heidenhain TNC 640 Programming Manual

Download

TNC 640

User’s Manual DIN/ISO Programming

NC Software 340590-05 340591-05 340595-05

English (en) 1/2015

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 ManualDIN/ISO Programming | 1/2015

Controls of the TNC

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Fundamentals

About this manual

The symbols used in this manual are described below.

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

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 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: tnc-userdoc@heidenhain.de.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

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

TNC model NC software number

TNC 640 340590-05 TNC 640 E 340591-05 TNC 640 Programming Station 340595-05

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 ManualDIN/ISO Programming | 1/2015

Fundamentals

TNC model, software and features

Software options

The TNC 640 features various software options that can be enabled by your machine tool builder. Each option is to be enabled separately and contains the following respective functions:

Hardware, options

■

1st additional axis for 4 axes plus spindle

■

2nd additional axis for 5 axes plus spindle

Software option 1 (option number 08) Rotary table machining

Coordinate transformation Interpolation

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

Interpolation

HEIDENHAIN DNC (option number 18)

Display step (Option number 23)

step

■

Programming of cylindrical contours as if in two axes Feed rate in distance per minute Working plane, tilting the ... Circle in 3 axes with tilted working plane (spacial arc)

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

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

Keeping the tool normal to the contour Tool radius compensation perpendicular to traversing and tool direction Linear in 5 axes (subject to export permit)

Communication with external PC applications over COM component

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

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

machine operating modes

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

languages

The machine manufacturer defines objects to be monitored

■

Three warning levels in manual operation

■

Program interrupt during automatic operation

■

Includes monitoring of 5-axis movements

■

Slovenian

■

Norwegian

■

Slovak

■

Latvian

■

Korean

■

Estonian

■

Turkish

■

Romanian

■

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

Software option for additional conversational languages (option number 41)

Lithuanian

■

DXF Converter software option (option number 42) Extracting contour programs

and machining positions from DXF data. Extracting contour sections from plainlanguage programs.

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

rate control for optimizing the machining conditions during series production

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

automatic testing and optimization of the machine kinematics

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

mode

Supported DXF format: AC1009 (AutoCAD R12)

■

For contours and point patterns

■

Simple and convenient specification of reference points

■

Select graphical features of contour sections from conversational

■

programs

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

■

Defining the limits of automatic feed rate control

■

Fully automatic feed control during program run

■

Backup/restore active kinematics

■

Test active kinematics

■

Optimize active kinematics

■

Switching between Milling/Turning mode of operation

■

Constant cutting speed

■

Tool-tip radius compensation

■

Turning cycles

■

Extended Tool Managment software option (option number 93)

Extended tool management, python-based

■

Remote Desktop Manager software option (option number 133)

Windows on a separate computer unitRemote operation of

■

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

Incorporated in the TNC interface

■

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

Feature Content Level (upgrade functions)

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

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

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

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

Intended place of operation

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

Legal information

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

Programming and Editing operating mode MOD function LICENSE INFO soft key

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 CAD Files", page 253).

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 364).

The machine manufacturer can now define any areas on the machine for collision monitoring ("Dynamic Collision Monitoring (Option #40)", page 377).

Writing and reading data in freely definable tables ("Freely definable tables", page 403).

The Adaptive Feed Control (AFC) function has been integrated ("Adaptive feed control AFC (Option #45)", page 384)

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 484).

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

New Active Chatter Control (ACC) software option ("Active Chatter Control ACC (Option #145)", page 396).

New manual probing cycle "Center line as datum" ("Setting a center line as datum ", page 531).

New function for rounding corners ("Rounding corners: M197", page 371).

External access to the TNC can now be blocked with a MOD function ("External access", page 579).

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

Changed 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 172).

The columns AFC and ACC were added to the tool table ("Enter tool data into the table", page 172).

Operation and positioning behavior of the manual probing cycles has been improved ("Using 3-D touch probes ", page 509).

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 77).

The FUNCTION TURNDATA SPIN rotational function has been expanded with an input option for maximum speed ("Program spindle speed", page 456).

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 524)

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Fundamentals

TNC model, software and features

New functions 34059x-04

New special operating mode ("Retraction after a power interruption", page 567).

New graphic simulation ("Graphics ", page 548). New MOD function "tool usage file" within the machine settings

group ("Tool usage file", page 582). New MOD function "set system time" within the systems settings

group ("Set the system time", page 584). New MOD group "graphic settings" ("Graphic settings",

page 578). 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 388).

With the new cutting data calculator you can calculate the spindle speed and the feed rate ("Cutting data calculator", page 147).

In the TURNDATA function, you can now define the effect of the tool compensation ("Tool compensation in the program", page 462).

Now you can activate and deactivate the active chatter compensation (ACC) by soft key ("Activating/deactivating ACC", page 397).

New if/then decisions were introduced in the jump commands ("Programming if-then decisions", page 301).

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 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).

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

Changed functions 34059x-04

The turning tool table was expanded by the column NAME ("Tool data", page 463).

Now up to 4 functions are allowed in an NC block ("Fundamentals", page 352).

New soft keys for value transfer have been introduced in the pocket calculator ("Operation", page 144).

The distance-to-go display can now also be displayed in the input system ("Select the position display", page 585).

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 ManualDIN/ISO Programming | 1/2015

Fundamentals

TNC model, software and features

New functions 34059x-05

The tool management was expanded by the column PITCH ("Enter tool data into the table", page 172).

The turning tool table was expanded by the columns YL and DYL ("Tool data", page 463).

In the tool management, several lines can now be added at the end of the table ("Tool management (Option #93)", page 190).

Any turning tool table can be selected for the program test ("Test Run", page 560).

Programs with .HU and .HC endings can be selected and processed in all operating modes.

The functions and have been added ("Calling any program as a subprogram").

New FEED DWELL function for programming repeating dwell times ("Dwell time FUNCTION FEED DWELL").

The control automatically writes upper case letters at the start of a block "Programming path functions", page 220.

The D18 functions have been expanded ("D18: Reading system data", page 313).

The DCM function can be activated and deactivated from the NC program ("Activating and deactivating collision monitoring", page 382).

USB data carriers can be locked with the SELinux security software ("SELinux security software", page 90).

The posAfterContPocket machine parameter has been added that influences positioning after an SL cycle ("Machine-specific user parameters", page 608).

Protective zones can be defined in the MOD menu ("Entering traverse limits", page 581).

Write protection is possible for single lines in the preset table ("Saving the datums in the preset table", page 501).

New manual probing function for aligning a plane ("Measuring 3-D basic rotation", page 525).

New function for aligning the machining plane without rotary axes ("Tilt the working plane without rotary axes", page 434).

CAD files can be opened without Option #42 ("CAD Viewer", page 255).

New software option #131 Spindle Sychronism ("Software options", page 8).

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

TNC model, software and features

Modified functions 34059x-05

With tool selection, the control also displays columns XL and ZL from the turning tool table in the pop-up window ("Tool call", page 461).

The input range of the DOC column in the pocket table has been expanded to 32 characters ("Pocket table for tool changer").

Commands D15, D31 and D32 from predecessor controls no longer generate ERROR blocks during import. When simulating or running an NC program with these commands, the control interrupts the NC program with an error message that helps you to find an alternative implementation.

Miscellaneous functions M104, M105, M112, M114, M124, M134, M142, M150, M200 - M204 from predecessor controls no longer generate ERROR blocks during import. When simulating or running an NC program with these miscellaneous functions, the control interrupts the NC program with an error message that helps you to find an alternative implementation ("Comparison: Miscellaneous functions").

The maximum file size of files output with D16 F-Print has been increased from 4kB to 20kB.

The Preset.PR preset table is write-protected in Programming operating mode ("Saving the datums in the preset table").

The input range of the Q parameter list for defining the QPARA tab on the status display consists of 132 input positions ("Displaying Q parameters (QPARA tab)", page 82).

Manual calibration of the touch probe with less pre-positionings ("Calibrating a 3-D touch trigger probe ").

The position display takes into account the DL oversizes programmed in the T block, selectable as an oversize of the workpiece or tool ("Delta values for lengths and radii", page 171).

In single blocks, the control executes each point singly with point pattern cycles and G79 PAT ("Program run", page 562).

Rebooting the control is no longer possible with the END key, but with the soft key ("Switch-off", page 482).

The control displays the contouring feed rate in manual mode ("Spindle speed S, feed rate F and miscellaneous function M", page 494).

Deactivate tilting in manual mode is only possible via the 3D-ROT menu ("To activate manual tilting:", page 538).

The machine parameter maxLineGeoSearch has been increased to a maximum of 100000 ("Machine-specific user parameters", page 608).

The names of the software options #8, #9 and #21 have been changed ("Software options", page 8).

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Fundamentals

TNC model, software and features

New and modified cycle functions 34059x-05

New cycle G880 (Option #50), see "ZAHNRAD ABWÄLZFRÄSEN (Zyklus 880, DIN/ISO: G880)"

New cycle G292 (Option #96), see "INTERPOLATIONSDREHEN KONTURSCHLICHTEN (Zyklus 292, DIN/ISO: G292, Softwareoption

96)" New cycle G291 COUPLG.TURNG.INTERP. (Option #96), see

"INTERPOLATIONSDREHEN KOPPLUNG (Zyklus 291, DIN/ISO: G291, Softwareoption 96)"

New cycle G239 for LAC (Load Adapt. Control) load-dependent adaptation of control parameters (Option #143), see "BELADUNG ERMITTELN (Zyklus 239 DIN/ISO: G239, Software-Option 143)"

Cycle G270 CONTOUR TRAIN DATA has been added (Option #19), see "KONTURZUG-DATEN (Zyklus 270, DIN/ISO: G270, SoftwareOption 19)"

Cycle G139 has been added (Option #1), see "ZYLINDER-MANTEL (Zyklus 39, DIN/ISO: G139, Software-Option 1)"

The character set of machining cycle G225 has been expanded with the CE character, ß, the @ character and system time, see "ENGRAVING (Cycle 225, DIN/ISO: G225)"

Cycles G252-G254 have been expanded with the optional parameter Q439

Cycle G122 has been expanded with the optional parameters Q401, Q404, see "ROUGHING (Cycle 22, DIN/ISO: G122, software option 19)"

Cycle G484 has been expanded with the optional parameter Q536, see "Calibrate the wireless TT 449 (Cycle 484, DIN/ISO: G484, software option 17 Touch Probe Functions software option 17)"

Cycles G841 SIMPLE REC. TURNG., RADIAL DIR., G842 , G851 , G852 have been expanded with plunge feed rate Q488

Eccentric turning with cycle G800 is possible with Option #50, see "ADAPT ROTARY COORDINATE SYSTEM(Cycle 800, DIN/ISO: G800)"

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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

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

3 Programming: Fundamentals, File Management........................................................................93

4 Programming: Programming aids.............................................................................................. 139

5 Programming: Tools..................................................................................................................... 167

6 Programming: Programming contours...................................................................................... 203

7 Programming: Data Transfer from CAD Files............................................................................ 253

8 Programming: Subprograms and program section repeats.................................................... 273

9 Programming: Q Parameters.......................................................................................................291

10 Programming: Miscellaneous functions.....................................................................................351

11 Programming: Special functions.................................................................................................373

12 Programming: Multiple Axis Machining.................................................................................... 411

13 Programming: Pallet editor......................................................................................................... 445

14 Programming: Turning Operations............................................................................................. 451

15 Manual operation and setup.......................................................................................................479

16 Positioning with Manual Data Input.......................................................................................... 541

17 Test run and program run........................................................................................................... 547

18 MOD functions..............................................................................................................................575

19 Tables and overviews...................................................................................................................607

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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

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

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

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

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

Creating a cycle program........................................................................................................................58

1.4 Graphically testing the first part.........................................................................................................60

Selecting the correct operating mode.................................................................................................... 60

Selecting the tool table for the test run.................................................................................................60

Choosing the program you want to test................................................................................................ 61

Selecting the screen layout and the view.............................................................................................. 61

Starting the test run................................................................................................................................62

1.5 Setting up tools.................................................................................................................................... 63

Selecting the correct operating mode.................................................................................................... 63

Preparing and measuring tools............................................................................................................... 63

The tool table TOOL.T............................................................................................................................ 64

The pocket table TOOL_P.TCH................................................................................................................65

1.6 Workpiece setup....................................................................................................................................66

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

Clamping the workpiece......................................................................................................................... 66

Datum setting with 3-D touch probe...................................................................................................... 67

1.7 Running the first program................................................................................................................... 68

Selecting the correct operating mode.................................................................................................... 68

Choosing the program you want to run................................................................................................. 68

Start the program....................................................................................................................................68

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

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

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

Programming: In HEIDENHAIN conversational and DIN/ISO..................................................................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........................................................................................................................................... 74

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

Program Run, Full Sequence and Program Run, Single Block................................................................75

2.4 Status displays...................................................................................................................................... 76

General status display.............................................................................................................................76

Additional status displays........................................................................................................................77

2.5 Window Manager..................................................................................................................................84

Task bar................................................................................................................................................... 85

2.6 Remote Desktop Manager (Option #133)........................................................................................... 86

Introduction............................................................................................................................................. 86

Configuring connections – Windows Terminal Service.......................................................................... 86

Configuring the connection – VNC......................................................................................................... 88

Starting and stopping the connection.....................................................................................................89

2.7 SELinux security software....................................................................................................................90

2.8 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels......................................91

3-D touch probes.................................................................................................................................... 91

HR electronic handwheels...................................................................................................................... 92

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

3 Programming: Fundamentals, File Management........................................................................93

3.1 Fundamentals........................................................................................................................................ 94

Position encoders and reference marks................................................................................................. 94

Reference system................................................................................................................................... 94

Reference system on milling machines..................................................................................................95

Designation of the axes on milling machines.........................................................................................95

Polar coordinates..................................................................................................................................... 96

Absolute and incremental workpiece positions......................................................................................97

Selecting the datum................................................................................................................................98

3.2 Opening programs and entering......................................................................................................... 99

Organization of an NC program in DIN/ISO format................................................................................ 99

Define the blank: G30/G31................................................................................................................... 100

Opening a new part program............................................................................................................... 103

Programming tool movements in DIN/ISO...........................................................................................104

Actual position capture..........................................................................................................................105

Editing a program..................................................................................................................................106

The TNC search function...................................................................................................................... 109

3.3 File Management: Fundamentals......................................................................................................111

Files....................................................................................................................................................... 111

Displaying externally generated files on the TNC.................................................................................113

Data Backup.......................................................................................................................................... 113

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

3.4 Working with the File Manager.........................................................................................................114

Directories............................................................................................................................................. 114

Paths......................................................................................................................................................114

Overview: Functions of the file manager............................................................................................. 115

Calling the File Manager....................................................................................................................... 116

Selecting drives, directories and files...................................................................................................117

Creating a new directory...................................................................................................................... 118

Creating a new file................................................................................................................................118

Copying a single file..............................................................................................................................118

Copying files into another directory......................................................................................................119

Copying a table..................................................................................................................................... 120

Copying a directory...............................................................................................................................120

Choosing one of the last files selected................................................................................................121

Deleting a file........................................................................................................................................122

Deleting a directory...............................................................................................................................122

Tagging files.......................................................................................................................................... 123

Renaming a file..................................................................................................................................... 124

Sorting files........................................................................................................................................... 124

Additional functions...............................................................................................................................125

Additional tools for management of external file types........................................................................126

Data transfer to/from an external data medium................................................................................... 133

The TNC in a network.......................................................................................................................... 135

USB devices on the TNC......................................................................................................................136

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

4 Programming: Programming aids.............................................................................................. 139

4.1 Adding comments...............................................................................................................................140

Application............................................................................................................................................. 140

Entering comments during programming.............................................................................................140

Inserting comments after program entry............................................................................................. 140

Entering a comment in a separate block..............................................................................................140

Functions for editing of the comment..................................................................................................141

4.2 Display of NC Programs.....................................................................................................................142

Syntax highlighting................................................................................................................................ 142

Scrollbar.................................................................................................................................................142

4.3 Structuring programs..........................................................................................................................143

Definition and applications.................................................................................................................... 143

Displaying the program structure window / Changing the active window............................................143

Inserting a structuring block in the program window...........................................................................143

Selecting blocks in the program structure window.............................................................................. 143

4.4 Calculator............................................................................................................................................. 144

Operation...............................................................................................................................................144

4.5 Cutting data calculator.......................................................................................................................147

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

4.6 Programming graphics....................................................................................................................... 150

Generate/do not generate graphics during programming.....................................................................150

Generating a graphic for an existing program...................................................................................... 151

Block number display ON/OFF..............................................................................................................152

Erasing the graphic............................................................................................................................... 152

Showing grid lines.................................................................................................................................152

Magnification or reduction of details.................................................................................................... 153

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

4.7 Error messages.................................................................................................................................... 154

Display of errors....................................................................................................................................154

Open the error window........................................................................................................................ 154

Closing the error window..................................................................................................................... 154

Detailed error messages.......................................................................................................................155

INTERNAL INFO soft key......................................................................................................................155

Clearing errors.......................................................................................................................................156

Error log.................................................................................................................................................156

Keystroke log.........................................................................................................................................157

Informational texts................................................................................................................................ 158

Saving service files............................................................................................................................... 158

Calling the TNCguide help system....................................................................................................... 158

4.8 TNCguide context-sensitive help system.........................................................................................159

Application............................................................................................................................................. 159

Working with the TNCguide................................................................................................................. 160

Downloading current help files.............................................................................................................164

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

5 Programming: Tools..................................................................................................................... 167

5.1 Entering tool-related data.................................................................................................................. 168

Feed rate F............................................................................................................................................168

Spindle speed S.................................................................................................................................... 169

5.2 Tool data...............................................................................................................................................170

Requirements for tool compensation................................................................................................... 170

Tool number, tool name........................................................................................................................ 170

Tool length L......................................................................................................................................... 170

Tool radius R......................................................................................................................................... 170

Delta values for lengths and radii.........................................................................................................171

Entering tool data into the program..................................................................................................... 171

Enter tool data into the table............................................................................................................... 172

Importing tool tables.............................................................................................................................180

Pocket table for tool changer................................................................................................................181

Call tool data......................................................................................................................................... 184

Tool change........................................................................................................................................... 186

Tool usage test......................................................................................................................................188

Tool management (Option #93)............................................................................................................ 190

5.3 Tool compensation..............................................................................................................................198

Introduction........................................................................................................................................... 198

Tool length compensation..................................................................................................................... 198

Tool radius compensation..................................................................................................................... 199

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

6 Programming: Programming contours...................................................................................... 203

6.1 Tool movements..................................................................................................................................204

Path functions....................................................................................................................................... 204

FK free contour programming.............................................................................................................. 204

Miscellaneous functions M...................................................................................................................204

Subprograms and program section repeats......................................................................................... 205

Programming with Q parameters......................................................................................................... 205

6.2 Fundamentals of Path Functions.......................................................................................................206

Programming tool movements for workpiece machining.....................................................................206

6.3 Approaching and departing a contour............................................................................................. 209

Starting point and end point................................................................................................................. 209

Tangential approach and departure....................................................................................................... 211

Overview: Types of paths for contour approach and departure............................................................212

Important positions for approach and departure...................................................................................213

Approaching on a straight line with tangential connection: APPR LT................................................... 214

Approaching on a straight line perpendicular to the first contour point: APPR LN............................... 215

Approaching on a circular path with tangential connection: APPR CT..................................................216

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

APPR LCT.............................................................................................................................................. 217

Departing in a straight line with tangential connection: DEP LT.......................................................... 218

Departing in a straight line perpendicular to the last contour point: DEP LN....................................... 218

Departing on a circular path with tangential connection: DEP CT........................................................219

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT.............. 219

6.4 Path contours - Cartesian coordinates............................................................................................. 220

Overview of path functions.................................................................................................................. 220

Programming path functions.................................................................................................................220

Straight line in rapid traverse G00 or straight line with feed rate F G01.............................................. 221

Inserting a chamfer between two straight lines...................................................................................222

Corner rounding G25............................................................................................................................ 223

Circle center I, J................................................................................................................................... 224

Circular path C around circle center CC............................................................................................... 225

CircleG02/G03/G05 with defined radius............................................................................................... 226

Circle G06 with tangential connection..................................................................................................228

Example: Linear movements and chamfers with Cartesian coordinates.............................................. 229

Example: Circular movements with Cartesian coordinates.................................................................. 230

Example: Full circle with Cartesian coordinates................................................................................... 231

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

6.5 Path contours – Polar coordinates....................................................................................................232

Overview............................................................................................................................................... 232

Zero point for polar coordinates: pole I, J............................................................................................ 233

Straight line in rapid traverse G10 or straight line with feed rate F G11...............................................233

Circular path G12/G13/G15 around pole I, J......................................................................................... 234

Circle G16 with tangential connection..................................................................................................234

Helix.......................................................................................................................................................235

Example: Linear movement with polar coordinates............................................................................. 237

Example: Helix...................................................................................................................................... 238

6.6 Path contours – FK free contour programming...............................................................................239

Fundamentals........................................................................................................................................ 239

FK programming graphics..................................................................................................................... 241

Initiating the FK dialog.......................................................................................................................... 242

Pole for FK programming...................................................................................................................... 242

Free straight line programming.............................................................................................................243

Free circular path programming............................................................................................................ 244

Input options......................................................................................................................................... 245

Auxiliary points...................................................................................................................................... 248

Relative data..........................................................................................................................................249

Example: FK programming 1................................................................................................................ 251

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

7 Programming: Data Transfer from CAD Files............................................................................ 253

7.1 CAD viewer and DXF converter screen layout.................................................................................254

CAD viewer and DXF converter screen layout..................................................................................... 254

7.2 CAD Viewer..........................................................................................................................................255

Application............................................................................................................................................. 255

7.3 DXF converter (Option #42)............................................................................................................... 256

Application............................................................................................................................................. 256

Working with the DXF converter..........................................................................................................257

Opening a DXF file............................................................................................................................... 257

Basic settings........................................................................................................................................258

Setting layers.........................................................................................................................................260

Defining the datum............................................................................................................................... 261

Selecting and saving a contour.............................................................................................................263

Selecting and saving machining positions............................................................................................ 267

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

8 Programming: Subprograms and program section repeats.................................................... 273

8.1 Labeling Subprograms and Program Section Repeats................................................................... 274

Label......................................................................................................................................................274

8.2 Subprograms....................................................................................................................................... 275

Operating sequence..............................................................................................................................275

Programming notes...............................................................................................................................275

Programming a subprogram................................................................................................................. 275

Calling a subprogram............................................................................................................................ 276

8.3 Program-section repeats.................................................................................................................... 277

Label G98.............................................................................................................................................. 277

Operating sequence..............................................................................................................................277

Programming notes...............................................................................................................................277

Programming a program section repeat............................................................................................... 278

Calling a program section repeat..........................................................................................................278

8.4 Any desired program as subprogram............................................................................................... 279

Overview of the soft keys.................................................................................................................... 279

Operating sequence..............................................................................................................................280

Programming notes...............................................................................................................................280

Calling any program as a subprogram..................................................................................................281

8.5 Nesting................................................................................................................................................. 283

Types of nesting....................................................................................................................................283

Nesting depth........................................................................................................................................283

Subprogram within a subprogram........................................................................................................ 284

Repeating program section repeats......................................................................................................285

Repeating a subprogram.......................................................................................................................286

8.6 Programming examples..................................................................................................................... 287

Example: Milling a contour in several infeeds...................................................................................... 287

Example: Groups of holes.................................................................................................................... 288

Example: Group of holes with several tools.........................................................................................289

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

9 Programming: Q Parameters.......................................................................................................291

9.1 Principle and overview of functions................................................................................................. 292

Programming notes...............................................................................................................................294

Calling Q parameter functions.............................................................................................................. 295

9.2 Part families—Q parameters in place of numerical values............................................................. 296

Application............................................................................................................................................. 296

9.3 Describing contours with mathematical functions......................................................................... 297

Application............................................................................................................................................. 297

Overview............................................................................................................................................... 297

Programming fundamental operations..................................................................................................298

9.4 Angle functions................................................................................................................................... 299

Definitions............................................................................................................................................. 299

Programming trigonometric functions.................................................................................................. 299

9.5 Calculation of circles...........................................................................................................................300

Application............................................................................................................................................. 300

9.6 If-then decisions with Q parameters................................................................................................ 301

Application............................................................................................................................................. 301

Unconditional jumps..............................................................................................................................301

Programming if-then decisions............................................................................................................. 301

9.7 Checking and changing Q parameters............................................................................................. 302

Procedure.............................................................................................................................................. 302

9.8 Additional functions............................................................................................................................304

Overview............................................................................................................................................... 304

D14: Displaying error messages........................................................................................................... 305

D16 – Formatted output of text and Q parameter values.....................................................................309

D18: Reading system data....................................................................................................................313

D19 – Transfer values to the PLC.........................................................................................................322

D20 – NC and PLC synchronization......................................................................................................322

D29 – Transfer values to the PLC.........................................................................................................323

D37 – EXPORT......................................................................................................................................323

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

9.9 Entering formulas directly..................................................................................................................324

Entering formulas..................................................................................................................................324

Rules for formulas.................................................................................................................................326

Programming example.......................................................................................................................... 327

9.10 String parameters............................................................................................................................... 328

String processing functions.................................................................................................................. 328

Assigning string parameters................................................................................................................. 329

Chain-linking string parameters.............................................................................................................329

Converting a numerical value to a string parameter.............................................................................330

Copying a substring from a string parameter.......................................................................................331

Converting a string parameter to a numerical value.............................................................................332

Checking a string parameter.................................................................................................................333

Finding the length of a string parameter..............................................................................................334

Comparing alphabetic sequence...........................................................................................................335

Reading out machine parameters......................................................................................................... 336

9.11 Preassigned Q parameters.................................................................................................................339

Values from the PLC: Q100 to Q107....................................................................................................339

Active tool radius: Q108........................................................................................................................339

Tool axis: Q109......................................................................................................................................339

Spindle status: Q110.............................................................................................................................340

Coolant on/off: Q111............................................................................................................................. 340

Overlap factor: Q112............................................................................................................................. 340

Unit of measurement for dimensions in the program: Q113................................................................340

Tool length: Q114.................................................................................................................................. 340

Coordinates after probing during program run..................................................................................... 341

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

130.........................................................................................................................................................341

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

TNC........................................................................................................................................................341

Measurement results from touch probe cycles (see also User’s Manual for Cycle Programming).......342

9.12 Programming examples..................................................................................................................... 344

Example: Ellipse.................................................................................................................................... 344

Example: Concave cylinder machined with spherical cutter.................................................................346

Example: Convex sphere machined with end mill................................................................................348

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

10 Programming: Miscellaneous functions.....................................................................................351

10.1 Entering miscellaneous functions M and STOP...............................................................................352

Fundamentals........................................................................................................................................ 352

10.2 M functions for program run inspection, spindle and coolant.......................................................353

Overview............................................................................................................................................... 353

10.3 Miscellaneous functions for coordinate data...................................................................................354

Programming machine-referenced coordinates: M91/M92.................................................................. 354

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130...................356

10.4 Miscellaneous functions for path behavior......................................................................................357

Machining small contour steps: M97................................................................................................... 357

Machining open contour corners: M98................................................................................................ 358

Feed rate factor for plunging movements: M103.................................................................................359

Feed rate in millimeters per spindle revolution: M136.........................................................................360

Feed rate for circular arcs: M109/M110/M111.......................................................................................361

Calculating the radius-compensated path in advance (LOOK AHEAD): M120......................................362

Superimposing handwheel positioning during program run: M118...................................................... 364

Retraction from the contour in the tool-axis direction: M140...............................................................366

Suppressing touch probe monitoring: M141........................................................................................ 368

Deleting basic rotation: M143...............................................................................................................369

Automatically retract tool from the contour at an NC stop: M148....................................................... 370

Rounding corners: M197.......................................................................................................................371

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

11 Programming: Special functions.................................................................................................373

11.1 Overview of special functions........................................................................................................... 374

Main menu for SPEC FCT special functions........................................................................................ 374

Program defaults menu........................................................................................................................ 375

Functions for contour and point machining menu................................................................................ 375

Menu of various DIN/ISO functions......................................................................................................376

11.2 Dynamic Collision Monitoring (Option #40).....................................................................................377

Function.................................................................................................................................................377

Graphic display of the collision objects................................................................................................ 378

Collision monitoring in the manual operating modes........................................................................... 380

Collision monitoring in the Program Run operating modes..................................................................381

Activating and deactivating collision monitoring................................................................................... 382

11.3 Adaptive feed control AFC (Option #45).......................................................................................... 384

Application............................................................................................................................................. 384

Defining the AFC basic settings........................................................................................................... 386

Recording a teach-in cut....................................................................................................................... 388

Activating/deactivating AFC...................................................................................................................392

Log file.................................................................................................................................................. 393

Tool breakage/tool wear monitoring......................................................................................................394

Spindle load monitoring........................................................................................................................ 395

11.4 Active Chatter Control ACC (Option #145).......................................................................................396

Application............................................................................................................................................. 396

Activating/deactivating ACC...................................................................................................................397

11.5 Defining DIN/ISO Functions...............................................................................................................398

Overview............................................................................................................................................... 398

11.6 Creating Text Files...............................................................................................................................399

Application............................................................................................................................................. 399

Opening and exiting text files...............................................................................................................399

Editing texts.......................................................................................................................................... 400

Deleting and re-inserting characters, words and lines..........................................................................400

Editing text blocks.................................................................................................................................401

Finding text sections.............................................................................................................................402

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

11.7 Freely definable tables....................................................................................................................... 403

Fundamentals........................................................................................................................................ 403

Creating a freely definable table...........................................................................................................403

Editing the table format........................................................................................................................404

Switching between table and form view..............................................................................................405

D26 – Open a freely definable table.................................................................................................... 406

D27 – Write to a freely definable table................................................................................................ 407

D28 – Read from a freely definable table............................................................................................ 408

11.8 Dwell time FUNCTION FEED DWELL................................................................................................409

Programming dwell time.......................................................................................................................409

Resetting dwell time............................................................................................................................. 410

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

12 Programming: Multiple Axis Machining.................................................................................... 411

12.1 Functions for multiple axis machining............................................................................................. 412

12.2 The PLANE Function: Tilting the working plane (Software Option 8)........................................... 413

Introduction........................................................................................................................................... 413

Overview............................................................................................................................................... 414

Defining the PLANE function................................................................................................................415

Position display......................................................................................................................................415

Resetting the PLANE function.............................................................................................................. 416

Defining the working plane with the spatial angle: PLANE SPATIAL....................................................417

Defining the working plane with the projection angle: PLANE PROJECTED....................................... 419

Defining the working plane with the Euler angle: PLANE EULER........................................................420

Defining the working plane with two vectors: PLANE VECTOR.......................................................... 422

Defining the working plane via three points: PLANE POINTS..............................................................424

Defining the working plane via a single incremental spatial angle: PLANE SPATIAL............................426

Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)......................................427

Specifying the positioning behavior of the PLANE function.................................................................429

Tilt the working plane without rotary axes...........................................................................................434

12.3 Inclined-tool machining in a tilted plane (Option #9)..................................................................... 435

Function.................................................................................................................................................435

Inclined-tool machining via incremental traverse of a rotary axis......................................................... 435

12.4 Miscellaneous functions for rotary axes.......................................................................................... 436

Feed rate in mm/min on rotary axes A, B, C: M116 (Option #8).......................................................... 436

Shortest-path traverse of rotary axes: M126........................................................................................437

Reducing display of a rotary axis to a value less than 360°: M94........................................................438

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

(Option #9).............................................................................................................................................439

Selecting tilting axes: M138................................................................................................................. 442

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

M144 (Option #9).................................................................................................................................. 443

12.5 Peripheral Milling: 3-D radius compensation with M128 and radius compensation (G41/

G42).......................................................................................................................................................444

Application............................................................................................................................................. 444

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

13 Programming: Pallet editor......................................................................................................... 445

13.1 Pallet management............................................................................................................................. 446

Application............................................................................................................................................. 446

Select pallet table................................................................................................................................. 448

Exiting the pallet file............................................................................................................................. 448

Run pallet file........................................................................................................................................ 448

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

14 Programming: Turning Operations............................................................................................. 451

14.1 Turning Operations on Milling Machines (Option #50)................................................................... 452

Introduction........................................................................................................................................... 452

14.2 Basic functions (Option 50)............................................................................................................... 453

Switching between milling/turning mode of operation......................................................................... 453

Graphical display of turning operations.................................................................................................455

Program spindle speed......................................................................................................................... 456

Feed rate............................................................................................................................................... 457

14.3 Unbalance functions (Option #50).................................................................................................... 458

Unbalance while turning....................................................................................................................... 458

Measure Unbalance cycle.....................................................................................................................460

14.4 Tools in turning mode (Option #50).................................................................................................. 461

Tool call..................................................................................................................................................461

Tool compensation in the program....................................................................................................... 462

Tool data................................................................................................................................................ 463

Tool tip radius compensation TRC........................................................................................................ 468

14.5 Turning program functions (Option #50).......................................................................................... 469

Recessing and undercutting..................................................................................................................469

Blank form update TURNDATA BLANK................................................................................................ 475

Inclined turning......................................................................................................................................476

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

15 Manual operation and setup.......................................................................................................479

15.1 Switch-on, switch-off..........................................................................................................................480

Switch-on...............................................................................................................................................480

Switch-off...............................................................................................................................................482

15.2 Moving the machine axes..................................................................................................................483

Note.......................................................................................................................................................483

Moving the axis with the machine axis direction buttons.................................................................... 483

Incremental jog positioning...................................................................................................................483

Traverse with electronic handwheels....................................................................................................484

15.3 Spindle speed S, feed rate F and miscellaneous function M......................................................... 494

Application............................................................................................................................................. 494

Entering values......................................................................................................................................494

Adjusting spindle speed and feed rate................................................................................................. 495

Activating feed-rate limitation............................................................................................................... 495

15.4 Optional safety concept (Functional safety FS)............................................................................... 496

Miscellaneous........................................................................................................................................496

Explanation of terms............................................................................................................................. 497

Checking the axis positions.................................................................................................................. 498

Activating feed-rate limitation............................................................................................................... 498

Additional status displays......................................................................................................................499

15.5 Datum management with the preset table......................................................................................500

Note.......................................................................................................................................................500

Saving the datums in the preset table................................................................................................. 501

Activating the datum.............................................................................................................................506

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

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

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

Setting datum with an end mill............................................................................................................ 507

Using touch probe functions with mechanical probes or measuring dials............................................508

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

15.7 Using 3-D touch probes..................................................................................................................... 509

Overview............................................................................................................................................... 509

Functions in touch probe cycles........................................................................................................... 511

Selecting touch probe cycles................................................................................................................513

Recording measured values from the touch-probe cycles................................................................... 514

Writing measured values from the touch probe cycles in a datum table............................................. 515

Writing measured values from the touch probe cycles in the preset table..........................................516

15.8 Calibrating a 3-D touch trigger probe...............................................................................................517

Introduction........................................................................................................................................... 517

Calibrating the effective length............................................................................................................. 518

Calibrating the effective radius and compensating center misalignment............................................. 519

Displaying calibration values................................................................................................................. 522

15.9 Compensating workpiece misalignment with 3-D touch probe.................................................... 523

Introduction........................................................................................................................................... 523

Identifying basic rotation.......................................................................................................................524

Saving a basic rotation in the preset table...........................................................................................524

Compensation of workpiece misalignment by rotating the table.........................................................524

Displaying a basic rotation.................................................................................................................... 525

Canceling a basic rotation.....................................................................................................................525

Measuring 3-D basic rotation................................................................................................................525

15.10Datum setting with 3-D touch probe................................................................................................527

Overview............................................................................................................................................... 527

Datum setting in any axis..................................................................................................................... 527

Corner as datum................................................................................................................................... 528

Circle center as datum..........................................................................................................................529

Setting a center line as datum............................................................................................................. 531

Measuring workpieces with a 3-D touch probe................................................................................... 532

15.11Tilting the working plane (Option #8).............................................................................................. 535

Application, function..............................................................................................................................535

Traversing reference points in tilted axes............................................................................................. 537

Position display in a tilted system........................................................................................................ 537

Limitations on working with the tilting function...................................................................................537

To activate manual tilting:..................................................................................................................... 538

Setting the current tool-axis direction as the active machining direction..............................................539

Setting the datum in a tilted coordinate system.................................................................................. 540

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

16 Positioning with Manual Data Input.......................................................................................... 541

16.1 Programming and executing simple machining operations...........................................................542

Positioning with manual data input (MDI)............................................................................................ 542

Protecting and erasing programs in $MDI............................................................................................545

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

17 Test run and program run........................................................................................................... 547

17.1 Graphics................................................................................................................................................548

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

Speed of the Setting test runs.............................................................................................................549

Overview: Display modes..................................................................................................................... 550

3-D view................................................................................................................................................ 551

Plan view...............................................................................................................................................554

Projection in three planes..................................................................................................................... 554

Repeating graphic simulation................................................................................................................556

Tool display............................................................................................................................................556

Measurement of machining time......................................................................................................... 557

17.2 Showing the workpiece blank in the working space......................................................................558

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

17.3 Functions for program display.......................................................................................................... 559

Overview............................................................................................................................................... 559

17.4 Test Run................................................................................................................................................560

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

17.5 Program run.........................................................................................................................................562

Application............................................................................................................................................. 562

Running a part program........................................................................................................................ 563

Interrupt machining............................................................................................................................... 564

Moving the machine axes during an interruption................................................................................. 565

Resuming program run after an interruption........................................................................................ 565

Retraction after a power interruption....................................................................................................567

Any entry into program (mid-program startup).....................................................................................569

Returning to the contour.......................................................................................................................571

17.6 Automatic program start....................................................................................................................572

Application............................................................................................................................................. 572

17.7 Optional block skip............................................................................................................................. 573

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

Inserting the "/" character......................................................................................................................573

Erasing the "/" character........................................................................................................................573

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

17.8 Optional program-run interruption....................................................................................................574

Application............................................................................................................................................. 574

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

18 MOD functions..............................................................................................................................575

18.1 MOD function...................................................................................................................................... 576

Selecting MOD functions......................................................................................................................576

Changing the settings........................................................................................................................... 576

Exiting MOD functions..........................................................................................................................576

Overview of MOD functions................................................................................................................ 577

18.2 Graphic settings.................................................................................................................................. 578

18.3 Machine settings.................................................................................................................................579

External access..................................................................................................................................... 579

Entering traverse limits......................................................................................................................... 581

Tool usage file....................................................................................................................................... 582

Select kinematics.................................................................................................................................. 583

18.4 System settings...................................................................................................................................584

Set the system time............................................................................................................................. 584

18.5 Select the position display................................................................................................................ 585

Application............................................................................................................................................. 585

18.6 Setting the unit of measure.............................................................................................................. 586

Application............................................................................................................................................. 586

18.7 Displaying operating times................................................................................................................586

Application............................................................................................................................................. 586

18.8 Software numbers...............................................................................................................................587

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

18.9 Entering the code number................................................................................................................. 587

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Contents

18.10Setting up data interfaces..................................................................................................................588

Serial interfaces on the TNC 640......................................................................................................... 588

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

Setting the RS-232 interface.................................................................................................................588

Setting the BAUD RATE (baudRate)..................................................................................................... 588

Setting the protocol (protocol).............................................................................................................. 589

Setting data bits (dataBits)....................................................................................................................589

Check parity (parity).............................................................................................................................. 589

Setting the stop bits (stopBits).............................................................................................................589

Setting handshaking (flowControl)........................................................................................................ 590

File system for file operations (fileSystem).......................................................................................... 590

Block Check Character (bccAvoidCtrlChar)............................................................................................590

Condition of RTS line (rtsLow)..............................................................................................................590

Define behavior after reception of ETX (noEotAfterEtx).......................................................................591

Settings for data transfer with the TNCserver PC software.................................................................591

Setting the operating mode of the external device (fileSystem).......................................................... 592

Data transfer software.......................................................................................................................... 592

18.11 Ethernet interface................................................................................................................................594

Introduction........................................................................................................................................... 594

Connection options............................................................................................................................... 594

Configuring the TNC............................................................................................................................. 594

18.12Firewall................................................................................................................................................. 600

Application............................................................................................................................................. 600

18.13Configure HR 550 FS wireless handwheel....................................................................................... 603

Application............................................................................................................................................. 603

Assigning the handwheel to a specific handwheel holder................................................................... 603

Setting the transmission channel..........................................................................................................604

Selecting the transmitter power........................................................................................................... 604

Statistical data.......................................................................................................................................605

18.14Load machine configuration.............................................................................................................. 606

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

19 Tables and overviews...................................................................................................................607

19.1 Machine-specific user parameters.....................................................................................................608

Application............................................................................................................................................. 608

19.2 Connector pin layout and connection cables for data interfaces...................................................620

RS-232-C/V.24 interface for HEIDENHAIN devices...............................................................................620

Non-HEIDENHAIN devices....................................................................................................................622

Ethernet interface RJ45 socket............................................................................................................ 623

19.3 Technical Information..........................................................................................................................624

19.4 Overview tables...................................................................................................................................632

Fixed cycles...........................................................................................................................................632

Miscellaneous functions....................................................................................................................... 633

19.5 Functions of the TNC 640 and the iTNC 530 compared................................................................. 635

Comparison: Specifications...................................................................................................................635

Comparison: Data interfaces.................................................................................................................635

Comparison: Accessories......................................................................................................................636

Comparison: PC software..................................................................................................................... 636

Comparison: Machine-specific functions.............................................................................................. 637

Comparison: User Functions.................................................................................................................637

Comparator: Cycles...............................................................................................................................644

Comparison: Miscellaneous functions.................................................................................................. 647

Comparison: Touch probe cycles in the Manual Operation and El. Handwheel modes........................649

Comparison: Touch probe cycles for automatic workpiece inspection................................................. 650

Comparison: Differences in programming............................................................................................ 651

Comparison: Differences in Test Run, functionality..............................................................................656

Comparison: Differences in Test Run, operation.................................................................................. 656

Comparison: Differences in Manual Operation, functionality............................................................... 656

Comparison: Differences in Manual Operation, operation....................................................................658

Comparison: Differences in Program Run, operation........................................................................... 658

Comparison: Differences in Program Run, traverse movements..........................................................659

Comparison: Differences in MDI operation.......................................................................................... 663

Comparison: Differences in programming station................................................................................ 664

19.6 DIN/ISO function overview................................................................................................................665

DIN/ISO Function Overview TNC 640.................................................................................................. 665

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with

the TNC 640

First Steps with the TNC 640

1.1 Overview

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

The following topics are included in this chapter:

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

1.2 Machine switch-on

Acknowledging the power interruption and moving to the reference points

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

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

Press the CE key: The TNC compiles the PLC program

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

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

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

Further information on this topic

Traversing the reference marks: see "Switch-on", page 480 Operating modes: see "Programming", page 74

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

ENT

1.3 Programming the first part

Selecting the correct operating mode

You can write programs only in Programming mode:

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

Further information on this topic

Operating modes: see "Programming", page 74

The most important TNC keys

Key Functions for conversational guidance

Confirm entry and activate the next dialog prompt

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 operating state

Further information on this topic

Writing and editing programs: see "Editing a program", page 106

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.3 Programming the first part

Opening a new program/file management

Press the PGM MGT key: The TNC opens the file manager. The file management of the TNC is arranged much like the file management on a PC with the Windows Explorer. The file management enables you to manage data on the internal memory of the TNC

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

Confirm with the ENT key: The control asks you for the unit of measurement for the new program

Select 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 114

Creating a new program: see "Opening programs and entering", page 99

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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: Enter the 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: Enter the 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: Enter the 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: Enter the largest Z coordinate of the workpiece blank with respect to the reference point, e.g. 0. Confirm with the ENT key. The TNC concludes the dialog

Example NC blocks

%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

Defining the workpiece blank: page 103

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 *

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 G17

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 G00 soft key if you want to enter a rapid traverse motion

Programming the first part 1.3

Press the G90 soft key for absolute values

Retract tool: Press the orange axis key Z and enter the value for the position to be approached, e.g.

250. Press the ENT key Activate no radius compensation: Press the G40

soft key Confirm Miscellaneous function M? with the END

key: The TNC saves 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 G00 soft key if you want to enter a rapid

traverse motion Preposition the tool in the working plane: Press

the orange X axis key and enter the value for the position to be approached, e.g. –20

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

Activate no radius compensation: Press the G40 soft key

Confirm Miscellaneous function M? with the END key: The TNC saves 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 G00 soft key if you want to enter a rapid traverse motion

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.3 Programming the first part

Activate no radius compensation: Press the G40 soft key

Miscellaneous function M? Switch on the spindle and coolant, e.g. M13, confirm with the END key: The TNC saves the entered positioning block

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

Enter the coordinates of the contour starting point

1 in X and Y, e.g. 5/5. Confirm with the ENT key

Activate radius compensation to the left of the path: Press the G41 soft key

Feed rate F=? Enter the machining feed rate, e.g. 700 mm/min, save your entry with the END key

Enter 26 to approach the contour: Define for the circular arc, save entries with the END key

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

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

Define chamfer G24 on contour point 3: Enter 10 mm, save with the END key

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

Define chamfer G24 on contour point 4: Enter 20 mm, save with the END key

Move to 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 of the departing arc

Depart contour: Enter coordinates outside of the workpiece in X and Y, e.g. -20/-20, confirm with the ENT key

Activate no radius compensation: Press the G40 soft key

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

Press the G00 soft key if you want to enter a rapid traverse motion

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

Activate no radius compensation: Press the G40 soft key

MISCELLANEOUS FUNCTION M? Enter M2 to end the program and confirm with the END key: The TNC saves the entered positioning block

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Further information on this topic

Complete example with NC blocks: see "Example: Linear

movements and chamfers with Cartesian coordinates",

page 229

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

page 99

Approaching/departing contours: see "Approaching and

departing a contour"

Programming contours: see "Overview of path functions",

page 220

Tool radius compensation: see "Tool radius compensation ",

page 199

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

inspection, spindle and coolant ", page 353

Programming the first part 1.3

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.3 Programming the first part

Creating a cycle program

The holes (depth of 20 mm) shown in the figure at right are to be drilled with a standard drilling cycle. You have already defined the workpiece blank.

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

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 G00 soft key if you want to enter a rapid traverse motion

Press the G90 soft key for absolute values Retract tool: Press the orange axis key Z and enter

the value for the position to be approached, e.g.

250. Press the ENT key Activate no radius compensation: Press the G40

soft key Miscellaneous function M? Switch on the spindle

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

Call the cycle menu

Display the drilling cycles

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

Enter 0 to approach the first drilling position: Enter the coordinates of the drilling position, call the cycle with M99

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

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

Miscellaneous function M? Enter M2 to end the program and confirm with the END key: The TNC saves the entered positioning block

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Example NC blocks

%C200 G71 *

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

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

N30 T5 G17 S4500 *

N40 G00 G90 Z+250 G40 *

N50 G200

Q200=2 ;SET-UP CLEARANCE

Q201=-20 ;DEPTH

Q206=250 ;FEED RATE FOR PLNGNG

Q202=5 ;

Q210=0 ;DWELL TIME AT TOP

Q203=-10 ;SURFACE COORDINATE

Q204=20 ;2ND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT DEPTH

N60 G00 X+10 Y+10 M13 M99 *

N70 G00 X+10 Y+90 M99 *

N80 G00 X+90 Y+10 M99 *

N90 G00 X+90 Y+90 M99 *

N100 G00 Z+250 M2 *

N99999999 %C200 G71 *

Programming the first part 1.3

Definition of workpiece blank

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 99

Cycle programming: See User’s Manual for Cycles, "Cycle

fundamentals / Overviews"

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.4 Graphically testing the first part

Selecting the correct operating mode

You can test programs in the Test Run mode:

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

Further information on this topic

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

page 73

Testing programs: see "Test Run", page 560

Selecting the tool table for the test run

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

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

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

Press the 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:\table directory

Move the highlight to the right onto the files

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

Press the END key: Exit the file manager

Further information on this topic

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

page 172

Testing programs: see "Test Run", page 560

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Choosing the program you want to test

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

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

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

Further information on this topic

Selecting a program: see "Working with the File Manager",

page 114

Selecting the screen layout and the view

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

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

Press the FURTHER VIEW OPTIONS soft key

Graphically testing the first part 1.4

Shift the soft-key row and select the desired view by soft key

The TNC features the following views:

Soft keys Function

Volume view

Volume view and tool paths

Tool paths

Further information on this topic

Graphic functions: see "Graphics ", page 548

Running a test run: see "Test Run", page 560

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.4 Graphically testing the first part

Starting the test run

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

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

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

Press the START soft key: The TNC resumes the test run after a break

Further information on this topic

Running a test run: see "Test Run", page 560

Graphic functions: see "Graphics ", page 548

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

runs", page 549

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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

Setting up tools 1.5

Preparing and measuring tools

Clamp the required tools in their tool holders

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, see page 65

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.5 Setting up tools

The tool table TOOL.T

In the tool table TOOL.T (permanently saved under TNC:\table\), save the tool data such as length and radius, but also further toolspecific information that the TNC needs to perform its functions.

To enter tool data in the tool table TOOL.T, proceed as follows:

Display the tool table: The TNC shows 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 172

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

The pocket table TOOL_P.TCH

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

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

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

Display the tool table: 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.

Setting up tools 1.5

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 181

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.6 Workpiece setup

Selecting the correct operating mode

Workpieces are set up in the or mode

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

Further information on this topic

Operating mode : see "Moving the machine axes", page 483

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.

Further information on this topic

Setting datums with 3-D touch probe: see "Datum setting with

3-D touch probe ", page 527

Setting datums without 3-D touch probe: see "Datum setting

without a 3-D touch probe", page 507

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Datum setting with 3-D touch probe

Insert a 3-D touch probe: In the Positioning with Manual Data

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

then return to the Manual Operation mode

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

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

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

defined direction until it contacts the workpiece and then automatically returns to its starting point

Use the axis-direction keys to pre-position the touch probe to a position near the second touch point on the first workpiece edge

Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point

Use the axis-direction keys to pre-position the touch probe to a position near the first touch point on the second workpiece edge

Select the probing direction via soft key Press NC start: The touch probe moves in the

defined direction until it contacts the workpiece and then automatically returns to its starting point

Use the axis-direction keys to pre-position the touch probe to a position near the second touch point on the second workpiece edge

Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point

Then the TNC shows the coordinates of the measured corner point

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

Workpiece setup 1.6

Further information on this topic

Datum setting: see "Datum setting with 3-D touch probe ",

page 527

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

First Steps with the TNC 640

1.7 Running the first program

Selecting the correct operating mode

You can run programs either in the Single Block or the Full Sequence mode:

Press the operating mode key: The TNC goes into the Program Run, Single Block mode and the TNC executes the program block by block. You have to confirm each block with the NC start key

Press the Program Run, Full Sequence operating mode key: The TNC switches to that mode and runs the program after NC start up to a program interruption or to the end of the program

Further information on this topic

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

page 73

Running programs: see "Program run", page 562

Choosing the program you want to run

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

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

If desired, use the arrow keys to select the program that you want to run. Load with the ENT key

Further information on this topic

File Management: see "Working with the File Manager",

page 114

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 562

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.1 The TNC 640

HEIDENHAIN TNC controls are workshop-oriented contouring controls that enable you to program conventional milling and drilling operations right at the machine in an easy-to-use conversational programming language. They are designed for milling, drilling and boring 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: In HEIDENHAIN conversational and DIN/ISO

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 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 or with error messages when the file is opened.

Please also note the detailed description of the differences between the iTNC 530 and the TNC 640, see "Functions of the TNC 640 and the iTNC 530 compared", page 635.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 thin bars immediately above the soft-key row indicate the number of soft-key rows that can be called with the keys to the right and left that are used to switch the soft keys. The bar representing the active soft-key row is highlighted

3 Soft-key selection keys 4 Keys for switching the soft keys 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 Keys for switching the soft keys for machine tool builders

Setting the screen layout

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

To change the screen layout:

Press the screen layout key: The soft-key row shows the available layout options, see "Modes of Operation"

Select the desired screen layout

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

8 9

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 Alpha-numeric keyboard for entering texts and file names, as

well as for DIN/ISO programming

3 Programming modes 4 Machine operating modes 5 Initiating programming dialogs 6 7 Numerical input and axis selection 8 Touchpad 9 Mouse buttons 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.

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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)

Soft key Window

Positions

Modes of Operation 2.3

Left: positions, right: status display

Left: positions, right: collision object

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

Soft key Window

Program

Left: program, right: status display

Left: program, right: collision object

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.3 Modes of Operation

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

Soft key Window

Program

Left: program, right: program structure

Left: program, right: programming graphics

Test Run

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

Soft keys for selecting the screen layout

Soft key Window

Program

Left: program, right: status display

Left: program, right: graphics

Graphic

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Program Run, Full Sequence and Program Run, Single Block

In the Program run full sequence mode of operation the TNC executes a 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. With point pattern cycles and CYCL CALL PAT, the control stops after each point.

Soft keys for selecting the screen layout

Soft key Window

Program

Modes of Operation 2.3

Left: program, right: status display

Left: program, right: graphics

Graphic

Left: program, right: collision object

Collision body

Soft key Window

Pallet table

Left: program, right: pallet table

Left: pallet table, right: status display

Left: pallet table, right: graphics

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.4 Status displays

General status display

The general 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 only, and during

Positioning with Manual Data Input. In the Manual Operation and El. Handwheel modes the status

display appears in the large window.

Information in the status display

Icon Meaning

ACTL. Position display: Actual, nominal or distance-to-go

coordinates mode Machine axes; the TNC displays auxiliary axes in

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

Number of the active presets from the preset table. If the datum was set manually, the TNC displays the text MAN behind the symbol

F S M The displayed feed rate in inches corresponds to

one tenth of the effective value. Spindle speed S, feed rate F and active M functions

Axis is clamped

Axis can be moved with the handwheel

Axes are moving under a basic rotation

Axes are moving under a 3-D basic rotation

Axes are moving in a tilted working plane

The M128 is active

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Icon Meaning

No active program

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 (Option #40)

Status displays 2.4

The Adaptive Feed Function (AFC) is active (Option #45)

The Active Chatter Control feature (ACC) is active (Option #145)

The CTC function is active (Option #141)

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 screen layout with additional status display: In the right half of the screen, the TNC shows the OVERVIEW status form

To select an additional status display

Switch the soft-key rows until the STATUS soft keys appear

Either select the additional status display directly by soft key, e.g. positions and coordinates, or

use the switch-over soft keys to select the desired view

The available status displays described below can be selected either directly by soft key or with the switch-over soft keys.

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.4 Status displays

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

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 ManualDIN/ISO Programming | 1/2015

Program section repeat/Subprograms (LBL tab)

Soft key Meaning

Status displays 2.4

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 subprograms with block number in which the subprogram was called and the label number that was called

Active fixed cycle

Active values of Cycle 32 Tolerance

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.4 Status displays

Active miscellaneous functions M (M tab)

Soft key Meaning

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 ManualDIN/ISO Programming | 1/2015

Information on tools (TOOL tab)

Soft key Meaning

Display of active tool:

T: Tool number and tool name

RT: Number and name of a replacement tool Tool axis Tool length and tool 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

Status displays 2.4

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 tolerance in the tool table was exceeded

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.4 Status displays

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

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

Press the Q PARAMETER LIST soft key. The TNC opens a pop-up window. For each parameter type (Q, QL, QR, QS), define the parameter numbers you wish to control. Separate single Q parameters with a comma, and connect sequential Q parameters with a hyphen, e.g. 1,3,200-208. The input range per parameter type is 132 characters.

The display in the QPARA tab always contains eight decimal places. The result of Q1 = COS 89.999 is shown by the control as 0.00001745 for example. Very large or very small values are displayed by the control in exponential notation. The result of Q1 = COS 89.999 * 0.001 is shown by the control as +1.74532925e-08, whereby e-08 corresponds to the factor of 10-8.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Adaptive Feed Control (AFC tab, Option #45)

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

Soft key Meaning

Status displays 2.4

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.5 Window Manager

The machine tool builder determines the available functions and behavior of the window manager. Refer to your machine manual.

The TNC features the Xfce window manager. Xfce is a standard application for UNIX-based operating systems, and is used to manage graphical user interfaces. The following functions are possible with the window manager:

Display a task bar for switching between various applications (user interfaces).

Manage an additional desktop, on which special applications from your machine tool builder can run.

Control the focus between NC-software applications and those of the machine tool builder.

The size and position of pop-up windows can be changed. It is also possible to close, minimize and restore the pop-up windows.

The TNC shows a star in the upper left of the screen if an application of the window manager or the window manager itself has caused an error In this case, switch to the window manager and correct the problem. If required, refer to your machine manual.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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 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 Remote Desktop Manager (Option #133): Display and remote

operation of external computer units Diagnostics: Available only to authorized specialists to start

diagnostic functions

Settings: Configuration of miscellaneous settings

Date/Time: Set the date and time Language: System dialog language setting. During startup

the TNC overwrites this setting with the language setting of the machine parameter CfgLanguage

Network: Network settings of the control Screensaver: Screensaver settings SELinux: Security software settings for Linux-based

operating systems

Shares: Settings for external network drives VNC: Setting for external softwares that access for

maintenance purposes on the control for example (Virtual

Network Computing)

WindowManagerConfig: Available only to authorized specialists for setting the window manager

Firewall: Firewall settings see "Firewall", page 600

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 Management: Fundamentals", page 111)

Window Manager 2.5

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.6 Remote Desktop Manager (Option #133)

Introduction

The Remote Desktop Manager enables you to display external computer units on the TNC screen that are connected via Ethernet and to operate them over the TNC. You can also start programs specifically under HeROS or display web pages of an external server.

The following connection options are available:

Windows Terminal Server (RDP): Displays the desktop of a remote Windows computer on the control

Windows Terminal Server (RemoteFX): Displays the desktop of a remote Windows computer on the control

VNC: Connection to an external computer (e.g. HEIDENHAINIPC). Displays the desktop of a remote Windows or Unix computer on the control

Switch-off/restart of a computer: Available only to authorized specialists

World Wide Web: Available only to authorized specialists SSH: Available only to authorized specialists XDMCP: Available only to authorized specialists User-defined connection: Available only to authorized

specialists

HEIDENHAIN assures a functioning connection between HeROS 5 and the IPC 6341. HEIDENHAIN cannot guarantee the correct function of any other combinations or connections to external devices.

Configuring connections – Windows Terminal Service

Configuring an external computer

You do not need additional software for your external computer for connecting to the Windows Terminal Service.

Proceed as follows to configure the external computer, e.g. in the Windows 7 operating system:

After pressing the Windows start button select the menu item

System control via the task bar

Select the System menu item Select the Advanced system settings menu item Select the Remote tab

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Remote Desktop Manager (Option #133) 2.6

In the Remote support area, activate the function Permit

remote support connection with this computer

In the Remote desktop area, activate the function Permit

connections from computers on which any version of remote desktop is installed

Confirm the settings via the OK button

Configuring the TNC

Depending on the operating system of your external computer and the protocol used in accordance with this, select either Windows Terminal Service (RDP) or Windows Terminal Service (RemoteFX).

Configure the TNC as follows:

After pressing the green HEIDENHAIN button, select the menu item Remote Desktop Manager via the task bar

Press the New connection button in the Remote Desktop Manager window

Select the menu item Windows Terminal Service (RDP) or

Windows Terminal Service (RemoteFX)

Specify the required connection information in the Edit connection window

Setting Meaning Input

Connection name

Restarting after end of connection

Automatic starting upon login

Add to favorites

Move to the following workspace

Release USB mass memory

Name of the connection in the Remote Desktop Manager Required Behavior with terminated connection:

Always restart Never restart Always after an error Ask after an error

Connection automatically established during control power-up Required

Connection icon in the task bar:

Double click with left mouse button: The control starts the connection

Single click with left mouse button: The control changes to the desktop of the connection

Single click with right mouse button: The control displays the connection menu

Number of desktop for the connection, whereby desktops 0 and 1 are reserved for the NC software

Enable access to connected USB mass memory Required

Required

Computer

User name

Password

Windows domain Full screen mode or user-

defined window size

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Host name or IP address of the external computer Required Name of the user Required User password Required Domain of the external computer Required Size of the connection window Required

Introduction

2.6 Remote Desktop Manager (Option #133)

Setting Meaning Input

Entries in the Advanced options area

Available only to authorized specialists Optional

Configuring the connection – VNC

Configuring an external computer

You do not need an additional VNC server for your external computer for connecting to VNC.

Install and configure the VNC server, e.g. the TightVNC server, before configuring the TNC.

Configuring the TNC

Configure the TNC as follows:

Select the Remote Desktop Manager menu item via the task bar

Press the New connection button in the Remote Desktop Manager window

Select the VNC menu item Specify the required connection information in the

Edit connection window

Setting Meaning Input

Connection name

Restarting after end of connection

Automatic starting upon login

Add to favorites

Move to the following workspace

Release USB mass memory

Computer

Name of the connection in the Remote Desktop Manager Required Behavior with terminated connection:

Always restart Never restart Always after an error Ask after an error

Connection automatically established during control power-up Required

Connection icon in the task bar:

Double click with left mouse button: The control starts the connection

Single click with left mouse button: The control changes to the desktop of the connection

Single click with right mouse button: The control displays the connection menu

Number of desktop for the connection, whereby desktops 0 and 1 are reserved for the NC software

Permit access to connected USB mass memory Required Host name or IP address of the external computer Required

Required

Password Full screen mode or user-

defined window size

Permit further connections (share)

Password for connecting to the VNC server Required Size of the connection window Required

Enable access to the VNC server also by other VNC connections Required

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Remote Desktop Manager (Option #133) 2.6

Setting Meaning Input

View only Entries in the Advanced

options area

The external computer cannot be operated in display mode Required Available only to authorized specialists Optional

Starting and stopping the connection

Once a connection has been configured, it is shown as an icon in the Remote Desktop Manager window. Click the connection icon with the right mouse key to open a menu in which the display can be started and stopped.

Use the right DIADUR key on the keyboard to change to Desktop 3 and back to the TNC interface. You can also use the task bar to get to this desktop.

If the desktop of the external connection or the external computer is active, all inputs from the mouse and the keyboard are transmitted there.

All connections are canceled automatically when the HEROS 5 operating system is shut down. Please note, however, that only the connection is canceled, whereas the external computer or the external system is not shut down automatically.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

2.7 SELinux security software

SELinux is an extension for Linux-based operating systems.

SELinux is an additional security software package based on Mandatory Access Control (MAC) and protects the system against the running of unauthorized processes or functions and therefore protects against viruses and other malware.

MAC means that each action must be specifically permitted otherwise the TNC will not run it. The software is intended as protection in addition to the normal access restriction in Linux. Certain processes and actions can only be executed if the standard functions and access control of SELinux permit it.

The SELinux installation of the TNC is prepared to permit running of only those programs installed with the HEIDENHAIN NC software. Other programs cannot be run with the standard installation.

The access control of SELinux under HEROS 5 is regulated as follows:

The TNC runs only those applications installed with the HEIDENHAIN NC software.

Files in connection with the security 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.

USB data carriers cannot be deselected 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 ManualDIN/ISO Programming | 1/2015

Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

2.8 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

The triggering touch probes TS 220, TS 440, TS 444, TS 640 and TS 740

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.

2.8

Handwheels

TT 140 tool touch probe for tool measurement

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Introduction

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

HR electronic handwheels

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

Programming:

Fundamentals, File

Management

Programming: Fundamentals, File Management

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.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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.

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 ManualDIN/ISO Programming | 1/2015

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

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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

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 ManualDIN/ISO Programming | 1/2015

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.

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

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.

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 ManualDIN/ISO Programming | 1/2015

Programming: Fundamentals, File Management

3.2 Opening programs and entering

Define the blank: G30/G31

Immediately after initiating a new program, you define an unmachined workpiece blank. If you wish to define the blank at a later stage, press the SPEC FCT key, the 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 rectangular 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

100

TNC 640 | User's ManualDIN/ISO Programming | 1/2015

heidenhain TNC 640 Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

TNC 640

Controls of the TNC

Keys on visual display unit

Alphanumeric keyboard

Programming modes

Program/file management, TNC functions

Machine operating modes

Navigation keys

Potentiometer for feed rate and spindle speed

Cycles, subprograms and program section repeats

Tool functions

Special functions

Entering and editing coordinate axes and numbers

Programming path movements

Fundamentals

About this manual

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

TNC model, software and features

Software options

Feature Content Level (upgrade functions)

Intended place of operation

Legal information

New functions

Contents

1.1 Overview

1.2 Machine switch-on

Acknowledging the power interruption and moving to the reference points

1.3 Programming the first part

Selecting the correct operating mode

The most important TNC keys

Opening a new program/file management

Defining a workpiece blank

Program layout

Programming a simple contour

Creating a cycle program

1.4 Graphically testing the first part

Selecting the correct operating mode

Selecting the tool table for the test run

Choosing the program you want to test

Selecting the screen layout and the view

Starting the test run

1.5 Setting up tools

Selecting the correct operating mode

Preparing and measuring tools

The tool table TOOL.T

The pocket table TOOL_P.TCH

1.6 Workpiece setup

Selecting the correct operating mode

Clamping the workpiece

Datum setting with 3-D touch probe

1.7 Running the first program

Selecting the correct operating mode

Choosing the program you want to run

Start the program

Introduction

2.1 The TNC 640

Programming: In HEIDENHAIN conversational and DIN/ISO

Compatibility

Visual display unit and operating panel 2.2

Display screen

Setting the screen layout

Control Panel

2.3 Modes of Operation

Manual Operation and El. Handwheel

Positioning with Manual Data Input

Programming

Test Run

Program Run, Full Sequence and Program Run, Single Block

2.4 Status displays

General status display

Additional status displays

2.5 Window Manager

Task bar

Introduction

2.6 Remote Desktop Manager (Option #133)

Configuring connections – Windows Terminal Service