HEIDENHAIN TNC 410 User Manual

Download

Page 1

TNC 410

NC-Software 286 060-xx 286 080-xx

User’s Manual

Conversational

Programming

English (en)

6/2001

Page 2

Controls on the visual display unit

Split screen layout

Toggle display between machining and programming modes

Soft keys for selecting functions in screen

Shift soft-key rows for the soft keys

Change screen settings

Controls on the TNC

(BC 120 only)

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 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

HELP functions

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

APPR

Approach/depart contour

DEP

Free contour programming

Straight line

Circle center/pole for polar coordinates

Circle with center

Circle with radius

Tangential circle

CHF

Chamfer

RND

Corner rounding

Tool functions

TOOL

DEF

Enter or call tool length and radius

CALL

Cycles, subprograms and program section repeats

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

End block

Clear numerical entry or TNC error message

DEL

Abort dialog, delete program section

Confirm entry and resume dialog

Page 3

Page 4

TNC Models, Software and Features

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

TNC Model NC Software No.

TNC 410 286 060-xx TNC 410 286 080-xx

The machine tool builder adapts the useable features of the TNC to his machine by setting machine parameters. Therefore, 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

■ Tool measurement with the TT 120

■ Rigid tapping

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.

Contents

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.

IHEIDENHAIN TNC 410

Page 5

Contents

Page 6

Contents

Introduction

Manual Operation and Setup

Positioning with Manual Data Input

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

2 3 4 5 6 7 8 9

Digitizing

MOD Functions

Tables and Overviews

13 14 15

IIIHEIDENHAIN TNC 410

Page 7

1 INTRODUCTION ..... 1

1.1 The TNC 410 ..... 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 ..... 12

2 MANUAL OPERATION AND SETUP ..... 13

2.1 Switch-On ..... 14

2.2 Moving the Machine Axes ..... 15

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 18

2.4 Setting the Datum (Without a 3-D Touch Probe) ..... 19

3 POSITIONING WITH MANUAL DATA INPUT (MDI) ..... 21

3.1 Programming and Executing Simple Positioning Blocks ..... 22

4 PROGRAMMING: FUNDAMENTALS OF NC, FILE MANAGEMENT, PROGRAMMING AIDS ..... 25

4.1 Fundamentals of NC ..... 26

4.2 File Management ..... 31

4.3 Creating and Writing Programs ..... 34

4.4 Interactive Programming Graphics ..... 39

4.5 Adding Comments ..... 40

4.6 HELP Function ..... 41

5 PROGRAMMING: TOOLS ..... 43

5.1 Entering Tool-Related Data ..... 44

5.2 Tool Data ..... 45

5.3 Tool Compensation ..... 52

5.4 Measuring Tools with the TT 120 ..... 56

Contents

Page 8

6 PROGRAMMING: PROGRAMMING CONTOURS ..... 63

6.1 Overview of Tool Movements ..... 64

6.2 Fundamentals of Path Functions ..... 65

6.3 Contour Approach and Departure ..... 68

Overview: Types of paths for contour approach and departure ..... 68

Important positions for approach and departure ..... 68

Approaching on a straight line with tangential connection: APPR LT ..... 70

Approaching on a straight line perpendicular to the first contour point: APPR LN ..... 70

Approaching on a circular arc with tangential connection: APPR CT ..... 71

Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT ..... 72

Departing tangentially on a straight line: DEP LT ..... 73

Departing on a straight line perpendicular to the last contour point: DEP LN ..... 73

Departing tangentially on a circular arc: DEP CT ..... 74

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT ..... 75

6.4 Path Contours — Cartesian Coordinates ..... 76

Overview of path functions ..... 76

Straight line L ..... 77

Inserting a chamfer CHF between two straight lines ..... 77

Circle center CC ..... 78

Circular path C around circle center CC ..... 79

Circular path CR with defined radius ..... 80

Circular path CT with tangential connection ..... 81

Corner Rounding RND ..... 82

Example: Linear movements and chamfers with Cartesian coordinates ..... 83

Example: Circular movements with Cartesian coordinates ..... 84

Example: Full circle with Cartesian coordinates ..... 85

6.5 Path Contours – Cartesian Coordinates ..... 86

Polar coordinate origin: Pole CC ..... 86

Straight line LP ..... 87

Circular path CP around pole CC ..... 87

Circular path CTP with tangential connection ..... 88

Helical interpolation ..... 88

Example: Linear movement with polar coordinates ..... 90

Example: Helix ..... 91

Contents

VHEIDENHAIN TNC 410

Page 9

6.6 Path Contours – FK Free Contour Programming ..... 92

Fundamentals ..... 92

Graphics during FK programming ..... 92

Contents

7 PROGRAMMING: MISCELLANEOUS FUNCTIONS ..... 103

Initiating the FK dialog ..... 93

Free programming of straight lines ..... 94

Free programming of circular arcs ..... 94

Auxiliary points ..... 96

Relative data ..... 97

Closed contours ..... 97

Example: FK programming 1 ..... 98

Example: FK programming 2 ..... 99

Example: FK programming 3 ..... 100

7.1 Entering Miscellaneous Functions M and STOP ..... 104

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 105

7.3 Miscellaneous Functions for Coordinate Data ..... 105

Programming machine-referenced coordinates: M91/M92 ..... 105

7.4 Miscellaneous Functions for Contouring Behavior ..... 107

Smoothing corners: M90 ..... 107

Entering contour transitions between contour elements: M112 ..... 108

Contour filter: M124 ..... 110

Machining small contour steps: M97 ..... 112

Machining open contours: M98 ..... 113

Feed rate factor for plunging movements: M103 ..... 114

Constant feed rate at the tool cutting edge: M109/M110/M111 ..... 115

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 115

7.5 Miscellaneous Functions for Rotary Axes ..... 117

Shorter-path traverse of rotary axes: M126 ..... 117

Reducing display of a rotary axis to a value less than 360°: M94 ..... 117

Contents

Page 10

8 PROGRAMMING: CYCLES ..... 119

8.1 General Overview of Cycles ..... 120

8.2 Point Tables ..... 122

Creating a point table ..... 122

Selecting point tables in the program. ..... 122

Calling a cycle in connection with point tables ..... 123

8.3 Drilling Cycles ..... 124

PECKING (Cycle 1) ..... 124

DRILLING (Cycle 200) ..... 126

REAMING (Cycle 201) ..... 127

BORING (Cycle 202) ..... 128

UNIVERSAL DRILLING (Cycle 203) ..... 129

BACK BORING (Cycle 204) ..... 131

TAPPING with a floating tap holder (Cycle 2) ..... 133

RIGID TAPPING GS (Cycle 17) ..... 134

Example: Drilling cycles ..... 135

Example: Drilling cycles ..... 136

Example: Calling drilling cycles in connection with point tables ..... 137

8.4 Cycles for Milling Pockets, Studs and Slots ..... 139

POCKET MILLING (Cycle 4) ..... 140

POCKET FINISHING (Cycle 212) ..... 141

STUD FINISHING (Cycle 213) ..... 143

CIRCULAR POCKET MILLING (Cycle 5) ..... 144

CIRCULAR POCKET FINISHING (Cycle 214) ..... 146

CIRCULAR STUD FINISHING (Cycle 215) ..... 147

SLOT MILLING (Cycle 3) ..... 149

SLOT (Slot milling) with reciprocating plunge cut (Cycle 210) ..... 150

CIRCULAR SLOT with reciprocating plunge-cut (Cycle 211) ..... 152

Example: Milling pockets, studs and slots ..... 154

Example: Roughing and finishing a rectangular pocket in connection with point tables ..... 156

8.5 Cycles for Machining Hole Patterns ..... 158

CIRCULAR PATTERN (Cycle 220) ..... 159

LINEAR PATTERN (Cycle 221) ..... 160

Example: Circular hole patterns ..... 162

Contents

VIIHEIDENHAIN TNC 410

Page 11

8.6 SL cycles ..... 164

Contents

8.7 Cycles for multipass milling ..... 176

8.8 Coordinate Transformation Cycles ..... 181

8.9 Special Cycles ..... 190

CONTOUR GEOMETRY (Cycle 14) ..... 165

Overlapping contours ..... 166

Pilot drilling (Cycle 15) ..... 168

ROUGH-OUT (Cycle 6) ..... 169

CONTOUR MILLING (Cycle 16) ..... 171

Example: Rough-out a pocket ..... 172

Example: Pilot drilling, roughing-out and finishing overlapping contours ..... 174

MULTIPASS MILLING (Cycle 230) ..... 176

RULED SURFACE (Cycle 231) ..... 178

Example: Multipass milling ..... 180

DATUM SHIFT (Cycle 7) ..... 182

DATUM SHIFT with datum tables (Cycle 7) ..... 182

MIRROR IMAGE (Cycle 8) ..... 184

ROTATION (Cycle 10) ..... 185

SCALING FACTOR (Cycle 11) ..... 186

AXIS-SPECIFIC SCALING (Cycle 26) ..... 187

Example: Coordinate transformation cycles ..... 188

DWELL TIME (Cycle 9) ..... 190

PROGRAM CALL (Cycle 12) ..... 190

ORIENTED SPINDLE STOP (Cycle 13) ..... 191

9 PROGRAMMING: SUBPROGRAMS AND PROGRAM SECTION REPEATS ..... 193

9.1 Marking Subprograms and Program Section Repeats ..... 194

9.2 Subprograms ..... 194

9.3 Program section repeats ..... 195

9.4 Program as Subprogram ..... 196

9.5 Nesting ..... 197

Subprogram within a subprogram ..... 197

Repeating program section repeats ..... 198

Repeating a subprogram ..... 199

9.6 Programming Examples ..... 200

Example: Milling a contour in several infeeds ..... 200

Example: Groups of holes ..... 201

Example: Groups of holes with several tools ..... 202

VIII

Contents

Page 12

10 PROGRAMMING: Q PARAMETERS ..... 205

10.1 Principle and Overview ..... 206

10.2 Part Families — Q Parameters in Place of Numerical Values ..... 207

10.3 Describing Contours Through Mathematical Functions ..... 208

10.4 Trigonometric Functions ..... 210

10.5 If-Then Decisions with Q Parameters ..... 211

10.6 Checking and Changing Q Parameters ..... 212

10.7 Additional Functions ..... 213

10.8 Entering Formulas Directly ..... 219

10.9 Preassigned Q Parameters ..... 222

10.10 Programming Examples ..... 224

Example: Ellipse ..... 224

Example: Concave cylinder machined with spherical cutter ..... 2267

Example: Convex sphere machined with end mill ..... 228

11 TEST RUN ND PROGRAM RUN ..... 231

11.1 Graphics ..... 232

11.2 Test run ..... 236

11.3 Program run ..... 238

11.4 Blockwise Transfer: Running Longer Programs ..... 245

11.5 Optional Block Skip ..... 246

11.6 Optional Program Run Interruption ..... 246

Contents

12 3-D TOUCH PROBES ..... 247

12.1 Touch Probe Cycles in the Manual and Electronic Handwheel modes. ..... 248

12.2 Setting the Datum with a 3-D Touch Probe ..... 251

12.3 Measuring Workpieces with a 3-D Touch Probe ..... 254

13 DIGITIZING ..... 259

13.1 Digitizing with a Triggering Touch Probe (Optional) ..... 260

13.2 Programming Digitizing Cycles ..... 261

13.3 Meander Digitizing ..... 262

13.4 Contour Line Digitizing ..... 263

13.5 Using Digitized Data in a Part Program ..... 265

IXHEIDENHAIN TNC 410

Page 13

14 MOD FUNCTIONS ..... 267

14.1 Selecting, Changing and Exiting the MOD Functions ..... 268

14.2 System Information ..... 268

Contents

14.3 Code Number ..... 269

14.4 Setting the Data Interface ..... 269

14.5 Machine-Specific User Parameters ..... 271

14.6 Position Display Types ..... 272

14.7 Unit of Measurement ..... 272

14.8 Select the Programming Language ..... 273

14.9 Enter Axis Traverse Limits ..... 274

14.10 The HELP Function ..... 275

15 TABLES AND OVERVIEWS ..... 277

15.1 General User Parameters ..... 278

Input possibilities for machine parameters ..... 278

Selecting user parameters ..... 278

External data transfer ..... 279

3-D touch probes and digitizing ..... 280

TNC displays, TNC editor ..... 282

Machining and program run ..... 287

Electronic handwheels ..... 289

15.2 Pin Layout and Connecting Cable for the Data Interface ..... 290

15.3 Technical Information ..... 292

TNC features ..... 292

Programmable functions ..... 293

TNC Specifications ..... 294

15.4 TNC Error Messages ..... 295

TNC error messages during programming ..... 295

TNC error messages during test run and program run ..... 296

TNC error messages during digitizing ..... 299

15.5 Changing the Buffer Battery ..... 300

Contents

Page 14

Introduction

Page 15

1.1 The TNC 410

HEIDENHAIN TNC controls are shop-floor programmable contouring controls for milling, drilling and boring machines, as well as machining centers with up to four axes. You can program conventional milling, drilling and boring operations right at the machine with the easily understandable interactive conversational guidance. You can also change the angular position of the spindle under program control.

1.1 The TNC 410

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 during test run. It is also possible to program in ISO format or DNC mode.

You can enter a program while the TNC is running another.

Compatibility

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

1 Introduction

Page 16

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.

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 right and left. 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

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.

. The lines immediately above the

Move picture to the left or downward

Move picture to the right or upward

1.2 Visual Display Unit and Keyboard

3HEIDENHAIN TNC 410

Page 17

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

You select the screen layout yourself: In the PROGRAMMING AND

1.2 Visual Display Unit and Keyboard

EDITING mode of operation, for example, you can have the TNC show program blocks in the left window while the right window displays programming graphics. You could also display help graphics for cycle definition in the right window instead, or display only program blocks in one large window. The available screen windows depend on the selected operating mode.

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row shows the available layout options.

Select the desired screen layout.

1 Introduction

Page 18

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, MOD functions, HELP functions

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 in the foldout of the 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

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 and set the datums.

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

The same selection is available as in the Positioning with MDI mode. The TNC always shows the positions at left in the divided screen.

5HEIDENHAIN TNC 410

Page 19

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 blocks

Left: program, right: general program information

Left: program, right: positions and

1.3 Modes of Operation

coordinates

Left: program, right: information on tools

Left: Program, right: coordinate transformations

Programming and Editing

In this mode of operation you can write your part programs. The FK free programming feature, the various cycles and the Q parameter functions help you with programming and add necessary information. If desired, you can have the programming graphics show the individual steps.

Soft keys for selecting the screen layout

Screen windows Soft key

Program blocks

Left: program, right: help graphics for cycle programming

Left: program blocks, right: programming graphics

Interactive Programming Graphics

1 Introduction

Page 20

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

Screen windows Soft key

Program blocks

Test run graphics

Left: program, right: test run graphics

Left: program, right: general program information

Left: program, right: positions and coordinates

Left: program, right: information on tools

1.3 Modes of Operation

Left: Program, right: coordinate transformations

7HEIDENHAIN TNC 410

Page 21

Program Run, Full Sequence and Program Run, Single Block

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

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

Soft keys for selecting the screen layout

Screen windows Soft key

Program blocks

1.3 Modes of Operation

Left: program, right: general program information

Left: program, right: positions and coordinates

Left: program, right: information on tools

Left: Program, right: coordinate transformations

Left: program, right: tool measurement

1 Introduction

Page 22

1.4 Status Displays

“General” status displays

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

In the Manual mode,Electronic Handwheel mode, and Positioning with MDI mode the position display appears in the large window.

Information in the status display

Symbol Meaning

ACTL. Actual or nominal coordinates of the current position

X Y Z

S F M

Machine axes

Spindle speed S, feed rate F and active M functions

Program run started

Axis locked

Axes are moving under a basic rotation.

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:

1.4 Status Displays

Call the soft-key row for screen layout.

Select the layout option for the additional status display, e.g. positions and coordinates.

9HEIDENHAIN TNC 410

Page 23

You can also choose between the following additional status displays:

General program information

Name of main program Active programs Active machining cycle Circle center CC (pole)

1.4 Status Displays

Dwell time counter Active program section repeats/Counter for current

program section repeat (5/3: 5 repetitions programmed, 3 remaining to be run)

Operating time

Positions and coordinates

Position display Type of position display, e.g. actual positions Angle of a basic rotation

1 Introduction

Page 24

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

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 (Cycle 11 or Cycle 26)

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

1.4 Status Displays

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.

11HEIDENHAIN TNC 410

Page 25

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.

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 optical switch.

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

HR electronic handwheels

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

1 Introduction

Page 26

Manual Operation and Setup

Page 27

2.1 Switch-On

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

Switch on the power supply for control and machine.

2.1 Switch-On

The TNC automatically initiates the following dialog

Memory Test

The TNC memory is automatically checked.

Power Interrupted

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

PLC-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.

Manual Operation Traverse Reference Points

Cross the reference points in any sequence:

Press and hold the machine axis direction button for each axis until the reference point has been traversed, or

Cross the reference points with several axes at

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

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

2 Manual Operation and Setup

Page 28

2.2 Moving the Machine Axes

Traversing with the machine axis direction buttons is a machine-dependent function. Your machine manual provides more detailed information.

To traverse with the machine axis direction buttons:

Select the Manual Operation mode.

Press the machine axis direction button and

hold it as long as you wish the axis to move.

...or 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.

15HEIDENHAIN TNC 410

Page 29

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

Page 30

Incremental jog positioning

With incremental jog positioning you can move a machine axis by a preset distance each time you press the corresponding machine axis direction button.

Select the Electronic Handwheel or Manual

mode of operation.

Select incremental jog positioning, set the soft key to On.

JOG INCREMENT =

Enter the jog increment in mm, e.g. 8 mm, or

Enter the jog increment via soft key (preset softkey values).

Press the machine axis direction button as often as desired.

2.2 Moving the Machine Axes

17HEIDENHAIN TNC 410

Page 31

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

In the operating modes Manual and Electronic Handwheel, enter the spindle speed S and the miscellaneous function M using soft keys. The miscellaneous functions are described in Chapter 7 ”Programming: Miscellaneous Functions.” The feed rate is defined in a machine parameter and can be changed only with the override knobs (see next page).

Entering values

Example: Enter 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.

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

Proceed in the same way to enter the miscellaneous functions M.

Changing the spindle speed S and feed rate F

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.

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

2 Manual Operation and Setup

Page 32

2.4 Setting the Datum (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.

To prepare the TNC:

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.

Set the datum

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 the axis.

Datum Set

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.

ÿÿÿ

Zero tool in spindle axis: Set the display to a

known workpiece position (here, 0) or enter the

thickness the tool radius.

of the shim. In the tool axis, offset

on it. Then enter a

2.4 Setting the Datum

19HEIDENHAIN TNC 410

Page 33

Page 34

Positioning with Manual Data Input (MDI)

Page 35

3.1 Programming and Executing Simple Positioning Blocks

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

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

To start program run, press the machine START button.

Limitations:

The following functions are not available:

- - Tool radius compensation

- FK free contour programming

- Programming graphics and program-run graphics

- The programmable probing functions

- Subprograms, Program section repetitions

- The path functions CT, CR, RND and CHF

- PGM CALL

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.

3.1 Programming and Executing Simple Positioning Blocks

First you pre-position the tool in L blocks (straight-line blocks) to the hole center coordinates at a setup clearance of 5 mm above the workpiece surface. Then drill the hole with Cycle 1 PECKING.

0 BEGIN PGM $MDI MM 1 TOOL DEF 1 L+0 R+5 2 TOOL CALL 1 Z S2000

3 L Z+200 R0 FMAX 4 L X+50 Y+50 R0 FMAX M3 5 L Z+5 F2000

Define tool: zero tool, radius 5 Call tool: tool axis Z Spindle speed 2000 rpm Retract tool (FMAX = rapid traverse) Move the tool at FMAX to a position above the borehole, spindle on Position tool to 5 mm above hole

3 Positioning with Manual Data Input (MDI)

Page 36

6 CYCL DEF 1.0 PECKING 7 CYCL DEF 1.1 SET UP 5 8 CYCL DEF 1.2 DEPTH -20 9 CYCL DEF 1.3 PECKG 10 10 CYCL DEF 1.4 DWELL 0.5 11 CYCL DEF 1.5 F250 12 CYCL CALL 13 L Z+200 R0 FMAX M2 14 END PGM $MDI MM

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

Example 2

Correcting workpiece misalignment on machines with rotary tables

Use the 3-D touch probe to rotate the coordinate system. See ”12.1 Touch probe cycles in the Manual and Electronic Handwheel Mode” section ”Compensating workpiece misalignment.”

Write down the Rotation Angle and cancel the Basic Rotation.

Define PECKING cycle: 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 PECKING cycle Retract tool End of program

Select operating mode: Positioning with MDI.

Select the axis of the rotary table, enter the

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

Conclude entry.

Press the machine START button: The rotation of the table corrects the misalignment. After the NC start the highlight is moved onto the next block.

3.1 Programming and Executing Simple Positioning Blocks

23HEIDENHAIN TNC 410

Page 37

Protecting and erasing programs in $MDI

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

Select operating mode: Programming and Editing

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

Move the highlight to the $MDI file.

Select „Copy file“: Press the COPY soft key

Target file =

BOREHOLE

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

Copy the file.

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

Erasing the contents of the $MDI file is done in a similar way:

3.1 Programming and Executing Simple Positioning Blocks

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.

If you wish to switch between conversational and ISO programming with the MOD function, you need to delete the current file $MDI.*, and then select again the Positioning with MDI operating mode.

For further information, refer to section 4.2 “File Management.”

3 Positioning with Manual Data Input (MDI)

Page 38

Programming:

Fundamentals of NC, File Management, Programming Aids

Page 39

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 TNC 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

Page 40

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 up to 4 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 shows the assignment of secondary axes and rotary axes to the main axes.

4.1 Fundamentals of NC

V+

W+

C+

B+

A+

U+

27HEIDENHAIN TNC 410

Page 41

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

■ Polar Radius, the distance from the circle center CC to the

position, and the

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

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

4.1 Fundamentals of NC

See figure to the lower right.

Setting the pole and the angle reference axis

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

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

XY +X YZ +Y ZX +Z

0°

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

Page 42

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 prefix “I” before the axis.

Example 2: Holes dimensioned in relative coordinates

Absolute coordinates of hole

X= 10 mm Y= 10 mm

referenced to hole Hole referenced to hole

Hole IX= 20 mm IX= 20 mm

IY= 10 mm IY= 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

+IPA

+IPR

+IPA

0°

29HEIDENHAIN TNC 410

Page 43

Selecting the datum

A production drawing identifies a certain point on the workpiecee — usually a cornerr — 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 8.8 “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

Page 44

4.2 File Management

Files in the TNC Type

Files and file management

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 tables as files.

File names

The name of a file can have up to 8 characters. The special characters @, $, _, %, # and & are permitted. When you store programs and tables 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

The TNC permits only one file type per file name. You cannot assign several file types to the same name.

The TNC can manage up to 64 files. Their total size, however, must not exceed 256 KB.

Working with the file manager

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.

Programs

in HEIDENHAIN conversational format .H in ISO format .I

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

4.2 File Management

To call the file manager

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

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 Meaning

File name Name with up to 8 characters

and file type Properties of the file:

M Program is selected

in a Program Run operating mode

P Protect a file 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

31HEIDENHAIN TNC 410

Page 45

Select a file

Call the file manager.

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

Move the highlight up or down

Delete 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

4.2 File Management

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.

Copy 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.

Rename 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.

Converting an FK program into HEIDENHAIN conversational format

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

ú To select the converting function,

press the CONVERT FK->H soft key (2nd soft-key row).

ú Enter the name of the destination file. ú To execute conversion, press the ENT

key.

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

Page 46

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.

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 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.

4.2 File Management

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.

ú Move 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.

33HEIDENHAIN TNC 410

Page 47

4.3 Creating and Writing Programs

Organization of an NC program in HEIDENHAIN conversational format

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

The TNC numbers the blocks in ascending sequence. The first block of a program is identified by “BEGIN PGM,” the

program name and the active unit of measure. 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 is identified by “END PGM,” the program name and the active unit of measure.

4.3 Creating and Writing Programs

Defining the blank form — BLK FORM

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

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

entered as absolute values.

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

entered as absolute or incremental values.

The TNC can display the graphic only if the short side of the BLK FORM is longer than 1/64 of the long side.

Block:

10 L X+10 Y+5 R0 F100 M3

Path function Words

Block number

MIN

MAX

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

Page 48

Creating a new part program

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 soft key.

File name =

NEW Entering new program names

Select the file type, e.g. HEIDENHAIN conversational: Press the .H soft key.

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

4.3 Creating and Writing Programs

Confirm your entry with the ENT key.

35HEIDENHAIN TNC 410

Page 49

Define the blank

Open the dialog for blank definition: Press the BLK FORM soft key

Working spindle axis X/Y/Z ?

Enter the spindle axis.

Def BLK FORM: Min corner?

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

-40

Def BLK FORM: Max-corner?

4.3 Creating and Writing Programs

100

The program blocks window shows the following BLK FORM definition

BEGIN PGM NEW MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 2 BLK FORM 0.2 X+100 Y+100 Z+0 END PGM NEW MM

The TNC automatically generates the block numbers as well as the BEGIN and END blocks.

End the dialog MIN-corner entry.

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

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

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

Page 50

Programming tool movements in HEIDENHAIN conversational format

To program a block, initiate the dialog by pressing a function key. In the screen headline, the TNC then asks you for all the information necessary to program the desired function.

Dialog initiation in an example

Initiate the dialog.

Coordinates ?

Enter the target coordinate for the X axis.

Enter the target coordinate for the Y axis, and go to the next question with ENT.

Radius comp.: RL/RR/no comp. ?

Enter “No radius compensation” and go to the next question with ENT.

Functions during the dialog Key

Ignore the dialog question

4.3 Creating and Writing Programs

End the dialog immediately, save the block

Feed rate ? F=

100

The program blocks window will display the following line:

3 L X+10 Y+5 R0 F100 M3

Enter a feed rate of 100 mm/min for this path contour; go to the next question with ENT.

Miscellaneous function M ?

Enter the miscellaneous function directly, e.g M3 for ”spindle on,” or

enter miscellaneous functions that require additional input values, e.g. M120: Press M120 and enter the values.

Press the END key to end the dialog and save the entered block.

Abort the dialog and erase the block

37HEIDENHAIN TNC 410

Page 51

Editing program lines

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

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.

4.3 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 blocks at any desired location

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

initiate the dialog.

Inserting the previously edited (deleted) block at any desired 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.

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.

Jump 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

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.

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.

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

Page 52

4.4 Interactive Programming Graphics

While you are writing the part program, you can have the TNC generate a graphic illustration of the programmed contour. The TNC represents movements in a negative spindle axis direction with a white circle (circle diameter = machine tool diameter).

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.

To generate 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.

Functions Soft key

Generate interactive graphic blockwise

Generate a complete graphic or complete it after RESET + START

4.4 Interactive Programming Graphics

Additional functions are listed in the table at right.

To erase the graphic:

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

Stop the programming graphics This soft key only appears while the TNC generates the interactive graphics

39HEIDENHAIN TNC 410

Page 53

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:

Principle Soft key

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

Enlarge the frame overlay — press and

4.5 Adding Comments

hold the soft key to magnify the detail

Shift the frame

ú With the WINDOW DETAIL soft key, Confirm the

selected area.

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

4.5 Adding Comments

To explain or identify program steps you can enter comment blocks.

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 Programming: Fundamentals of NC, File Management, Programming Aids

Page 54

4.6 HELP Function

Certain TNC programming functions are explained in more detail in the HELP function. 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)

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

4.6 HELP Function

End the HELP function

Press the END soft key twice.

41HEIDENHAIN TNC 410

Page 55

Page 56

Programming:

Tools

Page 57

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. For further information refer to section 6.2 “Fundamentals of Path Contours.”

Rapid traverse

If you wish to program rapid traverse, enter FMAX. To enter FMAX, press the ENT key or the FMAX soft key as soon as the dialog question “Feed rate F = ?” appears on the TNC screen.

Duration of effect

A feed rate entered as a numerical value remains in effect until a

5.1 Entering Tool-Related Data

block with a different feed rate is reached. F MAX is only effective in the block in which it is programmed. After the block with F MAX is executed, the feed rate will return to the last feed rate entered as a numerical value.

Changing the spindle speed 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 a TOOL CALL block.

Programmed change

In the part program, you can change the spindle speed in a TOOL CALL block by entering the spindle speed only:

ú To program a tool call, press the TOOL CALL key. ú Ignore the dialog question for “Tool number ?” with

the NO ENT key.

ú Ignore the dialog question for “Working spindle axis X/

Y/Z ?” with the NO ENT key.

ú Enter the new spindle speed for the dialog question

“Spindle speed S= ?”, and confirm with END.

Changing the spindle speed during program run

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

5 Programming: Tools

Page 58

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 TOOL DEF or (and) separately in a tool table. 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 number

Each tool is identified by a number between 0 and 254. 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 Enter the value in the TOOL DEF block or in the tool table by

pressing the actual-position-capture soft key

2 If you determine the length L with a tool presetter, this value can

be entered directly in the TOOL DEF block without further calculations.

45HEIDENHAIN TNC 410

Page 59

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 in the TOOL CALL block of the part program.

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 TOOL CALL 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 TOOL DEF block of the part program.

ú To select tool definition, press the TOOL DEF key. 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: Enter the compensation value

for the tool radius.

DL<0

DR<0

DR>0

DL>0

During the dialog, you can take the values for length and radius directly from the position display with the soft keys „CUR.POS X, CUR.POS Y or CUR.POS Z“.

If you use the black key for actual-position capture, the TNC saves the value of the active tool axis for the tool length. If no tool axis is active, the TNC saves the value of the axis that has been defined in the probing function calibration menu as the touch probe axis.

Resulting NC block:

4 TOOL DEF 5 L+10 R+5

5 Programming: Tools

Page 60

Entering tool data in tables

You can define and store up to 254 tools and their tool data in a tool table. (The maximum number of tools in the table can be set in machine parameter 7260). See also the Editing Functions at a later stage in this Chapter.

Tool table: Available input data

You must use the tool table if:

■ your machine tool has an automatic tool changer

■ you want to measure tools automatically with the

TT 120 touch probe (see section 5.4 “Measuring Tools”)

5.2 Tool Data

Abbr. Input

T Number by which the tool is called in the program

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 DL Delta value for tool length DR Delta value for tool radius R TL Set tool lock

(TL:Tool Lock

RT Number of sister tool,if available,

as Replacement Tool (RT) (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. DOC Comment on tool (up to 16 characters) PLC Information on this tool that is

sent to the PLC

Dialog

–

Tool name?

Tool length? Tool radius? Tool length oversize? Tool radius oversize? Tool locked ?

Replacement tool?

Maximum tool age ?

Maximum tool life for TOOL CALL?

Current tool life?

Tool description? PLC status?

47HEIDENHAIN TNC 410

Page 61

Tool table: Tool data required for automatic tool measurement

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).

5.2 Tool Data

RTOL Permissible deviation from tool radius R for

DIRECT. Cutting direction of the tool for measuring the tool

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

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

LBREAK Permissible deviation from tool length L for

RBREAK Permissible deviation from tool radius R for breakage

Input range: 0 to 0.9999 mm

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

during rotation

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

to MP6530 (see section 15.1 +General User Parameters+) between upper edge of stylus and lower edge of tool. Preset value: 0

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

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 (M3 = –) ?

Tool offset: radius ?

Tool offset: length ?

Breakage tolerance: length ?

Breakage tolerance: radius ?

5 Programming: Tools

Page 62

Editing tool tables

The tool table that is active during execution of the part program is designated TOOL.T. Tool.T is automatically active in a Program Run operating mode. In the Programming and Editing mode, tool tables can also have other names.

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 Call the file manager. ú Select an existing file with the extension .T and press

the COPY soft key. Enter a new file name and confirm with the ENT 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 (see figure at upper right). You can overwrite the stored values, or enter new values at any position. The available editing functions are illustrated in the table at right.

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

Editing functions for tool tables Soft key

Go to the previous page of the table

Go to the next page of the table

Move highlight to the left

Move highlight to the right

Lock tool in TL column

To leave the tool table:

ú Finish editing the tool table: Press the ”End” soft key or the END

key.

ú Call the file manager and select a file of a different type, e.g. a

part program.

If you edit the tool table parallel to tool change the TNC does not interrupt the program run. However, the changed data does not become effective until the next tool call.

User parameter MP7266 defines which data can be entered in the tool table and in what sequence the data is displayed.

Do not lock tool in TL column

Confirm actual positions, e.g. for Z axis

Confirm entered value Select the next column in the table. If the highlight is at the end of the line, then jump to the first column of the next line.

Delete incorrect numerical value, re-establish preset value

Re-establish the last value stored

49HEIDENHAIN TNC 410

Page 63

Pocket table for tool changer

The TOOLP.TCH (TOOL Pocket)table must be programmed to enable automatic tool change.

To select the pocket table:

ú In the Programming and Editing mode,

5.2 Tool Data

ú In a machine operating mode

ú call the file manager. ú Move the highlight to TOOLP.TCH. Confirm with the

ENT key.

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

key.

ú To select the pocket table,

press the POCKET TABLE soft key

ú Set the EDIT soft key to ON

Editing functions for pocket tables Soft key

When you have opened the pocket table, you can edit the tool data by moving the cursor to the desired position in the table with the arrow keys (see figure at upper right). You can overwrite the stored values, or enter new values at any position.

You may not use a tool number twice in the pocket table. If you do so the TNC will output an error message when you exit the table.

You can enter the following information on a tool into a pocket table

Abbr. Input

P Pocket number of the tool in the tool magazine T Tool number ST Special tool with a large radius requiring several pockets

in the tool magazine. If your special tool takes up pockets in front of and behind its actual pocket, these additional pockets need to be locked (status L).

F Fixed tool number.

The tool is always returned to the same pocket. L Locked pocket PLC Information on this tool pocket that is to be

sent to the PLC

Select previous page in table

Select next page in table

Move the highlight one column to the left

Move the highlight one column to the right

Reset pocket table

Dialog

– Tool number? Special tool ?

Fixed pocket?

Locked pocket? PLC status?

5 Programming: Tools

Page 64

Calling tool data

A TOOL CALL block in the part program is defined with the following data:

ú Select the tool call function with the TOOL CALL key. ú Tool number: Enter the number of the tool. The tool

must already be defined in a TOOL DEF block or in the tool table.

ú Working spindle axis X/Y/Z: Enter the tool axis. Parallel

axes U, V and W are permitted.

ú Spindle speed S ú Tool length oversize: Enter the delta value for the tool

length.

ú Tool radius oversize: Enter the delta value for the tool

radius.

Example:

Call tool number 5 in the tool axis Z with a spindle speed 2500 rpm. The tool length is to be programmed with an oversize of 0.2 mm, the tool radius with an undersize of 1 mm.

20 TOOL CALL 5 Z S2500 DL+0.2 DR-1

The character D preceding L and R designates delta values.

Manual tool change

To change the tool manually, stop the spindle and move the tool to the tool change position:

ú Move to the tool change position under program

control.

ú Interrupt program run (see section 11.3 “Program

Run”).

ú Change the tool. ú Resume the program run (see section 11.3

“Program Run”).

Automatic tool change

If your machine tool has automatic tool changing capability, the program run is not interrupted. When the TNC reaches a TOOL CALL, it replaces the inserted tool by another from the tool magazine.

Automatic tool change if the tool life expires: M101

This function can vary depending on the individual machine tool. Your machine manual provides more information on M101.

5.2 Tool Data

Tool preselection with tool tables

When you use a tool table, enter a TOOL DEF block to preselect the next tool to be selected. Simply enter the tool number or a corresponding Q parameter, or type a tool name in quotation marks.

Tool change

The tool change function can vary depending on the individual machine tool. Your machine manual provides more information on M101.

Tool change position

A tool change position must be approachable without collision. With the miscellaneous functions M91 and M92, you can enter machinereferenced (rather than workpiece-referenced) coordinates for the tool change position. If TOOL CALL 0 is programmed before the first tool call, the TNC moves the tool spindle in the tool axis to a position that is independent of the tool length.

The TNC automatically changes the tool if the tool life TIME2 expires during program run. To use this miscellaneous function, activate M101 at the beginning of the program. M101 is reset with M102.

The tool is not always changed immediately, but, depending on the workload of the control, a few NC blocks later.

Prerequisites for standard NC blocks with radius compensation R0, RR, RL

The radius of the replacement tool must be the same as that of the original tool. If the radii are not equal, the TNC displays an error message and does not replace the tool.

51HEIDENHAIN TNC 410

Page 65

5.3 Tool Compensation

The TNC adjusts the spindle path in the tool axis by the compensation value for the tool length. In the working plane, it compensates the tool radius.

If you are writing the part program directly on the TNC, the tool radius compensation is effective only in the working plane. The TNC accounts for the compensation value in up to five axes including the rotary axes.

Tool length compensation

Length compensation becomes effective automatically as soon as a tool is called and the tool axis moves. To cancel length

5.3 Tool Compensation

compensation call a tool with the length L=0.

If you cancel a positive length compensation with TOOL CALL 0, the distance between tool and workpiece will be reduced.

After TOOL CALL, the path of the tool in the tool axis, as entered in the part program, is adjusted by the difference between the length of the previous tool and that of the new one.

For tool length compensation, the TNC takes the delta values from both the TOOL CALL block and the tool table into account:

Compensation value = L + DL

TOOL CALL

+ DL

L is the tool length L from the TOOL DEF block or tool

table

TOOL CALL

is the oversize for length DL in the TOOL CALL block (not taken into account by the position display)

TAB

is the oversize for length DL in the tool table

TAB

, where

Tool radius compensation

The NC block for programming a tool movement contains:

■ RL or RR for compensation in the tool radius

■ R+ or R– for radius compensation in single-axis movements

■ R0 if no radius compensation is required

Radius compensation becomes effective as soon as a tool is called and is moved in the working plane with RL or RR. To cancel radius compensation, program a positioning block with R0.

5 Programming: Tools

Page 66

For tool radius compensation, the TNC takes the delta values from

both the TOOL CALL block and the tool table into account: Compensation value = R + DR

TOOL CALL

+ DR

TAB

, where

R is the tool radius R from the TOOL DEF block or tool

table

TOOL CALL

is the oversize for radius DR in the TOOL CALL block (not taken into account by the position display)

TAB

is the oversize for radius DR in the tool table

Tool movements without radius compensation: R0

The tool center moves in the working plane to the programmed path or coordinates.

Applications: Drilling and boring, pre-positioning (see figure at center right)

Tool movements with radius compensation: RR and RL RR The tool moves to the right of the programmed contour

RL The tool moves to the left of the programmed contour

The tool center moves along the contour at a distance equal to the radius. “Right” or “left” are to be understood as based on the direction of tool movement along the workpiece contour (see illustrations on the next page).

Between two program blocks with different radius compensations (RR and RL) you must program at least one block without radius compensation (that is, with R0).

Radius compensation does not come into effect until the end of the block in which it is first programmed.

You can also activate the radius compensation for secondary axes in the working plane. Program the secondary axes too in each following block, since otherwise the TNC will execute the radius compensation in the principal axis again.

Whenever radius compensation is activated with RR/RL or canceled with R0, the TNC positions the tool perpendicular to the programmed starting or end position. Position the tool at a sufficient distance from the first or last contour point to prevent the possibility of damaging the contour.

5.3 Tool Compensation

53HEIDENHAIN TNC 410

Page 67

Entering radius compensation

When you program a path contour, the following dialog question is displayed after entry of the coordinates:

Radius comp.: RL/RR/no comp. ?

To select tool movement to the left of the contour, press the RL soft key, or

To select tool movement to the right of the contour, press the RR soft key, or

5.3 Tool Compensation

To select tool movement without radius compensation or to cancel radius compensation, press the ENT key or the R0 soft key.

To terminate the dialog, press the END key.

5 Programming: Tools

Page 68

Radius compensation: Machining corners

Outside corners

If you program radius compensation, the TNC moves the tool in a transitional arc around corners. The tool “rolls around” the corner point. If necessary, the TNC reduces the feed rate at outside corners to reduce machine stress, for example at very great changes of direction.

Inside corners

The TNC calculates the intersection of the tool center paths at inside corners under radius compensation. From this point it then starts the next contour element. This prevents damage to the workpiece. The permissible tool radius, therefore, is limited by the geometry of the programmed contour.

To prevent the tool from damaging the contour, be careful not to program the starting or end position for machining inside corners at a corner of the contour.

Machining corners without radius compensation

If you program the tool movement without radius compensation, you can change the tool path and feed rate at workpiece corners with the miscellaneous functions M90 and M112.See ”7.4 Miscellaneous Functions for Contouring Behavior.”

5.3 Tool Compensation

RL RL

55HEIDENHAIN TNC 410

Page 69

5.4 Measuring Tools with the TT 120

The TNC and the machine tool must be set up by the machine tool builder for use of the TT 120 touch probe.

Some cycles and functions may not be provided on your machine tool. Refer to your machine manual.

In conjunction with the TNC’s tool measurement cycles, the TT 120 enables you to measure tools automatically. The compensation values for tool length and radius can be stored in the central tool file TOOL.T and are accounted for in the next tool call. The following types of tool measurement are provided:

■ Tool measurement while the tool is at standstill

■ Tool measurement while the tool is rotating

■ Measurement of individual teeth

You can define the tool measurement cycles in the PROGRAMMING AND EDITING mode of operation. The following cycles are available:

■ TCH PROBE 30.0 TT CALIBRATE

■ TCH PROBE 31.0 TOOL LENGTH

■ TCH PROBE 32.0 TOOL RADIUS

The measuring cycles can be used only when the central tool file TOOL.T is active.

Before working with the measuring cycles, you must first enter all the required data into the central tool file

5.4 Tool Measurement with the TT 120 Touch Probe

and call the tool to be measured with TOOL CALL.

Setting the machine parameters

The TNC uses the feed rate for probing defined in MP6520 when measuring a tool at standstill.

When measuring a rotating tool, the TNC automatically calculates the spindle speed and feed rate for probing.

5 Programming: Tools

Page 70

The spindle speed is calculated as follows

MP6570

n =

r • 0.0063

where

n = spindle speed in rpm MP6570 = maximum permissible cutting speed in m/min r = active tool radius in mm

The feed rate for probing is calculated from: v = meas. tolerance • where v = feed rate for probing in mm/min

meas. tolerance = meas. tolerance in mm, depending on MP6507

n = speed in rpm

MP6507 determines the calculation of the probing feed rate: MP6507=0:

The measuring tolerance remains constant — regardless of the tool radius. With very large tools, however, the feed rate for probing is reduced to zero. The smaller you set the maximum permissible rotational speed (MP6570) and the permissible tolerance (MP6510), the sooner you will encounter this effect.

MP6507=1: The measuring tolerance is adjusted relative to the size of the tool radius. This ensures a sufficient feed rate for probing even with large tool radii. The TNC adjusts the measuring tolerance according to the following table:

Tool radius Meas. tolerance

up to 30 mm MP6510 30 to 60 mm 2 • MP6510 60 to 90 mm 3 • MP6510 90 to 120 mm 4 • MP6510

MP6507=2: The feed rate for probing remains constant, the error of measurement, however, rises linearly with the increase in tool radius:

Measuring tolerance =

where r = tool radius in mm

MP6510= maximum permissible error of measurement

5 mm

r • MP6510

5.4 Tool Measurement with the TT 120 Touch Probe

57HEIDENHAIN TNC 410

Page 71

Displaying the measuring results

You can display the results of tool measurement in the additional status display when your screen layout includes PGM and T PROBE STATUS (in the machine operating modes). The TNC then shows the program blocks in the left and the measuring results in the right screen window. The measuring results that exceed the permissible wear tolerance are marked in the status display with an asterisk “∗”; the results that exceed the permissible breakage tolerance are marked with the character B.

Calibrating the TT 120 touch probe

Before calibrating the touch probe, you must enter the exact length and radius of the calibrating tool into the tool table TOOL.T.

The position of the TT 120 within the machine working space must be defined by setting the machine parameters 6580.0 to 6580.2.

If you change the setting of any of the machine parameters

6580.0 to 6580.2, you must recalibrate the TT 120.

The TT 120 is calibrated automatically with the measuring cycle TCH PROBE 30. The TNC also measures the center misalignment of the calibrating tool automatically by rotating the spindle by 180° after the first half of the calibration cycle. The calibrating tool must be a precisely cylindrical part, for example a cylinder pin. The resulting calibration values are stored in the TNC memory and are accounted for during subsequent tool measurement.

ú To program the calibration cycle, press the TOUCH

PROBE key in the Programming and Editing mode of

5.4 Tool Measurement with the TT 120 Touch Probe

operation.

ú Select measuring cycle 30 TT CALIBRATE: Press

TT CALIBR. soft key

ú Clearance height: Enter the position in the spindle axis

at which there is no danger of collision with the workpiece or fixtures. The clearance height is referenced to the active workpiece datum. If you enter such a small clearance height that the tool tip would lie below the level of the probe contact, the TNC automatically positions the tool above the level of the probe contact (safety zone from MP6540)

NC sample blocks

6 TOOL CALL 1 Z 7 TCH PROBE 30.0 TT CALIBRATE 8 TCH PROBE 30.1 HEIGHT: +90

5 Programming: Tools

Page 72

Measuring the tool length

Before measuring a tool for the first time, enter the following data on the tool into the tool table TOOL.T: the approximate radius, the approximate length, the number of teeth, and the cutting direction.

The tool length is measured with the cycle TCH PROBE 31 TOOL LENGTH. Depending on the input parameters you can measure the length of a tool by one of the following methods:

■ If the tool diameter is larger than the diameter of the measuring

surface of the TT 120, you can measure the tool while it is rotating (Enter TT:R-OFFS = R in the TOOL.T).

■ If the tool diameter is smaller than the diameter of the measuring

surface of the TT 120, or if you are measuring the length of a drill or spherical cutter, you can measure the tool while it is at standstill (Enter TT:R-OFFS = 0 in the TOOL.T).

■ If the tool diameter is larger than the diameter of the measuring

surface of the TT 120, you can measure the individual teeth of the tool while it is at standstill.

Measuring cycle for measuring a tool during rotation

The TNC determines the longest tooth of a rotating tool by positioning the tool to be measured at an offset to the center of the touch probe system and then moving it toward the measuring surface until it contacts the surface. The offset is programmed in the tool table under Tool offset: Radius (TT: R-OFFS; preset value: R = tool radius).

Measuring cycle for measuring a tool during standstill (e.g. for drills)

The TNC positions the tool to be measured over the center of the measuring surface. It then moves the tool toward the measuring surface of the TT 120 (without rotation of the spindle) until the tool contacts the surface. To activate this function, enter zero for the Tool offset: Radius (TT: R-OFFS) in the tool table.

5.4 Tool Measurement with the TT 120 Touch Probe

Measuring cycle for measuring individual teeth

The TNC pre-positions the tool to be measured to a position at the side of the touch probe head. The distance from the tip of the tool to the upper edge of the touch probe head is defined in MP6530. You can enter an additional offset with Tool offset: Length (TT: LOFFS) in the tool table. The TNC probes the tool radially during rotation to determine the starting angle for measuring the individual teeth. It then measures the length of each tooth by changing the corresponding angle of spindle orientation. To activate this function, program TCH PROBE 31 = 1 for cutter measurement.

59HEIDENHAIN TNC 410

Page 73

5.4 Tool Measurement with the TT 120 Touch Probe

ú To program the calibration cycle, press the TOUCH

PROBE key in the Programming and Editing mode of operation.

ú Select measuring cycle 31 TT TOOL LENGTH: Press

TOOL LENGTH soft key

ú Measure tool=0 / Check tool=1: Select whether the

tool is to be measured for the first time or whether a tool that has already been measured is to be inspected. If the tool is being measured for the first time, the TNC overwrites the tool length L in the central tool file TOOL.T by the delta value DL = 0. If you wish to inspect a tool, the TNC compares the measured length with the tool length L that is stored in TOOL.T. It then calculates the positive or negative deviation from the stored value and enters it into TOOL.T as the delta value DL. The deviation can also be used for Q parameter Q115. If the delta value is greater than the permissible tool length tolerance for wear or break detection, the TNC will lock the tool (status L in TOOL.T).

ú Parameter number for result?: Parameter number in

which the TNC stores the status of the measurement:

0.0: Tool is within tolerance

1.0: Tool is worn out (LTOL exceeded)

2.0: Tool is broken (LBREAK exceeded) If you do not wish to use the result of measurement within the program, answer the dialog prompt with NO ENT.

ú Clearance height: Enter the position in the spindle axis

ú Probe the teeth? 0=No / 1=Yes:

Choose whether or not the TNC is to measure the individual teeth.

Resulting NC blocks for measuring a rotating tool for the first time and storing the status in Q1

6 TOOL CALL 12 Z 7 TCH PROBE 31.0 CAL. tool length 8 TCH PROBE 31.1 CHECK: 0 Q1 9 TCH PROBE 31.2 height: +120 10 TCH PROBE 31.3 PROBING THE TEETH:0

Resulting NC blocks for inspecting a tool and measuring the individual teeth, but not saving the status

6 TOOL CALL 12 Z 7 TCH PROBE 31.0 CAL. tool length 8 TCH PROBE 31.1 check: 1 9 TCH PROBE 31.2 height: +120 10 TCH PROBE 31.3 PROBING THE TEETH:1

5 Programming: Tools

Page 74

Measuring the tool radius

The tool radius is measured with the cycle TCH PROBE 32 TOOL RADIUS. Depending on the input parameters you can measure the radius of a tool by:

■ Measuring the tool while it is rotating

■ Measuring the tool while it is rotating and subsequently

measuring the individual teeth.

Measuring cycle

The TNC pre-positions the tool to be measured to a position at the side of the touch probe head. The distance from the tip of the milling tool to the upper edge of the touch probe head is defined in MP6530. The TNC probes the tool radially while it is rotating. If you have programmed a subsequent measurement of individual teeth, the TNC measures the radius of each tooth with the aid of oriented spindle stops.

ú To program the measuring cycle, press the TOUCH

PROBE key in the Programming and Editing mode of operation.

ú Select measuring cycle 32 TT TOOL RADIUS: Press

TOOL RADIUS soft key

ú Measure tool=0 / Check tool=1: Select whether the

tool is to be measured for the first time or whether a tool that has already been measured is to be inspected. If the tool is being measured for the first time, the TNC overwrites the tool radius R in the central tool file TOOL.T by the delta value DR = 0. If you wish to inspect a tool, the TNC compares the measured radius with the tool radius R that is stored in TOOL.T. It then calculates the positive or negative deviation from the stored value and enters it into TOOL.T as the delta value DR. The deviation can also be used for Q parameter Q116. If the delta value is greater than the permissible tool radius tolerance for wear or break detection, the TNC will lock the tool (status L in TOOL.T).

Resulting NC blocks for measuring a rotating tool for the first time and storing the status in Q1

7 TOOL CALL 12 Z 8 TCH PROBE 32.0 CAL. tool radius 9 TCH PROBE 32.1 CHECK: 0 Q1 10 TCH PROBE 32.2 height: +120 11 TCH PROBE 32.3 PROBING THE TEETH:0

Resulting NC blocks for inspecting a tool and measuring the individual teeth, but not saving the status

7 TOOL CALL 12 Z 8 TCH PROBE 32.0 CAL. tool radius 9 TCH PROBE 32.1 check: 1 10 TCH PROBE 32.2 height: +120 11 TCH PROBE 32.3 PROBING THE TEETH:1

5.4 Tool Measurement with the TT 120 Touch Probe

61HEIDENHAIN TNC 410

Page 75

ú Parameter number for result?: Parameter number in

which the TNC stores the status of the measurement:

0.0: Tool is within tolerance

1.0: Tool is worn (RTOL exceeded)

2.0: Tool is broken (RBREAK exceeded) If you do not wish to use the result of measurement within the program, answer the dialog prompt with NO ENT.

ú Clearance height: Enter the position in the spindle axis

ú Cutter measurement 0=No / 1=Yes:

Choose whether or not the TNC is to measure the individual teeth.

5.4 Tool Measurement with the TT 120 Touch Probe

5 Programming: Tools

Page 76

Programming:

Programming Contours

Page 77

6.1 Overview of Tool Movements

Path functions

A workpiece contour is usually composed of several contour elements such as straight lines and circular arcs. With the path functions, you can program the tool movements for straight lines and circular arcs.

Free contour (FK) programming

If a production drawing is not dimensioned for NC and the dimensions given are not sufficient for creating a part program, you can program the workpiece contour with the FK free contour programming and have the TNC calculate the missing data.

With FK programming, you also program tool movements for

straight lines and circular arcs.

Miscellaneous functions M

6.1 Overview of Tool Movements

With the TNC’s miscellaneous functions you can affect

■ program run, such as a program interruption

■ machine functions, such as switching spindle rotation and coolant

supply on and off

■ contouring behavior of the tool.

R40

Subprograms and program section repeats

If a machining sequence occurs several times in a program, you can save time and reduce the chance of programming errors by entering the sequence once and then defining it as a subprogram or program section repeat. If you wish to execute a specific program section only under certain conditions, you also define this machining sequence as a subprogram. In addition, you can have a part program call a separate program for execution.

How subprograms and program section repeats are used in programming is described in Chapter 9.

Programming with Q parameters

Instead of programming numerical values in a part program, you enter markers called Q parameters. You assign the values to the Q parameters separately with the Q parameter functions. You can use the Q parameters for programming mathematical functions that control program execution or describe a contour.

In addition, parametric programming enables you to measure with the 3-D touch probe during program run.

Programming with Q parameter is described in Chapter 10.

11510

6 Programming: Programming Contours

Page 78

6.2 Fundamentals of Path Functions

Programming tool movements for workpiece machining

You create a part program by programming the path functions for the individual contour elements in sequence. You usually do this by entering the coordinates of the end points of the contour elements given in the production drawing. The TNC calculates the actual path of the tool from these coordinates, and from the tool data and radius compensation.

The TNC moves all axes programmed in a single block simultaneously.

Movement parallel to the machine axes

The program block contains only one coordinate. The TNC thus moves the tool parallel to the programmed axis.

Depending on the individual machine tool, the part program is executed by movement of either the tool or the machine table on which the workpiece is clamped. Nevertheless, you always program path contours as if the tool moves and the workpiece remains stationary.

Example:

L X+100

The tool retains the Y and Z coordinates and moves to the position X=100. See figure at upper right.

Movement in the main planes

The program block contains two coordinates. The TNC thus moves the tool in the programmed plane.

Example:

L X+70 Y+50

Path function for “straight line” Coordinate of the end point

100

6.2 Fundamentals of Path Functions

The tool retains the Z coordinate and moves in the X/Y plane to the position X=70, Y=50. See figure at center right.

Three-dimensional movement

The program block contains three coordinates. The TNC thus moves the tool in space to the programmed position.

Example:

L X+80 Y+0 Z-10

This example is illustrated in the figure at lower right.

-10

65HEIDENHAIN TNC 410

Page 79

Circles and circular arcs

The TNC moves two axes simultaneously in a circular path relative to the workpiece. You can define a circular movement by entering the circle center CC.

When you program a circle, the TNC assigns it to one of the main planes. This plane is defined automatically when you set the spindle axis during a tool call:

Spindle axis Main plane ZXY, also

UV, XV, UY

YZX, also

WU, ZU, WX

XYZ, also

VW, YW, VZ

You can program circles that do not lie parallel to a main plane by using Q parameters (see Chapter 10).

Direction of rotation DR for circular movements

When a circular path has no tangential transition to another contour element, enter the direction of rotation DR:

6.2 Fundamentals of Path Functions

Clockwise direction of rotation: DR– Counterclockwise direction of rotation: DR+

Radius compensation

The radius compensation must be in the block in which you move to the first contour element. You cannot begin radius compensation in a circle block. It must be activated beforehand an a straight-line block or approach block (APPR block).

Pre-positioning

Before running a part program, always pre-position the tool to prevent the possibility of damaging it or the workpiece.

DR+

DR–

6 Programming: Programming Contours

Page 80

Creating the program blocks with the path function keys

The gray path function keys initiate the plain language dialog. The TNC asks you successively for all the necessary information and inserts the program block into the part program.

Example — programming a straight line:

Initiate the programming dialog (here, for a straight line).

Coordinates ?

Radius comp.: RL/RR/no comp. ?

Feed rate ? F=

100

Enter the feed rate (here, 100 mm/min), and

Enter the coordinates of the straight-line end point.

Select the radius compensation (here, press the RL soft key — the tool moves to the left of the programmed contour).

confirm your entry with ENT.

6.2 Fundamentals of Path Functions

Miscellaneous function M ?

The part program now contains the following line:

L X+10 Y+5 RL F100 M3

Enter a miscellaneous function (here, M3), and terminate the dialog with END.

Enter a miscellaneous function with parameter: e.g. press the soft key M120 and enter the requested parameter.

67HEIDENHAIN TNC 410

Page 81

6.3 Contour Approach and Departure

Overview: Types of paths for contour approach and departure

The functions for contour approach and departure are activated with the APPR/DEP key. You can then select the desired path function with the corresponding soft key:

Function Soft keys: Approach Departure

Straight line with tangential connection

Straight line perpendicular to a contour point

Circular arc with tangential connection

Circular arc with tangential connection to the contour. Approach and departure to an auxiliary point outside of the contour on a tangentially connecting line.

6.3 Contour Approach and Departure

Approaching and departing a helix

The tool approaches and departs a helix on its extension by moving in a circular arc that connects tangentially to the contour. You program helix approach and departure with the APPR CT and DEP CT functions.

Important positions for approach and departure

■ Starting point P

You program this position in the block before the APPR block. P lies outside the contour and is approached without radius compensation (R0).

■ Auxiliary point P

Some of the paths for approach and departure go through an auxiliary point P APPR or DEP block.

■ First contour point P

You program the first contour point PA in the APPR block. The last contour point P

■ If the APPR block also contains a Z axis coordinate, the TNC will

first move the tool to P the entered depth in the tool axis.

■ End point P

The position PN lies outside of the contour and results from your input in the DEP block. If the DEP block also contains a Z axis coordinate, the TNC will first move the tool to P plane, and then move it to the entered depth in the tool axis.

that the TNC calculates from your input in the

and last contour point P

can be programmed with any path function.

in the working plane, and then move it to

in the working

6 Programming: Programming Contours

Page 82

You can enter the position data in absolute or incremental coordinates and in Cartesian or polar coordinates.

The TNC does not check whether the programmed contour will be damaged when moving from the actual position to the auxiliary point P

. Use the test graphics to simulate approach and departure

before executing the part program. When approaching the contour, allow sufficient distance between

the starting point P

and the first contour point PA to assure that the

TNC will reach the programmed feed rate for machining. The TNC moves the tool from the actual position to the auxiliary

point P

at the feed rate that was last programmed.

Radius compensation

For the TNC to interpret an APPR block as an approach block you must program a change in compensation from R0 to RL/RR. The TNC automatically cancels the radius compensation in a DEP block. If you wish to program a contour element with the DEP block (no change in compensation), then you need to program the active radius compensation again (2nd soft-key row, if the F element is highlighted).

If no change in compensation is programmed in an APPR or in a DEP block, the TNC makes the contour connection as follows:

Function Contour connection

APPR LT Tangential connection to the following

contour element

APPR LN Perpendicular connection to the following

contour element

APPR CT without angle of traverse/without radius:

Tangentially connecting circular arc between the preceding and the following contour element.

without angle of traverse/with radius:

Tangentially connecting circular arc with programmed radius to the following contour element

with angle of traverse/without radius:

Tangentially connecting circular are with angle of traverse to the following contour element

with angle of traverse/with radius:

Tangentially connecting circular arc with connecting line and angle of traverse to the following contour element

APPR LCT Tangent with connecting tangential

circular arc to the following contour element

Abbreviation Meaning

APPR Approach DEP Departure L Line C Circle T Tangential

(smooth connection)

N Normal (perpendicular)

Function Contour connection

DEP LT Tangential connection to the

preceding contour element

DEP LN Perpendicular connection to the

preceding contour element

DEP CT without angle of traverse/without radius:

Tangentially connecting circular arc between the preceding and the following contour element

without angle of traverse/with radius:

Tangentially connecting circular arc with programmed radius to the preceding contour element

with angle of traverse/without radius:

Tangentially connecting circular arc with angle of traverse to the preceding contour element

with angle of traverse/with radius:

Tangentially connecting circular arc with connecting line and angle of traverse to the preceding contour element

DEP LCT Tangent with tangentially

connecting circular arc to the preceding contour element

6.3 Contour Approach and Departure

69HEIDENHAIN TNC 410

Page 83

Approaching on a straight line with tangential connection: APPR LT

The tool moves on a straight line from the starting point PS to an auxiliary point P on a straight line that connects tangentially to the contour. The auxiliary point P distance LEN.

ú Use any path function to approach the starting point P

Example NC blocks

7 L X+40 Y+10 R0 FMAX M3 8 APPR LT X+20 Y+20 Z-10 LEN15 RR F100 9 L X+35 Y+35

6.3 Contour Approach and Departure

10 L ...

. It then moves from PHto the first contour point P

is separated from the first contour point PA by the

ú Initiate the dialog with the APPR/DEP key and APPR LT

soft key:

ú Coordinates of the first contour point P ú LEN: Distance from the auxiliary point P

contour point P

ú Radius compensation for machining

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

The tool moves on a straight line from the starting point PS to an auxiliary point P on a straight line perpendicular to the first contour element. The auxiliary point P distance LEN plus the tool radius.

ú Use any path function to approach the starting point P ú Initiate the dialog with the APPR/DEP key and APPR LN soft key:

. It then moves from PHto the first contour point P

is separated from the first contour point PA by the

ú Coordinates of the first contour point P ú Length: Distance from the auxiliary point P

contour point P

Always enter LEN as a positive value!

ú Radius compensation RR/RL for machining

to the first

P RR

Approach PS without radius compensation PA with radius comp. RR End point of the first contour element Next contour element

Example NC blocks

7 L X+40 Y+10 R0 FMAX M3 8 APPR LN X+10 Y+20 Z-10 LEN+15 RR F100 9 L X+20 Y+35 10 L ...

Approach PS without radius compensation PA with radius comp. RR, distance PH to PA: LEN=15 End point of the first contour element Next contour element

6 Programming: Programming Contours

Page 84

Approaching on a circular arc with tangential connection: APPR CT

The tool moves on a straight line from the starting point PS to an auxiliary point P following a circular arc that is tangential to the first contour element.

The arc from P center angle CCA. The direction of rotation of the circular arc is automatically derived from the tool path for the first contour element.

ú Use any path function to approach the starting point P ú Initiate the dialog with the APPR/DEP key and APPR CT soft key:

Example NC blocks

7 L X+40 Y+10 R0 FMAX M3 8 APPR CT X+10 Y+20 Z-10 CCA180 R+10 RR F100 9 L X+20 Y+35 10 L ...

. It then moves from PH to the first contour point P

to PA is determined through the radius R and the

ú Coordinates of the first contour point P ú Center angle CCA of the arc

■ CCA can be entered only as a positive value.

■ Maximum input value 360°

ú Radius R of the circular arc

■ If the tool should approach the workpiece in the

direction defined by the radius compensation: Enter R as a positive value.

■ If the tool should approach the workpiece opposite to

the radius compensation: Enter R as a negative value.

ú Radius compensation RR/RL for machining

CCA= 180°

R10

Approach PS without radius compensation PA with radius comp. RR, Radius R=10 End point of the first contour element Next contour element

4010

6.3 Contour Approach and Departure

71HEIDENHAIN TNC 410

Page 85

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

The tool moves on a straight line from the starting point PS to an auxiliary point P on a circular arc.

The arc is connected tangentially both to the line P to the first contour element. Once these lines are known, the radius then suffices to completely define the tool path.

ú Use any path function to approach the starting point P ú Initiate the dialog with the APPR/DEP key and APPR LCT soft key:

Example NC blocks

7 L X+40 Y+10 R0 FMAX M3 8 APPR LCT X+10 Y+20 Z-10 R10 RR F100

6.3 Contour Approach and Departure

9 L X+20 Y+35 10 L ...

. It then moves from PH to the first contour point P

– PH as well as

ú Coordinates of the first contour point P ú Radius R of the arc

Always enter R as a positive value.

ú Radius compensation for machining

Approach PS without radius compensation PA with radius compensation RR, radius R=10 End point of the first contour element Next contour element

P RR

R10

4010

6 Programming: Programming Contours

Page 86

Departing tangentially on a straight line: DEP LT

The tool moves on a straight line from the last contour point PE to the end point P element. P

ú Program the last contour element with the end point P

radius compensation.

ú Initiate the dialog with the APPR/DEP key and DEP LT soft key:

Example NC blocks

23 L Y+20 RR F100 24 DEP LT LEN12.5 F100 25 L Z+100 FMAX M2

. The line lies in the extension of the last contour

is separated from PE by the distance LEN.

and

ú LEN: Enter the distance from the last contour element

to the end point PN.

12.5

P R0

Last contour element: PE with radius compensation Depart contour by LEN = 12.5 mm Retract in Z, return to block 1, end program

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

The tool moves on a straight line from the last contour point PE to the end point P last contour point P plus the tool radius.

ú Program the last contour element with the end point P

radius compensation.

ú Initiate the dialog with the APPR/DEP key and DEP LN soft key:

Example NC blocks

23 L Y+20 RR F100 24 DEP LN LEN+20 F100 25 L Z+100 FMAX M2

. The line departs on a perpendicular path from the

. PN is separated from PE by the distance LEN

and

ú LEN: Enter the distance from the last contour element

to the end point PN.

Important: Always enter LEN as a positive value!

Last contour element: PE with radius compensation Depart perpendicular to contour by LEN = 20 mm Retract in Z, return to block 1, end program

6.3 Contour Approach and Departure

73HEIDENHAIN TNC 410

Page 87

Departing tangentially on a circular arc: DEP CT

The tool moves on a circular arc from the last contour point PE to the end point P contour element.

ú Program the last contour element with the end point P

radius compensation.

ú Initiate the dialog with the APPR/DEP key and DEP CT soft key:

Example NC blocks

23 L Y+20 RR F100 24 DEP CT CCA 180 R+8 F100

6.3 Contour Approach and Departure

25 L Z+100 FMAX M2

. The arc is tangentially connected to the last

ú Center angle CCA of the arc ú Radius R of the circular arc

■ If the tool should depart the workpiece in the direction

of the radius compensation (i.e. to the right with RR or to the left with RL): Enter R as a positive value.

■ If the tool should depart the workpiece on the

direction opposite to the radius compensation: Enter R as a negative value.

and

180°

Last contour element: PE with radius compensation Center angle=180°, arc radius= 8 mm Retract in Z, return to block 1, end program

6 Programming: Programming Contours

Page 88

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

The tool moves on a circular arc from the last contour point PE to an auxiliary point P straight line. The arc is tangentially connected both to the last contour element and to the line from P known, the radius R then suffices to completely define the tool path.

ú Program the last contour element with the end point P

radius compensation.

ú Initiate the dialog with the APPR/DEP key and DEP LCT soft key:

Example NC blocks

23 L Y+20 RR F100 24 DEP LCT X+10 Y+12 R8 F100 25 L Z+100 FMAX M2

. It then moves from PH to the end point PN on a

to PN. Once these lines are

ú Enter the coordinates of the end point P ú Radius R of the arc

Always enter R as a positive value

and

P R0

Last contour element: PE with radius compensation Coordinates PN, arc radius = 8 mm Retract in Z, return to block 1, end program

6.3 Contour Approach and Departure

75HEIDENHAIN TNC 410

Page 89

6.4 Path Contours — Cartesian Coordinates

Overview of path functions

Function Path function key

Line L

CHamFer

Circle Center

Circle

Circle by Radius

Circle Tangential

6.4 Path Contours — Cartesian Coordinates

Corner RouNDing

Tool movement

Straight line

Chamfer between two straight lines

No tool movement

Circular arc around a circle center CC to an arc end point

Circular arc with a certain radius

Circular arc with tangential connection to the preceding contour element

Circular arc with tangential connection to the preceding and subsequent contour elements

Required input

Coordinates of the straight-line end point

Chamfer side length

Coordinates of the circle center or pole

Coordinates of the arc end point, direction of rotation

Coordinates of the arc end point, arc radius, direction of rotation

Coordinates of the arc end point

Rounding-off radius R

FK free contour programming

Straight line or circular path with any connection to the preceding contour element

6 Programming: Programming Contours

See section 6.6

Page 90

Straight line L

The TNC moves the tool in a straight line from its current position to the straight-line end point. The starting point for the straight line is the end point that was programmed in the preceding block.

ú Enter the coordinates of the end point for the line.

Further entries, if necessary:

ú Radius compensation RL/RR/R0 ú Feed rate F ú Miscellaneous function M

Example NC blocks

7 L X+10 Y+40 RL F200 M3 8 L IX+20 IY-15 9 L X+60 IY-10

Actual position capture

In a positioning block you can capture the coordinates of the current tool position:

ú Select the Programming and Editing mode of operation. ú Open a new block or move the highlight to a coordinate within an

existing block.

ú Press the actual-position-capture key: The TNC stores

the coordinates of the highlighted axis.

6.4 Path Contours — Cartesian Coordinates

Inserting a chamfer CHF between two straight lines

The chamfer enables you to cut off corners at the intersection of two straight lines.

■ The blocks before and after the CHF block must be in the same

working plane.

■ The radius compensation before and after the chamfer block must

be the same.

■ An inside chamfer must be large enough to accommodate the

current tool.

ú Chamfer side length: Enter the length of the chamfer

Further entries, if necessary:

ú Feed rate F (only effective in CHF block)

Please observe the notes on the next page!

77HEIDENHAIN TNC 410

Page 91

Example NC blocks

7 L X+0 Y+30 RL F300 M3 8 L X+40 IY+5 9 CHF 12 10 L IX+5 Y+0

You cannot start a contour with a CHF block A chamfer is possible only in the working plane. The feed rate for chamferring is taken from the

preceding block. The corner point is cut off by the chamfer and is not part

of the contour.

Circle center CC

You can define a circle center CC for circles that are programmed with the C key (circular path C). This is done in the following ways:

■ Entering the Cartesian coordinates of the circle center

■ Using the circle center defined in an earlier block

■ Capturing the coordinates with the actual-position-capture key

ú Coordinates CC: Enter the circle center coordinates

If you want to use the last programmed position, do

6.4 Path Contours — Cartesian Coordinates

Example NC blocks

5 CC X+25 Y+25

10 L X+25 Y+25 11 CC

The program blocks 10 and 11 do not refer to the illustration.

not enter any coordinates.

Duration of effect

The circle center definition remains in effect until a new circle center is programmed. You can also define a circle center for the secondary axes U, V and W.

Entering the circle center CC incrementally

If you enter the circle center with incremental coordinates, you have programmed it relative to the last programmed position of the tool.

6 Programming: Programming Contours

Page 92

The only effect of CC is to define a position as a circle center — the tool does not move to the position.

The circle center also serves as the pole for polar coordinates.

Circular path C around circle center CC

Before programming a circular path C, you must first enter the circle center CC. The last programmed tool position before the C block is used as the circle starting point.

ú Move the tool to the circle starting point.

ú Enter the coordinates of the circle center.

ú Enter the coordinates of the arc end point ú Direction of rotation DR

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

Example NC blocks

5 CC X+25 Y+25 6 L X+45 Y+25 RR F200 M3 7 C X+45 Y+25 DR+

6.4 Path Contours — Cartesian Coordinates

Full circle

Enter the same point you used as the starting point for the end point in a C block.

The starting and end points of the arc must lie on the circle.

Input tolerance: up to 0.016 mm.

DR+

DR–

79HEIDENHAIN TNC 410

Page 93

Circular path CR with defined radius

The tool moves on a circular path with the radius R.

ú Enter the coordinates of the arc end point. ú Radius R

Note: The algebraic sign determines the size of the arc.

ú Direction of rotation DR

Note: The algebraic sign determines whether the arc is concave or convex.

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

Full circle

For a full circle, program two CR blocks in succession: The end point of the first semicircle is the starting point of the

second. The end point of the second semicircle is the starting point of the first. See figure at upper right.

E1=S

S1=E

Central angle CCA and arc radius R

The starting and end points on the contour can be connected with four arcs of the same radius:

Smaller arc: CCA<180° Enter the radius with a positive sign R>0

6.4 Path Contours — Cartesian Coordinates

Larger arc: CCA>180° Enter the radius with a negative sign R<0

The direction of rotation determines whether the arc is curving outward (convex) or curving inward (concave):

Convex: Direction of rotation DR– (with radius compensation RL) Concave: Direction of rotation DR+ (with radius compensation RL)

Example NC blocks

See figures at middle and lower right.

10 L X+40 Y+40 RL F200 M3 11 CR X+70 Y+40 R+20 DR (arc 1)

11 CR X+70 Y+40 R+20 DR+ (arc 2)

11 CR X+70 Y+40 R-20 DR- (arc 3)

11 CR X+70 Y+40 R-20 DR+ (arc 4)

Please observe the notes on the next page!

DR+

40 70

DR+

40 70

6 Programming: Programming Contours

Page 94

The distance from the starting and end points of the arc diameter cannot be greater than the diameter of the arc.

The maximum radius is 9999.999 mm. You can also enter rotary axes A, B and C.

Circular path CT with tangential connection

The tool moves on an arc that starts at a tangent with the previously programmed contour element.

A transition between two contour elements is called “tangential” when there is no kink or corner at the intersection between the two contours — the transition is smooth.

The contour element to which the tangential arc connects must be programmed immediately before the CT block. This requires at least two positioning blocks.

ú Enter the coordinates of the arc end point.

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

Example NC blocks

7 L X+0 Y+25 RL F300 M3 8 L X+25 Y+30 9 CT X+45 Y+20 10 L Y+0

6.4 Path Contours — Cartesian Coordinates

A tangential arc is a two-dimensional operation: the coordinates in the CT block and in the contour element preceding it must be in the same plane of the arc.

81HEIDENHAIN TNC 410

Page 95

Corner Rounding RND

The RND function is used for rounding off corners. The tool moves on an arc that is tangentially connected to both the

preceding and subsequent contour elements. The rounding arc must be large enough to accommodate the tool.

ú Rounding-off radius: Enter the radius of the arc. ú Feed rate for rounding the corner.

Example NC blocks

5 L X+10 Y+40 RL F300 M3 6 L X+40 Y+25 7 RND R5 F100 8 L X+10 Y+5

In the preceding and subsequent contour elements, both coordinates must lie in the plane of the rounding arc.

The corner point is cut off by the rounding arc and is not part of the contour.

A feed rate programmed in the RND block is effective only in that block. After the RND block, the previous feed rate becomes effective again.

6.4 Path Contours — Cartesian Coordinates

You can also use an RND block for a tangential contour approach if you do not want to use an APPR function.

6 Programming: Programming Contours

Page 96

Example: Linear movements and chamfers with Cartesian coordinates

0 BEGIN PGM LINEAR MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+10 4 TOOL CALL 1 Z S4000 5 L Z+250 R0 FMAX 6 L X-10 Y-10 R0 F MAX 7 L Z-5 R0 F1000 M3 8 APPR LT X+5 Y+5 LEN10 RL F300

9 L Y+95 10 L X+95 11 CHF 10 12 L Y+5 13 CHF 20 14 L X+5 15 DEP LT LEN10 R0 F1000 16 L Z+250 R0 FMAX M2 17 END PGM LINEAR MM

Define blank form for graphic workpiece simulation

Define tool in the program Call tool in the spindle axis and with the spindle speed S Retract tool in the spindle axis at rapid traverse FMAX Pre-position the tool Move to working depth at feed rate F = 1000 mm/min Approach the contour at point 1 on straight lines with tangential connection Move to point 2 Point 3: first straight line for corner 3 Program chamfer with length 10 mm Point 4: 2nd straight line for corner 3, 1st straight line for corner 4 Program chamfer with length 20 mm Move to last contour point 1, second straight line for corner 4 Depart the contour on a straight line with tangential connection Retract in the tool axis, end of program

6.4 Path Contours — Cartesian Coordinates

83HEIDENHAIN TNC 410

Page 97

Example: Circular movements with Cartesian coordinates

0 BEGIN PGM CIRCULAR MM

6.4 Path Contours — Cartesian Coordinates

1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+10 4 TOOL CALL 1 Z S4000 5 L Z+250 R0 FMAX 6 L X-10 Y-10 R0 F MAX 7 L Z-5 R0 F1000 M3 8 APPR LCT X+5 Y+5 R5 RL F300

9 L X+5 Y+85 10 RND R10 F150 11 L X+30 Y+85 12 CR X+70 Y+95 R+30 DR- 13 L X+95 14 L X+95 Y+40 15 CT X+40 Y+5

16 L X+5 17 DEP LCT X-20 Y-20 R5 R0 F1000 18 L Z+250 R0 FMAX M2 19 END PGM CIRCULAR MM

Define blank form for graphic workpiece simulation

Define tool in the program Call tool in the spindle axis and with the spindle speed S Retract tool in the spindle axis at rapid traverse FMAX Pre-position the tool Move to working depth at feed rate F = 1000 mm/min Approach the contour at point 1 on a circular arc with tangential connection Point 2: first straight line for corner 2 Insert radius with R = 10 mm, feed rate: 150 mm/min Move to point 3: Starting point of the arc with CR Move to point 4: End point of the arc with CR, radius 30 mm Move to point 5 Move to point 6 Move to point 7: End point of the arc, radius with tangential connection to point 6, TNC automatically calculates the radius Move to last contour point 1 Depart the contour on a circular arc with tangential connection Retract in the tool axis, end of program

R10

R30

4030 70

6 Programming: Programming Contours

Page 98

Example: Full circle with Cartesian coordinates

0 BEGIN PGM C-CC MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+12.5 4 TOOL CALL 1 Z S3150 5 CC X+50 Y+50 6 L Z+250 R0 F MAX 7 L X-40 Y+50 R0 F MAX 8 L Z-5 R0 F1000 M3 9 APPR LCT X+0 Y+50 R5 RL F300

10 C X+0 DR- 11 DEP LCT X-40 Y+50 R5 R0 F1000

12 L Z+250 R0 FMAX M2 13 END PGM CCC MM

Define the blank form

Define the tool Call the tool Define the circle center Retract the touch probe Pre-position the tool Move to working depth Approach the starting point of the circle on a circular arc with tangential connection Move to the circle end point (= circle starting point) Depart the contour on a circular arc with tangential connection Retract in the tool axis, end of program

6.4 Path Contours — Cartesian Coordinates

85HEIDENHAIN TNC 410

Page 99

6.5 Path Contours – Cartesian Coordinates

With polar coordinates you can define a position in terms of its angle PA and its distance PR relative to a previously defined pole CC. See section ”4.1 Fundamentals of NC.”

Polar coordinates are useful with:

■ Positions on circular arcs

■ Workpiece drawing dimensions in degrees, e.g. bolt hole circles

Overview of path functions with polar coordinates

Function Path function keys

Line LP

Circular arc CP +

Circular arc CTP +

6.5 Path Contours — Polar Coordinates

Helical interpolation +

Polar coordinate origin: Pole CC

You can define the pole CC anywhere in the part program before blocks containing polar coordinates. Enter the pole in Cartesian coordinates as a circle center in a CC block.

ú Coordinates CC: Enter Cartesian coordinates for the

pole, or: If you want to use the last programmed position, do

not enter any coordinates.

Tool movement

Straight line

Circular path around circle center/ pole CC to arc end point

Circular arc with tangential connection to the preceding contour element

Combination of a circular and a linear movement

Required input

Polar radius, polar angle of the straight-line end point

Polar angle of the arc end point, direction of rotation

Polar radius, polar angle of the arc end point

Polar radius, polar angle of the arc end point, coordinate of the end point in the tool axis

6 Programming: Programming Contours

Page 100

Straight line LP

The tool moves in a straight line from its current position to the straight-line end point. The starting point for the straight line is the end point that was programmed in the preceding block.

ú Polar-coordinates radius PR: Enter the distance from

the pole CC to the straight-line end point.

ú Polar-coordinates angle PA: Angular position of the

straight-line end point between –360° and +360° The sign of PA depends on the angle reference axis:

Angle from angle reference axis to PR is counterclockwise: PA>0 Angle from angle reference axis to PR is clockwise: PA<0

Example NC blocks

12 CC X+45 Y+25 13 LP PR+30 PA+0 RR F300 M3 14 LP PA+60 15 LP IPA+60 16 LP PA+180

60°

Circular path CP around pole CC

The polar coordinate radius PR is also the radius of the arc. It is defined by the distance from the starting point to the pole CC. The last programmed tool position before the CP block is the starting point of the arc.

ú Polar coordinates angle PA: Angular position of the

arc end point between –5400° and +5400°

ú Direction of rotation DR

Example NC blocks

18 CC X+25 Y+25 19 LP PR+20 PA+0 RR F250 M3 20 CP PA+180 DR+

For incremental coordinates, enter the same sign for DR and PA.

6.5 Path Contours — Polar Coordinates

R20

87HEIDENHAIN TNC 410

HEIDENHAIN TNC 410 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual