heidenhain TNC 310 Programming Manual

Download

TNC 310

NC Software 286 140-xx 286 160-xx

User's Manual

HEIDENHAIN Conversational

Programming

English (en)

4/2003

Controls on the visual display unit

Split screen layout

Numerical input, editing

... Numbers

Soft keys

Shift the soft-key rows

Machine control keys

Axis direction

Controls on the TNC

Rapid traverse

Direction of spindle rotation

Coolant

Tool release

Spindle ON/OFF

NC start/NC stop

Override control knobs for feed rate/spindle speed

100

S %

100

F %

Mode of operation

Manual Operation

Decimal point

Change arithmetic sign

Confirm entry and resume dialog

End block

Clear numerical entry or TNC error message

Abort dialog, delete program section

Programming aids

MOD functions

HELP function

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

Move highlight

Move highlight, skip dialog question

Select blocks and cycles directly

Positioning with Manual Data Input (MDI)

Program Run/Test Run

Programming and Editing

TNC Models, Software and Features

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

TNC Model NC Software No.

TNC 310 286 140-xx TNC 310 M 286 160-xx

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

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

■ Probing function for the 3-D touch probe

■ Rigid tapping cycle

■ Boring cycle

■ Back boring cycle

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

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

Contents

Location of use

The TNC complies with the limits for a Class A device in accordance with the specifications in EN 55022, and is intended for use primarily in industrially-zoned areas.

IHEIDENHAIN TNC 310

Contents

Introduction

Manual Operation and Setup

Positioning with Manual Data Input (MDI)

Programming: Fundamentals, File Management, Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Cycles

Programming: Subprograms and Program Section Repeats

Programming: Q Parameters

Test Run and Program Run

3-D Touch Probes

Contents

3 4 5 6 7 8

9 10 11 12

MOD Functions

Tables and Overviews

13 14

IIIHEIDENHAIN TNC 310

1 INTRODUCTION.....1

1.1 The TNC 310.....2

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

Contents

1.3 Modes of Operation.....4

1.4 Status Displays.....7

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels.....11

2 MANUAL OPERATION AND SETUP.....13

2.1 Switch-On.....14

2.2 Moving the Machine Axes.....15

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

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

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

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

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

4.1 Fundamentals of NC.....26

4.2 File management.....31

4.3 Creating and Writing Programs.....34

4.4 Interactive Programming Graphics.....39

4.5 HELP function.....41

5 PROGRAMMING: TOOLS.....43

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

5.2 Tool Data.....45

5.3 Tool Compensation.....51

Contents

6 PROGRAMMING: PROGRAMMING CONTOURS.....55

6.1 Overview of Tool Movements.....56

6.2 Fundamentals of Path Functions.....57

6.3 Contour Approach and Departure.....60

Overview: Types of paths for contour approach and departure.....60

Important positions for approach and departure.....60

Approaching on a straight line with tangential connection: APPR LT.....62

Approaching on a straight line perpendicular to the first contour point: APPR LN.....62

Approaching on a circular arc with tangential connection: APPR CT.....63

Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT.....64

Departing tangentially on a straight line: DEP LT.....65

Departing on a straight line perpendicular to the last contour point: DEP LN.....65

