HEIDENHAIN CNC Pilot 4290 User Manual

Download

CNC PILOT 4290

NC Software 368 650-xx V7

User’s Manual

English (en)

10/2004

Data input keypad

Manual operating mode

Machine operating panel

Cycle Start

Automatic mode

Programming modes (DIN PLUS, simulation, TURN PLUS)

Organization modes (parameter, service, transfer)

Display error status

Call the info system

ESC (escape)

■ Go back by one menu level

■ Close dialog box, do not save

INS (insert)

■ Insert list element

■ Close dialog box, save data

ALT (alter)

■ Change the list element

DEL (delete)

■ Deletes the list element

■ deletes the selected character or the character to

the left of the cursor.

. . . Numbers for value input and soft-key

selection

Decimal point

Cycle Stop

Feed Stop

Spindle Stop

Spindle on – M3/M4 direction

Spindle jog – M3/M4 direction (The spindle turns until you press the key.

Manual direction keys +X/–X

Manual direction keys +Z/–Z

Manual direction keys +Y/–Y

Rapid traverse key

Slide change key

Spindle change key

Spindle speed at the programmed value

Minus as algebraic sign

”Continue key” for special functions (e.g. marking)

Arrow keys

Page forward, page backward

■ Change to previous/next screen page

■ Change to previous/next dialog box

■ Switch between input windows

Enter – Confirmation of input

Increase/decrease spindle speed by 5%

Override dial for feed rate

Touch pad with right and left mouse key

CNC PILOT 4290, Software and Functions

This manual describes functions that are available in the CNC PILOT 4290 with NC software number 368 650-xx (Release 7.0). For programming the Y-axis, please refer to the User's Manual ”CNC PILOT 4290 with Y-Axis”. It is not described in this manual.

The machine manufacturer adapts the features offered by the control to the capabilities of the specific lathe by setting machine parameters. Therefore, some of the functions described in this manual may not be among the features provided by the CNC PILOT on your machine tool.

Some of the CNC PILOT functions which are not available on every machine are:

■ Machining with the C axis

■ Machining with the Y-axis

■ Full-surface machining

■ Tool monitoring

■ Graphically supported interactive contour definition

■ Automatic or graphically supported interactive DIN PLUS program

generation

Please contact your machine manufacturer for detailed information on the features that are supported by your machine tool.

Many machine manufacturers and HEIDENHAIN offer programming courses for the CNC PILOT controls. We recommend these courses as an effective way of improving your programming skills and sharing information and ideas with other CNC PILOT users.

HEIDENHAIN also offers the PC software DataPilot 4290, which is designed for use with the CNC PILOT 4290. The DataPilot is suitable for both shop-floor programming as well as off-location program creation and testing. It is also ideal for training purposes. DataPilot can be run on WINDOWS 95, WINDOWS 98, WINDOWS ME, WINDOWS NT 4.0 or WINDOWS 2000.

Intended place of operation

The CNC PILOT 4290 complies with EN 55022, Class A, and is intended primarily for operation in industrially zoned areas.

Contents

Introduction and Fundamentals

Basics of operation

Manual Control and Automatic Modes

DIN PLUS

Graphic Simulation

TURN PLUS

Parameter

Operating Resources

Service and Diagnosis

Transfer

Tables and overviews

2 3 4 5 6 7 8 9

Contents

HEIDENHAIN CNC PILOT 4290

1 Introduction and Fundamentals..... 1

1.1 The CNC PILOT..... 2

1.2 The Operating Modes..... 5

Contents

1.3 Expansion Stages (Options)..... 6

1.4 Fundamentals..... 7

1.5 Tool Dimensions..... 10

2 Basics of Operation..... 11

2.1 User Interface..... 12

2.1.1 Screen Displays..... 12

2.1.2 Controls and Displays..... 13

2.1.3 Selection of Operating Modes..... 14

2.1.4 Selection of Functions, Data Input..... 14

2.2 The Info System..... 16

2.3 The Error System..... 17

2.3.1 Direct Error Messages..... 17

2.3.2 Error Display, PLC Display..... 17

2.4 Data Backup..... 19

2.5 Explanation of Terms..... 19

3 Manual Control and Automatic mode..... 21

3.1 Switch-On, Switch-Off, Reference Run..... 22

3.1.1 Switch-On and Traversing the Reference Marks..... 22

3.1.2 Switch-Off..... 23

3.2 Manual Operating Mode..... 24

3.2.1 Entering machine data..... 25

3.2.2 M Commands..... 25

3.2.3 Manual Turning Operations..... 26

3.2.4 Handwheel..... 26

3.2.5 Spindle and Axis Direction Keys..... 27

3.2.6 Slide/Spindle change key..... 27

3.3 Tool Lists, Tool Life Management..... 28

3.3.1 Setting Up a Tool List..... 29

3.3.2 Comparing a Tool List with an NC Program..... 31

3.3.3 Transferring the Tool List from an NC Program..... 32

3.3.4 Tool Life Management..... 33

3.4 Setup Functions..... 34

3.4.1 Defining the Tool Change Position..... 34

3.4.2 Shifting the Workpiece Datum..... 35

3.4.3 Defining the protection zone..... 36

3.4.4 Setting up the Chucking Table..... 37

3.4.5 Setting up Machine Dimensions..... 38

3.4.6 Measuring Tools..... 39

Contents

3.5 Automatic Mode of Operation..... 41

3.5.1 Program Selection..... 41

3.5.2 Defining a Start Block..... 42

3.5.3 Program Sequence Modification..... 43

3.5.4 Compensation..... 44

3.5.5 Tool Life Management..... 45

3.5.6 Inspection Mode..... 46

3.5.7 Block Display..... 48

3.5.8 Graphic Display..... 49

3.5.9 Post-Process Measuring Status Display..... 51

3.6 Machine Display..... 52

3.7 Load Monitoring..... 54

3.7.1 Reference Machining..... 54

3.7.2 Production Using Load Monitoring..... 55

3.7.3 Editing Limit Values..... 56

3.7.4 Analyzing Reference Machining..... 57

3.7.5 Machining Using Load Monitoring..... 57

3.7.6 Load Monitoring Parameters..... 58

4 DIN PLUS..... 59

4.1 DIN Programming..... 60

4.1.1 Introduction..... 60

4.1.2 DIN PLUS Screen..... 61

4.1.3 Linear and Rotary Axes..... 62

4.1.4 Units of Measurement..... 63

4.1.5 Elements of the DIN Program..... 63

4.2 Programming Notes..... 65

4.2.1 Parallel Editing..... 65

4.2.2 Address Parameters..... 65

4.2.3 Contour Programming..... 66

4.2.4 Tool Programming..... 68

4.2.5 Fixed cycles..... 69

4.2.6 NC Subprograms..... 70

4.2.7 Template Control..... 70

4.2.8 NC Program Interpretation..... 70

4.3 The DIN PLUS Editor..... 71

4.3.1 Main Menu..... 72

4.3.2 Geometry Menu..... 75

4.3.3 Machining Menu..... 76

4.3.4 Block Menu..... 77

Contents

HEIDENHAIN CNC PILOT 4290

III

4.4 Program Section Codes..... 79

Contents

4.5 Geometry Commands..... 84

4.6 Machining Commands..... 110

4.7 Turning Cycles..... 122

4.8 Thread Cycles..... 140

4.9 Drilling cycles..... 143

4.10 C-Axis Machining..... 148

4.11 Milling Cycle Group..... 152

4.12 Special functions..... 159

4.4.1 PROGRAMMKOPF [PROGRAM HEAD]..... 79

4.4.2 TURRET..... 80

4.4.3 CHUCKING EQUIPMENT..... 82

4.4.4 Contour Definition..... 82

4.4.5 BEARBEITUNG [MACHINING]..... 83

4.4.6 UNTERPROGRAMM [SUBPROGRAM]..... 83

4.5.1 Definition of Blank..... 84

4.5.2 Basic Contour Elements..... 84

4.5.3 Contour Form Elements..... 86

4.5.4 Help Commands for Contour Definition..... 92

4.5.5 Contour Position..... 95

4.5.6 Front and Rear Face Contours..... 96

4.5.7 Lateral Surface Contours..... 102

4.5.8 Circular Pattern with Circular Slots..... 108

4.6.1 Assigning the Contour to the Operation..... 110

4.6.2 Tool Positioning without Machining..... 110

4.6.3 Simple Linear and Circular Movements..... 111

4.6.4 Feed Rate and Spindle Speed..... 113

4.6.5 Cutter Radius Compensation (TRC/MCRC)..... 115

4.6.6 Zero Point Shift..... 116

4.6.7 Oversizes, Safety Clearances..... 118

4.6.8 Tools, Types of Compensation..... 120

4.7.1 Contour-Based Turning Cycles..... 122

4.7.2 Simple Turning Cycles..... 134

4.10.1 General C-Axis Functions..... 148

4.10.2 Front/Rear Face Machining..... 149

4.10.3 Lateral Surface Machining..... 150

4.12.1 Chucking Equipment in Simulation..... 159

4.12.2 Slide Synchronization..... 160

4.12.3 Spindle Synchronization, Workpiece Transfer..... 161

4.12.4 Contour Follow-Up..... 164

4.12.5 In-Process Measuring..... 165

Contents

4.12.6 Post-Process Measuring..... 166

4.12.7 Load Monitoring..... 167

4.13 Other G Functions..... 168

4.14 Data Input and Data Output..... 173

4.14.1 Input/Output of # Variables..... 173

4.14.2 Input/Output of V Variables..... 174

4.15 Programming Variables..... 175

4.15.1 # Variables..... 175

4.15.2 V Variables..... 177

4.15.3 Program Branches, Program Repeats, Conditional Block Execution..... 179

4.16 Subprograms..... 182

4.17 M Functions..... 183

4.18 Programming Notes and Examples..... 184

4.18.1 Programming Machining Cycles..... 184

4.18.2 Contour Repetitions..... 184

4.18.3 Full-Surface Machining..... 187

5 Graphic Simulation..... 195

5.1 Simulation Mode of Operation..... 196

5.1.1 Graphic Elements, Displays..... 197

5.1.2 Basics of Operation..... 200

5.2 Main Menu..... 201

5.3 Contour Simulation..... 203

5.3.1 Contour-Simulation Functions..... 203

5.3.2 Dimensioning..... 204

5.4 Machining Simulation..... 205

5.5 Motion Simulation..... 207

5.6 Zoom Function..... 208

5.7 3-D View..... 209

5.8 Checking the

5.9 Time Calculation..... 212

5.10 Synchronous Point Analysis..... 213

6 TURN PLUS..... 215

6.1 TURN PLUS Mode of Operation..... 216

6.2 Program Management..... 217

6.2.1 TURN PLUS Files..... 217

6.2.2 Program Head..... 218

6.3 Workpiece Description..... 219

6.3.1 Entering the Contour of a Blank Part..... 219

6.3.2 Input of the Finished Part Contour..... 220

6.3.3 Superimposing form elements..... 221

6.3.4 Integrating a Contour Train..... 222

Contents

HEIDENHAIN CNC PILOT 4290

Contents

6.4 Contours of Workpiece Blanks..... 228

6.5 Contour of Finished Part..... 229

6.6 C-Axis Contours..... 242

6.7 Manipulating Contours..... 256

6.8 Importing DXF Contours..... 263

6.9 Assigning attributes..... 267

6.10 User Aids..... 273

6.11 Preparing a Machining Process..... 277

6.3.5 Entering Contours Machined with the C Axis..... 223

6.3.6 Basics of Operation..... 225

6.3.7 Help Functions for Element Definition..... 226

6.5.1 Basic Contour Elements..... 229

6.5.2 Form elements..... 232

6.5.3 Overlay Elements..... 239

6.6.1 Contours on the Front and Rear Face..... 242

6.6.2 Contours of the Lateral Surface..... 249

6.7.1 Editing the Contours of a Blank Part..... 256

6.7.2 Trimming..... 256

6.7.3 Change..... 258

6.7.4 Deleting..... 259

6.7.5 Inserting..... 260

6.7.6 Transformations..... 261

6.7.7 Connect..... 262

6.7.8 Resolve..... 262

6.8.1 Fundamentals..... 263

6.8.2 Configuring the DXF Import..... 264

6.8.3 DXF-Import..... 266

6.8.4 Transferring and Organizing DXF Files..... 266

6.9.1 Attributes for Workpiece Blanks..... 267

6.9.2 Oversize..... 267

6.9.3 Feed rate/peak-to-valley height..... 267

6.9.4 Precision stop..... 268

6.9.5 Separation Points..... 268

6.9.6 Machining Attributes..... 269

6.10.1 Calculator..... 273

6.10.2 Digitizing..... 274

6.10.3 Inspector – Checking Contour Elements..... 274

6.10.4 Unresolved Contour Elements..... 275

6.10.5 Error Messages..... 276

6.11.1 Chucking a Workpiece..... 277

6.11.2 Setting Up a Tool List..... 284

Contents

6.12 Interactive Working Plan Generation (IWG)..... 286

6.12.1 Tool call..... 287

6.12.2 Cutting Data..... 288

6.12.3 Cycle specification..... 288

6.12.4 Roughing..... 289

6.12.5 Recessing..... 294

6.12.6 Drilling..... 299

6.12.7 Finishing..... 301

6.12.8 Thread Machining(G31)..... 306

6.12.9 Milling..... 307

6.12.10 Special Machining Tasks (SM)..... 309

6.13 Automatic Working Plan Generation (AWG)..... 310

6.13.1 Generating a Machining Plan..... 310

6.13.2 Machining Sequence..... 311

6.14 Control Graphics..... 321

6.15 Configuration..... 322

6.16 Machining Information..... 324

6.16.1 Tool Selection, Turret Assignment..... 324

6.16.2 Cutting Parameters..... 325

6.16.3 Coolant..... 325

6.16.4 Hollowing..... 326

6.16.5 Inside Contours..... 326

6.16.6 Drilling..... 328

6.16.7 Full-Surface Machining..... 328

6.16.9 Shaft Machining..... 330

6.17 Example..... 332

7 Parameters..... 337

7.1 Parameter Mode of Operation..... 338

7.1.1 Parameters..... 338

7.1.2 Editing Parameters..... 339

7.2 Machine Parameters..... 341

7.3 Control Parameters..... 348

7.4 Set-Up Parameters..... 355

7.5 Machining Parameters..... 357

Contents

HEIDENHAIN CNC PILOT 4290

VII

8 Operating Resources..... 371

8.1 Tool Database..... 372

8.1.1 Tool Editor..... 372

Contents

9 Service and Diagnosis..... 401

10 Transfer..... 411

11 Tables and overviews..... 425

8.1.2 Tool Types (Overview)..... 375

8.1.3 Tool Parameters..... 377

8.1.4 Multipoint Tools, Tool Life Monitoring..... 384

8.1.5 Explanation of Tool Data..... 385

8.1.6 Tool Holder, Mounting Position..... 387

8.2 Chucking Equipment Database..... 390

8.2.1 Chucking Equipment Editor..... 390

8.2.2 Chucking Equipment Data..... 392

8.3 Technology Database (Cutting Values)..... 399

9.1 Service Mode of Operation..... 402

9.2 Service Functions..... 402

9.2.1 Access Authorization..... 402

9.2.2 System Service..... 403

9.2.3 Fixed-Word Lists..... 404

9.3 Maintenance System..... 405

9.4 Diagnosis..... 408

10.1 The Transfer Mode of Operation..... 412

10.2 Transfer Systems..... 413

10.2.1 General Information..... 413

10.2.2 Configuring for Data Transfer..... 414

10.3 Data Transfer..... 417

10.3.1 Enabling, Data Types..... 417

10.3.2 Transmitting and Receiving Files..... 418

10.4 Parameters and Operating Resources..... 420

10.4.1 Converting Parameters and Operating Resources..... 420

10.4.2 Saving Parameters and Operating Resources..... 422

10.5 File Organization..... 423

11.1 Undercut and Thread Parameters..... 426

11.1.1 Undercut DIN 76, Parameters..... 426

11.1.2 Undercut DIN 509 E, Parameters..... 427

11.1.3 Undercut DIN 509 F, Parameters..... 427

11.1.4 Thread Parameters..... 428

11.1.5 Thread Pitch..... 429

11.2 Technical Information..... 433

11.3 Peripheral Interfaces..... 437

VIII

Contents

Introduction and Fundamentals

1.1 The CNC PILOT

The CNC PILOT is a contouring control designed for lathes and turning centers. In addition to turning operations, you can perform milling and drilling operations with the C-axis or the Y-axis. The CNC PILOT supports parallel machining of up to 4 workpieces in programming, testing and production. Full-surface machining is supported on lathes with:

■ Rotating gripper

■ Movable opposing spindle

■ Multiple spindles, slides and tool carriers

1.1 The CNC PILOT

The CNC PILOT controls up to 6 slides, 4 spindles and 2 C axes.

Programming

Depending on the type and complexity of the parts to be machined and your organization, you can choose the type of programming best suited to your tasks.

In TURN PLUS you describe the contour of the blank and finished part with interactive graphics. Then you call the automatic working plan generation (AWG), and the NC program will be generated fully automatically at a keystroke. Alternately, you can choose the interactive working plan generation (IWG). When using the IWG, you determine the sequence of machining and other technical details.

Every working step is shown in the control graphics and can be corrected immediately. The result of program creation with TURN PLUS is a structured DIN PLUS program.

TURN PLUS minimizes the number of entries required, but it requires that the the tool data and cutting data has already been entered.

If TURN PLUS fails to create the optimal NC program for technologically sophisticated machining operations, or if you primarily want to reduce the machining time, program the NC program in DIN PLUS.

DIN PLUS supports the separation of the geometric description from the machining of the workpiece. Powerful cycles are available for programming in DIN PLUS. The ”simple geometry programming” function calculates coordinates if the dimensions used in the drawing are not suitable for NC programs.

Alternately, you can machine your workpiece in DIN PLUS with linear and circular movements and simple turning cycles, as you are accustomed to in conventional DIN programming.

Both TURN PLUS and DIN PLUS support machining with the C-axis or Y-axis and full-surface machining.

The Graphic Simulation feature enables you to subject your NC programs to a realistic test. The CNC PILOT displays the machining of up to 4 workpieces in the working space. Workpiece blanks and finished parts, chucking equipment and tools are shown to scale.

You can program your NC programs and test them -even during machining operations- directly on the machine.

Regardless of whether you are machining a simple or complex part, producing a single part or a series of parts, or a whole batch on a turning center, the CNC PILOT always gives you optimum support.

1 Introduction and Fundamentals2

The C-axis

With a C-axis you can drill and mill a workpiece on its front, back and lateral surfaces.

During use of the C-axis, one axis interpolates linearly or circularly with the spindle in the given working plane, while the third axis interpolates linearly.

The CNC PILOT supports part program creation with the C-axis in:

■ DIN PLUS

■ TURN PLUS contour definition

■ TURN PLUS working plan generation

TheY-axis

With a Y-axis you can drill and mill a workpiece on its front, back and lateral surfaces.

During use of the Y-axis, two axes interpolate linearly or circularly in the given working plane, while the third axis interpolates linearly. This enables you to machine slots or pockets, for example, with plane floors and perpendicular edges. By defining the spindle angle, you can determine the position of the milling contour on the workpiece.

The CNC PILOT supports part program creation with the Y-axis in:

■ DIN PLUS

■ TURN PLUS contour definition

■ TURN PLUS working plan generation

1.1 The CNC PILOT

3HEIDENHAIN CNC PILOT 4290

Full-surface machining

The CNC PILOT supports full-surface machining for all common machine designs. The features include anglesynchronous part transfer with rotating spindle, traversing to a stop, controlled parting, and coordinate transformation. This ensures efficient full-surface machining and simple programming.

The CNC PILOT supports full surface machining in:

■ DIN PLUS

■ TURN PLUS contour definition

■ TURN PLUS working plan generation

1.1 The CNC PILOT

1 Introduction and Fundamentals4

1.2 The Operating Modes

The functions of the CNC PILOT are grouped into the following operating modes:

Manual operating mode

In the Manual mode you set up the machine and move the axes manually.

Automatic mode

The NC programs are run in Automatic mode. You control and monitor the machining of the workpiece.

DIN PLUS programming mode

In ”DIN PLUS,” you can create structured NC programs. You first define the geometry of the blank and finished part, and then program the individual operations.

Simulation programming mode

The Simulation mode shows a graphic representation of programmed contours, the paths of traverse and cutting operations.The working space, tools and chucking equipment are shown true to scale.

During simulation, the CNC PILOT calculates the machining and idle-machine times for every tool. For lathes with several slides, the Synchronous point analysis enables you to optimize your NC program.

TURN PLUS programming mode

In ”TURN PLUS” you describe the contour of the workpiece using interactive graphics. For Automatic Working plan Generation (AWG), you select the material and chucking equipment. The CNC PILOT will generate the NC program automatically at a keystroke. As an alternative, you can create the working plan with the aid of interactive graphics (IAG).

Parameter organization mode

The system behavior of the CNC PILOT is controlled with parameters. In this mode, you set the parameters to adapt the control to your situation.

In addition, in this mode you describe the operating resources (tools and chucking equipment) and the cutting values.

Service organization mode

In ”Service” mode, you log on for password-protected functions, select the conversational language and make the system settings. This operating mode also provides diagnostic functions for commissioning and checking the system.

Transfer organization mode

In ”Transfer” you exchange the files with other systems, organize your programs and make data backups.

The actual control is not accessible to the machinist. You should know, however, that your CNC PILOT has an integrated hard disk on which all TURN PLUS and DIN PLUS programs that you enter are stored. This allows you to save a vast number of programs.

For data exchange and data backup, you can use the Ethernet interface. Data exchange is also possible over the serial interface. (RS232).

1.2 Modes of Operation

5HEIDENHAIN CNC PILOT 4290

1.3 Expansion Stages (Options)

The machine manufacturer configures the CNC PILOT according to the capabilities of the specific lathe. The following upgrades (options) are available, which enable you to adapt the control to your specific requirements:

■ TURN PLUS

Graphically supported interactive contour definition

■ Graphic description of the workpiece for blank and finished part

■ Geometry-programming function for calculating and displaying

missing contour data

■ Simple input of standard form elements like chamfers, rounding

arcs, recesses, undercuts, threads, fits, etc.

■ Easy-to-use transformations like shifting, rotating, mirroring or

multiplying

DIN PLUS program generation with interactive graphics

■ Selection of the appropriate machining method

■ Selection of the tools and definition of the cutting data

Expansion Stages (Options)

■ Direct graphic control of machining process

■ Immediate compensation possibility

Automatic DIN PLUS program generation

■ Automatic selection of tools

■ Automatic generation of working plan

■ TURN PLUS – extension by C-axis or Y-axis

■ C-axis: representation of programmed contour in the following

views: XC plane (front/rear end) and ZC plane (unrolled surface)

■ Y-axis: representation of programmed contour in the following

views: XY plane (front/rear end) YZ plane (side view)

■ Hole and figure patterns

■ Fixed cycles

■ Interactive or automatic working plan generation – also for

machining with the C-axis or Y-axis

■ TURN PLUS – extension by opposing spindle

■ Rechucking with expert program

■ Interactive or automatic generation of working plan – also for

rechucking and 2nd setup

■ In-process measuring

■ With triggering probe

■ For measuring tools

■ For measuring workpieces

■ Post-process measuring

■ Connection of measuring system via RS-232 interface

■ Evaluation of measuring results in Automatic mode

This operating manual describes all options.The operating sequences described in this manual may therefore deviate from those on your machine whenever a certain option is not supported by your system.

Options can usually be retrofitted. Your machine manufacturer can give you more information on retrofitting.

1 Introduction and Fundamentals6

1.4 Fundamentals

Axis designations The cross slide is referred to as the X-axis and the saddle as the Z- axis.

All X-axis values that are displayed or entered are regarded as diameters. In TURN PLUS you can define whether the X-axis values are to be interpreted as diameters or radii.

Lathes with Y-axis: The Y-axis is perpendicular to the X-axis and Z-axis (Cartesian system).

When programming paths of traverse, remember to:

■ Program a positive value to depart the workpiece.

■ Program a negative value to approach the workpiece.

Coordinate system

The coordinates entered for the principal axes X, Y and Z are referenced to the workpiece zero point – exceptions to this rule will be indicated.

Angles entered for the C-axis are referenced to the ”zero point of the C-axis” (precondition: the C-axis has been configured as a principal axis).

1.4 Fundamentals

Absolute coordinates

If the coordinates of a position are referenced to the workpiece zero point, they are referred to as absolute coordinates. Each position on a workpiece is clearly defined by its absolute coordinates.

7HEIDENHAIN CNC PILOT 4290

Incremental coordinates

Incremental coordinates are always referenced to the last programmed position. They specify the distance from the last active position and the subsequent position. Each position on a workpiece is clearly defined by its incremental coordinates.

1.4 Fundamentals

Polar coordinates

Positions located on the face or lateral surface can either be entered in Cartesian coordinates or polar coordinates.

When programming with polar coordinates, a position on the workpiece is clearly defined by the entries for diameter and angle.

You can enter polar coordinates as absolute or incremental values.

Units of measurement

You can program and operate the CNC PILOT either in the metric or inch system. The units of measurement listed in the table below apply to all inputs and displays.

Measure Metric inch

Coordinates mm inch

Lengths mm inch

Angles Degrees Degrees

Spindle speed rpm rpm

Cutting speed m/min ft/min

Feed per revolution mm/rev inch/rev

Feed per minute mm/min inch/min

Acceleration m/s

ft/s

1 Introduction and Fundamentals8

Machine reference points

Machine zero point

The point of intersection of the X-axis with the Z-axis is called the machine zero point. On a lathe, the machine zero point is usually the point of intersection of the spindle axis and the spindle surface. The machine zero point is designated with the letter M.

Workpiece zero point

For machining a workpiece, it is easier to reference all input data to a zero point located on the workpiece. By programming the zero point used in the workpiece drawing, you can take the dimensions directly from the drawing, without further calculation. This point is the ”workpiece zero point.” The workpiece zero point is designated with the letter W.

Reference marks

Whether the control ”forgets” the positions of the machine axes when it is switched off depends on the position encoders used. If the positions are lost, you must pass over the fixed reference points after switching on the CNC PILOT. The system knows the distances of the reference points to the machine datum.

1.4 Fundamentals

9HEIDENHAIN CNC PILOT 4290

1.5 Tool Dimensions

The CNC PILOT requires information on the specific tools for a variety of tasks, such as calculating the cutting radius compensation or the proportioning of cuts.

Tool length

All position values that are programmed and displayed are referenced to the distance between the tool tip and workpiece zero point. Since the control only knows the absolute position of the tool carrier (slide), it needs the dimensions XE and ZE to calculate and display the position of the tool tip. For milling and drilling tools operating with the Yaxis, the CNC PILOT additionally needs the dimension in Y.

1.5 Tool Dimensions

Tool compensation

The tool tip is subjected to wear during machining processes. To compensate for this wear, the CNC PILOT uses compensation values. The system automatically adds the compensation values to the values for length.

Tooth and cutter radius compensation (TRC)

The tip of a lathe tool has a certain radius. When machining tapers, chamfers and radii, this results in inaccuracies which the CNC PILOT compensates with its cutting radius compensation function.

Programmed paths of traverse are referenced to the theoretical tool tip S. The TRC function compensates for this error by calculating a new path of traverse, the equidistant line.

Milling cutter radius compensation (MRC)

In milling operations, the outside diameter of the milling cutter determines the contour. When the MRC function is not active, the system defines the center of the cutter as reference point for the paths of traverse. The MRC function compensates for this error by calculating a new path of traverse, the equidistant line.

1 Introduction and Fundamentals10

Basics of Operation

2.1 User Interface

2.1.1 Screen Displays

1 Operating mode line

Show the status of the operating modes.

■ The active mode of operation is shown with a

dark-gray background.

■ Programming and organization modes:

– The selected mode is shown at the right of the symbol

2.1 User Interface

– Additional information such as the selected program, submode, etc. are shown below the operating mode symbol.

2 Menu bar and pull-down menus

For function selection

3 Working window

Size and content depend on the operating mode. Some programming and organization modes overlap the machine display.

4 Machine display

Current status of the machine (tool position, the cycle and spindle situation, active tool, etc.). The machine display is configurable.

5 Status line

■ Simulation, TURN PLUS: display of current

settings or information on the next operating steps

■ Other operating modes: display of the last error

message

6 Calendar date and service ”traffic light”

■ Display of date and time

■ A color background signals a error or a PLC

message

■ The ”service traffic light” shows the servicing

state of the machine (see ” system”)

7 Soft-key row

Shows the current meaning of the soft keys.

8 Vertical soft-key row

Shows the current meaning of the soft keys. For more information: see the machine manual

9.3

Maintenance

2 Basics of Operation12

2.1.2 Controls and Displays

Screen with

■ Horizontal and vertical soft keys: The meaning is

shown above or next to the soft keys Additional keys (same function as on the operating panel):

■ ESC

■ INS

Operating panel with

■ Alphanumeric keyboard with integrated

numeric keypad

■ Keys for Operating mode selection

■ Touch pad: For cursor positioning (menu or soft

key selection, selection from lists, selecting edit boxes, etc.)

Machine operating panel with

■ Operating elements for the manual and

automatic operation of the lathe (cycle keys, manual direction keys, etc.)

■ Handwheel for exact positioning in manual

operation

■ Override button for feed-rate override

Operation of the touch pad

Normally, you can use the touch pad as an alternative to the cursor keys. In the following, the keys below the touch pad are referred to as the left and right mouse keys.

The functions and operation of the touch pad are similar to the mouse operation of the Windows operating systems.

■ Single click of the left mouse key or single touch on

the touch pad:

■ The cursor is positioned in lists or input windows.

■ Menu items, soft keys or buttons are activated

■ Double-click of the left mouse key or double touch

on the touch pad: In lists, the selected element is activated (the input window is activated)

■ Single-click with the right mouse key:

■ Same function as the ESC key – prerequisite: the

ESC key is allowed in this situation (for example to go back by one menu level)

■ Same function as the left mouse key when

selection soft keys or buttons

2.1 User Interface

13HEIDENHAIN CNC PILOT 4290

2.1.3 Selection of Operating Modes

You can switch the operating mode at any time. After the change, the new mode starts in the function in which it was last exited.

In the programming and organization modes a difference is made between the following situations:

■ No operating mode is selected (no entry next to the operating mode

symbol): Select the desired mode from the menu.

■ Operating mode selected (indicated next to the operating mode

symbol): The functions of this operating mode are available. Within

2.1 User Interface

the programming or organization modes, you can switch the modes by soft key or by repeatedly pressing the corresponding mode key.

2.1.4 Selection of Functions, Data Input

Menu bar and pull-down menu

The individual menu items are preceded by a 9-field symbol with one field highlighted. This field represents the field on the numeric keypad. Press the key whose position corresponds to the position of the highlighted field.

The function selection begins in the menu row, then goes to the pulldown menus. In the pull-down menu, press again the numeric key assigned to the menu item – or alternatively, select the menu item with touch pad or with the ”page up/page down” keys and press Enter.

Soft-key row

The meaning of the soft keys is dependent on the current operating situation.

Some soft keys work like ”toggle switches”. A function is active when the associated field in the function-key row is highlighted in color. The setting remains in effect until the function is switched off.

Keys for operating mode selection:

Manual operating mode

Automatic operating mode

Programming modes

Organization modes

List Operations

DIN PLUS programs, tool lists, parameter lists, etc. are displayed as lists. You can scroll through a list with the touch pad or arrow keys to check data, to select the position where you wish to enter data, or to highlight items for operations like deleting, copying, editing, etc.

After having selected the desired list position or a list item, press the ENTER, INS, ALT or DEL key to execute the operation.

Continued

2 Basics of Operation14

Data Input

Data are entered and edited in input windows. An input window consists of severalinput fields. You position the cursor with the touch pad or with the page up/page down keys to the input box.

Once the cursor is located in the box, you can enter your data. Existing data are overwritten. With the right/left arrow keys you can place the cursor on a position within the input box in order to delete or add characters. The up/down arrow keys or Enter confirm and terminate the entry.

Some dialogs have more input fields than a window can show. In these cases, more than one input window appears on the screen, one superimposed on the other. You will recognize this through the window number in the top line. To toggle between input windows, use the Page Up/Page Dn keys.

By pressing the ”OK” button, you confirm the data entered or edited. Independent of the position of the cursor, you can press the INS key as an alternative. If you leave the input window by pressing the ”Cancel” button or the ESC key, entries or changes will be lost.

If the dialog consists of more than one input window, you already confirm the data when pressing the PageUp/PageDn key.

Buttons

The CNC PILOT allows you to choose various options via different buttons such as the ”OK” and ”Cancel” buttons for terminating a dialog box or the buttons contained in the ”Extended inputs” window.

Select the required button and press ENTER.

Note: Instead of selecting the ”OK” or ”Cancel” button, you can press the INS or ESC key.

2.1 User Interface

15HEIDENHAIN CNC PILOT 4290

2.2 The Info System

The info system calls excerpts from the User's Manual to the screen. The system is structured in info topics comparable to the chapters of a book. In the top line of the information window, the topic you selected and the page number are shown.

The info system gives you information on the current operating situation (context-sensitive help). Also, you can select the info topics through the table of contents or the subject index. Simply select the desired topic or word and click ”Topic select” (or

2.2 The Info System

Enter).

Cross references in the text are highlighted. Place the cursor on the desired cross reference and call the topic with ”Topic select.” ”Topic return” switches back to the previous topic.

Error display

When an error message occurs, press the info key, or place the cursor on the error message in the ”display of errors” and then press the info key, to get further information on the respective error.

Call the info system

End the info system

Soft keys

Calls the

■ Selected cross reference

■ Topic from the table of contents

■ Topic from the subject index

Returns to the most recent info topic

Calls the table of contents with the overview of info topics. The table of contents is arranged in several levels.

Calls the subject index

Switches to the previous topic.

Switches to the next topic.

(or page up key) previous info page

(or page down key) next info page

2 Basics of Operation16

2.3 The Error System

2.3.1 Direct Error Messages

Direct error messages appear whenever immediate error correction is possible. Confirm the message by pressing ENTER and correct the error. Example: The input value of the parameter is out of range.

Information of the error message:

■ Error description: Explains the error

■ Error number: For service inquiries

■ Time of day When the error occurred (for your

information).

Symbols

Warning

The program run/operation continues. The CNC PILOT indicates the problem.

Error

The program run/operation is stopped. Yo u must correct the error before you can continue the current job.

2.3.2 Error Display, PLC Display

Error Display

If during the system start or during program run or other operation an error occurs, it is indicated in the date box, displayed in the status line, and saved in the error display.

The date and time remain highlighted in red until all of the errors have been canceled.

Notes on using TURN PLUS:

Opens the ”error display”

2.3 The Error System

Further information on the error marked with the cursor

Exits the error display

Deletes the error message marked with the cursor

Deletes all error messages.

Continued

17HEIDENHAIN CNC PILOT 4290

Information of the error message:

■ Error description: Explains the error

■ Error number: For service inquiries

■ Channel number: Slide for which the error

occurred.

■ Time of day When the error occurred (for your

information).

■ Error class (only with errors):

■ Background: The message serves for

information only, or it is a minor error.

■ Cancel: The running process (cycle run, traverse

command, etc.) was aborted. You can resume

2.3 The Error System

operation once the error has been cleared.

■ Emergency stop: Traverse and the execution of

the DIN program were stopped. You can resume operation once the error has been cleared.

■ Reset: Traverse and the execution of the DIN pro-

gram were stopped. Switch off the control for a moment, then restart. Contact your machine manufacturer if the error occurs again.

System Error, Internal Error

If a system error or internal error occurs, write down all information on the displayed message and inform your machine manufacturer. You cannot correct an internal error. Switch off the control and restart.

Warnings during Simulation

In the event of problems during simulation of an NC program, the CNC PILOT displays a warning in the

5.1.2

status line (see ”

Notes on Operation”).

PLC display

The PLC window is used for PLC messages and the PLC diagnosis. Your machine manual provides more detailed information on the PLC window.

To call the PLC window, open the error window with the Error status key and then press ”PLC Diagnosis” soft key.

To exit the PLC status display, press the ESC key; to switch to the error window, use the ”CNC Diagnosis” soft key.

Soft keys

Switch to PLC display

Deletes all error messages

Return to error display

2 Basics of Operation18

2.4 Data Backup

The CNC PILOT stores NC programs, operating-resource data and parameters on the hard disk. Since the possibility of damage to the hard disk due to excessive vibration or shock cannot be eliminated, HEIDENHAIN recommends making regular backup copies of your programs, operating resource data and parameters on a PC.

You can use DataPilot 4290, the WINDOWS ”Explorer” or other suitable programs for backing up your data on a PC.

For data exchange and data backup, you can use the Ethernet

interface. Data exchange is also possible over the serial interface (RS-232) (see ”

10.2

Data Transfer Methods”).

2.5 Explanation of Terms

■ Cursor: In lists, or during data input, a list item, an input box or a

character is highlighted. This ”highlight” is called a cursor.

■ Arrow keys: The cursor is moved with the ”page up/page down”

arrow keys or the touch pad.

■ Navigate: You can move the cursor within a list or an input box to

any position you would like to check, change, delete or add to. In other words, you ”navigate” through the list.

■ Active/inactive functions, menu items: Functions or soft keys

that currently unavailable are shown dimmed.

■ Dialog box: Dialog boxes are also called input windows.

■ Editing: ”Editing” is changing, deleting and adding to parameters,

commands, etc., within programs, tool data or parameters.

■ Default value: If the parameters of DIN commands or other

parameters are preassigned values, these values are referred to as ”default values.”

■ Bytes: The capacity of a storage disk is indicated in ”bytes.” Since

the CNC features a hard disk, the individual program lengths (file sizes) are expressed in bytes.

■ Extension: File names consist of the actual file name and the ”file

name extension.” The name part and the extension part are separated by ”.”.The extension indicates the type of file. Examples:

■ ”*.NC” DIN programs

■ ”*.NCS” DIN subprograms

■ ”*.MAS” Machine parameters

2.4 Data Backup; 2.5 Explanation of Terms

19HEIDENHAIN CNC PILOT 4290

Manual Control and Automatic mode

HEIDENHAIN CNC PILOT 4290

3.1 Switch-On, Switch-Off, Reference Run

3.1.1 Switch-On and Traversing the Reference Marks

In the screen dialog line, the CNC PILOT shows you step by step how to proceed when starting the system. The the CNC PILOT asks you to select an operating mode.

Whether the reference run is necessary depends on the encoders installed in your machine:

■ EnDat encoder: Reference run is not necessary

■ Distance-coded encoders: The position of the axes

is ascertained after a short reference run

■ Standard encoder: The axes move to familiar,

machine-based points

”Reference automatic” means that all axes make reference runs. ”Reference jog” only one axis does.

Reference automatic (all axes)

Select ”Ref – Reference automatic.”

3.1 Switch-On, Switch-Off, Reference Run

”Status of reference run approach” informs you of the current status. Axes that have not been referenced are shown in gray.

Either set the slides that need to find a reference or set ”All slides” (”reference automatic” dialog box)

The axis move to find the reference

Interrupts the reference run. Cycle start resumes the run.

Cancels the reference run

After completion of the reference run:

■ The position display is activated.

■ The automatic mode is selectable.

■ The Sequence, in which the axis make their reference

run is defined in machine parameters 203, 253, .. .

■ Exiting the ”Reference automatic” dialog box: Press

Cycle stop

The software limit switches are active only after you have traversed the reference marks.

Monitoring the EnDat encoders

If your machine is equipped with EnDat encoders, the control saves the axis positions during switch-off. During switch-on, the CNC PILOT compares for each axis the position during switch-on with the position saved during switch-off.

If there is a difference, one of the following messages appears:

■ ”Axis was moved after the machine was switched off.”

Check the current position and confirm it if the axis was in fact moved.

■ ”Saved encoder position of the axis is invalid”

This message is correct if the control has been switched on for the first time, or if the encoder or other control components involved were exchanged.

■ ”Parameters were changed. Saved encoder position of the axis is

invalid.” This message is correct if configuration parameters were changed.

The cause for one of the messages listed above could be a defect in the encoder or in the control. Please contact your machine supplier if the problem recurs.

3 Manual Control and Automatic mode22

Reference jog (single axis)

Select ”Ref – Reference jog.”

”Status of reference run approach” informs you of the current status. Axes that have not been referenced are shown in gray.

Set slides and axes (”reference jog” dialog box)

The reference run is continued as long as you keep pressing the key. To interrupt the reference run, release the key.

Cancels the reference run

After completion of the reference run:

■ The position display is active for the axis that has

been referenced.

■ If all axes have been referenced, you can select

automatic mode.

Exiting the ”Reference jog” dialog box: Press cycle stop

The software limit switches are only active after you have traversed the reference marks.

3.1 Switch-On, Switch-Off, Reference Run

3.1.2 Switch-Off

Switching off the CNC PILOT. Confirm the subsequent request with OK. The control is shut down in an orderly manner. After a few seconds, CNC PILOT requests you to switch off the machine.

”Shutdown” is available in the programming and organization modes if no operating mode is selected.

Proper switch-off is recorded in the error log file.

HEIDENHAIN CNC PILOT 4290

3.2 Manual Operating Mode

The Manual control mode offers various functions for setting up the machine, for measuring tool dimensions and for manually machining workpieces.

The machine display in the lower section of the screen shows the tool position and further machine data.

Options of operation:

■ Manual mode of operation

With the ”machine keys” and the handwheel, you can control the spindle and move the axes to machine the workpiece.

■ Setting up the machine

Functions for entering the tools being used, setting the workpiece zero point, the tool change position, the protective-zone dimensions, etc.

■ Measuring tool dimensions

Functions for measuring the tool by touching the workpiece or by use of measuring devices.

■ Configuring the screen display

3.2 Manual Control Operating Mode

The CNC PILOT supports various types of machine display.

In Automatic mode, the data are entered and displayed in 1 millimeters or in inches, depending on the setting of the control parameter 1.

Remember: If the machine has not been

referenced:

■ The position display is not valid

■ The software limit switches are

nonoperational.

Soft keys

■ Assigns a handwheel to an axis

■ Defines the handwheel interpolation factor

Switches the machine display

Turret one position backward

Turret one position forward

3 Manual Control and Automatic mode24

3.2.1 Entering machine data

”F” (feed rate) pull-down menu:

■ Feed per revolution

Select ”Feed per revolut.” Enter the feed rate in mm/rev (or inches/rev)

■ Feed per minute

Select ”Feed per minute.” Enter the feed rate in mm/min (or inches/min) and

press OK.

”S” (spindle speed) pull-down menu:

■ Spindle speed

Select ”Speed S.” Enter the speed in rpm

■ Constant cutting speed

Select ”V constant.” Enter the cutting speed in m/min (or ft/min) and

press OK.

■ Spindle point stop

To switch to the required spindle, press the

Spindle change key.

Select ”Spindle point stop.” Enter position Cycle start: The spindle is positioned

Cycle stop: Exit the dialog box

Menu item ”T” (Tool):

Select ”T” Enter the turret position

You can enter a constant cutting speed only for slides with an X axis.

3.2 Manual Control Operating Mode

Tool change functions:

■ Moving the tool into position

■ Offsetting ”new” tool dimensions

■ Showing the ”new” actual values in the position display.

3.2.2 M Commands

”M” (M functions) pull-down menu:

■ The M number is known: Select ”M direct” and

enter the number.

■ M menu: To select the M function, use the menu.

After input/selection of the M function:

Cycle start: The M function is executed

Cycle stop: Exit the dialog box

The content of the M menu depends on the machine. Yours may differ from the example shown here.

HEIDENHAIN CNC PILOT 4290

3.2.3 ManualTurning Operations

”Manual” pull-down menu:

Simple longitudinal and transverse turning operations

Select ”Constant feed.” Select the direction of feed (”Constant feed”

dialog box).

Control the feed rate with the cycle keys.

G functions

Select ”G function.” Enter the G number and the function parameter;

press OK.

The G function is executed.

The following G functions are permitted:

■ G30 – Rear-face machining

■ G710 – Adding tool dimensions

■ G720 – Spindle synchronization

■ G602..G699 – PLC functions

Manual NC programs

Depending on the configuration of a lathe, the machine manufacturer can includes NC programs

3.2 Manual Control Operating Mode

supporting the machinist in manually operating the lathe (Example: Switching to rear-face machining). Refer to the machine manual.

With constant speed, a feed rate per revolution must be defined.

3.2.4 Handwheel

Assign the handwheel to one of the principle axes or the C axis, and enter the feed rate or angle of rotation per handwheel increment (”Handwheel axes” dialog box).

The handwheel assignment and speed ratio are shown in the machine display (the axis letter and the decimal place of the handwheel traverse ratio are marked).

The cancel the handwheel assignment, press the ”Handwheel” soft key with opened dialog box.

The handwheel assignment is canceled by:

■ Switching to another slide.

■ Changing the operating mode.

■ Pressing an axis direction key.

■ Selecting the handwheel assignment again.

3 Manual Control and Automatic mode26

3.2.5 Spindle and Axis Direction Keys

The keys of the machine operating panel are used for machining a workpiece manually and for special functions such as positioning or determining compensation values (actual position capture, scratching, etc.).

To activate tools, define the spindle speed and feed rate, etc., use the menus.

To move the slide diagonally, press the X and Z-axis direction keys simultaneously.

Spindle keys

Switch the spindle on in M3/M4 direction.

Jog the spindle in M3/M4 direction. The spindle rotates as long as the key is held. Jog speed: machine parameters 805, 855, ...

Spindle stop

Axis direction keys (jog keys)

Move slide in X direction.

Move slide in Z direction.

Move slide in Y direction.

3.2.6 Slide/Spindle change key

■ On lathes with more than one slide, the axis

direction keys control the selected slide.

■Selection of the slide: Slide change key

■ Display of the selected slide: Machine display

■ On lathes with more than one spindle, the spindle

keys on the selected spindle.

■ Select the spindle: Spindle change key

■ Display of the selected spindle: Machine display.

■ For setup functions referring to one slide or spindle

(workpiece zero point, tool change point, etc.), you specify the slide/spindle with the slide/spindle change key.

■ The machine display usually contains display

elements for spindle and slide. To switch between these elements, use the Slide/Spindle change key

3.6

(see

”Machine Display”).

To move the slide in rapid traverse: Simultaneously press the rapid traverse key and the axis direction key. Rapid traverse velocity: Machine parameters 204, 254, ...

Slide/Spindle change key

Switch over to the next slide

Switch over to the next spindle

3.2 Manual Control Operating Mode

HEIDENHAIN CNC PILOT 4290

3.3 Tool Lists, Tool Life Management

The tool list (turret table) indicates the current tool carrier assignment. To compile a tool list, enter the ID numbers of the tools.

You can use the entries in the TURRET section of the NC program to set up the tool list. The ”Compare list” and ”Accept list” functions refer to the NC program last interpreted in automatic mode.

Tool life data

Apart from ID numbers and tool type descriptions, the tool list includes data for tool life management:

■ Status

Shows the remaining tool life/quantity.

■ Ready for use

When the tool life has expired/the defined number of parts has been produced, the tool is ”not ready for use” any longer.

■ Atw (replacement tool)

If a tool is ”not ready for use,” a replacement tool is

3.3 Tool Lists, Tool Life Management

inserted.

Simple tools

With the setup functions, you can only enter tools registered in the database. If the NC program uses ”simple tools,” proceed as follows:: Run an interpretation of the NC program; the CNC PILOT automatically updates the tool list.h

If the positions in the tool list are occupied by ”old”

tools, the confirmation request - ”Update tool list?”

- appears. The tools are only entered after you have confirmed the request.

Tools that are not registered in the database are identified by the code ”_AUTO_xx” (xx: T number), and not by an ID number.

■ The parameters of simple tools are defined in the NC

program

■ The tool life data are evaluation only if the tool life

management is active.

Danger of collision

■ Compare the tool list with the current tool carrier

assignment and check the tool data before running a program.

■ The tool list and the dimensions of the tools entered

must correspond to the actual facts, because the CNC PILOT uses the data for slide movements, protective-zone monitoring, etc.

3 Manual Control and Automatic mode28

3.3.1 Setting Up a Tool List

A tool list can also be set up without using an NC program.

Enter a new tool

Select ”Setting up - Tool list - Compile list”

Select the tool location

ENTER (or INS key) – opens the setup dialog box

Enter the ID number

Take the tool from the database

Enter the tool type – the CNC PILOT displays all tools of this type mask

Enter the ID number – the CNC PILOT displays all the tools of this ID mask

Select the tool

Take the tool from the database

3.3 Tool Lists, Tool Life Data

Soft keys

Delete tool

Take the tool from the ”ID number clipboard”

Delete the tool and place in the ”ID number clipboard”

Exit the tool database

Delete the tool

Select ”Setting up - Tool list - Compile list”

Select the tool location

or the DEL key deletes the tool

HEIDENHAIN CNC PILOT 4290

Edit the tool parameters

Entries in the tool database - sorted by tool typep

Entries in the tool database - sorted by tool ID number

Continued

Changing the tool pocket

Select ”Setting up - Tool list - Compile list”

Select tool location

Deletes the tool and saves it in the ”ID number clipboard”

Select a new tool location

Take the tool from the ”ID number clipboard”

3.3 Tool Lists, Tool Life Data

If the location was occupied, the previous tool is taken into the clipboard.

3 Manual Control and Automatic mode30

3.3.2 Comparing a Tool List with an NC Program

The CNC PILOT compares the current tool list with the entries in the NC program last translated in automatic mode.

Comparing a tool list

Select ”Setting up - Tool list - Compare list” The CNC PILOT shows the current contents of the tool list and marks deviations from the programmed tool list.

Select marked tool location

Nominal-actual comparison

Press ENTER (or INS key). The CNC PILOT opens the ”nominal-actual comparison” dialog box.

Accept the ID number of the ”nominal tool” in the tool list or

Look for the tool in the database

3.3 Tool Lists, Tool Life Data

Soft keys

Delete the tool

Take the tool from the ”ID number clipboard”

The CNC PILOT shows the following tools marked:

■ Actual tool ≠ nominal tool

■ Actual – not occupied; nominal – occupied

The entries in the TURRET section are considered nominal tools (reference:TURRET section of the NC program most recently interpreted in Automatic mode).

Tool locations that are not assigned in the NC program cannot be selected.

Danger of collision

■ Tool pockets that are occupied but,

according to the NC program, are not needed, are not marked.

■ The CNC PILOT compensates the tool

actually entered – even if it does not match the nominal assignment.

HEIDENHAIN CNC PILOT 4290

Delete the tool and place in the ”ID number clipboard”

Edit the tool parameters

Entries in the tool database - sorted by tool typep

Entries in the tool database - sorted by tool ID numberr

Accept the ID number of the ”nominal tool” in the tool list

3.3.3 Transferring theTool List from an NC Program

The CNC PILOT transfers the new tool assignment from the TURRET section (reference: the NC program last interpreted in Automatic mode).

Transferring the tool list

Select ”Setting up - Tool list - Accept list”

Depending on the previous turret assignment, the following might occur:

■ Tool not used

The CNC PILOT enters the new tools in the tool list. Positions that were occupied in the old tool list, but

3.3 Tool Lists, Tool Life Data

are not used in the new list, are retained. If a tool shall remain in the tool carrier, no further action is required; if not, delete the tool:

■ Actual tool location differs from location in tool

list

A tool is not entered when its newly assigned location differs from the location specified in the tool list. The CNC PILOT displays a message indicating this error. Change the tool location.

As long as a tool position differs from the nominal assignment it remains highlighted.

Soft keys

Delete the tool

Take the tool from the ”ID number clipboard”

Danger of collision

■ Tool locations that are occupied but,

according to the NC program, are not needed, are kept.

■ The CNC PILOT compensates the tool

actually entered – even if it does not match the nominal assignment.

Delete the tool and place in the ”ID number clipboard”

Edit the tool parameters

Entries in the tool database - sorted by tool typep

Entries in the tool database - sorted by tool ID number

3 Manual Control and Automatic mode32

3.3.4 Tool Life Management

The tool life management allows you to define the sequence of exchange and declare the tool to be ready for use. The tool life/quantity is defined in the tool database (see section ” Life Monitoring”).

The ”Tool life management” dialog box is used both for entering and displaying the tool life data.

You can use the variable-programming function in your NC program to evaluate sequential events that you enter in ”Event 1” and ”Event 2” (see section

4.15.2

V Variables”).

”

Tool life management parameters

■ Repl. tool (replacement tool): T number (turret

position) of the replacement tool

■ Event 1: Sequential event that is triggered when

the life of a tool has expired/a tool has produced the defined quantity – Event 21..59

■ Event 2: Sequential event that is triggered when

the life of the last tool of the interchange chain has expired/the tool has produced the defined quantity – Event 21..59

■ Ready for use: Set the tool to ”ready for use” or

”not ready for use” (applies to tool life management only).

Entering the tool life parameters

Select ”Setting up – Tool list – Tool life management”; the CNC PILOT displays the tools entered.

Select the tool location.

Press ENTER – the CNC PILOT opens the ”Tool life management” dialog box.

Enter the replacement tool and the tool life parameters; press OK.

”New cutter” sets the tool life/quantity to the value programmed in the database and sets the tool to ready for use.

8.1.7

Multiple Tools, Tool

3.3 Tool Lists, Tool Life Data

Update tool life management data

Select ”Setting up - Tool list – Update tool life management.”

Confirm the confirmation request with OK; the CNC PILOT sets the tool life/quantity to the value defined in the database and sets all tools in the tool list to ready for use.

The CNC PILOT displays the ”Tool list - tool life management” for inspection.

Application example: The cutting edges of all tools used have been replaced. Part production is to be continued, using the tool life management function.

HEIDENHAIN CNC PILOT 4290

3.4 Setup Functions

3.4.1 Defining the Tool Change Position

With the ISO command G14, the machine slide moves to the tool change point. Always program the tool change point as far from the workpiece as possible to allow the turret to rotate to any position.

Defining the tool change position

For more than one slide: Define the desired slide (with the Slide change key)

3.4 Setup Functions

Select ”Setting up – Tool change point.”

The CNC PILOT displays the currently valid position in the ”Set tool change point” dialog box.

Entering the tool change point

Enter a new position

Soft keys

Capture tool change point

Move slide to the tool change position

Confirms the slide position as tool change point

Confirms the position of individual axes

The tool change point is managed in the setup parameters (Select: „Act. Para – Setting up (menu) – Tool change point – ..“).

The coordinates of the tool change position are entered and displayed as distance between machine datum and tool carrier datum. Since these values are not shown in the position display, it is advisable to move to the tool change point and ”capture” the position.

■ Assigns a handwheel to an axis

■ Defines the handwheel interpolation factor

Switch the machine display

Enter the feed per revolution

Enter the constant surface speed

Enter the M function

Accept the axis position as tool change point(or Y or Z axis)

Accept the slide position as tool change point

3 Manual Control and Automatic mode34

3.4.2 Shifting theWorkpiece Datum

Shifting the Workpiece Datum

For more than one slide: Define the desired slide (with the Slide change key)

Position the tool

Select ”Setting up - Shift zero point.”

The ”Shift zero point” dialog box displays the current workpiece zero point.

Enter the workpiece zero point

Enter a ”zero point shift”

Contact position = tool zero point

Touch the end face with the tool

Accept the tool contact position as

workpiece zero point

Workpiece zero point relative to the contact position

Touch the end face with the tool

Accept the tool contact position

3.4 Setup Functions

Soft keys

■ Assigns a handwheel to an axis

■ Defines the handwheel interpolation factor

Switches the machine display

Enter the feed per revolution

Enter the measured value (distance of the tool contact position from the workpiece zero point)

The tool zero point is managed in the setup parameters (Select: „Act. Para – Setting up (menu) – Tool zero point – ..“).

■ The ”displacement” is with respect to

the machine zero point.

■ You can also offset the workpiece zero

point for the X and Y axes.

HEIDENHAIN CNC PILOT 4290

Enter the constant surface speed

Enter the M function

Define the Z position as tool zero point (or X or Y position)

Specify the tool zero point relative to the current Z position (or X or Y position)

3.4.3 Defining the protection zone

Defining the protection zone

Insert any tool (T0 is not permitted).

Select ”Setting up - Selection zones”

Enter the protection zone parameters

Enter the limit values.

3.4 Setup Functions

Capturing the protection zone parameters per axis

For each input box:

Select the input field Position the tool to the protection zone limit

Accept the axis position as protection zone parameter

Capturing positive/negative protection zone parameters

Select any positive or negative input field Position the tool to the protection zone limit

Accept all positive/negative axis positions

Soft keys

■ Assigns a handwheel to an axis

■ Defines the handwheel interpolation factor

Switch the machine display

Enter the feed per revolution

The parameters serve for protection zone monitoring - not as software limit switches.

Protection zone parameters:

■ are expressed with respect to the

machine zero point

■ are managed in the machine parameters

1116, 1156, ..

■ X value are radius dimensions

■ 99999/–99999 means: no monitoring of

this side of the protection zone

Enter the constant surface speed

Enter the M function

Accept the X position as ”protection zone –X” parameter (or +X, –Y, +Y, –Z, +Z position)

Accept the axis positions as positive/negative protection zone parameter

3 Manual Control and Automatic mode36

3.4.4 Setting up the ChuckingTable

The chucking table is evaluated by the concurrent graphics.

Setting up the chucking table

Select ”Setting up – Chucking table – Main spindle (or Tailstock)

Select the ID number from the chucking database

Chucking equipment for spindles

The definition of the clamping form (”Grip. form”) presupposes the definition of the chuck jaws. Set the clamp form by soft key – it is graphically illustrated.

To switch to the chucking assignment of further spindles, press the Page Up/Page Dn keys.

Parameters for ”spindle x” (main spindle, spindle 1, ..)

■ Chucking ID (identification number): Reference to

database.

■ Chuck jaws ID (identification number): Reference to

database.

■ Chuck supplement ID (identification number):

Reference to database.

■ Clamp form (for chuck jaws): Define internal/

external chucking and the level of chuck jaws used

■ Clamping diameter: The diameter at which the

workpiece is clamped. (Workpiece diameter when clamped externally; inside diameter when internal clamping is used)

”Tailstock” parameters

■ Sleeve center ID (identification number): Reference

to database.

3.4 Setup Functions

Soft keys

Edit the chucking equipment parameters

Entries in the chucking database – sorted by chuck type

Entries in the chucking database – sorted by chuck ID number

”Continue” – Define the clamp form

HEIDENHAIN CNC PILOT 4290

3.4.5 Setting up Machine Dimensions

You can evaluate machine dimensions in the variable programming of the NC program.

The ”Set machine dimensions” function accounts for the dimensions 1..9 and the ”configured axes” for each dimension.

Setting up machine dimensions

Select ”Setting up - Machine dimensions.”

3.4 Setup Functions

Enter the machine dimension number

Enter the machine dimensions

Enter the values (”Set machine dimension x” dialog box).

Capturing a single machine dimension

Select the input field Move the axis to the desired position

Confirm the axis position as machine dimension (or Y or Z position)

Soft keys

■ Assigns a handwheel to an axis

■ Defines the handwheel interpolation factor

Capturing all machine dimensions

Move the slides to the desired positions

Confirm the axis positions of the slides as machine dimensions

OK – enter the next machine dimension Cancel – Exit the machine dimension setup

Machine dimensions are managed in machine parameter 7.

Machine dimensions are given with respect to the machine zero point.

Switch the machine display

Enter the feed per revolution

Enter the constant surface speed

Enter the M function

Accept the axis position as machine dimension X (or Y or Z axis)

Accept the axis positions of the slides as machine dimensions

3 Manual Control and Automatic mode38

3.4.6 MeasuringTools

Define the type of tool measurement in machine parameter 6:

■ 0: Contact with tool

■ 1: Measure with touch probe

■ 2: Measure with measuring optics

MeasuringTools

Position the tool

Select ”Setting up - Tool setup – Tool measuring.” The ”Tool measuring T...” dialog box indicates the current tool dimensions.

Enter the machine dimensions

Enter the dimensions

Find the tool dimensions by touching the

workpiece with the tool

Select the input field ”X” Touch off the diameter, retract in Z direction

Confirm the diameter as measured value

Select the Z input field Touch the face with the tool, then retract in the X

direction

Confirm the Z position of the tool as the measured value

3.4 Setup Functions

Soft keys

■ Assign a handwheel to an axis

■ Define the handwheel interpolation factor

Switch the machine display

Enter the feed per revolution

Enter the constant surface speed

Measuring tools with the touch probe

for each input field:

Select the X/Z input field Move the tool tip in X/Z direction to the probe; the

CNC PILOT saves the X/Z dimension

Retract the tool – retract the touch probe

Measuring the tools with measuring optics

For each input field

Select the X/Z input field Align the tool point in the X/Z direction with the

cross hairs

Accept the value

HEIDENHAIN CNC PILOT 4290

Enter the M function

Accept the X position as measured value X (or Y or Z position)

■ The entries in the ”Enter measured value” dialog box are

given with respect to the workpiece zero point.

■ The compensation values of the tool are deleted.

■ The measured tool dimensions are entered in the

database.

Continued

Determining tool-compensation values

Move the tool into position

Select ”Setting up - Tool setup – Tool compensation”

Assign the handwheel to the X axis – move the tool by the compensation value

Assign the handwheel to the Z axis – move the tool by the compensation value

3.4 Setup Functions

The CNC PILOT loads the compensation values

Soft keys

■ Assign a handwheel to an axis

■ Define the handwheel interpolation factor

Switch the machine display

Enter the feed per revolution

Enter the constant surface speed

Enter the M function

Accept the tool compensation values

3 Manual Control and Automatic mode40

3.5 Automatic Mode of Operation

In Automatic mode, the data are entered and displayed in 1 millimeters or in inches, depending on the setting of the control parameter 1. The setting in the ”program head” of the NC program governs the execution of the NC part program - it has no influence on operation or display.

3.5.1 Program Selection

The CNC PILOT interprets the NC program before it can be activated with Cycle Start. ”#-Variables” are entered during the translation process. A ”restart” prevents a new translation, while a ”new start” forces a new translation.

Program selection

Select ”Prog – Program selection” Select the NC program

The NC program is loaded without previous translation, if:

■ No changes were made in the program or the tool

list.

■ The lathe was not switched off since the program

was last selected.

Restart

Select ”Prog – Restart”

The last active NC program is loaded without without previous translation, if:

■ No changes were made in the program or the tool

list.

■ The lathe was not switched off since the program

was last selected.

New start

Select ”Prog – New start”

The NC program is loaded and translated. (Use for starting an NC program containing # variables.)

From DIN PLUS

Select ”Prog – From DIN PLUS”

The NC program selected in DIN PLUS is loaded and translated.

■ If the ”turret table” of the NC program is

not the currently valid one, there is a warning.

■ The name of the NC program is retained

until you select another program – even if the lathe was switched off in the meantime.

3.5 Automatic Mode of Operation

Soft keys

Switch to ”graphic display”

Switch the machine display

Define block display for more channels

Display basic blocks (individual paths of traverse)

Suppress/permit variable output

Set single block mode

Program stop at M01 (optional stop)

Run a start-block search

HEIDENHAIN CNC PILOT 4290

3.5.2 Defining a Start Block

Defining a Start Block

Activating a start block search

Position the cursor on the start block. (The soft keys support your search.)

The CNC PILOT switches back into automatic mode and jumps to the start block.

Start the NC program with the selected NC block.

3.5 Automatic Mode of Operation

Exit the start block search without default start block.

■ Select a suitable start block. If program

run is started by a specific start block, the CNC PILOT automatically provides all the programmed and essential data for this NC program (excluding interchange of the correct tool and paths of traverse).

■ On machines with more than on slide,

select a suitable start block on all slides before you press the Accept soft key.

Danger of collision

■ If the start block includes a T command,

the CNC PILOT first rotates the turret.

■ The first traversing instruction is

executed from the current tool position.

Soft keys

Switch the machine display

Define block display for more channels

Display basic blocks (individual paths of traverse)

Preset the T number – the cursor is positioned with this T number on the next T command

Preset the T number – the cursor is positioned to the block number

Preset the L number – the cursor is positioned with this L number to the next subprogram call

Run a start-block search

3 Manual Control and Automatic mode42

3.5.3 Program Sequence Modification

Skip levels:

■ The program blocks which are marked as active

skip levels are not executed when the program is being carried out.

■ Skip levels: 0..9

■ For multiple skip levels, enter a sequence of digits

■ Deactivate the skip level: No entries in ”Level No.”

Operation:

Select menu item ”Process - Skip level” Enter the level number

Quantity

■ Counting range: 0..9999

■ Quantity = 0: Production without quantity limitation;

the counter is increased by one after each program run.

■ Quantity > 0: The CNC PILOT produces the defined

quantity; the counter is reduced by one after each program run.

■ Quantity counting is retained even if the machine

has been switched off in the meantime.

■ When an NC program is activated with ”Program

selection,” the CNC PILOT resets the quantity counter.

■ When a program has completed a production lot,

the NC program cannot be restarted by the Cycle Start key. To start the NC program again, press ”Re-start.”

Operation:

Select menu item ”Process – Quantity” Enter the quantity

V variables

■ The ”V variables” dialog box serves for input and

display of variables.

■ V variables are defined at the beginning of the NC

program. The meaning is specified in the NC program.

Operation:

Select the menu item ”Process – V variables” – the CNC PILOT shows the variables defined in the NC program

Press ”Edit” if you wish to change the variables

Status of skip levels

Display field:

Markings:

■ Upper row: entered skip levels

■ Lower row: the skip levels detected by the ”block execution”

(active skip levels)

The CNC PILOT accounts for activated/deactivated skip levels after approx. 10 blocks (reason: block scan during the execution of NC blocks).

3.5 Automatic Mode of Operation

HEIDENHAIN CNC PILOT 4290

Continued

Single-block mode

Only one NC command (basic block) is executed at a time. The CNC PILOT then goes into the ”cycle stop” condition.The subsequent blocks are started with Cycle Start.

Optional STOP

The CNC PILOT stops at the M01 command and goes into the cycle stop condition. Cycle start resumes the program run.

Status of optional stop

Optional stop off

Optional stop on

Feed rate override F% (0% .. 150%)

Feed rate override is controlled manually with a knob on the on the machine operating panel. The machine display shows the current feed rate override.

Spindle speed override S% (50% .. 150%)

The spindle speed override or the reset to the

3.5 Automatic Mode of Operation

programmed speed is controlled with the keys of the machine operating panel. The machine display shows the current spindle speed override.

3.5.4 Compensation

■ Tool compensation

Select ”Comp - Tool compensation”

The CNC PILOT enters the T number and current compensation values of the active tool. You can enter a differentT number.

Enter the compensation values

Values entered here are added to the existing compensation values.

Tool compensation:

■ Become effective when the next

traverse starts.

■ Are transferred to the database.

■ Values of max. 1 mm can be entered.

Keys for spindle speed override

Rotational speed to 100% (of the programmed value)

Increase speed by 5%

Reduce speed by 5%

3 Manual Control and Automatic mode44

■ Additive compensation

Select ”Comp - Additive cormpensation.”

Enter the compensation number (901 to 916); the CNC PILOT displays the current compensation values.

Enter the compensation values

Values entered here are added to the existing compensation values.

Additive compensation:

■ are activated with G149 ..

■ are managed in setup parameter 10

■ can be changed by no more than 1 mm

3.5 Automatic Mode of Operation

3.5.5 Tool Life Management

Select ”Comp - Tool life management.” This tool list with the current tool life data is

displayed

Select the tool ENTER opens the ”Tool life management” dialog

box

■ Set to ”ready for use” - or

■ update the tool life data with a ”new cutter.”

HEIDENHAIN CNC PILOT 4290

3.5.6 Inspection Mode

This function interrupts the program sequence, checks and corrects the ”active tool,” inserts a new cutting edge and continues the NC program from the point of interruption.

The inspection cycle is executed as follows:: Interrupt the program sequence and retract the tool.Check the tool, and replace the cutting edge if necessary.n Return the tool.

■ Cutting edge OK: Continue the automatic

program run.

■ New cutting edge: Define the compensation

values by ”scratching,” and continue the automatic program run.

When the tool is retracted, the CNC PILOT stores the first five traverse movements. Each change in direction corresponds to a path of traverse.

The NC program run can be continued before the point of interruption. Specify the distance to the

3.5 Automatic Mode of Operation

interruption point. If the value is greater than the distance between the start of the NC block and the interruption point, program sequence begins at the start of the interrupted NC block.

■ During the inspection process you can

turn the turret, press the spindle keys, etc.

■ If the turret was turned, the return

motion program inserts the ”correct” tool.

■ When changing the cutting edge, select

the compensation values so that the tool stops in front of the workpiece.

■ In the cycle stop condition you can

interrupt the inspection cycle with ESC and switch to ”Manual control.”

Inspection mode

Interrupt the program run

Select ”Insp(ection)”

To retract the tool, use the axis-direction keys.

If necessary, swivel the turret.

Inspect the tool; if necessary, replace it.

Conclude the inspection process - the CNC PILOT loads the return motion program (”_SERVICE”).

The ”Tool compensation” dialog box appears. Enter the compensation values, and confirm with OK.

If you are using a new cutting edge, modify the tool compensation so that the tool - when returning - comes to a stop in front of the workpiece.

If necessary, activate the spindle.

Starts the return motion program.

Continued

3 Manual Control and Automatic mode46

Inspection mode – continued

The ”Scrambled takeoff on restart?” dialog box appears; Enter Yes/No, and press OK.

Scrambled takeoff – Yes:

The ”Start from interruption point (IP) / before interruption point” dialog box appears.

■ From UP: No further dialog box.

■ Before UP: Specify the distance from the point of

interruption to the starting point of the tool (Dialog ”Distance from interruption point”).

The return motion program positions the tool on/ before the interruption point and continues the program without stopping.

The inspection cycle has been completed.

Scrambled takeoff – NO:

The ”Start from interruption point (IP) / before interruption point” dialog box appears.

■ From UP: No further dialog box.

■ Before UP: Specify the distance from the point of

interruption to the starting point of the tool (Dialog ”Distance from interruption point”).

The return motion program positions the tool on/ before the interruption point and stops.

Application example: Cutting edge has been replaced.

Select ”Insp(ection)” again.

The ”Scratch with tool” dialog box opens (for information)

Assign the handwheel to the X/Z axis and ”scratch” the workpiece.

Press ”Accept value” to save the compensation values defined per handwheel.

The program run continues

3.5 Automatic Mode of Operation

HEIDENHAIN CNC PILOT 4290

3.5.7 Block Display

Block display – basic block display

The block display lists the NC blocks according to the programmed sequence. The basic-block display shows the individual paths of traverse – the cycles are ”resolved.” The numbering of the basic blocks is independent of the programmed block numbers.

In the block display and basic-block display, the cursor is located on the block being executed.

Channel display

For lathes with several slides (channels), you can activate block display for up to 3 channels.

Basic block on/off

Switching the channel display

To add a channel, press the soft key again; in the block display, only channel

3.5 Automatic Mode of Operation

Menu item ”display - ...”

■ Font size: Enlarges/reduces the characters in the

block display

■ Load monitoring – see ”

Load Monitoring”

1 is shown.

Variable output

Pressing the soft key enables the variable soft key output (with PRINTA). Otherwise the variable output is suppressed.

3.7.2

Production under

3 Manual Control and Automatic mode48

3.5.8 Graphic Display

The ”Automatic graphics” function displays the programmed blank and finished part and the paths of traverse. This enables process control of non-visible areas during production and provides an oversight of production status, etc.

All machining operations, including milling, are depicted in the turning window (XZ view).

Activate the graphic – if the graphic was already active, the screen is adapted to the current machining status.

Return to block display

Settings:

Line: Each tool movement is

represented as a line, referenced to the theoretical tool tip.

Cutting path: depicts the surface covered by the ”cutting area” of the tool with hatch marks. You can see the area that will actually be machined, with the geometry of the respective tool already accounted for (see ”

5.1

Simulation Mode of Operation”).

The white dot: (small white rectangle) represents the theoretical tool point.

Tool: The tool contour is depicted. (Precondition: Proper tool description in the tool database.)

Standard: The system displays the complete path of traverse block by block Motion: Depicts the metal removal in synchronism to the machining sequence.

Prerequisites:

■ Workpiece blank is programmed

■ Activate the ”motion” function

before starting the NC program.

■ If an NC program is repeated (M99),

the ”Motion” function becomes active with the next program run.

3.5 Automatic Mode of Operation

Soft keys

Return to block display

Activate the zoom function

Set to Single block mode

Depiction of traverse paths: Line or (cutting) trace

Tool depiction: Point of light or tool

■ ”Motion” appears only for lathes with one slide.

■ If no blank part was programmed, the standard blank

form (control parameter 23) is assumed.

HEIDENHAIN CNC PILOT 4290

Continued

Enlarging, reducing, selecting a section for enlargement

When you call the zoom function, a red frame appears with which you can select the detail you wish to isolate.

Detail:

■ Enlarge: ”Page forward”

■ Reduce: ”Page back”

■ Shift: Cursor keys

Zoom settings by touch pad

Prerequisite: Simulation in ”stop condition”

Position the cursor to one corner of the section

While holding the left mouse key, pull the cursor to

the opposite corner of the section

Right mouse key: Return to standard size

Standard settings: See soft-key table

3.5 Automatic Mode of Operation

Exit the zoom function

After having enlarged a detail to a great extent, select ”Workpiece maximum” or ”Work space,” and then isolate a new detail.

Soft keys

Return to block display

Cancels the zoom settings last used and displays the last standard setting (”Workpiece maximum” or ”Work space”).

Switches back to the last zoom/setting used. You can select ”Previous zoom” more than once.

Shows the workpiece in the largest possible magnification

Shows the working space including the tool change position.

In the ”Coordinate system” dialog box, you specify the dimensions of the simulation window and the position of the workpiece zero point.

3 Manual Control and Automatic mode50

3.5.9 Post-Process Measuring Status Display

Selection: Menu item ”Display – PPM Status”

(automatic mode)

The ”PPM Info” dialog box contains information on the status of the measured values and displays the transferred results:

■ ”Measured-value coupling” (control parameter 10)

■ Off: Measuring results are immediately

transferred. Previous values are overwritten.

■ On: Measuring results are not transferred until

the previous results have been processed.

■ Measured values valid: Status of the measured

values (after the measured values have been transferred with G915, the status ”No” is displayed).

■ #939: Total result of last measurement.

■ #940..956: Measuring results last transferred by the

measuring function.

If you select ”Init,” the post-process measuring function is re-initialized and all measured values are deleted.

3.5 Automatic Mode of Operation

The post-process measuring function stores the measured values received in the clipboard. The ”PPM Info” dialog box displays in #939..956 the values contained in the clipboard not the variables.

HEIDENHAIN CNC PILOT 4290

3.6 Machine Display

The machine display of the CNC PILOT can be configured. Per slide, you can configure up to 6 displays in Manual mode and Automatic mode.

Switches to the ”next configured display”

To switch to the display of the following slide, press the Change slide key. With the spindle change key you can display the next spindle.

3.6 Machine Display

The ”display elements” table explains the standard display fields. For more display fields, see ” Parameters”

You can set the values of the Position display in ”Display setting” (machine parameter 17):

■ 0: Actual values

■ 1: Lag

■ 2: Distance to go

■ 3: Distance between tool tip and position

of slide

■ 4: Slide position

■ 5: Distance between reference cams

and zero pulse

■ 6: Nominal position value

■ 7: Distance between tool tip and slide

position

■ 8: IPO nominal position

7.3

Control

Display elements

Position display (actual value display)

Distance from tool point to tool zero point

■ Empty box: Reference mark in this axis not yet traversed

■ White axis letter No enabling

Position display (actual value display) C

Position of the C axis.

■ ”Index”: Indicates the C axis „0/1“

■ Empty box: C axis is not active

■ White axis letter: No enabling

Distance-to-go display

Distance remaining in the current traverse command

■ Bar graphic: Distance to go in millimeters

■ Box at lower left: Actual position

■ Box at lower right: Distance to go

T display – without tool life monitoring

■ T number of active tool

■ Tool compensation values

T display – with tool life monitoring

■ T number of the active tool

■ Tool life data

Continued

3 Manual Control and Automatic mode52

Display elements (continued)

Cycle status (slide display)

Quantity of workpieces/time per workpiece

■ Number of finished workpieces in this batch

■ Machining time of current workpiece

■ Entire production time of this batch

Load display

Load of the spindle motors/axis drives with regard to rated torque

D display – additive compensation

■ Number of the active compensation

■ Compensation values

Slide display

■ White symbol: No enabling

■ Number: Selected slides

■ Cycle state: see table

■ Bar diagram: Feed rate override ”in %”

■ Upper box: Feed rate override

■ Lower box: Current feed rate – with stationary spindle: Nominal

feed rate (gray print)

■ Slide number in blue background: Rear side machining active

Spindle display

■ White symbol: No enabling

■ Number in spindle symbol: Gear range

■ ”H”/number: Selected spindle

■ Spindle status: See table

■ Bar diagram: Spindle speed override ”in %”

■ Upper box: Spindle speed override

■ Lower box: Current speed – with position control (M19): Spindle

position – with stationary spindle: Nominal speed (gray print)

Automatic mode – Cycle Start

Automatic mode – Feed Stop

Automatic mode – Cycle Stop

Manual control

3.6 Machine Display

Inspection cycle

Machine in setup mode

Spindle status (spindle display)

Direction of spindle rotation M3

Direction of spindle rotation M4

Spindle stopped

Spindle position-controlled (M19)

C-axis is ”active”

Overview of enabled elements

Shows the enabling status of up to 6 NC channels, 4 spindles, and 2 C-axes. Enabled elements are marked in green.

■ Display group at left: Enabled elements

F=feed rate; D=data; S=spindle; C=C-axis.

1..6: Number of slides/ of spindle, of C axis

■ Display group at center: Status

Zy – left dash: Cycle on/off. Zy – right dash: Feed Stop. R=traversing the reference marks; A=automatic mode; H=manual control; F=retracting (after traversing the limit switches); I = Inspection mode; E = Setup switch;

■ Display group at right: Spindle

Display for ”direction of rotation left/right.” Both active: Positioning of spindle (M19).

HEIDENHAIN CNC PILOT 4290

3.7 Load Monitoring

The load monitoring function of the CNC PILOT compares the current torque, or the values for work, with the values from a ”reference run.”

If ”torque limit 1” or the ”work limit” is exceeded, the CNC PILOT marks the tool as ”worn out.” If ”torque limit 2” is exceeded, the CNC PILOT assumes tool breakage and stops machining (feed stop). Violations of limit values are reported as error messages.

The load monitoring identifies worn tool in the ”tool diagnosis bits.” If you are using the tool life

3.7 Load Monitoring

management function, the CNC PILOT will manage

4.2.4

the replacement of tools (see ” Programming”). You can also evaluate the ”tool diagnosis bits” in the NC program.

The load monitoring function defines the monitoring zones and the drives to be monitored (G995) in the NC program. The torque limits of a monitoring zone depend on the maximum torque determined by the reference machining cycle.

Tool

The CNC PILOT checks the values for torque and work in each interpolator cycle and displays the values in a time reference grid of 20 ms. The limit values are calculated from the reference values and the limit factor (control parameter 8). You can later change the limit values in ”Edit load parameters.”

■ Make sure that the conditions for reference machining

comply with those for production (feed-rate/speed override, tool quality, etc.).

■ Up to four components are monitored per monitoring

zone.

■ Using ”G996 Type of load monitoring,” you can control

the hiding the rapid traverses paths and the monitoring of torque and/or work.

■ The graphic and numeric displays are relative to the rated

torque values.

3.7.1 Reference Machining

The reference machining cycle (registration of nominal values) determines the reference values for the maximal permissible torque and work of each monitoring zone.

CNC PILOT executes a reference machining cycle if:

■ The parameters for monitoring have not been

entered.

■ You press ”Yes” in the ”Reference machining”

dialog box (after having selected the program).

Selection: ”Display – Load monitoring – Load monitoring display” (Automatic mode).

”Taking nominal values” submenu

■ ”Curves” menu item

Assign the input fields ”curves 1...4” to the drives. The value in ”Display grid” influences the accuracy

and velocity of the graphical display. A small value increases the accuracy of the display (values: 4, 9, 19, 39 seconds per image).

■ ”Mode” menu group

■ Line graphics: Display torque values over the

time axis

Continued

3 Manual Control and Automatic mode54

■ Bar graphic: Graphically display torque values

and mark the peak values

■ Save/do not save measured values

The measured values must be saved for later analysis of reference machining. Check the setting in the ”Save data” (”Write data”) display field.

■ Overwrite/Do not overwrite limit values

If you wish to retain the limit values after a new reference machining cycle, select ”Do not overwrite limit values.”

■ Pause stops the display

■ Continue continues the display

■ Auto: returns to the automatic menu

Additional information

■ Zone number: Current monitoring zone.

Negative algebraic sign: Production is not monitored (example: skipping the paths of rapid traverse).

■ Tool: Active Tool.

■ Selected drives: The drives are listed and the

current torques are displayed.

■ Block display

3.7 Load Monitoring

Block display has no influence on reference machining.

3.7.2 Production Using Load Monitoring

If you wish to use the load monitoring function for your machining processes, you must activate it in the NC program (G996).

Display torque values and limit values:

”Display – Load monitoring – Display” (Automatic operating mode).

”Load monitoring display” submenu:

■ ”Curves” menu item

Enter the required drives in the input fields ”Curves 1 to 4”.

■ Line graphics: One curve

■ Bar graphics: Up to four curves

Display grid: See §

■ ”Mode” menu group

■ Line graphic Display the torque values over the

time axis and limit values – limit values are gray: nonmonitored area (rapid traverse paths are hidden).

■ Bar graphic Displays current torque values,

previous ”work” and all limit values of the monitoring zone

3.7.1

Reference Machining”

■ Pause Stops the display

■ Continue Resumes the display

■ Auto Returns to the automatic menu

HEIDENHAIN CNC PILOT 4290

3.7.3 Editing Limit Values

The function for editing the load parameters allows you to analyze reference machining cycles and optimize limit values.

The CNC PILOT displays the program name of the loaded monitoring parameters in the header.

Selection: ”Display – Load monitoring – Edit” (Automatic mode).

3.7 Load Monitoring

”Load parameter editor” submenu

■ ”Act. load” (Load current file) menu item:

Monitoring parameters of the active NC program.

■ ”Load” menu item: Monitoring parameters you

have selected.

■ ”Edit” menu item: Display and edit the limit

values.

■ ”Delete reference values” menu item: Delete the

load parameters of the NC program.

■ Auto Returns to the automatic menu

Editing the load parameters

The ”Display and adjust load parameters” dialog box displays the parameters of one component of one monitoring zone, which can then be edited. The bar graphic shows all components of the monitoring zone (the larger bar displays the values for performance; the smaller bar displays the values for work). The selected component is highlighted. Enter the monitoring zone and select the component. The CNC PILOT displays the reference values. The limit values for performance and work, which are displayed, can be edited. The tool (T number) is displayed for information.

Buttons of the dialog box:

■ Saving: Store the limit values of the component in

the specified zone.

■ End (or ESC key): Exit the dialog box.

■ File: Switch to ”Line graphics.” Precondition: The

values measured during the reference machining cycle have been stored.

3 Manual Control and Automatic mode56

3.7.4 Analyzing Reference Machining

The torque and the limit values of the selected component are shown ”over time.” Limit values ”gray”: nonmonitored area (hiding rapid traverse paths).

The CNC PILOT also displays the values of the cursor position.

Selection: ”File” button (”Display and set load parameters” dialog box).

”Analyzer (file display)” submenu:

■ ”Set cursor” pull-down menu; using the right/left

arrow key, position the cursor at the:

■ Start of file

■ Start of the next zone

■ Zone maximum

■ ”Display” menu item: Select the component from

the ”Display file” dialog box.

■ ”Setting – Zoom” menu item: Set the zoom

factor. (Small values increase the accuracy of the display and reduce the step size of the cursor.)

The settings defined for the grid, the time reference grid of the measured value registration and the cursor position are shown in the line below the graphic display (relative to the start of reference machining). Time ”0:00.00 sec” = Start of reference machining cycle.

Switch back to ”Edit load parameters”

3.7 Load Monitoring

3.7.5 Machining Using Load Monitoring

It is advisable to use the load-monitoring function when - due to a dull cutting edge - a machining process requires a considerably higher torque than with a new cutting edge. As a rule, drives that are subjected to considerable loads should be monitored usually the main spindle.

Due to the relatively small torque variations, it is difficult to monitor machining operations with small cutting depths.

A decrease in torque cannot be identified.

HEIDENHAIN CNC PILOT 4290

Defining the monitoring zones: The reference values for torque depend on the maximum torque values of the zone. Therefore, lower torque values cannot always be monitored.

Facing with constant cutting speed: The spindle is monitored as long as the acceleration is 15% of the mean value from maximum acceleration and maximum braking deceleration (machine parameters 811, ...). Since acceleration increases as a result of the increase in rotational speed, the CNC PILOT usually only monitors the period after the first cut.

Experimental values for the machining of steel

■ For longitudinal turning, ensure that the cutting depth is greater than

1 mm.

■ For recessing, ensure that the cutting depth is greater than 1 mm.

■ For hole drilling, ensure that the diameter drilled is between 6 and

10 mm.

3.7.6 Load Monitoring Parameters

Machine parameters for load monitoring (spindle: 809, 859, ...; C-

axis: 1010, 1060; linear axes: 1110, 1160, ...)

■ Start time for monitoring [0 to 1000 ms] is calculated when rapid

traverse movements have been skipped:

■ Spindles: A limit value is calculated from the acceleration and

brake ramps. As long as nominal acceleration exceeds the limit value, the monitoring function is deactivated. If nominal acceleration drops below the limit value, the monitoring function is delayed by the ”start time for monitoring.”

■ Linear axes and C-axis: After rapid traverse has changed to feed

3.7 Load Monitoring

rate, the monitoring function is delayed by the ”start time for monitoring.”

■ Number of measured values to be averaged [1..50]

The mean value reduces the sensitivity to short peaks.

■ Maximum torque of the drive [Nmm]

■ Delay in reaction P1, P2 [0 to 1000 ms]: The CNC PILOT indicates

that torque limit 1/2 has been exceeded after the time ”P1/P2” has passed.

Control parameter 8 ”Load monitoring settings”

■ Factor for torque limit value 1, 2

■ Factor for work limit value

Limit value = reference value * factor for limit value

■ Minimum torque [% of rated torque]: Reference values below

this value are raised to this minimum torque value. This prevents that limit values are exceeded as a result of minor differences in torque.

■ maximum file size [KB]: If the data exceed the ”maximum file

size,” the ”oldest measured values” are overwritten. Approximate value: For one component per minute of program run time approximately 12 KB.

Control parameter 15 ”bit codes for load monitoring”:

Assigns the bits number used in G995 to the drives (logical axes).

3 Manual Control and Automatic mode58

DIN PLUS

4.1 DIN Programming

Example: Structured DIN PLUS program

4.1.1 Introduction

The CNC PILOT supports conventional DIN programming and DIN PLUS programming.

Conventional DIN programming

You program the basic contour with line segments, circular arcs and simple turning cycles. For conventional DIN programming, the ”simple tool description” is sufficient (see section ”

DIN PLUS – Programming

The geometrical description of the workpiece and the

4.1 DIN Programming

machining process are separated. You first program the geometry of the blank and finished part. Then you machine the workpiece, using contour-related turning cycles. The contour follow-up function can be activated for each machining step, including individual paths of traverse and simple turning cycles. The CNC PILOT optimizes the machining process as well as the paths for approach and departure (no noncutting passes).

Depending on the type and complexity of your machining task, you can use simple DIN programming or DIN PLUS programming.

NC program sections

The CNC PILOT supports the division of the NC program into individual program sections. Sections containing set-up information and organizational data are included.

NC program sections:

■ Program head (organizational data and setup

information)

■ Tool list (turret table)

■ Chucking-equipment table

■ Definition of blank

■ Definition of finished part

■ Machining of workpiece

Parallel operation

While you are editing and testing programs, your machine can execute another NC program.

4.4.2

Turret”).

PROGRAMMKOPF [PROGRAM HEAD]

#MATERIAL St 60-2 #EINSPANNDURCHM [CLAMPING DIAMETER] 120 #AUSSPANNLAENGE [CLAMPING LENGTH] 106 #SPANNDRUCK [CLAMPING PRESSURE] 20 #SCHLITTEN [SLIDE] $1 #SYNCHRO 0

REVOLVER 1 [TURRET]

T1 ID”342-300.1” T2 ID”111-80-080.1” T3 ID”112-16-080.1” T4 ID”121-55-040.1” T5 ID”122-20-040.1” T6 ID”151-600.2”

SPANNMITTEL [CHUCKING EQUIPMENT] [zero offset Z282 ] H1 ID”KH250” H2 ID”KBA250-77” Q4.

ROHTEIL [BLANK]

N1 G20 X120 Z120 K2

FERTIGTEIL [FINISHED PART]

N2 G0 X60 Z-115 N3 G1 Z-105 . . .

BEARBEITUNG [MACHINING]

N22 G59 Z282 N23 G65 H1 X0 Z-152 N24 G65 H2 X120 Z-118 N25 G14 Q0 [Predrilling-30mm-Outside-Centric-Front face] N26T1 N27 G97 S1061 G95 F0.25 M4 . . .

ENDE [END]

4 DIN PLUS60

4.1.2 DIN PLUS Screen

1 Menu bar

2 Display of loaded NC programs. The selected

program is marked.

3 Full, double or triple editing window. The selected

window is marked.

4 Contour display (or machine display)

5 Soft keys

Parallel editing

You can edit up to eight NC program/subprograms in parallel. The CNC PILOT displays NC programs as desired in either a full, double, or triple window.

Main menus and submenus

The functions of the DIN PLUS editor are contained in the main menu and various submenus. The submenus can be called by

■ Selecting the desired menu items

■ Positioning the cursor in the program section

Soft keys

Soft keys are available for fast switching to ”neighboring operating modes” for changing the editing window and for activating the graphic.

Soft keys

Change to the simulation operating mode

Change to the TURN PLUS mode

4.1 DIN Programming

Switch the NC program

Switch the editing window

Select full-size window (one editing window)

Select double or triple window

Activate the graphics

HEIDENHAIN CNC PILOT 4290

4.1.3 Linear and Rotary Axes

Principle axes: Coordinates of the X, Y and Z axes refer to the

workpiece zero point. Any deviations from this rule will be indicated.

Note for negative X-coordinates:

■ Not permitted for contour definition.

■ Not permitted for turning cycles.

■ Contour regeneration is interrupted.

■ The direction of rotation of arcs (G2/G3, G12/G13) must

be adjusted manually.

■ The position for tooth and cutter-radius compensation

(G41/G42) must be adjusted manually.

4.1 DIN Programming

C axis: Angle data are with respect to the zero point of the C axis.

(Precondition: The C axis has been configured as a principal axis.)

For C-axis contours and C-axis operations, the following applies:

■ Positions on the front/rear face are entered in Cartesian

coordinates (XK, YK), or polar coordinates (X, C).

■ Positions on the lateral surface are entered in polar coordinates

(Z, C). Instead of C, the ”linear value CY” is used (”unrolled” reference diameter).

Secondary axes (auxiliary axes): In addition to the principle axes, the CNC PILOT supports:

■ U: Linear axis in X direction

■ V: Linear axis in Y direction

■ W: Linear axis in Z direction

■ A: Rotary axis around X

■ B: Rotary axis around Y

■ C: Rotary axis around Z

Principal axes

The auxiliary axes are only programmed in the MACHINING section, using the functions G0 to G3, G12, G13, G30, G62 and G701. Circular interpolation is only possible in the principal axes.

Rotary axes (auxiliary axes) are programmed in the MACHINING section, using G15.

■ The DIN editor respects only address letters of the

configured axes.

■ The behavior of the rotary axis C depends on whether it

is configured as principle or secondary. The ”C axis functions” G100..G113 apply for the principle axis C.

Linear axes as secondary axes

Rotary axes as secondary axes

4 DIN PLUS62

4.1.4 Units of Measurement

You can use the metric or inch system for writing NC programs. The unit of measure is defined in the ”Unit” box (see ” Head”). After the unit of measure has been defined, it cannot be edited. Units of measure used: See ”

1. 4

Fundamentals.”

4.4.1

Program

4.1.5 Elements of the DIN Program

A DIN program consists of the following elements:

■ Program number

■ Program section codes

■ NC blocks

■ Commands for structuring the program

■ Comment blocks

The program number begins with ”%” followed by up to 8 characters (numbers, upper case letters or underscore; no mutated vowels or ”ß”) and the extension ”nc” for main programs or ”ncs” for subprograms. The first character must be a number or a letter.

Program section code: When you create a new DIN program, certain program section codes are already entered. You can add new codes or delete existing ones, depending on your program requirements. A DIN program must contain at least the MACHINING and END section codes.

NC blocks start with the letter ”N” followed by a block number (with up to four digits). The block numbers do not affect the sequence in which the program blocks are executed. They are only intended for identifying the individual blocks.

The NC blocks of the PROGRAM HEAD, TURRET and CHUCKING EQUIPMENT sections are not included in the ”block number organization” of the DIN editor.

An NC block contains NC commands such as positioning, switching or organizational commands. Traversing and switching commands begin with ”G” or ”M” followed by a number (G1, G2, G81, M3, M30, ...) and the address parameters. Organizational commands consist of ”key words” (WHILE, RETURN, etc.), or of a combination of letters/ numbers.

You can also program NC blocks containing only variable calculations.

You can program various NC commands in an NC block provided that they do not contain the same address letters and do not have opposing functionalities.

4.1 DIN Programming

HEIDENHAIN CNC PILOT 4290

Continued

Examples

■ Permissible combination:

N10 G1 X100 Z2 M8

■ Impermissible combination:

N10 G1 X100 Z2 G2 X100 Z2 R30 (same address letters used more than once)

or N10 M3 M4 – opposing functionality

NC address parameters

Address parameters consist of 1 or 2 letter(s) followed by a

■ A value

■ A mathematical expression

4.1 DIN Programming

■ A ”?” (simplified geometry programming VGP)

■ An ”i” to designate incremental address parameters (examples:

Xi..., Ci..., XKi..., YKi..., etc.)

■ A # variable (calculated during NC program interpretation)

■ A V variable (calculated during run time)

Examples:

■ X20 (absolute dimension)

■ Zi–35.675 (incremental dimension)

■ X? (Simple geometry programming)

■ X#12 (Programming of variables)

■ X{V12+1} (Programming of variables)

■ X(37+2)*SIN(30) (Mathematical term)

Program branches and repeats

■ You can use program jumps, repeats and subprograms to structure

a program. Example: Machining the beginning/end of a bar etc.

■ Skip level: Influences the execution of individual NC blocks

■ Slide code: you can assign the NC blocks to the indicated slides

provided that your lathe is equipped with more than one slide.

Input and output

With ”input” the machine operator can influence the flow of the NC program. Using ”output” functions, you can communicate with the machinist. Example: The machinist is required to check measuring points and update compensation values.

Comments

These are enclosed in parentheses ”[...].” They are located at the end of an NC block or in a separate NC block.

4 DIN PLUS64

4.2 Programming Notes

4.2.1 Parallel Editing

The CNC PILOT

■ runs up to eight NC program/subprograms in parallel

■ provides up to three editing windows

”Switch windows” soft key

Switch the NC program

Editing window

Double or triple window: Selected in ”Config – Window – ...” (main menu).

Load the desired NC program.

Load NC program in the next free window:

Select ”Prog – Load – Main program/Subprogram”

Load NC program in selected window:

Select and activate free editing window Select ”Prog – Load – Main program/Subprogram”

Switching between NC programs and windows

■ By soft key: see table

■ By touch pad:

■ To switch NC programs: Click the NC program in the program title

bar

■ To switch editing windows: Click the desired window

Save the NC program

■ ”Prog – Save”: Saves the NC program of the active window. The

NC program stays in the editing window – you can continue editing it.

■ ”Prog – Save as”: Saves the NC program of the active window

under a new program name. In the ”Saving NC program” dialog box you specify whether the editing window is closed.

■ „Prog – Save all”: Saves the NC programs of all active windows.

The NC programs remain in the editing windows – you can continue editing them.

Switch the editing window

Select full-size window (one editing window)

Select double or triple window

4.2 Basics of Programming

4.2.2 Address Parameters

You can use absolute or incremental coordinates for programming. If no entry is made for X, Y, Z, XK, YK, C, the coordinates of the block previously executed will be retained (modal).

CNC PILOT calculates missing coordinates in the principal axes X, Y or Z if you program ”?” (simplified geometry programming).

The machining functions G0, G1, G2, G3, G12 and G13 are modal. This means that the CNC PILOT uses the previous G command if the address parameters X, Y, Z, I or K in the following block have been programmed without a G function provided that the address parameters have been programmed as absolute values.

Continued

HEIDENHAIN CNC PILOT 4290

The CNC PILOT supports the use of variables and mathematical expressions as address parameters.

Editing address parameters

Call the dialog box. Place the cursor in the required input box.

■ Enter/edit values, or

■ CONTINUE soft key: The ”Extended input” dialog

box appears

■ Program ”?” (simplified geometry programming).

■ Switch from ”Incremental” to ”Absolute,” or

vice versa.

■ Activate the input of variables.

CNC PILOT only shows the ”Extended inputs” permitted in the respective input

4.2 Basics of Programming

box.

4.2.3 Contour Programming

The ”contour follow-up” function and contour-turning cycles require the previous description of the blank and finished part. For milling and drilling with the C or Y axis, contour definition is a precondition if you wish to use fixed cycles.

Remember with Contours for turning:

■ Describe a continuous contour.

■ The direction of the contour description is

independent of the direction of machining.

■ CNC PILOT closes open contours paraxially.

■ Contour descriptions must not extend beyond the

turning center.

■ The contour of the finished part must lie within the

contour of the blank part.

■ When machining bars, only define the required

section as blank.

■ Contour definitions are valid for the complete NC

program, even if the workpiece is rechucked for machining the rear face.

■ In the fixed cycles you program ”reference values”

referenced to the contour description.

Continued

4 DIN PLUS66

To describe blank parts, use

■ G20 ”Blank part macro” for standard parts (cylinder, hollow

cylinder).

■ G21 ”Cast-part macro” for blank-part contours based on finished-

part contours.

■ Individual contour elements (such as are used for finished-part

contours) if use of G20 or G21 is not possible.

To describe finished parts, use individual contour elements. The contour elements or the complete contour can be assigned attributes which are accounted for during the machining of the workpiece (example: roughness, allowances, etc.).

For intermediate machining steps, define auxiliary contours.Auxiliary contours are programmed in the same way as finished-part descriptions.You can program one contour definition per AUXILIARY CONTOUR. The number of auxiliary contours in a program is not limited.

Contours for machining with the C/Y axis

Contours that are milled or drilled are programmed within the FINISHED PART section. The machining planes are defined as FRONT, FRONT_Y, SURFACE, SURFACE_Y, etc. You can repeatedly use the section codes, or program various contours within one section code.

Up to four contour per NC program

The CNC PILOT support up to four contour groups (workpiece blank and finished part) in one NC program.

The code CONTOUR introduces the description of a contour group. Parameters on zero point shift and the coordinate system define the position of the contour in the working space. A G99 in the machining section assigns the machining to a contour.

Contour generation during simulation:

You can save contours generated in the simulation and insert it in the NC program. Example: You describe the workpiece blank and finished part, and simulate the machining of the first setup. Then you save the contour. You define a shift of the workpiece zero point and/or a mirror image. The simulation saves the ”generated contour” as the workpiece blank and the originally defined finished part contour taking the zero point shift and mirroring into account.

In DIN PLUS, you insert into the program the workpiece blank and finished part contour that you generated during simulation (block menu – ”Insert contour”).

Contour follow-up

CNC PILOT takes the blank part as a basis and accounts for each cut and each cycle of the turning operation when following up the contour. Thus you can inspect the current contour of the workpiece during each machining stage. With the ”contour follow-up” function, the CNC PILOT optimizes the paths for approach and departure and avoids noncutting passes.

4.2 Basics of Programming

HEIDENHAIN CNC PILOT 4290

Continued

The contour follow-up function can also be used for auxiliary contours.

Preconditions for contour follow-up:

■ Definition of blank

■ Proper description of tools (”simple definition of

tools” is not sufficient)

The contour follow-up function can be used only for turning contours; it cannot be used for contours with the C or Y axis.

Contour simulation

During editing CNC PILOT displays programmed contours in up to two graphic windows.

■ Selection of the graphic window: ”Graphic –

Window” menu item

4.2 Basics of Programming

■ Back to machine display: ”Graphic – Graphic OFF”

menu item

Activate graphic window or update the contour

Note:

■ The starting point of the turning contour is marked

by a ”small box.”

■ When the cursor is located on a block of the

”BLANK or FINISHED PART” section the corresponding contour element is highlighted in red and the direction of contour definition is indicated.

■ When programming fixed cycles, you can use the

displayed contour for establishing block references.

■ The CNC PILOT starts at the pattern base when

displaying contours on lateral surfaces (reference diameter for SURFACE).

4.2.4 Tool Programming

The designations of the tool pockets are fixed by the machine tool builder. Each tool holder has a unique T number.

In the ”T command” (MACHINING section) you program the position of the tool holder, and therefore the position to which the tool carrier rotates. The CNC PILOT retrieves the assignment of the tools to the turret positions from the TURRET section, or the tool list (in case the T number is not defined in TURRET).

■ Additions/changes on the contours are not considered

until GRAPHIC is selected again.

■ Unambiguous NC block numbers are a prerequisite for

the ”contour display”!

Continued

4 DIN PLUS68

Multipoint tools

For tools with more than one point (multiple tools) the T number is followed by an „. S”.

T number S S: Number of the cutting edge [0 to 4] (0=main cutter - may be omitted)

In the TURRET section, you define only the main cutting edge.

When a cutting edge of a multiple tool has become dull, the tool life management function marks all cutting edges ”worn-out.”

Examples:

■ T3 or T3.0 – Turret position 3; Main cutting edge

■ T12.2 – position to which the turret rotates 12; cutting point 2

Replacement tools

If you wish to use the Tool life monitoring function, you must define an ”tool interchange chain.” As soon as a tool is worn out, the CNC PILOT interchanges a replacement tool. The CNC PILOT does not stop the program run until the last tool of the tool interchange chain is worn out.

In the TURRET section and the T commands, you program the first tool to be interchanged.The CNC PILOT inserts the replacement tool automatically.

When programming variables (access to tool compensation or tool diagnosis bits), you also address the first tool of the chain. The CNC PILOT automatically addresses the ”active tool.”

3.3.4

You can define replacement tools in ”Setup” (see ”

Tool Life

Management”).

4.2 Basics of Programming

4.2.5 Fixed cycles

HEIDENHAIN recommends programming a fixed cycle in the following steps: (see: ”

■ Insert tool.

■ Define the cutting data.

■ Position the tool in front of the working area.

■ Define the safety clearance.

■ Call a cycle.

■ Retract the tool.

■ Approach the tool change position.

HEIDENHAIN CNC PILOT 4290

4.18.1

Programming a Fixed Cycle”):

Danger of collision!

If cycle-programming steps are omitted when a program is optimized:

■ A special feed rate remains in effect up

to the next feed-rate command (example: finishing feed for recessing cycles).

■ Several cycles return diagonally to the

starting point if you use the standard programming (example: roughing cycles).

4.2.6 NC Subprograms

Subprograms are used to program the contour or the machining process.

In the subprograms, transfer parameters are available as variables. You can fix the designation of the transfer parameter (see ” Subprograms”).

In every subprogram, the variables #256 to #285 are available for internal calculations.

Subprograms can be nested up to six times. This means that a subprogram calls in a further subprogram, etc.

If a subprogram is to be executed repeatedly, enter the number of times the subprogram is to be repeated in the parameter Q.

The CNC PILOT distinguishes between local andexternal

subprograms. Local subprograms and the NC main program are

4.2 Basics of Programming

stored in the same file. Local subprograms can only be called in from their corresponding main programs. External subprograms are stored in separate NC files and can be called in from any NC main program or other NC subprograms.

Expert programs

The machine manufacturer usually provides subroutines, which are tailored to the machine configuration, for complex processes such as workpiece transfer for full-surface machining. (Example: workpiece transfer for full-surface machining). Refer to the machine manual.

4.2.7 Template Control

”Templates” are predefined NC code blocks integrated in the NC program.They reduce programming input and help standardize the program format.

Templates are defined by the machine tool builder. Your machine tool builder can tell you whether he offers templates and how they can be used.

4.16

4.2.8 NC Program Interpretation

For variable programming and user communication, keep in mind that the CNC PILOT interprets the complete NC program before it can be run (see ”

The CNC PILOT differentiates between:

■ #-variables are calculated during the interpretation of the NC

program.

■ V-variables are calculated at runtime, which means during the

execution of an NC block.

■ Input/output during NC program interpretation.

■ Input/output during NC program run.

3.5

Automatic Mode of Operation).

4 DIN PLUS70

4.3 The DIN PLUS Editor

Select menu items

The submenus can be called by

■ Selecting the desired menu items

■ Positioning the cursor in the program section

From the submenu back to the main menu

When you call the menu items ”Geometry,” ”Processing,” ”Turret assignment” or ”Chucking equipment,” the CNC PILOT jumps to the corresponding program section. - When you position the cursor in the BLANK, FINISHED PART or MACHINING section, the CNC PILOT switches to the corresponding submenu.

Creating NC blocks

The insertion of new NC blocks varies depending on the program section.

■ After the ”Editing program head” dialog box has been concluded,

the CNC PILOT automatically creates the blocks of the program head (code ”#”).

■ In the TURRET and CHUCKING EQUIPMENT sections, you can

insert a new block by pressing the INS key.

■ When you program a contour or a machining process, or within a

subprogram, the CNC PILOT automatically creates new NC blocks. Alternately, you can add NC blocks by pressing the INS key.

The new NC block is inserted below the cursor position.

Deleting elements of an NC block

Position the cursor on an element of the NC block (NC block

number, G or M command, address parameter, etc.), or the section code.

Press the DEL key. The element highlighted by the cursor and all

the related elements are deleted. (Example: If the cursor is located on a G command, the address parameters are also deleted.)

4.3The DIN PLUS Editor

Before deleting a complete NC block, CNC PILOT displays a confirmation request. Individual elements of an NC block including G or M functions are deleted immediately.

Editing elements of an NC block

Position the cursor on an element of the NC block (NC block

number, G or M command, address parameter, etc.), or the section code.

Press ENTER or double-click with the left mouse key. The CNC

PILOT activates a dialog box which displays the block number, the number of the G or M function, or the address parameters of the G function, which can then be edited.

When you edit NC words (G, M, T), the CNC PILOT additionally activates a dialog box for editing the address parameters.

When editing section codes, you can only change the associated parameters (Example: Number of the turret).

Continued

HEIDENHAIN CNC PILOT 4290

”Conversational” or ”free” editing

You usually select the NC functions from the menus and edit the address parameters in dialog boxes. You can also select ”Free input” (”NC Bl” pull-down menu) and edit the NC program. For ”free editing,” the maximum length of a block is 128 characters per line.

Block references

When editing G commands related to the contour (MACHINING section), you can switch to contour simulation and select the block references from the contour displayed, using the arrow keys.

G commands

The G commands are divided into:

■ Geometry commandsfor describing the blank and finished part.

You can use additional ”auxiliary commands” (allowance, surface quality, etc.) to influence the machining process.

4.3The DIN PLUS Editor

■ Machining commands for the MACHINING section.

4.3.1 Main Menu

”Prog” pull-down menu (NC program management):

■ Load – loads stored NC programs:

The CNC PILOT displays existing NC main programs or

subprograms.

Select the NC program

■ New – creates new NC main programs or subprograms:

Enter a program name. Select main program or subprogram. To activate the ”Editing program head” window, select ”Program

head.”

■ Close – Closes the selected NC program without saving it

■ Save – Saves the selected NC program – the program stays open

for editing

■ Save as – Saves the selected NC program under a given name

”Do not close/Close”: Select whether to close the editing window

or leave it open to continue editing the NC program

”Save as ...”: Enter the program name

■ Save all – Saves all loaded NC programs

Some G functions are used for blank/ finished-part definition and in the MACHINING section. When copying or shifting NC blocks, keep in mind that ”geometry” functions are used only for describing a contour, while ”machining” functions are used only in the MACHINING section.

When you exit ”DIN PLUS” operating mode, the NC programs are saved automatically. The old version of the NC program is overwritten.

”Head” pull-down menu (NC program head):

■ Program head: activates the ”Editing program head” dialog box.

■ Turret assignment: positions the cursor in the TURRET section.

■ Chucking equipment: positions the cursor in the CHUCKING

EQUIPMENT section.

Continued

4 DIN PLUS72

”Geometry” pull-down menu (contour programming):

■ Blank – Chuck piece/bar G20: creates an NC

block in the BLANK section, switches to the ”Geometry” menu and activates the ”Chuck part cylinder/tube G20” dialog box.

■ Blank – Casting G21: creates an NC block in the

BLANK section, switches to the ”Geometry” menu and activates the ”Casting G21” dialog box.

■ Blank – Free contour: positions the cursor in the

BLANK section and switches to the Geometry menu.

■ Finished part: positions the cursor in the

FINISHED PART section and switches to the Geometry menu.

Single menu items

■ Programming: switches to the Machining submenu

and positions the cursor in the MACHINING section.

■ PAb (Program Section codes) – inserts new section

codes:

Select the desired section code and press

ENTER.

The CNC PILOT inserts the section code at the

correct position.

■ Block: switches to the block-editing functions (see

4.5.5

section ”

Block menu”).

”NC Bl” pull-down menu

■ Program beginning Positions the cursor to the

beginning of the program

■ Program end: Positions the cursor to the program

end

■ Search function - Search block

Enter the block number. The CNC PILOT positions the cursor on the block

number provided that it exists.

■ Search function - Search word

Enter the NC word to be searched for ( G

command, address parameter, etc.).

The cursor skips to the first NC block containing the word searched for. The CNC PILOT searches from the cursor position to the end of the program, then continues searching from the start of the program.

■ Increment Numerical interval between NC blocks

The increment entered remains in effect for the active NC program only.

4.3The DIN PLUS Editor

DIN PLUS main menu

Prog (NC program management)

Head: Edit the NC program head (program head, turret

assignment, chucking equipment table)

Geo: Program the contour of the blank and finished part (submenu ”Geometry”)

Pro(gramming): Program the machining of the workpiece (”Machining” submenu)

PA b: Insert program section codes

Block: Switch to the block submenu containing functions

for moving, copying or deleting NC blocks

NC Bl: Functions for block numbering, searching and ”free” editing

Configuration of the DIN PLUS screen display (with/ without graphical display)

Graphics: Select graphic simulation window, switch the contour simulation ON/OFF

HEIDENHAIN CNC PILOT 4290

Continued

■ Block numbering: The number ”interval” is specified for the first

NC block; for each following block the ”interval” is added. Block references in contour-related G commands and subprogram calls are corrected automatically. The sequence of the NC blocks is retained.

■ New: free input

Position the cursor. Select ”New: free input.” Enter NC block The new NC block is inserted below the cursor position.

■ Modify: free input

Position the cursor on the NC block to be edited.

4.3The DIN PLUS Editor

Select ”New: modified input.” Edit the NC block

”Config(uration)” menu group:

■ Aux. pict.:Select whether you wish to display the help graphics.

■ Window – Full-size window/Double window/Triple window:

Select the number of editing windows

■ Font size – smaller/larger: Change the font size within the editing

window

■ Font size – Adjust fonts: Set the font size of the selected window

in all editing windows

■ Settings – Save: Saves the current editor condition (window

setting, all loaded NC programs)

■ Settings – Load: Loads the lasts save condition of the editor

■ Settings – Auto-save on: Saves the current editor condition when

CNC PILOT is switched off

■ Settings – Auto-save off: No saving of the editor condition when

the CNC PILOT is switched off

”Graphics” pull-down menu

■ Graphic ON: activates contour simulation.

■ Graphic - OFF: deactivates contour simulation and activates the

machine display.

■ Window (selection of simulation window): Select a maximum of

two windows. The contour simulation is activated by selecting ”Graphic ON.”

4 DIN PLUS74

4.3.2 Geometry Menu

The ”Geometry” submenu contains G functions and instructions for the BLANK and FINISHED PART sections.

Selecting a G function:

■ The G number is known: Select ”G” and enter the

number.

■ The G number is not known:

Select ”G.”

Press the CONTINUE soft key

Select the G function from the list of G numbers

■ ”G menu”: To select the desired G function, use the

pull-down menu.

”Instr(uctions)” pull-down menu:

■ DIN PLUS words – calls selection list containing:

■ Instructions for structuring the program.

■ Instructions for input/output.

■ Section codes for contours with the C/Y axis.

■ Variables – Enter a variable or mathematical

expression

■ FRONT, SURFACE, REAR SIDE

The dialog box for entering the contour position (reference plane/reference diameter) appears.

Enter the Z position/diameter

The CNC PILOT inserts the section code below the position of the cursor.

■ AUXILIARY CONTOUR (TEMPORARY) – inserts

the section code below the position of the cursor.

■ Comment line – Enter a comment. The comment

is inserted above the position of the cursor.

Single menu item:

■ Graphic – Activates/deactivates contours in the

graphic window.

4.3The DIN PLUS Editor

Geometry submenu

G: Direct input of the G number / Calls the G list

Line: Activates the G1 Geo dialog box

CirClockwise arc, counterclockwise with incremental or ab-

solute center dimensioning

Form Elements of the contour, subprogram call, reference plane for pocket/island

Attributes (auxiliary commands) for contour definition

Front: Basic elements, figures or patterns of the contour

on the front or rear face (machining with the C axis)

HEIDENHAIN CNC PILOT 4290

Surface: Basic elements, figures or patterns on the lateral surface (machining with the C axis)

Instructions for structuring the program and for section codes

Graphics: Activate/update the contour in the graphic simulation windows

4.3.3 Machining Menu

The ”Machining” submenu contains G and M functions as well as further functions for the MACHINING section.

Selecting a G function:

■ The G number is known: Select ”G” and enter the

number.

■ The G number is not known:

Select ”G.” Press the CONTINUE soft key Select the G function from the list of G numbers

■ ”G menu”: To select the desired G function, use the

pull-down menu.

4.3The DIN PLUS Editor

Selecting an M function:

■ The M number is known: Select ”M” and enter the

number.

■ M menu: To select the M function, use the menu.

Single menu items

■ T – Tool call

Program the T number (see ”

4.6.7

Tools, Types of Compensation”). A list containing the tools indicated in the TURRET section is displayed.

■ F- calls ”G95 - ”Feed per revolution.”

■ S- calls ”G96 – Cutting speed.”

”Instr(uctions)” pull-down menu:

■ DIN PLUS words – calls selection list containing:

■ Instructions for structuring the program.

■ Instructions for input/output. n

■ Variables – Enter a variable or mathematical

expression

■ / Skip level

Enter skip level 1 to 9. The CNC PILOT inserts the skip level before the

NC block (example: /3 N 100 G...).

■ $ Slide:

Enter the ”Slide number”; more than one slide

number -one after the other- can be entered.

The DIN editor inserts the slide number before the

NC block (example: $1$2 N 100 G...).

Machining submenu

G: Enter number of G function/call the list of G functions

G menu: Pull-down menus containing G functions appear

M: Enter the M number

M Menu: Opens pull-down menus containing M functions

T:Tool call

F: Call ”G95 - ”Feed per revolution”

S: Calls ”G96 – Cutting speed”

Instructions for structuring the program

Graphics: Activate/update the contour in the graphic

simulation windows

Continued

4 DIN PLUS76

■ L call external – (see ”

4.16

Subprograms”). Select the subprogram and press RETURN Enter the transfer parameters. The CNC PILOT inserts the subprogram call.

■ L call internal – (see ”

4.16

Subprograms”).

Enter the name of the subprogram (number of the

first block of the subprogram).

Enter the transfer parameters. The CNC PILOT inserts the subprogram call.

■ Comment line

Enter the comment – the comment is inserted

above the cursor position.

■ Template selection – Select from the available

templates. Prerequisite:The machine manufacturer has defined templates

■ The working plan – ”collects” all comments that

begin with ”// ...” and places them before the MACHINING section. This gives you a summary of the functions in the NC program or subprogram.

Menu item:

■ Graphic – Activates/deactivates contours in the

graphic window.

4.3.4 Block Menu

This function enables NC program sections (several successive NC blocks) to be moved, copied, deleted or exchanged between NC programs.

To define an NC block, highlight the first and last line of the block. Then select the desired function from the ”Edit” menu.

In order to exchange blocks between NC programs, copy the block to the clipboard. Then read in the block from the clipboard. A block remains in the clipboard until it is overwritten by another block.

Single menu items

■ Start Mark:

Position the cursor on the beginning of a block. Press ”Start mark.”

■ End mark:

Position the cursor on the end of a block. Press ”End mark.”

4.3The DIN PLUS Editor

Continued

HEIDENHAIN CNC PILOT 4290

”Edit” pull-down menu

■ Cut:

■ Stores the highlighted block in the clipboard.

■ Deletes the block.

■ Copy to clipboard – copies the highlighted block to the clipboard.

■ Paste from clipboard:

Position the cursor where you wish to insert the block. Select ”Paste from clipboard.” The block is inserted at the position indicated by the cursor.

■ Delete – deletes the highlighted block definitively (it is not stored in

the clipboard).

■ Displace:

Position the cursor where you wish to insert the block. Select ”Displace.”

4.3The DIN PLUS Editor

The highlighted block is moved from its initial position to the

position indicated by the cursor.

■ Copy and paste:

Position the cursor where you wish to insert the block. Select ”Copy and paste.” The block is inserted at/copied to the position indicated by the

cursor.

Single menu items

■ Cancel – all markings are canceled.

■ Insert contour – inserts the most recent workpiece blank and

finished part contour in the simulation below the cursor position

As an alternative of the block menu, you can use the usual WINDOWS key combinations for marking, deleting, shifting etc.:

■ Marking by moving the cursor keys while holding the shift key.

■ Ctrl + C: Copy the marked text to the clipboard

■ Shift + Del(ete): Delete the marked text and save it in the clipboard

■ Ctrl + V: Insert text from the clipboard at the cursor position

■ Del(ete): Delete the marked text

4 DIN PLUS78

4.4 Program Section Codes

A new DIN program is already provided with section codes. You can add new codes or delete existing ones, depending on your program requirements. A DIN program must contain at least the MACHINING and END section codes.

Overview of program section codes

PROGRAMMKOPF [PROGRAM HEAD] TURRET MAGAZINE CHUCKING EQUIPMENT KONTUR [CONTOUR] ROHTEIL [BLANK] FERTIGTEIL [FINISHED PART] HILFSKONTUR [AUXILIARY CONTOUR] BEARBEITUNG [MACHINING] ENDE [END] UNTERPROGRAMM [SUBPROGRAM] RETURN

4.4 Program Section Codes

Machining with the C axis

FRONT REAR SIDE SURFACE

4.4.1 PROGRAMMKOPF [PROGRAM HEAD]

The PROGRAM HEAD comprises:

■ Slides: NC program is run only on the given slides

(input:„$1, $2, ...”) – no input: NC program is run for every slide.

■ Unit: Unit of measure ”metric/inches” – no input:

The unit of measure defined in control parameter 1 is used

■ The other codes containorganizational

information and set-up information that do not

influence the program run.

Information contained in the program head is preceded by ”#” in the DIN program.

The ”Unit” can be programmed only when a new program is being created (set under PROGRAM HEAD). It is not possible to post-edit this entry.

HEIDENHAIN CNC PILOT 4290

Definition of the variable display

Call: ”Variable display” button in the ”Editing program

head” dialog box

In the dialog box you define up to 16 V variables that control the program process. In automatic mode and in the simulation you define whether the variables are to be asked for during program run. As an alternative, the program version is run with the default values.

For each variable you define:

■ Variable number

■ Default value (initialization value)

■ Description (text, with which this variable is

asked for during program run)

The definition of the variable display is an alternative to programming with INPUTA/PRINTA commands.

4.4 Program Section Codes

4.4.2 TURRET

TURRET x (x: 1..6) defines the turret assignment of tool carrier x. You enter the ID number directly (”Tools” dialog box), or you take it from the tool database. You can access the tool database with the ”Type list” or ”ID list” soft key.

Alternately, you can define the tool parameters in the NC program.

Enter the tool data:

„ Select ”Head – Turret assignment.” Position the cursor in the TURRET section. Press the INS key. Edit the ”Tool” dialog box.

Edit the tool data:

Position the cursor. Press RETURN or double-click with the left mouse

key

Edit the ”Tool” dialog box.

Parameters of the ”Tool” dialog box:

■ T-number: Position on the tool carrier.

■ ID (ID number): Reference to the database – no

input: Data saved in the database as ”temporary tools.”.

Continued

Access to the tool database by soft key

Edit the tool parameters

Entries in the tool database - sorted by tool type

Entries in the tool database - sorted by tool ID number

4 DIN PLUS80

Extended input:

No constraints for the use of the tool.

Only the tool tip is shown in the simulation.

First you define the tool type, then you edit the tool parameters.

The tool parameters are shown in the parameters of the first dialog

8.1

box to the tool editor (see ”

The data are saved in the database during program compilation

Tool Database).

only if you enter the ID number.

Simple tool:

Only suitable for simple traverse paths and turning cycles

(G0...G3, G12, G13; G81...G88).

No contour regeneration.

Tooth/cutter radius compensation.

Simple tools are not included in the database.

For the meaning of the parameters, refer to the table below.

Simple tools Dialog box NC program Meaning

Tool type WT Tool type and machining direction

X dimension (xe) X Setup dimension

Y dimension (ye) Y Setup dimension

Z dimension (ze) Z Setup dimension

Radius R (rs) R Cutting radius of turning tools

Cutting width B (sb) B Cutting width of recessing and button tools

Diameter I (df) I Milling or drilling diameter

Example: TURRET -- Table REVOLVER 1 [TURRET]

T1 ID”342-300.1” [Tool from the database]

T2 WT1 X50 Z50 R0.2 B6 [simple tool description]

T3 WT122 X15 Z150 H0 V4 R0.4 A93 C55 I9 K70 [extended

tool description – not transferred to database]

■ If you do not program the TURRET,

the tools entered in the ”tool list” are used

3.3.1

(see ”

■ The names ”_SIM...” and ”_AUTO...”

Setting Up the Tool List”).

are reserved for temporary tools (simple tools and tools without ID number). Tool entries are valid as long as the NC program is activated in the simulation or Automatic mode.

4.4 Program Section Codes

T4 ID”Erw.1” WT112 X20 Z150 H2 V4 R0.8A95 C80 B9 K70

[extended tool description – with transfer to database]

. . .

HEIDENHAIN CNC PILOT 4290

4.4.3 CHUCKING EQUIPMENT

CHUCKING EQUIPMENT x (x: 1 to 4) defines spindle assignment x. Using the identification numbers of chuck, jaws and adapters (lathe center, etc.), you create the chucking equipment table. It is evaluated in the simulation (G65).

Enter chucking equipment data:

„ Select ”Header – Chucking equipment” Position the cursor in the CHUCKING EQUIPMENT section. Press the INS key. Edit the ”Chucking equipment” dialog box.

Edit the CHUCKING EQUIPMENT data:

Position the cursor. Press ENTER

4.4 Program Section Codes

Edit the ”Chucking equipment” dialog box.

Parameters of the ”Chucking equipment” dialog box:

H: Number of chucking equipment (reference to G65).

■ H=1: Chuck

■ H=2: Jaw

■ H=3: Adapter - spindle

■ H=4: Adapter - tailstock

ID: Identification number of chucking equipment (reference to

database). X: Gripping diameter of jaws Q: Chuck form of jaws (see G65)

The chucking equipment table is used for the simulation graphics – it does not influence the execution of the program.

Example: CHUCKING EQUIPMENT table SPANNMITTEL 1 [CHUCKING EQUIPMENT]

H1 ID”KH250” H2 ID”KBA250-77”

. . .

4.4.4 Contour Definition

KONTUR [CONTOUR]

Assigns the following workpiece blank and finished part description to a contour.

Parameters

Q: Number of the contour – 1..4 X, Z: Zero point shift (reference: machine zero) V: Position of the coordinate system

■ 0: The machine coordinate system applies

■ 2: Mirrored machine coordinate system (Z direction opposite

to the machine coordinate system)

4 DIN PLUS82

ROHTEIL [BLANK]

Program section for defining the contour of the blank part.

FERTIGTEIL [FINISHED PART]

Program section for defining the contour of the finished part. To define the finished part, use additional section codes such as FRONT, SURFACE, etc.

FRONT, REARSIDE

designates contours on the front and rear face

Parameters

Z: Position of the contour on the front/rear face – default: 0

SURFACE

identifies contours on the lateral surface.

Parameters

X: Reference diameter of lateral-surface contours.

HILFSKONTUR [AUXILIARY CONTOUR]

designates further turning contours (intermediate contours).

For several independent contour definitions for drilling/milling, use the program section codes (FRONT END, REAR END, etc.).

Examples for section codes in the finished part definitions . . . ROHTEIL [BLANK]

N1 G20 X100 Z220 K1

FERTIGTEIL [FINISHED PART]

N2 G0 X60 Z-80 N3 G1 Z-70

. . . STIRN Z-25 [FRONT]

N31 G308 P-10 N32 G402 Q5 K110 A0 Wi72 V2 XK0 YK0 N33 G300 B5 P10 W118 A0 N34 G309

STIRN Z0 [FRONT]

N35 G308 P-6 N36 G307 XK0 YK0 Q6 A0 K34.641 N37 G309

. . .

4.4 Program Section Codes

4.4.5 BEARBEITUNG [MACHINING]

Program section for machining a workpiece. This code must be programmed.

ENDE [END]

Ends your NC program. This code must be programmed. It replaces M30.

4.4.6 UNTERPROGRAMM [SUBPROGRAM]

If you define a subprogram within your NC program (within the same file), it is designated with SUBPROGRAM, followed by the name of the subprogram (max. 8 characters).

RETURN

ends your NC subprogram.

HEIDENHAIN CNC PILOT 4290

4.5 Geometry Commands

4.5.1 Definition of Blank

Chuck piece: bar/tube G20 Geo

Contour of a cylinder/hollow cylinder.

Parameters

■ Diameter of a cylinder hollow cylinder

■ Diameter of circumference of a polygonal blank

Z: Length of blank K: Right edge (distance between workpiece zero point and right

edge) I: Inside diameter for hollow cylinders

4.5 Geometry Commands

Cast part G21 Geo

Generates the workpiece blank contour from the finished part contour – plus the ”equidistant allowance P.”

Parameters

P: Equidistant finishing allowance (reference: finished part contour) Q: Bore holes yes/no – default: Q=0

■ Q=0: Without bore holes

■ Q=1: With bore holes

4.5.2 Basic Contour Elements

Starting point of turning contour G0 Geo

Starting point of a turning contour.

Parameters

X, Z: Starting point of the contour (X diameter)

4 DIN PLUS84

Line segment in a contour G1-Geo

Parameters

X, Z: End point of contour element (X diameter) A: Angle to rotary axis – for angle direction see graphic support

window

Q: Selection of intersection – default: 0. End point, if the line

segment intersects a circular arc.

■ Q=0: near intersection

■ Q=1: distance intersection

B: Chamfer/rounding arc – transition to the next contour element.

Program the theoretical end point when you enter a chamfer/ rounding arc.

■ No entry in B: tangential transition

■ B=0: no tangential transition

■ B>0: Radius of the rounding arc

■ B<0: Width of chamfer

E: Special feed factor for chamfer/rounding arc in a finishing cycle

(0 < E <= 1) – default: 1 (special feed rate = active feed rate * E)

Circular arc in a contour

G2/G3 Geo – incremental center coordinates G12/G13 Geo – absolute center coordinates

Direction of rotation: see help graphic

Parameters

X, Z: End point of contour element (X diameter) R: Radius Q: Selection of intersection – default: 0. End point, if the circular arc

intersects a circular arc.

■ Q=0: Far intersection

■ Q=1: Near intersection

B: Chamfer/rounding arc – transition to the next contour element.

Program the theoretical end point when you enter a chamfer/ rounding arc.

■ No entry in B: tangential transition

■ B=0: no tangential transition

■ B>0: Radius of the rounding arc

■ B<0: Width of chamfer

E: Special feed factor for chamfer/rounding arc in a finishing cycle

(0 < E <= 1) – default: 1 (special feed rate = active feed rate * E)

4.5 Geometry Commands

Programming X, Z: Absolute,

incremental, modal or ”?”

G2 Geo

G2/G3 – incremental center:

I: Center (distance from starting point to center as radius) K: Center (distance from starting point to center)

G12/G13 – absolute center:

I: Center (radius) K: Center

Programming X, Z: Absolute, incremental, modal or ”?”

HEIDENHAIN CNC PILOT 4290

G13 Geo

4.5.3 Contour Form Elements

Recess (Standard) G22 Geo

Recess on a paraxial reference element (G1). G22 is assigned to the previously programmed reference element.

Parameters

X: Starting point of recess on the face (diameter) Z: Starting point of recess on the lateral surface I, K: Inside corner

■ I – recess on face: Recess end point (diameter value)

■ I – recess on lateral surface: Recess base (diameter value)

■ K – recess on face: Recess base

■ K – recess on lateral surface: Recess end point

Ii, Ki: Inside corner – incremental (pay attention to sign!)

4.5 Geometry Commands

■ Ii – recess on face: Recess width

■ Ii – recess on lateral surface: Recess depth

■ Ki – recess on face: Recess depth

■ Ki – recess on lateral surface: Recess end point (recess

width) B: Outside radius/chamfer (at both ends of the recess) – default: 0

■ B>0: Radius of rounding

■ B<0: Width of chamfer

R: Inside radius (in both corners of recess) – default: 0

Program either ”X” or ”Z”.

Recess (general) G23-Geo

Recess on a linear reference element (G1). G23 is assigned to the previously programmed reference element. On the lateral surface, the recess can be positioned on an inclined reference straight.

Parameters

H: Recess type – default: 0

■ H=0: Symmetrical recess

■ H=1: relief turn

X: Center point of recess on the end face (diameter) Z: Center point of recess on the lateral surface I: Recess depth and position

■ I>0: Recess to right of reference element

■ I<0: Recess to left of reference element

K: Recess width (without chamfer/rounding) U: Recess diameter (diameter of recess base) – use only if the

reference element runs parallel to the Z axis A: Recess angle – default: 0

■ With H=0: 0° <= A < 180° (angle between edges of recess)

■ With H=1: 0° < A <= 90° (angle between reference straight

and recess edge)

Continued

Simple recess

4 DIN PLUS86

B: Outside radius/chamfer; starting point near corner - default: 0

■ B>0: Radius of rounding

■ B<0: Width of chamfer

P: Outside radius/chamfer; starting point distant from corner -

default: 0

■P>0: Radius of rounding

■ P<0: Width of chamfer

R: Inside radius (in both corners of recess) – default: 0

The CNC PILOT refers the recess depth to the reference element. The recess base runs parallel to the reference element.

Thread with undercut G24-Geo

Linear base element with linear thread (external or internal thread; metric ISO fine-pitch thread DIN 13 Part 2, Series 1) and a subsequent thread undercut (DIN 76).

Calling the contour macro:

N..G1 X..Z..B.. /Starting point for thread N..G24 F..I..K..Z.. /Contours for thread and undercut N..G1 X.. /Next surface element

Parameters

F: Thread pitch I: Depth of undercut (radius) K: Width of undercut Z: End point of the undercut

Recess or free rotation

4.5 Geometry Commands

■ Use G24 only if the thread is cut in the definition

direction of the contour.

■ The thread is machined with G31.

HEIDENHAIN CNC PILOT 4290

Undercut contour G25-Geo

Generates the following undercut contours in paraxial inside contour corners. Program G25 after the first axis-parallel element.

Parameters

H: Type of undercut – default: 0

■ H=4: Undercut type U

■ H=0, 5: Undercut type DIN 509 E

■ H=6: Undercut type DIN 509 F

■ H=7: Thread undercut DIN 76

■ H=8: Undercut type H

■ H=9: Undercut type K

4.5 Geometry Commands

Undercut form U (H=4)

Parameters

I: Depth of undercut (radius) K: Width of undercut R: Inside radius (in both corners of recess) – default: 0 P: Outside radius/chamfer – default: 0

■ P>0: Radius of rounding

■ P<0: Width of chamfer

Calling the contour macro (example):

N..G1 Z.. /longitudinal element

N..G25 H..I..K.. .. /Undercut contour

N..G1 X.. /Next surface element

Undercut DIN 509 E (H=0, 5)

Parameters

I: Depth of undercut (radius) K: Width of undercut R: Undercut radius (in both corners of the undercut) W: Undercut angle

If you do not enter parameters, the CNC PILOT calculates them from

11.1.2

the diameter (see ”

Undercut Parameters DIN 509 E”).

Continued

4 DIN PLUS88

HEIDENHAIN CNC Pilot 4290 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual