MTS Logo
CNC Simulator for Turning & Milling - System Description

This document contains detailed information about the features of the MTS CNC Simulator for Turning & Milling Version  

Table of Contents

1 Software Concept of the Simulators

2 System Structure

3 Configuration

4 Tool Administration

5 Setup Mode

6 Automatic Mode

7 Programming Code

8 NC Program Generation

9. Special Functions

10. Transmission Program, Postprocessors and Generalized Postprocessor

11. Free Definable Programming Code

12. Programming Aids

Appendix: Hardware and Operating Systems


1 Software Concept of the Simulators

MTS GmbH looks back on more than ten years of experience in developing technical application software as well as CAD/CAM systems for mechanical engineering, with the main emphasis on CNC simulations of turning and milling technologies (laser cutting, punching and nibbling are in preparation). MTS systems are run-capable on IBM compatible PCs and can be adapted to all current CNC machines and control systems.

The CNC Simulators are employed in production as well as in vocational training and further education. We have made every effort to meet the complex requirements in both these fields of application by including appropriate new functions in the current Version 6.2 of our software, which makes the MTS Simulators one of the most efficient systems on the market today. This high performance is accompained by increased clarity and convenience of operation, due to the new user interface and function keys.

1.1 Performance Characteristics

Production Manual and Workshop-Oriented NC programming are among the most important fields of application of CNC Simulators in the production practice. Equally important is the facility to check and optimise generated NC programs and to make time calculations. 

Since the MTS Simulators can simulate all aspects of a CNC machine tool, they can also test NC programs for actual production; this includes checking for possible collisions as well as establishing workpart geometries (including thread geometries and roughness depths) based on the actual state of machining. No complicated changes of programming or control systems are necessary. Finally, a generalized postprocessor serves to translate NC programs into the programming code of any given CNC control system, so that they can be transmitted to the actual machine tool. 

The main performance characteristics of MTS Simulators are:

• open system qualities, in order to adapt the Simulators to different machine tools and control systems,
• configurable programming code based on the German Standard DIN 66025 and offering the full range of commands common to modern CNC control systems (including all standard machining cycles, contour strings, tool tip and cutter radius compensation),
• convenient NC programming with four different input modes available for specific tasks,
• dynamic update of the body lines of the workpart are dynamically updated during the machining simulation, achieved by a mathematical model of the workpart which allows even complex tool geometry; moreover, the theoretical roughing depth of each contour is generated from the given tool geometry, the course of the contour and the feedrate,
• collision tests, accounting for the geometry of elements in the entire working space (spindle, chuck, clamping device, tailstock, tool, turret/magazine) as well as for the actual machining, according to the tool motions programmed,
• measuring of the turning part, display of intersections and 3D-representations,
• storage and documentation of work results by easily handled NC program, workpart and status administration,
• convenient overall operation including such features as a setup form for automatic setup, an operating concept for Workshop-Oriented Programming (WOP) and a distinctly organised operation flow which corresponds to largely the actual handling of production machines and controls.

These characteristics make the Simulators a very effective means of support in industrial production; program errors can be avoided at an early stage and machine down times are reduced. Furthermore, the Simulators can be integrated into a complete CAD/CAM system environment, which helps minimise internal communication problems and ensures smooth production. 

CNC Training As the capacities of modern machine tools and flexible production systems increase, innovative professional training is required, to ensure that the trainees will be able to meet the new demands, such as high flexibility, an extended knowledge of systems and the ability to transfer such knowledge to new settings. For this reason, a self-disciplined learning and working is taken during vocational training, to promote a sense of professional responsibility in the trainees. 

In professional CNC training this objective is attained through a process of various stages. The MTS Simulators are not customised for a single learning path, but support a range of training concepts, offering a variety of possible solutions in NC programming and providing extensive information and help on every level.

Didactical Methods The MTS Simulator software is based on a didactic concept, which was developed in co-operation with the German "Federal Institute of Vocational Training" (BIBB) in Berlin, and which is constantly being improved. Relevant didactic criteria are: 

• training system with all typical characteristics but not restricted to a specific control system, 
• full information on the actual state of machining, in every program function,
• comprehensive error indication and correction facilities,
• a range of learning levels,
• opportunities for independent work.

The MTS Simulators keep the user continuously informed on the actual state of the machine, with all operational functions supported by user dialogues. Collision monitoring and error messages means that NC programscan be corrected instantly. Convenient programming aid is available at any time on graphic help screens. 

From a didactic point of view an important advantage of working with CNC Simulators, as compared with employing a real production machine for training purposes, is the possibility to reduce complex operational procedures to a number of simple operations at the beginning. Complexity can then be re-established with each successful step in the learning process. With the four different programming modes provided by the MTS Simulators (NC Editor; Interactive Programming; Workshop-Oriented Programming; Teach In) NC programs can be generated step by step, while each NC command programmed is immediately executed by the machine tool. This concept offers an easy way to understand the abstract programming language. The system's additional features, such as adaptation to specific machines, real time simulation and precise collision monitoring inclusive of technology data, add up to a comprehensive representation of CNC technology. Experience has shown that the simulators provide an effective but nevertheless gentle introduction to CNC technology, taking away the fear of making mistakes.

The MTS Simulators are designed to permit CNC training independent of specific control systems or specific manufacturer's products. One main educational objective of this training is to give qualified skilled workers a profound basic knowledge, along with the ability to adapt their skills to varying machine and control configurations. The voide range of CNC control systems available, increasingly with integrated CAD functions, demand highly-skilled, versatile operators. Versitility in this context is above all the ability to adapt to different machine configurations, which is precisly the ability promoted by the MTS Simulators. Several years of practical evaluation at AEG's CNC training centre in Berlin have proved the undeniable value of this approach.

1.2 Software Architecture

Programming Code The MTS Simulators for Milling and Turning are structured in a modular fashion; an extensive configuration program means the can be adapted to all current NC machine tools and CNC systems. Standard operating modes are the Setup Mode and the Automatic Mode; for purposes of NC program generation and optimisation there is a choice of three further operating modes: NC Editor, Interactive Programming and Teach In Mode. The system can be upgraded by installing a user interface for "Workshop-Oriented Programming" (WOP). MTS supplies a Programming Code (also referred to as "command code" in the following) which is designed for programming according to German Standard DIN 66025 (i.e. not adopting any specific manufacturer's code). It contains all standard commands common to modern CNC controls; with the programming of complex contour strings it allows geometry input such as lengths, angles, specification of tangential transitions etc. All standard machining cycles are available as well as tool tip and cutter radius compensation.
In order to ensure that the software is open to different CNC controls and can be adapted to other systems, there is the option of implementing the "Free definition Programming Code" along with the CNC Simulators. This program serves to assign the MTS Programming code to another command code in cases when the user decides to employ a different language (e.g. the one implemented in the machine control). 

For purposes of CNC training the PAL programming code is also available, since it is this which is used by the chambers of industry and commerce in examinations qualifying for a certificate of proficiency.

For data transmission between the CNC Simulators and a particular machine control a Generalized Postprocessor is employed, which enables the user to determine the reciprocal reference of commands in the program translation. 

In addition MTS offers a choice of more than seventy postprocessors for the translation of specific DIN-based controls. These are linked to the Transmission Program which allows variable configuration of interfaces as well as the definition of control characters for data transmission.

CAD/CAM System Among the most important recent advancements in the field of CNC technology has been the development of CAD/CAM interfaces serving to convert CAD design data via NC programming systems into NC programs with the ultimate aim of achieving computer-assisted integration of design and production. For applications in this field MTS GmbH has developed the INCAD system, which can be implemented with no difficulty as an extension to the MTS Simulators. 

INCAD constitutes an Integrated NC and CAD System, functioning both as a full-range CAD system and as a very convenient NC programming system. Among its outstanding features are a uniform user interface, serving both programs, and a direct link to the Generalized Postprocessor, facilitating the adjustment to workshop conditions.

The CAD system of INCAD offers a number of very effective and user-friendly functions for the generation, modification and documentation of design drawings. Exchange of geometry data with other CAD systems is realised through data communication in the IGES, resp. DXF formats.

The NC programming system features separate tool and technology administration, which can be generated and edited by the user. Automatic generation of NC programs (which includes contour strings as well as all current machining cycles) is established through a process of reducing a design to single contours and subsequently assigning technology data and machining methods. A graphically supported interactive dialogue guides the user through this procedure. The reproduction of specific machine and control configurations in the CNC simulators means that NC programs for turning and milling can be tested and optimized before being sent to a real production machine.

All in all the MTS software modules add up to a fully integrated CAD/CAM package, offering practice-oriented and customised solutions for production and training.

2 System Structure

2.1 Survey of Machining Functions

Machine Type The Simulator for Turning emulates a single-slide lathe, with powered tools and C, Y and B axis operation available as an upgrade. The CNC Simulator for Milling represents a 3D-milling machine with vertical or horizontal spindle position. 

Main machining modes available are the following:

• Setup Mode,
• Automatic Mode,
• NC Programming.

The uniform WOP operating concept applies to each of the CNC Simulators, and includes function keys, menu guidance and program dialogues. Auxiliary functions to facilitate program generation and optimisation are measuring, zooming, display of intersections and 3D-representation as well as a number of programming- and controlling aids.

Realistic simulation of the machine tool and its controls is an important precondition for flexibility of application; with MTS Simulators provide the user can define the geometry of the working space and the various machine elements such as spindle, chuck, fixtures, tools, turret, tailstock etc. These parameters are considered in the simulation and computation of the workpart geometry which, with an accuracy of 1 µm , is based on the actual machining, not on the programmed address values. Exact collision checks, taking all machine components into account, are carried out during program execution; errors are denoted in plaintext messages.

Configuration An extensive Configuration Program serves to adapt the MTS Simulators to specific machine and control conditions, as well as to the computer hardware employed. Configuration possibilities are: 

• Machine configuration: specifications of the machine tool (machine parameters) including geometry data and technical specifications.
• Control system configuration: definition of the programming code, specific default settings concerning the logic of controls, such as execution of subprograms, machining cycles, modal commands etc.
• Computer hardware configuration: specifications of the hardware employed, interfaces, periphery, graphic mode etc.

Each configuration is stored in a separate configuration file, which allows quick and convenient alternation between different default settings.

CNC Simulation In the Automatic Mode NC programs are executed and tested in real-time simulation. The graphic-dynamical representation of the machining gives a view of either the entire workspace or a zoomed detail. During the turning simulation body lines (apparent and true edges) are dynamically updated. The same applies to the displayed intersections during the milling simulation. The display shows the NC blocks being executed, while the co-ordinates and technology data are shown in the menu field. Machining times and down times are also calculated.
NC Programming In the Programming Mode there are of four different ways to generate an NC program: 

• The NC Editor supports direct entry or editing of NC blocks via its programming interface, especially suited for NC programs. Each NC block entered is subject to an automatic syntax check ("syntax" in this context being the internal structure of the NC blocks). There is also a check to ensure that the values entered fall within the permitted ranges.
• The Interactive Programming Mode, constituting a reciprocal completion of the Automatic mode and the Editor, is the easiest and most effective way to start on NC programming. During program generation each NC block entered is immediately executed in the simulation, including collision tests.
• Teach-In is a special kind of interactive programming. While the workpart is tooled manually, as in the Setup Mode, the tool paths generated in this way are automatically converted into G-commands (corresponding to DIN 66025) and inserted into the NC program.
• Using the WOP interface, complex contours can be programmed without any further aid. A dialogue system serves to query the geometry data given in the drawing: in addition to co-ordinate values the input of lengths, angles or tangential transitions is possible. Every unequivocally defined partial contour is graphically displayed; if various solutions are possible, they will be offered for selection. Chamfers and roundings can be inserted into a contour string by entering the chamfer width or the radius. All contours generated in the WOP mode can be measured and zoomed.

Data Administration The systems data administration is designed for convenient data protection and documentation of NC programs and configuration files. Further possibilities are the creation of subroutines and workpart files. Any state of machining can be stored and reloaded when further machining of a semi-finished part is desired. 

A new feature of the system is the so-called "Setup Form Interpreter". A setup form contains all information necessary to set up the machine automatically for a specific NC program. At the same time a setup form can be automatically generated from any machine status.

In addition to these applications the CNC Simulators provide a number of special functions designed for convenience of operation. Among these are:

• re-chucking (flipping) the workpart,
• display of sections and 3D - representation,
• measuring and zooming,
• display of traverse paths,
• a variety of programming aids.

2.2 Graphic Representation

Version 5.3 of the simulator software now features vector-scan display (based on the mathematical model), which results in an even faster and more precise screen representation of machining procedures. In the turning and milling simulations the basic layout of operation and display has been left unchanged, so as to maintain uniform operation in both MTS CNC Simulators. The screen is subdivided into three areas: 

• working space,
• information field,
• function keys.

Machining Area The upper part of the screen shows a graphic representation of the working area of the CNC machine tool, including clamping devices, workpart and tool. The size of this window can be adjusted even during the machining. With the Simulator for Turning, either the surface view (with dynamically updated true and apparent edges) or a full or half section of the workpiece is shown. Threads and roughness depths are included in the representation. The milling simulation displays the workpart and the cutter in top view. Intersections through the cutter centre in the X/Z and X/Y plane can be viewed in separate overlay windows, they are dynamically updated in the course of the machining (see Ch. 9.4 below for detailed information on sections display and 3D-representation). With all relevant information graphically presented, the machining process can be supervised in the best possible way.
Information Field In the information field in the right margin of the screen the following information on the status of the system and the machine is listed: 

• current tool co-ordinates,
• spindle speed, feedrate, active tool and compensation register,
• cutting speed,
• coolant and spindle engine status,
• increment or in automatic mode, the leght (min.) of the NC program run,
• blank dimensions (resp. in the automatic mode: the modal commands).

The keys <F1> to <F8> at the bottom of the screen serve to control the applicable functions of the CNC Simulator.

Dialog In the line immediately above the function keys plaintext messages are displayed when an error is made. During interactive programming this line provides user prompts (see Diagr. 25). 

In automatic mode the line above is used to display the NC block being executed.

The colours used in the display can be edited at will (depending on the graphic card employed), e.g. to match the display of a given CNC machine tool.

2.3 Operation and Input Devices

There are two different ways to operate the CNC Simulator:
PC-Keyboard If a PC keyboard is used, all functions are controlled by function keys. To help the user get med to the system quickly, all functions are arranged in layers of a hierarchical menu which has a uniform user interface in the MTS CNC Simulators.
Graphics tablet When the CAD system INCAD is employed concurrently with the Simulators, the PC must be equipped with a "mouse" or a graphics tablet. The tablet can be used as a CNC keyboard by applying the touchpad foil of the simulator to it. 

Other CNC control foils may be used instead of the original MTS foil as long as the allocation of symbols, characters and digits is appropriately configured for each overlay. The user can then work with a variety of keyboard layouts at comparatively low cost. 

Concurrent use of different input media is also possible.

3 Configuration

Since an important feature of the MTS Simluators is the emulation of different NC machine tools, an extensive configuration program is provided to set the default machine control parameters and to adapt the software to the computer hardware (any IBM compatible PC and its periphery). 

All configuration data (with machine, control and hardware parameters grouped separately) are stored in configuration files to be named by the user. This allows convenient "switching" between different configurations. The configuration files can be password-protected against unauthorised access.

The current Version 5.3 of the system offers considerably extended configuration possibilities, especially with regard to the components of the machine working space. This further increases the practical applicability of the simulators:

Working Space In addition to the overall dimensions of the working space, the tool travel range and the reference points must be defined. Furthermore, the machine model discriminates between stationary and mobile components of the working space, both of which are largely configurable.
Chuck System The chuck system of the Simulator for Turning consists of the spindle and the chuck with configurable chuck jaws. Turning between tips is possible as well. The user also defines the geometrical dimensions of tailstock and sleeve. 

In the Simulator for Milling the workpart can be held either by a magnetic chuck, by a vice or by any number of gripping jaws.

4 Tool Administration

The standard equipment of the CNC Simulator includes almost every type of tool with a parameterized geometry of cutting edge and toolholder. Additional tools can be defined with the help of tool administration. Turning tools for instance are defined by specification of the parameters for tip radius, plunge-, insert- and clearance angle, side length of insert and length of toolholder. Any new tool thus defined will be stored in the tool file. 

A similar procedure applies to the Simulator for Milling; standard tools already defined are universal, angular, spherical and T-slot cutters and drills.

5 Setup Mode

In the setup mode (or manual mode) all necessary preparatory activities can be carried out, such as selection of tools (in the turret or in the tool magazine), definition of the blank, selection of a clamping device etc. The input related to functional requirements (such as moving to the reference point, specifying tool compensation values, touching the workpart to define the zero point) is mandatory. Once a machine status has been defined this way, it can be set down in a "setup form" which is assigned to an NC program. Invoking this NC program will then effect the automatic setup of the appropriate simulated machine tool.
Blank / Chuck The procedure of manually setting up the blank and the chuck (and the tailstock, if applicable) is carried out with the help of a special interactive menu. Blank dimensions must be specified, a clamping device be selected and the chucking length defined. In all there is a choice of eleven clamping positions (as configured - see above, Ch.3). 

Appropriate error messages will appear if invalid blank dimensions have been entered, if the spindle is active, or if tool or tailstock are too close to the workpart.

Instead of defining a blank, prefabricated parts (e.g. castings) can be selected from a "parts file" to be inserted as a blank or a semi-finished part for further machining. Geometry data of such parts will automatically be read from the parts file. Conversely each semi-finished part can be stored in a file to be re-loaded at a later point in time.

Re-chucking In both simulators workparts can be flipped (re-chucked) any number of times.
Tool Selection The CNC Simulator for Turning provides a turret which holds a maximum of 16 tools. The Simulator for Milling provides the same number of tools in the magazine. For training purposes tools from the tool file can be mounted in all tool position (from T01 to T16) as default setting, so as to simulate the equipment of an actual machine tool. This configuration means that the turret or the magazine is automatically equipped with this tool selection each time the simulator system is booted. 

The set of tools can of course be modified in the setup mode. All tools mounted will be graphically displayed; the same applies to the total set of tools in the tool file (cf. above, Ch. 4 ).

Offset Values Only tools previously defined can be employed for machining in the CNC Simulators. Therefore, as a rule, after program start or after any change in the allocation of tools the applicable offset values (co-ordinates, radii and quadrants of turning tools) must be specified, so that the offset can be computed in the control system. A total of 99 offset value storage files are available. The appropriate file for each tool can be activated by entering the last two digits of the four-digit tool number. 

The predefined ("gauged") offset values of each tool can be read in from the tool file. When a "reference tool" has been defined, the offset values can alternately be established by "touching" the workpiece. Faulty offset values will of course lead to inaccurate machining or even collisions. At the same time it is possible as in general practice to create finishing allowances by entering slightly different offset values.

Feed times As an additional function the feed times (in seconds) of each tool employed can be ascertained. The engagement time of a tool (measured from the start of an NC program run) is indicated in the menu, and from this taking into account the theoretical tool life, the remaining tool life can be calculated. This is an important aspect of preparatory activities.The feed times are retained and cumulated, even through a sequence of NC program executions. They are however reset to zero each time a tool change or a manual input is effected.
Reference Point As with the setup of the actual machine tool, the approach of the reference point is indispensable in the CNC Simulators; it serves to establish the zero position for incremental measuring along the axes. Approach of the reference point is also a precondition for defining the workpart zero and for execution of NC programs in the Automatic Mode.
Workpart Zero Setting the workpart zero is possible in any position by "zeroing" the co-ordinates. Usually this will be effected by touching the workpart. Alternatively the co-ordinate values of the tool tip resp. the cutter centre can be redefined.
Manual Mode Among the special features of the CNC Simulators is the option of moving the spindle carriage, resp. the tool, in jog motion, e.g. to execute a "manual" pre-tooling of the workpart. This machining is of course also simulated in real time, including feedrate, spindle speed, feedrate override and collision checks. In the manual mode the co-ordinates of the tool nose, resp. the cutter centre are continuously updated and accordingly displayed in the course of the machining. The incremental steps can be set to either 1.0, 0.1 or 0.01 mm. Further options in this operational mode are: tool change, entering of spindle speeds and feedrate values, switching on and off the coolant.

6 Automatic Mode

The automatic mode serves to execute and test in real time simulation NC programs which have been generated in the CNC Simulators, in the INCAD system or by application of some other programming system. The automatic run includes collision checks and offers a variety of ways to optimise NC programs, especially when the extensive configuration opportunities are being drawn on.
Display Screen representation of the machining is dynamically updated and the actual tool co-ordinates as well as the NC blocks being executed are indicated. The machining times and feed times are calculated concurrently. The accurate and comprehensive collision monitoring puts the user in a position to quickly ascertain and immediately correct any program errors. In addition to this, programs can be executed blockwise, in the so-called "single block mode". 

As well as normal program termination, the automatic run can be temporarily suspended to invoke such functions as measuring, zooming or 3D representation. The program run can also be terminated to call up a different machining procedure.

Override / Test Run During the automatic run the machining times and down times are continuously computed. They are directly dependent on the feedrate override which is configurable within a range of 10% to 150%. Tool change times are calculated according to the values configured and are added to the machine down times. 

When the test run function is activated, the machining simulation is of course much faster than the actual machining would be in fact the speed of the simulation also depends on the performance of the Personal Computer employed. This does not however impede the exact calculation of machining times during the test run.

When the system is reset to the setup mode after program execution, the established feed times of the respective tools (cf. above Ch. 4) can be displayed.

With any NC program the traverse paths can be displayed, with feed motion and rapid traverse marked in different colours.

7 Programming Code

7.1 Configurable MTS Control

"Programming Code" or "Command Code" stands for the entirety of G-functions, cycles and machine commands, including all parameters and their combinations, which can be effected by a CNC control system. Especially in those sectors of program design which are not covered by the German Standard (DIN), there is a great variety of manufacturer-specific solutions with the effect that programs can not easily be run under different control systems. 

The programming code (the syntax) of the MTS Simulators has therefore been conceived as an open system: it is not fixed but can be edited or redefined by employing the "Free Definition Programming Code" to create a "Cross-Reference File". Thus the user can generate his own programming code, orientated on the DIN blocks, on which his subsequent NC programming will be based.

As all further generation of programming codes is based on the standard command code supplied with the MTS Simulators, this code is designed to provide a most comprehensive syntax. Among its commands are the following:

1 cf. Ch.11 for a detailed description of the "Freely Configurable Programming Code"

2 "Syntax" means here and in the following the formal structure of NC commands, i.e. the selection and assignation of parameters and the signs to the specified values.

Turning and Milling:
G00 Rapid Traverse
G01 - G03 Linear and Circle Interpolation
G04 Dwell Time
G09 In-position Programming
G22 Subroutines with a Maximum of elevenfold Nesting
G23 Repetition of Program Parts
G24 Unconditional Jump
G25 Moving to the Reference Point
G26 Moving to the Tool-Change Position
G40 - G42 Tool Nose Compensation / Cutter Radius Compensation
G54 - G58 Setting the Zero Point
G53, G59 Zero Shift
G71 - G73 Programming of Contour Strings
G90 - G91 Absolute / Incremental Co-ordinates
G31 Threading Cycles
G33 Special Threads
G36 Path limits for G83
G57 Finishing Allowance for Cycles G81 - G83
G65, G66 Straight and Cross Roughing Cycle, Tapered Contour
G75, G76 Straight and Cross Roughing Cycle, Rectangular Contour
G81, G82 Straight and Cross Roughing Cycle, any following Contour
G83 Roughing Parallel to Contours, Repeated Cycle
G84 Deep Drilling Cycle
G78, G85 Undercuts
G79, G86 Grooves
G87, G88 Radius resp. Chamfer Cycle
G92 Spindle Speed Limitation
G94, G95 Feedrate mm p. min / p. rev.
G96, G97 Constant Cutting Speed / Constant Spindle Speed
G10 Rapid Traverse by Polar Coordinates
G11 - G13 Linear and Circular Interpolation by Polar Coordinates
G45 - G47 Approach and Retreat Information for Cutter Radius Compensation.
G81 - G86 Drilling, Reaming, Thread Milling Cycles
G87 - G88 Pockets (Rectangle, Circle)
G89 Pins
G67 Rectangular Pocket
G61, G77 Drilling (Cycle) Pattern on a Circle
G78 Drilling (Cycle) Pattern on a Straight Line
Apart from these G-functions machine functions (activated by "M" as a first character) as well as other switching functions (denoted by characters "F," "S" and "T") are also available. NC programming with parameters or subroutines is of course possible too.
Data Formats As already mentioned, the CNC Simulators can be configured to operate with different programming codes. If the respective NC commands, including formats, keywords and register values, have been properly assigned, the user will be in a position to emulate the programming code of a foreign CNC control. For training purposes this offers a double advantage:
Data Transmission 1. As the generated NC programs are run-capable without further modifications (except, if necessary, the transmission control characters) postprocessors are no longer needed for the transmission of programs to the actual CNC machine tool (Cf. below, Ch.10). 

2. Different programming codes (esp. the PAL code, cf. below, Ch.7.5) can be used in the training to point out the peculiarities of these codes and to make the trainees acquainted with their application.

7.2 Segment Contour Programming (Contour Strings)

When programming is done directly from design drawings which have not been dimensioned according to NC requirements, the task will be much facilitated by the possibility of entering the geometry data of a sequence of chained contour segments, so-called "contour strings". Instead of entering the co-ordinates of a corner point or circle centre (parameters according to German Standard DIN 66025) the contour string commands G71 (straight line), G72 (circular arc, clockwise) and G73 (circular arc, counterclockwise) allow direct input of further design data such as angles, lengths, tangential tranistions etc. This relieves the user from the chore of intermediate calculations. 

The MTS control system provides programming of multiple-point contour strings and open contours, including sequences of "undefined" spans (entities). The "intermediate points" will be computed by the system (see Diagr.). Even contours of high geometric complexity can therefore be programmed easily, starting out from the design drawing of the part. No special mathematical knowledge or further aid is necessary. The process can be further facilitated by employing the "WOP-Interface" (see Ch. 7.4) which is specially designed for segment contour programming and offers convenient user guidance.

Diagram 19 

Extract from a Program

Example of contour string programming: 

Program: %321 Syntax: correct


N017 G01 Z+010.000 
N019 G00 X+250.000 Y+050.000 Z+010.000 T1111 
N021 G42 X+190.000 Y+060.000 G46 A+005.000 G01 Z-020.000 (CRC, semicirc. approach 
N023 G73 I+155.000 J+060.000 P070 P001 (circular arc ccw, tangential transition 
N025 G72 B+080.000 P000 (circular arc cw, tangential transition 
N027 G73 I+035.000 J+060.000 B+020.000 P070 P001 P000 (circular arc ccw, tang. 
N029 G73 B+120.000 P000 (circular arc ccw, tangential transition


N031 G73 X+185.000 I+155.000 J+060.000 B+035.000 P070 P000 P002 (cir. arc ccw, t.


N033 G40 G46 A+010.000

Explanations: [The character "(" denotes the beginning of comments in the program] 

N021: Activation of cutter radius compens. to the right of the contour, with semicircular approach;

N023: circular arc (counterclockwise), 1st entity of an open four-point contour string, with absolute centre co-ordinates (P070); choice of alternate solutions (P001);

N025: tangential transition (P000) onto clockwise circular arc, 2nd entity of the open four-point contour string, with radius B specified only;

N027: tangential transition (P000) onto counterclockwise circular arc , 3rd entity of the open four-point contour string, with absolute centre co-ordinates (P070), radius specification; choice of alternate solutions.

In the following this entity is treated as the 1st entity of a closed four-point contour string;

N029: tangential transition (P000) onto counterclockwise circular arc , 2nd entity of the closed four-point contour string, with radius only;

N031: tangential transition (P000) onto counterclockwise circular arc , 3rd entity of the closed four-point contour string, with absolute (P070) centre co-ordinates and end co-ordinate in X, radius B specified and choice No.2 of alternate solutions (P002);

N033 Deactivation of cutter radius compensation, with semicircular retreat.

7.3 Cutter Radius / Tool Tip Compensation

CRC The MTS Simulators naturally provide cutter radius- and tool tip compensation, which is a standard feature of modern CNC controls. 

In the CNC Simulator for Milling the invocation of G41 or G42 allows cutting along the programmed contour with the appropriate cutter radius compensation (CRC). Additionally the approach and retreat movements of the tool can be programmed with the applicable NC commands: G45 (contour parallel approach / retreat), G46 (semicircular approach / retreat), G47 (quadrant approach / retreat).

As a special feature, the number of contour segments anticipated in the computing of the cutter radius compensation can be configured (only anticipation of the next span is a standard with CNC controls).

Tool Tip Compensation Accordingly, the commands G41 or G42 in the CNC Simulator for Turning invoke tip radius compensation of the inserts, taking the "working quadrant" into account. The working quadrant determines the position of the centre of the tool, relative to the tool cutting point, as defined in the tool configuration. In addition, this procedure of predefining ("gauging") helps the user understand the effects of cutter radius compensation and learn about the technically unavoidable radiusing of internal corners.

7.4 Cycles

As already mentioned, almost all the work cycles found in CNC controls have been built in to the CNC Simulators, so as to fulfil our primary aim of providing a whole range of CNC controls which can be reproduced by application of the freely configurable programming code. 

In the following overview most of the common standard cycles available as well as some complex machining procedures are listed:

Diagram 22 

Extract from a Program

Examples and explanations of cycle programming: 

Program: %220200 Syntax: correct


N105 G87 X+030.000 Y+030.000 Z-030.000 B+005.000 I-050.000 K+020.000 (rect. pock. 
N110 G78 X+020.000 Y+020.000 A+000.000 D+050.000 S0003 (invoc. of a repeated cyc. 
N115 G88 Z-050.000 B+015.000 I+060.000 K+015.000 W+020.000 (circ. pockets cycle 
N120 G79 X+170.000 Y+050.000 (invocation of a single cycle 
N125 G00 Z-020.000 T0404 M03 F050.000 S0500 
N130 G83 Z-028.000 K+015.000 A+000.500 B+000.500 D+005.000 (deep drilling cycle 
N135 X+192.000


N140 G77 X+170.000 Y+050.000 A+000.000 B+022.000 D+060.000 S0003 (inv. of a cyc.


N145 G00 X+162.000 Y+050.000 Z-023.000 T0909 M03

Explanations: [The character "(" denotes the beginning of comments in the program] 

N105: Rectangular pocket cycle, with specification of finished size, depth of pockets, corner radius and tool adjustments;

N110: Repeated cycle for machining along a straight line, with co-ordinates for the first execution, specification of angles, of distances between and number of pockets;

N115: Circular pockets cycle, with specification of radius and depth of pockets, the clearance plane and the tool adjustments;

N120: Single cycle, with specification of co-ordinates;

N125: Tool change, tool adjustment and machining data;

N130: Deep drilling cycle, with chip breaking, specification of drilling depth; 1st drilling level, dwell times and degression;

N135: Tool adjustment in X;

N140: Cycle for machining along circular arcs, with arc centre co-ordinates and radius, specification of cycle start angle, difference angles between starting positions of subsequent invocations, number of repetitions.

Capabilities of the MTS Programming Code:
CNC Turning:
CNC Milling:
Segment Contour Programming 

Tool Tip Compensation

Segment Contour Programming 

Cutter Radius Compensation with Approach / Retreat Statement

Cutting Cycles: • straight or cross turning 
• contour parallel with/without movement limitation
• optional (non-monotonous) follow-up contours
• interrupted cut for chip breaking
• automatic check for remaining chips
Drilling Cycles: 

Drilling Patterns:

Pocket Cycles:

• deep hole drilling (with chip breaking) 

• tapping

• boring
• reaming
• on a straight line (cycle)
• on a circular arc (cycle)
• rectangular pocket

Repeated Cycles: 

Thread Cycles:

• combinable with other 

• standard threads
• tapered threads
• special threads

• circular pocket 
• pins
Undercuts: • according to DIN 76 and DIN 509, form E or F
Grooves: • chamfered or radiused or 
• with slanted sides
Deep Drilling Cycles
These NC programs can be extended by subprograms (with a maximum tenfold nesting) and can be standardised by using parameters (parameter programming, including calculating functions).

8 NC Program Generation

Both simulators have four programming modes:
Programming Modes • Editor, 
• Interactive Programming,
• Teach In,
• Workshop-Oriented Programming (WOP). 

Each of these modes is designed to meet specific requirements, and with their clear layout and error messages they all offer convenient user guidance during program generation. It is possible to switch from one mode to another at any time during programming, and so to exploit the advantages of the different input systems.

8.1 NC Editor

The NC Editor provides a programming interface customised for convenient input or editing of NC blocks. Each classification letter defined in the programming code has a fixed format, which states the number of spaces before and behind the decimal point and whether input of signs is permitted. These formats are freely configurable.
Input of NC Blocks • In the course of programming only the input of address, sign and value is required, the complete format (e.g. "X+1" => "X+001.000") will then be established automatically and classification letters will be sorted. The sequence of classification letters within a program line is either established in accordance with DIN 66025 or may be defined by the user.
Editing Functions NC block numbers are also automatically assigned. Renumbering an NC program or specific segments of a program is as easily effected as searching for a word, reading-in other NC programs, printing hardcopies etc. Editing functions available are: input, overwriting, deleting, copying and shifting of classification letters, values, NC blocks and program segments.
Error Check During program generation the editor takes care of the important task of formal error detection: a syntax check is carried out line by line. As long as all input is error-free this procedure will run unnoticed indicated only by the remark "syntax correct", in the status area at the top of the editor screen. If however an NC block whose formal structure is invalid (e.g. "G41" and "G40" programmed in the same line) has been entered and confirmed, the respective line will be marked in red and an error message ("syntax not correct") will appear.

8.2 Interactive Programming

Display The screen layout in Interactive Programming is the same as in Automatic Mode, except that the line above the function keys, normally showing the current NC block, is now used for the program generation. Each NC block entered is executed on-line as soon as it has been confirmed. Two types of error correction are provided: 

1. a plaintext error message appears (e.g. "Collision")

The user can undo the machining effected by the faulty block by striking any key. Immediate correction in the respective program line is possible, then the simulation can be re-activated.

Dialog 2. a prompt appears: "Adopt NC block?" 

In this case the Simulator has successfully executed the programmed machining. It is now up to the programmer to decide (in the course of an interactive entry sequence) whether to accept the result. If approved, the NC block is adopted as part of the program being created and the system will be ready for input of the next program line. If the user discards the result, the machining effected by this block will be undone (as in the case of errors) where cycles are concerned, this may amount to a considerable number of cancelled movements.

The immedeate simulation of NC command execution and the direct correction of input errors has been widely approved in the practice of CNC training. Interactive Programming provides a clear, application-oriented introduction to programming, which is a perfect learning aid. In addition, it can be used alongside "Workshop-Oriented Programming", whenever the programming of complex contour geometries is required.

8.3 Teach-In

Teach-In is a special mode of Interactive Programming. As in the setup mode, the tool is manually controlled while the tool-paths generated in the course of machining are automatically converted into basic G-functions and inserted into the NC program.

8.4 Workshop-Oriented Programming

Although segment contour programming (as described above, Ch. 7.2) does much to facilitate the programmer's task, some serious problems may still arise with complex geometries. As practice has shown, the input of NC blocks is often at such a high level of abstraction that the problems can not immediately are resolved even by invoking programming aids and further information on geometry input possibilities.
WOP Interface To resolve such complex input problems, a new programming mode has been developed which is especially designed to meet the requirements of production practice. The so-called "Workshop-Oriented Programming" mode (WOP) is basically a programming interface for CNC technologies. It was originally conceived in the context of a project sponsored by the German Ministry of Research and Development, but it has not been declared a DIN Standard. The general idea of this concept is that the generation of NC programs should be possible by employing only softkey functions and by an interactive programming procedure. At each stage in the programming the workpart geometry is graphically displayed (in a way similar to a CAD program). Whenever there are several mathematical solutions, these are offered for selection. 

The WOP interface provided by MTS has all of these features plus some additional capabilities for convenience fo use:

• The MTS WOP interface can easily be installed to function with the CNC Simulators. Consequently, it is possible different programming modes to switch through, so as to make full use of the respective advantages of each system.

• In the course of NC programming the generated contour and the generating NC block are displayed together on the screen. That means, that the results of programming can be checked immedeately and the input correct if necessary. Geometry definitions are directly linked to the program generation.

• Conversely all programmed contours can be read in to be ready for editing by the functions of the WOP interface.

• The MTS programming code allows for programming of multiple-point contour strings and open contours, including sequences of "undefined" spans (entities). The user is relieved of extensive calculations, as the programming system confines the dialogue to prompts concerning a selection of valid parameters, inclusive of rounding and chamfering data. Thus the programmer can be certain of the contour being unequivocally defined and of its being executed on the workpart. In addition to this, auxiliary diagrams are available to help with the parameter input.

WOP programming generally starts out with the definition of a contour segment (entity) as a straight line or a circular arc (clockwise or counterclockwise) with either a tangential or non-tangential transition. The system then offers a choice of geometry input possibilities, including a check on the mathematical validity of inputs. If the contour entered is sufficiently determined, it will be graphically displayed online.

Input Parameters
of the WOP
CNC Turning
Straight line with/without tangential transition G71
Corner coordinates X and Z
Gradient AW
Distance L
Rounding radius Rc
Length of chamfer Fc
Circular arc (clockwise/counterclockwise) with/without tangential transition. G72 or G73
End coordinates X and Z
Centre coordinates I and K
Arc radius B
Start angle / end angle AW and EW
Rounding radius Rc
For close inspection each contour can be magnified and dimensioned according to the DIN Standard. A further special feature of the WOP programming interface is the automatic (definite and irreversible) assignation of programmed contours to the applicable DIN commands. It is possible to switch to a different programming mode without differences in the NC Syntax causing problems.

9. Special Functions

To facilitate the generation and checking of NC programs, each CNC Simulator provides a number of special functions, including: 

• Magnification of details: zooming,
• Measuring (especially dimensioning of threads),
• Accounting for roughing depths,
• Display of intersections,
• 3D-representation.

9.1 Zoom

As mentioned above, the displayed sector of the working space of the machine tool can be edited at any time during machining, and zoomed details of the machining can be viewed. The workpart is displayed with its rotating edges; those internal corners which are rounded by the tip radius (so-called "apparent edges") are represented by two thin lines ending a short distance from the body edges. 

The zoom function is also available with Workshop-Oriented Programming and Measuring.

Thread Geometry As a new feature with Version 5.3 of the software the geometry of threads is considered and can be displayed online, so that lead and depth of threads as well as nominal and minor diameters can be exactly dimensioned.

9.2 Measuring

The "Measuring" function serves to check the workpart geometry which results from the machining. It can be activated at any time during turning, and also during interactive programming. Two types of dimensioning are possible: 

• entity dimensioning specifies all geometry data (start and end point, transition angles, lengths, circle centres etc.) of contour segments (straight lines or arcs), 
• point dimensioning establishes the distances of contour points from a definable dimension zero (with an accuracy of 1/1000 mm). 

During dimensioning the zoom or magnifying function can be activated for separate dimensioning of a workpart detail. Repeated magnification is possible, the maximum being a detail of 6/1000 mm by 8/1000 mm magnified to fill the screen.

9.3 Roughness Depths

To verify the surface quality the theoretical roughing depth is established with each cutting cycle. In accordance with German Standard DIN 4768, Part 1, the maximum roughing depth and the mean value of surface roughness can be measured.
9.4 Display of Intersections
For screen representation of the machining MTS has conceived a solution which requires extensive mathematical computation:
CNC Turning In the MTS turning simulation the tool tip geometry is not simplified; any generalized polygon of lines and arcs can be assumed as a cutting edge. The complexity of the resulting area can be appreciated even from the simple example of a standard disposable insert, defined by a straight line, an arc and a straight line, moving along a circular arc. 

Therefore, for each basic G function the area covered by the cutting edge is computed and brought to coincidence with the actual workpart contour - i.e. integrated into the internal mathematical model of the workpart. A theoretical roughing depth, established from the cutting edge geometry and the feed motion, is attributed to each contour span.

It follows from this calculation, that the only linkage between the generated geometry and the NC program data is the resulting tool motion. Furthermore this data model allows the graphic representation of body lines (true and apparent edges), relieve cuts, thread geometries and roughing depths, as well as a variety of intersections through the workpart. As a rule internal machining is displayed in half or full section, while external machining is displayed either in half section or in external view.

CNC Milling In the MTS milling simulation vertical intersection areas (through the cutter centre, in the X/Z and Y/Z planes, according to G 17) can be inserted as additional windows in the screen representation of the workpart, the jaws and the tool. These inserts will be displayed above and to the right of the workpart and will be dynamically updated in the course of the machining. 

The (dynamically updated) motion of the cutter (with its spindle) can be viewed in a further overlay window, inserted in the intersection display. In this way the user always has three views of the machining process, which means convenient and precise control of the NC program execution.

Finally, the screen display as described above can be complemented by screen representations of freely definable intersections through the workpart. This mode of display allows free movement of section areas in the X and Y axes, independent of the cutter centre position. Once more the intersection display is dynamically updated. A line (which of course can be edited) indicates the Z plane.

9.5 3D Representations

As a further support feature the system can display of 3D representations of the workpart from any visual angle, at any time during machining. For a view of internal machining, the user can define circular sectors (CNC Turning), resp. quadrants of the workpart (CNC Milling) to be removed in the 3D representation.

10. Transmission Program, Postprocessors and Generalized Postprocessor

Data Transmission NC programs which have been generated or edited with MTS software can be read-in to the control system of a CNC machine tool and subsequently be executed. Conversely, it is also possible provided certain requirements are met to transmit NC programs from the machine control system to the MTS Simulators, e.g. for modification or test run purposes. 

The transmission program is designed to transmit NC programs without any changes of format or syntax. Certain control characters, such as for encoding program start and program end or line feed can be defined by the user. To facilitate the interface configuration and to ensure a perfect interconnection, the transmission program allows the link between the Simulator and the target machine control to be tested before it is actually established.

Postprocessors NC programs written in the MTS- or PAL programming code must be translated into the code of the machine control before they can be read by the control system. For these purpose a variety of postprocessors are available, each designed for a specific control system and for adjustment to the respective interfaces. 

The postprocessors change the MTS-coded programs into basic NC blocks which correspond to the DIN standard and whose syntax is compatible with the dialect of DIN used in the target control. At present more than seventy postprocessors are available. 

The most economic solution for the translation of NC programs is the Generalized Postprocessor, which enables the user to determine cross-references of commands in the translation. Provided that these features are supported by the target control system, the performance characteristics of the Generalized Postprocessor are the following:

• Addresses are changed if necessary,
• Formats of values of the addresses are adapted to the control,
• Subroutines are kept during the translation,
• Parameters are retained or added,
• Cycles are transformed into the respective cycles of the target control,
• Segment contour programming is kept while being translated into G-functions.

The capabilities of the target control system as well as of the MTS software are used to the full in the translation. With its user-defined command references between the source and the object code, the Generalized Postprocessor is a powerful and universal tool which can adapt the MTS software to a wide variety of CNC control systems.

At present the following postprocessors are available:
CNC Milling:
CNC Turning
Anton CNC 3300 
Bosch CC200M
Bosch CC300M
Bosch CC320M
Bosch CNC Alpha 3
Deckel Contour 2
Deckel Contour 3
Deckel Dialog 4
Deckel Dialog 11
DIN (66025) Milling
Emcotronic M 1
Emcotronic TM 02
Engelhardt CNC 3300
Fanuc MF-M4
Fanuc MF-M5
Fanuc Series 0-MB
Fanuc Series 00-MB
Fanuc Series 0-MC
Heckler & Koch 781
Heckler & Koch 783
Heidenhain TNC 151/155 (DIN/ISO)
Heidenhain TNC 355 (DIN/ISO)
Heidenhain TNC 360 (DIN/ISO) 
Heidenhain TNC 407/415 (DIN/ISO)
Heidenhain TNC 151/155 (Klartext)
Heidenhain TNC 355 (Klartext)
Heidenhain TNC 360 (Klartext)
Heidenhain TNC 407/415 (Klartext)
Maho CNC 332 M (Klartext)
Maho CNC 332 (DIN/ISO)
Maho CNC 332 (Klartext)
Maho CNC 432
Maho CNC 532 M
NUM 720 F
NUM 750 F
NUM 760 F
Seibu EDM-EW 30NT
Sinumerik 3 M
Sinumerik 6M-B
Sinumerik 7M
Sinumerik 810 M
Sinumerik 820M
Sinumerik 850M
Sinumerik 880M
Acramatic Cincinnati Milacron 
Anton CNC 3300
Bosch CC200T
Bosch CNC Alpha 2
CC 4200T
DIN (66025) Turning
Emcotronic T 1
Emcotronic TM 02
Engelhardt CNC 3300T
Fagor 8020T
Fanuc Series 0-TB
Fanuc Series 00-TB
Fanuc Series 10-TB
Fanuc Series 15-TA
Fanuc Series 15-TF
Fanuc Series 15-TTA
Fanuc Series 150-TTA
Fanuc Series 6-TB
Gildemeister EPL 1 
Gildemeister EPL 2
Lux Turn
Maho graziano Spa CNC MG 423T
Maho CNC 432 T
NUM 720 T
NUM 750 T
NUM 760 T
Okuma OSP 500L-G
Sinumerik 3 T
Sinumerik 8 T
Sinumerik 810 T
Sinumerik 820 T
Sinumerik 850 T
Sinumerik 880T
Tiger III
Traub TX 8D
Traub TX 8F
Status: 29.11.1996
Postprocessors for other control systems can be developed on request

11. Free Definable Programming Code

The programming codes of CNC systems, although based on the German Standard DIN 66025, do vary from manufacturer to manufacturer. Exploiting the freedom of the standard, each system is designed to facilitate NC programming by providing segment contour programming and specific machine cycles. We have therefore developed an individual programming code for MTS Simulators, which is non manufactorer-specific and which fulfils two major requirements: it permits all contour strings and machining cycles common to other control systems by way of its superior "command standard" and at the same time guarantees convenient NC programming. The success which the MTS system has achieved in CNC training fully endorses the strategy adopted. 

In addition to the MTS and PAL programmings codes we also offer a software module, which allows the application of any other NC syntax in the CNC Simulators. Provided you have the "Free Definition Programming Code" license, NC blocks of the foreign syntax can be assigned to the respective MTS syntax blocks. In this way a foreign command code can be used to generate NC programs in the CNC Simulators.

A definable programming code file serves to convert the various NC commands. The comprehensive "command standard" of the MTS programming code means that even NC commands from a foreign programming code can be assigned to MTS-coded commands. The "translation" of single NC blocks is then carried out, based on there cross-references.

Each new programming code file is generated with the help of a special editor, which can be invoked from the configuration program. Programming codes which are already part of the configuration can easily be selected or edited for use with a task in one of the CNC Simulators.

1 For a description of the MTS Programming Code cf. above. Ch.7.

12. Programming Aids

Programming aids, which are classified by subject, can be activated at any stage in the operation of the CNC Simulators. The help windows inform the user of the effects of a G-command or cycle. Directories and general surveys of the subject matter are provided for quick orientation. In this way the user has access to most of the programming instructions even during the actual machining process. 

Once the help function has been activated, any number of help windows can be called up. The user can browse through sub-headings, e.g. to compare related commands, or jump from subject to subject to obtain wider information. During interactive programming or program generation with the NC Editor the programming level can be re-activated alongside the help function, and an NC block corrected or entered directly.

The programming aids are designed to support the basic didactical concept of the CNC Simulators. On one level, the user is provided with immediate answers to any questions he may have, while on another level, help windows providing information on wider aspects of programming are available. The reputation of the MTS Simulators for learner-friendliness is due in no small way to there extensive help facilities.

Appendix: Hardware and Operating Systems

The CNC Simulator software is run-capable on IBM compatible PCs under MS-DOS (from Version 3.00 upwards). A UNIX version of the software is also available. 

Hardware requirements for running the MS-DOS Version 5.3 of the MTS CNC Simulator package are as follows:

• 4 MB of RAM
• a 80386, 80486 or pentium processor
• 8 MB to 10 MB of available storage capacity on hard disk, depending on the extent of the software employed
• a floppy disk drive (5 ¼" or 3 ½")
• a serial interface, if a graphic tablet or mouse is to be used
• a parallel interface to connect the software protection module (hardlock); this interface can also be used to connect a printer
• one of the video cards listed in the following:

- HVGA (1024 x 768 pixels)
- SVGA (800 x 600 pixels)
- VGA (640 x 480 pixels)

For use with 80386-processors
• a mathematical coprocessor is not required but highly recommendable (because of the extensive mathematical calculations necessary)

Optional enhancements of the systems are:
• additional interfaces for peripheral devices (e.g. tape reader/ puncher, plotter, mouse-devices [Microsoft, Genius etc.]) or a direct connection to a CNC machine tool.

Hardcopy Output of hardcopies requires a printer driver compatible with the graphics card and the printer used.

CNC Simulators for Turning and Milling - System Description - Version 5.3
© MTS Mathematisch Technische Software-Entwicklung GmbH
Kaiserin-Augusta-Allee 101 • D-10553 Berlin • Tel.: +49/30/34 99 600 • Fax: +49/30/34 99 60 25 • e-Mail:

Deckel is a registered trademark of the Friedrich Deckel AG. EPL is a registered trademark of the Gildemeister AG. MAHO is a registered trademark of the MAHO AG. MS-DOS is a registered trademark of the Microsoft Corporation. Hercules is a registered trademark of the Hercules Corporation. HP is a registered trademark of the Hewlett-Packard Corporation. IBM is a registered trademark of the International Business Machines Corporation. Olivetti is a registered trademark of the Ing. C. Olivetti & C., S.p.A. DIN: Deutsche Industrie Norm, Deutsches Institut für Normung e.V.


Descubra nuestra Software para la Formaciσn Profesional y para la Producciσn !



Materials de Informacion: [ TOPCAM/TOPTURN/TOPMILL
[ MTS presente en las Ferias... | [ Home | FAQ | Support | Pedidos | Acerca de MTS | Socios | Download ]

Para mayores informaciones escriba directamente a:
Nuestro equipo de servicio al cliente puede comunicarse con Vd. directamente en los idiomas: inglιs, alemαn, espaρol y francιs.
Copyright &COPY; 1996-2006 MTS GmbH Berlin • Letztes Update: 04.01. 2006