Departing tangentially on a circular arc: DEP CT.....66

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT.....67

6.4 Path Contours — Cartesian Coordinates.....68

Overview of path functions.....68

Straight line L.....69

Inserting a chamfer CHF between two straight lines.....69

Circle center CC.....70

Circular path C around circle center CC.....71

Circular path CR with defined radius.....72

Circular path CT with tangential connection.....73

Corner Rounding RND.....74

Example: Linear movements and chamfers with Cartesian coordinates.....75

Example: Circular movements with Cartesian coordinates.....76

Example: Full circle with Cartesian coordinates.....77

6.5 Path Contours—Polar Coordinates.....78

Polar coordinate origin: Pole CC.....78

Straight line LP.....79

Circular path CP around pole CC.....79

Circular path CTP with tangential connection.....80

Helical interpolation.....81

Example: Linear movement with polar coordinates .....83

Example: Helix .....84

Contents

VHEIDENHAIN TNC 310

7 PROGRAMMING: MISCELLANEOUS FUNCTIONS.....85

7.1 Entering Miscellaneous Functions M and STOP.....86

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant.....87

Contents

7.3 Miscellaneous Functions for Coordinate Data.....87

7.4 Miscellaneous Functions for Contouring Behavior.....89

7.5 Miscellaneous Function for Rotary Axes.....92

8 PROGRAMMING: CYCLES.....93

8.1 General Overview of Cycles.....94

8.2 Drilling Cycles.....96

PECKING (Cycle 1).....96

DRILLING (Cycle 200).....98

REAMING (Cycle 201).....99

BORING (Cycle 202).....100

UNIVERSAL DRILLING (Cycle 203).....101

BACK BORING (Cycle 204).....103

TAPPING with a floating tap holder (Cycle 2).....105

RIGID TAPPING (Cycle 17).....106

Example: Drilling cycles.....107

Example: Drilling cycles .....108

8.3 Cycles for Milling Pockets, Studs and Slots.....109

POCKET MILLING (Cycle 4).....110

POCKET FINISHING (Cycle 212).....111

STUD FINISHING (Cycle 213).....113

CIRCULAR POCKET MILLING (Cycle 5).....114

CIRCULAR POCKET FINISHING (Cycle 214).....116

CIRCULAR STUD FINISHING (Cycle 215) .....117

SLOT MILLING (Cycle 3).....119

SLOT with reciprocating plunge-cut (Cycle 210).....120

CIRCULAR SLOT with reciprocating plunge-cut (Cycle 211) .....122

Example: Milling pockets, studs and slots.....124

Contents

8.4 Cycles for Machining Hole Patterns.....126

CIRCULAR PATTERN (Cycle 220).....127

LINEAR PATTERN (Cycle 221) .....128

Example: Circular hole patterns.....130

8.5 Cycles for multipass milling.....132

MULTIPASS MILLING (Cycle 230).....132

RULED SURFACE (Cycle 231).....134

Example: Multipass milling.....136

8.6 Coordinate Transformation Cycles .....137

DATUM SHIFT (Cycle 7).....138

DATUM SHIFT with datum tables (Cycle 7).....138

MIRROR IMAGE (Cycle 8).....140

ROTATION (Cycle 10).....141

SCALING FACTOR (Cycle 11) .....142

Example: Coordinate transformation cycles.....143

8.7 Special Cycles .....145

DWELL TIME (Cycle 9) .....145

PROGRAM CALL (Cycle 12).....145

ORIENTED SPINDLE STOP (Cycle 13) .....146

Contents

9 PROGRAMMING: SUBPROGRAMS AND PROGRAM SECTION REPEATS.....147

9.1 Labeling Subprograms and Program Section Repeats.....148

9.2 Subprograms.....148

9.3 Program Section Repeats.....149

9.4 Nesting.....151

Subprogram within a subprogram .....151

Repeating program section repeats.....152

Repeating a subprogram.....153

Example: Milling a contour in several infeeds .....154

Example: Groups of holes .....155

Example: Groups of holes with several tools .....156

VIIHEIDENHAIN TNC 310

10 PROGRAMMING: Q PARAMETERS.....159

10.1 Principle and Overview.....160

10.2 Part Families — Q Parameters in Place of Numerical Values.....161

Contents

10.3 Describing Contours through Mathematical Operations.....162

10.4 Trigonometric Functions .....164

10.5 If-Then Decisions with Q Parameters .....165

10.6 Checking and Changing Q Parameters .....166

10.7 Additional Functions .....167

10.8 Entering Formulas Directly.....173

10.9 Preassigned Q Parameters.....176

10.10 Programming Examples.....178

Example: Ellipse.....178

Example: Concave cylinder machined with spherical cutter .....180

Example: Convex sphere machined with end mill .....182

11 TEST RUN AND PROGRAM RUN.....185

11.1 Graphics.....186

11.2 Test run.....190

11.3 Program Run.....192

11.4 Blockwise Transfer: Running Longer Programs.....199

11.5 Optional Program Run Interruption.....200

12 3-D TOUCH PROBES.....201

12.1 Touch Probe Cycles in the Manual Operation Mode.....202

Calibrating a touch trigger probe.....203

Compensating workpiece misalignment.....204

12.2 Setting the Datum with a 3-D Touch Probe.....205

12.3 Measuring Workpieces with a 3-D Touch Probe.....208

VIII

Contents

13 MOD FUNCTIONS.....211

13.1 Selecting, Changing and Exiting the MOD Functions.....212

13.2 System Information.....212

13.3 Entering the Code Number.....213

13.4 Setting the Data Interface.....213

13.5 Machine-Specific User Parameters.....216

13.6 Position Display Types.....216

13.7 Unit of Measurement.....216

13.8 Axis Traverse Limits .....217

13.9 Running the HELP File.....218

14 TABLES AND OVERVIEWS.....219

14.1 General User Parameters.....220

Input possibilities for machine parameters.....220

Selecting general user parameters.....220

External data transfer.....221

3-D Touch Probes.....222

TNC displays, TNC editor.....222

Machining and program run.....224

Electronic handwheels.....225

14.2 Pin Layout and Connecting Cable for the Data Interface.....226

RS-232-C/V.24 Interface .....226

14.3 Technical Information.....227

TNC features.....227

Programmable functions.....228

TNC Specifications.....228

14.4 TNC Error Messages.....229

TNC error messages during programming.....229

TNC error messages during test run and program run.....229

14.5 Exchanging the Buffer Battery.....232

Contents

IXHEIDENHAIN TNC 310

Introduction

1.1 The TNC 310

HEIDENHAIN TNC controls are shop-floor programmable contouring controls for milling, drilling and boring machines.

You can program conventional milling, drilling and boring operations right at the machine with the easily understandable interactive conversational guidance. The TNC 310 can control up to 4 axes. Instead of the fourth axis, you can also change the angular position of the spindle under program control.

1.1 The TNC 310

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

Programming: HEIDENHAIN conversational format

HEIDENHAIN conversational programming is an especially easy method of writing programs. Interactive graphics illustrate the individual machining steps for programming the contour. Workpiece machining can be graphically simulated during test run.

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

Compatibility

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

In addition, the TNC can also run programs with functions that cannot be programmed directly on the TNC 310 itself, such as:

■ FK free contour programming

■ Contour cycles

■ ISO programs

■ Program call with PGM CALL

1 Introduction

1.2 Visual Display Unit and Keyboard

Visual display unit

The figure at right shows the keys and controls on the VDU:

Setting the screen layout Soft key selector keys Switching the soft-key rows Header

When the TNC is on, the selected operating mode is shown in the screen header. Dialog prompts and TNC messages also appear here (unless the TNC is showing only graphics).

Soft keys In the right margin the TNC indicates additional functions in a softkey row. You can select these functions by pressing the keys immediately beside them are rectangular boxes indicating the number of soft-key rows. These rows can be called with the box representing the active soft-key row is filled in.

Screen layout

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

. Directly beneath the soft-key row

outside right and left. The

1.2 Visual Display Unit and Keyboard

To change the screen layout:

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

Select the desired screen layout.

3HEIDENHAIN TNC 310

Keyboard

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

MOD function, HELP function

Numerical input Dialog buttons Arrow keys and GOTO jump command Modes of Operation Machine control buttons Override control knobs for feed rate/spindle speed

1.3 Modes of Operation

The functions of the individual keys are described in the foldout of the front cover. The exact functioning of the machine control buttons, e.g. NC START, is described in more detail in your Machine Manual.

1.3 Modes of Operation

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

Manual Operation and Electronic Handwheel

The Manual Operation mode is required for setting up the machine tool. In this operating mode, you can position the machine axes manually or by increments. Datums can be set by the usual scratching method or by using the TS 220 triggering touch probe. The TNC also supports the manual traverse of the machine axes using a HR electronic handwheel.

Soft keys for selecting the screen layout

Screen windows Soft key

Positions

Left: positions, right: general program information

Left: positions, right: positions and Coordinates

Screen windows Soft key

Left: positions, right: information on tools

Left: positions, right: coordinate transformations

1 Introduction

Positioning with Manual Data Input (MDI)

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

Soft keys for selecting the screen layout

Screen windows Soft key

Program

Left: program blocks, right: general program information

Left: program blocks, right: positions and Coordinates

Left: program blocks, right: tool tools

Left: program blocks, right: coordinate transformations

Left: program blocks, right: help graphics for cycle programming (2nd soft-key level)

Programming and Editing

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

Soft keys for selecting the screen layout

1.3 Modes of Operation

Screen windows Soft key

Program

Left: program blocks, right: help graphics for cycle programming

Left: program blocks, right: programming graphics

Interactive Programming Graphics

5HEIDENHAIN TNC 310

Test run

In the Test Run mode of operation, the TNC checks programs and program sections for errors, such as geometrical incompatibilities, missing or incorrect data within the program or violations of the work space. This simulation is supported graphically in different display modes. Use a soft key to activate the test run in the Program Run operating mode.

Soft keys for selecting the screen layout

Screen windows Soft key

Program

n Test run graphics

1.3 Modes of Operation

Left: program blocks, right: general program information

Left: program blocks, right: positions and Coordinates

Left: program blocks, right: tool tools

Left: program blocks, right: coordinate transformations

1 Introduction

Program Run/Single Block and Program Run/Full Sequence

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

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

Soft keys for selecting the screen layout

Screen windows Soft key

Program

Left: program blocks, right: general program information

Left: program blocks, right: positions and Coordinates

Left: program blocks, right: tool tools

Left: program blocks, right: coordinate transformations

1.4 Status Displays

“General” status display

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

In the operating modes Manual Operation and Electronic Handwheel and Positioning with MDI the status display appears in the large window

7HEIDENHAIN TNC 310

Information in the status display

The Meaning

ACTL. Actual or nominal coordinates of the current position

X Y Z Machine axes

S F M Spindle speed S, feed rate F and active M functions

1.4 Status Displays

ROT Axes are moving

Program run started

Axis locked

plain

Additional status displays

The additional status displays contain detailed information on the program run. They can be called in all operating modes, except in the Manual Operation mode.

To switch on the additional status display:

Call the soft-key row for screen layout.

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

You can also choose between the following additional status displays:

8 1 Introduction

General program information

Name of main program / Active block number Program called via Cycle 12 Active machining cycle Circle center CC (pole) Dwell time counter

Number of the active subprogram or active program section repeats/ Counter for current program section repeat (5/3: 5 repetitions programmed, 3 remaining to be run)

Operating time

Positions and coordinates

Name of main program / Active block number Position display Type of position display, e.g. distance-to-go Angle of a basic rotation

1.4 Status Displays

9HEIDENHAIN TNC 310

Information on tools

T: Tool number Tool axis Tool length and radius Oversizes (delta values) from TOOL CALL block

1.4 Status Displays

Coordinate transformations

Name of main program / Active block number Active datum shift (Cycle 7) Active rotation angle (Cycle 10) Mirrored axes (Cycle 8) Active scaling factor (Cycle 11)

For further information, refer to section 8.6 “Coordinate Transformation Cycles.”

1 Introduction

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

3-D Touch Probes

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

■ Automatically align workpieces

■ Quickly and precisely set datums

TS 220 touch trigger probe

This touch probe is particularly effective for automatic workpiece alignment, datum setting and workpiece measurement. The TS 220 transmits the triggering signals to the TNC via cable.

