Important initial information

Overview

The control provides various operating modes that are suitable for different tasks, e.g. programming, testing, or machining.

Key	Function
	Manual operation
	Electronic handwheel
	Positioning with Manual Data Input
	Program Run, Single Block
	Program Run, Full Sequence

Key	Function
	Programming
	Test Run

This subdivision allows you to perform multiple tasks in parallel. For example, you can create and test a new NC program while machining.

Tip

For further details on the various operating modes, see the following interaction: Selecting an operating mode.

General information

1	Directories nc_prog for NC programs table for tables tncguide for the help system
2	Drives RS 232: serial interface TNC: hard disk for the control USB if applicable
3	Active path or file name
4	File window Existing directories on the selected drive Existing files in the selected directory
5	Directory window Existing directories on the selected drive Existing subdirectories in the selected directory

Information	Explanation
	The file is permanently protected against erasing and editing with the Protect soft key.
	The file is temporarily protected against erasing and editing, because it is being run on the machine.
File name	Files with file type
Byte	Size of each file in bytes
Status	M: The file has been selected in Program Run mode S: The file has been selected in Test Run mode E: The file has been selected in the Programming mode +: File contains dependent files, e.g. structuring items
Date	Date of last modification
Time	Time of last modification

Control-specific file types

The control provides you with the following file types among others:

Files	Application	Type
Programs	In HEIDENHAIN Klartext format According to DIN/ISO	.H .I
Tables	Tool table Turning tool table Touch probe table Pocket table Datum table Points table Preset table Pallet table Freely definable table Backup files	.T .TRN .TP .TCH .D .PNT .PR .P .TAB .BAK
Texts	ASCII files Log files Help files	.A .TXT .CHM

Tip

If some files are missing in the file management display, this is due to the active operating mode or the active filter settings.

To select the file type shown, proceed as follows:
		Switch to the Programming operating mode
		Press the PGM MGT key
		Press the SELECT TYPE soft key
		Press the SHOW ALL soft key Alternative: Press the soft key for the desired file type

File types not commonly used in the control

Several additional tools are installed on the control, used to display the following files. Some of the files can also be edited.

Files	Type
PDF files	.PDF
Tables	.XLS .CSV
Text files	.TXT .INI
Graphic files	.BMP .GIF .JPG .PNG
Internet files	.HTML

Permitted characters

File names on the control must comply with the following 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. Table names must start with a letter.

1 / 4

NC program structure

1 / 2

Structure of an NC program

Each NC program consists of multiple NC blocks. Each NC block consists of multiple words.

Example
5 L X+20 Y-10 R0 F1000 M3

Word	Meaning
5	Block number
L	Path function
X+20 Y-10	End point coordinates
R0	Radius compensation
F1000	Feed rate
M3	Miscellaneous function

The control numbers all NC blocks in your NC program in ascending order.

The first NC block is identified by BEGIN PGM, the program name, and the active unit of measure.

The next blocks contain information on:

Workpiece blank
Tool calls
Approaching a safe position
Feed rate and spindle speed
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.

Tip

HEIDENHAIN recommends: After each tool call, traverse to a safe position from which the control can position the tool for machining without causing a collision!

Syntax elements

The control displays syntax elements with various colors according to their meaning. Color-highlighting makes the NC programs easier to read and clearer.

Color highlighting of syntax elements
Use	Color
Standard color	Black
Comments	Green
Block numbers	Violet
Numerical values	Blue
Modal feed rate data	Brown
Maximum feed rate	Orange
Text, e.g. in calls	Wine red

Tip

Screen content can be shifted with the mouse using the scroll bar at the right edge of the program window. In addition, the size and position of the scrollbar indicates program length and cursor position.

Figure: The video shows the NC program structure.

1 / 2

Tool definition

1 / 2

Defining the tools

You must define the tools to be used so that the control can determine the tool center path and execute tool compensations.

Define a tool in the following ways:

With the TOOL DEF function
In the tool table
In Extended Tool Management (option 93)

The TOOL DEF function enables you to enter tool data directly in your NC program.

Key	Meaning	Function
	Tool Definition Define the tool	Define the tool in the NC program Pre-position the tool changer

Machine

Refer to your machine manual.

If you work with tool tables, the TOOL DEF key is usually assigned the "Pre-position tool changer" function.

Tool number or tool name
Tool length L
Tool radius R

Example
TOOL DEF 5 L+47 R+5

Manual

For information on tool management, please refer to the User’s Manual.

Editing the tool table

The tool table provides more input options than the TOOL DEF function. As soon as a tool table is active, that table is binding.

You can work with several tool tables. For the program run, the tool table with the TOOL.T file name will be used.

Edit the TOOL.T tool table as follows:
		Switch to a machine mode of operation, e.g. Manual operation
		Press the TOOL TABLE soft key
		Set the EDIT soft key to ON

Select the desired view as follows:
		Press the screen layout key
		Press the soft key for the desired layout

Tip

When programming the HIT exercises and additional HIT examples, you only need the tools that are already available. There is no need to create your own tools in the tool table.

1 / 2

Path functions

1 / 7

Overview

The control provides various path functions for the different tool movements.

Key		Function
		Approach /depart from contour
		FK free contour programming
		Straight line
		Circle center / pole for polar coordinates
		Circular arc with center
		Circular arc with radius
		Circular arc with tangential transition
		Chamfer / Rounding

Tip

We will discuss the most important path functions on the next pages.

The Contour Programming learning module contains detailed information on the path functions, as well as descriptions of the additional functions APPR, DEP, and FK.

Straight line L

The control moves the tool in a straight line from its current position to the end point of the straight line. The starting point is the end point of the preceding block.

Circular movement C with circle center CC

You can define a circle center for circles that you have programmed with the C key (circular path C) This is done in the following ways:

Enter the Cartesian coordinates of the circle center in the working plane, or
Use the position last programmed, or
Take over the coordinates with the Actual-position-capture key

Before programming a circular arc C, you must first specify the circle center CC. The last programmed tool position will be the starting point of the arc.

Circular movement CR

The tool moves on a circular path with the radius R.

Circular movement CT

The tool moves on an arc that connects tangentially to the previously programmed contour element.

A connection between two contour elements is called tangential when there is no kink or corner at the intersection between the two contours—the transition is smooth.

The contour element to which the tangential arc connects must be programmed immediately before the CT block. This requires at least two positioning blocks.

Chamfer CHF

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

Rounding arc RND

The RND function creates rounding arcs at contour corners.

The tool moves on an arc that connects tangentially to both the preceding and subsequent contour elements.

The rounding arc must be machinable with the called tool.

1 / 7

Dialog guidance

Overview of keys

The control offers you the following keys for dialog guidance:

Key	Meaning	Application
	Enter Confirm	Confirm/Save value Move to next dialog
	Arrow key	Confirm/Save value Enter next coordinate
	No Enter Do not confirm	Do not confirm value Move to next dialog
	Clear Entry Acknowledge message	Delete input value
	End of Block End block	Confirm block without further input Cancel function
	Delete Block Delete	Delete program line Cancel modification

Important M Functions

Overview

Miscellaneous functions, also known as M functions, enable you to control the program run and specific machine functions.
Depending on the control system used, you can enter a minimum of two miscellaneous functions in each positioning block of your NC program.

The following miscellaneous functions are standardized according to DIN 66025:

Number		Function
M00		Program STOP Spindle STOP Coolant OFF
M1		Optional program STOP Can be activated via soft key When NC start is pressed again, continue with next block
M2		Program STOP Spindle STOP Coolant OFF Return jump to block 1 of the NC program Clear the status display (depends on the clearMode machine parameter)
M3		Spindle ON, clockwise
M4		Spindle ON, counterclockwise
M5		Spindle STOP
M8		Coolant ON
M9		Coolant OFF
M13		Spindle ON, clockwise Coolant ON
M14		Spindle ON, counterclockwise Coolant ON
M30		Same as M2