HEIDENHAIN TNC 426B User Manual

Download

TNC 410 TNC 426 TNC 430

NC Software 286 060-xx 286 080-xx 280 472-xx 280 473-xx 280 474-xx 280 475-xx

User's Manual

ISO Programming

4/99

Controls on the visual display unit

Split screen layout

Switch between machining or programming modes

Soft keys for selecting functions in screen

Switching the soft-key rows

Changing the screen settings

Controls on the TNC

(only BC 120)

Typewriter keyboard for entering letters and symbols

W E

F S T M

Comments

ISO programs

File name

Machine operating modes

Manual Operation

Electronic Handwheel

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

PGM MGT

External data transfer

PGM

Enter program call in a program

CALL

MOD

MOD functions

HELP

Displaying help texts for NC error messages

CALC

Pocket calculator

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

Move highlight

GOTO

Go directly to blocks, cycles and parameter functions

Override control knobs for feed rate/spindle speed

100

F %

100

S %

Programming path movements (only conversational)

APPR

Approach/depart contour

DEP

FK free contour programming

Straight line

Circle center/pole for polar coordinates

Circle with center

Circle with radius

Circular arc with tangential connection

CHF

Chamfer

RND

Corner rounding

Tool data (only conversational)

TOOL

DEF

Entering and calling tool length and

TOOL CALL

radius

Cycles, subprograms, and program section repeats (only conversational)

CYCL

DEF

LBL SET

Define and call cycles

CALL

LBL

Enter and call labels for

CALL

subprogramming and program section repeats

STOP

Program stop in a program

TOUCH

Enter touch probe functions in a program

PROBE

Coordinate axes and numbers, editing

...

Select coordinate axes or enter

them in a program

Numbers

Decimal point

Change arithmetic sign

Polar coordinates

Incremental dimensions

Q parameters

Capture actual position

Skip dialog questions, delete words

ENT

END

Clear numerical entry or TNC error message

DEL

Confirm entry and resume dialog

End block

Abort dialog, delete program section

TNC Models, Software and Features

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

TNC Model NC Software No.

TNC 410 286 060-xx TNC 410 286 080-xx TNC 426 CB, TNC 426 PB 280 472-xx TNC 426 CF, TNC 426 PF 280 473-xx TNC 430 CA, TNC 430 PA 280 472-xx TNC 430 CE, TNC 430 PE 280 473-xx TNC 426 CB, TNC 426 PB 280 474-xx TNC 426 CF, TNC 426 PF 280 475-xx TNC 426 M 280 474-xx TNC 426 ME 280 475-xx TNC 430 CA, TNC 430 PA 280 474-xx TNC 430 CE, TNC 430 PE 280 475-xx TNC 430 M 280 474-xx TNC 430 ME 280 475-xx

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

■ Probing function for the 3-D touch probe

■ Digitizing option (conversational programming only)

■ Tool measurement with the TT 120 (conversational

programming only)

■ Rigid tapping

■ Returning to the contour after an interruption

Please contact your machine tool builder to become familiar with the individual implementation of the control on your machine.

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

Touch Probe Cycles User's Manual:

In addition to this manual, another manual is available describing all the touch probe functions of the TNC 426 / TNC 430. Please contact HEIDENHAIN if you require a copy of this User's Manual. ID number: 329 203-xx.

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.

Contents

IHEIDENHAIN TNC 410, TNC 426, TNC 430

Contents

Introduction

Manual Operation and Setup

Positioning with Manual Data Input (MDI)

Programming: Fundamentals of NC, File Management, Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Cycles

Programming: Subprograms and Program Section Repeats

Programming: Q Parameters

Test Run and Program Run

3-D Touch Probes

Contents

3 4 5 6 7 8 9

MOD Functions

Tables and Overviews

13 14

IIIHEIDENHAIN TNC 410, TNC 426, TNC 430

1 INTRODUCTION ..... 1

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

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

Contents

1.3 Modes of Operation ..... 5

1.4 Status Displays ..... 9

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

2 MANUAL OPERATION AND SETUP ..... 15

2.1 Switch-on, Switch-off ..... 16

2.2 Moving the Machine Axes ..... 17

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 19

2.4 Datum Setting (Without a 3-D Touch Probe) ..... 20

2.5 Tilt the working plane (not TNC 410) ..... 21

3 POSITIONING WITH MANUAL DATA INPUT (MDI) ..... 25

3.1 Program and Run Simple Machining Operations ..... 26

4 PROGRAMMING: FUNDAMENTALS OF NC, FILE MANAGEMENT,

PROGRAMMING AIDS, PALLET MANAGEMENT ..... 31

4.1 Fundamentals of NC ..... 32

4.2 File Management: Fundamentals ..... 37

4.3 Standard file management TNC 426, TNC 430 ..... 38

4.4 Expanded File Management TNC 426, TNC 430 ..... 43

4.5 File Management for the TNC 410 ..... 56

4.6 Creating and Writing Programs ..... 59

4.7 Programming Graphics (not TNC 426, TNC 430) ..... 66

4.8 Adding Comments ..... 68

4.9 Creating Text Files (not TNC 410) ..... 69

4.10 The Pocket Calculator (not TNC 410) ..... 72

4.11 Direct Help for NC Error Messages (not TNC 410) ..... 73

4.12 Help Function (not TNC 426, TNC 430) ..... 74

4.13 Pallet Management (not TNC 410) ..... 75

Contents

5 PROGRAMMING: TOOLS ..... 77

5.1 Entering Tool-Related Data ..... 78

5.2 Tool Data ..... 79

5.3 Tool Compensation ..... 90

6 PROGRAMMING: PROGRAMMING CONTOURS ..... 95

6.1 Overview of Tool Movements ..... 96

6.2 Fundamentals of Path Functions ..... 97

6.3 Contour Approach and Departure ..... 99

6.4 Path Contours — Cartesian Coordinates ..... 102

Overview of path functions ..... 102

Straight line at rapid traverse G00, Straight line with feed rate G01 F . . . ..... 103

Inserting a chamfer between two straight lines ..... 103

Circle center I, J ..... 104

Circular path G02/G03/G05 around the circle center I, J ..... 104

Circular path G02/G03/G05 with defined radius ..... 105

Rounding corners G25 ..... 108

Example: Linear movements and chamfers with Cartesian coordinates ..... 109

Example: Circular movements with Cartesian coordinates ..... 110

Example: Full circle with Cartesian coordinates ..... 111

6.5 Path Contours—Polar Coordinates ..... 112

Zero point for polar coordinates: pole I, J ..... 112

Straight line at rapid traverse G10, Straight line with feed rate G11 F . . . ..... 113

Circular path G12/G13/G15 around pole I, J ..... 113

Circular path G16 with tangential approach ..... 114

Helical interpolation ..... 114

Example: Linear movement with polar coordinates ..... 116

Example: Helix ..... 117

Contents

VHEIDENHAIN TNC 410, TNC 426, TNC 430

7 PROGRAMMING: MISCELLANEOUS FUNCTIONS ..... 119

7.1 Entering Miscellaneous Functions M ..... 120

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 121

Contents

7.3 Miscellaneous Functions for Coordinate Data ..... 121

7.4 Miscellaneous Functions for Contouring Behavior ..... 124

Smoothing corners: M90 ..... 124

Entering contour transitions between two contour elements: M112 (not TNC 426, TNC 430) ..... 125

Contour filter: M124 (not TNC 426, TNC 430) ..... 127

Machining small contour steps: M97 ..... 129

Machining open contours: M98 ..... 130

Feed rate factor for plunging movements: M103 ..... 131

Feed rate in micrometers per spindle revolution: M136

(only TNC 426, TNC 430 with NC software 280 474-xx) ..... 131

Feed rate at circular arcs: M109/M110/M111 ..... 132

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 132

Superimposing handwheel positioning during program run: M118 (not TNC 410) ..... 133

7.5 Miscellaneous Functions for Rotary Axes ..... 134

Feed rate in mm/min on rotary axes A, B, C: M116 (not TNC 410) ..... 134

Shorter-path traverse of rotary axes: M126 ..... 134

Reducing display of a rotary axis to a value less than 360°: M94 ..... 135

Automatic compensation of machine geometry when working with tilted axes: M114

(not TNC 410) ..... 136

Maintaining the position of the tool tip when positioning with tilted axes (TCPM*): M128 ..... 137

Exact stop at corners with nontangential transitions: M134 ..... 139

Selection of tilting axes: M138 (only TNC 426, TNC 430 with NC software 280 474-xx) ..... 139

7.6 Miscellaneous Functions for Laser Cutting Machines (not TNC 410) ..... 140

Contents

8 PROGRAMMING: CYCLES ..... 141

8.1 General Information on Cycles ..... 142

8.2 Point Tables (only TNC 410) ..... 144

Creating a point table ..... 144

Selecting point tables in the program ..... 144

Calling a cycle in connection with point tables ..... 145

8.3 Drilling Cycles ..... 146

PECKING (Cycle G83) ..... 146

DRILLING (Cycle G200) ..... 148

REAMING (Cycle G201) ..... 149

BORING (Cycle G202) ..... 150

UNIVERSAL DRILLING (Cycle G203) ..... 151

BACK BORING (Cycle G204) ..... 153

UNIVERSAL PECKING (Cycle G205, only with the TNC 426, TNC 430 with NC software 280 474-xx) ..... 155

BORE MILLING (Cycle G208, only with the TNC 426, TNC 430 with NC software 280 474-xx) ..... 157

TAPPING with a floating tap holder (Cycle G84) ..... 159

TAPPING NEW with floating tap holder (Cycle G206, only with TNC 426, TNC 430

with NC software 280 474-xx) ..... 160

RIGID TAPPING (Cycle G85) ..... 162

RIGID TAPPING NEW(Cycle G207, only with the TNC 426, TNC 430 with NC software 280 474-xx) ..... 163

THREAD CUTTING (Cycle G86, not TNC 410) ..... 165

Example: Drilling cycles ..... 166

Example: Drilling cycles ..... 167

Example: Calling drilling cycles in connection with point tables (only with TNC 410) ..... 168