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

HR electronic handwheels

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

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

11HEIDENHAIN TNC 310

Manual Operation and Setup

2.1 Switch-On

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

ú Switch on the power supply for control and machine.

2.1 Switch-On

The TNC automatically initiates the following dialog

Memory test

The TNC memory is automatically checked.

Power interrupted

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

TRANSLATE PLC program

The PLC program of the TNC is automatically compiled.

Relay Ext. DC Voltage Missing

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

Traverse Reference Points

Cross the reference points in any sequence:

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

Cross the reference points with several axes at

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

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

2 Manual Operation and Setup

2.2 Moving the Machine Axes

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

Traverse the axis with the axis direction keys

Select the Manual Operation mode.

Press the axis direction button and hold it as long as you wish the axis to move.

...or move the axis continuously:

and Press and hold the axis direction button, then

press the NC START button: The axis continues to move after you release the keys.

2.2 Moving the Machine Axes

Press the NC STOP key to stop the axis.

You can move several axes at a time with these two methods.

15HEIDENHAIN TNC 310

Traversing with the HR 410 electronic handwheel

The portable HR 410 handwheel is equipped with two permissive buttons. The permissive buttons are located below the star grip. You can only move the machine axes when an permissive button is depressed (machine-dependent function).

The HR 410 handwheel features the following operating elements:

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

are set by the machine tool builder) Direction in which the TNC moves the selected axis

2.2 Moving the Machine Axes

Machine function (set by the machine tool builder)

The red indicators show the axis and feed rate you have selected.

To move an axis:

Select the Manual Operation mode.

Activate handwheel, set soft key to ON

Press the permissive button.

Select the axis on the handwheel

Select the feed rate.

or Move the active axis in the positive or negative

direction.

2 Manual Operation and Setup

Incremental jog positioning

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

Select the Manual Operation mode.

Select incremental jog positioning, set the soft key to ON

JOG INCREMENT?

Enter the jog increment in millimeters

(here, 8 mm).

Select the jog increment via soft key (select 2nd or 3rd soft-key row)

Press the axis direction button to position as often as desired

2.2 Moving the Machine Axes

17HEIDENHAIN TNC 310

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

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

Entering values

Example: Entering the spindle speed S

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

SPINDLE SPEED S=

1000 Enter the desired spindle speed,

and confirm with the NC START button

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

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

Changing the spindle speed and feed rate

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

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

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

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

18 2 Manual Operation and Setup

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

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

Preparation

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

Datum setting

Fragile workpiece? If the workpiece surface must not be scratched, you can lay a metal shim of know thickness

tool axis datum value that is larger than the desired datum by the

value

Select the Manual Operation mode.

Move the tool slowly until it touches the workpiece surface.

Select the function for setting the datum

Select the axis.

DATUM SET Z=

Zero tool in spindle axis: Set the display to a

known workpiece position (here, 0) or enter the

thickness the tool radius.

of the shim. In the tool axis, offset

on it. Then enter a

2.4 Setting the Datum

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

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

19HEIDENHAIN TNC 310

Positioning with Manual Data Input (MDI)

3.1 Programming and Executing Simple Positioning Blocks

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

To start program run, press the machine START button.

Limitations:

The following functions are not available:

- Tool radius compensation

- Programming graphics

- Programmable probing functions

- Subprograms, program section repeats

- Path functions CT, CR, RND and CHF

- Cycle 12 PGM CALL

Example 1

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

3.1 Programming and Executing Simple Positioning Blocks

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

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

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

Define tool: zero tool, radius 5 Call tool: tool axis Z Spindle speed 2000 rpm Retract tool (FMAX = rapid traverse) Pos. tool aboveholeatFMAX , spindle On

3 Positioning with Manual Data Input (MDI)

5 L Z+5 F2000 6 CYCL DEF 1.0 PECKING 7 CYCL DEF 1.1 SET UP 5 8 CYCL DEF 1.2 DEPTH -20 9 CYCL DEF 1.3 PECKG 10 10 CYCL DEF 1.4 DWELL 0.5 11 CYCL DEF 1.5 F250 12 CYCL CALL 13 L Z+200 R0 FMAX M2 14 END PGM $MDI MM

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

ling Cycles.”

Position tool to 5 mm above hole Define PECKING cycle: Setup clearance of the tool above the hole Total hole depth (Algebraic sign=working direction) Depth of each infeed before retraction Dwell time in seconds at the hole bottom Feed rate for pecking Call PECKING cycle Retract tool End of program

3.1 Programming and Executing Simple Positioning Blocks

23HEIDENHAIN TNC 310

Protecting and erasing programs in $MDI

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

Select operating mode: Programming and Editing

Call up the file manager: PGM NAME soft key

Move the highlight to the $MDI file.

Select „Copy file“: Press the COPY soft key

Target file =

1225 Enter the name under which you want to save

the current contents of the $MDI file.

Copy the file.

Exit the file manager: END key

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

3.1 Programming and Executing Simple Positioning Blocks

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

24 3 Positioning with Manual Data Input (MDI)

Programming:

Fundamentals of NC, File Management, Programming Aids

4.1 Fundamentals of NC

Position encoders and reference marks

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

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

4.1 Fundamentals of NC

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

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

X (Z,Y)

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

Reference system

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

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

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

Reference systems on milling machines

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

The TNC 310 can control up to 4 axes. The axes U, V and W are secondary linear axes parallel to the main axes X, Y and Z, respectively. Rotary axes are designated as A, B and C. The illustration shows the assignment of secondary axes and rotary axes to the main axes.

4.1 Fundamentals of NC

V+

W+

C+

B+

A+

U+

27HEIDENHAIN TNC 310

Polar coordinates

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

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

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

position, and the

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

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

4.1 Fundamentals of NC

See figure at lower right.

Definition of pole and angle reference axis

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

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

XY +X YZ +Y ZX +Z

0°

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

Absolute and relative workpiece positions

Absolute workpiece positions

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

Example 1: Holes dimensioned in absolute coordinates

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

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

Hole Hole

Relative workpiece positions

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

To program a position in incremental coordinates, enter the prefix “I”(soft key) before the axis.

Example 2: Holes dimensioned with relative coordinates

Absolute coordinates of hole

X= 10 mm Y= 10 mm

referenced to hole Hole referenced to hole

Hole IX= 20 mm IX= 20 mm

IY= 10 mm IY= 10 mm

Absolute and incremental polar coordinates

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

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

10 10

3010

4.1 Fundamentals of NC

+IPA

+IPR

+IPA

0°

29HEIDENHAIN TNC 310

Selecting the datum

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

If the production drawing is dimensioned in relative coordinates, simply use the coordinate transformation cycles. For further information, refer to section 8.6 “Coordinate Transformation Cycles.”

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

4.1 Fundamentals of NC

at a position or corner on the workpiece, which is the most suitable for deducing the dimensions of the remaining workpiece positions.

The fastest, easiest and most accurate way of setting the datum is by using a 3-D touch probe from HEIDENHAIN. For further information, refer to section 12.2 “Setting the Datum with a 3-D Touch Probe.”

Example

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

to are referenced to a relative datum with the

to without any further

to , which

750

320

150

7 6

-150

0,1

300

325

450 900

950

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

4.2 File management

Files and file management

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

File names

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

35720 .H

File name File type

Files in the TNC Type

Programs

in HEIDENHAIN conversational format .H

4.2 File Management

Table for

Tools .T

The TNC can manage up to 64 files. Their total size, however, must not exceed 128 MB.

Working with the file manager

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

Calling the file manager

Press the PGM NAME soft key: the TNC displays the file management window

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

Table for Datums .D

display. Meaning

FILE NAME Name with up to 8 characters

and file type Number following the name: File size in bytes

Status Properties of the file:

M Program is in a

Program Run mode of operation.

P File is protected against

editing and erasure

(Protected)

31HEIDENHAIN TNC 310

Selecting a file

Calling the file manager

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

Move the highlight up or down.

Deleting a file

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

ú To select the erasing function,

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

ú To confirm erasure: Press the YES

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

Enter the first or more numbers of the file you wish to select and

4.2 File Management

then press the GOTO key: The highlight moves to the first file that matches these numbers.

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

Copying a file

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

ú Press the COPY soft key to select the copying

function.

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

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

Renaming a file

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

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

changed.

ú To execute renaming, press the ENT key.

Protecting a file/Canceling file protection

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

ú To enable file protection, press the

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

You also need to enter the code number 86357. To cancel file protection, enter the code number

86357.

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

Read in/read out files

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

The TNC provides the following functions:

Functions for reading in/reading out files Soft key

Read in all files

Only read in selected files; To accept a file suggested by the TNC, press the YES soft key; Press the NO soft key if you do not want to accept it.

Read in the selected file: Enter the file name

Read out the selected file: Move the highlight to the desired file and confirm with ENT

Read out all of the files in the TNC memory

Display the file directories of the external unit on your TNC screen

4.2 File Management

33HEIDENHAIN TNC 310

4.3 Creating and Writing Programs

Organization of an NC program in HEIDENHAIN conversational format.

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

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

program name and the active unit of measure. The subsequent blocks contain information on:

■ The blank form:

■ tool definitions and tool calls,

■ Feed rates and spindle speeds as well as

■ Path contours, cycles and other functions

The last block of a program is identified by “END PGM,” the pro- gram name and the active unit of measure.

4.3 Creating and Writing Programs

Defining the blank form — BLK FORM

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

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

entered as absolute values.

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

entered as absolute or incremental values.

Block:

10 L X+10 Y+5 R0 F100 M3

Path function Words

Block number

MAX

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

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

MIN

Creating a new part program

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

Program initiation in an example:

Select the Programming and Editing mode of operation.

Call up the file manager: Press the PGM NAME soft key

File name =

3056 Enter the new program number and confirm

your entry with the ENT key.

File name = 3056.H

Select the default setting for unit of measurement (mm): Press the ENT key, or

Switch to inches: Press the MM/INCH soft key

and confirm with ENT.

4.3 Creating and Writing Programs

35HEIDENHAIN TNC 310

Define the blank

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

Working spindle axis X/Y/Z ?

Enter the spindle axis.

Def BLK FORM: Min corner?

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

the MIN point.

-40

Def BLK FORM: Max-corner?

4.3 Creating and Writing Programs

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

the MAX point.

100

The program blocks window shows the following BLK FORM definition

0 BEGIN PGM 3056 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 END PGM 3056 MM

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

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

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

Programming tool movements in conversational format

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

Example of a dialog

Initiate the dialog.

Coordinates ?

10 Enter the target coordinate for the X axis.

5 Enter the target coordinate for the Y axis,

and go to the next question with ENT.

Radius comp. RL/RR/no comp. ?

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

Feed rate ? F=

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

contour; go to the next question with ENT.

Miscellaneous function M ?

3 Enter the miscellaneous function M3 “spindle

ON”; pressing the ENT key will terminate this dialog.

Functions during the dialog Key

Ignore the dialog question

End the dialog immediately

Abort the dialog and erase the block

4.3 Creating and Writing Programs

The program blocks window will display the following line:

3 L X+10 Y+5 R0 F100 M3

37HEIDENHAIN TNC 310

Editing program lines

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

Selecting blocks or words Soft keys/keys

Move from one block to the next

Scrolling through the program

ú Press the GOTO key ú Enter the block number and confirm with ENT, and the TNC will

go to the indicated block, or

ú Press one of the superimposed soft keys to scroll to another page

(see table at top right.)

Looking for the same words in different blocks

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

4.3 Creating and Writing Programs

Select a block with the arrow keys.

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

Inserting blocks at any desired location

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

initiate the dialog.

Inserting the previously edited (deleted) block at any location

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

just edited (deleted.)

ú If you wish to insert a block you have stored in the buffer memory,

press the soft key INSERT NC BLOCK

Select individual words in a block

Go to the previous page

Go to the next page

Jump to beginning of program

Jump to beginning End

Erasing blocks and words Key

Set the value of the selected word to zero

Erase an incorrect number

Clear a (non-blinking) error message

Delete the selected word

Delete the selected block (cycle)

Editing and inserting words

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

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

ú To accept the change, press the END key.

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

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

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

4.4 Interactive Programming Graphics

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

To generate/not generate graphics during programming:

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

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

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

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

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

AUTO DRAW ON does not simulate program section repeats.

To generate a graphic for an existing program:

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

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

ú To generate graphics, press the RESET + START

soft key.

Additional functions are listed in the table at right.

To erase the graphic:

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

Functions Soft key

Generate interactive graphics blockwise

Generate a complete graphic or complete it after RESET + START

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

4.4 Interactive Programming Graphics

39HEIDENHAIN TNC 310

Magnifying or reducing a detail

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

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

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

Function Soft key

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

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

Move the frame overlay to the left: Press and hold the soft key. Move the frame overlay to the right: Press and hold the arrow to the right soft key

4.4 Interactive Programming Graphics

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

ú Confirm the selected section with the WINDOW

DETAIL soft key

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

4.5 HELP function

Certain TNC programming functions are explained in more detail in the HELP function. You can select a HELP topic using the soft keys

Select the HELP function

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

Help topics / Functions Soft key

M functions

Cycle parameters

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

Go to previous page

Go to next page

Go to beginning of file

Go to end of file

Select search functions; Enter a number, Begin search with ENT key

The HELP provided by the machine manufacturer can only be displayed and not executed.

4.5 HELP Function

End the HELP function

Press the END key.

41HEIDENHAIN TNC 310

Programming:

Tools

5.1 Entering Tool-Related Data

Feed rate F

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

Input

You can enter the feed rate in every positioning block. For further information refer to section 6.2 “Fundamentals of Path Contours.”

Rapid traverse

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

Duration of effect

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

5.1 Entering Tool-Related Data

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

Changing during program run

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

Spindle speed S

The spindle speed S is entered in revolutions per minute (rpm) in a TOOL CALL block.

Programmed change

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

ú To program a tool call, press the

TOOL CALL soft key (3rd soft-key row)

ú Ignore the dialog question for „Tool number ?“ with

the right arrow key

ú Ignore the dialog question for „Working spindle axis

X/Y/Z ?“ with the right arrow key

ú Enter the new spindle speed for the dialog

question “Spindle speed S= ?”.

Changing during program run

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

5 Programming: Tools

5.2 Tool Data

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

Tool data can be entered either directly in the part program with TOOL DEF or (and) separately in tool tables. The TNC will consider all of the data entered when executing the part program.

Tool number

Each tool is identified by a number between 0 and 254. The tool number 0 is automatically defined as the zero tool with the

length L=0 and the radius R=0. In tool tables, tool 0 should also be defined with L=0 and R=0.

Tool length L

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

that of a zero tool L

For the algebraic sign:

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

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

To determine the length:

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

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

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

zero tool.

ú Enter the value in the TOOL DEF block or in the tool table by

pressing the „ACTUAL POSITION“ key

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

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

5.2 Tool Data

45HEIDENHAIN TNC 310

Tool radius R

You can enter the tool radius R directly.

Delta values for lengths and radii

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

5.2 Tool Data

delta value describes a tool undersize (DR<0). Enter the delta values when you are programming with TOOL CALL.

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

DR<0

Entering tool data into the program

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

ú To select tool definition, press the TOOL DEF key. ú Enter the Tool number: Each tool is uniquely

identified by its number. When the tool table is active, enter tool numbers greater than 99 (dependent on MP7260)

ú Enter the tool length: Enter the compensation

value for the tool length.

ú Enter the Tool radius.

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

Resulting NC block:

4 TOOL DEF 5 L+10 R+5

DR>0

DL<0

DL>0

5 Programming: Tools

Entering tool data in tables

You can define and store up to 254 tools and their tool data in the tool table (the maximum number of tools in the table can be set in machine parameter 7260).

Tool table: Available input data

Abbr. Input

T Number by which the tool is called in the program L Value for tool length compensation L R Compensation value for the tool radius R

Editing the tool table

The tool table has the name TOOL.T is automatically active in a program run operating mode.

To open the tool table TOOL.T:

ú Select any machine operating mode.

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

key.

ú Set the EDIT soft key to ON.

ú Select the Programming and Editing mode of operation.

ú Calls the file manager. ú Move the highlight to TOOL.T. Confirm with the

ENT key.

Dialog

–

Tool length? Tool radius?

5.2 Tool Data

When you have opened the tool table, you can edit the tool data by moving the cursor to the desired position in the table with the arrow keys (see figure at center right). You can overwrite the stored values, or enter new values at any position. The available editing functions are illustrated in the table on the next page.

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

To leave the tool table:

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

part program.

47HEIDENHAIN TNC 310

Editing functions for tool tables Soft key

Take the value from the position display

Select previous page in table (2nd soft-key row)

5.2 Tool Data

Select next page in table (2nd soft-key row)

Move the highlight one column to the left

Move the highlight one column to the right

Delete incorrect numerical value, re-establish preset value

Re-establish the last value stored

Move the highlight back to beginning of line

5 Programming: Tools

Calling tool data

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

ú Select the tool call function with the TOOL CALL

key

ú Tool number: Enter the number of the tool. The

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

ú Working spindle axis X/Y/Z: Enter the tool axis. ú Spindle speed S ú Tool length oversize: Enter the delta value for the

tool length.

ú Tool radius oversize: Enter the delta value for the

tool radius.

Example:

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

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

The character D preceding L and R designates delta values.

Tool change

The tool change function can vary depending on the individual machine tool. Refer to your machine tool manual.

5.2 Tool Data

Tool change position

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

Manual tool change

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

ú Move to the tool change position under program control. ú Interrupt program run (see section 11.3 “Program Run”). ú Change the tool. ú Resume the program run (see section 11.3 “Program Run”).

49HEIDENHAIN TNC 310

Pocket table for tool changer

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

To select the pocket table:

ú In the Programming and Editing mode,

5.2 Tool Data

ú In a machine operating mode

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

ENT key.

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

key.

ú To select the pocket table,

press the POCKET TABLE soft key

ú Set the EDIT soft key to ON

Editing functions for pocket table Soft key

Select previous page in table (2nd soft-key row)

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

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

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

Abbr. Input

P Pocket number of the tool in the tool magazine T Tool number ST Special tool with large radius requiring more than one

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

F Fixed tool number.

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

sent to the PLC

Select next page in table (2nd soft-key row)

Move the highlight one column to the left

Move the highlight one column to the right

Reset pocket table

Dialog

–

Tool number? Special tool ?

Fixed pocket?

Locked pocket? PLC status?

5 Programming: Tools

5.3 Tool Compensation

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

If you are writing the part program directly on the TNC, the tool radius compensation is effective only in the working plane.

Tool length compensation

Length compensation becomes effective automatically as soon as a tool is called and the tool axis moves. To cancel length compensation call a tool with the length L=0.

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

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

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

Compensation value = L + DL L is the tool length L from the TOOL DEF block or tool

table

TOOL CALL

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

TOOL CALL

where

5.3 Tool Compensation

Tool radius compensation

The NC block for programming a tool movement contains:

■ RL or RR for compensation in the tool radius

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

■ R0 if no radius compensation is required

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

51HEIDENHAIN TNC 310

For tool radius compensation, the TNC takes the delta values from the TOOL CALL block into account:

Compensation value = R + DR

TOOL CALL,

where

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

table

TOOL CALL

is the oversize for radius DR in the TOOL CALL block

(not taken into account by the position display)

Tool movements without radius compensation: R0

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

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

5.3 Tool Compensation

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

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

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

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

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

5 Programming: Tools

Entering radius compensation

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

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

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

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

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

To terminate the dialog, press the END key.

5.3 Tool Compensation

53HEIDENHAIN TNC 310

Radius compensation: Machining corners

Outside corners

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

Inside corners

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

5.3 Tool Compensation

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

Machining corners without radius compensation

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

RL RL

5 Programming: Tools

Programming:

Programming Contours

6.1 Overview of Tool Movements

Path functions

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

Miscellaneous functions M

With the TNC’s miscellaneous functions you can affect

■ Program run, e.g., a program interruption

■ Machine functions, such as switching spindle rotation and coolant

supply on and off

■ Contouring behavior of the tool

Subprograms and program section repeats

6.1 Overview of Tool Movements

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

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

R40

11510

6 Programming: Programming Contours

6.2 Fundamentals of Path Functions

Programming tool movements for workpiece machining

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

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

Movement parallel to the machine axes

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

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

Example:

L X+100

L Path function for “straight line” X+100 Coordinate of the end point

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

Movement in the main planes

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

Example:

L X+70 Y+50

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

100

6.2 Fundamentals of Path Functions

Three-dimensional movement

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

Example:

L X+80 Y+0 Z-10

See figure at lower right.

-10

57HEIDENHAIN TNC 310

Circles and circular arcs

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

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

Spindle axis Main plane ZXY

YZX XYZ

Direction of rotation DR for circular movements

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

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

Radius compensation

Radius compensation must be programmed before the block containing the coordinates for the first contour element. You cannot

6.2 Fundamentals of Path Functions

begin radius compensation in a circle block. It must be activated beforehand in a straight-line block.

Pre-positioning

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

DR+

DR–

6 Programming: Programming Contours

Creating the program blocks with the path function keys

Use the path function keys to open a conversational dialog. The TNC asks you successively for all the necessary information and inserts the program block into the part program.

You may not program controlled and non-controlled axes in the same block.

Example — programming a straight line:

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

Coordinates ?

10 Enter the coordinates of the straight-line end

point.

Transfer the coordinates of the selected axis: Press ACTUAL POSITION soft key (second softkey row)

6.2 Fundamentals of Path Functions

Radius comp.: RL/RR/NOcomp. ?

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

Feed rate F=

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

confirm your entry with ENT.

Miscellaneous function M ?

3 Enter a miscellaneous function (here, M3), and

terminate the dialog with ENT.

The part program now contains the following line:

L X+10 Y+5 RL F100 M3

59HEIDENHAIN TNC 310

6.3 Contour Approach and Departure

Overview: Types of paths for contour approach and departure

The functions for contour approach and departure are activated with the APPR/DEP key. You can then select the following contour forms using soft keys.

Function Soft keys: Approach Departure

Straight line with tangential connection

Straight line perpendicular to a contour point

Circular arc with tangential connection

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

6.3 Contour Approach and Departure

Approaching and departing a helix

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

Important positions for approach and departure

■ Starting point P

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

■ Auxiliary point P

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

■ First contour point P

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

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

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

■ End point P

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

that the TNC calculates from your input in the

and last contour point P

can be programmed with any path function.

in the working plane, and then move it to

in the working

6 Programming: Programming Contours

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

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

. Use the test graphics to simulate approach and departure

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

the starting point P

and the first contour point PA to assure that the

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

point P

at the feed rate that was last programmed.

