Introduction to TopTurn CNC simulator turning Version 7.1

Mathematisch Technische 

Software-Entwicklung GmbH 

Introduction to TopTurn 

CNC simulator turning 

Version 7.1 

© MTS GmbH • Kaiserin-Augusta-Allee 101 • D-10553 Berlin • Tel.: +49 / 30 / 349 960 - 0 • Fax: +49 / 30 / 349 960 - 25

MTS – Introduction to TopTurn Version 7.1 

Introduction to TopTurn 

Version V7.1 

© MTS Mathematisch Technische Software-Entwicklung GmbH 

Kaiserin-Augusta-Allee 101 • D - 10553 Berlin • Tel.: (030) 349 960 0 • Fax: 349 960 25 

Berlin, 2006. 

Any form of reproduction, including photo-mechanical copies and copies in electronic form, requires our prior authorization. 

We are always grateful for improvement suggestions and reports on any errors detected 

Seite: 2 © MTS GmbH 2006


1.0. INTRODUCTION ...................................................................................................................................... 5 

1.1. HOW OPERATING ELEMENTS ARE REPRESENTED IN TOPTURN.................................................. 5 

1.2. STARTING OF TOPTURN....................................................................................................................... 6 

1.3. NOTES ON SETTING UP A CONFIGURATIONTYPE............................................................................ 7 

2.0. TOPTURN – THE CNC SIMULATOR TURNING .................................................................................... 8 

2.1. AUTOMATIC MODE ................................................................................................................................ 9 

2.2. INTERACTIVE MODE ............................................................................................................................ 10 

2.3. SINGLE BLOCK MODE......................................................................................................................... 11 

2.4. TOOL TRACING .................................................................................................................................... 12 

2.5. MEASURING AND INSPECTION.......................................................................................................... 13 

2.6. 3D REPRESENTATION AND SURFACE FINISH................................................................................. 14 

2.7. 2D REPRESENTATION......................................................................................................................... 15 

3.0. THE NC EDITOR.................................................................................................................................... 17 

3.1. SETUP SHEET....................................................................................................................................... 18 

3.2. KEYBOARD LAYOUT FOR NC EDITOR FUNCTIONS........................................................................ 19 

3.3. NC DIALOG PROGRAMMING .............................................................................................................. 20 

3.4. ADDITIONAL INFORMATION TO MTS NC EDITOR ........................................................................... 21 

4.0 THE “TURNING” SET-UP DIALOG........................................................................................................ 22 

4.1. OPEN THE DIALOG WINDOW AND ASSIGN A PROGRAM NAME .................................................... 22 

4.2. SELECT THE CLAMPING DEVICE AND CLAMPING CONFIGURATION.......................................... 22 

4.3. WERKSTÜCKMAßE UND NULLPUNKT DEFINIEREN ....................................................................... 23 

4.4. SELECT THE MACHINING TOOL SET ................................................................................................ 24 

4.5. PROGRAM FOR EXERCISES 01.DNC................................................................................................. 25 

5.0. SETUP MODE OVERVIEW.................................................................................................................... 26 

5.1. CLAMPING DEVICES, CLAMPING METHODS OF BLANK MATERIAL SHAPES............................ 26 

5.2. TOOL TURRETS, TOOL MOUNTINGS AND TOOLS........................................................................... 26 

5.3. TOOL LIBRARY..................................................................................................................................... 27 

5.4. AXIS MOTIONS IN SETUP MODE ........................................................................................................ 27 

6.0. PREPARATIONS FOR PROGRAMMING ............................................................................................. 28 

6.1. PRODUCTION PLANNING AND TECHNOLOGY ................................................................................ 29 

© MTS GmbH 2006 Seite: 3


6.2. SETUP FORM FOR “TURNING WORKPART 1” ................................................................................. 31 

6.3. PRODUCTION SHEET FOR „TURNING WORKPART 1” ................................................................... 32 

Sequence of machining steps........................................................................................................................ 32 

7.0. SETTING UP THE MACHINE ................................................................................................................ 33 

8.0. NC PROGRAMMING IN MTS PROGRAMMING KEY .......................................................................... 43 

8.1. INSIDE STRAIGHT ROUGHING CYCLE G81 ...................................................................................... 44 

8.2. DRILLING CYCLE G84.......................................................................................................................... 45 

8.3. OUTSIDE STRAIGHT ROUGHING CYCLE G81 .................................................................................. 46 

8.4. INSIDE STRAIGHT ROUGHING CYCLE G81 ...................................................................................... 46 

8.5. INSIDE FINISHING................................................................................................................................. 47 

8.6. OUTSIDE FINISHING............................................................................................................................. 47 

8.7. OUTSIDE THREAD-CUTTING CYCLE G31 ......................................................................................... 48 

8.8. OUTSIDE GROOVE-CUTTING CYCLE G79......................................................................................... 49 

8.9. INSIDE GROOVE-CUTTING.................................................................................................................. 50 

9.0. QUALITY CONTROL – MEASURING OF WORKPART....................................................................... 51 

10.0 APPENDICES ........................................................................................................................................ 52 

10.1. NC PROGRAM %3................................................................................................................................. 53 

10.2. WORKPART DRAWING ........................................................................................................................ 56 

10.3. WORKING TEMPLATES ....................................................................................................................... 57 

Tool data / magazine or turret positions ........................................................................................................ 57 

Sequence of machining steps........................................................................................................................ 58 

NC-Code ........................................................................................................................................................ 59 

10.4. NOTICE FOR ADMINISTRATING AND ORGANISING OF SETUP TURNING ................................... 60 

10.5. SYSTEM INFORMATION....................................................................................................................... 62 



1.0. Introduction 

The individual chapters of this manual explain the essential functions involved in operating and handling the 

system. The functions described here are also intended to give you a general idea of the system’s capabilities 

(as well as the possibilities offered for implementing dedicated training courses). 

These not only include the creation of NC programs and simulating and checking their quality, but also many 

other realistic ways of teaching the trainees basic CNC machine tool functions using computer support. 

The examples used in the simulation are available in the programming keys of all CNC control systems supplied 

by our company. 

Trainees are guided through system operation step-by-step, enabling them to learn the underlying principles 

and the operation of the CNC simulator in a very short time. 

After some introductory explanations, we will first show you how to set up the simulator according to a work plan 

and how to create a setup sheet. 

1.1. How operating elements are represented in TopTurn 

The operating elements and the meaning of their functions are shown by the simulator as 10 function buttons in 

a menu bar at the bottom of the screen corresponding to the function keys of a PC or control keyboard. 

Main menu: 

To activate the desired function, either move the mouse pointer to the respective function button and click on 

the leftt-hand mouse button , or press the appropriate function key … of the PC keyboard. This 

enables you to adapt system operation to your preferences. 

To help you follow the explanations more easily, the functions which you have to select from the menu 

structures are shown in the explanatory and instruction texts with a coloured or darker background, or are 

indicated by symbols representing PC keys. 

To begin with, you only need to carry out the individual steps as instructed. 

If the desired result is not achieved due to an input error, please observe the following notes: 

• You can return to the main menu or the start-up status of the simulator at any time by pressing the or 

key. Depending on how far down the menu tree you are, you may have to press the key several times. 

• To select or de-select functions, use the keys … . This may pull up a new menu. 

• Generally, a function is concluded or accepted by pressing . If you have navigated through several 

menus in order to select a specific function, you will have to exit each menu, one at a time by pressing 

or the appropriate number of times. This, too, will return you to the main menu. 

Instead of using the function keys the windows toolbar can be used for operation 



1.2. Starting of TopTurn 

Click on the Windows START button in the task bar, select the Programs folder and then (sofar you have not 

changed the folder name when installing the software) the MTS-CNC English folder to access the MTS 

programs TopTurn, TopMill or TopCAM. 

The respective documentation / training manuals are stored in PDF format in the Help subfolder. 

If you start TOPCAM, the start-up menu will offer you the following software modules for selection: 

TopCAM 

A CAD system with integrated NC programming for 

turning/lathe work with up to 5 axes and milling work 

with 3 axes 

TopTurn 

NC programming module, either control-systemspecific 

or of neutral ISO control system type, with 

simulation and collision detection; optionally available 

with opposite spindle and up to 7 axes 

TopMill 

NC programming module, either control-systemspecific 

or of neutral ISO control system type, with 

simulation and collision detection in 3 axes 

When you start up the TURNING software for the first time, an MTS configuration group with the MTS 

programming key will always be active:: 

MTS TM -___.___.042x0500x1000 x MTS TM CONTROL 

If you have not purchased the MTS programming key, which is independent of the type of control system, but 

have a turning/lathe work control system using e. g. PAL94 command codes or SINUMERIK 820T, the Start 

Turning button is not active after you have installed the software. In this case, you first have to select a 

corresponding configuration group. This activates the Start Turning button. This configuration group selection 

is memorized for subsequent program starts. 

Click left hand mouse button to select 

a configuration group 

Info on the machine tool axes, tailstock 

in the selected configuration 



1.3. Notes on setting up a configurationtype 

You can skip over this chapter when first learning to operate the software. 

The name of a configuration group is always related to a particular combination of machine tool and control 

system configurations. These are saved and managed by the Configuration Administration. For instance, a lathe 

will be configured according to the manufacturer’s instructions. The definitive properties will include the 

machining space, tool travel ranges, tool magazine type and the tool positions, number of NC axes, whether a 

opposite spindle, headstock or tailstock are installed etc. 

The control configuration will comprise the CNC programming syntax, the allocation of the optional 

postprocessor and the control settings. 

A postprocessor is always needed for translating an MTS 

or PAL program into a specific control system code. The 

same as with the programming key, this will be activated 

after the target control system has been selected. 

Which of these modules are available will depend on which software level you have purchased. You can add 

modules whenever required. 

In the following illustration, both modules, i. e. the programming key and the postprocessor are available. The 

Postprocessor and Start turning buttons are therefore enabled and activated. 

Driving tool 5 axes machining (X, Z, Y, B, C) main 

spindle and Counterspindel 

Programming key of the control Sinumerik 810D 

with 5 axes simulation 

Cycle postprocessor for translating programs into 

the Sinumerik 810 D NC code for 5 axes 

Transfer of the NC data between the PC AND THE nc 

machine tool 

If you have not purchased a programming key for your postprocessor, then the 

enabled. 

button is not 

Before continuing, re-check the active configuration group. 

Now start the CNC simulator by double-clicking on the button. The simulator will either use the 

MTS TM -___.___.042x0500x1000 x MTS TM CONTROL 

configuration group as in the example bevor, or the one which you have purchased. 



2.0. TopTurn – the CNC simulator turning 

The CNC simulator has three different operating modes: 

NC Editor 

Automatic mode 

Setup mode 

Setup dialog 

For teaching purposes, it is best to start with the 

get familiar with the various types of simulation. 

. This means that the trainee will first 

We switch the simulator to 3D 

Let us start by explaining some features of the initial screen display. 

The power-on state of the CNC simulator is 

determined by a setup sheet. This describes a specific 

simulator setup which is determined by the following 

components: 

• a lathe chuck with clamping jaws, 

• the workpiece blank / blank material and 

• tooling setup with tool positions in the tool 

magazine. 

The start setup sheet is stored as header in an NC 

program. In each control system, it is stored under the 

program administration and is named 

. The user can adapt this setup 

sheet individually or can change its name of in the 

respective control system configuration. 

To activate the program and set up 

the system, select by mouse pointer 

or press the key. This returns the simulator to its 

original power-on state. 

Header of the setup sheet as are 

shown by the NC editor. 

For further information on setup sheets, refer to Chapter 3.1, 



2.1. Automatic mode 

We want to run an NC program on a CNC machine tool. To enable this process, the program first has to be 

loaded into the control system’s memory. The following description illustrates the individual steps required to 

operate the MTS system in this mode. 

Press key , or select the button to open the NC Program Administration, which will 

display a list of all NC programs for this control system 

Double-click on the file name to load 

this NC Program into the machine tool memory for further processing. 

With mouse click you can activate further functions of the explorer: 

e.g. copy program to diskette, 

delete, rename etc.. 

In our example, the program has been selected. Press to confirm the 

action. The system will display a new menu. This offers you four different types of simulation. We shall start 

byselecting automatic mode . 

Automatic mode 

Interactive mode 

Single block 

Tool tracing 

To start the simulation in automatic mode, press the key. The CNC program currently loaded into the 

machine memory is run automatically from the first to the last block. 

The right-hand pane shows important system 

information on the operating state of the virtual CNC 

lathe: 

• current co-ordinates of the X and Z axis (as well 

as of the optional additional axes), 

• cutting speed, rotation speed, tool feed, 

tool number, 

• direction of spindle rotation, machining time, 

• active G code and 

• override & runtime 

The lower section of the simulation window shows a 

section of the program with the NC block currently 

being processed by TopTurn 



2.2. Interactive mode 

Interactive mode, called up by pressing the key, enables the user to write, tocreate, edit and run an NC 

program in dialog with the software. The CNC simulator runs the NC program block-by-block. The program can 

be corrected at any time. After being executed by the simulator, any block can be rejected so that you can reedit 

it and then re-run on the simulator. During this process, the workpiece will be continuously updated, or, if 

the block is rejected, the workpiece will be returned to its former condition. 

Let us run the NC program in . 

Initially, the program administration is opened: 

Double-click left on the programm in 

order to transfer it to the machine program memory. 

This will get the program wunning in interactive mode. After editing and confirmation every NC block will be 

simulated and this block will be represented for editing after simulation. 

Execute an NC block: 

Accept NC block [Y/N] 

Execute an NC block 


In this operating mode, the NC code can be edited 

again as follows: 

Reject the block by pressing the or . Using 

the keyboard, edit the current block. 


Instead of you may press also . 



If you wish to change the speed at which the simulation is run, use the function . This 

function is available on all modern machine tools, both during machining work and during tooling and set-up 

(zero-position scratching, setting zero co-ordinates). 

To access the various functions for altering the time taken to run the simulation, press the button. Try using the individual options offered in the menu bar. To apply your settings, press key . 

You may change the settings at any time. 

Important: The override setting affects the calculated machining time. As opposed to this, the slow-motion and 

test run on/off functions do not affect calculated machining times. 

2.3. Single block mode 

The function is used when running in Automatic mode and requires the operator to confirm the 

execution of each NC block or record individually. 

The NC-Program should be executed in the operating mode 

. 

Click on or press the 

with to run the NC block. 

or confirm 

Note: 

You can switch over between the simulation modes Automatic mode, Single block and Interactive mode 

even after simulation of an NC program has been started. 



2.4. Tool tracing 

The function is used to display the tool travel paths described by the selected NC program e. g. 

. 

The program is run and the programmed 3D tool tracing of the the tool tip are displayed graphically and each 

tool is shown in different colors. 

Careful and precise evaluation of the programmed tool movements in rapid speed and subsequent correction of 

the NC program can lead to considerable reductions in manufacturing times. 

With the toolbar you can manipulate the graphic display of the tool tracing and you can also alternatively insert 

the workpart. 

Note: 

The currently selected NC program can be run in any of the simulation modes. 

 

 

 

 

If the setup sheet interpreter is activated, every time an NC program is started the CNC simulator will be set up 

according to the setup sheet in the header of the NC program. This has the advantage that the original 

workpiece blank is always placed back on the machine whenever the program is restarted. 



2.5. Measuring and inspection 

Irrespective of the simulation mode you have selected and the NC code already processed, you can use the 

button at any time to call up functions for displaying and checking the workpiece in its actual 

state. 

The button gives you access to simulator functions relevant to the topic of quality analysis 

and checking of your own work. 

The trainee is offered a comprehensive range of functions for checking the results of the work he/she has done. 

The function , or is used to make a “specifications/as is” 

comparison in order to check whether the programmed workpiece contour really matches the drawing 

specifications. 

Now try using the various functions offered, e. g. to examine the effect of the cutting tool radius compensation 

on the workpiece contours by measuring the workpiece alternately with compensation on and off. 

Exit with . 



2.6. 3D representation and surface finish 

The viewing angle, viewer distance and zoom factor, 

as well as a cut-away section angle, can be set to suit 

your requirements. In the sections menu, you can 

define the cut-away segment.. 

To obtain a full-screen display, press + , you 

can only switch back to the normal user interface by 

pressing the key. With the toolbar you can also 

obtain a permanent 3D representation of the selected 

tool 

Roughness depth analyse 

, calls up a function to analyse the workpiece 

contour by individual contour entities, one at a time. 

Using the cutting tool geometry and feed, the system 

will calculate and display the surface and determine 

the roughness depth average value. To obtain more 

detailed information on the currently selected contour 

entity, press keys and . 



2.7. 2D representation 

The functions accessed by the or 

three ways: 

key allow you to modify the on-screen display mode in 

• Workpiece views 

• Zoom functions 

• NC code line display 

To apply the setting changes made in the , press the key; to reject them, press . 

A rectangular zoom section will be defined by the two 

points of a section diagonal.To define a zoom section, 

click with the left-hand mouse button on one edge 

of the rectangle and drag the mouse pointer to the 

diagonally opposite corner of the rectangle.. 

You can always switch back instantly to the overall 

view of the machining space or to a standard display 

related to the workpiece blank. 

After selecting the new display mode, exit the menu by clicking on the button or by pressing . The 

selected view mode will remain in force until it is changed again. (Except when the NC program itself calls up a 

window setting). The simulator will return to the function which was selected at the time you called up the 

functions. 



The following workpiece geometry views can be selected: outside view, half-section (top or bottom half) and full 

longitudinal section. 

Outside view display 

Display showing bottom half-section 

Display showing full section 

The button or key calls up a 

function which you can use to define the number of 

lines of NC code to be displayed in automatic mode. 



3.0. The NC Editor 

The initial menu of the NC editor provides access to the following functions: 

• Edit the current NC program 

• not assigned 

• Select an NC program from the Administration in order to edit it, or to create a new program 

• not assigned 

• Print the NC program 

• Transfer the NC program to the machine tool in DNC mode 

• Return to setup mode 

• Return to automatic mode 

• 

As you already learned in the section on , you can select a program or create a new 

program using the file selection dialog. 

This offers various ways of opening or creating a program. Press or click on , and enter 

a program name. 

If a program with this name already exists, it will be opened for editing, if not, you will be shown a message: 

“Program does not exist! Create program [Y/N]?”. In the latter case, press the [Y] key to create a new 

program and [N] [to abort. 

You can also select a program by clicking or pressing . The selected name is then 

copied into the simulator’s status bar when the dialog window is closed. You can subsequently open it with 

or by using other functions. 

The NC program is to be opened for viewing. It contains all 

required information, from the setup data for simulation 

right down to the NC code of the program. 

After you have marked the NC program with a single 

left mouse click , you can click on the right-hand 

mouse button to call up further supplementary 

functions. 



3.1. Setup sheet 

A setup sheet stored as header of an NC program always has the same structure. It comprises the following 

groups: 

• Machine tool and control system configuration names, 

• Workpiece blank and geometry 

• Clamping devices and their positioning 

• Active tool in the machining position 

• Tools in the tool magazine, tool positions including tool correction values 

In the main menu, click on or press 

in order to access the setup form menu. 

After the simulator was set-up in setup mode you can save this setup in a respective setup sheet: 

Press and enter a program name. 

Setup sheet information 

• () Beginning and end marks for the setup sheet interpreter 

• ( Setup sheet line which is to be processed by the interpreter 

• (( Comments, these are not to be processed by the interpreter 

When you create a new setup sheet, the command (meaning “end of program”) will be the only NC line 

to be added to the setup sheet. Without the error message “unanticipated end of program” will be 

displayed when you are working in automatic mode or when the setup sheet is being used as a startup setup 

sheet. 



3.2. Keyboard layout for NC editor functions 

The section of the program that can currently be edited is always shown between two horizontal rules. To select 

a word, use the cursor key . You can change, delete or write new code as you wish. 

Confirm and conclude your entries by pressing the 

key. 

Browse a page at a time 

Browse block by block 

or 

or 

Insert a line: + 

Delete a line: + 

Inset a word: 

Delete a word: 

• Link programs 

• Group operation 

• Renumber the NC program 

To insert another NC program in front of the currently selected line, call up the appropriate function by pressing 

the key or clicking on on . This is an important function that is needed for creating 

modification copies, for instance. 

The group operation function, called up by pressing the key, enables you to mark a block of multiple 

complete lines, including the beginning and end marks, and then carry out operations such as shift, copy or 

delete block. 

The Renumber functions called up by pressing enable you to renumber the NC program from a first 

program number up to another program number by specifying a start number and a numbering increment. 



3.3. NC dialog programming 

To enter dialog programming mode, press the key or click on . This is a universal MTS 

software function which can be adapted to all types of NC controls. When you press the key, the current 

work line is analyzed to locate commands for which a dialog screen is available. If a fitting dialog screen is 

found, it will be displayed and the respective input parameter values shown in the dialog screen. 

Dialog screen 

List of contentc 

In the above example, this is an MTS straight roughing machining cycle call G81 with three addresses: X, Z and 

I, as well as supplementary parameters which have not yet been assigned values in the example. You can 

change the address values and also add values from the dialog screen. To enter all values into the actual NC 

program, click on the button. 

If no key word is found, the dialog programming module will call up the list of contents showing all available 

commands, allowing you to select one of these by clicking on “Parameter” . The corresponding dialog 

screen is then opened so that you can enter the desired values. Click on to confirm your input. The 

corresponding new NC code line will replace the line originally selected. If you have accessed the end of the NC 

program, a new line will be appended to the existing NC program. (This operation also applies to multiple-line 

NC programming commands, provided that the selected NC control system supports these). 

You can either enter a numerical value, or in the case of switch functions, select the respective function setting. 

In this procedure, the permissible value ranges are checked and a distinction is made between mandatory 

addresses and optional addresses. You also have the option of using an alternative address combination, e. g. 

defining an arc by I and K instead of by the radius. 

In dialog programming of more complex cycles, you 

can also call up the corresponding Windows help 

screens if available for this specific control.. 



3.4. Additional information to MTS NC editor 

The function key Dialog/Help can also be activated by pressing the key combination + , or by clicking 

on with the right mouse button , to get into a help box for tool magazine informations. 

Enter T in the input field and confirm with 

magazine equipment of the CNC simulator. 

, then you will get the information display of the actual tool 

Here you can get additional informations about the 

marked tool. 

Note: 

The modification of the tool equipment is not possible 

in this helpscreen. 

Press 

to leave this tool magazine information. 



4.0 The “turning” set-up dialog 

Four simple steps to create a setup sheet 

The set-up dialog assists you to create a setup sheet for a new programming task quickly. First, the clamping 

device - e.g a chuck and jaws - is selected. Then the workpiece - a cylinder or a pipe - is defined, the workpiece 

origin is specified and the new program is completed by adding a suitable set of tools. After the procedure is 

finished, the controls read in the setup sheet in the form of a program header, and the user can immediately 

start to key in the new program. 

4.1. Open the dialog window and assign a program name 

To open the set-up dialog, press key . Enter a 

new name for the CNC program you wish to create, 

e. g. "Exercise 01" and then open the program 

4.2. Select the clamping device and clamping configuration 

Select the clamping device. 

Explanation: 

7 different clamping devices are offered for selection. A clamping depth definition is not necessary in case of 

peak clamping. In this case the workpart must have a centering. Is the workpart a pipe, an external and internal 

diameter must be entered. 



Select the clamping device 

KFD-HS 130 min.46 max.118 Et=18 

Determine the clamping depth of the workpart 

Input: 18 mm 

Next open the tab: 

Blank/Zero point 

Explanation: 

Observe the range of values in the display field. If a value cannot be evaluated, then it is shown in red in the 

input field and is not processed. 

Selection of the vise corresponds to the standard in the „Turning“ clamping device library. 


KFD-HS 130 describes the lathe chuck, min. 46 til max. 118 mm describes the opening range of the respective 

jaw and Et=18 mm is the maximum clamping depth possible for a workpart. 

4.3. Werkstückmaße und Nullpunkt definieren 

Specify the workpart dimensions: 

Input length = 120 mm, 

Input width = 60 mm 

and enter a zero point shift from front side into the 

material. 

Input 

Z= -2 mm 


Tools 

Explanation: 

The position of the workpiece origin can be specified by selecting a value in the center input field of this tab. 

A total of 2 possible workpart origins are offered for selection: right or left from the workpart. 

Additionally this point can be moved incrementally in Z ± direction from the selected point. 



4.4. Select the machining tool set 

Select the tool set e.g. 94-03 and inform about the 

tooling of the turret magazine. 


Compensation value 

Explanation: 

The tool set determines which tools are to be made available on the setup sheet. 

You find here a list of compensation values. 

Explanation: 

Select the compensation values tab in order to obtain 

more detailed tool information. 

Confirm your input by clicking on the button to 

create the new setup sheet. This is then read in by the 

CNC machine tool in Automatic mode – Interactive 

programming – and you can then start programming 

the machine. 

The CNC program can be created immediately. 

The machine origin (zero point) specified in the dilaog 

is entered at the bottom of the setup sheet and can 

then be activated with the assigned command, e.g. 

G54. 

Below is an excerpt from the setup sheet: 

( 

( WORKPART ZERO-POINT 

( G54 X200.000 Y+150.000 Z+105.000 



4.5. Program for exercises 01.dnc 

() 

(( 06.04.2006 16:57 

( 

( CONFIGURATION 

( MACHINE MTS01 TM-016_-R1_-060x0646x0920 

( CONTROL MTS TM01 

( 

( PART 

( CYLINDER D+060.000 L+120.000 

( 

( MAIN SPINDLE WITH WORKPART 

( CHUCK KFD-HS 130 

( STEP JAW HM-110_130-02.001 

( TYPE OF CHUCK EXTERNAL CHUCK OUTSIDE STEP JAW 

( CHUCKING DEPTH E18.000 

(( Right side of the part: Z+230.000 

( 

( TOOLS 

( T01 "DIN69880 V 30\Left corner tool\CL-SCLCL-2020 L 1208 ISO30" 

( T02 "DIN69880 V 30\Left corner tool\CL-SVACL-2020 L 1604 ISO30" 

( T03 "DIN69880 V 30\Left corner tool\CL-MTJNL-2020 L 1608 ISO30" 

( T04 "DIN69880 V 30\Round horizontal\CT-SRDCN-2016 L 0603 ISO30" 

( T05 "DIN69880 V 30\Left corner tool\CL-SDJCL-2020 L 1208 ISO30" 

( T06 "DIN69880 V 30\Recessing tool\EA-SGTFL-2012 L 02.5-0 ISO30" 

( T07 "DIN69880 V 30\Left threading tool\TL-LHTR-2020 R 60 1.50 ISO30" 


( T09 "DIN69880 V 30\Left corner tool\CL-SVJCL-2020 L 1604 ISO30" 

( T10 "DIN69880 V 30\Twist drill\DR-18.00 130 R HSS ISO30" 

( T11 EMPTY 

( T12 EMPTY 


( T14 "DIN69880 V 30\Recessing tool\ER-SGTFL-1212 L 01.6-0 ISO30" 

( 

( TOOL COMPENSATION 

( D01 T01 Q3 R0.800 X+070.0 Z+045.000 G000.000 E005.005 I-0.800 K-000.800 A+004.375 L011.855 N01 


( D03 T03 Q3 R0.800 X+070.0 Z+045.000 G000.000 E027.130 I-0.800 K-000.800 A+002.372 L015.678 N01 

( D04 T04 Q8 R3.000 X+070.0 Z+034.000 G006.000 E090.000 I-3.000 K+000.000 A+000.000 L003.000 N01 






( D10 T10 Q7 R0.000 X+000.0 Z+204.000 G018.000 E059.000 I+0.000 K+000.000 A+000.000 L000.000 N01 





( 

( WORKPART ZEROPOINTS 


( G54 X000.000 Z+228.000 

( 

() 

N0010 G54 



5.0. Setup mode overview 

The setup mode integrated into the TopTurn has a very wide function range. The following chapters provide a 

brief synopsis of the various options offered. 

5.1. Clamping devices, clamping methods of blank material shapes 

5.2. Tool turrets, tool mountings and tools 

Tool length compensation 

1.Ouadrant: K= R I= R 

2.Ouadrant: K=-R I= R 

3.Ouadrant: K=-R I=-R 

4.Ouadrant: K= R I=-R 

5.Ouadrant: K= R I= 0 

6.Ouadrant: K= 0 I= R 

7.Ouadrant: K=-R I= 0 

8.Ouadrant: K= 0 I=-R 

P = Tool holder reference point 

B1 = Length compensation in X 

A1 = Length compensation in Z 

F1 = Cutting radius 

F1 gives the values for I and K 

E1 = Value for I 

D1 = Value for K 



5.3. Tool library 

Currently, the software handles about 700 turning tools in 20 tool types (extendable by the user). 

5.4. Axis motions in setup mode 

Motion control keys: 

or 

or 

move along Z axis in feedrate 

move along X axis in feedrate 

+ or move along Z axis in rapid speed 

+ or move along X axis in rapid speed 

To move the tool turret around in the machining space, press the respective motion control keys just as on a 

real machine tool. The workpiece coordinate origin can also be determined by zero-point scratching. 

With the technology menu, or the direct hot-keys: 

switch spindle 3, 4 or 5, lubricant 7, 8 or 9 

rotation speed 1000 

feed rate 0.220 

turret tool position 0202 

you can set the correct speed, feed, tool, spindle and machining lubricant by numerical input 



6.0. Preparations for programming 

Before starting to write an NC program, you must study the drawings and production specifications carefully. As 

soon as all the information required for creating a program is available, you can start planning the individual 

machining steps. It is important to take into consideration which machine tool the respective workpiece is to be 

produced on and which tools and clamping devices are available on that machine tool. 

Appendix 1 contains a complete drawing of the part (“Drehteil 1”, page ) used in our example. 

• Analyze the workshop drawing 

• Fixing the work plan 

• Select the clamping devices and the required tools (setup sheet) 

• Write the NC program 

study 

work order 

study 

workshop drawing 

tools 

programmer 

clamping 

devices 

work plan 

set-up form 

program sheet 

Typical work preparation and planning forms 



6.1. Production planning and technology 

1 

Machining step 

Determine 

Blank 

dimensions 

Type of tool, position in turret 

cutting data 

Calinder D: 80 mm L: 122 mm 

Material: AlMg1 

Chuck: KFD-HS 130 

Clamp blank Chuck jaws: HM-110_130-02.001 

2 Determine 

origin of Clamping depth: 18.0 mm 

workpiece 

coordinates 

3 

4 Facing LEFT HANDED CORNER CUTTER 

CL-SCLCL-2020/L/1208 ISO30 

Machining step diagram 

T0101 G96 S260 M04 

G95 F0.250 M08 

5 Straight 

roughing 

external profile 

LEFT HANDED CORNER CUTTER 

CL-SCLCL-2020/L/1208 ISO30 

T0101 G96 S260 M04 

G95 F0.350 M08 

6 Drilling TWIST DRILL 

DR-18.00/130/R/HSS ISO30 

T0606 G97 S1200 M03 

G95 F0.220 M08 

7 Straight 

roughing 

internal profile 

BORING TOOL (POSTAXIAL) 

BI-SCAAL-1010/L/0604 ISO30 

T0808 G96 S220 M04 

G95 F0.250 M08 



Production planning (continued) 

Machining step 

6 Finishing 

internal profile 

Type of tool, position in turret 

cutting data 

BORING TOOL (POSTAXIAL) 

BI-SCAAL-1010/L/0604 ISO30 

Machining step diagram 

T1010 G96 S300 M04 

G95 F0.100 M08 

7 Finishing 

external profile 

LEFT HANDED CORNER CUTTER 

CL-SVJCL-2020/L/1604 ISO30 

T0202 G96 S360 M04 

G95 F0.100 M08 

8 External 

Threading 

LEFT HANDED THREADING TOOL 

TL-LHTR-2020/R/60/1.50 ISO30 

T0303 G97 S1000 M03 

G95 F1.5 M08 

9 Cutting three 

external 

grooves 

EXTERNAL RECESSING TOOL7 

RI-GHILL-1013/L/01.10 ISO30 

T0404 G97 S1000 M04 

G95 F0.150 M08 

10 Cutting internal 

groove 

INSIDE RECESSING TOOL (POSTAXIAL) 

RI-GHILL-1013/L/01.10 ISO30 

T1212 G97 S01000 M04 

G95 F000.150 M08 

The setup sheet is to be compiled on the basis of this work plan. 



6.2. Setup form for “Turning workpart 1” 

CNC 

Turning 

Setup Sheet 

Mathematisch Technische Software-Entwicklung GmbH Datum : 

Program No. Turning workpart 1 

Programmer MTS 

Drawings No. 2704 

Designation Turning workpart 1 

Material: AlMg1 

Raw part/blank 80 x 122 

Clamping mode: Inside 

Clamping device: Chuck 

Clamping depth back stop 18 mm 

Tailstock position: 800 

Other info: 

MTS TM 

Tool data / magazine or turret positions 

Station Tool designation Tool File No. Compensation data Ag. 

01 LEFT HANDED CORNER 

CUTTER 

CL-SCLCL-2020/L/1208 ISO30 X 60,0 

Z 43,0 

06 TWIST DRILL DR-18.00/130/R/HSS ISO30 X 0,0 

Z 210,0 

08 BORING TOOL (POSTAXIAL) BI-SCAAL-1010/L/0604 ISO30 X –6,77 

Z 160,0 

10 BORING TOOL (POSTAXIAL) BI-SCAAL-1010/L/0604 ISO30 X –6,77 

Z 160,0 

02 LEFT HANDED CORNER 

CUTTER 

03 LEFT HANDED THREADING 

TOOL 

04 EXTERNAL RECESSING 

TOOL 

12 INSIDE RECESSING TOOL 

(POSTAXIAL) 

CL-SVJCL-2020/L/1604 ISO30 X 70,0 

Z 43,0 

TL-LHTR-2020/R/60/1.50 ISO30 X 70,0 

Z 38,783 

ER-SGTFL-1212/L/01.8-0 ISO30 X 60,0 

Z 40,2 

RI-GHILL-1013/L/01.10 ISO30 X –11,5 

Z 125,9 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

R 0,8 

Quadr. 7 

R 0,0 

Quadr. 7 

R 0,4 

Quadr. 2 

R 0,4 

Quadr. 2 

R 0,4 

Quadr. 3 

R 0,217 

Quadr. 8 

R 0,160 

Quadr. 3 

R 0,1 

Quadr. 2 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

01 

02 

03 

04 

05 

06 

07 

08 

09 



6.3. Production sheet for „Turning workpart 1” 


Turning 

Production Sheet 


Program No . Turning workpart 1 

Programmer MTS 

Drawings No. 2704 

Designation Turning workpart 

Material AlMg1 

Raw part/blank 80 x 122 

Steuerung 

MTS TM 

Sequence of machining steps 

Nr. Machining step NC programming code Tool Cutting data 

position 

01 Facing G01 T01 F 0,25 N 

V c 260 

02 Straight roughing external profile G81 Straight roughing cycle T01 F 0,35 N 

V c 260 

03 Drilling G84 Drilling cycle T06 F 0,22 N 1200 

V c 

04 Straight roughing internal profile G81 Straight roughing cycle T08 F 0,25 N 

V c 220 

05 Finishing internal profile G41 G01 G02 G03 

G23 

T10 F 0,10 N 

V c 300 

06 Finishing external profile G42 G01 G02 G03 G85 

G23 

T02 F 0,10 N 

V c 300 

07 External threading G31 threading cycle T03 F 1,5 N1000 

V c 

08 Cutting three external grooves G79 grooving cycle T04 F 0,15 N1000 

V c 

09 Cutting internal groove G01 T12 F 0,10 N1000 

V c 

10 F N 

V c 

11 

12 F N 

V c 

13 F N 

V c 

14 F N 

V c 

15 F N 

V c 

16 F n 

V c 

17 F n 

V c 

18 F n 

V c 



7.0. Setting up the machine 

This chapter explains how to set up the CNC simulator for an exercise. This involves the following steps: 

• Selecting a blank, blank material, the clamping device and clamping method, clamping device changes 

• Assigning tools to tool turret positions and creating new tool data 

• Generating the setup sheet 

Exercise: 

A cylindrical aluminium alloy (AlMg1) blank, 80 x 122 mm is to be clamped against a back stop (18 mm) in a jaw 

chuck. In the setup mode menu, click on or press to select the workpiece/clamping menu. 

First select the desired material from the material table by pressing , then enter the blank geometry – a 

cylinder in our example. (However, material selection is not mandatory on the CNC simulator). 

Select the material group 

Select the material and press 

to confirm. 

Enter the dimensions of the blank in the top right-hand 

input fields: 

• Enter the cylinder geometry data: 

In filed D: enter : 80 

im field L: enter : 122 

To confirm your entries for the workpiece blank and 

register, press 

Information to the material AlMg1 

You have now defined the blank, the next step is to 

clamp it on the machine tool. 



To change clamping mode, press or click left 

The coloured frame marks the currently selected type. 

To confirm your selection, press .. 

The last set-up to be used determines the currently 

suggested clamping method. As the current jaws only 

permit a maximum clamping depth of 15…16 mm, a 

new chuck combination must be set up on the 

machine. 

To access the chuck menu, press . 

Here again, you may change the clamping method for your workpiece. In our example, this is not necessary 

To accept the selected clamping method, press 

call up the chuck device library. 

to 

First select a suitable lathe chuck. 

Open the lathe chuck library. 

Clamping and chuck devices are stored, by name, in a special library. You can modify these in order to comply 

with the tooling available in the respective workshop. 



Click on to select the required item in the library 

KFD-HS 130, then press to confirm. 

Next, you must select suitable stepped jaws. 

Chuck jaw selection, explanation of designations inside 

the name: 

HM 

(hard alloy) 

110_130 (suitatble 

for the chuck and blank diameter) 

-02 (number of Steps in the jaw) 

-001 (serial number) 

With this, you have equipped your machine tool with a 

new chuck with stepped jaws. 

You can still make changes at any time. The other 

clamping devices are released in relation to the 

method of clamping selected before. 

Press in order to install the combination on the 

simulator. 

Press 

in order to select type HM-110_130-02.001 

Of course, you can also define other chucks and stepped jaws as you wish. 



Now the workpiece blank has to be clamped in the 

chuck. 

Press in order to select the main spindle for 

clamping the workpiece. 

Now clamp the workpiece 

Press several times to move the workpiece into 

the chuck area. 

Press to close the chuck. 

Press several times to move the workpiece until it 

rests against the jaw stop. 

Press to conclude and accept the clamping setup. 

Note: 

The clamping device combination of chuck and jaw type can clamp 

workpieces with a diameter of 50 mm up to 116 mm and can grip these up to a length of 18 mm to the jaw stop. 

When creating a setup sheet, this informations will be saved as header in an NC program. Open this program in 

the NC editor and you will see the following entry: 

( ZYLINDER D080.000 L122.000. 

If you use the editor to change the dimension entries e. g. to D060.000 L050.000, a blank with these dimensions 

will be used in the simulator the next time the program is started. If you have chosen a blank diameter which is 

too small or too big for the combination of chuck and jaws, e. g. D040, an error message will be generated. 



Assigning tools to tool stations on the turret 

The tool turret currently installed has 16 tool positions (“stations”). (You can change this in the configuration 

settings). Use the mouse pointer to select the turret position. The associated tool in this position is shown more 

largely on the screen. 

You will have to mount the tools on the turret to comply with your production sheet. 

T01 LEFT HANDED CORNER CUTTER CL-SCLCL-2020/L/1208 ISO30 

Select position T01 and with double click 

tool library. 

open the 

Press 

to select the tool type library. 

Select tool type 

Use the mouse to locate the tool called 

and select it with 

. This tool is then mounted on turret position T01. 

In the two preceding steps, you have replaced a tool in the tool turret. To locate this tool, you have searched 

through a tool type for a tool with a specific name. 

The tool T02 < CL-SVJCL-2020/L/1604 ISO30> ist suitable for tooling. 



We will now show you an alternative method, using the tool set-up for position T03 as an example. We need a 

thread-cutting tool for cutting an external thread with a pitch of 1.5 mm. 

Thus, the first step is to search for all tools suitable for cutting threads with a 1.5 mm pitch. 

Select position T03 and then press with double click 

to open the tool library. 

Press 

to select the tool type library. 

Select tool type 

With mouse click we select in the list field 

. All left handed thread cutting tools are then 

ordered in the pitch parameter Pmin. 



Now scroll all left handed thread cutting tools suitable 

for cutting threads with a 1.5 mm pitch. Select one of 

the two availabel tools. 

Press to select and confirm the tool with the 

designation . Now 

this tool has been mounted in position T03. 

We have now shown you two different ways of selecting tools and mounting them on the turret. You can now 

mount the other tools of your setup sheet on your own. 

You can press the tool bar button to remove an unnecessary marked tool from the turret. 

Tool table synopsis: 

T01 LEFT HANDED CORNER CUTTER CL-SCLCL-2020 L 1208 ISO30 

T02 LEFT HANDED CORNER CUTTER CL-SVJCL-2020 L 1604 ISO30 

T03 LEFT HANDED THREADING TOOL TL-LHTR-2020 R 60 1.50 ISO30 

T04 EXTERNAL RECESSING TOOL ER-SGTFL-1212 L 01.8-0 ISO30 

T05 TWIST DRILL DR-18.00 130 R HSS ISO30 

T08 BORING TOOL (POSTAXIAL) BI-SCAAL-1010 L 0604 ISO30 

T10 BORING TOOL (POSTAXIAL) BI-SCAAL-1010 L 0604 ISO30 

T12 INSIDE RECESSING TOOL (POSTAXIAL) RI-GHILL-1013 L 01.10 ISO30 



The tool for position T12 of type inside recessing tool RI-GHILL-1013 L 01.10 ISO30, is currently not available in 

the library. 

Using the tool function we will enter the respective tool data and create a new tool. 

The tool management enables you to create new tool data in the individual tool types as well as to edit or delete 

existing tool data. 

We select position T12 and select the tool 

management. 

Press 

to open the tool type library. 

Since a large amount of data is required, it is helpful to 

select an existing, similar tool to use as a template. 

Mark the selected tool < RI-GHILL-1013 L/01.30 

ISO30> to be processed per mouse click . Open 

with mouse click a context menu and select 

function “create”. 

The selected tool is read in as a copy. 

Next, select a new name for the the tolol and write the 

selected tool name in the entry field. 

RI-GHILL-1013 L/01.10 ISO30 



We select with mouse click tool parameter set 

cutting plate. 

The new tool data can be edited in the respective 

parameters 

You can now select with the input field. 

Write the following values and enter the required data: 

Broad, upper: 2.9 

Broad, bottom: 3.2 

. 

After you have modified all required data you can now 

genererate the tool. 

Confirm by pressing . The new tool is stored 

under the tool type in the tool 

management. You come back to the tool type list view 

of the tool management. 

Exit tool management with . 

Now the new tool has to be assigned to position T12 

on the tool turret. 

We move the tool into position 12 as before 

When all tools are selected for tooling, leave the tool 

magazine with 

Now tooling is completed. Our next step is to generate a setup sheet. 



In the main menu press 

to call up the setup form menu. 

Press 

to generate a new setup sheet. 

Enter a program name e.g. . 

Save with or or press to quit. The setup 

sheet has been created as header for the NC program. 

Call up the NC Editor and open the new NC 

program. 

If you wish you can exit the NC editor by pressing 

The next chapter will outline one of the methods for 

creating NC programs. 



8.0. NC programming in MTS programming key 

This chapter describes how the editor can be used in combination with interactive programming and dialog 

programming as an NC programming method. 

Using the NC editor, delete the “M30” command at the 

end of the setup form section by positioning the cursor 

on [M] and pressing . 

The beginning of the NC program will be written block 

by block. Exit the editor after block N40 and change 

over to interactive programming mode, a second 

optional method of generating NC programs with 

TopTurn. 

Each NC command block is run individually. 

N0010 G90 

N0015 G54 

N0020 G00 X+100.000 Z+0150.000 

N0025 G92 S4000 

N0030 G96 F0000.250 S0260 

N0035 T0101 M04 

N0040 G00 X+082.000 Z+0000.000 

N0045 G01 X-001.600 

N0050 G00 X+082.000 Z+0002.000 

N0055 G57 X+000.500 Z+0000.200 

After the facing, a straight roughing turning cycle follows, as mentioned in the production sheet.. 



8.1. Inside straight roughing cycle G81 

We shall enter the canned cycle call in dialog programming mode by pressing . 

G81 Straight roughing cycle will be selected. 

In the command overview you select the cycle with 

mouse click and press on to confirm 

Enter the cycle parameter values into the respective 

fields in the form screen, then click on to save 

them to the program. 

N0060 G81 X+033.000 Z+002.000 I+003.000 

Now enter the contour description in interactive mode: 

N0065 G01 Z+0000.000 

N0070 X+036.000 Z-0001.500 

N0075 Z-0030.000 

N0080 X+040.000 

N0085 X+060.000 Z-0050.000 

N0090 Z-0095.000 

N0095 X+074.000 

N0100 X+084.000 Z-0100.000 

N0105 G80 

Once the cycle call G80 is entered, the NC program will 

be run. 

Note: In interactive mode the programmed contour will be shown graphically. 



8.2. Drilling cycle G84 

Technology and tool change 

for drilling cycle programing. 

N0110 G00 X+150.000 Z+0100.000 

N0115 G97 S1200 M08 F0000.150 

N0120 T0505 M03 

N0125 G00 Z+0002.000 

N0130 G00 X+000.000 

Call up dialog programming mode in order to program the drilling cycle. 


mouse click and press on to confirm. 

The NC command line thus created reads: 

Enter the cycle parameter values into the input 

screen, then click on to save them to the 

program. 

Drilling cycle 

N0135 G84 Z-0095.326 A+000.200 B+000.200 

D+010.000 K+020.000 



8.3. Outside straight roughing cycle G81 


N0140 G00 X+150.000 Z+0150.000 

N0145 G92 S4000 

N0150 G96 F0000.250 S0220 

N0155 T0808 M04 

N0160 G00 X+015.000 Z+0001.500 

N0165 G57 X-001.000 Z-0000.100 

8.4. Inside straight roughing cycle G81 

Inside straight roughing cycle and contour description 

N0170 G81 X+021.000 Z+0001.000 I+002.000 

N0175 G01 X+020.000 Z-0000.500 

N0180 Z-0035.000 

N0185 G01 X+024.000 Z-0038.464 

N0190 Z-0076.536 

N0195 X+020.000 Z-0080.000 

N0200 Z-0091.000 

N0205 X+013.000 

N0210 G80 



8.5. Inside finishing 

Technology and tool change, finishing with repeated program sections. 

N0215 G00 X+100.000 Z+0150.000 

N0220 G92 S4000 

N0225 G96 F0000.100 S0300 

N0230 T1010 M04 

N0235 G57 X+000.000 Z+0000.000 

N0240 G41 G00 X+021.000 Z+0001.500 

N0245 G01 X+021.000 Z+0000.000 

N0250 G23 O0175 Q0205 

N0255 G40 

N0260 G00 Z+0002.000 

8.6. Outside finishing 

Technology and tool change, finishing with repeated 

program sections. 

N0265 G00 X+100.000 Z+0150.000 

N0270 G92 S4500 

N0275 G96 F0000.100 S0360 

N0280 T0202 M04 

N0285 G42 G00 X+033.000 Z+0001.500 

N0290 G01 Z+0000.000 

N0295 G01 X+036.000 Z-0001.500 

N0300 G85 X+036.000 Z-0030.000 I+001.100 

K+005.300 

N0305 G23 O0080 Q0100 

N0310 G40 



8.7. Outside thread-cutting cycle G31 

Technology and tool change for calling up thread-cutting 

cycle. 

N0315 G00 X+100.000 Z+0150.000 

N0320 G97 F001.500 S1000 

N0325 T0303 M03 

N0330 G00 X+038.000 Z+0004.000 

Dialog programming the threadding cycle 





program. 

The NC command line thus created: 

N0340 G31 X+036.000 Z-0027.600 F0001.500 

D+000.920 S0006 F0001* 

N0345 M05 



8.8. Outside groove-cutting cycle G79 


N0350 G00 X+100.000 Z+0150.000 

N0355 G92 S4000 

N0360 G96 F0000.150 S0260 

N0365 T0404 M04 

N0370 G00 X+062.000 Z-0063.500 

Dialog programming the groove-cutting cycle G79 





program. 

Cutting three external grooves 

N0380 G79 X+054.000 Z-0064.500 I+000.300 

K+000.300 J+002.000 A+000.200 D-002.600 

W+000.300 O0005 Q0005 

N0380 G79 X+054.000 Z-0072.500 I+000.300 

K+000.300 J+002.000 A+000.200 D-002.600 

W+000.300 O0005 Q0005 

N0380 G79 X+054.000 Z-0080.500 I+000.300 

K+000.300 J+002.000 A+000.200 D-002.600 

W+000.300 O0005 Q0005 



8.9. Inside groove-cutting 

Technology and tool change and inside groove-cutting 

N0390 G00 X+100.000 Z+0150.000 

N0395 G97 F0000.100 S1000 

N0400 T1212 M04 

N0405 G00 X+018.000 Z+0002.000 

N0410 Z-0002.600 

N0415 G01 X+021.000 

N0420 X+018.000 

N0425 G00 Z-0023.700 

N0430 G01 X+021.000 

N0435 X+018.000 

N0440 G00 Z+0002.000 

N0445 G00 X+100.000 Z+0150.000 

N0450 M30 

3D representation of the workpart created by the entered program 



9.0. Quality control – Measuring of workpart 



10.0 Appendices 

Sample 

Drawing 

Template 

Template 

Template 

Information 

NC program 

Turning workpart1 

setup form (setup sheet) 

work plan 

NC programming sheet 

hardlock 



10.1. NC Program %3 

() 

(( 12.4.2006 10:09 

( 

( CONFIGURATION 

( MACHINE MTS01 TM-016_-R1_-060x0646x0920 

( CONTROL MTS TM01 

( 

( FINISHED PART %040____TN08-TR01-16-TM1 

( 

( PART 

( CYLINDER D080.000 L122.000 

( MATERIAL "N\Aluminium\AlMgSi0.5" 

( DENSITY 002.70 

( 

( MAIN SPINDLE WITH WORKPART 

( CHUCK "Chuck Turning\Jaw chuck\KFD-HS 130" 

( STEP JAW "Jaw\Step jaw\HM-110_130-02.001" 

( TYPE OF CHUCK EXTERNAL CHUCK OUTSIDE STEP JAW 

( CHUCKING DEPTH E18.000 


( 

( 

( TAILSTOCK 

( TAILSTOCK POSITION Z+1095.000 

( 

( CURRENT TOOL T01 

( TOOLS 

( T01 "DIN69880 V 30\Left corner tool\CL-SCLCL-2020 L 1208 ISO30" 

( T02 "DIN69880 V 30\Left corner tool\CL-SVJCL-2020 L 1604 ISO30" 


( T04 "DIN69880 V 30\Recessing tool\ER-SGTFL-1212 L 01.8-0 ISO30" 

( T05 "DIN69880 V 30\Twist drill\DR-18.00 130 R HSS ISO30" 

( T06 EMPTY 

( T07 EMPTY 

( T08 "DIN69880 V 30\Inside turning tool postaxial\BI-SCAAL-1010 L 0604 ISO30" 

( T09 EMPTY 

( T10 "DIN69880 V 30\Inside turning tool postaxial\BI-SCAAL-1010 L 0604 ISO30" 

( T11 EMPTY 

( T12 "DIN69880 V 30\Inside recessing tool postaxial\RI-GHILL-1013 L 01.10 ISO30" 

( T13 EMPTY 

( T14 EMPTY 

( T15 EMPTY 

( T16 EMPTY 

( 

( TOOL COMPENSATION 






( D08 T08 Q2 R000.400 X-008.238 Z+0170.000 G000.000 E032.079 I+000.400 K-000.400 A+002.721 L005.992 N01 



( 

( WORKPART ZEROPOINTS 


( G54 X+000.000 Z+0231.000 

( 

() 

N0010 G90 

N0015 G54 

N0020 G00 X+100.000 Z+0150.000 

N0025 G92 S4000 

N0030 G96 F0000.250 S0260 

N0035 T0101 M04 

N0040 G00 X+082.000 Z+0000.000 

N0045 G01 X-001.600 

N0050 G00 X+082.000 Z+0002.000 



N0055 G57 X+000.500 Z+0000.200 

N0060 G81 X+033.000 Z+0002.000 I+003.000 

N0065 G01 Z+0000.000 

N0070 X+036.000 Z-0001.500 

N0075 Z-0030.000 

N0080 X+040.000 

N0085 X+060.000 Z-0050.000 

N0090 Z-0095.000 

N0095 X+074.000 

N0100 X+084.000 Z-0100.000 

N0105 G80 

N0110 G00 X+150.000 Z+0100.000 

N0115 G97 S1200 M08 F0000.150 

N0120 T0505 M03 

N0125 G00 Z+0002.000 

N0130 G00 X+000.000 

N0135 G84 Z-0095.326 A+000.200 B+000.200 D+010.000 K+020.000 

N0140 G00 X+150.000 Z+0150.000 

N0145 G92 S4000 

N0150 G96 F0000.250 S0220 

N0155 T0808 M04 

N0160 G00 X+015.000 Z+0001.500 

N0165 G57 X-001.000 Z-0000.100 

N0170 G81 X+021.000 Z+0001.000 I+002.000 

N0175 G01 X+020.000 Z-0000.500 

N0180 Z-0035.000 

N0185 G01 X+024.000 Z-0038.464 

N0190 Z-0076.536 

N0195 X+020.000 Z-0080.000 

N0200 Z-0091.000 

N0205 X+013.000 

N0210 G80 

N0215 G00 X+100.000 Z+0150.000 

N0220 G92 S4000 

N0225 G96 F0000.100 S0300 

N0230 T1010 M04 

N0235 G57 X+000.000 Z+0000.000 

N0240 G41 G00 X+021.000 Z+0001.500 

N0245 G01 X+021.000 Z+0000.000 

N0250 G23 O0175 Q0205 

N0255 G40 

N0260 G00 Z+0002.000 

N0265 G00 X+100.000 Z+0150.000 

N0270 G92 S4500 

N0275 G96 F0000.100 S0360 

N0280 T0202 M04 

N0285 G42 G00 X+033.000 Z+0001.500 

N0290 G01 Z+0000.000 

N0295 G01 X+036.000 Z-0001.500 

N0300 G85 X+036.000 Z-0030.000 I+001.100 K+005.300 

N0305 G23 O0080 Q0100 

N0310 G40 

N0315 G00 X+100.000 Z+0150.000 

N0320 G00 X+100.000 Z+0150.000 

N0325 G97 F0001.500 S1000 

N0330 T0303 M03 

N0335 G00 X+038.000 Z+0004.000 

N0340 G31 X+036.000 Z-0027.600 F0001.500 D+000.920 S0006 F0001* 

N0345 M05 

N0350 G00 X+100.000 Z+0150.000 

N0355 G92 S4000 

N0360 G96 F0000.150 S0260 

N0365 T0404 M04 

N0370 G00 X+062.000 Z-0063.500 

N0380 G79 X+054.000 Z-0064.500 I+000.300 K+000.300 J+002.000 A+000.200 D-002.600 W+000.300 O0005 Q0005 

N0380 G79 X+054.000 Z-0072.500 I+000.300 K+000.300 J+002.000 A+000.200 D-002.600 W+000.300 O0005 Q0005 

N0380 G79 X+054.000 Z-0080.500 I+000.300 K+000.300 J+002.000 A+000.200 D-002.600 W+000.300 O0005 Q0005 

N0390 G00 X+100.000 Z+0150.000 

N0395 G97 F0000.100 S1000 

N0400 T1212 M04 

N0405 G00 X+018.000 Z+0002.000 



N0410 Z-0002.600 

N0415 G01 X+021.000 

N0420 X+018.000 

N0425 G00 Z-0023.700 

N0430 G01 X+021.000 

N0435 X+018.000 

N0440 G00 Z+0002.000 

N0445 G00 X+100.000 Z+0150.000 

N0450 M30 



10.2. Workpart drawing 



10.3. Working templates 


Turning 

Program No. 

Programmer 

Drawing No. 

Designation 

Material: 

Raw part/blank : 

Setup Sheet 


Clamping mode 

Clamping device 

Clamping depth 

Tailstock/vise position 

CNC control 

Tool data / magazine or turret positions 

Station Tool designation Tool file No. Compensation data Ag. 

X 

Z 0 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

X 

Z 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 

R 

Quadr. 




Turning 

Production Sheet 


Program No. 

Programmer 

Drawing No. 

Designation 

Material 

Raw part/blank 

CNC control 

Sequence of machining steps 

Nr. Maching step NC programming code Tool Cutting data 

position 

01 F N 

V c 

02 F N 

V c 

03 F N 

V c 

04 F N 

V c 

05 F N 

V c 

06 F N 

V c 

07 F N 

V c 

08 F N 

V c 

09 F N 

V c 

10 F N 

V c 

11 F N 

V c 

12 F N 

V c 

13 F N 

V c 

14 F N 

V c 

15 F N 

V c 

16 F n 

V c 

17 F n 

V c 

18 F n 

V c 

19 F n 

V c 




Turning 

Programming Sheet 


Program No. 

Programmer 

Drawing No. 

Designation 

Material 

Raw part/blank 

NC-Code 

N G X Z I K F M T 

05 

10 

15 

20 

25 

30 

35 

40 

45 

50 

55 

60 

65 

70 

75 

80 

85 

90 

95 

100 

105 

110 

115 



10.4. Notice for administrating and organising of setup turning 

The data available in the setup dialogue are read from already existing setup sheets. Those sheets can be 

found in the file: 

.\MTS-CNC Deutsch\Setup_T\ 

mtssetup.sct 

The data mtssetup.sct .(Turning) contains the corresponding informations on the setup dialog. They can be at 

any time edited and extended for new clamping devices. 

Excerpt Source File mtssetup.scm 

[HAUPTSPINDEL] 

INFO=KFD-HS 130 min.42 max.118 Et=30 

DATEI=KFD-HS 130-42-118-E30-A.dnc 

LMIN=10 

LMAX=300 

DMIN=42 

DMAX=118 

IMIN=30 

IMAX=80 

EMIN=5 

EMAX=30 

CMIN=1 

CMAX=6 

Meaning 

= Keyword 

= Name Clamping device 

= Setup sheet with clamping device 

= min. workpart size 

= max. workpart size 

= min. outside diameter 

= max. outside diameter 

= min. inside diameter 

= max. inside diameter 

= min. clamping depth 

= max. clamping depth 

= min. center diameter 

= max. center diameter 

New tool set: 

During setup assign the tools from the tool administration to the corresponding tool positions. Leave the 

magazine with exact correction values and create a new setup sheet. Tool set 05.dnc. 

Consider, that every tool correction values must be listed, otherwise the new workpart set will not be shown in 

the setup dialog. 

Copy the setup sheet Tool set 05.dnc into .\MTS-CNC Deutsch\Setup_T\. 

The new tool set is automatically shown in the list field and is available for new setup. 



Clamping device overview 

CNC-Programm INFO für clamping device Clamping 

picture 

KFD-HS 130-42-118-E30-A.dnc 

KFD-HS 130-42-118-E33-A.dnc 

KFD-HS 130-42-118-E40-A.dnc 

KFD-HS 160-60-148-E30-A.dnc 

KFD-HS 160-60-148-E33-A.dnc 

KFD-HS 160-60-148-E40-A.dnc 







KFD-HS 130-46-118-E10.dnc 

KFD-HS 130-42-118-E15.dnc 

KFD-HS 130-46-118-E18.dnc 

KFD-HS 160-50-148-E12.dnc 

KFD-HS 160-50-148-E18.dnc 

KFD-HS 160-56-148-E22.dnc 







KFD-HS 130-48-114-E10-I.dnc 

KFD-HS 130-48-114-E15-I.dnc 

KFD-HS 130-48-114-E18-I.dnc 

KFD-HS 160-74-162-E04-I.dnc 

KFD-HS 160-74-162-E15-I.dnc 

KFD-HS 160-68-156-E25-I.dnc 







KFD-HS 160-114-184-E40-I.dnc 

KFD-HS 160-114-193-E425-I.dnc 

KFD-HS 160-114-196-E44-I.dnc 


KFD-HS 160 min.114 max.193 Et=42.5 

KFD-HS 160 min.114 max.196 Et=44.0 

KFD-HS 130-46-118-E30-A-RS-02MT2.dnc 






KFD-HS 130 min.46 max.118 Et=30 RS 02-MT2 






KFD-HS 130-42-118-E15-RS-02MT2.dnc 












FDSC 046-60-100-02-MT2.dnc 

FDSC 070-90-200-04-MT3.dnc 

FDSC 046 min.060 max.100 02-MT2 

FDSC 070 min.090 max.200 04-MT3 



10.5. System Information 

* Windows NT 2000 or XP: 

Administrator right must be available in order to install the software. The software must have read and write 

rights in the installation folder. 

* Windows NT: 

The dialog programming of the simulator requires the Internet Explorer 4.01 SP2 (or higher). 

If for technical reasons once 

is not activ, the system must be checked. 

With right mouse click on 

you open a meu. 

Under Info for TopMill the number of the hardlock is shown. 

Compare it with the number of the software licence you have purchased. 

If hardlock number 0 is shown, there is a mistake in the system or in the software installation. 

• Search in Windows functions for a file name: 

• Hardlock.sys (WINNT-2000 XP). 

• Examine the attachment of the hardlock on the LPT-Port.

Introduction to TopTurn CNC simulator turning Version 7.1

You also want an ePaper? Increase the reach of your titles

Delete template?

Save as template?