HEIDENHAIN TNC 640 User Manual

Page 1

TNC 640

User's Manual
HEIDENHAIN Conversational Programming
NC Software 340590-02 340591-02 340594-02
English (en) 5/2013
Page 2

Controls of the TNC

Controls of the TNC

Keys on visual display unit

Key Function
Select split screen layout
Toggle the display between machining and programming modes
Soft keys for selecting functions on screen
Shifting between soft-key rows

Alphanumeric keyboard

Key Function
File names, comments
DIN/ISO programming

Programming modes

Key Function
Programming
Test run

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

Machine operating modes

Key Function
Manual operation
Electronic handwheel
Positioning with manual data input
Program run, single block
Program run, full sequence
Show 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
2
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 3

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
Enter program stop in a program

Tool functions

Key Function
Define tool data in the program
Call tool data

Special functions

Key Function
Show special functions
Select the next tab in forms
Up/down one dialog box or button

Entering and editing coordinate axes and numbers

Key Function
Select coordinate axes or enter
. . . .
. . . .
them in a program
Numbers
Decimal point / Reverse algebraic sign

Programming path movements

Key Function
Approach/depart contour
FK free contour programming
Straight line
Circle center/pole for polar coordinates
Circular arc with center
Circle with radius
Circular arc with tangential connection
Chamfer/Corner rounding
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
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
3
Page 4
Controls of the TNC
4
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 5

Fundamentals

Page 6
Fundamentals

About this manual

About this manual
The symbols used in this manual are described below.
This symbol indicates that important notes about the function described must be regarded.
This symbol indicates that there is one or more of the following risks when using the described function:
Danger to workpiece Danger to fixtures Danger to tool Danger to machine Danger to operator
This symbol indicates a possibly dangerous situation that may cause light injuries if not avoided.
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.

Would you like any changes, or have you found any errors?

We are continuously striving to improve our documentation for you. Please help us by sending your requests to the following e-mail address: tnc-userdoc@heidenhain.de.
6
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 7

TNC model, software and features

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
TNC 640 340590-02 TNC 640 E 340591-02 TNC 640 Programming Station 340594-02
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 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 Cycle Programming:
All of the cycle functions (touch probe cycles and fixed cycles) are described in the Cycle Programming User’s Manual. Please contact HEIDENHAIN if you require a copy of this User’s Manual. ID: 892905-xx
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
7
Page 8
Fundamentals
TNC model, software and features

Software options

The TNC 640 features various software options that can be enabled by your machine tool builder. Each option is to be enabled separately and contains the following respective functions:
Hardware, options
1st additional axis for 4 axes plus spindle
2nd additional axis for 5 axes plus spindle
Software option 1 (option number 08) Rotary table machining
Coordinate transformation Interpolation
Software option 2 (option number 09) 3-D machining
Interpolation
HEIDENHAIN DNC (option number 18)
Display step (Option number 23)
step
Programming of cylindrical contours as if in two axes Feed rate in distance per minute Working plane, tilting the ... Circle in 3 axes with tilted working plane (spacial arc)
Motion control with minimum jerk 3-D tool compensation through surface normal vectors Using the electronic handwheel to change the angle of the swivel head
during program run without affecting the position of the tool point. (TCPM = Tool Center Point Management)
Keeping the tool normal to the contour Tool radius compensation perpendicular to traversing and tool direction Linear in 5 axes (subject to export permit)
Communication with external PC applications over COM component
Linear axes to 0.01 µmInput resolution and display Rotary axes to 0.00001°
Dynamic Collision Monitoring (DCM) software option (option number 40) Collision monitoring in all
machine operating modes
Software option for additional conversational languages (option number 41) Additional conversational
languages
8
The machine manufacturer defines objects to be monitored
Three warning levels in manual operation
Program interrupt during automatic operation
Includes monitoring of 5-axis movements
Slovenian
Norwegian
Slovak
Latvian
Korean
Estonian
Turkish
Romanian
Lithuanian
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 9
TNC model, software and features
DXF Converter software option (option number 42) Extracting contour
programs and machining positions from DXF data. Extracting contour sections from plain-language programs.
Adaptive Feed Control (AFC) software option (option number 45) Function for adaptive feed-
rate control for optimizing the machining conditions during series production
KinematicsOpt software option (option number 48) Touch-probe cycles for
automatic testing and optimization of the machine kinematics
Mill-Turning software option (option number 50) Functions for milling/turning
mode
Supported DXF format: AC1009 (AutoCAD R12)
For contours and point patterns
Simple and convenient specification of reference points
Select graphical features of contour sections from conversational
programs
Recording the actual spindle power by means of a teach-in cut
Defining the limits of automatic feed rate control
Fully automatic feed control during program run
Backup/restore active kinematics
Test active kinematics
Optimize active kinematics
Switching between Milling/Turning mode of operation
Constant cutting speed
Tool-tip radius compensation
Turning cycles
Extended Tool Managment software option (option number 93)
Extended tool management, python-based
Remote Desktop Manager software option (option number 133)
Windows on a separate computer unitRemote operation of
external computer units (e.g. Windows PC) via the TNC user interface
Incorporated in the TNC interface
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
9
Page 10
Fundamentals
Cross Talk Compensation (CTC) software option (option number 141)
TNC model, software and features
Compensation of axis couplings
Position Adaptive Control (PAC) software option (option number 142) Changing control
parameters
Load Adaptive Control (LAC) software option (option number 143)
parameters
Active Chatter Control (ACC) software option (option number 145)
Fully automatic function for chatter control during machining
Determination of dynamically caused position deviation through axis
acceleration Compensation of the TCP
Changing of the control parameters depending on the position of the
axes in the working space Changing of the control parameters depending on the speed or
acceleration of an axis
Automatic determination of workpiece weight and frictional forcesDynamic changing of control
Continuous adaptation of the parameters of the adaptive precontrolling
to the actual weight of the workpiece during machining
10
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 11
TNC model, software and features

Feature Content Level (upgrade functions)

Along with software options, significant further improvements of the TNC software are managed via the Feature Content Level 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.

Intended place of operation

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.

Legal information

This product uses open source software. Further information is available on the control under
Programming and Editing operating mode MOD function LICENSE INFO soft key
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
11
Page 12
Fundamentals
TNC model, software and features

New functions

New functions 34059x-02
DXF files can be opened directly on the TNC in order to extract contours and point patterns (Programming: Data transfer from DXF files or plain-language contours, page 243).
The active tool-axis direction can now be activated in manual mode and during handwheel superimposition as a virtual tool axis (Superimposing handwheel positioning during program run: M118 , page 360).
The machine manufacturer can now define any areas on the machine for collision monitoring (Dynamic Collision Monitoring (software option), page 371).
Writing and reading data in freely definable tables (Freely definable tables, page 402).
The Adaptive Feed Control (AFC) function has been integrated (Adaptive Feed Control Software Option (AFC), page 377)
New touch probe cycle 484 for calibrating the wireless TT 449 tool touch probe (see User's Manual for Cycles).
The new HR 520 and HR 550 FS handwheels are supported (Traverse with electronic handwheels, page 490).
New machining cycle 225 ENGRAVING (see User’s Manual for Cycle Programming)
New Active Chatter Control (ACC) software option (Active Chatter Control (ACC; software option), page 389).
New manual probing cycle "Center line as datum" (Setting a center line as datum , page 535).
New function for rounding corners (Rounding corners: M197, page 366).
External access to the TNC can now be blocked with a MOD function (External access, page 584).
12
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 13
TNC model, software and features
Modified functions 34059x-02
The maximum number of characters for the NAME and DOC fields in the tool table has been increased from 16 to 32 (Enter tool data into the table, page 160).
The columns AFC and ACC were added to the tool table (Enter tool data into the table, page 160).
Operation and position behavior of the manual probing cycles has been improved (Using 3-D touch probes , page 514).
Predefined values can now be entered into a cycle parameter with the PREDEF function in cycles (see User’s Manual for Cycle Programming).
The status display has been expanded with the AFC tab (Additional status displays, page 76).
The FUNCTION TURNDATA SPIN rotational function has been expanded with an input option for maximum speed (Program spindle speed, page 464).
A new optimization algorithm is now used with the KinematicsOpt cycles (see User’s Manual for Cycle Programming).
With Cycle 257, circular stud milling, a parameter is now available with which you can determine the approach position on the stud (see User's Manual for Cycle Programming)
With Cycle 256, rectangular stud, a parameter is now available with which you can determine the approach position on the stud (see User's Manual for Cycle Programming).
With the "Basic Rotation" probing cycle, workpiece misalignment can now be compensated for via a table rotation (Compensation of workpiece misalignment by rotating the table, page 528)
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
13
Page 14
Fundamentals
TNC model, software and features
14
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 15

Contents

1 First Steps with the TNC 640......................................................................................................... 47
2 Introduction.......................................................................................................................................69
3 Programming: Fundamentals, file management...........................................................................89
4 Programming: Programming aids................................................................................................ 131
5 Programming: Tools....................................................................................................................... 155
6 Programming: Programming contours........................................................................................ 191
7 Programming: Data transfer from DXF files or plain-language contours................................. 243
8 Programming: Subprograms and program section repeats...................................................... 261
9 Programming: Q Parameters.........................................................................................................277
10 Programming: Miscellaneous functions.......................................................................................347
11 Programming: Special functions.................................................................................................. 367
12 Programming: Multiple Axis Machining...................................................................................... 409
13 Programming: Pallet editor........................................................................................................... 453
14 Programming: Turning Operations............................................................................................... 459
15 Manual operation and setup.........................................................................................................485
16 Positioning with Manual Data Input............................................................................................ 547
17 Test run and program run............................................................................................................. 553
18 MOD functions................................................................................................................................581
19 Tables and overviews.....................................................................................................................605
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
15
Page 16
Contents
16
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 17
1 First Steps with the TNC 640......................................................................................................... 47
1.1 Overview................................................................................................................................................. 48
1.2 Machine switch-on.................................................................................................................................48
Acknowledging the power interruption and moving to the reference points...........................................48
1.3 Programming the first part...................................................................................................................49
Selecting the correct operating mode..................................................................................................... 49
The most important TNC keys.................................................................................................................49
Creating a new program/file management.............................................................................................. 50
Defining a workpiece blank......................................................................................................................51
Program layout......................................................................................................................................... 52
Programming a simple contour................................................................................................................53
Creating a cycle program......................................................................................................................... 56
1.4 Graphically testing the first part..........................................................................................................58
Selecting the correct operating mode..................................................................................................... 58
Selecting the tool table for the test run..................................................................................................58
Choosing the program you want to test................................................................................................. 59
Selecting the screen layout and the view............................................................................................... 59
Starting the test run.................................................................................................................................60
1.5 Setting up tools..................................................................................................................................... 61
Selecting the correct operating mode..................................................................................................... 61
Preparing and measuring tools................................................................................................................ 61
The tool table TOOL.T............................................................................................................................. 62
The pocket table TOOL_P.TCH.................................................................................................................63
1.6 Workpiece setup.....................................................................................................................................64
Selecting the correct operating mode..................................................................................................... 64
Clamping the workpiece.......................................................................................................................... 64
Workpiece alignment with 3-D touch probe............................................................................................ 65
Datum setting with 3-D touch probe....................................................................................................... 66
1.7 Running the first program.................................................................................................................... 67
Selecting the correct operating mode..................................................................................................... 67
Choosing the program you want to run.................................................................................................. 67
Start the program.....................................................................................................................................67
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
17
Page 18
Contents
2 Introduction.......................................................................................................................................69
2.1 The TNC 640........................................................................................................................................... 70
Programming: HEIDENHAIN conversational and ISO formats.................................................................70
Compatibility.............................................................................................................................................70
2.2 Visual display unit and operating panel..............................................................................................71
Display screen..........................................................................................................................................71
Setting the screen layout.........................................................................................................................71
Control Panel............................................................................................................................................72
2.3 Modes of Operation...............................................................................................................................73
Manual Operation and El. Handwheel.....................................................................................................73
Positioning with Manual Data Input.........................................................................................................73
Programming............................................................................................................................................ 73
Test Run................................................................................................................................................... 74
Program Run, Full Sequence and Program Run, Single Block.................................................................74
2.4 Status displays....................................................................................................................................... 75
"General" status display............................................................................................................................75
Additional status displays.........................................................................................................................76
2.5 Window Manager...................................................................................................................................83
Task bar.................................................................................................................................................... 84
2.6 SELinux security software.....................................................................................................................85
2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels.......................................86
3-D touch probes..................................................................................................................................... 86
HR electronic handwheels....................................................................................................................... 87
18
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 19
3 Programming: Fundamentals, file management...........................................................................89
3.1 Fundamentals......................................................................................................................................... 90
Position encoders and reference marks.................................................................................................. 90
Reference system.................................................................................................................................... 90
Reference system on milling machines...................................................................................................91
Designation of the axes on milling machines..........................................................................................91
Polar coordinates...................................................................................................................................... 92
Absolute and incremental workpiece positions....................................................................................... 93
Selecting the datum.................................................................................................................................94
3.2 Opening programs and entering.......................................................................................................... 95
Organization of an NC program in HEIDENHAIN Conversational format.................................................95
Define the blank: BLK FORM.................................................................................................................. 95
Opening a new part program.................................................................................................................. 96
Programming tool movements in conversational.....................................................................................97
Actual position capture.............................................................................................................................99
Editing a program...................................................................................................................................100
The TNC search function....................................................................................................................... 103
3.3 File manager: Fundamentals...............................................................................................................105
Files........................................................................................................................................................ 105
Displaying externally generated files on the TNC..................................................................................107
Data Backup........................................................................................................................................... 107
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
19
Page 20
Contents
3.4 Working with the file manager.......................................................................................................... 108
Directories.............................................................................................................................................. 108
Paths.......................................................................................................................................................108
Overview: Functions of the file manager.............................................................................................. 109
Calling the file manager......................................................................................................................... 110
Selecting drives, directories and files....................................................................................................111
Creating a new directory....................................................................................................................... 112
Creating a new file.................................................................................................................................112
Copying a single file...............................................................................................................................112
Copying files into another directory.......................................................................................................113
Copying a table...................................................................................................................................... 114
Copying a directory................................................................................................................................ 115
Choosing one of the last files selected.................................................................................................115
Deleting a file.........................................................................................................................................116
Deleting a directory................................................................................................................................116
Tagging files........................................................................................................................................... 117
Renaming a file...................................................................................................................................... 118
Sorting files............................................................................................................................................ 118
Additional functions................................................................................................................................119
Additional tools for management of external file types.........................................................................120
Data transfer to/from an external data medium.................................................................................... 125
The TNC in a network............................................................................................................................127
USB devices on the TNC.......................................................................................................................128
20
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 21
4 Programming: Programming aids................................................................................................ 131
4.1 Adding comments................................................................................................................................132
Application.............................................................................................................................................. 132
Entering comments during programming..............................................................................................132
Inserting comments after program entry.............................................................................................. 132
Entering a comment in a separate block...............................................................................................132
Functions for editing of the comment...................................................................................................133
4.2 Display of NC Programs...................................................................................................................... 134
Syntax highlighting................................................................................................................................. 134
Scrollbar..................................................................................................................................................134
4.3 Structuring programs...........................................................................................................................135
Definition and applications..................................................................................................................... 135
Displaying the program structure window / Changing the active window.............................................135
Inserting a structuring block in the (left) program window.................................................................... 135
Selecting blocks in the program structure window............................................................................... 135
4.4 Calculator.............................................................................................................................................. 136
Operation................................................................................................................................................136
4.5 Programming graphics........................................................................................................................ 138
Generating / not generating graphics during programming................................................................... 138
Generating a graphic for an existing program....................................................................................... 138
Block number display ON/OFF...............................................................................................................139
Erasing the graphic................................................................................................................................ 139
Showing grid lines..................................................................................................................................139
Magnification or reduction of details..................................................................................................... 140
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
21
Page 22
Contents
4.6 Error messages..................................................................................................................................... 141
Display of errors.....................................................................................................................................141
Open the error window......................................................................................................................... 141
Closing the error window...................................................................................................................... 141
Detailed error messages........................................................................................................................142
INTERNAL INFO soft key.......................................................................................................................142
Clearing errors........................................................................................................................................143
Error log..................................................................................................................................................143
Keystroke log..........................................................................................................................................144
Informational texts................................................................................................................................. 145
Saving service files................................................................................................................................ 145
Calling the TNCguide help system........................................................................................................ 146
4.7 TNCguide context-sensitive help system..........................................................................................147
Application.............................................................................................................................................. 147
Working with the TNCguide.................................................................................................................. 148
Downloading current help files.............................................................................................................. 152
22
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 23
5 Programming: Tools....................................................................................................................... 155
5.1 Entering tool-related data................................................................................................................... 156
Feed rate F.............................................................................................................................................156
Spindle speed S..................................................................................................................................... 157
5.2 Tool data................................................................................................................................................158
Requirements for tool compensation.................................................................................................... 158
Tool number, tool name......................................................................................................................... 158
Tool length L.......................................................................................................................................... 158
Tool radius R.......................................................................................................................................... 158
Delta values for lengths and radii.......................................................................................................... 159
Entering tool data into the program...................................................................................................... 159
Enter tool data into the table.................................................................................................................160
Importing tool tables..............................................................................................................................169
Pocket table for tool changer.................................................................................................................170
Call tool data.......................................................................................................................................... 173
Tool change............................................................................................................................................ 175
Tool usage test.......................................................................................................................................178
Tool management (software option)...................................................................................................... 180
5.3 Tool compensation............................................................................................................................... 187
Introduction.............................................................................................................................................187
Tool length compensation...................................................................................................................... 187
Tool radius compensation...................................................................................................................... 188
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
23
Page 24
Contents
6 Programming: Programming contours........................................................................................ 191
6.1 Tool movements................................................................................................................................... 192
Path functions........................................................................................................................................ 192
FK free contour programming................................................................................................................192
Miscellaneous functions M....................................................................................................................192
Subprograms and program section repeats.......................................................................................... 193
Programming with Q parameters.......................................................................................................... 193
6.2 Fundamentals of Path Functions........................................................................................................194
Programming tool movements for workpiece machining......................................................................194
6.3 Approaching and departing a contour...............................................................................................198
Overview: Types of paths for contour approach and departure.............................................................198
Important positions for approach and departure....................................................................................199
Approaching on a straight line with tangential connection: APPR LT.................................................... 201
Approaching on a straight line perpendicular to the first contour point: APPR LN................................ 201
Approaching on a circular path with tangential connection: APPR CT...................................................202
Approaching on a circular path with tangential connection from a straight line to the contour: APPR
LCT......................................................................................................................................................... 203
Departing in a straight line with tangential connection: DEP LT........................................................... 204
Departing in a straight line perpendicular to the last contour point: DEP LN........................................ 204
Departing on a circular path with tangential connection: DEP CT.........................................................205
Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT...............205
6.4 Path contours - Cartesian coordinates...............................................................................................206
Overview of path functions................................................................................................................... 206
Straight line L.........................................................................................................................................207
Inserting a chamfer between two straight lines....................................................................................208
Corner rounding RND.............................................................................................................................209
24
Circle center CC..................................................................................................................................... 210
Circular path C around circle center CC................................................................................................ 211
Circle CR with defined radius................................................................................................................ 212
Circle CT with tangential connection.....................................................................................................214
Example: Linear movements and chamfers with Cartesian coordinates............................................... 215
Example: Circular movements with Cartesian coordinates................................................................... 216
Example: Full circle with Cartesian coordinates.................................................................................... 217
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Page 25
6.5 Path contours – Polar coordinates..................................................................................................... 218
Overview................................................................................................................................................ 218
Zero point for polar coordinates: pole CC..............................................................................................219
Straight line LP.......................................................................................................................................219
Circular path CP around pole CC........................................................................................................... 220
Circle CTP with tangential connection...................................................................................................220
Helix........................................................................................................................................................221
Example: Linear movement with polar coordinates.............................................................................. 223
Example: Helix........................................................................................................................................224
6.6 Path contours – FK free contour programming................................................................................ 225
Fundamentals......................................................................................................................................... 225
FK programming graphics...................................................................................................................... 227
Initiating the FK dialog........................................................................................................................... 229
Pole for FK programming....................................................................................................................... 229
Free straight line programming..............................................................................................................230
Free circular path programming............................................................................................................. 231
Input options.......................................................................................................................................... 232
Auxiliary points....................................................................................................................................... 235
Relative data...........................................................................................................................................236
Example: FK programming 1................................................................................................................. 238
Example: FK programming 2................................................................................................................. 239
Example: FK programming 3................................................................................................................. 240
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
25
Page 26
Contents
7 Programming: Data transfer from DXF files or plain-language contours................................. 243
7.1 Processing DXF Files (Software Option)........................................................................................... 244
Application.............................................................................................................................................. 244
Opening a DXF file.................................................................................................................................245
Working with the DXF converter...........................................................................................................245
Basic settings.........................................................................................................................................246
Setting layers..........................................................................................................................................248
Defining the datum................................................................................................................................ 249
Selecting and saving a contour..............................................................................................................251
Selecting and saving machining positions............................................................................................. 255
26
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 27
8 Programming: Subprograms and program section repeats...................................................... 261
8.1 Labeling Subprograms and Program Section Repeats.................................................................... 262
Label....................................................................................................................................................... 262
8.2 Subprograms........................................................................................................................................ 263
Operating sequence...............................................................................................................................263
Programming notes................................................................................................................................263
Programming a subprogram...................................................................................................................263
Calling a subprogram............................................................................................................................. 264
8.3 Program-section repeats..................................................................................................................... 265
Label LBL............................................................................................................................................... 265
Operating sequence...............................................................................................................................265
Programming notes................................................................................................................................265
Programming a program section repeat................................................................................................ 265
Calling a program section repeat...........................................................................................................266
8.4 Any desired program as subprogram................................................................................................ 267
Operating sequence...............................................................................................................................267
Programming notes................................................................................................................................267
Calling any program as a subprogram................................................................................................... 268
8.5 Nesting.................................................................................................................................................. 269
Types of nesting.....................................................................................................................................269
Nesting depth.........................................................................................................................................269
Subprogram within a subprogram......................................................................................................... 270
Repeating program section repeats.......................................................................................................271
Repeating a subprogram........................................................................................................................272
8.6 Programming examples.......................................................................................................................273
Example: Milling a contour in several infeeds.......................................................................................273
Example: Groups of holes..................................................................................................................... 274
Example: Group of holes with several tools..........................................................................................275
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
27
Page 28
Contents
9 Programming: Q Parameters.........................................................................................................277
9.1 Principle and overview of functions.................................................................................................. 278
Programming notes................................................................................................................................279
Calling Q parameter functions............................................................................................................... 280
9.2 Part families—Q parameters in place of numerical values.............................................................. 281
Application.............................................................................................................................................. 281
9.3 Describing contours with mathematical functions.......................................................................... 282
Application.............................................................................................................................................. 282
Overview................................................................................................................................................ 282
Programming fundamental operations...................................................................................................283
9.4 Angle functions (trigonometry)..........................................................................................................284
Definitions...............................................................................................................................................284
Programming trigonometric functions................................................................................................... 284
9.5 Calculation of circles............................................................................................................................285
Application.............................................................................................................................................. 285
9.6 If-then decisions with Q parameters................................................................................................. 286
Application.............................................................................................................................................. 286
Unconditional jumps...............................................................................................................................286
Programming if-then decisions.............................................................................................................. 286
Abbreviations used:................................................................................................................................287
9.7 Checking and changing Q parameters...............................................................................................288
Procedure............................................................................................................................................... 288
9.8 Additional functions.............................................................................................................................290
Overview................................................................................................................................................ 290
FN 14: ERROR: Displaying error messages...........................................................................................291
FN 16: F-PRINT: Output of formatted texts and Q parameter values.....................................................295
FN 18: SYS-DATUM READ: Reading system data................................................................................. 299
FN 19: PLC: Transfer values to PLC...................................................................................................... 308
FN 20: WAIT FOR: NC and PLC synchronization.................................................................................. 308
FN 29: PLC: Transfer values to the PLC................................................................................................310
FN 37: EXPORT......................................................................................................................................310
28
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 29
9.9 Accessing tables with SQL commands............................................................................................. 311
Introduction.............................................................................................................................................311
A transaction.......................................................................................................................................... 312
Programming SQL commands...............................................................................................................314
Overview of the soft keys..................................................................................................................... 314
SQL BIND...............................................................................................................................................315
SQL SELECT.......................................................................................................................................... 316
SQL FETCH............................................................................................................................................ 318
SQL UPDATE..........................................................................................................................................319
SQL INSERT...........................................................................................................................................319
SQL COMMIT........................................................................................................................................ 320
SQL ROLLBACK..................................................................................................................................... 320
9.10 Entering formulas directly...................................................................................................................321
Entering formulas...................................................................................................................................321
Rules for formulas..................................................................................................................................323
Programming example........................................................................................................................... 324
9.11 String parameters................................................................................................................................ 325
String processing functions................................................................................................................... 325
Assigning string parameters.................................................................................................................. 326
Chain-linking string parameters..............................................................................................................326
Converting a numerical value to a string parameter..............................................................................327
Copying a substring from a string parameter........................................................................................328
Converting a string parameter to a numerical value..............................................................................329
Checking a string parameter..................................................................................................................330
Finding the length of a string parameter...............................................................................................331
Comparing alphabetic sequence............................................................................................................332
Reading machine parameters.................................................................................................................333
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
29
Page 30
Contents
9.12 Preassigned Q parameters.................................................................................................................. 336
Values from the PLC: Q100 to Q107.....................................................................................................336
Active tool radius: Q108.........................................................................................................................336
Tool axis: Q109.......................................................................................................................................336
Spindle status: Q110.............................................................................................................................. 337
Coolant on/off: Q111...............................................................................................................................337
Overlap factor: Q112.............................................................................................................................. 337
Unit of measurement for dimensions in the program: Q113.................................................................337
Tool length: Q114................................................................................................................................... 337
Coordinates after probing during program run.......................................................................................338
Deviation between actual value and nominal value during automatic tool measurement with the TT
130..........................................................................................................................................................338
Tilting the working plane with mathematical angles: rotary axis coordinates calculated by the TNC.....338
Measurement results from touch probe cycles (see also User’s Manual for Cycle Programming)........339
9.13 Programming examples.......................................................................................................................341
Example: Ellipse..................................................................................................................................... 341
Example: Concave cylinder machined with spherical cutter..................................................................343
Example: Convex sphere machined with end mill.................................................................................345
30
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 31
10 Programming: Miscellaneous functions.......................................................................................347
10.1 Entering miscellaneous functions M and STOP................................................................................348
Fundamentals......................................................................................................................................... 348
10.2 M functions for program run inspection, spindle and coolant........................................................349
Overview................................................................................................................................................ 349
10.3 Miscellaneous functions for coordinate data....................................................................................350
Programming machine-referenced coordinates: M91/M92....................................................................350
Moving to positions in a non-tilted coordinate system with a tilted working plane: M130.................... 352
10.4 Miscellaneous functions for path behavior.......................................................................................353
Machining small contour steps: M97.................................................................................................... 353
Machining open contour corners: M98..................................................................................................354
Feed rate factor for plunging movements: M103..................................................................................355
Feed rate in millimeters per spindle revolution: M136..........................................................................356
Feed rate for circular arcs: M109/M110/M111........................................................................................357
Calculating the radius-compensated path in advance (LOOK AHEAD): M120.......................................358
Superimposing handwheel positioning during program run: M118....................................................... 360
Retraction from the contour in the tool-axis direction: M140................................................................362
Suppressing touch probe monitoring: M141......................................................................................... 363
Deleting basic rotation: M143................................................................................................................364
Automatically retract tool from the contour at an NC stop: M148........................................................ 365
Rounding corners: M197........................................................................................................................366
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
31
Page 32
Contents
11 Programming: Special functions.................................................................................................. 367
11.1 Overview of special functions............................................................................................................ 368
Main menu for SPEC FCT special functions......................................................................................... 368
Program defaults menu..........................................................................................................................369
Functions for contour and point machining menu................................................................................. 369
Menu of various conversational functions............................................................................................. 370
11.2 Dynamic Collision Monitoring (software option)..............................................................................371
Function..................................................................................................................................................371
Collision monitoring in the manual operating modes............................................................................ 373
Collision monitoring in Automatic operation.......................................................................................... 375
Graphic depiction of the protected space............................................................................................. 376
11.3 Adaptive Feed Control Software Option (AFC).................................................................................377
Application.............................................................................................................................................. 377
Defining the AFC basic settings............................................................................................................ 379
Recording a teach-in cut........................................................................................................................ 382
Activating/deactivating AFC....................................................................................................................385
Log file....................................................................................................................................................386
Tool breakage/tool wear monitoring.......................................................................................................387
Spindle load monitoring......................................................................................................................... 388
11.4 Active Chatter Control (ACC; software option).................................................................................389
Application.............................................................................................................................................. 389
Activating/deactivating ACC....................................................................................................................389
11.5 Working with the Parallel Axes U, V and W..................................................................................... 390
Overview................................................................................................................................................ 390
FUNCTION PARAXCOMP DISPLAY.......................................................................................................391
FUNCTION PARAXCOMP MOVE...........................................................................................................391
FUNCTION PARAXCOMP OFF.............................................................................................................. 392
FUNCTION PARAXMODE......................................................................................................................392
FUNCTION PARAXMODE OFF.............................................................................................................. 393
11.6 File functions........................................................................................................................................ 394
Application.............................................................................................................................................. 394
Defining file functions............................................................................................................................ 394
32
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 33
11.7 Definition of a datum shift..................................................................................................................395
Overview................................................................................................................................................ 395
TRANS DATUM AXIS............................................................................................................................. 395
TRANS DATUM TABLE.......................................................................................................................... 396
TRANS DATUM RESET..........................................................................................................................397
11.8 Creating Text Files................................................................................................................................398
Application.............................................................................................................................................. 398
Opening and exiting text files................................................................................................................398
Editing texts........................................................................................................................................... 399
Deleting and re-inserting characters, words and lines...........................................................................399
Editing text blocks..................................................................................................................................400
Finding text sections..............................................................................................................................401
11.9 Freely definable tables.........................................................................................................................402
Fundamentals......................................................................................................................................... 402
Creating a freely definable table............................................................................................................402
Editing the table format.........................................................................................................................403
Switching between table and form view...............................................................................................404
FN 26: TAPOPEN: Open a freely definable table.................................................................................. 405
FN 27: TAPWRITE: Write to a freely definable table.............................................................................406
FN 28: TAPREAD: Read from a freely definable table.......................................................................... 407
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
33
Page 34
Contents
12 Programming: Multiple Axis Machining...................................................................................... 409
12.1 Functions for multiple axis machining.............................................................................................. 410
12.2 The PLANE Function: Tilting the Working Plane (Software Option 1)............................................411
Introduction.............................................................................................................................................411
Defining the PLANE function.................................................................................................................413
Position display.......................................................................................................................................413
Resetting the PLANE function............................................................................................................... 414
Defining the working plane with the spatial angle: PLANE SPATIAL.................................................... 415
Defining the working plane with the projection angle: PLANE PROJECTED........................................ 417
Defining the working plane with the Euler angle: PLANE EULER.........................................................418
Defining the working plane with two vectors: PLANE VECTOR........................................................... 420
Defining the working plane via three points: PLANE POINTS...............................................................422
Defining the working plane via a single incremental spatial angle: PLANE SPATIAL.............................424
Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function)...................................... 425
Specifying the positioning behavior of the PLANE function..................................................................427
12.3 Inclined-tool machining in a tilted machining plane (software option 2).......................................432
Function..................................................................................................................................................432
Inclined-tool machining via incremental traverse of a rotary axis.......................................................... 432
Inclined-tool machining via normal vectors............................................................................................433
12.4 Miscellaneous functions for rotary axes........................................................................................... 434
Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1)............................................... 434
Shortest-path traverse of rotary axes: M126.........................................................................................435
Reducing display of a rotary axis to a value less than 360°: M94.........................................................436
Maintaining the position of the tool tip when positioning with tilted axes (TCPM): M128 (software option
2).............................................................................................................................................................437
Selecting tilting axes: M138...................................................................................................................440
Compensating the machine’s kinematics configuration for ACTUAL/NOMINAL positions at end of block:
M144 (software option 2)...................................................................................................................... 441
12.5 FUNCTION TCPM (software option 2)............................................................................................... 442
Function..................................................................................................................................................442
Defining the TCPM FUNCTION............................................................................................................. 442
Mode of action of the programmed feed rate...................................................................................... 443
Interpretation of the programmed rotary axis coordinates....................................................................443
Type of interpolation between the starting and end position................................................................ 445
Resetting the TCPM FUNCTION........................................................................................................... 446
34
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 35
12.6 Three-dimensional tool compensation (software option 2)............................................................ 447
Introduction.............................................................................................................................................447
Definition of a normalized vector...........................................................................................................448
Permitted tool shapes............................................................................................................................ 449
Using other tools: Delta values............................................................................................................. 449
3-D compensation without TCPM......................................................................................................... 449
Face Milling: 3D compensation with TCPM.......................................................................................... 450
Peripheral Milling: 3-D radius compensation with TCPM and radius compensation (RL/RR)................. 451
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
35
Page 36
Contents
13 Programming: Pallet editor........................................................................................................... 453
13.1 Pallet Management.............................................................................................................................. 454
Application.............................................................................................................................................. 454
Select pallet table.................................................................................................................................. 456
Exiting the pallet file.............................................................................................................................. 456
Run pallet file......................................................................................................................................... 456
36
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 37
14 Programming: Turning Operations............................................................................................... 459
14.1 Turning Operations on Milling Machines (Software Option 50)......................................................460
Introduction.............................................................................................................................................460
14.2 Basis Functions (Software Option 50)............................................................................................... 461
Switching between milling/turning mode of operation.......................................................................... 461
Graphical display of turning operations..................................................................................................463
Program spindle speed.......................................................................................................................... 464
Feed rate................................................................................................................................................ 465
Tool call...................................................................................................................................................465
Tool compensation in the program........................................................................................................ 466
Tool data................................................................................................................................................. 467
Tool tip radius compensation TRC......................................................................................................... 472
Recessing and undercutting...................................................................................................................473
Inclined turning.......................................................................................................................................479
14.3 Unbalance Functions........................................................................................................................... 481
Unbalance while turning........................................................................................................................ 481
Measure Unbalance cycle......................................................................................................................483
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
37
Page 38
Contents
15 Manual operation and setup.........................................................................................................485
15.1 Switch-on, switch-off...........................................................................................................................486
Switch-on................................................................................................................................................486
Switch-off................................................................................................................................................488
15.2 Moving the machine axes...................................................................................................................489
Note........................................................................................................................................................489
Moving the axis with the machine axis direction buttons..................................................................... 489
Incremental jog positioning....................................................................................................................489
Traverse with electronic handwheels.....................................................................................................490
15.3 Spindle speed S, feed rate F and miscellaneous function M.......................................................... 500
Application.............................................................................................................................................. 500
Entering values.......................................................................................................................................500
Adjusting spindle speed and feed rate.................................................................................................. 501
Activating feed-rate limitation................................................................................................................ 501
15.4 Functional safety FS (option)..............................................................................................................502
Miscellaneous.........................................................................................................................................502
Explanation of terms.............................................................................................................................. 503
Checking the axis positions................................................................................................................... 504
Overview of permitted feed rates and speeds......................................................................................505
Activating feed-rate limitation................................................................................................................ 505
Additional status displays.......................................................................................................................506
15.5 Datum setting without a 3-D touch probe........................................................................................507
Note........................................................................................................................................................507
Preparation..............................................................................................................................................507
Workpiece presetting with axis keys.....................................................................................................507
Datum management with the preset table........................................................................................... 508
15.6 Using 3-D touch probes.......................................................................................................................514
Overview................................................................................................................................................ 514
Functions in touch probe cycles............................................................................................................ 516
Selecting touch probe cycles.................................................................................................................518
Recording measured values from the touch-probe cycles.....................................................................519
Writing measured values from the touch probe cycles in a datum table.............................................. 520
Writing measured values from the touch probe cycles in the preset table........................................... 521
38
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 39
15.7 Calibrating a 3-D touch trigger probe................................................................................................522
Introduction.............................................................................................................................................522
Calibrating the effective length.............................................................................................................. 523
Calibrating the effective radius and compensating center misalignment.............................................. 524
Displaying calibration values.................................................................................................................. 526
15.8 Compensating workpiece misalignment with 3-D touch probe......................................................527
Introduction.............................................................................................................................................527
Identifying basic rotation........................................................................................................................528
Saving a basic rotation in the preset table............................................................................................528
Compensation of workpiece misalignment by rotating the table..........................................................528
Displaying a basic rotation..................................................................................................................... 529
Canceling a basic rotation......................................................................................................................529
15.9 Datum Setting with 3-D Touch Probe................................................................................................530
Overview................................................................................................................................................ 530
Datum setting in any axis...................................................................................................................... 530
Corner as datum.................................................................................................................................... 531
Circle center as datum...........................................................................................................................533
Setting a center line as datum...............................................................................................................535
Measuring workpieces with a 3-D touch probe.....................................................................................536
Using touch probe functions with mechanical probes or measuring dials.............................................539
15.10 Tilting the working plane (software option 1)..................................................................................540
Application, function...............................................................................................................................540
Traversing reference points in tilted axes.............................................................................................. 542
Position display in a tilted system......................................................................................................... 542
Limitations on working with the tilting function....................................................................................542
To activate manual tilting:...................................................................................................................... 543
Setting the current tool-axis direction as the active machining direction...............................................544
Setting the datum in a tilted coordinate system................................................................................... 545
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
39
Page 40
Contents
16 Positioning with Manual Data Input............................................................................................ 547
16.1 Programming and executing simple machining operations............................................................548
Positioning with manual data input (MDI)............................................................................................. 548
Protecting and erasing programs in $MDI.............................................................................................551
40
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 41
17 Test run and program run............................................................................................................. 553
17.1 Graphics.................................................................................................................................................554
Application.............................................................................................................................................. 554
Speed of the Setting test runs.............................................................................................................. 555
Overview: Display modes...................................................................................................................... 556
Plan view................................................................................................................................................557
Projection in three planes...................................................................................................................... 557
3-D view................................................................................................................................................. 558
Magnifying details.................................................................................................................................. 560
Repeating graphic simulation.................................................................................................................561
Tool display.............................................................................................................................................561
Measurement of machining time...........................................................................................................562
3-D line graphics.................................................................................................................................... 563
17.2 Showing the workpiece blank in the working space.......................................................................565
Application.............................................................................................................................................. 565
17.3 Functions for program display............................................................................................................566
Overview................................................................................................................................................ 566
17.4 Test Run.................................................................................................................................................567
Application.............................................................................................................................................. 567
17.5 Program run..........................................................................................................................................570
Application.............................................................................................................................................. 570
Running a part program......................................................................................................................... 571
Interrupt machining................................................................................................................................ 572
Moving the machine axes during an interruption.................................................................................. 573
Resuming program run after an interruption......................................................................................... 573
Any entry into program (mid-program startup)......................................................................................575
Returning to the contour........................................................................................................................577
17.6 Automatic program start.....................................................................................................................578
Application.............................................................................................................................................. 578
17.7 Optional block skip.............................................................................................................................. 579
Application.............................................................................................................................................. 579
Inserting the "/" character.......................................................................................................................579
Erasing the "/" character......................................................................................................................... 579
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
41
Page 42
Contents
17.8 Optional program-run interruption.....................................................................................................580
Application.............................................................................................................................................. 580
42
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 43
18 MOD functions................................................................................................................................581
18.1 MOD function....................................................................................................................................... 582
Selecting MOD functions.......................................................................................................................582
Changing the settings............................................................................................................................ 582
Exiting MOD functions...........................................................................................................................582
Overview of MOD functions..................................................................................................................583
18.2 Machine settings.................................................................................................................................. 584
External access...................................................................................................................................... 584
Select kinematics................................................................................................................................... 586
18.3 Position Display Types......................................................................................................................... 587
Application.............................................................................................................................................. 587
18.4 Unit of Measurement...........................................................................................................................588
Application.............................................................................................................................................. 588
18.5 Displaying operating times................................................................................................................. 588
Application.............................................................................................................................................. 588
18.6 Software numbers................................................................................................................................589
Application.............................................................................................................................................. 589
18.7 Entering the code number.................................................................................................................. 589
Application.............................................................................................................................................. 589
18.8 Setting up data interfaces...................................................................................................................590
Serial interfaces on the TNC 640.......................................................................................................... 590
Application.............................................................................................................................................. 590
Setting the RS-232 interface..................................................................................................................590
Setting the BAUD RATE (baudRate)...................................................................................................... 590
Setting the protocol (protocol)............................................................................................................... 591
Setting data bits (dataBits).....................................................................................................................591
Check parity (parity)............................................................................................................................... 591
Setting the stop bits (stopBits)..............................................................................................................591
Setting handshaking (flowControl)......................................................................................................... 592
File system for file operations (fileSystem)........................................................................................... 592
Settings for data transfer with the TNCserver PC software..................................................................592
Setting the operating mode of the external device (fileSystem)........................................................... 593
Data transfer software........................................................................................................................... 594
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
43
Page 44
Contents
18.9 Ethernet interface.................................................................................................................................596
Introduction.............................................................................................................................................596
Connection options................................................................................................................................ 596
Configuring the TNC.............................................................................................................................. 596
18.10 Configure HR 550 FS wireless handwheel........................................................................................ 602
Application.............................................................................................................................................. 602
Assigning the handwheel to a specific handwheel holder.................................................................... 602
Setting the transmission channel...........................................................................................................603
Selecting the transmitter power............................................................................................................ 603
Statistical data........................................................................................................................................604
44
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 45
19 Tables and overviews.....................................................................................................................605
19.1 Machine-specific user parameters......................................................................................................606
Application.............................................................................................................................................. 606
19.2 Connector pin layout and connection cables for data interfaces....................................................616
RS-232-C/V.24 interface for HEIDENHAIN devices................................................................................616
Non-HEIDENHAIN devices.....................................................................................................................618
Ethernet interface RJ45 socket............................................................................................................. 618
19.3 Technical Information...........................................................................................................................619
19.4 Overview tables....................................................................................................................................627
Fixed cycles............................................................................................................................................627
Miscellaneous functions.........................................................................................................................628
19.5 Functions of the TNC 640 and the iTNC 530 compared.................................................................. 630
Comparison: Specifications....................................................................................................................630
Comparison: Data interfaces..................................................................................................................630
Comparison: Accessories.......................................................................................................................631
Comparison: PC software...................................................................................................................... 631
Comparison: Machine-specific functions............................................................................................... 632
Comparison: User functions.................................................................................................................. 632
Comparison: Cycles................................................................................................................................639
Comparison: Miscellaneous functions................................................................................................... 641
Comparison: Touch probe cycles in the Manual Operation and El. Handwheel modes.........................643
Comparison: Touch probe cycles for automatic workpiece inspection.................................................. 644
Comparison: Differences in programming............................................................................................. 645
Comparison: Differences in Test Run, functionality............................................................................... 649
Comparison: Differences in Test Run, operation................................................................................... 649
Comparison: Differences in Manual Operation, functionality................................................................ 649
Comparison: Differences in Manual Operation, operation.....................................................................651
Comparison: Differences in Program Run, operation............................................................................ 651
Comparison: Differences in Program Run, traverse movements...........................................................652
Comparison: Differences in MDI operation........................................................................................... 656
Comparison: Differences in programming station................................................................................. 657
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
45
Page 46
Page 47
1
First Steps with
the TNC 640
Page 48
1
First Steps with the TNC 640

1.1 Overview

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 Programming the first part Graphically testing the first part Setting up tools Workpiece setup Running the first program

1.2 Machine switch-on

Acknowledging the power interruption and moving to the reference points

Switch-on and crossing over the reference points can vary depending on the machine tool. Refer to your machine manual.
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 interrupted" in the screen header
Press the CE key: The TNC compiles the PLC program
Switch on the control voltage: The TNC checks operation of the emergency stop circuit and goes into the reference run mode
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 486 Operating modes: See "Programming", page 73
48
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 49

1.3 Programming the first part

Selecting the correct operating mode

You can write programs only in Programming mode:
Press the Programming operating mode key: The TNC switches to Programming mode
Further information on this topic
Operating modes: See "Programming", page 73

The most important TNC keys

Functions for conversational guidance Key
Confirm entry and activate the next dialog prompt
1
Programming the first part 1.3
Ignore the dialog question
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 100
Overview of keys: See "Controls of the TNC", page 2
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
49
Page 50
1
First Steps with the TNC 640
1.3 Programming the first part

Creating a new program/file management

Press the PGM MGT key: The TNC opens the file manager. 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
Use the arrow keys to select the folder in which you want to open the new file
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
To select the unit of measure, press the MM or INCH soft key: The TNC automatically starts the workpiece blank definition (See "Defining a workpiece blank", page 51)
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 108
Creating a new program: See "Opening programs and entering", page 95
50
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 51
Programming the first part 1.3

Defining 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:
Working plane in graphic: XY?: Enter the active spindle axis. Z is saved as default setting. Accept with the ENT key
Workpiece blank def.: minimum X: Smallest X coordinate of the workpiece blank with respect to the reference point, e.g. 0. Confirm with the ENT key
Workpiece blank def.: minimum Y: Smallest Y coordinate of the workpiece blank with respect to the reference point, e.g. 0. Confirm with the ENT key
1
Workpiece blank def.: minimum Z: Smallest Z coordinate of the workpiece blank with respect to the reference point, e.g. –40. Confirm with the ENT key
Workpiece blank def.: maximum X: Largest X coordinate of the workpiece blank with respect to the reference point, e.g.
100. Confirm with the ENT key Workpiece blank def.: maximum Y: Largest Y coordinate of
the workpiece blank with respect to the reference point, e.g.
100. Confirm with the ENT key Workpiece blank def.: maximum Z: Largest Z coordinate of
the workpiece blank with respect to the reference point, e.g. 0. Confirm with the ENT key. The TNC concludes the dialog
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
Further information on this topic
Defining the workpiece blank: page 96
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
51
Page 52
1
First Steps with the TNC 640
1.3 Programming the first part

Program layout

NC programs should be arranged consistently in a similar manner. This makes it easier to find your place, accelerates programming 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
preposition immediately to workpiece depth. If required, switch on
the spindle/coolant 5 Contour approach 6 Contour machining 7 Contour departure 8 Retract the tool, end program
Further information on this topic
Contour programming: See "Tool movements", page 192
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
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 program
Further information on this topic
Cycle programming: See User’s Manual for Cycles
Cycle program layout
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
52
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 53
Programming the first part 1.3

Programming 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.
Call the tool: Enter the tool data. Confirm each of your entries with the ENT key. Do not forget the tool axis
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
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
1
Confirm Feed rate F=? with the ENT key: Move at rapid traverse (FMAX)
Confirm the Miscellaneous function M? with theEND key: The TNC saves the entered positioning block
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
Press the orange Y axis key and enter the value for the position to be approached, e.g. –20. Confirm with the ENT key
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
Confirm Feed rate F=? with the ENT key: Move at rapid traverse (FMAX)
Confirm the Miscellaneous function M? with the END key: The TNC saves the entered positioning block
Move the tool to workpiece depth: Press the orange axis key and enter the value for the position to be approached, e.g. –5. Confirm with the ENT key
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
Feed rate F=? Enter the positioning feed rate, e.g. 3000 mm/min and confirm with the ENT key
Miscellaneous function M? Switch on the spindle and coolant, e.g. M13. Confirm with the END key: The TNC saves the entered positioning block
Move to the contour: Press the APPR/DEP key: The TNC shows a soft-key row with approach and departure functions
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
53
Page 54
1
First Steps with the TNC 640
1.3 Programming the first part
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
Center angle? Enter the approach angle, e.g. 90°, and confirm with the ENT key
Circle radius? Enter the approach radius, e.g. 8 mm, and confirm with the ENT key
Confirm the Radius comp.: RL/RR/no comp? with the RL soft key: Activate the radius compensation to the left of the programmed contour
Feed rate F=? Enter the machining feed rate, e.g. 700 mm/min, and confirm your entry with the END key
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
Move to contour point 3: Enter the X coordinate 95 and save your entry with the END key
Define the chamfer at contour point 3: Enter the chamfer width 10 mm and save with the END key
Move to contour point 4: Enter the Y coordinate 5 and save your entry with the END key
Define the chamfer at contour point 4: Enter the chamfer width 20 mm and save with the END key
Move to contour point 1: Enter the X coordinate 5 and save your entry with the END key
Depart the contour
54
Select the departure function DEP CT Center angle? Enter the departure angle, e.g. 90°,
and confirm with the ENT key Circle radius? Enter the departure radius, e.g. 8
mm, and confirm with the ENT key Feed rate F=? Enter the positioning feed rate, e.g.
3000 mm/min and confirm with the ENT key Miscellaneous function M? Switch off the coolant,
e.g. M9, with the END key: The TNC saves the entered positioning block
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Page 55
Enter 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
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
Confirm Feed rate F=? with the ENT key: Move at rapid traverse (FMAX)
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 215
Creating a new program: See "Opening programs and entering",
page 95
Approaching/departing contours: See " Approaching and
departing a contour", page 198
Programming contours: See "Overview of path functions",
page 206
Programmable feed rates: See "Mögliche Vorschubeingaben"
Tool radius compensation: See "Tool radius compensation",
page 188
Miscellaneous functions (M): See "M functions for program run
inspection, spindle and coolant ", page 349
1
Programming the first part 1.3
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
55
Page 56
1
First Steps with the TNC 640
1.3 Programming the first part

Creating 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.
Call the tool: Enter the tool data. Confirm each of your entries with the ENT KEY. DO NOT FORGET THE TOOL AXIS
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
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
Confirm Feed rate F=? with the ENT key: Move at rapid traverse (FMAX)
Confirm the Miscellaneous function M? with theEND key: The TNC saves the entered positioning block
Call the cycle menu
Display the drilling cycles
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
Call the menu for special functions
Display the functions for point machining
Select the pattern definition
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
Display the menu for defining the cycle call
56
Run the drilling cycle on the defined pattern: Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX) Miscellaneous function M? Switch on the spindle
and coolant, e.g. M13. Confirm with the END key: The TNC saves the entered positioning block
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Page 57
Enter 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
Confirm Radius comp.: RL/RR/no comp? by pressing the ENT key: Do not activate the radius compensation
Confirm Feed rate F=? with the ENT key: Move at rapid traverse (FMAX)
Miscellaneous function M? Enter M2 to end the program and confirm with the END key: The TNC saves the entered positioning block
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 ;SET-UP CLEARANCE
Q201=-20 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGNG
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 BOTTOM
7 CYCL CALL PAT FMAX M13
8 L Z+250 R0 FMAX M2
9 END PGM C200 MM
1
Programming the first part 1.3
Definition of workpiece blank
Tool call Retract the tool Define the machining positions
Define the cycle
Spindle and coolant on, call the cycle Retract the tool, end program
Further information on this topic
Creating a new program: See "Opening programs and entering",
page 95
Cycle programming: See User’s Manual for Cycles
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
57
Page 58
1
First Steps with the TNC 640

1.4 Graphically testing the first part

1.4 Graphically testing the first part

Selecting the correct operating mode

You can test programs only in the Test Run mode:
Press the Test Run operating mode key: the TNC switches to that mode
Further information on this topic
Operating modes of the TNC: See "Modes of Operation",
page 73
Testing programs: See "Test Run", page 567

Selecting the tool table for the test run

You only need to execute this step if you have not activated a tool table in the Test Run mode.
Press the PGM MGT key: The TNC opens the file manager
Press the SELECT TYPE soft key: The TNC shows a soft-key menu for selection of the file type to be displayed
Press the SHOW ALL soft key: The TNC shows all saved files in the right window
Move the highlight to the left onto the directories
Move the highlight to the TNC:\ directory
Move the highlight to the right onto the files
Move the highlight to the file TOOL.T (active tool table) and load with the ENT key: TOOL.T receives the status S and is therefore active for the test run
Press the END key: Exit the file manager
Further information on this topic
Tool management: See "Enter tool data into the table",
page 160
Testing programs: See "Test Run", page 567
58
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 59

Choosing the program you want to test

Press the PGM MGT key: The TNC opens the file manager
Press the LAST FILES soft key: The TNC opens a pop-up window with the most recently selected files
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 108

Selecting the screen layout and the view

1
Graphically testing the first part 1.4
Press the key for selecting the screen layout. The TNC shows all available alternatives in the soft-key row
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
Select the desired view via soft key Plan view
Projection in three planes
3-D view
Further information on this topic
Graphic functions: See "Graphics ", page 554
Running a test run: See "Test Run", page 567
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
59
Page 60
1
First Steps with the TNC 640
1.4 Graphically testing the first part

Starting the test run

Press the RESET + START soft key: The TNC simulates the active program up to a programmed break or to the program end
While the simulation is running, you can use the soft keys to change views
Press the STOP soft key: The TNC interrupts the test run
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 567
Graphic functions: See "Graphics ", page 554
Adjusting the test speed: See "Speed of the Setting test runs",
page 555
60
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 61

1.5 Setting up tools

Selecting the correct operating mode

Tools are set up in the Manual Operation mode:
Press the Manual Operation operating mode key: the TNC switches to that mode
Further information on this topic
Operating modes of the TNC: See "Modes of Operation",
page 73
1
Setting up tools 1.5

Preparing and measuring tools

Clamp the required tools in their chucks
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
When measuring on the machine: Place the tools into the tool
changer page 63
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
61
Page 62
1
First Steps with the TNC 640
1.5 Setting up tools

The tool table TOOL.T

In the tool table TOOL.T (permanently saved under TNC:\TABLE\), save the tool data such as length and radius, but also further tool­specific information that the TNC needs to perform its functions.
To enter tool data in the tool table TOOL.T, proceed as follows:
Display the tool table
Edit the tool table: Set the EDITING soft key to ON With the upward or downward arrow keys you can
select the tool number that you want to edit With the rightward or leftward arrow keys you can
select the tool data that you want to edit To exit the tool table, press the END key
Further information on this topic
Operating modes of the TNC: See "Modes of Operation",
page 73
Working with the tool table: See "Enter tool data into the table",
page 160
62
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 63

The pocket table TOOL_P.TCH

The function of the pocket table depends on the machine. Refer to your machine manual.
In the pocket table TOOL_P.TCH (permanently saved under TNC: \TABLE\) you specify which tools your tool magazine contains.
To enter data in the pocket table TOOL_P.TCH, proceed as follows:
Display the tool table
Display the pocket table Edit the pocket table: Set the EDITING soft key to
ON
1
Setting up tools 1.5
With the upward or downward arrow keys you can select the pocket number that you want to edit
With the rightward or leftward arrow keys you can select the data that you want to edit
To leave the pocket table, press the END key
Further information on this topic
Operating modes of the TNC: See "Modes of Operation",
page 73
Working with the pocket table: See "Pocket table for tool
changer", page 170
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
63
Page 64
1
First Steps with the TNC 640

1.6 Workpiece setup

1.6 Workpiece setup

Selecting the correct operating mode

Workpieces are set up in the Manual Operation or Electronic Handwheel mode
Press the Manual Operation operating mode key: the TNC switches to that mode
Further information on this topic
Manual Operation mode: See "Moving the machine axes",
page 489

Clamping 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.
64
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 65

Workpiece alignment with 3-D touch probe

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)
Select the probing functions: The TNC displays the available functions in the soft-key row
Measure the basic rotation: The TNC displays the basic rotation menu. To identify the basic rotation, probe two points on a straight surface of the workpiece
Use the axis-direction keys to preposition the touch probe to a position near the first contact point
Select the probing direction via soft key
1
Workpiece setup 1.6
Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point
Use the axis-direction keys to preposition the touch probe to a position near the second contact point
Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point
Then the TNC shows the measured basic rotation Press SET BASIC ROTATION soft key to select the
displayed value as the active rotation. Press the END soft key to exit the menu
Further information on this topic
MDI operating mode: See "Programming and executing simple
machining operations", page 548
Workpiece alignment: See "Compensating workpiece
misalignment with 3-D touch probe ", page 527
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
65
Page 66
1
First Steps with the TNC 640
1.6 Workpiece setup

Datum setting with 3-D touch probe

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
Select the probing functions: The TNC displays the available functions in the soft-key row
Set the datum at a workpiece corner, for example Position the touch probe near the first touch point
on the first workpiece edge Select the probing direction via soft key Press NC start: The touch probe moves in the
defined direction until it contacts the workpiece and then automatically returns to its starting point
Use the axis-direction keys to pre-position the touch probe to a position near the second touch point on the first workpiece edge
Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point
Use the axis-direction keys to pre-position the touch probe to a position near the first touch point on the second workpiece edge
Select the probing direction via soft key Press NC start: The touch probe moves in the
defined direction until it contacts the workpiece and then automatically returns to its starting point
Use the axis-direction keys to pre-position the touch probe to a position near the second touch point on the second workpiece edge
Press NC start: The touch probe moves in the defined direction until it contacts the workpiece and then automatically returns to its starting point
Then the TNC shows the coordinates of the measured corner point
Set to 0: Press the SET DATUM soft key Press the END soft key to close the menu
Further information on this topic
Datum setting: See "Datum Setting with 3-D Touch Probe ",
page 530
66
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 67

1.7 Running the first program

Selecting the correct operating mode

You can run programs either in the Single Block or the Full Sequence mode:
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 start key
Press the Program Run, Full Sequence operating mode key: The TNC switches to that mode and runs the program after NC start up to a program interruption or to the end of the program
Further information on this topic
Operating modes of the TNC: See "Modes of Operation",
page 73
Running programs: See "Program run", page 570
1
Running the first program 1.7

Choosing the program you want to run

Press the PGM MGT key: The TNC opens the file manager
Press the LAST FILES soft key: The TNC opens a pop-up window with the most recently selected files
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 108

Start the program

Press the NC start key: The TNC runs the active program
Further information on this topic
Running programs: See "Program run", page 570
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
67
Page 68
Page 69
2

Introduction

Page 70
2
Introduction

2.1 The TNC 640

2.1 The TNC 640
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 and drilling machines, as well as machining centers, with up to 18 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 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 and 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 FK free contour programming feature performs the necessary calculations automatically. Workpiece machining can be graphically simulated either during or before actual machining.
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

Machining programs created on HEIDENHAIN contouring controls (starting from the TNC 150 B) may not always run on the TNC 640. If NC blocks contain invalid elements, the TNC will mark them as ERROR blocks when the file is opened.
See "Functions of the and the iTNC 530 compared". Please also note the detailed description of the differences between the iTNC 530 and the TNC 640
70
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 71
1
7
7
2
5
4
3
4
6
8
Visual display unit and operating panel 2.2

2.2 Visual display unit and operating panel

Display screen

The TNC is shipped with a 19-inch TFT flat-panel display.
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 operating 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 soft­key row. You can select these functions by pressing the keys immediately below them. The lines immediately above the soft-key row indicate the number of soft-key rows that can be called with the black arrow keys to the right and left. The bar representing the active soft-key row is highlighted
2
3 Soft-key selection keys 4 Shifting between soft-key rows 5 Setting the screen layout 6 Shift key for switchover between machining and programming
modes
7 Soft-key selection keys for machine tool builders 8 Switching the soft-key rows for machine tool builders

Setting the screen layout

You select the screen layout yourself: In the Programming 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 screen layout key: The soft-key row shows the available layout options, see "Operating modes", page 62
Select the desired screen layout
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
71
Page 72
2
2
3
4
5
8 9
6
7
10
1
Introduction
2.2 Visual display unit and operating panel

Control Panel

The TNC 640 is delivered with an integrated keyboard. The figure to the right shows the operating elements of the operating panel:
1 Alphabetic keyboard for entering texts and file names, and for
ISO programming.
2
3 Programming modes 4 Machine operating modes 5 Initiation of programming dialogs 6 Navigation keys and GOTO jump command 7 Numerical input and axis selection 8 Touchpad 9 Mouse function keys 10 USB connection
The functions of the individual keys are described on the inside front cover.
File management Calculator MOD function HELP function
Some machine manufacturers do not use the standard operating panel from HEIDENHAIN. Refer to your machine manual.
Machine panel buttons, e.g. NC START or NC STOP, are described in the manual for your machine tool.
72
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 73

2.3 Modes of Operation

Manual Operation and El. 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 El. 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
Positions
2
Modes of Operation 2.3
Left: positions, right: status display

Positioning with Manual Data Input

This mode of operation is used for programming simple traversing movements, such as for face milling or prepositioning.
Soft keys for selecting the screen layout
Window Soft key
Program
Left: program blocks, right: status display

Programming

In this mode of operation you can write your part programs. The FK free programming feature, the various cycles and the Q parameter functions help you with programming and add necessary information. If desired, you can have the programming graphics show the programmed paths of traverse.
Soft keys for selecting the screen layout
Window Soft key
Program
Left: program, right: program structure
Left: program, right: programming graphics
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
73
Page 74
2
Introduction
2.3 Modes of Operation

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 working space. This simulation is supported graphically in different display modes.
Soft keys for selecting the screen layout: See "Program Run, Full Sequence and Program Run, Single Block", page 74.

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
Left: program, right: program structure
Left: program, right: status
Left: program, right: graphics
Graphics
Window Soft key
Pallet table
Left: program, right: pallet table
Left: pallet table, right: status
74
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 75

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 Operation and El. Handwheel modes the status display appears in the large window.
Information in the status display
Icon Meaning
ACTL. Position display: Actual, nominal or distance-to-go
coordinates mode 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
Number of the active presets from the preset table. If the datum was set manually, the TNC displays the text MAN behind the symbol
F S M The displayed feed rate in inches corresponds to
one tenth of the effective value. Spindle speed S, feed rate F and active M functions
Axis is clamped
2
Status displays 2.4
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
No active program
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
75
Page 76
2
Introduction
2.4 Status displays
Icon Meaning
Program run has started
Program run is stopped
Program run is being aborted
Turning mode is active
The Dynamic Collision Monitoring function (DCM) is active
The Adaptive Feed Function (AFC) is active (software option)

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 Programming and Editing mode of operation.
To switch on the additional status display:
Call the soft-key row for screen layout
Select the 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:
Switch the soft-key rows until the STATUS soft keys appear
Either select the additional status display directly by soft key, e.g. positions and coordinates, or
use the switch-over soft keys to select the desired view
The available status displays described below can be selected either directly by soft key or with the switch-over soft keys.
Please note that some of the status information described below is not available unless the associated software option is enabled on your TNC.
76
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 77
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
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
2
Status displays 2.4
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
Current machining time in percent Current time Active programs
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
77
Page 78
2
Introduction
2.4 Status displays
Program section repeat/Subprograms (LBL tab)
Soft key Meaning
No direct selection possible
Information on standard cycles (CYC tab)
Soft key Meaning
No direct selection possible
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
78
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 79
Active miscellaneous functions M (M tab)
Soft key Meaning
2
Status displays 2.4
No direct selection possible
Positions and coordinates (POS tab)
Soft key Meaning
List of the active M functions with fixed meaning
List of the active M functions that are adapted by your machine manufacturer
Type of position display, e.g. actual position
Tilt angle of the working plane Angle of a basic rotation Active kinematics
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
79
Page 80
2
Introduction
2.4 Status displays
Information on tools (TOOL tab)
Soft key Meaning
Display of active tool:
T: Tool number and name RT: Number and name of a replacement tool
Tool axis Tool length 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 programmed tool and replacement tool
Tool measurement (TT tab)
The TNC displays the TT tab only 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 permissible tolerance in the tool table was exceeded
80
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 81
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 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
2
Status displays 2.4
For further information, refer to the User's Manual for Cycles, "Coordinate Transformation Cycles."
Displaying Q parameters (QPARA tab)
Soft key Meaning
Display the current values of the defined Q parameters
Display the character strings of the defined string parameters
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
81
Page 82
2
Introduction
2.4 Status displays
Adaptive Feed Control (AFC tab, software option)
The TNC displays the AFC tab only if the function is active on your machine.
Soft key Meaning
No direct selection possible
Active tool (number and name)
Cut number Current factor of the feed potentiomenter 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
82
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 83

2.5 Window Manager

The machine tool builder determines the scope of function and behavior of the window manager. Refer to your machine manual.
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 task bar for switching between various applications
(user interfaces).
Manage an additional desktop, on which special applications
from 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.
2
Window Manager 2.5
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.
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
83
Page 84
2
Introduction
2.5 Window Manager

Task bar

In the task bar you can choose different workspaces by mouse click. The TNC provides the following workspaces:
Workspace 1: Active mode of operation
Workspace 2: Active programming mode
Workspace 3: Manufacturer's applications (optionally available)
In the task bar you can also select other applications that you have started together with the TNC (switch for example to the PDF
viewer or TNCguide)
Click the green HEIDENHAIN symbol to open a menu in which you can get information, make settings or start applications. The following functions are available:
About Xfce: Information on the Windows manager Xfce
About HEROS: Information about the operating system of the
TNC
NC Control: Start and stop the TNC software. Only permitted
for diagnostic purposes
Web Browser: Start Mozilla Firefox
Diagnostics: Available only to authorized specialists to start
diagnostic functions
Settings: Configuration of miscellaneous settings
Date/Time: Set the date and time Language: Language setting for the system dialogs. During
startup the TNC overwrites this setting with the language setting of MP 7230
Network: Network setting Reset WM-Conf: Restore basic settings of the Windows
Manager. May also reset settings implemented by your machine manufacturer
Screensaver: Settings for the screen saver; several are available
Shares: Configure network connections
Tools: Only for authorized users. The applications available
under tools can be started directly by selecting the pertaining
file type in the file management of the TNC See "File manager:
Fundamentals", page 105
84
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 85
SELinux security software 2.6

2.6 SELinux security software

SELinux is an extension for Linux-based operating systems.
SELinux is an additional security software package based on Mandatory Access Control (MAC) and protects the system against the running of unauthorized processes or functions and therefore protects against viruses and other malware.
MAC means that each action must be specifically permitted otherwise the TNC will not run it. The software is intended as protection in addition to the normal access restriction in Linux. Certain processes and actions can only be executed if the standard functions and access control of SELinux permit it.
The SELinux installation of the TNC is prepared to permit running of only those programs installed with the HEIDENHAIN NC software. Other programs cannot be run with the standard installation.
2
The access control of SELinux under HEROS 5 is regulated as follows:
The TNC runs only those applications installed with the
HEIDENHAIN NC software.
Files in connection with the safety of the software (SELinux
system files, HEROS 5 boot files etc.) may only be changed by
programs that are selected explicitly.
New files generated by other programs must never be
executed.
There are only two processes that are permitted to execute new
files:
Starting a software update: A software update from HEIDENHAIN can replace or change system files.
Starting the SELinux configuration: The configuration of SELinux is usually password-protected by your machine tool builder. Refer here to the relevant machine tool manual.
HEIDENHAIN generally recommends activating SELinux because it provides additional protection against attacks from outside.
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
85
Page 86
2
Introduction
2.7 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic
Handwheels
2.7 Accessories: HEIDENHAIN 3-D Touch
Probes and Electronic Handwheels

3-D touch probes

The various HEIDENHAIN 3-D touch probes enable you to:
Automatically align workpieces
Quickly and precisely set datums
Measure the workpiece during program run
Measure and inspect tools
All of the cycle functions (touch probe cycles and fixed cycles) are described in the Cycle Programming User’s Manual. Please contact HEIDENHAIN if you require a copy of this User’s Manual. ID: 892905-xx
TS 220, TS 440, TS 444, TS 640 und TS 740 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 cost-effective 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 the actual value.
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.
86
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 87
2
Accessories: HEIDENHAIN 3-D Touch Probes and Electronic

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 panel-mounted handwheels, HEIDENHAIN also offers the HR 410 portable handwheel.
2.7
Handwheels
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
87
Page 88
Page 89
3
Programming:
Fundamentals, file
management
Page 90
3
Programming: Fundamentals, file management

3.1 Fundamentals

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.
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.

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.
90
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 91

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 TNC 640 can control up to 18 axes optionally. 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
Fundamentals 3.1

Designation of the axes on milling machines

The X, Y and Z axes on your milling machine are also referred to as tool axis, principal axis (1st axis) and secondary axis (2nd axis). The assignment of the tool axis is decisive for the assignment of the principal and secondary axes.
Tool axis Principal axis Secondary axis
X Y Z Y Z X Z X Y
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
91
Page 92
3
Programming: Fundamentals, file management
3.1 Fundamentals

Polar coordinates

If the production drawing is dimensioned in Cartesian coordinates, you also write the NC program using Cartesian coordinates. For parts containing circular arcs or angles it is often simpler to give the dimensions in polar coordinates.
While the Cartesian coordinates X, Y and Z are three-dimensional and can describe points in space, polar coordinates are two­dimensional and describe points in a plane. Polar coordinates have their datum at a circle center (CC), or pole. A position in a plane can be clearly defined by the:
Polar Radius, the distance from the circle center CC to the
position, and the
Polar Angle, the value of the angle between the angle 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.
Coordinates of the pole (plane)
X/Y +X Y/Z +Y Z/X +Z
Reference axis of the angle
92
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 93

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 an NC program in incremental coordinates, you thus program the tool to move by the distance between the previous and the subsequent nominal positions. This is why they are 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
3
Fundamentals 3.1
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 angle reference axis.
Incremental polar coordinates always refer to the last programmed nominal position of the tool.
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
93
Page 94
3
Programming: Fundamentals, file management
3.1 Fundamentals

Selecting 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 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 from which the dimensions of the remaining workpiece positions can be most easily measured.
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 Cycle Programming 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.
94
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 95
Block number
Path functions
Words
Block
Opening programs and entering 3.2

3.2 Opening programs and entering

Organization of an NC program in HEIDENHAIN Conversational format

A part program consists of a series of program blocks. The figure at right illustrates the elements of a block.
The TNC numbers the blocks in ascending sequence. The first block of a program is identified by BEGIN PGM, the
program name and the active unit of measure. The subsequent blocks contain information on:
The workpiece blank
Tool calls
Approaching a safe position
Feed rates and spindle speeds, as well as
Path contours, cycles and other functions
3
The last block of a program is identified by END PGM the program name and the active unit of measure.
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, the PROGRAM DEFAULTS soft 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 workpiece blank 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 workpiece blank if you wish to run a graphic test for the program!
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
95
Page 96
3
Programming: Fundamentals, file management
3.2 Opening programs and entering

Opening 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 mode of operation
Call the file manager: Press the PGM MGT key
Select the directory in which you wish to store the new program:
FILE NAME = ALT.H
Enter the new program name and confirm your entry with the ENT key.
Select the unit of measure: Press the MM or INCH soft key. The TNC switches the screen layout and initiates the dialog for defining the BLK FORM (workpiece blank)
WORKING PLANE IN GRAPHIC: XY
Enter spindle axis, e.g. Z
WORKPIECE BLANK DEF.: MINIMUM
Enter in sequence the X, Y and Z coordinates of the MIN point and confirm each of your entries with the ENT key
WORKPIECE BLANK DEF.: MAXIMUM
Enter in sequence the X, Y and Z coordinates of the MAX point and confirm each of your entries with the ENT key
Example: Display the BLK form in the NC program
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
The TNC automatically generates the block numbers as well as the BEGIN and END blocks.
Program begin, name, unit of measure Spindle axis, MIN point coordinates MAX point coordinates Program end, name, unit of measure
96
If you do not wish to define a blank form, cancel the dialog at Working plane in graphic: XY by pressing the DEL key.
The TNC can display the graphics only if the shortest side is at least 50 µm long and the longest side is no longer than 99 999.999 mm.
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
Page 97
Opening programs and entering 3.2

Programming tool movements in conversational

To program a block, initiate the dialog by pressing a function key. In the screen headline, the TNC then asks you for all the information necessary to program the desired function.
If you enter DIN/ISO functions via a connected USB keyboard, make sure that capitalization is active.
Example of a positioning block
Open block
3
COORDINATES ?
10 (Enter the target coordinate for the X axis)
20 (Enter the target coordinate for the Y axis)
go to the next question with ENT.
RADIUS COMP.: RL/RR/NO COMP.?
Enter "No radius compensation" and go to the next question with ENT.
FEED RATE F=? / F MAX = ENT
100 (Enter a feed rate of 100 mm/min for this path contour)
go to the next question with ENT.
MISCELLANEOUS FUNCTION M ?
Enter 3 (miscellaneous function M3 "Spindle ON").
The TNC ends this dialog by pressing the ENT key.
The program-block window displays the following line:
3 L X+10 Y+5 R0 F100 M3
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
97
Page 98
3
Programming: Fundamentals, file management
3.2 Opening programs and entering
Possible feed rate input
Functions for setting the feed rate Soft key
Rapid traverse, non-modal. Exception: If defined before an APPR block, FMAX is also in effect for moving to an auxiliary point (See "Important positions for approach and departure", page 199)
Traverse feed rate automatically calculated in
TOOL CALL
Move at the programmed feed rate (unit of measure is mm/min or 1/10 inch/min). With rotary axes, the TNC interprets the feed rate in degrees/min, regardless of whether the program is written in mm or inches
Define the feed per revolution (units in mm/ rev or inch/rev). Caution: In inch-programs, FU cannot be combined with M136
Define the tooth feed (units in mm/tooth or inch/tooth). The number of teeth must be defined in the tool table in the CUT. column
Functions for conversational guidance Key
Ignore the dialog question
End the dialog immediately
Abort the dialog and erase the block
98
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Page 99
Opening programs and entering 3.2

Actual position capture

The TNC enables you to transfer the current tool position into the program, for example during
Positioning-block programming
Cycle programming
To transfer the correct position values, proceed as follows:
Place the input box at the position in the block where you want
to insert a position value
Select the actual-position-capture function: In the soft-key row the TNC displays the axes whose positions can be transferred
Select the axis: The TNC writes the current position of the selected axis into the active input box
3
In the working plane the TNC always captures the coordinates of the tool center, even though tool radius compensation is active.
In the tool axis the TNC always captures the coordinates of the tool tip and thus always takes the active tool length compensation into account.
The TNC keeps the soft-key row for axis selection active until you deactivate it by pressing the actual­position-capture key again. This behavior remains in effect even if you save the current block and open a new one with a path function key. If you select a block element in which you must choose an input alternative via soft key (e.g. for radius compensation), then the TNC also closes the soft-key row for axis selection.
The actual-position-capture function is not allowed if the tilted working plane function is active.
TNC 640 | User's Manual HEIDENHAIN Conversational Programming | 5/2013
99
Page 100
3
Programming: Fundamentals, file management
3.2 Opening programs and entering

Editing a program

You cannot edit a program while it is being run by the TNC in a machine operating mode.
While you are creating or editing a part program, you can select any desired line in the program or individual words in a block with the arrow keys or the soft keys:
Function Soft key/Keys
Go to previous page
Go to next page
Go to beginning of program
Go to end of program
Change the position of the current block on the screen. Press this soft key to display additional program blocks that are programmed before the current block
Change the position of the current block on the screen. Press this soft key to display additional program blocks that are programmed after the current block
Move from one block to the next
Select individual words in a block
To select a certain block, press the GOTO key, enter the desired block number, and confirm with the ENT key. Or: Enter the block number step and press the N LINES soft key to jump over the entered number of lines upward or downward
100
HEIDENHAIN Conversational Programming | 5/2013
TNC 640 | User's Manual
Loading...