8.4 Cycles for milling pockets, studs and slots ..... 170

POCKET MILLING (Cycles G75, G76) ..... 171

POCKET FINISHING (Cycle G212) ..... 172

STUD FINISHING (Cycle G213) ..... 174

CIRCULAR POCKET MILLING (Cycles G77, G78) ..... 175

CIRCULAR POCKET FINISHING (Cycle G214) ..... 177

CIRCULAR STUD FINISHING (Cycle G215) ..... 178

SLOT MILLING (Cycle G74) ..... 180

SLOT with reciprocating plunge-cut (Cycle G210) ..... 181

CIRCULAR SLOT with reciprocating plunge-cut (Cycle G211) ..... 183

Example: Milling pockets, studs and slots ..... 185

Contents

VIIHEIDENHAIN TNC 410, TNC 426, TNC 430

8.5 Cycles for Machining Hole Patterns ..... 186

Contents

8.6 SL Cycles Group I ..... 191

8.7 SL Cycles Group II (not TNC 410) ..... 197

8.8 Cycles for Face Milling ..... 216

CIRCULAR PATTERN (Cycle 220) ..... 187

LINEAR PATTERN (Cycle 221) ..... 188

Example: Circular hole patterns ..... 191

CONTOUR GEOMETRY (Cycle G37) ..... 192

PILOT DRILLING (Cycle G56) ..... 193

ROUGH-OUT (Cycle G57) ..... 194

CONTOUR MILLING (Cycle G58/G59) ..... 196

CONTOUR GEOMETRY (Cycle G37) ..... 199

Overlapping contours ..... 199

CONTOUR DATA (Cycle G120) ..... 201

PILOT DRILLING (Cycle G121) ..... 202

ROUGH-OUT (Cycle G122) ..... 203

FLOOR FINISHING (Cycle G123) ..... 204

SIDE FINISHING (Cycle G124) ..... 205

CONTOUR TRAIN (Cycle G125) ..... 206

CYLINDER SURFACE (Cycle G127) ..... 208

CYLINDER SURFACE slot milling (Cycle G128, only in TNC 426, TNC 430 with

NC software 280 474-xx) ..... 210

Example: Pilot drilling, roughing-out and finishing overlapping contours ..... 212

Example: Cylinder surface ..... 214

Example: Contour train ..... 215

RUN DIGITIZED DATA (Cycle G60, not TNC 410) ..... 216

MULTIPASS MILLING (Cycle G230) ..... 218

RULED SURFACE (Cycle 231) ..... 220

Example: Multipass milling ..... 222

VIII

Contents

8.9 Coordinate transformation cycles ..... 223

DATUM SHIFT (Cycle G54) ..... 224

DATUM SHIFT with datum tables (Cycle G53) ..... 225

MIRROR IMAGE (Cycle G28) ..... 228

ROTATION (Cycle G73) ..... 229

SCALING FACTOR (Cycle G72) ..... 230

WORKING PLANE (Cycle G80, not TNC 410) ..... 231

Example: Coordinate transformation cycles ..... 236

8.10 Special Cycles ..... 238

DWELL TIME (Cycle G04) ..... 238

PROGRAM CALL (Cycle G39) ..... 238

ORIENTED SPINDLE STOP (Cycle G36) ..... 239

TOLERANCE (Cycle G62, not TNC 410) ..... 240

9 PROGRAMMING: SUBPROGRAMS AND PROGRAM SECTION REPEATS ..... 241

9.1 Marking Subprograms and Program Section Repeats ..... 242

9.2 Subprograms ..... 242

9.3 Program Section Repeats ..... 243

9.4 Program as Subprogram ..... 244

9.5 Nesting ..... 245

9.6 Programming Examples ..... 248

Example: Milling a contour in several infeeds ..... 248

Example: Groups of holes ..... 249

Example: Groups of holes with several tools ..... 250

Contents

10 PROGRAMMING: Q PARAMETERS ..... 253

10.1 Principle and Overview ..... 254

10.2 Part Families — Q Parameters in Place of Numerical Values ..... 255

10.3 Describing Contours Through Mathematical Functions ..... 256

10.4 Trigonometric Functions ..... 258

10.5 If-Then Decisions with Q Parameters ..... 259

10.6 Checking and Changing Q Parameters ..... 260

10.7 Additional Functions ..... 261

10.8 Entering Formulas Directly ..... 263

10.9 Preassigned Q Parameters ..... 266

10.10 Programming Examples ..... 269

Example: Ellipse ..... 269

Example: Concave cylinder machined with spherical cutter ..... 271

Example: Convex sphere machined with end mill ..... 273

IXHEIDENHAIN TNC 410, TNC 426, TNC 430

11 TEST RUN AND PROGRAM RUN ..... 275

11.1 Graphics ..... 276

11.2 Functions for Program Display in Program Run and Test Run ..... 281

Contents

11.3 Test run ..... 282

11.4 Program Run ..... 284

11.5 Blockwise Transfer: Running Long Programs (not with TNC 426, TNC 430) ..... 292

11.6 Optional block skip ..... 293

11.7 Optional Program Run Interruption (not TNC 426, TNC 430) ..... 293

12 3-D TOUCH PROBES ..... 295

12.1 Touch Probe Cycles in the Manual and Electronic Handwheel ..... 296

12.2 Setting the Datum with a 3-D Touch Probe ..... 304

12.3 Measuring Workpieces with a 3-D Touch Probe ..... 307

13 MOD FUNCTIONS ..... 313

13.1 Selecting, Changing and Exiting the MOD Functions ..... 314

13.2 System Information (not TNC 426, TNC 430) ..... 315

13.3 Software Numbers and Option Numbers TNC 426, TNC 430 ..... 316

13.4 Code Number ..... 316

13.5 Setting the Data Interface for the TNC 410 ..... 317

Setting the OPERATING MODE of the external device ..... 317

Setting the BAUD RATE ..... 317

13.6 Setting Up the Data Interfaces for TNC 426, TNC 430 ..... 318

13.7 Software for Data Transfer ..... 320

13.8 Ethernet Interface (only TNC 426, TNC 430) ..... 322

13.9 Configuring PGM MGT (not TNC 410) ..... 329

13.10 Machine-Specific User Parameters ..... 329

13.11 Showing the Workpiece in the Working Space (not TNC 410) ..... 329

13.12 Position Display Types ..... 331

13.13 Unit of Measurement ..... 331

13.14 Programming Language for MDI ..... 332

13.15 Selecting the Axes for Generating L Blocks (not TNC 410, only Conversational Dialog) ..... 332

13.16 Axis Traverse Limits, Datum Display ..... 332

13.17 The HELP Function ..... 334

13.18 Operating Time (via Code Number for TNC 410) ..... 334

Contents

TABLES AND OVERVIEWS ..... 335

14.1 General User Parameters ..... 336

14.2 Pin Layout and Connecting Cable for the Data Interfaces ..... 352

14.3 Technical Information ..... 356

14.4 Exchanging the Buffer Battery ..... 360

14.5 Addresses (ISO) ..... 360

Contents

XIHEIDENHAIN TNC 410, TNC 426, TNC 430

Introduction

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

HEIDENHAIN TNC controls are workshop-oriented contouring controls that enable you to program conventional machining operations right at the machine in an easy-to-use conversational programming language. They are designed for milling, drilling and boring machines, as well as for machining centers. The TNC 410 can control up to 4 axes, the TNC 426 up to 5 axes, and the TNC 430 up to 9 axes. You can also change the angular position of the spindle under program control.

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

Programming: HEIDENHAIN conversational and ISO formats

HEIDENHAIN conversational programming is an especially easy method of writing programs. Interactive graphics illustrate the individual machining steps for programming the contour. If a production drawing is not dimensioned for NC, the HEIDENHAIN FK free contour programming carries out the necessary calculations automatically. Workpiece machining can be graphically simulated either during or before actual machining. It is also possible to program in ISO format or DNC mode.

You can enter a program while the control is running another. With the TNC 426, TNC 430 it is also possible to test one program while another is being run.

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

Compatibility

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

1 Introduction

1.2 Visual Display Unit and Keyboard

Visual display unit

The TNC is available with either a color CRT screen (BC 120) or a TFT flat panel display (BF 120. The figures at right show the keys and controls on the BC 120 (upper right) and the BF 120 (middle right).

Header When the TNC is on, the selected operating modes are shown in the screen header. With the TNC 426, TNC 430, the machine operating modes are on the left and the programming modes are on the 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).

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 soft-key row indicate the number of soft-key rows that can be called with the black arrow keys to the The line representing the active soft-key row is highlighted.

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

modes

. The lines immediately above the

outside right and left.

1.2 Visual Display Unit and Keyboard

Keys on BC 120 only

Screen demagnetization; Exit main menu for screen settings

Select main menu for screen settings; In the main menu: Move highlight downward In the submenu: Reduce value

In the main menu: Move highlight upward In the submenu: Increase value

In the main menu: Select submenu

In the submenu: Exit submenu

See next page for the screen settings.

Move picture to the left or downward

Move picture to the right or upward

3HEIDENHAIN TNC 410, TNC 426, TNC 430

Main menu dialog Function

BRIGHTNESS Adjust brightness CONTRAST Adjust contrast H-POSITION Adjust horizontal position H-SIZE Adjust picture width V-POSITION Adjust vertical position V-SIZE Adjust picture height SIDE-PIN Correct barrel-shaped distortion TRAPEZOID Correct trapezoidal distortion ROTATION Correct tilting COLOR TEMP Adjust color temperature R-GAIN Adjust strength of red color B-GAIN Adjust strength of blue color RECALL No function

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

Screen layout

1.2 Visual Display Unit and Keyboard

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 (only TNC 410). The available screen windows depend on the selected operating mode.

To change the screen layout:

Press the switch-over key: The soft-key row shows the available layout options (see section

1.3 ”Modes of Operation”).

Select the desired screen layout.

1 Introduction

Keyboard

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

Alphanumeric keyboard for entering texts and file names, as well as for programming in ISO format

File management, pocket calculator (not TNC 410), MOD function, HELP function

Programming modes Machine operating modes Initiation of programming dialog Arrow keys and GOTO jump command Numerical input and axis selection

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

1.3 Modes of Operation

The TNC offers the following modes of operation for the various functions and working steps that you need to machine a workpiece:

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 describe above, TNC 410: see screen layout with program run, full sequence)

Screen windows Soft key

Positions

Left: positions. Right: status display.

5HEIDENHAIN TNC 410, TNC 426, TNC 430

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

Program

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

1.3 Modes of Operation

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

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

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

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

1 Introduction

Programming and Editing

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

Soft keys for screen layout (not for TNC 426, TNC 430)

Screen windows Soft key

Program

Left: program. Right: help graphics for cycle programming

Left: program. Right: programming graphics

Interactive Programming Graphics

1.3 Modes of Operation

7HEIDENHAIN TNC 410, TNC 426, TNC 430

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.

