Page 1
User’s Manual
HEIDENHAIN
Conversational
TNC 640
NC Software
340 590-01
340 591-01
340 594-01
English (en)
4/2012
Page 2
Controls of the TNC
1
50
0
50
100
F %
1
50
0
50
100
S %
Keys on visual display unit
Key Function
Split screen layout
Toggle the display between machining
and programming modes
Soft keys for selecting functions on
screen
Switch the soft-key rows
Alphanumeric keyboard
Key Function
File names, comments
DIN/ISO programming
Machine operating modes
Key Function
Manual Operation
Electronic Handwheel
Program/file management, TNC functions
Key Function
Select or delete programs and files,
external data transfer
Define program call, select datum and
point tables
Select MOD functions
Display help text for NC error messages,
call TNCguide
Display all current error messages
Show 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
Programming modes
Key Function
Positioning with Manual Data Input
Program Run, Single Block
Program Run, Full Sequence
Cycles, subprograms and program section repeats
Key Function
Define touch probe cycles
Programming and Editing
Define and call cycles
Test Run
Enter and call labels for subprogramming
and program section repeats
Enter program stop in a program
Page 3
Tool functions
Key Function
Define tool data in the program
Coordinate axes and numbers: Entering and editing
Key Function
Select coordinate axes or
enter them into the program
Call tool data
Programming path movements
Key Function
Approach/depart contour
FK free contour programming
Straight line
Circle center/pole for polar coordinates
Circle with center
Circle with radius
Circular arc with tangential connection
Chamfer/Corner rounding
Numbers
Decimal point / Reverse algebraic sign
Polar coordinate input / Incremental
values
Q parameter programming /
Q parameter status
Save actual position or values from
calculator
Skip dialog questions, delete words
Confirm entry and resume dialog
Conclude block and exit entry
Clear numerical entry or TNC error
message
Abort dialog, delete program section
Special functions
Key Function
Show special functions
Select the next tab in forms
Up/down one dialog box or button
Page 4
Page 5
About this Manual
The symbols used in this manual are described below.
This symbol indicates that important notes about the
function described must be 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 that the described function must be
adapted by the machine tool builder. The function
described may therefore vary depending on the machine.
This symbol indicates that you can find detailed
information about a function in another manual.
About this Manual
Would you like any changes, or have you found any errors?
We are continuously striving to improve documentation for you.
Please help us by sending your requests to the following e-mail
address: tnc-userdoc@heidenhain.de.
HEIDENHAIN TNC 640 5
Page 6
TNC Model, Software and Features
This manual describes functions and features provided by TNCs as of
the following NC software numbers.
TNC model NC software number
TNC 640 340 590-01
TNC 640 E 340 591-01
TNC 640 Programming Station 340 594-01
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
TNC Model, Software and Features
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 a separate manual. Please contact
HEIDENHAIN if you need a copy of this User’s Manual.
ID: 892 905-xx
6
Page 7
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:
Software option 1 (option number #08)
Cylinder surface interpolation (Cycles 27, 28 and 29)
Feed rate in mm/min for rotary axes: M116
Tilting the machining plane (plane functions, Cycle 19 and 3D-ROT
soft key in the Manual Operation mode)
Circle in 3 axes with tilted working plane
Software option 2 (option number #09)
5-axis interpolation
3-D machining:
M128: Maintaining the position of the tool tip when positioning
with tilted axes (TCPM)
FUNCTION TCPM: Maintaining the position of the tool tip when
positioning with tilted axes (TCPM) in selectable modes
M144: Compensating the machine’s kinematic configuration for
ACTUAL/NOMINAL positions at end of block
LN blocks (3-D compensation)
TNC Model, Software and Features
HEIDENHAIN DNC (option number #18)
Communication with external PC applications over COM
component
Additional conversational language (option number #41)
Function for enabling the conversational languages Slovenian,
Slovak, Norwegian, Latvian, Estonian, Korean, Turkish, Romanian,
Lithuanian.
Display step (option number #23)
Input resolution and display step:
Linear axes down to 0.01 µm
Rotary axes to 0.00001°
Double speed (option number #49)
Double-speed control loops are used primarily for high-speed
spindles as well as for linear motors and torque motors
HEIDENHAIN TNC 640 7
Page 8
KinematicsOpt software option (option number #48)
Touch-probe cycles for inspecting and optimizing the machine
accuracy
Software option Mill-Turning (option number #50)
Functions for milling/turning mode:
Switching between Milling/Turning mode of operation
Constant cutting speed
Tool-tip radius compensation
Turning cycles
Extended Tool Management software option
(option number #93)
Tool management that can be changed by the machine
manufacturer using Python scripts
TNC Model, Software and Features
8
Page 9
Feature content level (upgrade functions)
Along with software options, significant further improvements of the
TNC software are managed via the Feature Content Level (FCL)
upgrade functions. Functions subject to the FCL are not available
simply by updating the software on your TNC.
All upgrade functions are available to you without
surcharge when you receive a new machine.
Upgrade functions are identified in the manual with FCL n, where n
indicates the sequential number of the feature content level.
You can purchase a code number in order to permanently enable the
FCL functions. For more information, contact your machine tool
builder or HEIDENHAIN.
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
U Programming and Editing operating mode
U MOD function
U LICENSE INFO soft key
TNC Model, Software and Features
HEIDENHAIN TNC 640 9
Page 10
TNC Model, Software and Features
10
Page 11
Contents
First Steps with the TNC 640
1
Introduction
2
Programming: Fundamentals,
File Management
3
Programming: Programming Aids
4
Programming: Tools
5
Programming: Programming Contours
6
Programming: Subprograms and
Program Section Repeats
7
Programming: Q Parameters
8
Programming: Miscellaneous Functions
9
Programming: Special Functions
10
Programming: Multiple Axis Machining
11
Programming: Pallet Editor
12
Programming: Turning Operations
13
Manual Operation and Setup
14
Positioning with Manual Data Input
15
Test Run and Program Run
16
MOD Functions
17
Tables and Overviews
18
HEIDENHAIN TNC 640 11
Page 12
Page 13
1 First Steps with the TNC 640 ..... 35
1.1 Overview ..... 36
1.2 Machine Switch-On ..... 37
Acknowledging the power interruption and moving to the reference points ..... 37
1.3 Programming the First Part ..... 38
Selecting the correct operating mode ..... 38
The most important TNC keys ..... 38
Creating a new program/file management ..... 39
Defining a workpiece blank ..... 40
Program layout ..... 41
Programming a simple contour ..... 42
Creating a cycle program ..... 45
1.4 Graphically Testing the First Program ..... 48
Selecting the correct operating mode ..... 48
Selecting the tool table for the test run ..... 48
Choosing the program you want to test ..... 49
Selecting the screen layout and the view ..... 49
Starting the program test ..... 49
1.5 Tool Setup ..... 50
Selecting the correct operating mode ..... 50
Preparing and measuring tools ..... 50
The tool table TOOL.T ..... 50
The pocket table TOOL_P.TCH ..... 51
1.6 Workpiece Setup ..... 52
Selecting the correct operating mode ..... 52
Clamping the workpiece ..... 52
Aligning the workpiece with a 3-D touch probe system ..... 53
Datum setting with a 3-D touch probe ..... 54
1.7 Running the First Program ..... 55
Selecting the correct operating mode ..... 55
Choosing the program you want to run ..... 55
Starting the program ..... 55
HEIDENHAIN TNC 640 13
Page 14
2 Introduction ..... 57
2.1 The TNC 640 ..... 58
Programming: HEIDENHAIN conversational and ISO formats ..... 58
Compatibility ..... 58
2.2 Visual Display Unit and Keyboard ..... 59
Visual display unit ..... 59
Setting the screen layout ..... 60
Operating panel ..... 61
2.3 Operating Modes ..... 62
Manual Operation and El. Handwheel ..... 62
Positioning with Manual Data Input ..... 62
Programming and Editing ..... 63
Test Run ..... 63
Program Run, Full Sequence and Program Run, Single Block ..... 64
2.4 Status Displays ..... 65
"General" status display ..... 65
Additional status displays ..... 67
2.5 Window Manager ..... 74
Soft-key row ..... 75
2.6 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels ..... 76
3-D touch probes ..... 76
HR electronic handwheels ..... 77
14
Page 15
3 Programming: Fundamentals, File Management ..... 79
3.1 Fundamentals ..... 80
Position encoders and reference marks ..... 80
Reference system ..... 80
Reference system on milling machines ..... 81
Designation of the axes on milling machines ..... 81
Polar coordinates ..... 82
Absolute and incremental workpiece positions ..... 83
Setting the datum ..... 84
3.2 Creating and Writing Programs ..... 85
Organization of an NC program in HEIDENHAIN Conversational ..... 85
Define the blank: BLK FORM ..... 85
Creating a new part program ..... 86
Programming tool movements in conversational format ..... 88
Actual position capture ..... 90
Editing a program ..... 91
The TNC search function ..... 95
3.3 File Management: Fundamentals ..... 97
Files ..... 97
Showing externally created files on the TNC ..... 99
Data backup ..... 99
3.4 Working with the File Manager ..... 100
Directories ..... 100
Paths ..... 100
Overview: Functions of the file manager ..... 101
Calling the file manager ..... 102
Selecting drives, directories and files ..... 103
Creating a new directory ..... 105
Creating a new file ..... 105
Copying a single file ..... 106
Copying files into another directory ..... 107
Copying a table ..... 108
Copying a directory ..... 108
Choosing one of the last files selected ..... 109
Deleting a file ..... 109
Deleting a directory ..... 110
Marking files ..... 111
Renaming a file ..... 112
File sorting ..... 112
Additional functions ..... 113
Additional tools for management of external file types ..... 114
Data transfer to or from an external data medium ..... 119
The TNC in a network ..... 121
USB devices on the TNC ..... 122
HEIDENHAIN TNC 640 15
Page 16
4 Programming: Programming Aids ..... 123
4.1 Adding Comments ..... 124
Application ..... 124
Entering comments during programming ..... 124
Inserting comments after program entry ..... 124
Entering a comment in a separate block ..... 124
Functions for editing of the comment ..... 125
4.2 Display of NC Programs ..... 126
Syntax highlighting ..... 126
Scrollbar ..... 126
4.3 Structuring Programs ..... 127
Definition and applications ..... 127
Displaying the program structure window / Changing the active window ..... 127
Inserting a structuring block in the (left) program window ..... 127
Selecting blocks in the program structure window ..... 127
4.4 On-Line Calculator ..... 128
Operation ..... 128
4.5 Programming Graphics ..... 130
Generating / not generating graphics during programming ..... 130
Generating a graphic for an existing program ..... 130
Block number display ON/OFF ..... 131
Erasing the graphic ..... 131
Showing grid lines ..... 131
Magnifying or reducing a detail ..... 131
4.6 Error Messages ..... 132
Display of errors ..... 132
Open the error window ..... 132
Closing the error window ..... 132
Detailed error messages ..... 133
INTERNAL INFO soft key ..... 133
Clearing errors ..... 134
Error log ..... 134
Keystroke log ..... 135
Informational texts ..... 136
Saving service files ..... 136
Calling the TNCguide help system ..... 136
4.7 Context-Sensitive Help System ..... 137
Application ..... 137
Working with the TNCguide ..... 138
Downloading current help files ..... 142
16
Page 17
5 Programming: Tools ..... 145
5.1 Entering Tool-Related Data ..... 146
Feed rate F ..... 146
Spindle speed S ..... 147
5.2 Tool Data ..... 148
Requirements for tool compensation ..... 148
Tool numbers and tool names ..... 148
Tool length L ..... 148
Tool radius R ..... 148
Delta values for lengths and radii ..... 149
Entering tool data into the program ..... 149
Entering tool data in the table ..... 150
Pocket table for tool changer ..... 157
Calling tool data ..... 160
Tool change ..... 161
Tool management (software option) ..... 166
5.3 Tool Compensation ..... 173
Introduction ..... 173
Tool length compensation ..... 173
Tool radius compensation ..... 174
HEIDENHAIN TNC 640 17
Page 18
6 Programming: Programming Contours ..... 177
6.1 Tool Movements ..... 178
Path functions ..... 178
FK free contour programming ..... 178
Miscellaneous functions M ..... 178
Subprograms and program section repeats ..... 178
Programming with Q parameters ..... 178
6.2 Fundamentals of Path Functions ..... 179
Programming tool movements for workpiece machining ..... 179
6.3 Contour Approach and Departure ..... 183
Overview: Types of paths for contour approach and departure ..... 183
Important positions for approach and departure ..... 184
Approaching on a straight line with tangential connection: APPR LT ..... 186
Approaching on a straight line perpendicular to the first contour point: APPR LN ..... 186
Approaching on a circular path with tangential connection: APPR CT ..... 187
Approaching on a circular arc with tangential connection from a straight line to the contour: APPR LCT ..... 188
Departing on a straight line with tangential connection: DEP LT ..... 189
Departing on a straight line perpendicular to the last contour point: DEP LN ..... 189
Departing on a circular path with tangential connection: DEP CT ..... 190
Departing on a circular arc tangentially connecting the contour and a straight line: DEP LCT ..... 190
6.4 Path Contours—Cartesian Coordinates ..... 191
Overview of path functions ..... 191
Straight line L ..... 192
Inserting a chamfer between two straight lines ..... 193
Corner rounding RND ..... 194
Circle center CCI ..... 195
Circular path C around circle center CC ..... 196
Circular path CR with defined radius ..... 197
Circular path CT with tangential connection ..... 199
6.5 Path Contours—Polar Coordinates ..... 204
Overview ..... 204
Zero point for polar coordinates: pole CC ..... 205
Straight line LP ..... 205
Circular path CP around pole CC ..... 206
Circular path CTP with tangential connection ..... 207
Helical interpolation ..... 208
18
Page 19
6.6 Path Contours—FK Free Contour Programming ..... 212
Fundamentals ..... 212
Graphics during FK programming ..... 214
Initiating the FK dialog ..... 215
Pole for FK programming ..... 216
Free programming of straight lines ..... 216
Free programming of circular arcs ..... 217
Input possibilities ..... 218
Auxiliary points ..... 222
Relative data ..... 223
HEIDENHAIN TNC 640 19
Page 20
7 Programming: Subprograms and Program Section Repeats ..... 231
7.1 Labeling Subprograms and Program Section Repeats ..... 232
Labels ..... 232
7.2 Subprograms ..... 233
Operating sequence ..... 233
Programming notes ..... 233
Programming a subprogram ..... 233
Calling a subprogram ..... 233
7.3 Program Section Repeats ..... 234
Label LBL ..... 234
Operating sequence ..... 234
Programming notes ..... 234
Programming a program section repeat ..... 234
Calling a program section repeat ..... 234
7.4 Separate Program as Subprogram ..... 235
Operating sequence ..... 235
Programming notes ..... 235
Calling any program as a subprogram ..... 236
7.5 Nesting ..... 237
Types of nesting ..... 237
Nesting depth ..... 237
Subprogram within a subprogram ..... 238
Repeating program section repeats ..... 239
Repeating a subprogram ..... 240
7.6 Programming Examples ..... 241
20
Page 21
8 Programming: Q Parameters ..... 247
8.1 Principle and Overview ..... 248
Programming notes ..... 249
Calling Q-parameter functions ..... 250
8.2 Part Families—Q Parameters in Place of Numerical Values ..... 251
Application ..... 251
8.3 Describing Contours through Mathematical Operations ..... 252
Application ..... 252
Overview ..... 252
Programming fundamental operations ..... 253
8.4 Trigonometric Functions ..... 254
Definitions ..... 254
Programming trigonometric functions ..... 255
8.5 Circle Calculations ..... 256
Application ..... 256
8.6 If-Then Decisions with Q Parameters ..... 257
Application ..... 257
Unconditional jumps ..... 257
Programming If-Then decisions ..... 257
Abbreviations used: ..... 258
8.7 Checking and Changing Q Parameters ..... 259
Procedure ..... 259
8.8 Additional Functions ..... 261
Overview ..... 261
FN 14: ERROR: Displaying error messages ..... 262
FN 16: F-PRINT: Formatted output of text and Q-parameter values ..... 267
FN 18: SYS-DATUM READ ..... 271
FN 19: PLC: Transfer values to the PLC ..... 280
FN 20: WAIT FOR: NC and PLC synchronization ..... 280
FN 29: PLC: Transfer values to the PLC ..... 282
FN37: EXPORT ..... 283
8.9 Accessing Tables with SQL Commands ..... 284
Introduction ..... 284
A Transaction ..... 285
Programming SQL commands ..... 287
Overview of the soft keys ..... 287
SQL BIND ..... 288
SQL SELECT ..... 289
SQL FETCH ..... 292
SQL UPDATE ..... 293
SQL INSERT ..... 293
SQL COMMIT ..... 294
SQL ROLLBACK ..... 294
HEIDENHAIN TNC 640 21
Page 22
8.10 Entering Formulas Directly ..... 295
Entering formulas ..... 295
Rules for formulas ..... 297
Programming example ..... 298
8.11 String Parameters ..... 299
String processing functions ..... 299
Assigning string parameters ..... 300
Chain-linking string parameters ..... 301
Converting a numerical value to a string parameter ..... 302
Copying a substring from a string parameter ..... 303
Converting a string parameter to a numerical value ..... 304
Checking a string parameter ..... 305
Finding the length of a string parameter ..... 306
Comparing alphabetic priority ..... 307
Reading machine parameters ..... 308
8.12 Preassigned Q Parameters ..... 311
Values from the PLC: Q100 to Q107 ..... 311
Active tool radius: Q108 ..... 311
Tool axis: Q109 ..... 312
Spindle status: Q110 ..... 312
Coolant on/off: Q111 ..... 312
Overlap factor: Q112 ..... 312
Unit of measurement for dimensions in the program: Q113 ..... 313
Tool length: Q114 ..... 313
Coordinates after probing during program run ..... 313
Deviation between actual value and nominal value during automatic tool measurement with the TT 130 ..... 314
Tilting the working plane with mathematical angles: rotary axis coordinates calculated by the TNC ..... 314
Measurement results from touch probe cycles (see also User’s Manual for Touch Probe Cycles) ..... 315
8.13 Programming Examples ..... 317
22
Page 23
9 Programming: Miscellaneous Functions ..... 325
9.1 Entering Miscellaneous Functions M and STOP ..... 326
Fundamentals ..... 326
9.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant ..... 327
Overview ..... 327
9.3 Miscellaneous Functions for Coordinate Data ..... 328
Programming machine-referenced coordinates: M91/M92 ..... 328
Moving to positions in a non-tilted coordinate system with a tilted working plane: M130 ..... 330
9.4 Miscellaneous Functions for Contouring Behavior ..... 331
Machining small contour steps: M97 ..... 331
Machining open contour corners: M98 ..... 333
Feed rate factor for plunging movements: M103 ..... 334
Feed rate in millimeters per spindle revolution: M136 ..... 335
Feed rate for circular arcs: M109/M110/M111 ..... 336
Calculating the radius-compensated path in advance (LOOK AHEAD): M120 ..... 337
Superimposing handwheel positioning during program run: M118 ..... 339
Retraction from the contour in the tool-axis direction: M140 ..... 340
Suppressing touch probe monitoring: M141 ..... 341
Delete basic rotation: M143 ..... 341
Automatically retract tool from the contour at an NC stop: M148 ..... 342
HEIDENHAIN TNC 640 23
Page 24
10 Programming: Special Functions ..... 343
10.1 Overview of Special Functions ..... 344
Main menu for SPEC FCT special functions ..... 344
Program defaults menu ..... 345
Functions for contour and point machining menu ..... 345
Menu of various conversational functions ..... 346
10.2 Working with the Parallel Axes U, V and W ..... 347
Overview ..... 347
FUNCTION PARAXCOMP DISPLAY ..... 348
FUNCTION PARAXCOMP MOVE ..... 349
FUNCTION PARAXCOMP OFF ..... 350
FUNCTION PARAXMODE ..... 351
FUNCTION PARAXMODE OFF ..... 352
10.3 File Functions ..... 353
Application ..... 353
Defining file functions ..... 353
10.4 Defining Coordinate Transformations ..... 354
Overview ..... 354
TRANS DATUM AXIS ..... 354
TRANS DATUM TABLE ..... 355
TRANS DATUM RESET ..... 355
10.5 Creating Text Files ..... 356
Application ..... 356
Opening and exiting text files ..... 356
Editing texts ..... 357
Deleting and re-inserting characters, words and lines ..... 358
Editing text blocks ..... 359
Finding text sections ..... 360
24
Page 25
11 Programming: Multiple Axis Machining ..... 361
11.1 Functions for Multiple Axis Machining ..... 362
11.2 The PLANE Function: Tilting the Working Plane (Software Option 1) ..... 363
Introduction ..... 363
Define the PLANE function ..... 365
Position display ..... 365
Reset the PLANE function ..... 366
Defining the machining plane with spatial angles: PLANE SPATIAL ..... 367
Defining the machining plane with projection angles: PROJECTED PLANE ..... 369
Defining the machining plane with Euler angles: EULER PLANE ..... 371
Defining the working plane with two vectors: VECTOR PLANE ..... 373
Defining the working plane via three points: PLANE POINTS ..... 375
Defining the machining plane with a single, incremental spatial angle: PLANE RELATIVE ..... 377
Tilting the working plane through axis angle: PLANE AXIAL (FCL 3 function) ..... 378
Specifying the positioning behavior of the PLANE function ..... 380
11.3 Inclined-Tool Machining in a Tilted Plane (Software Option 2) ..... 385
Function ..... 385
Inclined-tool machining via incremental traverse of a rotary axis ..... 385
Inclined-tool machining via normal vectors ..... 386
11.4 Miscellaneous Functions for Rotary Axes ..... 387
Feed rate in mm/min on rotary axes A, B, C: M116 (software option 1) ..... 387
Shorter-path traverse of rotary axes: M126 ..... 388
Reducing display of a rotary axis to a value less than 360°: M94 ..... 389
Maintaining the position of the tool tip when positioning with tilted axes (TCPM): M128 (software option
2) ..... 390
Selecting tilting axes: M138 ..... 392
Compensating the machine’s kinematics configuration for ACTUAL/NOMINAL positions at end of block: M144
(software option 2) ..... 393
11.5 TCPM FUNCTION (Software Option 2) ..... 394
Function ..... 394
Defining the TCPM FUNCTION ..... 395
Mode of action of the programmed feed rate ..... 395
Interpretation of the programmed rotary axis coordinates ..... 396
Type of interpolation between the starting and end position ..... 397
Resetting the TCPM FUNCTION ..... 398
11.6 Three-Dimensional Tool Compensation (Software Option 2) ..... 399
Introduction ..... 399
Definition of a normalized vector ..... 400
Permissible tool shapes ..... 401
Using other tools: Delta values ..... 401
3-D compensation without TCPM ..... 402
Face milling: 3-D compensation with TCPM ..... 402
Peripheral milling: 3-D radius compensation with TCPM and radius compensation (RL/RR) ..... 404
HEIDENHAIN TNC 640 25
Page 26
12 Programming: Pallet Editor ..... 407
12.1 Pallet Editor ..... 408
Application ..... 408
Selecting a pallet table ..... 410
Exiting the pallet file ..... 410
Executing the pallet file ..... 411
26
Page 27
13 Programming: Turning Operations ..... 413
13.1 Turning Operations on Milling Machines (Software Option 50) ..... 414
Introduction ..... 414
13.2 Basis Functions (Software Option 50) ..... 415
Switching between milling/turning mode of operation ..... 415
Graphical display of turning operations ..... 417
Programming the speed ..... 418
Feed rate ..... 419
Tool call ..... 420
Tool compensation in the program ..... 420
Tool data ..... 421
Tool tip radius compensation TRC ..... 423
Recessing and undercutting ..... 424
Inclined turning ..... 431
13.3 Unbalance Functions ..... 433
Unbalance while turning ..... 433
Measure Unbalance cycle ..... 435
HEIDENHAIN TNC 640 27
Page 28
14 Manual Operation and Setup ..... 437
14.1 Switch-On, Switch-Off ..... 438
Switch-on ..... 438
Switch-off ..... 440
14.2 Moving the Machine Axes ..... 441
Note ..... 441
Moving the axis using the machine axis direction buttons ..... 441
Incremental jog positioning ..... 442
Traversing with the HR 410 electronic handwheel ..... 443
14.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M ..... 444
Application ..... 444
Entering values ..... 444
Changing the spindle speed and feed rate ..... 445
Activating feed-rate limitation ..... 446
14.4 Datum Setting without a 3-D Touch Probe ..... 447
Note ..... 447
Preparation ..... 447
Workpiece presetting with axis keys ..... 448
Datum management with the preset table ..... 449
14.5 Using the 3-D Touch Probe ..... 455
Overview ..... 455
Selecting touch probe cycles ..... 455
Writing the measured values from touch probe cycles in datum tables ..... 456
Writing the measured values from touch probe cycles in the preset table ..... 456
14.6 Calibrating a 3-D Touch Probe ..... 457
Introduction ..... 457
Calibrating the effective length ..... 458
Calibrating the effective radius and compensating center misalignment ..... 459
Displaying calibration values ..... 460
14.7 Compensating Workpiece Misalignment with a 3-D Touch Probe ..... 461
Introduction ..... 461
Measuring a basic rotation ..... 462
Saving a basic rotation in the preset table ..... 462
Displaying a basic rotation ..... 462
Canceling a basic rotation ..... 462
28
Page 29
14.8 Datum Setting with a 3-D Touch Probe ..... 463
Overview ..... 463
Datum setting in any axis ..... 463
Corner as datum ..... 464
Circle center as datum ..... 465
Measuring workpieces with a 3-D touch probe ..... 466
Using touch probe functions with mechanical probes or dial gauges ..... 469
14.9 Tilting the Working Plane (Software Option 1) ..... 470
Application, function ..... 470
Traversing reference points in tilted axes ..... 472
Position display in a tilted system ..... 472
Limitations on working with the tilting function ..... 472
Activating manual tilting ..... 473
Setting the current tool-axis direction as the active machining direction ..... 474
Setting the datum in a tilted coordinate system ..... 475
HEIDENHAIN TNC 640 29
Page 30
15 Positioning with Manual Data Input ..... 477
15.1 Programming and Executing Simple Machining Operations ..... 478
Positioning with Manual Data Input (MDI) ..... 478
Protecting and erasing programs in $MDI ..... 481
30
Page 31
16 Test Run and Program Run ..... 483
16.1 Graphics ..... 484
Application ..... 484
Setting the speed of the test run ..... 485
Overview of display modes ..... 486
Plan view ..... 486
Projection in 3 planes ..... 487
3-D view ..... 488
Magnifying details ..... 490
Repeating graphic simulation ..... 491
Displaying the tool ..... 491
Measuring the machining time ..... 492
3-D line graphics ..... 493
16.2 Showing the Blank in the Working Space ..... 495
Application ..... 495
16.3 Functions for Program Display ..... 496
Overview ..... 496
16.4 Test Run ..... 497
Application ..... 497
16.5 Program run ..... 499
Application ..... 499
Running a part program ..... 500
Interrupting machining ..... 501
Moving the machine axes during an interruption ..... 502
Resuming program run after an interruption ..... 503
Mid-program startup (block scan) ..... 504
Returning to the contour ..... 506
16.6 Automatic Program Start ..... 507
Application ..... 507
16.7 Optional block skip ..... 508
Application ..... 508
Inserting the "/" character ..... 508
Erasing the "/" character ..... 508
16.8 Optional Program-Run Interruption ..... 509
Application ..... 509
HEIDENHAIN TNC 640 31
Page 32
17 MOD Functions ..... 511
17.1 Selecting MOD Functions ..... 512
Selecting the MOD functions ..... 512
Changing the settings ..... 512
Exiting the MOD functions ..... 512
Overview of MOD functions ..... 513
17.2 Software Numbers ..... 514
Application ..... 514
17.3 Entering Code Numbers ..... 515
Application ..... 515
17.4 Setting the Data Interfaces ..... 516
Serial interfaces on the TNC 640 ..... 516
Application ..... 516
Setting the RS-232 interface ..... 516
Setting the baud rate (baudRate) ..... 516
Setting the protocol (protocol) ..... 516
Setting the data bits (dataBits) ..... 517
Parity check (parity) ..... 517
Setting the stop bits (stopBits) ..... 517
Setting the handshake (flowControl) ..... 517
Settings for data transfer with the TNCserver PC software ..... 518
Setting the operating mode of the external device (fileSystem) ..... 518
Software for data transfer ..... 519
17.5 Ethernet Interface ..... 521
Introduction ..... 521
Connection possibilities ..... 521
Configuring the TNC ..... 522
17.6 Position Display Types ..... 528
Application ..... 528
17.7 Unit of Measurement ..... 529
Application ..... 529
17.8 Displaying Operating Times ..... 530
Application ..... 530
32
Page 33
18 Tables and Overviews ..... 531
18.1 Machine-Specific User Parameters ..... 532
Application ..... 532
18.2 Pin Layouts and Connecting Cables for the Data Interfaces ..... 540
RS-232-C/V.24 interface for HEIDENHAIN devices ..... 540
Non-HEIDENHAIN devices ..... 541
Ethernet interface RJ45 socket ..... 541
18.3 Technical Information ..... 542
18.4 Exchanging the Buffer Battery ..... 549
HEIDENHAIN TNC 640 33
Page 34
34
Page 35
First Steps with the TNC 640
Page 36
1.1 Overview
This chapter is intended to help TNC beginners quickly learn to handle
the most important procedures. For more information on a respective
topic, see the section referred to in the text.
The following topics are included in this chapter:
Machine Switch-On
1.1 Overview
Programming the First Part
Graphically Testing the First Program
Tool Setup
Workpiece Setup
Running the First Program
36 First Steps with the TNC 640
Page 37
1.2 Machine Switch-On
Acknowledging the power interruption and moving to the reference points
Switch-on and crossing the reference points can vary
depending on the machine tool. Your machine manual
provides more detailed information.
U Switch on the power supply for control and machine. The TNC starts
the operating system. This process may take several minutes. Then
the TNC will display the message "Power interruption."
U Press the CE key: The TNC compiles the PLC program
U Switch on the control voltage: The TNC checks
operation of the emergency stop circuit and goes into
the reference run mode
U Cross the reference points manually in the displayed
sequence: For each axis press the machine START
button. If you have absolute linear and angle encoders
on your machine there is no need for a reference run
The TNC is now ready for operation in the Manual Operation mode.
Further information on this topic
Traversing the reference marks: See "Switch-on" on page 438
Operating modes: See "Programming and Editing" on page 63
1.2 Machine Switch-On
HEIDENHAIN TNC 640 37
Page 38
1.3 Programming the First Part
Selecting the correct operating mode
You can write programs only in the Programming and Editing mode:
U Press the operating modes key: The TNC goes into
the Programming and Editing mode
Further information on this topic
Operating modes: See "Programming and Editing" on page 63
The most important TNC keys
Functions for conversational guidance Key
Confirm entry and activate the next dialog
prompt
Ignore the dialog question
1.3 Programming the First Part
End the dialog immediately
Abort dialog, discard entries
Soft keys on the screen with which you select
functions appropriate to the active state
Further information on this topic
Writing and editing programs: See "Editing a program" on page 91
Overview of keys: See "Controls of the TNC" on page 2
38 First Steps with the TNC 640
Page 39
Creating a new program/file management
U Press the PGM MGT key: The TNC displays the file
management. The file management of the TNC is
arranged much like the file management on a PC with
the Windows Explorer. The file management enables
you to manipulate data on the TNC hard disk
U Use the arrow keys to select the folder in which you
want to open the new file
U Enter a file name with the extension .H: The TNC then
automatically opens a program and asks for the unit
of measure for the new program
U To select the unit of measure, press the MM or INCH
soft key: The TNC automatically starts the workpiece
blank definition (see "Defining a workpiece blank" on
page 40)
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" on page 100
Creating a new program: See "Creating and Writing Programs" on
page 85
1.3 Programming the First Part
HEIDENHAIN TNC 640 39
Page 40
Defining a workpiece blank
Y
X
Z
MAX
MIN
-40
100
100
0
0
Immediately after you have created a new program, the TNC starts the
dialog for entering the workpiece blank definition. Always define the
workpiece blank as a cuboid by entering the MIN and MAX points,
each with reference to the selected reference point.
After you have created a new program, the TNC automatically initiates
the workpiece blank definition and asks for the required data:
U Working plane in graphic: XY?: Enter the active spindle axis. Z is
saved as default setting. Accept with the ENT key
U Workpiece blank def.: Minimum X: Enter the smallest X coordinate
of the workpiece blank with respect to the reference point, e.g. 0.
Confirm with the ENT key
U Workpiece blank def.: Minimum Y: Enter the smallest Y coordinate
of the workpiece blank with respect to the reference point, e.g. 0.
Confirm with the ENT key
U Workpiece blank def.: Minimum Z: Enter the smallest Z coordinate
of the workpiece blank with respect to the reference point, e.g. –40.
Confirm with the ENT key
U Workpiece blank def.: Maximum X: Enter the largest X coordinate
1.3 Programming the First Part
of the workpiece blank with respect to the reference point, e.g. 100.
Confirm with the ENT key
U Workpiece blank def.: Maximum Y: Enter the largest Y coordinate
of the workpiece blank with respect to the reference point, e.g. 100.
Confirm with the ENT key
U Workpiece blank def.: Maximum Z: Enter the 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: (see page 86)
40 First Steps with the TNC 640
Page 41
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
pre-position immediately to workpiece depth. If required, switch
on the spindle/coolant
5 Move to the contour
6 Machine the contour
7 Leave the contour
8 Retract the tool, end the program
Further information on this topic:
Contour programming: See "Tool Movements" on page 178
Recommended program layout for simple cycle programs
1 Call tool, define tool axis
2 Retract the tool
3 Define the machining positions
4 Define the fixed cycle
5 Call the cycle, switch on the spindle/coolant
6 Retract the tool, end the program
Further information on this topic:
Cycle programming: See User’s Manual for Cycles
Example: Layout of contour machining programs
0 BEGIN PGM BSPCONT MM
1 BLK FORM 0.1 Z X... Y... Z...
2 BLK FORM 0.2 X... Y... Z...
3 TOOL CALL 5 Z S5000
4 L Z+250 R0 FMAX
5 L X... Y... R0 FMAX
6 L Z+10 R0 F3000 M13
7 APPR ... RL F500
...
16 DEP ... X... Y... F3000 M9
17 L Z+250 R0 FMAX M2
18 END PGM BSPCONT MM
Example: Program layout for cycle programming
0 BEGIN PGM BSBCYC MM
1 BLK FORM 0.1 Z X... Y... Z...
2 BLK FORM 0.2 X... Y... Z...
3 TOOL CALL 5 Z S5000
4 L Z+250 R0 FMAX
5 PATTERN DEF POS1( X... Y... Z... ) ...
6 CYCL DEF...
7 CYCL CALL PAT FMAX M13
8 L Z+250 R0 FMAX M2
9 END PGM BSBCYC MM
1.3 Programming the First Part
HEIDENHAIN TNC 640 41
Page 42
Programming a simple contour
X
Y
9
5
95
5
10
10
20
20
1
4
2
3
The contour shown to the right is to be milled once to a depth of 5 mm.
You have already defined the workpiece blank. After you have initiated
a dialog through a function key, enter all the data requested by the
TNC in the screen header.
U Call the tool: Enter the tool data. Confirm each of your
entries with the ENT key. Do not forget the tool axis
U Retract the tool: Press the orange axis key Z in order
to get clear in the tool axis, and enter the value for the
position to be approached, e.g. 250. Confirm with the
ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Confirm the Miscellaneous function M? with the
END key: The TNC saves the entered positioning
block
1.3 Programming the First Part
U Preposition the tool in the working plane: Press the
orange X axis key and enter the value for the position
to be approached, e.g. –20
U Press the orange Y axis key and enter the value for the
position to be approached, e.g. –20. Confirm with the
ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Confirm the Miscellaneous function M? with the
END key: The TNC saves the entered positioning
block
U Move the tool to workpiece depth: Press the orange
axis key and enter the value for the position to be
approached, e.g. –5. Confirm with the ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
U Feed rate F=? Enter the positioning feed rate, e.g.
3000 mm/min and confirm with the ENT key
U Miscellaneous function M? Switch on the spindle and
coolant, e.g. M13. Confirm with the END key: The TNC
saves the entered positioning block
42 First Steps with the TNC 640
Page 43
U Move to the contour: Press the APPR/DEP key: The
TNC shows a soft-key row with approach and
departure functions
U Select the approach function APPR CT: Enter the
coordinates of the contour starting point 1 in X and Y,
e.g. 5/5. Confirm with the ENT key
U Center angle? Enter the approach angle, e.g. 90°, and
confirm with the ENT key
U Circle radius? Enter the approach radius, e.g. 8 mm,
and confirm with the ENT key
U Confirm the Radius comp.: RL/RR/no comp? with the
RL soft key: Activate the radius compensation to the
left of the programmed contour
U Feed rate F=? Enter the machining feed rate, e.g. 700
mm/min, and confirm your entry with the END key
U Machine the contour and move to contour point 2: You
only need to enter the information that changes. In
other words, enter only the Y coordinate 95 and save
your entry with the END key
U Move to contour point 3: Enter the X coordinate 95
and save your entry with the END key
U Define the chamfer at contour point 3: Enter the
chamfer width 10 mm and save with the END key
U Move to contour point 4: Enter the Y coordinate 5 and
save your entry with the END key
U Define the chamfer at contour point 4: Enter the
chamfer width 20 mm and save with the END key
U Move to contour point 1: Enter the X coordinate 5 and
save your entry with the END key
1.3 Programming the First Part
HEIDENHAIN TNC 640 43
Page 44
U Depart the contour
U Select the departure function DEP CT
U Center angle? Enter the departure angle, e.g. 90°, and
confirm with the ENT key
U Circle radius? Enter the departure radius, e.g. 8 mm,
and confirm with the ENT key
U Feed rate F=? Enter the positioning feed rate, e.g.
3000 mm/min and save it with the ENT key
U Miscellaneous function M? Switch off the coolant,
e.g. M9, with the END key: The TNC saves the entered
positioning block
U Retract the tool: Press the orange axis key Z in order
to get clear in the tool axis, and enter the value for the
position to be approached, e.g. 250. Confirm with the
ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
1.3 Programming the First Part
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Miscellaneous function M? Enter M2 to end the
program and confirm with the END key: The TNC
saves the entered positioning block
Further information on this topic
Complete example with NC blocks: See "Example: Linear
movements and chamfers with Cartesian coordinates" on page 200
Creating a new program: See "Creating and Writing Programs" on
page 85
Approaching/departing contours: See "Contour Approach and
Departure" on page 183
Programming contours: See "Overview of path functions" on page
191
Programmable feed rates: See "Possible feed rate input" on page 89
Tool radius compensation: See "Tool radius compensation" on page
174
Miscellaneous functions (M): See "Miscellaneous Functions for
Program Run Control, Spindle and Coolant" on page 327
44 First Steps with the TNC 640
Page 45
Creating a cycle program
X
Y
20
10
100
100
10
90
9080
The holes (depth of 20 mm) shown in the figure at right are to be drilled
with a standard drilling cycle. You have already defined the workpiece
blank.
U Call the tool: Enter the tool data. Confirm each of your
entries with the ENT key. Do not forget the tool axis
U Retract the tool: Press the orange axis key Z in order
to get clear in the tool axis, and enter the value for the
position to be approached, e.g. 250. Confirm with the
ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Confirm the Miscellaneous function M? with the
END key: The TNC saves the entered positioning
block
U Call the cycle menu
U Display the drilling cycles
U Select the standard drilling cycle 200: The TNC starts
the dialog for cycle definition. Enter all parameters
requested by the TNC step by step and conclude each
entry with the ENT key. In the screen to the right, the
TNC also displays a graphic showing the respective
cycle parameter
1.3 Programming the First Part
HEIDENHAIN TNC 640 45
Page 46
U Call the menu for special functions
U Display the functions for point machining
U Select the pattern definition
U Select point entry: Enter the coordinates of the 4
points and confirm each with the ENT key. After
entering the fourth point, save the block with the END
key
U Display the menu for defining the cycle call
U Run the drilling cycle on the defined pattern:
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Miscellaneous function M? Switch on the spindle and
coolant, e.g. M13. Confirm with the END key: The TNC
saves the entered positioning block
U Retract the tool: Press the orange axis key Z in order
1.3 Programming the First Part
to get clear in the tool axis, and enter the value for the
position to be approached, e.g. 250. Confirm with the
ENT key
U Confirm Radius comp.: RL/RR/no comp? by pressing
the ENT key: Do not activate the radius compensation
U Confirm Feed rate F=? with the ENT key: Move at
rapid traverse (FMAX)
U Miscellaneous function M? Enter M2 to end the
program and confirm with the END key: The TNC
saves the entered positioning block
Example NC blocks
0 BEGIN PGM C200 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
Definition of workpiece blank
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
Tool call
Retract the tool
Define machining positions
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)
46 First Steps with the TNC 640
Page 47
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 DEPTH
7 CYCL CALL PAT FMAX M13
8 L Z+250 R0 FMAX M2
9 END PGM C200 MM
Further information on this topic
Creating a new program: See "Creating and Writing Programs" on
page 85
Cycle programming: See User’s Manual for Cycles
Define the cycle
Spindle and coolant on, call the cycle
Retract in the tool axis, end program
1.3 Programming the First Part
HEIDENHAIN TNC 640 47
Page 48
1.4 Graphically Testing the First
Program
Selecting the correct operating mode
You can test programs only in the Test Run mode:
U Press the operating modes key: The TNC goes into
the Test Run mode
Further information on this topic
Operating modes of the TNC: See "Operating Modes" on page 62
Testing programs: See "Test Run" on page 497
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.
U Press the PGM MGT key: The TNC displays the file
manager
U Press the SELECT TYPE soft key: The TNC shows a
soft-key menu for selection of the file type to be
displayed
U Press the SHOW ALL soft key: The TNC shows all
saved files in the right window
1.4 Graphically Testing the First Program
U Move the highlight to the left onto the directories
U Move the highlight to the TNC:\ directory
U Move the highlight to the right onto the files
U Move the highlight to the file TOOL.T (active tool
table) and load with the ENT key: TOOL.T receives
the status S and is therefore active for the Test Run
U Press the END key: Leave the file manager
Further information on this topic
Tool management: See "Entering tool data in the table" on page 150
Testing programs: See "Test Run" on page 497
48 First Steps with the TNC 640
Page 49
Choosing the program you want to test
U Press the PGM MGT key: The TNC displays the file
manager
U Press the LAST FILES soft key: The TNC opens a
pop-up window with the most recently selected files
U Use the arrow keys to select the program that you
want to test. Load with the ENT key
Further information on this topic
Selecting a program: See "Working with the File Manager" on page
100
Selecting the screen layout and the view
U Press the key for selecting the screen layout. The TNC
shows all available alternatives in the soft-key row
U Press the PROGRAM + GRAPHICS soft key: In the
left half of the screen the TNC shows the program; in
the right half it shows the workpiece blank
U Select the desired view via soft key
U Plan view
U Projection in three planes
U 3-D view
Further information on this topic
Graphic functions: See "Graphics" on page 484
Running a test run: See "Test Run" on page 497
Starting the program test
U Press the RESET + START soft key: The TNC
simulates the active program up to a programmed
break or to the program end
U While the simulation is running, you can use the soft
keys to change views.
U Press the STOP soft key: The TNC interrupts the test
run
U Press the START soft key: The TNC resumes the test
run after a break
Further information on this topic
Running a test run: See "Test Run" on page 497
Graphic functions: See "Graphics" on page 484
Adjusting the test speed: See "Setting the speed of the test run" on
page 485
1.4 Graphically Testing the First Program
HEIDENHAIN TNC 640 49
Page 50
1.5 Tool Setup
Selecting the correct operating mode
Tools are set up in the Manual Operation mode:
U Press the operating modes key: The TNC goes into
the Manual Operation mode
Further information on this topic
1.5 Tool Setup
Operating modes of the TNC: See "Operating Modes" on page 62
Preparing and measuring tools
U Clamp the required tools in their chucks
U When measuring with an external tool presetter: Measure the tools,
note down the length and radius, or transfer them directly to the
machine through a transfer program
U When measuring on the machine: Place the tools into the tool
changer (see page 51)
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 tool-specific
information that the TNC needs to perform its functions.
To enter tool data in the tool table TOOL.T, proceed as follows:
U Display the tool table
U Edit the tool table: Set the EDITING soft key to ON
U With the upward or downward arrow keys you can
select the tool number that you want to edit
U With the rightward or leftward arrow keys you can
select the tool data that you want to edit
U To leave the tool table, press the END key
Further information on this topic
Operating modes of the TNC: See "Operating Modes" on page 62
Working with the tool table: See "Entering tool data in the table" on
page 150
50 First Steps with the TNC 640
Page 51
The pocket table TOOL_P.TCH
The function of the pocket table depends on the machine.
Your machine manual provides more detailed information.
In the pocket table TOOL_P.TCH (permanently saved under
TNC:\TABLE\) you specify which tools your tool magazine contains.
To enter data in the pocket table TOOL_P.TCH, proceed as follows:
U Display the tool table
U Display the pocket table
U Edit the pocket table: Set the EDITING soft key to ON
U With the upward or downward arrow keys you can
select the pocket number that you want to edit
U With the rightward or leftward arrow keys you can
select the data that you want to edit
U To leave the pocket table, press the END key
Further information on this topic
Operating modes of the TNC: See "Operating Modes" on page 62
Working with the pocket table: See "Pocket table for tool changer"
on page 157
1.5 Tool Setup
HEIDENHAIN TNC 640 51
Page 52
1.6 Workpiece Setup
Selecting the correct operating mode
Workpieces are set up in the Manual Operation or Electronic
Handwheel mode
U Press the operating modes key: The TNC goes into
the Manual Operation mode
Further information on this topic
Manual Operation mode: See "Moving the Machine Axes" on page
441
1.6 Workpiece Setup
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.
52 First Steps with the TNC 640
Page 53
Aligning the workpiece with a 3-D touch probe system
U Insert the 3-D touch probe: In the Manual Data Input (MDI) operating
mode, run a TOOL CALL block containing the tool axis, and then return
to the Manual Operation mode (in MDI mode you can run an
individual NC block independently of the others)
U Select the probing functions: The TNC displays the
available functions in the soft-key row
U Measure the basic rotation: The TNC displays the
basic rotation menu. To identify the basic rotation,
probe two points on a straight surface of the
workpiece
U Use the axis-direction keys to pre-position the touch
probe to a position near the first contact point
U Select the probing direction via soft key
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Use the axis-direction keys to pre-position the touch
probe to a position near the second contact point
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Then the TNC shows the measured basic rotation
U Press SET BASIC ROTATION soft key to select the
displayed value as the active rotation. Press the END
soft key to exit the menu
1.6 Workpiece Setup
Further information on this topic
MDI operating mode: See "Programming and Executing Simple
Machining Operations" on page 478
Workpiece alignment: See "Compensating Workpiece Misalignment
with a 3-D Touch Probe" on page 461
HEIDENHAIN TNC 640 53
Page 54
Datum setting with a 3-D touch probe
U Insert the 3-D touch probe: In the MDI mode, run a TOOL CALL block
containing the tool axis and then return to the Manual Operation
mode
U Select the probing functions: The TNC displays the
available functions in the soft-key row
U Set the datum at a workpiece corner, for example
U Position the touch probe near the first touch point on
the first workpiece edge
U Select the probing direction via soft key
1.6 Workpiece Setup
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Use the axis-direction keys to pre-position the touch
probe to a position near the second touch point on the
first workpiece edge
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Use the axis-direction keys to pre-position the touch
probe to a position near the first touch point on the
second workpiece edge
U Select the probing direction via soft key
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Use the axis-direction keys to pre-position the touch
probe to a position near the second touch point on the
second workpiece edge
U Press NC start: The touch probe moves in the defined
direction until it contacts the workpiece and then
automatically returns to its starting point
U Then the TNC shows the coordinates of the measured
corner point
U Set to 0: Press the SET DATUM soft key
U Press the END soft key to close the menu
Further information on this topic
Datum setting: See "Datum Setting with a 3-D Touch Probe" on page
463
54 First Steps with the TNC 640
Page 55
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:
U Press the operating mode key: The TNC goes into the
Program Run, Single Block mode and the TNC
executes the program block by block. You have to
confirm each block with the NC start key
U Press the operating mode key: The TNC goes into the
Program Run, Full Sequence mode and the TNC
executes the program after NC start up to a program
break or to the end of the program
Further information on this topic
Operating modes of the TNC: See "Operating Modes" on page 62
Running programs: See "Program run" on page 499
Choosing the program you want to run
U Press the PGM MGT key: The TNC displays the file
manager
U Press the LAST FILES soft key: The TNC opens a pop-
up window with the most recently selected files
U If desired, use the arrow keys to select the program
that you want to run. Load with the ENT key
Further information on this topic
File management: See "Working with the File Manager" on page 100
Starting the program
U Press the NC start button: The TNC executes the
active program
Further information on this topic
Running programs: See "Program run" on page 499
1.7 Running the First Program
HEIDENHAIN TNC 640 55
Page 56
1.7 Running the First Program
56 First Steps with the TNC 640
Page 57
Introduction
Page 58
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
2.1 The TNC 640
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 HEIDENHAIN FK
free contour programming 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.
Please also note the detailed description of the differences
between the iTNC 530 and the TNC 640 (see "Comparison:
Functions of the TNC 640 and the iTNC 530" on page 555).
58 Introduction
Page 59
2.2 Visual Display Unit and
1
3
4
4
5
77
8
2
1
6
7
Keyboard
Visual display unit
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 soft-key
row. You can select these functions by pressing the keys
immediately below them. The lines immediately above the softkey row indicate the number of soft-key rows that can be called
with the black arrow keys to the right and left. The bar
representing the active soft-key row is highlighted.
3 Soft-key selection keys
4 Switching the 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
2.2 Visual Display Unit and Keyboard
HEIDENHAIN TNC 640 59
Page 60
Setting the screen layout
You select the screen layout yourself: In the PROGRAMMING AND
EDITING mode of operation, for example, you can have the TNC show
program blocks in the left window while the right window displays
programming graphics. You could also display the program structure
in the right window instead, or display only program blocks in one large
window. The available screen windows depend on the selected
operating mode.
To change the screen layout:
Press the SPLIT SCREEN key: The soft-key row
shows the available layout options (see "Operating
Modes", page 62)
Select the desired screen layout
2.2 Visual Display Unit and Keyboard
60 Introduction
Page 61
Operating panel
1
9
5
8
1
3
2
4
6
7
10
The TNC 640 is delivered with an integrated keyboard. The figure at
right shows the controls and displays of the keyboard:
1 Alphabetic keyboard for entering texts and file names, and for
ISO programming.
2 File manager
On-line calculator
MOD function
HELP function
3 Programming modes
4 Machine operating modes
5 Initiation of programming dialog
6 Arrow keys and GOTO jump command
7 Numerical input and axis selection
8 Touchpad
9 Navigation keys
10 USB connection
The functions of the individual keys are described on the inside front
cover.
Some machine manufacturers do not use the standard
operating panel from HEIDENHAIN. Please refer to your
machine manual in these cases.
Machine panel buttons, e.g. NC START or NC STOP, are
described in the manual for your machine tool.
2.2 Visual Display Unit and Keyboard
HEIDENHAIN TNC 640 61
Page 62
2.3 Operating Modes
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
2.3 Operating Modes
Positions
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 pre-positioning.
Soft keys for selecting the screen layout
Window Soft key
Program
Left: program blocks, right: status display
62 Introduction
Page 63
Programming and Editing
In this mode of operation you can write your part programs.
The FK free programming feature, the various cycles and the
Q parameter functions help you with programming and add necessary
information. If desired, 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 blocks, right: graphics
Test Run
In the Test Run mode of operation, the TNC checks programs and
program sections for errors, such as geometrical incompatibilities,
missing or incorrect data within the program or violations of the
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 64.
2.3 Operating Modes
HEIDENHAIN TNC 640 63
Page 64
Program Run, Full Sequence and Program Run, Single Block
In the Program Run, Full Sequence mode of operation the TNC
executes a part program continuously to its end or to a manual or
programmed stop. You can resume program run after an interruption.
In the Program Run, Single Block mode of operation you execute each
block separately by pressing the machine START button.
Soft keys for selecting the screen layout
Window Soft key
Program
2.3 Operating Modes
Left: program, right: program structure
Left: program, right: status
Left: program, right: graphics
Graphics
Soft keys for selecting the screen layout for pallet tables (software
option Pallet management)
Window Soft key
Pallet table
Left: program blocks, right: pallet table
Left: pallet table, right: status
64 Introduction
Page 65
2.4 Status Displays
ACTL.
X Y Z
F S M
"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
Symbol Meaning
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.
2.4 Status Displays
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
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.
HEIDENHAIN TNC 640 65
Page 66
Symbol Meaning
No active program
Program run has started
Program run is stopped
Program run is being aborted
2.4 Status Displays
Turning mode is active
66 Introduction
Page 67
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
2.4 Status Displays
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.
HEIDENHAIN TNC 640 67
Page 68
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
2.4 Status Displays
General program information (PGM tab)
Soft key Meaning
No direct
selection
possible
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
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
68 Introduction
Page 69
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
2.4 Status Displays
HEIDENHAIN TNC 640 69
Page 70
Active miscellaneous functions M (M tab)
Soft key Meaning
No direct
selection
possible
List of the active M functions with fixed meaning
List of the active M functions that are adapted by
your machine manufacturer
2.4 Status Displays
70 Introduction
Page 71
Positions and coordinates (POS tab)
Soft key Meaning
Type of position display, e.g. actual position
Tilt angle of the working plane
Angle of a basic rotation
Information on tools (TOOL tab)
Soft key Meaning
T: Tool number and name
RT: Number and name of a replacement tool
Tool axis
Tool lengths and radii
Oversizes (delta values) from the tool table (TAB) and
the TOOL CALL (PGM)
Tool age, maximum tool age (TIME 1) and maximum
tool age for TOOL CALL (TIME 2)
Display of the active tool and the (next) replacement
tool
2.4 Status Displays
HEIDENHAIN TNC 640 71
Page 72
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
2.4 Status Displays
Coordinate transformations (TRANS tab)
Soft key Meaning
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
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
For further information, refer to the User's Manual for Cycles,
"Coordinate Transformation Cycles."
72 Introduction
Page 73
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
Press the Q PARAMETER LIST soft key. The TNC opens a
pop-up window in which you can enter the desired range
for display of the Q parameters or string parameters.
Multiple Q parameters are entered separated by commas
(e.g. Q 1,2,3,4). To define display ranges, enter a hyphen
(e.g. Q 10-14).
2.4 Status Displays
HEIDENHAIN TNC 640 73
Page 74
2.5 Window Manager
The machine tool builder determines the scope of function
and behavior of the window manager. The machine tool
manual provides further information.
The TNC features the Xfce window manager. Xfce is a standard
application for UNIX-based operating systems, and is used to manage
graphical user interfaces. The following functions are possible with the
window manager:
Display a task bar for switching between various applications (user
interfaces).
Manage an additional desktop, on which special applications from
2.5 Window Manager
your machine tool builder can run.
Control the focus between NC-software applications and those of
the machine tool builder.
The size and position of pop-up windows can be changed. It is also
possible to close, minimize and restore the pop-up windows.
The TNC shows a star in the upper left of the screen if an
application of the window manager or the window
manager itself has caused an error. In this case, switch to
the window manager and correct the problem. If required,
refer to your machine manual.
74 Introduction
Page 75
Soft-key row
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 operation 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 Management:
Fundamentals" on page 97)
2.5 Window Manager
HEIDENHAIN TNC 640 75
Page 76
2.6 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 touch probe functions are described in the
User’s Manual for Cycle Programming. Please contact
HEIDENHAIN if you need a copy of this User’s Manual.
ID: 892 905-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 costeffective alternative for applications where digitizing is not frequently
required.
The TS 640 (see figure) and the smaller TS 440 feature infrared
transmission of the triggering signal to the TNC. This makes them
highly convenient for use on machines with automatic tool changers.
Principle of operation: HEIDENHAIN triggering touch probes feature a
wear resisting optical switch that generates an electrical signal as
soon as the stylus is deflected. This signal is transmitted to the
control, which stores the current position of the stylus as the actual
value.
2.6 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels
76 Introduction
Page 77
TT 140 tool touch probe for tool measurement
The TT 140 is a triggering 3-D touch probe for tool measurement and
inspection. Your TNC provides three cycles for this touch probe with
which you can measure the tool length and radius automatically either
with the spindle rotating or stopped. The TT 140 features a particularly
rugged design and a high degree of protection, which make it
insensitive to coolants and swarf. The triggering signal is generated by
a wear-resistant and highly reliable optical switch.
HR electronic handwheels
Electronic handwheels facilitate moving the axis slides precisely by
hand. A wide range of traverses per handwheel revolution is available.
Apart from the HR 130 and HR 150 panel-mounted handwheels,
HEIDENHAIN also offers the HR 410 portable handwheel.
HEIDENHAIN TNC 640 77
2.6 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels
Page 78
2.6 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels
78 Introduction
Page 79
Programming: Fundamentals, File Management
Page 80
3.1 Fundamentals
Y
X
Z
X (Z,Y)
X
MP
Y
X
Z
Position encoders and reference marks
The machine axes are equipped with position encoders that register
the positions of the machine table or tool. Linear axes are usually
equipped with linear encoders, rotary tables and tilting axes with angle
encoders.
When a machine axis moves, the corresponding position encoder
generates an electrical signal. The TNC evaluates this signal and
calculates the precise actual position of the machine axis.
3.1 Fundamentals
If there is a power interruption, the calculated position will no longer
correspond to the actual position of the machine slide. To recover this
association, incremental position encoders are provided with
reference marks. The scales of the position encoders contain one or
more reference marks that transmit a signal to the TNC when they are
crossed over. From that signal the TNC can re-establish the
assignment of displayed positions to machine positions. For linear
encoders with distance-coded reference marks, the machine axes
need to move by no more than 20 mm, for angle encoders by no more
than 20°.
With absolute encoders, an absolute position value is transmitted to
the control immediately upon switch-on. In this way the assignment
of the actual position to the machine slide position is re-established
directly after switch-on.
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.
80 Programming: Fundamentals, File Management
Page 81
Reference system on milling machines
+X
+Y
+Z
+X
+Z
+Y
W+
C+
B+
V+
A+
U+
Y
X
Z
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.
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 minor axis (2nd axis). The assignment
of the tool axis is decisive for the assignment of the principal and
minor axes.
Tool axis Principal axis Minor axis
XYZ
YZX
3.1 Fundamentals
ZXY
HEIDENHAIN TNC 640 81
Page 82
Polar coordinates
X
Y
0°
30
10
CC
PR
PA
1
PA
2
PR
PR
PA
3
X
Z
Y
X
Z
Y
X
Z
Y
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 two-dimensional
and describe points in a plane. Polar coordinates have their datum at a
circle center (CC), or pole. A position in a plane can be clearly defined
by the:
Polar Radius, the distance from the circle center CC to the position,
3.1 Fundamentals
and the
Polar Angle, the value of the angle between the 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) Angle reference axis
X/Y +X
Y/Z +Y
Z/X +Z
82 Programming: Fundamentals, File Management
Page 83
Absolute and incremental workpiece positions
X
Y
2
1
3
10 30 50
10
20
30
X
Y
20
10 10
20
10
10
5
4
6
X
Y
0°
30
10
CC
PR
PA
+IPA
PR
PR
+IPA
+IPR
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 a chain dimensions.
To program a position in incremental coordinates, enter the function "I"
before the axis.
Example 2: Holes dimensioned in incremental coordinates
Absolute coordinates of hole 4
X = 10 mm
Y = 10 mm
Hole 5, with respect to 4 Hole 6, with respect to 5
X = 20 mm X = 20 mm
Y = 10 mm Y = 10 mm
3.1 Fundamentals
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.
HEIDENHAIN TNC 640 83
Page 84
Setting the datum
Y
X
Z
MAX
MIN
X
Y
325
320
0
450 900
950
150
-150
750
0
300
±
0,1
21
3 4
7
6
5
A production drawing identifies a certain form element of the
workpiece, usually a corner, as the absolute datum. When setting the
datum, you first align the workpiece along the machine axes, and then
move the tool in each axis to a defined position relative to the
workpiece. Set the display of the TNC either to zero or to a known
position value for each position. This establishes the reference system
for the workpiece, which will be used for the TNC display and your part
program.
If the production drawing is dimensioned in relative coordinates,
simply use the coordinate transformation cycles (see User’s Manual
3.1 Fundamentals
for Cycles, Cycles for Coordinate Transformation).
If the production drawing is not dimensioned for NC, set the datum at
a position or corner on the workpiece 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 Touch Probe Cycles User’s Manual.
Example
The workpiece drawing shows holes (1 to 4) whose dimensions are
shown with respect to an absolute datum with the coordinates X=0
Y=0. Holes 5 to 7 are dimensioned with respect to a relative datum
with the absolute coordinates X=450, Y=750. With the DATUM SHIFT
cycle you can temporarily set the datum to the position X=450, Y=750,
to be able to program holes 5 to 7 without further calculations.
84 Programming: Fundamentals, File Management
Page 85
3.2 Creating and Writing Programs
10 L X+10 Y+5 R0 F100 M3
Block number
Path function
Words
Block
Organization of an NC program in HEIDENHAIN Conversational
A part program consists of a series of program blocks. The figure at
right illustrates the elements of a block.
The TNC numbers the blocks in ascending sequence.
The first block of a program is identified by BEGIN PGM, the program
name and the active unit of measure.
The subsequent blocks contain information on:
Workpiece blank
Tool calls
Approaching a safe position
Feed rates and spindle speeds, as well as
Path contours, cycles and other functions
The last block of a program is identified by END PGM the program name
and the active unit of measure.
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 blank form is
defined by two of its corner points:
MIN point: the smallest X, Y and Z coordinates of the blank form,
entered as absolute values
MAX point: the largest X, Y and Z coordinates of the blank form,
entered as absolute or incremental values
You only need to define the workpiece blank if you wish
to run a graphic test for the program!
3.2 Creating and Writing Programs
HEIDENHAIN TNC 640 85
Page 86
Creating a new part program
You always enter a part program in the Programming and Editing
mode of operation. An example of program initiation:
Select the Programming and Editing operating mode
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
3.2 Creating and Writing Programs
WORKING PLANE IN GRAPHIC: XY
initiates the dialog for defining the BLK FORM
(workpiece blank)
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
86 Programming: Fundamentals, File Management
Page 87
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 generates the block numbers as well as the BEGIN and END
blocks automatically.
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.
Program begin, name, unit of measure
Spindle axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure
3.2 Creating and Writing Programs
HEIDENHAIN TNC 640 87
Page 88
Programming tool movements in conversational
20
format
To program a block, initiate the dialog by pressing a function key. In the
screen header, the TNC then asks you for all the information
necessary to program the desired function.
Example of a positioning block
Start block.
COORDINATES?
Enter the target coordinate for the X axis
Enter the target coordinate for the Y axis, and go to
the next question with ENT
TOOL RADIUS COMP: RL/RR/NO COMP?
3.2 Creating and Writing Programs
FEED RATE F=? / F MAX = ENT
MISCELLANEOUS FUNCTION M?
The program-block window displays the following line:
3 L X+10 Y+5 R0 F100 M3
Enter "No radius compensation" and go to the next
question with ENT
Enter a feed rate of 100 mm/min for this path contour;
go to the next question with ENT
Enter the miscellaneous function M3 "spindle ON."
Pressing the ENT key terminates this dialog
88 Programming: Fundamentals, File Management
Page 89
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" on page
184)
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
3.2 Creating and Writing Programs
End the dialog immediately
Abort the dialog and erase the block
HEIDENHAIN TNC 640 89
Page 90
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:
U Place the input box at the position in the block where you want to
insert a position value
U Select the actual-position-capture function: In the
soft-key row the TNC displays the axes whose
positions can be transferred
U Select the axis: The TNC writes the current position of
the selected axis into the active input box
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.
3.2 Creating and Writing Programs
The TNC keeps the soft-key row for axis selection active
until you deactivate it by pressing the actual-positioncapture 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.
90 Programming: Fundamentals, File Management
Page 91
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
3.2 Creating and Writing Programs
HEIDENHAIN TNC 640 91
Page 92
Function Soft key/Key
Set the selected word to zero
Erase an incorrect number
Clear a (non-blinking) error message
Delete the selected word
Delete the selected block
Erase cycles and program sections
Insert the block that you last edited or deleted
Inserting blocks at any desired location
U Select the block after which you want to insert a new block and
3.2 Creating and Writing Programs
initiate the dialog
Editing and inserting words
U Select a word in a block and overwrite it with the new one. The
plain-language dialog is available while the word is highlighted
U To accept the change, press the END key
If you want to insert a word, press the horizontal arrow key repeatedly
until the desired dialog appears. You can then enter the desired value.
92 Programming: Fundamentals, File Management
Page 93
Looking for the same words in different blocks
To use this function, set the AUTO DRAW soft key to OFF.
To select a word in a block, press the arrow keys
repeatedly until the highlight is on the desired word
Select a block with the arrow keys
The word that is highlighted in the new block is the same as the one
you selected previously.
If you have started a search in a very long program, the
TNC shows a progress display window. You then have the
option of canceling the search via soft key.
Finding any text
U To select the search function, press the FIND soft key. The TNC
displays the Find text: dialog prompt
U Enter the text that you wish to find
U To find the text, press the EXECUTE soft key
3.2 Creating and Writing Programs
HEIDENHAIN TNC 640 93
Page 94
Marking, copying, deleting and inserting program sections
The TNC provides certain functions for copying program sections
within an NC program or into another NC program—see the table
below.
To copy a program section, proceed as follows:
U Select the soft-key row containing the marking functions
U Select the first (last) block of the section you wish to copy
U To mark the first (last) block, press the SELECT BLOCK soft key. The
TNC then highlights the first character of the block and the CANCEL
SELECTION soft key appears
U Move the highlight to the last (first) block of the program section you
wish to copy or delete. The TNC shows the marked blocks in a
different color. You can end the marking function at any time by
pressing the CANCEL SELECTION soft key
U To copy the selected program section, press the COPY BLOCK soft
key. To delete the selected section, press the DELETE BLOCK soft
key. The TNC stores the selected block
U Using the arrow keys, select the block after which you wish to insert
the copied (deleted) program section
To insert the section into another program, select the
corresponding program using the file manager and then
3.2 Creating and Writing Programs
mark the block after which you wish to insert the copied
block.
U To insert the block, press the INSERT BLOCK soft key
U To end the marking function, press the CANCEL SELECTION soft
key
Function Soft key
Switch the marking function on
Switch the marking function off
Delete the marked block
Insert the block that is stored in the buffer
memory
Copy the marked block
94 Programming: Fundamentals, File Management
Page 95
The TNC search function
+40
The search function of the TNC enables you to search for any text
within a program and replace it by a new text, if required.
Finding any text
U If required, select the block containing the word you wish to find
U Select the search function: The TNC superimposes
the search window and displays the available search
functions in the soft-key row (see table of search
functions)
U Enter the text to be searched for. Please note that the
search is case-sensitive
U Start the search process: The TNC moves to the next
block containing the text you are searching for
U Repeat the search process: The TNC moves to the
next block containing the text you are searching for
U End the search function
3.2 Creating and Writing Programs
HEIDENHAIN TNC 640 95
Page 96
Finding/Replacing any text
The find/replace function is not possible if
a program is protected
the program is currently being run by the TNC
When using the REPLACE ALL function, ensure that you
do not accidentally replace text that you do not want to
change. Once replaced, such text cannot be restored.
U If required, select the block containing the word you wish to find.
U Select the Search function: The TNC superimposes
the search window and displays the available search
functions in the soft-key row
U Enter the text to be searched for. Please note that the
search is case-sensitive. Then confirm with the ENT
key
U Enter the text to be inserted. Please note that the
entry is case-sensitive
U Start the search process: The TNC moves to the next
occurrence of the text you are searching for
3.2 Creating and Writing Programs
U To replace the text and then move to the next
occurrence of the text, press the REPLACE soft key.
To replace all text occurrences, press the REPLACE
ALL soft key. To skip the text and move to its next
occurrence press the FIND soft key
U End the search function
96 Programming: Fundamentals, File Management
Page 97
3.3 File Management:
Fundamentals
Files
Files in the TNC Ty p e
Programs
In HEIDENHAIN format
In DIN/ISO format
.H
.I
Tables for
Tools
Tool changers
Pallets
Datums
Points
Presets
Touch probes
Turning tools
Backup files
Dependent data (such as structure items)
Texts as
ASCII files
Log files
Help files
When you write a part program on the TNC, you must first enter a
program name. The TNC saves the program to the hard disk as a file
with the same name. The TNC can also save texts and tables as files.
The TNC provides a special file management window in which you can
easily find and manage your files. Here you can call, copy, rename and
erase files.
You can manage an almost unlimited number of files with the TNC.
The available memory is at least 21 GB. A single NC program can be
up to 2 GB in size.
Depending on the setting, the TNC generates a backup file
(*.bak) after editing and saving of NC programs. This can
reduce the memory space available to you.
.T
.TCH
.P
.D
.PNT
.PR
.TP
.TRN
.BAK
.DEP
.A
.TXT
.CHM
3.3 File Management: Fundamentals
HEIDENHAIN TNC 640 97
Page 98
File names
When you store programs, tables and texts as files, the TNC adds an
extension to the file name, separated by a point. This extension
indicates the file type.
PROG20 .H
File name File type
File names should not exceed 25 characters, otherwise the TNC
cannot display the entire file name.
File names on the TNC must comply with this standard: The Open
Group Base Specifications Issue 6 IEEE Std 1003.1, 2004 Edition
(Posix-Standard). Accordingly, the file names may include the
characters below:
A B C D E F G H I J K L M N O P Q R S T U V W X Y Z a b c d e f g h i
j k l m n o p q r s t u v w x y z 0 1 2 3 4 5 6 7 8 9 . _ -
You should not use any other characters in file names in order to
prevent any file transfer problems.
The maximum limit for the path and file name together is
82 characters (see "Paths" on page 100).
3.3 File Management: Fundamentals
98 Programming: Fundamentals, File Management
Page 99
Showing externally created files on the TNC
The TNC features several additional tools which you can use to display
the files shown in the table below. Some of the files can also be
edited.
File types Ty p e
PDF files
Excel spreadsheets
Internet files
pdf
xls
csv
html
Text files txt
ini
Image files bmp
gif
jpg
png
For further information about displaying and editing the listed file
types: See “Additional tools for management of external file types” on
page 114..
Data backup
We recommend saving newly written programs and files on a PC at
regular intervals.
The TNCremoNT data transmission freeware from HEIDENHAIN is a
simple and convenient method for backing up data stored on the TNC.
You additionally need a data medium on which all machine-specific
data, such as the PLC program, machine parameters, etc., are stored.
Ask your machine manufacturer for assistance, if necessary.
Saving the contents of the entire hard disk (> 2 GB) can
take up to several hours. In this case, it is a good idea to
save the data outside of work hours, e.g. during the night.
Take the time occasionally to delete any unneeded files so
that the TNC always has enough hard-disk space for
system files (such as the tool table).
3.3 File Management: Fundamentals
Depending on operating conditions (e.g., vibration load),
hard disks generally have a higher failure rate after three to
five years of service. HEIDENHAIN therefore
recommends having the hard disk inspected after three to
five years.
HEIDENHAIN TNC 640 99
Page 100
3.4 Working with the File Manager
TNC:\
AUFTR1
NCPROG
WZTAB
A35K941
ZYLM
TESTPROG
HUBER
KAR25T
Directories
To ensure that you can easily find your files, we recommend that you
organize your hard disk into directories. You can divide a directory into
further directories, which are called subdirectories. With the –/+ key or
ENT you can show or hide the subdirectories.
Paths
A path indicates the drive and all directories and subdirectories under
which a file is saved. The individual names are separated by a
backslash "\".
The path, including all drive characters, directory and the
file name, including the extension, must not exceed 82
characters!
Drive designations must not include more than 8
uppercase letters.
Example
3.4 Working with the File Manager
The directory AUFTR1 was created on the TNC:\ drive. Then, in the
AUFTR1 directory, the directory NCPROG was created and the part
program PROG1.H was copied into it. The part program now has the
following path:
TNC:\AUFTR1\NCPROG\PROG1.H
The chart at right illustrates an example of a directory display with
different paths.
100 Programming: Fundamentals, File Management
Loading...