HEIDENHAIN TNC 360 User Manual

Download

Page 1

HEIDENHAIN

February 1994

User's Manual ISO Programming

TNC 360

Page 2

Keys and Controls on the TNC 360

HKJ

ENT

Controls on the Visual Display Unit

Brightness

Contrast

Override Knobs

100

Machine Operating Modes

F %

S %

MANUAL OPERATION ELECTRONIC HANDWHEEL POSITIONING WITH MANUAL DATA INPUT PROGRAM RUN, SINGLE BLOCK

Feed rate

Spindle speed

Address Letters for ISO Programming

Block number

TOUCH PROBE

G function Feed rate / Dwell time with G04 / Scaling factor Miscellaneous function (M function) Spindle speed in rpm Parameter definition Polar angle/Rotation angle in cycle G73 X, Y, Z coordinate of circle center/pole Assign a label number with G98/

Jump to a label number/ Tool length with G99

Polar radius/ Rounding radius with G25, G26, G27 Chamfer with G24 Circle radius with G02, G03, G05 Tool radius with G99

Tool definition with G99/ Tool call

Set a datum with the 3D touch probe system

PROGRAM RUN, FULL SEQUENCE

Programming Modes

PROGRAMMING AND EDITING TEST RUN

Program and File Management

PGM

CALL

EXT

MOD

Moving the Cursor and Selecting Blocks, Cycles and Parameter Functions with GOTO

GOTO

Graphics

MOD

BLK

FORM

Select programs and files Delete programs and files Enter program call in a program External data transfer Supplementary modes

Move the cursor (highlight) Go directly to blocks, cycles and

parameter functions

Graphic operating modes Define blank form, reset blank form

Entering Numbers and Coordinate Axes, Editing

ENT

END

DEL

...

Select or enter coordinate axes

in a program

Numbers Decimal point Algebraic sign Actual position capture Ignore dialog queries, delete words Confirm entry and resume dialog Conclude block Clear numerical entry

or TNC message Abort dialog; delete program sections

MAGN

START

Magnify detail Start graphic simulation

Page 3

TNC Guideline:

From workpiece drawing to program-controlled machining

Step Task TNC Refer to

operating mode Section

Preparation

1 Select tools —— ——

2 Set workpiece datum

for coordinate system —— ——

3 Determine spindle speeds

and feed rates —— 11.4

4 Switch on machine —— 1.3

5 Traverse reference marks or 1.3, 2.1

6 Clamp workpiece —— ——

7 Set the datum /

Reset position display ...

7a ... with the 3D touch probe or 2.5

7b ... without the 3D touch probe or 2.3

Entering and testing part programs

8 Enter part program

or download over external 5 to 8 data interface or or 10

9 Test part program for errors 3.1

10 Test run: Run program

block by block without tool 3.2

EXT

11 If necessary: Optimize

part program 5 to 8

Machining the workpiece

12 Insert tool and

run part program 3.2

Page 4

Sequence of Program Steps

Milling an outside contour

Programming step Key/Function Refer to Section

1 Create or select program 4.4

Input: Program number

Unit of measure for programming

2 Define workpiece blank for graphic display G30/G31 4.4 3 Define tool(s) G99 4.2

Input: Tool number T...

Tool length L... Tool radius R...

4 Call tool data T... 4.2

Input: Tool number

Spindle axis G17 Spindle speed S...

5 Tool change

Input: Feed rate (rapid traverse) G00 e.g. 5.4

Radius compensation G40 Coordinates of the tool change position X... Y... Z... Miscellaneous function (tool change) M06

6 Move to starting position 5.2/5.4

Input: Feed rate (rapid traverse) G00

Coordinates of the starting position X... Y... Radius compensation G40 Miscellaneous function (spindle on, clockwise) M03

PGM

7 Move tool to (first) working depth 5.4

Input: Feed rate (rapid traverse) G00

Coordinate of the (first) working depth Z...

8 Move to first contour point 5.2/5.4

Input: Linear interpolation G01

Radius compensation for machining G41/G42 Coordinates of the first contour point X... Y... Machining feed rate F...

if desired, with smooth approach: program G26 after this block 9 Machining to last contour point 5 to 8

Input: Enter all necessary values for

each contour element if desired, with smooth departure: program G27 after the last radius-compensated block

10 Move to end position 5.2/5.4

Input: Feed rate (rapid traverse) G00

Cancel radius compensation G40

Coordinates of the end position X... Y...

Miscellaneous function (spindle stop) M05 11 Retract tool in spindle axis 5.2/5.4

Input: Feed rate (rapid traverse) G00

Coordinate above the workpiece Z...

Miscellaneous function (end of program) M02

12 End of program

Page 5

How to use this manual

This manual describes functions and features available on the TNC 360 from NC software number 259 900 08.

This manual describes all available TNC functions. However, since the machine builder has modified (with machine parameters) the available range of TNC functions to interface the control to his specific machine, this manual may describe some functions which are not available on your TNC.

TNC functions which are not available on every machine are, for example:

• Probing functions for the 3D touch probe system

• Rigid tapping If in doubt, please contact the machine tool builder.

TNC programming courses are offered by many machine tool builders as well as by HEIDENHAIN. We recommend these courses as an effective way of improving your programming skill and sharing information and ideas with other TNC users.

TNC 360

Page 6

The TNC beginner can use the manual as a workbook. The first part of the manual deals with the basics of NC technology and describes the TNC functions. It then introduces the techniques of conversational programming. Each new function is thoroughly described when it is first introduced, and the numerous examples can be tried out directly on the TNC. The TNC beginner should work through this manual from beginning to end to ensure that he is capable of fully exploiting the features of this powerful tool.

For the TNC expert, this manual serves as a comprehensive reference work. The table of contents and cross references enable him to quickly find the topics and information he needs. Easy-to-read dialog flowcharts show him how to enter the required data for each function.

The dialog flow charts consist of sequentially arranged instruction boxes. Each key is illustrated next to an explanation of its function to aid the beginner when he is performing the operation for the first time. The experienced user can use the key sequences illustrated in the left part of the flowchart as a quick overview. The TNC dialogs in the instruction boxes are always presented on a gray background.

Layout of the dialog flowcharts

Dialog initiation keys

DIALOG PROMPT (ON TNC SCREEN)

e.g.

Answer the prompt with these keys

NEXT DIALOG QUESTION

Press this key

Or press this key

. . .

ENT

The functions of the keys are explained here.

Function of the key.

A dashed line means that either the key above or below it can be

Function of an alternative key.

The trail of dots indicates that:

• the dialog is not fully shown, or

• the dialog continues on the next page.

pressed.

TNC 360

Page 7

Contents User's Manual TNC 360

ISO Programming

Introduction

Manual Operation and Setup

Test Run and Program Run

Programming

Programming Tool Movements

Subprograms and Program Section Repeats

Programming with Q Parameters

Cycles

External Data Transfer

MOD-Functions

Tabels, Overviews and Diagrams

1 2 3 4 5 6 7 8

9 10 11

Page 8

1 Introduction

1.1 The TNC 360 .......................................................................................... 1-2

The Operating Panel .................................................................................................... 1-3

The Screen .................................................................................................................. 1-3

TNC Accessories ......................................................................................................... 1-5

1.2 Fundamentals of Numerical Control (NC).......................................... 1-6

Introduction ................................................................................................................. 1-6

What is NC? ................................................................................................................ 1-6

The part program ......................................................................................................... 1-6

Programming ............................................................................................................... 1-6

Reference system ....................................................................................................... 1-7

Cartesian coordinate system ....................................................................................... 1-7

Additional axes ............................................................................................................ 1-8

Polar coordinates ......................................................................................................... 1-8

Setting the pole ........................................................................................................... 1-9

Setting the datum ........................................................................................................ 1-9

Absolute workpiece positions ................................................................................... 1-11

Incremental workpiece positions .............................................................................. 1-11

Programming tool movements.................................................................................. 1-13

Position encoders ...................................................................................................... 1-13

Reference marks ...................................................................................................... 1-13

1.3 Switch-On ........................................................................................... 1-14

1.4 Graphics and Status Display ............................................................. 1-15

Plan view ................................................................................................................... 1-15

Projection in three planes .......................................................................................... 1-16

3D view .................................................................................................................... 1-16

Status display ............................................................................................................ 1-18

1.5 Programs ............................................................................................. 1-19

Program directory ...................................................................................................... 1-19

Selecting, erasing and protecting programs .............................................................. 1-20

TNC 360

Page 9

2 Manual Operation and Setup

2.1 Moving the Machine Axes ................................................................... 2-2

Traversing with the machine axis direction buttons .................................................... 2-2

Traversing with the electronic handwheel .................................................................. 2-3

Working with the HR 330 Electronic Handwheel ........................................................ 2-3

Incremental jog positioning ......................................................................................... 2-4

Positioning with manual data input (MDI) ................................................................... 2-4

2.2 Spindle Speed S, Feed Rate F and Miscellaneous Function M ........ 2-5

To enter the spindle speed S ...................................................................................... 2-5

To enter the miscellaneous function M....................................................................... 2-6

To change the spindle speed S ................................................................................... 2-6

To change the feed rate F ........................................................................................... 2-6

2.3 Setting the Datum without a 3D Touch Probe .................................. 2-7

Setting the datum in the tool axis ............................................................................... 2-7

Setting the datum in the working plane ...................................................................... 2-8

2.4 3D Touch Probe System ...................................................................... 2-9

3D Touch probe applications ....................................................................................... 2-9

Selecting the touch probe menu ................................................................................. 2-9

Calibrating the 3D touch probe.................................................................................. 2-10

Compensating workpiece misalignment ................................................................... 2-12

2.5 Setting the Datum with the 3D Touch Probe System .................... 2-14

Setting the datum in a specific axis .......................................................................... 2-14

Corner as datum ........................................................................................................ 2-15

Circle center as datum .............................................................................................. 2-17

2.6 Measuring with the 3D Touch Probe System .................................. 2-19

Finding the coordinate of a position on an aligned workpiece .................................. 2-19

Finding the coordinates of a corner in the working plane ......................................... 2-19

Measuring workpiece dimensions ............................................................................ 2-20

Measuring angles ...................................................................................................... 2-21

TNC 360

Page 10

3 Test Run and Program Run

3.1 Test Run ................................................................................................ 3-2

To do a test run ........................................................................................................... 3-2

3.2 Program Run ......................................................................................... 3-3

To run a part program .................................................................................................. 3-3

Interrupting machining ................................................................................................ 3-4

Resuming program run after an interruption ............................................................... 3-5

3.3 Blockwise Transfer: Executing Long Programs ................................. 3-6

Jumping over blocks ................................................................................................... 3-7

TNC 360

Page 11

4 Programming

4.1 Editing Part Programs .......................................................................... 4-2

Layout of a program .................................................................................................... 4-2

Editing functions.......................................................................................................... 4-3

4.2 Tools ...................................................................................................... 4-5

Determining tool data .................................................................................................. 4-5

Entering tool data into the program............................................................................. 4-7

Entering tool data in program 0 ................................................................................... 4-8

Calling tool data ........................................................................................................... 4-9

Tool change ................................................................................................................. 4-9

4.3 Tool Compensation Values ............................................................... 4-11

Effect of tool compensation values ........................................................................... 4-11

Tool radius compensation ......................................................................................... 4-11

Machining corners ..................................................................................................... 4-13

4.4 Program Creation ............................................................................... 4-14

To create a new part program ................................................................................... 4-14

Defining the blank form ............................................................................................. 4-14

4.5 Entering Tool-Related Data ............................................................... 4-17

Feed rate F ................................................................................................................ 4-17

Spindle speed S ......................................................................................................... 4-18