Program Run, Full Sequence and Program Run, Single Block

1.3 Modes of Operation

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

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

Soft keys for selecting the screen layout

Screen windows Soft key

Program

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

Left: program blocks, right: graphics (only TNC 426, TNC 430)

Graphics (only TNC 426, TNC 430)

Screen windows Soft key

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

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

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

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

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

1 Introduction

1.4 Status Displays

“General” status display

The status display 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 operating modes Manual and Electronic Handwheel, the status display is shown in the large window.

Information in the status display

The Meaning

ACTL. Actual or nominal coordinates of the current position

X Y Z 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

F S M The displayed feed rate in inches corresponds to

one tenth of the effective value. Spindle speed S, feed rate F and active M functions

Program run started

# Axis locked

Axis can be moved with the handwheel

Axes are moving in a tilted working plane (not TNC 410)

1.4 Status Displays

Axes are moving under a basic rotation

9HEIDENHAIN TNC 410, TNC 426, TNC 430

Additional status displays

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

To switch on the additional status display:

Call the soft-key row for screen layout.

1.4 Status Displays

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

Select the layout option for the 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.

1 Introduction

General program information

Name of main program Active programs Active machining cycle Circle center CC (pole) Operating time Dwell time counter

Positions and coordinates

Position display Type of position display, e.g. actual positions Tilting angle for the working plane (not TNC 410) Angle of a basic rotation

1.4 Status Displays

11HEIDENHAIN TNC 410, TNC 426, TNC 430

Information on tools

T: Tool number and name RT: Number and name of a replacement tool

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

table (TAB) Tool life, maximum tool life (TIME 1) and maximum tool life for

1.4 Status Displays

TOOL CALL (TIME 2) Display of the active tool and the (next) replacement tool

Coordinate transformations

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

For further information, refer to section 8.8 “Coordinate Transformation Cycles.”

Tool measurement

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

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

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

Cutting edge number with the corresponding measured value. If the measured value is followed by an asterisk, the allowable tolerance in the tool table was exceeded.

1 Introduction

Active miscellaneous functions M

(only TNC 426, TNC 430 with NC software 280 474-xx)

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

manufacturer.

1.4 Status Displays

13HEIDENHAIN TNC 410, TNC 426, TNC 430

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

■ Digitize 3-D surfaces (option), and

■ Measure and inspect tools

TS 220 and TS 630 touch trigger probes

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

The TS 630 features infrared transmission of the triggering signal to the TNC. 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.

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

TT 120 tool touch probe for tool measurement

The TT 120 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 (only for conversational programming).

The TT 120 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

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

optical switch.

HR electronic handwheels

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

1 Introduction

Manual Operation and Setup

2.1 Switch-on, Switch-off

Switch-On

Switch-on and traversing the reference points can vary depending on the individual machine tool. Your machine manual provides more detailed information.

ú Switch on the power supply for control and machine.

The TNC automatically initiates the following dialog

Memory Test

The TNC memory is automatically checked.

2.1 Switch-on, Switch-off

Power Interrupted

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

Translate PLC Program

The PLC program of the TNC is automatically compiled.

Relay Ext. DC Voltage Missing

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

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

For the TNC 426, TNC 430:

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

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

Traversing the reference point in a tilted working plane

The reference point of a tilted coordinate system can be traversed by pressing the machine axis direction buttons. The “tilting the working plane” function (see section 2.5 “Tilting the Working Plane”) must be active in the Manual Operation mode. The TNC then interpolates the corresponding axes.

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

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

Manual Operation Traverse Reference Points

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

Cross the reference points in any sequence:

Press and hold the external direction button for each axis until the reference point has been traversed, or additionally for the TNC 410

Cross the reference points with several axes at

the same time: Use soft keys to select the axes (axes are then shown highlighted on the screen), and then press the machine START button.

Switch-off

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

ú Select the Manual mode

ú Select the function for run-down,

confirm again with the YES soft key.

ú When the TNC displays the message

„Now you can switch off the TNC“ in a superimposed window, you may cut off the power supply to the TNC.

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

2 Manual Operation and Setup

2.2 Moving the Machine Axes

Traversing with the machine axis direction buttons is a machine-dependent function. Refer to your machine tool manual.

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:

and Press and hold the machine axis direction

button, then press the machine START button: The axis continues to move after you release the keys.

2.2 Moving the Machine Axes

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 section 2.3 ”Spindle Speed S, Feed Rate F and Miscellaneous Functions M”). This function is not available on TNC 410.

17HEIDENHAIN TNC 410, TNC 426, TNC 430

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 an permissive button is depressed (machine-dependent function).

The HR 410 handwheel features the following operating elements:

EMERGENCY STOP Handwheel Permissive buttons Axis address keys Actual-position-capture key Keys for defining the feed rate (slow, medium, fast; the feed

rates are set by the machine tool builder)

2.2 Moving the Machine Axes

Direction in which the TNC moves the selected axis Machine function

(set by the machine tool builder)

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

during a program run.

To move an axis:

Select the Electronic Handwheel mode of operation

Press and hold the permissive button.

Select the axis.

Select the feed rate.

or Move the active axis in the positive or negative

direction.

2 Manual Operation and Setup

Incremental jog positioning

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

Select Manual or Electronic Handwheel mode of operation

Select incremental jog positioning: Switch the

INCREMENT soft key to ON

Jog increment:

Enter the jog increment in millimeters (here, 8

mm).

Enter the jog increment via soft key (preset softkey values). Not for TNC 426, TNC 430.

Press the machine axis direction button as often as desired.

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

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

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

19HEIDENHAIN TNC 410, TNC 426, TNC 430

Entering values

Example: Entering the spindle speed S

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

Spindle speed S =

1000 Enter the desired spindle speed,

and confirm your entry with the machine START button.

2.4 Setting the Datum

The spindle speed S with the entered rpm is started with a miscellaneous function.

Proceed in the same way to enter the feed rate F and the miscellaneous functions M.

For the feed rate F (not true for TNC 410):

■ If you enter F=0, then the lowest feed rate from MP1020 is

effective

■ F is not lost during a power interruption

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 knob for spindle speed override is effective only on machines with an infinitely variable spindle drive.

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

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

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

Preparation

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

2 Manual Operation and Setup

Datum setting

Fragile workpiece? If the workpiece surface must not be scratched, you can lay a metal shim of know thickness tool axis datum value that is larger than the desired datum by the

value

Select the Manual Operation mode.

Move the tool slowly until it touches the

workpiece surface.

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

Datum Set Z=

Zero tool in spindle axis: Set the display to a

known workpiece position (here, 0) or enter the

thickness 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.

of the shim. In the tool axis, offset

on it. Then enter a

2.5 Tilt the working plane (not TNC 410)

The functions for tilting the working plane are interfaced to the TNC and the machine tool by the machine tool builder. With specific swivel heads and tilting tables, the machine tool builder determines whether the entered angles are interpreted as coordinates of the tilt axes or as solid angles. Your machine manual provides more detailed information.

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.

10°

21HEIDENHAIN TNC 410, TNC 426, TNC 430

There are two functions available for tilting the working plane

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

mode (described below)

■ Tilting under program control: Cycle G80 WORKING PLANE in the

part program: see section ”8.9 Coordinate Transformation Cycles.”

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.

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

Machines 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

2.5 Tilt the working plane (not TNC 410)

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

Machines with swivel heads

■ 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 — 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).

2 Manual Operation and Setup

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 theManual Operation mode and the actual angle of the tilted axis was entered in the menu field.

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

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

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

Datum setting on machines with rotary tables

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 touch probe function Basic Rotation cannot

be used.

■ PLC positioning (determined by the machine tool

builder) is not possible.

■ Positioning blocks with M91/M92 are not

permitted.

The behavior of the TNC during datum setting depends on the machine.Your machine manual provides more detailed information.

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

MP 7500, bit 3=0

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

MP 7500, bit 3=1

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

2.5 Tilt the working plane (not TNC 410)

23HEIDENHAIN TNC 410, TNC 426, TNC 430

To activate manual tilting:

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

Enter the tilt angle.

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

To conclude entry, press the END soft key.

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

2.5 Tilt the working plane (not TNC 410)

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

If you set the function ”Tilt working plane” for the operating mode Program Run to Active, the tilt angle entered in the menu becomes active in the first block of the part program. If you are using Cycle G80 WORKING PLANE in the part program, the angular values defined in the cycle (starting at the cycle definition) are effective. Angular values entered in the menu will be overwritten.

2 Manual Operation and Setup

Positioning with Manual Data Input (MDI)

25HEIDENHAIN TNC 410, TNC 426, TNC 430

3.1 Program and Run Simple Machining Operations

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

Select the operating mode Positioning with MDI. Program the $MDI file as desired.

To start the selected block: Press the machine START button.

Limitations for TNC 410:

The following functions are not available:

- Tool radius compensation

- Programming and program run graphics

- Programmable probe functions

- Subprograms, program section repeats

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

- Program call with %

Limitations of the TNC 426, TNC 430:

The following functions are not available:

- Program call with %

- Program run graphics

3.1 Programming and Executing Simple Machining Operations

3 Positioning with Manual Data Input (MDI)

Example 1

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

First you pre-position the tool with G00 and G01 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 G83 PECKING.

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

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

N50 G01 Z+2 F2000 * N60 G83

P01 +2 P02 -20 P03 +10 P04 0.5

P05 250 * N70 G79 * N80 G00 G40 Z+200 M2 * N99999 %$MDI G71 *

Define tool: zero tool, radius 5 Call tool: spindle axis Z, Spindle speed 2000 rpm Retract tool (rapid traverse) Move the tool at rapid traverse to a position above the hole. Spindle on. Position tool to 5 mm above hole Define Cycle G83 PECKING: Setup clearance of the tool above the hole Total hole depth (Algebraic sign=working direction) Depth of each infeed before retraction Dwell time in seconds at the hole bottom Feed rate for pecking Call Cycle G83 Retract tool End of program

The straight-line function is described in section 6.4 ”Path Contours — Cartesian Coordinates,” the G83 PECKING cycle in section 8.3 ”Drilling Cycles.”

3.1 Programming and Executing Simple Machining Operations

27HEIDENHAIN TNC 410, TNC 426, TNC 430

Example 2

Correcting workpiece misalignment on machines with rotary tables

Use the 3-D touch probe to rotate the coordinate system. See section ”12.1 Touch Probe Cycles in the Manual and Electronic Handwheel Modes,” section ”Compensating Workpiece Misalignment.”

