HEIDENHAIN iTNC 530 E User Manual

User’s Manual
HEIDENHAIN
Conversational
Programming

iTNC 530

NC Software
340 490-xx
340 491-xx
340 492-xx
340 493-xx
340 494-xx

English (en)
8/2005

Controls on the visual display unit

Split screen layout
Switch between machining or

programming modes
Soft keys for selecting functions in
screen

Switch the soft-key rows

Typewriter keyboard for entering letters and symbols

File names
Comments

ISO
programs

Machine operating modes

Manual Operation

Electronic Handwheel

smarT.NC

Positioning with Manual Data Input (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

Define program call, select datum and point tables

MOD Function

Display help texts for NC error messages

Display all current error messages

Pocket calculator

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

Move highlight

Go directly to blocks, cycles and parameter
functions

Override control knobs for feed rate/spindle speed

1

50

0

50

100

F %

1

50

0

50

100

S %

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

Define and call cycles
Enter and call labels for subprogramming and

program section repeats

Program stop in a program

Define touch probe cycles

Coordinate axes and numbers: Entering and editing

. . .

Select coordinate axes or
enter them into the program

. . .

Numbers

Decimal point / Reverse algebraic sign
Polar coordinate input/

Incremental dimensions

Q parameter programming/Q parameter status

Assume actual position or values from calculator

Skip dialog questions, delete words

Confirm entry and resume dialog

Conclude block, exit entry
Clear numerical entry or clear TNC error message

Abort dialog, delete program section

Special functions / smarT.NC

Show special functions

smarT.NC: Select next tab on form

smarT.NC: Select first input field in next/
previous frame

HEIDENHAIN iTNC 530 5

TNC Model, Software and Features

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

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

 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:

 Tool measurement with the TT

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

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

TNC model NC software number

iTNC 530 340 490-02

iTNC 530 E 340 491-02

iTNC 530 340 492-02

iTNC 530 E 340 493-02

iTNC 530 programming station 340 494-02

User’s Manual:

All TNC functions that have no connection with touch
probes are described in the User's Manual of the
iTNC 530. Please contact HEIDENHAIN if you need a copy
of this User’s Manual. ID number: 533 190-xx

User documentation:

The new smarT.NC operating mode is described in a
separate Pilot. Please contact HEIDENHAIN if you require
a copy of this Pilot. ID number: 533 191-xx.

6

Software options

The iTNC 530 features various software options that can be enabled
by you or your machine tool builder. Each option is to be enabled
separately and contains the following respective functions:

Software option 1

Cylinder surface interpolation (Cycles 27, 28, 29 and 39)

Feed rate in mm/min on rotary axes: M116

Tilting the machining plane (Cycle 19, PLANE function and 3-D ROT
soft key in the manual operating mode)

Circle in 3 axes (with tilted working plane)

Software option 2

Block processing time 0.5 ms instead of 3.6 ms

5 axis interpolation

Spline interpolation

3-D machining:

 M114: Automatic compensation of machine geometry when

working with tilted axes

 M128: Maintaining the position of the tool tip when positioning

with tilted axes (TCPM)

 FUNCTION TCPM: Maintaining the position of the tool tip when

positioning with tilted axes (TCPM) in selectable modes.

 M144: Compensating the machine’s kinematic configuration for

ACTUAL/NOMINAL positions at end of block

 Additional parameters finishing/roughing and tolerance for

rotary axes in Cycle 32 (G62)

 LN blocks (3-D compensation)

DXF Converter software option Description

Extract contours from DXF files (R12
format).

page 252

DCM software option Description

Function which monitors areas defined
by the machine manufacturer to
prevent collisions.

page 81

Additional dialog language software
option

Description

Slovenian. page 647

HEIDENHAIN iTNC 530 7

Feature content level (upgrade functions)

Along with software options, significant further improvements of the
TNC software are managed via the Feature Content Level. Functions
subject to the FCL are not available simply by updating the software
on your TNC. These functions are identified in the manual with FCL n,
where n indicates the sequential number of the feature content level.

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

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.

FCL-2 functions Description

3-D line graphics page 128

Virtual tool axis page 80

USB support of block devices (memory
sticks, hard disks, CD-ROM drives)

page 113

Filtering of externally created contours page 514

Possibility of assigning different depths
to each subcontour in the contour
formula

page 433

DHCP dynamic IP-address
management

page 617

Touch-probe cycle for global setting of
touch-probe parameters

User's Manual - Touch
Probe Cycles

smarT.NC: Graphic support of block
scan

smarT.NC Pilot

smarT.NC: Coordinate transformation smarT.NC Pilot

smarT.NC: PLANE function smarT.NC Pilot

8

Functions included in 340 49x-01 new since the
predecessor versions 340 422-xx and 340 423-xx

 A new form-based operating mode, smarT.NC, introduced. These

cycles are described in a separate user's document. In connection
with this the TNC operating panel was enhanced. There are some
new keys available for quicker navigation within smarT.NC (see
“Operating panel” on page 40).

 The single-processor versions supports pointing devices (mice) via

the USB interface.

 The tooth feed f

z

and feed per revolution fu can now be defined as

alternate feed entries See table “”.

 New CENTERING cycle (see “CENTERING (Cycle 240)” on page

305)

 New M function M150 for suppressing limit switch messages (see

“Suppress limit switch message: M150” on page 279)

 M128 is now also permitted for mid-program startup (see “Mid-

program startup (block scan)” on page 600).

 The number of available Q parameters was expanded to 2000 (see

“Principle and Overview” on page 532).

 The number of available label numbers was expanded to 1000. Now

label names can be assigned as well (see “Labeling Subprograms
and Program Section Repeats” on page 516).

 In the Q parameter functions FN9 to FN12 you can now also assign

label names as jump targets (see “If-Then Decisions with
Q Parameters” on page 540).

 Selectively machine points from a point table (see “Hiding single

points from the machining process” on page 299).

 The current time is also shown in the additional status display

window (see “General program information” on page 45).

 Several columns were added to the tool table (see “Tool table:

Standard tool data” on page 166).

 The Test Run can now also be stopped and continued within

machining cycles (see “Running a program test” on page 594).

HEIDENHAIN iTNC 530 9

TNC Model, Software and Features

New functions with 340 49x-02

 DXF files can be opened directly on the TNC, in order to extract

contours into a plain-language program (see “Generating Contour
Programs from DXF Data (Software Option)” on page 252)

 3-D line graphics are now available in the Programming and Editing

operating mode (see “3-D Line Graphics (FCL 2 Function)” on page

128)

 The active tool-axis direction can now be set as the active machining

direction for manual operation (see “Setting the current tool-axis
direction as the active machining direction (FCL 2 function)” on page

80)

 The machine manufacturer can now define any areas on the

machine for collision monitoring (see “Dynamic Collision Monitoring
(Software Option)” on page 81)

 Instead of the spindle speed S you can now define the cutting speed

Vc in m/min (see “Calling tool data” on page 175)

 The TNC can now display freely definable tables in the familiar table

view or as forms (see “Switching between table and form view” on
page 196)

 The function for converting FK programs to H was expanded.

Programs can now also be output in linearized format (see
“Converting FK programs into HEIDENHAIN conversational format”
on page 236)

 You can filter contours that were created using external

programming systems (see “Filtering Contours (FCL 2 Function)”
on page 514)

 For contours which you connect via the contour formula, you can

now assign separate machining depths for each subcontour (see
“Defining contour descriptions” on page 433)

 The single-processor version now supports not only pointing

devices (mice), but also USB block devices (memory sticks, disk
drives, hard disks, CD-ROM drives) (see “USB devices on the TNC
(FCL 2 function)” on page 113)

10

TNC Model, Software and Features

Functions changed in 340 49x-01 since the
predecessor versions 340 422-xx and 340 423-xx

 The layouts of the status display and additional status display were

redesigned (see “Status Displays” on page 44).

 Software 340 490 no longer supports the small resolution in

combination with the BC 120 screen (see “Visual display unit” on
page 39).

 New key layout of the TE 530 B keyboard unit (see “Operating

panel” on page 40)

 The entry range for the EULPR precession angle in the PLANE EULER

function was expanded (see “Defining the Machining Plane with
Euler Angles: EULER PLANE” on page 490)

 The plane vector in the PLANE EULER function no longer has to be

entered in standardized form (see “Defining the Machining Plane
with Two Vectors: VECTOR PLANE” on page 492)

 Positioning behavior of the CYCL CALL PAT function modified (see

“Calling a cycle in connection with point tables” on page 301)

 The tool types available for selection in the tool table were increased

in preparation for future functions.

 Instead of the last 10, you can now choose from the last 15 selected

files (see “Choosing one of the last files selected” on page 105)

HEIDENHAIN iTNC 530 11

TNC Model, Software and Features

Functions changed in 340 49x-02

 Access to the preset table was simplified. There are also new

possibilities for entering values in the preset table See table
“Manually saving the datums in the preset table”

 In inch-programs, the function M136 (feed rate in 0.1 inch/rev) can

no longer be combined with the function FU

 The feed-rate potentiometers of the HR 420 are no longer switched

over automatically when the handwheel is selected. The selection is
made via soft key on the handwheel. In addition, the pop-up window
for the active handwheel was made smaller, in order to improve the
view of the display beneath it (see “Potentiometer settings” on
page 60)

 The maximum number of contour elements for SL cycles was

increased to 8192, so that much more complex contours can be
machined (see “SL Cycles” on page 397)

 FN16: F-PRINT: The maximum number of Q-parameter values that

can be output per line in the format description file was increased to
32 (see “FN16: F-PRINT: Formatted output of texts or Q parameter
values” on page 548)

 The soft keys START and START SINGLE BLOCK in the Program

Test mode of operation were switched, so that the soft-key
alignment is the same in all modes of operation (Programming and
Editing, smarT.NC, Test) (see “Running a program test” on page

594)

 The design of the soft keys was revised completely

HEIDENHAIN iTNC 530 13

Contents

Introduction

1

Manual Operation and Setup

2

Positioning with Manual Data Input
(MDI)

3

Programming: Fundamentals of File
Management, Programming Aids

4

Programming: Tools

5

Programming: Programming Contours

6

Programming: Miscellaneous Functions

7

Programming: Cycles

8

Programming: Special Functions

9

Programming: Subprograms and
Program Section Repeats

10

Programming: Q Parameters

11

Test Run and Program Run

12

MOD Functions

13

Tables and Overviews

14

iTNC 530 with Windows 2000 (Option)

15

HEIDENHAIN iTNC 530 15

1.1 The iTNC 530 ..... 38

Programming: HEIDENHAIN conversational, smarT.NC and ISO formats ..... 38

Compatibility ..... 38

1.2 Visual Display Unit and Operating Panel ..... 39

Visual display unit ..... 39

Screen layout ..... 39

Operating panel ..... 40

1.3 Modes of Operation ..... 41

Manual operation and electronic handwheel ..... 41

Positioning with Manual Data Input (MDI) ..... 41

Programming and editing ..... 42

Test Run ..... 42

Program Run, Full Sequence and Program Run, Single Block ..... 43

1.4 Status Displays ..... 44

“General” status display ..... 44

Additional status displays ..... 45

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels ..... 49

3-D touch probes ..... 49

HR electronic handwheels ..... 50

1 Introduction ..... 37

16

2.1 Switch-On, Switch-Off ..... 52

Switch-on ..... 52

Switch-off ..... 54

2.2 Moving the Machine Axes ..... 55

Note ..... 55

To traverse with the machine axis direction buttons: ..... 55

Incremental jog positioning ..... 56

Traversing with the HR 410 electronic handwheel ..... 57

HR 420 Electronic Handwheel ..... 58

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 64

Function ..... 64

Entering values ..... 64

Changing the spindle speed and feed rate ..... 65

2.4 Datum Setting (Without a 3-D Touch Probe) ..... 66

Note ..... 66

Preparation ..... 66

Datum setting with axis keys ..... 67

Datum management with the preset table ..... 68

2.5 Tilting the Working Plane (Software Option 1) ..... 75

Application, function ..... 75

Traversing the reference points in tilted axes ..... 76

Setting the datum in a tilted coordinate system ..... 77

Datum setting on machines with rotary tables ..... 77

Datum setting on machines with spindle-head changing systems ..... 77

Position display in a tilted system ..... 78

Limitations on working with the tilting function ..... 78

Activating manual tilting ..... 79

Setting the current tool-axis direction as the active machining direction (FCL 2 function) ..... 80

2.6 Dynamic Collision Monitoring (Software Option) ..... 81

Function ..... 81

Collision monitoring in the manual operating modes ..... 81

Collision monitoring in Automatic operation ..... 83

3.1 Programming and Executing Simple Machining Operations ..... 86

Positioning with Manual Data Input (MDI) ..... 86

Protecting and Erasing Programs in $MDI ..... 88

2 Manual Operation and Setup ..... 51

3 Positioning with Manual Data Input (MDI) ..... 85

HEIDENHAIN iTNC 530 17

4.1 Fundamentals ..... 90

Position encoders and reference marks ..... 90

Reference system ..... 90

Reference system on milling machines ..... 91

Polar coordinates ..... 92

Absolute and incremental workpiece positions ..... 93

Setting the datum ..... 94

4.2 File Management: Fundamentals ..... 95

Files ..... 95

Data backup ..... 96

4.3 Working with the file manager ..... 97

Directories ..... 97

Paths ..... 97

Overview: Functions of the File Manager ..... 98

Calling the File Manager ..... 99

Selecting drives, directories and files ..... 100

Creating a new directory (only possible on the drive TNC:\) ..... 102

Copying a single file ..... 103

Copying a directory ..... 105

Choosing one of the last files selected ..... 105

Deleting a file ..... 106

Deleting a directory ..... 106

Tagging files ..... 107

Renaming a file ..... 108

Additional functions ..... 108

Data transfer to or from an external data medium ..... 109

Copying files into another directory ..... 111

The TNC in a Network ..... 112

USB devices on the TNC (FCL 2 function) ..... 113

4.4 Creating and Writing Programs ..... 114

Organization of an NC program in HEIDENHAIN conversational format ..... 114

Defining the blank form – BLK FORM ..... 114

Creating a new part program ..... 115

Programming tool movements in conversational format ..... 117

Actual position capture ..... 119

Editing a program ..... 120

The TNC search function ..... 124

4 Fundamentals of NC, File Management, Programming Aids, Pallet Management ..... 89

18

4.5 Interactive Programming Graphics ..... 126

To generate/not generate graphics during programming: ..... 126

Generating a graphic for an existing program ..... 126

Block number display ON/OFF ..... 127

Erase the graphic ..... 127

Magnifying or reducing a detail ..... 127

4.6 3-D Line Graphics (FCL 2 Function) ..... 128

Function ..... 128

Functions of the 3-D line graphics ..... 129

Highlighting NC blocks in the graphics ..... 131

Block number display ON/OFF ..... 131

Erase the graphic ..... 131

4.7 Structuring Programs ..... 132

Definition and applications ..... 132

Displaying the program structure window / Changing the active window ..... 132

Inserting a structuring block in the (left) program window ..... 132

Selecting blocks in the program structure window ..... 132

4.8 Adding Comments ..... 133

Function ..... 133

Entering comments during programming ..... 133

Inserting comments after program entry ..... 133

Entering a comment in a separate block ..... 133

Functions for editing of the comment ..... 134

4.9 Creating Text Files ..... 135

Function ..... 135

Opening and exiting text files ..... 135

Editing texts ..... 136

Deleting and inserting characters, words and lines ..... 137

Editing text blocks ..... 138

Finding text sections ..... 139

4.10 Integrated Pocket Calculator ..... 140

Operation ..... 140

4.11 Immediate Help for NC Error Messages ..... 141

Displaying error messages ..... 141

Display HELP ..... 141

HEIDENHAIN iTNC 530 19

4.12 List of all current error messages ..... 142

Function ..... 142

Show error list ..... 142

Window contents ..... 143

4.13 Pallet Management ..... 144

Function ..... 144

Selecting a pallet table ..... 146

Leaving the pallet file ..... 146

Executing the pallet file ..... 147

4.14 Pallet Operation with Tool-Oriented Machining ..... 148

Function ..... 148

Selecting a pallet file ..... 152

Setting up the pallet file with the entry form ..... 153

Sequence of tool-oriented machining ..... 157

Leaving the pallet file ..... 158

Executing the pallet file ..... 158

20

5.1 Entering Tool-Related Data ..... 162

Feed rate F ..... 162

Spindle speed S ..... 163

5.2 Tool Data ..... 164

Requirements for tool compensation ..... 164

Tool numbers and tool names ..... 164

Tool length L ..... 164

Tool radius R ..... 165

Delta values for lengths and radii ..... 165

Entering tool data into the program ..... 165

Entering tool data in tables ..... 166

Using an external PC to overwrite individual tool data ..... 171

Pocket table for tool changer ..... 172

Calling tool data ..... 175

Tool change ..... 176

5.3 Tool Compensation ..... 178

Introduction ..... 178

Tool length compensation ..... 178

Tool radius compensation ..... 179

5.4 Three-Dimensional Tool Compensation (Software Option 2) ..... 182

Introduction ..... 182

Definition of a normalized vector ..... 183

Permissible tool forms ..... 184

Using other tools: Delta values ..... 184

3-D compensation without tool orientation ..... 185

Face Milling: 3-D compensation with and without tool orientation ..... 186

Peripheral Milling: 3-D radius compensation with workpiece orientation ..... 188

5.5 Working with Cutting Data Tables ..... 190

Note ..... 190

Applications ..... 190

Table for workpiece materials ..... 191

Table for tool cutting materials ..... 192

Table for cutting data ..... 192

Data required for the tool table ..... 193

Working with automatic speed / feed rate calculation ..... 194

Changing the table structure ..... 195

Switching between table and form view ..... 196

Data transfer from cutting data tables ..... 197

Configuration file TNC.SYS ..... 197

5 Programming: Tools ..... 161

HEIDENHAIN iTNC 530 21

6.1 Tool Movements ..... 200

Path functions ..... 200

FK Free Contour Programming ..... 200

Miscellaneous functions M ..... 200

Subprograms and program section repeats ..... 200

Programming with Q parameters ..... 200

6.2 Fundamentals of Path Functions ..... 201

Programming tool movements for workpiece machining ..... 201

6.3 Contour Approach and Departure ..... 205

Overview: Types of paths for contour approach and departure ..... 205

Important positions for approach and departure ..... 205

Approaching on a straight line with tangential connection: APPR LT ..... 208

Approaching on a straight line perpendicular to the first contour point: APPR LN ..... 208

Approaching on a circular path with tangential connection: APPR CT ..... 209

Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT ..... 210

Departing on a straight line with tangential connection: DEP LT ..... 211

Departing on a straight line perpendicular to the last contour point: DEP LN ..... 211

