HEIDENHAIN TNC 640 User Manual

TNC 640

User’s Manual
DIN/ISO Programming

NC Software
340590-04
340591-04
340595-04

English (en)
3/2014

Controls of the TNC

Controls of the TNC

Keys on visual display unit

Key Function

Select split screen layout

Toggle the display between
machining and programming
modes

Soft keys for selecting functions on
screen

Shifting between soft-key rows

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

NO

ENT

Cycles, subprograms and program section repeats

Key Function

Define touch probe cycles

Define and call cycles

Enter and call labels for
subprogramming and program
section repeats

Enter program stop in a program

Tool functions

Key Function

Define tool data in the program

Call tool data

Special functions

Key Function

Show special functions

Select the next tab in forms

Up/down one dialog box or button

Entering and editing coordinate axes and numbers

Key Function

Select coordinate axes or enter

. . .

. . .

them in a program

Numbers

Decimal point / Reverse algebraic
sign

Programming path movements

Key Function

Approach/depart contour

FK free contour programming

Straight line

Circle center/pole for polar
coordinates

Circular arc with center

Circle with radius

Circular arc with tangential
connection

Chamfer/Corner rounding

Polar coordinate input /
Incremental values

Q-parameter programming/
Q-parameter status

Save actual position or values from
calculator

Skip dialog questions, delete
words

Confirm entry and resume dialog

Conclude block and exit entry

Clear numerical entry or TNC error
message

Abort dialog, delete program
section

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

3

Controls of the TNC

4

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Fundamentals

Fundamentals

About this manual

About this manual

The symbols used in this manual are described below.

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

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

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

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

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

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

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

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

6

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 340590-04

TNC 640 E 340591-04

TNC 640 Programming Station 340595-04

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 for DIN/ISO Programming | 3/2014

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:

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 down 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

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

■

8

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 feed­rate 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

Synchronizing Functions software option (option number 135)

Real Time Coupling (RTC)

Incorporated in the TNC interface

■

Coupling of axes

■

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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 229).

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 340).

The machine manufacturer can now define any areas on the
machine for collision monitoring ("Dynamic Collision Monitoring
(software option)", page 351).

Writing and reading data in freely definable tables ("Freely definable
tables", page 377).

The Adaptive Feed Control (AFC) function has been integrated
("Adaptive Feed Control Software Option (AFC)", page 357)

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 458).

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 370).

New manual probing cycle "Center line as datum" ("Setting a center
line as datum ", page 503).

New function for rounding corners ("Rounding corners: M197",
page 346).

External access to the TNC can now be blocked with a MOD
function ("External access", page 553).

12

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

TNC model, software and features

New 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 164).

The columns AFC and ACC were added to the tool table ("Enter tool
data into the table", page 164).

Operation and position behavior of the manual probing cycles has
been improved ("Using 3-D touch probes ", page 482).

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 turning function has been
expanded with an input option for maximum speed ("Program
spindle speed", page 432).

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 496)

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

13

Fundamentals

TNC model, software and features

New functions 34059x-04

New special operating mode Retraction ("Retraction after a power
interruption", page 540).

New graphic simulation ("Graphics ", page 522).
New MOD function "tool usage file" within the machine settings

group ("Tool usage file", page 555).
New MOD function "set system time" within the systems settings

group ("Set the system time", page 557).
New MOD group "graphic settings" ("Graphic settings",

page 552).
With the new syntax for the adaptive feed control (AFC) you

can start or end a teach-in step ("Recording a teach-in cut",
page 362).

With the new cutting data calculator you can calculate the spindle
speed and the feed rate ("Cutting data calculator", page 139).

In the TURNDATA function, you can now define the effect of
the tool compensation ("Tool compensation in the program",
page 434).

Now you can activate and deactivate the active chatter
compensation (ACC) by soft key ("Activating/deactivating ACC",
page 371).

New if/then decisions were introduced in the jump commands
("Programming if-then decisions", page 271).

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

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

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

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

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

14

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

TNC model, software and features

Changed functions 34059x-04

The turning tool table was expanded by the column NAME ("Tool
data", page 435).

Now up to 4 functions are allowed in an NC block ("Fundamentals",
page 328).

New soft keys for value transfer have been introduced in the pocket
calculator ("Operation", page 136).

The distance-to-go display can now also be displayed in the input
system ("Position Display Types", page 558).

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

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

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

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

15

Fundamentals

TNC model, software and features

16

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Contents

1 First Steps with the TNC 640....................................................................................................... 49

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

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

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

5 Programming: Tools..................................................................................................................... 159

6 Programming: Programming contours...................................................................................... 195

7 Programming: Data transfer from DXF files or plain-language contours............................... 229

8 Programming: Subprograms and program section repeats.................................................... 247

9 Programming: Q Parameters.......................................................................................................263

10 Programming: Miscellaneous functions.....................................................................................327

11 Programming: Special functions.................................................................................................347

12 Programming: Multiple Axis Machining.................................................................................... 383

13 Programming: Pallet editor......................................................................................................... 421

14 Programming: Turning Operations............................................................................................. 427

15 Manual operation and setup.......................................................................................................453

16 Positioning with Manual Data Input.......................................................................................... 515

17 Test run and program run........................................................................................................... 521

18 MOD functions..............................................................................................................................549

19 Tables and overviews...................................................................................................................579

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

17

Contents

18

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

1 First Steps with the TNC 640....................................................................................................... 49

1.1 Overview................................................................................................................................................ 50

1.2 Machine switch-on................................................................................................................................50

Acknowledging the power interruption and moving to the reference points..........................................50

1.3 Programming the first part..................................................................................................................51

Selecting the correct operating mode.................................................................................................... 51

The most important TNC keys................................................................................................................51

Creating a new program/file management............................................................................................. 52

Defining a workpiece blank.................................................................................................................... 53

Program layout........................................................................................................................................ 54

Programming a simple contour...............................................................................................................55

Creating a cycle program........................................................................................................................ 57

1.4 Graphically testing the first part.........................................................................................................59

Selecting the correct operating mode.................................................................................................... 59

Selecting the tool table for the test run.................................................................................................59

Choosing the program you want to test................................................................................................ 60

Selecting the screen layout and the view.............................................................................................. 60

Starting the test run................................................................................................................................61

1.5 Setting up tools.................................................................................................................................... 62

Selecting the correct operating mode.................................................................................................... 62

Preparing and measuring tools............................................................................................................... 62

The tool table TOOL.T............................................................................................................................ 63

The pocket table TOOL_P.TCH................................................................................................................64

1.6 Workpiece setup....................................................................................................................................65

Selecting the correct operating mode.................................................................................................... 65

Clamping the workpiece......................................................................................................................... 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 for DIN/ISO Programming | 3/2014

19

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

20

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 DIN/ISO format................................................................................ 95

Define the blank: G30/G31..................................................................................................................... 96

Opening a new part program................................................................................................................. 97

Programming tool movements in DIN/ISO............................................................................................. 99

Actual position capture..........................................................................................................................100

Editing a program..................................................................................................................................101

The TNC search function...................................................................................................................... 104

3.3 File manager: Fundamentals..............................................................................................................106

Files....................................................................................................................................................... 106

Displaying externally generated files on the TNC.................................................................................108

Data Backup.......................................................................................................................................... 108

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

21

Contents

3.4 Working with the file manager......................................................................................................... 109

Directories............................................................................................................................................. 109

Paths......................................................................................................................................................109

Overview: Functions of the file manager............................................................................................. 110

Calling the file manager........................................................................................................................ 111

Selecting drives, directories and files...................................................................................................112

Creating a new directory...................................................................................................................... 113

Creating a new file................................................................................................................................113

Copying a single file..............................................................................................................................113

Copying files into another directory......................................................................................................114

Copying a table..................................................................................................................................... 115

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

Choosing one of the last files selected................................................................................................116

Deleting a file........................................................................................................................................117

Deleting a directory...............................................................................................................................117

Tagging files.......................................................................................................................................... 118

Renaming a file..................................................................................................................................... 119

Sorting files........................................................................................................................................... 119

Additional functions...............................................................................................................................120

Additional tools for management of external file types........................................................................121

Data transfer to/from an external data medium................................................................................... 126

The TNC in a network.......................................................................................................................... 128

USB devices on the TNC......................................................................................................................129

22

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 Cutting data calculator.......................................................................................................................139

Application............................................................................................................................................. 139

4.6 Programming graphics....................................................................................................................... 142

Generate/do not generate graphics during programming.....................................................................142

Generating a graphic for an existing program...................................................................................... 142

Block number display ON/OFF..............................................................................................................143

Erasing the graphic............................................................................................................................... 143

Showing grid lines.................................................................................................................................143

Magnification or reduction of details.................................................................................................... 144

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

23

Contents

4.7 Error messages.................................................................................................................................... 145

Display of errors....................................................................................................................................145

Open the error window........................................................................................................................ 145

Closing the error window..................................................................................................................... 145

Detailed error messages.......................................................................................................................146

INTERNAL INFO soft key......................................................................................................................146

Clearing errors.......................................................................................................................................147

Error log.................................................................................................................................................147

Keystroke log.........................................................................................................................................148

Informational texts................................................................................................................................ 149

Saving service files............................................................................................................................... 149

Calling the TNCguide help system....................................................................................................... 150

4.8 TNCguide context-sensitive help system.........................................................................................151

Application............................................................................................................................................. 151

Working with the TNCguide................................................................................................................. 152

Downloading current help files............................................................................................................. 156

24

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

5 Programming: Tools..................................................................................................................... 159

5.1 Entering tool-related data.................................................................................................................. 160

Feed rate F............................................................................................................................................160

Spindle speed S.................................................................................................................................... 161

5.2 Tool data...............................................................................................................................................162

Requirements for tool compensation................................................................................................... 162

Tool number, tool name........................................................................................................................ 162

Tool length L......................................................................................................................................... 162

Tool radius R......................................................................................................................................... 162

Delta values for lengths and radii......................................................................................................... 163

Entering tool data into the program..................................................................................................... 163

Enter tool data into the table............................................................................................................... 164

Importing tool tables.............................................................................................................................172

Pocket table for tool changer................................................................................................................173

Call tool data......................................................................................................................................... 176

Tool change........................................................................................................................................... 178

Tool usage test......................................................................................................................................181

Tool management (software option)..................................................................................................... 183

5.3 Tool compensation.............................................................................................................................. 190

Introduction........................................................................................................................................... 190

Tool length compensation..................................................................................................................... 190

Tool radius compensation..................................................................................................................... 191

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

25

Contents

6 Programming: Programming contours...................................................................................... 195

6.1 Tool movements.................................................................................................................................. 196

Path functions....................................................................................................................................... 196

Miscellaneous functions M...................................................................................................................196

Subprograms and program section repeats......................................................................................... 196

Programming with Q parameters......................................................................................................... 196

6.2 Fundamentals of Path Functions.......................................................................................................197

Programming tool movements for workpiece machining.....................................................................197

6.3 Approaching and departing a contour............................................................................................. 200

Starting point and end point................................................................................................................. 200

Tangential approach and departure....................................................................................................... 202

Overview: Types of paths for contour approach and departure............................................................203

Important positions for approach and departure...................................................................................204

Approaching on a straight line with tangential connection: APPR LT................................................... 205

Approaching on a straight line perpendicular to the first contour point: APPR LN............................... 205

Approaching on a circular path with tangential connection: APPR CT..................................................206

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

APPR LCT.............................................................................................................................................. 206

Departing in a straight line with tangential connection: DEP LT.......................................................... 207

Departing in a straight line perpendicular to the last contour point: DEP LN....................................... 207

Departing on a circular path with tangential connection: DEP CT........................................................207

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT.............. 208

6.4 Path contours - Cartesian coordinates............................................................................................. 209

Overview of path functions.................................................................................................................. 209

Programming path functions.................................................................................................................209

26

Straight line in rapid traverse G00 Straight line with feed rate G01 F.................................................. 210

Inserting a chamfer between two straight lines...................................................................................211

Corner rounding G25............................................................................................................................ 212

Circle center I, J................................................................................................................................... 213

Circular path C around circle center CC............................................................................................... 214

CircleG02/G03/G05 with defined radius............................................................................................... 215

Circle G06 with tangential connection..................................................................................................217

Example: Linear movements and chamfers with Cartesian coordinates.............................................. 218

Example: Circular movements with Cartesian coordinates.................................................................. 219

Example: Full circle with Cartesian coordinates................................................................................... 220

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

6.5 Path contours – Polar coordinates.................................................................................................... 221

Overview............................................................................................................................................... 221

Zero point for polar coordinates: pole I, J............................................................................................ 222

Straight line in rapid traverse G10 Straight line with feed rate G11 F...................................................222

Circular path G12/G13/G15 around pole I, J......................................................................................... 223

Circle G16 with tangential connection.................................................................................................. 223

Helix.......................................................................................................................................................224

Example: Linear movement with polar coordinates............................................................................. 226

Example: Helix...................................................................................................................................... 227

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

27

Contents

7 Programming: Data transfer from DXF files or plain-language contours............................... 229

7.1 Processing DXF Files (Software Option).......................................................................................... 230

Application............................................................................................................................................. 230

Opening a DXF file............................................................................................................................... 231

Working with the DXF converter..........................................................................................................231

Basic settings........................................................................................................................................232

Setting layers.........................................................................................................................................234

Defining the datum............................................................................................................................... 235

Selecting and saving a contour.............................................................................................................237

Selecting and saving machining positions............................................................................................ 241

28

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

8 Programming: Subprograms and program section repeats.................................................... 247

8.1 Labeling Subprograms and Program Section Repeats................................................................... 248

Label...................................................................................................................................................... 248

8.2 Subprograms....................................................................................................................................... 249

Operating sequence..............................................................................................................................249

Programming notes...............................................................................................................................249

Programming a subprogram................................................................................................................. 249

Calling a subprogram............................................................................................................................ 250

8.3 Program-section repeats.................................................................................................................... 251

Label G98.............................................................................................................................................. 251

Operating sequence..............................................................................................................................251

Programming notes...............................................................................................................................251

Programming a program section repeat............................................................................................... 251

Calling a program section repeat..........................................................................................................252

8.4 Any desired program as subprogram............................................................................................... 253

Operating sequence..............................................................................................................................253

Programming notes...............................................................................................................................253

Calling any program as a subprogram.................................................................................................. 254

8.5 Nesting................................................................................................................................................. 255

Types of nesting....................................................................................................................................255

Nesting depth........................................................................................................................................255

Subprogram within a subprogram........................................................................................................ 256

Repeating program section repeats......................................................................................................257

Repeating a subprogram.......................................................................................................................258

8.6 Programming examples..................................................................................................................... 259

Example: Milling a contour in several infeeds...................................................................................... 259

Example: Groups of holes.................................................................................................................... 260

Example: Group of holes with several tools.........................................................................................261

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

29

Contents

9 Programming: Q Parameters.......................................................................................................263

9.1 Principle and overview of functions................................................................................................. 264

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

Calling Q parameter functions.............................................................................................................. 266

9.2 Part families—Q parameters in place of numerical values............................................................. 267

Application............................................................................................................................................. 267

9.3 Describing contours with mathematical functions......................................................................... 268

Application............................................................................................................................................. 268

Overview............................................................................................................................................... 268

Programming fundamental operations..................................................................................................269

9.4 Angle functions (trigonometry).........................................................................................................270

Definitions............................................................................................................................................. 270

Programming trigonometric functions.................................................................................................. 270

9.5 If-then decisions with Q parameters................................................................................................ 271

Application............................................................................................................................................. 271

Unconditional jumps..............................................................................................................................271

Programming if-then decisions............................................................................................................. 271

9.6 Checking and changing Q parameters............................................................................................. 272

Procedure.............................................................................................................................................. 272

9.7 Additional functions............................................................................................................................274

Overview............................................................................................................................................... 274

D14: Displaying error messages........................................................................................................... 275

D18: Reading system data....................................................................................................................279

30

D19: Transfer values to PLC................................................................................................................. 288

D20: NC and PLC synchronization........................................................................................................288

D29: Transfer values to the PLC...........................................................................................................290

D37 EXPORT.........................................................................................................................................290

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

9.8 Accessing tables with SQL commands............................................................................................ 291

Introduction........................................................................................................................................... 291

A transaction......................................................................................................................................... 292

Programming SQL commands..............................................................................................................294

Overview of the soft keys.................................................................................................................... 294

SQL BIND..............................................................................................................................................295

SQL SELECT......................................................................................................................................... 296

SQL FETCH........................................................................................................................................... 298

SQL UPDATE.........................................................................................................................................299

SQL INSERT..........................................................................................................................................299

SQL COMMIT....................................................................................................................................... 300

SQL ROLLBACK.................................................................................................................................... 300

9.9 Entering formulas directly..................................................................................................................301

Entering formulas.................................................................................................................................. 301

Rules for formulas.................................................................................................................................303

Programming example.......................................................................................................................... 304

9.10 String parameters............................................................................................................................... 305

String processing functions.................................................................................................................. 305

Assigning string parameters................................................................................................................. 306

Chain-linking string parameters.............................................................................................................306

Converting a numerical value to a string parameter.............................................................................307

Copying a substring from a string parameter.......................................................................................308

Converting a string parameter to a numerical value.............................................................................309

Checking a string parameter.................................................................................................................310

Finding the length of a string parameter..............................................................................................311

Comparing alphabetic sequence...........................................................................................................312

Reading machine parameters............................................................................................................... 313

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

31

Contents

9.11 Preassigned Q parameters................................................................................................................. 316

Values from the PLC: Q100 to Q107....................................................................................................316

Active tool radius: Q108........................................................................................................................316

Tool axis: Q109......................................................................................................................................316

Spindle status: Q110............................................................................................................................. 317

Coolant on/off: Q111............................................................................................................................. 317

Overlap factor: Q112............................................................................................................................. 317

Unit of measurement for dimensions in the program: Q113................................................................317

Tool length: Q114.................................................................................................................................. 317

Coordinates after probing during program run..................................................................................... 318

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

TT 130....................................................................................................................................................318

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

TNC........................................................................................................................................................318

Measurement results from touch probe cycles (see also User’s Manual for Cycle Programming).......319

9.12 Programming examples..................................................................................................................... 321

Example: Ellipse.................................................................................................................................... 321

Example: Concave cylinder machined with spherical cutter.................................................................323

Example: Convex sphere machined with end mill................................................................................325

32

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

10 Programming: Miscellaneous functions.....................................................................................327

10.1 Entering miscellaneous functions M and STOP...............................................................................328

Fundamentals........................................................................................................................................ 328

10.2 M functions for program run inspection, spindle and coolant.......................................................329

Overview............................................................................................................................................... 329

10.3 Miscellaneous functions for coordinate data...................................................................................330

Programming machine-referenced coordinates: M91/M92.................................................................. 330

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130................... 332

10.4 Miscellaneous functions for path behavior......................................................................................333

Machining small contour steps: M97................................................................................................... 333

Machining open contour corners: M98................................................................................................ 334

Feed rate factor for plunging movements: M103.................................................................................335

Feed rate in millimeters per spindle revolution: M136.........................................................................336

Feed rate for circular arcs: M109/M110/M111.......................................................................................337

Calculating the radius-compensated path in advance (LOOK AHEAD): M120......................................338

Superimposing handwheel positioning during program run: M118...................................................... 340

Retraction from the contour in the tool-axis direction: M140...............................................................342

Suppressing touch probe monitoring: M141........................................................................................ 343

Deleting basic rotation: M143...............................................................................................................344

Automatically retract tool from the contour at an NC stop: M148....................................................... 345

Rounding corners: M197.......................................................................................................................346

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

33

Contents

11 Programming: Special functions.................................................................................................347

11.1 Overview of special functions........................................................................................................... 348

Main menu for SPEC FCT special functions........................................................................................ 348

Program defaults menu........................................................................................................................ 349

Functions for contour and point machining menu................................................................................ 349

Menu of various DIN/ISO functions......................................................................................................350

11.2 Dynamic Collision Monitoring (software option)............................................................................ 351

Function.................................................................................................................................................351

Collision monitoring in the manual operating modes........................................................................... 353

Collision monitoring in Automatic operation......................................................................................... 355

Graphic depiction of the protected space............................................................................................ 356

11.3 Adaptive Feed Control Software Option (AFC)................................................................................357

Application............................................................................................................................................. 357

Defining the AFC basic settings........................................................................................................... 359

Recording a teach-in cut....................................................................................................................... 362

Activating/deactivating AFC...................................................................................................................365

Log file.................................................................................................................................................. 367

Tool breakage/tool wear monitoring......................................................................................................368

Spindle load monitoring........................................................................................................................ 369

11.4 Active Chatter Control (ACC; software option)................................................................................370

Application............................................................................................................................................. 370

Activating/deactivating ACC...................................................................................................................371

11.5 Defining DIN/ISO Functions...............................................................................................................372

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

11.6 Creating Text Files...............................................................................................................................373

Application............................................................................................................................................. 373

Opening and exiting text files...............................................................................................................373

Editing texts.......................................................................................................................................... 374

Deleting and re-inserting characters, words and lines..........................................................................374

Editing text blocks.................................................................................................................................375

Finding text sections.............................................................................................................................376

34

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

11.7 Freely definable tables....................................................................................................................... 377

Fundamentals........................................................................................................................................ 377

Creating a freely definable table...........................................................................................................377

Editing the table format........................................................................................................................377

Switching between table and form view..............................................................................................379

D26: TAPOPEN: Open a freely definable table.................................................................................... 380

D27: TAPWRITE: Write to a freely definable table...............................................................................381

D28: TAPREAD: Read from a freely definable table.............................................................................382

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

35

Contents

12 Programming: Multiple Axis Machining.................................................................................... 383

12.1 Functions for multiple axis machining............................................................................................. 384

12.2 The PLANE Function: Tilting the Working Plane (Software Option 1)...........................................385

Introduction........................................................................................................................................... 385

Defining the PLANE function................................................................................................................387

Position display......................................................................................................................................387

Resetting the PLANE function.............................................................................................................. 388

Defining the working plane with the spatial angle: PLANE SPATIAL....................................................389

Defining the working plane with the projection angle: PLANE PROJECTED....................................... 391

Defining the working plane with the Euler angle: PLANE EULER........................................................392

Defining the working plane with two vectors: PLANE VECTOR.......................................................... 394

Defining the working plane via three points: PLANE POINTS..............................................................396

Defining the working plane via a single incremental spatial angle: PLANE SPATIAL............................398

Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)......................................399

Specifying the positioning behavior of the PLANE function.................................................................401

12.3 Inclined-tool machining in a tilted machining plane (software option 2)......................................406

Function.................................................................................................................................................406

Inclined-tool machining via incremental traverse of a rotary axis......................................................... 406

12.4 Miscellaneous functions for rotary axes.......................................................................................... 407

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1).............................................. 407

Shortest-path traverse of rotary axes: M126........................................................................................408

Reducing display of a rotary axis to a value less than 360°: M94........................................................409

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

option 2)................................................................................................................................................ 410

Selecting tilting axes: M138................................................................................................................. 413

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

M144 (software option 2)...................................................................................................................... 414

12.5 FUNCTION TCPM (software option 2).............................................................................................. 415

Function.................................................................................................................................................415

Defining the TCPM FUNCTION............................................................................................................ 415

Mode of action of the programmed feed rate..................................................................................... 416

Interpretation of the programmed rotary axis coordinates...................................................................416

Type of interpolation between the starting and end position............................................................... 418

Resetting the TCPM FUNCTION.......................................................................................................... 419

36

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

12.6 Peripheral Milling: 3-D radius compensation with TCPM and radius compensation (G41/

G42).......................................................................................................................................................420

Application............................................................................................................................................. 420

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

37

Contents

13 Programming: Pallet editor......................................................................................................... 421

13.1 Pallet Management............................................................................................................................. 422

Application............................................................................................................................................. 422

Select pallet table................................................................................................................................. 424

Exiting the pallet file............................................................................................................................. 424

Run pallet file........................................................................................................................................ 424

38

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

14 Programming: Turning Operations............................................................................................. 427

14.1 Turning Operations on Milling Machines (Software Option 50).....................................................428

Introduction........................................................................................................................................... 428

14.2 Basis Functions (Software Option 50).............................................................................................. 429

Switching between milling/turning mode of operation......................................................................... 429

Graphical display of turning operations.................................................................................................431

Program spindle speed......................................................................................................................... 432

Feed rate............................................................................................................................................... 433

Tool call..................................................................................................................................................433

Tool compensation in the program....................................................................................................... 434

Tool data................................................................................................................................................ 435

Tool tip radius compensation TRC........................................................................................................ 440

Recessing and undercutting..................................................................................................................441

Inclined turning......................................................................................................................................447

14.3 Unbalance Functions.......................................................................................................................... 449

Unbalance while turning....................................................................................................................... 449

Measure Unbalance cycle.....................................................................................................................451

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

39

Contents

15 Manual operation and setup.......................................................................................................453

15.1 Switch-on, switch-off..........................................................................................................................454

Switch-on............................................................................................................................................... 454

Switch-off...............................................................................................................................................456

15.2 Moving the machine axes..................................................................................................................457

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

Moving the axis with the machine axis direction buttons.................................................................... 457

Incremental jog positioning...................................................................................................................457

Traverse with electronic handwheels....................................................................................................458

15.3 Spindle speed S, feed rate F and miscellaneous function M......................................................... 468

Application............................................................................................................................................. 468

Entering values......................................................................................................................................468

Adjusting spindle speed and feed rate................................................................................................. 469

Activating feed-rate limitation............................................................................................................... 469

15.4 Functional safety FS (option)............................................................................................................ 470

Miscellaneous........................................................................................................................................470

Explanation of terms............................................................................................................................. 471

Checking the axis positions.................................................................................................................. 472

Activating feed-rate limitation............................................................................................................... 473

Additional status displays......................................................................................................................474

15.5 Datum setting without a 3-D touch probe.......................................................................................475

Note.......................................................................................................................................................475

Preparation.............................................................................................................................................475

Workpiece presetting with axis keys....................................................................................................475

Datum management with the preset table.......................................................................................... 476

15.6 Using 3-D touch probes..................................................................................................................... 482

Overview............................................................................................................................................... 482

Functions in touch probe cycles........................................................................................................... 484

Selecting touch probe cycles................................................................................................................486

Recording measured values from the touch-probe cycles................................................................... 487

Writing measured values from the touch probe cycles in a datum table............................................. 488

Writing measured values from the touch probe cycles in the preset table.......................................... 489

40

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

15.7 Calibrating a 3-D touch trigger probe...............................................................................................490

Introduction........................................................................................................................................... 490

Calibrating the effective length............................................................................................................. 491

Calibrating the effective radius and compensating center misalignment............................................. 492

Displaying calibration values................................................................................................................. 494

15.8 Compensating workpiece misalignment with 3-D touch probe.................................................... 495

Introduction........................................................................................................................................... 495

Identifying basic rotation.......................................................................................................................496

Saving a basic rotation in the preset table...........................................................................................496

Compensation of workpiece misalignment by rotating the table.........................................................496

Displaying a basic rotation.................................................................................................................... 497

Canceling a basic rotation.....................................................................................................................497

15.9 Datum Setting with 3-D Touch Probe...............................................................................................498

Overview............................................................................................................................................... 498

Datum setting in any axis..................................................................................................................... 498

Corner as datum................................................................................................................................... 499

Circle center as datum..........................................................................................................................501

Setting a center line as datum............................................................................................................. 503

Measuring workpieces with a 3-D touch probe................................................................................... 504

Using touch probe functions with mechanical probes or measuring dials............................................507

15.10Tilting the working plane (software option 1).................................................................................508

Application, function..............................................................................................................................508

Traversing reference points in tilted axes............................................................................................. 510

Position display in a tilted system........................................................................................................ 510

Limitations on working with the tilting function...................................................................................510

To activate manual tilting:..................................................................................................................... 511

Setting the current tool-axis direction as the active machining direction..............................................512

Setting the datum in a tilted coordinate system.................................................................................. 513

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

41

Contents

16 Positioning with Manual Data Input.......................................................................................... 515

16.1 Programming and executing simple machining operations...........................................................516

Positioning with manual data input (MDI)............................................................................................ 516

Protecting and erasing programs in $MDI............................................................................................519

42

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

17 Test run and program run........................................................................................................... 521

17.1 Graphics................................................................................................................................................522

Application............................................................................................................................................. 522

Speed of the Setting test runs............................................................................................................. 523

Overview: Display modes..................................................................................................................... 524

Plan view...............................................................................................................................................525

Projection in three planes..................................................................................................................... 525

3-D view................................................................................................................................................ 526

Repeating graphic simulation................................................................................................................529

Tool display............................................................................................................................................529

Measurement of machining time......................................................................................................... 530

17.2 Showing the workpiece blank in the working space......................................................................531

Application............................................................................................................................................. 531

17.3 Functions for program display.......................................................................................................... 532

Overview............................................................................................................................................... 532

17.4 Test Run................................................................................................................................................533

Application............................................................................................................................................. 533

17.5 Program run.........................................................................................................................................535

Application............................................................................................................................................. 535

Running a part program........................................................................................................................ 536

Interrupt machining............................................................................................................................... 537

Moving the machine axes during an interruption................................................................................. 538

Resuming program run after an interruption........................................................................................ 538

Retraction after a power interruption....................................................................................................540

Any entry into program (mid-program startup).....................................................................................543

Returning to the contour.......................................................................................................................545

17.6 Automatic program start....................................................................................................................546

Application............................................................................................................................................. 546

17.7 Optional block skip............................................................................................................................. 547

Application............................................................................................................................................. 547

Inserting the "/" character......................................................................................................................547

Erasing the "/" character........................................................................................................................ 547

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

43

Contents

17.8 Optional program-run interruption....................................................................................................548

Application............................................................................................................................................. 548

44

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

18 MOD functions..............................................................................................................................549

18.1 MOD function...................................................................................................................................... 550

Selecting MOD functions......................................................................................................................550

Changing the settings........................................................................................................................... 550

Exiting MOD functions..........................................................................................................................550

Overview of MOD functions................................................................................................................ 551

18.2 Graphic settings.................................................................................................................................. 552

18.3 Machine settings................................................................................................................................. 553

External access..................................................................................................................................... 553

Tool usage file....................................................................................................................................... 555

Select kinematics.................................................................................................................................. 556

18.4 System settings...................................................................................................................................557

Set the system time............................................................................................................................. 557

18.5 Position Display Types........................................................................................................................558

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

18.6 Unit of Measurement......................................................................................................................... 559

Application............................................................................................................................................. 559

18.7 Displaying operating times................................................................................................................559

Application............................................................................................................................................. 559

18.8 Software numbers...............................................................................................................................560

Application............................................................................................................................................. 560

18.9 Entering the code number................................................................................................................. 560

Application............................................................................................................................................. 560

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

45

Contents

18.10 Setting up data interfaces..................................................................................................................561

Serial interfaces on the TNC 640......................................................................................................... 561

Application............................................................................................................................................. 561

Setting the RS-232 interface.................................................................................................................561

Setting the BAUD RATE (baudRate)..................................................................................................... 561

Setting the protocol (protocol).............................................................................................................. 562

Setting data bits (dataBits)....................................................................................................................562

Check parity (parity).............................................................................................................................. 562

Setting the stop bits (stopBits).............................................................................................................562

Setting handshaking (flowControl)........................................................................................................ 563

File system for file operations (fileSystem).......................................................................................... 563

Settings for data transfer with the TNCserver PC software.................................................................563

Setting the operating mode of the external device (fileSystem).......................................................... 564

Data transfer software.......................................................................................................................... 565

18.11 Ethernet interface................................................................................................................................567

Introduction........................................................................................................................................... 567

Connection options............................................................................................................................... 567

Configuring the TNC............................................................................................................................. 567

18.12Firewall................................................................................................................................................. 573

Application............................................................................................................................................. 573

18.13Configure HR 550 FS wireless handwheel....................................................................................... 576

Application............................................................................................................................................. 576

Assigning the handwheel to a specific handwheel holder................................................................... 576

Setting the transmission channel..........................................................................................................577

Selecting the transmitter power........................................................................................................... 577

Statistical data.......................................................................................................................................578

18.14Load machine configuration.............................................................................................................. 578

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

46

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

19 Tables and overviews...................................................................................................................579

19.1 Machine-specific user parameters.....................................................................................................580

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

19.2 Connector pin layout and connection cables for data interfaces...................................................590

RS-232-C/V.24 interface for HEIDENHAIN devices...............................................................................590

Non-HEIDENHAIN devices....................................................................................................................592

Ethernet interface RJ45 socket............................................................................................................ 593

19.3 Technical Information..........................................................................................................................594

19.4 Overview tables...................................................................................................................................602

Fixed cycles...........................................................................................................................................602

Miscellaneous functions....................................................................................................................... 603

19.5 Functions of the TNC 640 and the iTNC 530 compared................................................................. 605

Comparison: Specifications................................................................................................................... 605

Comparison: Data interfaces.................................................................................................................605

Comparison: Accessories......................................................................................................................606

Comparison: PC software..................................................................................................................... 606

Comparison: Machine-specific functions.............................................................................................. 607

Comparison: User functions................................................................................................................. 607

Comparator: Cycles............................................................................................................................... 614

Comparison: Miscellaneous functions.................................................................................................. 617

Comparison: Touch probe cycles in the Manual Operation and El. Handwheel modes........................618

Comparison: Touch probe cycles for automatic workpiece inspection................................................. 620

Comparison: Differences in programming............................................................................................ 621

Comparison: Differences in Test Run, functionality.............................................................................. 626

Comparison: Differences in Test Run, operation.................................................................................. 626

Comparison: Differences in Manual Operation, functionality............................................................... 626

Comparison: Differences in Manual Operation, operation....................................................................628

Comparison: Differences in Program Run, operation........................................................................... 628

Comparison: Differences in Program Run, traverse movements..........................................................629

Comparison: Differences in MDI operation.......................................................................................... 633

Comparison: Differences in programming station................................................................................ 634

19.6 DIN/ISO function overview................................................................................................................635

DIN/ISO Function Overview TNC 640.................................................................................................. 635

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

47

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

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

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

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

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

Further information on this topic

Traversing the reference marks: See "Switch-on", page 454
Operating modes: See "Programming", page 73

50

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

NO

ENT

1.3 Programming the first part

Selecting the correct operating mode

You can write programs only in Programming mode:

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

Further information on this topic

Operating modes: See "Programming", page 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 101

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

51

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

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

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

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

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

Further information on this topic

File management: See "Working with the file manager",
page 109

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

52

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Programming the first part 1.3

Defining a workpiece blank

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

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

Spindle axis Z – Plane XY: Enter the active spindle axis. G17 is
saved as default setting. Accept with the ENT key

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

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

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

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

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

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

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

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

1

Example NC blocks

%NEW G71 *

N10 G30 G17 X+0 Y+0 Z-40 *

N20 G31 X+100 Y+100 Z+0 *

N99999999 %NEW G71 *

Further information on this topic

Define the blank: page 97

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

53

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 in the program"

Layout of contour machining
programs

%BSPCONT G71 *

N10 G30 G71 X... Y... Z... *

N20 G31 X... Y... Z... *

N30 T5 G17 S5000 *

N40 G00 G40 G90 Z+250 *

N50 X... Y... *

N60 G01 Z+10 F3000 M13 *

N70 X... Y... RL F500 *

...

N160 G40 ... X... Y... F3000 M9 *

N170 G00 Z+250 M2 *

N99999999 BSPCONT G71 *

Recommended program layout for simple cycle programs

1 Call tool, define tool axis
2 Retract the tool
3 Define the fixed cycle
4 Move to the machining position
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

%BSBCYC G71 *

N10 G30 G71 X... Y... Z... *

N20 G31 X... Y... Z... *

N30 T5 G17 S5000 *

N40 G00 G40 G90 Z+250 *

N50 G200... *

N60 X... Y... *

N70 G79 M13 *

N80 G00 Z+250 M2 *

N99999999 BSBCYC G71 *

54

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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

Press the L key to open a program block for a
linear movement

Press the left arrow key to switch to the input
range for G codes

Press the G0 soft key if you want to enter a rapid
traverse motion

1

Programming the first part 1.3

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

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

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

Press the L key to open a program block for a
linear movement

Press the left arrow key to switch to the input
range for G codes

Press the G0 soft key if you want to enter a rapid
traverse motion

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

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

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

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

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

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

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

Miscellaneous function M? Switch on the spindle

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

Enter 26 to move to the contour: Define the
rounding radius of the approaching arc

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

55

1

First Steps with the TNC 640

1.3 Programming the first part

Machine the contour and move to the contour
point 2: You only need to enter the information
that changes. In other words, enter only the Y
coordinate 95 and save your entry with the END
key

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

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

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

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

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

Enter 27 to depart from the contour: Define the
rounding radius of the departing arc

Enter 0. To retract the tool, select : Press the
orange axis key Z in order to get clear in the tool
axis, and enter the value for the position to be
approached, e.g. 250. Press the ENT key

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

MISCELLANEOUS FUNCTION M? Enter M2 to enter

end of program, then confirm with the END key.
The TNC saves the entered positioning block

Further information on this topic

Complete example with NC blocks: See "Example: Linear

movements and chamfers with Cartesian coordinates",

page 218

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

page 95

Approaching/departing contours: See "Approaching and

departing a contour"

Programming contours: See "Overview of path functions",

page 209

Tool radius compensation: See "Tool radius compensation ",

page 191

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

inspection, spindle and coolant ", page 329

56

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Programming the first part 1.3

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

Press the L key to open a program block for a
linear movement

Press the left arrow key to switch to the input
range for G codes

Press the G0 soft key if you want to enter a rapid
traverse motion

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

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

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

Call the cycle menu

1

Display the drilling cycles

Select standard drilling cycle 200: The TNC starts
the dialog for cycle definition. Enter all parameters
requested by the TNC step by step and conclude
each entry with the ENT key. In the screen to the
right, the TNC also displays a graphic showing the
respective cycle parameter

Enter 0 to move to the first drilling position: Enter
the coordinates of the drilling position, switch-on
the coolant and spindle, and call the cycle via M99

Enter 0 to move to a further drilling position:
Enter the coordinates of the respective drilling
positions, and call the cycle with M99

Enter 0. To retract the tool, select : Press the
orange axis key Z in order to get clear in the tool
axis, and enter the value for the position to be
approached, e.g. 250. Press the ENT key

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

Miscellaneous function M? Enter M2 to enter end
of program, then confirm with the END key. The
TNC stores the entered positioning block

Example NC blocks

%C200 G71 *

N10 G30 G17 X+0 Y+0 Z-40 *

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Definition of workpiece blank

57

1

First Steps with the TNC 640

1.3 Programming the first part

N20 G31 X+100 Y+100 Z+0 *

N30 T5 G17 S4500 *

N40 G00 G40 G90 Z+250 *

N50 G200 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

N60 X+10 Y+10 M13 M99 *

N70 X+10 Y+90 M99 *

N80 X+90 Y+10 M99 *

N90 X+90 Y+90 M99 *

N100 G00 Z+250 M2 *

N99999999 %C200 G71 *

Tool call

Retract the tool

Define the cycle

Spindle and coolant on, call the cycle

Call the cycle

Call the cycle

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, "Cycle

fundamentals / Overviews"

58

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Graphically testing the first part 1.4

1.4 Graphically testing the first part

Selecting the correct operating mode

You can test programs only in the Test Run mode:

Press the operating-mode key: The TNC goes into
the Test Run operating mode

Further information on this topic

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

page 73

Testing programs: See "Test Run", page 533

1

Selecting the tool table for the test run

You only need to execute this step if you have not activated a tool
table in the Test Run mode.

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

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

Press the DEFAULT soft key: The TNC shows all
saved files in the right window

Move the highlight to the left onto the directories

Move the highlight to the TNC:\ directory

Move the highlight to the right onto the files

Move the highlight to the file TOOL.T (active tool
table) and load with the ENT key: TOOL.T receives
the status S and is therefore active for the test run

Press the END key: Exit the file management

Further information on this topic

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

page 164

Testing programs: See "Test Run", page 533

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

59

1

First Steps with the TNC 640

1.4 Graphically testing the first part

Choosing the program you want to test

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

Press the LAST FILES soft key: The TNC opens a
pop-up window with the most recently selected
files

Use the arrow keys to select the program that you
want to test. Load with the ENT key

Further information on this topic

Selecting a program: See "Working with the file manager",

page 109

Selecting the screen layout and the view

Press the key for selecting the screen layout: The
TNC displays all available alternatives in the soft­key row

Press the PROGRAM+GRAPHICS soft key: In
the left half of the screen the TNC shows the
program; in the right half it shows the workpiece
blank

Press the FURTHER VIEW OPTIONS soft key

Move the soft-key row further and select the
desired view by soft key

The TNC features the following views:

Soft key Function

Plan view

Projection in three planes

3-D view

Further information on this topic

Graphic functions: See "Graphics ", page 522

Running a test run: See "Test Run", page 533

60

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Starting the test run

Press the RESET + START soft key: The TNC
simulates the active program up to a programmed
break or to the program end

While the simulation is running, you can use the
soft keys to change views

Press the STOP soft key: The TNC interrupts the
test run

Press the START soft key: the TNC resumes the
test run after an interruption.

Further information on this topic

Running a test run: See "Test Run", page 533

Graphic functions: See "Graphics ", page 522

Adjust the simulation speed: See "Speed of the Setting test

runs", page 523

1

Graphically testing the first part 1.4

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

61

1

First Steps with the TNC 640

1.5 Setting up tools

1.5 Setting up tools

Selecting the correct operating mode

Tools are set up in the Manual Operation mode:

Press the operating-mode key: The TNC switches
to the Manual mode of operation

Further information on this topic

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

page 73

Preparing and measuring tools

Clamp the required tools in their chucks

When measuring with an external tool presetter: Measure the

tools, note down the length and radius, or transfer them directly

to the machine through a transfer program

When measuring on the machine: store the tools in the tool

changer page 64

62

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 164

1

Setting up tools 1.5

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

63

1

First Steps with the TNC 640

1.5 Setting up tools

The pocket table TOOL_P.TCH

The function of the pocket table depends on the
machine. Refer to your machine manual.

In the pocket table TOOL_P.TCH (permanently saved under TNC:
\TABLE\) you specify which tools your tool magazine contains.

To enter data in the pocket table TOOL_P.TCH, proceed as follows:

Displaying the tool table: The TNC shows the tool
table

Display the pocket table: The TNC shows the
pocket table

Edit the pocket table: Set the EDIT soft key to ON
With the upward or downward arrow keys you can

select the pocket number that you want to edit
With the rightward or leftward arrow keys you can

select the data that you want to edit
Exit the pocket table: press the END key.

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 173

64

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

1.6 Workpiece setup

Selecting the correct operating mode

Workpieces are set up in the Manual Operation or Electronic
Handwheel mode

Press the operating-mode key: The TNC switches
to the Manual mode of operation

Further information on this topic

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

page 457

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.

1

Workpiece setup 1.6

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

65

1

First Steps with the TNC 640

1.6 Workpiece setup

Datum setting with 3-D touch probe

Insert a 3-D touch probe Insert the 3-D touch probe: In the MDI

mode, run a TOOL CALL block containing the tool axis and then

return to the Manual Operation mode

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

Set the datum at a workpiece corner, for example
Position the touch probe near the first touch point

on the first workpiece edge
Select the probing direction via soft key
Press NC start Press NC start: The touch probe

moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the second touch
point on the first workpiece edge

Press NC start Press NC start: The touch probe
moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the first touch point
on the second workpiece edge

Select the probing direction via soft key
Press NC start Press NC start: The touch probe

moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Use the axis-direction keys to pre-position the
touch probe to a position near the second touch
point on the second workpiece edge

Press NC start Press NC start: The touch probe
moves in the defined direction until it contacts the
workpiece and then automatically returns to its
starting point

Then the TNC shows the coordinates of the
measured corner point

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

Further information on this topic

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

page 498

66

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

1.7 Running the first program

Selecting the correct operating mode

You can run programs either in the Single Block or the Full
Sequence mode:

Press the operating-mode key: The TNC goes into
the Program Run, Single Block mode and the
TNC executes the program block by block. You
have to confirm each block with the NC start key

Press the operating-mode key: The switches
to the Program Run, Full Sequence operating
mode: The TNC switches to that mode and
runs the program after NC start up to a program
interruption or to the end of the program

Further information on this topic

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

page 73

Running programs: See "Program run", page 535

1

Running the first program 1.7

Choosing the program you want to run

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

Press the LAST FILES soft key: The TNC opens a
pop-up window with the most recently selected
files

If desired, use the arrow keys to select the
program that you want to run. Load with the ENT
key

Further information on this topic

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

page 109

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 535

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 TNC 640 and the iTNC 530
compared", page 605. Please also note the
detailed description of the differences between the
iTNC 530 and the TNC 640

70

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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

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

2

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 for DIN/ISO Programming | 3/2014

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
7 Numerical input and axis selection
8 Touchpad
9 Mouse function keys
10 USB connection

File management
Calculator
MOD function
HELP function

Navigation keys and GOTO jump command

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

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

2.4 Status displays

"General" status display

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

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

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

Positioning with Manual Data Input (MDI).
In the Manual Operation and El. Handwheel modes the status

display appears in the large window.

Information in the status display

Icon Meaning

ACTL. Position display: Actual, nominal or distance-to-go

coordinates mode

2

Status displays 2.4

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

Number of the active presets from the preset
table. If the datum was set manually, the TNC
displays the text MAN behind the symbol

F S M The displayed feed rate in inches corresponds to

one tenth of the effective value. Spindle speed S,
feed rate F and active M functions

Axis is clamped

Axis can be moved with the handwheel

Axes are moving under a basic rotation

Axes are moving in a tilted working plane

The M128 function or TCPM FUNCTION is active

No active program

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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)

The Active Chatter Control feature (ACC) is active
(software option)

The Cross Talk Compensation (CTC) is active
(software option)

Additional status displays

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

To switch on the additional status display:

Call the soft-key row for screen layout

Select the layout option for the additional status
display: In the right half of the screen, the TNC
shows the OVERVIEW status form

To select an additional status display:

Switch the soft-key rows until the STATUS soft
keys appear

Either select the additional status display directly
by soft key, e.g. positions and coordinates, or

use the switch-over soft keys to select the desired
view

The available status displays described below can be selected
either directly by soft key or with the switch-over soft keys.

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

76

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Overview

After switch-on, the TNC displays the Overview status form,
provided that you have selected the PROGRAM+STATUS screen
layout (or POSITION + STATUS). The overview form contains a
summary of the most important status information, which you can
also find on the various detail forms.

Soft key Meaning

Position display

Tool information

Active M functions

Active coordinate transformations

Active subprogram

Active program section repeat

Program called with PGM CALL

Current machining time

Name of the active main program

2

Status displays 2.4

General program information (PGM tab)

Soft key Meaning

No direct
selection
possible

Name of the active main program

Circle center CC (pole)

Dwell time counter

Machining time when the program was
completely simulated in the Test Run operating
mode

Current machining time in percent

Current time

Active programs

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 G53

Active datum shift (Cycle G54); The TNC
displays an active datum shift in up to 8 axes

Mirrored axes (Cycle G28)

Active basic rotation

Active rotation angle (Cycle G73)

Active scaling factor/factors (Cycles G72); 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 for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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 the machine parameter CfgLanguage

Network: Network setting
Reset WM-Conf: Restore basic settings of the Windows

Manager. May also reset settings implemented by your
machine manufacturer

Screensaver: Settings for the screen saver; several are
available

Shares: Configure network connections
Firewall: Configuring the Firewall See "Firewall", page 573

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 106)

84

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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

The TS 220, TS 440, TS 444, TS 640 and TS 740 triggering touch
probes edge finder

These touch probes are particularly effective for automatic
workpiece alignment, datum setting and workpiece measurement.
The TS 220 transmits the triggering signals to the TNC via cable
and is a cost-effective alternative for applications where digitizing is
not frequently required.

The TS 640 (see figure) and the smaller TS 440 feature infrared
transmission of the triggering signal to the TNC. This makes
them highly convenient for use on machines with automatic tool
changers.

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

TT 140 tool touch probe for tool measurement

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

86

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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. 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 for DIN/ISO Programming | 3/2014

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 H.

Coordinates of the pole
(plane)

X/Y +X

Y/Z +Y

Z/X +Z

Reference axis of the angle

92

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

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 G91 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

G91 X = 20 mm G91 X = 20 mm

G91 Y = 10 mm G91 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 for DIN/ISO Programming | 3/2014

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Block number

Path function

Words

Block

Opening programs and entering 3.2

3.2 Opening programs and entering

Organization of an NC program in DIN/ISO 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 of a part program automatically
depending on machine parameter blockIncrement (105409). The
machine parameter blockIncrement (105409) defines the block
number increment.

The first block of a program is identified by %, the program name
and the active unit of measure.

The subsequent blocks contain information on:

The workpiece blank

Tool calls

Approaching a safe position

Feed rates and spindle speeds, as well as

Path contours, cycles and other functions
The last block of a program is identified by N99999999 the

program name and the active unit of measure.

3

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

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

95

3

Programming: Fundamentals, file management

3.2 Opening programs and entering

Define the blank: G30/G31

Immediately after initiating a new program, you define a cuboid,
unmachined workpiece blank. If you wish to define the blank at a
later stage, press the spec fct key, the PROGRAM DEFAULTS soft
key, and then the BLK FORM soft key. The TNC needs this definition
for graphic simulation.

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

The TNC can depict various types of blank forms.

Soft key Function

Define a workpiece blank

Define a cylindrical blank

Define a rotationally symmetric blank

Rectangular blank

The sides of the cuboid lie parallel to the X, Y and Z axes. This
blank is defined by two of its corner points:

MIN point G30: the smallest X, Y and Z coordinates of the blank

form, entered as absolute values

MAX point G31: the largest X, Y and Z coordinates of the blank

form, entered as absolute or incremental values

Example: Display the BLK FORM in the NC program

%NEW G71 *

N10 G30 G17 X+0 Y+0 Z-40 *

N20 G31 X+100 Y+100 Z+0 *

N99999999 %NEW G71 *

Program begin, name, unit of measure

Spindle axis, MIN point coordinates

MAX point coordinates

Program end, name, unit of measure

96

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Opening programs and entering 3.2

Cylindrical blank

The cylindrical blank form is defined by the dimensions of the
cylinder:

R: Radius of the cylinder

L: Length of the cylinder

DIST: Distance from datum to cylinder end

RI: Inside radius for a hollow cylinder

The DIST and RI parameters are optional and do not
need to be programmed.

Example: Display the BLK FORM CYLINDER in the NC program

0 BEGIN PGM NEW MM

1 BLK FORM CYLINDER Z R50 L105 DIST+5 RI10

2 END PGM NEW MM

Program begin, name, unit of measure

Spindle axis, radius, length, distance, inside radius

Program end, name, unit of measure

3

Rotationally symmetric blank of any shape

You define the contour of the rotationally symmetric blank in a
subprogram. In the workpiece blank definition you refer to the
contour description:

DIM_D, DIM_R: Diameter or radius of the rotationally

symmetrical blank form

LBL: Subprogram with the contour description

The subprogram can be designated with a number,
an alphanumeric name, or a QS parameter.

Example: Display the BLK FORM ROTATION in the NC program

0 BEGIN PGM NEW MM

1 BLK FORM ROTATION Z DIM_R LBL1

2 M30

3 LBL 1

4 L X+0 Z+1

5 L X+50

6 L Z-20

7 L X+70

8 L Z-100

9 L X+0

10 L Z+1

11 LBL 0

12 END PGM NEW MM

Program begin, name, unit of measure

Spindle axis, manner of interpretation, subprogram number

End of main program

Beginning of subprogram

Beginning of contour

End of contour

End of subprogram

Program end, name, unit of measure

Opening a new part program

You always enter a part program in the PROGRAMMING AND
EDITING mode of operation. An example of program initiation:

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

97

3

Z

Programming: Fundamentals, file management

3.2 Opening programs and entering

Select the PROGRAMMING mode of operation

To call the file manager, Press the PGM MGT key.

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

.I

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

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

Select a rectangular workpiece blank: Press the
soft key for a rectangular blank form

WORKING PLANE IN GRAPHIC: XY

Enter spindle axis, e.g. Z

WORKPIECE BLANK DEF.: MINIMUM

Enter in sequence the X, Y and Z coordinates of
the MIN point and confirm each of your entries
with the ENT key

WORKPIECE BLANK DEF.: MAXIMUM

Enter in sequence the X, Y and Z coordinates of
the MAX point and confirm each of your entries
with the ENT key

Example: Display the BLK form in the NC program

%NEW G71 *

N10 G30 G17 X+0 Y+0 Z-40 *

N20 G31 X+100 Y+100 Z+0 *

N99999999 %NEW G71 *

The TNC automatically generates the first and last blocks of the
program.

Program begin, name, unit of measure

Spindle axis, MIN point coordinates

MAX point coordinates

Program end, name, unit of measure

If you do not wish to define a blank form, cancel the
dialog at Working plane in graphic: XY by pressing
the DEL key.

98

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

Y

Opening programs and entering 3.2

Programming tool movements in DIN/ISO

Press the SPEC FCT key to program a block. Press the PROGRAM
FUNCTIONS soft key, and then the DIN/ISO soft key. You can also
use the gray contouring keys to get the corresponding G code.

If you enter DIN/ISO functions via a connected USB
keyboard, make sure that capitalization is active.

Example of a positioning block

Enter 1 and press the ENT key to open the block

COORDINATES ?

10 (Enter the target coordinate for the X axis)

3

20 (Enter the target coordinate for the Y axis)

go to the next question with ENT.

MILLINGDEFINITIONPOINTPATH

Enter 40 and confirm with ENT to traverse without
tool radius compensation, or

Move to the left or right of the programmed
contour: Select G41 or G42 by soft key

FEED RATE F=?

100 (Enter a feed rate of 100 mm/min for this path contour)

go to the next question with ENT.

MISCELLANEOUS FUNCTION M ?

Enter 3 (miscellaneous function M3 "Spindle ON").

With the END key, the TNC ends this dialog.

The program-block window displays the following line:

N30 G01 G40 X+10 Y+5 F100 M3 *

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014

99

3

Programming: Fundamentals, file management

3.2 Opening programs and entering

Actual position capture

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

Positioning-block programming

Cycle programming
To transfer the correct position values, proceed as follows:

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

to insert a position value

Select actual-position capture: In the soft-key row
the TNC displays the axes whose positions can be
transferred

Select an axis: The TNC writes the current position
of the selected axis into the active input box

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.

100

TNC 640 | User's Manual for DIN/ISO Programming | 3/2014