Write down the Rotation Angle and cancel the Basic Rotation.

Select operating mode: Positioning with MDI.

Select the axis of the rotary table, enter the

rotation angle you wrote down previously and set the feed rate. For example: G00 G40 G90 C+2.561 F50

Conclude entry.

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

3.1 Programming and Executing Simple Machining Operations

3 Positioning with Manual Data Input (MDI)

Save or delete programs from %$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).

Tag the %$MDI file

Select „Copy file“: Press the COPY soft key

Target file =

Hole

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

TNC 410: Start copying by pressing the ENT key

TNC 426, TNC 430: Press the EXECUTE soft key to start copying

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.

TNC 426, TNC 430:

The %$MDI file may not be selected in the Programming and Editing mode during the erasure procedure.

3.1 Programming and Executing Simple Machining Operations

29HEIDENHAIN TNC 410, TNC 426, TNC 430

Programming:

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

4.1 Fundamentals of NC

Position encoders and reference marks

The machine axes are equipped with position encoders that register the positions of the machine table or tool. When a machine axis moves, the corresponding position encoder generates an electrical signal. The TNC evaluates this signal and calculates the precise actual position of the machine axis.

If there is an interruption of power, the calculated position will no longer correspond to the actual position of the machine slide. The CNC can re-establish this relationship with the aid of reference marks when power is returned. The scales of the position encoders contain one or more reference marks that transmit a signal to the TNC when they are crossed over. From the signal the TNC identifies

4.1 Fundamentals of NC

that position as the machine-axis reference point and can reestablish the assignment of displayed positions to machine axis positions.

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

X (Z,Y)

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

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

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

Reference systems on milling machines

When using a milling machine, you orient tool movements to the Cartesian coordinate system. The illustration at right shows how the Cartesian coordinate system describes the machine axes. The figure at right illustrates the “right-hand rule” for remembering the three axis directions: the middle finger is pointing in the positive direction of the tool axis from the workpiece toward the tool (the Z axis), the thumb is pointing in the positive X direction, and the index finger in the positive Y direction.

The TNC 410 can control a maximum of 4 axes, the TNC 426 a maximum of 5 axes and the TNC 430 a maximum of 9 axes. The axes U, V and W are secondary linear axes parallel to the main axes X, Y and Z, respectively. Rotary axes are designated as A, B and C. The illustration at lower right shows the assignment of secondary axes and rotary axes to the main axes.

4.1 Fundamentals of NC

V+

W+

C+

B+

A+

U+

33HEIDENHAIN TNC 410, TNC 426, TNC 430

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 twodimensional and describe points in a plane. Polar coordinates have their datum at the so-called pole. A position in a plane can be clearly defined by the

■ Polar radius R: the distance from the pole to the position, and the

■ Polar angle H, the size of the angle between the reference axis

and the line that connects the pole with the position.

4.1 Fundamentals of NC

See figure at lower right.

Definition of pole and angle reference axis

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

0°

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

I and J +X J and K +Y K and I +Z

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Absolute and relative workpiece positions

Absolute workpiece positions

Absolute coordinates are position coordinates that are referenced to the datum of the coordinate system (origin). Each position on the workpiece is uniquely defined by its absolute coordinates.

Example 1: Holes dimensioned in absolute coordinates

Hole X=10 mm X=30 mm X=50 mm

Y=10 mm Y=20 mm Y=30 mm

Hole Hole

Relative workpiece positions

Relative coordinates are referenced to the last programmed nominal position of the tool, which serves as the relative (imaginary) datum. When you write a part program in incremental coordinates, you thus program the tool to move by the distance between the previous and the subsequent nominal positions. Incremental coordinates are therefore also referred to as chain dimensions.

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

Example 2: Holes dimensioned with relative coordinates

Absolute coordinates of hole

X= 10 mm Y= 10 mm

referenced to hole Hole referenced to hole

Hole G91 X= 20 mm G91 X= 20 mm

G91 Y= 10 mm G91 Y= 10 mm

Absolute and incremental polar coordinates

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

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

10 10

3010

4.1 Fundamentals of NC

G91+R

G91+H

0°

35HEIDENHAIN TNC 410, TNC 426, TNC 430

Selecting 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. For further information, refer to section 8.9 ”Coordinate Transformation Cycles.”

If the production drawing is not dimensioned for NC, set the datum

4.1 Fundamentals of NC

at a position or corner on the workpiece, which is the most 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. For further information, refer to section 12.2 “Setting the Datum with a 3-D Touch Probe.”

Example

The workpiece drawing at right illustrates the holes are dimensioned to an absolute datum with the coordinates X=0 Y=0. The holes absolute coordinates X=450 Y=750. By using the DATUM SHIFT cycle you can shift the datum temporarily to the position X=450, Y=750 and program the holes calculations.

to are referenced to a relative datum with the

to without any further

to , which

750

320

150

-150

0,1

300

325

450 900

950

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

4.2 File Management: Fundamentals

Files

When you write a part program on the TNC, you must first enter a file name. The TNC then stores the program as a file with the same name. You can also store text and tables as files.

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

In the TNC 410 you can manage a max. 64 files with a total of up to 128 KB.

The TNC 426, TNC 430 can manage any number of files. However, their total size must not exceed 1.5 gigabytes.

File names

The name of a file can have up to 16 characters (TNC 410: 8 characters). When you store programs, tables and texts as files, the TNC adds an extension to the file name, separated by a point. This extension identifies the file type (see table at right).

PROG20 .H

File name File type

Data backup TNC 426, TNC 430

We recommend saving newly written programs and files on a PC at regular intervals. You can do this with the cost-free backup program TNCBACK.EXE from HEIDENHAIN. Your machine tool builder can provide you with a copy of TNCBACK.EXE.

You also need a floppy disk on which all the machine-specific data (PLC program, machine parameters, etc.) of your machine tool are stored. Please contact your machine tool builder for more information on both the backup program and the floppy disk.

Files in the TNC Type

Programs

in HEIDENHAIN conversational format .H in ISO format .I

Tables for

Tools .T Tool changer (TNC 410: 1 table) .TCH Datums .D Points .PNT Pallets (not TNC 410) .P

Text as ASCII files (not TNC 410) .A

4.2 File Management: Fundamentals

Saving the contents of the entire hard disk (up to 1.5 GB) can take up to several hours. In this case, it is a good idea to save the data outside of working hours, (e.g. overnight), or to use the PARALLEL EXECUTE function to copy in the background while you work.

37HEIDENHAIN TNC 410, TNC 426, TNC 430

4.3 Standard file management TNC 426, TNC 430

Use the standard file manager if you want to store all of the files in one directory, or if you are used to working with the file manager on old TNC controls.

Set the MOD function PGM MGT to Standard (see section 13.9) .

Calling the file manager

Press the PGM MGT: The TNC displays the file management window (see Fig. at top right)

The window shows you all of the files that are stored in the TNC. Each file is shown with additional information, see table at center right.

Display Meaning

FILE NAME Name with max. 16 characters

and file type

BYTE File size in bytes

Selecting a file

Calling the file manager

4.3 Standard File Management TNC 426, TNC 430

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

Move the highlight up or down.

or Select a file: Press the SELECT soft key

or ENT

STATUS Property of the file:

E Program is in the

Programming and Editing mode of operation

S Program is in the

Program is selected in the Test RUN mode of operation

M Program is in the

Program Run mode of operation.

P File is protected against

editing and erasure (Protected)

Display of long file directories Soft key

Move pagewise up through the file directory.

Move pagewise down through the file directory

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Deleting a file

Calling the file manager

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

Move the highlight up or down.

Delete a file: Press the DELETE soft key

Delete ........ file ?

Press the YES soft key to confirm, or

the NO soft key to abort.

Copying a file

Calling the file manager

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

Move the highlight up or down.

Copy a file: Press the COPY soft key

Target file =

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

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

4.3 Standard File Management TNC 426, TNC 430

39HEIDENHAIN TNC 410, TNC 426, TNC 430

Data transfer to or from an external data medium

Before you can transfer data to an external data medium, you must set the interface (see section 13.6 ”Setting the Data Interfaces for TNC 426, TNC 430”).

Calling the file manager

Activate data transfer: press the EXT soft key. In the left half of the screen, the TNC shows all of

files that are stored on the TNC, and in the

the right half of the screen, stored on the external data medium.

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

Move the highlight up and down within a

window

Move the highlight from the left to the right

window, and vice versa.

all of the files that are

If you are transferring from the TNC to the external medium, move the highlight in the left window onto the file that is to be transferred.

4.3 Standard File Management TNC 426, TNC 430

If you are transferring from the external medium to the TNC, move the highlight in the right window onto the file that is to be transferred.

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

Transfer several files: Press TAG (marking functions, see table on right), or

transfer all files by pressing the TNC EXT soft key

Tagging functions Soft key

Tag a single file

Tag all files

Untag a single file

Untag all files

Copy all tagged files

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

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

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

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

Selecting one of the last 10 files selected

Calling the file manager

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

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

Move the highlight up or down.

or Select a file: Press the SELECT soft key

or ENT

4.3 Standard File Management TNC 426, TNC 430

41HEIDENHAIN TNC 410, TNC 426, TNC 430

Renaming a file

Calling the file manager

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

Move the highlight up or down.

To rename the file, press the RENAME key.

Target file =

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

Protect file / Cancel file protection

Calling the file manager

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

4.3 Standard File Management TNC 426, TNC 430

Move the highlight up or down.

Press the PROTECT soft key to enable file protection The file now has status P, or

To cancel file protection, press the UNPROTECT soft key. The P status is canceled.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

4.4 Expanded File Management TNC 426, TNC 430

Select the file manager with additional functions if you wish to store files in various different directories.

Set the MOD function PGM MGT (see section 13.9) to Enhanced!

See also section 4.2 ”File Management: Fundamentals”!

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 up into further directories, which are called subdirectories.

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

no longer sorts them alphabetically!

Directory names

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

Paths

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

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

TNC:\AUFTR1\NCPROG\PROG1.I The chart at right illustrates an example of a directory display with

different paths.

TNC:\

AUFTR1

NCPROG WZTAB

A35K941

ZYLM TESTPROG

HUBER

4.4 Expanded File Management TNC 426, TNC 430

KAR25T

43HEIDENHAIN TNC 410, TNC 426, TNC 430

Overview: Functions of the expanded file manager

Function Soft key

Copy (and convert) individual files

Display a specific file type

Display the last 10 files that were selected

Erase a file or directory

Tag a file

Renaming a file

Protect a file against editing and erasure

Cancel file protection

Network drive management (Ethernet option only)

Copying a directory

Display all the directories of a particular drive

4.4 Expanded File Management TNC 426, TNC 430

Delete directory with all its subdirectories

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Calling the file manager

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

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

In the lower part of the narrow window the TNC shows all directories file symbol to the left and the directory name to the right. The TNC displays a subdirectory to the right of and below its parent directory. The selected (active) directory is depicted in a different color.

The wide window at on the right side shows all the files stored in the selected directory. Each file is shown with additional information that is illustrated in the table on the next page.

of the selected drive. A drive is always identified by a

that are

Display Meaning

FILE NAME Name with max. 16 characters

and file type

BYTE File size in bytes

STATUS Property of the file:

E Program is in the

Programming and Editing mode of operation

4.4 Expanded File Management TNC 426, TNC 430

S Program is in the

Program is selected in the Test RUN mode of operation

M Program is in the

Program Run mode of operation.

P File is protected against

editing and erasure (Protected)

DATE Date the file

was last changed

TIME Time the file

was last changed

45HEIDENHAIN TNC 410, TNC 426, TNC 430

To select drives, directories and files:

Calling the file manager

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

Move the highlight from the left to the right

window, and vice versa.

Move the highlight up and down within a

window

Move the highlight one page up or

down within a window

1st step: select drive:

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

or Select drive: Press the SELECT soft key

or ENT

4.4 Expanded File Management TNC 426, TNC 430

2nd step: select directory:

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

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

3rd step: select a file:

Press the SELECT TYPE soft key

Press the soft key for the desired file type, or

Press the SHOW ALL soft key to display all files

Move the highlight to the desired file in the right window

or The selected file is opened in the

operating mode from which you have the called file manager: Press ENT or the SELECT soft key.

To create a new directory (only possible on the TNC's hard disk drive):

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

NEW

Create \NEW directory ?

Enter the new file name, and confirm with ENT.

Press the YES soft key to confirm, or

the NO soft key to abort.

4.4 Expanded File Management TNC 426, TNC 430

47HEIDENHAIN TNC 410, TNC 426, TNC 430

Copying a file

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

ú Press the COPY soft key to select the copying

function.

ú Enter the name of the destination file and confirm your entry with

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

Copying a table

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

■ The target table must exist.

■ The file to be copied must only contain the columns or lines you

want to replace.

Example:

With a tool presetter you have measured the length and radius of 10 new tools. The tool presetter then generates the tool table TOOL.T with 10 lines (for the 10 tools) and the columns

■ Tool number

■ Tool length

4.4 Expanded File Management TNC 426, TNC 430

■ Tool radius

If you wish to copy this file to the TNC, the TNC asks if you wish to overwrite the existing TOOL.T tool table:

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

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

■ If you press the REPLACE FIELDS soft key, the TNC merely

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

Copying a directory

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

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Selecting one of the last 10 files selected

Calling the file manager

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

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

Move the highlight up or down.

or Select a file: Press the SELECT soft key

or ENT

Deleting a file

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

ú To select the erasing function, press the DELETE soft

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

ú To confirm, press the YES soft key;

To abort erasure, press the NO soft key.

4.4 Expanded File Management TNC 426, TNC 430

Erase a directory

ú Erase all files and subdirectories stored in the directory that you

wish to erase.

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

ú To select the erasing function, press the DELETE soft

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

ú To confirm, press the YES soft key;

To abort erasure, press the NO soft key.

49HEIDENHAIN TNC 410, TNC 426, TNC 430

Tagging files

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

Move the highlight to the first file.

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

Tagging functions Soft key

Tagging single files

Tag all files in the directory

Untag a single file

Untag all files

Tag a file by pressing the TAG FILE soft key.

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

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

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

Delete the tagged files by

4.4 Expanded File Management TNC 426, TNC 430

pressing END to end the marking function, and then DELETE to delete the tagged files.

Renaming a file

ú Move the highlight to the file you wish to rename.

ú Select the renaming function. ú Enter the new file name; the file type cannot be

changed.

ú To execute renaming, press the ENT key.

Copy all tagged files

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Additional Functions

Protecting a file/Canceling file protection

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

ú To select the additional functions, press the MORE

FUNCTIONS key.

ú To enable file protection, press the PROTECT soft key.

The file now has status P.

To cancel file protection, proceed in the same way using the UNPROTECT soft key.

Erase a directory together with all its subdirectories and files.

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

to erase.

ú To select the additional functions, press the MORE

FUNCTIONS key.

ú Press DELETE ALL to erase the directory together

with its subdirectories.

ú To confirm, press the YES soft key;

To abort erasure, press the NO soft key.

4.4 Expanded File Management TNC 426, TNC 430

51HEIDENHAIN TNC 410, TNC 426, TNC 430

Data transfer to or from an external data medium

Before you can transfer data to an external data medium, you must set the interface (see section 13.6 ”Setting the Data Interfaces for TNC 426, TNC 430”).

Calling the file manager

Select the screen layout for data transfer: press the WINDOW soft key. In the left half of the screen, the TNC shows all of the stored on the TNC, and in the right half of the screen, external data medium.

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

Move the highlight up and down within a

window

Move the highlight from the left to the right

window, and vice versa.

all of the files that are stored on the

files that are

If you are transferring from the TNC to the external medium, move the highlight in the left window onto the file that is to be transferred.

4.4 Expanded File Management TNC 426, TNC 430

If you are transferring from the external medium to the TNC, move the highlight in the right window onto the file that is to be transferred.

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

To transfer several files, use the TAG soft key (in the second soft-key row, see also Tagging functions earlier on in this chapter), or

transfer all files by pressing the TNC EXT soft key

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

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

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

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

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

4.4 Expanded File Management TNC 426, TNC 430

53HEIDENHAIN TNC 410, TNC 426, TNC 430

Copying files into another directory

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

In the right window:

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

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

In the left window:

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

ENT to display them.

ú Display the file tagging functions.

ú Move the highlight to the file you want to copy and

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

ú Copy the tagged files into the target directory.

For additional tagging functions see „Tagging files“. If you have marked files in the left and right windows, the TNC

copies from the directory in which the highlight is located.

Overwriting files

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

ú Press the YES soft key to overwrite all files, or ú Press the NO soft key if no file is to be overwritten

4.4 Expanded File Management TNC 426, TNC 430

ú To confirm each file separately before overwriting it, press the

CONFIRM key.

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

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

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

To connect the Ethernet card to your network, refer to Chapter ”13.8 Ethernet Interface”!

The TNC logs error messages during network operation (see section ”13.8 Ethernet Interface”).

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

Connecting and disconnecting network drives

Function Soft key

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

(see screen at upper right). All the functions

ú To select the program management: Press the PGM

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

ú To manage the network drives: Press the ”Network”

soft key. In the right-hand window the network drives available for access. With the following soft keys you can define the connection for each drive.

the TNC shows

Printing the file with a network printer

If you have defined a network printer (see section ”13.8 Ethernet Interface”), you can print the files directly:

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

one printer, the TNC will print the file immediately.

Delete network connection

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

Do not network connection automatically when the TNC is switched on

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

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

4.4 Expanded File Management TNC 426, TNC 430

55HEIDENHAIN TNC 410, TNC 426, TNC 430

4.5 File Management for the TNC 410

Files in the TNC 410 Type

Programs

in HEIDENHAIN conversational format .H in ISO format .I

Tables for Tools .T Tool pockets .TCH Datums .D Points .PNT

This section informs you about the meaning of the individual screen information, and describes how to select files and directories. If you are not yet familiar with the TNC file manager, we recommend that you read this section completely and test the individual functions on your TNC.

Calling the file manager

4.5 File Management for the TNC 410

Press the PGM MGT key: the TNC displays the file management window

Display Meaning

File name Name with up to 8 characters

and file type Properties of the file:

M Program is in the

Program Run mode of operation.

P File is protected against

editing and erasure (Protected)

The window shows you all of the files that are stored in the TNC. Each file is shown with additional information that is illustrated in the table on the next page.

Display of long file directories Soft key

Move pagewise up through the file directory.

Move pagewise down through the file directory

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Selecting a file

Calling the file manager

Use the arrow keys to move the highlight to the desired file:

Move the highlight up or down.

Deleting a file

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

ú To select the erasing function, press

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

ú To confirm erasure press the YES soft

key. Abort with the NO soft key if you do not wish to erase the file.

Enter the first or more letters of the file you wish to select and then press the GOTO key: The highlight moves to the first file that matches these letters.

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

Copying a file

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

ú Press the COPY soft key to select the copying

function.

ú Enter the name of the destination file and confirm your entry with

the ENT key: The TNC copies the file. The original file is retained.

Renaming a file

ú Move the highlight to the file you wish to rename.

ú Select the renaming function. ú Enter the new file name; the file type cannot be

changed.

ú To execute renaming, press the ENT key.

Protecting a file/Canceling file protection

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

ú To enable file protection, press the

PROTECT/UNPROTECT soft key. The file now has status P.

To cancel file protection, proceed in the same way using the PROTECT/UNPROTECT soft key. You also need to enter the code number 86357.

4.5 File Management for the TNC 410

57HEIDENHAIN TNC 410, TNC 426, TNC 430

Read in/read out files

ú To read in or read out files: Press the ENT soft key. The

TNC provides the functions described below.

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

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

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

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

data medium.

Read in offered file

ú List all files of a certain file type.

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

ú Output all files stored in the TNC to an

external device.

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

ú Display a list of files stored in the

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

4.5 File Management for the TNC 410

ú For example: list all HEIDENHAIN conversational

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

Read in a specific file

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

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

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

Read out a specific file

ú Select the function for reading out a single file.

úMove the highlight to the file that you wish to read

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

ú To terminate the function for reading out specific files:

press the END key.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

4.6 Creating and Writing Programs

Organization of an NC program in ISO format.

A part program consists of a series of program blocks. The figure at right illustrates the elements of a block.

The TNC automatically numbers the program blocks in ascending sequence, if you have set a block number increment in MP7220 (see „14.1 General User Parameters“)

The first block of a program is identified by “%” the program name and the active unit of measure G70/G71.

The subsequent blocks contain information on:

■ The blank form:

■ Tool definitions and tool calls,

■ Feed rates and spindle speeds as well as

■ Path contours, cycles and other functions

The last block of a program begins with N999 999 and is identified with ”%”, the program name and the active unit of measure.

Define blank form: G30/G31

Immediately after initiating a new program, you define a cuboid workpiece blank. This definition is needed for the TNC’s graphic simulation feature. The sides of the workpiece blank may be max. 100 000 mm long (TNC 410: 30 000 mm) and lie parallel to the axes X, Y and Z. The ratio of the side lengths must be less than 200:1. The blank form is defined by two of its corner points:

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

form, entered as absolute values.

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

form, entered as absolute or incremental values.

Block:

N100 G00 G40 X+10 Y+5 M3

Path function Words

Block number

MAX

4.6 Creating and Writing Programs

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

MIN

59HEIDENHAIN TNC 410, TNC 426, TNC 430

Opening a new part program TNC 426, TNC 430

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

Open new program for the TNC 410

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

Program initiation in an example:

Select the Programming and Editing mode of operation.

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

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

File name = OLD.I

NEW

4.6 Creating and Writing Programs

Enter the new program name and confirm your

entry with the ENT key.

To select the unit of measure, press the MM or INCH soft key. The TNC changes to the program window

Program initiation in an example:

Select the Programming and Editing mode of operation.

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

File name =

NEW Entering new program names

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

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

Confirm your entry with the ENT key.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Define the workpiece blank

30 Define MIN point

17 Define spindle axis (here Z)

0 Enter in sequence the X, Y and Z coordinates

of the MIN point.

-40

To terminate the block, press the END key.

31 Define MAX point

90 Define absolute/incremental input

4.6 Creating and Writing Programs

100 Enter in sequence the X, Y and Z coordinates of

the MAX point.

100

To terminate the block, press the END key.

The program blocks window shows the following BLK FORM definition

%NEW G71 * N10 G30 G17 X+0 Y+0 Z-40 * N20 G31 G90 X+100 Y+100 Z+0 * N999999 %NEW G71 *

The TNC automatically generates the first and last blocks of the program.

Program begin, name, unit of measure Tool axis, MIN point coordinates MAX point coordinates Program end, name, unit of measure

61HEIDENHAIN TNC 410, TNC 426, TNC 430

Program tool movements

To program a block, select an ISO function key on the alphabetic keyboard. With the TNC 410 you can also use the gray path function keys to get the corresponding G code.

Example of a positioning block

1 Start block

40 Enter „No radius compensation“

10 Enter the target coordinate for the X axis.

5 Enter the target coordinate for the Y axis.

4.6 Creating and Writing Programs

100 Enter a feed rate of 100 mm/min for this path

contour.

3 Enter the miscellaneous function M3 “spindle

ON”; pressing the END key will terminate the block.

The program blocks window will display the following line:

N30 G01 G40 X+10 Y+5 F100 M3 *

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Editing a program with TNC 426, TNC 430

While you are creating or editing a part program, you can select any desired line in the program or individual words in a block with the arrow keys or the soft keys (see table at right).

Inserting blocks at any desired location

ú Select the block after which you want to insert a new block and

initiate the dialog.

Selecting blocks or words Soft keys/keys

Move from one block to the next

Select individual words in a block

Editing and inserting words

ú Select a word in a block and overwrite it with the new one. The

plain-language dialog is available while the word is highlighted.

ú To accept the change, press the END key.

If you want to insert a word, press the horizontal arrow key repeatedly until the desired dialog appears. You can then enter the desired value.

Looking for the same words in different blocks

To select a word in a block, press the arrow keys repeatedly until the highlight is on the desired word.

Select a block with the arrow keys.

The word that is highlighted in the new block is the same as the one you selected previously.

Erasing blocks and words Key

Set the selected word to zero

Erase an incorrect number

Clear a (non-blinking) error message

Delete the selected word

Delete the selected block

Erase cycles and program sections: First select the last block of the cycle or program section to be erased, then erase with the DEL key.

4.6 Creating and Writing Programs

63HEIDENHAIN TNC 410, TNC 426, TNC 430

Marking, copying, deleting and inserting program sections

The TNC provides certain functions (listed in table at right) for copying program sections within an NC program or into another NC program.

To copy a program section, proceed as follows:

ú Select the soft-key row using the marking function. ú Select the first (last) block of the section you wish to copy. ú To mark the first (last) block: Press the SELECT BLOCK soft key.

The TNC then highlights the first character of the block and superimposes the soft key CANCEL SELECTION.

ú Move the highlight to the last (first) block of the program section

you wish to copy or delete. The TNC shows the marked blocks in a different color. You can end the marking function at any time by pressing the CANCEL SELECTION soft key.

ú To copy the selected program section: Press the COPY BLOCK

soft key, and to delete the selected section: Press the DELETE BLOCK soft key. The TNC stores the selected block.

ú Using the arrow keys, select the block after which you wish to

insert the copied (deleted) program section.

4.6 Creating and Writing Programs

To insert the section into another program, select the corresponding program using the File Manager and then mark the block after which you wish to insert the copied block.

Function Soft key

Switch on marking function

Switch off marking function

Delete marked block

Insert block that is stored in the buffer memory

Copy marked block

ú To insert the block: Press the INSERT BLOCK soft key

Regenerating the block number increment

If you have deleted, moved or added program sections, you can have the TNC renumber the blocks through the ORDER N function.

ú To regenerate the block numbering: Press the ORDER N soft key.

The TNC displays the conversational prompt ”Block nr. increment =.”

ú Enter the desired block number increment. The value defined in

MP7220 is overwritten.

ú To number the blocks: Press the ENT key. ú To cancel the change: Press the END key or the END soft key.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Editing a program with the TNC 410

While you are creating or editing a part program, you can select any desired line in the program or individual words in a block with the arrow keys (see table at right). While you are entering a new block the TNC identifies the block with a * as long as the block has not been saved.

Function Soft keys/keys

Go to the previous page

Go to the next page

Inserting blocks at any desired location

ú Select the block after which you want to insert a new block and

initiate the dialog.

Editing and inserting words

ú Select a word in a block and overwrite it with the new one. The

plain-language dialog is available while the word is highlighted.

ú To save your changes, press the END key. ú To reject the change, press the DEL key.

If you want to insert a word, press the horizontal arrow key repeatedly until the desired dialog appears. You can then enter the desired value.

Looking for the same words in different blocks

To select a word in a block, press the arrow keys repeatedly until the highlight is on the desired word.

Select a block with the arrow keys.

The word that is highlighted in the new block is the same as the one you selected previously.

Go to beginning of program

Go to end of program

Move from one block to the next

Select individual words in a block

Search for a sequence of characters

Erasing blocks and words Key

Set the selected word to zero

Erase an incorrect number

Clear a (non-blinking) error message

Delete the selected word

In a block: Restore previously saved version

4.6 Creating and Writing Programs

Finding any text

ú To select the search function, press the FIND soft key.

The TNC displays the dialog prompt FIND TEXT:

ú Enter the text that you wish to find. ú To find the text, press the EXECUTE soft key.

Inserting the previously edited (deleted) block at any location

ú Select the block after which you want to insert the block you have

just edited (deleted) and press the INSERT NC BLOCK soft key.

Block display

If a block is so long that the TNC cannot display it in one line (for example in a fixed cycle), this will be indicated with ”>>” at the right edge of the screen.

Delete the selected block (cycle)

Delete the program sections: First select the last block of the program section to be erased, then erase with the DEL key.

65HEIDENHAIN TNC 410, TNC 426, TNC 430

4.7 Programming Graphics (not TNC 426, TNC 430)

While you are writing the part program, you can have the TNC generate a graphic illustration of the programmed contour.

To generate/not generate graphics during programming:

ú To switch the screen layout to displaying program blocks to the

left and graphics to the right, press the SPLIT SCREEN key and PGM + GRAPHICS soft key.

ú Set the AUTO DRAW soft key to ON. While you are

entering the program lines, the TNC generates each path contour you program in the graphics window in the right screen half.

If you do not wish to have graphics generated during programming, set the AUTO DRAW soft key to OFF.

Even when AUTO DRAW is switched ON, graphics are not generated for program section repeats.

Generating a graphic for an existing program

ú Use the arrow keys to select the block up to which you want the

graphic to be generated, or press GOTO and enter the desired block number.

ú To generate graphics, press the RESET + START soft

key.

Additional functions are listed in the table at right.

To erase the graphic:

4.7 Programming Graphics (not TNC 426 B, TNC 430)

ú Shift the soft-key row (see figure at right) ú Delete graphic: Press CLEAR GRAPHIC soft key

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Magnifying or reducing a detail

You can select the graphics display by selecting a detail with the frame overlay. You can now magnify or reduce the selected detail.

ú Select the soft-key row for detail magnification/reduction

(second row, see figure at right) The following functions are available:

Function Soft key

Reduce the frame overlay — press and hold the soft key to reduce the detail

Enlarge the frame overlay — press and hold the soft key to magnify the detail

ú With the WINDOW DETAIL soft key, Confirm the

selected area.

With the WINDOW BLK FORM soft key, you can restore the original section.

Functions Soft key

Generate interactive graphic blockwise

Generate a complete graphic or complete it after RESET + START

Interrupt interactive graphics This soft key only appears while the TNC generates the interactive graphics

4.7 Programming Graphics (not TNC 426 B, TNC 430)

67HEIDENHAIN TNC 410, TNC 426, TNC 430

4.8 Adding Comments

You can add comments to any desired block in the part program to explain program steps or make general notes. There are three possibilities to add comments:

1. Adding comments during program input (not

TNC 410)

ú Enter the data for a program block, then press the

semicolon key “;” on the alphabetic keyboard — the TNC displays the dialog prompt COMMENT ?

ú Enter your comment and conclude the block by

4.8 Adding Comments

pressing the END key.

2. Adding comments after program input

(not TNC 410)

ú Select the block to which a comment is to be

added.

ú Move to the required block using the arrow keys,

then press the semicolon key on the alphabetic keyboard _ the TNC displays the dialog prompt COMMENT ?

ú Enter your comment and conclude the block by

pressing the END key.

3. To enter a comment in a separate block:

ú Select the block after which the comment is to be

inserted.

ú Initiate the programming dialog with the

semicolon key “;” on the alphabetic keyboard.

ú Enter your comment and conclude the block by

pressing the END key.

4 Programmieren: Grundlagen, Datei-Verwaltung,

Programmierhilfen, Paletten-Verwaltung

4.9 Creating Text Files (not TNC 410)

You can use the TNC’s text editor to write and edit texts. Typical applications:

■ Recording test results

■ Documenting working procedures

■ Creating formularies

Text files are type .A files (ASCII files). If you want to edit other types of files, you must first convert them into type .A files.

Opening and exiting text files

ú Select the Programming and Editing mode of operation. ú To call the file manager, press the PGM MGT key. ú To display type .A files, press the SELECT TYPE and then the

SHOW .A soft keys.

ú Select a file and open it with the SELECT soft key or ENT key,

or create a new file by entering the new file name and confirming your entry with the ENT key.

To leave the text editor, call the file manager and select a file of a different file type, for example a part program.

Cursor movements Soft key

Move one word to the right

Move one word to the left

4.9 Creating Text Files (not TNC 410)

Editing texts

The first line of the text editor is an information headline which displays the file name, and the location and writing mode of the cursor:

File: Name of the text file Line: Line in which the cursor is presently located Column: Column in which the cursor is presently located Insert: Insert new text, pushing the existing text to the

right

Overwrite: Write over the existing text, erasing it where it is

replaced with the new text.

The text is inserted or overwritten at the location of the cursor. You can move the cursor to any desired position in the text file by pressing the arrow keys.

The line in which the cursor is presently located is depicted in a different color. A line can have up to 77 characters. To start a new line, press the RET key or the ENT key.

Go to the next screen page

Go to the previous screen page

Go to beginning of file

Go to end of file

Editing functions Key

Begin a new line

Erase the character to the left of the cursor

Insert a blank space

Switch between upper and lower + case letters

69HEIDENHAIN TNC 410, TNC 426, TNC 430

Erasing and inserting characters, words and lines

With the text editor, you can erase words and even lines, and insert them at any desired location in the text. See the table at right.

Delete functions Soft key

Delete and temporarily store a line

To move a word or line to a different location:

ú Move the cursor to the word or line you wish to erase and insert

at a different place in the text.

ú Press the DELETE WORD or DELETE LINE soft key: the text is put

in the buffer memory

ú Move the cursor to the location where you wish insert the text,

and press the RESTORE LINE/WORD soft key.

Editing text blocks

You can copy and erase text blocks of any size, and insert them at other locations. Before carrying out any of these editing functions, you must first select the desired text block:

ú To select a text block, move the cursor to the first character of the

text you wish to select.

ú Press the SELECT BLOCK soft key.

4.9 Creating Text Files (not TNC 410)

After selecting the desired text block, you can edit the text with the following soft keys:

Function Soft key

ú Move the cursor to the last character of the text you

wish to select. You can select whole lines by moving the cursor up or down directly with the arrow keys — the selected text is shown in a different color.

Delete and temporarily store a word

Delete and temporarily store a character

Insert a line or word from temporary storage

Delete the selected text and store temporarily

Store marked block temporarily without erasing (copy )

If necessary, you can now insert the temporarily stored block at a different location

ú Move the cursor to the location where you want to insert the

temporarily stored text block.

ú Press the INSERT BLOCK soft key _ the text block in

inserted.

You can insert the temporarily stored text block as often as desired.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

To transfer the selected text to a different file:

ú Select the text block as described previously.

ú Press the APPEND TO FILE soft key — the TNC

displays the dialog prompt Destination file =

ú Enter the path and name of the target file. The TNC

appends the selected text to the end of the specified file. If no target file with the specified name is found, the TNC creates a new file with the selected text.

To insert another file at the cursor position:

ú Move the cursor to the location in the text where you wish to

insert another file.

ú Press the READ FILE soft key.

The TNC displays the dialog prompt File name =

ú Enter the path and name of the file you want to insert.

Finding text sections

With the text editor, you can search for words or character strings in a text. Two functions are available:

1. Finding the current text

The search function is to find the next occurrence of the word in which the cursor is presently located:

ú Move the cursor to the desired word. ú To select the search function, press the FIND soft key. ú Press the FIND CURRENT WORD soft key

2. Finding any text

ú To select the search function, press the FIND soft key.

The TNC displays the dialog prompt Find text:

ú Enter the text that you wish to find. ú To find the text, press the EXECUTE soft key.

To leave the search function, press the END soft key.

4.9 Creating Text Files (not TNC 410)

71HEIDENHAIN TNC 410, TNC 426, TNC 430

4.10 The Pocket Calculator (not TNC 410)

The TNC features an integrated pocket calculator with the basic mathematical functions.

With the CALC key you can open and close an additional window for calculations. You can move the window to any desired location on the TNC screen with the arrow keys.

The calculator is operated with short commands through the alphabetic keyboard. The commands are shown in a special color in the calculator window:

Mathematical function Command

Addition + Subtraction – Multiplication * Division : Sine S Cosine C Tangent T Arc sine AS Arc cosine AC Arc tangent AT Powers ^

4.10 The Pocket Calculator (not TNC 410)

Square root Q Inversion / Parenthetic calculations ( ) p (3.14159265359) P Display result =

ARC SIN COS TAN

+–∗ :

X^YSQR1/X PI

( ) CE =

789 456 123

–

If you are writing a program and the programming dialog is active, you can use the actual-position-capture key to transfer the result to the highlight position in the current block.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

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

The TNC automatically generates error messages when it detects problems such as

■ Incorrect data input

■ Logical errors in the program

■ Contour elements that are impossible to machine

■ Incorrect use of the touch probe system

An error message that contains a program block number was caused by an error in the indicated block or in the preceding block. The TNC error messages can be canceled with the CE key, after the cause of the error has been removed.

If you require more information on a particular error message, press the HELP key. A window is then superimposed where the cause of the error is explained and suggestions are made for correcting the error.

Display HELP

if an error message appears at the top of screen:

ú To display Help, press the HELP key ú Read the description of the error and the possibilities

for correcting it. Close the Help window with the CE, thus canceling the error message

ú Remove the cause of the error as described in the

Help window.

The TNC displays the Help text automatically if the error message is flashing. The TNC needs to be restarted after flashing error messages. Press the END key and hold for two seconds.

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

73HEIDENHAIN TNC 410, TNC 426, TNC 430

4.12 Help Function (not TNC 426, TNC 430)

The help function of the TNC includes a description of all of the ISO functions. You can select a HELP topic using the soft keys.

Select the HELP function

ú Press the HELP key ú Select a topic: Press one of the available soft keys

Help topics / Functions Soft key

ISO programming: G functions

ISO programming: D functions

ISO programming: M functions

ISO programming: Address letters

Cycle parameters

HELP that is entered by the machine manufacturers (optional, not executable)

4.12 HELP Function (not TNC 426, TNC 430)

Go to next page

Go to previous page

Go to beginning of file

Go to end of file

Select search functions; Enter text, Begin search with ENT key

End the HELP function

Press the END key twice.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

4.13 Pallet Management (not TNC 410)

Pallet table management is a machine-dependent function. The standard functional range will be described in the following. Refer to your machine manual for more information.

Pallet tables are used for machining centers with pallet changer: The pallet table calls the part programs that are required for the different pallets, and activates datum shifts or datum tables.

You can also use pallet tables to run in succession several programs that have different datums.

Pallet tables contain the following information:

■ PAL/PGM (entry obligatory): Identification for pallet or NC program

(select with ENT or NO ENT)

■ NAME (entry obligatory): Pallet or program name. The machine

tool builder determines the pallet name (see Machine Manual). The program name must be stored in the same directory as the pallet table. Otherwise you must enter the full path name for the program.

■ DATUM (entry optional): Name of the datum table. The datum

table must be stored in the same directory as the pallet table. Otherwise you must enter the full path name for the datum table. Datums from the datum table can be activated in the NC program with Cycle 7 DATUM SHIFT

■ X, Y, Z (entry optional; other axes also possible): For pallet names,

the programmed coordinates are referenced to the machine datum. For NC programs, the programmed coordinates are referenced to the pallet datum. These entries overwrite the datum that you last set in the Manual mode of operation. With the miscellaneous function M104 you can reactivate the datum that was last set. With the ”actual-position-capture” key, the TNC opens a window that enables you to have the TNC enter various points as datums (see next page):

Function Soft key

Select beginning of table

Select end of table

4.13 Pallet Management (not TNC 410)

Select previous page in table

Select next page in table

Insert the last line in the table

Delete the last line in the table

Go to the beginning of the next line

Add the entered number of lines to the end of the table

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

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

75HEIDENHAIN TNC 410, TNC 426, TNC 430

Position Meaning

Actual values Enter the coordinates of the current tool

position relative to the active coordinate system.

Reference values Enter the coordinates of the current tool

position relative to the machine datum.

ACTL measured values Enter the coordinates relative to the active

coordinate system of the datum last probed in the Manual operating mode.

REF measured values Enter the coordinates relative to the

machine datum of the datum last probed in the Manual operating mode.

With the arrow keys and ENT, select the position that you wish to confirm. Then press the ALL VALUES soft key so that the TNC saves the respective coordinates of all active axes in the pallet table. With the PRESENT VALUE soft key, the TNC saves the coordinates of the axis on which the highlight in the pallet table is presently located.

If you have not defined a pallet before an NC program, the programmed coordinates are then referenced to the machine datum.

4.13 Pallet Management (not TNC 410)

To select a pallet table:

ú Call the file manager in the operating mode Programming and

Editing: Press the PGM MGT key.

ú Display all .P files: Press the soft keys SELECT TYPE and

SHOW .P.

ú Select a pallet table with the arrow keys, or enter a new file name

to create a new table.

ú Confirm your entry with the ENT key.

To execute the pallet file

In machine parameter 7683, set whether the pallet table is to be executed blockwise or continuously (see „14.1 General User Parameters“).

ú Select the file manager in the operating mode

Program Run, Full Sequence or Program Run, Single Block: Press the PGM MGT key.

ú Display all .P files: Press the soft keys SELECT

TYPE and SHOW .P.

ú Select pallet table with the arrow keys and

confirm with ENT.

ú Execute pallet table: Press the NC Start button.

The TNC executes the pallets as set in Machine Parameter 7683.

To leave the pallet file:

ú To select the file manager, press the Taste PGM MGT key. ú To select a different type of file, press the SELECT TYPE soft key

and the soft key for the desired file type, for example SHOW.H.

ú Select the desired file.

4 Programming: Fundamentals of NC, File Management,

Programming Aids, Pallet Management

Programming:

Tools

5.1 Entering Tool-Related Data

Feed rate F

The feed rate is the speed (in millimeters per minute or inches per minute) at which the tool center moves. The maximum feed rates can be different for the individual axes and are set in machine parameters.

Input

You can enter the feed rate in every positioning block or in a separate block. Press the F key on the alphabetic keyboard.

Rapid traverse

If you wish to program rapid traverse, enter G00.

Duration of effect

A feed rate entered as a numerical value remains in effect until a block with a different feed rate is reached. If the new feed rate is G00 (rapid traverse), the last programmed feed rate is once again

5.1 Entering Tool-Related Data

valid after the next block with G01.

Changing during program run

You can adjust the feed rate during program run with the feed-rate override knob.

Spindle speed S

The spindle speed S is entered in revolutions per minute (rpm) in any block (e.g. during tool call).

Programmed change

In the part program, you can change the spindle speed with an S block:

ú Press the S key on the alphabetic keyboard ú Enter the new spindle speed

Changing during program run

You can adjust the spindle speed during program run with the spindle-speed override knob.

5 Programming: Tools

5.2 Tool Data

You usually program the coordinates of path contours as they are dimensioned in the workpiece drawing. To allow the TNC to calculate the tool center path — i.e. the tool compensation — you must also enter the length and radius of each tool you are using.

Tool data can be entered either directly in the part program with G99 or separately in tool tables. In a tool table, you can also enter additional data on the specific tool. The TNC will consider all the data entered for the tool when executing the part program.

5.2 Tool Data

Tool numbers and tool names

Each tool is identified by a number between 0 and 254. If you are working with tool tables, you can use higher numbers (not TNC 410) and you can also enter a tool name for each tool (not TNC 410).

The tool number 0 is automatically defined as the zero tool with the length L=0 and the radius R=0. In tool tables, tool 0 should also be defined with L=0 and R=0.

Tool length L

There are two ways to determine the tool length L: 1 The length L is the difference between the length of the tool and

that of a zero tool L

For the algebraic sign:

■ The tool is longer than the zero tool L>L

■ The tool is shorter than the zero tool: L<L

To determine the length:

ú Move the zero tool to the reference position in the tool axis

(e.g. workpiece surface with Z=0).

ú Set the datum in the tool axis to 0 (datum setting). ú Insert the desired tool. ú Move the tool to the same reference position as the zero tool. ú The TNC displays the difference between the current tool and the

zero tool.

ú Using the key for ”actual position capture” (TNC 426 B, TNC 430)

or the soft key ACT. POS. Z (TNC 410), transfer the value to the G99 block or the tool table.

2 Determine the tool length L with a tool presetter. This allows you

to enter the determined value directly in the G99 tool definition block without further calculations.

79HEIDENHAIN TNC 410, TNC 426, TNC 430

Tool radius R

You can enter the tool radius R directly.

Delta values for lengths and radii

Delta values are offsets in the length and radius of a tool. A positive delta value describes a tool oversize (DR>0). If you are

5.2 Tool Data

programming the machining data with an allowance, enter the oversize value with T.

A negative delta value describes a tool undersize (DR<0). An undersize is entered in the tool table for wear.

Delta values are usually entered as numerical values. In a T block, you can also assign the values to Q parameters.

Input range: You can enter a delta value with up to ± 99.999 mm.

Entering tool data into the program

The number, length and radius of a specific tool is defined in the G99 block of the part program.

ú Select tool definition. Press ENT to confirm. ú Enter the Tool number: Each tool is uniquely identified

by its number.

ú Enter the tool length: Enter the compensation value

for the tool length.

ú Enter the Tool radius.

DL<0

DR<0

DR>0

DL>0

In the programming dialog, you can transfer the value for tool length directly into the input line.

TNC 426, TNC 430:

Press the actual-position-capture key. You only need to make sure that the highlight in the status display is placed on the tool axis.

TNC 410:

Press the ACT. POS. Z soft key.

Resulting NC block:

N40 G99 T5 L+10 R+5 *

5 Programming: Tools

Entering tool data in tables

You can define and store up to 32767 tools and their tool data in a tool table (TNC 410: 254 tools). In Machine Parameter 7260, you can define how many tool places are to be reserved by the TNC when a new table is set up. See also the Editing Functions at a later stage in this Chapter. For the TNC 426, TNC 430 with the NC software number 280 474-xx, in order to be able to assign various compensation data to a tool (indexing tool number), machine parameter 7262 must not be equal to 0.

Tool table: Available input data

Abbr. Input

T Number by which the tool is called in the program

You must use tool tables if

■ your machine tool has an automatic tool changer,

■ you want to measure tools automatically with the

TT 120 touch probe (only conversational programming)

5.2 Tool Data

Dialog Width of column

–

NAME Name by which the tool is called in the program

L Value for tool length compensation R Compensation value for the tool radius R R2 Tool radius R2 for toroid cutters

(only for 3-D radius compensation or graphical representation of a machining operation with spherical or

toroid cutters, not TNC 410) DL Delta value for tool length DR Delta value for tool radius R DR2 Delta value for tool radius R2 (not TNC 410) LCUTS Tooth length of the tool for Cycle G122 ANGLE Maximum plunge angle of the tool for reciprocating

plunge-cut in Cycles G122 and G208 TL Set tool lock

(TL:Tool Lock RT Number of replacement tool,

if available

(see also TIME2)

TIME1 Maximum tool life in minutes. This

function can vary depending on the individual machine

tool. Your machine manual provides more information

on TIME1. TIME2 Maximum tool life in minutes during TOOL CALL.

If the current tool age exceeds this value,

the TNC changes the tool

during the next TOOL CALL

(see also CUR.TIME) CUR.TIME Time in minutes the tool has been in use:

The TNC automatically counts

the current tool age.

A starting value can be entered for used tools.

Continued on next page

Tool name?

Tool length? Tool radius? Tool radius 2?

Tool length oversize? Tool radius oversize? Tool radius oversize 2 ? Tool length in the tool axis? Maximum plunge angle?

Tool locked? Yes = ENT / No = NO ENT Replacement tool?

Maximum tool age ?

Maximum tool life for TOOL CALL?

Current tool life?

81HEIDENHAIN TNC 410, TNC 426, TNC 430

Abbr. Input

DOC Comment on tool (up to 16 characters) PLC Information on this tool that is to be sent to the PLC

Only TNC 426, TNC 430 with NC Software 280 474-xx

PLC-VAL Value of this tool that is to be sent to the PLC

5.2 Tool Data

Tool table: Tool data required for automatic tool measurement (only conversational programming)

Dialog Width of column

Tool description? PLC status?

PLC value?

Abbr. Input

CUT. Number of teeth (20 teeth maximum) LTOL Permissible deviation from tool length L for

wear detection. If the entered value is exceeded, the TNC locks the tool(status L). Input range: 0 to 0.9999 mm

RTOL Permissible deviation from tool radius R for

wear detection. If the entered value is exceeded, the TNC locks the tool(status L). Input range: 0 to 0.9999 mm

DIRECT. Cutting direction of the tool for measuring the tool

during rotation

TT:R-OFFS Tool length measurement: tool offset between

stylus center and tool center. Preset value: Tool radius R

TT:L-OFFS Tool radius measurement: tool offset in addition

to MP6530 (see „14.1 General User Parameters) between upper surface of stylus and lower surface of tool. Preset value: 0

LBREAK Permissible deviation from tool length L for

breakage detection. If the entered value is exceeded, the TNC locks the tool (status L). Input range: 0 to 0.9999 mm

RBREAK Permissible deviation from tool radius R for

breakage detection. If the entered value is exceeded, the TNC locks the tool (status L). Input range: 0 to 0.9999 mm

Dialog

Number of teeth ? Wear tolerance: length ?

Wear tolerance: radius ?

Cutting direction (M03 = –) ?

Tool offset: radius ?

Tool offset: length ?

Breakage tolerance: length ?

Breakage tolerance: radius ?

5 Programming: Tools

Editing tool tables

The tool table that is active during execution of the part program is designated TOOL.T. TOOL.T must be stored in the directory TNC:\ and can be edited in any of the machine operating modes. Other tool tables that are used for archiving or test runs are given different file names with the extension .T .

To open the tool table TOOL.T:

ú Select any machine operating mode.

ú To select the tool table, press the TOOL TABLE soft

key.

ú Set the EDIT soft key to ON.

To open any other tool table

ú Select the Programming and Editing mode of operation.

ú Calling the file manager ú To select the file type, press the SELECT TYPE soft

key.

ú To show type .T files, press the SHOW soft key. ú Select a file or enter a new file name. Conclude your

entry with the ENT key or SELECT soft key.

When you have opened the tool table, you can edit the tool data by moving the cursor to the desired position in the table with the arrow keys or the soft keys (see figures at upper and center right). You can overwrite the stored values, or enter new values at any position. Refer to the table (on the next page) for additional editing functions.

If the TNC cannot show all positions in the tool table in one screen page, the highlight bar at the top of the table will display the symbol >> or << .

5.2 Tool Data

To leave the tool table:

ú Finish editing the tool table: Press the END key. ú Call the file manager and select a file of a different type, e.g. a

part program.

83HEIDENHAIN TNC 410, TNC 426, TNC 430

Editing functions for tool tables TNC 426, TNC 430 Soft key

Editing functions for Tool Table TNC 410 Soft key

Select beginning of table

Select end of table

Select previous page in table

5.2 Tool Data

Select next page in table

Look for the tool name in the table

Show tool information in columns or show the information on one tool on one screen page

Move to beginning of line

Move to end of line

Copy the highlighted field

Insert the copied field

Add the entered number of lines (tools) to the end of the table

Select previous page in table

Select next page in table

Move highlight to the left

Move highlight to the right

Lock tool in TL column

Do not lock tool in TL column

Confirm actual positions, e.g. for Z axis

Confirm entered value Select next column in the table

Delete incorrect value, restore previous value

Restore last value stored

Only TNC 426 B, TNC 430 with the NC software 280 474-xx:

Insert a line for the indexed tool number after the active line. The function is only active if you are permitted to store various compensation data for a tool (machine parameter 7262 not equal to 0). The TNC inserts a copy of the tool data after the last available index and increases the index by 1

Delete current line (tool)

Display / Do not display pocket numbers

Display all tools / only those tools that are stored in the pocket table

5 Programming: Tools

HEIDENHAIN TNC 426B User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual