heidenhain TNC 124 User Manual

July 2004

User's Manual

TNC Guideline:

From workpiece drawing to
program-controlled machining

Step Task TNC operating Starting

mode on page

Preparation

1 Select tools  

2 Set workpiece datum for

coordinate system  

3 Determine spindle speeds

and feed rates as desired 107, 116

4 Switch on TNC and machine  17

5 Cross over reference marks 17

6 Clamp workpiece  

7 Set datum /

Reset position display ...

7a ... with the probing functions 33

7b ... without the probing functions 31

Entering and testing part programs

8 Enter part program or

download over external
data interface 59

9 Test run: Run part program

block by block without tool 103

10 If necessary: Optimize

part program 59

Machining the workpiece

12 Insert tool and

run part program 105

Screen

MOD

INFO HELP

7

8 9

4 5 6

1 2 3

–

0

ENT

CE

+

´

Y

–

Z

´

´

–

+

X

X

–

´

Y

+

Z

100

150

50

F %

GOTO

NC

I

I

NC

0

0

HEIDENHAIN

Operating

mode or

function

Plain language
dialog line

Operating mode sym­bols (current mode is
highlighted)

Soft-key row
(with 5 soft
keys)

Input line

Tool number
and tool axis

Spindle brake

Screen in the operating modes

PROGRAMMING AND
EDITING and
PROGRAM RUN

Current

block

Spindle speed

Feed rate

Soft keys

Selected
datum

Miscellaneous

function M

Current

positions

Status line

Controlling machine functions

MOD

INFO HELP

7

8 9

4 5 6

1 2 3

–

0

ENT

CE

+

´

Y

–

Z

´

´

–

+

X

X

–

´

Y

+

Z

100

150

50

F %

GOTO

NC

I

I

NC

0

0

HEIDENHAIN

Power supply

Counterclockwise

spindle rotation

EMERGENCY STOP

Spindle brake

Clockwise
spindle rotation

50

100

Symbol for
soft-key row

+

´

Y

–

Z

´

+

X

–

Y

Z

´

–

X

´

+

150

F %

Machine axis
direction keys;
Rapid traverse
key

Feed rate
override

Coolant

Release tool

Selecting functions and programming

MOD

INFO HELP

7

8 9

4 5 6

1 2 3

–

0

ENT

CE

+

´

Y

–

Z

´

´

–

+

X

X

–

´

Y

+

Z

100

150

50

F %

GOTO

NC

I

I

NC

0

0

HEIDENHAIN

5 soft keys

(functions vary

according to

associated fields

on screen)

Change parameters
and settings

MOD

INFO HELP

7 8 9

4 5 6

1 2 3

Select or deselect
INFO functions

Select or deselect
HELP screens

Numeric input keys

0

Clear entries or

error messages

Page through indi-

vidual soft-key rows

Access program blocks to

make changes, or switch

operating parameters

Selecting operating modes; Start or stop NC and spindle

MOD

INFO HELP

7

8 9

4 5 6

1 2 3

–

0

ENT

CE

+

´

Y

–

Z

´

´

–

+

X

X

–

´

Y

+

Z

100

150

50

F %

GOTO

NC

I

I

NC

0

0

HEIDENHAIN

OPERATION

POSITIONING WITH

MANUAL

CE

MDI

–

ENT

GOTO

PROGRAM RUN

Change sign

Confirm entry

Incremental
dimensions

Return to previous
soft-key level

Go to program block
or operating param­eter

Select programs
and program blocks

PROGRAMMING AND
EDITING

Spindle ON

Spindle OFF

I

I

NC

NC

0

0

Start NC

I key)

(NC-

Stop NC

Contents

Software Version................................................................................................. 7

TNC 124.............................................................................................................. 7

About This Manual .............................................................................................. 8

Special Notes in this Manual .............................................................................. 9

TNC Accessories .............................................................................................. 10

1 Fundamentals of Positioning ................................................... 11

Coordinate system and coordinate axes ........................................................... 11

Datums and positions ....................................................................................... 12

Machine axis movements and position feedback ............................................... 14

Angular positions .............................................................................................. 15

2 Working with the TNC 124  First Steps ..................................17

Before you start ................................................................................................ 17

Switch-on .......................................................................................................... 17

Operating modes .............................................................................................. 18

HELP, MOD and INFO functions ....................................................................... 18

Selecting soft-key functions .............................................................................. 19

Symbols on the TNC screen ............................................................................. 19

On-screen operating instructions ....................................................................... 20

Error messages ................................................................................................ 21

Selecting the unit of measurement .................................................................... 21

Selecting position display types........................................................................ 22

Traverse limits ................................................................................................... 22

3 Manual Operation and Setup .................................................... 23

Feed rate F, spindle speed S and miscellaneous function M ............................. 23

Moving the machine axes .................................................................................. 25

Entering tool length and radius .......................................................................... 28

Calling the tool data .......................................................................................... 29

Selecting datum points ..................................................................................... 30

Datum setting: Approaching positions and entering actual values...................... 31

Functions for datum setting ............................................................................... 33

Measuring diameters and distances .................................................................. 33

4 Positioning with Manual Data Input (MDI) ................................ 38

Before you machine the workpiece .................................................................... 38

Taking the tool radius into account .................................................................... 38

Feed rate F, spindle speed S and miscellaneous function M ............................. 39

Entering and moving to positions ....................................................................... 41

Pecking and tapping ......................................................................................... 43

Hole patterns .................................................................................................... 48

Bolt hole circle patterns .................................................................................... 49

Linear hole patterns .......................................................................................... 53

Rectangular pocket milling ................................................................................ 57

5 Programming ............................................................................. 59

Operating mode PROGRAMMING AND EDITING ............................................. 59

Entering a program number ............................................................................... 60

Deleting programs ............................................................................................. 60

Editing programs ............................................................................................... 61

Contents

Editing program blocks ..................................................................................... 62

Editing existing programs .................................................................................. 63

Deleting program blocks ................................................................................... 64

Feed rate F, spindle speed S and miscellaneous function M ............................ 65

Entering program interruptions .......................................................................... 67

Calling the tool data in a program ...................................................................... 68

Calling datum points ......................................................................................... 69

Entering dwell time ........................................................................................... 70

6 Programming Workpiece Positions .........................................71

Entering workpiece positions ............................................................................ 71

Transferring positions: Teach-In mode ............................................................... 73

7 Drilling, Milling Cycles and Hole Patterns in Programs ..........77

Entering a cycle call ......................................................................................... 78

Drilling cycles in programs ................................................................................ 78

Hole patterns in programs ................................................................................. 85

Rectangular pockets in programs ...................................................................... 91

8 Subprograms and Program Section Repeats ......................... 94

Subprograms .................................................................................................... 95

Program section repeats ................................................................................... 97

9 Transferring Files Over the Data Interface ............................. 100

Transferring a program into the TNC ................................................................ 100

Reading a program out of the TNC .................................................................. 101

Transferring tool tables and datum tables ........................................................ 102

10 Executing programs ................................................................ 103

Single block .................................................................................................... 104

Full sequence ................................................................................................. 105

Interrupting program run .................................................................................. 105

11 Positioning Non-Controlled Axes........................................... 106

12 Cutting Data Calculator, Stopwatch and

Pocket Calculator: The INFO Functions ................................107

Cutting data: Calculate spindle speed S and feed rate F ................................. 108

Stopwatch ....................................................................................................... 109

Pocket calculator functions ............................................................................. 109

13 User Parameters: The MOD Function ....................................111

Entering user parameters ................................................................................ 111

TNC 124 user parameters ............................................................................... 112

14 Tables, Overviews and Diagrams........................................... 113

Miscellaneous functions (M functions) ............................................................. 113

Pin layout and connecting cable for the data interface ..................................... 115

Diagram for machining .................................................................................... 116

Technical information ...................................................................................... 117

Accessories .................................................................................................... 118

Subject Index ........................................................................... 119

Software Version

This User's Manual is for TNC 124 models with the following software
version:

The x's can be any numbers.

For detailed technical information refer to the Technical
Manual for the TNC 124.

NC and PLC software numbers

The NC and PLC software numbers of your unit are displayed on the
TNC screen after switch-on.

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.

TNC 124

Progr. 246 xxx-16.

TNC family

What is NC? NC stands for Numerical Control, that is, control of a
machine tool by means of numbers. Modern controls such as the
TNC have a built-in computer for this purpose and are therefore called
CNC (Computerized Numerical Control).

From the very beginning, the TNCs from HEIDENHAIN were devel­oped specifically for shop-floor programming by the machinist. This
is why they are called TNC, or Touch Numerical Controls.

The TNC 124 is a straight cut control for boring machines and milling
machines with up to three axes. It also features position display of a
fourth axis.

Conversational programming

Workpiece machining is defined in a part program. It contains a
complete list of instructions for machining a part, for example, the
target position coordinates, the feed rate and the spindle speed.

You begin programming each machining step by simply pressing a
key or soft key. The TNC then asks for all the information that it
needs to execute the step.

TNC 124 7

About This Manual

If you're new to TNC, you can use the operating instructions as a
step-by-step workbook. This part begins with a short introduction to
the basics of coordinate systems and position feedback, and pro­vides an overview of the available features. Each feature is explained
in detail, using an example  so you won't get lost too deeply in
the theory. As a beginner you should work through all the examples
presented.

The examples are intentionally brief; it generally won't take you
longer than 10 minutes to enter the example data.

If you're already proficient with TNC, you can use the operating
instructions as a comprehensive review and reference guide. The
clear layout and the subject index make it easy to find the desired
topics.

Dialog flowcharts

Dialog flowcharts are used for each example in this manual.
They are laid out as follows:

The operating mode is indicated above the first dialog flowchart.

This area shows the
keys to press.

This area shows the key function or work step.
If necessary, supplementary information will also be included.

Prompt

This area shows the
keys to press.

A prompt appears with some actions (not always) at the top of the
screen.

If two flowcharts are divided by a broken line, and words by or,
this means that you can follow either of the instructions.

Some flowcharts also show the screen that will appear after you
press the correct keys.

Abbreviated flowcharts

Abbreviated flowcharts supplement the examples and explanations.
An arrow ( ä ) indicates a new input or a work step.

This area shows the key function or work step.
If necessary, supplementary information will also be included.

If there is an arrow at the end of the flowchart, this means that it
continues on the next page.

8 TNC 124

Special Notes in this Manual

Particularly important information is presented separately in shaded
boxes. Be sure to carefully pay attention to these notes. If you ig­nore these notes your TNC may not function as required, or damage
the workpiece or tool.

Symbols used in the notes

Each note is identified by a symbol to the left. Your manual uses
three different symbols which have the following meanings:

General note,

e.g., indicating the behavior of the control.

Note with reference to the machine manufacturer,
e.g., indicating that a specific function must be enabled
for your machine tool.

Important note,

e.g., indicating that a special tool is required for the
function.

TNC 124 9

TNC Accessories

Electronic handwheel

Electronic handwheels facilitate precise manual control of the axis
slides. Like a conventional machine tool, the machine slide moves in
direct relation to the rotation of the handwheel. A wide range of
traverses per handwheel revolution is available.

The HR 410 Electronic Handwheel

10 TNC 124

1 Fundamentals of Positioning

1

Fundamentals of Positioning

Coordinate system and coordinate axes

Reference system

In order to define positions on a surface, a reference system is
required. For example, positions on the earth's surface can be
defined absolutely by their geographic coordinates of longitude and
latitude. The term coordinate comes from the Latin word for that
which is arranged. In contrast to the relative definition of a position
that is referenced to a known location, the network of horizontal and
vertical lines on the globe constitutes an absolute reference system.

The Greenwich observatory illustrated in Fig. 1.1 is located at 0° lon­gitude, and the equator at 0° latitude.

0° 90°90°

Greenwich

60°

30°

0°

30°

60°

Cartesian coordinate system

On a TNC-controlled milling or drilling machine tool, workpieces are
normally machined according to a workpiece-based Cartesian coordi­nate system (a rectangular coordinate system named after the
French mathematician and philosopher Renatus Cartesius, who lived
from 1596 to 1650). The Cartesian coordinate system is based on
three coordinate axes designated X, Y and Z which are parallel to the
machine guideways.

The figure to the 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.

Axis designations

X, Y and Z are the main axes of the Cartesian coordinate system.
The additional axes U, V and W are secondary linear axes parallel to
the main axes. Rotary axes are designated as A, B and C (see Fig.

1.3).

Fig. 1.1: The geographic coordinate system

Fig. 1.2: Designations and directions of the

is an absolute reference system

+Y

+Y

axes on a milling machine

+Z

+X

+Z

+X

Z

Y

W+

C+

B+

V+

A+

X

U+

Fig. 1.3: Main, additional and rotary axes in

TNC 124 11

the Cartesian coordinate system

1 Fundamentals of Positioning

Y

X

Z

Datums and positions

Setting the datum

The workpiece drawing identifies a certain point on the workpiece
(usually a corner) as the absolute datum and perhaps one or more
other points as relative datums. The datum setting procedure estab­lishes these points as the origin of the absolute or relative coordinate
systems: The workpiece, which is aligned with the machine axes, is
moved to a certain position relative to the tool and the display is set
either to zero or to another appropriate value (e.g., to compensate
the tool radius).

Example: Coordinates of hole1:

X = 10 mm
Y = 5 mm
Z = 0 mm (hole depth: Z =  5 mm)

The datum of the Cartesian coordinate system

1

is located 10 mm from hole

on the X axis and

5 mm from it in the Y axis (in negative direction).

The TNC's probing functions facilitate finding and setting datums.

Fig. 1.4: The workpiece datum represents

the origin of the Cartesian coordi­nate system

Z

Y

X

1

5

10

1

Fig. 1.5: Hole

defines the coordinate

system

12 TNC 124

1 Fundamentals of Positioning

Y

X

Z

1

20

10

Z=15mm

X=20mm

Y=10mm

15

I

Z=–15mm

Y

X

Z

2

10

5

5

15

20

10

10

I

X=10mm

I

Y=10mm

3

0

0

Datums and Positions

Absolute workpiece positions

Each position on the workpiece is uniquely identified by its absolute
coordinates.

Example: Absolute coordinates of the position

X=20mm
Y=10mm
Z=15mm

If you are drilling or milling a workpiece according to a workpiece
drawing with absolute coordinates, you are moving the tool to the
value of the coordinates.

1

:

Incremental workpiece positions

A position can also be referenced to the preceding nominal posi­tion. In this case the relative datum is always the last pro­grammed position. Such coordinates are referred to as incre-
mental coordinates (increment = increase). They are also
called incremental or chain dimensions (since the positions are
defined as a chain of dimensions). Incremental coordinates are
designated with the prefix

Example: Incremental coordinates of position

position

2

Absolute coordinates of position2:
X=10mm

Y= 5mm
Z=20mm

Incremental coordinates of position

IX= 10mm
IY= 10mm
IZ=15mm

If you are drilling or milling a workpiece according to a drawing with
incremental coordinates, you are moving the tool by the value of the
coordinates.

I.

3

referenced to

3

:

Fig. 1.6: Position definition through absolute

coordinates

Fig. 1.7: Position definition through incremental

coordinates

TNC 124 13

1 Fundamentals of Positioning

Y

X

Z

Machine axis movements and position feedback

Programming tool movements

During workpiece machining, an axis position is changed either by
moving the tool or by moving the machine table on which the
workpiece is fixed.

When entering tool movements in a part program you
always program as if the tool is moving and the work­piece is stationary.

+Y

+Z

+X

Position feedback

The position feedback encoders  linear encoders for linear axes,
angle encoders for rotary axes  convert the movement of the ma­chine axes into electrical signals. The control evaluates these sig­nals and constantly calculates the actual position of the machine
axes.

If there is an interruption in power, the calculated position will no
longer correspond to the actual position. When power is restored,
the TNC can re-establish this relationship.

Reference marks

The scales of the position encoders contain one or more reference
marks. When a reference mark is passed over, it generates a signal
which identifies that position as the reference point (scale reference
point = machine reference point). With the aid of this reference mark
the TNC can re-establish the assignment of displayed values to ma­chine axis positions.

If the position encoders feature distance-coded reference marks,
each axis need only move a maximum of 20 mm (0.8 in.) for linear
encoders, and 20° for angle encoders.

Fig. 1.8: On this machine the tool moves in

the Y and Z axes; the workpiece
moves in the X axis.

Fig. 1.9: Linear position encoder, here for

the X axis

Fig. 1.10: Linear scales: above with distance-

coded reference marks, below with
one reference mark

14 TNC 124

1 Fundamentals of Positioning

Angular positions

For angular positions, the following reference axes are defined:

Plane Angle reference axis

X / Y + X

Y / Z + Y

Z / X + Z

Y

–270°

+45°

+180°

Algebraic sign for direction of rotation

Positive direction of rotation is counterclockwise if the working plane
is viewed in negative tool axis direction (see Fig. 1.11).

Example: Angle in the working plane X / Y

Angle Corresponds to the ...

+ 45° ... bisecting line between +X and +Y

± 180° ... negative X axis

 270° ... positive Y axis

–180°

Fig. 1.11: Angle and the angle reference

axis, here in the X / Y plane

X

TNC 124 15

1 Fundamentals of Positioning

NOTES

16 TNC 124

2 Working with the TNC 124  First Steps

2
Working with the TNC 124  First Steps

Before you start

You must cross over the reference marks after every switch-on.
From the positions of the reference marks, the TNC automatically re­establishes the relationship between axis slide positions and
display values that you last defined by setting the datum.

Setting up a new datum point automatically stores the new relation­ship between axis positions and display values.

Switch-on

0 ä 1

MEMORY TEST

Please wait...

POWER INTERRUPTED

CE

RELAY EXT. DC VOLTAGE MISSING

CROSS OVER REFERENCE MARKS

For each axis:

or

Press and hold suc­cessively:

NC

´

+

X

+

Y

´

+

Z

Switch on the TNC and the machine tool.

The internal memory of the TNC is checked automatically.

Clear the TNC message indicating that the power was interrupted.

Switch on the control voltage.
The TNC automatically checks the function of the EMERGENCY STOP button.

Move the axes in the displayed sequence across the reference marks

Move the axes in the displayed sequence across the reference marks.

or

Cross the reference marks in any sequence:
Press the machine axis direction button until the moving
axis disappears from the screen.
Sequence in this example: X AXIS, Y AXIS, Z AXIS

The TNC 124 is now ready for operation in the
MANUAL OPERATION mode.

TNC 124 17

2 Working with the TNC 124  First Steps

Operating modes

Selecting the operating mode determines which functions are avail­able to you.

Available functions Mode Key

Move the machine axes MANUAL
 with the direction keys, OPERATION
 with the electronic hand-

wheel,
 by incremental jog positioning;
Datum setting 
also with probing functions
(e.g. circle center as datum);
Enter and change spindle speed
and miscellaneous functions

Enter positioning blocks and POSITIONING
execute them block by block; WITH
Enter hole patterns and MDI
execute them block by block;
Change spindle speed, feed
rate, miscellaneous functions;
Enter tool data;

Store work steps for small-lot PROGRAMMING
production by AND EDITING
 Keyboard entry
 Teach-in;
Transferring programs
through the data interface

Executing programs PROGRAM
 continuously RUN
 blockwise

You can switch to another operating mode at any time by pressing
the key for the desired mode.

HELP, MOD and INFO functions

You can call the HELP, MOD and INFO functions at any time.

To call a function:

ä

Press the function key for that function.

To leave a function:

ä

Press the same function key again.

Functions Designation Key

On-screen operating HELP
instructions:
graphics and text explaining
the current screen contents

User parameters: MOD
To redefine the TNC's basic
operating characteristics

Cutting data calculator, INFO
stopwatch, pocket calculator

HELP

MOD

INFO

18 TNC 124

2 Working with the TNC 124  First Steps

Selecting soft-key functions

The soft-key functions are grouped into one or more rows. The TNC
indicates the number of rows by a symbol at the bottom right of the
screen.

If no symbol is visible, that means that all pertinent functions are al­ready shown. The highlighted rectangle in the symbol indicates the
current row.

Overview of functions

Function Key

Page through the soft-key rows: forwards

Page through the soft-key rows: backwards

Go back one soft-key level

The TNC displays the soft keys with the main functions
of an operating mode whenever you press the key for
that mode.

Symbols on the TNC screen

The TNC continuously informs you of the current operating status.
The symbols are displayed on the screen

 next to the designations of the coordinate axes or
 in the status line at the bottom of the screen.

Symbol Function/Meaning

T ... Tool, for example T 1

*)

S ...

*)

F ...

M ... Miscellaneous function, e.g. M 3

...

ACTL. TNC displays actual values

NOML. TNC displays nominal values

REF TNC displays the reference position

LAG TNC displays the servo lag

*

®

®

®

Spindle speed, e.g. S 1000 [rpm]

Feed rate, e.g. F 200 [mm/min]

Datum, e.g.: 1

Control active

®

Spindle brake active

Spindle brake inactive

Axis can be moved with the
electronic handwheel

Fig. 2.1: The symbol for soft-key rows at

the bottom right of the screen.
Here, the first row is being dis­played.

)

*

A highlighted F or S symbol means that the feed rate or
spindle has not been enabled by the PLC.

TNC 124 19

2 Working with the TNC 124  First Steps

On-screen operating instructions

The integrated operating instructions provide information and assist­ance in any situation.

To call the operating instructions:

➤ Press the HELP key.
➤ Use the paging keys if the explanation extends over more than

one screen page.

To leave the operating instructions:
➤ Press the HELP key again.

Example: On-screen operating instructions for datum setting

(PROBE CENTERLINE)

The PROBE CENTERLINE function is described in this manual on
page 34.

➤ Select the MANUAL OPERATION mode.
➤ Press the paging key to display the second screen page.
➤ Press the HELP key.

The first page of the operating instructions for the probing
functions appears.

Page reference at the lower right of the screen:
the number in front of the slash is the current page, the number

behind the slash is the total number of pages.
The on-screen operating instructions now contain the following

information on PROBING FUNCTIONS (on three pages):
 Overview of the probing functions (page 1)
 Graphic illustration of all probing functions

(pages 2 and 3)

➤ To leave the operating instructions:

Press HELP again.
The screen returns to the menu for the probing functions.

➤ Press (for example) the soft key Centerline.
➤ Press HELP.

The screen now displays operating instructions  spread over
three pages  on the function PROBE CENTERLINE including:

 Overview of all work steps (page 1)
 Graphic illustration of the probing sequence (page 2)
 Information on how the TNC reacts and on datum setting

(page 3)

➤ To leave the on-screen operating instructions:

Press HELP again.

Fig. 2.2: On-screen operating instructions

for PROBE, page 1

Fig. 2.3: On-screen operating instructions

for PROBE CENTERLINE,
page 1

Fig. 2.4: On-screen operating instructions

for PROBE CENTERLINE,
page 2

20 TNC 124

2 Working with the TNC 124  First Steps

Error messages

If an error occurs while you are working with the TNC, a message will
come up on the screen.

To call an explanation of the error:
➤ Press the HELP key.

To clear the error message:

➤ Press the CE key.

Blinking error messages

W A R N I N G !

Blinking error messages mean that the operational
reliability of the TNC has been impaired.

If a blinking error message occurs:

➤ Note down the error message displayed on the screen.
➤ Switch off the TNC and machine tool.
➤ Attempt to correct the problem with the power off.
➤ If the error cannot be corrected or if the blinking error message

recurs, notify your customer service agency.

Selecting the unit of measurement

Positions can be displayed in millimeters or inches. If you choose
inches, inch will be displayed at the top of the screen.

To change the unit of measurement:

➤ Press MOD.
➤ Page to the soft-key row containing the user parameter

mm or inch.

➤ Choose the soft key mm or inch to change to the other unit.
➤ Press MOD again.

For more information on user parameters, see Chapter 13.

Fig. 2.5: The inch indicator

TNC 124 21

2 Working with the TNC 124  First Steps

Selecting position display types

The TNC can display various position values for a specific tool
position.

The positions indicated in Fig. 2.6 are:
 Starting position of the tool

 Target position of the tool
 Workpiece datum
 Scale reference point

The TNC position display can be set to show the following types of
information:

 Nominal position NOML.

The value presently commanded by the TNC.

 Actual position ACTL.

The position at which the tool is presently located as referenced
to the workpiece datum.

 Servo lag LAG

3

The difference between nominal and actual positions
(NOML. – ACTL.)

 Actual position as referenced to the scale reference point REF

To change the position display

➤ Press MOD.
➤ Page to the soft-key row containing the user parameter

Posit.

➤ Press the soft key for selecting the position display type and

change to the other display type.

➤ Select the desired display type.
➤ Press MOD again.

For more information on user parameters, see Chapter 13.

1

2

3

A

Z

W

M

1

M

2

Fig. 2.6: Tool and workpiece positions

4

A

W

4

Z

Traverse limits

The maximum range of traverse of the machine axes is set by the
machine manufacturer.

Z

Z

max

Z

min

X

min

Fig. 2.7: Traverse limits define the machine's

actual working envelope

X

max

X

Y

max

Y

min

Y

22 TNC 124

3 Manual Operation and Setup

3
Manual Operation and Setup

The machine manufacturer may define a method of
moving the axes that varies from what is described in
this manual.

On the TNC 124 you can move the machine axes with:
 the direction keys,
 the electronic handwheel,
 incremental jog positioning, or
 positioning with manual data input MDI (see Chapter 4).

In the MANUAL OPERATION and POSITIONING WITH MDI
modes of operation (see Chapter 4) you can also enter and change:

 Feed rate F (the feed rate can only be entered in

POSITIONING WITH MDI)
 Spindle speed S
 Miscellaneous function M

Feed rate F, spindle speed S and miscellaneous function M

To change the feed rate F:

You can vary the feed rate F infinitely by turning the knob for feed
rate override on the TNC control panel.

Feed rate override

You can vary the feed rate F from
0% to 150% of the set value

100

15050

F %

0

+

´

Y

–

Z

´

+

Z

F%

´

–

X

´

+

X

–

Y

100

50

Fig. 3.1: Feed rate override on the TNC con-

trol panel

150

TNC 124 23

3 Manual Operation and Setup

Feed Rate F, Spindle Speed S and Miscellaneous Function M

Entering and changing the spindle speed S

The machine manufacturer determines which spindle
speeds are allowed on your TNC.

Example: Entering the spindle speed S

Select S for the spindle speed function.

Spindle speed ?

9

5 0

NC

To change the spindle speed S:

You can vary the spindle speed S infinitely by turning the knob for
spindle speed override  if provided  on the TNC control panel.

Spindle speed override

You can vary the spindle speed S from
0% to 150% of the set value

Entering a miscellaneous function M

The machine manufacturer determines which miscel­laneous functions are available on your TNC and which
effects they have.

Enter the spindle speed, for example 950 rpm.

Change the spindle speed.

100

15050

S %

0

Example: Entering a miscellaneous function

Select M for miscellaneous function.

Miscell a n e o u s function M ?

3

NC

24 TNC 124

Enter the miscellaneous function, for example M 3: spindle ON, clockwise.

Execute the miscellaneous function.

3 Manual Operation and Setup

Moving the machine axes

The TNC control panel includes six direction keys. The keys for the X
and Y axes are identified with a prime mark (X', Y'). This means that
the traversing directions indicated on these keys correspond to
movement of the machine table.

Traversing with the direction keys

The direction key defines at the same time
 the coordinate axis, for example X
 the traversing direction, for example negative: X

X

´

+

Z

´

–

Y

X

+

´

–

On machine tools with central drives you can only move one axis
at a time.

If you are moving a machine axis with the direction key, the TNC au­tomatically stops moving the axis as soon as you release the key.

For continuous movement:

You can also move the machine axes continuously:
The axis continues to move after you release the key.
To stop the axis press the key indicated below in example 2.

Rapid traverse

To move an axis at rapid traverse:
➤ Press the rapid traverse key and the direction key together.

Example: Moving the machine axis in the Z+ direction with the

direction key (retract tool):

Example 1: Moving the machine axes

Operating mode: MANUAL OPERATION

–

Y

Fig. 3.2: The direction keys on the TNC con-

trol panel, with the key for rapid
traverse in the center

Z

Y

Z

´

+

X

Press and hold:

Example 2: For continuous movement of the machine axes

Operating mode: MANUAL OPERATION

Together:

NC

0

TNC 124 25

´

+

Z

NC

´

+

Z

Press the direction key, here for the positive Z direction (Z'+) and hold it
as long as you wish the axis to move.

Start movement of the axis: Press the direction key, here for the positive
Z direction (Z'+) together with the NC-

Stop the axis.

I k ey .

3 Manual Operation and Setup

Moving the Machine Axes

Traversing with the electronic handwheel

Electronic handwheels can be connected only to ma­chines with preloaded drives. The machine manufacturer
can tell you whether electronic handwheels can be
connected on your machine.

You can connect the following HEIDENHAIN electronic handwheels
to your TNC 124:

 HR 410 portable handwheel
 HR 130 integral handwheel

Direction of traverse

The machine manufacturer determines in which direction the
handwheel must be turned to move an axis in a specific direction.

If you are working with the HR 410 portable handwheel

The HR 410 portable handwheel is equipped with two permissive but-

➂. You can move the machine axes with the handwheel ➁ only

tons
if a permissive button is depressed.

1

2

3

4

X

IV

V

Y

Z

–

+

FCT

FCT

FCT

B

A

C

5

6

7

8

Other features of the HR 410:

 Axis selection keys X, Y and Z

➃ .

 The axes can be moved continuously with the + and  direction

➆ .

keys
 Three keys for slow, medium and fast traverse
 Actual-position-capture key

➄ for transferring positions or tool

➅ .

data in teach-in mode directly from the position display into the

program or tool table (without having to type the numbers).
 Three keys for machine functions

➇ defined by the machine

tool builder.
 EMERGENCY STOP button

➀ for immediate machine shut-

down in case of danger. This safety feature is additional to the

permissive buttons.
 Magnetic holding pads on the back of the handwheel enable you

to place it within easy reach on a flat metal surface.

Example: Moving a machine axis with the HR 410 electronic handwheel,

for example the Y axis

Operating mode: MANUAL MODE

Select the Electronic handwheel function.
The handwheel symbol is displayed next to the X for the X coordinate.

Fig. 3.3: The HR 410 portable electronic

handwheel

Y

The handwheel symbol is shifted to the selected coordinate axis.

Select the traverse per revolution: large, medium, or small,
as preset by the machine tool builder.

Press the permissive button! Turn the handwheel to move the machine axis.

26 TNC 124

Select the coordinate axis at the handwheel.

3 Manual Operation and Setup

Moving the Machine Axes

Incremental jog positioning

Incremental jog positioning enables you to move a machine axis by
the increment you have preset each time you press the correspond­ing direction key.

Current jog increment

If you enter a jog increment, the TNC stores the entered value and
displays it right of the highlighted input line for Infeed.

The programmed jog increment is effective until a new value is en­tered by keyboard or soft key.

Maximum input value

0.001 mm £ jog increment £ 99.999 mm

Changing the feed rate F

You can increase or decrease the feed rate F by turning the knob for
feed rate override.

Example: Moving the machine axis in the X+ direction by incremental

jog positioning

Fig. 3.4: TNC screen for incremental jog

positioning

Z

Operating mode: MANUAL OPERATION

Select the Jog Increm. function.

Infeed :
0 . 0 0 0

Enter the infeed (5 mm)  by soft key.

or

ENT

5

or

Enter the infeed (5 mm)  with the keyboard and confirm your entry with ENT.

Infeed :
0 . 0 0 0 5 . 0 0 0

´

+

X

Move the machine axis by the entered infeed, for example in the
X+ direction.

5 5

510

X

TNC 124 27

3 Manual Operation and Setup

Entering tool length and radius

Enter the lengths and radii of your tools in the TNC's tool table. The
TNC will then take the entered data into account for datum setting
and all other machining processes.

You can enter up to 99 tools.

The tool length is the difference in length DL between the tool and
the zero tool.

To enter the tool length directly move the tool until it touches the
workpiece and transfer the tool position coordinate by using the ac­tual position capture function.

Sign for the length difference DL

If the tool is longer than the zero tool: DL > 0
If the tool is shorter than the zero tool: DL < 0

Example: Entering the tool length and radius

into the tool table

Tool number: e.g. 7

Tool length: L = 12 mm

Tool radius: R = 8 mm

Z

T

1

R

1

∆L

=0

1

Fig. 3.5: Tool length and radius

Z

T

2

R

2

T

0

R

R

3

>0

∆L

2

T

7

7

MOD

T

3

∆L3<0

X

1

or

MOD

/

Select the user parameters.

Go to the soft-key row containing Tool Table.

Open the tool table.

Tool number ?

ENT

7

Enter the tool number (such as 7) and confirm your entry with ENT.

Tool length ?

ENT

2

Enter the tool length (12 mm) and confirm your entry with ENT.

or

L

=0

0

X

L7>0

Capture the actual position in the tool axis by pressing the soft key.

or

or

Capture the actual position in the tool axis by pressing key on the handwheel.

28 TNC 124

3 Manual Operation and Setup

Tool radius ?

MOD

ENT

8

MOD

Calling the tool data

The lengths and radii of your tools must first be entered into the
TNC's tool table (see previous page).

Before you start workpiece machining, select the tool you are using
from the tool table. To call the desired tool, move the highlight to the
tool, select the axis with the corresponding soft key and press the
soft key Tool Table.

The TNC then takes into account the stored tool data when you
work with tool compensation (e.g., with hole patterns).

You can also call the tool data with the command
TOOL CALL in a program.

Enter the tool radius (8 mm) and confirm your entry with ENT.

Depart the user parameters.

Example: Calling the tool data

MOD

/

Tool number ?

ENT

5

Fig. 3.6: The tool table on the TNC screen

Select the user parameters.

Go to the first soft-key row containing Tool Table.

Select the tool table.

Enter the tool number (here: 5) and confirm your entry with ENT.

Select the Tool axis (Z).

Activate the tool and depart the user parameters.

TNC 124 29

3 Manual Operation and Setup

Selecting datum points

The TNC 124 can store up to 99 datum points in a datum table. In
most cases this will free you from having to calculate the axis travel
when working with complicated workpiece drawings containing sev­eral datums, or when several workpieces are clamped to the ma­chine table at the same time.

For each datum point, the datum table contains the positions that
the TNC 124 assigned to the reference point on the scale of each
axis (REF values) during datum setting. Note that if you change the
REF values in the table, this will move the datum point.

The TNC 124 displays the number of the current datum at the lower
right of the screen.

To select the datum:

In all operating modes:

MOD

➤ Press MOD and go to the soft key row containing

Datum Table.

➤ Choose the soft key Datum Table.

➤ Select the datum you are using from the datum table.

➤ Leave the datum table:

Press MOD again.

In the MANUAL OPERATION and POSITIONING WITH MDI
modes of operation:

➤ Press the vertical arrow keys.

The machine manufacturer determines whether quick
datum selection via arrow keys is enabled on your
TNC.

In the PROGRAMMING AND EDITING / PROGRAM RUN modes
of operation:

➤ You can also select a datum point by entering the command

DATUM in a program.

30 TNC 124

3 Manual Operation and Setup

Y

X

2

1

Z

Datum setting: Approaching positions and entering actual values

The easiest way to set datum points is to use the TNC's probing
functions. A description of the probing functions starts on page 33.

Of course, you can also set datum points in the conventional man­ner by touching the edges of the workpiece one after the other with
the tool and entering the tool positions as datum points (see exam­ples on this page and the next).

Example: Setting a workpiece datum without the probing function

Working plane: X / Y

Tool axis: Z

Tool radius: R = 5 mm

Axis sequence in
this example: X - Y - Z

Preparation

➤ Select the desired datum point

(see Selecting datum points).

➤ Insert the tool.
➤ Press MOD and go to the soft-key row containing

Tool Table.

➤ Select the user parameter Tool Table.
➤ Select the tool you will use to set the datum.
➤ Leave the tool table:

Press the soft key Tool Call.

➤ Activate the spindle, for example with the miscellaneous

function M 3.

TNC 124 31

3 Manual Operation and Setup

Datum Setting: Approaching Positions and Entering Actual Values

Operating mode: MANUAL OPERATION

Select the Datum function.

Select the X axis.

Touch edge1with the tool.

Datum setting
X = + 0

5

ENT

Enter the position of the tool center (X =  5 mm)
and
transfer the X coordinate of the datum.

Select the Y axis.

Touch edge

Datum setting
Y = – 5

ENT

Transfer the Y coordinate of the datum.

Select the Z axis.

Touch the workpiece surface.

2

with the tool.

Datum setting
Z = – 5

0

ENT

32 TNC 124

Enter the position of the tool tip (Z = 0 mm)
and
transfer the Z coordinate of the datum.

3 Manual Operation and Setup

Functions for datum setting

It is very easy to set datum points with the TNC's probing functions.
These functions do not require a touch probe system or an edge
finder since you simply probe the workpiece edges with the tool.

The following probing functions are available:
 Workpiece edge as datum:

Edge

 Centerline between two workpiece edges:

Centerline

 Center of a hole or cylinder:

Circle Center

With Circle Center, the hole must be in a main plane.
The three main planes are formed by the axes X / Y, Y / Z
and Z / X.

Preparations for all probing functions

➤ Select the desired datum point

(see Selecting datum points).

➤ Insert the tool.
➤ Press MOD and go to the soft-key row containing

Tool Table.

➤ Select the user parameter Tool Table.
➤ Select the tool you will use to set the datum.
➤ Leave the tool table:

Press the soft key Tool Call.

➤ Activate the spindle, for example with the miscellaneous

functionM 3.

To abort the probing function

While the probing function is active, the TNC displays the soft key
Escape. Choose this soft key to return to the opening state of the
selected probing function.

Measuring diameters and distances

With the probing function Centerline the TNC calculates the dis-
tance between the two probed edges of a workpiece; with the Cir-
cle Center function it determines the diameter of the probed cir­cle.

The calculated distance and diameter are displayed on the TNC
screen between the position displays.

If you want to measure the distance between two edges or a diam­eter without setting a datum:

➤ Probe the workpiece as described on page 35

(Centerline) and page 36 (Circle Center).

As soon as the TNC displays the distance or diameter:

➤ Do not enter a datum coordinate. Simply press the soft key

Escape.

Fig. 3.7: On-screen operating instructions

for the probing functions

TNC 124 33

3 Manual Operation and Setup

Functions for Datum Setting

Example: Probe workpiece edge, display position of workpiece

edge and set the edge as a datum

The probed edge lies parallel to the Y axis.

The coordinates of the datum can be set by probing edges or sur­faces and capturing them as datums as described below.

Operating modes: MANUAL OPERATION/ELECTRONIC

HANDWHEEL/JOG INCREMENT

Z

Y

X?

X

/

Go to the second soft-key row.

Select Edge.

Select the axis for which the coordinate is to be set: X axis.

Probe in X axis

Move the tool towards the workpiece until it makes contact.

Store the position of the workpiece edge.

Retract the tool from the workpiece.

Ente r value for X

+ 0

2

0

ENT

34 TNC 124

0 is offered as a default value for the coordinate.
Enter the desired coordinate for the workpiece edge, for example X = 20 mm
and
set the coordinate as a datum for this workpiece edge.

3 Manual Operation and Setup

Functions for Datum Setting

Example: Set centerline between two workpiece edges as datum

The position of the centerline

1

edges

The centerline is parallel to the Y axis.

Desired coordinate
of the centerline: X = 5 mm

Operating modes: MANUAL OPERATION/ELECTRONIC

HANDWHEEL/JOG INCREMENT

and2 .

M

is determined by probing the

Z

Y

2

1

M

X?

X

/

Go to the second soft-key row.

Select Centerline.

Select the axis for which the coordinate is to be set: X axis.

Probe 1st edge in X

Move the tool towards workpiece edge1until it makes contact.

Store the position of the edge.

Probe 2nd edge in X

Move the tool towards workpiece edge

2

until it makes contact.

Store the position of the edge.
Screen display is frozen;
the distance between the two edges is displayed below the selected axis.

Retract the tool from the workpiece.

Enter value for X
+ 0

5

ENT

TNC 124 35

Enter coordinate (X = 5 mm)
and
transfer coordinate as datum for the centerline.

3 Manual Operation and Setup

Functions for Datum Setting

Example: Probe the circumference of a hole

and set the center of the hole as a datum

Main plane: X / Y plane

Tool axis: Z

X coordinate of the
circle center: X = 50 mm

Y coordinate of
circle center: Y = 0 mm

Operating mode: MANUAL OPERATION/ELECTRONIC

HANDWHEEL/JOG INCREMENT

Y

2

3 4

0

X?

X

1

/

Go to the second soft-key row.

Select Circle Center.

Select plane containing the circle (main plane): Plane X/Y.

Probe 1 s t poin t in X / Y

Move tool towards first point1on the circumference until it makes contact.

Store position of the bore hole wall.

Retract tool from bore hole wall.

Probe three additional points on the circumference in the same manner.
Further information appears on the screen. Store positions with Note.

Enter center point X
X = 0

0

5

ENT

Enter first coordinate (X = 50 mm)
and
transfer coordinate as datum for the circle center.

Enter center point Y
Y = 0

ENT

36 TNC 124

Ac cept d efault entry Y = 0 mm.

3 Manual Operation and Setup

NOTES

TNC 124 37

4 Positioning with MDI

4
Positioning with Manual Data Input (MDI)

For many simple machining processes, for example if a machining
process is to be executed only once, or if you are machining simple
geometrical shapes, it would be too time-consuming to enter the in­dividual machining steps in an NC program.

In the POSITIONING WITH MDI mode of operation you can enter
all data directly instead of storing them in a part program.

Simple milling and drilling operations

Enter the following nominal position data manually in the POSI­TIONING WITH MDI mode of operation:

 Coordinate axis
 Position value
 Radius compensation

The TNC then moves the tool to the desired position.

Pecking and tapping, hole patterns, rectangular pocket milling

The POSITIONING WITH MDI mode of operation also supports
the TNC Cycles (see Chapter 7):

 Pecking
 Tapping
 Bolt hole circle patterns
 Linear hole patterns
 Rectangular pocket

Before you machine the workpiece

➤ Select the desired datum point

(see Selecting datum points).

➤ Insert the tool.
➤ Pre-position the tool to prevent the possibility of damaging the

tool or workpiece.

➤ Select an appropriate feed rate F.
➤ Select an appropriate spindle speed S.

Taking the tool radius into account

The TNC can compensate for the tool radius (see Fig. 4.1).
This allows you to enter workpiece dimensions directly from the

drawing. The remaining distance is then automatically lengthened
(R+) or shortened (R) by the tool radius.

Entering tool data

➤ Press MOD.
➤ Choose the soft key Tool Table.
➤ Enter the tool number.
➤ Enter the tool length.
➤ Enter the tool radius.
➤ Select the tool axis via soft key.
➤ Press the Tool Call soft key.

Y

R

0

R+

R–

Fig. 4.1: Tool radius compensation

X

38 TNC 124

4 Positioning with MDI

Feed rate F, spindle speed S and miscellaneous function M

In the POSITIONING WITH MDI mode of operation you can also enter

and change the following information:

 Feed rate F

 Spindle speed S

 Miscellaneous function M

Feed rate F after an interruption of power

If you have entered a feed rate F in the POSITIONING WITH MDI

mode of operation, the TNC will move the axes with this feed rate after

an interruption of power as soon as power is restored.

Entering and changing the feed rate F

Example: Entering the feed rate F

Select F for the feed rate function.

Feed rate ?

5

0 0

ENT

Changing the feed rate F

You can vary the feed rate F infinitely by turning the knob for feed
rate override on the TNC control panel.

Feed rate override

You can vary the feed rate F from
0% to 150 % of the entered value.

Enter the feed rate F, for example 500 mm/min.

Confirm the feed rate F for the next positioning step.

100

15050

F %

0

+

´

Y

–

Z

´

+

Z

F%

´

–

X

´

+

X

–

Y

100

50

Fig. 4.2: Knob for feed rate override on the

TNC control panel

150

TNC 124 39

4 Positioning with MDI

Feed Rate F, Spindle Speed S and Miscellaneous Function M

Entering and changing the spindle speed S

The machine manufacturer determines which spindle
speeds are allowed on your TNC.

Example: Entering the spindle speed S

Select S for the spindle speed function.

Spindle speed ?

9

5 0

NC

To change the spindle speed S:

You can vary the spindle speed S infinitely by turning the knob for
spindle speed override  if provided  on the TNC control panel.

Spindle speed override

You can vary the spindle speed S from
0% to 150% of the set value.

Entering a miscellaneous function M

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

Enter the spindle speed S, for example 950 rpm.

Change the spindle speed S.

100

15050

S %

0

Example: Entering a miscellaneous function

Select M for the miscellaneous functions.

Miscellaneous function M ?

3

NC

40 TNC 124

Enter the miscellaneous function M, for example M 3: spindle ON, clockwise.

Execute the miscellaneous function M.

4 Positioning with MDI

Entering and moving to positions

For simple machining operations, you can program the coordinates
directly in the POSITIONING WITH MDI mode of operation.

Example: Milling a shoulder

The coordinates are entered as absolute dimensions; the datum is
the workpiece zero.

1

Corner
Corner
Corner
Corner

Preparation:

➤ Select the desired datum point

➤ Enter the tool data.
➤ Pre-position the tool to an appropriate location

➤ Move the tool to milling depth.

: X = 0 mm Y = 2 0 mm

2

: X = 30 mm Y = 20 mm

3

: X = 30 mm Y = 50 mm

4

: X = 60 mm Y = 50 mm

(see Selecting datum points).

(such as X = Y =  20 mm).

Y

50

20

0

1 2

0

3 4

30

X

60

Operating mode: POSITIONING WITH MDI

Select the Y axis.

Nominal position value ?

2

0

Enter the nominal position value for corner point1: Y = + 20 mm
and
select tool radius compensation: R +.

NC

Move the tool to the programmed position.

Select the X axis.

Nominal position value ?

03

Enter the nominal position value for corner point2: X = + 30 mm
and
select tool radius compensation: R .

NC

Move the tool to the programmed position.

TNC 124 41

4 Positioning with MDI

Entering and Moving to Positions

Nominal position value ?

5

0

Select the Y axis.

Enter the nominal position value for corner point3: Y = + 50 mm
and
select tool radius compensation: R +.

NC

Move the tool to the programmed position.

Select the X axis.

Nominal position value ?

6

0

NC

Enter the nominal position value for corner point4: X = + 60 mm,
tool radius compensation is already set to R +.

Move the tool to the programmed position.

42 TNC 124

4 Positioning with MDI

Pecking and tapping

The TNC cycles for pecking and tapping (see Chapter 7) are available
in the POSITIONING WITH MDI mode of operation.

Use the soft keys on the second soft-key row to select the desired
type of hole and enter the required data. These data can usually be
taken from the workpiece drawing (hole depth, infeed depth, etc.).

The TNC controls the machine tool and calculates additional data
such as the advanced stop distance if the hole is to be drilled in sev­eral infeeds.

Pecking and tapping in hole patterns

The functions for pecking and tapping are also available in combina­tion with the hole pattern functions Circle Pattern and Linear Pattern.

Pecking and tapping processes

The input data for pecking and tapping can also be entered as
cycles in a part program. You will find detailed information on how
the TNC controls pecking and tapping operations in Chapter7. (See
page 79 for pecking and page 82 for tapping).

Pre-positioning the drill for pecking and tapping

Pre-position the drill in the Z axis to a position above the workpiece.
In the X and Y axes (working plane), pre-position the drill to the hole

position. The hole position is approached without radius compensation
(input R0).

Input data for pecking

 Clearance height at which the drill can traverse in the working

plane without damaging the workpiece;
Enter an absolute value together with the algebraic sign.

 Setup clearance at which the drill is located above the work-

piece.

 Coordinate of the workpiece surface;

Enter an absolute value together with the algebraic sign.
 Hole depth; the algebraic sign determines the working direction.
 Infeed depth
 Dwell time of the drill at the bottom of the hole.
 Machining feed rate

Input data for tapping

 Clearance height at which the drill can traverse in the working

plane without damaging the workpiece;

Enter an absolute value together with the algebraic sign.
 Setup clearance at which the drill is located above the work-

piece.
 Coordinate of the workpiece surface;

Enter an absolute value together with the algebraic sign.
 Hole depth; the algebraic sign determines the working direction.
 Dwell time of the drill at the end of thread.
 Machining feed rate

TNC 124 43

4 Positioning with MDI

Example: PECKING

X coordinate of the hole: 30 mm
Y coordinate of the hole: 20 mm

Clearance height: + 50 mm
Setup clearance

Workpiece surface: + 0 mm
Hole depth

B

: 15mm
Pecking depth
Dwell time: 0.5 s
Pecking feed rate: 80 mm/min
Hole diameter: e.g. 6 mm

Preparation

➤ Pre-position the tool over the workpiece.

Operating mode: POSITIONING WITH MDI

A

:2mm

C

: 5mm

Select the X axis.

20

A

B

C

Y

0

0

X

30

Nominal position value ?

3

0

NC

Enter the nominal position value for pre-positioning in the X axis:
X = + 30 mm

and
select tool radius compensation R 0.

Pre-position the tool in the X axis.

Select the Y axis.

Nominal position value ?

2

0

NC

Enter the nominal position value for pre-positioning in the Y axis: Y = + 20 mm.
Tool radius compensation is already set to R 0.

Pre-position the tool in the Y axis.

44 TNC 124

4 Positioning with MDI

Pecking

5

/

Go to the second soft-key row.

Select Pecking.

Clearance height ?

ENT

0

Enter the clearance height of the tool over the workpiece (+ 50 mm).
Confirm your entry.

Setup clearance ?

ENT

2

Enter setup clearance
Confirm your entry.

Surface ?

ENT

0

Enter the coordinate of the workpiece surface (0 mm).
Confirm your entry.

Hole depth ?

1 5

ENT

Enter hole depth
Confirm your entry.

A

B

(– 15 mm).

(2 mm).

Pecking depth ?

ENT

5

Enter pecking depth
Confirm your entry.

C

(5 mm).

Dwell time ?

0

ENT

5

Enter the dwell time for chip breaking (0.5 s).
Confirm your entry.

Feed rate ?

0

NC

ENT

8

Enter the feed rate for drilling (F = 80 mm/min).
Confirm your entry.

Drill.

TNC 124 45

4 Positioning with MDI

Example: TAPPING

X coordinate of the hole: 30 mm
Y coordinate of the hole: 20 mm
Pitch p: 0.8 mm
Spindle speed S: 100 rpm
Clearance height: + 50 mm
Setup clearance
Workpiece surface: 0 mm
Thread depth

B

Dwell time: 0.4 s
Feed rate F = S  p: 80 mm/min

Preparation

➤ Pre-position the tool over the workpiece.

ä

For tapping right-hand threads activate the spindle with M 3.

Operating mode: POSITIONING WITH MDI

A

:3mm

:  20 mm

Select the X axis.

20

A

B

Y

0

0

X

30

Nominal position value ?

3

0

NC

Enter the nominal position value for pre-positioning in the X axis:
X = + 30 mm

and
select tool radius compensation R 0.

Pre-position the tool in the X axis.

Select the Y axis.

Nominal position value ?

2

0

NC

Enter the nominal position value for pre-positioning in the Y axis: Y = + 20 mm.
Tool radius compensation is already set to R 0.

Pre-position the tool in the Y axis.

46 TNC 124

4 Positioning with MDI

Tapping

5 0

3

0

2

/

Go to the second soft-key row.

Select Tapping.

Clearance height ?

ENT

Enter the clearance height of the tool over the workpiece (+ 50 mm).
Confirm your entry.

Setup clearance ?

ENT

Enter setup clearance

Surface ?

ENT

Enter the coordinate of the workpiece surface (0 mm).
Confirm your entry.

Hole depth ?

ENT

0

Enter hole depth

B

(– 20 mm). Confirm your entry.

A

(3 mm). Confirm your entry.

Dwell time ?

0

ENT

4

Enter the dwell time (0.4 s). Confirm your entry.

Feed rate ?

0

NC

ENT

8

Enter the feed rate for tapping (80 mm/min).
Confirm your entry.

Drill.

TNC 124 47

4 Positioning with MDI

Hole patterns

The hole pattern functions Circle Pattern and Linear
Pattern are available in the POSITIONING WITH MDI mode of

operation.

Use the soft keys to select the desired hole pattern function and en­ter the required data. These data can usually be taken from the
workpiece drawing (number of holes, coordinates of the first hole,
etc.).

The TNC then calculates the positions of all holes in the pattern, and
displays the pattern graphically on the screen.

Type of hole

At the hole positions that were calculated for the pattern you
canexecute either

 pecking or
 tapping operations.

Enter the required data for pecking or tapping (see pages 43 to 47).

If you do not wish to drill at the calculated hole positions, or if you
want to drill the holes manually:

➤ Choose the soft key No Entry for Type of hole ? .

Fig. 4.3: On-screen operating instructions:

graphic for bolt hole circle pattern
(full circle)

Pre-positioning the drill

Pre-position the drill in the Z axis to a position above the workpiece
surface. The TNC then pre-positions the drill in the X and Y axes
(working plane) above each hole position.

Bolt hole circle patterns

If you are drilling a Circle Pattern in the POSITIONING
WITH MDI mode of operation, enter the following data:

 Full circle or circle segment
 Number of holes
 Center point coordinates and radius of the circle
 Starting angle (position of first hole)
 Circle segment only: angle step between the holes
 Bore hole or tap hole

Linear hole patterns

If you are drilling a Linear Pattern in the POSITIONING
WITH MDI mode of operation, enter the following data:

 Coordinates of the first hole
 Number of holes per row
 Spacing between holes on a row
 Angle between the first row and the X axis
 Number of rows
 Spacing between rows
 Bore hole or tap hole

Fig. 4.4: On-screen operating instructions:

graphic for bolt hole circle pattern
(circle segment)

48 TNC 124

4 Positioning with MDI

Bolt hole circle patterns

Information required:
 Full circle or circle segment
 Number of holes
 Center point coordinates and radius of the circle
 Starting angle (position of first hole)
 Circle segment only: angle step between the holes
 Bore hole or tap hole

The TNC calculates the coordinates of all holes.

Bolt hole circle graphic

The graphic enables verification of the hole pattern before you start
machining. It is also useful when:

 selecting holes directly
 executing holes separately
 skipping holes

Overview of functions

Function Soft key/Key

Switch to full circle

Switch to circle segment

Go to next-highest
input line

Go to next-lowest
input line

Confirm entry values

Fig. 4.5: TNC graphic for bolt hole circle

patterns

ENT

TNC 124 49

4 Positioning with MDI

Bolt Hole Circle Patterns

Example: Entering data and executing bolt hole circles

The work steps Enter circle pattern data, Display graphic and
Drill are described separately in this example.

Hole data

Enter the hole data separately (see pages 43 and 44) before enter­ing the circle pattern data.

Clearance height: +50 mm

A

Setup clearance

:3mm
Workpiece surface: 0 mm
Hole depth
Pecking depth

B

: 20mm

C

:5mm
Dwell time: 0.4 s
Feed rate: 80 mm/min

Circle pattern data

Number of holes: 8
Center point coordinates: X = 50 mm

Y = 50 mm
Bolt hole circle radius: 20 mm
Starting angle: angle between

X axis and first hole 30°

50

Z

A

C

B

Y

30°

R20

1st step: Enter circle pattern data

Operating mode: POSITIONING WITH MDI

/

0

0

Go to the second soft-key row in the operating mode
POSITIONING WITH MDI.

Select Circle Pattern.

Select Full Circle.

50

X

50 TNC 124

4 Positioning with MDI

Bolt Hole Circle Patterns

Number of holes ?

ENT

8

Center point X ?

5 0

Center point Y ?

5 0

Radius ?

2

0

ENT

ENT

ENT

Enter the data and call the dialog.

Enter the number of holes (8).
Confirm your entry.

Enter the X coordinate of the center of the bolt hole circle (X = 50 mm).
Confirm your entry.

Enter the Y coordinate of the center of the bolt hole circle (Y = 50 mm).
Confirm your entry.

Enter the radius of the bolt hole circle (20 mm).
Confirm you entry.

3 0

Starting angle ?

ENT

Enter the starting angle from the X axis to the first hole (30°).
Confirm your entry.

Type of hole ?

Choose Pecking for drilling bore holes at the hole positions in the pattern.

TNC 124 51

4 Positioning with MDI

Bolt Hole Circle Patterns

2nd step: Display graphic

The graphic makes it easy to verify the entered data.
The solid circle represents the currently selected hole.

The direction of rotation for bolt hole circle graphics
is influenced with a user parameter (see Chapter 13).

The TNC can mirror the coordinate axes for bolt hole
circle graphics (see Chapter 13).

The TNC displays the bolt hole
circle graphically on the screen.

Here, a full circle with 8 holes is
shown. The first hole is at 30°.
The coordinates of the hole are
given at the bottom of the screen.

3rd step: Drill

Before you start drilling verify the data entered in the drilling cycle!

The direction of rotation for bolt hole circles is influenced
with a user parameter (see Chapter 13).

Start the bolt hole circle function.

NC

NC

NC

Pre-position in the first coordinate axis.

Pre-position in the second coordinate axis.

Drill. The TNC drills the bolt hole as defined by the input data for Pecking
(or Tapping).

NC

Drill the next hole and all remaining holes.

Functions for drilling and graphic

Function Soft key

Go to next hole

Return to last hole

End graphic/drilling

52 TNC 124

4 Positioning with MDI

Linear hole patterns

Information required:
 Coordinates of the first hole
 Number of holes per row
 Spacing between holes on a row
 Angle between the first row and the angle reference axis
 Number of rows
 Spacing between rows
 Bore hole or tap hole

The TNC calculates the coordinates of all holes.

Linear hole pattern graphic

The graphic enables verification of the hole pattern before you start
machining. It is also useful when:

 selecting holes directly
 executing holes separately
 skipping holes

Overview of functions

Function Key

Go to the next-highest
input line

Go to the next-lowest
input line

Confirm entry values

ENT

Fig. 4.6: TNC graphic for linear hole patterns

TNC 124 53

4 Positioning with MDI

Linear Hole Patterns

Example: Entering data and executing rows of holes

The work steps Enter linear pattern data, Display graphic and
Drill are described separately in this example.

Hole data

Enter the hole data separately (see pages 43 and 44) before enter­ing the linear pattern data.

Clearance height: +50 mm

A

Setup clearance

:3mm
Workpiece surface: 0 mm
Hole depth
Pecking depth

B

: 20mm

C

:5mm
Dwell time: 0.4 s
Feed rate: 80 mm/min

Linear pattern data

1

X coordinate of hole
Y coordinate of hole

: X = 2 0 m m

1

: Y = 15 mm
Number of holes per row: 4
Hole spacing: +10 mm

Angle between rows and
X axis: 18°
Number or rows: 3
Row spacing: +12 mm

1st step: Enter linear pattern data

Operating mode: POSITIONING WITH MDI

15

Z

A

C

B

Y

10

1

0

12

18°

X

0

20

/

Go to the second soft-key row in the operating mode
POSITIONING WITH MDI.

Select Linear Pattern.

54 TNC 124

4 Positioning with MDI

Linear Hole Patterns

1st hole X ?

2

0

1st hole Y ?

1 5

Holes per row ?

ENT

4

Hole spacing ?

1

0

Angle ?

1 8

ENT

ENT

ENT

ENT

1

Enter the X coordinate of hole
Confirm your entry.

Enter the Y coordinate of hole1(Y = 1 5 m m ) .
Confirm your entry.

Enter the number of holes per row (4).
Confirm your entry.

Enter the spacing between holes in the row (10 mm).
Confirm your entry.

Enter the angle between the X axis and the hole pattern (18°).
Confirm your entry.

(X = 20 mm) .

3

1 2

Number of rows ?

ENT

Enter the number of rows (3).
Confirm your entry.

Row spacing ?

ENT

Enter the spacing between rows (12 mm).
Confirm your entry.

Type of hole ?

Choose Pecking for drilling bore holes at the hole positions in the pattern.

TNC 124 55

4 Positioning with MDI

Linear Hole Patterns

2nd step: Display graphic

The graphic makes it easy to verify the entered data.
The solid circle represents the currently selected hole.

The TNC can mirror the coordinate axes for linear hole
pattern graphics if the corresponding user parameter is set
(see Chapter 13).

The TNC displays the pattern
graphically on the screen.
Here, 3 rows of 4 holes are shown.

1st hole at X=20 mm, Y=10 mm
Hole spacing 10 mm
Angle between rows and X axis: 18°
Row spacing 12 mm

Coordinates of the current hole are
shown at the bottom of the screen.

3rd step: Drill

Before you start drilling verify the data entered in the drilling cycle!

NC

NC

NC

NC

Functions for drilling and graphic

Function Soft key

Go to next hole

Start the linear hole pattern function.

Pre-position in the first coordinate axis.

Pre-position in the second coordinate axis.

Drill. The TNC drills the bolt hole as defined by the input data for Pecking
(or Tapping).

Drill the next and all remaining holes.

Return to last hole

End graphic/drilling

56 TNC 124

4 Positioning with MDI

Rectangular pocket milling

The TNC cycle for rectangular pocket milling is available in the PO­SITIONING WITH MDI mode of operation.

The input data for milling a rectangular pocket can also be entered
as a cycle in a part program (see Chapter 7).

Select the Pocket Milling soft key on the second soft-key row and
enter the required data. These data can usually be taken from the
workpiece drawing (side length, depth of the pocket, etc.).

The TNC controls the machine tool and calculates the tool path for
area clearance.

For the procedure and input data required for programming a rec­tangular pocket, see Chapter 7.

TNC 124 57

4 Positioning with MDI

Example: RECTANGULAR POCKET

Clearance height: + 80 mm
Safety clearance: 2 mm

Workpiece surface: + 0 mm
Milling depth:  20 mm
Pecking depth: 7 mm
Pecking feed rate: 80 mm/min
Pocket center in X: 50 mm

Pocket center in Y: 40 mm
Side length in X: 80 mm
Side length in Y: 60 mm

Milling feed rate: 100 mm/min
Direction of milling rotation: 0: CLIMB

Finishing allowance: 0.5 mm

Operating mode: POSITIONING WITH MDI

/

Go to the second soft-key row.

Select Pocket Milling.

–20
–30

80
70

40

10

Z

0

X

Y

R10

0

0

10

50

90

X

100

Clearance height ?

8

ENT

0

Enter the clearance height of the tool over the workpiece (HEIGHT +80 mm).
Confirm your entry.

Setup clearance ?

ENT

2

Enter the setup clearance (DIST 2 mm).
Confirm your entry.

Surface ?

ENT

0







NC

Enter the coordinate of the workpiece surface (SURF 0 mm).
Confirm your entry.

After you have entered all the data, start the rectangular pocket milling cycle.

58 TNC 124

5 Programming

5
Programming

Operating mode PROGRAMMING AND EDITING

In the PROGRAMMING AND EDITING mode of operation you can
store the individual work steps that are required for recurring
machining operations, for example for small-lot production.

Programs in the TNC

Programs contain the work steps for workpiece machining. You can
edit programs, add work steps and run them as often as you wish.

The External mode enables you to store programs with the HEI-
DENHAIN FE 401 floppy disk unit and load them into the TNC again
on demandyou don't need to retype them. You can also transfer
programs to a personal computer or printer.

Storage capacity

The TNC 124 can store a maximum of 20 programs with a total of
2000 NC blocks. A single program can contain a maximum of 1000
NC blocks.

Position display during programming

In the PROGRAMMING AND EDITING mode of operation, the TNC
continuously displays the current positions at the bottom of the screen
to left of the lowest soft key.

Fig. 5.1: The first soft-key row in the operat-

ing mode PROGRAMMING AND

EDITING

Programmable functions

 Nominal position values
 Feed rate F, spindle speed S and miscellaneous function M
 Tool call
 Pecking and tapping cycles
 Bolt hole circle and linear hole patterns
 Program section repeats:

A section of a program only has to be entered once and can then
be run up to 999 times in succession.

 Subprograms:

A section of a program only has to be entered once and can then

be run at various points in the program.
 Datum call
 Dwell time
 Interrupt program

Transfer position: Teach-In mode

This mode allows you to transfer the actual positions of the tool di­rectly into a program, such as the nominal positions for workpiece
machining, etc.

In many cases the Teach-In function will save you considerable pro­gramming work.

What happens with finished programs?

For workpiece machining, programs are executed in the operating
mode PROGRAM RUN. See Chapter 10 for an explanation of this
mode.

TNC 124 59

5 Programming

Entering a program number

Select a program and identify it by a number between 0 and
99999999 which you assign it.

Operating mode: PROGRAMMING AND EDITING

Select Program Manage.

Go to the program directory.

or

/

Program directory

The program directory appears when you choose the soft key Pro­gram Number. The number in front of the slash is the program

number, the number behind the slash is the number of blocks in the
program.

A program always contains at least two blocks.

Program number ?

1

/

ENT

When you select the unit of measurement with the soft
key inch/mm, the TNC overwrites the user parameter
inch/mm.

Create a new program or select an existing program,
such as program number 1.

or

Select an existing program with the cursor keys.

Choose the unit of measurement.

Confirm your entry.
The selected program can now be entered, edited and run.

Deleting programs

If you no longer wish to keep a program in memory,
you can delete it:

➤ Press the soft key Program Manage.
➤ Press the soft key Delete Program.
➤ Enter the program number.
➤ Press ENT to delete the program.

60 TNC 124

5 Programming

Editing programs

Operating mode: PROGRAMMING AND EDITING

Select a program (see previous page).

The first soft-key row provides

/

/

functions for
 Selecting program management
 Entering coordinates

The second soft-key row provides
the following functions:

 Enter labels for subprograms

and program section repeats
 Call tool data
 Interrupt program with Stop
 Delete program blocks

The third soft-key row provides
cycles for entering:

 Cycle definition for pecking,

tapping, bolt hole circles and

/

/

linear hole patterns
 Cycle call
 Datum call
 Dwell time
 Teach-In

The fourth soft-key row provides
the functions
 Feed rate F
 Miscellaneous function M
 Spindle speed S

TNC 124 61

5 Programming

Editing program blocks

Current block

The current block is shown between the two dashed lines. New
blocks are inserted behind the current block. When the END PGM
block is between the dashed lines, no new blocks can be inserted.

Overview of functions

Function Soft key/Key

Go up one block

Go down one block

Clear numerical entry

Delete current block

Going directly to a program block

Scrolling to the desired block with the arrow keys can be time-con­suming with long programs. A quicker way is to use the GOTO func­tion. This enables you to move directly to the block you wish to
change or add new blocks behind.

Operating mode: PROGRAMMING AND EDITING

GOTO

Block number ?

5 8

ENT

CE

Press the GOTO key.

Enter a block number, such as 58.

Confirm your entry.
Block number 58 is now the currently selected block.

62 TNC 124

5 Programming

Editing existing programs

You can edit existing programs, for example to correct keying er­rors. The TNC supports you with plain language dialogs  just as
when you are creating a new program.

Confirm your changes

You must confirm each change with the ENT key for it to become
effective!

Example: Changing a program number

➤ Select the BEGIN or END block.
➤ Enter a new program number.
➤ Confirm the change with ENT.

Example: Editing a program block

Operating mode: PROGRAMMING AND EDITING

/

2 0

ENT

Overview of functions

Function Key

Select the next-lowest program block

Select the next-highest program block

Go directly to program block number

Select program block to edit

Move to the block you wish to change.

Select the block.

Edit the block, for example enter a new nominal position value (here, 20).

Confirm the change.

GOTO

Confirm change

ENT

TNC 124 63

5 Programming

Deleting program blocks

You can delete any blocks in existing programs except the BEGIN
and END blocks.

When a block is deleted, the TNC automatically renumbers the re­maining blocks. The block before the deleted block then becomes
the current block.

Example: Deleting a program block

Operating mode: PROGRAMMING AND EDITING

/

/

It is also possible to delete an entire program section:

➤ Select the last block of the program section to be deleted.
➤ Press the soft key Delete Block repeatedly until all

blocks in the program section have been deleted.

Move to the block you wish to delete
(or use the GOTO key).

Go to the second soft-key row.

Press Delete Block.

64 TNC 124

5 Programming

Feed rate F, spindle speed S and miscellaneous function M

Besides the geometry for workpiece machining, you must also enter
the following information:

 Feed rate F in [mm/min]
 Miscellaneous function M
 Spindle speed S in [rpm]

The feed rate F, miscellaneous function M and spindle speed S are
programmed in separate blocks and become effective as soon as the
TNC has executed the blocks in which they are programmed.
These program blocks must be entered in the program befo r e t he
positioning blocks for which they are intended.

Entering the feed rate F

The feed rate F is modally effective. This means that the entered
feed rate remains in effect until a new feed rate is programmed.

Exception: Rapid traverse F MAX

Rapid traverse F MAX

You can also move the machine axes at rapid traverse (F MAX). The
feed rate for rapid traverse F MAX is preset in a machine parameter
by the machine manufacturer.
F MAX is not modally effective.

After the block with F MAX is executed, the feed rate returns to the
value that was programmed previously.

Programming example:

Operating mode: PROGRAMMING AND EDITING

/

Feed rate ?

5

0

0

or

The feed rate can be varied infinitely during program
run by turning the knob for feed rate override on the TNC
control panel.

ENT

Go to the fourth soft-key row.

Select Feed rate F.

Enter the feed rate F, such as F = 500 mm/min.
Confirm entry. Input range: 0 to 30 000 mm/min.

or

Select rapid traverse F MAX.

TNC 124 65

5 Programming

Feed Rate F, Spindle Speed S and Miscellaneous Function M

Entering the spindle speed S

The machine manufacturer determines which spindle
speeds are allowed on your TNC.

The spindle speed S is modally effective. This means that the
entered spindle speed remains in effect until a new spindle speed is
programmed.

Programming example

Operating mode: PROGRAMMING AND EDITING

/

Spindle speed ?

9

9

The spindle speed can be varied infinitely during program
run by turning the knob for spindle speed override on the
TNC control panel.

Entering a miscellaneous function M

With the miscellaneous functions (M functions) you can influence,
for example, direction of spindle rotation and program run.

Chapter 14 provides an overview of all miscellaneous functions that
can be programmed on the TNC 124.

The machine manufacturer determines which miscel­laneous functions are available on your TNC and which
functions they have.

ENT

0

Go to the fourth soft-key row.

Select Spindle speed S.

Enter the spindle speed S, such as S = 990 rpm.
Confirm entry. Input range: 0 to 9999.999 rpm.

Programming example

Operating mode: PROGRAMMING AND EDITING

/

Go to the fourth soft-key row.

Select Miscellaneous function M.

Miscellaneous function M ?

ENT

3

66 TNC 124

Select the miscellaneous function, such as M 3 (spindle ON, clockwise).
Confirm entry.

5 Programming

Entering program interruptions

You can divide a program into sections with stop marks. The TNC
then only executes the next block when you resume program run.

Operating mode: PROGRAMMING AND EDITING

/

Resuming program run after an interruption

➤ Press the NC-

I key.

Go to the second soft-key row.

Press STOP to insert a program interruption.

TNC 124 67

5 Programming

Calling the tool data in a program

Chapter 3 explained how to enter the length and radius of your tools
in the tool table.

The tool data stored in the table can also be called from a program.
Then if you change the tool during program run you don't need to se­lect the new tool data from the tool table every time.

The TOOL CALL command automatically pulls the tool length and
radius from the tool table.

You define the tool axis for program run in the program.

If you enter a different tool axis in the program than is
stored in the table, the TNC stores the new tool axis in
the table.

Operating mode: PROGRAMMING AND EDITING

Fig. 5.2: The tool table on the TNC screen

/

Tool number ?

ENT

4

Tool axis ?

or

Working without TOOL CALL

If a part program is written without TOOL CALL the TNC will use
the data of the tool that was programmed previously.

When you are changing tools, you can also go to the tool table from
the operating mode PROGRAM RUN to call the new tool data.

Go to the second soft-key row.

Call tool data from the tool table.

Enter the tool number (such as 4) under which the tool data are stored
in the tool table. Confirm entry.
Input range: 0 to 99.

Enter the tool axis (such as Z).
The program contains the tool call block TOOL CALL 4 Z.

or

Choose No Entry for the Tool axis, if the program already contains a
TOOL CALL block with tool data.

The program contains the tool call block TOOL CALL 4.

68 TNC 124

5 Programming

Calling datum points

The TNC 124 can store up to 99 datum points in a datum table. You
can call a datum point from the datum table during program run by
simply pressing the soft key Datum Call and entering the block
DATUM XX. This automatically calls the datum point entered for XX
during program run.

Operating mode: PROGRAMMING AND EDITING

/

Go to the third soft-key row.

Call a datum point from the table.

D a t u m n u m b e r ?

5

ENT

Enter the datum number (such as 5).
Confirm entry. Input range: 1 to 99.

TNC 124 69

5 Programming

Entering dwell time

You can enter a dwell time in the part program by pressing the soft
key Dwell Time and defining the block DWELL XXXX.XXX.
When the DWELL block is executed, continuation of the running
program is delayed by the time entered in seconds for DWELL.

Operating mode: PROGRAMMING AND EDITING

/

Go to the third soft-key row.

Call dwell time.

D w e l l t i m e i n s e c o n d s ?

8

ENT

Enter the dwell time in seconds (such as 8).
Confirm entry. Input range: 0 to 9999.999.

70 TNC 124

6 Programming Workpiece Positions

6
Programming Workpiece Positions

Entering workpiece positions

For many simple machining processes it is often sufficient to simply
describe the workpiece to be machined by the coordinates of the po­sitions to which the tool should move.

There are two possibilities of entering these coordinates in a
program:

 Keying in the coordinates with the keyboard, or
 Transferring the tool position with the Teach-In function

Entries for a complete part program

Having the TNC execute a machining process requires more than
entering coordinates in a program. A complete part program requires
the following data:

A BEGIN block and an END block (automatically generated by

the TNC)
 Feed rate F
 Miscellaneous function M
 Spindle speed S
 Calling the tool with TOOL CALL

Entering feed rate F, miscellaneous function M, spindle speed S and
TOOL CALL in a part program is described in Chapter 5.

Important information on programming and machining

The following information is intended to help you in quickly and easily
machining the programmed workpiece.

Movements of tool and workpiece

During workpiece machining on a milling or drilling machine, an axis
position is changed either by moving the tool or by moving the ma­chine table on which the workpiece is fixed.

When entering tool movements in a part program you
always program as if the tool is moving and the work­piece is stationary.

Pre-positioning

Pre-position the tool to prevent the possibility of damaging the
tool or workpiece. The best pre-position lies on the extension of the
tool path.

Feed rate F and spindle speed S

Adjust the feed rate F and spindle speed S to your tool, workpiece
material and machining operation.
The TNC then calculates the feed rate F and spindle speed S with
the INFO function (see Chapter 12).

In the appendix you will find a diagram which will aid you in
selecting the appropriate feed rate F for tapping.

TNC 124 71

6 Programming Workpiece Positions

Entering Workpiece Positions

Programming example: Milling a shoulder

The coordinates are programmed in absolute dimensions.
The datum is the workpiece zero.

1

Corner
Corner
Corner
Corner

: X = 0 mm Y = 2 0 m m

2

: X = 30 mm Y = 20 mm

3

: X = 30 mm Y = 50 mm

4

: X = 60 mm Y = 50 mm

Summary of all programming steps

➤ In the main menu PROGRAMMING AND EDITING go to

Program Manage.

➤ Key in the number of the program you want to work on, and

press ENT.

➤ Enter the nominal positions.

Running a finished program

When a program is finished it can be run in the PROGRAM RUN
mode (see Chapter 10).

Example of entry:Entering a nominal position into a program

(block 11 in this example)

Y

50

20

0

1 2

0

3 4

30

X

60

Select the coordinate axis (X axis).

Nominal position value ?

3

0

ENT

Program blocks

0 BEGIN PGM 10 MM Start of program, program number and unit of measurement
1 F 9999 High feed rate for pre-positioning

2 Z+20 Clearance height
3 X–20 R0 Pre-position the tool in the X axis
4 Y–20 R0 Pre-position the tool in the Y axis
5 Z–10 Move tool to milling depth

6 TOOL CALL 1 Z Call the tool, such as tool 1, tool axis Z

7 S 1000 Spindle speed
8M 3 Spindle ON, clockwise

9 F 200 Machining feed rate

10 Y+20 R+ Y coordinate, corner

11 X+30 R– X coordinate, corner

12 Y+50 R+ Y coordinate, corner
13 X+60 R+ X coordinate, corner

14 F 9999 High feed rate for retracting
15 Z+20 Clearance height
16 M 2 Stop program run, spindle OFF, coolant OFF

17 END PGM 10 MM End of program, program number and unit of measurement

Enter the nominal position value, for example 30 mm
and

select tool radius compensation R .

Confirm the entry. The nominal position is now the current block
(between the dashed lines).

1

2

3

4

72 TNC 124

6 Programming Workpiece Positions

Transferring positions: Teach-In mode

Teach-In programming offers the following two options:

 Enter nominal position, transfer nominal position to program,

move to position.
 Move to a position and transfer the actual value to a program

via soft key or through the actual-value-capture key on the

handwheel.

You can change transferred position values during Teach-In.

Preparation

➤ With Program number select the program you want transfer

positions to.
➤ Select the tool data from the tool table.

Feed rate F for Teach-In

Before starting the Teach-In process define the feed rate at which the
tool should move during Teach-In:

➤ Select the Teach-In function and enter a block with the desired

feed rate F first.
➤ Press the NC-

I key.

Overview of functions

Function Soft key/Key

Go to the next block

Go to the previous block

Delete the current block

TNC 124 73

6 Programming Workpiece Positions

Transferring Positions: Teach-In Mode

Programming example: Generate a program while machining a pocket

With Teach-In you first machine a workpiece according to the
workpiece drawing dimensions.

The TNC then transfers the coordinates directly into the program.
Pre-positioning and retraction movements can be selected as de­sired and entered like drawing dimensions.

1

Corner point
Corner point
Corner point
Corner point

: X = 15 mm Y = 12 mm

2

: X = 15 mm Y = 47 mm

3

: X = 53 mm Y = 47 mm

4

: X = 53 mm Y = 12 mm

Pocket depth: Z =  10 mm (for example)

Operating mode: PROGRAMMING AND EDITING

Select Teach-In.

Example: Transferring the Y coordinate of corner point

3

i nt o a p r og ra m

Select the coordinate axis (Y axis).

Y

47

12

0

53

3

4

X

2

1

0

15

Nominal position value ?

4 7

NC

Enter the nominal position value (such as 47 mm)
and

select tool radius compensation R .

Move to the programmed coordinate.
Then enter and transfer any other coordinates.

74 TNC 124

6 Programming Workpiece Positions

Y

X

Z

Transferring Positions: Teach-In Mode

Programming example: Touch island with tool

and transfer positions to program

This example illustrates how to generate a program containing the
actual positions of the tool.

When you then run the program:
➤ Use a tool which has the same radius as the tool you used

during the Teach-In process.
➤ If you use a different tool, you must enter all program blocks

with radius compensation. Then enter the difference between

the radii of the two tools as the tool radius for machining:

Radius of the tool for machining

 Radius of the tool for Teach-In
= Tool radius to be entered for machining

Selecting radius compensation

The current radius compensation is highlighted at the top of the
screen. If you wish to change the radius compensation:

➤ Press the soft key Radius Comp.

Operating mode: PROGRAMMING AND EDITING

Select Teach-In.

/

Example: Transfer Z coordinate (workpiece surface)

to a p rog ra m

´

–

Z

or

Z

Page to the second soft-key row.

Move the tool until it touches the workpiece surface.

Store the position in the tool axis (Z) with the soft key at the TNC

or

with the actual-position-capture key on the handwheel.

TNC 124 75

6 Programming Workpiece Positions

Transferring Positions: Teach-In Mode

Changing nominal positions after they have been transferred

Positions which you have transferred into a program with Teach-In
can be changed. It is not necessary to leave the Teach-In mode to
do so.

Enter the new value in the input line.

Example: Changing a block transferred with Teach-In

Operating mode: PROGRAMMING AND EDITING, Teach-In

/

With the arrow keys (or GOTO), move to the block you wish to change.

Select the block.

Nominal position value ?

3

0

ENT

Functions for changing a Teach-In program

Function Soft key

Enter feed rate F

Enter miscellaneous function M

Enter a new nominal position value
and
change the tool radius compensation (for example).

Confirm your changes.

Enter spindle speed S

Delete current block

76 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

7

Drilling, Milling Cycles and Hole Patterns in Programs

The cycles for pecking or tapping, hole patterns, and rectangular
pocket milling can also be written to a program (see Chapter 4).
Each piece of information is then stored in a separate program
block. These blocks are identified by CYCL after the block
number, followed by a number.

The cycles contain all information required by the TNC for machin­ing a hole, hole pattern or rectangular pocket.

The TNC 124 features six different cycles:

Drilling cycles

• CYCL 1.0 PECKING

• CYCL 2.0 TAPPING

Hole patterns

• CYCL 5.0 FULL CIRCLE

• CYCL 6.0 CIRCLE SEGMENT

• CYCL 7.0 LINEAR HOLE PATTN

Rectangular pocket milling

• CYCL 4.0 RECTANGULAR POCKET

Cycles must be complete

Do not delete any blocks from a cycle because this will result in
the error message CYCLE INCOMPLETE when the program is
executed.

Drilling cycles must be called

The TNC runs a drilling cycle whenever it reaches a cycle call
(CYCL CALL) during execution of the program. A cycle call always
calls the drilling cycle that was programmed before the cycle call.

The TNC automatically executes a hole pattern or rectangular
pocket as soon as it reaches it during execution of the program. If
you wish to repeatedly execute hole patterns or rectangular pock­ets, you must enter the data repeatedly or write them in a
subprogram (see Chapter 8).

Entering cycles

Press the Cycle Def. soft key in the third soft-key row and se-
lect the desired cycle. The TNC automatically asks for all data re­quired for executing the cycle.

TNC 124 77

7 Drilling, Milling Cycles and Hole Patterns in Programs

Entering a cycle call

A drilling cycle must be called at the location in a part program at
which the cycle is to be executed.

Operating mode: PROGRAMMING AND EDITING

/

Drilling cycles in programs

The following two cycles are available on the TNC 124:
 CYCL 1.0 PECKING
 CYCL 2.0 TAPPING

Cycle 1.0 PECKING

Cycle 1.0 PECKING is used for drilling holes in several infeeds.

During machining the TNC advances the tool in several infeeds,
retracting the tool each time to setup clearance.

Cycle 2.0 TAPPING

The TAPPING cycle requires a floating tap holder.

Go to the third soft-key row.

Enter a cycle call (CYCL CALL).

Cycle 2.0 TAPPING is used for cutting threads.

The thread is cut in one pass. After a dwell time at the end of
thread, the direction of spindle rotation is reversed and the tool re­tracted.

Signs for the input values in the drilling cycles

Enter the clearance height

O

workpiece surface

as absolute values  together with the al-

H

and the coordinate of the

gebraic sign.

The algebraic sign for hole depth (thread length)
the working direction. If you are drilling in the negative axis direc­tion, enter a negative sign for hole depth.

Fig. 7.1 also illustrates setup clearance
depth

C

.

Pre-positioning the drill

Before executing the cycle, pre-position the drill in the tool axis and
in the working plane. The coordinates for pre-positioning can be en­tered into the program before the cycle.

A

and the infeed

B

determines

A

C

B

O

Fig. 7.1: Absolute and incremental input

C

values for drilling cycles

H

78 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

PECKING

If you program Cycle 1.0 PECKING, the TNC drills to the pro­grammed hole depth in several infeeds.

Process

The pecking cycle is illustrated in Fig. 7.2 and Fig. 7.3.

I:

The TNC pre-positions the tool at setup clearance above the
workpiece surface.

II:

The tool drills to the first pecking depth at the programmed ma­chining feed rate F. After reaching the first pecking depth, the tool
retracts at rapid traverse (F MAX) to setup clearance .

C

III:

The TNC pre-positions the tool at rapid traverse to the first infeed
depth , minus the advanced stop distance . The tool then
advances with another infeed .

C

C

t

I

A

A

II

A

C

A

IV:

The TNC retracts the tool again and repeats the drilling process
(drilling/retracting) until the programmed hole depth is reached.

After a dwell time at the hole bottom, the tool is retracted to clear­ance height at rapid traverse (F MAX) for chip breaking.

Advanced stop distance

The advanced stop distance for the drilling operation is auto­matically calculated by the TNC:

Hole depth up to 30 mm: = 0.6 mm
Hole depth between 30 mm and 350 mm: = 0.02  hole depth
Hole depth exceeding 350 mm: = 7 mm

Input data for Cycle 1.0 PECKING

 Clearance height - HEIGHT

Position in the tool axis at which the TNC can move the tool in

the working plane without damaging the workpiece.
 Setup clearance - DIST

The TNC advances the tool from clearance height to setup

clearance at rapid traverse.
 Workpiece surface - SURF

Absolute coordinate of the workpiece surface.
 Hole depth - DEPTH

Distance between workpiece surface and bottom of hole (tip of

drill taper).
 Pecking depth - PECKG

Infeed per cut.
 Dwell time - DWELL in [s]

Amount of time the tool remains at the hole depth for cutting

free the drill taper.
 Feed rate - F in [mm/min]

Traversing speed of the tool while drilling.

Fig. 7.2: Steps I and II in Cycle

B

III

t

t

t

t

t

A

Fig. 7.3: Steps III and IV in Cycle 1.0

B

C

1.0 PECKING

A

C

t

C

PECKING

IV

A

B

Hole depth and infeed depth

The infeed depth does not have to be a multiple of the hole depth.
If the infeed depth is programmed greater than the hole depth, or
equals the hole depth, the tool will drill to the programmed hole
depth in one operation.

TNC 124 79

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

Programming example: Cycle 1.0 PECKING

X coordinate of the hole: 30 mm
Y coordinate of the hole: 20 mm
Hole diameter: 6 mm
Clearance height HEIGHT: + 50 mm
Setup clearance DIST : 2 mm

A

Coordinate of the
workpiece surface SURF: 0 mm

Hole depth DEPTH :  15 mm
Pecking depth PECKG : 5 mm

B

C

Dwell time DWELL: 0.5 s
Machining feed rate F: 80 mm/min

Example: Entering Cycle 1.0 PECKING in a part program

Operating mode: PROGRAMMING AND EDITING

20

A

B

C

Y

0

0

X

30

/

Page to the third soft-key row.

Select Cycle Definition.

Enter Cycle 1.0 PECKING in a part program.

Clearance height ?

5

ENT

0

Enter the clearance height (HEIGHT = 50 mm).
Confirm your entry.

Setup clearance ?

ENT

2

Enter the setup clearance (DIST = 2 mm).
Confirm your entry.

Workpiece surface ?

ENT

0

Enter the coordinate of the workpiece surface (SURF = 0 mm).
Confirm your entry.

A

Hole depth ?

1 5

ENT

Enter the hole depth (DEPTH = – 15 mm).
Confirm your entry.

B

Pecking depth ?

ENT

5

Enter the pecking depth (PECKG = 5 mm).
Confirm your entry.

80 TNC 124

C

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

Dwell time ?

0

ENT

5

Enter the dwell time for chip breaking (DWELL = 0.5 s).
Confirm your entry.

Feed rate ?

8

Program blocks

0 BEGIN PGM 20 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+600 Tool-change position

3 X+30 Pre-positioning in the X axis
4 Y+20 Pre-positioning in the Y axis
5 TOOL CALL 8 Z Call the tool for pecking, such as tool 8, tool axis Z
6 S 1500 Spindle speed
7M 3 Spindle ON, clockwise

8 CYCL 1.0 PECKING Cycle data for Cycle 1.0 PECKING follow
9 CYCL 1.1 HEIGHT +50 Clearance height
10 CYCL 1.2 DIST 2 Setup clearance above the workpiece surface
11 CYCL 1.3 SURF + 0 Absolute coordinate of the workpiece surface
12 CYCL 1.4 DEPTH –15 Hole depth
13 CYCL 1.5 PECKG 5 Depth per infeed
14 CYCL 1.6 DWELL 0.5 Dwell time at bottom of hole
15 CYCL 1.7 F 80 Machining feed rate

16 CYCL CALL Cycle call

17 M 2 Stop program run, spindle STOP, coolant OFF

18 END PGM 20 MM End of program, program number, unit of measurement

ENT

0

Enter the feed rate for drilling (F = 80 mm/min).
Confirm your entry.

Cycle 1.0 PECKING is executed in the operating mode
PROGRAM RUN (see Chapter 10).

TNC 124 81

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

TAPPING

With Cycle 2.0 TAPPING you can cut right-hand and left-hand
threads.

No effect of the override controls during tapping

When Cycle 2.0 TAPPING is being run, the knobs for spindle
speed override control and feed rate override control are disabled.

Required floating tap holder

A floating tap holder is required for executing Cycle 2.0 TAPPING.
The floating tap holder compensates the tolerances for the pro­grammed feed rate F and the programmed spindle speed S.

Tapping right-hand and left-hand threads
Right-hand thread: Spindle ON with miscellaneous function M 3

Left-hand thread: Spindle ON with miscellaneous function M 4

Process

The tapping cycle is illustrated in Fig. 7.4 and Fig. 7.5.

I:

The TNC pre-positions the tool at setup clearance above the
workpiece surface.

II:

The tool drills to the end of thread at the feed rate F.

B

III:

When the tool reaches the end of thread, the direction of spindle
rotation is reversed. After the programmed dwell time the tool is re­tracted to clearance height.

IV:

Above the workpiece, the direction of spindle rotation is reversed
once again.

A

I

II

A

B

B

Calculating the feed rate F
Formula for calculation: F = S  p in [mm/min], where
S: Spindle speed in [rpm]
p: Pitch in [mm]

Input data for Cycle 2.0 TAPPING

 Clearance height - HEIGHT

Position in the tool axis at which the TNC can move the tool in
the working plane without damaging the workpiece.

 Setup clearance - DIST

The TNC advances the tool from clearance height to setup
clearance at rapid traverse.
Standard value: DIST = 4  thread pitch p

 Workpiece surface - SURF

Absolute coordinate of the workpiece surface

 Thread length - DEPTH

Distance between workpiece surface and end of thread.

 Dwell time - DWELL in [s]

A dwell time prevents wedging of the tool when retracted.
Further information is available from the machine manufacturer.
Standard value: DWELL = 0 to 0.5 s

 Feed rate - F in [mm/min]

Traversing speed of the tool during tapping

Fig. 7.4: Steps I and II in Cycle

III

A

B

Fig. 7.5: Steps III and IV in Cycle

2.0 TAPPING

A

2.0 TAPPING

IV

A

82 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

Programming example: Cycle 2.0 TAPPING

Right-hand thread
X coordinate of the hole: 30 mm
Y coordinate of the hole: 20 mm
Pitch p: 0.8 mm
Spindle speed S: 100 rpm
Clearance height HEIGHT: + 50 mm

Setup clearance DIST : 3 mm

A

Coordinate of the
workpiece surface SURF:0 mm

Thread depth DEPTH :  20 mm

B

Dwell time DWELL: 0.4 s
Feed rate F = S  p: 80 mm/min

Example: Entering Cycle 2.0 TAPPING into a part program

Operating mode: PROGRAMMING AND EDITING

20

A

B

Y

0

0

X

30

/

Page to the third soft-key row.

Select Cycle Definition.

Enter Cycle 2.0 TAPPING in a part program.

Clearance height ?

5

ENT

0

Enter the clearance height (HEIGHT = 50 mm).
Confirm your entry.

Setup clearance ?

ENT

3

Enter the setup clearance (DIST = 3 mm).
Confirm your entry.

Workpiece surface ?

ENT

0

Enter the coordinate of the workpiece surface (SURF = 0 mm).
Confirm your entry.

A

Hole depth ?

ENT

0

2

Enter the hole depth (DEPTH = – 20 mm).
Confirm your entry.

TNC 124 83

B

7 Drilling, Milling Cycles and Hole Patterns in Programs

Drilling Cycles in Programs

Dwell time ?

0

ENT

4

Enter the dwell time (DWELL = 0.4 s).
Confirm your entry.

Feed rate ?

8

Program blocks

0 BEGIN PGM 30 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+600 Tool-change position

3 X+30 Pre-positioning in the X axis
4 Y+20 Pre-positioning in the Y axis
5 TOOL CALL 4 Z Call the tool for tapping, such as tool 4, tool axis Z
6 S 100 Spindle speed
7M 3 Spindle ON, clockwise (right-hand thread)

8 CYCL 2.0 TAPPING Cycle data for Cycle 2.0 TAPPING follow
9 CYCL 2.1 HEIGHT +50 Clearance height
10 CYCL 2.2 DIST 3 Setup clearance above the workpiece surface
11 CYCL 2.3 SURF + 0 Absolute coordinate of the workpiece surface
12 CYCL 2.4 DEPTH –20 Hole depth (thread length)
13 CYCL 2.5 DWELL 0.4 Dwell time at the end of thread
14 CYCL 2.6 F 80 Machining feed rate

15 CYCL CALL Cycle call

16 M 2 Stop program run, spindle STOP, coolant OFF

17 END PGM 30 MM End of program, program number, unit of measurement

ENT

0

Enter the feed rate for tapping (F = 80 mm/min).
Confirm your entry.

Cycle 2.0 TAPPING is executed in the operating mode
PROGRAM RUN (see Chapter 10).

84 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole patterns in programs

The information for the hole patterns Circle Pattern and
Linear Pattern (see Chapter 4) can also be written to a pro-

gram.

Executing holes in hole patterns

The TNC either drills bore holes or tap holes at the hole positions in
the pattern. The bore hole or tap hole data, such as setup clear­ance and hole depth, must be programmed in a cycle.

The TNC then executes the holes according to the selected cycle
that is programmed before the hole pattern cycle.

Hole pattern graphics

The hole patterns in a program can be displayed graphically.

Programming example: Cycle 5.0 Circle Pattern (full circle)

Number of holes NO. :8
Center point coordinates: CCX = 50 mm

CCY = 50 mm
Bolt circle radius RAD: 20 mm
Starting angle between

X axis and first hole START: 30°

Hole data

A description of Cycle 1.0 Pecking
starts on page 79.

Clearance height HEIGHT: + 50 mm
Setup clearance DIST:2 mm
Coordinate of the

workpiece surface SURF:0 mm
Hole depth DEPTH:  15 mm
Pecking depth PECKG:5 mm
Dwell time DWELL: 0.5 s
Feed rate F: 80 mm/min

Example: Entering bolt hole circle data into a program

Operating mode: PROGRAMMING AND EDITING

50

Y

30°

R20

0

0

50

X

/

Page to the third soft-key row.

Select Cycle Definition.

Select Circle Pattern.
The soft-key row switches to a deeper level.

TNC 124 85

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole Patterns in Programs

Type of bolt circle ?

Select Full Circle. The TNC calculates the hole positions on a full circle.

Number of holes ?

ENT

8

Enter the number of holes (NO. = 8).
Confirm your entry.

Center point X ?

5

ENT

0

Enter the X coordinate of the bolt circle center (CCX = 50 mm).
Confirm your entry.

Center point Y ?

5

ENT

0

Enter the Y coordinate of the bolt circle center (CCY = 50 mm).
Confirm your entry.

Radius ?

2

ENT

0

Enter the radius of the bolt circle (RAD = 20 mm).
Confirm your entry.

Starting angle ?

3

ENT

0

Enter the starting angle from the X axis to the first hole
(START = 30°). Confirm your entry.

Type of hole ?

Choose Pecking for drilling bore holes at the hole positions in the pattern.

86 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole Patterns in Programs

Program blocks

0 BEGIN PGM 40 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+600 Tool-change position
3 TOOL CALL 3 Z Call the tool for drilling, for example tool 3, tool axis Z
4 S 100 Spindle speed
5M 3 Spindle ON, clockwise

6 CYCL 1.0 PECKING Cycle data for Cycle 1.0 PECKING follow
7 CYCL 1.1 HEIGHT +50 Clearance height
8 CYCL 1.2 DIST 2 Setup clearance above the workpiece surface
9 CYCL 1.3 SURF + 0 Absolute coordinate of the workpiece surface
10 CYCL 1.4 DEPTH –15 Hole depth
11 CYCL 1.5 PECKG 5 Depth per infeed
12 CYCL 1.6 DWELL 0.5 Dwell time at bottom of hole
13 CYCL 1.7 F 80 Machining feed rate

14 CYCL 5.0 FULL CIRCLE Cycle data for Cycle 5.0 FULL CIRCLE follow
15 CYCL 5.1 NO. 8 Number of holes
16 CYCL 5.2 CCX +50 X coordinate of the center of the bolt circle
17 CYCL 5.3 CCY +50 Y coordinate of the center of the bolt circle
18 CYCL 5.4 RAD 20 Radius
19 CYCL 5.5 START +30 Starting angle of first hole
20 CYCL 5.6 TYPE 1:PECK Drill bore holes

21 M 2 Stop program run, spindle STOP, coolant OFF

22 END PGM 40 MM End of program, program number, unit of measurement

For a circle segment (CYCL 6.0 CIRCLE SEGMENT)
you also enter the angle step (STEP) between the holes
(after the starting angle).

The bolt hole circle is then executed in the operating mode
PROGRAM RUN (see Chapter 10).

TNC 124 87

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole Patterns in Programs

Programming example: Cycle 7.0 Linear hole pattern

X coordinate of the first hole : POSX = 20 mm
Y coordinate of the first hole : POSY = 15 mm

1

1

Number of holes per row NO.HL:4
Hole spacing HLSPC:10mm
Angle between hole row

and X axis ANGLE: 18°
Number of rows NO.RW:3
Row spacing RWSPC:12mm

Hole data

A description of Cycle 1.0 Pecking
starts on page 79.

Clearance height HEIGHT:+ 50mm
Setup clearance DIST:2mm
Coordinate of the

workpiece surface SURF:0mm
Hole depth DEPTH: 15mm
Infeed depth PECKG:5mm
Dwell time DWELL: 0.5 s
Feed rate F: 80 mm/min

Example: Entering data for linear hole pattern into a program

Operating mode: PROGRAMMING AND EDITING

15

0

Y

10

1

12

18°

X

0

20

/

Page to the third soft-key row.

Select Cycle Definition.

Select Linear Pattern.

88 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole Patterns in Programs

1 s t h o l e X ?

2

ENT

0

Enter the X coordinate of hole (POSX = 20 mm).
Confirm your entry.

1 s t h o l e Y ?

1

ENT

5

Enter the Y coordinate of hole (POSY = 15 mm).
Confirm your entry.

Holes per row ?

ENT

4

Enter the number of holes per row (NO.HL = 4).
Confirm your entry.

Hole spacing ?

1

ENT

0

Enter the hole spacing (HLSPC = 10 mm).
Confirm your entry.

Angle ?

1

ENT

8

Enter the angle between the X axis and the rows of holes
(ANGLE = 18°). Confirm your entry.

1

1

Number of rows ?

ENT

3

Enter the number of rows (NO.RW = 3).
Confirm your entry.

Row spacing ?

1

ENT

2

Enter the row spacing (RWSPC = 12 mm).
Confirm your entry.

Type of hole ?

Choose Pecking for drilling bore holes at the hole positions in the pattern.

TNC 124 89

7 Drilling, Milling Cycles and Hole Patterns in Programs

Hole Patterns in Programs

Program blocks

0 BEGIN PGM 50 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+600 Tool-change position
3 TOOL CALL 5 Z Call the tool for pecking, such as tool 5, tool axis Z
4 S 1000 Spindle speed
5M 3 Spindle ON, clockwise

6 CYCL 1.0 PECKING Cycle data for Cycle 1.0 PECKING follow
7 CYCL 1.1 HEIGHT +50 Clearance height
8 CYCL 1.2 DIST 2 Setup clearance above the workpiece surface
9 CYCL 1.3 SURF + 0 Absolute coordinate of the workpiece surface
10 CYCL 1.4 DEPTH –15 Hole depth
11 CYCL 1.5 PECKG 5 Depth per infeed
12 CYCL 1.6 DWELL 0.5 Dwell time at bottom of hole
13 CYCL 1.7 F 80 Machining feed rate

14 CYCL 7.0 LINEAR HOLE PATTN Cycle data for Cycle 7.0 LINEAR HOLE PATTN follow
15 CYCL 7.1 POSX +20 X coordinate of first hole
16 CYCL 7.2 POSY +15 Y coordinate of first hole
17 CYCL 7.3 NO.HL 4 Number of holes per row
18 CYCL 7.4 HLSPC +10 Distance between holes on the row
19 CYCL 7.5 ANGLE +18 Angle between the rows and the X axis
20 CYCL 7.6 NO.RW 3 Number of rows
21 CYCL 7.7 RWSPC +12 Spacing between rows
22 CYCL 7.8 TYPE 1:PECK Pecking

23 M 2 Stop program run, spindle STOP, coolant OFF

24 END PGM 50 MM End of program, program number, unit of measurement

1

1

The hole pattern is then executed in the operating mode
PROGRAM RUN (see Chapter 10).

90 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Rectangular pockets in programs

The TNC makes it easier to clear out rectangular pockets. You
need only enter the dimensions of the pocket; the TNC calculates
the tool path for you.

Process

The cycle process is illustrated in Figures 7.6, 7.7 and 7.8.

I:

The TNC pre-positions the tool in the tool axis at the clearance

H

height
in the tool axis to the setup clearance

, moves it in the working plane to the pocket center, then

A

II:

The TNC drills at the pecking feed rate to the first pecking

C

depth

.

III:

The TNC clears out the pocket at the milling feed rate along the
path illustrated in Fig. 7.8 below (in this case with climb milling).

IV:

The pecking and the roughing process are repeated down to the
programmed depth
the tool in the pocket center back to the clearance height

Input data for Cycle 4.0 RECTANGULAR POCKET

 Clearance height  HEIGHT

The absolute position in the tool axis at with the tool can move
in the working plane without danger of collision.

 Setup clearance  DIST

The tool moves at rapid traverse from the clearance height to
the setup clearance.

 Workpiece surface  SURF

Absolute coordinate of the workpiece surface.

 Milling depth  DEPTH

Distance between workpiece surface and bottom of pocket.

 Pecking depth  PECKG

Infeed per drilling cut.

 Pecking feed rate  F

Tool traversing speed during pecking.

 Pocket center in X  POSX

Point in the longitudinal axis at which the pocket center is
located.

 Pocket center in Y  POSY

Point in the transverse axis at which the pocket center is
located.

 Side length in X  LNGTH X

Length of the pocket in the longitudinal axis.

 Side length in Y  LNGTH Y

Length of the pocket in the transverse axis.

 Milling feed rate  F

Traversing speed of the tool in the working plane.

 Direction DIRCTN

Input value 0: climb milling (Fig. 7.8: clockwise)
Input value 1: upcut milling (counterclockwise)

 Finishing allowance - ALLOW

Finishing allowance in the working plane.

B

. Then the TNC ends the cycle by moving

H

A

B

C

MX

MY

X

Y

I

Z

H

A

X

.

Fig. 7.6: Step I in Cycle

4.0 RECTANGULAR POCKET

II

H

.

Z

Fig. 7.7: Step II in Cycle

4.0 RECTANGULAR POCKET

C

B

X

III

X

MX

Y

Y

MY

Fig. 7.8: Step III in Cycle

4.0 RECTANGULAR POCKET

R

X

TNC 124 91

7 Drilling, Milling Cycles and Hole Patterns in Programs

Rectangular Pockets in Programs

Example: Cycle 4.0 RECTANGULAR POCKET

Clearance height: + 80 mm
Setup clearance: 2 mm

Workpiece surface: + 0 mm
Milling depth:  20 mm
Pecking depth: 7 mm
Pecking feed rate: 80 mm/min
Pocket center in X: 50 mm

Pocket center in Y: 40 mm
Side length in X: 80 mm
Side length in Y: 60 mm

Milling feed rate: 100 mm/min
Direction: 0: CLIMB

Finishing allowance: 0.5 mm

Example: Entering Cycle 4.0 RECTANGULAR POCKET

into a part program

Operating mode: PROGRAMMING AND EDITING

/

Page to the third soft-key row.

–20
–30

80
70

40

10

Z

0

X

Y

R10

0

0

10

50

90

X

100

Select Cycle Definition.

Enter Cycle 4.0 RECTANGULAR POCKET in a part program.

Clearance height ?

8

ENT

0

Enter the clearance height (HEIGHT = 80 mm).
Confirm your entry.

Setup clearance ?

ENT

2

Enter the setup clearance (DIST = 2 mm).
Confirm your entry.

Workpiece surface ?

ENT

0







Enter the coordinate of the workpiece surface (SURF = 0 mm).
Confirm your entry.

92 TNC 124

7 Drilling, Milling Cycles and Hole Patterns in Programs

Rectangular Pockets in Programs

Program blocks

0 BEGIN PGM 55 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+600 Tool-change position

3 X-100 Pre-positioning in the X axis
4 Y-100 Pre-positioning in the Y axis
5 TOOL CALL 7 Z Call the tool for pocket milling, such as tool 7, tool axis Z
6 S 800 Spindle speed
7M 3 Spindle ON, clockwise

8 CYCL 4.0 RECTANGULAR

POCKET Cycle data for Cycle 4.0 RECTANGULAR POCKET follow
9 CYCL 4.1 HEIGHT + 80 Clearance height
10 CYCL 4.2 DIST 2 Setup clearance above the workpiece surface
11 CYCL 4.3 SURF + 0 Absolute coordinate of the workpiece surface
12 CYCL 4.4 DEPTH – 20 Milling depth
13 CYCL 4.5 PECKG 7 Depth per infeed
14 CYCL 4.6 F 80 Pecking feed rate
15 CYCL 4.7 POSX + 50 Pocket center in X
16 CYCL 4.8 POSY + 40 Pocket center in Y
17 CYCL 4.9 LNGTHX 80 Side length X
18 CYCL 4.10 LNGTHY 60 Side length Y
19 CYCL 4.11 F 100 Milling feed rate
20 CYCL 4.12 DIRCTN 0: CLIMB Climb milling
21 CYCL 4.13 ALLOW 0.5 Finishing allowance

22 M 2 Stop program run, spindle STOP, coolant OFF
23 END PGM 55 MM End of program, program number, unit of measurement

Cycle 4.0 RECTANGULAR POCKET is executed in the operating mode
PROGRAM RUN (see Chapter 10).

TNC 124 93

8 Subprograms and Program Section Repeats

8
Subprograms and Program Section Repeats

Subprograms and program section repeats only need to be entered
once in the program. You can then run them up to 999 times.

Subprograms can be run at any point in the program, while program
section repeats are run several times in succession.

Inserting program marks (labels)

You identify subprograms and program section repeats with labels
(abbreviated in the program to LBL).

Labels 1 to 99

Labels 1 to 99 identify the beginning of a subprogram or a program
section which is to be repeated.

Label 0

Label 0 is used only to identify the end of a subprogram.

Label call

In the program, subprograms and program sections are called with
the command CALL LBL.

The command CALL LBL 0 is not allowed.

Subprograms:
After a CALL LBL block in the program, the TNC executes the
called subprogram.

Program section repeats:
The TNC repeats the program section located before the CALL LBL
block. You enter the number of repeats with the CALL LBL com-
mand.

Fig. 8.1: On-screen operating instructions

for subprogram (page 5 shown)

Nesting program sections

Subprograms and program section repeats can also be nested. For
example, a subprogram can in turn call another subprogram.

Maximum nesting depth: 8 l ev el s

Fig. 8.2: On-screen operating instructions

for program section repeats

(page 3 shown)

94 TNC 124

8 Subprograms and Program Section Repeats

Subprograms

Programming example: Subprogram for slots

Slot lengths: 20 mm + tool diameter
Slot depths:  10 mm

Slot diameters: 8 mm (= tool diameter)
Infeed point coordinates

1

Slot
Slot
Slot

: X = 20 mm Y = 10 mm

2

: X = 40 mm Y = 50 mm

3

: X = 60 mm Y = 40 mm

This example requires a center-cut end mill (ISO 1641)!

Example: Inserting label for subprogram

Operating mode: PROGRAMMING AND EDITING

/

Go to the second soft-key row.

Insert a label (LBL) for a subprogram.
The TNC offers the lowest available number.

Label number ?

50

40

10

Y

8

20

2

3

20

1

X

40

60

0

0

Accept the default label number.

or

Enter a label number (here, 1). Confirm your entry.
The current block now contains the label LBL 1.

or

1

ENT

ENT

The beginning of a subprogram (or a program section repeat) is now
marked with the label. Enter the program blocks for the subprogram
after the LBL block.

Label 0 (LBL 0) is used only to identify the end of a subprogram.

Example: Entering a subprogram call: CALL LBL

/

Go to the second soft-key row.

Call label.
The TNC offers the label number which was last set.

TNC 124 95

8 Subprograms and Program Section Repeats

Subprograms

Label number ?

ENT

or

1

ENT

Accept the default label number.

or

Enter a label number (here, 1). Confirm your entry.
The current block now contains the called label: CALL LBL 1.

For subprograms you can ignore the question Repeat REP ?.
Press the soft key to confirm that a subprogram is being called.

After the CALL LBL block in the operating mode PROGRAM RUN,
the TNC executes those blocks in the subprogram that are located
between the LBL block with the called number and the next block
containing LBL 0.

Note that the subprogram will be executed at least once even without
a CALL LBL block.

Program blocks

0 BEGIN PGM 60 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+20 Clearance height
3 X+20 R0 X coordinate infeed point slot
4 Y+10 R0 Y coordinate infeed point slot

1

1

5 TOOL CALL 7 Z Call tool data, here tool 7, tool axis Z
6 S 1000 Spindle speed
7M 3 Spindle ON, clockwise

8 CALL LBL 1 Call subprogram 1: execute blocks 17 to 23

9 X+40 R0 X coordinate infeed point slot
10 Y+50 R0 Y coordinate infeed point slot

2

2

11 CALL LBL 1 Call subprogram 1: execute blocks 17 to 23

12 X+60 R0 X coordinate infeed point slot
13 Y+40 R0 Y coordinate infeed point slot

3

3

14 CALL LBL 1 Call subprogram 1: execute blocks 17 to 23

15 Z+20 Clearance height
16 M 2 Stop program run, spindle STOP, coolant OFF

1 7 LBL 1 Start of subprogram 1
1 8 F 200 Machining feed rate during subprogram
19 Z–10 Infeed to slot depth
20 IY+20 R0 Mill slot
2 1 F 9999 High feed rate for retracting and pre-positioning
22 Z+2 Retract
2 3 LBL 0 End of subprogram 1

24 END PGM 60 MM End of program, program number, unit of measurement

96 TNC 124

8 Subprograms and Program Section Repeats

Program section repeats

A program section repeat is entered like a subprogram. The end of
the program section is identified simply by the command to repeat
the section.

Label 0 is therefore not set.

Display of the CALL LBL block with a program section repeat

The screen displays (for example): CALL LBL 1 REP 10 / 10 .

The two numbers with the slash between them indicate that this is a
program section repeat. The number in front of the slash is the
number of repeats you entered. The number behind the slash is the
number of repeats remaining to be performed.

Programming example: Program section repeat for slots

Slot lengths: 16 mm + tool diameter
Slot depths:  12 mm
Incremental offset

of the infeed point : 15 mm
Slot diameter: 6 mm (= tool diameter)
Infeed point coordinates

1

Slot

: X = 30 mm Y = 10 mm

70

55

40

Y

6

16

This example requires a center-cut end mill (ISO 1641)!

Example: Label for a program section repeat

Operating mode: PROGRAMMING AND EDITING

/

Go to the second soft-key row.

Insert a label for a program section repeat (LBL).
The TNC offers the lowest available label number as a default.

Label number ?

ENT

or

ENT

1

Enter the blocks for the program section repeat after the
LBL block.

Accept the default label number.

or

Enter a label number (here, 1). Confirm entry.
The current block now contains the set label: LBL 1.

25

10

1

0

0

30

X

TNC 124 97

8 Subprograms and Program Section Repeats

Program Section Repeats

Example: Entering a program section repeat: CALL LBL

/

Go to the second soft-key row.

Call label.
The TNC offers the label number that was last set.

Label number ?

ENT

or

1

ENT

Accept the default label number.

or

Enter a label number (here, 1). Confirm your entry.
The current block now contains the called label: CALL LBL 1.

Repeat REP ?

ENT

4

After a CALL LBL block in the operating mode PROGRAM RUN, the
TNC repeats those program blocks that are located behind the LBL
block with the called number and before the CALL LBL block.

Note that the program section will always be executed one more
time than the programmed number of repeats.

Enter the number of repeats (here, 4).
Confirm your entry.

Program blocks

0 BEGIN PGM 70 MM Start of program, program number, unit of measurement

1 F 9999 High feed rate for pre-positioning
2 Z+20 Clearance height
3 TOOL CALL 9 Z Call tool data, here tool 9, tool axis Z
4 S 1800 Spindle speed
5M 3 Spindle ON, clockwise

6 X+30 R0 X coordinate infeed point slot
7 Y+10 R0 Y coordinate infeed point slot

1

1

8 LBL 1 Start of program section 1
9 F 150 Machining feed rate during program section repeat
10 Z-12 Infeed
11 IX+16 R0 Mill slot
1 2 F 9999 High feed rate for retracting and pre-positioning
13 Z+2 Retract
14 IX-16 R0 Positioning in X
15 IY+15 R0 Positioning in Y
1 6 CALL LBL 1 REP 4 / 4 Repeat program section 1 four times

17 Z+20 Clearance height
18 M 2 Stop program run, spindle STOP, coolant OFF
19 END PGM 70 MM End of program, program number, unit of measurement

98 TNC 124

8 Subprograms and Program Section Repeats

NOTES

TNC 124 99

9 Transferring Files Over the Data Interface

9
Transferring Files Over the Data Interface

The TNC 124 features an RS-232-C interface for external data stor­age on a device such as the HEIDENHAIN FE 401 floppy disk unit or
a PC.
Programs, tool tables and datum tables can also be archived on dis­kette and loaded back into the TNC again as required.

Pin layout, wiring and connections for the data interface
are described on page 115 and in the Technical Manual
for the TNC 124.

Functions for data transfer

Function Soft key/Key

Directory of programs stored
in the TNC

Directory of programs stored
on the FE

Abort data transfer

 Toggle between FE and EXT
 Show further programs

Transferring a program into the TNC

Operating mode: PROGRAMMING AND EDITING

Select Program Manage.

Select Extern.

File number ?

5

If you are transferring programs from a PC into the TNC
(EXTsetting), the PC must send the programs.

100 TNC 124

Enter the program number (here, 5).

Select external device (for diskette unit or PC with HEIDENHAIN data transfer
software TNC.EXE use FE setting; for PC without TNC.EXE use EXT setting).

Press Start Input to transfer the program to the TNC.
The message Loading file: appears on the TNC screen.