/2013

6.5 Path contours – Polar coordinates..................................................................................................... 218

Overview................................................................................................................................................ 218

Zero point for polar coordinates: pole CC..............................................................................................219

Straight line LP.......................................................................................................................................219

Circular path CP around pole CC........................................................................................................... 220

Circle CTP with tangential connection...................................................................................................220

Helix........................................................................................................................................................221

Example: Linear movement with polar coordinates.............................................................................. 223

Example: Helix........................................................................................................................................224

6.6 Path contours – FK free contour programming................................................................................ 225

Fundamentals......................................................................................................................................... 225

FK programming graphics...................................................................................................................... 227

Initiating the FK dialog........................................................................................................................... 229

Pole for FK programming....................................................................................................................... 229

Free straight line programming..............................................................................................................230

Free circular path programming............................................................................................................. 231

Input options.......................................................................................................................................... 232

Auxiliary points....................................................................................................................................... 235

Relative data...........................................................................................................................................236

Example: FK programming 1................................................................................................................. 238

Example: FK programming 2................................................................................................................. 239

Example: FK programming 3................................................................................................................. 240

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

25

Contents

7 Programming: Data transfer from DXF files or plain-language contours................................. 243

7.1 Processing DXF Files (Software Option)........................................................................................... 244

Application.............................................................................................................................................. 244

Opening a DXF file.................................................................................................................................245

Working with the DXF converter...........................................................................................................245

Basic settings.........................................................................................................................................246

Setting layers..........................................................................................................................................248

Defining the datum................................................................................................................................ 249

Selecting and saving a contour..............................................................................................................251

Selecting and saving machining positions............................................................................................. 255

26

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

8 Programming: Subprograms and program section repeats...................................................... 261

8.1 Labeling Subprograms and Program Section Repeats.................................................................... 262

Label....................................................................................................................................................... 262

8.2 Subprograms........................................................................................................................................ 263

Operating sequence...............................................................................................................................263

Programming notes................................................................................................................................263

Programming a subprogram...................................................................................................................263

Calling a subprogram............................................................................................................................. 264

8.3 Program-section repeats..................................................................................................................... 265

Label LBL............................................................................................................................................... 265

Operating sequence...............................................................................................................................265

Programming notes................................................................................................................................265

Programming a program section repeat................................................................................................ 265

Calling a program section repeat...........................................................................................................266

8.4 Any desired program as subprogram................................................................................................ 267

Operating sequence...............................................................................................................................267

Programming notes................................................................................................................................267

Calling any program as a subprogram................................................................................................... 268

8.5 Nesting.................................................................................................................................................. 269

Types of nesting.....................................................................................................................................269

Nesting depth.........................................................................................................................................269

Subprogram within a subprogram......................................................................................................... 270

Repeating program section repeats.......................................................................................................271

Repeating a subprogram........................................................................................................................272

8.6 Programming examples.......................................................................................................................273

Example: Milling a contour in several infeeds.......................................................................................273

Example: Groups of holes..................................................................................................................... 274

Example: Group of holes with several tools..........................................................................................275

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

27

Contents

9 Programming: Q Parameters.........................................................................................................277

9.1 Principle and overview of functions.................................................................................................. 278

Programming notes................................................................................................................................279

Calling Q parameter functions............................................................................................................... 280

9.2 Part families—Q parameters in place of numerical values.............................................................. 281

Application.............................................................................................................................................. 281

9.3 Describing contours with mathematical functions.......................................................................... 282

Application.............................................................................................................................................. 282

Overview................................................................................................................................................ 282

Programming fundamental operations...................................................................................................283

9.4 Angle functions (trigonometry)..........................................................................................................284

Definitions...............................................................................................................................................284

Programming trigonometric functions................................................................................................... 284

9.5 Calculation of circles............................................................................................................................285

Application.............................................................................................................................................. 285

9.6 If-then decisions with Q parameters................................................................................................. 286

Application.............................................................................................................................................. 286

Unconditional jumps...............................................................................................................................286

Programming if-then decisions.............................................................................................................. 286

Abbreviations used:................................................................................................................................287

9.7 Checking and changing Q parameters...............................................................................................288

Procedure............................................................................................................................................... 288

9.8 Additional functions.............................................................................................................................290

Overview................................................................................................................................................ 290

FN 14: ERROR: Displaying error messages...........................................................................................291

FN 16: F-PRINT: Output of formatted texts and Q parameter values.....................................................295

FN 18: SYS-DATUM READ: Reading system data................................................................................. 299

FN 19: PLC: Transfer values to PLC...................................................................................................... 308

FN 20: WAIT FOR: NC and PLC synchronization.................................................................................. 308

FN 29: PLC: Transfer values to the PLC................................................................................................310

FN 37: EXPORT......................................................................................................................................310

28

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

9.9 Accessing tables with SQL commands............................................................................................. 311

Introduction.............................................................................................................................................311

A transaction.......................................................................................................................................... 312

Programming SQL commands...............................................................................................................314

Overview of the soft keys..................................................................................................................... 314

SQL BIND...............................................................................................................................................315

SQL SELECT.......................................................................................................................................... 316

SQL FETCH............................................................................................................................................ 318

SQL UPDATE..........................................................................................................................................319

SQL INSERT...........................................................................................................................................319

SQL COMMIT........................................................................................................................................ 320

SQL ROLLBACK..................................................................................................................................... 320

9.10 Entering formulas directly...................................................................................................................321

Entering formulas...................................................................................................................................321

Rules for formulas..................................................................................................................................323

Programming example........................................................................................................................... 324

9.11 String parameters................................................................................................................................ 325

String processing functions................................................................................................................... 325

Assigning string parameters.................................................................................................................. 326

Chain-linking string parameters..............................................................................................................326

Converting a numerical value to a string parameter..............................................................................327

Copying a substring from a string parameter........................................................................................328

Converting a string parameter to a numerical value..............................................................................329

Checking a string parameter..................................................................................................................330

Finding the length of a string parameter...............................................................................................331

Comparing alphabetic sequence............................................................................................................332

Reading machine parameters.................................................................................................................333

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

29

Contents

9.12 Preassigned Q parameters.................................................................................................................. 336

Values from the PLC: Q100 to Q107.....................................................................................................336

Active tool radius: Q108.........................................................................................................................336

Tool axis: Q109.......................................................................................................................................336

Spindle status: Q110.............................................................................................................................. 337

Coolant on/off: Q111...............................................................................................................................337

Overlap factor: Q112.............................................................................................................................. 337

Unit of measurement for dimensions in the program: Q113.................................................................337

Tool length: Q114................................................................................................................................... 337

Coordinates after probing during program run.......................................................................................338

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

130..........................................................................................................................................................338

Tilting the working plane with mathematical angles: rotary axis coordinates calculated by the TNC.....338

Measurement results from touch probe cycles (see also User’s Manual for Cycle Programming)........339

9.13 Programming examples.......................................................................................................................341

Example: Ellipse..................................................................................................................................... 341

Example: Concave cylinder machined with spherical cutter..................................................................343

Example: Convex sphere machined with end mill.................................................................................345

30

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

10 Programming: Miscellaneous functions.......................................................................................347

10.1 Entering miscellaneous functions M and STOP................................................................................348

Fundamentals......................................................................................................................................... 348

10.2 M functions for program run inspection, spindle and coolant........................................................349

Overview................................................................................................................................................ 349

10.3 Miscellaneous functions for coordinate data....................................................................................350

Programming machine-referenced coordinates: M91/M92....................................................................350

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130.................... 352

10.4 Miscellaneous functions for path behavior.......................................................................................353

Machining small contour steps: M97.................................................................................................... 353

Machining open contour corners: M98..................................................................................................354

Feed rate factor for plunging movements: M103..................................................................................355

Feed rate in millimeters per spindle revolution: M136..........................................................................356

Feed rate for circular arcs: M109/M110/M111........................................................................................357

Calculating the radius-compensated path in advance (LOOK AHEAD): M120.......................................358

Superimposing handwheel positioning during program run: M118....................................................... 360

Retraction from the contour in the tool-axis direction: M140................................................................362

Suppressing touch probe monitoring: M141......................................................................................... 363

Deleting basic rotation: M143................................................................................................................364

Automatically retract tool from the contour at an NC stop: M148........................................................ 365

Rounding corners: M197........................................................................................................................366

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

31

Contents

11 Programming: Special functions.................................................................................................. 367

11.1 Overview of special functions............................................................................................................ 368

Main menu for SPEC FCT special functions......................................................................................... 368

Program defaults menu..........................................................................................................................369

Functions for contour and point machining menu................................................................................. 369

Menu of various conversational functions............................................................................................. 370

11.2 Dynamic Collision Monitoring (software option)..............................................................................371

Function..................................................................................................................................................371

Collision monitoring in the manual operating modes............................................................................ 373

Collision monitoring in Automatic operation.......................................................................................... 375

Graphic depiction of the protected space............................................................................................. 376

11.3 Adaptive Feed Control Software Option (AFC).................................................................................377

Application.............................................................................................................................................. 377

Defining the AFC basic settings............................................................................................................ 379

Recording a teach-in cut........................................................................................................................ 382

Activating/deactivating AFC....................................................................................................................385

Log file....................................................................................................................................................386

Tool breakage/tool wear monitoring.......................................................................................................387

Spindle load monitoring......................................................................................................................... 388

11.4 Active Chatter Control (ACC; software option).................................................................................389

Application.............................................................................................................................................. 389

Activating/deactivating ACC....................................................................................................................389

11.5 Working with the Parallel Axes U, V and W..................................................................................... 390

Overview................................................................................................................................................ 390

FUNCTION PARAXCOMP DISPLAY.......................................................................................................391

FUNCTION PARAXCOMP MOVE...........................................................................................................391

FUNCTION PARAXCOMP OFF.............................................................................................................. 392

FUNCTION PARAXMODE......................................................................................................................392

FUNCTION PARAXMODE OFF.............................................................................................................. 393

11.6 File functions........................................................................................................................................ 394

Application.............................................................................................................................................. 394

Defining file functions............................................................................................................................ 394

32

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

11.7 Definition of a datum shift..................................................................................................................395

Overview................................................................................................................................................ 395

TRANS DATUM AXIS............................................................................................................................. 395

TRANS DATUM TABLE.......................................................................................................................... 396

TRANS DATUM RESET..........................................................................................................................397

11.8 Creating Text Files................................................................................................................................398

Application.............................................................................................................................................. 398

Opening and exiting text files................................................................................................................398

Editing texts........................................................................................................................................... 399

Deleting and re-inserting characters, words and lines...........................................................................399

Editing text blocks..................................................................................................................................400

Finding text sections..............................................................................................................................401

11.9 Freely definable tables.........................................................................................................................402

Fundamentals......................................................................................................................................... 402

Creating a freely definable table............................................................................................................402

Editing the table format.........................................................................................................................403

Switching between table and form view...............................................................................................404

FN 26: TAPOPEN: Open a freely definable table.................................................................................. 405

FN 27: TAPWRITE: Write to a freely definable table.............................................................................406

FN 28: TAPREAD: Read from a freely definable table.......................................................................... 407

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

33

Contents

12 Programming: Multiple Axis Machining...................................................................................... 409

12.1 Functions for multiple axis machining.............................................................................................. 410

12.2 The PLANE Function: Tilting the Working Plane (Software Option 1)............................................411

Introduction.............................................................................................................................................411

Defining the PLANE function.................................................................................................................413

Position display.......................................................................................................................................413

Resetting the PLANE function............................................................................................................... 414

Defining the working plane with the spatial angle: PLANE SPATIAL.................................................... 415

Defining the working plane with the projection angle: PLANE PROJECTED........................................ 417

Defining the working plane with the Euler angle: PLANE EULER.........................................................418

Defining the working plane with two vectors: PLANE VECTOR........................................................... 420

Defining the working plane via three points: PLANE POINTS...............................................................422

Defining the working plane via a single incremental spatial angle: PLANE SPATIAL.............................424

Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)...................................... 425

Specifying the positioning behavior of the PLANE function..................................................................427

12.3 Inclined-tool machining in a tilted machining plane (software option 2).......................................432

Function..................................................................................................................................................432

Inclined-tool machining via incremental traverse of a rotary axis.......................................................... 432

Inclined-tool machining via normal vectors............................................................................................433

12.4 Miscellaneous functions for rotary axes........................................................................................... 434

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1)............................................... 434

Shortest-path traverse of rotary axes: M126.........................................................................................435

Reducing display of a rotary axis to a value less than 360°: M94.........................................................436

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

2).............................................................................................................................................................437

Selecting tilting axes: M138...................................................................................................................440

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

M144 (software option 2)...................................................................................................................... 441

12.5 FUNCTION TCPM (software option 2)............................................................................................... 442

Function..................................................................................................................................................442

Defining the TCPM FUNCTION............................................................................................................. 442

Mode of action of the programmed feed rate...................................................................................... 443

Interpretation of the programmed rotary axis coordinates....................................................................443

Type of interpolation between the starting and end position................................................................ 445

Resetting the TCPM FUNCTION........................................................................................................... 446

34

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

12.6 Three-dimensional tool compensation (software option 2)............................................................ 447

Introduction.............................................................................................................................................447

Definition of a normalized vector...........................................................................................................448

Permitted tool shapes............................................................................................................................ 449

Using other tools: Delta values............................................................................................................. 449

3-D compensation without TCPM......................................................................................................... 449

Face Milling: 3D compensation with TCPM.......................................................................................... 450

Peripheral Milling: 3-D radius compensation with TCPM and radius compensation (RL/RR)................. 451

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

35

Contents

13 Programming: Pallet editor........................................................................................................... 453

13.1 Pallet Management.............................................................................................................................. 454

Application.............................................................................................................................................. 454

Select pallet table.................................................................................................................................. 456

Exiting the pallet file.............................................................................................................................. 456

Run pallet file......................................................................................................................................... 456

36

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

14 Programming: Turning Operations............................................................................................... 459

14.1 Turning Operations on Milling Machines (Software Option 50)......................................................460

Introduction.............................................................................................................................................460

14.2 Basis Functions (Software Option 50)............................................................................................... 461

Switching between milling/turning mode of operation.......................................................................... 461

Graphical display of turning operations..................................................................................................463

Program spindle speed.......................................................................................................................... 464

Feed rate................................................................................................................................................ 465

Tool call...................................................................................................................................................465

Tool compensation in the program........................................................................................................ 466

Tool data................................................................................................................................................. 467

Tool tip radius compensation TRC......................................................................................................... 472

Recessing and undercutting...................................................................................................................473

Inclined turning.......................................................................................................................................479

14.3 Unbalance Functions........................................................................................................................... 481

Unbalance while turning........................................................................................................................ 481

Measure Unbalance cycle......................................................................................................................483

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

37

Contents

15 Manual operation and setup.........................................................................................................485

15.1 Switch-on, switch-off...........................................................................................................................486

Switch-on................................................................................................................................................486

Switch-off................................................................................................................................................488

15.2 Moving the machine axes...................................................................................................................489

Note........................................................................................................................................................489

Moving the axis with the machine axis direction buttons..................................................................... 489

Incremental jog positioning....................................................................................................................489

Traverse with electronic handwheels.....................................................................................................490

15.3 Spindle speed S, feed rate F and miscellaneous function M.......................................................... 500

Application.............................................................................................................................................. 500

Entering values.......................................................................................................................................500

Adjusting spindle speed and feed rate.................................................................................................. 501

Activating feed-rate limitation................................................................................................................ 501

15.4 Functional safety FS (option)..............................................................................................................502

Miscellaneous.........................................................................................................................................502

Explanation of terms.............................................................................................................................. 503

Checking the axis positions................................................................................................................... 504

Overview of permitted feed rates and speeds......................................................................................505

Activating feed-rate limitation................................................................................................................ 505

Additional status displays.......................................................................................................................506

15.5 Datum setting without a 3-D touch probe........................................................................................507

Note........................................................................................................................................................507

Preparation..............................................................................................................................................507

Workpiece presetting with axis keys.....................................................................................................507

Datum management with the preset table........................................................................................... 508

15.6 Using 3-D touch probes.......................................................................................................................514

Overview................................................................................................................................................ 514

Functions in touch probe cycles............................................................................................................ 516

Selecting touch probe cycles.................................................................................................................518

Recording measured values from the touch-probe cycles.....................................................................519

Writing measured values from the touch probe cycles in a datum table.............................................. 520

Writing measured values from the touch probe cycles in the preset table........................................... 521

38

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

15.7 Calibrating a 3-D touch trigger probe................................................................................................522

Introduction.............................................................................................................................................522

Calibrating the effective length.............................................................................................................. 523

Calibrating the effective radius and compensating center misalignment.............................................. 524

Displaying calibration values.................................................................................................................. 526

15.8 Compensating workpiece misalignment with 3-D touch probe......................................................527

Introduction.............................................................................................................................................527

Identifying basic rotation........................................................................................................................528

Saving a basic rotation in the preset table............................................................................................528

Compensation of workpiece misalignment by rotating the table..........................................................528

Displaying a basic rotation..................................................................................................................... 529

Canceling a basic rotation......................................................................................................................529

15.9 Datum Setting with 3-D Touch Probe................................................................................................530

Overview................................................................................................................................................ 530

Datum setting in any axis...................................................................................................................... 530

Corner as datum.................................................................................................................................... 531

Circle center as datum...........................................................................................................................533

Setting a center line as datum...............................................................................................................535

Measuring workpieces with a 3-D touch probe.....................................................................................536

Using touch probe functions with mechanical probes or measuring dials.............................................539

15.10 Tilting the working plane (software option 1)..................................................................................540

Application, function...............................................................................................................................540

Traversing reference points in tilted axes.............................................................................................. 542

Position display in a tilted system......................................................................................................... 542

Limitations on working with the tilting function....................................................................................542

To activate manual tilting:...................................................................................................................... 543

Setting the current tool-axis direction as the active machining direction...............................................544

Setting the datum in a tilted coordinate system................................................................................... 545

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

39

Contents

16 Positioning with Manual Data Input............................................................................................ 547

16.1 Programming and executing simple machining operations............................................................548

Positioning with manual data input (MDI)............................................................................................. 548

Protecting and erasing programs in $MDI.............................................................................................551

40

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

17 Test run and program run............................................................................................................. 553

17.1 Graphics.................................................................................................................................................554

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

Speed of the Setting test runs.............................................................................................................. 555

Overview: Display modes...................................................................................................................... 556

Plan view................................................................................................................................................557

Projection in three planes...................................................................................................................... 557

3-D view................................................................................................................................................. 558

Magnifying details.................................................................................................................................. 560

Repeating graphic simulation.................................................................................................................561

Tool display.............................................................................................................................................561

Measurement of machining time...........................................................................................................562

3-D line graphics.................................................................................................................................... 563

17.2 Showing the workpiece blank in the working space.......................................................................565

Application.............................................................................................................................................. 565

17.3 Functions for program display............................................................................................................566

Overview................................................................................................................................................ 566

17.4 Test Run.................................................................................................................................................567

Application.............................................................................................................................................. 567

17.5 Program run..........................................................................................................................................570

Application.............................................................................................................................................. 570

Running a part program......................................................................................................................... 571

Interrupt machining................................................................................................................................ 572

Moving the machine axes during an interruption.................................................................................. 573

Resuming program run after an interruption......................................................................................... 573

Any entry into program (mid-program startup)......................................................................................575

Returning to the contour........................................................................................................................577

17.6 Automatic program start.....................................................................................................................578

Application.............................................................................................................................................. 578

17.7 Optional block skip.............................................................................................................................. 579

Application.............................................................................................................................................. 579

Inserting the "/" character.......................................................................................................................579

Erasing the "/" character......................................................................................................................... 579

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

41

Contents

17.8 Optional program-run interruption.....................................................................................................580

Application.............................................................................................................................................. 580

42

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

18 MOD functions................................................................................................................................581

18.1 MOD function....................................................................................................................................... 582

Selecting MOD functions.......................................................................................................................582

Changing the settings............................................................................................................................ 582

Exiting MOD functions...........................................................................................................................582

Overview of MOD functions..................................................................................................................583

18.2 Machine settings.................................................................................................................................. 584

External access...................................................................................................................................... 584

Select kinematics................................................................................................................................... 586

18.3 Position Display Types......................................................................................................................... 587

Application.............................................................................................................................................. 587

18.4 Unit of Measurement...........................................................................................................................588

Application.............................................................................................................................................. 588

18.5 Displaying operating times................................................................................................................. 588

Application.............................................................................................................................................. 588

18.6 Software numbers................................................................................................................................589

Application.............................................................................................................................................. 589

18.7 Entering the code number.................................................................................................................. 589

Application.............................................................................................................................................. 589

18.8 Setting up data interfaces...................................................................................................................590

Serial interfaces on the TNC 640.......................................................................................................... 590

Application.............................................................................................................................................. 590

Setting the RS-232 interface..................................................................................................................590

Setting the BAUD RATE (baudRate)...................................................................................................... 590

Setting the protocol (protocol)............................................................................................................... 591

Setting data bits (dataBits).....................................................................................................................591

Check parity (parity)............................................................................................................................... 591

Setting the stop bits (stopBits)..............................................................................................................591

Setting handshaking (flowControl)......................................................................................................... 592

File system for file operations (fileSystem)........................................................................................... 592

Settings for data transfer with the TNCserver PC software..................................................................592

Setting the operating mode of the external device (fileSystem)........................................................... 593

Data transfer software........................................................................................................................... 594

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

43

Contents

18.9 Ethernet interface.................................................................................................................................596

Introduction.............................................................................................................................................596

Connection options................................................................................................................................ 596

Configuring the TNC.............................................................................................................................. 596

18.10 Configure HR 550 FS wireless handwheel........................................................................................ 602

Application.............................................................................................................................................. 602

Assigning the handwheel to a specific handwheel holder.................................................................... 602

Setting the transmission channel...........................................................................................................603

Selecting the transmitter power............................................................................................................ 603

Statistical data........................................................................................................................................604

44

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

19 Tables and overviews.....................................................................................................................605

19.1 Machine-specific user parameters......................................................................................................606

Application.............................................................................................................................................. 606

19.2 Connector pin layout and connection cables for data interfaces....................................................616

RS-232-C/V.24 interface for HEIDENHAIN devices................................................................................616

Non-HEIDENHAIN devices.....................................................................................................................618

Ethernet interface RJ45 socket............................................................................................................. 618

19.3 Technical Information...........................................................................................................................619

19.4 Overview tables....................................................................................................................................627

Fixed cycles............................................................................................................................................627

Miscellaneous functions.........................................................................................................................628

19.5 Functions of the TNC 640 and the iTNC 530 compared.................................................................. 630

Comparison: Specifications....................................................................................................................630

Comparison: Data interfaces..................................................................................................................630

Comparison: Accessories.......................................................................................................................631

Comparison: PC software...................................................................................................................... 631

Comparison: Machine-specific functions............................................................................................... 632

Comparison: User functions.................................................................................................................. 632

Comparison: Cycles................................................................................................................................639

Comparison: Miscellaneous functions................................................................................................... 641

Comparison: Touch probe cycles in the Manual Operation and El. Handwheel modes.........................643

Comparison: Touch probe cycles for automatic workpiece inspection.................................................. 644

Comparison: Differences in programming............................................................................................. 645

Comparison: Differences in Test Run, functionality............................................................................... 649

Comparison: Differences in Test Run, operation................................................................................... 649

Comparison: Differences in Manual Operation, functionality................................................................ 649

Comparison: Differences in Manual Operation, operation.....................................................................651

Comparison: Differences in Program Run, operation............................................................................ 651

Comparison: Differences in Program Run, traverse movements...........................................................652

Comparison: Differences in MDI operation........................................................................................... 656

Comparison: Differences in programming station................................................................................. 657

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

45

1

First Steps with

the TNC 640

1

First Steps with the TNC 640

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 control and machine. The TNC
starts the operating system. This process may take several
minutes. Then the TNC will display the message "Power
interrupted" in the screen header

Press the CE key: The TNC compiles the PLC
program

Switch on the 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 axis press the
machine START button. 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 486
Operating modes: See "Programming", page 73

48

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

1.3 Programming the first part

Selecting the correct operating mode

You can write programs only in Programming mode:

Press the Programming operating mode key: The
TNC switches to Programming mode

Further information on this topic

Operating modes: See "Programming", page 73

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 100

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

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

49

1

First Steps with the TNC 640

1.3 Programming the first part

Creating a new program/file management

Press the PGM MGT key: The TNC opens the
file manager. 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 a file name with the extension .H: The TNC
then automatically opens a program and asks for
the unit of measure for the new program

To select the unit of measure, press the MM
or INCH soft key: The TNC automatically starts
the workpiece blank definition (See "Defining a
workpiece blank", page 51)

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 108

Creating a new program: See "Opening programs and entering",
page 95

50

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

Programming the first part 1.3

Defining a workpiece blank

Immediately after you have created a new program, the TNC starts
the dialog for entering the workpiece blank definition. Always
define the workpiece blank as a cuboid by entering the MIN and
MAX points, each with reference to the selected reference point.

After you have created a new program, 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

1

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

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

Defining the workpiece blank: page 96

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

51

1

First Steps with the TNC 640

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", page 192

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 | 5/2013

TNC 640 | User's Manual

Programming the first part 1.3

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.
Confirm with the ENT key

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation

1

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

Confirm the Miscellaneous function M? with
theEND key: The TNC saves the entered
positioning block

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

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

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation

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

Confirm the Miscellaneous function M? with the
END key: The TNC saves the entered positioning
block

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

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the 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. Confirm with the END key:
The TNC saves the entered positioning block

Move to the contour: Press the APPR/DEP key:
The TNC shows a soft-key row with approach and
departure functions

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

53

1

First Steps with the TNC 640

1.3 Programming the first part

Select the approach function APPR CT: Enter the
coordinates 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

Confirm the Radius comp.: RL/RR/no comp? with
the RL soft key: Activate the 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 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

Move to contour point 3: Enter the X coordinate 95
and save your entry with the END key

Define the chamfer at contour point 3: Enter the
chamfer width 10 mm and save with the END key

Move to contour point 4: Enter the Y coordinate 5
and save your entry with the END key

Define the chamfer at contour point 4: Enter the
chamfer width 20 mm and save with the END key

Move to contour point 1: Enter the X coordinate 5
and save your entry with the END key

Depart the contour

54

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, with the END key: The TNC saves the
entered positioning block

TNC 640 | User's Manual

HEIDENHAIN Conversational Programming | 5/2013

Enter 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.
Confirm with the ENT key

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation

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

MISCELLANEOUS FUNCTION M? ENTER M2 to end
the program and 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 215

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

page 95

Approaching/departing contours: See " Approaching and

departing a contour", page 198

Programming contours: See "Overview of path functions",

page 206

Programmable feed rates: See "Mögliche Vorschubeingaben"

Tool radius compensation: See "Tool radius compensation",

page 188

Miscellaneous functions (M): See "M functions for program run

inspection, spindle and coolant ", page 349

1

Programming the first part 1.3

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

55

1

First Steps with the TNC 640

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 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.
Confirm with the ENT key

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation

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

Confirm the Miscellaneous function M? with
theEND key: The TNC saves the entered
positioning block

Call the cycle menu

Display the drilling cycles

Select the 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

56

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. Confirm with the END key:
The TNC saves the entered positioning block

TNC 640 | User's Manual

HEIDENHAIN Conversational Programming | 5/2013

Enter 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.
Confirm with the ENT key

Confirm Radius comp.: RL/RR/no comp? by
pressing the ENT key: Do not activate the radius
compensation

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

Miscellaneous function M? Enter M2 to end the
program and confirm with the END key: The TNC
saves 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 ;PLUNGING DEPTH

Q210=0 ;DWELL TIME AT TOP

Q203=-10 ;SURFACE COORDINATE

Q204=20 ;2ND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT BOTTOM

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 95

Cycle programming: See User’s Manual for Cycles

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

57

1

First Steps with the TNC 640

1.4 Graphically testing the first part

1.4 Graphically testing the first part

Selecting the correct operating mode

You can test programs only in the Test Run mode:

Press the Test Run operating mode key: the TNC
switches to that mode

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 73

Testing programs: See "Test Run", page 567

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
manager

Press the SELECT TYPE soft key: The TNC shows
a soft-key menu for selection of the file type to be
displayed

Press the SHOW ALL 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 manager

Further information on this topic

Tool management: See "Enter tool data into the table",

page 160

Testing programs: See "Test Run", page 567

58

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

Choosing the program you want to test

Press the PGM MGT key: The TNC opens the file
manager

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 108

Selecting the screen layout and the view

1

Graphically testing the first part 1.4

Press the key for selecting the screen layout. The
TNC shows all available alternatives in the soft-key
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

Select the desired view via soft key
Plan view

Projection in three planes

3-D view

Further information on this topic

Graphic functions: See "Graphics ", page 554

Running a test run: See "Test Run", page 567

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

59

1

First Steps with the TNC 640

1.4 Graphically testing the first part

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 a break

Further information on this topic

Running a test run: See "Test Run", page 567

Graphic functions: See "Graphics ", page 554

Adjusting the test speed: See "Speed of the Setting test runs",

page 555

60

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

1.5 Setting up tools

Selecting the correct operating mode

Tools are set up in the Manual Operation mode:

Press the Manual Operation operating mode key:
the TNC switches to that mode

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 73

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: Place the tools into the tool

changer page 63

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

61

1

First Steps with the TNC 640

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 73

Working with the tool table: See "Enter tool data into the table",

page 160

62

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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:

Display the tool table

Display the pocket table
Edit the pocket table: Set the EDITING soft key to

ON

1

Setting up tools 1.5

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

To leave the pocket table, press the END key

Further information on this topic

Operating modes of the TNC: See "Modes of Operation",

page 73

Working with the pocket table: See "Pocket table for tool

changer", page 170

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

63

1

First Steps with the TNC 640

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 Manual Operation operating mode key:
the TNC switches to that mode

Further information on this topic

Manual Operation mode: See "Moving the machine axes",

page 489

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 | 5/2013

TNC 640 | User's Manual

Workpiece alignment with 3-D touch probe

Insert the 3-D touch probe: In the Manual Data Input (MDI)

operating mode, run a TOOL CALL block containing the tool axis,

and then return to the Manual Operation mode (in MDI mode

you can run an individual NC block independently of the others)

Select the probing functions: The TNC displays the
available functions in the soft-key row

Measure the basic rotation: The TNC displays the
basic rotation menu. To identify the basic rotation,
probe two points on a straight surface of the
workpiece

Use the axis-direction keys to preposition the
touch probe to a position near the first contact
point

Select the probing direction via soft key

1

Workpiece setup 1.6

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 preposition the
touch probe to a position near the second contact
point

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 measured basic rotation
Press SET BASIC ROTATION soft key to select the

displayed value as the active rotation. Press the
END soft key to exit the menu

Further information on this topic

MDI operating mode: See "Programming and executing simple

machining operations", page 548

Workpiece alignment: See "Compensating workpiece

misalignment with 3-D touch probe ", page 527

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

65

1

First Steps with the TNC 640

1.6 Workpiece setup

Datum setting with 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 the
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: 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: 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: 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: 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

Set to 0: Press the SET DATUM soft key
Press the END soft key to close the menu

Further information on this topic

Datum setting: See "Datum Setting with 3-D Touch Probe ",

page 530

66

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

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 Program Run, Full Sequence operating
mode key: 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 73

Running programs: See "Program run", page 570

1

Running the first program 1.7

Choosing the program you want to run

Press the PGM MGT key: The TNC opens the file
manager

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 108

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 570

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

67

2

Introduction

2

Introduction

2.1 The TNC 640

2.1 The TNC 640

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 18 axes. You
can also change the angular position of the spindle under program
control.

An integrated hard disk provides storage for as many programs as
you like, even if they were created off-line. For quick calculations
you can call up the on-screen pocket calculator at any time.

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 640.
If NC blocks contain invalid elements, the TNC will mark them as
ERROR blocks when the file is opened.

See "Functions of the and the iTNC 530 compared".
Please also note the detailed description of the
differences between the iTNC 530 and the TNC 640

70

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

1

7

7

2

5

4

3

4

6

8

Visual display unit and operating panel 2.2

2.2 Visual display unit and operating panel

Display screen

The TNC is shipped with a 19-inch TFT 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

2

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

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

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

71

2

2

3

4

5

8
9

6

7

10

1

Introduction

2.2 Visual display unit and operating panel

Control Panel

The TNC 640 is delivered with an integrated keyboard. The figure to
the right shows the operating elements of the operating panel:

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 Navigation keys and GOTO jump command
7 Numerical input and axis selection
8 Touchpad
9 Mouse function keys
10 USB connection

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

File management
Calculator
MOD function
HELP function

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.

72

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

73

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.

Soft keys for selecting the screen layout: See "Program Run, Full
Sequence and Program Run, Single Block", page 74.

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

Graphics

Window Soft key

Pallet table

Left: program, right: pallet table

Left: pallet table, right: status

74

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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
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

2

Status displays 2.4

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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

75

2

Introduction

2.4 Status displays

Icon Meaning

Program run has started

Program run is stopped

Program run is being aborted

Turning mode is active

The Dynamic Collision Monitoring function (DCM)
is active

The Adaptive Feed Function (AFC) 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 and Editing mode of operation.

To switch on the additional status display:

Call the soft-key row for screen layout

Select the screen layout with 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.

Please note that some of the status information
described below is not available unless the
associated software option is enabled on your TNC.

76

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

77

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

78

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

79

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

80

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

81

2

Introduction

2.4 Status displays

Adaptive Feed Control (AFC tab, software option)

The TNC displays the AFC tab only if the function is
active on your machine.

Soft key Meaning

No direct
selection
possible

Active tool (number and name)

Cut number
Current factor of the feed potentiomenter in

percent
Active spindle load in percent
Reference load of the spindle
Current spindle speed
Current deviation of the speed
Current machining time
Line diagram, in which the current spindle load

and the value commanded by the TNC for the
feed-rate override are shown

82

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

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.

2

Window Manager 2.5

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.

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

83

2

Introduction

2.5 Window Manager

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 MP 7230

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

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 105

84

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

SELinux security software 2.6

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.

2

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.

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

85

2

Introduction

2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

Handwheels

2.7 Accessories: HEIDENHAIN 3-D Touch

Probes and Electronic Handwheels

3-D touch probes

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: 892905-xx

TS 220, TS 440, TS 444, TS 640 und TS 740 touch trigger probes

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

86

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual

2

Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

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.

2.7

Handwheels

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

87

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.

90

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 can control up to 18 axes optionally. 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

91

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

92

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

93

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.

94

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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

3

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

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

Define the blank: BLK FORM

Immediately after initiating a new program, you define a cuboid
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. This definition is needed for the
TNC’s graphic simulation feature. The sides of the workpiece blank
lie parallel to the X, Y and Z axes and can be up to 100 000 mm
long. The workpiece 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

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

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

95

3

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

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.

Select the unit of measure: Press the MM or INCH
soft key. The TNC switches the screen layout and
initiates the dialog for defining the BLK FORM
(workpiece blank)

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

96

If you do not wish to define a blank form, cancel the
dialog at Working plane in graphic: XY by pressing
the DEL key.

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

TNC 640 | User's Manual

HEIDENHAIN Conversational Programming | 5/2013

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.

If you enter DIN/ISO functions via a connected USB
keyboard, make sure that capitalization is active.

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").

The TNC ends this dialog by pressing the ENT key.

The program-block window displays the following line:

3 L X+10 Y+5 R0 F100 M3

TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

97

3

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 199)

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

98

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | 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 the actual-position-capture function: In the
soft-key row the TNC displays the axes whose
positions can be transferred

Select the axis: The TNC writes the current
position of the selected axis into the active input
box

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 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013

99

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

100

HEIDENHAIN Conversational Programming | 5/2013

TNC 640 | User's Manual