HEIDENHAIN iTNC 530 User Manual

Download

Page 1

User’s Manual HEIDENHAIN Conversational

iTNC 530

NC Software 340 490-05 340 491-05 340 492-05 340 493-05 340 494-05

English (en) 12/2008

Page 2

Controls of the TNC

Keys on visual display unit

Key Function

Split screen layout

Toggle display between machining and programming modes

Soft keys for selecting functions on screen

Shift between soft-key rows

Alphanumeric keyboard

Key Function

File names, comments

DIN/ISO programming

Machine operating modes

Key Function

Manual Operation

Electronic Handwheel

Program/file management, TNC functions

Key Function

Select or delete programs and files, external data transfer

Define program call, select datum and point tables

Select MOD functions

Display help text for NC error messages, call TNCguide

Display all current error messages

Show pocket calculator

Navigation keys

Key Function

Move highlight

Go directly to blocks, cycles and parameter functions

Potentiometer for feed rate and spindle speed

Feed rate Spindle speed

smarT.NC

Positioning with Manual Data Input

Program Run, Single Block

Program Run, Full Sequence

Programming modes

Key Function

Programming and Editing

Test Run

100

S %

100

F %

Cycles, subprograms and program section repeats

Key Function

Define touch probe cycles

Define and call cycles

Enter and call labels for subprogramming and program section repeats

Program stop in a program

Page 3

Tool functions

Key Function

Define tool data in the program

Coordinate axes and numbers: Entering and editing

Key Function

. . .

Select coordinate axes or enter them into the program

Call tool data

Programming path movements

Key Function

Approach/depart contour

FK free contour programming

Straight line

Circle center/pole for polar coordinates

Circle with center

Circle with radius

Circular arc with tangential connection

Chamfering/Corner rounding

. . .

Numbers

Decimal point / Reverse algebraic sign

Polar coordinate input / Incremental values

Q parameter programming / Q parameter status

Save actual position or values from calculator

Skip dialog questions, delete words

Confirm entry and resume dialog

Conclude block and exit entry

Clear numerical entry or TNC error message

Abort dialog, delete program section

Special functions / smarT.NC

Key Function

Show special functions

smarT.NC: Select next tab on form

smarT.NC: Select first input field in previous/next frame

Page 4

Page 5

About this Manual

The symbols used in this manual are described below.

This symbol indicates that important notes about the function described must be adhered to.

This symbol indicates that using the function described runs one or more than one of the following risks:

 Danger to workpiece  Danger to fixtures  Danger to tool  Danger to machine  Danger to operator

This symbol indicates that the described function must be adapted by the machine tool builder. The function described may therefore vary depending on the machine.

This symbol indicates that you can find detailed information about a function in another manual.

About this Manual

Do you desire any changes, or have you found any errors?

We are continuously striving to improve documentation for you. Please help us by sending your requests to the following e-mail address: tnc-userdoc@heidenhain.de.

HEIDENHAIN iTNC 530 5

Page 6

TNC Model, Software and Features

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

TNC model NC software number

iTNC 530 340 490-05

iTNC 530 E 340 491-05

iTNC 530 340 492-05

iTNC 530 E 340 493-05

iTNC 530 programming station 340 494-05

The suffix E indicates the export version of the TNC. The export version of the TNC has the following limitations:

 Simultaneous linear movement in up to 4 axes

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

TNC Model, Software and Features

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

 Tool measurement with the TT

Please contact your machine tool builder to become familiar with the features of your machine.

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

User’s Manual for Cycles:

All of the cycle functions (touch probe cycles and fixed cycles) are described in a separate manual. Please contact HEIDENHAIN if you require a copy of this User’s Manual. ID: 670 388-xx

smarT.NC user documentation:

The smarT.NC operating mode is described in a separate Pilot. Please contact HEIDENHAIN if you require a copy of this Pilot. ID: 533 191-xx

Page 7

Software options

The iTNC 530 features various software options that can be enabled by you or your machine tool builder. Each option is to be enabled separately and contains the following respective functions:

Software option 1

Cylinder surface interpolation (Cycles 27, 28, 29 and 39)

Feed rate in mm/min for rotary axes: M116

Tilting the machining plane (Cycle 19, PLANE function and 3-D ROT soft key in the Manual Operation mode)

Circle in 3 axes with tilted working plane

Software option 2

Block processing time 0.5 ms instead of 3.6 ms

5-axis interpolation

Spline interpolation

3-D machining:

 M114: Automatic compensation of machine geometry when

working with swivel axes

 M128: Maintaining the position of the tool tip when positioning

with swivel axes (TCPM)

 FUNCTION TCPM: Maintaining the position of the tool tip when

positioning with swivel axes (TCPM) in selectable modes

 M144: Compensating the machine’s kinematics configuration for

ACTUAL/NOMINAL positions at end of block

 Additional parameters for finishing/roughing and tolerance for

rotary axes in Cycle 32 (G62)

 LN blocks (3-D compensation)

TNC Model, Software and Features

DCM Collision software option Description

Function that monitors areas defined by the machine manufacturer to prevent collisions.

DXF Converter software option Description

Extract contours and machining positions from DXF files (R12 format).

HEIDENHAIN iTNC 530 7

Page 365

Page 240

Page 8

Additional dialog language software option

Function for enabling the conversational languages Slovenian, Slovak, Norwegian, Latvian, Estonian, Korean, Turkish, Romanian, Lithuanian

Global Program Settings software option Description

Function for superimposing coordinate transformations in the Program Run modes, handwheel superimposed traverse in virtual axis direction.

AFC software option Description

Function for adaptive feed-rate control for optimizing the machining conditions during series production.

KinematicsOpt software option Description

Touch-probe cycles for inspecting and optimizing the machine accuracy.

TNC Model, Software and Features

Description

Page 620

Page 380

Page 391

User’s Manual for Cycles

Page 9

Feature content level (upgrade functions)

Along with software options, significant further improvements of the TNC software are managed via the Feature Content Level (FCL) upgrade functions. Functions subject to the FCL are not available simply by updating the software on your TNC.

All upgrade functions are available to you without surcharge when you receive a new machine.

Upgrade functions are identified in the manual with FCL n, where n indicates the sequential number of the feature content level.

You can purchase a code number in order to permanently enable the FCL functions. For more information, contact your machine tool builder or HEIDENHAIN.

FCL 4 functions Description

Graphical depiction of the protected space when DCM collision monitoring is active

Page 370

Handwheel superimposition in stopped condition when DCM collision monitoring is active

3-D basic rotation (set-up compensation) Machine Manual

FCL 3 functions Description

Touch probe cycle for 3-D probing User’s Manual for Cycles

Touch probe cycles for automatic datum setting using the center of a slot/ridge

Feed-rate reduction for the machining of contour pockets with the tool being in full contact with the workpiece

PLANE function: Entry of axis angle Page 442

User documentation as a contextsensitive help system

smarT.NC: Programming of smarT.NC and machining can be carried out simultaneously

smarT.NC: Contour pocket on point pattern

smarT.NC: Preview of contour programs in the file manager

Page 369

User’s Manual for Cycles

Page 150

Page 118

smarT.NC Pilot

TNC Model, Software and Features

smarT.NC: Positioning strategy for machining point patterns

HEIDENHAIN iTNC 530 9

smarT.NC Pilot

Page 10

FCL 2 functions Description

3-D line graphics Page 142

Virtual tool axis Page 541

USB support of block devices (memory sticks, hard disks, CD-ROM drives)

Filtering of externally created contours Page 405

Possibility of assigning different depths to each subcontour in the contour formula

DHCP dynamic IP-address management Page 598

Touch-probe cycle for global setting of touch-probe parameters

smarT.NC: Graphic support of block scan smarT.NC Pilot

smarT.NC: Coordinate transformation smarT.NC Pilot

smarT.NC: PLANE function smarT.NC Pilot

Intended place of operation

TNC Model, Software and Features

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

Page 128

User’s Manual for Cycles

User’s Manual for Touch Probe Cycles

Legal information

This product uses open source software. Further information is available on the control under

U Programming and Editing operating mode U MOD function U LEGAL INFORMATION soft key

Page 11

New functions in 340 49x-01 since the predecessor versions 340 422-xx/340 423-xx

 A new form-based operating mode, smarT.NC, has been

introduced. These cycles are described in a separate user's document. In connection with this the TNC operating panel was enhanced. There are some new keys available for quicker navigation within smarT.NC

 The single-processor version supports pointing devices (mice) via

the USB interface.

 The tooth feed f

alternate feed entries (see “Possible feed rate input” on page 103).

 New cycle CENTERING (see User’s Manual for Cycles)  New M function M150 for suppressing limit switch messages (see

“Suppress limit switch message: M150” on page 358)

 M128 is now also permitted for mid-program startup (see “Mid-

program startup (block scan)” on page 572)

 The number of available Q parameters was expanded to 2000 (see

“Principle and Overview” on page 274).

 The number of available label numbers was expanded to 1000. Now

label names can be assigned as well (see “Labeling Subprograms and Program Section Repeats” on page 258).

 In the Q parameter functions FN9 to FN12 you can now also assign

label names as jump targets (see “If-Then Decisions with Q Parameters” on page 284).

 Selectively machine points from a point table (see User's Manual for

Cycles)

 The current time is also shown in the additional status display

window (see “General program information (PGM tab)” on page

83).

 Several columns were added to the tool table (see “Tool table:

Standard tool data” on page 162).

 The Test Run can now also be stopped and resumed within

machining cycles (see “Running a program test” on page 563).

and feed per revolution fu can now be defined as

340 422-xx/340 423-xx

HEIDENHAIN iTNC 530 11

New functions in 340 49x-01 since the predecessor versions

Page 12

New functions with 340 49x-02

 DXF files can be opened directly on the TNC, in order to extract

contours into a plain-language program (see “Processing DXF Files (Software Option)” on page 240)

 3-D line graphics are now available in the Programming and Editing

operating mode (see “3-D Line Graphics (FCL2 Function)” on page

142)

 The active tool-axis direction can now be set as the active machining

direction for manual operation (see “Setting the current tool-axis direction as the active machining direction (FCL 2 function)” on page

541)

 The machine manufacturer can now define any areas on the

machine for collision monitoring (see “Dynamic Collision Monitoring (Software Option)” on page 365)

 Instead of the spindle speed S you can now define the cutting speed

Vc in m/min (see “Calling tool data” on page 173)

 The TNC can now display freely definable tables in the familiar table

view or as forms (see “Switching between table and form view” on page 422)

 The function for converting FK programs to H was expanded.

New functions with 340 49x-02

Programs can now also be output in linearized format (see “Converting FK programs into HEIDENHAIN conversational format” on page 224)

 You can filter contours that were created using external

programming systems (see “Filtering Contours (FCL 2 Function)” on page 405)

 For contours which you connect via the contour formula, you can

now assign separate machining depths for each subcontour (see User's Manual for Cycles)

 The single-processor version now supports not only pointing

devices (mice), but also USB block devices (memory sticks, disk drives, hard disks, CD-ROM drives) (see “USB devices on the TNC (FCL 2 function)” on page 134)

Page 13

New functions with 340 49x-03

 The Adaptive Feed Control function (AFC) was introduced (see

“Adaptive Feed Control Software Option (AFC)” on page 391)

 The global parameter settings function makes it possible to set

various transformations and settings in the program run modes (see “Global Program Settings (Software Option)” on page 380).

 The TNC now features a context-sensitive help system, the

TNCguide (see “The Context-Sensitive Help System TNCguide (FCL3 Function)” on page 150).

 Now you can extract point files from DXF files(see “Selecting and

storing machining positions” on page 250).

 Now, in the DXF converter, you can divide or lengthen laterally

joined contour elements (see “Dividing, extending and shortening contour elements” on page 249).

 In the PLANE function the working plane can now also be defined

directly by its axis angle (see “Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)” on page 442).

 In Cycle 22 ROUGH-OUT, you can define a feed-rate reduction if the

tool is cutting on its entire circumference (FCL3 function, see User's Manual for Cycles)

 In Cycle 208 BORE MILLING, you can now choose between climb or

up-cut milling (see User's Manual for Cycles)

 String processing has been introduced in Q parameter programming

(see “String Parameters” on page 312)

 A screen saver can be activated through machine parameter 7392

(see “General User Parameters” on page 620)

 The TNC now also supports a network connection over the NFS V3

protocol (see “Ethernet Interface” on page 591)

 The maximum manageable number of tools in a pocket table was

increased to 9999 (see “Pocket table for tool changer” on page 170)

 Parallel programming is possible with smarT.NC (see “Select

smarT.NC programs” on page 118)

 The system time can now be set through the MOD function (see

“Setting the System Time” on page 615)

New functions with 340 49x-03

HEIDENHAIN iTNC 530 13

Page 14

New functions with 340 49x-04

 The global parameter settings function makes it possible to activate

handwheel superimposed traverse in the active tool axis direction (virtual axis) (see “Virtual axis VT” on page 390)

 Machining patterns can now easily be defined with PATTERN DEF

(see User's Manual for Cycles)

 Program defaults valid globally can now be defined for machining

cycles (see User's Manual for Cycles)

 Now, in Cycle 209 TAPPING WITH CHIP BREAKING, you can define a

factor for the retraction shaft speed, so that you can depart the hole faster (see User's Manual for Cycles)

 In Cycle 22 ROUGH-OUT, you can now define the fine-roughing

strategy (see User's Manual for Cycles)

 In the new Cycle 270 CONTOUR TRAIN DATA, you can define the type

of approach of Cycle 25 CONTOUR TRAIN (see User's Manual for Cycles)

 New Q-parameter function for reading a system datum was

introduced (see “Copying system data to a string parameter,” page

317)

New functions with 340 49x-04

 New functions for copying, moving and deleting files from within

the NC program were introduced (see “File Functions,” page 406)

 DCM: Collision objects can now be shown three-dimensionally

during machining (see “Graphic depiction of the protected space (FCL4 function),” page 370)

 DXF converter: New settings possibility introduced, with which the

TNC automatically selects the circle center when loading points from circular elements (see “Basic settings,” page 242)

 DXF converter: Element information is shown in an additional info

window (see “Selecting and saving a contour,” page 247)

 AFC: A line diagram is now shown in the additional AFC status

display (see “Adaptive Feed Control (AFC tab, software option)” on page 89)

 AFC: Control settings parameters selectable by machine tool builder

(see “Adaptive Feed Control Software Option (AFC)” on page 391)

 AFC: The spindle reference load currently being taught is shown in

a pop-up window in the teach-in mode. In addition, the learning phase can be restarted at any time via soft key (see “Recording a teach-in cut” on page 395).

 AFC: The dependent file <name>.H.AFC.DEP can now also be

modified in the Programming and Editing operating mode (see “Recording a teach-in cut” on page 395)

Page 15

 The maximum path permitted for LIFTOFF was increased to 30 mm

(see “Automatically retract tool from the contour at an NC stop: M148” on page 357)

 File management was adapted to the file management of smarT.NC

(see “Overview: Functions of the file manager” on page 114)

 New function for generating service files was introduced (see

“Generating service files” on page 149)

 A window manager was introduced (see “Window Manager” on

page 90)

 The new dialog languages Turkish and Romanian were introduced

(software option, Page 620)

New functions with 340 49x-04

HEIDENHAIN iTNC 530 15

Page 16

New functions with 340 49x-05

 DCM: Integrated fixture management (see “Fixture Monitoring

(Software Option)” on page 372)

 DCM: No collision checking in the Test Run mode(see “Collision

monitoring in the Test Run mode of operation” on page 371)

 DCM: Management of tool-carrier kinematics has been simplified

(see “Tool-carrier kinematics” on page 168)

 Processing DXF data: Fast point selection via mouse area (see

“Quick selection of hole positions in an area defined by the mouse” on page 252)

 Processing DXF data: Fast point selection via diameter input (see

“Quick selection of hole positions in an area defined by the mouse” on page 252)

 DXF data processing: Polyline support was integrated (see

“Processing DXF Files (Software Option)” on page 240)

 AFC: Smallest occurring feed rate will now also be saved in the log

file (see “Log file” on page 399)

 AFC: Monitoring for tool breakage/tool wear (see “Tool

breakage/tool wear monitoring” on page 401)

New functions with 340 49x-05

 AFC: Direct monitoring of spindle load (see “Spindle load

monitoring” on page 401)

 Global program settings: Function also partially effective with

M91/M92 blocks (see “Global Program Settings (Software Option)” on page 380)

 Pallet preset table added (see “Pallet datum management with the

pallet preset table,” page 477 or see “Application,” page 474 or see “Storing measured values in the pallet preset table,” page 521 or see “Saving the basic rotation in the preset table,” page 526)

 The additional status display now has an additional tab, i.e. PAL, on

which an active pallet preset is displayed (see “General pallet information (PAL tab)” on page 84)

 New tool management (see “Tool management” on page 179)  New column R2TOL in the tool table (see “Tool table: Tool data

required for automatic tool measurement” on page 164)

 Tools can now also be selected during tool call by soft key directly

from TOOL.T (see “Calling tool data” on page 173)

 TNCguide: Context sensitivity has been improved in that when the

cursor is engaged it jumps to the appropriate description (see “Calling the TNCguide” on page 151)

 Lithuanian dialog added, machine parameter 7230 (see “List of

general user parameters” on page 621)

 M116 allowed in combination with M128 (see “Feed rate in

mm/min on rotary axes A, B, C: M116 (software option 1)” on page

455)

 Introduction of local and nonvolatile Q parameters QL and QR (see

“Principle and Overview” on page 274)

 The MOD function can now test the data medium (see “Checking

the Data Carrier” on page 614)

 New Cycle 241 for Single-Fluted Deep-Hole Drilling (see User’s

Manual for Cycles)

Page 17

 Touch probe cycle 404 (SET BASIC ROTATION) was expanded by

parameter Q305 (Number in table) in order to write basic rotations to the preset table (see User's Manual for Cycles)

 Touch probe cycles 408 to 419: The TNC now also writes to line 0

of the preset table when the display value is set (see User's Manual for Cycles)

 Touch probe cycle 416 (Datum on Circle Center) was expanded by

parameter Q320 (safety clearance) (see User's Manual for Cycles)

 Touch probe cycles 412, 413, 421 and 422: Additional parameter

Q365 (type of traverse) (see User's Manual for Cycles)

 Touch probe cycle 425 (Measure Slot) was expanded by parameters

Q301 (Move to clearance height) and Q320 (setup clearance) (see User's Manual for Cycles)

 Touch probe cycle 450 (Save Kinematics) was expanded by input

option 2 (Display saving status) in parameter Q410 (mode) (see User's Manual for Cycles)

 Touch probe cycle 451 (Measure Kinematics) was expanded by

parameters Q423 (number of circular measurements) and Q432 (set preset) (see User's Manual for Cycles)

 New touch probe cycle 452 (Preset Compensation) simplifies the

measurement of tool changer heads (see User's Manual for Cycles)

 New touch probe cycle 484 for calibrating the wireless TT 449 tool

touch probe (see User's Manual for Cycles)

New functions with 340 49x-05

HEIDENHAIN iTNC 530 17

Page 18

Changed functions in 340 49x-01 since the predecessor versions 340 422-xx/340 423-xx

 The layouts of the status display and additional status display were

redesigned (see “Status Displays” on page 81)

 Software 340 490 no longer supports the small resolution in

combination with the BC 120 screen (see “Visual display unit” on page 75)

 New key layout of the TE 530 B keyboard unit (see “Operating

panel” on page 77)

 The entry range for the EULPR precession angle in the PLANE EULER

function was expanded (see “Defining the machining plane with

340 422-xx/340 423-xx

Euler angles: EULER PLANE” on page 435)

 The plane vector in the VECTOR PLANE function no longer has to be

entered in standardized form (see “Defining the machining plane with two vectors: VECTOR PLANE” on page 437)

 Positioning behavior of the CYCL CALL PAT function has been

modified (see User's Manual for Cycles)

 The tool types available for selection in the tool table were increased

in preparation for future functions

 Instead of the last 10, you can now choose from the last 15 selected

files (see “Choosing one of the last files selected” on page 123)

Changed functions in 340 49x-01 since the predecessor versions

Page 19

Functions changed in 340 49x-02

 Access to the preset table was simplified. There are also new

possibilities for entering values in the preset table. See table “Manually saving the datums in the preset table”

 In inch-programs, the function M136 (feed rate in 0.1 inch/rev) can

no longer be combined with the FU function

 The feed-rate potentiometers of the HR 420 are no longer switched

over automatically when the handwheel is selected. The selection is made via soft key on the handwheel. In addition, the pop-up window for the active handwheel was made smaller, in order to improve the view of the display beneath it (see “Potentiometer settings” on page 503)

 The maximum number of contour elements for SL cycles was

increased to 8192, so that much more complex contours can be machined (see User's Manual for Cycles)

 FN16: F-PRINT: The maximum number of Q-parameter values that

can be output per line in the format description file was increased to 32 (see “FN 16: F-PRINT: Formatted output of text and Q parameter values” on page 294)

 The soft keys START and START SINGLE BLOCK in the Program

Test mode of operation were switched, so that the soft-key alignment is the same in all modes of operation (Programming and Editing, smarT.NC, Test) (see “Running a program test” on page

563)

 The design of the soft keys was revised completely

Functions changed in 340 49x-02

HEIDENHAIN iTNC 530 19

Page 20

Changed functions with 340 49x-03

 In Cycle 22 you can now define a tool name also for the coarse

roughing tool (see User's Manual Cycles)

 In the PLANE function, an FMAX can now be programmed for the

automatic rotary positioning (see “Automatic positioning: MOVE/TURN/STAY (entry is mandatory)” on page 444)

 When running programs in which non-controlled axes are

programmed, the TNC now interrupts the program run and displays a menu for returning to the programmed position (see “Programming of noncontrolled axes (counter axes)” on page 569)

 The tool usage file now also includes the total machining time,

which serves as the basis for the progress display in percent in the Program Run, Full Sequence mode (see “Tool usage test” on page

576)

 The TNC now also takes the dwell time into account when

calculating the machining time in the Test Run mode (see “Measuring the machining time” on page 559)

 Arcs that are not programmed in the active working plane can now

also be run as spatial arcs (see “Circular path C around circle center CC” on page 205)

 The EDIT OFF/ON soft key on the pocket table can be deactivated

by the machine tool builder (see “Pocket table for tool changer” on page 170)

Changed functions with 340 49x-03

 The additional status display has been revised. The following

improvements have been introduced (see “Additional status displays” on page 82):

 A new overview page with the most important status displays

were introduced

 The individual status pages are now displayed as tabs (as in

smarT.NC). The individual tabs can be selected with the Page soft keys or with the mouse

 The current run time of the program is shown in percent by a

progress bar

 The tolerance values set in Cycle 32 are displayed  Active global program settings are displayed, provided that this

software option was enabled

 The status of the Adaptive Feed Control (AFC) is displayed,

provided that this software option was enabled

Page 21

Changed functions with 340 49x-04

 DCM: Retraction after collision simplified (see “Collision monitoring

in the manual operating modes,” page 367)

 The input range for polar angles was increased (see “Circular path

CP around pole CC” on page 215)

 The value range for Q-parameter assignment was increased (see

“Programming notes,” page 276)

 The pocket-, stud- and slot-milling cycles 210 to 214 were removed

from the standard soft-key row (CYCL DEF > POCKETS/STUDS/SLOTS). For reasons of compatibility, the cycles will still be available, and can be selected via the GOTO key

 The soft-key rows in the Test Run operating mode were modified to

those of the smarT.NC operating mode

 Windows XP is now used on the dual-processor version (see

“Introduction” on page 648)

 Conversion from FK to H was moved to the special functions (SPEC

FCT) (see “Converting FK programs into HEIDENHAIN conversational format” on page 224)

 Filtering of contours was moved to the special functions (SPEC FCT)

(see “Filtering Contours (FCL 2 Function)” on page 405)

 Loading of values from the pocket calculator was changed (see “To

transfer the calculated value into the program” on page 139)

Changed functions with 340 49x-04

HEIDENHAIN iTNC 530 21

Page 22

Changed functions with 340 49x-05

 GS global program settings: Form was redesigned (see “Global

Program Settings (Software Option),” page 380)

 The menu for network configuration was revised (see “Configuring

the TNC” on page 594)