Radius compensation

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

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

Function Contour connection

APPR LT Tangential connection to the following

Contour element

APPR LN Perpendicular connection to the following

Contour element

APPR CT without angle of traverse/without radius:

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

without angle of traverse/with radius:

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

with angle of traverse/without radius:

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

with angle of traverse/with radius:

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

APPR LCT Tangent with connecting tangential

circular arc to the following contour element

Abbreviation Meaning

APPR Approach DEP Departure L Line C Circle T Tangential

(smooth connection)

N Normal (perpendicular)

Function Contour connection

DEP LT Tangential connection to the

preceding contour element

DEP LN Perpendicular connection to the

preceding contour element

DEP CT without angle of traverse/without

radius:

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

without angle of traverse/with radius:

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

with angle of traverse/without radius:

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

with angle of traverse/with radius:

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

DEP LCT Tangent with tangentially

connecting circular arc to the preceding contour element

6.3 Contour Approach and Departure

61HEIDENHAIN TNC 310

Approaching on a straight line with tangential connection: APPR LT

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

ú Use any path function to approach the starting point P

Example NC blocks

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

6.3 Contour Approach and Departure

10 L ...

. It then moves from PHto the first contour point P

is separated from the first contour point PA by the

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

LT soft key:

ú Coordinates of the first contour point P

ú LEN: Distance from the auxiliary point P

first contour point P

ú Radius compensation for machining

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

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

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

. It then moves from PHto the first contour point P

is separated from the first contour point PA by the

ú Coordinates of the first contour point P

ú Length: Distance from the auxiliary point P

first contour point P

Always enter LEN as a positive value!

ú Radius compensation RR/RL for machining

to the

P RR

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

Example NC blocks

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

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

6 Programming: Programming Contours

Approaching on a circular arc with tangential connection: APPR CT

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

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

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

Example NC blocks

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

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

to PA is determined through the radius R and the

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

■ CCA can be entered only as a positive value.

■ Maximum input value 360°

ú Radius R of the circular arc

■ If the tool should approach the workpiece in the

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

■ If the tool should approach the workpiece opposite

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

ú Radius compensation RR/RL for machining

CCA= 180°

R10

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

4010

6.3 Contour Approach and Departure

63HEIDENHAIN TNC 310

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

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

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

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

Example NC blocks

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

6.3 Contour Approach and Departure

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

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

– PH as well as

ú Coordinates of the first contour point P

ú Radius R of the arc

Always enter R as a positive value.

ú Radius compensation for machining

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

P RR

R10

4010

6 Programming: Programming Contours

Departing tangentially on a straight line: DEP LT

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

ú Program the last contour element with the end point P

radius compensation.

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

Example NC blocks

23 L Y+20 RR F100 24 DEP LT LEN12.5 R0 F100 25 L Z+100 FMAX M2

. The line lies in the extension of the last contour

is separated from PE by the distance LEN.

ú LEN: Enter the distance from the last contour

element P

to the end point PN.

and

12.5

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

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

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

ú Program the last contour element with the end point P

radius compensation.

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

Example NC blocks

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

. The line departs on a perpendicular path from the

. PN is separated from PE by the distance LEN

and

ú LEN: Enter the distance from the last contour

element P

to the end point PN.

Important: Always enter LEN as a positive value!

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

6.3 Contour Approach and Departure

65HEIDENHAIN TNC 310

Departing tangentially on a circular arc: DEP CT

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

ú Program the last contour element with the end point P

radius compensation.

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

Example NC blocks

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

6.3 Contour Approach and Departure

25 L Z+100 FMAX M2

. The arc is tangentially connected to the last

ú Center angle CCA of the arc

ú Radius R of the circular arc

■ If the tool should depart the workpiece in the

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

■ If the tool should depart the workpiece on the

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

and

180°

Last contour element: PE with radius compensation Center angle=180°, arc radius=10 mm Retract in Z, return to block 1, end program

6 Programming: Programming Contours

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

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

ú Program the last contour element with the end point P

radius compensation.

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

Example NC blocks

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

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

to PN. Once these lines are

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

Always enter R as a positive value

and

Last contour element: PE with radius compensation Coordinates PN, arc radius = 10 mm Retract in Z, return to block 1, end program

6.3 Contour Approach and Departure

67HEIDENHAIN TNC 310

6.4 Path Contours — Cartesian Coordinates

Overview of path functions

Function Contour function soft key

Line L

CHamFer

Circle Center

Circle

Circle by Radius

Circle Tangential Circle Tangential

6.4 Path Contours — Cartesian Coordinates

Corner RouNDing

Tool movement

Straight line

Chamfer between two straight lines

No tool movement

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

Circular arc with a certain radius

Circular arc with tangential connection to the preceding contour element

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

Required input

Coordinates of the straight-line end point

Chamfer side length

Coordinates of the circle center or pole

Coordinates of the arc end point, direction of rotation

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

Coordinates of the arc end point

Rounding-off radius R

6 Programming: Programming Contours

Straight line L

The tool moves on a straight line from its current position to the line end point. The starting point is the end point of the preceding block.

ú Enter the coordinates of the end point.

Further entries, if necessary:

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

Example NC blocks

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

Inserting a chamfer CHF between two straight lines

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

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

working plane.

■ The radius compensation before and after the chamfer block must

be the same.

■ An inside chamfer must be large enough to accommodate the

current tool.

ú Chamfer side length: Enter the length of the

chamfer

Further entries, if necessary:

ú Feed rate F (only effective in CHF block)

6.4 Path Contours — Cartesian Coordinates

Example NC blocks

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

You cannot start a contour with a CHF block A chamfer is possible only in the working plane. If you have not programmed a feed rate in the CHF block,

the TNC will move at the last programmed feed rate. A feed rate programmed in the CHF block is effective

only in that block. After the CHF block, the previous feed rate becomes effective again.

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

69HEIDENHAIN TNC 310

Circle center CC

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

■ Entering the Cartesian coordinates of the circle center

■ Using the circle center defined in an earlier block

■ Capturing the coordinates with the

„ACTUAL POSITION“ soft key

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Coordinates CC: Enter the circle center coordinates

If you want to use the last programmed position, do not enter any coordinates.

Example NC blocks

5 CC X+25 Y+25

10 L X+25 Y+25 11 CC

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

Duration of effect

The circle center definition remains in effect until a new circle

6.4 Path Contours — Cartesian Coordinates

center is programmed.

Entering the circle center CC incrementally

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

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

The circle center is also the pole for polar coordinates.

6 Programming: Programming Contours

Circular path C around circle center CC

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

ú Move the tool to the circle starting point.

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Enter the coordinates of the circle center.

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

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

Example NC blocks

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

Full circle

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

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

Input tolerance: up to 0.016 mm.

6.4 Path Contours — Cartesian Coordinates

71HEIDENHAIN TNC 310

Circular path CR with defined radius

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

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

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

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

ú Direction of rotation DR

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

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

E1=S

S1=E

Full circle

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

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

Central angle CCA and arc radius R

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

6.4 Path Contours — Cartesian Coordinates

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

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

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

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

Example NC blocks

See figures at middle and lower right.

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

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

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

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

DR+

40 70

DR+

40 70

Please observe the notes on the next page!

6 Programming: Programming Contours

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

The maximum possible radius is 30 m.

Circular path CT with tangential connection

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

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

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

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Enter the coordinates of the arc end point.

Further entries, if necessary:

ú Feed rate F ú Miscellaneous function M

Example NC blocks

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

30 25

6.4 Path Contours — Cartesian Coordinates

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

73HEIDENHAIN TNC 310

Corner Rounding RND

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

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

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

Example NC blocks

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

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

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

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

6.4 Path Contours — Cartesian Coordinates

rate becomes effective again. You can also use an RND block for a tangential contour

approach if you do not want to use an APPR function.

6 Programming: Programming Contours

Example: Linear movements and chamfers with Cartesian coordinates

0 BEGIN PGM 10 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+10 4 TOOL CALL 1 Z S4000 5 L Z+250 R0 F MAX 6 L X-20 Y-10 R0 F MAX 7 L Z-5 R0 F1000 M3 8 L X+5 Y+5 RL F300 9 RND R2 10 L Y+95 11 L X+95 12 CHF 10 13 L Y+5 14 CHF 20 15 L X+5 16 RND R2 17 L X-20 R0 F1000 18 L Z+250 R0 F MAX M2 19 END PGM 10 MM

Define blank form for graphic workpiece simulation

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

6.4 Path Contours — Cartesian Coordinates

75HEIDENHAIN TNC 310

Example: Circular movements with Cartesian coordinates

0 BEGIN PGM 20 MM

6.4 Path Contours — Cartesian Coordinates

1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+10 4 TOOL CALL 1 Z S4000 5 L Z+250 R0 F MAX 6 L X-20 Y-20 R0 F MAX 7 L Z-5 R0 F1000 M3 8 L X+5 Y+5 RL F300 9 RND R2 10 L Y+85 11 RND R10 F150 12 L X+30 13 CR X+70 Y+95 R+30 DR14 L X+95 15 L Y+40 16 CT X+40 Y+5

17 L X+5 18 RND R2 19 L X-20 Y-20 R0 F1000 20 L Z+250 R0 F MAX M2 21 END PGM 20 MM

Define blank form for graphic workpiece simulation

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

R10

R30

4030 70

6 Programming: Programming Contours

Example: Full circle with Cartesian coordinates

0 BEGIN PGM 30 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+12.5 4 TOOL CALL 1 Z S3150 5 CC X+50 Y+50 6 L Z+250 R0 F MAX 7 L X-40 Y+50 R0 F MAX 8 L Z-5 R0 F1000 M3 9 L X+0 Y+50 RL F300 10 RND R2 11 C X+0 DR12 RND R2 13 L X-40 Y+50 R0 F1000 14 L Z+250 R0 F MAX M2 15 END PGM 30 MM

Define the workpiece blank

Define the tool tool call Define the circle center Retract the tool Pre-position the tool Move to working depth Approach starting point of circle Tangential approach to circle with R=2 mm Move to the circle end point (= circle starting point) Tangential departure from circle with R=2 mm Retract tool in the working plane Retract tool in the spindle axis, end of program

6.4 Path Contours — Cartesian Coordinates

77HEIDENHAIN TNC 310

6.5 Path Contours— Polar Coordinates

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

Polar coordinates are useful with:

■ Positions on circular arcs

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

Overview of path functions with polar coordinates

Function Contour function soft keys

Tool movement

Required input

Line LP

Circular arc CP +

Circular arc CTP +

6.5 Path Contours — Polar Coordinates6.5 Path Contours — Polar Coordinates

Helix + (Helix)

Straight line

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

Circular path with tangential connection to the preceding contour element

Combination of a circular and a linear movement

Polar coordinate origin: Pole CC

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

ú Select circle functions: Press the „CIRCLE“ soft key

ú Coordinates CC: Enter Cartesian coordinates for

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

do not enter any coordinates.

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

Polar angle of the arc end point, direction of rotation

Polar radius, polar angle of the arc end point

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

6 Programming: Programming Contours

Straight line LP

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

ú Select straight line function: Press the L soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row). Polar coordinates-radius PR: Enter the distance from the pole CC to the straightline end point.

ú Polar-coordinates angle PA: Angular position of the

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

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

Example NC blocks

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

60°

6.5 Path Contours — Polar Coordinates

Circular path CP around pole CC

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

ú Select circle functions: Press the „CIRCLE“ soft key

ú Select circular path C: Press the C soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú Polar coordinates angle PA: Angular position of the

arc end point between –5400° and +5400°

ú Direction of rotation DR

R20

79HEIDENHAIN TNC 310

Example NC blocks

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

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

Circular path CTP with tangential connection

The tool moves on a circular path, starting tangentially from a preceding contour element.

ú Select circle functions: Press the „CIRCLE“ soft key

120°

ú Select the circular path CT: Press the CT soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú Polar coordinates radius PR: Distance from the arc

end point to the pole CC.

ú Polar coordinates angle PA: Angular position of the

arc end point.

6.5 Path Contours — Polar Coordinates6.5 Path Contours — Polar Coordinates

Example NC blocks

12 CC X+40 Y+35 13 L X+0 Y+35 RL F250 M3 14 LP PR+25 PA+120 15 CTP PR+30 PA+30 16 L Y+0

The pole CC is not the center of the contour arc!

R25

R30

30°

6 Programming: Programming Contours

Helical interpolation

A helix is a combination of a circular movement in a main plane and a linear movement perpendicular to this plane.

A helix is programmed only in polar coordinates.

Application

■ Large-diameter internal and external threads

■ Lubrication grooves

Calculating the helix

To program a helix, you must enter the total angle through which the tool is to move on the helix in incremental dimensions, and the total height of the helix.

For calculating a helix that is to be cut in a upward direction, you need the following data:

Thread revolutions n

Total height h Incremental total angle IPA

Starting coordinate Z

Shape of the helix

The table below illustrates in which way the shape of the helix is determined by the work direction, direction of rotation and radius compensation.

Internal thread Work direction Direction Radius compensation

Right-handed Z+ DR+ RL Left-handed Z+ DR– RR Right-handed Z– DR– RR Left-handed Z– DR+ RL

External thread

Right-handed Z+ DR+ RR Left-handed Z+ DR– RL Right-handed Z– DR– RL Left-handed Z– DR+ RR

Thread revolutions + thread overrun at the start and end of the thread Thread pitch P x thread revolutions n Thread revolutions x 360° + angle for beginning of thread + angle for thread overrun Thread pitch P x (thread revolutions + thread overrun at start of thread)

6.5 Path Contours — Polar Coordinates

81HEIDENHAIN TNC 310

Programming a helix

6.5 Path Contours — Polar Coordinates

Always enter the same algebraic sign for the direction of rotation DR and the incremental total angle IPA. The tool may otherwise move in a wrong path and damage the contour.

For the total angle IPA, you can enter a value from –5400° to +5400°. If the thread has of more than 15 revolutions, program the helix in a program section repeat (see section 9.2 ”Program Section Repeats”).

ú Select circle functions: Press the „CIRCLE“ soft key

ú Select circular path C: Press the C soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú Polar coordinates angle: Enter the total angle of

tool traverse along the helix in incremental dimensions. After entering the angle, identify the

tool axis using a soft key.

ú Enter the coordinate for the height of the helix in

incremental dimensions.

ú Direction of rotation DR

Clockwise helix: DR– Counterclockwise helix: DR+

ú Radius compensation RL/RR/R0

Enter the radius compensation according to the table above.

270°

Example NC blocks

12 CC X+40 Y+25 13 Z+0 F100 M3 14 LP PR+3 PA+270 RL F50 15 CP IPA–1800 IZ+5 DR– RL F50

6 Programming: Programming Contours

Example: Linear movement with polar coordinates

100

60°

R45

0 BEGIN PGM 40 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+7.5 4 TOOL CALL 1 Z S4000 5 CC X+50 Y+50 6 L Z+250 R0 F MAX 7 LP PR+60 PA+180 R0 F MAX 8 L Z-5 R0 F1000 M3 9 LP PR+45 PA+180 RL F250 10 RND R1 11 LP PA+120 12 LP PA+60 13 LP PA+0 14 LP PA-60 15 LP PA-120 16 LP PA+180 17 RND R1 18 LP PR+60 PA+180 R0 F1000 19 L Z+250 R0 F MAX M2 20 END PGM 40 MM

Define the workpiece blank

Define the tool tool call Define the datum for polar coordinates Retract the tool Pre-position the tool Move to working depth Approach the contour at point 1 Tangential approach to circle with R=1 mm Move to point 2 Move to point 3 Move to point 4 Move to point 5 Move to point 6 Move to point 1 Tangential departure from circle with R=1 mm Retract tool in the working plane Retract tool in the spindle axis, end of program

100

6.5 Path Contours — Polar Coordinates

83HEIDENHAIN TNC 310

Example: HelixExample: HelixExample: HelixExample: HelixExample: HelixExample: HelixExample: Helix

100

6.5 Path Contours — Polar Coordinates

0 BEGIN PGM 50 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-20 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL DEF 1 L+0 R+5 4 TOOL CALL 1 Z S1400 5 L Z+250 R0 F MAX 6 L X+50 Y+50 R0 F MAX 7 CC 8 L Z-12.75 R0 F1000 M3 9 LP PR+32 PA-180 RL F100 10 RND R2 11 CP IPA+3240 IZ+13,5 DR+ F200 12 RND R2 13 L X+50 Y+50 R0 F MAX 14 L Z+250 R0 F MAX M2 15 END PGM 50 MM

Define the workpiece blank

Define the tool tool call Retract the tool Pre-position the tool Transfer the last programmed position as the pole Move to working depth Approach contour Tangential approach to circle with R=2 mm Helical interpolation Tangential departure from circle with R=2 mm Retract tool in the working plane Retract tool in the spindle axis, end of program

100

M64 x 1,5

To cut a thread with more than 16 revolutions

... 8 L Z-12.75 R0 F1000 9 LP PR+32 PA-180 RL F100 10 LBL 1 11 CP IPA+360 IZ+1.5 DR+ F200 12 CALL LBL 1 REP 24

Identify beginning of program section repeat Enter the thread pitch as an incremental IZ dimension Program the number of repeats (thread revolutions)

6 Programming: Programming Contours

Programming:

Miscellaneous functions

7.1 Entering Miscellaneous Functions M and STOP

With the TNC's miscellaneous functions - also called M functions you can affect:

■ Program run, e.g., a program interruption

■ Machine functions, such as switching spindle rotation and coolant

supply on and off

■ Contouring behavior of the tool

The machine tool builder may add some M functions that are not described in this User's Manual. Your machine manual provides more detailed information.

M functions are always entered at the end of a positioning block. The TNC then displays the following dialog question:

Miscellaneous function M ?

Only enter the number of the M function in the programming dialog.

In the MANUAL OPERATION operating mode, the M functions are entered with the M soft key.

Please note that some F functions become effective at the start of a positioning block, and others at the end.

M functions come into effect in the block in which they are called. Unless the M function is only effective blockwise, it is canceled in a subsequent block or at the end of the program. Some M functions are effective only in the block in which they are called.

7.1 Entering Miscellaneous Functions M and STOP

Entering an M function in a STOP block

If you program a STOP block, the program run or test run is interrupted at the block, for example for tool inspection. You can also enter an M function in a STOP block:

ú To program an interruption of program run,

press the STOP key.

ú Enter miscellaneous function M

Example NC block

87 STOP M6

7 Programming: Miscellaneous functions

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant

M Effect M00 Stop program run

Spindle STOP Coolant OFF

M01 Stop program run M02 Stop program run

Spindle STOP Coolant OFF Go to block 1 Clear the status display (dependent on machine parameter 7300)

M03 Spindle ON clockwise M04 Spindle ON counterclockwise M05 Spindle STOP M06 Tool change

Spindle STOP Program run stop (dependent on machine parameter 7440)

M08 Coolant ON M09 Coolant OFF M13 Spindle ON clockwise

Coolant ON

M14 Spindle ON counterclockwise

Coolant ON

M30 Same as M02

Effective at

Block end

Block end Block end

Block start Block start Block end Block end

Block start Block end Block start

Block start

7.3 Miscellaneous functions for Coordinate Data

Block end

7.3 Miscellaneous Functions for Coordinate Data

Programming machine-referenced coordinates: M91/M92

Scale reference point

On the scale, a reference mark indicates the position of the scale reference point.

Machine datum

The machine datum is required for the following tasks:

■ Defining the limits of traverse (software limit switches)

■ Moving to machine-referenced positions (such as tool change

positions)

■ Setting the workpiece datum

X (Z,Y)

7.2 Miscellaneous functions for Program Run Control, Spindle and Coolant;

87HEIDENHAIN TNC 310

The distance in each axis from the scale reference point to the machine datum is defined by the machine tool builder in a machine parameter.

Standard behavior

The TNC references coordinates to the workpiece datum (see “Datum setting”).

Behavior with M91 — Machine datum

If you want the coordinates in a positioning block to be referenced to the machine datum, end the block with M91.

The coordinate values on the TNC screen are referenced to the machine datum. Switch the display of coordinates in the status display to REF (see section 1.4 “Status Displays”).

Behavior with M92 — Additional machine datum

In addition to the machine datum, the machine tool builder can also define an additional machine-based position as a reference point.

For each axis, the machine tool builder defines the distance between the machine datum and this additional machine datum. Refer to the machine manual for more information.

If you want the coordinates in a positioning block to be based on the additional machine datum, end the block with M92.

Radius compensation remains the same in blocks that are programmed with M91 or M92. The tool length, however, is not compensated.

7.3 Miscellaneous Functions for Coordinate Data

Effect

M91 and M92 are effective only in the blocks in which they are programmed with M91 or M92.

M91 and M92 become effective at the start of block.

Workpiece datum

The figure at right shows coordinate systems with the machine datum and workpiece datum.

7 Programming: Miscellaneous functions

heidenhain TNC 310 Programming Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Introduction

1.1 The TNC 310

1.2 Visual Display Unit and Keyboard

1.3 Modes of Operation

1.4 Status Displays

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

Manual Operation and Setup

2.1 Switch-On

2.2 Moving the Machine Axes

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

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

Positioning with Manual Data Input (MDI)

3.1 Programming and Executing Simple Positioning Blocks

4.1 Fundamentals of NC

4.2 File Management

4.3 Creating and Writing Programs

4.4 Interactive Programming Graphics

4.5 HELP Function

5.1 Entering Tool-Related Data

5.2 Tool Data

5.3 Tool Compensation

6.1 Overview of Tool Movements

6.2 Fundamentals of Path Functions

Overview: Types of paths for contour approach and departure

6.3 Contour Approach and Departure

Important positions for approach and departure

Approaching on a straight line with tangential connection: APPR LT

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

Approaching on a circular arc with tangential connection: APPR CT

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

Departing tangentially on a straight line: DEP LT

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

Departing tangentially on a circular arc: DEP CT

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

Overview of path functions

6.4 Path Contours — Cartesian Coordinates

Straight line L

Inserting a chamfer CHF between two straight lines

Circle center CC

Circular path C around circle center CC

Circular path CR with defined radius

Circular path CT with tangential connection

Corner Rounding RND

Example: Linear movements and chamfers with Cartesian coordinates

Example: Circular movements with Cartesian coordinates

Example: Full circle with Cartesian coordinates

6.5 Path Contours— Polar Coordinates

Polar coordinate origin: Pole CC

Straight line LP

Circular path CP around pole CC

Circular path CTP with tangential connection

Helical interpolation

Example: Linear movement with polar coordinates

Example: HelixExample: HelixExample: HelixExample: HelixExample: HelixExample: HelixExample: Helix

7.1 Entering Miscellaneous Functions M and STOP

7.3 Miscellaneous functions for Coordinate Data