HEIDENHAIN TNC 410 User Manual

TNC 410
TNC 426
TNC 430

NC Software
286 060-xx
286 080-xx
280 476-xx
280 477-xx

User’s Manual

ISO Programming

English (en)

8/2002

Controls on the visual display unit

Split screen layout
Switch between machining or

programming modes
Soft keys for selecting functions in screen

Switching the soft-key rows
Changing the screen settings

(only BC 120)

Typewriter keyboard for entering letters and symbols

File names
Comments

ISO
programs

Machine operating modes

MANUAL OPERATION

ELECTRONIC HANDWHEEL

POSITIONING WITH MDI

PROGRAM RUN, SINGLE BLOCK

PROGRAM RUN, FULL SEQUENCE

Programming modes

PROGRAMMING AND EDITING

TEST RUN

Program/file management, TNC functions

Select or delete programs and files
External data transfer

Enter program call in a program

MOD functions

Display help texts for NC error messages

Pocket calculator

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

Go directly to blocks, cycles and parameter

Move highlight

functions

Override control knobs for feed rate/spindle speed

50

100

0

1

F %

50

50

100

0

1

S %

50

Programming path movements

Approach/depart contour

FK free contour programming

Straight line

Circle center/pole for polar coordinates

Circular arc with center

Circular arc with radius

Circular arc with tangential connection

Chamfer

Corner rounding

Tool functions

Enter and call tool length and radius

Cycles, subprograms and program section
repeats

Program stop in a program

Enter touch probe functions in a program

Define and call cycles
Enter and call labels for subprogramming and

program section repeats

Coordinate axes and numbers: Entering and editing

. . .

. . .

Decimal point

Change arithmetic sign

Polar coordinates

Incremental dimensions

Q parameters

Capture actual position

Skip dialog questions, delete words

Confirm entry and resume dialog

End block
Clear numerical entry or TNC error

or delete error message
Abort dialog, delete program section

Select coordinate axes or
enter them into the program

Numbers

TNC models, software and features

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

TNC model NC software no.

TNC 426 CB, TNC 426 PB 280 476-xx

TNC 426 CF, TNC 426 PF 280 477-xx

TNC 426 M 280 476-xx

TNC 426 ME 280 477-xx

TNC 430 CA, TNC 430 PA 280 476-xx

TNC 430 CE, TNC 430 PE 280 477-xx

TNC 430 M 280 476-xx

TNC 430 ME 280 477-xx

TNC 410 286 060-xx

TNC 410 286 080-xx

The suffixes E and F indicate the export versions of the TNC The
export versions of the TNC have the following limitations:

n Linear movement is possible in no more than 4 axes simultaneously.

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

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

n Probing function for the 3-D touch probe
n Digitizing option
n Tool measurement with the TT 130
n Rigid tapping
n Returning to the contour after an interruption

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

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

Touch Probe Cycles User's Manual:

All of the touch probe functions are described in a separate
manual. Please contact HEIDENHAIN if you require a copy
of this User's Manual. ID number: 329 203-xx.

HEIDENHAIN TNC 410, TNC 426, TNC 430 I

Location of use

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.

New features of the NC software 280 476-xx

n Thread milling cycles 262 to 267 (see “Fundamentals of thread

milling” on page 208)

n Tapping Cycle 209 with chip breaking (see “TAPPING WITH CHIP

BREAKING (Cycle G209, not TNC 410)” on page 206)

n Cycle 247(see “DATUM SETTING (Cycle G247, not TNC 410)” on

page 299)

n Entering two miscellaneous functions M (see “Entering

Miscellaneous Functions M” on page 148)

n Program stop with M01 (see “Optional Program Run Interruption”

on page 386)

n Starting NC programs automatically (see “Automatic Program Start

(not TNC 410)” on page 383)

n Selecting the screen layout for pallet tables (see “Screen layout for

executing pallet tables” on page 95)

n New columns in the tool table for managing TS calibration data (see

“Entering tool data in tables” on page 101)

n Management of unlimited calibration data with the TS triggering

touch probes (see User’s Manual for Touch Probe Cycles)

n Cycles for automatic tool measurement with the TT tool touch probe

in ISO (see User's Manual for Touch Probe Cycles)

n New Cycle 440 for measuring the axial displacement of a machine

with the TT tool touch probe (see User's Manual for Touch Probe
Cycles)

n Support of Teleservice functions (see “Teleservice (not TNC 410)”

on page 418)

n Setting the display mode for blocks with more than one line, e.g. for

cycle definitions (see “General User Parameters” on page 422)

n M142 (see “Erasing modal program information: M142 (not TNC

410)” on page 163)

n M143 (see “Erasing the basic rotation: M143 (not TNC 410)” on

page 163)

n M144 (see “Compensating the machine's kinematic configuration

for ACTUAL/NOMINAL positions at end of block: M144 (not TNC

410)” on page 171)

n External access with the LSV-2 interface (see “Permitting/

Restricting external access” on page 419)

II

Changed features of the NC software 280 476-xx

n The feed-rate unit for M136 was changed from µm/rev to mm/rev.

(see “Feed rate in millimeters per spindle revolution: M136 (not TNC

410)” on page 159)

n The size of the contour memory for SL cycles was doubled. (see “SL

Cycles Group II (not TNC 410)” on page 265)

n M91 and M92 are now also possible with tilted working plane. (see

“Positioning in a tilted coordinate system” on page 306)

n Display of the NC program during the execution of pallet tables (see

“Program Run, Full Sequence and Program Run, Single Block” on
page 8) and (see “Screen layout for executing pallet tables” on page

95)

New/Changed Descriptions in this Manual

n TNCremoNT (see “Data transfer between the TNC and

TNCremoNT” on page 398)

n Summary of input formats (see “Input format and unit of TNC

functions” on page 443)

n Mid-program startup of pallet tables (see “Mid-program startup

(block scan)” on page 380)

n Exchanging the buffer battery (see “Exchanging the Buffer Battery”

on page 445)

HEIDENHAIN TNC 410, TNC 426, TNC 430 III

Contents

Introduction

1

Manual Operation and Setup

Positioning with Manual Data Input
(MDI)

Programming: Fundamentals of File
Management, Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Cycles