4.6 Entering Miscellaneous Functions and STOP .................................. 4-19

4.7 Actual Position Capture ..................................................................... 4-20

TNC 360

Page 12

5 Programming Tool Movements

5.1 General Information on Programming Tool Movements ................. 5-2

5.2 Contour Approach and Departure ...................................................... 5-4

Starting and end positions ........................................................................................... 5-4

Smooth approach and departure ................................................................................. 5-6

5.3 Path Functions ...................................................................................... 5-7

General information ..................................................................................................... 5-7

Machine axis movement under program control ........................................................ 5-7

Overview of path functions ......................................................................................... 5-9

5.4 Path Contours - Cartesian Coordinates ............................................ 5-10

Straight line at rapid traverse G00 ............................................................................. 5-10

Straight line with feed rate G01 F ... ......................................................................... 5-10

Chamfer G24 ............................................................................................................. 5-13

Circles and circular arcs - General information .......................................................... 5-15

Circle center I, J, K ................................................................................................... 5-16

Circular path G02/G03/G05 around the circle center I, J, K ...................................... 5-18

Circular path G02/G03/G05 with defined radius ........................................................ 5-21

Circular path G06 with tangential connection............................................................ 5-24

Corner rounding G25 ................................................................................................. 5-26

5.5 Path Contours - Polar Coordinates ................................................... 5-28

Polar coordinate origin: Pole I, J, K ........................................................................... 5-28

Straight line at rapid traverse G10 ............................................................................. 5-28

Straight line with feed rate G11 F ... ......................................................................... 5-28

Circular path G12/G13/G15 around pole I, J, K .......................................................... 5-30

Circular path G16 with tangential connection............................................................ 5-32

Helical interpolation ................................................................................................... 5-33

5.6 M Functions for Contouring Behavior and Coordinate Data.......... 5-36

Smoothing corners: M90 ........................................................................................... 5-36

Machining small contour steps: M97 ........................................................................ 5-37

Machining open contours: M98 ................................................................................ 5-38

Programming machine-referenced coordinates: M91/M92 ...................................... 5-39

5.7 Positioning with Manual Data Input (MDI) ...................................... 5-41

TNC 360

Page 13

6 Subprograms and Program Section Repeats

6.1 Subprograms ........................................................................................ 6-2

Principle ...................................................................................................................... 6-2

Operating limits ........................................................................................................... 6-2

Programming and calling subprograms ....................................................................... 6-3

6.2 Program Section Repeats .................................................................... 6-5

Principle ...................................................................................................................... 6-5

Programming notes ..................................................................................................... 6-5

Programming and calling a program section repeat .................................................... 6-5

6.3 Main Program as Subprogram ............................................................ 6-8

Principle ...................................................................................................................... 6-8

Operating limits ........................................................................................................... 6-8

To call a main program as a subprogram .................................................................... 6-8

6.4 Nesting .................................................................................................. 6-9

Nesting depth .............................................................................................................. 6-9

Subprogram in a subprogram ...................................................................................... 6-9

Repeating program section repeats .......................................................................... 6-11

Repeating subprograms ............................................................................................ 6-12

TNC 360

Page 14

7 Programming with Q Parameters

7.1 Part Families — Q Parameters Instead of Numerical Values ........... 7-3

7.2 Describing Contours Through Mathematical Functions................... 7-5

Overview ..................................................................................................................... 7-5

7.3 Trigonometric Functions ..................................................................... 7-7

Overview ..................................................................................................................... 7-7

7.4 If-Then Operations with Q Parameters .............................................. 7-8

Jumps ...................................................................................................................... 7-8

Overview ..................................................................................................................... 7-8

7.5 Checking and Changing Q Parameters............................................. 7-10

7.6 Output of Q Parameters and Messages ........................................... 7-11

Displaying error messages ........................................................................................ 7-11

Output through an external data interface ................................................................ 7-11

Assigning values for the PLC .................................................................................... 7-11

7.7 Measuring with the 3D Touch Probe During Program Run............ 7-12

7.8 Examples for Exercise ........................................................................ 7-14

Rectangular pocket with corner rounding and tangential approach .......................... 7-14

Bolt hole circles ......................................................................................................... 7-15

Ellipse .................................................................................................................... 7-17

Machining a hemisphere with an end mill................................................................. 7-19

TNC 360

Page 15

8 Cycles

8.1 General Overview of Cycles ................................................................ 8-2

8.2 Simple Fixed Cycles.............................................................................. 8-4

8.3 SL Cycles ............................................................................................. 8-15

Programming a cycle ................................................................................................... 8-2

Dimensions in the tool axis ......................................................................................... 8-3

PECKING G83 .............................................................................................................. 8-4

TAPPING with floating tap holder G84 ........................................................................ 8-6

RIGID TAPPING G85 ................................................................................................... 8-8

SLOT MILLING G74 .................................................................................................... 8-9

POCKET MILLING G75/G76 ...................................................................................... 8-11

CIRCULAR POCKET MILLING G77/G78 ................................................................... 8-13

CONTOUR GEOMETRY G37 .................................................................................... 8-16

ROUGH-OUT G57 ..................................................................................................... 8-17

Overlapping contours ................................................................................................ 8-19

PILOT DRILLING G56................................................................................................ 8-25

CONTOUR MILLING G58/G59 .................................................................................. 8-26

8.4 Cycles for Coordinate Transformations ........................................... 8-29

DATUM SHIFT G54 ................................................................................................... 8-30

MIRROR IMAGE G28 ................................................................................................ 8-33

ROTATION G73 ......................................................................................................... 8-35

SCALING FACTOR G72 ............................................................................................. 8-36

8.5 Other Cycles ........................................................................................ 8-38

DWELL TIME G04 ..................................................................................................... 8-38

PROGRAM CALL G39 ............................................................................................... 8-38

ORIENTED SPINDLE STOP G36 ............................................................................... 8-39

TNC 360

Page 16

9 External Data Transfer

9.1 Menu for External Data Transfer......................................................... 9-2

Blockwise transfer....................................................................................................... 9-2

9.2 Pin Layout and Connecting Cable for Data Interfaces ...................... 9-3

RS-232-C/V.24 Interface .............................................................................................. 9-3

9.3 Preparing the Devices for Data Transfer ............................................ 9-4

HEIDENHAIN devices ................................................................................................. 9-4

Non-HEIDENHAIN devices ......................................................................................... 9-4

TNC 360

Page 17

10 MOD Functions

10.1 Selecting, Changing and Exiting the MOD Functions..................... 10-2

10.2 NC and PLC Software Numbers ........................................................ 10-2

10.3 Entering the Code Number................................................................ 10-3

10.4 Setting the External Data Interfaces ................................................ 10-3

BAUD RATE .............................................................................................................. 10-3

RS-232-C Interface .................................................................................................... 10-3

10.5 Machine-Specific User Parameters ................................................... 10-4

10.6 Selecting Position Display Types ...................................................... 10-4

10.7 Selecting the Unit of Measurement ................................................. 10-5

10.8 Selecting the Programming Language............................................. 10-5

10.9 Setting the Axis Traverse Limits ....................................................... 10-6

TNC 360

Page 18

11 Tables, Overviews, Diagrams

11.1 General User Parameters ................................................................... 11-2

Selecting the general user parameters ..................................................................... 11-2

Parameters for external data transfer ....................................................................... 11-2

Parameters for 3D touch probes ............................................................................... 11-4

Parameters for TNC displays and the editor ............................................................. 11-4

Parameters for machining and program run .............................................................. 11-7

Parameters for override behavior and electronic handwheel .................................... 11-9

11.2 Miscellaneous Functions (M Functions) ......................................... 11-11

Miscellaneous functions with predetermined effect............................................... 11-11

Vacant miscellaneous functions .............................................................................. 11-12

11.3 Preassigned Q Parameters .............................................................. 11-13

11.4 Diagrams for Machining .................................................................. 11-15

Spindle speed S ....................................................................................................... 11-15

Feed rate F .............................................................................................................. 11-16

Feed rate F for tapping ............................................................................................ 11-17

11.5 Features, Specifications and Accessories ...................................... 11-18

TNC 360 .................................................................................................................. 11-18

Accessories ............................................................................................................. 11-20

11.6 TNC Error Messages ......................................................................... 11-21

TNC error messages during programming .............................................................. 11-21

TNC error messages during test run and program run............................................ 11-22

11.7 Address letters (ISO programming) ............................................... 11-25

G Functions ............................................................................................................. 11-25

Other address letters .............................................................................................. 11-26

Parameter definitions .............................................................................................. 11-27

TNC 360

Page 19

1 Introduction

1.1 The TNC 360

Control

The TNC 360 is a shop-floor programmable contouring control for milling machines, boring machines and machining centers with up to four axes. The spindle can be rotated to a given angular stop position (oriented spindle stop).

Visual display unit and operating panel

The monochrome screen clearly displays all information necessary for operating the TNC. In addition to the CRT monitor (BE 212), the TNC 360 can also be used with a flat luminescent screen (BF 110). The keys on the operating panel are grouped according to their functions. This simplifies programming and the application of the TNC functions.

Programming

The TNC 360 is programmed in ISO format. Programming with the easy to understand HEIDENHAIN plain language dialog format is also possible and is described in the TNC 360 User's Manual for HEIDENHAIN Conversational Programming.

Graphics

The graphic simulation enables you to test programs before actual machining. Various types of graphic representation can be selected.

Compatibility

The TNC 360 can execute any part program that was programmed on a TNC 150B HEIDENHAIN control or any subsequent version.

TNC 3601-2

Page 20

1 Introduction

1.1 The TNC 360

The Operating Panel

The keys on the TNC operating panel are grouped according to their functions:

• Program selection

• Address letters

• External data transfer

• Probing functions

• Editing functions

• Jump instruction GOTO

• Arrow keys

• Address letters

• NO ENT key

• Tool-related address letters

Graphic operating modes

PGM

EXT

GOTO

STOP

ENT

MOD

PGM

CALL

PGM

RND

DEL

TOUCH PROBE

CYCL

CALL

DEF

TOOL

CALL

DEF

GRAPHICS

BLK

MAGN START

FORM

100

150

F %

ENT

LBL

CALL

SET

7 8

0 Q

5 2 3

DEF

9 6

• Numerical entries

• Axis selection

END

Operating modes

100

150

S %

MOD

HEIDENHAIN

Override controls for spindle speed and feed rate

The functions of the individual keys are described on the inside front cover. An overview of the address letters used for ISO programming is provided in Chapter 11.

The machine operating buttons, such as for NC start, are described in the manual for your machine tool.

In this manual they are shown in gray.

The Screen

Brightness control (BE 212 only)

Header

The header of the screen shows the selected operating mode. Dialog questions and TNC messages also appear there.

TNC 360 1-3

Page 21

1 Introduction

1.1 The TNC 360

Screen Layout

MANUAL and EL. HANDWHEEL operating modes:

A machine operating mode has been selected

• Coordinates

• Selected axis

• ❊ means:

control is in operation

• Status display, e.g. feed rate F, miscellaneous function M

A program run operating mode has been selected

Section of selected program

Status display

The screen layout is the same in the operating modes PROGRAM RUN, PROGRAMMING AND EDITING and TEST RUN. The current block is shown between two horizontal lines.

TNC 3601-4

Page 22

1 Introduction

1.1 The TNC 360

TNC Accessories

3D Touch Probe Systems

The TNC features the following functions for the HEIDENHAIN 3D touch probe systems:

• Automatic workpiece alignment (compensation of workpiece misalignment)

• Datum setting

• Measurements of the workpiece can be performed during program run

• Digitizing 3D forms (optional, only available with HEIDENHAIN plain language dialog programming)

The TS 120 touch probe system is connected to the control via cable, while the TS 510 communicates by means of infrared light.

Fig. 1.5: HEIDENHAIN 3D Touch Probe Systems TS 120 and TS 511

Floppy Disk Unit

The HEIDENHAIN FE 401 floppy disk unit serves as an external memory for the TNC, allowing you to store your programs externally on diskette.

The FE 401 can also be used to transfer programs that were written on a PC into the TNC. Extremely long programs which exceed the TNC's memory capacity are “drip fed” block by block. The machine executes the transferred blocks and erases them immediately, freeing memory for further blocks from the FE.

Electronic Handwheels

Electronic handwheels provide precise manual control of the axis slides. As on conventional machines, turning the handwheel moves the axis by a defined amount. The traverse distance per revolution of the handwheel can be adjusted over a wide range.

Fig. 1.6: HEIDENHAIN FE 401 Floppy Disk Unit

Portable handwheels, such as the HR 330, are connected to the TNC by cable. Built-in handwheels, such as the HR 130, are built into the machine operating panel.

An adapter allows up to three handwheels to be connected simultaneously. Your machine tool builder can tell you more about the handwheel configuration of your machine.

Fig. 1.7: The HR 330 Electronic Handwheel

TNC 360 1-5

Page 23

1 Introduction

1.2 Fundamentals of Numerical Control (NC)

Introduction

This chapter addresses the following topics:

• What is NC?

• The part program

• Programming

• Reference system

• Cartesian coordinate system

• Additional axes

• Polar coordinates

• Setting the pole

• Datum setting

• Absolute workpiece positions

• Incremental workpiece positions

• Programming tool movements

• Position encoders

• Reference mark evaluation

What is NC?

NC stands for Numerical Control. Simply put, numerical control is the operation of a machine by means of coded instructions. Modern controls such as the HEIDENHAIN TNCs have a built-in computer for this purpose. Such a control is therefore also called a CNC (Computer Numerical Control).

The part program

A part program is a complete list of instructions for machining a workpiece. It contains such information as the target position of a tool movement, the tool path — i.e. how the tool should move towards the target position — and the feed rate. The program must also contain information on the radius and length of the tools, the spindle speed and the tool axis.

Programming

The TNC is programmed in the ISO format; some programming sections, however, are guided by dialog prompting. The single commands (words) can be entered in any sequence within a block (except G90/G91). The TNC automatically sorts the single commands as soon as the block is concluded.

TNC 3601-6

Page 24

1 Introduction

0° 90°90°

0°

30°

60°

Greenwich

1.2 Fundamentals of NC

Reference system

In order to define positions one needs a reference system. For example, positions on the earth's surface can be defined "absolutely" by their geographic coordinates of longitude and latitude. The term "coordinate" comes from the Latin word for "that which is arranged", i.e. dimensions used for determining or defining positions. The network of horizontal and vertical lines around the globe constitutes an "absolute reference system" – in contrast to the "relative" definition of a position that is referenced, for example, to some other, known location.

Cartesian coordinate system

On a TNC controlled milling machine a workpiece is normally machined according to a workpiece-referenced Cartesian coordinate system (a rectangular coordinate system named after the French mathematician and philosopher René Descartes, Latin: Renatus Cartesius; 1596 to 1650). The Cartesian coordinate system is based on three coordinate axes X, Y and Z, which are parallel to the machine guideways. The figure to the 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.

Fig. 1.8: The geographic coordinate system

is an absolute reference system

Fig. 1.9: Designations and directions of the

axes on a milling machine

TNC 360 1-7

Page 25

1 Introduction

1.2 Fundamentals of NC

Additional axes

The TNC can control machines that have more than three axes. U, V and W are secondary linear axes parallel to the main axes X, Y and Z, respec-

tively (see illustration). Rotary axes are also possible. They are designated as axes A, B and C.

W+

C+

B+

V+

A+

Polar coordinates

The Cartesian coordinate system is especially useful for parts whose dimensions are mutually perpendicular. But when workpieces contain circular arcs, or when dimensions are given in degrees, it is often easier to use polar coordinates. In contrast to Cartesian coordinates, which are three-dimensional, polar coordinates can only describe positions in a plane.

The datum for polar coordinates is the pole I, J, K. To describe a position in polar coordinates, think of a scale whose zero point is rigidly connected to the pole but which can be freely rotated in a plane around the pole.

Positions in this plane are defined by:

• Polar Radius R: The distance from the pole I, J

to the defined position.

• Polar Angle H: The angle between the refer-

ence axis and the scale.

U+

Fig. 1.10: Arrangement and designation of

the auxiliary axes

J = 10

Fig. 1.11: Positions on an arc with polar coordinates

I = 30

TNC 3601-8

Page 26

1 Introduction

1.2 Fundamentals of NC

Setting the pole

The pole is defined by setting two Cartesian coordinates. These two coordinates also determine the reference axis for the polar angle PA.

Coordinates of the pole Reference axis of the angle

I, J +X

J, K +Y

K, I +Z

Fig. 1.12: Polar coordinates and their associated reference axes

Setting the datum

The workpiece drawing identifies a certain prominent point on the workpiece (usually a corner) as the "absolute datum" and perhaps one or more other points as relative datums. The process of datum setting establishes these points as the origin of the absolute or relative coordinate systems: The workpiece, which is aligned with the machine axes, is moved to a certain position relative to the tool and the display is set either to zero or to another appropriate position value (e.g. to compensate the tool radius).

0°

Fig. 1.13: The workpiece datum serves as

the origin of the Cartesian coordinate system

TNC 360 1-9

Page 27

1 Introduction

1.2 Fundamentals of NC

Example:

Drawings with several relative datums (according to ISO 129 or DIN 406, Part 11; Figure 171)

1225

750

320

125

250

216,5

250

-250

-125

-216,5

125 0

-125

-216,5

-250

150 0

-150

300±0,1

325

450

700

900

950

Example:

Coordinates of the point ➀:

X = 10 mm Y = 5 mm Z = 0 mm

The datum of the Cartesian coordinate system is located 10 mm away from point ➀ on the X axis and 5 mm on the Y axis.

The 3D Touch Probe System from HEIDENHAIN is an especially convenient and efficient way to find and set datums.

Fig. 1.15: Point ➀ defines the coordinate

system.

TNC 3601-10

Page 28

1 Introduction

Z=15mm

X=20mm

Y=10mm

Z=–15mm

X=10mm

Y=10mm

1.2 Fundamentals of NC

Absolute workpiece positions

Each position on the workpiece is clearly defined by its absolute coordinates.

Example: Absolute coordinates of the position ➀:

X = 20 mm Y = 10 mm Z = 15 mm

If you are drilling or milling a workpiece according to a workpiece drawing with absolute coordinates, you are moving the tool to the coordinates.

Incremental workpiece positions

A position can be referenced to the previous nominal position: i.e. the relative datum is always the last programmed position. Such coordinates are referred to as incremental coordinates (increment = growth), or also incremental or chain dimensions (since the positions are defined as a chain of dimensions). Incremental coordinates are designated with G91.

Example: Incremental coordinates of the position ➂

referenced to position ➁ Absolute coordinates of the position ➁ :

X = 10 mm Y = 5 mm Z = 20 mm

Incremental coordinates of the position ➂ : IX = 10 mm IY = 10 mm IZ = –15 mm

If you are drilling or milling a workpiece according to a workpiece drawing with incremental coordinates, you are moving the tool by the coordinates.

An incremental position definition is therefore intended as an immediately relative definition. This is also the case when a position is defined by the distance-to-go to the target position (here the relative datum is located at the target position). The distance-to-go has a negative algebraic sign if the target position lies in the negative axis direction from the actual position.

The polar coordinate system can also express both types of dimensions:

• Absolute polar coordinates always refer to the pole I, J and the angle reference axis.

• Incremental polar coordinates always refer to

the last programmed nominal position of the tool.

Fig. 1.16: Position ➀ of the example

"absolute workpiece positions"

Fig. 1.17: Positions ➁ and ➂ of the example

"incremental workpiece positions"

G91R

G91H G91H

J = 10

0°

TNC 360 1-11

Fig. 1.18: Incremental dimensions in polar coordinates (designated

with "G91")

I = 30

Page 29

1 Introduction

1.2 Fundamentals of NC

Example: Workpiece drawing with coordinate dimensioning

(according to ISO 129 or DIN 406, Part 11; Figure 179)

2.1

2.2

2.3

3.4

3.5

3.6

3.7 3

3.8

3.9

3.10 Y2

2 1.3

3.3

3.11

3.2

3.1

3.12

1.21.1

Dimensions in mm

Coordinate Coordinates origin

Pos. X1 X2 Y1 Y2 r ϕ d

11 00 1 1.1 325 320 Ø 120 H7 1 1.2 900 320 Ø 120 H7 1 1.3 950 750 Ø 200 H7 1 2 450 750 Ø 200 H7 1 3 700 1225 Ø 400 H8 2 2.1 –300 150 Ø 50 H11 2 2.2 –300 0 Ø 50 H11 2 2.3 –300 –150 Ø 50 H11 3 3.1 250 0° Ø 26 3 3.2 250 30° Ø 26 3 3.3 250 60° Ø 26 3 3.4 250 90° Ø 26 3 3.5 250 120° Ø 26 3 3.6 250 150° Ø 26 3 3.7 250 180° Ø 26 3 3.8 250 210° Ø 26 3 3.9 250 240° Ø 26 3 3.10 250 270° Ø 26 3 3.11 250 300° Ø 26 3 3.12 250 330° Ø 26

TNC 3601-12

Page 30

1 Introduction

1.2 Fundamentals of NC

Programming tool movements

An axis position is changed either by moving the tool or by moving the machine table on which the workpiece is fixed, depending on the individual machine tool.

You always program as if the tool is moving and the workpiece is stationary.

If the machine table moves in one or several axes, the corresponding axes are designated on the machine operating panel with a prime mark (e.g. X’, Y’). When an axis is designated with a prime mark, the programmed direction of axis movement is the opposite direction of tool movement relative to the workpiece.

Position encoders

The position encoders – linear encoders for linear axes, angle encoders for rotary axes – convert the movement of the machine axes into electrical signals. The control evaluates these signals and constantly calculates the actual position of the machine axes.

If there is an interruption in power, the calculated position will no longer correspond to the actual position. When power is returned, the TNC can re-establish this relationship.

Reference marks

The scales of the position encoders contain one or more reference marks. When a reference mark is passed over, it generates a signal which identifies that position as the machine axis reference point. With the aid of these reference marks the TNC can re-establish the assignment of displayed positions to machine axis positions.

Fig. 1.20: On this machine the tool moves in

the Y and Z axes; the machine table moves in the positive X' axis direction.

Fig. 1.21: Linear position encoder, here for

the X axis

If the position encoders feature distance-coded reference marks, each axis need only move a maximum of 20 mm (0.8 in.) for linear encoders, and 20° for angle encoders.

Fig. 1.22: Linear scales: above with

distance-coded-reference marks, below with one reference mark

TNC 360 1-13

Page 31

1 Introduction

1.3 Switch-On

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

MEMORY TEST

The TNC memory is automatically checked.

POWER INTERRUPTED

Message from the TNC indicating that the power was interrupted. Clear the message.

TRANSLATE PLC PROGRAM

The PLC program of the TNC is automatically translated.

RELAY EXT. DC VOLTAGE MISSING

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

MANUAL OPERATION

TRAVERSE REFERENCE POINTS

To cross over the reference marks in the displayed sequence: Press the machine START button for each axis.

To cross over the reference marks in any sequence: For each axis, press and hold down the machine axis direction button until the reference mark has been crossed over.

, , ...

The TNC is now ready for operation in the MANUAL OPERATION mode.

TNC 3601-14

Page 32

1 Introduction

1.4 Graphics and Status Display

The TNC features various graphic display modes for testing programs. To be able to use this feature, you must select a program run operating mode.

Workpiece machining is simulated graphically in the display modes:

• Plan view

• Projection in three planes

• 3D view

With the fast internal image generation, the TNC calculates the contour and displays a graphic only of the completed part.

Select display mode

GRAPHICS

MOD

2 x

Select display mode menu.

Plan view

Select desired display mode.

ENT

Confirm selection.

Start graphic display

GRAPHICS

START

Start graphic simulation in the selected display mode.

The START key repeats a graphic simulation as often as desired.

Rotary axis movements cannot be graphically simulated. An attempted test run will result in an error message.

In this mode, contour height is shown by image brightness. The deeper the contour, the darker the image.

Number of depth levels: 7

This is the fastest of the three display modes.

Fig. 1.23: TNC graphics, plan view

TNC 360 1-15

Page 33

1 Introduction

1.4 Graphics and Status Display

Projection in three planes

Here the program is displayed as in a technical drawing, with a plan view and two orthographic sections. A conical symbol near the graphic indicates whether the display is in first angle or second angle projection according to ISO 6433, Part 1. The type of projection can be selected with MP 7310.

Moving the sectional planes

The sectional planes can be moved to any position with the arrow keys. The position of the sectional plane is displayed on the screen while it is being moved.

3D view

This mode displays the simulated workpiece in three-dimensional space.

Fig. 1.24: TNC graphics, projection in three planes

Fig. 1.25: TNC graphics, 3D view

Rotating the 3D view

In the 3D view, the image can be rotated around the vertical axis with the horizontal arrow keys. The angle of orientation is indicated with a special symbol:

rotation

900 rotation

1800 rotation

rotation

270

Fig. 1.26: Rotated 3D view

3D view, not true to scale

If the height-to-side ratio is between 0.5 and 50, a non-scaled 3D view can be selected with the vertical arrow keys. This view improves the resolution of the shorter workpiece side.

The angle orientation symbol also indicates the angle of orientation of the non-scaled 3D view.

TNC 3601-16

Page 34

1 Introduction

1.4 Graphics and Status Display

Detail magnification of a 3D graphic

Fig. 1.27: Detail magnification of a 3D graphic

GRAPHICS

MAGN

Select function for detail magnification.

Select sectional plane.

Set / reset section.

If desired: switch dialog for transfer of detail.

TRANSFER DETAIL = ENT

ENT

Magnify detail.

Details can be magnified in any display mode. The abbreviation MAGN appears on the screen to indicate that the image is magnified.

Return to non-magnified view

GRAPHICS

BLK

FORM

Press BLK FORM to display the workpiece in its programmed size.

TNC 360 1-17

Page 35

1 Introduction

1.4 Graphics and Status Display

Status Display

The status display in a program run operating mode shows the current coordinates as well as the following information:

• Type of position display (ACTL, NOML, ...)

• Axis locked ( in front of the axis)

• Number of current tool T

• Tool axis

• Spindle speed S

• Feed rate F

• Active miscellaneous function M

• TNC is in operation (indicated by ❊)

• Machines with gear ranges:

Gear range following "/" character (depends on machine parameter)

Bar graphs can be used to indicate analog quantities such as spindle speed and feed rate in the status display. These bar graphs must be activated by the machine tool builder.

Fig. 1.28: Status display in a program run operating mode

TNC 3601-18

Page 36

1 Introduction

1.5 Programs

The TNC 360 can store up to 32 part programs at once. The part programs can be written in HEIDENHAIN plain language dialog or according to ISO. ISO programs are indicated with “ISO”.

Each program is identified by a number with up to eight characters.

Program directory

The program directory is called with the PGM NR key. To erase programs in the TNC memory, press the CL PGM key.

The program directory provides the following information:

• Program number

• Program type (HEIDENHAIN or ISO)

• Program size in bytes, where one byte is the equivalent of one character.

Action Mode of Call program

operation directory with...

Create (a program) ...

Edit ...

Erase ...

Test ...

Execute ...

Fig. 1.29: Program management functions

PGM

Fig. 1.30: Program directory on the TNC screen

TNC 360 1-19

Page 37

1 Introduction

1.5 Programs

Selecting, erasing and protecting programs

To select a program:

PGM

PROGRAM NUMBER ?

ENT

To erase a program:

PGM

ERASE = ENT / END = NO ENT

Call the program management.

Use the arrow keys to highlight the program.

Enter the desired program number, for example 15.

Confirm your selection.

Press CL PGM to call the program management.

Use the arrow keys to highlight the program.

ENT

Erase the program or abort.

ENT

To protect a program:

PGM

Call the program management.

PROGRAM NUMBER = ?

e.g.

ENT

Enter the number of the program to be protected, for example program number 5.

Use the arrow key to highlight the first block.

END

Enter the function for program protection, conclude the block.

Resulting NC block: %5 G71 G50 *

Removing edit protection

To remove edit protection re-select the program and enter the code number 86357 with the corresponding MOD function (see page 10-3).

TNC 3601-20

Page 38

1 Introduction

1.5 Programs

To remove edit protection:

Select the protected program, for example program number 5.

0 BEGIN 5 MM P

MOD

VACANT BYTES =

repeatedly

CODE NUMBER

8 6

5 7

Select MOD functions.

Activate the CODE NUMBER function.

Enter the code number 86357: Edit protection is removed, the "P" disappears.

TNC 360 1-21

Page 39

2 Manual Operation and Setup

2.1 Moving the Machine Axes

Traversing with the machine axis direction buttons

MANUAL OPERATION

e.g.

You can move several axes at once in this way.

For continuing movement:

MANUAL OPERATION

e.g.

together

You can only move one axis at a time with this method.

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

Press and hold the machine axis direction button, then press the machine START button. The axis continues to move after you release the keys.

To stop the axis, press the machine STOP button.

TNC 3602-2

Page 40

2 Manual Operation and Setup

2.1 Moving the Machine Axes

Traversing with the electronic handwheel

ELECTRONIC HANDWHEEL

INTERPOLATION FACTOR: 1 3

e.g.

Now move the selected axis with the electronic handwheel. If you are using the portable handwheel, first press the enabling switch on its back.

Interpolation

factor

0 1 2 3 4 5 6 7 8 9

Fig. 2.1: Interpolation factors and paths of traverse

ENT

Traverse in mm per

revolution

20.000

10.000

Enter the desired interpolation factor (see table below).

Select the axis that you wish to move: for portable handwheels, at the handwheel; for integral handwheels, at the TNC keyboard.

5.000

2.500

1.250

0.625

0.312

0.156

0.078

0.039

0.019

Fig. 2.2: HR 330 Electronic Handwheel

The smallest programmable interpolation factor depends on the individual machine tool. Positioning with the electronic handwheel can also be carried out in the operating mode PROGRAMMING AND EDITING (depending on MP7641).

Working with the HR 330 Electronic Handwheel

Attach the electronic handwheel to a steel surface with the mounting magnets such that it cannot be operated unintentionally.

Be sure not to press the axis direction buttons unintentionally when you remove the handwheel from its position as long as the enabling switch (between the magnets) is depressed.

If you are using the handwheel for machine setup, press the enabling switch. Only then can you move the axes with the axis direction buttons.

TNC 360 2-3

Page 41

2 Manual Operation and Setup

8 8

816

2.1 Moving the Machine Axes

Incremental jog positioning

With incremental jog positioning, a machine axis will move by a preset increment each time you press the corresponding machine axis direction button.

Fig. 2.3: Incremental jog positioning in the

ELECTRONIC HANDWHEEL

INTERPOLATION FACTOR: 4

Select incremental jog positioning.

Select incremental jog positioning by pressing the handwheel mode key again.

ELECTRONIC HANDWHEEL

JOG-INCREMENT: 4 8

e.g.

ENT

Enter the jog increment, for example 8 mm.

Press the machine axis direction button as often as desired.

X axis

Incremental jog positioning must be enabled by the machine tool builder.

Positioning with manual data input (MDI)

Page 5-41 describes positioning by manually entering the target coordinates for the tool.

TNC 3602-4

Page 42

2 Manual Operation and Setup

2.2 Spindle Speed S, Feed Rate F and Miscellaneous Function M

The following values can be entered and changed in the MANUAL OPERATION and ELECTRONIC HANDWHEEL modes of operation:

• Miscellaneous function M

• Spindle speed S

• Feed rate F (can be changed but not entered)

For part programs these functions are entered or edited directly in the PROGRAMMING AND EDITING operating mode.

To enter the spindle speed S

N10 S

e.g.

A miscellaneous function M starts spindle rotation at the entered speed S.

END

Fig. 2.4: Knobs for spindle speed and feed

rate overrides

Select the S function key.

Enter the spindle speed S, for example 1000 rpm.

Confirm the spindle speed S with the machine START button.

TNC 360 2-5

Page 43

2 Manual Operation and Setup

2.2 Spindle Speed S, Feed Rate F and Miscellaneous Function M

To enter the miscellaneous function M

N10 M

ENT

e.g.

Chapter 11 provides an overview of the miscellaneous functions.

To change the spindle speed S

100

15050

S %

The spindle speed override will function only if your machine tool is equipped with a stepless spindle drive.

Select the M function key.

Enter the desired miscellaneous function M, for example M6.

Activate the miscellaneous function M with the machine START button.

Turn the spindle speed override knob: Adjust the spindle speed S to between 0% and 150% of the last entered value.

To change the feed rate F

In the MANUAL OPERATION mode the feed rate is set through a machine parameter.

100

15050

F %

Turn the feed rate override knob: Adjust the feed rate to between 0% and 150% of the last entered value.

TNC 3602-6

Page 44

2 Manual Operation and Setup

2.3 Setting the Datum without a 3D Touch Probe

You fix a datum by setting the TNC position display to the coordinates of a known point on the workpiece. The fastest, easiest and most accurate way of setting the datum is by using a 3D touch probe system from HEIDENHAIN (see page 2-14).

To prepare the TNC:

Clamp and align the workpiece.

Insert the zero tool with known radius into the spindle.

Select the MANUAL OPERATION mode.

Ensure that the TNC is showing actual position values (see p. 10-4).

Setting the datum in the tool axis

Protective arrangement: If the workpiece surface must not be scratched, you can lay a metal shim of known thickness d on it. Then enter a tool axis datum value that is larger than the desired datum by the value d.

Move the tool until it touches workpiece surface.

e.g.

Fig. 2.5: Datum setting in the tool axis; right with protective shim

Select the tool axis.

DATUM SET Z =

ENT

e.g.

5 0

e.g.

TNC 360 2-7

ENT

For a zero tool: Set the display to Z = 0 or enter thickness d of the shim.

For a preset tool: Set the display to the length L of the tool, for example Z=50 mm, or enter the sum Z=L+d.

Page 45

2 Manual Operation and Setup

2.3 Setting the Datum without a 3D Touch Probe

Setting the datum in the working plane

Move the zero tool until it touches the side of the workpiece.

e.g.

ENT

–R

Fig. 2.6: Setting the datum in the working plane; plan view (upper

right)

Select the axis.

Enter the position of the tool center (here X = –5 mm) in the selected axis. Be careful to enter the correct algebraic sign.

Repeat the process for all axes in the working plane.

TNC 3602-8

Page 46

2 Manual Operation and Setup

2.4 3D Touch Probe System

3D Touch probe applications

The TNC provides touch functions for application of a HEIDENHAIN 3D touch probe. Typical applications for the touch probe system are:

• Compensating workpiece misalignment (basic rotation)

• Datum setting

• Measuring:

- Lengths and positions on the workpiece

- Angles

- Circle radii

- Circle centers

• Measurements under program control

• Digitizing 3D surfaces (optional, only available with HEIDENHAIN plain language dialog programming.)

The TNC must be specially prepared by the machine tool builder for the use of a 3D touch probe.

After you press the machine START button, the touch probe begins executing the selected probe function. The machine tool builder sets the feed rate F at which the probe approaches the workpiece. When the 3D touch probe contacts the workpiece, it

• transmits a signal to the TNC, which stores the coordinates of the probed position

• stops moving

• returns to its starting position in rapid traverse

Selecting the touch probe menu

Fig. 2.7: HEIDENHAIN TS 120 three-

dimensional touch probe system

max

Fig. 2.8: Feed rates during probing

MANUAL OPERATION

ELECTRONIC HANDWHEEL

TOUCH PROBE

CALIBRATION EFFECTIVE LENGTH CALIBRATION EFFECTIVE RADIUS BASIC ROTATION SURFACE = DATUM CORNER = DATUM CIRCLE CENTER = DATUM

TNC 360 2-9

Select the menu of touch probe functions.

Page 47

2 Manual Operation and Setup

2.4 3D Touch Probe System

Calibrating the 3D Touch Probe

The touch probe system must be calibrated

• for commissioning

• after a stylus breaks

• when the stylus is changed

• when the probe feed rate is changed

• in case of irregularities, such as those resulting from machine heating. During calibration, the TNC finds the “effective” length of the stylus and

the “effective” radius of the ball tip. To calibrate the 3D touch probe, clamp a ring gauge with known height and known internal radius to the machine table.

To calibrate the effective length

Set the datum in the tool axis such that for the machine tool table, Z=0.

TOUCH PROBE

SURFACE = DATUM

Fig. 2.9: Calibrating the touch probe length

ENT

CALIBRATION EFFECTIVE LENGTH

TOOL AXIS = Z

e.g.

Move the touch probe to a position just above the ring gauge.

Select the calibration function for the touch probe length.

Z+ Z–

If necessary, enter the tool axis, for example Z.

Move the highlight to DATUM.

Enter the height of the ring gauge, for example 5 mm.

If necessary, change the displayed traverse direction.

The 3D touch probe contacts the upper surface of the ring gauge.

TNC 3602-10

Page 48

2 Manual Operation and Setup

2.4 3D Touch Probe System

To calibrate the effective radius

Position the ball tip in the bore hole of the ring gauge.

Fig. 2.10: Calibrating the touch probe radius

TOUCH PROBE

Displaying calibration values

The effective length and radius of the 3D touch probe are stored in the TNC for use whenever the touch probe is needed again. The stored values are displayed the next time the calibration function is called.

SURFACE = DATUM

ENT

CALIBRATION EFFECTIVE RADIUS

X+ X– Y+ Y–

RADIUS RING GAUGE = 0

ENT

4 x

Select the calibration function for the ball-tip radius.

Select RADIUS RING GAUGE.

Enter the radius of the ring gauge, for example 5 mm.

The 3D touch probe contacts one position on the bore for each axis direction.

TNC 360 2-11

Page 49

2 Manual Operation and Setup

2.4 3D Touch Probe System

Compensating workpiece misalignment

The TNC electronically compensates workpiece misalignment by computing a “basic rotation.” Set the ROTATION ANGLE to the angle at which a workpiece surface should be oriented with respect to the angle reference axis (see p. 1-9) of the working plane.

A B

TOUCH PROBE

SURFACE = DATUM

ENT

Select the BASIC ROTATION probe function.

BASIC ROTATION

X+ X- Y+ Y–

ROTATION ANGLE =

e.g.

ENT

Enter the nominal value of the ROTATION ANGLE.

Move the ball tip to a starting position

X + X – Y + Y –

Select the probing direction.

Fig. 2.11: Basic rotation of a workpiece, probing procedure for com-

near the first touch point 1.

pensation (right). The dashed line is the nominal position; the angle PA is being compensated.

Move the ball tip to a starting position

Probe the workpiece.

near the second touch point 2.

Probe the workpiece.

A basic rotation is kept in non-volatile storage and is effective for all subsequent program runs and graphic simulations.

TNC 3602-12

Page 50

2 Manual Operation and Setup

2.4 3D Touch Probe System

Displaying basic rotation

The angle of the basic rotation is shown in the rotation angle display. When a basic rotation is active the abbreviation ROT is highlighted in the status display.

To cancel a basic rotation:

Select BASIC ROTATION again.

Fig. 2.12: Displaying the angle of an active basic rotation

ROTATION ANGLE =

ENT

END

Set the ROTATION ANGLE to 0.

Terminate the probe function.

TNC 360 2-13

Page 51

2 Manual Operation and Setup

2.5 Setting the Datum with the 3D Touch Probe System

The following functions for setting the datum on an aligned workpiece are listed for in the TCH PROBE menu:

• Datum setting in any axis with SURFACE = DATUM

• Setting a corner as datum with CORNER = DATUM

• Setting the datum at a circle center with CIRCLE CENTER = DATUM

Setting the datum in a specific axis

Select the probe function SURFACE = DATUM.

Move the touch probe to a starting position near the touch point.

SURFACE = DATUM

X + X – Y + Y – Z + Z –

Select the probing direction and the axis in which you wish to set the datum, for example Z in the Z– direction.

Probe the workpiece.

Enter the nominal coordinate of the DATUM.

e.g.

ENT

Fig. 2.13: Probing for the datum in the Z axis

TNC 3602-14

Page 52

2 Manual Operation and Setup

2.5 Setting the Datum with the 3D Touch Probe System

Corner as datum

Y=?

Fig. 2.14: Probing procedure for finding the coordinates of the

Select the CORNER = DATUM probe function.

To use the points that were just probed for a basic rotation:

TOUCH POINTS OF BASIC ROTATION?

ENT

Transfer the touch point coordinates to memory.

X=?

corner P

Move the touch probe to a starting position near the first touch point on the side that was not probed for basic rotation.

CORNER = DATUM

X + X – Y + Y –

Move the touch probe to a starting position near the second touch point on the same side.

DATUM X =

e.g.

ENT

Select the probing direction.

Probe the workpiece.

Enter the first coordinate of the datum, for example in the X axis.

. . .

TNC 360 2-15

Page 53

2 Manual Operation and Setup

2.5 Setting the Datum with the 3D Touch Probe System

. . .

Select the second coordinate.

DATUM Y =

e.g.

ENT

END

Enter the second coordinate of the datum, for example in the Y axis.

Terminate the probe function.

If you do not wish to use points that were just probed for a basic rotation:

TOUCH POINTS OF BASIC ROTATION?

ENT

Ignore the dialog prompt.

Probe both workpiece sides twice.

Enter the datum coordinates.

TNC 3602-16

Page 54

2 Manual Operation and Setup

2.5 Setting the Datum with the 3D Touch Probe System

Circle center as datum

With this function you can set the datum at the center of bore holes, circular pockets, cylinders, journals, circular islands etc.

Inside circle

The TNC automatically probes the inside wall in all four coordinate axis directions.

For incomplete circles (circular arcs) you can choose the appropriate probing direction.

Y+

X–

X+

Y–

Select the CIRCLE CENTER = DATUM probe function.

Move the touch probe to a position approximately in the center of the circle.

CIRCLE CENTER = DATUM

X + X – Y + Y –

4 x

DATUM X =

e.g.

ENT

The probe touches four points on the inside of the circle.

Enter the first coordinate of the circle center, for example in the X axis.

Fig. 2.15: Probing an inside cylindrical

surface to find the center

Select the second coordinate.

DATUM Y =

e.g.

TNC 360 2-17

END

ENT

Enter the second coordinate of the circle center, for example in the Y axis.

Terminate the probe function.

Page 55

2 Manual Operation and Setup

X–

X+

Y+

Y–

2.5 Setting the Datum with the 3D Touch Probe System

Outside circle

Select the CIRCLE CENTER = DATUM probe function.

Move the touch probe to a starting position near the first touch point

CIRCLE CENTER = DATUM

X + X – Y + Y –

Repeat the probing process for points

Select the probing direction.

Probe the workpiece.

and 4 (see Fig. 2.16).

2, 3

Enter the coordinates of the circle center.

Fig. 2.16: Probing an outside cylindrical

outside of the circle.

surface to find the center

After the probing procedure is completed, the TNC displays the coordinates of the circle center and the circle radius PR.

TNC 3602-18

Page 56

2 Manual Operation and Setup

2.6 Measuring with the 3D Touch Probe System

With the 3D touch probe system you can determine

• Position coordinates, and from them,

• dimensions and angles on the workpiece.

Finding the coordinate of a position on an aligned workpiece

Select the SURFACE = DATUM probe function.

Move the touch probe to a starting position near the touch point.

SURFACE = DATUM

X + X – Y + Y – Z + Z –

The TNC displays the coordinate of the touch point as DATUM.

Select the probing direction and the axis in which you wish to find the coordinate.

Probe the workpiece.

Finding the coordinates of a corner in the working plane

Find the coordinates of the corner point as described under “Corner as datum.” The TNC displays the coordinates of the probed corner as DATUM.

TNC 360 2-19

Page 57

2 Manual Operation and Setup

2.6 Measuring with the 3D Touch Probe System

Measuring workpiece dimensions

Select the SURFACE = DATUM probe function.

Move the probe to a starting position near the first touch point 1.

SURFACE = DATUM

X + X – Y + Y – Z + Z –

Use the arrow keys to select the probing direction.

Fig. 2.17: Measuring lengths with the 3D

touch probe

If you will need the current datum later, write down the value that appears in the DATUM display.

DATUM X =

ENT

END

Re-select the SURFACE = DATUM probe function.

Move the touch probe to a starting position near the second touch point

Probe the workpiece.

Set the DATUM to 0.

Terminate the dialog.

. . .

TNC 3602-20

Page 58

2 Manual Operation and Setup

2.6 Measuring with the 3D Touch Probe System

. . .

SURFACE = DATUM

X + X – Y + Y – Z + Z –

The value displayed as DATUM is the distance between the two points on the coordinate axis.

To return to the datum that was active before the length measurement:

Select the SURFACE = DATUM probe function.

Probe the first touch point again.

Set the datum to the value that you wrote down previously.

END

Select the probing direction with the arrow keys – same axis as for 1.

Probe the workpiece.

Terminate the dialog.

Measuring angles

You can also use the 3D touch probe system to measure angles in the working plane. You can measure

• the angle between the angle reference axis and a workpiece side, or

• the angle between two sides. The measured angle is displayed as a value of maximum 90°.

To find the angle between the angle reference axis and a side of the workpiece:

Select the BASIC ROTATION probe function.

ROTATION ANGLE =

If you will need the current basic rotation later, write down the value that appears under ROTATION ANGLE.

Make a basic rotation with the side of the workpiece (see “Compensating workpiece misalignment”).

. . .

TNC 360 2-21

Page 59

2 Manual Operation and Setup

2.6 Measuring with the 3D Touch Probe

. . .

The angle between the angle reference axis and the side of the workpiece appears as the ROTATION ANGLE in the BASIC ROTATION function.

Cancel the basic rotation.

Restore the previous basic rotation by setting the ROTATION ANGLE to the value that you wrote down previously.

To measure the angle between two sides of a workpiece:

Fig. 2.18: Measuring the angle between two

Select the BASIC ROTATION probe function.

ROTATION ANGLE =

If you will need the current basic rotation later, write down the value that appears under ROTATION ANGLE.

Make a basic rotation for the first side (see “Compensating workpiece misalignment“).

Probe the second side as for a basic rotation, but do not set the ROTATION ANGLE to zero!

The angle PA between the workpiece sides appears as the ROTATION ANGLE in the BASIC ROTATION function.

Cancel the basic rotation.

sides of a workpiece

Restore the previous basic rotation by setting the ROTATION ANGLE to the value that you wrote down previously.

TNC 3602-22

Page 60

3 Test Run and Program Run

3.1 Test Run

In the TEST RUN mode of operation the TNC checks programs and program sections for the following errors without moving the machine axes:

• Geometrical incompatibility

• Missing data

• Impossible jumps

The following TNC functions can be used in the TEST RUN operating mode:

• Test interruption at any block

• Optional block skip

To do a test run

TEST RUN TO BLOCK NUMBER =

e.g.

ENT

Test the entire program.

Test the program up to the entered block, for example block 10.

Test run functions

Function Key

• Interrupt the test run

• Continue test run after interruption

ENT

TNC 3603-2

Page 61

3 Test Run and Program Run

3.2 Program Run

In the PROGRAM RUN / FULL SEQUENCE mode of operation the TNC executes a part program continuously to its end or up to a program stop.

In the PROGRAM RUN /SINGLE BLOCK mode of operation you execute each block separately by pressing the machine START button.

The following TNC functions can be used during a program run:

• Interrupt program run

• Start program run from a certain block

• Blockwise transfer of very long programs from external storage

• Checking/changing Q parameters

• Graphic simulation of a program run

To run a part program

• Clamp the workpiece to the machine table.

• Set the datum

• Select the program.

PROGRAM RUN / SINGLE BLOCK

PROGRAM RUN / FULL SEQUENCE

Select the part program.

GOTO

ENT

Go to the first block of the program.

Run the part program.

Only in mode

PROGRAM RUN /

SINGLE BLOCK

Run each block of the part program separately.

repeatedly

The feed rate and spindle speed can be changed with the override knobs.

TNC 360 3-3

Page 62

3 Test Run and Program Run

3.2 Program Run

Interrupting machining

There are various ways to interrupt a program run:

• Programmed interruptions

• External STOP key

• Switching to PROGRAM RUN / SINGLE BLOCK

• EMERGENCY STOP button

If the TNC registers an error during program run, it automatically interrupts machining.

Programmed interruptions

Interruptions can be programmed directly in the part program. The part program is interrupted at a block containing one of the following entries:

• G38

• Miscellaneous functions M0, M02 or M30

• Miscellaneous function M06, if the machine tool builder has assigned a stop function

To interrupt or abort machining immediately:

The block which the TNC is currently executing is not completed.

Interrupt machining.

The ❊ sign in the status display blinks.

The part program can be aborted with the D key.

The ❊ sign disappears from the status display.

To interrupt machining by switching to the PROGRAM RUN / SINGLE BLOCK operating mode:

You can interrupt the program run at the end of the current block.

Abort program run.

Select PROGRAM RUN / SINGLE BLOCK.

TNC 3603-4

Page 63

3 Test Run and Program Run

3.2 Program Run

Resuming program run after an interruption

When a program run is interrupted the TNC stores:

• The data of the last called tool

• Active coordinate transformations

• The coordinates of the last defined circle center

• The count of a running program section repeat

• The number of the last block that calls a subprogram or a program section repeat

Resuming program run with the START button

You can resume program run by pressing the machine START button if the program was interrupted in one of the following ways:

• Pressing the machine STOP button

• A programmed interruption

• Pressing the EMERGENCY STOP button (machine-dependent function).

Resuming program run after an error

• If the error message is not blinking:

Remove the cause of the error.

Clear the error message from the screen.

Restart the program.

• If the error message is blinking:

ON0I

OFF

Switch off the TNC and the machine.

Remove the cause of the error.

Restart the program.

• If you cannot correct the error:

Write down the error message and contact your repair service agency.

TNC 360 3-5

Page 64

3 Test Run and Program Run

3.3 Blockwise Transfer: Executing Long Programs

Part programs that occupy more memory than the TNC provides can be “drip fed” block by block from an external storage device.

During program run, the TNC transfers program blocks from a floppy disk unit or PC through its data interface, and erases them after execution.

To prepare for blockwise transfer:

• Prepare the data interface.

• Configure the data interface with the MOD function (see page 10-3).

• If you wish to transfer a part program from a PC, adapt the TNC and PC to each other (see pages 9-4 and 11-2).

• Ensure that the transferred program meets the following requirements:

- The highest block number must not exceed 65534. However, the

block numbers can repeat themselves as often as necessary.

- All programs called from the transferred program must be present in

the TNC memory

- The transferred program must not contain:

Subprograms Program section repetitions The function D 15:PRINT

- The TNC can store up to 20 G99 blocks.

PROGRAM RUN / SINGLE BLOCK

TEST RUN

EXT

PROGRAM NUMBER

e.g.

1 0

ENT

Select the function for blockwise transfer.

Enter the program number and start data transfer.

Execute the transferred program blocks.

If the data transfer is interrupted, press the machine START button again.

TNC 3603-6

Page 65

3 Test Run and Program Run

3.3 Blockwise Transfer: Executing Long Programs

Jumping over blocks

The TNC can jump to any desired block in the program to begin transfer. The preceding blocks are ignored during a program run.

Select the program and start transfer.

GOTO

e.g.

ENT

Enter the block number at which you wish to begin data transfer, for example 150.

Execute the transferred blocks, starting with the block number that you entered.

TNC 360 3-7

Page 66

4 Programming

In the PROGRAMMING AND EDITING mode of operation you can do such things as

• creating,

• adding to, and

• editing files.

This chapter describes basic functions and programming input that do not cause machine axis movement. The entry of geometry for workpiece machining is described in the next chapter.

4.1 Editing Part Programs

Layout of a program

A part program consists of individual program blocks.

Block:

The TNC numbers the blocks in ascending order. The block number increment is defined through the machine parameter MP 7220 (see page 11-5). Program blocks contain units of information called "words".

Fig. 4.1: Program blocks contain words of specific information

Function Key

• Continue the dialog

• Ignore the dialog question

• End the block

• Erase the block / Erase the word

N10 G00 G40 G90 X+100 Y+20 M3

Path

function Block Words Number

ENT

END

DEL

TNC 3604-2

Page 67

4 Programming

4.1 Editing Part Programs

Editing functions

Editing means entering, adding to or changing commands and information for the TNC.

The TNC enables you to

• Enter data with the keyboard

• Select desired blocks and words

• Insert and erase blocks and words

• Correct erroneously entered values and commands

• Easily clear TNC messages from the screen

Types of input

Numbers, coordinate axes and radius compensation are entered directly by keyboard. You can set the algebraic sign either before, during or after a numerical entry.

Selecting blocks and words

• To call a block with a certain block number:

GOTO

e.g.

ENT

Block number 10 is highlighted.

• To move one block forward or backward:

Press the vertical arrow keys.

• To select individual words in a block:

Press the horizontal arrow keys.

• To find the same word in other blocks:

Select the word in the block.

Jump to the same word in other blocks.

Inserting blocks

Additional program blocks can be inserted behind any existing block (except the N9999 block).

e.g.

GOTO

ENT

Select the block in front of the desired insertion.

Program the new block.

4-3TNC 360

Page 68

4 Programming

4.1 Editing Part Programs

Editing and inserting words

Highlighted words can be changed as desired: simply overwrite the old value with the new one. After entering the new information, press a horizontal arrow key to remove the highlight from the block or confirm the change with the END key. You can also insert new words into a specific block by moving the highlight to the desired block with the horizontal arrow keys.

Erasing blocks and words

Function Key

• Set the selected number to 0

• Erase an incorrect number

• Clear a non-blinking error message

• Delete the selected word

• Delete the selected block

• Erase program sections: First select the last block of the program

section to be erased.

DEL

TNC 3604-4

Page 69

4 Programming

4.2 Tools

Each tool is identified by a number.

The tool data, consisting of the:

• Length L, and

• Radius R are assigned to the tool number.

The tool data can be entered:

• into the individual part program in a G99 block, or

• once for each tool into a common tool table that is stored as program 0.

Once a tool is defined, the TNC then associates its dimensions with the tool number and accounts for them when executing positioning blocks.

Determining tool data

Tool number

Each tool is designated with a number between 0 and 254.

The tool with the number 0 is defined as having length L = 0 and radius R = 0. In tool tables, T0 should also be defined with L = 0 and R = 0.

Tool radius R

The radius of the tool is entered directly.

Tool length L

The compensation value for the tool length is measured

• as the difference in length between the tool and a zero tool, or

• with a tool pre-setter.

A tool pre-setter eliminates the need to define a tool in terms of the difference between its length and that of another tool.

4-5TNC 360

Page 70

4 Programming

4.2 Tools

Determining tool length with a zero tool

For the sign of the tool length L: L > L

L < L0A negative value means the tool is

A positive value means the tool is longer than the zero tool.

shorter than the zero tool.

L >0

L <0

Fig. 4.2: Tool lengths can be given as the difference from the zero

tool

Move the zero tool to the reference position in the tool axis (e.g. workpiece surface with Z = 0).

If necessary, set the datum in the tool axis to 0.

Change tools.

Move the new tool to the same reference position as the zero tool.

The TNC displays the compensation value for the length L of the tool.

Write the value down and enter it later.

Enter the display value by using the "actual position capture" function (see page 4-20).

TNC 3604-6

Page 71

4 Programming

4.2 Tools

Entering tool data into the program

The following data can be entered for each tool in the part program:

• Tool number

• Tool length compensation value L

• Tool radius R

To enter tool data in the program block:

e.g.

1 0

e.g.

ENT

END

Designate the tool with a number, for example 5.

Enter the compensation value for the tool length, for example L = 10mm.

Enter the tool radius, for example R = 5mm.

TOOL NUMBER T

TOOL LENGTH L

TOOL RADIUS R

Resulting NC block: G99 T5 L+10 R+5

You can enter the tool length L directly in the tool definition by using the "actual position capture" function (see page 4-20).

4-7TNC 360

Page 72

4 Programming

4.2 Tools

Entering tool data in program 0

The data for all tools can be entered in a common tool table. The number of tools in the table is selected through the machine parameter MP 7260.

If your machine uses an automatic tool changer, the tool data must be stored in the tool table.

Editing the tool table (program 0)

PROGRAMMING AND EDITING

PGM

Call the program directory.

PROGRAM NUMBER =

ENT

Select the tool table.

In the ELECTRONIC HANDWHEEL and MANUAL modes of operation, you can call the tool table at any time by simply pressing ENT.

Data in the tool table

The tool table contains further information in addition to the tool dimensions.

Abbreviation

P L R

Fig. 4.3: Tool table

Input

Tool number: the number with which the tool is called in a

part program Special tool with large radius requiring more than one

pocket in the tool magazine. A certain number of pockets is kept vacant on each side of the special tool. The letter S then appears in front of the tool number.

Pocket number of the tool in the magazine Compensation value for the Length of the tool

Radius of the tool

Dialog

–

SPECIAL TOOL? YES = ENT / NO = NO ENT

POCKET NUMBER? TOOL LENGTH L? TOOL RADIUS R?

TNC 3604-8

Page 73

4 Programming

4.2 Tools

Calling tool data

The following data can be programmed in the T block:

• Tool number, Q parameter

• Working plane with G17/G18 or G19

• Spindle speed S

To call the tool data:

Resulting NC block: T5 G17 S500

Tool pre-selection with tool tables

If you are using tool tables, you can indicate which tool you will next need by entering a G51 block. Simply enter the tool number or a corresponding Q parameter.

Tool change

Automatic tool change

If your machine is built for automatic tool changing, the TNC controls the replacement of the inserted tool by another from the tool magazine. The program run is not interrupted.

TOOL NUMBER?

e.g.

END

Enter the number of the tool as it was defined in the tool table or in a "G99" block, for example 5.

Select the spindle axis Z.

Enter the desired spindle speed, for example S = 500 rpm.

Manual tool change

To change the tool manually, stop the spindle and move the tool to the tool change position. Sequence of action:

• Move to the tool change position (under program control, if desired)

• Interrupt program run (see page 3-4)

• Change the tool

• Continue the program run (see page 3-5)

4-9TNC 360

Page 74

4 Programming

4.2 Tools

Tool change position

A tool change position must lie next to or above the workpiece to prevent tool collision. With the miscellaneous functions M91 and M92 (see page 5-

39) you can enter machine-referenced rather than workpiecereferenced coordinates for the tool change position.

If T0 is programmed before the first tool call, the TNC moves the spindle to an uncompensated position.

If a positive length compensation value was in effect before T0, the clearance to the workpiece is reduced.

TNC 3604-10

Page 75

4 Programming

4.3 Tool Compensation Values

For each tool, 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.

Effect of tool compensation values

Tool length

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

Fig. 4.4: The TNC must compensate the length and radius of the tool

To cancel length compensation, call a tool with the length L = 0.

Tool radius

Radius compensation becomes effective as soon as a tool is called and is moved in the working plane with G41 or G42.

To cancel radius compensation, program a positioning block with G40.

Tool radius compensation

Tool traverse can be programmed:

• Without radius compensation: G40

• With radius compensation: G41or G42

• As single-axis movements with G43 or G44

Fig. 4.5: Programmed contour (–––, +) and the path of the tool

center (- - -)

4-11TNC 360

Page 76

4 Programming

4.3 Tool Compensation Values

Traverse without radius compensation: G40

The tool center moves to the programmed coordinates.

Applications:

• Drilling and boring

• Pre-positioning

Fig. 4.6: These drilling positions are entered without radius compen-

Traverse with radius compensation G41, G42

The tool center moves to the left (G41) or to the right (G42) of the programmed contour at a distance equal to the tool radius. "Right" or "left" is meant as seen in the direction of tool movement as if the workpiece were stationary.

G41

sation

G42

Fig. 4.7: The tool moves to the left (G41) or to the right (G42) of the workpiece during milling

Between two program blocks with differing radius compensation you must program at least one block without radius compensation (that is, with G40). Radius compensation is not in effect until the end of the block in which it is first programmed.

Shortening or lengthening single-axis movements G43, G44

This type of radius compensation is possible only for single-axis movements in the working plane: The programmed tool path is shortened (G44) or lengthened (G43) by the tool radius.

Applications:

• Single-axis machining

• Occasionally for pre-positioning the tool, such as for cycle G47: SLOT MILLING.

• G43 and G44 are activated by programming a positioning block with only one axis.

• The machine tool builder may block the entry of single-axis positioning blocks through a machine parameter.

TNC 3604-12

Page 77

4 Programming

4.3 Tool Compensation Values

Machining corners

Outside corners

The TNC moves the tool in a transitional arc around outside corners. The tool "rolls around" the corner point.

If necessary, the feed rate F is automatically reduced at outside corners to reduce machine strain, for example for very sharp changes in direction.

If you work without radius compensation, you can influence the machining of outside corners with the miscellaneous function M90 (see page 5-36).

G41

Fig. 4.8: The tool "rolls around" outside corners

Inside corners

The TNC calculates the intersection of the tool center paths at inside corners. From this point it then starts the next contour element. This prevents damage to the workpiece at inside corners.

When two or more inside corners adjoin, the chosen tool radius must be small enough to fit in the programmed contour.

G41

S S

Fig. 4.9: Tool path for inside corners

G41

4-13TNC 360

Page 78

4 Programming

4.4 Program Creation

To create a new part program

PGM

Select any program.

PROGRAM NUMBER=

e.g.

MM=G71 / INCH=G70

e.g.

Defining the blank form

If you wish to use the graphic workpiece simulation you must first define a rectangular workpiece blank. Its sides lie parallel to the X, Y and Z axes and can be up to 30 000 mm long.

ENT

Call the file directory.

Enter the name of the new program, for example 743.

Select the unit of measurement used in the program, for example millimeters (G71), conclude the block.

MAX

The ratio of the blank-form side lengths must be less than 84:1.

MIN and MAX points

The blank form is defined by two of its corner points:

• The MIN point — the smallest X, Y and Z coordinates of the blank form, entered as absolute values.

• The MAX point — the largest X, Y and Z coordinates of the blank form, entered as absolute values or incremental values.

MIN

Fig. 4.10: The MIN and MAX points define

the blank form

TNC 3604-14

Page 79

4 Programming

4.4 Program Creation

e.g.

1 1

END

0 0

END

G function for entering the MIN point.

Select the tool axis: G17 designates the Z axis.

Enter the MIN point coordinates for the X, Y and Z axes; confirm the block with END.

G function for entering the MAX point.

Enter an absolute value, or

Enter an incremental value.

Enter the MAX point coordinates for the X, Y and Z axes; confirm the block with END.

4-15TNC 360

Page 80

4 Programming

4.4 Program Creation

The entered program section appears on the TNC screen:

% 743 G71

Block 1: Program beginning, name, unit of measure.

N10 G30 G17 X+0 Y+0 Z-40

Block 2: Spindle axis, MIN point coordinates.

N20 G31 G90 X+100 Y+100 Z+0

Block 3: MAX point coordinates.

N9999 % 743 G71

Block 4: Program end, name, unit of measure.

The unit of measure used in the program appears behind the program name (G71 = mm).

❊❊

❊

❊❊

❊

❊❊

❊

❊❊

❊

❊❊

TNC 3604-16

Page 81

4 Programming

4.5 Entering Tool-Related Data

Besides the tool data and compensation, you must also enter the following information:

• Feed rate F

• Spindle speed S

• Miscellaneous functions M

The tool-related data can be determined with the aid of diagrams (see page 11-15).

Feed rate F

The feed rate is the speed in mm/min (or inch/min) with which the tool center moves.

Input range: F = 0 to 30 000 mm/min (1181 inch/min)

The maximum feed rate is set in machine parameters individually for each axis.

S S

Fig. 4.11: Feed rate F and spindle speed S of the tool

To set the feed rate:

e.g.

Rapid traverse

You can program rapid traverse directly with the G00 function.

Duration of feed rate F

A feed rate that is entered as a numerical value remains in effect until the control executes a block in which another feed rate has been programmed.

If the new feed rate is G00 (rapid traverse), the feed rate will return to the last numerically entered feed rate as soon as the next block with G01 is executed.

Changing the feed rate F

You can vary the feed rate by turning the knob for feed rate override on the operating panel (see page 2-6).

1 0 0

Enter the feed rate F, for example F = 100 mm/min.

4-17TNC 360

Page 82

4 Programming

4.5 Entering Tool-Related Data

Spindle speed S

The spindle speed S is entered in revolutions per minute (rpm). Input range:

S = 0 to 99 999 rpm

To change the spindle speed S in the part program:

Resulting NC block: T1 G17 S1000

To change the spindle speed S during program run:

e.g.

100

END

15050

S %

Enter the spindle speed S, for example 1000 rpm.

You can vary the spindle speed S on machines with stepless ballscrew drives by turning the override knob on the operating panel.

TNC 3604-18

Page 83

4 Programming

4.6 Entering Miscellaneous Functions and STOP

The M functions (M for miscellaneous) affect:

• Program run

• Machine functions

• Tool behavior On the inside back cover of this manual you will find a list of M functions

that are predetermined for the TNC. The list indicates whether an M function begins at the start or at the end of the block in which it is programmed.

You can program several M functions in one NC block as long as they are independent of each other. The M function list on the inside back cover of this manual shows the different groups of M functions.

Some M functions are not effective on certain machines. The machine tool builder may also add some of his own M functions.

A program run or test run is interrupted when it reaches an NC block containing the function G38.

If you wish to interrupt the program run or test run for a certain duration, use the cycle G04: DWELL TIME (see page 8-38).

4-19TNC 360

Page 84

4 Programming

4.7 Actual Position Capture

Sometimes you may want to enter the actual position of the tool in a specific axis as a coordinate in a part program. Instead of reading the actual position values and entering them with the numeric keypad, you can simply press the "actual position capture" key. This feature can be used, for example, to enter the tool length.

To capture the actual position:

Fig. 4.12: Storing the actual position in the TNC

MANUAL OPERATION

Move the tool to the position that you wish to capture.

PROGRAMMING AND EDITING

Select or create the program block in which you wish to enter the actual position of the tool.

e.g.

Enter the radius compensation according to the position of the tool relative to the workpiece.

Select the axis in which you wish to capture a coordinate, for example the X axis.

Transfer the actual position coordinate to the program.

TNC 3604-20

Page 85

5 Programming Tool Movements

5.1 General Information on Programming Tool Movements

A tool movement is always programmed as if the tool is moving and the workpiece is stationary.

Always pre-position the tool at the beginning of a part program to prevent the possibility of damaging the tool or workpiece. In addition, radius compensation and a path function must be active.

Example of an NC block: N30 G00 G40 G90 Z+100 *

Path functions

Each element of the workpiece contour is entered separately using path functions. The various path functions produce:

• Straight lines

• Circular arcs You can also program a combination of the two

(helical paths).

The contour elements are executed in sequence to machine the programmed contour.

Fig. 5.1: A contour consists of a combination of straight lines and

circular arcs

G01

G 01

I, J

G01

G02

Fig. 5.2: Contour elements are programmed and executed in sequence

5-2 TNC 360

Page 86

5 Programming Tool Movements

5.1 General Information on Programming Tool Movements

Subprograms and program section repeats

If a machining sequence repeats itself in a program, you can enter the sequence once and define it as a subprogram or program section repeat.

Programming possibilities:

• To repeat a machining routine immediately after it is executed (program section repeat)

• To insert a machining routine at certain locations in a program (subprogram)

• To call a separate program for execution or test run within the main program (main program as subprogram)

Cycles

Common machining routines are delivered with the control as standard cycles. The TNC features fixed cycles for:

• Pecking

• Tapping

• Slot milling

• Pocket and island milling

Coordinate transformation cycles can be used to change the coordinates of a machining sequence in a defined way, i.e.:

• Datum shift

• Mirroring

• Rotation

• Enlarging / Reducing

Parameter programming

Instead of numerical values you enter markers in the program, so-called parameters, which are defined through mathematical functions or logical comparisons. You can use parametric programming for:

• Conditional and unconditional jumps

• Measurements with the 3D touch probe during program run

• Output of values and messages

• Transferring values to and from memory

The following mathematical functions are available:

• Assign

• Addition/Subtraction

• Multiplication/Division

• Angle measurement/Trigonometry

etc.

TNC 360

5-3

Page 87

5 Programming Tool Movements

G40

5.2 Contour Approach and Departure

An especially convenient way to approach and depart a workpiece is on a tangential arc. This is done with the "smooth approach" function (G26) (see page 5-6).

Starting and end positions

Starting position

The tool moves from the starting position to the first contour point. The starting position is programmed without radius compensation.

The starting position must be:

• approachable without collision

• near the first contour point

• located to prevent contour damage during workpiece approach If you choose a starting position within the hatch marked area of Fig. 5.3

the tool will damage the contour as it approaches the first contour point.

The best starting position S lies on the extension of the tool path for machining the first contour element.

First contour point

Workpiece machining starts at the first contour point. The tool moves on a radius-compensated path to this point.

Approaching the starting point in the spindle axis

The spindle moves to its working depth as it approaches the starting position S.

If there is any danger of collision, move the spindle axis separately to the starting position.

Example: G00 G40 X ... Y ... Positioning in X/Y

Z–10 Positioning in Z

Fig. 5.3 : Starting position S for contour

approach

G41

Fig. 5.4 : First contour point A for machin-

ing

Fig. 5.5 : Move the spindle axis separately if

there is any danger of collision

5-4 TNC 360

Page 88

5 Programming Tool Movements

5.2 Contour Approach and Departure

End position

The end position, like the starting position, must be

• approachable without collision

• near the last contour point

• located to prevent contour damage during workpiece departure

The best end position E lies on the extension of the tool path. The end position can be located anywhere outside of the hatch marked area in Fig. 5.6. It is approached without radius compensation.

Departing the end position in the spindle axis

The spindle axis is moved separately when the end position is departed. Example: G00 G40 X ... Y ... approaching the end position

Z+50 retracting the tool

G40

Fig. 5.6 : End position E after machining

Common starting and end position

A common starting and end position

can be located outside of the

hatch marked area in the figures.

The best common starting and end position lies exactly between the extensions of the tool paths for machining the first and last contour elements.

A common starting and end position is approached without radius compensation.

Fig. 5.7 : Retract separately in the spindle

axis

G40

Fig. 5.8: Common starting and end position

TNC 360

5-5

Page 89

5 Programming Tool Movements

5.2 Contour Approach and Departure

Smooth approach and departure

The tool approaches and departs the workpiece at a tangent if you select the function G26 for approach and the function G27 for departure. This prevents dwell marks on the workpiece surface.

Starting and end positions

The starting workpiece and near the first and last contour elements, respectively.

The tool paths to the starting and end positions are programmed without radius compensation.

Input

• During contour approach, the function G26 is entered after the block in which the first contour point is programmed, i.e. after the first block with radius compensation G41/G42.

• During contour departure, the function G27 is entered after the block in which the last contour point is programmed, i.e. after the last block with radius compensation G41/G42.

and end E positions of machining lie outside of the

G41

G40

Fig. 5.9: Smooth approach onto a contour

G41

Program example

. . .

G00 G40 G90 X ... Y ... ............................................... Starting position

G01 G41 X ... Y ... F350 ..............................................First contour point

G26 R ... ..................................................................... Smooth approach

. . .

Contour elements

. . .

X ... Y ... ...................................................................... Last contour point

G27 R ... ..................................................................... Smooth departure

G00 G40 X ... Y ... .......................................................End position

G40

Fig. 5.10: Smooth departure from a contour

For proper execution of the functions G26/G27, a radius must be chosen such that the arc can connect the starting or end position with the contour point.

5-6 TNC 360

Page 90

5 Programming Tool Movements

5.3 Path Functions

General information

Part program input

To create a part program you enter the dimensional information given on the workpiece drawing. The workpiece coordinates are programmed as absolute values (G90) or as relative values (G91).

You usually program a contour element by entering its end point. The TNC automatically calculates the tool path from the tool data and the radius compensation.

The first machining block after the tool call must contain the following G functions:

Path function e.g. G00 Radius compensation e.g. G40 Absolute or incremental programming e.g. G90

Machine axis movement under program control

All machine axes programmed in a single NC block are moved simultaneously.

Paraxial movement

Paraxial movement means that the tool path is parallel to the programmed axis.

Number of axes programmed in the NC block: 1

Movement in the main planes

With this type of movement the tool moves to the programmed position on a straight line or a circular arc in a "working plane".

Number of axes programmed in the NC block: 2

G00 X +100

100

Fig. 5.11: Paraxial movement

G00 X +70 Y +50

TNC 360

Fig. 5.12: Movement in a main plane

(X/Y plane)

5-7

Page 91

5 Programming Tool Movements

5.3 Path Functions

Movement of three machine axes (3D movement)

The tool moves in a straight line to the programmed position. Number of axes programmed in the NC block: 3

Exception: A helical path is created by combining a circular movement in

a plane with a linear movement perpendicular to the plane.

L X +80 Y 0 Z –10

Fig. 5.13: Three-dimensional tool movement

5-8 TNC 360

Page 92

5 Programming Tool Movements

5.3 Path Functions

Overview of path functions

Function in Cartesian in polar

Straight line at rapid traverse. G00 G10

Straight line with a programmed feed rate. G01 G11

Chamfer with chamfer length R. G24 A chamfer is inserted between two intersecting straight lines.

Circle center – at the same time a reference for polar coordinates. I, J, K I,J,K do not generate a movement.

Circular movement in the clockwise direction (CW). G02 G12

Circular movement in the counterclockwise direction (CCW). G03 G13

Input

coordinates coordinates

A circular path can be programmed by entering:

• Circle center I, J, K and end point, or

• Circle radius and end point.

Circular path with no direction of rotation defined. G05 G15 The circular path is programmed by entering circle center and end point. The direction of rotation is taken from the last programmed circular movement (G02/G12 or G03/G13).

Circular movement with tangential connection. G06 G16 A circular arc is connected tangentially with the previously programmed contour element. The end point of the circular arc is entered in the part program.

Corner rounding with radius R. G25 A circular arc is inserted to connect tangentially both with the preceding and the subsequent contour elements.

TNC 360

5-9

Page 93

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

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

To program a straight line, you enter:

• The coordinates of the end point

• If necessary: Radius compensation, feed rate, miscellaneous function

The tool moves in a straight line from its starting position to the end point

To program a straight line:

. The starting position S was reached in the previous block.

If necessary

e.g.

Straight line at rapid traverse.

Identify coordinates as relative values, for example G91 X–50 mm.

Press the orange axis selection key, for example X.

Fig. 5.14: A linear movement

e.g.

If necessary

e.g.

. .

Enter the coordinate of the end point.

If the coordinate is negative, press the +/- key once, for example X = –50 mm.

Enter all further coordinates of the end point.

. . .

5-10 TNC 360

Page 94

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

. . .

e.g.

Resulting NC block: N25 G00 G42 G91 X+50 G90 Y+10 Z–20 M3 *

ENT

END

The tool must move to the left of the programmed contour to compensate its own radius.

The tool must move to the right of the programmed contour to compensate its own radius.

The tool moves directly to the end point.

Enter a miscellaneous function, for example M3 (spindle on, clockwise rotation).

Conclude the block with END as soon as all coordinates are entered.

TNC 360

5-11

Page 95

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Example for exercise: Milling a rectangle

Coordinates of the corner points:

X = 5 mm Y = 5 mm

X = 5 mm Y = 95 mm

X = 95 mm Y = 95 mm

X = 95 mm Y = 5 mm

Milling depth: Z = –10mm

100

–10

Part program

%S512I G71 * ............................................................ Begin program; program name S512I;

................................................................................... dimensions in millimeters

N10 G30 G17 X+0 Y+0 Z–20 *

N20 G31 G90 X+100 Y+100 Z+0 * ............................ Define blank form for graphic workpiece simulation

(MIN and MAX point)

N30 G99 T1 L+0 R+5 * .............................................. Define tool in the program

N40 T1 G17 S2500 * .................................................. Call tool in the spindle axis Z (G17);

spindle speed S = 2500 rpm

N50 G00 G40 G90 Z+100 M06 * ............................... Retract in the spindle axis; rapid traverse; miscellaneous

function for tool change

N60 X–10 Y–10 * ....................................................... Pre-position near the first contour point

N70 Z–10 M03 * ........................................................ Pre-position in Z; spindle on

N80 G01 G41 X+5 Y+5 F150 * .................................. Move to point 1 with radius compensation

N90 Y+95 * ................................................................ Move to corner point

N100 X+95 * .............................................................. Move to corner point

N110 Y+5 * ................................................................ Move to corner point

N120 X+5 * ................................................................ Move to corner point 1, conclude milling

N130 G00 G40 X–10 Y–10 M05 * .............................. Retract in X and Y, cancel radius compensation,

spindle STOP

N140 Z+100 M02 *.................................................... Move tool to setup clearance, spindle OFF, coolant OFF,

................................................................................... program stop, return jump to block 1

N9999 %S512I G71 * ................................................ End of program

2 3 4

100

5-12 TNC 360

Page 96

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Chamfer G24

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

You enter the length L to be removed from each side of the corner.

Prerequisites:

• 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.

Fig. 5.15: Chamfer from S to

Fig. 5.16: Tool radius too large

• You cannot start a contour with a G24 block.

• A chamfer is only possible in the working plane.

• The feed rate for chamfering is taken from the previous block.

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

To program a chamfer:

ENT

Select the chamfer function.

CHAMFER SIDE LENGTH?

e.g.

END

Resulting NC block: G24 R5

Enter the length to be removed from each side of the corner, for example 5 mm.

TNC 360

5-13

Page 97

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Example for exercise: Chamfering a corner

Coordinates of the corner point

Chamfer length: LF = 10 mm

Milling depth: Z = –15 mm

Tool radius: R = +10 mm

: X=95mm

Y=5mm

100

–15

95 100

Part program

%S514I G71 * ............................................................ Begin program

N10 G30 G17 X+0 Y+0 Z–20 * .................................. Workpiece blank MIN point

N20 G31 G90 X+100 Y+100 Z+0 * ............................ Workpiece blank MAX point

N30 G99 T5 L+5 R+10 * ............................................ Tool definition

N40 T5 G17 S2000 * .................................................. Tool call

N50 G00 G40 G90 Z+100 M06 * ............................... Retract spindle and insert tool

N60 X–10 Y–5 * ......................................................... Pre-position in X, Y

N70 Z–15 M03 * ........................................................ Pre-position to the working depth, spindle on

N80 G01 G42 X+5 Y+5 F200 * .................................. Move with radius compensation and reduced feed to

................................................................................... the first contour point

N90 X+95 * ................................................................ Program the first straight line for corner E

N100 G24 R10 * ........................................................ Chamfer block: inserts a chamfer with L = 10 mm

N110 Y+100 * ............................................................ Program the second straight line for corner E

N120 G00 G40 X+110 Y+110 * ................................. Retract the tool in X, Y and Z, cancel radius

................................................................................... compensation

N130 Z+100 M02 *.................................................... Move tool to setup clearance

N9999 %S514I G71 *

5-14 TNC 360

Page 98

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Circles and circular arcs - General information

The TNC can control two machine axes simultaneously to move the tool in a circular path.

Circle center I, J, K

You can define a circular movement by entering its center.

A circle center can also serve as reference (pole) for polar coordinates.

Fig. 5.17: Circular arc and circle center

Direction of rotation

When there is no tangential transition to another contour element, enter the mathematical direction of rotation, where

• a clockwise direction of rotation is mathematically negative: function G02

• a counterclockwise direction of rotation is mathematically positive: function G03

Fig. 5.18: Circle center coordinates

G03

Fig. 5.19: Direction of rotation for circular movements

G02

TNC 360

5-15

Page 99

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Radius compensation in circular paths

You cannot begin radius compensation in a circle block. It must be activated beforehand in a line block.

Circles in the main planes

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

Spindle axis

Main plane

Circle center

You can program circles that do not lie parallel to a main plane by using Q parameters (see Chapter 7).

Circle center I, J, K

If you program an arc using the functions G02/G03/G05, you must first define the circle center by:

• entering the Cartesian coordinates of the circle center

• using the circle center defined in an earlier block

• capturing the actual position

You can define the last programmed position as circle center/pole by programming G29.

Fig. 5.20: Defining the spindle axis also defines the main plane and the

circle center designations

XY G17

ZX G18

YZ G19

I J

K I

J K

5-16

Duration of a circle center definition

A circle center definition remains effective until a new circle center is defined.

Fig. 5.21: Circle center I, J

TNC 360

Page 100

5 Programming Tool Movements

5.4 Path Contours - Cartesian Coordinates

Entering I, J, K in relative values

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

G91 J

G91 I

Fig. 5.22: Incremental circle center coordinates

• The circle center I, J, K also serves as pole for polar coordinates.

• I, J, K defines a position as a circle center. The resulting contour is located on the circle, not on the circle center.

To program a circle center (pole):

Select the coordinate axis for the circle center.

Enter the coordinate for the circle center on this axis, for example I = 20 mm.

Select the second coordinate axis, for example J.

Enter the coordinate of the circle center, for example J = –10 mm.

e.g.

END

TNC 360

Resulting NC block: I+20 J–10 *

5-17

HEIDENHAIN TNC 360 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual