HEIDENHAIN ITNC 530 - PILOT SMART NC User manual

Pilot
smarT.NC
NC Software
340 490-06, 606 420-01
340 491-06, 606 421-01
340 492-06
340 493-06
340 494-06
English (en)
6/2010
iTNC 530

3
The smarT.NC Pilot
The smarT.NC Pilot
... is the concise programming guide for the smarT.NC
operating mode of the iTNC 530. For complete information on
programming and operating the iTNC 530, refer to the User’s
Manual.
Symbols in the Pilot
Certain symbols are used in the Pilot to denote specific types of
information:
Control NC software number
iTNC 530 340 490-06
iTNC530 with HSCI 606 420-01
iTNC 530, export version 340 491-06
iTNC 530, export version with
HSCI 606 421-01
iTNC 530 with Windows XP 340 492-06
iTNC 530 with Windows XP,
export version 340 493-06
iTNC 530 programming station 340 494-06
Important note!
The TNC and the machine tool must be prepared by
the machine tool builder to perform this function!
Warning: danger for the user or machine!

4
Contents
The smarT.NC Pilot .................................................................................................................................................... 3
Quick Guide ................................................................................................................................................................ 5
Fundamentals ............................................................................................................................................................. 16
Defining Machining Operations .................................................................................................................................. 45
Defining Machining Positions ..................................................................................................................................... 149
Defining Contours ...................................................................................................................................................... 172
Processing DXF Files (Software Option) .................................................................................................................... 182
Graphically Testing and Running a Unit Program ....................................................................................................... 207

5
Quick Guide
Quick Guide
For the first time, select the new operating mode
and create a new program
USelect the smarT.NC operating mode: The TNC is found in
the file management (see figure at right). If the TNC is not
located in the file management: Press the PGM MGT key
UIn order to write a new machining program, press the NEW
FILE soft key. smarT.NC opens a pop-up window
UEnter a file name with the extension .HU, and confirm with
ENT
UConfirm with the MM (or INCH) soft key or screen button.
smarT.NC creates an .HU program with the selected units
of measurement and automatically inserts the program
header form. This form contains in addition to the workpiece
blank definition the most important presettings valid for the
rest of the program
USelect the standard values and save the program header
form: Press the END key: You can now define the working
steps

6
Quick Guide
Exercise 1: Simple drilling operations in smarT.NC
Task
Centering bolt hole circle, drilling and tapping
Prerequisites
The following tools must be defined in the tool table TOOL.T:
NC center drill, diameter 10 mm
Drill, diameter 5 mm
Tap M6
50
50
20
M6
¬80
0
0
0

7
Quick Guide
Defining centering
UInsert a machining step: Press the INSERT soft key
UInserting a machining step
UInsert drilling operation: The TNC displays a soft key row
with the available drilling operations
USelect centering: The TNC displays the overview form for
defining the entire centering operation
USpecify tool: Press the SELECT soft key for the TNC to
display the contents of the tool table TOOL.T in a pop-up
window
UMove the highlight with the cursor keys onto the NC center
drill and enter it into the form with the ENT key. As an
alternative, you may also enter the tool number directly and
confirm the entry with the ENT key
UEnter the spindle speed and confirm entry with the ENT key
UEnter the centering feed rate and confirm entry with the ENT
key
USwitch to depth entry via soft key and confirm entry with the
ENT key. Enter the desired depth
USelect the Positiondetail form with the key for switching the
tabs
USwitch to bolt hole circle definition. Enter required bolt hole
circle data and confirm each entry with the ENT key
USave the form with the END key. Definition of the centering
operation is complete

8
Quick Guide
Defining drilling
USelect drilling: Press the UNIT 205 soft key for the TNC to
display the form for drilling operations
USpecify tool: Press the SELECT soft key for the TNC to
display the contents of the tool table TOOL.T in a pop-up
window
UMove the highlight with the cursor keys onto the NC drill and
enter it into the form with the ENT key
UEnter the spindle speed and confirm entry with the ENT key
UEnter the drilling feed rate and confirm entry with the ENT
key
UEnter the drilling depth and confirm entry with the ENT key
UEnter infeed depth, save the form with the END key
You do not need to define the drilling positions again. The
TNC automatically uses the previously defined positions, i.e.
those defined for the centering operation.

9
Quick Guide
Defining tapping
UOne level upwards via the BACK soft key
UInsert tapping operation: Press the THREAD soft key for the
TNC to display a soft key row with the available tapping
operations
USelect rigid tapping: Press the UNIT 209 soft key for the TNC
to display the form for defining tapping operations
USpecify tool: Press the SELECT soft key for the TNC to
display the contents of the tool table TOOL.T in a pop-up
window
UMove the highlight with the cursor keys onto the tap and
enter it into the form with the ENT key
UEnter the spindle speed and confirm entry with the ENT key
UEnter the depth of thread and confirm with the ENT key
UEnter the thread pitch, save the form with the END key
You do not need to define the drilling positions again. The
TNC automatically uses the previously defined positions, i.e.
those defined for the centering operation.

10
Quick Guide
Test run
USelect the initial soft key row with the smarT.NC key (home
function)
USelect the Test Run submode
UStart the test run: The TNC simulates the machining
operations defined by you
USelect the initial soft key row with the smarT.NC key (home
function) after program end
Running a program
USelect the initial soft key row with the smarT.NC key (home
function)
USelect the Program Run submode
UStart the program run: The TNC runs the machining
operations defined by you
USelect the initial soft key row with the smarT.NC key (home
function) after program end

11
Quick Guide
Exercise 2: Simple milling operations in smarT.NC
Task
Roughing and finishing a circular pocket with a tool
Prerequisites
The following tool must be defined in the tool table TOOL.T:
End mill, diameter 10 mm
50
50
15
¬80
20
0
0
0

12
Quick Guide
Defining circular pocket
UInsert a machining step: Press the INSERT soft key
UInserting a machining step
UInsert pocket machining: Press the POCKETS/STUDS soft
key for the TNC to display a soft key row with the available
milling operations
USelect circular pocket: Press the UNIT 252 soft key. The TNC
displays the form for circular pocket machining The
machining operation is set to roughing and finishing
USpecify tool: Press the SELECT soft key for the TNC to
display the contents of the tool table TOOL.T in a pop-up
window
UMove the highlight onto the end mill with the cursor keys
and enter it into the form with the ENT key
UEnter the spindle speed and confirm entry with the ENT key
UEnter the plunging feed rate and confirm with the ENT key
UEnter the milling feed rate and confirm with the ENT key
UEnter the circular pocket diameter and confirm with the ENT
key
UEnter depth, infeed depth and finishing allowance for the
side and confirm each time with the ENT key
UEnter X and Y center point coordinates for the circular
pocket, confirm each time with the ENT key
USave the form with the END key. Definition of the circular
pocket operation is complete
UTest and run the newly created program as previously
described

13
Quick Guide
Exercise 3: Contour milling in smarT.NC
Task
Roughing and finishing a contour with a tool
Prerequisites
The following tool must be defined in the tool table TOOL.T:
End mill, diameter 22 mm
10 80 90
10
0
0
70
90
6x45°
1
2
R8
3
4
5
6

14
Quick Guide
Defining contour machining
UInsert a machining step: Press the INSERT soft key
UInserting a machining step
UInsert contour machining: Press the CONTR. PGM soft key
for the TNC to display a soft key row with the available
contour operations
USelect contour train machining: Press the UNIT 125 soft key.
The TNC displays the form for a contour operation
USpecify tool: Press the SELECT soft key for the TNC to
display the contents of the tool table TOOL.T in a pop-up
window
UMove the highlight onto the end mill with the cursor keys
and enter it into the form with the ENT key
UEnter the spindle speed and confirm entry with the ENT key
UEnter the plunging feed rate and confirm with the ENT key
UEnter the milling feed rate and confirm with the ENT key
UEnter coordinates of workpiece upper edge, depth, infeed
depth and finishing allowance for the side and confirm each
time with the ENT key
USelect type of milling, radius compensation and type of
approach via soft keys and confirm each time with the ENT
key
UEnter the approach parameters and confirm each time with
the ENT key

15
Quick Guide
UThe input field Contour name is active. Create a new contour
program: smarT.NC displays a pop-up window for entering
the contour name. Enter the name of the contour, confirm
with the ENT key. smarT.NC is now in contour programming
mode
UDefine the starting point of the contour in X and Y with the L
key: X=10, Y=10, save with the END key
UApproach point 2with the L key: X=90, save with the END
key
UDefine a curvature radius of 8 mm with the RND key, save
with the END key
UApproach point 3with the L key: Y=80, save with the END
key
UApproach point 4with the L key: X=90, Y=70, save with the
END key
UApproach point 5with the L key: Y=10, save with the END
key
UDefine a chamfer of 6 mm with the CHF key, save with the
END key
UApproach end point 6with the L key: X=10, save with the
END key
USave contour program with the END key: smarT.NC now
again displays the form for defining contour machining
USave entire contour machining with the END key. Definition
of contour machining is complete
UTest and run the newly created program as previously
described

16
Fundamentals
Fundamentals
Introduction to smarT.NC
With smarT.NC you can easily write structured conversational programs
in separate working steps (units) and, if you want, edit them with the
conversational editor. Since the only data basis for smarT.NC is the
conversational program, you can modify data with the conversational
editor, for example, and show them in the form view.
Immediately understandable input forms in the right half of the screen
make it easier to define the required machining parameters, which are
also displayed in a help graphic (lower left quarter of the screen). The
structured program layout in a tree diagram (top left quarter of the screen)
provides you with a quick overview of the working steps in a part
program.
The separate and universal operating mode smarT.NC provides an
alternative to the well known conversational programming. As soon as
you have defined a machining step you can graphically test it and/or run
it in the new operating mode.
Parallel programming
You can also create and edit smarT.NC programs at the same time that
the TNC is running another program. Simply switch to the Programming
and Editing operating mode and open the desired smarT.NC program
there.
If you want to edit the smarT.NC program with the conversational editor,
select the OPEN WITH function in the file manager, and then press
CONVERSTL.

17
Fundamentals
Programs/Files
The TNC keeps its programs, tables and texts in files. A file designation
consists of two components:
smarT.NC uses mainly three file types:
Unit programs (file type .HU)
Unit programs are conversational programs that contain two additional
structuring elements: The beginning (UNIT XXX) and the end (END OF
UNIT XXX) of a machining step
Contour descriptions (file type .HC)
Contour descriptions are conversational programs. They must only
contain path functions that can be used to describe a contour in the
machining plane. The following elements are permitted: L, Cwith CC,
CT, CR, RND, CHF as well as the FPOL, FL, FLT, FC and FCT elements for FK
free contour programming
Point tables (file type .HP)
smarT.NC saves in point tables the machining positions that you
defined using the powerful pattern generator
Files in the TNC Ty p e
Programs
In HEIDENHAIN format
In DIN/ISO format .H .I
smarT.NC files
Structured unit programs
Contour descriptions
Point tables for machining positions
.HU
.HC
.HP
Tables for
Tools
Tool changers
Pallets
Datums
Presets (reference points)
Cutting data
Cutting materials, workpiece materials
.T
.TCH
.P
.D
.PR
.CDT
.TAB
Texts as
ASCII files
Help files .A .CHM
Drawing data as
DXF files .DXF
PROG20 .HU
File name File type
As a default, smarT.NC automatically saves all files in the
TNC:\smarTNC directory. However, you can also select any
other directory.

18
Fundamentals
Selecting the new operating mode the first time
USelect the smarT.NC operating mode: The file manager
of the TNC appears
USelect one of the available example programs with the
arrow keys and press ENTER, or
UIn order to write a new machining program, press the
NEW FILE soft key. smarT.NC opens a pop-up window
UEnter a file name with the extension .HU, and confirm
with ENT
UConfirm with the MM (or INCH) soft key or screen
button. smarT.NC creates an .HU program with the
selected units of measurement and automatically inserts
the program header form
UThe data for the program header form are mandatory,
since they are globally valid for the entire machining
program. The default values are specified internally.
Change the data if necessary, and save them with the
END key
UIn order to define machining steps, press the EDIT soft
key to select the desired machining step

19
Fundamentals
File management with smarT.NC
As mentioned previously, smarT.NC differentiates between three file
types: unit programs (.HU), contour descriptions (.HC) and point tables
(.HP). These three file types can be selected and edited in the file
manager in the smarT.NC operating mode. Contour descriptions and
point tables can also be edited if you are currently defining a machining
unit.
You can also open DXF files from within smarT.NC in order to extract
contour descriptions (.HC files) and machining positions (.HP files) from
them (software option).
The file manager in smarT.NC can also be fully operated with the mouse.
You can even use the mouse to change the sizes of the windows within
the file manager. Click the horizontal or vertical separating line, and drag
it to the desired position with the mouse.

20
Fundamentals
Calling the file manager
UTo select the file manager, press the PGM MGT key: The TNC displays
the file manager window (the figure at right shows the default setting).
If the TNC displays a different screen layout, press the WINDOW soft
key on the second soft-key row)
The top window on the left shows the available drives and directories.
Drives designate devices with which data are stored or transferred. A
drive can be the hard disk of the TNC, directories connected via the
network, or USB devices. A directory is always identified by a folder
symbol to the left and the directory name to the right. Subdirectories are
shown to the right of and below their parent directories. A triangle
pointing to the right in front of the folder symbol indicates that there are
further subdirectories, which can be shown with the right arrow key.
The lower window on the left shows a preview of the file contents if an
.HP or .HC file is highlighted.