Programming: Subprograms and
Program Section Repeats

Programming: Q Parameters

Test Run and Program Run

MOD Functions

2
3
4
5
6
7
8
9

10

11

12

Tables and Overviews

13

1 Introduction ..... 1

1.1 The TNC 410, the TNC 426 and the TNC 430 ..... 2

Programming: HEIDENHAIN conversational and ISO formats ..... 2

Compatibility ..... 2

1.2 Visual Display Unit and Keyboard ..... 3

Visual display unit ..... 3

Screen layout ..... 4

Keyboard ..... 5

1.3 Modes of Operation ..... 6

Manual Operation and Electronic Handwheel ..... 6

Positioning with Manual Data Input (MDI) ..... 6

Programming and editing ..... 7

Test Run ..... 7

Program Run, Full Sequence and Program Run, Single Block ..... 8

1.4 Status Displays ..... 10

“General” status display ..... 10

Additional status displays ..... 11

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels ..... 14

3-D touch probes ..... 14

HR electronic handwheels ..... 15

HEIDENHAIN TNC 410, TNC 426, TNC 430 VII

2 Manual Operation and Setup ..... 17

2.1 Switch-on, Switch-Off ..... 18

Switch-on ..... 18

Additional functions for the TNC 426, TNC 430 ..... 19

Switch-off ..... 19

2.2 Moving the Machine Axes ..... 20

Note ..... 20

To traverse with the machine axis direction buttons: ..... 20

Traversing with the HR 410 electronic handwheel ..... 21

Incremental jog positioning ..... 22

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 23

Function ..... 23

Entering values ..... 23

Changing the spindle speed and feed rate ..... 23

2.4 Datum Setting (Without a 3-D Touch Probe) ..... 24

Note ..... 24

Preparation ..... 24

Datum setting ..... 25

2.5 Tilting the Working Plane (not TNC 410) ..... 26

Application, function ..... 26

Traversing the reference points in tilted axes ..... 27

Setting the datum in a tilted coordinate system ..... 27

Datum setting on machines with rotary tables ..... 28

Position display in a tilted system ..... 28

Limitations on working with the tilting function ..... 28

To activate manual tilting: ..... 29

3 Positioning with Manual Data Input (MDI) ..... 31

3.1 Programming and Executing Simple Machining Operations ..... 32

Positioning with Manual Data Input (MDI) ..... 32

Protecting and erasing programs in $MDI ..... 35

VIII

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

Pallet Management ..... 37

4.1 Fundamentals ..... 38

Position encoders and reference marks ..... 38

Reference system ..... 38

Reference system on milling machines ..... 39

Polar coordinates ..... 40

Absolute and incremental workpiece positions ..... 41

Setting the datum ..... 42

4.2 File Management: Fundamentals ..... 43

Files ..... 43

Data backup TNC 426, TNC 430 ..... 44

4.3 Standard File Management TNC 426, TNC 430 ..... 45

Note ..... 45

Calling the file manager ..... 45

Selecting a file ..... 46

Deleting a file ..... 46

Copying a file ..... 47

Data transfer to or from an external data medium ..... 48

Selecting one of the last 10 files selected ..... 50

Renaming a file ..... 50

Converting an FK program into HEIDENHAIN conversational format ..... 51

Protecting a file / Canceling file protection ..... 52

4.4 Expanded File Management TNC 426, TNC 430 ..... 53

Note ..... 53

Directories ..... 53

Paths ..... 53

Overview: Functions of the expanded file manager ..... 54

Calling the file manager ..... 55

Selecting drives, directories and files ..... 56

Creating a new directory (only possible on the drive TNC:\) ..... 57

Copying a single file ..... 58

Copying a directory ..... 59

Choosing one of the last 10 files selected. ..... 59

Deleting a file ..... 59

Deleting a directory ..... 60

Tagging files ..... 60

Renaming a file ..... 61

Additional functions ..... 61

Data transfer to or from an external data medium ..... 62

Copying files into another directory ..... 63

The TNC in a network (applies only for Ethernet interface option) ..... 64

HEIDENHAIN TNC 410, TNC 426, TNC 430 IX

4.5 File Management for the TNC 410 ..... 66

Calling the file manager ..... 66

Selecting a file ..... 66

Deleting a file ..... 67

Copying a file ..... 68

Data transfer to or from an external data medium ..... 69

4.6 Creating and Writing Programs ..... 71

Organization of an NC program in ISO format ..... 71

Define blank form: G30/G31 ..... 71

Creating a new part program TNC 426, TNC 430 ..... 72

Creating a new part program TNC 410 ..... 73

Define the workpiece blank ..... 74

Programming tool movements ..... 76

Editing a program with TNC 426, TNC 430 ..... 77

Editing a program with TNC 410 ..... 81

4.7 Interactive Programming Graphics (only TNC 410) ..... 83

To generate/not generate graphics during programming: ..... 83

Generating a graphic for an existing program ..... 83

Magnifying or reducing a detail ..... 84

4.8 Adding Comments ..... 85

Function ..... 85

Adding comments during program input (not TNC 410) ..... 85

Adding comments after program input (not TNC 410) ..... 85

Entering a comment in a separate block ..... 85

4.9 Creating Text Files (not TNC 410) ..... 86

Function ..... 86

Opening and exiting text files ..... 86

Editing texts ..... 87

Erasing and inserting characters, words and lines ..... 88

Editing text blocks ..... 88

Finding text sections ..... 89

4.10 Integrated Pocket Calculator (not TNC 410) ..... 90

Operation ..... 90

4.11 Direct Help for NC Error Messages (not TNC 410) ..... 91

Displaying error messages ..... 91

Display HELP ..... 91

4.12 Pallet Management (not TNC 410) ..... 92

Function ..... 92

Selecting a pallet table ..... 94

Leaving the pallet file ..... 94

Executing the pallet file ..... 94

X

5 Programming: Tools ..... 97

5.1 Entering Tool-Related Data ..... 98

Feed rate F ..... 98

Spindle speed S ..... 98

5.2 Tool Data ..... 99

Requirements for tool compensation ..... 99

Tool numbers and tool names ..... 99

Tool length L ..... 99

Tool radius R ..... 100

Delta values for lengths and radii ..... 100

Entering tool data into the program ..... 100

Entering tool data in tables ..... 101

Pocket table for tool changer ..... 107

Calling tool data ..... 109

Tool change ..... 110

5.3 Tool Compensation ..... 111

Introduction ..... 111

Tool length compensation ..... 111

Tool radius compensation ..... 112

5.4 Peripheral Milling: 3-D Radius Compensation with Workpiece Orientation ..... 115

Function ..... 115

HEIDENHAIN TNC 410, TNC 426, TNC 430 XI

6 Programming: Programming Contours ..... 117

6.1 Tool Movements ..... 118

Path functions ..... 118

Miscellaneous functions M ..... 118

Subprograms and program section repeats ..... 118

Programming with Q parameters ..... 118

6.2 Fundamentals of Path Functions ..... 119

Programming tool movements for workpiece machining ..... 119

6.3 Contour Approach and Departure ..... 122

Starting point and end point ..... 122

Tangential approach and departure ..... 124

6.4 Path Contours—Cartesian Coordinates ..... 126

Overview of path functions ..... 126

Straight line at rapid traverse G00

Straight line with feed rate G01 F. . . ..... 127

Inserting a chamfer CHF between two straight lines ..... 128

Rounding corners G25 ..... 129

Circle center I, J ..... 130

Circular path G02/G03/G05 around circle center I, J ..... 131

Circular path G02/G03/G05 with defined radius ..... 132

Circular path G06 with tangential approach ..... 134

6.5 Path Contours—Polar Coordinates ..... 139

Overview of path functions with polar coordinates ..... 139

Zero point for polar coordinates: pole I, J ..... 139

Straight line at rapid traverse G10

Straight line with feed rate G11 F . . . ..... 140

Circular path G12/G13/G15 around pole I, J ..... 140

Circular arc with tangential connection ..... 141

Helical interpolation ..... 141

XII

7 Programming: Miscellaneous Functions ..... 147

7.1 Entering Miscellaneous Functions M ..... 148

Fundamentals ..... 148

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 149

Overview ..... 149

7.3 Miscellaneous Functions for Coordinate Data ..... 150

Programming machine-referenced coordinates: M91/M92 ..... 150

Activating the most recently set datum: M104 (not with TNC 410) ..... 152

Moving to positions in an untilted coordinate system with a tilted working plane: M130 (not with TNC 410) ..... 152

7.4 Miscellaneous Functions for Contouring Behavior ..... 153

Smoothing corners: M90 ..... 153

Insert rounding arc between straight lines: M112 (TNC 426, TNC 430) ..... 154

Entering contour transitions between contour elements: M112 (TNC 410) ..... 154

Contour filter: M124 (not TNC 426, TNC 430) ..... 156

Machining small contour steps: M97 ..... 157

Machining open contours: M98 ..... 158

Feed rate factor for plunging movements: M103 ..... 158

Feed rate in millimeters per spindle revolution: M136 (not TNC 410) ..... 159

Feed rate at circular arcs: M109/M110/M111 ..... 160

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 160

Superimposing handwheel positioning during program run: M118 (not TNC 410) ..... 162

Erasing modal program information: M142 (not TNC 410) ..... 163

Erasing the basic rotation: M143 (not TNC 410) ..... 163

7.5 Miscellaneous Functions for Rotary Axes ..... 164

Feed rate in mm/min on rotary axes A, B, C: M116 (not TNC 410) ..... 164

Shorter-path traverse of rotary axes: M126 ..... 165

Reducing display of a rotary axis to a value less than 360°: M94 ..... 166

Automatic compensation of machine geometry when working with tilted axes: M114 (not TNC 410) ..... 167

Maintaining the position of the tool tip when positioning with tilted axes (TCPM*): M128 (not TNC 410) ..... 168

Exact stop at corners with nontangential transitions: M134 (not TNC 410) ..... 169

Selecting tilting axes: M138 (not TNC 410) ..... 170

Compensating the machine's kinematic configuration for ACTUAL/NOMINAL positions at end of block: M144

(not TNC 410) ..... 171

7.6 Miscellaneous Functions for Laser Cutting Machines (not TNC 410) ..... 172

Principle ..... 172

Output the programmed voltage directly: M200 ..... 172

Output voltage as a function of distance: M201 ..... 172

Output voltage as a function of speed: M202 ..... 173

Output voltage as a function of time (time-dependent ramp): M203 ..... 173

Output voltage as a function of time (time-dependent pulse): M204 ..... 173

HEIDENHAIN TNC 410, TNC 426, TNC 430 XIII

8 Programming: Cycles ..... 175

8.1 Working with Cycles ..... 176

Defining a cycle using soft keys ..... 176

Calling a cycle ..... 177

Working with the secondary axes U/V/W ..... 179

8.2 Point Tables ..... 180

Function ..... 180

Creating a point table ..... 180

Selecting a point table in the program ..... 181

Calling a cycle in connection with point tables ..... 182

8.3 Cycles for Drilling, Tapping and Thread Milling ..... 183

Overview ..... 183

PECKING (Cycle G83) ..... 185

DRILLING (Cycle G200) ..... 186

REAMING (Cycle G201) ..... 187

BORING (Cycle G202) ..... 189

UNIVERSAL DRILLING (Cycle G203) ..... 191

BACK BORING (Cycle G204) ..... 193

UNIVERSAL PECKING (Cycle G205, not TNC 410) ..... 195

BORE MILLING (Cycle G208, not TNC 410) ..... 197

TAPPING with a floating tap holder (Cycle G84) ..... 199

TAPPING NEW with floating tap holder (Cycle G206, not TNC 410) ..... 200

RIGID TAPPING (Cycle G85) ..... 202

RIGID TAPPING NEW (Cycle G207, not TNC 410) ..... 203

THREAD CUTTING (Cycle G86, not TNC 410) ..... 205

TAPPING WITH CHIP BREAKING (Cycle G209, not TNC 410) ..... 206

Fundamentals of thread milling ..... 208

THREAD MILLING (Cycle G262, not TNC 410) ..... 210

THREAD MILLING/COUNTERSINKING (Cycle G263, not TNC 410) ..... 212

THREAD DRILLING/MILLING (Cycle G264) not TNC 410) ..... 216

HELICAL THREAD DRILLING/MILLING (Cycle G265, not TNC 410) ..... 220

OUTSIDE THREAD MILLING (Cycle G267, not TNC 410) ..... 223

8.4 Cycles for Milling Pockets, Studs and Slots ..... 231

Overview ..... 231

POCKET MILLING (Cycles G75, G76) ..... 232

POCKET FINISHING (Cycle G212) ..... 234

STUD FINISHING (Cycle G213) ..... 236

CIRCULAR POCKET MILLING (Cycle G77, G78) ..... 238

CIRCULAR POCKET FINISHING (Cycle G214) ..... 240

CIRCULAR STUD FINISHING (Cycle G215) ..... 242

SLOT MILLING (Cycle G74) ..... 244

SLOT with reciprocating plunge-cut (Cycle G210) ..... 246

CIRCULAR SLOT with reciprocating plunge-cut (Cycle G211) ..... 248

XIV

8.5 Cycles for Machining Hole Patterns ..... 252

Overview ..... 252

CIRCULAR PATTERN (Cycle G220) ..... 254

LINEAR PATTERN (Cycle G221) ..... 256

8.6 SL Cycles Group I ..... 259

Fundamentals ..... 259

Overview of SL Cycles, Group I ..... 260

CONTOUR GEOMETRY (Cycle G37) ..... 261

PILOT DRILLING (Cycle G56) ..... 262

ROUGH-OUT (Cycle G57) ..... 263

CONTOUR MILLING (Cycle G58/G59) ..... 264

8.7 SL Cycles Group II (not TNC 410) ..... 265

Fundamentals ..... 265

Overview of SL Cycles ..... 266

CONTOUR GEOMETRY (Cycle G37) ..... 267

Overlapping contours ..... 267

CONTOUR DATA (Cycle G120) ..... 270

PILOT DRILLING (Cycle G121) ..... 271

ROUGH-OUT (Cycle G122) ..... 272

FLOOR FINISHING (Cycle G123) ..... 273

SIDE FINISHING (Cycle G124) ..... 274

CONTOUR TRAIN (Cycle G125) ..... 275

CYLINDER SURFACE (Cycle G127) ..... 277

CYLINDER SURFACE slot milling (Cycle G128) ..... 279

8.8 Cycles for Multipass Milling ..... 287

Overview ..... 287

RUN DIGITIZED DATA (Cycle G60, not TNC 410) ..... 288

MULTIPLASS MILLING (Cycle G230) ..... 289

RULED SURFACE (Cycle G231) ..... 291

8.9 Coordinate Transformation Cycles ..... 294

Overview ..... 294

Effect of coordinate transformations ..... 294

DATUM SHIFT (Cycle G54) ..... 295

DATUM SHIFT with datum tables (Cycle G53) ..... 296

DATUM SETTING (Cycle G247,

not TNC 410) ..... 299

MIRROR IMAGE (Cycle G28) ..... 300

ROTATION (Cycle G73) ..... 302

SCALING FACTOR (Cycle G72) ..... 303

WORKING PLANE (Cycle G80, not TNC 410) ..... 304

8.10 Special Cycles ..... 311

DWELL TIME (Cycle G04) ..... 311

PROGRAM CALL (Cycle G39) ..... 311

ORIENTED SPINDLE STOP (Cycle G36) ..... 312

TOLERANCE (Cycle G62, not TNC 410) ..... 313

HEIDENHAIN TNC 410, TNC 426, TNC 430 XV

9 Programming: Subprograms and Program Section Repeats ..... 315

9.1 Labeling Subprograms and Program Section Repeats ..... 316

Labels ..... 316

9.2 Subprograms ..... 317

Operating sequence ..... 317

Programming notes ..... 317

Programming a subprogram ..... 317

Calling a subprogram ..... 317

9.3 Program Section Repeats ..... 318

Label G98 ..... 318

Operating sequence ..... 318

Programming notes ..... 318

Programming a program section repeat ..... 318

Calling a program section repeat ..... 318

9.4 Separate Program as Subprogram ..... 319

Operating sequence ..... 319

Programming notes ..... 319

Calling any program as a subprogram ..... 319

9.5 Nesting ..... 320

Types of nesting ..... 320

Nesting depth ..... 320

Subprogram within a subprogram ..... 320

Repeating program section repeats ..... 321

Repeating a subprogram ..... 322

XVI

10 Programming: Q Parameters ..... 329

10.1 Principle and Overview ..... 330

Programming notes ..... 330

Calling Q parameter functions ..... 331

10.2 Part Families—Q Parameters in Place of Numerical Values ..... 332

Example NC blocks ..... 332

Example ..... 332

10.3 Describing Contours through Mathematical Operations ..... 333

Function ..... 333

Overview ..... 333

Programming fundamental operations ..... 334

10.4 Trigonometric Functions ..... 336

Definitions ..... 336

Programming trigonometric functions ..... 337

10.5 If-Then Decisions with Q Parameters ..... 338

Function ..... 338

Unconditional jumps ..... 338

Programming If-Then decisions ..... 338

Abbreviations used: ..... 339

10.6 Checking and Changing Q Parameters ..... 340

Procedure ..... 340

10.7 Additional Functions ..... 341

Overview ..... 341

D14: ERROR: Output error messages ..... 341

D15: PRINT: Output of texts or Q parameter values ..... 345

D19: PLC: Transferring values to the PLC ..... 346

10.8 Entering Formulas Directly ..... 347

Entering formulas ..... 347

Rules for formulas ..... 349

Programming example ..... 350

10.9 Preassigned Q Parameters ..... 351

Values from the PLC: Q100 to Q107 ..... 351

Active tool radius: Q108 ..... 351

Tool axis: Q109 ..... 351

Spindle status: Q110 ..... 351

Coolant on/off: Q111 ..... 352

Overlap factor: Q112 ..... 352

Unit of measurement for dimensions in the program: Q113 ..... 352

Tool length: Q114 ..... 352

Coordinates after probing during program run ..... 352

Deviation between actual value and nominal value during automatic tool measurement with the TT 130 ..... 353

Tilting the working plane with mathematical angles (not TNC 410): Rotary axis coordinates calculated by the

TNC ..... 353

Results of measurements with touch probe cycles (see also Touch Probe Cycles User's Manual) ..... 354

HEIDENHAIN TNC 410, TNC 426, TNC 430 XVII

11 Test Run and Program Run ..... 363

11.1 Graphics ..... 364

Function ..... 364

Overview of display modes ..... 364

Plan view ..... 365

Projection in 3 planes ..... 366

3-D view ..... 367

Magnifying details ..... 367

Repeating graphic simulation ..... 369

Measuring the machining time ..... 370

11.2 Functions for Program Display ..... 371

Overview ..... 371

11.3 Test Run ..... 372

Function ..... 372

11.4 Program Run ..... 374

Function ..... 374

Running a part program ..... 375

Running a part program containing coordinates from non-controlled axes (not TNC 426, TNC 430) ..... 376

Interrupting machining ..... 377

Moving the machine axes during an interruption ..... 378

Resuming program run after an interruption ..... 379

Mid-program startup (block scan) ..... 380

Returning to the contour ..... 382

11.5 Automatic Program Start (not TNC 410) ..... 383

Function ..... 383

11.6 Blockwise Transfer: Running Long Programs (not with TNC 426, TNC 430) ..... 384

Function ..... 384

Blockwise program transfer ..... 384

11.7 Optional block skip ..... 385

Function ..... 385

11.8 Optional Program Run Interruption ..... 386

Function ..... 386

XVIII

12 MOD Functions ..... 387

12.1 MOD functions ..... 388

Selecting the MOD functions ..... 388

Changing the settings ..... 388

Exiting the MOD functions ..... 388

Overview of MOD Functions TNC 426, TNC 430 ..... 388

12.2 System Information (not TNC 426, TNC 430) ..... 390

Function ..... 390

12.3 Software Numbers and Option Numbers (not TNC 410) ..... 391

Function ..... 391

12.4 Code Numbers ..... 392

Function ..... 392

12.5 Setting the Data Interface for the TNC 410 ..... 393

Selecting the setup menu ..... 393

Setting the OPERATING MODE of the external device ..... 393

Setting the BAUD RATE ..... 393

Creating the memory for blockwise transfer ..... 393

Setting the block buffer ..... 393

Data transfer between the TNC 410 and TNCremo ..... 394

12.6 Setting the Data Interfaces for TNC 426, TNC 430 ..... 395

Selecting the setup menu ..... 395

Setting the RS-232 interface ..... 395

Setting the RS-422 interface ..... 395

Setting the OPERATING MODE of the external device ..... 395

Setting the BAUD RATE ..... 395

Assign ..... 396

Software for data transfer ..... 397

12.7 Ethernet Interface (not TNC 410) ..... 400

Introduction ..... 400

Installing an Ethernet card ..... 400

Connection possibilities ..... 400

Configuring the TNC ..... 401

12.8 Configuring PGM MGT (not TNC 410) ..... 406

Function ..... 406

Changing the setting ..... 406

12.9 Machine-Specific User Parameters ..... 407

Function ..... 407

HEIDENHAIN TNC 410, TNC 426, TNC 430 XIX

12.10 Showing the Workpiece in the Working Space (not TNC 410) ..... 408

Function ..... 408

12.11 Position Display Types ..... 410

Function ..... 410

12.12 Unit of Measurement ..... 411

Function ..... 411

12.13 Select the Programming Language for $MDI ..... 412

Function ..... 412

12.14 Selecting the Axes for Generating L Blocks (not TNC 410) ..... 413

Function ..... 413

12.15 Enter the Axis Traverse Limits, Datum Display ..... 414

Function ..... 414

Working without additional traverse limits ..... 414

Find and enter the maximum traverse ..... 415

Datum display ..... 415

Axis traverse limits for

test run (not TNC 426, TNC 430) ..... 415

12.16 The HELP Function ..... 416

Function ..... 416

Selecting and executing a HELP function ..... 416

12.17 Operating Time (via Code Number for TNC 410) ..... 417

Function ..... 417

12.18 Teleservice (not TNC 410) ..... 418

Function ..... 418

Calling/Exiting Teleservice ..... 418

12.19 External Access (not TNC 410) ..... 419

Function ..... 419

XX

13 Tables and Overviews ..... 421

13.1 General User Parameters ..... 422

Input possibilities for machine parameters ..... 422

Selecting general user parameters ..... 422

13.2 Pin Layout and Connecting Cable for the Data Interfaces ..... 436

RS-232-C/V.24 Interface HEIDEHAIN devices ..... 436

Non-HEIDENHAIN devices ..... 437

RS-422/V.11 interface (not TNC 410) ..... 438

Ethernet interface RJ45 socket (option, not TNC 410) ..... 439

Ethernet interface BNC socket (option, not TNC 410) ..... 439

13.3 Technical Information ..... 440

TNC features ..... 440

13.4 Exchanging the Buffer Battery ..... 445

TNC 410 CA/PA, TNC 426 CB/PB, TNC 430 CA/PA ..... 445

TNC 410 M, TNC 426 M, TNC 430 M ..... 445

13.5 Addresses (ISO) ..... 446

G functions ..... 446

Assigned addresses ..... 449

Parameter functions ..... 450

HEIDENHAIN TNC 410, TNC 426, TNC 430 XXI

Introduction

1

1.1 The TNC 410, the TNC 426 and
the TNC 430

HEIDENHAIN TNC controls are workshop-oriented contouring
controls that enable you to program conventional machining
operations right at the machine in an easy-to-use conversational
programming language. They are designed for milling, drilling and
boring machines, as well as for machining centers. The TNC 410 can
control up to 4 axes, the TNC 426 up to 5 axes, and the TNC 430 up to
9 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 or by digitizing. For quick
calculations you can call up the on-screen pocket calculator at any
time.

Keyboard and screen layout are clearly arranged in such a way that the
functions are fast and easy to use.

Programming: HEIDENHAIN conversational and ISO formats

HEIDENHAIN conversational programming 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 HEIDENHAIN FK
free contour programming does 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

1.1 The TNC 410, the TNC 426 and the TNC 430

another. With the TNC 426, TNC 430 it is also possible to test one
program while another is being run.

Compatibility

The TNC can execute all part programs that were written on
HEIDENHAIN controls TNC 150 B and later.

2 1 Introduction

1.2 Visual Display Unit and
Keyboard

Visual display unit

The TNC is available with either a color CRT screen (BC 120) or a TFT
flat panel display (BF 120). The figure at top right shows the keys and
controls on the BC 120, and the figure at center right shows those of
the BF 120.

1 Header

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

2 Soft keys

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

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

modes

1

1

2

4

3

1

5

7

9

8

10

4

6

1

1.2 Visual Display Unit and Keyboard

Keys on BC 120 only

7 Screen demagnetization; Exit main menu for screen settings
8 Select main menu for screen settings:

n In the main menu: Move highlight downward
n In the submenu: Reduce value or move picture to the left or

downward

9 n In the main menu: Move highlight upward

n In the submenu: Increase value or move picture to the right or

upward

10 n In the main menu: Select submenu

n In the submenu: Exit submenu

Main menu dialog Function

BRIGHTNESS Adjust brightness

CONTRAST Adjust contrast

H-POSITION Adjust horizontal position

HEIDENHAIN TNC 410, TNC 426, TNC 430 3

5

1

1

2

4

6

4

11

3

1

Main menu dialog Function

V-POSITION Adjust vertical position

V-SIZE Adjust picture height

SIDE-PIN Correct barrel-shaped distortion

TRAPEZOID Correct trapezoidal distortion

ROTATION Correct tilting

COLOR TEMP Adjust color temperature

R-GAIN Adjust strength of red color

B-GAIN Adjust strength of blue color

RECALL No function

The BC 120 is sensitive to magnetic and electromagnetic noise, which
can distort the position and geometry of the picture. Alternating fields
can cause the picture to shift periodically or to become distorted.

Screen layout

You select the screen layout yourself: In the Programming and Editing

1.2 Visual Display Unit and Keyboard

mode of operation, for example, you can have the TNC show program
blocks in the left window while the right window displays
programming graphics (only TNC 410). The available screen windows
depend on the selected operating mode.

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row
shows the available layout options (see “Modes of
Operation,” page 6).

Select the desired screen layout.

4 1 Introduction

Keyboard

The figure at right shows the keys of the keyboard grouped according
to their functions:

1 Alphabetic keyboard for entering texts and file names, as well as

for programming in ISO format

2 n File management

n Pocket calculator (not TNC 410)
n MOD functions
n HELP functions

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

The functions of the individual keys are described on the inside front
cover. Machine panel buttons, e.g. NC START, are described in the
manual for your machine tool.

1

5

2

1

4

1

5

33

7

6

1.2 Visual Display Unit and Keyboard

HEIDENHAIN TNC 410, TNC 426, TNC 430 5

1.3 Modes of Operation

Manual Operation and Electronic Handwheel

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

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

Soft keys for selecting the screen layout (select
as described above, TNC 410: see screen layout
with program run, full sequence)

1.3 Modes of Operation

Screen windows Soft key

Positions

Left: positions, right: status display

Positioning with Manual Data Input (MDI)

This mode of operation is used for programming
simple traversing movements, such as for face
milling or pre-positioning. You can also define point
tables for setting the digitizing range in this mode.

Soft keys for selecting the screen layout

Screen windows Soft key

Program

Left: program. Right: status display
(only TNC 426, TNC 430)

Left: program. Right: general
program information (only TNC 410)

Left: program. Right: positions and
coordinates (only TNC 410)

Left: program. Right: information on
tools (only TNC 410)

Left: program. Right: coordinate
transformations (only TNC 410)

6 1 Introduction

Programming and editing

In this mode of operation you can write your part
programs. The various cycles and Q-parameter
functions help you with programming and add
necessary information.

Soft keys for selecting the screen layout (only
TNC 410)

Screen windows Soft key

Program

Left: program. Right: help graphics
for cycle programming

Left: program. Right: programming
graphics

Interactive 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 work
space. This simulation is supported graphically in
different display modes.

Soft keys for selecting the screen layout: see
“Program Run, Full Sequence and Program Run,
Single Block,” page 8.

1.3 Modes of Operation

HEIDENHAIN TNC 410, TNC 426, TNC 430 7

Program Run, Full Sequence and Program Run, Single Block

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

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

Soft keys for selecting the screen layout

Screen windows Soft key

Program

1.3 Modes of Operation

Left: program. Right: status display
(only TNC 426, TNC 430)

Left: program. Right: graphics (only
TNC 426, TNC 430)

Graphics (only TNC 426, TNC 430)

Left: program. Right: general
program information (only TNC 410)

Left: program. Right: positions and
coordinates (only TNC 410)

Left: program. Right: information on
tools (only TNC 410)

Left: program. Right: coordinate
transformations (only TNC 410)

Left: program. Right: tool
measurement (only TNC 410)

Soft keys for selecting the screen layout for
pallet tables (only TNC 426, TNC 430): see next
page.

8 1 Introduction

Soft keys for selecting the screen layout for pallet
tables (only TNC 426, TNC 430)

Screen windows Soft key

Pallet table

Left: program. Right: pallet table

Left: pallet table. Right: status

Left: pallet table. Right: graphics

1.3 Modes of Operation

HEIDENHAIN TNC 410, TNC 426, TNC 430 9

1.4 Status Displays

ACTL

“General” status display

The status display 1 informs you of the current state of the machine
tool. It is displayed automatically in the following modes of operation:

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

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

n Positioning with Manual Data Input (MDI).

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

1.4 Status Displays

Information in the status display

Symbol Meaning

.

Actual or nominal coordinates of the current position

1

1

X Y Z

F S M

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

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

Program run started

Axis locked

Axis can be moved with the handwheel

Axes are moving in a tilted working plane (only TNC
426, TNC 430)

Axes are moving under a basic rotation

1

1

10 1 Introduction

Additional status displays

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

To switch on the additional status display:

Call the soft-key row for screen layout.

Select the layout option for the additional status
display.

To select an additional status display:

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

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

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

General program information

1 Name of main program
2 Active programs
3 Active machining cycle
4 Circle center CC (pole)
5 Operating time
6 Dwell time counter

1.4 Status Displays

1

2

3

4

5

HEIDENHAIN TNC 410, TNC 426, TNC 430 11

6

Positions and coordinates

1 Position display
2 Type of position display, e.g. actual position
3

Tilting angle for the working plane (only TNC 426, TNC 430)

4 Angle of a basic rotation

1.4 Status Displays

Information on tools

1 n T: Tool number and name

n RT: Number and name of a replacement tool

2 Tool axis
3 Tool length and radii
4 Oversizes (delta values) from TOOL CALL (PGM) and the tool

table (TAB)

5 Tool life, maximum tool life (TIME 1) and maximum tool life for

TOOL CALL (TIME 2)

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

1

3

4

1

2

4

5

2

3

6

Coordinate transformations

1 Name of main program
2 Active datum shift (Cycle 7)
3 Active rotation angle (Cycle 10)
4 Mirrored axes (Cycle 8)
5 Active scaling factor(s) (Cycles 11 / 26)
6 Scaling datum

(see “Coordinate Transformation Cycles” on page 294)

12 1 Introduction

1

2

6

5

3

4

Tool measurement

1 Number of the tool to be measured
2 Display whether the tool radius or the tool length is being

measured

3 MIN and MAX values of the individual cutting edges and the

result of measuring the rotating tool (DYN = dynamic
measurement)

4 Cutting edge number with the corresponding measured value. If

the measured value is followed by an asterisk, the allowable
tolerance in the tool table was exceeded

Active miscellaneous functions M (not TNC 410)

1 List of the active M functions with fixed meaning.
2 List of the active M functions with function assigned by machine

manufacturer.

1

23

4

1.4 Status Displays

1

2

HEIDENHAIN TNC 410, TNC 426, TNC 430 13

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

3-D touch probes

With the various HEIDENHAIN 3-D touch probe systems you can:

n Automatically align workpieces
n Quickly and precisely set datums
n Measure the workpiece during program run
n Digitize 3-D surfaces (option), and
n Measure and inspect tools

All of the touch probe functions are described in a separate
manual. Please contact HEIDENHAIN if you require a copy
of this User's Manual. ID number: 329 203-xx.

TS 220, TS 630 and TS 632 touch trigger probes

These touch probes are particularly effective for automatic workpiece
alignment, datum setting, workpiece measurement and for digitizing.
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 630 and TS 632 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-resistant optical switch that generates an electrical
signal as soon as the stylus is deflected. This signal is transmitted to
the TNC, which stores the current position of the stylus as an actual
value.

During digitizing the TNC generates a program containing straight line
blocks in HEIDENHAIN format from a series of measured position
data. You can then output the program to a PC for further processing
with the SUSA evaluation software. This evaluation software enables
you to calculate male/female transformations or correct the program
to account for special tool shapes and radii that differ from the shape
of the stylus tip. If the tool has the same radius as the stylus tip you
can run these programs immediately.

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

14 1 Introduction

TT 130 tool touch probe for tool measurement

The TT 130 is a triggering 3-D touch probe for tool measurement and
inspection. Your TNC provides three cycles for this touch probe with
which you can measure the tool length and radius automatically either
with the spindle rotating or stopped. The TT 130 features a particularly
rugged design and a high degree of protection, which make it
insensitive to coolants and swarf. The triggering signal is generated by
a wear-resistant and highly reliable optical switch.

HR electronic handwheels

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

HEIDENHAIN TNC 410, TNC 426, TNC 430 15

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

2

Manual Operation and Setup

2.1 Switch-on, Switch-Off

Switch-on

Switch-on and Traversing the Reference Points can vary
depending on the individual machine tool. Refer to your
machine manual.

Switch on the power supply for control and machine. The TNC
automatically initiates the following dialog

Memory Test

The TNC memory is automatically checked.

Power Interrupted

2.1 Switch-on, Switch-Off

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

Translate PLC program

The PLC program of the TNC is automatically compiled.

Relay Ext. DC Voltage Missing

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

Manual Operation
Traverse Reference Points

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

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

Cross the reference points with several axes at the
same time: Use soft keys to select the axes (axes are
then shown highlighted on the screen), and then
press the machine START button (only TNC 410).

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

18 2 Manual Operation and Setup

Additional functions for the TNC 426, TNC 430

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

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

Traversing the reference point in a tilted working plane

The reference point of a tilted coordinate system can be traversed by
pressing the machine axis direction buttons. The “tilting the working
plane” function must be active in the Manual Operation mode, see
“To activate manual tilting:,” page 29. The TNC then interpolates the
corresponding axes.

The NC START button is not effective. Pressing this button may result
in an error message.

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

Switch-off

2.1 Switch-on, Switch-Off

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

UUUU Select the Manual mode.

UUUU Select the function for shutting down, confirm again

with the YES soft key.

UUUU When the TNC displays the message Now you can

switch off the TNC in a superimposed window, you

may cut off the power supply to the TNC.

Inappropriate switch-off of the TNC can lead to data loss.

HEIDENHAIN TNC 410, TNC 426, TNC 430 19

2.2 Moving the Machine Axes

Note

Traversing with the machine axis direction buttons is a
machine-dependent function. The machine tool manual
provides further information.

To traverse with the machine axis direction buttons:

Select the Manual Operation mode.

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

2.2 Moving the Machine Axes

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

and

machine START button

To stop the axis, press the machine STOP button.

You can move several axes at a time with these two methods. You can
change the feed rate at which the axes are traversed with the
F soft key, see “Spindle Speed S, Feed Rate F and Miscellaneous
Functions M,” page 23.

20 2 Manual Operation and Setup

Traversing with the HR 410 electronic
handwheel

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

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

The HR 410 handwheel features the following operating elements:

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

are set by the machine tool builder)

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

1

2

4

6

8

3
4

5
7

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

during a program run.

To move an axis:

Select the Electronic Handwheel operating mode.

Press and hold the permissive button.

Select the axis.

Select the feed rate.

Move the active axis in the positive or negative
direction.

or

2.2 Moving the Machine Axes

HEIDENHAIN TNC 410, TNC 426, TNC 430 21

Incremental jog positioning

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

Select the Manual or Electronic Handwheel mode of
operation.

Z

Jog increment =

2.2 Moving the Machine Axes

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

Enter the jog increment in millimeters, i.e. 8 mm.

Press the machine axis direction button as often as
desired.

8

8

8

X

16

22 2 Manual Operation and Setup

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

Function

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

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

Entering values

Spindle speed S, miscellaneous function M

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

Spindle speed S =

1000

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

Feed rate F

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

The following is valid for feed rate F:

n If you enter F=0, then the lowest feed rate from MP1020 is effective
n F is not lost during a power interruption

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

Changing the spindle speed and feed rate

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

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

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

HEIDENHAIN TNC 410, TNC 426, TNC 430 23

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

Note

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

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

Preparation

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

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

24 2 Manual Operation and Setup

Datum setting

Fragile workpiece?

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

Select the Manual Operation mode.

Move the tool slowly until it touches the workpiece
surface.

Select an axis (all axes can also be selected via the
ASCII keyboard)

Datum Set Z=

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

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

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

Y

Z

X

Y

X

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

HEIDENHAIN TNC 410, TNC 426, TNC 430 25

2.5 Tilting the Working Plane (not
TNC 410)

Application, function

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

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

There are two functions available for tilting the working plane:

n 3-D ROT soft key in the Manual mode and Electronic Handwheel

mode, see “To activate manual tilting:,” page 29

n Tilting under program control, Cycle G80 WORKING PLANE in the part

program (see “WORKING PLANE (Cycle G80, not TNC 410)” on
page 304)

The TNC functions for “tilting the working plane” are coordinate
transformations in which the working plane is always perpendicular to

2.5 Tilting the Working Plane (not TNC 410)

the direction of the tool axis.
When tilting the working plane, the TNC differentiates between two

machine types:

n Machines with tilting tables:

n You must tilt the workpiece into the desired position for

machining by positioning the tilting table, for example with a G0
block.

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

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

n In calculating the transformed coordinate system, the TNC

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

Z

Y

B

10°

X

26 2 Manual Operation and Setup

n Machines with swivel heads

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

positioning the swivel head, for example with a G0 block.

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

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

n In calculating the transformed coordinate system, the TNC

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

Traversing the reference points in tilted axes

With tilted axes, you use the machine axis direction buttons to cross
over the reference points. The TNC interpolates the corresponding
axes. Be sure that the function for tilting the working plane is active in
the Manual Operation mode and the actual angle of the tilted axis was
entered in the menu field.

Setting the datum in a tilted coordinate system

After you have positioned the rotary axes, set the datum in the same
way as for a non-tilted system. The TNC then converts the datum for
the tilted coordinate system. If your machine tool features axis control,
the angular values for this calculation are taken from the actual
position of the rotary axis.

2.5 Tilting the Working Plane (not TNC 410)

You must not set the datum in the tilted working plane if
in machine parameter 7500 bit 3 is set. If you do, the TNC
will calculate the wrong offset.

If your machine tool is not equipped with axis control, you
must enter the actual position of the rotary axis in the
menu for manual tilting: The actual positions of one or
several rotary axes must match the entry. Otherwise the
TNC will calculate an incorrect datum.

HEIDENHAIN TNC 410, TNC 426, TNC 430 27

Datum setting on machines with rotary tables

The behavior of the TNC during datum setting depends on
the machine. Refer to your machine manual.

The TNC automatically shifts the datum if you rotate the table and the
tilted working plane function is active:

n MP 7500, bit 3=0

To calculate the datum, the TNC uses the difference between the
REF coordinate during datum setting and the REF coordinate of the
tilting axis after tilting. The method of calculation is to be used when
you have clamped your workpiece in proper alignment when the
rotary table is in the 0° position (REF value).

n MP 7500, bit 3=1

If you rotate the table to align a workpiece that has been clamped in
an unaligned position, the TNC must no longer calculate the offset
of the datum from the difference of the REF coordinates. Instead of
the difference from the 0° position, the TNC uses the REF value of
the tilting table after tilting. In other words, it assumes that you have
properly aligned the workpiece before tilting.

MP 7500 is effective in the machine parameter list, or, if
available, in the descriptive tables for tilted axis geometry.
Refer to your machine manual.

Position display in a tilted system

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

2.5 Tilting the Working Plane (not TNC 410)

Limitations on working with the tilting function

n The touch probe function Basic Rotation cannot be used.
n PLC positioning (determined by the machine tool builder) is not

possible.

n Positioning blocks with M91/M92 are not permitted.

28 2 Manual Operation and Setup

To activate manual tilting:

To select manual tilting, press the 3-D ROT soft key.
You can now select the desired menu items with the
arrow keys

Enter the tilt angle.

To set the desired operating mode in menu option "Tilt working plane"
to Active, select the menu option and shift with the ENT key.

To conclude entry, press the END key.

To reset the tilting function, set the desired operating modes in menu
"Tilt working plane" to Inactive.

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

If you set the function "Tilt working plane" for the operating mode
Program Run to Active, the tilt angle entered in the menu becomes
active in the first block of the part program. If you are using Cycle 19
WORKING PLANE in the part program, the angular values defined in the
cycle (starting at the cycle definition) are effective. Angular values
entered in the menu will be overwritten.

2.5 Tilting the Working Plane (not TNC 410)

HEIDENHAIN TNC 410, TNC 426, TNC 430 29

3

Positioning with Manual Data Input (MDI)

3.1 Programming and Executing
Simple Machining Operations

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

Positioning with Manual Data Input (MDI)

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

To start program run, press the machine START
button.

Limitations for TNC 410

The following functions are not available:

- Tool radius compensation

- Programming and program run graphics

- Programmable probe functions

- Subprograms, program section repeats

- Contouring functions G06, G02 and G03 with R, G24 and G25

- Program call with %

Limitations for TNC 426, TNC 430

The following functions are not available:

- Program call with %

- Program run graphics

3.1 Programming and Executing Simple Machining Operations

32 3 Positioning with Manual Data Input (MDI)

Example 1

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

First you pre-position the tool with straight-line blocks to the hole
center coordinates at a setup clearance of 5 mm above the workpiece
surface. Then drill the hole with Cycle G83 Pecking.

%$MDI G71 *
N10 G99 T1 L+0 R+5 *
N20 T1 G17 S2000 *

N30 G00 G40 G90 Z+200 *
N40 X+50 Y+50 M3 *

N50 G01 Z+2 F2000 *
N60 G83
P01 +2
P02 -20
P03 +10
P04 0.5
P05 250 *
N70 G79 *
N80 G00 G40 Z+200 M2 *
N99999 %$MDI G71 *

Z

Y

50

50

Define tool: zero tool, radius 5
Call tool: tool axis Z
Spindle speed 2000 rpm
Retract tool (rapid traverse)
Move the tool at rapid traverse to a position above

the hole
Spindle on
Position tool to 2 mm above hole
Define Cycle G83 PECKING:
Set-up clearance of the tool above the hole
Total hole depth (Algebraic sign=working direction)
Depth of each infeed before retraction
Dwell time in seconds at the hole bottom
Feed rate for pecking
Call Cycle G83 PECKING
Retract the tool
End of program

X

For details on the straight-line function G00 (see “Straight line at rapid
traverse G00 Straight line with feed rate G01 F. . .” on page 127), for
Cycle G83 PECKING (see “PECKING (Cycle G83)” on page 185).

HEIDENHAIN TNC 410, TNC 426, TNC 430 33

3.1 Programming and Executing Simple Machining Operations

Example 2: Correcting workpiece misalignment on machines
with rotary tables

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

Write down the rotation angle and cancel the Basic Rotation.

Select operating mode: Positioning with MDI.

Select the axis of the rotary table, enter the rotation
angle you wrote down previously and set the feed
rate. For example: G00 G40 G90 C+2.561 F50

Conclude entry.

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

3.1 Programming and Executing Simple Machining Operations

34 3 Positioning with Manual Data Input (MDI)

Protecting and erasing programs in $MDI

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

Select the Programming and Editing mode of
operation.

To call the file manager, press the PGM MGT key
(program management).

Move the highlight to the $MDI file.

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

Target file =

BOREHOLE

Erasing the contents of the $MDI file is done in a similar way: Instead
of copying the contents, however, you erase them with the DELETE
soft key. The next time you select the operating mode Positioning with
MDI, the TNC will display an empty $MDI file.

For further information, see “Copying a single file,” page 58.

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

TNC 410: Start copying by pressing the ENT key

TNC 426 B, TNC430: Press the EXECUTE soft key to
start copying

To close the file manager, press the END soft key.

TNC 426, TNC 430: If you wish to delete $MDI, then

n you must not have selected the Positioning with MDI

mode (not even in the background).

n you must not have selected the $MDI file in the

Programming and Editing mode.

3.1 Programming and Executing Simple Machining Operations

HEIDENHAIN TNC 410, TNC 426, TNC 430 35

4

Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.1 Fundamentals

Position encoders and reference marks

The machine axes are equipped with position encoders that register
the positions of the machine table or tool. 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. The control can

4.1 Fundamentals

re-establish this relationship with the aid of reference marks when
power is returned. The scales of the position encoders contain one or
more reference marks that transmit a signal to the TNC when the axes
pass over them. From the signal the TNC identifies that position as the
machine-axis reference point and can re-establish the assignment of
displayed positions to machine axis positions.

Linear encoders are generally used for linear axes. Rotary tables and
tilt axes have angle encoders. If the position encoders feature
distance-coded reference marks, you only need to move each axis a
maximum of 20 mm (0.8 in.) for linear encoders, and 20° for angle
encoders, to re-establish the assignment of the displayed positions to
machine axis positions.

X

MP

X (Z,Y)

Z

Y

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 (datum) you define within the coordinate system.
Relative coordinate values are also referred to as incremental
coordinate values.

X

Z

Y

X

38 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

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
at center right illustrates the “right-hand rule” for remembering the
three axis directions: the middle finger is pointing in the positive
direction of the tool axis from the workpiece toward the tool (the Z
axis), the thumb is pointing in the positive X direction, and the index
finger in the positive Y direction.

The TNC 410 can control a maximum of 4 axes, the TNC 426 a
maximum of 5 axes and the TNC 430 a maximum of 9 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.

+Y

+Z

+Y

+X

+Z

+X

4.1 Fundamentals

Z

V+

Y

W+

C+

B+

A+

X

U+

HEIDENHAIN TNC 410, TNC 426, TNC 430 39

Polar coordinates

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

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

n Polar Radius, the distance from the pole to the position, and the
n Polar Angle, the size of the angle between the reference axis and

4.1 Fundamentals

the line that connects the pole with the position.

See figure at upper right.

Definition of pole and 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) Reference axis of the angle

I and J +X

J and K +Y

K and I +Z

Y

R

H

2

H

10

3

R

CC

R

H

1

0°

X

30

Z

J

I

Z

Y

Z

Y

X

Y

K

J

K

I

X

X

40 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

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 a part program in incremental coordinates,
you thus program the tool to move by the distance between the
previous and the subsequent nominal positions. Incremental
coordinates are therefore also referred to as chain dimensions.

To program a position in incremental coordinates, enter the function
G91 before the axis.

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

Y = 10 mm
Hole 5, referenced to 4 Hole 6, referenced 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 reference
axis.

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

30

20

10

10

10 10

Y

3

1

2

1

1

1

4.1 Fundamentals

3010

50

Y

6

1

5

1

4

1

20

10

20

Y

X

X

G91+R

R

10

G91+H

R

G91+H

CC

R

H

0°

X

30

HEIDENHAIN TNC 410, TNC 426, TNC 430 41

Setting the datum

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

If the production drawing is dimensioned in relative coordinates,
simply use the coordinate transformation cycles. (see “Coordinate
Transformation Cycles” on page 294).

4.1 Fundamentals

If the production drawing is not dimensioned for NC, set the datum at
a position or corner on the workpiece which is suitable for deducing
the dimensions of the remaining workpiece positions.

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

Example

The workpiece drawing at right shows holes (1 to 4) whose
dimensions are shown with respect to an absolute datum with the
coordinates X=0 Y=0. The 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 the holes (5 to 7)
without further calculations.

750

320

Z

Y

MAX

X

MIN

Y

150

7

1

0

6

1

-150

5

1

0,1

±

300

1

1

3

1

0

4

1

2

1

325

450 900

950

42 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

X

4.2 File Management:
Fundamentals

Files

Files in the TNC Ty p e
Programs

In HEIDENHAIN format
In ISO format

Tables for

Tools
Tool changers
Pallets (not TNC 410)
Datums
Points
Cutting data (not TNC 410)
Cutting materials, workpiece materials (not
TNC 410)

Texts as

ASCII files (not TNC 410) .A

.H
.I

.T
.TCH
.P
.D
.PNT
.CDT
.TAB

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

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

In the TNC 410 you can manage a max. 64 files with a total of up to
256 KB.

The TNC 426, TNC 430 can manage any number of files. However,
their total size must not exceed 1500 MB.

File names

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

PROG20 .H
File name File type
Maximum Length See table “Files in the TNC.”

4.2 File Management: Fundamentals

HEIDENHAIN TNC 410, TNC 426, TNC 430 43

Data backup TNC 426, TNC 430

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

You can do this with the free backup program TNCBACK.EXE from
HEIDENHAIN. Your machine tool builder can provide you with a copy
of TNCBACK.EXE.

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

Saving the contents of the entire hard disk (up to 1500 MB)
can take up to several hours. In this case, it is a good idea
to save the data outside of working hours, (e.g. overnight),
or to use the PARALLEL EXECUTE function to copy in the
background while you work.

4.2 File Management: Fundamentals

44 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.3 Standard File Management
TNC 426, TNC 430

Note

The standard file management is best if you wish to save
all files in one directory, or if you are well practiced in the
file management of old TNC controls.

To use the standard file management, set the MOD
function PGM MGT (see “Configuring PGM MGT (not TNC

410)” on page 406) to Standard.

Calling the file manager

Press the PGM MGT key: The TNC displays the file
management window (see figure at right)

The window shows you all of the files that are stored in the TNC. Each
file is shown with additional information:

Display Meaning

FILE NAME Name with up to 16 characters and file type

BYTE File size in bytes

STATUS

E

S

M

P

HEIDENHAIN TNC 410, TNC 426, TNC 430 45

File properties:

Program is selected in the Programming and
Editing mode of operation.

Program is selected in the Test Run mode of
operation.

Program is selected in a program run
operating mode.

File is protected against editing and erasure.

4.3 Standard File Management TNC 426, TNC 430

Selecting a file

Call the file manager.

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

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To select the file: Press the SELECT soft key or the

or

ENT key.

Deleting a file

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to delete:

Moves the highlight up or down file by file in the

4.3 Standard File Management TNC 426, TNC 430

Delete ..... file?

46 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

window.

Moves the highlight up or down page by page in the
window.

To delete the file: Press the DELETE soft key.

Confirm with the YES soft key.

Abort with the NO soft key.

Copying a file

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to copy:

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To copy the file: Press the COPY soft key.

Target file =

Enter the new name, and confirm your entry with the EXECUTE soft
key or the ENT key. A status window appears on the TNC, informing
about the copying progress. As long as the TNC is copying, you can no
longer work, or

If you wish to copy very long programs, enter the new file name and
confirm with the PARALLEL EXECUTE soft key. The file will now be
copied in the background, so you can continue to work while the TNC
is copying.

HEIDENHAIN TNC 410, TNC 426, TNC 430 47

4.3 Standard File Management TNC 426, TNC 430

Data transfer to or from an external data medium

Before you can transfer data to an external data medium,
you must setup the data interface (see “Setting the Data
Interfaces for TNC 426, TNC 430” on page 395).

Call the file manager.

Activate data transfer: Press the EXT soft key. In the
left half of the screen (1) the TNC shows all files
saved on its hard disk. In the right half of the screen

(2) it shows all files saved on the external data

medium.

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

Moves the highlight up and down within a window.

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

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

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

12

Tagging functions Soft key

4.3 Standard File Management TNC 426, TNC 430

Tag a single file

Tag all files

Untag a single file

Untag all files

Copy all tagged files

48 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Transfer a single file: Press the COPY soft key, or

Transfer several files: Press the TAG soft key, or

Transfer all files: Press the TNC => EXT soft key.

Confirm with the EXECUTE soft key or with the ENT key. A status
window appears on the TNC, informing about the copying progress, or

If you wish to transfer more than one file or longer files, press the
PARALLEL EXECUTE soft key. The TNC then copies the file in the
background.

To stop transfer, press the TNC soft key. The
standard file manager window is displayed again.

HEIDENHAIN TNC 410, TNC 426, TNC 430 49

4.3 Standard File Management TNC 426, TNC 430

Selecting one of the last 10 files selected

Call the file manager.

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

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

Move the highlight up or down.

To select the file: Press the SELECT soft key or the

or

ENT key.

Renaming a file

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to rename:

4.3 Standard File Management TNC 426, TNC 430

Target file =

Enter the name of the new file and confirm your entry with the ENT
key or EXECUTE soft key.

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

Press the RENAME soft key to select the renaming
function

50 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Converting an FK program into HEIDENHAIN conversational format

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to convert:

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

Convert the file: Press the CONVERT FK –> H soft
key.

Target file =

Enter the name of the new file and confirm your entry with the ENT
key or EXECUTE soft key.

HEIDENHAIN TNC 410, TNC 426, TNC 430 51

4.3 Standard File Management TNC 426, TNC 430

Protecting a file / Canceling file protection

Call the file manager.

Use the arrow keys or arrow soft keys to move the highlight to the file
you wish to protect or whose protection you wish to cancel:

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To enable file protection: Press the PROTECT soft
key. The file now has status P, or

Press the UNPROTECT soft key to cancel file
protection. The P status is canceled.

4.3 Standard File Management TNC 426, TNC 430

52 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.4 Expanded File Management
TNC 426, TNC 430

Note

Use the advanced file manager if you wish to keep your
files in individual directories.

To use it, set the MOD function PGM MGT (see
“Configuring PGM MGT (not TNC 410)” on page 406).

See also “File Management: Fundamentals” on page 43.

Directories

To ensure that you can easily find your files, we recommend that you
organize your hard disk into directories. You can divide a directory into
further directories, which are called subdirectories.

The TNC can manage up to 6 directory levels!
If you save more than 512 files in one directory, the TNC

no longer sorts them alphabetically!

Directory names

The name of a directory can contain up to 8 characters and does not
have an extension. If you enter more than 8 characters for the
directory name, the TNC will display an error message.

Paths

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

Example

On drive TNC:\ the subdirectory AUFTR1 was created. Then, in the
directory AUFTR1 the directory NCPROG was created and the part
program PROG1.I was copied into it. The part program now has the
following path:

TNC:\AUFTR1\NCPROG\PROG1.I

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

HEIDENHAIN TNC 410, TNC 426, TNC 430 53

TNC:\

AUFTR1

NCPROG

WZTAB

A35K941

ZYLM

TESTPROG
HUBER

KAR25T

4.4 Expanded File Management TNC 426, TNC 430

Overview: Functions of the expanded file manager

Function Soft key

Copy (and convert) individual files

Display a specific file type

Display the last 10 files that were selected

Erase a file or directory

Tag a file

Renaming a file

Protect a file against editing and erasure

Cancel file protection

Network drive management (Ethernet option
only)

Copy a directory

Display all the directories of a particular drive

4.4 Expanded File Management TNC 426, TNC 430

Delete directory with all its subdirectories

54 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Calling the file manager

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

The narrow window at left shows three drives (1). If the TNC is
connected to a network, it also displayed the connected network
drives. Drives designate devices with which data are stored or
transferred. One drive is the hard disk of the TNC. Other drives are the
interfaces (RS232, RS422, Ethernet), which can be used, for example,
to connect a personal computer. The selected (active) drive is shown
in a different color.

In the lower part of the narrow window the TNC shows all directories

(2) of the selected drive. A drive is always identified by a file symbol

to the left and the directory name to the right. The control displays a
subdirectory to the right of and below its parent directory. The
selected (active) directory is depicted in a different color.

The wide window at right 3 shows you all of the files that are stored
in the selected directory. Information for each file is displayed in a
table to the right.

Display Meaning

FILE NAME Name with up to 16 characters and file type

1

2

3

BYTE File size in bytes

STATUS

E

S

M

P

DATE Date the file was last changed

TIME Time the file was last changed

HEIDENHAIN TNC 410, TNC 426, TNC 430 55

File properties:

Program is selected in the Programming and
Editing mode of operation.

Program is selected in the Test Run mode of
operation.

Program is selected in a program run
operating mode.

File is protected against editing and erasure.

4.4 Expanded File Management TNC 426, TNC 430

Selecting drives, directories and files

Call the file manager.

With the arrow keys or the soft keys, you can move the highlight to
the desired position on the screen:

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

Moves the highlight up and down within a window.

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

1st step: Select a drive

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

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

or

4.4 Expanded File Management TNC 426, TNC 430

2nd step: Select a directory

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

key.

56 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

3rd step: select a file

4

Press the SELECT TYPE soft key.

Press the soft key for the desired file type, or

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

*.H

Move the highlight to the desired file in the right window

or

Use wild card characters, e.g. to show all files of the
file type .H that begin with 4.

The selected file is opened in the operating mode
from which you have called the file manager: Press
the SELECT soft key or the ENT key.

Creating a new directory (only possible on the drive TNC:\)

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

NEW

Create \NEW directory?

Enter the new file name, and confirm with ENT.

4.4 Expanded File Management TNC 426, TNC 430

Press the YES soft key to confirm, or

Abort with the NO soft key.

HEIDENHAIN TNC 410, TNC 426, TNC 430 57

Copying a single file

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

UUUU Press the COPY soft key to select the copying

function.

UUUU Enter the name of the destination file and confirm your

entry with the ENT key or EXECUTE soft key: The
TNC copies the file into the active directory. The
original file is retained, or

UUUU Press the PARALLEL EXECUTE soft key to copy the

file in the background. Copying in the background
permits you to continue working while the TNC is
copying. This can be useful if you are copying very
large files that take a long time. While the TNC is
copying in the background you can press the INFO
PARALLEL EXECUTE soft key (under MORE
FUNCTIONS, second soft-key row) to check the
progress of copying.

Copying a table

If you are copying tables, you can overwrite individual lines or columns
in the target table with the REPLACE FIELDS soft key. Prerequisites:

n The target table must exist.
n The file to be copied must only contain the columns or lines you

want to replace.

The REPLACE FIELDS soft key does not appear when you
want to overwrite the table in the TNC with an external
data transfer software, such as TNCremoNT. Copy the
externally created file into a different directory, and then
copy the desired fields with the TNC file management.

Example
With a tool presetter you have measured the length and radius of 10

4.4 Expanded File Management TNC 426, TNC 430

new tools. The tool presetter then generates the tool table TOOL.T
with 10 lines (for the 10 tools) and the columns

n Tool number (column T)
n Tool length (column L)
n Tool radius (column R).

Copy this file to a directory other than the one containing the previous
TOOL.T. If you wish to copy this file over the existing table using the
TNC file management, the TNC asks if you wish to overwrite the
existing TOOL.T tool table:

UUUU If you press the YES soft key, the TNC will completely overwrite the

current TOOL.T tool table. After this copying process the new
TOOL.T table consists of 10 lines. The only remaining columns in
the table are tool number, tool length and tool radius.

UUUU Or, if you press the REPLACE FIELDS soft key, the TNC merely

overwrites the first 10 lines of the columns number, length and
radius in the TOOL.T file. The TNC does not change the data in the
other lines and columns.

58 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Copying a directory

Move the highlight in the left window onto the directory you want to
copy. Instead of the COPY soft key, press the COPY DIR soft key.
Subdirectories are also copied at the same time.

Choosing one of the last 10 files selected.

Call the file manager.

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

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

Moves the highlight up and down within a window.

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

or

Deleting a file

UUUU Move the highlight to the file you want to delete.

UUUU To select the erasing function, press the DELETE soft

key. The TNC inquires whether you really intend to
erase the file.

UUUU To confirm, press the YES soft key;

UUUU To abort erasure, press the NO soft key.

HEIDENHAIN TNC 410, TNC 426, TNC 430 59

4.4 Expanded File Management TNC 426, TNC 430

Deleting a directory

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

wish to erase.

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

UUUU To select the erasing function, press the DELETE soft

key. The TNC inquires whether you really intend to
erase the directory.

UUUU To confirm, press the YES soft key;

UUUU To abort erasure, press the NO soft key.

Tagging files

Tagging functions Soft key

Tag a single file

Tag all files in the directory

Untag a single file

Untag all files

Copy all tagged files

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

Move the highlight to the first file.

4.4 Expanded File Management TNC 426, TNC 430

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

Tag a file by pressing the TAG FILE soft key.

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

You can tag several files in this way, as desired.

60 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

To copy the tagged files, press the COPY TAG soft
key, or

Delete the tagged files by pressing END to end the
marking function, and then the DELETE soft key to
delete the tagged files.

Renaming a file

UUUU Move the highlight to the file you want to rename.

UUUU Select the renaming function.

UUUU Enter the new file name; the file type cannot be

changed.

UUUU To execute renaming, press the ENT key.

Additional functions

Protecting a file / Canceling file protection

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

UUUU To select the additional functions, press the MORE

FUNCTIONS soft key.

UUUU To enable file protection, press the PROTECT soft

key. The file now has status P.

UUUU To cancel file protection, proceed in the same way

using the UNPROTECT soft key.

Erase a directory together with all its subdirectories and files.

UUUU Move the highlight in the left window onto the directory you want

to erase.

UUUU To select the additional functions, press the MORE

FUNCTIONS soft key.

UUUU Press DELETE ALL to erase the directory together

with its subdirectories.

UUUU To confirm, press the YES soft key; To abort erasure,

press the NO soft key.

HEIDENHAIN TNC 410, TNC 426, TNC 430 61

4.4 Expanded File Management TNC 426, TNC 430

Data transfer to or from an external data medium

Before you can transfer data to an external data medium,
you must setup the data interface (see “Setting the Data
Interfaces for TNC 426, TNC 430” on page 395).

Call the file manager.

Select the screen layout for data transfer: press the
WINDOW soft key. In the left half of the screen (1)
the TNC shows all files saved on its hard disk. In the
right half of the screen (2) it shows all files saved on
the external data medium.

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

Moves the highlight up and down within a window.

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

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

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

12

Transfer a single file: Press the COPY soft key, or

4.4 Expanded File Management TNC 426, TNC 430

Transfer several files: Press the TAG soft key (in the
second soft-key row, see “Tagging files,” page 60),
or

Transfer all files: Press the TNC => EXT soft key.

62 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Confirm with the EXECUTE soft key or with the ENT key. A status
window appears on the TNC, informing about the copying progress, or

If you wish to transfer more than one file or longer files, press the
PARALLEL EXECUTE soft key. The TNC then copies the file in the
background.

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

To select another directory, press the PATH soft key and
then select the desired directory using the arrow keys and
the ENTkey!

Copying files into another directory

UUUU Select the screen layout with the two equally sized windows.
UUUU To display directories in both windows, press the PATH soft key.

In the right window

UUUU Move the highlight to the directory into which you wish to copy the

files, and display the files in this directory with the ENT key.

In the left window

UUUU Select the directory with the files that you wish to copy and press

ENT to display them.

UUUU Display the file tagging functions.

UUUU Move the highlight to the file you want to copy and tag

it. You can tag several files in this way, as desired.

UUUU Copy the tagged files into the target directory.

4.4 Expanded File Management TNC 426, TNC 430

Additional tagging functions: see “Tagging files,” page 60.
If you have marked files in the left and right windows, the TNC copies

from the directory in which the highlight is located.

HEIDENHAIN TNC 410, TNC 426, TNC 430 63

Overwriting files

If you copy files into a directory in which other files are stored under
the same name, the TNC will ask whether the files in the target
directory should be overwritten:

UUUU To overwrite all files, press the YES soft key, or
UUUU To overwrite no files, press the NO soft key, or
UUUU To confirm each file separately before overwriting it, press the

CONFIRM soft key.

If you wish to overwrite a protected file, this must also be confirmed
or aborted separately.

The TNC in a network (applies only for Ethernet interface option)

To connect the Ethernet card to your network, (see
“Ethernet Interface (not TNC 410)” on page 400).

The TNC logs error messages during network operation
(see “Ethernet Interface (not TNC 410)” on page 400).

If the TNC is connected to a network, the directory window 1 displays
up to 7 drives (see figure at right). All the functions described above
(selecting a drive, copying files, etc.) also apply to network drives,
provided that you have been given the corresponding rights.

Connecting and disconnecting network drive

UUUU To select the program management: Press the PGM

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

UUUU To manage the network drives: Press the NETWORK

soft key (second soft-key row). In the right-hand
window 2 the TNC shows the network drives

4.4 Expanded File Management TNC 426, TNC 430

available for access. With the following soft keys you
can define the connection for each drive.

1

2

Function Soft key

Establish network connection. If the connection is
active, the TNC shows an M in the Mnt column. You can
connect up to 7 additional drives with the TNC.

Delete network connection.

Automatically establish network connection
whenever the TNC is switched on. The TNC shows an
A in the Auto column if the connection is established
automatically.

Do not establish network connection automatically
when the TNC is switched on.

64 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

It may take some time to mount a network device. At the upper right
of the screen the TNC displays[READ DIR] to indicate that a connection
is being established. The maximum data transmission rate lies
between 200 and 1000 kilobaud, depending on the file type being
transmitted.

Printing file with a network printer

If you have defined a network printer (see “Ethernet Interface
(not TNC 410)” on page 400), you can print the files directly:

UUUU To call the file manager, press the PGM MGT key.
UUUU Move the highlight to the file you wish to print.
UUUU Press the KOPIEREN soft key.
UUUU Press the PRINT soft key: If you have define only one printer, the

TNC will print the file immediately. If you have defined more than
one printer, the TNC opens a window listing all defined printers. Use
the arrow keys to select the desired printer, then press ENT

HEIDENHAIN TNC 410, TNC 426, TNC 430 65

4.4 Expanded File Management TNC 426, TNC 430

4.5 File Management for the
TNC 410

Calling the file manager

Press the PGM MGT key: The TNC displays the file
management window (see figure at right)

The window shows you all of the files that are stored in the TNC. Each
file is shown with additional information:

Display Meaning

FILE NAME Name with up to 16 characters and file type

STATUS

M

P

4.5 File Management for the TNC 410

Selecting a file

Call the file manager.

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

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To select the file: Press the ENT key.

File properties:

Program is selected in a program run
operating mode.

File is protected against editing and erasure.

66 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Deleting a file

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to delete:

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To delete the file: Press the DELETE soft key.

Delete ..... file?

Confirm with the YES soft key.

Abort with the NO soft key.

4.5 File Management for the TNC 410

HEIDENHAIN TNC 410, TNC 426, TNC 430 67

Copying a file

Call the file manager.

Use the arrow keys or the arrow soft keys to move the highlight to the
file you wish to copy:

Moves the highlight up or down file by file in the
window.

Moves the highlight up or down page by page in the
window.

To copy the file: Press the COPY soft key.

Target file =

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

4.5 File Management for the TNC 410

68 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Data transfer to or from an external data medium

Before you can transfer data to an external data medium,
you must setup the data interface (see “Setting the Data
Interface for the TNC 410” on page 393).

Call the file manager.

Activate data transfer: Press the EXT soft key. In the
left half of the screen the TNC shows all files saved
on its hard disk. In the right half of the screen it shows
all files saved on the external data medium.

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

Moves the highlight up and down within a window.

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

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

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

4.5 File Management for the TNC 410

If a file to be read in already exists in the memory of the
TNC, the TNC displays the message File xxx already
exists. Read in file? In this case, answer the dialog
question with YES (file is the read in) or NO (file is not read
in).

Likewise, if a file to be read out already exists on the
external device, the TNC asks whether you wish to
overwrite the external file.

HEIDENHAIN TNC 410, TNC 426, TNC 430 69

Read in all files (file types: .H, .I, .T, .TCH, .D, .PNT)

UUUU Read in all of the files that are stored on the external

data medium.

Read in offered file

UUUU List all files of a certain file type.

UUUU For example: list all HEIDENHAIN conversational

programs. To read-in the listed program, press the
YES soft key. If you do not wish the read-in the
program, press NO.

Read in a specific file

UUUU Enter the file name. Confirm with the ENT key.

UUUU Select the file type, e.g. HEIDENHAIN dialog program.

If you with to read-in the tool table TOOL.T, press the TOOL TABLE
soft key. If you with to read-in the tool-pocket table TOOLP.TCH, press
the POCKET TABLE soft key.

Read out a specific file

UUUU Select the function for reading out a single file.

UUUU Move the highlight to the file that you wish to read

4.5 File Management for the TNC 410

out. Press ENT or the TRANSFER soft key to start the
transfer.

UUUU To terminate the function for reading out specific files:

press the END key.

Read out all files (file types: .H, .I, .T, . TCH, .D, .PNT)

UUUU Output all files stored in the TNC to an external device.

Display a file directory of the external device (file types: .H, .I, .T,
.TCH, .D, .PNT)

UUUU Display a list of files stored in the external device. The

files are displayed pagewise. To show the next page:
press the YES soft key. To return to the main menu:
press the NO soft key.

70 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.6 Creating and Writing Programs

Organization of an NC program in 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 in ascending sequence.
The first block of a program is identified by %, the program name and

the active unit of measure (G70/G71).
The subsequent blocks contain information on:

n The workpiece blank
n Tool definitions, tool calls
n Feed rates and spindle speeds, as well as
n Path contours, cycles and other functions

The last block of a program is identified by N999999, %, the program
name and the active unit of measure (G70/G71).

Define blank form: G30/G31

Blocks

N10 G00 G40 X+10 Y+5 F100 M3

Path function

Block number

Words

Immediately after initiating a new program, you define a cuboid
workpiece blank. This definition is needed for the TNC’s graphic
simulation feature. The sides of the workpiece blank lie parallel to the
X, Y and Z axes and may be up to 100 000 mm long (TNC 410: 30 000
mm). The blank form is defined by two of its corner points:

n MIN point G30: the smallest X, Y and Z coordinates of the blank

form, entered as absolute values.

n MAX point G31: the largest X, Y and Z coordinates of the blank form,

entered as absolute or incremental values (with G91).

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

The TNC can display the graphic only if the ratio of the
shortest to the longest side of the blank form is less than
1 : 64.

4.6 Creating and Writing Programs

HEIDENHAIN TNC 410, TNC 426, TNC 430 71

Creating a new part program TNC 426, TNC 430

You always enter a part program in the Programming and Editing
mode of operation:

Select the Programming and Editing mode of
operation.

To call the file manager, press the PGM MGT key.

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

File name = OLD.H

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

4.6 Creating and Writing Programs

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

72 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

Creating a new part program TNC 410

You always enter a part program in the Programming and Editing
mode of operation:

Select the Programming and Editing mode of
operation.

To call the file manager, press the PGM MGT key.

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

File name = OLD.H

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

Select the file type, e.g. ISO program: Press the .I soft
key.

If necessary, switch to inches as unit of measure:
Press the MM/INCH soft key.

Confirm your entry with the ENT key.

4.6 Creating and Writing Programs

HEIDENHAIN TNC 410, TNC 426, TNC 430 73

Define the workpiece blank

0

0

0

30

Spindle axis?

17

Def BLK FORM: Min-corner ?

-40

Define the MIN point and confirm your entry with the
ENT key.

Define the spindle axis (here Z).

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

To terminate the block, press the END key.

4.6 Creating and Writing Programs

31

Def BLK FORM: MAX-corner ?

Define the MAX point and confirm your entry with the
ENT key.

Define absolute/incremental input; can be defined
separately for each coordinate.

100

100

74 4 Programming: Fundamentals of NC, File Management, Programming Aids, Pallet Management

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

To terminate the block, press the END key.