Changed functions with 340 49x-05

Page 23

Table of Contents

First Steps with the iTNC 530

Introduction

Programming: Fundamentals, File Management

Programming: Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Data Transfer from DXF Files

Programming: Subprograms and Program Section Repeats

Programming: Q Parameters

Programming: Miscellaneous Functions

Programming: Special Functions

Programming: Multi-axis Machining

2 3 4 5 6 7 8 9

11 12 13

Programming: Pallet Management

Positioning with Manual Data Input

Test Run and Program Run

MOD Functions

Tables and Overviews

iTNC 530 with Windows XP (option)

HEIDENHAIN iTNC 530 23

14 15 16

17 18 19

Page 24

Page 25

1 First Steps with the iTNC 530 ..... 51

1.1 Overview ..... 52

1.2 Machine Switch-On ..... 53

Acknowledge the power interruption and move to the reference points ..... 53

1.3 Programming the First Part ..... 54

Select the correct operating mode ..... 54

The most important TNC keys ..... 54

Create a new program/file management ..... 55

Define a workpiece blank ..... 56

Program layout ..... 57

Program a simple contour ..... 58

Create a cycle program ..... 61

1.4 Graphically Testing the Program ..... 64

Select the correct operating mode ..... 64

Select the tool table for the test run ..... 64

Choose the program you want to test ..... 65

Select the screen layout and the view ..... 65

Start the program test ..... 66

1.5 Setting Up Tools ..... 67

Select the correct operating mode ..... 67

Prepare and measure tools ..... 67

The tool table TOOL.T ..... 67

The pocket table TOOL_P.TCH ..... 68

1.6 Workpiece Setup ..... 69

Select the correct operating mode ..... 69

Clamp the workpiece ..... 69

Align the workpiece with a 3-D touch probe system ..... 70

Set the datum with a 3-D touch probe ..... 71

1.7 Running the First Program ..... 72

Select the correct operating mode ..... 72

Choose the program you want to run ..... 72

Start the program ..... 72

HEIDENHAIN iTNC 530 25

Page 26

2 Introduction ..... 73

2.1 The iTNC 530 ..... 74

Programming: HEIDENHAIN conversational, smarT.NC and DIN/ISO formats ..... 74

Compatibility ..... 74

2.2 Visual Display Unit and Keyboard ..... 75

Visual display unit ..... 75

Sets the screen layout ..... 76

Operating panel ..... 77

2.3 Operating Modes ..... 78

Manual Operation and Electronic Handwheel ..... 78

Positioning with Manual Data Input ..... 78

Programming and Editing ..... 79

Test Run ..... 79

Program Run, Full Sequence and Program Run, Single Block ..... 80

2.4 Status Displays ..... 81

“General” status display ..... 81

Additional status displays ..... 82

2.5 Window Manager ..... 90

2.6 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels ..... 91

3-D touch probes ..... 91

HR electronic handwheels ..... 92

Page 27

3 Programming: Fundamentals, File Management ..... 93

3.1 Fundamentals ..... 94

Position encoders and reference marks ..... 94

Reference system ..... 94

Reference system on milling machines ..... 95

Polar coordinates ..... 96

Absolute and incremental workpiece positions ..... 97

Setting the datum ..... 98

3.2 Creating and Writing Programs ..... 99

Organization of an NC program in HEIDENHAIN Conversational ..... 99

Define the blank: BLK FORM ..... 99

Creating a new part program ..... 100

Programming tool movements in conversational format ..... 102

Actual position capture ..... 104

Editing a program ..... 105

The TNC search function ..... 109

3.3 File Management: Fundamentals ..... 111

Files ..... 111

Data backup ..... 112

3.4 Working with the File Manager ..... 113

Directories ..... 113

Paths ..... 113

Overview: Functions of the file manager ..... 114

Calling the file manager ..... 115

Selecting drives, directories and files ..... 116

Creating a new directory (only possible on the drive TNC:\) ..... 119

Creating a new file (only possible on the drive TNC:\) ..... 119

Copying a single file ..... 120

Copying files into another directory ..... 121

Copying a table ..... 122

Copying a directory ..... 123

Choosing one of the last files selected ..... 123

Deleting a file ..... 124

Deleting a directory ..... 124

Tagging files ..... 125

Renaming a file ..... 127

Additional functions ..... 128

Working with shortcuts ..... 130

Data transfer to or from an external data medium ..... 131

The TNC in a network ..... 133

USB devices on the TNC (FCL 2 function) ..... 134

HEIDENHAIN iTNC 530 27

Page 28

4 Programming: Programming Aids ..... 135

4.1 Adding Comments ..... 136

Function ..... 136

Entering comments during programming ..... 136

Inserting comments after program entry ..... 136

Entering a comment in a separate block ..... 136

Functions for editing of the comment ..... 137

4.2 Structuring Programs ..... 138

Definition and applications ..... 138

Displaying the program structure window / Changing the active window ..... 138

Inserting a structuring block in the (left) program window ..... 138

Selecting blocks in the program structure window ..... 138

4.3 Integrated Pocket Calculator ..... 139

Operation ..... 139

4.4 Programming Graphics ..... 140

Generating / Not generating graphics during programming: ..... 140

Generating a graphic for an existing program ..... 140

Block number display ON/OFF ..... 141

Erasing the graphic ..... 141

Magnifying or reducing a detail ..... 141

4.5 3-D Line Graphics (FCL2 Function) ..... 142

Function ..... 142

Functions of the 3-D line graphics ..... 142

Highlighting NC blocks in the graphics ..... 144

Block number display ON/OFF ..... 144

Erasing the graphic ..... 144

4.6 Immediate Help for NC Error Messages ..... 145

Displaying error messages ..... 145

Display HELP ..... 145

4.7 List of All Current Error Messages ..... 146

Function ..... 146

Show error list ..... 146

Window contents ..... 147

Calling the TNCguide help system ..... 148

Generating service files ..... 149

4.8 The Context-Sensitive Help System TNCguide (FCL3 Function) ..... 150

Function ..... 150

Working with the TNCguide ..... 151

Downloading current help files ..... 155

Page 29

5 Programming: Tools ..... 157

5.1 Entering Tool-Related Data ..... 158

Feed rate F ..... 158

Spindle speed S ..... 159

5.2 Tool Data ..... 160

Requirements for tool compensation ..... 160

Tool numbers and tool names ..... 160

Tool length L ..... 160

Tool radius R ..... 160

Delta values for lengths and radii ..... 161

Entering tool data into the program ..... 161

Entering tool data in the table ..... 162

Tool-carrier kinematics ..... 168

Using an external PC to overwrite individual tool data ..... 169

Pocket table for tool changer ..... 170

Calling tool data ..... 173

Tool change ..... 175

Tool usage test ..... 177

Tool management ..... 179

5.3 Tool Compensation ..... 182

Introduction ..... 182

Tool length compensation ..... 182

Tool radius compensation ..... 183

HEIDENHAIN iTNC 530 29

Page 30

6 Programming: Programming Contours ..... 187

6.1 Tool Movements ..... 188

Path functions ..... 188

FK free contour programming ..... 188

Miscellaneous functions M ..... 188

Subprograms and program section repeats ..... 188

Programming with Q parameters ..... 188

6.2 Fundamentals of Path Functions ..... 189

Programming tool movements for workpiece machining ..... 189

6.3 Contour Approach and Departure ..... 192

Overview: Types of paths for contour approach and departure ..... 192

Important positions for approach and departure ..... 193

Approaching on a straight line with tangential connection: APPR LT ..... 195

Approaching on a straight line perpendicular to the first contour point: APPR LN ..... 195

Approaching on a circular path with tangential connection: APPR CT ..... 196

Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT ..... 197

Departing on a straight line with tangential connection: DEP LT ..... 198

Departing on a straight line perpendicular to the last contour point: DEP LN ..... 198

Departure on a circular path with tangential connection: DEP CT ..... 199

Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT ..... 199

6.4 Path Contours—Cartesian Coordinates ..... 200

Overview of path functions ..... 200

Straight line L ..... 201

Inserting a chamfer between two straight lines ..... 202

Corner rounding RND ..... 203

Circle center CCI ..... 204

Circular path C around circle center CC ..... 205

Circular path CR with defined radius ..... 206

Circular path CT with tangential connection ..... 208

6.5 Path Contours—Polar Coordinates ..... 213

Overview ..... 213

Zero point for polar coordinates: pole CC ..... 214

Straight line LP ..... 214

Circular path CP around pole CC ..... 215

Circular path CTP with tangential connection ..... 216

Helical interpolation ..... 217

Page 31

6.6 Path Contours—FK Free Contour Programming ..... 221

Fundamentals ..... 221

Graphics during FK programming ..... 223

Converting FK programs into HEIDENHAIN conversational format ..... 224

Initiating the FK dialog ..... 225

Pole for FK programming ..... 226

Free programming of straight lines ..... 226

Free programming of circular arcs ..... 227

Input possibilities ..... 227

Auxiliary points ..... 231

Relative data ..... 232

HEIDENHAIN iTNC 530 31

Page 32

7 Programming: Data Transfer from DXF Files ..... 239

7.1 Processing DXF Files (Software Option) ..... 240

Function ..... 240

Opening a DXF file ..... 241

Basic settings ..... 242

Layer settings ..... 244

Specifying the reference point ..... 245

Selecting and saving a contour ..... 247

Selecting and storing machining positions ..... 250

Zoom function ..... 256

Page 33

8 Programming: Subprograms and Program Section Repeats ..... 257

8.1 Labeling Subprograms and Program Section Repeats ..... 258

Labels ..... 258

8.2 Subprograms ..... 259

Operating sequence ..... 259

Programming notes ..... 259

Programming a subprogram ..... 259

Calling a subprogram ..... 259

8.3 Program Section Repeats ..... 260

Label LBL ..... 260

Operating sequence ..... 260

Programming notes ..... 260

Programming a program section repeat ..... 260

Calling a program section repeat ..... 260

8.4 Separate Program as Subprogram ..... 261

Operating sequence ..... 261

Programming notes ..... 261

Calling any program as a subprogram ..... 261

8.5 Nesting ..... 263

Types of nesting ..... 263

Nesting depth ..... 263

Subprogram within a subprogram ..... 264

Repeating program section repeats ..... 265

Repeating a subprogram ..... 266

8.6 Programming Examples ..... 267

HEIDENHAIN iTNC 530 33

Page 34

9 Programming: Q Parameters ..... 273

9.1 Principle and Overview ..... 274

Programming notes ..... 276

Calling Q-parameter functions ..... 277

9.2 Part Families—Q Parameters in Place of Numerical Values ..... 278

Function ..... 278

9.3 Describing Contours through Mathematical Operations ..... 279

Function ..... 279

Overview ..... 279

Programming fundamental operations ..... 280

9.4 Trigonometric Functions ..... 281

Definitions ..... 281

Programming trigonometric functions ..... 282

9.5 Circle Calculations ..... 283

Function ..... 283

9.6 If-Then Decisions with Q Parameters ..... 284

Function ..... 284

Unconditional jumps ..... 284

Programming If-Then decisions ..... 284

Abbreviations used: ..... 285

9.7 Checking and Changing Q Parameters ..... 286

Procedure ..... 286

9.8 Additional Functions ..... 287

Overview ..... 287

FN 14: ERROR: Displaying error messages ..... 288

FN 15: PRINT: Output of texts or Q parameter values ..... 293

FN 16: F-PRINT: Formatted output of text and Q parameter values ..... 294

FN 18: SYS-DATUM READ: Read system data ..... 298

FN 19: PLC: Transfer values to the PLC ..... 304

FN 20: WAIT FOR: NC and PLC synchronization ..... 305

FN 25: PRESET: Setting a new datum ..... 307

9.9 Entering Formulas Directly ..... 308

Entering formulas ..... 308

Rules for formulas ..... 310

Programming example ..... 311

Page 35

9.10 String Parameters ..... 312

String processing functions ..... 312

Assigning string parameters ..... 313

Chain-linking string parameters ..... 314

Converting a numerical value to a string parameter ..... 315

Copying a substring from a string parameter ..... 316

Copying system data to a string parameter ..... 317

Converting a string parameter to a numerical value ..... 319

Checking a string parameter ..... 320

Finding the length of a string parameter ..... 321

Comparing alphabetic priority ..... 322

9.11 Preassigned Q Parameters ..... 323

Values from the PLC: Q100 to Q107 ..... 323

WMAT block: QS100 ..... 323

Active tool radius: Q108 ..... 323

Tool axis: Q109 ..... 324

Spindle status: Q110 ..... 324

Coolant on/off: Q111 ..... 324

Overlap factor: Q112 ..... 324

Unit of measurement for dimensions in the program: Q113 ..... 325

Tool length: Q114 ..... 325

Coordinates after probing during program run ..... 325

Deviation between actual value and nominal value during automatic tool measurement with the TT 130 ..... 326

Tilting the working plane with mathematical angles: rotary axis coordinates calculated by the TNC ..... 326

Measurement results from touch probe cycles (see also User’s Manual for Touch Probe Cycles) ..... 327

9.12 Programming Examples ..... 329

HEIDENHAIN iTNC 530 35

Page 36

10 Programming: Miscellaneous Functions ..... 337

10.1 Entering Miscellaneous Functions M and STOP ..... 338

Fundamentals ..... 338

10.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 340

Overview ..... 340

10.3 Miscellaneous Functions for Coordinate Data ..... 341

Programming machine-referenced coordinates: M91/M92 ..... 341

Activating the most recently entered datum: M104 ..... 343

Moving to positions in a non-tilted coordinate system with a tilted working plane: M130 ..... 343

10.4 Miscellaneous Functions for Contouring Behavior ..... 344

Smoothing corners: M90 ..... 344

Insert rounding arc between straight lines: M112 ..... 344

Do not include points when executing non-compensated line blocks: M124 ..... 345

Machining small contour steps: M97 ..... 346

Machining open contours corners: M98 ..... 348

Feed rate factor for plunging movements: M103 ..... 349

Feed rate in millimeters per spindle revolution: M136 ..... 350

Feed rate for circular arcs: M109/M110/M111 ..... 350

Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 351

Superimposing handwheel positioning during program run: M118 ..... 353

Retraction from the contour in the tool-axis direction: M140 ..... 354

Suppressing touch probe monitoring: M141 ..... 355

Delete modal program information: M142 ..... 356

Delete basic rotation: M143 ..... 356

Automatically retract tool from the contour at an NC stop: M148 ..... 357

Suppress limit switch message: M150 ..... 358

10.5 Miscellaneous Functions for Laser Cutting Machines ..... 359

Principle ..... 359

Output the programmed voltage directly: M200 ..... 359

Output voltage as a function of distance: M201 ..... 359

Output voltage as a function of speed: M202 ..... 360

Output voltage as a function of time (time-dependent ramp): M203 ..... 360

Output voltage as a function of time (time-dependent pulse): M204 ..... 360

Page 37

11 Programming: Special Functions ..... 361

11.1 Overview of Special Functions ..... 362

Main menu for SPEC FCT special functions ..... 362

Program defaults menu ..... 363

Functions for contour and point machining menu ..... 363

Menu of various conversational functions ..... 364

Menu of programming aids ..... 364

11.2 Dynamic Collision Monitoring (Software Option) ..... 365

Function ..... 365

Collision monitoring in the manual operating modes ..... 367

Collision monitoring in Automatic operation ..... 369

Graphic depiction of the protected space (FCL4 function) ..... 370

Collision monitoring in the Test Run mode of operation ..... 371

11.3 Fixture Monitoring (Software Option) ..... 372

Fundamentals ..... 372

Fixture templates ..... 373

Setting parameters for the fixture: FixtureWizard ..... 374

Placing the fixture on the machine ..... 376

Editing fixtures ..... 377

Removing fixtures ..... 377

Check the position of the measured fixture ..... 378

11.4 Global Program Settings (Software Option) ..... 380

Function ..... 380

Technical prerequisites ..... 382

Activating/deactivating a function ..... 383

Basic rotation ..... 385

Swapping axes ..... 386

Superimposed mirroring ..... 387

Additional, additive datum shift ..... 387

Axis locking ..... 388

Superimposed rotation ..... 388

Feed rate override ..... 388

Handwheel superimposition ..... 389

11.5 Adaptive Feed Control Software Option (AFC) ..... 391

Function ..... 391

Defining the AFC basic settings ..... 393

Recording a teach-in cut ..... 395

Activating/deactivating AFC ..... 398

Log file ..... 399

Tool breakage/tool wear monitoring ..... 401

Spindle load monitoring ..... 401

HEIDENHAIN iTNC 530 37

Page 38

11.6 Generate a Backward Program ..... 402

Function ..... 402

Prerequisites for the program to be converted ..... 403

Application example ..... 404

11.7 Filtering Contours (FCL 2 Function) ..... 405

Function ..... 405

11.8 File Functions ..... 406

Function ..... 406

Defining file functions ..... 406

11.9 Defining Coordinate Transformations ..... 407

Overview ..... 407

TRANS DATUM AXIS ..... 407

TRANS DATUM TABLE ..... 408

TRANS DATUM RESET ..... 408

11.10 Creating Text Files ..... 409

Function ..... 409

Opening and exiting text files ..... 409

Editing texts ..... 410

Deleting and inserting characters, words and lines ..... 411

Editing text blocks ..... 412

Finding text sections ..... 413

11.11 Working with Cutting Data Tables ..... 414

Note ..... 414

Applications ..... 414

Table for workpiece materials ..... 415

Table for tool cutting materials ..... 416

Table for cutting data ..... 416

Data required for the tool table ..... 417

Working with automatic speed / feed rate calculation ..... 418

Data transfer from cutting data tables ..... 419

Configuration file TNC.SYS ..... 419

11.12 Freely Definable Tables ..... 420

Fundamentals ..... 420

Creating a freely definable table ..... 420

Editing the table format ..... 421

Switching between table and form view ..... 422

FN 26: TABOPEN: Opening a freely definable table ..... 423

FN 27: TABWRITE: Writing to a freely definable table ..... 423

FN 28: TABREAD: Reading a freely definable table ..... 424

Page 39

12 Programming: Multiple Axis Machining ..... 425

12.1 Functions for Multiple Axis Machining ..... 426

12.2 The PLANE Function: Tilting the Working Plane (Software Option 1) ..... 427

Introduction ..... 427

Define the PLANE function ..... 429

Position display ..... 429

Reset the PLANE function ..... 430

Defining the machining plane with space angles: PLANE SPATIAL ..... 431

Defining the machining plane with projection angles: PROJECTED PLANE ..... 433

Defining the machining plane with Euler angles: EULER PLANE ..... 435

Defining the machining plane with two vectors: VECTOR PLANE ..... 437

Defining the machining plane via three points: POINTS PLANE ..... 439

Defining the machining plane with a single, incremental space angle: PLANE RELATIVE ..... 441

Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function) ..... 442

Specifying the positioning behavior of the PLANE function ..... 444

12.3 Inclined-Tool Machining in the Tilted Plane ..... 448

Function ..... 448

Inclined-tool machining via incremental traverse of a rotary axis ..... 448

Inclined-tool machining via normal vectors ..... 449

12.4 TCPM FUNCTION (Software Option 2) ..... 450

Function ..... 450

Define TCPM FUNCTION ..... 451

Mode of action of the programmed feed rate ..... 451

Interpretation of the programmed rotary axis coordinates ..... 452

Type of interpolation between the starting and end position ..... 453

Reset TCPM FUNCTION ..... 454

12.5 Miscellaneous Functions for Rotary Axes ..... 455

Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1) ..... 455

Shorter-path traverse of rotary axes: M126 ..... 456

Reducing display of a rotary axis to a value less than 360°: M94 ..... 457

Automatic compensation of machine geometry when working with tilted axes: M114 (software option 2) ..... 458

Maintaining the position of the tool tip when positioning with tilted axes (TCPM): M128 (software option

2) ..... 459

Exact stop at corners with nontangential transitions: M134 ..... 462

Selecting tilting axes: M138 ..... 462

Compensating the machine’s kinematics configuration for ACTUAL/NOMINAL positions at end of block: M144

(software option 2) ..... 463

HEIDENHAIN iTNC 530 39

Page 40

12.6 Three-Dimensional Tool Compensation (Software Option 2) ..... 464

Introduction ..... 464

Definition of a normalized vector ..... 465

Permissible tool forms ..... 466

Using other tools: Delta values ..... 466

3-D compensation without tool orientation ..... 467

Face milling: 3-D compensation with and without tool orientation ..... 467

Peripheral milling: 3-D radius compensation with workpiece orientation ..... 469

12.7 Contour Movements — Spline Interpolation (Software Option 2) ..... 471

Function ..... 471

Page 41

13 Programming: Pallet Editor ..... 473

13.1 Pallet Editor ..... 474

Application ..... 474

Selecting a pallet table ..... 476

Leaving the pallet file ..... 476

Pallet datum management with the pallet preset table ..... 477

Executing the pallet file ..... 479

13.2 Pallet Operation with Tool-Oriented Machining ..... 480

Application ..... 480

Selecting a pallet file ..... 485

Setting up the pallet file with the entry form ..... 485

Sequence of tool-oriented machining ..... 490

Leaving the pallet file ..... 491

Executing the pallet file ..... 491

HEIDENHAIN iTNC 530 41

Page 42

14 Manual Operation and Setup ..... 493

14.1 Switch-On, Switch-Off ..... 494

Switch-on ..... 494

Switch-off ..... 497

14.2 Moving the Machine Axes ..... 498

Note ..... 498

To traverse with the machine axis direction buttons: ..... 498

Incremental jog positioning ..... 499

Traversing with the HR 410 electronic handwheel ..... 500

HR 420 electronic handwheel ..... 501

14.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 506

Function ..... 506

Entering values ..... 506

Changing the spindle speed and feed rate ..... 507

14.4 Datum Setting without a 3-D Touch Probe ..... 508

Note ..... 508

Preparation ..... 508

Workpiece presetting with axis keys ..... 509

Datum management with the preset table ..... 510

14.5 Using the 3-D Touch Probe ..... 517

Overview ..... 517

Selecting probe cycles ..... 517

Recording measured values from the touch probe cycles ..... 518

Writing the measured values from touch probe cycles in datum tables ..... 519

Writing the measured values from touch probe cycles in the preset table ..... 520

Storing measured values in the pallet preset table ..... 521

14.6 Calibrating a 3-D Touch Probe ..... 522

Introduction ..... 522

Calibrating the effective length ..... 522

Calibrating the effective radius and compensating center misalignment ..... 523

Displaying calibration values ..... 524

Managing more than one block of calibrating data ..... 524

14.7 Compensating Workpiece Misalignment with a 3-D Touch Probe ..... 525

Introduction ..... 525

Measuring the basic rotation ..... 525

Saving the basic rotation in the preset table ..... 526

Saving the basic rotation in the pallet preset table ..... 526

Displaying a basic rotation ..... 526

Canceling a basic rotation ..... 526

Page 43

14.8 Datum Setting with a 3-D Touch Probe ..... 527

Overview ..... 527

Datum setting in any axis ..... 527

Corner as datum—using points that were already probed for a basic rotation ..... 528

Corner as datum—without using points that were already probed for a basic rotation ..... 528

Circle center as datum ..... 529

Center line as datum ..... 530

Setting datum points using holes/cylindrical studs ..... 531

Measuring Workpieces with a 3-D Touch Probe ..... 532

Using the touch probe functions with mechanical probes or dial gauges ..... 535

14.9 Tilting the Working Plane (Software Option 1) ..... 536

Application, function ..... 536

Traversing the reference points in tilted axes ..... 538

Setting the datum in a tilted coordinate system ..... 538

Datum setting on machines with rotary tables ..... 538

Datum setting on machines with spindle-head changing systems ..... 538

Position display in a tilted system ..... 539

Limitations on working with the tilting function ..... 539

Activating manual tilting ..... 540

Setting the current tool-axis direction as the active machining direction (FCL 2 function) ..... 541

HEIDENHAIN iTNC 530 43

Page 44

15 Positioning with Manual Data Input ..... 543

15.1 Programming and Executing Simple Machining Operations ..... 544

Positioning with Manual Data Input (MDI) ..... 544

Protecting and erasing programs in $MDI ..... 547

Page 45

16 Test Run and Program Run ..... 549

16.1 Graphics ..... 550

Application ..... 550

Overview of display modes ..... 552

Plan view ..... 552

Projection in 3 planes ..... 553

3-D view ..... 554

Magnifying details ..... 557

Repeating graphic simulation ..... 558

Displaying the tool ..... 558

Measuring the machining time ..... 559

16.2 Functions for Program Display ..... 560

Overview ..... 560

16.3 Test Run ..... 561

Application ..... 561

16.4 Program Run ..... 566

Application ..... 566

Running a part program ..... 567

Interrupting machining ..... 568

Moving the machine axes during an interruption ..... 570

Resuming program run after an interruption ..... 571

Mid-program startup (block scan) ..... 572

Returning to the contour ..... 575

Entering a program with the GOTO key ..... 575

Tool usage test ..... 576

16.5 Automatic Program Start ..... 578

Application ..... 578

16.6 Optional Block Skip ..... 579

Application ..... 579

Erasing the “/” character ..... 579

16.7 Optional Program-Run Interruption ..... 580

Application ..... 580

HEIDENHAIN iTNC 530 45

Page 46

17 MOD Functions ..... 581

17.1 Selecting MOD Functions ..... 582

Selecting the MOD functions ..... 582

Changing the settings ..... 582

Exiting the MOD functions ..... 582

Overview of MOD functions ..... 583

17.2 Software Numbers ..... 584

Function ..... 584

17.3 Entering Code Numbers ..... 585

Function ..... 585

17.4 Loading Service Packs ..... 586

Function ..... 586

17.5 Setting the Data Interfaces ..... 587

Function ..... 587

Setting the RS-232 interface ..... 587

Setting the RS-422 interface ..... 587

Setting the OPERATING MODE of the external device ..... 587

Setting the baud rate ..... 587

Assign ..... 588

Software for data transfer ..... 589

17.6 Ethernet Interface ..... 591

Introduction ..... 591

Connection possibilities ..... 591

Connecting the iTNC directly with a Windows PC ..... 592

Configuring the TNC ..... 594

17.7 Configuring PGM MGT ..... 601

Function ..... 601

Changing the PGM MGT setting ..... 601

Dependent files ..... 602

17.8 Machine-Specific User Parameters ..... 603

Function ..... 603

17.9 Showing the Workpiece in the Working Space ..... 604

Function ..... 604

Rotate the entire image ..... 605

17.10 Position Display Types ..... 606

Function ..... 606

17.11 Unit of Measurement ..... 607

Function ..... 607

17.12 Selecting the Programming Language for $MDI ..... 608

Function ..... 608

17.13 Selecting the Axes for Generating L Blocks ..... 609

Function ..... 609

Page 47

17.14 Entering the Axis Traverse Limits, Datum Display ..... 610

Function ..... 610

Working without additional traverse limits ..... 610

Find and enter the maximum traverse ..... 610

Datum display ..... 611

17.15 Displaying HELP Files ..... 612

Function ..... 612

Selecting HELP files ..... 612

17.16 Displaying Operating Times ..... 613

Function ..... 613

17.17 Checking the Data Carrier ..... 614

Function ..... 614

Performing the data carrier check ..... 614

17.18 Setting the System Time ..... 615

Function ..... 615

Selecting appropriate settings ..... 615

17.19 TeleService ..... 616

Function ..... 616

Calling/exiting TeleService ..... 616

17.20 External Access ..... 617

Function ..... 617

HEIDENHAIN iTNC 530 47

Page 48

18 Tables and Overviews ..... 619

18.1 General User Parameters ..... 620

Input possibilities for machine parameters ..... 620

Selecting general user parameters ..... 620

List of general user parameters ..... 621

18.2 Pin Layouts and Connecting Cables for the Data Interfaces ..... 635

RS-232-C/V.24 interface for HEIDENHAIN devices ..... 635

Non-HEIDENHAIN devices ..... 636

RS-422/V.11 interface ..... 637

Ethernet interface RJ45 socket ..... 637

18.3 Technical Information ..... 638

18.4 Exchanging the Buffer Battery ..... 646

Page 49

19 iTNC 530 with Windows XP (Option) ..... 647

19.1 Introduction ..... 648

End User License Agreement (EULA) for Windows XP ..... 648

General ..... 648

Specifications ..... 649

19.2 Starting an iTNC 530 Application ..... 650

Logging on to Windows ..... 650

19.3 Switching Off the iTNC 530 ..... 652

Fundamentals ..... 652

Logging a user off ..... 652

Exiting the iTNC application ..... 653

Shutting down Windows ..... 654

19.4 Network Settings ..... 655

Prerequisite ..... 655

Adjusting the network settings ..... 655

Controlling access ..... 656

19.5 Specifics About File Management ..... 657

The iTNC drive ..... 657

Data transfer to the iTNC 530 ..... 658

HEIDENHAIN iTNC 530 49

Page 50

Page 51

First Steps with the iTNC 530

Page 52

1.1 Overview

This chapter is intended to help TNC beginners quickly learn to handle the most important procedures. For more information on a respective topic, see the section referred to in the text.

The following topics are included in this chapter

 Machine Switch-On

1.1 Overview

 Programming the First Part  Graphically Testing the Program  SETTING UP TOOLS  Workpiece Setup  Running the First Program

52 First Steps with the iTNC 530

Page 53

1.2 Machine Switch-On

Acknowledge the power interruption and move to the reference points

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

U Switch on the power supply for control and machine. The TNC starts

the operating system. This process may take several minutes. Then the TNC will display the message “Power interruption.”

U Press the CE key: The TNC converts the PLC program U Switch on the control voltage: The TNC checks

operation of the emergency stop circuit and goes into the reference run mode

U Cross the reference points manually in the displayed

sequence: For each axis press the machine START button. If you have absolute linear and angle encoders on your machine there is no need for a reference run.

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

Further information on this topic

 Traversing the reference marks: See “Switch-on,” page 494  Operating modes:See “Programming and Editing,” page 79

1.2 Machine Switch-On

HEIDENHAIN iTNC 530 53

Page 54

1.3 Programming the First Part

Select the correct operating mode

You can write programs only in the Programming and Editing mode:

U Press the operating modes key: The TNC goes into

the Programming and Editing mode

Further information on this topic

 Operating modes:See “Programming and Editing,” page 79

The most important TNC keys

Functions for conversational guidance Key

Confirm entry and activate the next dialog prompt

Ignore the dialog question

1.3 Programming the First Part

End the dialog immediately

Abort dialog, discard entries

Soft keys on the screen with which you select functions appropriate to the active state

Further information on this topic

 Writing and editing programs: See “Editing a program,” page 105  Overview of keys: See “Controls of the TNC,” page 2

54 First Steps with the iTNC 530

Page 55

Create a new program/file management

U Press the PGM MGT key: the TNC displays the file

management. The file management of the TNC is arranged much like the file management on a PC with the Windows Explorer. The file management enables you to manipulate data on the TNC hard disk

U Use the arrow keys to select the folder in which you

want to open the new file

U Enter a file name with the extension .H: The TNC then

automatically opens a program and asks for the unit of measure for the new program

U To select the unit of measure: press the MM or INCH

soft key: The TNC automatically starts the workpiece blank definition (see “Define a workpiece blank” on page 56)

The TNC automatically generates the first and last blocks of the program. Afterwards you can no longer change these blocks.

Further information on this topic

 File management: See “Working with the File Manager,” page 113  Creating a new program: See “Creating and Writing Programs,”

page 99

1.3 Programming the First Part

HEIDENHAIN iTNC 530 55

Page 56

Define a workpiece blank

Immediately after you have created a new program, the TNC starts the dialog for entering the workpiece blank definition. Always define the workpiece blank as a cuboid by entering the MIN and MAX points, each with reference to the selected reference point.

After you have created a new program, the TNC automatically initiates the workpiece blank definition and asks for the required data:

U Spindle axis Z?: Enter the active spindle axis. Z is saved as default

setting. Accept with the ENT key

U Def BLK FORM: Min-corner?: Smallest X coordinate of the workpiece

blank with respect to the reference point, e.g. 0. Confirm with the ENT key

U Def BLK FORM: Min-corner?: Smallest Y coordinate of the workpiece

blank with respect to the reference point, e.g. 0. Confirm with the ENT key

U Def BLK FORM: Min-corner?: Smallest Z coordinate of the workpiece

blank with respect to the reference point, e.g. -40. Confirm with the ENT key

U Def BLK FORM: Max-corner?: Largest X coordinate of the workpiece

1.3 Programming the First Part

blank with respect to the reference point, e.g. 100. Confirm with the ENT key

U Def BLK FORM: Max-corner?: Largest Y coordinate of the workpiece

blank with respect to the reference point, e.g. 100. Confirm with the ENT key

U Def BLK FORM: Max-corner?: Largest Z coordinate of the workpiece

blank with respect to the reference point, e.g. 0. Confirm with the ENT key

Example NC blocks

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

100

MAX

-40

MIN

100

Further information on this topic

 Defining the workpiece blank: (See page 100)

56 First Steps with the iTNC 530

Page 57

Program layout

NC programs should be arranged consistently in a similar manner. This makes it easier to find your place and reduces errors.

Recommended program layout for simple, conventional contour machining

1 Call tool, define tool axis 2 Retract the tool 3 Pre-position the tool in the working plane near the contour starting

point

4 In the tool axis, position the tool above the workpiece, or pre-

position immediately to workpiece depth. If required, switch on the spindle/coolant

5 Move to the contour 6 Machine the contour 7 Leave the contour 8 Retract the tool, end the program

Further information on this topic:

 Contour programming: See “Tool Movements,” page 188

Recommended program layout for simple cycle programs 1 Call tool, define tool axis 2 Retract the tool 3 Define the machining positions 4 Define the fixed cycle 5 Call the cycle, switch on the spindle/coolant 6 Retract the tool, end the program

Further information on this topic:

 Cycle programming: See User’s Manual for Cycles

Example: Layout of contour machining programs

0 BEGIN PGM BSPCONT MM 1 BLK FORM 0.1 Z X... Y... Z... 2 BLK FORM 0.2 X... Y... Z... 3 TOOL CALL 5 Z S5000 4 L Z+250 R0 FMAX 5 L X... Y... R0 FMAX 6 L Z+10 R0 F3000 M13 7 APPR ... RL F500 ... 16 DEP ... X... Y... F3000 M9 17 L Z+250 R0 FMAX M2 18 END PGM BSPCONT MM

Example: Program layout for cycle programming

0 BEGIN PGM BSBCYC MM 1 BLK FORM 0.1 Z X... Y... Z... 2 BLK FORM 0.2 X... Y... Z... 3 TOOL CALL 5 Z S5000 4 L Z+250 R0 FMAX 5 PATTERN DEF POS1( X... Y... Z... ) ... 6 CYCL DEF... 7 CYCL CALL PAT FMAX M13 8 L Z+250 R0 FMAX M2 9 END PGM BSBCYC MM

1.3 Programming the First Part

HEIDENHAIN iTNC 530 57

Page 58

Program a simple contour

The contour shown to the right is to be milled once to a depth of 5 mm. You have already defined the workpiece blank. After you have initiated a dialog through a function key, enter all the data requested by the TNC in the screen header.

U Call the tool: Enter the tool data. Confirm each of your

entries with the ENT key. Do not forget the tool axis

U Retract the tool: Press the orange axis key Z in order

to get clear in the tool axis, and enter the value for the position to be approached, e.g. 250. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Activate the radius compensation

U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Confirm the Miscellaneous function M? with the

END key: The TNC saves the entered positioning block

1.3 Programming the First Part

U Preposition the tool in the working plane: Press the

orange X axis key and enter the value for the position to be approached, e.g. -20

U Press the orange Y axis key and enter the value for the

position to be approached, e.g. -20. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Do not activate the radius compensation

U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Confirm the Miscellaneous function M? with the

END key: The TNC saves the entered positioning block

U Move the tool to workpiece depth: Press the orange Y

axis key and enter the value for the position to be approached, e.g. -5. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Do not activate the radius compensation

U Feed rate F=? Enter the positioning feed rate, e.g.

3000 mm/min and confirm with the ENT key

U Miscellaneous function M? Switch on the spindle and

coolant, e.g. M13. Confirm with the END key: The TNC saves the entered positioning block

58 First Steps with the iTNC 530

Page 59

U Move to the contour: Press the APPR/DEP key: The

TNC shows a soft-key row with approach and departure functions

U Select the approach function APPR CT: Enter the

coordinates of the contour starting point 1 in X and Y, e.g. 5/5. Confirm with the ENT key

U Center angle? Enter the approach angle, e.g.90°, and

confirm with the ENT key

U Circle radius? Enter the approach radius, e.g. 8 mm,

and confirm with the ENT key

U Confirm the Radius comp.: RL/RR/no comp? with the

RL soft key: Activate the radius compensation to the left of the programmed contour

U Feed rate F=? Enter the machining feed rate, e.g. 700

mm/min, and confirm your entry with the END key

U Machine the contour and move to contour point 2: You

only need to enter the information that changes. In other words, enter only the Y coordinate 95 and save your entry with the END key

U Move to contour point 3: Enter the X coordinate 95

and save your entry with the END key

U Define the chamfer at contour point 3: Enter the

chamfer width 10 mm and save with the END key

U Move to contour point 4: Enter the Y coordinate 5 and

save your entry with the END key

U Define the chamfer at contour point 4: Enter the

chamfer width 20 mm and save with the END key

U Move to contour point 1: Enter the X coordinate 5 and

save your entry with the END key

1.3 Programming the First Part

HEIDENHAIN iTNC 530 59

Page 60

U Depart the contour

U Select the departure function DEP CT U Center angle? Enter the departure angle, e.g. 90°, and

confirm with the ENT key

U Circle radius? Enter the departure radius, e.g. 8 mm,

and confirm with the ENT key

U Feed rate F=? Enter the positioning feed rate, e.g.

3000 mm/min and confirm with the ENT key

U Miscellaneous function M? Switch off the coolant,

e.g. M9, with the END key: The TNC saves the entered positioning block

U Retract the tool: Press the orange axis key Z in order

to get clear in the tool axis, and enter the value for the position to be approached, e.g. 250. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Do not activate the radius compensation

1.3 Programming the First Part

U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Miscellaneous function M? Enter M2 to end the

program and confirm with the END key: The TNC saves the entered positioning block

Further information on this topic

 Complete example with NC blocks: See “Example: Linear

movements and chamfers with Cartesian coordinates,” page 209

 Creating a new program: See “Creating and Writing Programs,”

page 99

 Approaching/departing contours: See “Contour Approach and

Departure,” page 192

 Programming contours: See “Overview of path functions,” page

200

 Programmable feed rates: See “Possible feed rate input,” page 103  Tool radius compensation: See “Tool radius compensation,” page

183

 Miscellaneous functions (M): See “Miscellaneous Functions for

Program Run Control, Spindle and Coolant,” page 340

60 First Steps with the iTNC 530

Page 61

Create a cycle program

The holes (depth of 20 mm) shown in the figure at right are to be drilled with a standard drilling cycle. You have already defined the workpiece blank.

U Call the tool: Enter the tool data. Confirm each of your

entries with the ENT key. Do not forget the tool axis

U Retract the tool: Press the orange axis key Z in order

to get clear in the tool axis, and enter the value for the position to be approached, e.g. 250. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Activate the radius compensation

U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Confirm the Miscellaneous function M? with the

END key: The TNC saves the entered positioning block

U Call the cycle menu

U Display the drilling cycles

U Select the standard drilling cycle 200: The TNC starts

the dialog for cycle definition. Enter all parameters requested by the TNC step by step and conclude each entry with the ENT key. In the screen to the right, the TNC also displays a graphic showing the respective cycle parameter

100

9080

100

1.3 Programming the First Part

HEIDENHAIN iTNC 530 61

Page 62

U Call the menu for special functions

U Display the functions for point machining

U Select the pattern definition

U Select point entry: Enter the coordinates of the 4

points and confirm each with the ENT key. After entering the fourth point, save the block with the END key

U Display the menu for defining the cycle call

U Run the drilling cycle on the define pattern: U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Miscellaneous function M? Switch on the spindle and

coolant, e.g. M13. Confirm with the END key: The TNC saves the entered positioning block

U Retract the tool: Press the orange axis key Z in order

1.3 Programming the First Part

to get clear in the tool axis, and enter the value for the position to be approached, e.g. 250. Confirm with the ENT key

U Confirm Radius comp.: RL/RR/no comp? by pressing

the ENT key: Do not activate the radius compensation

U Confirm Feed rate F=? with the ENT key: Move at

rapid traverse (FMAX)

U Miscellaneous function M? Enter M2 to end the

program and confirm with the END key: The TNC saves the entered positioning block

62 First Steps with the iTNC 530

Page 63

Example NC blocks

0 BEGIN PGM C200 MM 1 BLK FORM 0.1 Z X+0 Y+0 Z-40 2 BLK FORM 0.2 X+100 Y+100 Z+0 3 TOOL CALL 5 Z S4500 4 L Z+250 R0 FMAX 5 PATTERN DEF

POS1 (X+10 Y+10 Z+0) POS2 (X+10 Y+90 Z+0) POS3 (X+90 Y+90 Z+0) POS4 (X+90 Y+10 Z+0)

6 CYCL DEF 200 DRILLING

Q200=2 ;SETUP CLEARANCE Q201=-20 ;DEPTH Q206=250 ;FEED RATE FOR PLNGN Q202=5 ;PLUNGING DEPTH Q210=0 ;DWELL TIME AT TOP Q203=-10 ;SURFACE COORDINATE Q204=20 ;2ND SET-UP CLEARANCE

Q211=0.2 ;DWELL TIME AT DEPTH 7 CYCL CALL PAT FMAX M13 8 L Z+250 R0 FMAX M2 9 END PGM C200 MM

Definition of workpiece blank

Tool call Retract the tool Defining Machining Positions

Define the cycle

1.3 Programming the First Part

Spindle and coolant on, call cycle Retract in the tool axis, end program

Further information on this topic

 Creating a new program: See “Creating and Writing Programs,”

page 99

 Cycle programming: See User’s Manual for Cycles

HEIDENHAIN iTNC 530 63

Page 64

1.4 Graphically Testing the Program

Select the correct operating mode

You can test programs only in the Test Run mode:

U Press the operating modes key: The TNC goes into

the Test Run mode

Further information on this topic

 Operating modes of the TNC: See “Operating Modes,” page 78  Testing programs: See “Test Run,” page 561

Select the tool table for the test run

You only need to execute this step is you have not activated a tool table in the Test Run mode.

U Press the PGM MGT key: the TNC displays the file

management

U Press the SELECT TYPE soft key: The TNC shows a

soft-key menu for selection of the file type to be

1.4 Graphically Testing the Program

displayed

U Press the SHOW ALL soft key: The TNC shows all

saved files in the right window

U Move the highlight to the left onto the directories

U Move the highlight to the TNC:\ directory

U Move the highlight to the right onto the files

U Move the highlight to the file TOOL.T (active tool

table) and load with the ENT key: TOOL.T receives that status S and is therefore active for the Test Run

U Press the END key: Leave the file manager

Further information on this topic

 Tool management: See “Entering tool data in the table,” page 162  Testing programs: See “Test Run,” page 561

64 First Steps with the iTNC 530

Page 65

Choose the program you want to test

U Press the PGM MGT key: the TNC displays the file

management

U Press the LAST FILES soft key: The TNC opens a pop-

up window with the most recently selected files

U Use the arrow keys to select the program that you

want to test. Load with the ENT key

Further information on this topic

 Selecting a program: See “Working with the File Manager,” page

113

Select the screen layout and the view

U Press the key for selecting the screen layout. The TNC

shows all available alternatives in the soft-key row

U Press the PROGRAM + GRAPHICS soft key: In the

left half of the screen the TNC shows the program; in the right half it shows the workpiece blank

U Select the desired view via soft key U Plan view

U Projection in three planes

1.4 Graphically Testing the Program

U 3-D view

Further information on this topic

 Graphic functions: See “Graphics,” page 550  Running a test run: See “Test Run,” page 561

HEIDENHAIN iTNC 530 65

Page 66

Start the program test

U Press the RESET + START soft key: The TNC

simulates the active program up to a programmed break or to the program end

U While the simulation is running you can use the soft

keys to change views

U Press the STOP soft key: The TNC interrupts the test

run

U Press the START soft key: The TNC resumes the test

run after a break

Further information on this topic

 Running a test run: See “Test Run,” page 561  Graphic functions: See “Graphics,” page 550  Adjusting the test speed:See “Setting the speed of the test run,”

page 551

1.4 Graphically Testing the Program

66 First Steps with the iTNC 530

Page 67

1.5 Setting Up Tools

Select the correct operating mode

Tools are set up in the Manual Operation mode:

U Press the operating modes key: The TNC goes into

the Manual Operation mode

Further information on this topic

 Operating modes of the TNC: See “Operating Modes,” page 78

Prepare and measure tools

U Clamp the required tools in their chucks U When measuring with an external tool presetter: Measure the tools,

note down the length and radius, or transfer them directly to the machine through a transfer program

U When measuring on the machine: Place the tools into the tool

changer (See page 68)

The tool table TOOL.T

In the tool table TOOL.T (permanently saved under TNC:\), save the tool data such as length and radius, but also further tool-specific information that the TNC needs to conduct its functions.

To enter tool data in the tool table TOOL.T, proceed as follows:

U Display the tool table U Edit the tool table: Set the EDITING soft key to ON U With the upward or downward arrow keys you can

select the tool number that you want to edit

U With the rightward or leftward arrow keys you can

select the tool data that you want to edit

U To leave the tool table, press the END key

Further information on this topic

 Operating modes of the TNC: See “Operating Modes,” page 78  Working with the tool table: See “Entering tool data in the table,”

page 162

1.5 Setting Up Tools

HEIDENHAIN iTNC 530 67

Page 68

The pocket table TOOL_P.TCH

The function of the pocket table depends on the machine. Your machine manual provides more detailed information.

In the pocket table TOOL_P.TCH (permanently saved under TNC:\) you specify which tools your tool magazine contains.

To enter data in the pocket table TOOL_P.TCH, proceed as follows:

U Display the tool table

1.5 Setting Up Tools

Further information on this topic

 Operating modes of the TNC: See “Operating Modes,” page 78  Working with the pocket table: See “Pocket table for tool changer,”

page 170

U Display the pocket table U Edit the pocket table: Set the EDITING soft key to ON U With the upward or downward arrow keys you can

select the pocket number that you want to edit

U With the rightward or leftward arrow keys you can

select the data that you want to edit

U To leave the pocket table, press the END key

68 First Steps with the iTNC 530

Page 69

1.6 Workpiece Setup

Select the correct operating mode

Workpieces are set up in the Manual Operation or Electronic Handwheel mode

U Press the operating modes key: The TNC goes into

the Manual Operation mode

Further information on this topic

 Manual mode: See “Moving the Machine Axes,” page 498

Clamp the workpiece

Mount the workpiece with a fixture on the machine table. If you have a 3-D touch probe on your machine, then you do not need to clamp the workpiece parallel to the axes.

If you do not have a 3-D touch probe available, you have to align the workpiece so that it is fixed with its edges parallel to the machine axes.

1.6 Workpiece Setup

HEIDENHAIN iTNC 530 69

Page 70

Align the workpiece with a 3-D touch probe system

U Insert the 3-D touch probe: In the Manual Data Input (MDI) operating

mode, run a TOOL CALL block containing the tool axis, and then return to the Manual Operation mode (in MDI mode you can run an individual NC block independently of the others)

U Select the probing functions: The TNC displays the

available functions in the soft-key row

U Measure the basic rotation: The NC displays the basic

rotation menu. To identify the basic rotation, probe two points on a straight surface of the workpiece

1.6 Workpiece Setup

U Use the axis-direction keys to pre-position the touch

probe to a position near the first contact point

U Select the probing direction via soft key U Press NC start: The touch probe moves in the defined

direction until it contacts the workpiece and then automatically returns to its starting point

U Use the axis-direction keys to pre-position the touch

probe to a position near the second contact point

U Press NC start: The touch probe moves in the defined

direction until it contacts the workpiece and then automatically returns to its starting point

U Then the TNC shows the measured basic rotation U Press the END key to close the menu and then

answer the question of whether the basic rotation should be transferred to the preset table by pressing the NO ENT key (no transfer)

Further information on this topic

 MDI operating mode:See “Programming and Executing Simple

Machining Operations,” page 544

 Workpiece alignment: See “Compensating Workpiece

Misalignment with a 3-D Touch Probe,” page 525

70 First Steps with the iTNC 530

Page 71

Set the datum with a 3-D touch probe

U Insert the 3-D touch probe: In the MDI mode, run a TOOL CALL block

containing the tool axis and then return to the Manual Operation mode

U Select the probing functions: The TNC displays the

available functions in the soft-key row

U Set the reference point at a tool corner, for example:

The TNC asks whether the prove points from the previously measured basic rotation should be loaded. Press the ENT key to load points

U Position the touch probe at a position near the first

touch point of the side that was not probed for basic rotation.

U Select the probing direction via soft key U Press NC start: The touch probe moves in the defined

direction until it contacts the workpiece and then automatically returns to its starting point

U Use the axis-direction keys to pre-position the touch

probe to a position near the second contact point

U Press NC start: The touch probe moves in the defined

direction until it contacts the workpiece and then automatically returns to its starting point

U Then the TNC shows the coordinates of the measured

corner point

U Set to 0: Press the SET DATUM soft key U Press the END to close the menu

1.6 Workpiece Setup

Further information on this topic

 Datum setting: See “Datum Setting with a 3-D Touch Probe,” page

527

HEIDENHAIN iTNC 530 71

Page 72

1.7 Running the First Program

Select the correct operating mode

You can run programs either in the Single Block or the Full Sequence mode:

U Press the operating mode key: The TNC goes into the

Program Run, Single Block mode and the TNC executes the program block by block. You have to confirm each block with the NC key

U Press the operating mode key: The TNC goes into the

Program Run, Full Sequence mode and the TNC executes the program after NC start up to a program break or to the end of the program

Further information on this topic

 Operating modes of the TNC: See “Operating Modes,” page 78  Running programs: See “Program Run,” page 566

1.7 Running the First Program

Choose the program you want to run

U Press the PGM MGT key: the TNC displays the file

management

U Press the LAST FILES soft key: The TNC opens a pop-

up window with the most recently selected files

U If desired, use the arrow keys to select the program

that you want to run. Load with the ENT key

Further information on this topic

 File management: See “Working with the File Manager,” page 113

Start the program

U Press the NC start button: The TNC executes the

active program

Further information on this topic

 Running programs: See “Program Run,” page 566

72 First Steps with the iTNC 530

Page 73

Introduction

Page 74

2.1 The iTNC 530

HEIDENHAIN TNC controls are workshop-oriented contouring controls that enable you to program conventional machining operations right at the machine in an easy-to-use conversational programming language. They are designed for milling, drilling and boring machines, as well as for machining centers. The iTNC 530 can control up to 12 axes. You can also change the angular position of the spindle under program control.

An integrated hard disk provides storage for as many programs as you like, even if they were created off-line. For quick calculations you can

2.1 The iTNC 530

call up the on-screen pocket calculator at any time. Keyboard and screen layout are clearly arranged in such a way that the

functions are fast and easy to use.

Programming: HEIDENHAIN conversational, smarT.NC and DIN/ISO formats

The HEIDENHAIN conversational programming format is an especially easy method of writing programs. Interactive graphics illustrate the individual machining steps for programming the contour. If a production drawing is not dimensioned for NC, the HEIDENHAIN FK free contour programming performs the necessary calculations automatically. Workpiece machining can be graphically simulated either during or before actual machining.

The smarT.NC operating mode offers TNC beginners an especially simple possibility to quickly and without much training create structured conversational dialog programs. Separate user documentation is available for smarT.NC.

It is also possible to program the TNCs in ISO format or DNC mode. You can also enter and test one program while the control is running

another.

Compatibility

The TNC can run all part programs that were written on HEIDENHAIN controls TNC 150 B and later. In as much as old TNC programs contain OEM cycles, the iTNC 530 must be adapted to them with the PC software CycleDesign. For more information, contact your machine tool builder or HEIDENHAIN.

74 Introduction

Page 75

2.2 Visual Display Unit and Keyboard

Visual display unit

The TNC is delivered with the BF 150 (TFT) color flat-panel display (see figure).

1 Header

When the TNC is on, the selected operating modes are shown in the screen header: the machining mode at the left and the programming mode at right. The currently active mode is displayed in the larger box, where the dialog prompts and TNC messages also appear (unless the TNC is showing only graphics).

2 Soft keys

In the footer the TNC indicates additional functions in a soft-key row. You can select these functions by pressing the keys immediately below them. The lines immediately above the softkey row indicate the number of soft-key rows that can be called with the black arrow keys to the right and left. The active soft-key row is indicated by brightened bar.

3 Soft-key selection keys 4 Shift between soft-key rows 5 Sets the screen layout 6 Shift key for switchover between machining and programming

modes

7 Soft-key selection keys for machine tool builders 8 Switches soft-key rows for machine tool builders

2.2 Visual Display Unit and Keyboard

HEIDENHAIN iTNC 530 75

Page 76

Sets the screen layout

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

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row shows the available layout options (see “Operating Modes,” page 78).

Select the desired screen layout.

2.2 Visual Display Unit and Keyboard

76 Introduction

Page 77

Operating panel

The TNC is delivered with the TE 530 keyboard unit. The figure shows the controls and displays of the TE 530 keyboard unit.

1 Alphabetic keyboard for entering texts and file names, and for ISO

programming. Dual-processor version: Additional keys for Windows operation

2  File management

 Calculator  MOD function  HELP function

3 Programming modes 4 Machine operating modes 5 Initiation of programming dialog 6 Arrow keys and GOTO jump command 7 Numerical input and axis selection 8 Touchpad: Only for operating the dual-processor version, soft

keys and smarT.NC

9 smarT.NC navigation keys

The functions of the individual keys are described on the inside front cover.

Some machine manufacturers do not use the standard operating panel from HEIDENHAIN. Please refer to your machine manual in these cases.

Machine panel buttons, e.g. NC START or NC STOP, are also described in the manual for your machine tool.

2.2 Visual Display Unit and Keyboard

HEIDENHAIN iTNC 530 77

Page 78

2.3 Operating Modes

Manual Operation and Electronic Handwheel

The Manual Operation mode is required for setting up the machine tool. In this mode of operation, you can position the machine axes manually or by increments, set the datums, and tilt the working plane.

The Electronic Handwheel mode of operation allows you to move the machine axes manually with the HR electronic handwheel.

Soft keys for selecting the screen layout (select as described previously)

Window Soft key

2.3 Operating Modes

Positions

Left: positions, right: status display

Left: positions, right: active collision objects (FCL4 function).

Positioning with Manual Data Input

This mode of operation is used for programming simple traversing movements, such as for face milling or pre-positioning.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program blocks, right: status display

Left: program blocks, right: active collision objects (FCL4 function). If this view is selected, then the TNC indicates a collision with a red frame around the graphics window.

78 Introduction

Page 79

Programming and Editing

In this mode of operation you can write your part programs. The FK free programming feature, the various cycles and the Q parameter functions help you with programming and add necessary information. If desired, the programming graphics or the 3-D line graphics (FCL 2 function) display the programmed traverse paths.

Soft keys for selecting the screen layout

Window Soft key

Program

Left: program blocks, right: program structure

Left: program blocks, right: graphics

Left: program blocks, right: 3-D line graphics

Test Run

In the Test Run mode of operation, the TNC checks programs and program sections for errors, such as geometrical incompatibilities, missing or incorrect data within the program or violations of the work space. This simulation is supported graphically in different display modes.

With the dynamic collision monitoring (DCM) software option you can test the program for potential collisions. As during program run, the TNC takes into account all permanent machine components defined by the machine manufacturer as well as all measured fixtures.

Soft keys for selecting the screen layout: see “Program Run, Full Sequence and Program Run, Single Block,” page 80.

2.3 Operating Modes

HEIDENHAIN iTNC 530 79

Page 80

Program Run, Full Sequence and Program Run, Single Block

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

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

Soft keys for selecting the screen layout

Window Soft key

Program

2.3 Operating Modes

Left: program, right: program structure

Left: program, right: status

Left: program, right: graphics

Graphics

Left: program blocks, right: active collision objects (FCL4 function). If this view is selected, then the TNC indicates a collision with a red frame around the graphics window.

Active collision objects (FCL4 function) If this view is selected, then the TNC indicates a collision with a red frame around the graphics window.

Soft keys for selecting the screen layout for pallet tables

Window Soft key

Pallet table

Left: program blocks, right: pallet table

Left: pallet table, right: status

Left: pallet table, right: graphics

80 Introduction

Page 81

2.4 Status Displays

“General” status display

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

 Program Run, Single Block and Program Run, Full Sequence, except

if the screen layout is set to display graphics only, and

 Positioning with Manual Data Input (MDI).

In the Manual mode and Electronic Handwheel mode the status display appears in the large window.

Information in the status display

Symbol Meaning ACTL.

Actual or nominal coordinates of the current position

2.4 Status Displays

X Y Z

F S M

Machine axes; the TNC displays auxiliary axes in lower-case letters. The sequence and quantity of displayed axes is determined by the machine tool builder. Refer to your machine manual for more information.

The displayed feed rate in inches corresponds to one tenth of the effective value. Spindle speed S, feed rate F and active M functions.

Program run started.

Axis is locked

Axis can be moved with the handwheel

Axes are moving under a basic rotation

Axes are moving in a tilted working plane

The M128 function or TCPM FUNCTION is active

The Dynamic Collision Monitoring function (DCM) is active

The Adaptive Feed Function (AFC) is active (software option)

HEIDENHAIN iTNC 530 81

Page 82

Symbol Meaning

One or more global program settings are active (software option)

Number of the active presets from the preset table. If the datum was set manually, the TNC displays the text MAN behind the symbol.

Additional status displays

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

2.4 Status Displays

Programming and Editing mode of operation.

To switch on the additional status display:

Call the soft-key row for screen layout.

Screen layout with additional status display: In the right half of the screen, the TNC shows the Overview status form.

To select an additional status display:

Shift the soft-key rows until the STATUS soft keys appear.

Either select the additional status display, e.g. positions and coordinates, or

use the soft keys to select the desired view.

With the soft keys or switch-over soft keys, you can choose directly between the available status displays.

Please note that some of the status information described below is not available unless the associated software option is enabled on your TNC.

82 Introduction

Page 83

Overview

After switch-on, the TNC displays the Overview status form, provided that you have selected the PROGRAM+STATUS screen layout (or POSITION + STATUS). The overview form contains a summary of the most important status information, which you can also find on the various detail forms.

Soft key Meaning

Position display in up to 5 axes

Tool information

Active M functions

Active coordinate transformations

Active subprogram

Active program section repeat

Program called with PGM CALL

Current machining time

Name of the active main program

General program information (PGM tab)

Soft key Meaning

No direct selection possible

Name of the active main program

Circle center CC (pole)

Dwell time counter

Machining time when the program was completely simulated in the Test Run operating mode

2.4 Status Displays

Current machining time in percent

Current time

Current/programmed contouring feed rate

Active programs

HEIDENHAIN iTNC 530 83

Page 84

General pallet information (PAL tab)

Soft key Meaning

No direct selection possible

Program section repeat/Subprograms (LBL tab)

Soft key Meaning

No direct selection possible

2.4 Status Displays

Information on standard cycles (CYC tab)

Soft key Meaning

No direct selection possible

Number of the active pallet preset

Active program section repeats with block number, label number, and number of programmed repeats/repeats yet to be run

Active subprogram numbers with block number in which the subprogram was called and the label number that was called

Active machining cycle

Active values of Cycle 32 Tolerance

84 Introduction

Page 85

Active miscellaneous functions M (M tab)

Soft key Meaning

No direct selection possible

List of the active M functions with fixed meaning

List of the active M functions that are adapted by your machine manufacturer

2.4 Status Displays

HEIDENHAIN iTNC 530 85

Page 86

Positions and coordinates (POS tab)

Soft key Meaning

Type of position display, e.g. actual position

Value traversed in virtual axis direction VT (only with “global program settings” software option)

Tilt angle of the working plane

Angle of a basic rotation

2.4 Status Displays

Information on tools (TOOL tab)

Soft key Meaning

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

Tool axis

Tool lengths and radii

Oversizes (delta values) from the tool table (TAB) and the TOOL CALL (PGM)

Tool life, maximum tool life (TIME 1) and maximum tool life for TOOL CALL (TIME 2)

Display of the active tool and the (next) replacement tool

86 Introduction

Page 87

Tool measurement (TT tab)

The TNC only displays the TT tab if the function is active on your machine.

Soft key Meaning

No direct selection possible

Number of the tool to be measured

Display whether the tool radius or the tool length is being measured

MIN and MAX values of the individual cutting edges and the result of measuring the rotating tool (DYN = dynamic measurement)

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

Coordinate transformations (TRANS tab)

Soft key Meaning

Name of the active datum table

Active datum number (#), comment from the active line of the active datum number (DOC) from Cycle 7

Active datum shift (Cycle 7); The TNC displays an active datum shift in up to 8 axes

Mirrored axes (Cycle 8)

Active basic rotation

2.4 Status Displays

Active rotation angle (Cycle 10)

Active scaling factor/factors (Cycles 11 / 26); The TNC displays an active scaling factor in up to 6 axes

Scaling datum

For further information, refer to the User's Manual for Cycles, "Coordinate Transformation Cycles."

HEIDENHAIN iTNC 530 87

Page 88

Global program settings 1 (GPS1 tab, software option)

The TNC only displays the tab if the function is active on your machine.

Soft key Meaning

No direct selection possible

Swapped axes

2.4 Status Displays

Superimposed datum shift

Superimposed mirroring

Global program settings 2 (GPS2 tab, software option)

The TNC only displays the tab if the function is active on your machine.

Soft key Meaning

No direct selection possible

Locked axes

Superimposed basic rotation

Superimposed rotation

Active feed rate factor

88 Introduction

Page 89

Adaptive Feed Control (AFC tab, software option)

The TNC only displays the AFC tab if the function is active on your machine.

Soft key Meaning

No direct selection possible

Active mode in which adaptive feed control is running

Active tool (number and name)

Cut number

Current factor of the feed potentiometer in percent

Active spindle load in percent

Reference load of the spindle

Current spindle speed

Current deviation of the speed

Current machining time

Line diagram, in which the current spindle load and the value commanded by the TNC for the feed-rate override are shown

2.4 Status Displays

HEIDENHAIN iTNC 530 89

Page 90

2.5 Window Manager

The machine tool builder determines the scope of function and behavior of the window manager. The machine tool manual provides further information.

The TNC features the XFCE window manager. XFCE is a standard application for UNIX-based operating systems, and is used to manage graphical user interfaces. The following functions are possible with the window manager:

 Display a taskbar for switching between various applications (user

interfaces).

 Manage an additional desktop, on which special applications from

2.5 Window Manager

your machine tool builder can run.

 Control the focus between NC-software applications and those of

the machine tool builder.

 The size and position of pop-up windows can be changed. It is also

possible to close, minimize and restore the pop-up windows.

The TNC shows a star in the upper left of the screen if an application of the window manager or the window manager itself has caused an error. In this case, switch to the window manager and correct the problem. If required, refer to your machine manual.

90 Introduction

Page 91

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

3-D touch probes

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

 Automatically align workpieces  Quickly and precisely set datums  Measure the workpiece during program run  Measure and inspect tools

All of the touch probe functions are described in the User’s Manual for Cycles. Please contact HEIDENHAIN if you require a copy of this User’s Manual. ID: 670 388-xx.

TS 220, TS 640 and TS 440 touch trigger probes

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

The TS 640 (see figure) and the smaller TS 440 feature infrared transmission of the triggering signal to the TNC. This makes them highly convenient for use on machines with automatic tool changers.

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

HEIDENHAIN iTNC 530 91

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

Page 92

TT 140 tool touch probe for tool measurement

The TT 140 is a triggering 3-D touch probe for tool measurement and inspection. Your TNC provides three cycles for this touch probe with which you can measure the tool length and radius automatically either with the spindle rotating or stopped. The TT 140 features a particularly rugged design and a high degree of protection, which make it insensitive to coolants and swarf. The triggering signal is generated by a wear-resistant and highly reliable optical switch.

HR electronic handwheels

Electronic handwheels facilitate moving the axis slides precisely by hand. A wide range of traverses per handwheel revolution is available. Apart from the HR 130 and HR 150 integral handwheels, HEIDENHAIN also offers the HR 410 and HR 420 portable handwheels. You will find a detailed description of HR 420 in Chapter 14 of this manual (see “HR 420 electronic handwheel” on page 501).

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

92 Introduction

Page 93

Programming: Fundamentals, File Management

Page 94

3.1 Fundamentals

Position encoders and reference marks

The machine axes are equipped with position encoders that register the positions of the machine table or tool. Linear axes are usually equipped with linear encoders, rotary tables and tilting axes with angle encoders.

When a machine axis moves, the corresponding position encoder generates an electrical signal. The TNC evaluates this signal and calculates the precise actual position of the machine axis.

3.1 Fundamentals

If there is a power interruption, the calculated position will no longer correspond to the actual position of the machine slide. To recover this association, incremental position encoders are provided with reference marks. The scales of the position encoders contain one or more reference marks that transmit a signal to the TNC when they are crossed over. From that signal the TNC can re-establish the assignment of displayed positions to machine positions. For linear encoders with distance-coded reference marks the machine axes need to move by no more than 20 mm, for angle encoders by no more than 20°.

With absolute encoders, an absolute position value is transmitted to the control immediately upon switch-on. In this way the assignment of the actual position to the machine slide position is re-established directly after switch-on.

X (Z,Y)

Reference system

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

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

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

94 Programming: Fundamentals, File Management

Page 95

Reference system on milling machines

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

The iTNC 530 can control up to 9 axes. The axes U, V and W are secondary linear axes parallel to the main axes X, Y and Z, respectively. Rotary axes are designated as A, B and C. The illustration at lower right shows the assignment of secondary axes and rotary axes to the main axes.

3.1 Fundamentals

V+

W+

C+

B+

A+

U+

HEIDENHAIN iTNC 530 95

Page 96

Polar coordinates

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

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

 Polar Radius, the distance from the circle center CC to the position,

3.1 Fundamentals

and the

 Polar Angle, the value of the angle between the reference axis and

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

Setting the pole and the angle reference axis

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

0°

Coordinates of the pole (plane)

X/Y +X

Y/Z +Y

Z/X +Z

Reference axis of the angle

96 Programming: Fundamentals, File Management

Page 97

Absolute and incremental workpiece positions

Absolute workpiece positions

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

Example 1: Holes dimensioned in absolute coordinates Hole 1 Hole 2 Hole 3

X = 10 mm X = 30 mm X = 50 mm Y = 10 mm Y = 20 mm Y = 30 mm

Incremental workpiece positions

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

To program a position in incremental coordinates, enter the function “I” before the axis.

Example 2: Holes dimensioned in incremental coordinates Absolute coordinates of hole 4 X = 10 mm

Y = 10 mm Hole 5, with respect to 4 Hole 6, with respect to 5

X = 20 mm X = 20 mm Y = 10 mm Y = 10 mm

Absolute and incremental polar coordinates

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

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

3.1 Fundamentals

10 30 50

10 10

+IPR

0°

+IPA

HEIDENHAIN iTNC 530 97

Page 98

Setting the datum

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

If the production drawing is dimensioned in relative coordinates, simply use the coordinate transformation cycles (see User’s Manual

3.1 Fundamentals

for Cycles, Cycles for Coordinate Transformation). If the production drawing is not dimensioned for NC, set the datum at

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

The fastest, easiest and most accurate way of setting the datum is by using a 3-D touch probe from HEIDENHAIN. See “Setting the Datum with a 3-D Touch Probe” in the Touch Probe Cycles User’s Manual.

Example

The workpiece drawing shows holes (1 to 4) whose dimensions are shown with respect to an absolute datum with the coordinates X=0 Y=0. Holes 5 to 7 are dimensioned with respect to a relative datum with the absolute coordinates X=450, Y=750. With the DATUM SHIFT cycle you can temporarily set the datum to the position X=450, Y=750, to be able to program holes 5 to 7 without further calculations.

750

320

MAX

MIN

150

6 5

-150

0,1 ±

300

3 4

325

450 900

950

98 Programming: Fundamentals, File Management

Page 99

3.2 Creating and Writing Programs

Organization of an NC program in HEIDENHAIN Conversational

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

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

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

 The workpiece blank  Tool calls  Approaching a safe position  Feed rates and spindle speeds, as well as  Path contours, cycles and other functions

The last block of a program is identified by END PGM the program name and the active unit of measure.

Block

10 L X+10 Y+5 R0 F100 M3

Path function

Block number

Words

Risk of collision!

After each tool call, HEIDENHAIN recommends always traversing to a safe position, from which the TNC can position the tool for machining without causing a collision!

Define the blank: BLK FORM

Immediately after initiating a new program, you define a cuboid workpiece blank. If you wish to define the blank at a later stage, press the SPEC FCT key and then the BLK FORM soft key. This definition is needed for the TNC’s graphic simulation feature. The sides of the workpiece blank lie parallel to the X, Y and Z axes and can be up to 100 000 mm long. The blank form is defined by two of its corner points:

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

entered as absolute values

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

entered as absolute or incremental values

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

3.2 Creating and Writing Programs

HEIDENHAIN iTNC 530 99

Page 100

Creating a new part program

You always enter a part program in the Programming and Editing mode of operation. An example of program initiation:

Select the Programming and Editing operating mode.

Press the PGM MGT key to call the file manager.

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

FILE NAME = OLD.H

Enter the new program name and confirm your entry with the ENT key.

To select the unit of measure, press the MM or INCH soft key. The TNC switches the screen layout and

3.2 Creating and Writing Programs

WORKING SPINDLE AXIS X/Y/Z?

initiates the dialog for defining the BLK FORM (workpiece blank).

Enter spindle axis, e.g. Z

DEF BLK FORM: MIN CORNER?

Enter in sequence the X, Y and Z coordinates of the MIN point and confirm each of your entries with the ENT key.

DEF BLK FORM: MAX CORNER?

Enter in sequence the X, Y and Z coordinates of the MAX point and confirm each of your entries with the ENT key.

100 Programming: Fundamentals, File Management

HEIDENHAIN iTNC 530 User Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Controls of the TNC

Keys on visual display unit

Alphanumeric keyboard

Machine operating modes

Program/file management, TNC functions

Navigation keys

Potentiometer for feed rate and spindle speed

Programming modes

Cycles, subprograms and program section repeats

Tool functions

Coordinate axes and numbers: Entering and editing

Programming path movements

Special functions / smarT.NC

About this Manual

Do you desire any changes, or have you found any errors?

TNC Model, Software and Features

Software options

Feature content level (upgrade functions)

Intended place of operation

Legal information

New functions in 340 49x-01 since the predecessor versions 340 422-xx/340 423-xx

New functions with 340 49x-02

New functions with 340 49x-03

New functions with 340 49x-04

New functions with 340 49x-05

Changed functions in 340 49x-01 since the predecessor versions 340 422-xx/340 423-xx

Functions changed in 340 49x-02

Changed functions with 340 49x-03

Changed functions with 340 49x-04

Changed functions with 340 49x-05

First Steps with the iTNC 530

1.1 Overview

Acknowledge the power interruption and move to the reference points

1.2 Machine Switch-On

Select the correct operating mode

The most important TNC keys

1.3 Programming the First Part

Create a new program/file management

Define a workpiece blank

Program layout

Program a simple contour

Create a cycle program

Select the correct operating mode

Select the tool table for the test run

1.4 Graphically Testing the Program

Choose the program you want to test

Select the screen layout and the view

Start the program test

Select the correct operating mode

Prepare and measure tools

The tool table TOOL.T

1.5 Setting Up Tools

The pocket table TOOL_P.TCH

Select the correct operating mode

Clamp the workpiece

1.6 Workpiece Setup

Align the workpiece with a 3-D touch probe system

Set the datum with a 3-D touch probe

Select the correct operating mode

1.7 Running the First Program

Choose the program you want to run

Start the program

Introduction

2.1 The iTNC 530

Programming: HEIDENHAIN conversational, smarT.NC and DIN/ISO formats

Compatibility

Visual display unit

2.2 Visual Display Unit and Keyboard

Sets the screen layout

Operating panel

Manual Operation and Electronic Handwheel

2.3 Operating Modes

Positioning with Manual Data Input

Programming and Editing

Test Run

Program Run, Full Sequence and Program Run, Single Block