Departure on a circular path with tangential connection: DEP CT ..... 212

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT ..... 212

6.4 Path Contours—Cartesian Coordinates ..... 213

Overview of path functions ..... 213

Straight Line L ..... 214

Inserting a Chamfer CHF between Two Straight Lines ..... 215

Corner Rounding RND ..... 216

Circle center CC ..... 217

Circular path C around circle center CC ..... 218

Circular path CR with defined radius ..... 219

Circular Path CT with Tangential Connection ..... 220

6.5 Path Contours—Polar Coordinates ..... 225

Overview ..... 225

Polar coordinate origin: Pole CC ..... 226

Straight line LP ..... 227

Circular path CP around pole CC ..... 227

Circular Path CTP with Tangential Connection ..... 228

Helical interpolation ..... 229

6 Programming: Programming Contours ..... 199

22

6.6 Path Contours—FK Free Contour Programming ..... 234

Fundamentals ..... 234

Graphics during FK programming ..... 235

Converting FK programs into HEIDENHAIN conversational format ..... 236

Initiating the FK dialog ..... 237

Free programming of straight lines ..... 238

Free programming of circular arcs ..... 238

Input possibilities ..... 239

Auxiliary points ..... 242

Relative data ..... 243

6.7 Contour Movements—Spline Interpolation (Software Option 2) ..... 250

Function ..... 250

6.8 Generating Contour Programs from DXF Data (Software Option) ..... 252

Function ..... 252

Opening a DXF file ..... 252

Basic settings ..... 253

Layer settings ..... 254

Datum specifying ..... 255

Contour selection, saving a contour program ..... 257

Zoom function ..... 258

HEIDENHAIN iTNC 530 23

7.1 Entering Miscellaneous Functions M and STOP ..... 260

Fundamentals ..... 260

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 261

Overview ..... 261

7.3 Miscellaneous Functions for Coordinate Data ..... 262

Programming machine-referenced coordinates: M91/M92 ..... 262

Activating the most recently entered datum: M104 ..... 264

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130 ..... 264

7.4 Miscellaneous Functions for Contouring Behavior ..... 265

Smoothing corners: M90 ..... 265

Insert rounding arc between straight lines: M112 ..... 266

Do not include points when executing non-compensated line blocks: M124 ..... 266

Machining small contour steps: M97 ..... 267

Machining open contours: M98 ..... 269

Feed rate factor for plunging movements: M103 ..... 270

Feed rate in millimeters per spindle revolution: M136 ..... 271

Feed rate for circular arcs: M109/M110/M111 ..... 271

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 272

Superimposing handwheel positioning during program run: M118 ..... 274

Retraction from the contour in the tool-axis direction: M140 ..... 275

Suppressing touch probe monitoring: M141 ..... 276

Delete modal program information: M142 ..... 277

Delete basic rotation: M143 ..... 277

Automatically retract tool from the contour at an NC stop: M148 ..... 278

Suppress limit switch message: M150 ..... 279

7.5 Miscellaneous Functions for Rotary Axes ..... 280

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1) ..... 280

Shorter-path traverse of rotary axes: M126 ..... 281

Reducing display of a rotary axis to a value less than 360°: M94 ..... 282

Automatic compensation of machine geometry when working with tilted axes: M114 (software option 2) ..... 283

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

option 2) ..... 284

Exact stop at corners with nontangential transitions: M134 ..... 286

Selecting tilting axes: M138 ..... 286

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

(software option 2) ..... 287

7 Programming: Miscellaneous Functions ..... 259

24

7.6 Miscellaneous Functions for Laser Cutting Machines ..... 288

Principle ..... 288

Output the programmed voltage directly: M200 ..... 288

Output voltage as a function of distance: M201 ..... 288

Output voltage as a function of speed: M202 ..... 289

Output voltage as a function of time (time-dependent ramp): M203 ..... 289

Output voltage as a function of time (time-dependent pulse): M204 ..... 289

HEIDENHAIN iTNC 530 25

8.1 Working with Cycles ..... 292

Machine-specific cycles ..... 292

Defining a cycle using soft keys ..... 293

Defining a cycle using the GOTO function ..... 293

Calling cycles ..... 295

Working with the secondary axes U/V/W ..... 297

8.2 Point Tables ..... 298

Function ..... 298

Creating a point table ..... 298

Hiding single points from the machining process ..... 299

Selecting a point table in the program ..... 300

Calling a cycle in connection with point tables ..... 301

8.3 Cycles for Drilling, Tapping and Thread Milling ..... 303

Overview ..... 303

CENTERING (Cycle 240) ..... 305

DRILLING (Cycle 200) ..... 307

REAMING (Cycle 201) ..... 309

BORING (Cycle 202) ..... 311

UNIVERSAL DRILLING (Cycle 203) ..... 313

BACK BORING (Cycle 204) ..... 315

UNIVERSAL PECKING (Cycle 205) ..... 317

BORE MILLING (Cycle 208) ..... 320

TAPPING NEW with floating tap holder (Cycle 206) ..... 322

RIGID TAPPING without a floating tap holder NEW (Cycle 207) ..... 324

TAPPING WITH CHIP BREAKING (Cycle 209) ..... 326

Fundamentals of thread milling ..... 328

THREAD MILLING (Cycle 262) ..... 330

THREAD MILLING/COUNTERSINKING (Cycle 263) ..... 332

THREAD DRILLING/MILLING (Cycle 264) ..... 336

HELICAL THREAD DRILLING/MILLING (Cycle 265) ..... 340

OUTSIDE THREAD MILLING (Cycle 267) ..... 344

8 Programming: Cycles ..... 291

26

8.4 Cycles for Milling Pockets, Studs and Slots ..... 353

Overview ..... 353

RECTANGULAR POCKET (Cycle 251) ..... 354

CIRCULAR POCKET (Cycle 252) ..... 359

SLOT MILLING (Cycle 253) ..... 363

CIRCULAR SLOT (Cycle 254) ..... 368

POCKET FINISHING (Cycle 212) ..... 373

STUD FINISHING (Cycle 213) ..... 375

CIRCULAR POCKET FINISHING (Cycle 214) ..... 377

CIRCULAR STUD FINISHING (Cycle 215) ..... 379

SLOT (oblong hole) with reciprocating plunge-cut (Cycle 210) ..... 381

CIRCULAR SLOT (oblong hole) with reciprocating plunge-cut (Cycle 211) ..... 384

8.5 Cycles for Machining Point Patterns ..... 390

Overview ..... 390

CIRCULAR PATTERN (Cycle 220) ..... 391

LINEAR PATTERN (Cycle 221) ..... 393

8.6 SL Cycles ..... 397

Fundamentals ..... 397

Overview of SL Cycles ..... 399

CONTOUR (Cycle 14) ..... 400

Overlapping contours ..... 401

CONTOUR DATA (Cycle 20) ..... 404

PILOT DRILLING (Cycle 21) ..... 405

ROUGH-OUT (Cycle 22) ..... 406

FLOOR FINISHING (Cycle 23) ..... 407

SIDE FINISHING (Cycle 24) ..... 408

CONTOUR TRAIN (Cycle 25) ..... 409

CYLINDER SURFACE (Cycle 27, software option 1) ..... 411

CYLINDER SURFACE slot milling (Cycle 28, software option 1) ..... 413

CYLINDER SURFACE ridge milling (Cycle 29, software option 1) ..... 416

CYLINDER SURFACE outside contour milling (Cycle 39, software option 1) ..... 418

8.7 SL Cycles with Contour Formula ..... 431

Fundamentals ..... 431

Selecting a program with contour definitions ..... 432

Defining contour descriptions ..... 433

Entering a contour formula ..... 434

Overlapping contours ..... 435

Contour machining with SL Cycles ..... 437

8.8 Cycles for Multipass Milling ..... 441

Overview ..... 441

3-D DATA (Cycle 30) ..... 442

MULTIPASS MILLING (Cycle 230) ..... 443

RULED SURFACE (Cycle 231) ..... 445

FACE MILLING (Cycle 232) ..... 448

HEIDENHAIN iTNC 530 27

8.9 Coordinate Transformation Cycles ..... 456

Overview ..... 456

Effect of coordinate transformations ..... 456

DATUM SHIFT (Cycle 7) ..... 457

DATUM SHIFT with datum tables (Cycle 7) ..... 458

DATUM SETTING (Cycle 247) ..... 462

MIRROR IMAGE (Cycle 8) ..... 463

CONTOUR (Cycle 10) ..... 465

SCALING FACTOR (Cycle 11) ..... 466

AXIS-SPECIFIC SCALING (Cycle 26) ..... 467

WORKING PLANE (Cycle 19, software option 1) ..... 468

8.10 Special Cycles ..... 476

DWELL TIME (Cycle 9) ..... 476

PROGRAM CALL (Cycle 12) ..... 477

ORIENTED SPINDLE STOP (Cycle 13) ..... 478

TOLERANCE (Cycle 32, software option 2) ..... 479

9.1 The PLANE Function: Tilting the Working Plane (Software Option 1) ..... 482

Introduction ..... 482

Define the PLANE function ..... 484

Position display ..... 484

Reset the PLANE function ..... 485

9.2 Defining the Machining Plane with Space Angles: PLANE SPATIAL ..... 486

Function ..... 486

Input parameters ..... 487

9.3 Defining the Machining Plane with Projection Angles: PROJECTED PLANE ..... 488

Function ..... 488

Input parameters ..... 489

9.4 Defining the Machining Plane with Euler Angles: EULER PLANE ..... 490

Function ..... 490

Input parameters ..... 491

9.5 Defining the Machining Plane with Two Vectors: VECTOR PLANE ..... 492

Function ..... 492

Input parameters ..... 493

9.6 Defining the Machining Plane via Three Points: POINTS PLANE ..... 494

Function ..... 494

Input parameters ..... 495

9.7 Defining the Machining Plane with a Single, Incremental Space Angle: PLANE RELATIVE ..... 496

Function ..... 496

Input parameters ..... 497

Abbreviations used ..... 497

9 Programming: Special Functions ..... 481

28

9.8 Specifying the Positioning Behavior of the PLANE Function ..... 498

Overview ..... 498

Automatic positioning: MOVE/TURN/STAY (entry is mandatory) ..... 499

Selection of alternate tilting possibilities: SEQ +/– (entry optional) ..... 502

Selecting the type of transformation (entry optional) ..... 503

9.9 Inclined-Tool Machining in the Tilted Plane ..... 504

Function ..... 504

Inclined-tool machining via incremental traverse of a rotary axis ..... 504

Inclined-tool machining via normal vectors ..... 505

9.10 TCPM FUNCTION (Software Option 2) ..... 506

Function ..... 506

Define TCPM FUNCTION ..... 506

Mode of action of the programmed feed rate ..... 507

Interpretation of the programmed rotary axis coordinates ..... 508

Interpolation type between the starting and end position ..... 509

Reset TCPM FUNCTION ..... 510

9.11 Generate Backward Program ..... 511

Function ..... 511

Prerequisites for the program to be converted ..... 512

Application example ..... 513

9.12 Filtering Contours (FCL 2 Function) ..... 514

Function ..... 514

HEIDENHAIN iTNC 530 29

10.1 Labeling Subprograms and Program Section Repeats ..... 516

Labels ..... 516

10.2 Subprograms ..... 517

Operating sequence ..... 517

Programming notes ..... 517

Programming a subprogram ..... 517

Calling a subprogram ..... 517

10.3 Program Section Repeats ..... 518

Label LBL ..... 518

Operating sequence ..... 518

Programming notes ..... 518

Programming a program section repeat ..... 518

Calling a program section repeat ..... 518

10.4 Separate Program as Subprogram ..... 519

Operating sequence ..... 519

Programming notes ..... 519

Calling any program as a subprogram ..... 520

10.5 Nesting ..... 521

Types of nesting ..... 521

Nesting depth ..... 521

Subprogram within a subprogram ..... 521

Repeating program section repeats ..... 522

Repeating a subprogram ..... 523

10 Programming: Subprograms and Program Section Repeats ..... 515

30

11.1 Principle and Overview ..... 532

Programming notes ..... 533

Calling Q parameter functions ..... 533

11.2 Part Families—Q Parameters in Place of Numerical Values ..... 534

Example NC blocks ..... 534

Example ..... 534

11.3 Describing Contours through Mathematical Operations ..... 535

Function ..... 535

Overview ..... 535

Programming fundamental operations ..... 536

11.4 Trigonometric Functions ..... 537

Definitions ..... 537

Programming trigonometric functions ..... 538

11.5 Calculating Circles ..... 539

Function ..... 539

11.6 If-Then Decisions with Q Parameters ..... 540

Function ..... 540

Unconditional jumps ..... 540

Programming If-Then decisions ..... 540

Abbreviations used: ..... 541

11.7 Checking and Changing Q Parameters ..... 542

Procedure ..... 542

11.8 Additional Functions ..... 543

Overview ..... 543

FN14: ERROR: Displaying error messages ..... 544

FN15: PRINT: Output of texts or Q parameter values ..... 547

FN16: F-PRINT: Formatted output of texts or Q parameter values ..... 548

FN18: SYS-DATUM READ Read system data ..... 553

FN19: PLC: Transferring values to the PLC ..... 559

FN20: WAIT FOR: NC and PLC synchronization ..... 560

FN 25: PRESET: Setting a new datum ..... 561

FN26:TABOPEN: Opening a freely definable table ..... 562

FN27: TABWRITE: Writing to a freely definable table ..... 562

FN28:TABREAD: Reading a freely definable table ..... 563

11 Programming: Q Parameters ..... 531

HEIDENHAIN iTNC 530 31

11.9 Entering Formulas Directly ..... 564

Entering formulas ..... 564

Rules for formulas ..... 566

Programming example ..... 567

11.10 Preassigned Q Parameters ..... 568

Values from the PLC: Q100 to Q107 ..... 568

Active tool radius: Q108 ..... 568

Tool axis: Q109 ..... 568

Spindle status: Q110 ..... 569

Coolant on/off: Q111 ..... 569

Overlap factor: Q112 ..... 569

Unit of measurement for dimensions in the program: Q113 ..... 569

Tool length: Q114 ..... 569

Coordinates after probing during program run ..... 570

Deviation between actual value and nominal value during automatic tool measurement with the TT 130 ..... 570

Tilting the working plane with mathematical angles: Rotary axis coordinates calculated by the TNC ..... 570

Measurement results from touch probe cycles (see also User’s Manual for Touch Probe Cycles) ..... 571

32

12.1 Graphics ..... 582

Function ..... 582

Overview of display modes ..... 584

Plan view ..... 584

Projection in 3 planes ..... 585

3-D view ..... 586

Magnifying details ..... 589

Repeating graphic simulation ..... 590

Measuring the machining time ..... 591

12.2 Functions for Program Display ..... 592

Overview ..... 592

12.3 Test run ..... 593

Function ..... 593

12.4 Program Run ..... 596

Function ..... 596

Run a part program ..... 596

Interrupting machining ..... 597

Moving the machine axes during an interruption ..... 598

Resuming program run after an interruption ..... 599

Mid-program startup (block scan) ..... 600

Returning to the contour ..... 602

12.5 Automatic Program Start ..... 603

Function ..... 603

12.6 Optional Block Skip ..... 604

Function ..... 604

Erasing the “/” character ..... 604

12.7 Optional Program-Run Interruption ..... 605

Function ..... 605

12 Test Run and Program Run ..... 581

HEIDENHAIN iTNC 530 33

13.1 MOD Function ..... 608

Selecting the MOD functions ..... 608

Changing the settings ..... 608

Exiting the MOD functions ..... 608

Overview of MOD functions ..... 609

13.2 Software Numbers and Option Numbers ..... 610

Function ..... 610

13.3 Code Numbers ..... 611

Function ..... 611

13.4 Loading Service Packs ..... 612

Function ..... 612

13.5 Setting the Data Interfaces ..... 613

Function ..... 613

Setting the RS-232 interface ..... 613

Setting the RS-422 interface ..... 613

Setting the OPERATING MODE of the external device ..... 613

Setting the BAUD RATE ..... 613

Assign ..... 614

Software for data transfer ..... 615

13.6 Ethernet interface ..... 617

Introduction ..... 617

Connection possibilities ..... 617

Connecting the iTNC directly with a Windows PC ..... 618

Configuring the TNC ..... 620

13.7 Configuring PGM MGT ..... 625

Function ..... 625

Changing the PGM MGT setting ..... 625

Dependent files ..... 626

13.8 Machine-Specific User Parameters ..... 628

Function ..... 628

13.9 Showing the Workpiece in the Working Space ..... 629

Function ..... 629

Rotate the entire image ..... 630

13.10 Position Display Types ..... 631

Function ..... 631

13.11 Unit of Measurement ..... 632

Function ..... 632

13.12 Select the Programming Language for $MDI ..... 633

Function ..... 633

13 MOD Functions ..... 607

34

13.13 Selecting the Axes for Generating L Blocks ..... 634

Function ..... 634

13.14 Enter the Axis Traverse Limits, Datum Display ..... 635

Function ..... 635

Working without additional traverse limits ..... 635

Find and enter the maximum traverse ..... 635

Datum display ..... 636

13.15 Displaying HELP Files ..... 637

Function ..... 637

Selecting HELP files ..... 637

13.16 Display operating times ..... 638

Function ..... 638

13.17 TeleService ..... 639

Function ..... 639

Calling/exiting TeleService ..... 639

13.18 External Access ..... 640

Function ..... 640

HEIDENHAIN iTNC 530 35

14.1 General User Parameters ..... 642

Input possibilities for machine parameters ..... 642

Selecting general user parameters ..... 642

14.2 Pin Layout and Connecting Cable for the Data Interfaces ..... 656

RS-232-C/V.24 interface for HEIDENHAIN devices ..... 656

Non-HEIDENHAIN devices ..... 657

RS-422/V.11 interface ..... 658

Ethernet interface RJ45 socket ..... 658

14.3 Technical Information ..... 659

14.4 Exchanging the Buffer Battery ..... 666

15.1 Introduction ..... 668

End User License Agreement (EULA) for Windows 2000 ..... 668

General Information ..... 668

Specifications ..... 669

15.2 Starting an iTNC 530 Application ..... 670

Logging on to Windows ..... 670

Logging on as a TNC user ..... 670

Logging on as a local administrator ..... 671

15.3 Switching Off the iTNC 530 ..... 672

Fundamentals ..... 672

Logging a user off ..... 672

Exiting the iTNC application ..... 673

Shutting down Windows ..... 674

15.4 Network Settings ..... 675

Prerequisite ..... 675

Adjusting the network settings ..... 675

Controlling access ..... 676

15.5 Specifics About File Management ..... 677

The iTNC drive ..... 677

Data transfer to the iTNC 530 ..... 678

Overview tables ..... 687

Cycles ..... 687

Miscellaneous functions ..... 689

14 Tables and Overviews ..... 641

15 iTNC 530 with Windows 2000 (Option) ..... 667

Introduction

38 1 Introduction

1.1 The iTNC 530

1.1 The iTNC 530

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 iTNC 530 can
control up to 12 axes. You can also change the angular position of the
spindle under program control.

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

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

Programming: HEIDENHAIN conversational,
smarT.NC 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.

The smarT.NC operating mode offers TNC beginners an especially
simple possibility to quickly and without much training create
structured conversational dialog programs. Separate user
documentation is available for smarT.NC.

It is also possible to program in ISO format or DNC mode.
You can also enter and test one program while the control is running

another (does not apply to smarT.NC).

Compatibility

The TNC can run all part programs that were written on HEIDENHAIN
controls TNC 150 B and later. In as much as old TNC programs contain
OEM cycles, the iTNC 530 must be adapted to them with the PC
software CycleDesign. For more information, contact your machine
tool builder or HEIDENHAIN.

HEIDENHAIN iTNC 530 39

1.2 Visual Display Unit and Operating Panel

1.2 Visual Display Unit and
Operating Panel

Visual display unit

The TNC is delivered with the BF 150 (TFT) color flat-panel display (see
figure).

Screen layout

You select the screen layout yourself: In the PROGRAMMING AND
EDITING mode of operation, for example, you can have the TNC show
program blocks in the left window while the right window displays
programming graphics. You could also display the program structure
in the right window instead, or display only program blocks in one large
window. The available screen windows depend on the selected
operating mode.

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row
shows the available layout options (see “Modes of
Operation” on page 41).

Select the desired screen layout.

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 selection keys
4 Switches the soft-key rows
5 Sets the screen layout
6 Shift key for switchover between machining and programming

modes

7 Soft-key selection keys for machine tool builders
8 Switches soft-key rows for machine tool builders

1

3

1

1

4

4

5

1

6

7

8

2

40 1 Introduction

1.2 Visual Display Unit and Operating Panel

Operating panel

The TNC is delivered with the TE 530 operating panel. The figure
shows the controls and displays of the TE 530 keyboard unit.

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

1 Alphabetic keyboard for entering texts and file names, and for ISO

programming.
Dual-processor version: Additional keys for Windows operation

2  File Management

 Calculator
 MOD function
 HELP function

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
8 Touchpad: Only for operating the dual-processor version, soft

keys and smarT.NC

9 smarT.NC navigation keys

Some machine manufacturers do not use the standard
operating panel from HEIDENHAIN. Please refer to your
machine manual in these cases.

Machine panel buttons, e.g. NC START or NC STOP, are
also described in the manual for your machine tool.

1

2

3

5

1

4

6

77

1

79

8

HEIDENHAIN iTNC 530 41

1.3 Modes of Operation

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
previously)

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.

Soft keys for selecting the screen layout

Screen windows Soft key

Positions

Left: positions—Right: status display

Screen windows Soft key

Program

Left: program blocks—Right: status display

42 1 Introduction

1.3 Modes of Operation

Programming and editing

In this mode of operation you can write your part programs. The FK
free programming feature, the various cycles and the Q parameter
functions help you with programming and add necessary information.
If desired, the programming graphics or the 3-D line graphics (FCL 2
function) display the programmed traverse paths.

Soft keys for selecting the screen layout

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” on page 43.

Screen windows Soft key

Program

Left: program blocks, right: program structure

Left: program, right: programming graphics

Left: program, right: 3-D line graphics

HEIDENHAIN iTNC 530 43

1.3 Modes of Operation

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

Soft keys for selecting the screen layout for pallet tables

Screen windows Soft key

Program

Left: program blocks, right: program structure

Left: program, right: status

Left: program, right: graphics

Graphics

Screen windows Soft key

Pallet table

Left: program, right: pallet table

Left: pallet table, right: status

Left: pallet table, right: graphics

44 1 Introduction

1.4 Status Displays

1.4 Status Displays

“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:

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

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

 Positioning with Manual Data Input (MDI).

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

Information in the status display

Symbol Meaning

Actual or nominal coordinates of the current position.

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.

Axes are moving under a basic rotation.

PR Number of the active datum from the preset table. If

the datum was set manually, the TNC displays the
text MAN behind the symbol.

1

1

ACTL

.

X Y Z

F S M

HEIDENHAIN iTNC 530 45

1.4 Status Displays

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

Soft key Assignment Meaning

1 Name of the active main program

2 Active programs

3 Active machining cycle

4 Circle center CC (pole)

5 Machining time

6 Dwell time counter

7 Current time

4

6

1
2

3

5
6

7

46 1 Introduction

1.4 Status Displays

Positions and coordinates

Information on tools

Soft key Assignment Meaning

1 Position display

2 Type of position display, e.g. actual

position

3 Tilt angle of the working plane

4 Angle of a basic rotation

Soft key Assignment Meaning

1  T: Tool number and name

 RT: Number and name of a

replacement tool

2 Tool axis

3 Tool lengths 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

4

1

3

2

3

2

5

1

4

6

HEIDENHAIN iTNC 530 47

1.4 Status Displays

Coordinate transformations

See “Coordinate Transformation Cycles” on page 456.

Program section repeat/Subprograms

Soft key Assignment Meaning

1 Name of the active datum table

2 Active datum number (#), comment

from the active line of the active
datum number (DOC) from Cycle 7

3 Active datum shift (Cycle 7); The TNC

displays an active datum shift in up to
8 axes

4 Mirrored axes (Cycle 8)

5 Active rotation angle (Cycle 10)

6 Active scaling factor/factors (Cycles

11 / 26); The TNC displays an active
scaling factor in up to 6 axes

7 Scaling datum

Soft key Assignment Meaning

1 Active program section repeats with

block number, label number, and
number of programmed repeats/
repeats yet to be run

2 Active subprogram numbers with

block number in which the
subprogram was called and the label
number that was called

6

7

54

3

1
2

1

2

48 1 Introduction

1.4 Status Displays

Tool measurement

Active miscellaneous functions M

Soft key Assignment Meaning

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

Soft key Assignment Meaning

1 List of the active M functions with

fixed meaning

2 List of the active M functions that are

adapted by your machine
manufacturer

2

3

4

1

1

2

HEIDENHAIN iTNC 530 49

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

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:

 Automatically align workpieces
 Quickly and precisely set datums
 Measure the workpiece during program run
 Measure and inspect tools

TS 220 and TS 640 touch trigger probes

These touch probes are particularly effective for automatic workpiece
alignment, datum setting and workpiece measurement. The TS 220
transmits the triggering signals to the TNC via cable and is a cost­effective alternative for applications where digitizing is not frequently
required.

The TS 640 touch probe (see figure) features infrared transmission of
the triggering signal to the control. This makes it highly convenient for
use on machines with automatic tool changers.

Principle of operation: HEIDENHAIN triggering touch probes feature a
wear resisting optical switch that generates an electrical signal as
soon as the stylus is deflected. This signal is transmitted to the TNC,
which stores the current position of the stylus as an actual value.

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. Nr.: 329 203-xx.

50 1 Introduction

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

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 and HR 420 portable
handwheels. You will find a detailed description of HR 420 in Chapter
2 of this manual (see “HR 420 Electronic Handwheel” on page 58).

Manual Operation and Setup

52 2 Manual Operation and Setup

2.1 Switch-On, Switch-Off

2.1 Switch-On, Switch-Off

Switch-on

Switch on the power supply for control and machine. The TNC then
displays the following dialog:

The TNC memory is automatically checked.

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

The PLC program of the TNC is automatically compiled.

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

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.

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

MEMORY TEST

POWER INTERRUPTED

TRANSLATE PLC PROGRAM

RELAY EXT. DC VOLTAGE MISSING

MANUAL OPERATION
TRAVERSE REFERENCE POINTS

If your machine is equipped with absolute encoders, you
can leave out traversing the reference mark. In such a
case, the TNC is ready for operation immediately after the
machine control voltage is switched on.

HEIDENHAIN iTNC 530 53

2.1 Switch-On, Switch-Off

The TNC is now ready for operation 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
“Activating manual tilting” on page 79). The TNC then interpolates the
corresponding axes.

If available, you can also traverse the axes in the direction of the
current tool axis (see “Setting the current tool-axis direction as the
active machining direction (FCL 2 function)” on page 80).

If one of the two functions that were active before is active now, the
NC START button has no function. The TNC outputs a corresponding
error message.

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

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

If you use this function, then for non-absolute encoders
you must confirm the positions of the rotary axes, which
the TNC displays in a pop-up window. The position
displayed is the last active position of the rotary axes
before switch-off.

54 2 Manual Operation and Setup

2.1 Switch-On, Switch-Off

Switch-off

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

8 Select the Manual operating mode

8 Select the function for shutting down, confirm again

with the YES soft key.

8 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.

iTNC 530 with Windows 2000: See “Switching Off the
iTNC 530,” page 672.

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

HEIDENHAIN iTNC 530 55

2.2 Moving the Machine Axes

2.2 Moving the Machine Axes

Note

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

Move the axis continuously: Press and hold the
machine axis direction button, then press the
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” on page 64).

Traversing with the machine axis direction buttons can
vary depending on the machine tool. The machine tool
manual provides further information.

56 2 Manual Operation and Setup

2.2 Moving the Machine Axes

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.

Shift the soft-key row.

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.

JOG INCREMENT =

The maximum permissible value for infeed is 10 mm.

16

X

Z

8

8

8

HEIDENHAIN iTNC 530 57

2.2 Moving the Machine Axes

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:

The red indicator lights 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 if M118 is active.

Procedure:

Select the Electronic Handwheel operating mode.

Press and hold a permissive button.

Select the axis.

Select the feed rate.

Move the active axis in the positive direction, or

Move the active axis in the negative direction.

1 EMERGENCY OFF button
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)

2

4

6

8

1

3

4
5

7

58 2 Manual Operation and Setup

2.2 Moving the Machine Axes

HR 420 Electronic Handwheel

Unlike the HR 410, the HR 420 portable handwheel is equipped with
a display. In addition, you can run important setup functions through
the handwheel soft keys, e.g. setting datums or entering and running
M functions.

As soon as you press the handwheel activation key, it activates the
handwheel and deactivates the control panel. This is indicated by a
pop-up window on the TNC screen.

The HR 420 handwheel features the following operating elements:

If M118 is active, it is even possible to move the machine axes with the
handwheel during the program run.

1 EMERGENCY OFF button
2 Handwheel display for status display and function selection
3 Soft keys
4 Axis address keys
5 Handwheel activation key
6 Arrow keys for definition of handwheel sensitivity
7 Direction key by which the TNC moves the selected axis
8 Switch on the spindle (machine-specific M function)
9 Switch off the spindle (machine-specific M function)
10 NC-block creation key
11 NC start
12 NC stop
13 Permissive button
14 Handwheel
15 Spindle speed potentiometer
16 Feed rate potentiometer

Your machine manufacturer can make additional
functions of the HR 420 available. Please refer to your
machine manual.

2

5
7
8

1

3

4

6
7

9

11
12

14

16

15

13

10

6

HEIDENHAIN iTNC 530 59

2.2 Moving the Machine Axes

Display

The handwheel display has four lines (see figure). The TNC shows
there the following information:

Select the axis to be moved

You can activate directly through the axis address keys the principal
axes X, Y, Z and two other axes defined by the machine tool builder. If
you machine has more axes, proceed as follows.

8 Press the handwheel soft key F1 (AX): The TNC displays all active

axes on the handwheel display. The active axis blinks

8 Select the desired axis with the handwheel soft key F1 (->) or F2 (<-

) and confirm your selection with F3 (OK).

Set the handwheel sensitivity

The handwheel sensitivity defines the distance that an axis is to move
per handwheel revolution. The sensitivity levels are ready-defined and
are selectable with the handwheel arrow keys (unless incremental jog
is not active).

Selectable sensitivity levels: 0.01/0.02/0.05/0.1/0.2/0.5/1/2/5/10/20
[mm/revolution or degrees/revolution]

1 NOML X+1.563: Type of position display and position of the

selected axis

2 *: STIB (control is in operation)
3 S1000: Current spindle speed
4 F500: Feed rate at which the selected axis is moving
5 E: There is an error
6 3D: Tilted-working-plane function is active
7 2D: Basic rotation function is active
8 RES 5.0: Active handwheel resolution. Distance in mm/rev (°/rev

for rotary axes) that the selected axis moves for one handwheel
revolution

9 STEP ON or OFF: Incremental jog active or inactive. If the function

is active, the TNC also displays the active jog increment

10 Soft key row: Selection of various functions, described in the

following sections

1
3

8

2

4 to 7

9
10

60 2 Manual Operation and Setup

2.2 Moving the Machine Axes

Moving the Axes

Activate the handwheel: Press the handwheel key on
the HR 420. Now the TNC is operable only through
the HR 420. A pop-up window stating such appears
on the TNC screen.

Select the desired operating mode via the OPM soft key, if necessary
(see “Changing the modes of operation” on page 62).

If required, press and hold the permissive button

Use the handwheel to select the axis to be moved.
Select the additional axes via soft key

Move the active axis in the positive direction, or

Move the active axis in the negative direction.

Deactivate the handwheel: Press the handwheel key
on the HR 420. Now the TNC can be operated
through the control panel

Potentiometer settings

The potentiometers of the machine operating panel continue to be
active after you have activated the handwheel. If you want to use the
potentiometers on the handwheel, proceed as follows:

8 Press the CTRL and Handwheel keys in the HR 420. The TNC shows

the soft-key menu for selecting the potentiometers on the
handwheel display.

8 Press the HW soft key to activate the handwheel potentiometers.

If you have activated the potentiometers on the handwheel, you must
reactivate the potentiometers of the machine operating panel before
deselecting the handwheel. Proceed as follows:

8 Press the CTRL and Handwheel keys in the HR 420. The TNC shows

the soft-key menu for selecting the potentiometers on the
handwheel display.

8 Press the KBD soft key to activate the potentiometers of the

machine operating panel.

HEIDENHAIN iTNC 530 61

2.2 Moving the Machine Axes

Incremental Jog Positioning

With incremental jog positioning the TNC moves the currently active
handwheel axis by a preset distance defined by you.

8 Press the handwheel soft key F2 (STEP)
8 Activate incremental jog positioning: Press handwheel soft key 3

(ON)

8 Select the desired jog increment by pressing the F1 or F2 key. If you

press and hold the respective key, each time it reaches a decimal
value 0 the TNC increases the counting increment by a factor of 10.
If in addition you press the Ctrl key, the counting increment
increases to 1. The smallest possible jog increment is 0.0001 mm.
The largest possible is 10 mm

8 Confirm the selected jog increment with soft key 4 (OK)
8 With the + or – handwheel key, move the active handwheel axis in

the corresponding direction

Entering Miscellaneous Functions M

8 Press the handwheel soft key F3 (MSF)
8 Press the handwheel soft key F1 (M)
8 Select the desired M function number by pressing the F1 or F2 key
8 Execute the M function with the NC start key

Entering the spindle speed S

8 Press the handwheel soft key F3 (MSF)
8 Press the handwheel soft key F2 (S)
8 Select the desired speed by pressing the F1 or F2 key. If you press

and hold the respective key, each time it reaches a decimal value 0
the TNC increases the counting increment by a factor of 10. If in
addition you press the Ctrl key, the counting increment increases to
1000

8 Activate the new speed S with the NC start key

Enter the feed rate F

8 Press the handwheel soft key F3 (MSF)
8 Press the handwheel soft key F3 (F)
8 Select the desired feed rate by pressing the F1 or F2 key. If you

press and hold the respective key, each time it reaches a decimal
value 0 the TNC increases the counting increment by a factor of 10.
If in addition you press the Ctrl key, the counting increment
increases to 1000

8 Confirm the new feed rate F with the handwheel soft key F3 (OK)

62 2 Manual Operation and Setup

2.2 Moving the Machine Axes

Datum setting

8 Press the handwheel soft key F3 (MSF)
8 Press the handwheel soft key F4 (PRS)
8 If required, select the axis in which the datum is to be set
8 Reset the axis with the handwheel soft key F3 (OK), or with F1 and

F2 set the desired value and then confirm with F3 (OK). By also
pressing the Ctrl key, you can increase the counting increment to 10

Changing the modes of operation

With the handwheel soft key F4 (OPM), you can use the handwheel to
switch the mode of operation, provided that the current status of the
control allows a mode change.

8 Press the handwheel soft key F4 (OPM)
8 Select the desired operating mode by handwheel soft key

 MAN: Manual Operation
 MDI: Positioning with Manual Data Input
 SGL: Program Run, Single Block
 RUN: Program Run, Full Sequence

Generating a complete L Block

8 Select the Positioning with MDI operating mode
8 If required, use the arrow keys on the TNC keyboard to select the

NC block after which the new L block is to be inserted.

8 Actuate handwheel
8 Press the Generate-NC-block handwheel key: The TNC inserts a

complete L block containing all axis positions selected through the
MOD function

Use the MOD function to define the axis values to be
taken into an NC block (see “Selecting the Axes for
Generating L Blocks” on page 634).

If no axes are selected, the TNC displays the error
message No axes selected

HEIDENHAIN iTNC 530 63

2.2 Moving the Machine Axes

Features in the Program Run Modes of Operation

You can use the following functions in the Program Run modes of
operation:

 NC start (handwheel NC-start key)
 NC stop (handwheel NC-stop key)
 After the NC-stop key has been pressed: Internal stop (handwheel

soft keys MOP and then STOP)

 After the NC-stop key has been pressed: Manual axis traverse

(handwheel soft keys MOP and then MAN)

 Returning to the contour, after the axes were moved manually

during a program interruption (handwheel soft keys MOP and then
REPO). Operation is by handwheel soft key, which function similarly

to the control-screen soft keys (see “Returning to the contour” on
page 602)

 On/off switch for the Tilted Working Plane function (handwheel soft

keys MOP and then 3D)

64 2 Manual Operation and Setup

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

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

Function

In the Manual Operation and Electronic Handwheel operating modes,
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.”

Entering values

Spindle speed S, miscellaneous function M

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

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

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:

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

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

SPINDLE SPEED S =

1000

HEIDENHAIN iTNC 530 65

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

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.

66 2 Manual Operation and Setup

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

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

Note

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

Preparation

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

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

HEIDENHAIN iTNC 530 67

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

Datum setting with axis keys

Select the Manual Operation mode

Move the tool slowly until it touches (scratches) the
workpiece surface

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

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.

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.

DATUM SET Z=

Y

X

Z

X

Y

68 2 Manual Operation and Setup

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

Datum management with the preset table

Saving the datums in the preset table

The preset table has the name PRESET.PR, and is saved in the directory
TNC:\. PRESET.PR is editable only in the Manual and Electronic
Handwheel modes. In the Programming and Editing mode you can only

read the table, not edit it.
It is permitted to copy the preset table into another directory (for data

backup). Lines that were written by your machine tool builder are also
always write-protected in the copied tables. You therefore cannot edit
them.

Never change the number of lines in the copied tables! That could
cause problems when you want to reactivate the table.

To activate the preset table copied to another directory you have to
copy it back to the directory TNC:\.

You should definitely use the preset table if:

 Your machine is equipped with rotary axes (tilting table

or swivel head) and you work with the tilted working
plan function

 Your machine is equipped with a spindle-head changing

system

 Up to now you have been working with older TNC

controls with REF-based datum tables

 You wish to machine identical workpieces that are

differently aligned

The preset table can contain any number of lines
(datums). To optimize the file size and the processing
speed, you should use only as many lines as you need for
datum management.

For safety reasons, new lines can be inserted only at the
end of the preset table.

HEIDENHAIN iTNC 530 69

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

There are several methods for saving datums and/or basic rotations in
the preset table:

 Through probing cycles in the Manual or El. Handwheel modes (see

User’s Manual, Touch Probe Cycles, Chapter 2)

 Through the probing cycles 400 to 402 and 410 to 419 in automatic

mode (see User’s Manual, Touch Probe Cycles, Chapter 3)

 Manual entry (see description below)

Basic rotations from the preset table rotate the coordinate
system about the preset, which is shown in the same line
as the basic rotation.

When setting a preset, the TNC checks whether the
position of the tilting axes match the corresponding
values of the 3D ROT menu (depending on the MP
setting). Therefore:

 If the “Tilt working plane” function is not active, the

position displays for the rotary axes must = 0° (zero the
rotary axes if necessary).

 If the “Tilt working plane” function is active, the

position displays for the rotary axes must match the
angles entered in the 3D ROT menu.

The machine manufacturer can lock any lines in the preset
table in order to place fixed datums there (e.g. a center
point for a rotary table). Such lines in the preset table are
shown in a different color (default: red).

The line 0 in the preset table is write protected. In line 0,
the TNC always saves the datum that you most recently
set manually via the axis keys or via soft key. If the datum
set manually is active, the TNC displays the text PR MAN(0)
in the status display.

If you automatically set the TNC display with the touch­probe cycles for presetting, then the TNC does not store
these values in line 0.

70 2 Manual Operation and Setup

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

Manually saving the datums in the preset table

In order to set datums in the preset table, proceed as follows:

Select the Manual Operation mode

Move the tool slowly until it touches (scratches) the
workpiece surface, or position the measuring dial
correspondingly.

Displaying the preset table: The TNC opens the
preset table and sets the cursor to the active table
row.

Select functions for entering the presets: The TNC
display the available possibilities for entry in the soft­key row. See the table below for a description of the
entry possibilities.

Select the line in the preset table which you want to
change (the line number is the preset number).

If needed, select the column (axis) in the preset table
which you want to change.

Use the soft keys to select one of the available entry
possibilities (see the following table).

HEIDENHAIN iTNC 530 71

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

Function Soft key

Directly the assume the actual position of the
tool (the measuring dial) as the new datum: This
function only saves the datum in the axis whose
field is currently highlighted.

Assign any value to the actual position of the tool
(the measuring dial): This function only saves the
datum in the axis whose field is currently
highlighted. Enter the desired value in the pop-up
window.

Incrementally shift a datum already stored in the
table: This function only saves the datum in the
axis whose field is currently highlighted. Enter
the desired corrective value with the correct sign
in the pop-up window.

Directly enter the new datum without calculation
of the kinematics (axis-specific). Only use this
function if your machine has a rotary table, and
you want to set the datum to the center of the
rotary table by entering 0. This function only
saves the datum in the axis whose field is
currently highlighted. Enter the desired value in
the pop-up window.

Write the currently active datum to a selectable
line in the table: This function saves the datum in
all axes, and then activates the appropriate row in
the table automatically.

72 2 Manual Operation and Setup

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

Explanation of values saved in the preset table

 Simple machine with three axes without tilting device

The TNC saves in the preset table the distance from the workpiece
datum to the reference point (with the correct algebraic sign).

 Machine with swivel head

The TNC saves in the preset table the distance from the workpiece
datum to the reference point (with the correct algebraic sign).

 Machine with rotary table

The TNC saves in the preset table the distance from the workpiece
datum to the center of the rotary table (with the correct algebraic
sign).

 Machine with rotary table and swivel head

The TNC saves in the preset table the distance from the workpiece
datum to the center of the rotary table.

Keep in mind that moving an indexing feature on your
machine table (realized by changing the kinematics
description) requires you to redefine any workpiece-based
presets.

HEIDENHAIN iTNC 530 73

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

Editing the preset table

Editing function in table mode Soft key

Select beginning of table

Select end of table

Select previous page in table

Select next page in table

Select the functions for preset entry

Activate the datum of the selected line of the
preset table

Add the entered number of lines to the end of the
table (2nd soft-key row)

Copy the highlighted field (2nd soft-key row)

Insert the copied field (2nd soft-key row)

Reset the selected line: The TNC enters – in all
columns (2nd soft-key row)

Insert a single line at the end of the table
(2nd soft-key row)

Delete a single line at the end of the table
(2nd soft-key row)

74 2 Manual Operation and Setup

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

Activating the datum from the preset table in the Manual
operating mode

Select the Manual Operation mode

Display the preset table

Select the datum number that you want to activate, or

With the GOTO key, select the datum number that
you want to activate. Confirm with the ENT key.

Activate preset

Confirm activation of the datum. The TNC sets the
display and—if defined—the basic rotation

Leave the preset table

Activating the datum from the preset table in an NC program

To activate datums from the preset table during program run, use
Cycle 247. In Cycle 247 you define the number of the datum that you
want to activate (see “DATUM SETTING (Cycle 247)” on page 462).

When activating a datum from the preset table, the TNC
resets all coordinate transformations that were activated
with the following cycles:

 Cycle 7, Datum Shift
 Cycle 8, Mirroring
 Cycle 10, Rotation
 Cycle 11, Scaling
 Cycle 26, Axis-Specific Scaling

However, the coordinate transformation from Cycle 19,
Tilted Working Plane, remains active.

HEIDENHAIN iTNC 530 75

2.5 Tilting the Working Plane (Software Option 1)

2.5 Tilting the Working Plane
(Software Option 1)

Application, function

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 three functions available for tilting the working plane:

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

mode, see “Activating manual tilting” on page 79.

 Tilting under program control, Cycle 19 WORKING PLANE, in the part

program (see “WORKING PLANE (Cycle 19, software option 1)” on
page 468).

 Tilting under program control, PLANE function in the part program

(see “The PLANE Function: Tilting the Working Plane
(Software Option 1)” on page 482).

The TNC functions for “tilting the working plane” are coordinate
transformations in which the working plane is always perpendicular to
the direction of the tool axis.

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 rotary axes or as angular
components of a tilted plane. Refer to your machine
manual.

X

Z

Y

B

10°

76 2 Manual Operation and Setup

2.5 Tilting the Working Plane (Software Option 1)

When tilting the working plane, the TNC differentiates between two
machine types:

 Machine with tilting tables

 You must tilt the workpiece into the desired position for

machining by positioning the tilting table, for example with an L
block

 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.

 In calculating the transformed coordinate system, the TNC

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

 Machine with swivel head

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

positioning the swivel head, for example with an L block.

 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.

 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 that the actual angle of the tilted axis
was entered in the menu field.

HEIDENHAIN iTNC 530 77

2.5 Tilting the Working Plane (Software Option 1)

Setting the datum in a tilted coordinate system

After you have positioned the rotary axes, set the datum in the same
manner as for a non-tilted system. The behavior of the TNC during
datum setting depends on the settings of machine parameter 7500 in
your kinematics table:

 MP 7500, bit 5=0

With an active tilted working plane, the TNC checks during datum
setting in the X, Y and Z axes whether the current coordinates of the
rotary axes agree with the tilt angles that you defined (3D-ROT
menu). If the tilted working plane function is not active, the TNC
checks whether the rotary axes are at 0° (actual positions). If the
positions do not agree, the TNC will display an error message.

 MP 7500, bit 5=1

The TNC does not check whether the current coordinates of the
rotary axes (actual positions) agree with the tilt angles that you
defined.

Datum setting on machines with rotary tables

If you use a rotary table to align the workpiece, for example with
probing cycle 403, you must set the table position value to zero after
alignment and before setting the datum in the linear axes X, Y and Z.
The TNC will otherwise display an error message. Cycle 403 provides
you with an input parameter for this purpose (see User’s Manual for
Touch Probe Cycles, “Basic Rotation Compensation via Rotary Axis”).

Datum setting on machines with spindle-head
changing systems

If your machine is equipped with a spindle head changer, you should
use the preset table to manage your datums. Datums saved in preset
tables account for the active machine kinematics (head geometry). If
you exchange heads, the TNC accounts for the new head dimensions
so that the active datum is retained.

Always set a reference point in all three reference axes.
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.

78 2 Manual Operation and Setup

2.5 Tilting the Working Plane (Software Option 1)

Position display in a tilted system

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

Limitations on working with the tilting function

 The probing function for basic rotation is not available if you have

activated the working plane function in the Manual operating mode.

 PLC positioning (determined by the machine tool builder) is not

possible.

HEIDENHAIN iTNC 530 79

2.5 Tilting the Working Plane (Software Option 1)

Activating manual tilting

To select manual tilting, press the 3-D ROT soft key.

Use the arrow keys to move the highlight to the
Manual Operation menu item.

To activate manual tilting, press the ACTIVE soft key.

Use the arrow keys to position the highlight on the
desired rotary axis.

Enter the tilt angle.

To conclude entry, press the END key.

To reset the tilting function, set the desired operating modes in the
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 activate the “Tilt working plane” function for the Program Run
operating mode, the tilt angle entered in the menu becomes active in
the first block of the part program. If you use Cycle 19 WORKING PLANE
or the PLANE function in the machining program, the angle values
defined there are in effect. Angle values entered in the menu will be
overwritten.

80 2 Manual Operation and Setup

2.5 Tilting the Working Plane (Software Option 1)

Setting the current tool-axis direction as the
active machining direction (FCL 2 function)

In the Manual and El. Handwheel modes of operation you can use this
function to move the tool via the external direction keys or with the
handwheel in the direction that the tool axis is currently pointed. Use
this function if

 You want to retract the tool in the direction of the tool axis during

program interrupt of a 5-axis machining program.

 You want to machine with an inclined tool using the handwheel or

the external direction keys in the Manual operating mode.

To select manual tilting, press the 3-D ROT soft key.

Use the arrow keys to move the highlight to the
Manual Operation menu item.

To activate the current tool-axis direction as the active
machining direction, press the TOOL AXIS soft key.

To conclude entry, press the END key.

To reset the tilting function, set the Manual Operation menu item in
the “Tilt working plane” menu to inactive.

The symbol appears in the status display when the Move in tool-
axis direction function is active.

This function must be enabled by your machine
manufacturer. Refer to your machine manual.

The main axis of the active working plane (X with tool axis
Z) is always in the machine’s permanent main plane (Z/X
with tool axis Z).

This function is even available when you interrupt
program run and want to move the axes manually.

HEIDENHAIN iTNC 530 81

2.6 Dynamic Collision Monitoring (Software Option)

2.6 Dynamic Collision Monitoring
(Software Option)

Function

The machine manufacturer can define any objects that are monitored
by the TNC during all machining operations. If two objects monitored
for collision approach each other within a defined distance, the TNC
outputs an error message.

The TNC also monitors the current tool with the length and radius
entered in the tool table for collision (assuming a cylindrical tool).

The dynamic collision monitoring is active in all machine operating
modes, and is indicated by a symbol in the operating mode display.

Collision monitoring in the manual operating
modes

In the Manual and El. Handwheel operating modes, the TNC stops a
motion if two objects monitored for collision approach each other
within a specified distance. In addition, the TNC reduces the feed rate
significantly when the distance to the limit value triggering the error is
less than 5 mm.

There are three zones determining the TNC’s corrective behavior:

 Early warning: Two objects monitored for collision are within 14 mm

of each other

 Warning: Two objects monitored for collision are within 8 mm of

each other

 Error: Two objects monitored for collision are within 2 mm of each

other

The Dynamic Collision Monitoring DCM must be adapted
by the machine manufacturer for the TNC and for the
machine. Refer to your machine manual.

Please note that for certain tools (such as face milling
cutters), the diameter that would cause a diameter can be
greater than the dimensions defined in the tool­compensation data.

82 2 Manual Operation and Setup

2.6 Dynamic Collision Monitoring (Software Option)

Early warning zone

Two objects monitored for collision are within 12 to 14 mm of each
other The error message displayed (the machine manufacturer
determines the exact text) always starts with this text string: ]--[

8 Acknowledge the error message with the CE key.
8 Manually traverse the axes out of the danger zone. Pay attention to

the direction of traverse.

8 If applicable, remove the reason for the collision message.

Warning zone

Two objects monitored for collision are within 6 to 8 mm of each other
The error message displayed (the machine manufacturer determines
the exact text) always starts with this text string: ]-[

8 Acknowledge the error message with the CE key.
8 Manually traverse the axes out of the danger zone. Pay attention to

the direction of traverse.

8 If applicable, remove the reason for the collision message.

Error zone

Two objects monitored for collision are less than 2 mm from each
other The error message displayed (the machine manufacturer
determines the exact text) always starts with this text string: ][. In this
state you can only traverse the axes after deactivating collision
monitoring:

8 To select the menu for deactivating collision monitoring, press the

Collision Monitoring soft key (rear soft-key row).

8 Use the arrow keys to select the Manual Operation menu item.
8 To deactivate collision monitoring, press the ENT key, and the

symbol for collision monitoring in the operating mode display starts
to blink.

8 Acknowledge the error message with the CE key.
8 Manually traverse the axes out of the danger zone. Pay attention to

the direction of traverse.

8 If applicable, remove the reason for the collision message.
8 To reactivate collision monitoring, press the ENT key, and the

symbol for collision monitoring in the operating mode display
remains on again.

HEIDENHAIN iTNC 530 83

2.6 Dynamic Collision Monitoring (Software Option)

Collision monitoring in Automatic operation

The TNC monitors motions blockwise, i.e. it outputs a warning in the
block which would cause a collision, and interrupts program run. A
reduction of the feed rate, as with Manual operation, does not occur.

The handwheel superpositioning function with M118 is not
possible in combination with collision monitoring.

Positioning with Manual Data
Input (MDI)

86 3 Positioning with Manual Data Input (MDI)

3.1 Programming and Executing Simple Machining Operations

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 Positioning with MDI operating mode,
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 key.

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 in L blocks (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 1 PECKING.

Limitation
FK free contour programming, programming graphics and

program run graphics cannot be used. The $MDI file must
not contain a program call (PGM CALL).

Y

X

Z

50

50

0 BEGIN PGM $MDI MM
1 TOOL DEF 1 L+0 R+5

Define tool: zero tool, radius 5

2 TOOL CALL 1 Z S2000

Call tool: tool axis Z
spindle speed 2000 rpm

3 L Z+200 R0 FMAX

Retract tool (F MAX = rapid traverse)

4 L X+50 Y+50 R0 FMAX M3

Move the tool at F MAX to a position above the
hole,

spindle on

5 CYCL DEF 200 DRILLING

Define DRILLING cycle

Q200=5 ;SET-UP CLEARANCE

Set-up clearance of the tool above the hole

Q201=-15 ;DEPTH

Total hole depth (Algebraic sign=working direction)

HEIDENHAIN iTNC 530 87

3.1 Programming and Executing Simple Machining Operations

Straight line function L (see “Straight Line L” on page 214), DRILLING
cycle(see “DRILLING (Cycle 200)” on page 307).

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
Touch Probe 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: L C+2.561 F50

Conclude entry.

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

Q206=250 ;FEED RATE FOR PLNGNG

Feed rate for pecking

Q202=5 ;INFEED DEPTH

Depth of each infeed before retraction

Q210=0 ;DWELL TIME AT TOP

Dwell time after every retraction in seconds

Q203=-10 ;SURFACE COORDINATE

Coordinate of the workpiece surface

Q204=20 ;2ND SET-UP CLEARANCE

Set-up clearance of the tool above the hole

Q211=0.2 ;DWELL TIME AT DEPTH

Dwell time in seconds at the hole bottom

6 CYCL CALL

Call DRILLING cycle

7 L Z+200 R0 FMAX M2

Retract the tool

8 END PGM $MDI MM

End of program

88 3 Positioning with Manual Data Input (MDI)

3.1 Programming and Executing Simple Machining Operations

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.

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

Copy the file.

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

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” on page 103.

TARGET FILE =

If you wish to delete $MDI, then

 you must not have selected the Positioning with MDI

mode (not even in the background).

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

Programming and Editing mode.

BOREHOLE

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

90 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.1 Fundamentals

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. Linear axes are usually
equipped with linear encoders, rotary tables and tilting axes with angle
encoders.

When a machine axis moves, the corresponding position encoder
generates an electrical signal. The TNC evaluates this signal and
calculates the precise actual position of the machine axis.

If there is an interruption of power, the calculated position will no
longer correspond to the actual position of the machine slide. To
recover this association, incremental position encoders are provided
with reference marks. The scales of the position encoders contain one
or more reference marks that transmit a signal to the TNC when they
are crossed over. From the signal the TNC can re-establish the
assignment of displayed positions to machine positions. For linear
encoders with distance-coded reference marks the machine axes
need to move by no more than 20 mm, for angle encoders by no more
than 20°.

With absolute encoders, an absolute position value is transmitted to
the control immediately upon switch-on. In this way the assignment
of the actual position to the machine slide position is re-established
directly after switch-on.

Reference system

A reference system is required to define positions in a plane or in
space. The position data are always referenced to a predetermined
point and are described through coordinates.

The Cartesian coordinate system (a rectangular coordinate system) is
based on the three coordinate axes X, Y and Z. The axes are mutually
perpendicular and intersect at one point called the datum. A
coordinate identifies the distance from the datum in one of these
directions. A position in a plane is thus described through two
coordinates, and a position in space through three coordinates.

Coordinates that are referenced to the datum are referred to as
absolute coordinates. Relative coordinates are referenced to any other
known position (reference point) you define within the coordinate
system. Relative coordinate values are also referred to as incremental
coordinate values.

Y

X

Z

X (Z,Y)

X

MP

Y

X

Z

HEIDENHAIN iTNC 530 91

4.1 Fundamentals

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 “right­hand rule” is illustrated for remembering the three axis directions: the
middle finger points in the positive direction of the tool axis from the
workpiece toward the tool (the Z axis), the thumb points in the positive
X direction, and the index finger in the positive Y direction.

The iTNC 530 can control up to 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.

+X

+Y

+Z

+X

+Z

+Y

W+

C+

B+

V+

A+

U+

Y

X

Z

92 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.1 Fundamentals

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 a
circle center (CC), or pole. A position in a plane can be clearly defined
by the:

 Polar Radius, the distance from the circle center CC to the position,

and the

 Polar Angle, the size of the angle between the reference axis and

the line that connects the circle center CC with the position.

Setting the pole and the angle reference axis

The pole is set by entering two Cartesian coordinates in one of the
three planes. These coordinates also set the reference axis for the
polar angle PA.

Coordinates of the pole (plane) Reference axis of the angle

X/Y +X

Y/Z +Y

Z/X +Z

X

Y

0°

30

10

CC

PR

PA

1

PA

2

PR

PR

PA

3

X

Z

Y

X

Z

Y

X

Z

Y

HEIDENHAIN iTNC 530 93

4.1 Fundamentals

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

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 prefix “I”
before the axis.

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

Y = 10 mm

Absolute and incremental polar coordinates

Absolute polar coordinates always refer to the pole and the reference
axis.

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

Hole 1 Hole 2 Hole 3
X = 10 mm X = 30 mm X = 50 mm
Y = 10 mm Y = 20 mm Y = 30 mm

Hole 5, referenced to 4 Hole 6, referenced to 5
X = 20 mm X = 20 mm
Y = 10 mm Y = 10 mm

X

Y

30

20

50

3010

10

2

1

3

X

Y

20

10 10

20

10

10

5

4

6

X

Y

0°

30

10

CC

PR

PA

+IPA

PR

PR

+IPA

+IPR

94 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.1 Fundamentals

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 to either zero or 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 456).

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 “Setting the Datum
with a 3-D Touch Probe” in the Touch Probe Cycles User’s Manual.

Example

The workpiece drawing shows holes (1 to 4) whose dimensions are
shown with respect to an absolute datum with the coordinates X=0
Y=0. 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.

Y

X

Z

MAX

MIN

X

Y

325

320

0

450 900

950

150

-150

750

0

300

±

0,1

21

3 4

7
6

5

HEIDENHAIN iTNC 530 95

4.2 File Management: Fundamentals

4.2 File Management:
Fundamentals

Files

When you write a part program on the TNC, you must first enter a file
name. The TNC saves the program to the hard disk 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.

You can manage nearly any number of files with the TNC, at least

25 GB (dual-processor version: 13 GB).

File names

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

File names should not exceed 25 characters, otherwise the TNC
cannot display the entire file name. The characters * \ / “ ? < > .
are not permitted in file names.

Files in the TNC Ty p e
Programs

In HEIDENHAIN format
In ISO format

.H
.I

smarT.NC files

Structured unit program
Contour descriptions
Point tables for machining positions

.HU
.HC
.HP

Tables for

Tools
Tool changers
Pallets
Datums
Points
Presets
Cutting data
Cutting materials, workpiece materials
Dependent data (such as structure items)

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

Texts as

ASCII files .A

Drawing data as

ASCII files .DXF

PROG20 .H
File name File type

96 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.2 File Management: Fundamentals

Data backup

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

The TNCremoNT data transmission freeware from HEIDENHAIN is a
simple and convenient method for backing up data stored on the TNC.

You additionally need a data medium on which all machine-specific
data, such as the PLC program, machine parameters, etc., are stored.
Ask your machine manufacturer for assistance, if necessary.

Saving the contents of the entire hard disk (> 2 GB) can
take up to several hours. In this case, it is a good idea to
save the data outside of work hours, e.g. during the night.

Depending on operating conditions (e.g., vibration load),
hard disks generally have a higher failure rate after three to
five years of service. HEIDENHAIN therefore
recommends having the hard disk inspected after three to
five years.

HEIDENHAIN iTNC 530 97

4.3 Working with the file manager

4.3 Working with the file manager

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. With the –/+ key or
ENT you can show or hide the subdirectories.

Directory names

The name of a directory can contain up to 16 characters and does not
have an extension. If you enter more than 16 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.H was copied into it. The part program now has the
following path:

TNC:\AUFTR1\NCPROG\PROG1.H

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

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!

TNC:\

AUFTR1

NCPROG

WZTAB

A35K941

ZYLM

TESTPROG

HUBER

KAR25T

98 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.3 Working with the file manager

Overview: Functions of the File Manager

Function Soft key Page

Copy (and convert) individual files page 103

Select target directory page 103

Display a specific file type page 100

Display the last 10 files that were
selected

page 105

Erase a file or directory page 106

Tag a file page 107

Renaming a file page 108

Protect a file against editing and erasure page 108

Cancel file protection page 108

Manage network drives page 112

Copying a directory page 105

Display all the directories of a particular
drive

Delete directory with all its
subdirectories

page 108

HEIDENHAIN iTNC 530 99

4.3 Working with the file manager

Calling the File Manager

Press the PGM MGT key: The TNC displays the file
management window (see figure for default setting.
If the TNC displays a different screen layout, press
the WINDOW soft key.)

The narrow window on the left shows the available drives and
directories. 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. A directory is always identified by a
folder 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. A box with the + symbol in front of the folder symbol
indicates that there are further subdirectories, which can be shown
with the –/+ key or ENT.

The wide window on the right shows you all files that are stored in the
selected directory. Each file is shown with additional information,
illustrated in the table below.

Display Meaning

FILE NAME Name with up to 16 characters and file type

BYTE File size in bytes

STATUS

E

S

M

P

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 mode
of operation.

File is protected against editing and erasure.

DATE Date the file was last changed

TIME Time the file was last changed

100 4 Fundamentals of NC, File Management, Programming Aids, Pallet Management

4.3 Working with the file manager

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.

Step 1: Select drive

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

To select a drive, press the SELECT soft key, or

Press the ENT key.

Step 2: 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.