CNC Basics

208
CNC Basics MTS TeachWare Student’s Book MTS Mathematisch Technische Software-Entwicklung GmbH • Kaiserin-Augusta-Allee 101 • D-10553 Berlin Phone: +49 / 30 / 349 960 - 0 • Fax: +49 / 30 / 349 960 -25 • World Wide Web: http://www.mts-cnc.com • email: [email protected]

description

Catalogs MTSCNC training sofware

Transcript of CNC Basics

  • CNC Basics MTS TeachWare Students Book

    MTS Mathematisch Technische Software-Entwicklung GmbH Kaiserin-Augusta-Allee 101 D-10553 Berlin Phone: +49 / 30 / 349 960 - 0 Fax: +49 / 30 / 349 960 -25 World Wide Web: http://www.mts-cnc.com email: [email protected]

  • CNC-Basics

    MTS TeachWare Students Book

    MTS Mathematisch Technische Software-Entwicklung GmbH

    Kaiserin-Augusta-Allee 101 D-10553 Berlin

    Phone: +49 / 30 / 349 960 - 0

    Fax: +49 / 30 / 349 960 - 25

    eMail: [email protected]

    World Wide Web: http://www.mts-cnc.com

    Created by BK & BM, 2005.

  • All rights reserved, including photomechanical reproduction and storage on electric media

  • Contents

    Introduction into CNC Technology .................................................................................. 9

    1.1 History and Development of CNC Technology ................................................................................9 From conventional machine tool to Computer Integrated Manufacturing (CIM) ..............................9

    1.2 Conventional vs. CNC Machine Tool .............................................................................................11 Machine Structure ..........................................................................................................................11 Function..........................................................................................................................................11 Productivity .....................................................................................................................................12

    1.3 Characteristics of modern CNC machine tools ..............................................................................13 Controllable feed and rotation axis.................................................................................................13 Path measuring systems ................................................................................................................15 Main drive and work spindle...........................................................................................................17 Work part clamping devices ...........................................................................................................17 Tool change facilities ......................................................................................................................18 Security precautions on CNC machine tools..................................................................................19

    Control test CNC Basics.........................................................................................................................21

    Basic Geometry for CNC Machining .............................................................................. 23

    2.1 Coordinate systems on CNC machine tools ..................................................................................23 Types of coordinate systems..........................................................................................................23 Cartesian coordinate system..........................................................................................................23

    CNC-Exercise ...........................................................................................................................................28 Feed and Turning Axes on CNC Machines....................................................................................31

    CNC-Demo........................................................................................................................ 34

    CNC milling ...............................................................................................................................................34 CNC turning ..............................................................................................................................................35 2.2 NC Mathematics .............................................................................................................................36

    Basics of coordinate point calculations ..........................................................................................36 Calculation of NC coordinates........................................................................................................39

    2.3 Zero and reference points on CNC machine tools.........................................................................41 Types of zero and reference points................................................................................................41 Setting the work part zero point W on a CNC lathe .......................................................................44 Setting the work part zero point W on a CNC milling machine ......................................................45

    CNC exercise............................................................................................................................................47 2.4 Numeric Controls on CNC Machine Tools .....................................................................................53

    Control chain and control loop........................................................................................................53 CNC Control ...................................................................................................................................53 Types of CNC controls ...................................................................................................................56 DNC operation................................................................................................................................60

    2.5 Tool Compensations for CNC Machining.......................................................................................62

  • Inhalt

    Using tool compensation values.................................................................................................... 62 Tool length compensation for milling and turning.......................................................................... 62 Tool radius compensations............................................................................................................ 63 Tool measuring and adjusting with an adjusting device................................................................ 69 Tool measuring and setup using the CNC machine...................................................................... 71

    2.6 Path Measuring Systems............................................................................................................... 75 Infeeds, position control and position adjustment of the NC axis.................................................. 75 Path measuring.............................................................................................................................. 75

    CNC exercise ........................................................................................................................................... 77

    Control test Basic Geometry .......................................................................................83

    3 Technological Basics for CNC Machining...............................................................85

    3.1 CNC tool systems for turning and milling ...................................................................................... 85 Tool carriers ................................................................................................................................... 85 Tool holder ..................................................................................................................................... 85 Tungsten carbide indexable inserts............................................................................................... 86

    3.2 Structure and use of lathe tools for CNC machining ..................................................................... 87 Types of lathe tools and the corresponding ISO designation........................................................ 87 Cutting materials ............................................................................................................................ 88 Cutting edge geometry .................................................................................................................. 90 Abrasion and cutting edge............................................................................................................. 91 Cutting value .................................................................................................................................. 92 Examples: Calculating technological values for CNC machining.................................................. 94

    3.3 Structure and application of milling tools for CNC machining ....................................................... 95 Milling and milling operations......................................................................................................... 95 Types of milling tools ..................................................................................................................... 97 Cutting edge materials................................................................................................................... 99 Cutting geometry ......................................................................................................................... 100 Cutting values .............................................................................................................................. 102 Calculation examples of technological values for CNC machining ............................................. 104

    3.4 Calculation of technological data for CNC machining ................................................................. 107 Calculation examples of technological data for CNC turning ...................................................... 107 Calculation examples of technological data for CNC milling....................................................... 115

    3.5 CNC clamping systems ............................................................................................................... 119 Types of clamping systems ......................................................................................................... 119 Types and characteristics of clamping devices for turning.......................................................... 123 Types and characteristics of clamping devices for milling .......................................................... 132

    Control test Technological Basics............................................................................137

    MTS TeachWare CNC-Grundlagen Students Book 6

  • Contents

    4 Introduction into NC programming........................................................................ 139

    4.1 Work organization and flow of manual NC programming ............................................................139 Comparison of work preparation of conventional and CNC machining .......................................139 Organizing the steps of NC programming....................................................................................140 Programming procedure for manual NC programming at programming seat..............................143 Quality assurance during CNC production...................................................................................145

    4.2 NC programming basics...............................................................................................................146 NC programming standards (ISO)................................................................................................146 Structure of an NC program .........................................................................................................146 Structure of a program block ........................................................................................................147 Structure of a program word.........................................................................................................147 Comparison of programming codes/keys of various CNC controls .............................................149

    4.3 Introduction to manual NC programming .....................................................................................156 Procedure for manual NC programming ......................................................................................156 Manual NC programming Turning................................................................................................159 Manual NC programming Milling ..................................................................................................180

    2. Control test Introduction into NC programming............................................... 195

    MTS TeachWare CNC-Grundlagen Students Book 7

  • Instroduction into CNC technology

    2. Introduction into CNC Technology

    1.1 History and Development of CNC Technology

    From conventional machine tool to Computer Integrated Manufacturing (CIM) The idea of numerical control (NC) of machine tools emerged in 1949/50 at the MIT (Massachusetts Institute of Technology, Cambridge, USA) as a result of a US Air Force order to manufacture important airplane parts from full material rather than by riveting and welding material together. The templates and patterns needed for form cutting were however very complicated and could only be manufactured with a considerable time and cost increase when using conventional technology. Since how-ever the contours of the large parts could easily be represented as mathematical functions it was decided to develop a control to control a milling machine on this basis.

    NC

    19601950 1970 1980 1990

    CNCFFS

    CADCAD / CAM

    CIM

    NC Numerical control

    CNC Numerical control with inte-grated computer

    FFS Flexible manufacturing sys-tem

    CAD Computer aided draw-ing/design

    CAM Computer aided manufactur-ing

    CIM Computer integrated manu-facturing with planning, de-sign and manufacturing

    Figure 1 Development into CIM technology The technical realization of this idea required a control which interprets binary and digital entries for travel paths and switching operations in such a way that they could be understood and processed by the milling machine. Herewith the basic principle was formulated for the application of numerical controls. The rapid development of electronic data processing then enabled the practical realization. First a corresponding NC control was developed for a vertical milling machine. The machining path and switching information necessary for manufacturing was given on punch card. The idea was to control the infeed axis of the milling machine so that separately working motors control the axis movements of the tool carrier. The sequence of the travel path and switching information in form of code letters and numbers was called a NC program. This first NC machine tool already showed all the characteristics of the NC machines to be developed later on:

    Entry unit with numerical starting value for the travel path and switch information on a punch card. Computer control to process the travel path and switch information. Separate power supply for each infeed axis and spindle to control the movements of the tool and tool

    carrier.

    Measuring and control systems returning feedback to the controlling computer regarding the tool posi-tions.

    MTS TeachWare CNC-Grundlagen Students Book 9

  • Instroduction into CNC technology

    In the mid 50s almost all machine tool manufacturers began developing and manufacturing numerically con-trolled milling machines which were soon followed by NC lathes. The rapid development of new microele-tronic components, such us micro processors and micro computers, enhanced the development of NC con-trols to CNC (computerized numerical control) controls in the mid 70s. With the increased contribution of high-performance microprocessors it was possible to extend the opera-tions of the computer controlled machine tools. The current microcomputers and CNC controls as well as the PLC (programmable logic controller) of the machine tools have improved NC programming efficiency. Con-tour precision and machining speed of the tools as well as cutting power have continuously improved. Mod-ern CNC controls additionally offer a multitude of further characteristics. This has made it possible, for in-stance, to program complex tool geometries without using mathematical calculations. The continuous further development of CNC machine tools takes place in a reciprocal innovation exchange between the manufacturers of microelectronic components, CNC controls, tools and machine tools. Users also facilitate this increasingly rapid development by continuously demanding new and improved solutions. CNC machining centers, flexible production systems (FFS) and fully automated manufacturing (CIM) mark significant stages of this development which started in the 50s. The following list shows some of the current user requirements: interfaces with high performance for more rapid transfer of constantly increasing data complete machining centers with high precision, e.g. CNC lathes with 7-32 NC axis, several spindles and

    live milling tools for turning high speed machining for turning, milling and boring with maximum dynamic travel path accuracy development of servo motors whose scanning rate for defining the manufacturing dimensions becomes

    smaller and smaller (presently the scanning speed is already less than 1ms) minimizing the programming effort for the individual manufacturing tasks simple, high-performance NC programming systems with dynamic-interactive simulation of the machining

    processes graphic control error diagnosis of the CNC machine tool or of the complete machining system

    MTS TeachWare CNC-Grundlagen Students Book 10

  • Introduction into CNC Technology

    1.2 Conventional vs. CNC Machine Tool

    Machine Structure The CNC machine tools are basically built in the same way as conventional machine tools. The difference lies in the fact that the machine components relevant for turning and milling processes are controlled by computers. The movement directions of the components of a CNC controlled machine tool are specified by a coordinate system, which refers to the work part to be machined and shows axes located parallel to the main linear movement. The movements necessary for machining the individual machine tool assemblies (table, turret and others) are calculated, controlled and tested by a computer. For this purpose each machining direction has a separate measuring system to calculate the corresponding positions of the machine tool assemblies and to return this information to the control.

    Function In the following overview conventional, NC and CNC machine tools are compared in their basic functionality:

    Conventional Machine Tools

    NC Machine Tools CNC Machine Tools

    Entry: The qualified worker manually adjusts the machine tool according to the drawing, clamps the raw part as well as the tools and aligns them.

    Entry: The NC program is transmitted to the NC control using a punch card.

    Entry: NC programs can be entered into the CNC control either using a keyboard, disks or data interface (serial, Bus). Several NC programs are stored in an internal storage, whereby modern controls also use hard disks.

    Manual control: The qualified worker manually sets the machining values (number of rotations, infeed) and controls the machining using hand wheels.

    NC control: The NC control processes the path and feed information of the NC program and passes the corre-sponding control signals to the components of the NC machine.

    CNC control: The micro computer integrated in the CNC control and the corre-sponding software take over all control functions of the CNC ma-chine. Hereby internal storage are used for programs and sub-programs, machine data, tool and compensation values and fixed and free cycles. Frequently, error monitoring software is integrated in the CNC control.

    Dimension control: The qualified worker manually measures and verifies the dimen-sions of the work part and, if nec-essary, must repeat the machining process.

    NC machine: The NC machine ensures the di-mensional stability of the work part already during the machining process with the continuous feed-back from the measuring system and the servo motors.

    CNC machine: The CNC machine ensures the dimensional stability of the work part already during the machining process with the continuous feed-back from the measuring system and the servo motor, which is con-trolled by the number of rotations. Integrated measuring sensors make it possible to control the dimensions during the machining. In parallel to active machining it is possible to continue work on the CNC control, e.g. to test and opti-mize new NC programs.

    MTS TeachWare CNC-Grundlagen Students Book 11

  • Instroduction into CNC technology

    Productivity Advantages of the CNC machine tool 1. The higher machining speed of the CNC machine tool as well as decreased basic, auxiliary, preparation

    and finishing times on the machine increases productivity. The following factors are especially influential:

    programming directly on the machine tool with manual entries shared responsibility in a department responsible for work preparation for programming, materials and

    tools and due entry of the data at the CNC work seat storing recurrent machining processes of a tool specific program in form of subprograms optimizing NC programs on the control description of the work part shapes to be machined with simple geometry entries automatic infeed of the tool until the required dimension has been reached automatic initiation of all functions of the machine and direct intervention when identifying errors or

    disturbances automatic monitoring of the production through the CNC control (automatic measuring and testing) universal application of tools in tool clamping systems possibility to preset the tools outside of the machine tool without influencing machine run-time

    2. Constant quality of the work part and less scrap.

    3. Increased dimension precision of the work part through high basic precision of the machine tool (1/1000 mm)

    4. Short run-through-times through product organization and combination of split machining processes

    5. Improved machine utilization and rentability

    6. Improved production flexibility through machining systems and correspondingly rational production of small lots or single work parts with high complexity

    Due to the advantages mentioned above the CNC machine tools are prevalent in cutting production. The wide application field (see figure 2) is a typical characteristic of the CNC machine tools.

    1

    2

    3

    4

    larger lot sizes

    increased complexity and production precision

    CNC machine tools

    conventional machine tools

    Figure 2 Application field of CNC machine tools Requirements for using CNC machine tools To operate and program CNC machine tools the machine operator needs a higher qualification. Experience from conventional machining can not necessarily be transferred.

    MTS TeachWare CNC-Grundlagen Students Book 12

  • Introduction into CNC Technology

    1.3 Characteristics of modern CNC machine tools

    Controllable feed and rotation axis Work part machining on CNC machine tools requires controllable and adjustable infeed axes which are run by the servo motors independent of each other. The hand wheels typical of conventional machine tools are consequently redundant on a modern machine tool. CNC lathes (see figure 3) have at least 2 controllable or adjustable feed axes marked as X and Z.

    X

    Z

    Figure 3 Controllable NC axes on an automatic lathe

    CNC- milling machines (see figure 4) on the other hand have at least 3 controllable or adjustable feed axes marked as X, Y, Z.

    Z

    Y

    X

    Figure 4 Controllable NC axes on a milling machine

    MTS TeachWare CNC-Grundlagen Students Book 13

  • Instroduction into CNC technology

    In addition to the linear movements along the X, Y and Z axes it is possible to control rotation around each axis. These controllable rotation axes are marked with A, B and C (see figure 5).

    +Y

    +B

    +A

    +X

    +Z

    +C

    Figure 5 Feed and rotation axes in Cartesian coordinate system

    Often further controllable feed axes are needed. These are then marked as U, V, W. Additionally there are the adjustable rotation axes around which the machining table, head stock and tool holder can rotate inde-pendent of the feed axes. They are marked as A, B and C. The required tool and work part carriers are moved by feed drives. The feed drives meet the highest re-quirements due to high machining and iteration precision. The individual axis movements must be carried out with maximum feed speed and minimum positioning time. To meet these requirements a modern feed drive (see figure 6) consists of the following components:

    motor, mechanical gears against overload as well as electronic control ball screw drive for power transfer free from play sensor as path measuring system, mostly located at the free end of the axis power amplifier with analog or digital interfaces for CNC control For exact positioning the feed drives are connected with the measuring facilities. Each controllable axis of a CNC machine needs a path measuring system with automatic interpretation of the measuring signal. The most frequently used resolution for length measuring is 0.001 mm, however for the X axis of the lathe (di-ameter dimension) 0.0005 and for the precision grinding machine up to 0.0001 are customary.

    5

    12

    3

    4

    Figure 6 Feed drive for carrier with ball screw drive

    feed drive

    work table

    measuring system

    ball screw

    ball screw nut

    MTS TeachWare CNC-Grundlagen Students Book 14

  • Introduction into CNC Technology

    The embodiment of the measure is usually a ball circulating screw. If the spindle is set in motion by the mo-tor, then the spherical thread nut, which works almost free of play, moves in longitudinal direction and pushes the corresponding tool or work part carrier along the carrier track (see figure 7). The almost friction-free transfer of power from the spindle to the carrier is achieved through a system of balls. To guarantee the minimum of thread play the two halves of the ball thread nut are clamped against each other to achieve high and reproducible accuracy of production. Eventual pitch errors of the spherical contour spindle can be auto-matically rectified by the CNC control through the spindle pitch error compensation. Further mechanical pos-sibilities are for instance the rack/pinion and spindle/nut. If less accuracy is sufficient hydraulic drives are used as well.

    31

    4

    2

    3

    Figure 7 ball screw drive with play-free double nut

    ball screw nut

    Clamping ring

    balls

    Drive spindle

    The manufacturing tolerances resulting from the manufacturing process of the ball screw drive can be recti-fied by modern CNC controls using the spindle pitch error adjustment. For this purpose the tolerances are measured by laser measuring systems and stored in the CNC control.

    Path measuring systems Depending on the applied measuring device or scale direct and indirect position measuring are differentiated as well as absolute and incremental position measuring. The most accurate measuring values are achieved with direct measuring scales. In direct position measuring (see figure 8) the measuring scale is given in the carrier or on the machine table so that inaccuracies on spindle and drive connection have no influence on the value measured. The measuring values are specified by an optical pick-up on a scanning pattern of the measuring scale. The pick-up converts these values into electrical signals and transfers them to the control.

    Y

    X

    12

    Figure 8 Direct position measuring

    pick-up

    glass ruler with scale

    MTS TeachWare CNC-Grundlagen Students Book 15

  • Instroduction into CNC technology

    In indirect position measuring (see figure 9) the travel path is specified using the rotation of the ball circu-lating screw, which is equipped with a pulse disk as a measuring scale. A signal generator registers the rota-tions of the pulse disk and transfers them to the control. The control then calculates the exact carrier move-ments or its present positions based on the rotation pulses.

    X

    4

    3

    2

    1

    Figure 9 Indirect position measuring

    carrier

    pulse disk as a measuring scale

    spindle

    signal generator

    In absolute position measuring (see figure 10) a coded measuring scale immediately shows the position of the carrier with reference to one fixed orientation point on the machine. This point is the machine zero point, which is specified by the machine manufacturer. This method presupposes that the reading-in area of the measuring scale is as large as the machining area and that the coding of the measuring scale is binary. This is to enable the control to allocate a numerical value to each read-in position.

    M

    1 20 1 2 3 4 5 6 7 8

    Figure 10 Absolute position measuring

    binary-coded measuring scale

    current tool carrier position

    In incremental position measuring (see figure 11) a measuring scale with a simple grating consisting of light and dark fields is used. For a feed movement passing the sensor the sensor counts the number of light and dark fields and calculates the current carrier position based on the difference from the last carrier posi-tion.

    1 2 3 4

    Figure 11 Incremental position measuring

    ruled grating

    previous carrier position

    current carrier position

    carrier on reference point

    MTS TeachWare CNC-Grundlagen Students Book 16

  • Introduction into CNC Technology

    The control has once to be given one absolute position, which it then uses as a reference point when calcu-lating the current carrier position using incremental position measuring. Therefore, it is necessary to go to this absolute point once the control is started. This absolute point is called the reference point on the ma-chine. Each axes movement, even when traveled manually using the hand wheel or buttons, needs to be registered by the control. Since the control loses the control/information on mechanical movements when switched off the reference point has to be returned to each time the control is switched on.

    Main drive and work spindle The main drive of a CNC machine needs to transmit the necessary power output for machining the current work part. This power output is transmitted from the main drive to the drive of the corresponding work spin-dle. The friction loads of the mechanical parts of the machine are also to be considered. They ultimately determine the efficiency of the CNC machine. It is necessary to have a drive with high stability, i.e. the mo-ment of rotation has to be so that the current machining position remains unchanged even if the machining loads are high. In addition to this, the drive has to possess sufficient dynamics to master speed changes rapidly and without overshooting. The work spindle and the eventually available counter spindle were previously driven by a direct-current motor. To keep the cutting speed constant a stepless regulation of the rotation speed of these motors within a wide range, for instance to turn various diameters, is required. A disadvantage of the direct-current motor is the abrasion of the carbon brushes, which need to be regularly checked and changed if necessary. Thanks to the progressive development of microelectronic components three-phase motors are now mostly used. Their disadvantage, the complicated control of the number of rotations, has become irrelevant due to the price development in electronic controls. There are two types of three-phase motors: asynchronous and synchronous motors. They have consider-able advantages compared with direct-current motors. With identical dimensions higher rotation moments are achieved. Furthermore, up to three times higher number of rotation and much better power output is possible. These motors work without carbon brushes, without collectors or collecting rings and are corre-spondingly maintenance free. The spindle head of the work spindle is standardized to guarantee the maximum possible exchange of clamping devices. In CNC machines, the work spindle as well as many other parts are more solidly built than in conventional machine tools because of the considerably higher acceleration rate (10 to 40m/s) and higher machining performance.

    Work part clamping devices Work part clamping devices hold the work part in the correct and exact position on the work spindle for turn-ing or on the work table for milling. The work part must be clamped so that it is absolutely free from play, positioned correctly and exactly, and fully resistant to dynamic stresses. A multitude of work part clamping devices are available. In milling, loading and withdrawal of work parts will automatically be done by charging robots in the future (see MTS robot simulator ROBIN). For turning, mostly controllable jaw chucks of different types are used. These chucks are designed to allow pneumatically or hydraulically controlled automatic charging and ap-proach of the chucks. The clamping powers are adjustable. Depending on weight, material, length/diameter relation, clamping depth and other machining conditions the clamping powers have to be adjusted higher or lower. Chuck jaws for high number of rotations have a centrifugal force compensation so that the clamping power is not reduced by the contrary centrifugal force. This centrifugal force is realized for instance by compensation weights, which are connected with the clamping jaws by a lever. The centrifugal force of the compensation weight exerts then an opposite force to the centrifugal force of the chuck jaws. The clamping power is kept constant with this compensation. For machining between centers mostly drivers, face drivers and controlla-ble live turrets are used. For clamping small parts controllable collet systems are commonly used.

    MTS TeachWare CNC-Grundlagen Students Book 17

  • Instroduction into CNC technology

    In CNC milling the main function of the work part clamping devices is the correct positioning of the work parts. The work part clamping should allow a work part change which is as quick, easy to approach, cor-rectly and exactly positioned, reproducible as possible. For simple machining controllable, hydraulic chuck jaws are sufficient. For milling on all sides the complete machining should be possible with as few re-clamping as possible. For complicated milling parts milling fixtures, also with integrated automatic rotation, are being manufactured or built out of available modular systems to allow, as far as possible, complete ma-chining without re-clamping. Work part pallets, which are loaded with the next work part by the operator out-side the work room and then automatically taken into the right machining position, are increasingly being used.

    Tool change facilities

    Figure 12 Example of a turret

    CNC tool machines are equipped with controllable automatic tool change facilities. Depending on the type and application area these tool change facilities can simultaneously take various quantities of tools and set the tool called by the NC program into work-ing position. The most common types are: the tool turret the tool magazine. The tool turret (see figure 12) is mostly used for lathes and the tool magazine for milling machines. If a new tool is called by the NC program the turret rotates as long as the required tool achieves working position. Presently such a tool change only takes fractions of seconds.

    Depending on the type and size, the turrets of the CNC machines have 8 to 16 tool places. In large milling centers up to 3 turrets can be used simultaneously. If more than 48 tools are used tool magazines of differ-ent types are used in such machining centers allowing a charge of up to 100 and even more tools. There are longitudinal magazines, ring magazines, plate magazines and chain magazines (see figure 13) as well as cassette magazines.

    MTS TeachWare CNC-Grundlagen Students Book 18

  • Introduction into CNC Technology

    Figure 13 Example of a chain magazine

    1 2

    3

    4

    Figure 14 Automatic tool change facility

    milling tools

    tool gripper (tool changer)

    work spindle

    tool magazine

    In the tool magazine the tool change takes place using a gripping system also called tool changer (see figure 14). The change takes place with a double arm gripping device after a new tool has been called in the NC program as follows: Positioning the desired tool in magazine into tool changing position Taking the work spindle into changing position Revolving the tool gripping device to the old tool in the spindle and to the new tool in the magazine Taking the tools into the spindle and magazine and revolving the tool gripping device Placing the tools into the spindle sleeve or magazine Returning the tool gripping device into home position The tool change procedure takes between 6 to 15 seconds, whereby the quickest tool changers are able to make the tool change in merely one second.

    Security precautions on CNC machine tools The target of work security is to eliminate accidents and damages to persons, machines and facilities at work site. Basically the same work security precautions apply to working on CNC machines as to conventional ma-chine tools. They can be classified in three categories:

    Danger elimination Defects on machines and on all devices necessary for work need to be registered at once. Emergency exits have to be kept free. No sharp objects should be carried in clothing. Watches and rings are to be taken off.

    Screening and marking risky areas: The security precautions and corresponding notifications are not allowed to be removed or inacti-vated. Moving and intersecting parts must be screened.

    Eliminating danger exposure Protective clothing must be worn to protect from possible sparks and flashes.

    MTS TeachWare CNC-Grundlagen Students Book 19

  • Instroduction into CNC technology

    Protective glasses or protective shields must be worn to protect the eyes. Damaged electrical cables are not allowed to be used.

    When setting up and operating CNC machines the following is to be taken into consideration:

    In general, setting-up is allowed only on a machine which has been switched off. The only exceptions being the operations which required the machine power to be switched on, such as re-setting the work part with tools.

    The operator should not go to the rotation or work area of the machine since within this area the ma-chine can automatically rotate the turrethead or feed the tool carrier.

    The specific security precautions of the machine manufacturer have to be followed. The following security precautions are to be followed as well:

    Blocking system against loose parts or parts which have not been allocated correctly, against auto-generated movement of not fixed elements and against starting an automatic machining procedure before setting-up work has been completed.

    Blocking system of the work part clamping device when charging the CNC machine manually. Keeping the security distance between the parts of the neighbouring CNC machines coming closest to

    the machine in a system where CNC machines are connected with each other and

    protection against chips and coolant splashes. Sucking off the machine room air.

    Workshop Clarification of machine parts of CNC machines in the workshop. The parts of machine tools should be shown and explained on the available machine tools. Similarities and differences between conventional machine tools and CNC machine tools are to be emphasized.

    MTS TeachWare CNC-Grundlagen Students Book 20

  • Instroduction into CNC technology

    Control test CNC Basics

    1. Discuss relevant differences between CNC machine tools and conventional machine tools.

    1. Name characteristic features of numerically controlled machine tools!

    1. What are the advantages of CNC machine tools compared with conventional machine tools?

    1. Why is it necessary to have adjustable feed axes on CNC machines?

    1. Which components make up a modern feed drive?

    1. How many feed axes at minimum should be available on a CNC lathe?

    1. What are the feed axes called?

    1. How many feed axes at minimum should be available on a CNC milling machine?

    1. What are the feed axes called?

    1. Give some examples of controllable rotation axes on CNC machines!

    1. Which operations can be achieved by controllable rotation axes on CNC lathes?

    1. Which operations can be achieved by controllable rotation axes on CNC milling machines?

    1. Discuss the significance and function of a ball screw!

    1. Discuss the difference between direct and indirect position measuring?

    1. Discuss the difference between absolute and incremental position measuring?

    1. What are the advantages of main drive motors with controllable number of rotations?

    1. Which automatic tool installations are available on CNC machine tools?

    1. Which types of tool magazines are available on CNC milling machines?

    MTS TeachWare CNC-Grundlagen Students Book 21

  • Basic Geometry for CNC Machining

    MTS TeachWare CNC-Grundlagen Students Book 22

  • Basic Geometry for CNC Machining

    3. Basic Geometry for CNC Machining

    2.1 Coordinate systems on CNC machine tools

    Types of coordinate systems Coordinate systems enable the exact description of all points on a work plane or room. Basically there are two types of coordinate systems:

    Cartesian coordinate system and polar coordinate system.

    Cartesian coordinate system A Cartesian coordinate system, also called rectangular coordinate system includes for the exact description of the points

    two coordinate axes (two-dimensional Cartesian coordinate system) or also three coordinate axes (three-dimensional Cartesian coordinate system),

    located vertically to each other. In the two-dimensional Cartesian coordinate system, e.g. in the X, Y coordinate system, each point on the plane is explicitly defined (see figure 15). The distance from the Y axis is called the X coordinate and the distance from the X axis is called Y axis. These coordinates can either have a positive or a negative sign.

    Y

    X

    P1P2

    P3P4

    Figure 15 Cartesian coordinate system with 2 axis (X;Y)

    Example:

    P1 X= 80 Y= 40

    P2 X= -80 Y= 70

    P3 X= -50 Y= -40

    P4 X= 40 Y= -70

    If a work part drawing is placed in this coordinate system all important work points can be determined. De-pending on where the zero point of the work part is placed, it is possible to exactly define the points either with positive or also with negative coordinates.

    MTS TeachWare CNC-Grundlagen Students Book 23

  • Basic Geometry for CNC Machining

    The three-dimensional Cartesian coordinate system is necessary for the description and location specifica-tion of three-dimensional work parts, e.g. milling parts. To describe a point in space three coordinates are required. These are called X, Y or Z according to the corresponding axis (see figure 16). Such three-dimensional coordinate systems with positive and negative areas of the coordinate axis enable the exact description of all points, for instance in the operating space of a milling machine, regardless of where the zero point of the work part is positioned.

    X

    YZ

    P1

    P2

    Figure 16 Cartesian coordinate system with 3 axes (X,Y,Z)

    Example:

    P1 X= 30 Y= 20 Z= 0

    P2 X= 30 Y= 0 Z= -10

    The specifications of the three axes as well as the three coordinates is done as a so-called clockwise-rotating system and follows the right-hand-rule (see figure 17). The fingers of the right hand always show to the positive direction of each axis. This system is also called the clockwise-rotating coordinate system.

    +X

    +Y

    +Z

    Figure 17 Right-hand-rule

    MTS TeachWare CNC-Grundlagen Students Book 24

  • Basic Geometry for CNC Machining

    Polar coordinate system

    In the Cartesian coordinate system a point is described, for instance, by its X and Y coordinates. For rotation symmetrical contours, such as circular boring patterns, calculating the needed coordinates requires exten-sive computing. In the polar coordinate system a point is specified by its distance (radius r) to the point of origin and its angle () to a specified axis. The angle () refers to the X axis in the X,Y coordinate system. The angle is positive, if it is measured counterclockwise starting from the positive X axis (see figure 18). In the opposite direction it is negative (see figure 19).

    P

    Y

    X

    r

    P

    Y

    X

    r

    Figure 18 Polar coordinate system (positive angle )

    Figure 19 Polar coordinate system (negative angle )

    Rotation angle of axis Each of the 3 main axes X, Y and Z also have a rotation axis revolving around the corresponding angle. These rotation angles of the axes are indicated with A, B, C, whereby A rotates on the X, B on Y and C on Z axis (see figure 20). The rotation direction is positive if the rotation is clockwise when seen from the coordinate zero point in the positive coordinate direction (corresponds to the rotation of a screw with a right-hand thread or the rotation direction of a corkscrew). The specification of the angles A, B and C of the polar coordinates can be derived from figure 20. If the point which is to be approached is located on the X/Y plane of the coordinate system, then the polar coordinate angle corresponds to the rotation angle on the Z axis, i.e. C. On the Y/Z plane the polar coordinate angle corresponds to the rotation angle on X axis, i.e. A. In the X/Z plane it corresponds to the rotation angle Y, i.e. B.

    Figure 20

    MTS TeachWare CNC-Grundlagen Students Book 25

  • Basic Geometry for CNC Machining

    Axis angle of rotation with rotation direction

    Coordinate system definition with reference to machine or work part

    Machine coordinate system The machine coordinate system of the CNC machine tool is defined by the manufacturer and cannot be changed. The point of origin for this machine coordinate system, also called machine zero point M, cannot be shifted in its location (see figure 21). Work part coordinate system The work part coordinate system is defined by the programmer and can be changed. The location of the point of origin for the work part coordinate system, also called work part zero point W, can be specified as desired (see figure 22).

    M XY

    Z

    M Machine zero point

    X

    YZ

    W

    W Work part zero point

    Figure 21 Machine coordinate system

    Figure 22 Work part coordinate system

    CNC milling machine The design of the CNC machine specifies the definition of the respective coordinate system. Correspond-ingly, the Z axis is specified as the working spindle (tool carrier) in CNC milling machines (see figure 23), whereby the positive Z direction runs from the work part upwards to the tool.

    MTS TeachWare CNC-Grundlagen Students Book 26

  • Basic Geometry for CNC Machining

    For an easier calculation of the points needed for programming it is advisable to use the outer edges of the upper (see figure 24) or the lower area (see figure 25).

    Figure 23 Milling part in three-dimensional Cartesian coordinate system

    The X axis and the Y axis are usually parallel to the clamping plane of the work part. When standing in front of the machine the positive X direction runs to the right and the Y axis away from the viewer. The zero point of the coordinate system is rec-ommended to be placed on the outer edge of the work part.

    X

    YZ

    Figure 24 Work part zero point in the upper left outer edge

    Figure 25 Work part zero point in the lower left outer edge

    CNC lathes In the CNC lathes the working spindle (tool carrier) is specified as Z axis. This means the Z axis is identical to the rotation axis (see figure 26 and 27). The direction of the Z axis is specified so that the tool withdraws from the work part when moving to the positive axis direction. The X axis is located in a right angle to the Z axis. However, the direction of the X axis always depends on if the tool is located in front of (see figure 26) or behind (see figure 27) the rotation center.

    MTS TeachWare CNC-Grundlagen Students Book 27

  • Basic Geometry for CNC Machining

    W

    +X

    +Z

    W

    +X

    +Z

    Figure 26 Milling work part in Cartesian coordinate system with 2-axis tool in front of the rotation center

    Figure 27 Milling work part in Cartesian coordinate system with 2-axis tool behind the rotation center

    CNC-Exercise Working with different coordinate systems

    Y

    X

    a

    b

    c

    d

    Enter the coordinates of the points in the table.

    X Y

    a

    b

    c

    d

    MTS TeachWare CNC-Grundlagen Students Book 28

  • Basic Geometry for CNC Machining

    MTS TeachWare CNC-Grundlagen Students Book 29

    Y

    X

    Enter the following points in the diagram.

    X Y

    a 10 20

    b -80 -30

    c 40 -70

    d -30 50

    X

    YZ

    b

    ac

    d

    Enter the Cartesian coordinates of the points a to d in the table.

    X Y Z

    a

    b

    c

    d

  • Basic Geometry for CNC Machining

    Enter the Cartesian coordinates of the points a to h in the table.

    ab c

    d

    efg

    h

    X Y

    a

    b

    c

    d

    e

    f

    g

    h

    In a drawing milling work parts are specified by their diameter. Therefore, the diameter is also included for programming. Enter the Cartesian coordinates of the points a to g in the table. Determine the corresponding diameter val-ues of the X coordinates!

    a

    bc

    de

    fg

    X Z

    a

    b

    c

    d

    e

    f

    g

    MTS TeachWare CNC-Grundlagen Students Book 30

  • Basic Geometry for CNC Machining

    Feed and Turning Axes on CNC Machines

    Location and Designation of the NC axes

    CNC milling machines differ in their design with respect to the layout of the working spindles and the location of the NC axes (see figure 28 and 29). The Z axis is identical with the rotation axis of the working spindle. The positive Z direction is specified to run from the work part to the tool. Since a three-dimensional Cartesian coordinate system is used, the other two coordinate axes can be determined by the right-hand-rule.

    +Y

    -Y

    -X

    +X

    +Z

    -Z

    -Y

    +Y

    +Z

    -Z

    -X

    +X

    Figure 28 Axis on the vertical milling machine

    Figure 29 Axis on the horizontal milling machine

    In a CNC lathe the working spindle is defined as the Z axis (see figure 30). The positive Z direction runs from the work part to the tool. The X axis is vertical to the Z axis. The positive direction of the X axis runs here to the rear (tool behind the rotation center). One rotation axis - the C axis - is available when the working spin-dle is approached..

    +XC

    +Z

    Figure 30 Axes on the lathe

    MTS TeachWare CNC-Grundlagen Students Book 31

  • Basic Geometry for CNC Machining

    Directions of motion on CNC machine tools

    During machining relative motions between the work part and tool have to take place on the available axes. The axes of CNC machine tools are specified by their design (see chapter Location and marking of the NC axis). They refer to the work part, whereby a three-dimensional Cartesian coordinate system is used. It is always assumed that only the tool moves, even though tool carrier of the vertical milling machine shown below moves along the X and Z axes (see figure 31).

    +Y

    +X

    +Z

    Figure 31 Directions of motion on a milling machine

    To be able to program regardless of machine, the following definition is introduced.

    During programming it is always assumed that the tool moves. The coordinate system always refers to the work part.

    Using this definition the work part coordinates can always be applied to generate the NC program.

    NC compatible dimensioning

    Two different types of dimensioning are used in NC programming:

    absolute dimensioning and incremental dimensioning (incremental values).

    Absolute dimensioning always refers to the work part zero point, i.e. reference dimensions are used (see figure 32). In contrast, incremental dimensioning uses incremental values which are always measured from the current point to the next point (see figure 33). When turning, the X values for absolute dimensioning are diameter values, whereas for incremental dimen-sioning they refer to radius values.

    -Z

    +X

    -Z

    +X

    Figure 32 Example for absolute dimensioning

    Figure 33 Example for incremental dimensioning

    MTS TeachWare CNC-Grundlagen Students Book 32

  • Basic Geometry for CNC Machining

    MTS TeachWare CNC-Grundlagen Students Book 33

    Absolute dimensioning is recommended for programming, because of the following advantages compared with incremental dimensioning:

    measuring tolerances do not cumulate, changes of individual values do not necessarily influence the subsequent dimensions, one incorrect value does not lead to subsequent errors, absolute coordinates indicate the current traverse path distance from the tool, so that single program

    steps can be traced back more easily. NC compatible drawings should therefore avoid incremental values and use coordinate values referring to one reference point. Despite these advantages it is not always possible to avoid incremental dimensioning in programming. It is, for example, an advantage when several identical contour parts, such as recesses, are consecutively ma-chined.

  • Basic Geometry for CNC Machining

    4. CNC-Demo Controllable NC axes on the CNC simulator

    Similar to a real CNC machine tool, the CNC simulator also permits manual travel along the NC axes. Sub-sequently, the necessary steps on a CNC simulator are described.

    When entering data, only the indicated keys are to be pressed (for example, F5 corresponds to the function key F5)

    CNC milling

    Description Entry

    1. Call CNC milling in the main menu. F2 (Milling)

    2. Select setup mode. F3 (Setup mode) (NUM keyboard ON)

    3. Go to X, Y or Z axis and check the travel path. Press the corresponding key on the numerical keyboard.

    5 +X-X

    0Einfg

    +Z

    -Z

    +Y

    -Y

    64

    ,Entf

    3Bild

    9Bild

    7Pos 1

    1Ende

    8

    2

    6 4 9Bild

    1Ende

    8 2

    Travel directions available:

    ( + X - direction )

    ( - X - direction )

    ( + Y - direction )

    ( - Y - direction )

    ( + Z - direction )

    ( - Z - direction )

    The travel path can be checked using the displayed axis coordinates.

    4. Quit the setup menu F8 (Quit)

    CNC-Exercise: With the CNC simulator each student practices moving along the NC axes.

    MTS TeachWare CNC-Grundlagen Students Book 34

  • Basic Geometry for CNC Machining

    CNC turning

    Description Entry

    1. Call CNC turning in the main menu. F1 (Turning)

    2. Select setup mode. F3 (setup mode) (NUM keyboard ON)

    3. Go to the X or Z axis and check the travel path.

    Press the corresponding key on the numerical keyboard.

    5 +Z-Z

    0Einfg

    +X

    -X

    64

    ,Entf

    3Bild

    7Pos 1

    8

    2

    6 4 8 2

    Travel directions available:

    ( + Z - direction )

    ( - Z - direction )

    ( + X - direction )

    ( - X - direction )

    The travel path can be checked using the displayed axis coordinates.

    4. Quit the setup menu. F8 (Quit)

    CNC-Exercise: With the CNC simulator each student practices moving along the NC axes. Workshop Using the CNC machines available the students move along the controllable NC axes. Hereby the corre-sponding operation instructions of the machine have to be followed. Exercise: With the CNC simulator each student practices moving along the NC machine tool.

    MTS TeachWare CNC-Grundlagen Students Book 35

  • Basic Geometry for CNC Machining

    2.2 NC Mathematics

    Basics of coordinate point calculations When programming a CNC program the corresponding points of the contour to be machined have to be entered. In most cases it is possible to directly take these point from the drawing, providing the drawing di-mensions are NC compatible. In some cases it is however necessary to calculate coordinate points.

    Characteristic values of a triangle

    To calculate the missing coordinates the relations within a triangle are very helpful. There are various possi-bilities to describe a triangle. Some of the following characteristic values, such as corner points, angles or sides are used (see figure 34).

    A B

    C

    ab

    c

    Figure 34 Characteristic values of a triangle

    Corner points A, B and C mark the three corner points of a triangle. Angles , and are the corresponding angles in the corners of the triangle. Sides a, b and c mark the sides of the triangle op-posite to the corners A, B and C. The component parts of the triangle are al-ways marked counterclockwise.

    Angles of the triangle

    The angles of the triangle specify the type of the triangle. Depending on the sizes of the triangle angles the triangle is either an acute-angled, obtuse or right-angled triangle (see figure 35 - 37)

    A B

    C

    ab

    c

    A B

    C

    ab

    c

    A B

    C

    ab

    c

    Figure 35 Acute-angled triangle All angles are smaller than 90.

    Figure 36 Obtuse triangle One angle is larger than 90.

    Figure 37 right-angled triangle One angle is 90.

    For a triangle the relation applies: the sum of the triangle angles , and is always 180.

    + + = 180o With this formula it is possible to calculate one unknown angle if the other two angles are known.

    MTS TeachWare CNC-Grundlagen Students Book 36

  • Basic Geometry for CNC Machining

    Right-angled triangle

    The right-angled triangle (see figure 38) has a special significance in analytical geometry, since the sides of such a triangle stand in a certain mathematical relation to each other. The sides of a right-angled triangle have specific names:

    The longest side is located opposite the right angle and is called hypotenuse. The two sides of the triangle forming the right angle are each called cathetus

    or together the legs of the right-angled triangle. The side which is located opposite the angle is called counter cathetus. The side located adjacent to the angle is called adjacent cathetus.

    In a right-angled triangle the right angle (see figure 38) is described by a quarter circle and a point within the angle.

    2

    3

    1

    counter cathetus

    adjacent cathetus

    hypotenuse

    right angle

    Figure 38 Right-angled triangle

    The following applies for a right-angled triangle: In a right-angled triangle it is possible to calculate the length of an unknown side if the other two side lengths are known. For this, the Pythagorean theorem (see figure 39) is used.

    c

    a

    b

    bc

    a

    Figure 39 The Pythagorean theorem

    The Greek Pythagoras (approx. 580 - 496 BC) was the first to verify the following mathematical relation which was called after him

    the Pythagorean theorem

    The sum of the squares of the legs of a right triangle is equal to the

    square of the length of the hypote-nuse.

    or expressed as an equation:

    a b c2 2 2+ = With the corresponding transformation the sides of the triangle can be calculated as follows:

    a c b= 2 2

    b c a= 2 2

    c a b= +2 2

    MTS TeachWare CNC-Grundlagen Students Book 37

  • Basic Geometry for CNC Machining

    Trigonometric functions

    The trigonometric functions describe the relation between the angle and the sides of the right angle. With these trigonometric functions it is possible to calculate unknown side lengths if one angle and the length of one side is known. The choice of the trigonometric function between sine function (see figure 40), cosine function (see figure 41) or the tangent function (see figure 42) depends on which side and angle are known.

    1

    2

    counter cathetus

    hypotenuse

    sin counter cathetushypotenuse =

    Figure 40 Sine function

    1

    2

    adjacent cathetus

    hypotenuse

    cos adjacent cathetushypotenuse =

    Figure 41 Cosine function

    1

    2

    counter cathetus

    adjacent cathetus

    tan counter cathetusadjacent cathetus =

    Figure 42 Tangent function

    When calculating the unknown side the corresponding equations need to be transformed according to the following example:

    known values: the angle and the length of the adjacent cathetus

    unknown value: the length of the counter cathetus

    equation: tan counter cathetusadjacent cathetus = (see figure 42), resulting in:

    counter cathetus adjacent cathetus tan=

    MTS TeachWare CNC-Grundlagen Students Book 38

  • Basic Geometry for CNC Machining

    MTS TeachWare CNC-Grundlagen Students Book 39

    Calculation of NC coordinates Work part drawings are not always dimensioned NC-compatible. In addition to incremental values, angle values are also frequently given in drawings. Consequently, when programming manually the programmer has to calculate unknown Cartesian coordinates using the points to be programmed. In the following drawing the coordinates of the points b, c and f need to be calculated. The other points are known.

    25

    a b

    c d

    ef

    g

    X

    Y

    25

    X Y

    a 15 15

    b ? 15

    c ? 35

    d 85 35

    e 85 85

    f ? 85

    g 15 65

    Calculation of the point b:

    b 25

    ?

    dx

    known : x from center point = 65 mm

    unknown : x from point b = ?

    solution : x = 65 mm - dx

    dx = radius of the arc

    dx = 25 mm

    x = 65 mm - 25 mm

    x = 40 mm

    Calculation of the point c:

    c

    25

    ?

    dx

    dy

    known : x from center point = 65 mm

    radius of the arc r = 25 mm

    dy = 35 mm - 15 mm = 20 mm

    unknown : x from point c = ?

    solution : x = 65 mm + dx equation: dx r dy= 2 2

    ( )

    ( )dx mm mm= 25 202 2 dx mm= 225 2 dx mm= 15 x = 65 mm + 15 mm

    x = 80 mm

  • Basic Geometry for CNC Machining

    25

    fdx

    ?dy

    known : x from the beginning of the incline = 15 mm

    angle of the incline = 25 dy = 85 mm - 65 mm = 20 mm

    unknown : x from point f = ?

    solution : x = 15 mm + dx equation: counter cathetus = adjacent cathesis * tan

    dx = 20 mm * tan 25 dx = 20 mm * 0.4663 dx = 9.326 mm x = 15 mm + 9.326 mm

    x = 24.326 mm

    CNC exercise Enter the Cartesian coordinates from the center points of the drillings a to h in the table. Give all values rounded to three decimal points.

    abc

    d

    ef g

    h60

    X

    Y

    100

    100

    50

    50

    X Y

    a

    b

    c

    d

    e

    f

    g

    h

    Calculate the unknown coordinates in the following examples.

    30

    80

    80?

    90

    35

    ?

    5070

    85

    85

    unknown : Y coordinate unknown: Y coordinate

    MTS TeachWare CNC-Grundlagen Students Book 40

  • Control test Basic Geometry

    2.3 Zero and reference points on CNC machine tools

    Types of zero and reference points

    M machine zero point

    W work part zero point

    R reference point

    E tool reference point

    B tool setup point

    A tool shank point

    N tool change point

    ER

    N

    WM

    Figure 43 Location of the zero and reference points for turning

    Machine zero point M Each numerically controlled machine tool works with a machine coordinate system. The machine zero point is the origin of the machine-referenced coordi-nate system. It is specified by the machine manufac-turer and its position cannot be changed. In general, the machine zero point M is located in the center of the work spindle nose for CNC lathes and above the left corner edge of the work part carrier for CNC ver-tical milling machines.

    R

    N

    W

    AM

    Figure 44 Location of the zero and reference point for milling

    Reference point R A machine tool with an incremental travel path meas-uring system needs a calibration point which also serves for controlling the tool and work part movements. This calibration point is called the refer-ence point R. Its location is set exactly by a limit switch on each travel axis. The coordinates of the reference point, with reference to the machine zero point, always have the same value. This value has a set adjustment in the CNC control. After switching the machine on the reference point has to be ap-proached from all axes to calibrate the incremental travel path measuring system.

    MTS TeachWare CNC-Grundlagen Students Book 41

  • Basic Geometry for CNC Machining

    W

    M

    +X

    +Z

    WM

    +X

    +Z

    Figure 45 Work part zero point of the turned part

    Work part zero point W The work part zero point W is the origin of the work part-based coordinate system. Its location is speci-fied by the programmer according to practical criteria. The ideal location of the work part zero point allows the dimensions to be directly taken from the drawing. In case of turning the work part zero point is gener-ally in the center of the left or right side of the com-pleted part, depending on which side the dimension-ing was started from. The work part zero point can be shifted in the NC program, e.g. when a turned part is to be completely machined between centers on two sides. In this case it is advisable to alternately shift the work part zero point to the right or left side of the machined part.

    X

    YZ

    Figure 46 Work part zero point of a milled part.

    For milling, the outer corner point is usually chosen as the work part zero point, depending on which cor-ner point is selected as the reference point when dimensioning the work part.

    Tool reference point E A further important point in the machine work space is the tool reference point E. The tool reference point E of a CNC lathe is a fixed point on its tool carrier. On a CNC milling machine the tool reference point E is lo-cated on the tool spindle. The CNC control refers first to the tool reference point for all target point coordinates. When programming the target coordinates either the tool tip of the turning tool or the center of the milling tool is referred to. To be able to control exactly the tool tip in turning or the tools in milling along the desired machining travel path they have to be measured precisely. It is possible to measure the tools either outside the machine with a preset device or directly on the machine using special optics. When using an optic, the measured values are

    MTS TeachWare CNC-Grundlagen Students Book 42

  • Control test Basic Geometry

    directly entered into the machine storage. If however the preset device is used the measured values need to be entered manually for each tool into the corresponding compensation value storage of the control. Two additional points are needed to preset the tool outside the CNC machine. These are the tool setup point B and the tool shank point A.

    B

    R

    Q

    L

    Figure 47 Tool setup point of a turning tool

    Location of the tool setup point B on a turning tool B tool setup point L length = distance of the cutter tip to the tool setup

    point in X Q overhang = distance of the cutter tip to the tool

    setup point in Z R cutter radius

    B

    R

    L

    Figure 48 Tool setup point of a milling tool

    Location of the tool setup point at B of a milling tool B tool setup point L length = distance of the cutter tip to the tool setup

    point in Z R radius of the milling tool

    A

    Figure 49 Toolholding point of a turret

    Location of the toolholding point A on a turret A toolholding point

    If the tool system (tool post with tool) is placed into the tool carrier (i.e. a turret), then the tool setup point B and the toolholding point A fall together and make up the tool reference point E. Tool change point N The tool change point N is the point in the CNC machine work space on which the tools can be changed without collision. In most CNC controls the tool change point can be configured.

    MTS TeachWare CNC-Grundlagen Students Book 43

  • Basic Geometry for CNC Machining

    MTS TeachWare CNC-Grundlagen Students Book 44

    Setting the work part zero point W on a CNC lathe Setting the work part zero point W coordinates the work part zero point with the drawing zero point. The drawing dimensions can then be used directly for programming.

    M W

    zw

    Figure 50 Setting the work part zero point on a CNC lathe

    Setting the work part zero point is done with refer-ence to the machine zero point M of the CNC ma-chine. The machine zero point of a lathe is generally located on the rotation axis of the main spindle on the plane surface of the spindle flange on which the jaw chuck is flanged (see figure 50). Using the operation functions described below the distance between the machine zero point M and the work part zero point W is specified. This value zw, also called the zero point shift, is then entered into the CNC control.

    Procedure

    Starting situation: All machining tools have been measured and are available on the turret head. The clamping device is prepared and the work part has been correctly clamped.

    1. Switch on the spindle (counterclockwise rotation).

    1. Change the tool to set the work part zero point, i.e. rotate the turret head to the corresponding position, for instance T02.

    Note: The rotation area of the turret has to be checked first to avoid collision during rotation.

    3. Touch the front plane area of the work part: carefully move with the tool using the hand wheel or using the corresponding arrow keys of the keyboard of the CNC control until the cutting edge reaches a marking on the work part.

    3. Enter the desired plane area allowance (e.g. 0.5 mm) on the CNC control. Actuate with the zero key. (The dimensions are used to face the front surface in z=0)

    3. The CNC control then stores the value of the zero point shift zw. The work part zero point W is clearly specified since the X coordinate zero is located on the rotation axis.

    3. Because of eventual allowance the front side needs to be faced. This needs to be considered when pro-gramming the NC program.

  • Control test Basic Geometry

    Setting the work part zero point W on a CNC milling machine Similar to a lathe the work part zero point corresponds with the drawing zero point when the work part zero point W is set on a CNC milling machine. This allows the drawing data to be directly used for programming.

    R

    N

    W

    AM

    Figure 51 Setting the work part zero point on a CNC milling machine

    The work part zero point is set with reference to the machine zero point M. In most cases the machine zero point of a CNC vertical milling machine is lo-cated above the left corner edge of the machine table (see figure 51). With the operations described below the distance is specified between the machine zero point M and the work part zero point W in the three coordinates X, Y and Z. These values are then entered into the CNC control. Procedure Starting situation:

    The work part is adjusted and firmly clamped in the machine table. All tools are gauged to each other. The corresponding compensation values were en-tered into the CNC control. The zero setting tool is clamped and the spindle rotation is switched on. 1. Resetting Z direction

    W

    Z Y

    X

    Figure 52 Resetting in Z

    The machine table with the clamped work part is moved below the work spindle (in X and Y) in which the reset tool is clamped. Now the tool is recessed in Z direction to the work part surface (X, Y plane), with the spindle switched on (see figure 52), until a small marking is made on the work part (touching the work part) surface. After this the Z axis is reset and the Z value of the work part zero point W is transferred and stored into the CNC control using the IST key. 2. Resetting in X direction

    W

    Z Y

    X

    Figure 53 Resetting in X

    The tool is raised again and taken into the new reset-ting position for the X axis. With the spindle switched on it is moved along the side surface of the work part (Y, Z plane) in the X direction (see figure 53) until a small marking is made on the work part surface (touching the work part). When touching the work part in X axis the radius of the applied tool has to be considered when confirm-ing the value with the IST key, since the center point coordinates of the tool are always used in NC pro-gramming. If the milling tool of the adjacent figure has, for in-stance, a radius of 15 mm, then the value X=-15 is entered into the NC control and confirmed with IST. .

    MTS TeachWare CNC-Grundlagen Students Book 45

  • Basic Geometry for CNC Machining

    W

    Z Y

    X

    Figure 54 Resetting in Y

    3. Resetting in Y direction The last step is to take the tool to resetting position for the Y axis. With the spindle switched on, the tool is taken into Y direction (see figure 54), to the side surface of the work part (X, E Plane) until a small marking is done on the work part surface (touching the work part). When touching the work part in X axis the radius of the applied tool has to be considered when confirm-ing the value with the IST key, since the center point coordinates of the tool are always used in NC pro-gramming. If the tool of the adjacent figure has, for instance, a radius of 15 mm then the value Y=-15 is entered into the CNC control and confirmed with IST.

    MTS TeachWare CNC-Grundlagen Students Book 46

  • Control test Basic Geometry

    CNC exercise Setting the work part zero point W in the CNC simulator Turning

    By setting the work part zero point W the relation between the machine based and work part based coordi-nate system is created. The work part zero point corresponds to the drawing zero point. Consequently, the drawing dimensions can be used in programming. Using the operation steps described below the distance between the machine zero point M and the work part zero point W can be specified. This Z value is also called the zero shift zw.

    M W

    zw

    Starting situation:

    All machining tools are dimensioned and available on the turret head.

    The work part is clamped in chuck jaws. The work part zero point is located on the front

    plane surface, whereby an allowance of 1mm has to be considered.

    Description Entry

    1. Call CNC turning in the main menu. F1 (Turning)

    2. Select setup mode. F3 (Setup mode)

    3. Switch on the spindle in counterclockwise rotation.

    Type M04 using the keyboard and

    confirm.

    4. Change the tool for the definition of the work part zero point.

    Type T0404 using the keyboard and confirm.

    5. Move the lathe tool in rapid speed so that it is located in front of the front plane surface with a distance of approx. 5mm to the front plane surface.

    +Z

    +X

    Using the numeric keyboard press the corre-sponding arrow key simultaneously with the shift key:

    + 4 for rapid speed in -Z direction

    + 2 for rapid speed in -X direction

    5 +Z-Z

    0Einfg

    +X

    -X

    64

    ,Entf

    3Bild

    7Pos 1

    8

    2

    6 4 8 2

    Travel direction options:

    ( + Z - direction )

    ( - Z - direction )

    ( + X - direction )

    ( - X - direction )

    MTS TeachWare CNC-Grundlagen Students Book 47

  • Basic Geometry for CNC Machining

    6. Switch the increment from 1mm to 0,1mm or

    0,01 mm for further machining. . F3

    F5

    F2

    (Technology)

    (Increment)

    (Increment 0.1)

    7 Move the lathe tool in negative Z-direction until it touches the plane surface of the work part .

    4

    ESC

    F8

    Press the arrow key on the numeric keyboard.

    Then press

    and

    (Quit).

    8. Set the work part zero point in Z. F4 F4 F1

    F8

    (Tool datum)

    (Set datum)

    (Set Z coord.)

    Type z+1using the keyboard and confirm

    with (allowance of 1mm).

    The Z value can be checked for the current zero point using the displayed coordinates.

    9. Take the tool off in +Z direction and in +X direction .

    Using the numeric keyboard press the arrow key together with the shift key:

    + 6 for rapid speed in +Z direction

    + 8 for rapid speed in +X direction

    10. Quit the setup mode F8 F8 F8

    (Quit)

    (Quit)

    (Quit)

    MTS TeachWare CNC-Grundlagen Students Book 48

  • Control test Basic Geometry

    Setting the work part zero point W in the CNC simulator milling

    In milling, setting the work part zero point W coordinates the work part zero point with the drawing zero point. Please note that only the tool moves in the MTS simulator! Using the operation steps described below the distance between the machine zero point M and the work part zero point W in the three coordinates X, Y and Z is defined.

    W

    Z Y

    X

    Starting situation:

    All machining tools are dimensioned and avail-able in the magazine.

    The work part is adjusted and clamped on the machine table in the simulator.

    The location of the work part zero point should be the left top corner of the work part.

    Description Entry

    1. Call CNC milling in the main menu. F2 (Milling)

    2. Select the setup mode. F3 (Setup mode)

    3. Switch on the spindle in clockwise rotation.

    Type M03 using the keyboard and

    confirm.

    4. Change the tool to define the work part zero point.

    Type T0202 using the keyboard and

    confirm.

    5. Setting the zero point in Z direction Move the tool in rapid speed to a position approx. 5mm above the work part surface.

    W

    ZY

    X

    Using the numeric keyboard press the corre-sponding arrow key together with the shift key:

    Ex.: + 2 for rapid speed in -Z direction.

    5 +X-X

    0Einfg

    +Z

    -Z

    +Y

    -Y

    64

    ,Entf

    3Bild

    9Bild

    7Pos 1

    1Ende

    8

    2

    6

    4 9Bild

    1Ende

    8 2

    Further travel direction options:

    ( + X direction )

    ( - X direction )

    ( + Y direction )

    ( - Y direction )

    ( + Z direction )

    ( - Z direction )

    MTS TeachWare CNC-Grundlagen Students Book 49

  • Basic Geometry for CNC Machining

    6. Switch the increment from 1mm to 0,1mm or

    0,01mm for further machining. F3

    F5

    F2

    (Technology)

    (Increment)

    (Increment 0.1)

    7 Move the tool in negative Z direction until it touches the surface of the work part.

    2

    ESC

    F8

    Press the arrow key on the numeric keyboard

    Then press

    and

    (Quit).

    8. Set the work part zero point in Z. F4 F4 F3

    F8

    (Tool/ Datum)

    (Set Datum)

    (set Z coord.)

    Type in the data on the keyboard 0 and

    confirm it.

    Check Z by setting the zero point and using the dis-played coordinate values.

    9. Setting the zero point in X direction Withdraw the tool in +Z direction.

    Using the numeric keyboard press the arrow

    key together with the shift key:

    + 8 for rapid speed in +Z direction

    10. Move the tool in rapid speed to the new zero setting position approx. 5mm off the side sur-face.

    W

    ZY

    2

    1

    X

    Press the corresponding arrow key on the numeric keyboard

    together with the shift key:

    1) in -X direction

    + 4 for rapid speed in -X direction 2) in -Z direction

    + 2 for rapid speed in -Z direction

    MTS TeachWare CNC-Grundlagen Students Book 50

  • Control test Basic Geometry

    11. Move the tool in positive X direction until it

    touches the left side of the work part.

    6 ESC

    F8

    Press the arrow key on the numeric keyboard.

    Then press

    and

    (return).

    12. Set the work part zero point in X.

    Please note the tool radius!

    So, enter for the X coordinate the negative value of the radius of the applied tool, for in-stance -10.

    F4 F4 F1

    F8

    (tool, zero point)

    (set datum)

    (set X coordinate)

    Type -10 using the keyboard and confirm.

    Check the X by setting the zero point using the dis-played coordinate values.

    13. Setting the zero point in Y direction Take off the tool in -X direction and then in +Z direction.

    Using the numeric keyboard press the arrow key together with the shift key:

    + 4 for rapid speed in -X direction then

    + 8 for rapid speed in +Z direction.

    14. Take the tool in rapid speed to the new reset-ting position approx. 5mm off the front side.

    W

    ZY

    2

    1

    3X

    Using the numeric keyboard press the corre-sponding arrow key together with the shift key:

    1) in +X direction

    + 6 for rapid speed in +X direction 2) in -Y direction

    + 1Ende for rapid speed in -Y direction 3) in -Z direction

    + 2 for rapid speed in -Z

    MTS TeachWare CNC-Grundlagen Students Book 51

  • Basic Geometry for CNC Machining

    15. Take the tool in positive Y direction until it

    touches the front of the work part.

    9Bild ESC

    F8

    Press the arrow key on the numeric keyboard.

    Then press

    and

    (Quit).

    16. Set the work part zero point in Y.

    Please, note the tool radius!

    So, enter for the Y coordinate the negative value of the radius, for instance -10.

    F4 F4 F2

    F8

    (Tool/Datum)

    (set Datum)

    (set Y coord.)

    Type -10 using the keyboard and confirm

    key.

    Check the Y by setting the zero point using the dis-played coordinate values.

    17. Withdraw the tool in -Y and then in +Z direc-tion.

    use the numeric keyboard and press the ar-row key together with the shift key:

    + 1deEn for rapid speed in -Y direction, then

    + 8 for rapid speed in +Z

    18. F8 (Quit)

    19. Quit the setup mode menu. F8 (Quit)

    MTS TeachWare CNC-Grundlagen Students Book 52

  • Control test Basic Geometry

    2.4 Numeric Controls on CNC Machine Tools

    Control chain and control loop The current controls of the numeric-controlled machine tools are CNC controls. For the control it is characteristic to have an open movement path (see figure 55). The control gives the set value to the machine tool without controlling it directly. This is called a control chain.

    2

    3

    4

    1

    Figure 55 Function principle of a control chain

    input value (set value)

    output value (actual value)

    disturbance value

    control path

    Since such a control chain generates an incorrect output value it is connected with the control. The control is a sequence of operations which constantly recalculates and adjusts the actual value to reach the required value.This closed sequence of operations is called a control loop (see figure 56)..

    3

    4

    1

    5

    6

    2

    Figure 56 Function principle of a control loop

    entry value (set value)

    output value (actual value)

    disturbance value

    control path

    measuring equipment

    output value (actual value)

    In a CNC machine tool the principle of a control loop is applied as a position control for the axis.

    CNC Control

    Structure and function

    The CNC control is designed to decode a NC program and to process it as geometrical and technological information. Using CNC control it is possible to control or check the corresponding components of the CNC machine tool so that the desired work part is formed. The functions of the CNC control can be classified as data entry, data processing or data output (see figure 57).

    Data entry and data processing

    The data entry is done using the control panel consisting of a keyboard and monitor. Here the NC programs can be generated and managed, data can be entered or program simulations can be called . The NC pro-grams can also be read in or stored using external data carriers, such as data cassettes. It is also possible

    MTS TeachWare CNC-Grundlagen Students Book 53

  • Basic Geometry for CNC Machining

    to have an external data transmission to a computer (DNC operation) via serial interfaces or network input ports. It is then possible to generate (MTS system) and manage NC programs on this computer.

    1

    2

    X,Y,Z

    Y

    X

    3

    4

    5

    6 Z

    CNC control

    technological processing

    geometrical processing

    adjustment con-trol

    axis control

    actual position value

    data entry data processing data output

    Figure 57 Structure of a CNC control The data needed by the CNC machine tool to operate and machine the work part is generated out of the NC data by the data processing of the CNC control. The technological data is used e.g. for tool selection, for adjusting the spindle rotation speed, for selecting the spindle direction of rotation or for switching the coolant on and off. They are transmitted through the ad-justment control to the corresponding component of the CNC machine tool. The geometrical information of a NC program is translated from the CNC control into set values for the dif-ferent axial drives under consideration of the infeed values. The travel movements which are so created are continuously controlled by the position control loop of the feed axis. Travel movement using interpolation In technical applications by far all contour lines can be classified in straight lines and circular elements. This is the reason why the