heidenhain TNC 310 User Manual

TNC 310

NC-Software
286 040-xx

User’s Manual

Conversational

Programming

7/2000

Controls on the visual display unit

0

0

Split screen layout

Coordinate numbers, editing

... Numbers

Soft keys

Shift soft-key rows

Machine control buttons

Axis direction buttons

Controls on the TNC

Rapid traverse button

Spindle rotation direction

Coolant

Tool release

Spindle ON/OFF

NC start/NC stop

Override control knobs for feed rate/spindle speed

100

50

1

5

S %

0

100

50

1

5

F %

0

Machine operating modes

MANUAL OPERATION

Decimal point

Change arithmetic sign

Confirm entry and resume dialog

End block

Clear numerical entry or TNC error message

Abort dialog, delete program section

Programming aids

MOD functions

HELP functions

Moving the cursor, going directly to blocks, cycles and
parameter functions

Move highlight

Move highlight, skip dialog question

Select blocks and cycles directly

POSITIONING WITH MDI

PROGRAM RUN, SINGLE BLOCK

PROGRAMMING AND EDITING

TNC Models, Software and
Features

This manual describes functions and features provided by
the TNCs with the following NC software number.

TNC Model NC Software No.

TNC 310 286 040 xx

The machine tool builder adapts the useable features of the
TNC to his machine by setting machine parameters. There­fore, some of the functions described in this manual may
not be among the features provided by your machine tool.

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

■ Probing function for the 3-D touch probe

■ Digitizing option

■ Tool measurement with the TT 120

■ Rigid tapping

Please contact your machine tool builder to become familiar
with the individual implementation of the control on 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.

Contents

Location of use

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.

IHEIDENHAIN TNC 310

Contents

Introduction

1

Manual Operation and Setup

Positioning with Manual Data Input (MDI)

Programming: Fundamentals of NC,
File Management, Programming Aids

Programming: Tools

Programming: Programming Contours

Programming: Miscellaneous Functions

Programming: Cycles

Programming: Subprograms and Program
Section Repeats

Test Run and Program Run

3-D Touch Probes

MOD Functions

2

Contents

3
4
5
6
7
8

9
10
11
12

Tables and Overviews

13

IIIHEIDENHAIN TNC 310

1 INTRODUCTION 1

1.1 The TNC 310 2

1.2 Visual Display Unit and Keyboard 3

Contents

1.3 Modes of Operation 4

1.4 Status Displays 7

1.5 Accessories: HEIDENHAIN 3-D Touch Probes and Electronic Handwheels 11

2 MANUAL OPERATION AND SETUP 13

2.1 Switch-On 14

2.2 Moving the Machine Axes 15

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M 18

2.4 Datum Setting (Without a 3-D Touch Probe) 19

3 POSITIONING WITH MANUAL DATA INPUT (MDI) 21

3.1 Programming and Executing Simple Positioning Blocks 22

4 PROGRAMMING: FUNDAMENTALS OF NC, FILE MANAGEMENT, PROGRAMMING AIDS 23

4.1 Fundamentals of NC 24

4.2 File Management 29

4.3 Creating and Writing Programs 32

4.4 Interactive Programming Graphics 37

4.5 HELP Function 39

5 PROGRAMMING: TOOLS 41

5.1 Entering Tool-Related Data 42

5.2 Tool Data 43

5.3 Tool Compensation 48

IV

Contents

6 PROGRAMMING: PROGRAMMING CONTOURS 53

6.1 Overview of Tool Movements 54

6.2 Fundamentals of Path Functions 55

6.3 Path Contours — Cartesian Coordinates 58
Overview of path functions 58
Straight line L 59
Inserting a chamfer CHF between two straight lines 59
Circle center CC 60
Circular path C around circle center CC 61
Circular path CR with defined radius 62
Circular path CT with tangential connection 63
Corner Rounding RND 64
Example: Linear movements and chamfers with Cartesian coordinates 65
Example: Circular movements with Cartesian coordinates 66
Example: Full circle with Cartesian coordinates 67

6.4 Path Contours—Polar Coordinates 68
Polar coordinate origin: Pole CC 68
Straight line LP 69
Circular path CP around pole CC 69
Circular path CTP with tangential connection 70
Helical interpolation 71
Example: Linear movement with polar coordinates 73
Example: Helix 74

Contents

7 PROGRAMMING: MISCELLANEOUS FUNCTIONS 75

7.1 Entering Miscellaneous Functions M and STOP 76

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant 77

7.3 Miscellaneous Functions for Coordinate Data 77

7.4 Miscellaneous Functions for Contouring Behavior 79

7.5 Miscellaneous Function for Rotary Axes 82

VHEIDENHAIN TNC 310

8 PROGRAMMING: CYCLES 83

8.1 General Overview of Cycles 84

8.2 Drilling Cycles 86

Contents

PECKING (Cycle 1) 86
DRILLING (Cycle 200) 88
REAMING (Cycle 201) 89
BORING (Cycle 202) 90
UNIVERSAL DRILLING (Cycle 203) 91
TAPPING with a floating tap holder (Cycle 2) 93
RIGID TAPPING (Cycle 17) 94
Example: Drilling cycles 95
Example: Drilling cycles 96

8.3 Cycles for Milling Pockets, Studs and Slots 97
POCKET MILLING (Cycle 4) 98
POCKET FINISHING (Cycle 212) 99
STUD FINISHING (Cycle 213) 101
CIRCULAR POCKET MILLING (Cycle 5) 102
CIRCULAR POCKET FINISHING (Cycle 214) 104
CIRCULAR STUD FINISHING (Cycle 215) 105
SLOT MILLING (Cycle 3) 107
SLOT with reciprocating plunge-cut (Cycle 210) 108
CIRCULAR SLOT with reciprocating plunge-cut (Cycle 211) 110
Example: Milling pockets, studs and slots 112

8.4 Cycles for Machining Hole Patterns 114
CIRCULAR PATTERN (Cycle 220) 115
LINEAR PATTERN (Cycle 221) 116
Example: Circular hole patterns 118

8.5 Cycles for multipass milling 120
MULTIPASS MILLING (Cycle 230) 120
RULED SURFACE (Cycle 231) 122
Example: Multipass milling 124

VI

Contents

8.6 Coordinate transformation cycles 125
DATUM SHIFT (Cycle 7) 126
MIRROR IMAGE (Cycle 8) 127
ROTATION (Cycle 10) 128
SCALING FACTOR (Cycle 11) 129
Example: Coordinate transformation cycles 130

8.7 Special Cycles 132
DWELL TIME (Cycle 9) 132
PROGRAM CALL (Cycle 12) 132
ORIENTED SPINDLE STOP (Cycle 13) 133

9 PROGRAMMING: SUBPROGRAMS AND PROGRAM SECTION REPEATS 135

9.1 Marking Subprograms and Program Section Repeats 136

9.2 Subprograms 136

9.3 Program Section Repeats 137

9.4 Nesting 139
Subprogram within a subprogram 139
Repeating program section repeats 140
Repeating a subprogram 141

9.5 Programming Examples 142
Example: Milling a contour in several infeeds 142
Example: Groups of holes 143
Example: Groups of holes with several tools 144

Contents

10 TEST RUN AND PROGRAM RUN 147

10.1 Graphics 148

10.2 Test Run 152

10.3 Program Run 154

10.4 Optional Program Run Interruption 158

10.5 Blockwise Transfer: Running Longer Programs 158

11 3-D TOUCH PROBES 159

11.1 Touch probe cycles in the operating mode MANUAL OPERATION 160
Calibrating a touch trigger probe 161
Compensating workpiece misalignment 162

11.2 Setting the Datum with a 3-D Touch Probe 163

11.3 Measuring Workpieces with a 3-D Touch Probe 166

VIIHEIDENHAIN TNC 310

12 MOD FUNCTIONS 169

12.1 Selecting, Changing and Exiting the MOD Functions 170

12.2 System Information 170

Contents

12.3 Enter Code Number 171

12.4 Setting the Data Interface 171

12.5 Machine-Specific User Parameters 172

12.6 Position Display Types 172

12.7 Unit of Measurement 173

12.8 Enter Axis Traverse Limits 173

13 TABLES AND OVERVIEWS 175

13.1 General User Parameters 176
Input possibilities for machine parameters 176
Selecting general user parameters 176
External data transfer 177
3-D Touch Probes 178
TNC displays, TNC editor 178
Machining and program run 180
Electronic handwheels 180

13.2 Pin Layout and Connecting Cable for the Data Interface 181
RS-232-C/V.24 Interface 181

13.3 Technical Information 182
TNC features 182
Programmable functions 183
TNC Specifications 183

13.4 TNC Error Messages 184
TNC error messages during programming 184
TNC error messages during test run and program run 184

13.5 Exchanging the Buffer Battery 187

VIII

Contents

Introduction

1

1.1 The TNC 310

HEIDENHAIN TNC controls are shop-floor programmable
contouring controls for milling, drilling and boring machines.

You can program conventional milling, drilling and boring operations
right at the machine with the easily understandable interactive
conversational guidance. The TNC 310 can control up to 4 axes.
Instead of the fourth axis, you can also change the angular position
of the spindle under program control.

1.1 The TNC 310

Keyboard and screen layout are clearly arranged in a such way that
the functions are fast and easy to use.

Programming: HEIDENHAIN conversational format

HEIDENHAIN conversational programming is an especially easy
method of writing programs. Interactive graphics illustrate the
individual machining steps for programming the contour. Workpiece
machining can be graphically simulated during test run.

You can also enter one program while the TNC is running another.

Compatibility

The TNC can execute all part programs that were written on
HEIDENHAIN controls TNC 150 B and later.

2

1 Introduction

1.2 Visual Display Unit and Keyboard

Visual display unit

The figure at right shows the keys and controls on the VDU:

Setting the screen layout
Soft key selector keys
Switching the soft-key rows
Header

When the TNC is on, the selected operating mode is shown in
the screen header. Dialog prompts and TNC messages also
appear here (unless the TNC is showing only graphics).

Soft keys
In the right margin the TNC indicates additional functions in a soft­key row. You can select these functions by pressing the keys
immediately beside them
rectangular boxes indicating the number of soft-key rows. These
rows can be called with the
active soft-key row is filled in.

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 help
graphics for cycle definition in the right window instead, or display
only program blocks in one large window. The available screen
windows depend on the selected operating mode.

. Directly beneath the soft-key row are

shift key. The box representing the

1.2 Visual Display Unit and Keyboard

To change the screen layout:

Press the SPLIT SCREEN key: The soft-key row
shows the available layout options.

<

Select the desired screen layout.

3HEIDENHAIN TNC 310

Keyboard

The figure at right shows the keys of the keyboard grouped
according to their functions:

MOD function,
HELP function

Numerical input
Dialog buttons
Arrow keys and GOTO jump command
Modes of Operation
Machine control buttons
Override control knobs for feed rate/spindle speed

1.3 Modes of Operation

The functions of the individual keys are described in the foldout of
the front cover. The exact functioning of the machine control
buttons, e.g. NC START, is described in more detail in your Machine
Manual.

1.3 Modes of Operation

The TNC offers the following modes of operation for the various
functions and working steps that you need to machine a workpiece:

MANUAL OPERATION and ELECTRONIC
HANDWHEEL Operating Modes

The MANUAL OPERATION mode is required for setting up the
machine tool. In this operating mode, you can position the machine
axes manually or by increments. Datums can be set by the usual
scratching method or by using the TS 220 triggering touch probe.
The TNC also supports the manual traverse of the machine axes
using a HR electronic handwheel.

Soft keys for selecting the screen layout

There are no select options available. The TNC always shows the
position display.

4

1 Introduction

POSITIONING WITH MANUAL DATA INPUT (MDI)

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

There are no select options available. The TNC always shows the
position display.

PROGRAMMING AND EDITING

In this mode of operation you can write your part programs. The
various cycles help you with programming and add necessary
information. If desired, you can have the programming graphics
show the individual steps.

Soft keys for selecting the screen layout

Screen windows Soft key

Program blocks

Left: program blocks, right: help graphics for
cycle programming

Left: program blocks, right: programming graphics

Interactive Programming Graphics

1.3 Modes of Operation

5HEIDENHAIN TNC 310

TEST RUN

In the TEST RUN mode of operation, the TNC checks programs and
program sections for errors, such as geometrical incompatibilities,
missing or incorrect data within the program or violations of the
work space. This simulation is supported graphically in different
display modes. Use a soft key to activate the test run in the PRO­GRAM RUN operating mode.

Soft keys for selecting the screen layout

Screen windows Soft key

Program blocks

n Test run graphics

1.3 Modes of Operation

Left: program blocks, right: general
program information

Left: program blocks, right: positions and
coordinates

Left: program blocks, right: tool
information

Left: program blocks, right: coordinate
transformations

6

1 Introduction

PROGRAM RUN/SINGLE BLOCK and
PROGRAM RUN/FULL SEQUENCE

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 NC START button.

Soft keys for selecting the screen layout

Screen windows Soft key

Program blocks

Left: program blocks, right: general
program information

Left: program blocks, right: positions and
coordinates

Left: program blocks, right: tool
information

Left: program blocks, right: coordinate
transformations

1.4 Status Displays

1.4 Status Displays

“General” status display

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

In the operating modes MANUAL OPERATION and ELECTRONIC
HANDWHEEL and POSITIONING WITH MDI the status display
appears in the large window

.

7HEIDENHAIN TNC 310

Information in the status display

Symbol Meaning

ACTL.

X Y Z

S F M

1.4 Status Displays

ROT

Actual or nominal coordinates of the current position

Machine axes

Spindle speed S, feed rate F and active M functions

Program run started

Axis locked

Axes are moving
under a basic rotation.

Additional status displays

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

To switch on the additional status display:

Call the soft-key row for screen layout.

<

Select the layout option for the additional status
display, e.g. positions and coordinates.

8 1 Introduction

You can also choose between the following additional status
displays:

General program information

Name of main program / Active block number
Program called via Cycle 12
Active machining cycle
Circle center CC (pole)
Dwell time counter
Operating time

Positions and coordinates

Name of main program / Active block number
Position display
Type of position display, e.g. distance-to-go
Angle of a basic rotation

1.4 Status Displays

9HEIDENHAIN TNC 310

Information on tools

T: Tool number
Tool axis
Tool length and radius
Oversizes (delta values) from TOOL CALL block

1.4 Status Displays

Coordinate transformations

Name of main program / Active block number
Active datum shift (Cycle 7)
Active rotation angle (Cycle 10)
Mirrored axes (Cycle 8)
Active scaling factor (Cycle 11)

See also section 8.7 “Coordinate Transformation Cycles.”

10

1 Introduction

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

3-D Touch Probes

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

■ Automatically align workpieces

■ Quickly and precisely set datums

TS 220 touch trigger probe

This touch probe is particularly effective for automatic workpiece
alignment, datum setting and workpiece measurement. The TS 220
transmits the triggering signals to the TNC via cable.

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
TNC, which stores the current position of the stylus as an actual
value.

HR electronic handwheels

Electronic handwheels facilitate moving the axis slides precisely by
hand. A wide range of traverses per handwheel revolution is
available. Apart from the HR 130 and HR 150 integral handwheels,
HEIDENHAIN also offers the HR 410 portable handwheel.

1.5 Accessories: HEIDENHAIN 3-D Touch Probe and Electronic Handwheels

11HEIDENHAIN TNC 310

2

Manual Operation and Setup

2.1 Switch-On

Switch-on and traversing the reference points can
vary depending on the individual machine tool. Refer
to your machine manual for more information.

Switch on the power supply for control and machine.

The TNC automatically initiates the following dialog

2.1 Switch-On

MEMORY TEST

<

The TNC memory is automatically checked.

POWER INTERRUPTED

<

TNC message that the power was
interrupted — clear the message.

TRANSLATE PLC PROGRAM

<

The PLC program of the TNC is automatically translated.

RELAY EXT. DC VOLTAGE MISSING

<

Switch on the control voltage.
The TNC checks the functioning of the
EMERGENCY STOP circuit.

TRAVERSE REFERENCE POINTS

<

Cross the reference points in any sequence:

Press and hold the machine axis direction
button for each axis until the reference point
has been traversed, or

Cross the reference points with several axes

at the same time: Use softkeys to select the
axes (axes are then shown highlighted on
the screen), and then press the NC START
button.

The TNC is now ready for operation in the
MANUAL OPERATION mode.

14

2 Manual Operation and Setup

2.2 Moving the Machine Axes

Traversing the machine axes with the axis direction keys
is a machine-dependent function. Refer to your machine
tool manual for more information on operating times.

Traverse the axis with the axis direction keys

Select the MANUAL OPERATION mode.

<

Press the axis direction button and hold it as
long as you wish the axis to move.

...or move the axis continuously:

and Press and hold the axis direction button, then

press the NC START button: The axis continues
to move after you release the keys.

2.2 Moving the Machine Axes

Press the NC STOP key to stop the axis.

You can move several axes at a time with these two methods.

15HEIDENHAIN TNC 310

Traversing with the HR 410 electronic handwheel

The portable HR 410 handwheel is equipped with two permissive
buttons. The permissive buttons are located below the star grip.
You can only move the machine axes when an permissive button is
depressed (machine-dependent function).

The HR 410 handwheel features the following operating elements:

EMERGENCY STOP
Handwheel Modes
Permissive buttons
Axis address keys
Actual-position-capture key
Keys for defining the feed rate (slow, medium, fast; the feed rates

are set by the machine tool builder)
Direction in which the TNC moves the selected axis

2.2 Moving the Machine Axes

Machine function
(set by the machine tool builder)

The red indicators show the axis and feed rate you have selected.

To move an axis:

Select the MANUAL OPERATION mode.

<

Activate handwheel, set soft key to ON

<

Press the permissive button.

<

Select the axis on the handwheel

<

Select the feed rate.

<

or Move the active axis in the positive or negative

direction.

16

2 Manual Operation and Setup

16

X

Z

8

8

8

Incremental jog positioning

With incremental jog positioning you can move a machine axis by a
preset distance each time you press the corresponding axis
direction button.

Select the MANUAL OPERATION mode.

<

Select incremental jog positioning, set the
softkey to ON

JOG INCREMENT?

<

Enter the jog increment in millimeters (here,

8 mm), or

Select the jog increment via soft key (select 2nd
or 3rd soft-key row)

<

Press the axis direction button to position as
often as desired

2.2 Moving the Machine Axes

17HEIDENHAIN TNC 310

2.3 Spindle Speed S, Feed Rate F and
Miscellaneous Functions M

In the operating mode MANUAL OPERATION, you can enter the
spindle speed S and the miscellaneous functions M with soft keys.
The miscellaneous functions are described in Chapter 7
”Programming: Miscellaneous Functions.” The feed rate is defined
in a machine parameter and can be changed only with the override
knobs (see next page).

Entering values

Example: Entering the spindle speed S

To select the spindle speed, press the S soft
key.

SPINDLE SPEED S=

<

1000 Enter the desired spindle speed,

and confirm with the NC START button

The spindle speed S with the entered rpm is started with a
miscellaneous function.

Proceed in the same way to enter the miscellaneous functions M.

Changing the spindle speed and feed rate

With the override knobs you can vary the spindle speed S and feed
rate F from 0% to 150% of the set value.

The knob for spindle speed override is effective only on
machines with a stepless spindle drive.

The machine tool builder determines which
miscellaneous functions M are available on your TNC and
what effects they have.

2.3 Spindle Speed S, Feed Rate F and Miscellaneous Functions M

18 2 Manual Operation and Setup

2.4 Datum Setting
(Without a 3-D Touch Probe)

You fix a datum by setting the TNC position display to the
coordinates of a known position on the workpiece.

Preparation

Clamp and align the workpiece.
Insert the zero tool with known radius into the spindle.
Ensure that the TNC is showing the actual position values.

Y

Z

X

Y

X

Setting the datum

Fragile workpiece? If the workpiece surface must not be scratched,
you can lay a metal shim of know thickness
tool axis datum value that is larger than the desired datum by the

d

.

value

Select the MANUAL OPERATION mode.

<

Move the tool slowly until it touches the
workpiece surface.

<

Select the function for setting the datum

<

Select the axis.

DATUM SET Z=

<

Zero tool: Set the display to a known workpiece

position (here, 0) or enter the thickness
shim.

d

on it. Then enter a

d

of the

2.4 Setting the Datum

Repeat the process for the remaining axes.
If you are using a preset tool, set the display of the tool axis to the

length L of the tool or enter the sum Z=L+d.

19HEIDENHAIN TNC 310

3

Positioning with Manual Data
Input (MDI)

3.1 Programming and Executing
Simple Positioning Blocks

The operating mode POSITIONING WITH MANUAL DATA INPUT is
particularly convenient for simple positioning blocks and for
programming a tool call. You can write the individual blocks in
HEIDENHAIN conversational programming and execute them
immediately. The entered blocks are not stored by the TNC.

Select the POSITIONING WITH MDI mode of
operation.

<

Enter a simple positioning block without radius
compensation and feed rate,
e.g. X+25 R0 F50

<

Conclude entry.

<

Press the NC START button: The TNC executes
the entered block.

3.1 Programming and Executing Simple Positioning Blocks

22

3 Positioning with Manual Data Input (MDI)

4

Programming:

Fundamentals of NC,
File Management,
Programming Aids

4.1 Fundamentals of NC

Position encoders and reference marks

The machine axes are equipped with position encoders that
register the positions of the machine table or tool. When a machine
axis moves, the corresponding position encoder generates an
electrical signal. The TNC evaluates this signal and calculates the
precise actual position of the machine axis.

If there is an interruption of power, the calculated position will no
longer correspond to the actual position of the machine slide. The
TNC can re-establish this relationship with the aid of reference
marks when power is returned. 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 the signal the TNC identifies

4.1 Fundamentals of NC

that position as the machine-axis reference point and can re­establish the assignment of displayed positions to machine axis
positions.

Linear encoders are generally used for linear axes. Rotary tables
and tilt axes have angle encoders. If the position encoders feature
distance-coded reference marks, you only need to move each axis a
maximum of 20 mm (0.8 in.) for linear encoders, and 20° for angle
encoders, to re-establish the assignment of the displayed positions
to machine axis positions.

Z

Y

X

X

MP

X (Z,Y)

24

4 Programming: Fundamentals of NC, File Management, Programming Aids

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 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 (datum) you define within the coordinate
system. Relative coordinate values are also referred to as
incremental coordinate values.

Reference systems on milling machines

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

The TNC 310 can control up to 4 axes. The axes U, V and W are
secondary linear axes parallel to the main axes X, Y and Z,
respectively. Rotary axes are designated as A, B and C. The
illustration shows the assignment of secondary axes and rotary
axes to the main axes.

+Y

Z

Y

X

4.1 Fundamentals of NC

+Z

+Y

+X

+Z

+X

V+

Z

Y

W+

C+

B+

A+

X

U+

25HEIDENHAIN TNC 310

Polar coordinates

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

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

■ Polar Radius, the distance from the circle center CC to the

position, and the

■ Polar Angle, the size of the angle between the reference axis and

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

4.1 Fundamentals of NC

See figure to the lower right.

Definition of pole and 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) Reference axis of the angle

XY +X
YZ +Y
ZX +Z

10

Z

Y

PR

PA

2

PA

3

PR

CC

PA

PR

1

0°

X

30

Y

Z

Y

X

Z

Y

26

X

X

4 Programming: Fundamentals of NC, File Management, Programming Aids

Absolute and relative workpiece positions

Absolute workpiece positions

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

Example 1: Holes dimensioned in absolute coordinates

Hole
X=10 mm X=30 mm X=50 mm

Y=10 mm Y=20 mm Y=30 mm

Hole Hole

30

20

10

Y

3

2

1

Relative workpiece positions

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

To program a position in incremental coordinates, enter the prefix
“I”(soft key) before the axis.

Example 2: Holes dimensioned with relative coordinates

Absolute coordinates of hole

:

X= 10 mm
Y= 10 mm

referenced to hole Hole referenced to hole

Hole
IX= 20 mm IX= 20 mm

IY= 10 mm IY= 10 mm

Absolute and incremental polar coordinates

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

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

10

10 10

3010

50

4.1 Fundamentals of NC

Y

6

5

4

X

20

10

20

Y

X

10

PR

+IPA

+IPR

PR

+IPA

30

CC

PA

PR

0°

X

27HEIDENHAIN TNC 310

Selecting the datum

A production drawing identifies a certain point on the workpiecee
— usually a cornerr — as the absolute datum. Before setting the
datum, you align the workpiece with the machine axes and move
the tool in each axis to a known position relative to the workpiece.
You then set the TNC display to either zero or a predetermined
position value. 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. For further
information, refer to section 8.6 “Coordinate Transformation
Cycles.”

If the production drawing is not dimensioned for NC, set the datum

4.1 Fundamentals of NC

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

The fastest, easiest and most accurate way of setting the datum is
by using a 3-D touch probe from HEIDENHAIN. For further
information, refer to section 11.2 “Setting the Datum with a 3-D
Touch Probe.”

Example

The workpiece drawing at right illustrates the holes
are dimensioned to an absolute datum with the coordinates X=0
Y=0. The holes
absolute coordinates X=450 Y=750. By using the DATUM SHIFT
cycle you can shift the datum temporarily to the position X=450,
Y=750 and program the holes
calculations.

to are referenced to a relative datum with the

to without any further

to , which

750

320

Z

Y

X

Y

150

0

7
6

-150

0,1

5

±

300

1

3

0

2

4

28

325

450 900

950

4 Programming: Fundamentals of NC, File Management, Programming Aids

X

4.2 File Management

Files and file management

When you write a part program on the TNC, you must first enter a
file name. The TNC then stores the program as a file with the same
name. You can also store tables as files.

File names

The name of a file can have up to 8 characters. When you store
programs and tables as files, the TNC adds an extension to the file
name, separated by a point. This extension identifies the file type
(see table at right).

35720 .H

File name File type

The TNC can manage up to 64 files. Their total size, however, must
not exceed 128 MB.

Working with the file manager

This section informs you about the meaning of the individual
screen information, and describes how to select files. If you are not
yet familiar with the TNC file manager, we recommend that you
read this section completely and test the individual functions on
your TNC.

Call the file manager.

Press the PGM NAME soft key:
the TNC displays the file management window

Files in the TNC Type

Programs

in HEIDENHAIN conversational format .H

4.2 File Management

Table for

Tools .T

Display Meaning

FILE NAME Name with up to 8 characters

and file type Number following

the name:

File size in bytes

Status Properties of the file:

M Program is selected

in a Program Run
operating mode

P Protect a file against editing

and erasure (Protected)

The window shows all of the files that are stored in the TNC. Each
file is shown with additional information that is illustrated in the
table on the next page.

29HEIDENHAIN TNC 310

Select a file

Call the file manager.

<

Use the arrow keys to move the highlight to the desired file:

Move the highlight up or down

Delete a file

ú Move the highlight to the file you want to delete.

ú To select the erasing function,

press the DELETE soft key.
The TNC inquires whether you
really intend to erase the file.

ú To confirm erasure: Press the YES

soft key. Abort with the NO soft key
if you do not wish to erase the
directory

Enter the first or more numbers of the file you wish to select and

4.2 File Management

then press the GOTO key: The highlight moves to the first file that
matches these numbers.

<

The selected file is opened in the operating
mode from which you have the called file
manager: Press ENT.

Copy a file

ú Move the highlight to the file you wish to copy.

ú Press the COPY soft key to select the copying

function.

ú Enter the name of the destination file and confirm your entry with

the ENT key: The TNC copies the file. The original file is retained.

Rename a file

ú Move the highlight to the file you wish to rename.

ú Select the renaming function.
ú Enter the new file name; the file type cannot be

changed.

ú To execute renaming, press the ENT key.

Protecting a file/Canceling file
protection

ú Move the highlight to the file you want to protect.

ú To enable file protection, press the

PROTECT/UNPROTECT soft key.
The file now has status P.

To cancel file protection, proceed in the same way
using the PROTECT/UNPROTECT soft key. You also
need to enter the code number 86357.

30

4 Programming: Fundamentals of NC, File Management, Programming Aids

Read in/read out files

ú To read in or read out files: Press the ENT soft key.

The TNC provides the following functions:

Functions for reading in/reading out files Soft key

Read in all files

Only read in selected files; To accept a file
suggested by the TNC, press the YES soft key;
Press the NO soft key if you do not want to accept it.

Read in the selected file: Enter the file name

Read out the selected file: Move the highlight to
the desired file and confirm with ENT

Read out all of the files in the TNC memory

Display the file directories of the external unit on
your TNC screen

4.2 File Management

31HEIDENHAIN TNC 310

4.3 Creating and Writing Programs

Organization of an NC program in HEIDENHAIN
conversational format.

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

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

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

■ The blank form

■ tool definitions and tool calls,

■ 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.

4.3 Creating and Writing Programs

Defining the blank form — BLK FORM

Immediately after initiating a new program, you define a cuboid
workpiece blank. 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 30 000 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.

Block:

10 L X+10 Y+5 R0 F100 M3

Path function Words

Block number

Z

Y

MAX

X

32

The TNC can display the graphic only if the short side of
the BLK FORM is longer than 1/64 of the long side.

4 Programming: Fundamentals of NC, File Management, Programming Aids

MIN

Creating a new part program

You always enter a part program in the PROGRAMMING AND
EDITING mode of operation.

Program initiation in an example:

Select the PROGRAMMING AND EDITING
mode of operation.

<

Call up the file manager: Press the PGM NAME
soft key

FILE NAME=

<

3056

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

Program input : HDH / MM

<

Select the default setting for unit of
measurement (mm): Press the ENT key, or

Switch to using inches: Press the CHANGE MM/
INCH soft key

4.3 Creating and Writing Programs

33HEIDENHAIN TNC 310

Define the blank

Open the dialog for blank definition: Press the
BLK FORM soft key

WORKING SPINDLE AXIS X/Y/Z ?

<

Enter the spindle axis.

DEF BLK FORM: MIN-CORNER?

<

0

0

-40

DEF BLK FORM: MAX-CORNER?

4.3 Creating and Writing Programs

<

100

100

0

Enter in sequence the X, Y and Z coordinates of
the MIN point.

Enter in sequence the X, Y and Z coordinates of
the MAX point.

The program blocks window shows the following BLK FORM
definition

0 BEGIN PGM 3056 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 3056 MM

The TNC automatically generates the block numbers as well as the
BEGIN and END blocks.

34

4 Programming: Fundamentals of NC, File Management, Programming Aids

Program begin, name, unit of measure
Tool axis, MIN point coordinates
MAX point coordinates
Program end, name, unit of measure

Programming tool movements in conversational
format

To program a block, initiate the dialog by pressing a soft key. In the
screen headline, the TNC then asks you for all the information
necessary to program the desired function.

Example of a dialog

Initiate the dialog.

COORDINATES ?

10 Enter the target coordinate for the X axis.

5 Enter the target coordinate for the Y axis,

RADIUS COMP. RL/RR/NO COMP. ?

FEED RATE ? F=

100

MISCELLANEOUS FUNCTION M ?

3

<

<

and go to the next question with ENT.

<

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 will
terminate this dialog.

Functions during the dialog Key

Ignore the dialog question

End the dialog immediately

Abort the dialog and erase the block

4.3 Creating and Writing Programs

The program blocks window will display the following line:

3 L X+10 Y+5 R0 F100 M3

35HEIDENHAIN TNC 310

Editing program lines

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 (see table at right).

Selecting blocks or words Keys

Move from one block to the next

Looking for the same words in different blocks

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.

Inserting blocks at any desired location

ú Select the block after which you want to insert a new block and

4.3 Creating and Writing Programs

initiate the dialog.

Editing and inserting words

ú Select a word in a block and overwrite it with the new one. The

plain-language dialog is available while the word is highlighted.

ú To conclude editing, press the END key.

If you want to insert a word, press the horizontal arrow keys
repeatedly until the desired dialog appears. You can then enter the
desired value.

Select individual words in a block

Erasing blocks and words 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 (cycle)

Delete the program sections:
First select the last block of the
program section to be erased, then
erase with the DEL key.

36

4 Programming: Fundamentals of NC, File Management, Programming Aids

4.4 Interactive Programming Graphics

While you are writing the part program, you can have the TNC
generate a graphic illustration of the programmed contour.

To generate/not generate graphics during programming:

ú To switch the screen layout to displaying program blocks to the

left and graphics to the right, press the SPLIT SCREEN key and
PGM + GRAPHICS soft key.

ú Set the AUTO DRAW soft key to ON. While you are

entering the program lines, the TNC generates
each path contour you program in the graphics
window in the right screen half.

If you do not wish to have graphics generated during programming,
set the AUTO DRAW soft key to OFF.

AUTO DRAW ON does not simulate program section repeats.

To generate a graphic for an existing program:

ú Use the arrow keys to select the block up to which you want the

graphic to be generated, or press GOTO and enter the desired
block number.

ú To generate graphics, press the RESET + START

soft key.

Additional functions are listed in the table at right.

To erase the graphic:

ú Shift the soft-key row (see figure at right)
ú Delete graphic: Press CLEAR GRAPHIC soft key

Functions Soft key

Generate interactive graphics
blockwise

Generate a complete graphic
or complete it after
RESET + START

Interrupt interactive graphics
This soft key only appears while the
TNC generates the interactive graphics

4.4 Interactive Programming Graphics

37HEIDENHAIN TNC 310

Magnifying or reducing a detail

You can select the graphics display by selecting a detail with the
frame overlay. You can now magnify or reduce the selected detail.

ú Select the soft-key row for detail magnification/reduction

(last row, see figure at right)
The following functions are available:

Function Soft key

Reduce the frame overlay — press and
hold the soft key to reduce the detail

Enlarge the frame overlay — press and
hold the soft key to magnify the detail

Move the frame overlay to the left:
Press and hold the soft key. Move the frame
overlay to the right:
Press and hold the arrow to the right soft key

4.4 Interactive Programming Graphics

With the WINDOW BLK FORM soft key, you can restore the original
section.

ú Confirm the selected section with the WINDOW

DETAIL soft key

38

4 Programming: Fundamentals of NC, File Management, Programming Aids

4.5 HELP Function

Certain TNC programming functions are explained in more detail in
the HELP function. You can select a HELP topic using soft keys.

.

Select the HELP function

ú Press the HELP key
ú Select a topic: Press one of the available soft keys

Help topics / Functions Soft key

M functions

Cycle parameters

HELP that is entered by the machine
manufacturers (optional)

Go to previous page

Go to next page

Go to beginning of file

Go to end of file

Select search functions; Enter a number,
Begin search with ENT key

Leave HELP function

Press the END key or the HELP key.

4.5 HELP Function

39HEIDENHAIN TNC 310

Programming:

Tools

5

5.1 Entering Tool-Related Data

Feed rate F

The feed rate is the speed (in millimeters per minute or inches per
minute) at which the tool center moves. The maximum feed rates
can be different for the individual axes and are set in machine
parameters.

Input

You can enter the feed rate in every positioning block. For further
information refer to section 6.2 “Fundamentals of Path Contours.”

Rapid traverse

If you wish to program rapid traverse, enter FMAX. To enter F, press
the ENT key or the FMAX soft key as soon as the dialog question
“FEED RATE F = ?” appears on the TNC screen.

Duration of effect

A feed rate entered as a numerical value remains in effect until a

5.1 Entering Tool-Related Data

block with a different feed rate is reached. F MAX is only effective in
the block in which it is programmed. After the block with F MAX is
executed, the feed rate will return to the last feed rate entered as a
numerical value.

Changing the spindle speed during program run

You can adjust the feed rate during program run with the feed-rate
override knob.

Spindle speed S

The spindle speed S is entered in revolutions per minute (rpm) in a
TOOL CALL block.

Z

S

S

Y

F

X

Programmed change

In the part program, you can change the spindle speed in a TOOL
CALL block by entering the spindle speed only:

ú To program a tool call, press the

TOOL CALL soft key (3rd soft-key row)

ú Ignore the dialog question for „TOOL NUMBER ?“

with the right arrow key

ú Ignore the dialog question for „WORKING SPINDLE

AXIS X/Y/Z ?“ with the right arrow key

ú Enter the new spindle speed for the dialog

question “SPINDLE SPEED S= ?”.

Changing the spindle speed during program run

You can adjust the spindle speed during program run with the
spindle-speed override knob.

42

5 Programming: Tools

5.2 Tool Data

You usually program the coordinates of path contours as they are
dimensioned in the workpiece drawing. To allow the TNC to
calculate the tool center path — i.e. the tool compensation — you
must also enter the length and radius of each tool you are using.

Tool data can be entered either directly in the part program with
TOOL DEF or (and) separately in tool tables. The TNC will consider
all of the data entered when executing the part program.

Tool number

Each tool is identified by a number between 0 and 254. If you are
working with tool tables, each tool in the table is given a number
between 0
and 99.

The tool number 0 is automatically defined as the zero tool with the
length L=0 and the radius R=0. In tool tables, tool 0 should also be
defined with L=0 and R=0.

Tool length L

There are two ways to determine the tool length L:
1 The length L is the difference between the length of the tool and

that of a zero tool L

For the algebraic sign:

■ The tool is longer than the zero tool L>L

■ The tool is shorter than the zero tool: L<L

.

0

0

0

Z

L

0

5.2 Tool Data

X

To determine the length:

ú Move the zero tool to the reference position in the tool axis

(e.g. workpiece surface with Z=0).

ú Set the datum in the tool axis to 0 (datum setting).
ú Insert the desired tool.
ú Move the tool to the same reference position as the zero tool.
ú The TNC displays the difference between the current tool and the

zero tool.

ú Enter the value in the TOOL DEF block or in the tool table by

pressing the „ACTUAL POSITION“ key

2 If you determine the length L with a tool presetter, this value can

be entered directly in the TOOL DEF block without further
calculations.

43HEIDENHAIN TNC 310

Tool radius R

You can enter the tool radius R directly.

Delta values for lengths and radii

Delta values are offsets in the length and radius of a tool.
A positive delta value describes a tool oversize (DR>0), a negative

5.2 Tool Data

delta value describes a tool undersize (DR<0). Enter the delta
values when you are programming with TOOL CALL.

Input range: You can enter a delta value with up to ± 99.999 mm.

R

L

DR<0

R

Entering tool data into the program

The number, length and radius of a specific tool is defined in the
TOOL DEF block of the part program.

ú To select tool definition, press the TOOL DEF key.
ú Enter the TOOL NUMBER: Each tool is uniquely

identified by its number. When the tool table is
active, enter tool numbers greater than 99
(dependent on MP7260)

ú To enter the TOOL LENGTH, enter the

compensation value for the tool length.

ú Enter the TOOL RADIUS.

During the dialog, you can take the values for length and
radius directly from the position display with the soft
keys „CUR.POS X, CUR.POS Y or CUR.POS Z“.

Resulting NC block:

4 TOOL DEF 5 L+10 R+5

DR>0

DL<0

DL>0

44

5 Programming: Tools

Entering tool data in tables

You can define and store up to 99 tools and their tool data in the
tool table TOOL.T. (The maximum number of tools in the table can
be set in machine parameter 7260).

Tool table: Available input data

Abbr. Input

T Number by which the tool is called in the program
L Value for tool length compensation
R Tool radius R

Editing the tool table

The tool table has the file name TOOL.T. The
TOOL.T file can be edited in the PROGRAMMING AND EDITING
operating mode. TOOL.T is automatically active in a program run
operating mode.

To open the tool table TOOL.T:

Select the PROGRAMMING AND EDITING mode of operation.

ú call the file manager.
ú Move the highlight to TOOL.T. Confirm with the

ENT key.

When you have opened the tool table, you can edit the tool data by
moving the cursor to the desired position in the table with the
arrow keys (see figure at center right). You can overwrite the stored
values, or enter new values at any position. The available editing
functions are illustrated in the table on the next page.

To leave the tool table:

ú Finish editing the tool table: Press the END key.
ú Call the file manager and select a file of a different type, e.g. a

part program.

Dialog

–
TOOL LENGTH ?
TOOL RADIUS ?

5.2 Tool Data

45HEIDENHAIN TNC 310

Editing functions for tool tables Soft key

Take the value from the position
display

Go to the previous page of the table
(2nd soft-key row)

5.2 Tool Data

Go to the next page of the table
(2nd soft-key row)

Move the highlight one column to
the left

Move the highlight one column to
the right

Delete incorrect numerical value,
re-establish preset value

Re-establish the last value stored

Move the highlight back to beginning of line

46

5 Programming: Tools

Calling tool data

A TOOL CALL block in the part program is defined with the
following data:

ú Select the tool call function with the TOOL CALL

key

ú TOOL NUMBER: Enter the number of the tool. The

tool must already be defined in a TOOL DEF block
or in the tool table.

ú WORKING SPINDLE AXIS X/Y/Z: Enter the tool axis.
ú SPINDLE SPEED S
ú TOOL LENGTH OVERSIZE: Enter the delta value for

the tool length.

ú TOOL RADIUS OVERSIZE: Enter the delta value for

the tool radius.

Example:

Call tool number 5 in the tool axis Z with a spindle speed 2500 rpm.
The tool length is to be programmed with an oversize of 0.2 mm,
the tool radius with an undersize of 1 mm.

20 TOOL CALL 5 Z S2500 DL+0.2 DR-1

The character D preceding L and R designates delta values.

Tool change

The tool change function can vary depending on the
individual machine tool. Your machine manual provides
more information on M101.

5.2 Tool Data

Tool change position

A tool change position must be approachable without collision. With
the miscellaneous functions M91 and M92, you can enter machine­referenced (rather than workpiece-referenced) coordinates for the
tool change position. If TOOL CALL 0 is programmed before the
first tool call, the TNC moves the tool spindle in the tool axis to a
position that is independent of the tool length.

Manual tool change

To change the tool manually, stop the spindle and move the tool to
the tool change position:

ú Move to the tool change position under program control.
ú Interrupt program run (see section 10.3 “Program Run”).
ú Change the tool.
ú Resume the program run (see section 10.3 “Program Run”).

47HEIDENHAIN TNC 310

5.3 Tool Compensation

The TNC adjusts the spindle path in the tool axis by the
compensation value for the tool length. In the working plane, it
compensates the tool radius.

If you are writing the part program directly on the TNC, the tool
radius compensation is effective only in the working plane.

Tool length compensation

Length compensation becomes effective automatically as soon as a
tool is called and the tool axis moves. To cancel length
compensation call a tool with the length L=0.

5.3 Tool Compensation

For tool length compensation, the TNC takes the delta values from
the TOOL CALL block into account:

Compensation value = L + DL
L is the tool length L from the TOOL DEF block or tool

DL

If you cancel a positive length compensation with TOOL
CALL 0, the distance between tool and workpiece will
be reduced.

After TOOL CALL, the path of the tool in the tool axis, as
entered in the part program, is adjusted by the difference
between the length of the previous tool and that of the
new one.

where

TOOL CALL

TOOL CALL

table
is the oversize for length DL in the TOOL CALL block

(not taken into account by the position display)

Tool radius compensation

The NC block for programming a tool movement contains:

■ RL or RR for compensation in the tool radius

■ R+ or R– for radius compensation in single-axis movements

■ R0 if no radius compensation is required

Radius compensation becomes effective as soon as a tool is called
and is moved in the working plane with RL or RR. To cancel radius
compensation, program a positioning block with R0.

48

5 Programming: Tools

For tool radius compensation, the TNC takes the delta values from

R

R

R0

RL

the TOOL CALL block into account:
Compensation value = R + DR

TOOL CALL,

where

R is the tool radius R from the TOOL DEF block or tool

table

DR

TOOL CALL

is the oversize for radius DR in the TOOL CALL block
(not taken into account by the position display)

Tool movements without radius compensation: R0

The tool center moves in the working plane to the programmed
path or coordinates.

Applications: Drilling and boring, pre-positioning
(see figure at center right)

Tool movements with radius compensation: RR and RL
RR The tool moves to the right of the programmed contour
RL The tool moves to the left of the programmed contour

The tool center moves along the contour at a distance equal to the
radius. “Right” or “left” are to be understood as based on the
direction of tool movement along the workpiece contour (see
illustrations on the next page).

Between two program blocks with different radius
compensations (RR and RL) you must program at least
one block without radius compensation (that is, with R0).

Radius compensation does not come into effect until the
end of the block in which it is first programmed.

Whenever radius compensation is activated with RR/RL
or canceled with R0, the TNC positions the tool
perpendicular to the programmed starting or end
position. Position the tool at a sufficient distance from
the first or last contour point to prevent the possibility of
damaging the contour.

5.3 Tool Compensation

Z

Y

X

Y

X

49HEIDENHAIN TNC 310

Entering radius compensation

When you program a path contour, the following dialog question is
displayed after entry of the coordinates:

RADIUS COMP. RL/RR/NO COMP. ?

<

To select tool movement to the left of the
contour, press the RL soft key, or

To select tool movement to the right of the
contour, press the RR soft key, or

Y

RL

5.3 Tool Compensation

To select tool movement without radius
compensation or to cancel radius
compensation, press the ENT key or the R0 soft
key.

To terminate the dialog, press the END key.

X

Y

RR

X

50

5 Programming: Tools

Radius compensation: Machining corners

Outside corners

If you program radius compensation, the TNC moves the tool in a
transitional arc around corners. The tool “rolls around” the corner
point. If necessary, the TNC reduces the feed rate at outside
corners to reduce machine stress, for example at very great
changes of direction.

Inside corners

The TNC calculates the intersection of the tool center paths at
inside corners under radius compensation. From this point it then
starts the next contour element. This prevents damage to the
workpiece. The permissible tool radius, therefore, is limited by the
geometry of the programmed contour.

To prevent the tool from damaging the contour, be
careful not to program the starting or end position for
machining inside corners at a corner of the contour.

Machining corners without radius compensation

If you program the tool movement without radius compensation,
you can change the tool path and feed rate at workpiece corners
with the miscellaneous function M90. See ”7.4 Miscellaneous
Functions for Contouring Behavior.”

RL

5.3 Tool Compensation

RL RL

51HEIDENHAIN TNC 310

6

Programming:

Programming Contours

6.1 Overview of Tool Movements

Path functions

A workpiece contour is usually composed of several contour
elements such as straight lines and circular arcs. With the path
functions, you can program the tool movements for straight lines
and circular arcs.

Miscellaneous functions M

With the TNC’s miscellaneous functions you can affect

■ program run, such as a program interruption

■ machine functions, such as switching spindle rotation and coolant

supply on and off

■ contouring behavior of the tool.

Subprograms and program section repeats

6.1 Overview of Tool Movements

If a machining sequence occurs several times in a program, you can
save time and reduce the chance of programming errors by
entering the sequence once and then defining it as a subprogram
or program section repeat. If you wish to execute a specific pro­gram section only under certain conditions, you also define this
machining sequence as a subprogram. In addition, you can have a
part program call a separate program for execution.

How subprograms and program section repeats are used in
programming is described in Chapter 9.

L

L

CC

L

C

Y

80

60

40

CC

R40

54

11510

X

6 Programming: Programming Contours

6.2 Fundamentals of Path Functions

Programming tool movements for workpiece
machining

You create a part program by programming the path functions for
the individual contour elements in sequence. You usually do this by
entering the coordinates of the end points of the contour
elements given in the production drawing. The TNC calculates the
actual path of the tool from these coordinates, and from the tool
data and radius compensation.

The TNC moves all axes programmed in a single block
simultaneously.

Movement parallel to the machine axes

The program block contains only one coordinate. The TNC thus
moves the tool parallel to the programmed axis.

Depending on the individual machine tool, the part program is
executed by movement of either the tool or the machine table on
which the workpiece is clamped. Nevertheless, you always pro­gram path contours as if the tool moves and the workpiece remains
stationary.

Example:

L X+100
L

X+100

The tool retains the Y and Z coordinates and moves to the position
X=100. See figure at upper right.

Movement in the main planes

The program block contains two coordinates. The TNC thus moves
the tool in the programmed plane.

Example:

L X+70 Y+50

The tool retains the Z coordinate and moves in the XY plane to the
position X=70, Y=50. See figure at center right.

Path function for “straight line”
Coordinate of the end point

50

Z

Y

X

100

Z

6.2 Fundamentals of Path Functions

Y

X

70

Z

Three-dimensional movement

The program block contains three coordinates. The TNC thus moves
the tool in space to the programmed position.

Example:

L X+80 Y+0 Z-10

This example is illustrated in the figure at lower right.

Y

-10

X

80

55HEIDENHAIN TNC 310

Circles and circular arcs

The TNC moves two axes simultaneously in a circular path relative
to the workpiece. You can define a circular movement by entering
the circle center CC.

Y

When you program a circle, the TNC assigns it to one of the main
planes. This plane is defined automatically when you set the
spindle axis during a tool call:

Spindle axis Main plane
ZXY

YZX
XYZ

Direction of rotation DR for circular movements

When a circular path has no tangential transition to another contour
element, enter the direction of rotation DR:

Clockwise direction of rotation: DR–
Counterclockwise direction of rotation: DR+

Radius compensation

Radius compensation must be programmed before the block
containing the coordinates for the first contour element. You cannot

6.2 Fundamentals of Path Functions

begin radius compensation in a circle block. It must be activated
beforehand in a straight-line block.

Z

Y

Pre-positioning

Before running a part program, always pre-position the tool to
prevent the possibility of damaging it or the workpiece.

DR–

CC

Y

Y

C

C

X

CC

X

CC

X

DR+

CC

X

56

6 Programming: Programming Contours

Creating the program blocks with the path function keys

Use the path function keys to open a conversational dialog. The
TNC asks you successively for all the necessary information and
inserts the program block into the part program.

Example — programming a straight line:

Initiate the programming dialog (here, for a
straight line).

COORDINATES ?

<

10

Enter the coordinates of the straight-line end
point.

5

Transfer the coordinates of the selected axis:
Press ACTUAL POSITION soft key (second soft­key row)

RADIUS COMP. RL/RR/NO COMP. ?

<

Select the radius compensation (here, press the
RL soft key — the tool moves to the left of the
programmed contour).

FEED RATE F=

<

100

Enter the feed rate (here, 100 mm/min), and

confirm your entry with ENT.

MISCELLANEOUS FUNCTION M ?

<

3

Enter a miscellaneous function (here, M3), and

terminate the dialog with ENT.

The part program now contains the following line:

L X+10 Y+5 RL F100 M3

6.2 Fundamentals of Path Functions

57HEIDENHAIN TNC 310

6.3 Path Contours — Cartesian
Coordinates

Overview of path functions

Function Contour function soft key

Line L

CHamFer

Circle Center

Circle

Circle by Radius

Circle Tangential

6.3 Path Contours — Cartesian Coordinates

Corner RouNDing

Tool movement

Straight line

Chamfer between two straight lines

No tool movement

Circular arc around a circle
center CC to an arc end point

Circular arc with a certain radius

Circular arc with tangential connection
to the preceding contour element

Circular arc with tangential connection
to the preceding and subsequent contour
elements

Required input

Coordinates of the straight-line
end point

Chamfer side length

Coordinates of the circle center or
pole

Coordinates of the arc end point,
direction of rotation

Coordinates of the arc end point,
arc radius, direction of rotation

Coordinates of the arc end point

Rounding-off radius R

58

6 Programming: Programming Contours

Straight line L

The tool moves on a straight line from its current position to the
line end point. The starting point for the straight line is the end
point that was programmed in the preceding block.

ú Enter the COORDINATES of the end point.

Further entries, if necessary:

ú RADIUS COMPENSATION RL/RR/R0
ú FEED RATE F
ú MISCELLANEOUS FUNCTION M

Example NC blocks

7 L X+10 Y+40 RL F200 M3
8 L IX+20 IY-15
9 L X+60 IY-10

40

Y

15

10

10

20

X

60

Inserting a chamfer CHF between two straight lines

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

■ The blocks before and after the CHF block must be in the same

working plane.

■ The radius compensation before and after the chamfer block must

be the same.

■ An inside chamfer must be large enough to accommodate the

current tool.

ú CHAMFER SIDE LENGTH: Enter the length of the

chamfer

Example NC blocks

7 L X+0 Y+30 RL F300 M3
8 L X+40 IY+5
9 CHF 12
10 L IX+5 Y+0

You cannot start a contour with a CHF block
A chamfer is possible only in the working plane.
The feed rate for chamferring is taken from the

preceding block.
The corner point is cut off by the chamfer and is not part

of the contour.

30

Y

6.3 Path Contours — Cartesian Coordinates

X

Y

5

12

40

12

5

X

59HEIDENHAIN TNC 310

Circle center CC

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

■ Entering the Cartesian coordinates of the circle center

■ Using the circle center defined in an earlier block

■ Capturing the coordinates with the

„ACTUAL POSITION“ soft key

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú COORDINATES CC: Enter the circle center

coordinates
If you want to use the last programmed position,

do not enter any coordinates.

Example NC blocks

5 CC X+25 Y+25

or

10 L X+25 Y+25
11 CC

The program blocks 10 and 11 do not refer to the illustration.

Duration of effect

6.3 Path Contours — Cartesian Coordinates

The circle center definition remains in effect until a new circle
center is programmed.

Z

Y

CC

Y

CC

X

CC

X

Entering the circle center CC incrementally

If you enter the circle center with incremental coordinates, you
have programmed it relative to the last programmed position of the
tool.

The only effect of CC is to define a position as a circle
center — the tool does not move to the position.

The circle center also serves as the pole for polar
coordinates.

60

6 Programming: Programming Contours

Circular path C around circle center CC

Before programming a circular path C, you must first enter the
circle center CC. The last programmed tool position before the C
block is used as the circle starting point.

ú Move the tool to the circle starting point.

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Enter the COORDINATES of the circle center.

ú Enter the COORDINATES of the arc end point
ú DIRECTION OF ROTATION DR

Further entries, if necessary:

ú FEED RATE F
ú MISCELLANEOUS FUNCTION M

Y

E

CC

S

X

Example NC blocks

5 CC X+25 Y+25
6 L X+45 Y+25 RR F200 M3
7 C X+45 Y+25 DR+

Full circle

Enter the same point you used as the starting point for the end
point in a C block.

The starting and end points of the arc must lie on the
circle.

Input tolerance: up to 0.016 mm.

25

Y

DR+

CC

6.3 Path Contours — Cartesian Coordinates

DR–

25

45

X

61HEIDENHAIN TNC 310

Circular path CR with defined radius

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

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Enter the COORDINATES of the arc end point.
ú RADIUS R

Note: The algebraic sign determines the size of the
arc.

ú DIRECTION OF ROTATION DR

Note: The algebraic sign determines whether the
arc is concave or convex.

Further entries, if necessary:

ú FEED RATE F
ú MISCELLANEOUS FUNCTION M

Y

E1=S

R

2

S1=E

CC

2

X

Full circle

For a full circle, program two CR blocks in succession:
The end point of the first semicircle is the starting point of the

second. The end point of the second semicircle is the starting point
of the first. See figure at upper right.

Central angle CCA and arc radius R

The starting and end points on the contour can be connected with
four arcs of the same radius:

6.3 Path Contours — Cartesian Coordinates

Smaller arc: CCA<180°
Enter the radius with a positive sign R>0

Larger arc: CCA>180°
Enter the radius with a negative sign R<0

The direction of rotation determines whether the arc is curving
outward (convex) or curving inward (concave):

Convex: Direction of rotation DR– (with radius compensation RL)
Concave: Direction of rotation DR+ (with radius compensation RL)

Example NC blocks

See figures at middle and lower right.

10 L X+40 Y+40 RL F200 M3
11 CR X+70 Y+40 R+20 DR (arc 1)

or

11 CR X+70 Y+40 R+20 DR+ (arc 2)

or

11 CR X+70 Y+40 R-20 DR- (arc 3)

or

11 CR X+70 Y+40 R-20 DR+ (arc 4)

40

40

Y

1

DR+

ZW

R

R

2

X

40 70

Y

DR+

3

ZW

R

40 70

R

4

X

Please observe the notes on the next page!

62

6 Programming: Programming Contours

The distance from the starting and end points of the arc
diameter cannot be greater than the diameter of the arc.

The maximum possible radius is 30 m.

Circular path CT with tangential connection

The tool moves on an arc that starts at a tangent with the previously
programmed contour element.

A transition 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.

ú Select circle functions: Press the „CIRCLE“ soft key

(2nd soft-key row)

ú Enter the COORDINATES of the arc end point.

Further entries, if necessary:

ú FEED RATE F
ú MISCELLANEOUS FUNCTION M

Example NC blocks

7 L X+0 Y+25 RL F300 M3
8 L X+25 Y+30
9 CT X+45 Y+20
10 L Y+0

30
25

Y

20

25

45

X

6.3 Path Contours — Cartesian Coordinates

A tangential arc is a two-dimensional operation: the
coordinates in the CT block and in the contour element
preceding it must be in the same plane of the arc.

63HEIDENHAIN TNC 310

Corner Rounding RND

The RND function is used for rounding off corners.
The tool moves on an arc that is tangentially connected to both the

preceding and subsequent contour elements.
The rounding arc must be large enough to accommodate the tool.

ú ROUNDING-OFF RADIUS: Enter the radius of the

arc.

ú FEED RATE for rounding the corner.

Example NC blocks

5 L X+10 Y+40 RL F300 M3
6 L X+40 Y+25
7 RND R5 F100
8 L X+10 Y+5

In the preceding and subsequent contour elements,
both coordinates must lie in the plane of the rounding
arc.

The corner point is cut off by the rounding arc and is not
part of the contour.

A feed rate programmed in the RND block is effective
only in that block. After the RND block, the previous feed

6.3 Path Contours — Cartesian Coordinates

rate becomes effective again.
You can also use an RND block for a tangential contour

approach if you do not want to use an APPR function.

40

Y

R5

5

25

X

10

40

64

6 Programming: Programming Contours

Example: Linear movements and chamfers with Cartesian coordinatesExample: Linear movements and chamfers with Cartesian coordinates

0 BEGIN PGM 10 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+10
4 TOOL CALL 1 Z S4000
5 L Z+250 R0 F MAX
6 L X-20 Y-10 R0 F MAX
7 L Z-5 R0 F1000 M3
8 L X+5 Y+5 RL F300
9 RND R2
10 L Y+95
11 L X+95
12 CHF 10
13 L Y+5
14 CHF 20
15 L X+5
16 RND R2
17 L X-20 R0 F1000
18 L Z+250 R0 F MAX M2
19 END PGM 10 MM

Y

95

5

5

Define blank form for graphic workpiece simulation

Define tool in the program
Call tool in the spindle axis and with the spindle speed S
Retract tool in the spindle axis at rapid traverse FMAX
Pre-position the tool
Move to working depth at feed rate F = 1000 mm/min
Approach the contour at point 1
Tangential approach to circle with R=2 mm
Move to point 2
Point 3: first straight line for corner 3
Program chamfer with length 10 mm
Point 4: 2nd straight line for corner 3, 1st straight line for corner 4
Program chamfer with length 20 mm
Move to last contour point 1, second straight line for corner 4
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program

20

10

10

20

X

95

6.3 Path Contours — Cartesian Coordinates

65HEIDENHAIN TNC 310

Example: Circular movements with Cartesian coordinatesExample: Circular movements with Cartesian coordinates

Y

0 BEGIN PGM 20 MM

6.3 Path Contours — Cartesian Coordinates

1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+10
4 TOOL CALL 1 Z S4000
5 L Z+250 R0 F MAX
6 L X-20 Y-20 R0 F MAX
7 L Z-5 R0 F1000 M3
8 L X+5 Y+5 RL F300
9 RND R2
10 L Y+85
11 RND R10 F150
12 L X+30
13 CR X+70 Y+95 R+30 DR-
14 L X+95
15 L Y+40
16 CT X+40 Y+5

17 L X+5
18 RND R2
19 L X-20 Y-20 R0 F1000
20 L Z+250 R0 F MAX M2
21 END PGM 20 MM

95

85

40

5

Define blank form for graphic workpiece simulation

Define tool in the program
Call tool in the spindle axis and with the spindle speed S
Retract tool in the spindle axis at rapid traverse FMAX
Pre-position the tool
Move to working depth at feed rate F = 1000 mm/min
Approach the contour at point 1
Tangential approach to circle with R=2 mm
Point 2: first straight line for corner 2
Insert radius with R = 10 mm, feed rate: 150 mm/min
Move to point 3: Starting point of the arc with CR
Move to point 4: End point of the arc with CR, radius 30 mm
Move to point 5
Move to point 6
Move to point 7: End point of the arc, radius with tangential
connection to point 6, TNC automatically calculates the radius
Move to last contour point 1
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program

R10

5

R30

4030 70

95

X

66

6 Programming: Programming Contours

Example: Full circle with Cartesian coordinatesExample: Full circle with Cartesian coordinates

Y

0 BEGIN PGM 30 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+12.5
4 TOOL CALL 1 Z S3150
5 CC X+50 Y+50
6 L Z+250 R0 F MAX
7 L X-40 Y+50 R0 F MAX
8 L Z-5 R0 F1000 M3
9 L X+0 Y+50 RL F300
10 RND R2
11 C X+0 DR-
12 RND R2
13 L X-40 Y+50 R0 F1000
14 L Z+250 R0 F MAX M2
15 END PGM 30 MM

50

Define the blank form

Define the tool
Call the tool
Define the circle center
Retract the tool
Pre-position the tool
Move to working depth
Approach starting point of circle
Tangential approach to circle with R=2 mm
Move to the circle end point (= circle starting point)
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program

CC

50

X

6.3 Path Contours — Cartesian Coordinates

67HEIDENHAIN TNC 310

6.4 Path Contours—
Polar Coordinates

With polar coordinates you can define a position in terms of its
angle PA and its distance PR relative to a previously defined pole
CC. See section ”4.1 Fundamentals of NC.”

Polar coordinates are useful with:

■ Positions on circular arcs

■ Workpiece drawing dimensions in degrees, e.g. bolt hole circles

Overview of path functions with polar coordinates

Function Contour function soft keys

Tool movement

Required input

Line LP

Circular arc CP +

Circular arc CTP +

6.4 Path Contours– Polar Coordinates

Helix +
(Helix)

+

Straight line

Circular path around circle center/pole
CC to arc end point

Circular path with tangential
connection to the preceding contour
element

Combination of a circular and a linear
movement

Polar coordinate origin: Pole CC

You can define the pole CC anywhere in the part program before
blocks containing polar coordinates. Enter the pole in Cartesian
coordinates as a circle center in a CC block.

ú Select circle functions: Press the „CIRCLE“ soft key

ú COORDINATES CC: Enter Cartesian coordinates for

the pole, or:
If you want to use the last programmed position,

do not enter any coordinates.

Polar radius, polar angle of the
straight-line end point

Polar angle of the arc end point,
direction of rotation

Polar radius, polar angle of the arc
end point

Polar radius, polar angle of the arc
end point, coordinate of the end
point in the tool axis

Y

Y

C

C

CC

68

X

X

CC

6 Programming: Programming Contours

Straight line LP

The tool moves in a straight line from its current position to the
straight-line end point. The starting point for the straight line is the
end point that was programmed in the preceding block.

ú Select straight line function: Press the L soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row). POLAR COORDINATES­RADIUS PR: Enter the distance from the pole CC to
the straight-line end point.

ú POLAR COORDINATES-ANGLE PA: Angular

position of the straight-line end point between –
360° and +360°

The sign of PA depends on the angle reference
axis:
Angle from angle reference axis to PR is
counterclockwise: PA>0
Angle from angle reference axis to PR is clockwise:
PA<0

Example NC blocks

12 CC X+45 Y+25
13 LP PR+30 PA+0 RR F300 M3
14 LP PA+60
15 LP IPA+60
16 LP PA+180

25

Y

30

60°

60°

CC

X

45

6.4 Path Contours– Polar Coordinates

Circular path CP around pole CC

The polar coordinate radius PR is also the radius of the arc. It is
defined by the distance from the starting point to the pole CC. The
last programmed tool position before the CP block is the starting
point of the arc.

ú Select circle functions: Press the „CIRCLE“ soft key

ú Select circular path C: Press the C soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú POLAR COORDINATES-ANGLE PA: Angular

position of the arc end point between –5400° and
+5400°

ú DIRECTION OF ROTATION DR

25

Y

R20

CC

25

X

69HEIDENHAIN TNC 310

Example NC blocks

18 CC X+25 Y+25
19 LP PR+20 PA+0 RR F250 M3
20 CP PA+180 DR+

For incremental coordinates, enter the same sign for DR
and PA.

Circular path CTP with tangential connection

The tool moves on a circular path, starting tangentially from a
preceding contour element.

ú Select circle functions: Press the „CIRCLE“ soft key

Y

120°

ú Select the circular path CT: Press the CT soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú POLAR COORDINATES-RADIUS PR: Distance from

the arc end point to the pole CC.

6.4 Path Contours– Polar Coordinates

ú POLAR COORDINATES-ANGLE PA: Angular

position of the arc end point.

Example NC blocks

12 CC X+40 Y+35
13 L X+0 Y+35 RL F250 M3
14 LP PR+25 PA+120
15 CTP PR+30 PA+30
16 L Y+0

The pole CC is not the center of the contour arc!

35

CC

R25

40

R30

30°

X

70

6 Programming: Programming Contours

Helical interpolation

A helix is a combination of a circular movement in a main plane and
a linear movement perpendicular to this plane.

A helix is programmed only in polar coordinates.

Applications

■ Large-diameter internal and external threads

■ Lubrication grooves

Calculating the helix

To program a helix, you must enter the total angle through which
the tool is to move on the helix in incremental dimensions, and the
total height of the helix.

For calculating a helix that is to be cut in a upward direction, you
need the following data:

Z

Y

CC

X

Thread revolutions n

Total height h
Incremental
total angle IPA

Starting coordinate Z

Shape of the helix

The table below illustrates in which way the shape of the helix is
determined by the work direction, direction of rotation and radius
compensation.

Internal thread Work direct. Direction Radius compens.

Right-handed Z+ DR+ RL
Left-handed Z+ DR– RR
Right-handed Z– DR– RR
Left-handed Z– DR+ RL

External thread

Right-handed Z+ DR+ RR
Left-handed Z+ DR– RL
Right-handed Z– DR– RL
Left-handed Z– DR+ RR

Thread revolutions + thread overrun at
the start and end of the thread
Thread pitch P x thread revolutions n
Thread revolutions x 360° + angle for
beginning of thread + angle for thread
overrun
Thread pitch P x (thread revolutions +
thread overrun at start of thread)

6.4 Path Contours– Polar Coordinates

71HEIDENHAIN TNC 310

Programming a helix

6.4 Path Contours– Polar Coordinates

Always enter the same algebraic sign for the direction of
rotation DR and the incremental total angle IPA. The tool
may otherwise move in a wrong path and damage the
contour.

For the total angle IPA, you can enter a value from
–5400° to +5400°. If the thread has of more than 15
revolutions, program the helix in a program section
repeat (see section 9.2 “Program Section Repeats”).

ú Select circle functions: Press the „CIRCLE“ soft key

ú Select circular path C: Press the C soft key

ú Select entry of polar coordinates: Press the P soft

key (2nd soft-key row).

ú POLAR COORDINATES-ANGLE: Enter the total

angle of tool traverse along the helix in incremental
dimensions. After entering the angle, identify the

tool axis using a soft key.

ú Enter the COORDINATE for the height of the helix

in incremental dimensions.

ú Direction of rotation DR

Clockwise helix: DR–
Counterclockwise helix: DR+

ú RADIUS COMPENSATION RL/RR/R0

Enter the radius compensation according to the
table above.

25

Z

Y

CC

270°

R3

5

X

40

Example NC blocks

12 CC X+40 Y+25
13 Z+0 F100 M3
14 LP PR+3 PA+270 RL F50
15 CP IPA1800 IZ+5 DR RL F50

72

6 Programming: Programming Contours

Example: Linear movement with polar coordinates

100

50

Y

60°

R45

CC

5

0 BEGIN PGM 40 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+7.5
4 TOOL CALL 1 Z S4000
5 CC X+50 Y+50
6 L Z+250 R0 F MAX
7 LP PR+60 PA+180 R0 F MAX
8 L Z-5 R0 F1000 M3
9 LP PR+45 PA+180 RL F250
10 RND R1
11 LP PA+120
12 LP PA+60
13 LP PA+0
14 LP PA-60
15 LP PA-120
16 LP PA+180
17 RND R1
18 LP PR+60 PA+180 R0 F1000
19 L Z+250 R0 F MAX M2
20 END PGM 40 MM

5

50

Define the blank form

Define the tool
Call the tool
Define the datum for polar coordinates
Retract the tool
Pre-position the tool
Move to working depth
Approach the contour at point 1
Tangential approach to circle with R=1 mm
Move to point 2
Move to point 3
Move to point 4
Move to point 5
Move to point 6
Move to point 1
Tangential departure from circle with R=1 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program

100

X

6.4 Path Contours – Polar Coordinates

73HEIDENHAIN TNC 310

Example: Helix

Y

100

6.4 Path Contours – Polar Coordinates

0 BEGIN PGM 50 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+5
4 TOOL CALL 1 Z S1400
5 L Z+250 R0 F MAX
6 L X+50 Y+50 R0 F MAX
7 CC
8 L Z-12.75 R0 F1000 M3
9 LP PR+32 PA-180 RL F100
10 RND R2
11 CP IPA+3240 IZ+13,5 DR+ F200
12 RND R2
13 L X+50 Y+50 R0 F MAX
14 L Z+250 R0 F MAX M2
15 END PGM 50 MM

50

Define the blank form

Define the tool
Call the tool
Retract the tool
Pre-position the tool
Transfer the last programmed position as the pole
Move to working depth
Approach contour
Tangential approach to circle with R=2 mm
Helical interpolation
Tangential departure from circle with R=2 mm
Retract tool in the working plane
Retract tool in the spindle axis, end of program

CC

50

100

M64 x 1,5

X

To cut a thread with more than 16 revolutions

...
8 L Z-12.75 R0 F1000
9 LP PR+32 PA-180 RL F100
10 LBL 1
11 CP IPA+360 IZ+1.5 DR+ F200
12 CALL LBL 1 REP 24

74

Identify beginning of program section repeat
Enter the thread pitch as an incremental IZ dimension
Program the number of repeats (thread revolutions)

6 Programming: Programming Contours

7

Programming:

Miscellaneous Functions

7.1 Entering Miscellaneous Functions
M and STOP

With the TNC’s miscellaneous functions — also called M functions
— you can affect:

■ Program run, such as a program interruption

■ Machine functions, such as switching spindle rotation and coolant

supply on and off

■ Contouring behavior of the tool

The machine tool builder may add some M functions
that are not described in this User’s Manual. Refer to
your machine manual for more information.

M functions are always entered at the end of a positioning block.
The TNC then displays the following dialog question:

MISCELLANEOUS FUNCTION M ?

Only enter the number of the M function in the programming
dialog.

In the MANUAL OPERATION operating mode, the M functions are
entered with the M soft key.

Please note that some F functions become effective at the start of
a positioning block, and other at the end.

M functions come into effect in the block in which they are called.
Unless the M function is only effective blockwise, it is canceled in a
subsequent block or at the end of program. Some M functions are
effective only in the block in which they are called.

7.1 Entering Miscellaneous Functions M and STOP

Entering an M function in a STOP block

If you program a STOP block, the program run or test run is
interrupted at the block, for example for tool inspection. You can
also enter an M function in a STOP block:

ú To program an interruption of program run,

press the STOP key.

ú Enter a MISCELLANEOUS FUNCTION M.

Resulting NC block

87 STOP M6

76

7 Programming: Miscellaneous Functions

7.2 Miscellaneous Functions for Pro­gram Run Control, Spindle and
Coolant

M Effect
M00 Stop program run

Spindle STOP
Coolant OFF

M01 Stop program run
M02 Stop program run

Spindle STOP
Coolant OFF
Go to block 1
Clear the status display (dependent
on machine parameter 7300)

M03 Spindle ON clockwise
M04 Spindle ON counterclockwise
M05 Spindle STOP
M06 Tool change

Spindle STOP
Program run stop (dependent on
machine parameter 7440)

M08 Coolant ON
M09 Coolant OFF
M13 Spindle ON clockwise

Coolant ON

M14 Spindle ON counterclockwise

Coolant ON

M30 Same as M02

Effective at

Block end

Block end
Block end

Block start
Block start
Block end
Block end

Block start
Block end
Block start

Block start

Block end

7.3 Miscellaneous Functions for
Coordinate Data

Programming machine-referenced coordinates:
M91/M92

Scale reference point

On the scale, a reference mark indicates the position of the scale
reference point.

Machine datum

The machine datum is required for the following tasks:

■ Defining the limits of traverse (software limit switches)

■ Moving to machine-referenced positions (such as tool change

positions)

■ Setting the workpiece datum

X

MP

X (Z,Y)

7.2 Miscellaneous Functions for Program Run Control, Spindle and Coolant

77HEIDENHAIN TNC 310

The distance in each axis from the scale reference point to the
machine datum is defined by the machine tool builder in a machine
parameter.

Standard behavior

The TNC references coordinates to the workpiece datum (see
“Datum setting”).

Behavior with M91 — Machine datum

If you want the coordinates in a positioning block to be referenced
to the machine datum, end the block with M91.

The coordinate values on the TNC screen are referenced to the
machine datum. Switch the display of coordinates in the status
display to REF (see section 1.4 “Status Displays”).

Behavior with M92 — Additional machine datum

In addition to the machine datum, the machine tool
builder can also define an additional machine-based
position as a reference point.

For each axis, the machine tool builder defines the
distance between the machine datum and this additional
machine datum. Refer to the machine manual for more
information.

If you want the coordinates in a positioning block to be based on
the additional machine datum, end the block with M92.

Radius compensation remains the same in blocks that
are programmed with M91 or M92. The tool length,
however, is not compensated.

7.3 Miscellaneous Functions for Coordinate Data

Effect

M91 and M92 are effective only in the blocks in which they are
programmed with M91 or M92.

M91 and M92 become effective at the start of block.

Workpiece datum

The figure at right shows coordinate systems with the machine
datum and workpiece datum.

Z

Z

Y

Y

X

X

M

78

7 Programming: Miscellaneous Functions

7.4 Miscellaneous Functions for
Contouring Behavior

Smoothing corners: M90

Standard behavior

The TNC stops the tool briefly in positioning blocks without tool
radius compensation. This is called an accurate stop.

In program blocks with radius compensation (RR/RL), the TNC
automatically inserts a transition arc at outside corners.

Behavior with M90

The tool moves at corners with constant speed: This provides a
smoother, more continuous surface. Machining time is also
reduced. See figure at center right.

Example application: Surface consisting of a series of straight line
segments.

Effect

M90 is effective only in the blocks in which it is programmed with
M90.

M90 becomes effective at the start of block. Operation with servo
lag must be active.

Independently of M90, you can use machine parameter
MP7460 to set a limit value up to which the tool moves at
constant path speed (effective with servo lag and
feedforward control).

Y

X

Y

X

7.4 Miscellaneous Functions for Contouring Behavior

79HEIDENHAIN TNC 310

Machining small contour steps: M97

Standard behavior

The TNC inserts a transition arc at outside corners. If the contour
steps are very small, however, the tool would damage the contour.
See figure at upper right.

In such cases the TNC interrupts program run and generates the
error message “TOOL RADIUS TOOL LARGE.”

Behavior with M97

The TNC calculates the intersection of the contour elements — as
at inside corners — and moves the tool over this point. See figure
at lower right.

Program M97 in the same block as the outside corner.

Effect

M97 is effective only in the blocks in which it is programmed with
M97.

A corner machined with M97 will not be completely
finished. You may wish to rework the contour with a
smaller tool.

Y

X

Y

7.4 Miscellaneous Functions for Contouring Behavior

Example NC blocks

5 TOOL DEF L ... R+20
...
13 L X ... Y ... R.. F .. M97

14 L IY0.5 .... R .. F..

15 L IX+100 ...
16 L IY+0.5 ... R .. F.. M97
17 L X .. Y ...

S

13

14

Large tool radius

Move to contour point 13
Machine small contour step 13 to 14
Move to contour point 15
Machine small contour step 15 to 16
Move to contour point 17

S

16

17

15

X

80

7 Programming: Miscellaneous Functions

Machining open contours: M98

Standard behavior

The TNC calculates the intersections of the cutter paths at inside
corners and moves the tool in the new direction at those points.

If the contour is open at the corners, however, this will result in
incomplete machining (see figure at upper right).

Behavior with M98

With the miscellaneous function M98, the TNC temporarily
suspends radius compensation to ensure that both corners are
completely machined (see figure at lower right).

Effect

M98 is effective only in the blocks in which it is programmed with
M98.

M98 becomes effective at the end of block.

Example NC blocks

Move to the contour points 10, 11 and 12 in succession:

10 L X ... Y... RL F
11 L X... IY... M98
12 L IX+ ...

Y

S

S

X

Y

10

11

12

X

7.4 Miscellaneous Functions for Contouring Behavior

81HEIDENHAIN TNC 310

7.5 Miscellaneous Function for Rotary
Axes

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

Standard behavior

The TNC moves the tool from the current angular value to the
programmed angular value.

Example:
Current angular value: 538°
Programmed angular value: 180°
Actual path of traverse: –358°

Behavior with M94

At the start of block, the TNC first reduces the current angular value
to a value less than 360° and then moves the tool to the
programmed value. If several rotary axes are active, M94 will
reduce the display of all rotary axes.

Example NC blocks

To reduce display of all active rotary axes:

L M94

To reduce display of all active rotary axes and then move the tool in
the C axis to the programmed value:

7.5 Miscellaneous Function for Rotary Axes

L C+180 FMAX M94

Effect

M94 is effective only in the block in which M94 is programmed.
M94 becomes effective at the start of block.

82

7 Programming: Miscellaneous Functions

Programming:

Cycles

8

8.1 General Overview of Cycles

Group of Cycles Soft Key

Frequently recurring machining cycles that comprise several
working steps are stored in the TNC memory as standard cycles.
Coordinate transformations and other special cycles are also
provided as standard cycles. The table at right shows the various
cycle groups.

Fixed cycles with number starting with 200 use Q parameters as
transfer parametersParameters with specific functions that are
required in several cycles always have the same number: For
example, Q200 is always assigned the setup clearance, Q202 the
plunging depth, etc.

Defining a cycle

ú The soft-key row shows the available groups of

cycles

ú Press the soft key for the desired group of cycles,

for example DRILLING for the drilling cycles

8.1 General information on Cycles

ú Select a cycle, e.g. DRILLING The TNC initiates the

programming dialog and asks all required input
values. At the same time a graphic of the input
parameters is displayed in the right screen
window. The parameter that is asked for in the
dialog prompt is highlighted. Select the screen
layout PROGRAM + HELP GRAPHIC.

ú Enter all parameters asked by the TNC and

conclude each entry with the ENT key

ú The TNC terminates the dialog when all required

data have been entered

Cycles for pecking, reaming, boring
and tapping

Cycles for milling pockets, studs
and slots

Coordinate transformation cycles
which enable datum shift, rotation,
mirror image, enlarging and reducing
for various contours

Cycles for producing hole patterns,
such as circular or linear patterns

Cycles for face milling of flat or
twisted surfaces

Special cycles such as dwell time,
program call and oriented spindle stop

Resulting NC blocks

14 CYCL DEF 200 DRILLING
Q200=2
Q201=-40
Q206=250
Q202=5
Q210=0
Q203=-10
Q204=20

84

8 Programming: Cycles

Calling the Cycle

Prerequisites

The following data must always be programmed before a
cycle call

■ BLK FORM for graphic display (needed only for

test graphics)

■ Call the tool

■ Direction of spindle rotation (M functions M3/M4)

■ Cycle definition (CYCL DEF).

For some cycles, additional prerequisites must be
observed. They are described with the individual cycle.

The following cycles become effective automatically as soon as
they are defined in the part program. These cycles cannot and must
not be called:

■ Cycles for circular and linear hole patterns

■ Coordinate transformation cycles

■ DWELL TIME cycle

All other cycles are called as described below.
If the TNC is to execute the cycle once after the last programmed

block, program the cycle call with the miscellaneous function M99
or with CYCL CALL:

ú Press the CYCL CALL soft key to program a cycle

call

ú Enter a miscellaneous function, for example for

coolant supply.

8.1 General information on Cycles

If the TNC is to execute the cycle automatically after every
positioning block, program the cycle call with M89 (depending on
machine parameter 7440).

To cancel M89, enter

■ M99 or

■ CYCL CALL or

■ CYCL DEF

85HEIDENHAIN TNC 310

8.2 Drilling Cycles

The TNC offers 7 cycles for all types of drilling operations:

Cycle Soft Key

1 PECKING
Without automatic pre-positioning

200 DRILLING

8.2 Drilling Cycles

With automatic pre-positioning and
2nd set-up clearance

201 REAMING
With automatic pre-positioning and
2nd set-up clearance

202 BORING
With automatic pre-positioning and
2nd set-up clearance

203 UNIVERSAL DRILLING
With automatic pre-positioning, 2nd set-up
clearance, chip breaking, and decrement

2 TAPPING
With a floating tap holder

17 RIGID TAPPING
Without a floating tap holder

86

8 Programming: Cycles

PECKING (Cycle 1)

1 The tool drills from the current position to the first PECKING

DEPTH at the programmed FEED RATE F.

2 When it reaches the first pecking depth, the tool retracts in rapid

traverse FMAX to the starting position and advances again to the
first PECKING DEPTH minus the advanced stop distance t.

3 The advanced stop distance is automatically calculated by the

control:

■ At a total hole depth of up to 30 mm: t = 0.6 mm

■ At a total hole depth exceeding 30 mm: t = hole depth / 50

Maximum advanced stop distance: 7 mm

4 The tool then advances with another infeed at the programmed

FEED RATE F.

5 The TNC repeats this process (1 to 4) until the programmed

TOTAL HOLE DEPTH is reached.

6 After a dwell time at the hole bottom, the tool is returned to the

starting position in rapid traverse FMAX for chip breaking.

Before you begin programming, note the following:

Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION R0.

Program a positioning block for the starting point in the tool
axis (SET-UP CLEARANCE above the workpiece surface).

The algebraic sign for the cycle parameter TOTAL HOLE
DEPTH determines the working direction.

Z

X

8.2 Drilling Cycles

ú SET-UP CLEARANCE (incremental value):

Distance between tool tip (at starting position) and
workpiece surface

ú TOTAL HOLE DEPTH (incremental value):

Distance between workpiece surface and bottom
of hole (tip of drill taper)

ú PECKING DEPTH (incremental value):

Infeed per cut. The tool will drill to the DEPTH in
one movement if:

■ the PECKING DEPTH equals the TOTAL HOLE

DEPTH

■ the PECKING DEPTH is greater than the MILLING

DEPTH
The TOTAL HOLE DEPTH does not have to be a

multiple of the PECKING DEPTH.

ú DWELL TIME IN SECONDS: Amount of time the

tool
remains at the total hole depth for chip breaking

ú FEED RATE F: Traversing speed of the tool during

drilling in mm/min

87HEIDENHAIN TNC 310

DRILLING (Cycle 200)

1 The TNC positions the tool in the tool axis at rapid traverse FMAX

to the SET-UP CLEARANCE above the workpiece surface.

2 The tool drills to the first PLUNGING DEPTH at the programmed

FEED RATE F.

3 The tool is retracted to SET-UP CLEARANCE in FMAX, remains

there — if programmed— for the entered dwell time, and
advances again in FMAX to 0.2 mm above the first PLUNGING
DEPTH.

8.2 Drilling Cycles

4 The tool then drills deeper by the PLUNGING DEPTH at the

programmed FEED RATE F.

5 The TNC repeats this process (2 to 4) until the programmed TOTAL

HOLE DEPTH is reached.

6 At the hole bottom, the tool is retraced to SET-UP CLEARANCE or

— if programmed — to the 2ND SET-UP CLEARANCE in rapid
traverse FMAX.

Before you begin programming, note the following:

Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION R0.

The algebraic sign for the DEPTH parameter determines
the working direction.

Q203

Z

Q210

Q206

Q200

Q202

Q204

Q201

X

ú SET-UP CLEARANCE Q200 (incremental value):

Distance between tool tip and workpiece surface.

ú DEPTH Q201 (incremental value): Distance

between workpiece surface and bottom of hole (tip
of drill taper)

ú FEED RATE FOR PLUNGING Q206: Traversing

speed of the tool during drilling in mm/min

ú PLUNGING DEPTH Q202 (incremental value):

Infeed per cut. The tool will drill to the DEPTH in
one movement if:

■ the PLUNGING DEPTH is equal to the DEPTH

■ the PLUNGING DEPTH is greater than the

DEPTH
The DEPTH does not have to be a multiple of the

PLUNGING DEPTH.

ú DWELL TIME AT TOP Q210: Time in seconds that

the tool remains at SET-UP CLEARANCE after
having been retracted from the hole for chip
release.

88

8 Programming: Cycles

ú WORKPIECE SURFACE COORDINATE Q203 (absolu-

te): coordinate of workpiece surface

ú 2ND SET-UP CLEARANCE Q204 (incremental

value): Coordinate in the tool axis at which no
collision between tool and workpiece (clamping
devices) can occur.

REAMING (Cycle 201)

1 The TNC positions the tool in the tool axis at rapid traverse FMAX

to the programmed SET-UP CLEARANCE above the workpiece
surface.

2 The tool reams to the entered DEPTH at the programmed FEED

RATE F.

3 If programmed, the tool remains at the hole bottom for the

entered dwell time.

4 The tool then retracts to SET-UP CLEARANCE at the FEED RATE F,

and from there — if programmed — to the 2ND SET-UP
CLEARANCE in FMAX.

Before you begin programming, note the following:

Program a positioning block for the starting point (hole
center) in the working plane with RADIUS
COMPENSATION R0.

The algebraic sign for the DEPTH parameter determines
the working direction.

Q203

Z

Q206

8.2 Drilling Cycles

Q200

Q201

Q208

Q211

Q204

X

ú SET-UP CLEARANCE Q200 (incremental value):

Distance between tool tip and workpiece surface.

ú DEPTH Q201 (incremental value): Distance

between workpiece surface and bottom of hole

ú FEED RATE FOR PLUNGING Q206:

Traversingspeed of the tool during reaming in mm/
min

ú DWELL TIME AT DEPTH Q211: Time in seconds

that the tool remains at the hole bottom

ú RETRACTION FEED RATE Q208: Traversing speed

of the tool in mm/min when retracting from the
hole. If you enter Q208 = 0, the tool retracts at the
REAMING FEED RATE.

ú WORKPIECE SURFACE COORDINATE Q203 (absolu-

te): coordinate of workpiece surface

ú 2ND SET-UP CLEARANCE Q204 (incremental

value): Coordinate in the tool axis at which no
collision between tool and workpiece (clamping
devices) can occur.

89HEIDENHAIN TNC 310