CNC Basics MTS TeachWare Student’s Book
MTS Mathematisch Technische Software-Entwicklung GmbH •
Kaiserin-A ugusta-A llee 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 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 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
6
MTS TeachWare • CNC-Grundlagen • Student’s Book
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 • Student’s 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 however 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.
CIM CAD / CAM CAD FFS CNC
NC
CNC Numerical control with integrated computer FFS Flexible manufacturing system CAD Computer aided drawing/design CAM Computer aided manufacturing
NC
CIM 1950
1960
Numerical control
1970
1980
1990
Computer integrated manufacturing with planning, design 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 positions.
MTS TeachWare • CNC-Grundlagen • Student’s Book
9
Instroduction into CNC technology
In the mid 50s almost all machine tool manufacturers began developing and manufacturing numerically controlled milling machines which were soon followed by NC lathes. The rapid development of new microeletronic components, such us micro processors and micro computers, enhanced the development of NC controls to CNC (computerized numerical control) controls in the mid 70s. With the increased contribution of high-performance microprocessors it was possible to extend the operations 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. Contour precision and machining speed of the tools as well as cutting power have continuously improved. Modern CNC controls additionally offer a multitude of further characteristics. This has made it possible, for instance, to program complex tool geometries without using mathematical calculations. The continuous further development of CNC machine tools takes in a tools reciprocal innovation exchange between the manufacturers of microelectronic components, CNCplace controls, 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
10
MTS TeachWare • CNC-Grundlagen • Student’s Book
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
Entry:
CNC Machine Tools
Entry: The qualified worker manually The NC program is transmitted to adjusts the machine tool according the NC control using a punch card. to the drawing, clamps the raw part as well as the tools and aligns them.
Entry:
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 corresponding control signals to the components of the NC machine.
CNC control: The micro computer integrated in the CNC control and the corresponding software take over all control functions of the CNC machine. Hereby internal storage are used for programs and subprograms, machine data, tool and compensation values and fixed and free cycles. Frequently, error monitoring software is integrated in the CNC control.
Dimension control:
NC machine:
CNC machine:
The qualified worker manually measures and verifies the dimensions of the work part and, if necessary, must repeat the machining process.
The NC machine ensures the dimensional stability of the work part already during the machining process with the continuous feedback from the measuring system
The CNC machine ensures the dimensional stability of the work part already during the machining process with the continuous feedback from the measuring system
and the servo motors.
and the servo motor, which is controlled 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 optimize new NC programs.
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.
MTS TeachWare • CNC-Grundlagen • Student’s 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
larger lot sizes increased complexity and production precision
3
CNC machine tools conventional machine tools
4
2
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.
12
MTS TeachWare • CNC-Grundlagen • Student’s Book
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.
Z
X
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.
Y
X
Z
Figure 4 Controllable NC axes on a milling machine MTS TeachWare • CNC-Grundlagen • Student’s 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
+C
+Z
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 independent 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 requirements 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 (diameter dimension) 0.0005 and for the precision grinding machine up to 0.0001 are customary.
2 3
1
feed drive work table measuring system
4
ball screw
5
Figure 6 Feed drive for carrier with ball screw drive 14
MTS TeachWare • CNC-Grundlagen • Student’s Book
ball screw nut
Introduction into CNC Technology The embodiment of the measure is usually a ball circulating screw. If the spindle is set in motion by the motor, 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 frictionfree 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 automatically rectified by the CNC control through the spindle pitch error compensation. Further mechanical possibilities are for instance the rack/pinion and spindle/nut. If less accuracy is sufficient hydraulic drives are used as well.
2 ball screw nut
1
3
Clamping ring balls Drive spindle
3 4
Figure 7 ball screw drive with play-free double nut The manufacturing tolerances resulting from the manufacturing process of the ball screw drive can be rectified 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.
pick-up
X
glass ruler with scale
Y 1 2 Figure 8 Direct position measuring
MTS TeachWare • CNC-Grundlagen • Student’s Book
15
Instroduction into CNC technology In indirect position measuring (see figure 9) the travel path is specified using the rotation of the ball circulating screw, which is equipped with a pulse disk as a measuring scale. A signal generator registers the rotations of the pulse disk and transfers them to the control. The control then calculates the exact carrier movements or its present positions based on the rotation pulses.
1
carrier
2
pulse disk as a measuring scale spindle signal generator
3
X
4
Figure 9 Indirect position measuring 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.
1
012345 678
2 binary-coded measuring scale current tool carrier position
M
Figure 10 Absolute position measuring 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 position.
1
2
3
4 ruled grating previous carrier position current carrier position carrier on reference point
Figure 11 Incremental position measuring
16
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into CNC Technology
The control has once to be given one absolute position, which it then uses as a reference point when calculating 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 machine. 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 spindle. 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 moment 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 considerable 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 correspondingly 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 turning 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 approach 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 controllable live turrets are used. For clamping small parts controllable collet systems are commonly used.
MTS TeachWare • CNC-Grundlagen • Student’s 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, correctly 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 reclamping 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 machining without re-clamping. Work part pallets, which are loaded with the next work part by the operator outside the work room and then automatically taken into the right machining position, are increasingly being used.
Tool change facilities 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 working 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.
Figure 12 Example of a turret 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 different 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.
18
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into CNC Technology Figure 13 Example of a chain magazine
1
milling tools
2
tool gripper (tool changer) work spindle tool magazine
3 4
Figure 14 Automatic tool change facility 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 tool gripping device to the old tooland in the spindlethe and to gripping the new tool in the magazine Taking thethe tools into the spindle and magazine revolving tool 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 machine 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 inactivated. 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 • Student’s 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 machine 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 autogenerated 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.
20
MTS TeachWare • CNC-Grundlagen • Student’s Book
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 • Student’s Book
21
Basic Geometry for CNC Machining
22
MTS TeachWare • CNC-Grundlagen • Student’s Book
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 Example:
P2 P1 X
P1
X= 80
Y= 40
P2
X= -80
Y= 70
P3
X= -50
Y= -40
P4
X= 40
Y= -70
P3 P4 Figure 15 Cartesian coordinate system with 2 axis (X;Y)
If a work part drawing is placed in this coordinate system all important work points can be determined. Depending 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 • Student’s Book
23
Basic Geometry for CNC Machining The three-dimensional Cartesian coordinate system is necessary for the description and location specification 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.
Z
Y
Example:
P1
X= 30
Y= 20
Z=
0
P2
X= 30
Y=
Z= -10
P1 0
X P2
Figure 16 Cartesian coordinate system with 3 axes (X,Y,Z) The specifications of the three axes as well as the three coordinates is done as a so-called clockwiserotating 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.
+Y
+X
+Z Figure 17 Right-hand-rule 24
MTS TeachWare • CNC-Grundlagen • Student’s Book
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 extensive computing. In the polar coordinate system a point is specified by its distance (radius r) to the point of srcin and its angle (α) to a specified axis. The angle ( α) 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).
Y
Y
r
X
P
α α X
Figure 18 Polar coordinate system (positive angle α)
P
r Figure 19 Polar coordinate system (negative angle α)
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 • Student’s 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 srcin 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 srcin for the work part coordinate system, also called work part zero point W, can be specified as desired (see figure 22).
Z
Z
Y M
Y
X
W
M Machine zero point Figure 21 Machine coordinate system
X
W
Work part zero point
Figure 22 Work part coordinate system
CNC milling machine The design of the CNC machine specifies the definition of the respective coordinate system. Correspondingly, 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.
26
MTS TeachWare • CNC-Grundlagen • Student’s Book
Basic Geometry for CNC Machining 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 recommended to be placed on the outer edge of the work part.
Figure 23 Milling part in three-dimensional Cartesian coordinate system 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).
Z Y
X
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 • Student’s Book
27
Basic Geometry for CNC Machining
+X
W
+Z
+Z W
+X
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
Enter the coordinates of the points in the table. a b
X a X
b d c
28
c d
MTS TeachWare • CNC-Grundlagen • Student’s Book
Y
Basic Geometry for CNC Machining Y
Enter the following points in the diagram.
X
Y
a
10
20
b
-80
-30
c
40
-70
d
-30
50
X
Z Y a
Enter the Cartesian coordinates of the points a to d in the table. X
c
Y
Z
a b
X
c d
b
d
MTS TeachWare • CNC-Grundlagen • Student’s Book
29
Basic Geometry for CNC Machining Enter the Cartesian coordinates of the points a to h in the table.
X
g
f
a b
e
h
Y
c
a
d
d e
c
b
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 values of the X coordinates!
X
g
f
a
e
b
d
c
c
b a
d e f g
30
MTS TeachWare • CNC-Grundlagen • Student’s Book
Z
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.
+Z +Y -Z
-Y -X
+X
-X +X -Y
+Z
+Y
-Z
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 spindle is approached..
+X
C
+Z
Figure 30 Axes on the lathe
MTS TeachWare • CNC-Grundlagen • Student’s 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
+Z +X
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 dimensioning they refer to radius values.
+X
+X
-Z -Z
Figure 32 Example for absolute dimensioning
32
Figure 33 Example for incremental dimensioning
MTS TeachWare • CNC-Grundlagen • Student’s Book
Basic Geometry for CNC Machining 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 machined.
MTS TeachWare • CNC-Grundlagen • Student’s Book
33
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. Subsequently, 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.
+Z
8
7
Pos 1
-X
4
Ende
9
5 2 -Z
0
Einfg
6 4
Bild
1 -Y
+Y
Press the corresponding key on the numerical keyboard. Travel directions available: ( + X - direction ) ( - X - direction )
9
( + Y - direction )
1 Ende
( - Y - direction )
Bild
8
( + Z - direction )
,
2
( - Z - direction )
6 3
+X
Bild
Entf
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.
34
MTS TeachWare • CNC-Grundlagen • Student’s Book
Basic Geometry for CNC Machining
CNC turning Description
Entry
1. Call CNC turning in the main menu.
F1 (Turning)
2. Select setup mode.
F3
3. Go to the X or Z axis and check the travel path.
Press the corresponding key on the numerical keyboard. Travel directions available:
+X
7
Pos 1
8
6 4
-Z
4
5 2
6 3
(setup mode) (NUM keyboard ON)
+Z 8 2
( + Z - direction ) ( - Z - direction ) ( + X - direction ) ( - X - direction )
Bild
-X
0
,
Einfg
Entf
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 corresponding 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 • Student’s 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 dimensions 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 possibilities to describe a triangle. Some of the following characteristic values, such as corner points, angles or sides are used (see figure 34). Corner points A, B and C mark the three corner points of a triangle.
C
Angles α, β and γ are the corresponding angles in the corners of the triangle.
γ
b
a
Sides a, b and c mark the sides of the triangle opposite to the corners A, B and C.
β
α
A
The component parts of the triangle are always marked counterclockwise.
c
B
Figure 34 Characteristic values of a triangle 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)
C
C
C
γ
b
a
a
α
β
c
b
b α
A
B
Figure 35 Acute-angled triangle All angles are smaller than 90°.
A
β
c
Figure 36 Obtuse triangle One angle is larger than 90°.
a
α
B
A
β
c
Figure 37 right-angled triangle One angle is 90°.
For a triangle the relation applies: the sum of the triangle anglesα, β and γ is always 180°.
α + β + γ = 180o With this formula it is possible to calculate one unknown angle if the other two angles are known.
36
γ
γ
MTS TeachWare • CNC-Grundlagen • Student’s Book
B
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 α is called counter cathetus. The side located adjacent to the angle α 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.
counter cathetus 3
α
adjacent cathetus 1
hypotenuse
right angle 2
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. The Greek Pythagoras (approx. 580 - 496 BC) was the first to verify the following mathematical relation which was called after him the Pythagorean theorem
b² a² b
a c
The sum of the squares of the legs of a right triangle is equal to the square of the length of the hypotenuse. or expressed as an equation:
a2 + b2 = c 2 c²
With the corresponding transformation the sides of the triangle can be calculated as follows:
a = c 2 − b2 b = c 2 − a2
Figure 39 The Pythagorean theorem
c = a2 + b2
MTS TeachWare • CNC-Grundlagen • Student’s 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.
counter cathetus hypotenuse
2
α
1
sin α = counter cathetus hypotenuse Figure 40 Sine function
adjacent cathetus
α
hypotenuse
2
cos α =
adjacent cathetus hypotenuse
1
Figure 41 Cosine function
counter cathetus
α
adjacent cathetus
1
tan α = 2
counter cathetus adjacent 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 α =
counter cathetus (see figure 42), resulting in: adjacent cathetus
counter cathetus = adjacent cathetus • tan α
38
MTS TeachWare • CNC-Grundlagen • Student’s Book
Basic Geometry for CNC Machining
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.
Y f e
25
X
Y
a
15
15
b
?
15
c
?
35
d
85
35
e
85
85
f
?
85
g
15
65
g c
d
25
a
b
X Calculation of the point b: known :
b
x from center point = 65 mm
unknown : x from point b = ? 25
solution : x = 65 mm - dx dx = radius of the arc
dx
dx = 25 mm
?
x = 65 mm - 25 mm x = 40 mm
Calculation of the point c:
c
known :
x from center point = 65 mm radius of the arc r = 25 mm
y d
25
dy = 35 mm - 15 mm = 20 mm unknown : x from point c = ?
dx ?
solution : x = 65 mm + dx equation: dx = r 2 − dy 2 2 2 dx = ( 25mm ) − ( 20mm ) 2 dx = 225mm dx = 15mm
x = 65 mm + 15 mm x = 80 mm
MTS TeachWare • CNC-Grundlagen • Student’s Book
39
Basic Geometry for CNC Machining
?
known :
x from the beginning of the incline = 15 mm angle of the incline α = 25° dy = 85 mm - 65 mm = 20 mm
unknown : x from point f = ?
dx
solution : x = 15 mm + dx equation: counter cathetus = adjacent cathesis * tanα dx = 20 mm * tan 25° dx = 20 mm * 0.4663 dx = 9.326 mm x = 15 mm + 9.326 mm
f
y d 25
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.
Y X
c
a
b
b
a
d
c
0 0 1 6
0
d
h
e
e 0 5
g
f
Y
X
50
f g h
100
Calculate the unknown coordinates in the following examples.
5 80
70 50
5 3 30
5 8
0 8 ?
unknown : Y coordinate
40
?
unknown: Y coordinate
MTS TeachWare • CNC-Grundlagen • Student’s Book
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
Machine zero point M R E N
M
W
Each numerically controlled machine tool works with a machine coordinate system. The machine zero point is the srcin of the machine-referenced coordinate system. It is specified by the machine manufacturer 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 vertical milling machines.
Figure 43 Location of the zero and reference points for turning Reference point R
R M
A
N
A machine tool with an incremental travel path measuring system needs a calibration point which also serves for controlling the tool and work part movements. This calibration point is called the reference 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.After Thisswitching value hasthe a set adjustment in the CNC control. machine on the reference point has to be approached from all axes to calibrate the incremental travel path measuring system.
W
Figure 44 Location of the zero and reference point for milling
MTS TeachWare • CNC-Grundlagen • Student’s Book
41
Basic Geometry for CNC Machining
Work part zero point W
+X
M
+Z W
M
W
+Z
The work part zero point W is the srcin of the work part-based coordinate system. Its location is specified 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 generally in the center of the left or right side of the completed part, depending on which side the dimensioning was started from. The worke.g. partwhen zero apoint can beisshifted in the NC program, turned part 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
Figure 45 Work part zero point of the turned part
Z Y
For milling, the outer corner point is usually chosen as the work part zero point, depending on which corner point is selected as the reference point when dimensioning the work part.
X
Figure 46 Work part zero point of a milled 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 located 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
42
MTS TeachWare • CNC-Grundlagen • Student’s Book
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. Location of the tool setup point B on a turning tool
B L
B
Q
Q
R
R
tool setup point length = distance of the cutter tip to the tool setup point in X overhang = distance of the cutter tip to the tool setup point in Z cutter radius
L Figure 47 Tool setup point of a turning tool Location of the tool setup point at B of a milling tool
B L
B
R
tool setup point length = distance of the cutter tip to the tool setup point in Z radius of the milling tool
L
R Figure 48 Tool setup point of a milling tool Location of the toolholding point A on a turret
A
toolholding point
A
Figure 49 Toolholding point of a turret 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 • Student’s Book
43
Basic Geometry for CNC Machining
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. Setting the work part zero point is done with reference to the machine zero point M of the CNC machine.
W
M
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 z w, also called the zero point shift, is then entered into the CNC control.
zw
Figure 50 Setting the work part zero point on a CNC lathe 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 T02. tool to set the work part zero point, i.e. rotate the turret head to the corresponding position, for instance
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 programming the NC program.
44
MTS TeachWare • CNC-Grundlagen • Student’s Book
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. 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 located above the left corner edge of the machine table (see figure 51).
R M
A
N
W
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 entered into the CNC control. The zero setting tool is clamped and the spindle rotation is switched on. 1. Resetting Z direction Figure 51 Setting the work part zero point on a CNC milling machine Z
Y
W
X
The machine table with the clamped is moved below the work spindle (in X andwork Y) inpart 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
Figure 52 Resetting in Z Z
The tool is raised again and taken into the new resetting 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
Y
W
X
Figure 53 Resetting in X
small marking is part). made on the work part surface (touching the work When touching the work part in X axis the radius of the applied tool has to be considered when confirming the value with the IST key, since the center point coordinates of the tool are always used in NC programming. If the milling tool of the adjacent figure has, for instance, a radius of 15 mm, then the value X=-15 is entered into the NC control and confirmed with IST. .
MTS TeachWare • CNC-Grundlagen • Student’s Book
45
Basic Geometry for CNC Machining
Z
3. Resetting in Y direction
Y
W
X
Figure 54 Resetting in Y
46
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 confirming the value with the IST key, since the center point coordinates of the tool are always used in NC programming. If the tool of mm the then adjacent figureY=-15 has, for instance, a radius of 15 the value is entered into the CNC control and confirmed with IST.
MTS TeachWare • CNC-Grundlagen • Student’s Book
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 coordinate 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 z w. Starting situation:
• All machining tools are dimensioned and available on the turret head. work part is clamped in chuck jaws. •• The The work part zero point is located on the front
W
M
plane surface, whereby an allowance of 1mm has to be considered.
zw
Description
Entry
1. Call CNC turning in the main menu.
F1 (Turning)
2. Select setup mode.
F3
3. Switch on the spindle in counterclockwise rotation.
(Setup mode) Type „M04“ using the keyboard and confirm. Type „T0404“ using the keyboard and confirm.
4. Change the tool for the definition of the work part zero point. 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.
Using the numeric keyboard press the corresponding arrow key simultaneously with the shift key: + 4
+X
+
2
for rapid speed in -Z direction for rapid speed in -X direction
+Z Travel direction options:
+X
7
8
4
5
6
2
3
6
Pos 1
-Z
+Z
4 8
Bild
-X
0
Einfg
2
( + Z - direction ) ( - Z - direction ) ( + X - direction ) ( - X - direction )
, Entf
MTS TeachWare • CNC-Grundlagen • Student’s Book
47
Basic Geometry for CNC Machining
6. Switch the increment from 1mm to 0,1mm or 0,01 mm for further machining. .
7 Move the lathe tool in negative Z-direction until it touches the plane surface of the work part .
8. Set the work part zero point in Z.
F3
(Technology)
F5
(Increment)
F2
(Increment 0.1) Press the arrow key on the numeric keyboard.
4
Then press
ESC
and
F8
(Quit).
F4
(Tool datum)
F4
(Set datum)
F1 (Set Z coord.) Type „z+1“using the keyboard and confirm
F8
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 .
10. Quit the setup mode
48
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
F8
(Quit)
F8
(Quit)
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
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. Starting situation:
Y
Z
• All machining tools are dimensioned and available 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
W
X
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 Zdirection Move the tool in rapid speed to a position approx. 5mm above the work part surface.
Using the numeric keyboard press the corresponding arrow key together with the shift key: Ex.:
+ 2
for rapid speed in -Z direction.
Z W
X +Z
7 Pos 1 -X
8
4
5
+Y
9 Bild 6
Further travel direction options: 6
4
+X
9
Bild
1 Ende
1 -Y
2
Ende
3 Bild
-Z
0
Einfg
,
8 2
( + X direction ) ( - X direction ) ( + Y direction ) ( - Y direction ) ( + Z direction ) ( - Z direction )
Entf
MTS TeachWare • CNC-Grundlagen • Student’s Book
49
Basic Geometry for CNC Machining
6. Switch the increment from 1mm to 0,1mm or 0,01mm for further machining.
7 Move the tool in negative Z direction until it touches the surface of the work part.
8. Set the work part zero point in Z.
F3
(Technology)
F5
(Increment)
F2
(Increment 0.1) Press the arrow key on the numeric keyboard
2
Then press
ESC
and
F8
(Quit).
F4
(Tool/ Datum)
F4
(Set Datum)
F3
(set Z coord.) Type in the data on the keyboard „0“ and
F8
confirm it.
Check Z by setting the zero point and using the displayed 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
10. Move the tool in rapid speed to the new zero setting position approx. 5mm off the side surface.
1
together with the shift key: 1) in -X direction + 4
Y Z
2
50
for rapid speed in -X direction
2) in -Z direction + 2
W
for rapid speed in +Z direction
Press the corresponding arrow key on the numeric keyboard
for rapid speed in -Z direction
X
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
11. Move the tool in positive X direction until it touches the left side of the work part.
Press the arrow key on the numeric keyboard. 6
ESC
12. Set the work part zero point in X. Please note the tool radius! So, enter for the X coordinate the negative value the radius of the applied tool, for instanceof-10.
Then press and
F8
(return).
F4
(tool, zero point)
F4
(set datum)
F1 (set X coordinate) Type „-10“ using the keyboard and confirm.
F8 Check the X by setting the zero point using the displayed coordinate values.
13. Setting the zero point in Y direction Take off the tool in -X direction and then in +Z direction.
14. Take the tool in rapid speed to the new resetting position approx. 5mm off the front side.
Z
1
Y
+ 4
for rapid speed in -X direction then
+ 8
for rapid speed in +Z direction.
Using the numeric keyboard press the corresponding arrow key together with the shift key: 1) in +X direction + 6
2 W
Using the numeric keyboard press the arrow key together with the shift key:
for rapid speed in +X direction
2) in -Y direction
3
1 + Ende for rapid speed in -Y direction
X
3) in -Z direction + 2
for rapid speed in -Z
MTS TeachWare • CNC-Grundlagen • Student’s Book
51
Basic Geometry for CNC Machining
15. Take the tool in positive Y direction until it touches the front of the work part.
Press the arrow key on the numeric keyboard. 9 Bild
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.
Then press
ESC
and
F8
(Quit).
F4
(Tool/Datum)
F4
(set Datum)
F2
(set Y coord.) Type „-10“ using the keyboard and confirm
F8
key.
Check the Y by setting the zero point using the displayed coordinate values.
17. Withdraw the tool in -Y and then in +Z direction.
use the numeric keyboard and press the arrow key together with the shift key: 1 + En de for rapid speed in -Y direction, then
+ 8 18.
F8
(Quit)
19. Quit the setup mode menu.
F8
(Quit)
52
for rapid speed in +Z
MTS TeachWare • CNC-Grundlagen • Student’s Book
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.
1
input value (set value)
2
output value (actual value)
4
disturbance value control path 3
Figure 55 Function principle of a control chain
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)..
1
2 4
entry value (set value) output value (actual value) disturbance value
6
control path
3
measuring equipment 5
output value (actual value)
Figure 56 Function principle of a control loop 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 programs can also be read in or stored using external data carriers, such as data cassettes. It is also possible
MTS TeachWare • CNC-Grundlagen • Student’s 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.
CNC control
1
technological processing
Y
2
4
geometrical processing
X
adjustment control
5 3
X,Y,Z
6
axis control
Z
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 adjustment 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 different 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 majority of the CNC controls manufactured today are equipped only with straight line and circular interpolation. In our CNC controls interpolations of parabolas and cubic parabolas, helical interpolations and spline interpolations are also available. If a tool goes from the starting point to a target point which is not parallel to the axis it is a question of a straight line interpolation. To achieve a straight tool path the relevant axes have to be correspondingly adjusted to each other. The relation of the axis feeds defines then the direction of the straight lines (see figure 58 and 59).
Y
Y 1 1
2
1 2
1 X
aimed travel movement Figure 58 Relation of axial feeds
54
X aimed travel movement Figure 59 Relation of axial feeds
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ The best way to demonstrate the principle of tool feed along curves, lines and arcs on a plane is to use a plotter with a step motor. A step motor is controlled by current pulses. A positive or negative current pulse rotates the wave of the step motor with a jerk in a certain angle to the right or to the left. As a result, each of the two plotter axes can reach only a certain axial value. Therefore the plotter can only go to the points of a tight grid on its drawing area. Just like on a monitor screen an incline is drawn through the axis-parallel movement of the plotter (see figure 60).
1
aimed plotter movement movement in the X axis movement in the Y axis
2
3
Figure 60 Travel path of a plotter pen The same principle is used for the interpolator of a CNC control. It calculates the intermediate values needed for interpolation and transmits them as set values to the position control circles. In straight line interpolation two or three axes move simultaneously (see figure 61), whereby their travel movements are adjusted to each other in a certain relation. If the tool moves in a circular path from the starting point it is a question of a circular interpolation (see figure 62). The tool moves here either in clockwise or in counterclockwise direction. To achieve a circular tool path the travel movements of both axes, also depending on the path already traveled, have to be adjusted to each other. The axis movement corresponds to a sine or cosine curve. The overlay of the two axis makes out the arc. Z
X
X
Z
X X
Z
Travel path of a plotter pen
Figure 61 Straight line interpolation
Travel path of a plotter pen
Figure 62 Circular interpolation
MTS TeachWare • CNC-Grundlagen • Student’s Book
55
Basic Geometry for CNC Machining
Types of CNC controls The axis of the CNC machine tool receive their travel signals (commands) from the CNC control. These signals are coded and are based on the entered NC program. They are evaluated by the control and transmitted to the feed motor. The travel paths of the tools are exactly set. Depending on the type of the travel paths the following control type classification is used:
• point control • line control • path control:
- 2D path control - 2½ D path control - 3D path control Point control
It is the simplest control type. In case of a point control a target point is approached in rapid speed and a machining operation is carried out at the target point (see figure 63). In the same way several target points can be approached one after an other. The point control can be applied to work parts for which machining is made only at certain points, e.g. for machining surfaces by boring, reaming, recessing, threading, spot welding, punching.
Figure 63 Point control Line control
With the line control only tool travel paths which are parallel to axes and which have programmed infeed values can be controlled (see figure 64). The generated work part contours can only be parallel to axis. The line control can be applied in cases where machining is supposed to take place only on planes parallel to the guideways of the machine, e.g. for simple plane and straight turning, plane parallel milling or breakthrough milling where machining takes place in one direction at a time.
Figure 64 Line control
Path control
In path control it is possible to control any travel paths (straight, inclines, circular, splines) of the tool applied on planes or in space. It is possible to achieve any contour line (see figure 65) through the controlled interaction of two or more infeed motors.
Figure 65 Path control on a CNC machine
56
To be able to carry out the movements simultaneously on all machine axes all intermediate values located on the mathematically specified curve between the starting and end point need to be first calculated by the CNC control.
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
MTS TeachWare • CNC-Grundlagen • Student’s Book
57
Basic Geometry for CNC Machining Path controls are further classified depending on the number of axes which can be simultaneously controlled: 2 D path control
With the older 2 D path control it is possible to simultaneously control two axes. So it is possible to carry out straight and circular tool movements on one plane (see figure 65). If, for example, a 3 axes CNC milling machine has a 2 D path control it means that it is possible to mill contours in two axes. The third axes has to be entered separately. Figure 2D path66control 2 ½ D path control
The 2½ D path control makes it possible to carry out tool movements on several planes by switching the interpolation in each case on one of the three main planes. All three axes are controllable in 2½ D path control, however in every plane only two axes simultaneously. The third axes is the so-called infeed axis. Depending on the selected machining plane different axis can be controlled simultaneously so that it is possible to travel in the following directions:
- X/Y plane (see figure 67), - X/Z plane (see figure 68), - Y/Z plane (see figure 69).
Figure 67 2½D path control (X/Y plane)
Figure 68 2½D path control (X/Z plane)
Figure 69 2½D path control (Y/Z plane 3 D path control
In 3 D path controls three axes are interpolated simultaneously. Herewith it is possible to realize threedimensional tool movements. It enables complicated contours, e.g. in tool construction, especially in molded construction, to be machined in one clamping.
58
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
MTS TeachWare • CNC-Grundlagen • Student’s Book
59
Basic Geometry for CNC Machining
DNC operation Characteristics of DNC operation
DNC is the abbreviation of direct numerical control. It is the name of an operation mode in which several NC and CNC machines as well as further devices are connected with each other. These devices can be for instance tool presetting machines, measuring machines, programming seats and a central material and tool management (see figure 70).
CAD
NC-Programming
PS P
...
Local area Network (LAN)
Tool presetting machine Master computer Measuring machines
NC archive
...
Figure 70 Structure of a DNC system The connection between the components of a DNC system is realized by a data bus. This direct data transmission makes the conventional data carriers such as punch cards, magnetic stripes, discs as well as the corresponding recording and read-in instruments unnecessary. The significant characteristic of the DNC operation is the management and timely disposition of the information. To be able to calculate and distribute this information to the right position, interfaces are needed. Through the interfaces all the integrated parts of the DNC net are connected with the master computer. The master computer is able to calculate machine and production data, switch operation modes, address, read-in and record the correct storage location as well as automatically transmit them to the machine upstream computers. Data input and data processing in DNC operation
Through the structure of a DNC system (see figure 70) it is possible to enter data into different devices. These devices can be located far away from each other. Small NC programs can be written directly on the CNC machine tool. For writing extensive or complicated NC programs it is better to use an external programming work station. A DNC system generally includes the following basic functions.
• storage and management of NC programs • correct distribution of NC programs to the machines • re-transmission of the corrected and optimized NC programs from the machine to the master data storage medium
60
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
For this purpose there is a central management of the NC programs in the DNC system. The generated and optimized NC programs are transmitted to the corresponding computers through data links. In case the CNC machine tool is not equipped with a special DNC port a DNC terminal controls the organization of the data transmission between the CNC control and master computer. Depending on the model of a DNC system the following additional functions can be available:
• • • •
central tool management and tool compensation data
• • • • •
control of the material flow central storage of the current data bases
interface for tool presetting devices work part management set time value and definition of working sequences
central cooperation data and machine data acquisition (BDE, MDE) with graphical evaluation NC programming with postprocessor conversion graphical simulation with representation of the tool, clamping device and work part contour
Advantages of the DNC operation system
A DNC operation system has the following advantages compared with a solution with non-integrated CNC machine tools:
• improved workshop organization • immediate availability of programs and additional information • minimal standstill times of the CNC machine through the continuous provision of NC programs, tools and material
• reduced data entry errors • operating data and machine data acquisition (BDE, MDE) enable the user to control and record at any time the production data (machine operating times, out-of-service-times, down times, etc.), maintenance information and information on reasons for out-of-service-times
Workshop The different CNC control types are demonstrated on the CNC machine tools available.
If no CNC machine tools are available for point or line control these CNC control types can be simulated with the help of the corresponding work parts. Example:
• point control milling machine: go to boreholes
• line control milling machine: travel parallel to axis lathe: travel parallel to axis
• 2D path control milling machine: travel linear on two axis milling machine: travel in a circle lathe: machine a cone or rounding
• 2½ D path control milling machine: travel on various planes milling machine: travel in a circle on various planes
• 3 D path control milling machine: travel linear on two axis
MTS TeachWare • CNC-Grundlagen • Student’s Book
61
Basic Geometry for CNC Machining milling machine: travel on a circle in space
2.5
Tool Compensations for CNC Machining
Using tool compensation values Using the tool compensation values it is easy to program a work part without consideration of the actually applicable tool lengths or tool radii. The available work part drawing data can be directly used for programming. The tool data, lengths as well as radii of the milling machines or indexable inserts are automatically considered by the CNC control.
Tool length compensation for milling and turning A tool length compensationregarding the reference point enables the adjustment between the set and actual tool length, as in case of tool finishing. This tool length value has to be available for the control. For this it is necessary to measure the length L, i.e. the distance between the tool setup point B and the cutting tip, and to enter it into the control (see chapter on tool measuring page 69 ff.). In case of milling tools the length is defined in Z direction (see figure 71). B
tool setup point
L
length = distance of the cutting tip to the tool setup point in Z
R
radius of the milling tool
B
L
R Figure 71 Tool compensation values on a cutting tool In case of lathe tools the length L is defined in Z direction (see figure 72).
B
Q
B
tool setup point
L
length = distance of the cutting tip to the tool set-in point in Z
Q
overhang = distance of the cutting tip to the tool setup point in X
R
cutting radius
R L Figure 72 Tool compensation values on a lathe tool In the CNC control these tool compensation values are stored in the compensation value storage, whereby in most CNC controls it is possible to describe up to 99 tools. These values have to be activated during ma-
62
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ chining. This is done by calling the data within the NC program, e.g. with the address H or by specific places in the T word.
Tool radius compensations The CNC controls have an integrated cutter radius compensation for milling machines and tool tip compensation for lathes. Using these aids it is possible to directly program the finished contour of the work part.
Cutter radius compensation (milling)
To enable the tool to generate the programmed contour with high precision the tool center point has to travel on a path running parallel to the programmed path. This tool center point path is called equidisant (see figure 73).
1
Milling center point paths (equidisant) work part contour
2
Figure 73 Milling center point paths (equidisants) One equidisant is the tool center point path running in constant distance to the programmed path (contour) of the work part. In discontinuous path transitions, i.e. in the inner and outer corners (see figure 74 and 75), the transitions become equidisants, for instance, through insertion of arcs, in accordance with the controlspecific rules.
2 1
2
1
programmed path
programmed path
tool travel path
tool travel path
Figure 74 Inner corner in milling
Figure 75 Outer corner in milling
In case of inner corners an arc corresponding to the radius of the milling machine is created.
In case of outer corner the tool makes a compensating arc.
The CNC control calculates the contour-parallel milling center point path necessary for machining. The calculations are based on the radius value of the current milling tool, which is stored in the tool compensation
MTS TeachWare • CNC-Grundlagen • Student’s Book
63
Basic Geometry for CNC Machining value storage. The radius is not given in the NC program as such, the corresponding compensation switch is instead called. Due to the fact that machining can be done in two ways the NC control has to be informed if machining is to take place on the left or right of the programmed contour (see figure 76).
1
2 left of the contour right of the contour
3
programmed contours
Figure 76 Machining directions in milling radius correction
The following figures demonstrate the selection of the milling radius compensation which depends on the position of the tool with reference to the contour to be machined outside machining (see figure 77) and in inside machining (see figure 78).
2 1
1 2
3
left of the contour
left of the contour
right of the contour
right of the contour
programmed contour
programmed contour
Figure 77 Milling radius compensation in outside machining
64
3
Figure 78 Milling radius compensation in inside machining
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ If subsequent travel movements without milling radius compensation are to be done, for instance in borings, these have to be entered to the CNC control with the corresponding command. Tool nose compensation (turning)
In milling, milling radius compensation is used and in turning, tool nose correction, due to the fact that the control calculates the travel paths based on a theoretical tool nose of the lathe tool. This theoretical tool nose moves along the programmed path. Since the actual tool dimensions, i.e. tool nose radius of the lathe tool, are not considered errors are unavoidable. Consequently, as a rule, roundings remain in inside corners or the contours (see figure 79). In tool movements which are not parallel to X or Z axis considerable dimension and form deviations are the result (see figure 80). These errors can be avoided by using tool nose correction, also called tool nose compensation, in the CNC control. 3
3
4
4
3
5 3 2
5 2
1
Figure 79 Unavoidable error in turning: contour inside corner remains
1
Figure 80 Error in turning: cone is not true-to-size according to the programmed contour
programmed contour
programmed contour
theoretical cutting point
theoretical cutting point
theoretical tool tip
theoretical tool tip
actual tool tip
actual tool tip
contour corner remains unmachined because of the cutter radius
incorrect deviation from the programmed contour
The location of the actually traveled tool paths (equidisant see figure 81) is automatically calculated by the cutter radius compensation in modern CNC controls.The following three facts have to be considered: 1. The radius of the tool tip has to be available in the compensation value storage of the CNC control. 1. The location of the tool tip (cutter compensation value vector) has to be available for the CNC control. 1. The machining direction of the tool with reference to the contour has to be correspondingly programmed in NC programming.
programmed contour path 2
the center point path (equidisant) calculated by the CNC control on which the tool travels during machining
1
MTS TeachWare • CNC-Grundlagen • Student’s Book
65
Basic Geometry for CNC Machining Figure 81 Equidisant in turning To enable the control to correctly calculate the actual cutting point the so-called cutting tip is described for each tool by the cutter compensation vector (SRK vector). Hereby the SRK vector gives the position of the cutter tip in I and K (X and Y direction) with reference to the cutter center point (see figure 82). The SRK vector is defined in advance for each tool in the tool management of the MTS CNC simulator.
1
4
theoretical cutting edge
R
theoretical cutting tip
3
I
theoretical cutting tip cutting radius compensation value vector
1 R
2
cutting radius
K
Figure 82 Cutting radius compensation value vector Different cutting radius compensation value vectors have to be entered into the control depending on the fact in which machining quadrant the applied tools are located (see figure 83). When entering the compensation values I and K the signs of the resulting value have to be considered.
8 4
3
5
7
1
2 6
For the cutting radius R the value of the current tool has to be entered. 1. quadrant:
K=R
I=R
2. quadrant:
K = -R
I=R
3. quadrant:
K = -R
I = -R
4. quadrant:
K=R
I = -R
5. quadrant:
K=R
I=0
6. quadrant:
K=0
I=R
7. quadrant:
K = -R
I=0
8. quadrant:
K=0
I = -R
Figure 83 Values for the cutting radius compensation value vector which depend on the current machining quadrant of the tool.
66
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
The following example demonstrates how to define the compensation values I and K (see figure 84). cutting edge in machining quadrant 3 cutting edge radius R = 0,8 mm
The values I and K are as follows: K = -0,8
R
I
= -0,8
I K Figure 84 Example: Cutting edge radius compensation value
When calling the cutting edge radius compensation in the program the location of the turning tool in travel direction has to be entered into the CNC control by using the corresponding command: turning tool is located left of the contour in travel direction or turning tool is located right of the contour in travel direction The following figures demonstrate the programming of the cutting radius compensation in dependence upon the location of the tool with reference to the contour to be machined in case of outside machining (see figure 85 and figure 86) and in case of inside machining (see figure 87 and figure 88).
1
1
2
Figure 85 Cutting radius compensation in case of outside machining left of the contour machining direction of the tool left of the contour
2
Figure 86 Cutting radius compensation in case of outside machining right of the contour machining direction of the tool right of the contour
MTS TeachWare • CNC-Grundlagen • Student’s Book
67
Basic Geometry for CNC Machining
programmed contour
programmed contour
2
2
1
1
Figure 87 Cutting radius correction, inside machining, left of the contour.
Figure 88 Cutting radius correction, inside machining, right of the contour
machining direction of the tool left of the contour
machining direction of the tool right of the contour
programmed contour
programmed contour
Just like programming a milling work part it is possible to directly program the contour to be machined using the work part drawings data without data conversion. In turning as well, the selected cutting edge radius compensation has to be switched off with the corresponding command.
68
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
Tool measuring and adjusting with an adjusting device To guarantee efficient CNC machine capacity utilization the tool measurement (tool set-up) generally takes place outside the CNC machine. For this a universal tool measuring and setup device is used. The term „universal“ refers here to the fact that turning and milling tools are measured with different tool holders to define the corresponding setup values. Modern tool measuring and adjusting devices convey the calculated data directly to the CNC control or to an other data carrier or a printer via DNC for an output.
Structure and function of a tool setup device
A tool setup device is used to define the compensation values of turning or milling tools. It is not possible to correctly program a work part contour without the tool compensation values (see chapter on the milling radius compensation p.63 ff. or the tool nose compensation p. 65 ff).
Figure 89 Universal tool measuring and setup device A tool setup device consists in general of four main components:
• • • •
the base plate, the compound slide rest, the tool holder the tool shank
In addition to this, an electronic measuring device for measuring the tool compensation values and a storage medium for storing data, e.g. the milling radius R and length L, are available.
Tool measuring and setup
The following describes how to measure a turning tool using a tool setup device.
MTS TeachWare • CNC-Grundlagen • Student’s Book
69
Basic Geometry for CNC Machining
The target is to precisely define the length L and the overhang Q (see figure 90) of the turning tool to be able to give the CNC control the corresponding compensation values in X and Z.
B L
B
Q Q
tool set-up point length = distance of the cutting edge tip to the tool set-up point in Z overhang = distance of the cutting edge tip to the tool setup point in X
R
L Figure 90 Measuring a turning tool
• Clamp the turning tool to be measured in the tool shank corresponding to the current turret. • Switch on and adjust the tool measuring and setup device. • Measure the lathe tool. Using the control desk of the tool setup device the compound slide rest is moved with the lathe tool to be measured in X and Z (see figure 91).
X
Z
Figure 91 Display crosslines of a tool setup device with exact positioning of the tip of the turning tool The aim of the infeed is to adjust the tool cutting edge exactly on the display crosslines of the measuring device. Now the length L and the overhang Q of the lathe tool on the tool setup device display can be read-in. These values correspond to the compensation values of the clamped lathe tool in X and Z. • Store the measured compensation values The compensation values are now either manually listed for a later entry into the CNC machine, or they are directly carried into the CNC machine through a data link between the tool set-up device and the CNC control in DNC mode. • Declamp the turning tool The turning tool can now be declamped from the tool set-up device to allow a further tool to be measured.
70
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
Tool measuring and setup using the CNC machine Direct tool measuring on the CNC lathe
Measuring the tools directly on the CNC machine tool is only customary for CNC lathes. For direct tool measuring the work part is clamped together with the tool in any position (for instance machining a cylinder). The work part is then measured with reference to the machine zero point M. The measured values are entered in the tool compensation register of the CNC control. After that, the second tool is clamped, the tool slide is taken into the same position as it was for the first tool and the machined work part contour is worked out again. The control then calculates the compensation values for the second tool based on the new actual position of the tool slide. Direct tool measuring is time-consuming, requires however no additional investments. Defining the deviation between target and actual value with various aids Tool measuring using so-called zero tools on the CNC milling machine
A commonly applied method for tool measuring on CNC milling machine uses a zero tool to define the different lengths of the milling tools. The radius compensations of all tools have been defined and entered into the CNC control in advance. Procedure: With the first tool, also called zero tool, an area on the clamped work part is machined. For this tool the measured Z value is set zero. The next tool is clamped and then moved as far as to touch the work part surface. The current Z position can now be entered into the compensation register including its sign. Herewith the compensation values of the tool length become the deviation values of the zero tool length. This procedure will be repeated for all further tools. Tool measuring on the display of a CNC lathe
In the machining room of some CNC machines there is an optical system installed on a fixed point, whose position is known to the machine. The coordinates have been stored in the CNC control as parameters. The tools to be measured are clamped in any position and are taken one after the other to the center of the crosslines of the optical system using an electronic hand wheel (see figure 92). The control then calculates without further data entry the value overhang Q as well as the length L and stores these values in the tool compensation value register.
X
Z
Figure 92
MTS TeachWare • CNC-Grundlagen • Student’s Book
71
Basic Geometry for CNC Machining Inside optical measuring Advantages and disadvantages of direct tool measuring on CNC machine
Advantages
Disadvantages
• increased flexibility • improved design of machine work places • reduced investment since
• machine stand-still during measuring • high precision cannot be achieved
- tool setup devices - complicated tool holder systems are not needed
CNC exercise Working with tool compensation values in the MTS simulation
The MTS software, just like a real CNC machine tool, allows the user to allocate one or several compensation switches to each tool. With these switches the tool compensation values of the tool are called. Exercise: The following work part is to be machined, including rough turning and final turning, using a left corner turning tool and the set compensation switches. The corner turning tool T05
LEFT CORNER TOOL
CL-SDJCL-2020/L/1204 ISO30
is applied with the setting value for overhang Q and the length L to be entered in the compensation value register D25.
It is assumed: Setting-up the MTS simulator according to the following set-up data:
PART CYLINDER D060.000 L082.000 MATERIAL C 45 W-Nr: 1.0503 DENSITY 007.90 MAIN SPINDLE WITH WORKPART CHUCK KITAGAWA B-208 STEP JAW KITAGAWA-1 CHUCKING DEPTH E32.000 RIGHT SIDE OF THE PART: Z+209.500 TOOLS T05 LEFT CORNER TOOL CL-SDJCL-2020/R/1204 ISO30
72
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ Procedure:
Description
Entry
1. Call CNC turning in the main menu.
F1 (Turning)
2. Select setup mode.
F3
(Setup mode)
3. Select menu for the compensation value register.
F4
(Tool data)
F2
(Turret display)
4. Setting the additional compensation register No. 25.
Enter on the keyboard „25“ using
F1 (change values) confirm. Cutting point:
Z: +43.0 X: +60.5
Cutting radius:
R:
0.4
Size:
G:
0.0
Recessing angle:
E: 32.178
Compensation:
K: I:
-0.4 -0.4
The quadrant Q3 is automatically set by MTS when the arrow key or the tabulator key has been actuated subsequent to the entry of the values! Only then it is possible to accept/confirm the data.
5. Enter the data for the compensation register No. 25.
Use the keyboard to enter the data by pressing or by selecting the data one by one.
6. Quit the compensation register menu.
F8
(Quit)
F8
(Quit)
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
73
Basic Geometry for CNC Machining Now the NC program „BOLZEN“ can be simulated either in single step or in automatic run. Drawing
NC program: BOLZEN N010
G90
N015
G54
N020
F000.300
X+000.000
N025
G96
S0180
N030
G92
S3000
N035
G00
X+062.000
Z+000.000
N040
G01
X-001.000
M08
T0101
Z+207.500 M04
N045
Z+002.000
N050
G00
N055
F000.300
N060 N065
G00 X+050.000 Z+002.000 G01 Z-044.800 M08
X+120.000 T0525
N070
X+061.000
N075
G00
N080
X+040.000
N085
G01
N090
X+051.000
N095
G00
N100
X+030.000
N105
G01
N110
X+042.000
N115
G00
Z+040.000
M09
M04
Z+002.000 Z-044.800 Z+002.000 Z-014.800 Z+002.000
N120 T0505 M04 F000.160 N125
G00
X+030.000
N130
G01
Z-015.000
N135
X+040.000
N140
Z-045.000
N145
X+062.000
N150
G00
N155
M30
X+120.000
Z+040.000
M05
M09
Workshop Working with tool setup devices The students should individually define the compensation values of the tool on a real tool setup machine.
The necessary operation steps can be found in the operating manual of the applied tool setup machine.
• Optical measuring of tools on the CNC machine • Direct dimension measuring using the CNC machine The students should individually measure turning and milling tools on the CNC machine tools in workshop. The details of this procedure are given in the chapter „Tool measuring and setup using the CNC machine“. The operation steps on the CNC machine are given in the respective operation.
74
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
2.6
Path Measuring Systems
Infeeds, position control and position adjustment of the NC axis The CNC control invocates the travel movements of the tool or tool carriage using the NC program commands. Hereby the programmed coordinates have to be approached on the axis on a preset path (position) using the preset speed (infeed) in highest precision. The exact spatial position of the controllable and moving machine parts has to be constantly fed back to the CNC control. This is done by the position sensor whose data is fed into the position control loop (see figure 93). On the CNC machine tool the position of the tool carriage is constantly measured. Based on the change of time along the path, the current path position (actual value) as well as the path speed is calculated and compared with the programmed path (set value). For instance the machining forces as well as friction and play in guidance influence the feedback loop. They are called disturbance variables and are to be compensated by the control (CNC control). Approximately every millisecond the control delivers a new position set value to the position feedback loop, which the control aims for. Considering the high clock rate the control receives a new set value even before the previous set value has been achieved. This phenomenon of the position feedback loop is based on physical facts (i.e. too high infeed) and creates the so-called lag error.
1
2 5
4
input variable (set position value) output variable (actual position value) disturbance variables
7 3
3
motor 6
ball screw measuring equipment
Figure 93 Position feedback loop
output value (actual position value)
Path measuring To define the current position of the tool carriage (actual value of the position feedback loop) there is a path measuring system available for each travel axis of the CNC machine tool. Depending on the travel path different path measuring methods are applied. Absolute and incremental path measuring
For absolute path measuring (see figure 94) each pitch of the binary coded measuring scale indicates the exact numerical value. This value corresponds to an exact position of the tool slide opposite to the machine zero point M. This means that the current tool slide position can be directly conveyed to the CNC control at any time. The fact that the read-in area of the measuring scale has to be as large as the machining area is a disadvantage. In connection with the binary coding this results in large, technically complicated measuring scales.
MTS TeachWare • CNC-Grundlagen • Student’s Book
75
Basic Geometry for CNC Machining For incremental path measuring (see figure 95) counting pulses result from the constant change of light and dark fields of the ruled grating during the travel movement. These pulses are constantly added or subtracted by the CNC control. The current tool slide position is the difference of the new position to the last position. Therefore, after the CNC control has been switched on, the tool slide has to go once to an absolute point, the reference point, to enable the CNC control to calculate the absolute coordinates.
1
012345678
2
1
2
3
4
M
binary coded measuring scale
ruled grating
current tool slide position
last tool slide position current tool slide position tool slide on the reference point
Figure 94 absolute path measuring
Figure 95 incremental path measuring
In general, only incremental path measuring is applied in CNC machine tools due to the fact that the reference point can be gone to at any time. In case of welding line robots, however, collisions can occur with the work parts when going to the reference point. Therefore, absolute path measuring is required here.
76
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
CNC exercise Moving to the reference point CNC turning
Procedure: Description
Entry
1. Call CNC turning in the main menu.
F1 (turning)
2. Select setup mode.
F3
(setup mode)
3. Select ‘go to reference point’.
F2
(reference point)
Message: enter default value for the travel axis. 4. Select the order of the travel axis.
X Z
(first the X then the Z axis) or (first the Z and then the X axis) confirm
The system goes to the reference point automatically on both axes. The position can be read-in using the displayed axis coordinates.
5. Quit the setup mode.
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
77
Basic Geometry for CNC Machining Moving to the reference point CNC milling
Procedure: Description
Entry
1. Call CNC milling in the main menu.
F2
(milling)
2. Select the setup mode.
F3
(setup mode)
3. Select ‘go to reference point’. Message: Enter default value for the travel path. 4. Select the order of the travel axis.
(reference point)
F2 X
(1. the X , 2. the Y then the Z axis) or
Y
(1. the Y , 2. the X then the Z axis) or
Z
(1. the Z , 2. the X then the Y axis).
The system goes to the reference point automatically on both axes. The position can be read-in using the displayed axis coordinates.
5. Quit the setup mode menu.
78
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ Touching the turning tool on the plane surface
Procedure: 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.
Use the keyboard to enter „M04“ and
4. Change the tool to define the work part zero point.
Use the keyboard to enter „T0404“ 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.
Use the numeric keyboard to press the arrow key together with the shift key:
confirm.
+ 4
+X
+
2
for rapid speed in -Z direction for rapid speed in -X direction
+Z Further travel direction options:
+X
7
8
6
Pos 1
-Z
4
5
6
+Z
4 8
2
3 Bild
( - Z direction ) ( + X direction )
2
( - X direction )
F3
(technology)
F5
(increment)
F2
(increment 0.1)
-X
0
( + Z direction )
,
Einfg
Entf
6. Switch the increment from 1mm to 0,1mm or 0,01 mm for further machining.
7 Move the lathe tool in negative Z direction until it touches the plane surface of the work 4 part.
Now first press the arrow key on the numeric keyboard.
ESC
F8
and then press (Quit).
8. Quit the setup mode.
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
79
Basic Geometry for CNC Machining Touching the milling tool on the upper side
Procedure: 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.
Enter „M03“ using the keyboard and confirm.
4. Change the tool to define the work part zero point.
Enter „T0202“ using the keyboard and
5. Move the tool in rapid speed to a position approx. 5mm off the work part surface.
Use the numeric keyboard to press the arrow key together with the shift key:
confirm.
Ex.:
+ 2
for rapid speed in - Z direction.
Z W
X +Z
7
8
Pos 1
-X
4
5
+Y
4
9
Bild
6
Further travel direction options: 6
+X
9
Bild
1 Ende
1 -Y
2
Ende
3 Bild
-Z
0
,
Einfg
8 2
( + X direction ) ( - X direction ) ( + Y direction ) ( - Y direction ) ( + Z direction ) ( - Z direction )
Entf
6. Switch the increment from 1mm to 0,1mm or 0,01mm for further machining.
F3
(technology)
F5
(increment)
F2
(increment 0.1)
7 Move the tool in negative Z direction until it touches the surface of the work part.
Now press the arrow key on the numeric keyboard, 2 ESC
F8
then press and (Quit).
8. Quit the setup mode.
80
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“ Touching the milling tool on the lateral side
Procedure: 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.
Enter „M03“ using the keyboard and confirm.
4. Change the tool to define the work part zero point.
Enter „T0202“ using the keyboard and
5. Take the tool in rapid speed to the new resetting position approx. 5mm off the side surface.
Press the corresponding arrow key on the numeric keyboard
confirm.
1
together with the shift key: 1) in -X direction
Y
+ 4
2
Z
for rapid speed in - X direction
2) in -Z direction + 2
W
for rapid speed in -Z direction
X Further travel direction options:
+Z
8
7
Pos 1
-X
+Y
9
4
Bild
4
5
6
6
+X
9 Bild
1 Ende
1 -Y
2
Ende
3 Bild
-Z
0
,
Einfg
8 2
( + X direction ) ( - X direction ) ( + Y direction ) ( - Y direction ) ( + Z direction ) ( - Z direction )
Entf
6. Switch the increment from 1mm to 0,1mm or 0,01mm for further machining.
7. Move the tool in positive X direction until it touches the left side of the work part.
F3
(technology)
F5
(increment)
F2
(increment 0.1)
6
Now press the arrow key on the numeric keyboard,
ESC
then press
F8
and (return) key.
8. Quit the Setup mode.
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
81
Basic Geometry for CNC Machining Touching the milling tool on the front side
Procedure: 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
5. Take the tool in rapid speed to the new resetting position approx. 5mm off the front side.
Use the numeric keyboard to press the arrow key together with the shift key:
confirm.
1) in +X direction
1
Z
+ 6
2) in -Y direction
2
1 + En de for rapid speed in -Y direction
3
W
3) in -Z direction
X +Z
8
7
Pos 1
-X
+Y
9
5
6
+ 2
6
4
Bild
4
+X
9 Bild
1 Ende
1 -Y
2
Ende
3 Bild
-Z
0
,
Einfg
8 2
for rapid speed in -Z
Further travel direction options: ( + X direction ) ( - X direction ) ( + Y direction ) ( - Y direction ) ( + Z direction ) ( - Z direction )
Entf
6. Switch the increment from 1mm to 0,1mm or 0,01mm for further machining.
7. Take the tool in positive Y direction until it touches the front of the work part.
8. Quit the Setup mode.
82
for rapid speed in +X direction
F3
(Technology)
F5
(Increment)
F2
(Increment 0.1) Press the arrow key on the numeric keyboard.
9
Bild
Then press
ESC
and
F8
(Quit) key.
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Basic Geometry“
5.
Control test „Basic Geometry“
1.
Indicate the possible travel movements for turning in a coordinate system.
1.
Indicate the possible travel movements for milling in a coordinate system.
1.
For which applications is it reasonable to use the polar coordinate system in milling?
1.
Give two examples of control types on CNC milling machines.
1.
Which types of 2 ½ D path controls can be differentiated on CNC milling machines?
1.
How can the different possibilities of 2 ½ D path control be explained?
1.
Explain the zero and reference point on numerically controlled machine tools.
1.
Where should the work part zero point, which is set by the user, be positioned?
1.
What are the advantages of absolute programming?
1.
Why is incremental programming sometimes unavoidable?
1.
Incrementally dimension the sketched milling work part with absolute dimensions:
12.
What is the main difference between the principle of a control chain and a feedback loop?
12.
Discuss the control as an operation.
12.
Why is it necessary to have milling radius compensation in milling?
12.
Which values are considered by the tool compensation in milling?
12.
Why is it necessary to have cutting radius compensation in turning?
12.
Which values are considered by the tool compensation in turning?
12.
What is the significance of the working quadrants of the turning tool edge?
12.
List the different types of tool dimensioning.
MTS TeachWare • CNC-Grundlagen • Student’s Book
83
Basic Geometry for CNC Machining
84
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining 6.
3 Technological Basics for CNC Machining
3.1
CNC tool systems for turning and milling
CNC machine tools use special NC tools. These tools meet the following criteria:
• • • •
better milling performance with high stand still times short changing and setup times to enable economical production of small production lots standardized and rationalized tools improved tool management and flexible production
The NC tools are either a single tool or they are put together of the cutter edge holder and tool holder. To enable a quick tool change and to secure good exchangeability of the NC tools the tool carriers are standardized.
Tool carriers Special forms have been stablished for tool carriers. They differ from each other in their machining method. For turning tools a straight shank with toothing (see figure 96) is mostly used and for cutting tools a steepangle taper (see figure 97). Both tool shanks can be used with automatic and/or quick manual tool change.
Figure 96 Straight shank with toothing
Figure 97 Steep-angle taper
Tool holder Many lathe and milling tools are a combination of several components. Indexable inserts are used which are attached, for example with clamping devices (see figure 98).
1 Clamping finger
2
indexable insert
3
pin
4 Insert
5
indexable insert carrier
Figure 98 Example of a clamping system
MTS TeachWare • CNC-Grundlagen • Student’s Book
85
Basic Geometry for CNC Machining The main components of a modern lathe tool are the clamping holder or indexable insert holder, the indexable insert and the clamping device. The indexable inserts are placed in the holder which has two supporting edges and an insert. The insert serves to convey larger cutting forces and to protect the holder from damage in case of an eventual breach in the indexable insert. Since the indexable inserts are exposed to the cutting forces of the lathe and to the centrifugal forces of the milling machine, there is the danger of loosening supports or slipping tools. Clamping and screw clamping fixtures are therefore used to accurately fix and position the indexable inserts. The clamping fixtures and the indexable inserts are standardized to a large extent.
Tungsten carbide indexable inserts In CNC technology indexable inserts are increasingly being used since they achieve very high stand-still times and are easy to change. Indexable inserts have several cutting edges. This allows the insert to be rotated or turned when one edge of the insert becomes dull. Indexable inserts are made either of tungsten carbide or cutting ceramics (see chapter cutting materials pp. 88 ff.).They are sintered. This production method, in which metal powder is first pressed and then heat treated, enables economical indexable inserts to be manufactured in various designs (see figure 99).
S
B
E
T
P
H
R
Figure 99 Forms of indexable inserts Indexable inserts are classified according to their basic form, angles, cutting edges, tolerance class as well as their clamping system and main dimensions. Based on a norm sheet ISO 1832 / DIN-4987 the following example (see figure 100) shows the norm title of an indexable insert.
indexable insert ISO 1832 - ECMT 09 T3 08 FR - P10 Designation 1) 2) 3) 4) 5) 6) 7) 8) 9) 10)
Example
Norm main number basic form normal-clearance angle tolerance class face and clamping characteristics insert size
DIN 4987 E = orthorhombic 75° C = 7° M T = counterborehole 60°on face side length: 9,52 mm
insert thickness cutting edge radius cutting edge characteristics cutting direction cutting edge material
s = 3,97mm r = 0,8mm F = sharp edged R = right tungsten carbide P10
Figure 100 Description of an indexable insert
86
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
3.2
Structure and use of lathe tools for CNC machining
Types of lathe tools and the corresponding ISO designation The lathe tools, also called cutting tools, can be classified according to the following criteria: • according to the cutting material: − cutting tool edges out of high-speed steel, − cutting tool edges out of tungsten carbide, − cutting tool edges out of ceramics or − cutting tool edges out of diamond; • according to the location of the application area: − cutting tool for outer machining or − cutting tool for inner machining; • according to their form: − straight cutting tool, − offset cutting tool, − cranked cutting tool, − sharp cutting tool or − wide cutting tool; • according to the location of the major cutting edge − left cutting tool, − right cutting tool or − neutral cutting tool; • according to the application purpose e.g.: − recessing tool, − corner cutting tool or − tapping tool. Details of the cutting tools are described in the corresponding norms (ISO 243, 504 or 514). A selection of commonly used cutting tools is listed in the below table 101 according to their application area. These cutting tools are stored with all their dimensions in the tool management of the MTS turning simulator. They can be called from there for simulaton on the MTS turning simulator.
outer
inner
cutting tool corner cutting tool (right cutting) corner cutting tool (left cutting) copying lathe tool outer cutting tool (round cutting edge) inner cutting tool (preaxial) inner cutting tool (postaxial)
thread cutting tool outer tapping tool (right cutting) outer tapping tool (left cutting)
recessing tool outer recessing tool
inner recessing tool (preaxial) inner tapping tool (postaxial) inner recessing tool (postaxial) axial recessing tool
boring tool
inner tapping tool (preaxial)
axial
centering drill twist drill indexable insert reamer
Figure 101 Classification of cutting tools
MTS TeachWare • CNC-Grundlagen • Student’s Book
87
Basic Geometry for CNC Machining
Cutting materials Hard metals are primarily used as the cutting material for lathe tools. For certain types of cutting high-speed steels (HSS steels) are used. Their cutting surface is usually coated. In special cases ceramic materials (cutting ceramics) are used as indexable inserts and in some cases industrial diamonds as well. High-speed steels
High-speed steel is a high-alloyed tool steel (HSS = high-speed steel). It is highly durable and can therefore easily take impact loads. The cutting speed is considerable lower compared with hard metals and cutting ceramics. It is used for tools whose form, for instance boring and reaming tools, do not allow the use of indexable inserts or machining of thermoplastic plastics lightcolored alloys. HSS tools are frequently coated with a hard coat of titanium nitrid TiN. This extremely hard,and golden coating increases the abrasion resistance and allows higher cutting speeds. Hard metals
Hard metals are materials which are cintered as indexable inserts using hardening materials and a binding agent. In most cases the hardening materials are tungsten, titanium or tantalum carbide. Cobalt is used as a binding agent. Hard metals are considerably harder than HSS steels. They are extremely abrasion-resistent and allow very high working temperatures. They do, however, tolerate far less temperature fluctuation and impact exposure than the HSS steels. Hard metals can be classified according to the main cutting groups and cutting application groups. Main cutting groups
Cutting application groups Abbreviation
Materials
P01
P blue
P10 P20 P30 P40
K red
high resistance high abrasion cutting speed
precision machining, high cutting speed steel cast steel malleable cast iron short shipping
P50
M yellow
Applications superfinish high surfaceturning, quality
medium cutting speed
rough cutting interrupted cutting precision machining high cutting speed
high hardness high infeeds high abrasion resistance high cutting speed
M10
steel
M20 M30 M40
hard steel cast iron non-iron metals
medium cutting speed
K01
hard cast iron
precision machining
high hardness high infeeds high abrasion resistance high cutting speed
K10 K20
cast iron malleable cast iron short shipping plastics wood
rough cutting interrupted cutting
high hardness high infeeds
K30 K40
rough cutting interrupted cutting
Figure 102 Application areas of hard metals The abrasion resistance of hard metals can be increased with a corresponding coating. As coating materials titanium nitrid, titanium carbide and aluminium oxide are applied in several layers in vacuum in a temperature of 1000°C 88
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Cutting ceramics
Ceramic materials which are even harder than hard metals are used as cutting ceramics. Cutting ceramics allow a working temperature up to 1200°C. They are very brittle and sensitive to fluctuating cutting forces. Cutting ceramics are manufactured as indexable inserts and are clamped in the tool holder just like hard metals. Cutting ceramics are applied for cutting with constant cutting conditions, without coolant application. The cutting speed is higher than that of hard metals. They are ideal for cutting iron materials since they do not create built-up edges. They, however, cannot be used for aluminium alloys. The applicable cutting ceramics can be classified in the three following groups:
• oxide ceramics ceramics •• mixed nitrid ceramics Cutting ceramics alloys of pure Al2O3 are called oxide ceramics. They have no metallic binding agent. They are especially ideal for cutting iron alloys since they are highly abrasion resistant to them. In case of mixed ceramics hard materials are added to the Al 2O3 such as titanium carbide. Mixed ceramics are used for finishing gray-cast iron or steel as well as for cutting hardened iron materials. Nitrid ceramics are based on silicium nitrid Si3N4. This non-oxide cutting material is extremely brittle and sensitive to temperature fluctuations. High abrasion in cutting steel is a disadvantage. The nitrid ceramics is applied for machining gray cast iron.
Diamond
Diamands are harder than all other materials. They are extremely sensitive to impact, however create no built-up edges during machining. They are used for cutting non-iron materials and their alloys as well as for composite materials (GRP), hard metal, gas and ceramics. Diamands cannot be applied for machining steel. Here they have very high abrasion since the carbon atoms of diamonds are given off to the iron (diffusion abrasion).
MTS TeachWare • CNC-Grundlagen • Student’s Book
89
Basic Geometry for CNC Machining
Cutting edge geometry Each machining process requires its cutting edge geometry. Only this can guarantee ideal production times, long cutting-edge life and high surface quality. The angles of the tool cutting edge play a decisive role here (vgl. Abbildung 103).
α0 clearance angle
γ0
α0 β0
χ
r
λ ε
β0 wedge angle γ0
angle of rake
εr
angle of point
λs
angle of inclination
χr
adjustment angle
s
r
Figure Cutting103 geometries in turning Clearance angle :
The clearance angle reduces friction and heating up of the tool edge and the work part.
Wedge angle :
The size of the wedge angle depends on the hardness and toughness of the work part. The smaller the wedge angle the lighter the cutting, however, the larger the edge abrasion and the shorter the cutting edge life.
Angle of rake :
The angle of rake has an influence on chip building and cutting forces. The larger the angle of rake the smaller the cutting force, however, cutting edge breach and abrasion are increased because of total decarburization. Solid, medium hard materials require an angle of rake of approx. 10°. Hard and brittle materials require a small or even a negative angle of rake.
Adjustment angle : In the first place the entering angle has an influence on infeed force, on the forces against the work part clamping and work part as well as on the cutting width and thickness. In case of solid clamping situation an entering angle of 30 to 60° is selected. Only for thin shafts or right angled offsets 90° is selected for the adjustment angle. Inclination angle : For finishing a positive, for roughing a negative inclination angle is frequently selected. When negative angles of rake are used the cutting edge tip is exposed to less stress. When positive inclination angle is used the chip flow is directed away from the work part. Angle of point :
90
The larger the angle of point the better the stability of the tool edge and the better the heat removal.
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Abrasion and cutting edge During cutting the tools are subject to wear, also called abrasion. This is due to the cutting friction, the diffusion in high temperatures as well as to the chip flow. Due to the high temperature of the tool cutting edge small work part particles can be welded on to the tool face. A built-up edge can be created (see figure 105).
Figure 104 New lathe tool
Figure 105 Built-up edge
During the cutting process material particles continuously break off from the lathe tool. Correspondingly, the geometry of the tool cutting edge changes with the time. Depending on the choice of the tool cutting edge angle the abrasion can take different forms (see figure 106 to 109).
Figure 106 Open cutting edge wear
Figure 107 Chip surface wear
Figure 108 Crater wear
Figure 109 Edge rounding
Due to tool qualitysurface of the machining as well as thestability dimensional stability of the any workmore part are reduced. Aswear soonthe assurface the required quality or dimensional are not maintained the cutting-edge life of the tool has been reached. Cutting-edge life is the time during which the cutting edge is in operation and the following requirements are met: • Generation of required surface quality • Dimensional stability within the required tolerances When cutting-edge life has been reached it is necessary to change the tool or to resharpen it. When using indexable inserts the insert can be turned or changed. Prior to using the tool again tool dimensioning has to be done.
MTS TeachWare • CNC-Grundlagen • Student’s Book
91
Basic Geometry for CNC Machining
Cutting value Turning is a cutting operation with a circular cutting movement and an infeed which can be in any relation to the cutting direction. In most cases the cutting movement is made by the rotation of the work part and the infeed of the tool (see figure 110). The
• cutting speed vc and the • infeed speed vf overlap and result in a continuous cutting process. Cutting speed vc Cutting speed is the movement between the tool and the work part causing only a single chip removal during one rotation without infeed. The symbol for cutting speed is v c and is indicated in m/min.
In general the speed indicates the traversed path s within a certain period of time t. It is calculated as follows:
v=
s in path/time
t
The traversed path s for a work part rotation can be generated in turning using the work part diameter d on the cutting edge tip and the constant π:
s = π *d
in m
The starting point for the calculation of the cutting speed is now a time unit t = 1 min. The result is herewith cutting speed vc :
vc
=
π *d t
in m/min
The number or work part rotations in one minute is indicated as a number of rotations n (in rotations per minute):
t=
1
in min
n
As a result the following formula is achieved for the calculation of the cutting speed vc:
vc
= π *d * n
in m/min
vc n
n
vf
number of rotations
vinfeed speed f
in mm/
vcutting speed c
in m/min
vc
=π*d*n
Figure 110 Cutting values in turning
92
in U/min
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Infeed speed vf Together with the cutting movement Infeed allows a continuous chip removal during several rotations. The infeed speed vf is indicated in mm/min.
Often the infeed f is given in mm per rotation as well. The infeed f is the path the lathe tool makes in the infeed fixture during one spindle rotation. The following relation exists between these two forms:
vf = n *f
in mm / min
For each cutting process a certain infeed is required. Together with the spindle number of rotations n it defines the machining time for each travel path. Its value has a decisive influence on an ideal cutting force and on the sufrace quality of the machined surface. Chip size The chip diameter A describes the material diameter, which is cut in one cut (see figure 111). Its size largely defines the cutting force created.
Without considering the cutting edge radius, the chip diameter A is the product of the cutting depth a and 2 infeed f. It is given in mm . The cutting depth a, i.e. the depth of the tool cutting, is the value to be fed in step by step.
A = a *f
in mm
2
Using the entering angle κ it is possible to calculate the width b and the thickness h of the chip.
h = f *sin κ b=
a
in mm
in mm
sin κ
f
b
f a
a
κ h
a
cutting depth
κ
adjustment angle
f
infeed per rotation
b
chipping width
h
chipping thickness
Figure 111 Chipping sizes The following cutting values have to be selected always considering the specific appliction, and the lathe is to be correspondigly set up.
• cutting speed vc • infeed f • cutting depth a This requires extensive experience. As a support standard value tables are therefore available indicating the cutting values regarding the material to be cut and the cutting edge material.
MTS TeachWare • CNC-Grundlagen • Student’s Book
93
Basic Geometry for CNC Machining
Examples: Calculating technological values for CNC machining Cutting speed vc
vc
= π *d * n
in m/min
1. Example:
What is the cutting speed in plain turning if the cutting is done with a 60 mm diameter and number of rotations of 1500 1/mm.
datum:
d = 60 mm n = 1500 1/min
unknown:
vc in m/min
valid :
vc
= π *d *n
vc = solution:
π * 0,06 ⋅ m ⋅ 1500 1 min
vc = 283
m min
2. Example:
How many number rotations are required if the smallest diameter to be machined on the same work part with this cuttingofspeed is 12mm?
datum:
vc = 283 m/min d = 12 mm
unknown:
n in 1/min
valid :
vc = π *d * n , n=
vc
π *d 283m *m in* 0,012 m
n= solution:
94
or
π
n = 7511 1 min
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
3.3
Structure and application of milling tools for CNC machining
Milling and milling operations Milling is a cutting operation with a geometrically specified cutting edge in which the tool makes the rotating main movement, and the feed as well as the infeed movement are generally made by the work part (see figure 112).
1
rotation of the milling tool work part feed
2 Figure 112 Milling Milling operations are classified according to the position of the milling axis towards the work part, i.e. between face milling and peripheral milling. In case of face milling the milling axis is located vertically to the machining area (see figure 113). The work part surface is machined by the main cutting edges. Also, the work part surface is further finished with auxiliary cutting edges. In case of peripheral milling the milling axis is located parallel to the machining axis (see figure 114). The milling tool machines the work part surface with the main cutting edges (the peripheral cutting edges). Furthermore, a difference is made between synchronous and conventional milling.
Figure 113 Face milling
Figure 114 Plain-milling MTS TeachWare • CNC-Grundlagen • Student’s Book
95
Basic Geometry for CNC Machining Additionally, synchronous and conventional milling (see figure 115 and 116) are differentiated. In case of conventional milling the rotation direction of the milling tool is opposite to the feed direction of the work part (see figure 115). The milling tool chamfer edge starts with chip thickness zero. The milling tool cutting edge slides in front of the chip chamfer edge until the required minimum chip thickness has been achieved for chip building. The friction created by sliding results in high abrasion of the tool flanks and in hardening of the work part surface. This leads to a shorter cutting edge life of the tool compared with synchronous milling. Conventional milling is recommended to be used for machining work parts with hard surfaces (cast material) since the hard surface is cut through from inside. For synchronous milling the rotation direction of the milling tool and the feed movement of the work part are parallel (see figure 116). The tooth of the milling cutter immediately penetrates into the work part. Since the milling tool cutting edge is exposed to impact forces the feed drive needs to be playfree. Several cutters should always be in operation. The surface quality is flatter and duller when synchronous milling is used. Compared with conventional milling higher feed movements and cutting speeds within the same cutting edge life can be achieved.
1
1
Work part feed Figure 115 Conventional milling
Work part feed Figure 116 Synchronous milling
The tool cutting edge is subject to constant cutting interruptions in all milling operations. Due to the cutting path comma-form chips are cut with a changing chip thickness (see figure 117).
cutting chip
1
Figure 117 Milling plan
96
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Types of milling tools Milling tools can be classified according to the following criteria: • according to the type of the material to be cut in − tool type N (for normal steel), − tool type H (for soft, long-chipping materials), − tool type W (for hard, short-chipping materials), • according to the cutting material in − cutter with cutting edge of high-speed steel tool, − cutter with cutting edge of hardmetal, − cutter with cutting edge of ceramics or − cutter with cutting edge of diamond; • according to the type of the tool carrier − shell mill or; − end mill; • according to the milling form, for instance in − T slot cutter; − face milling cutter; − side mill or − form cutter; • according to the form of the milling tool tooth in − pointed teeth cutter or − back-off teeth cutter Details of milling tools are given in the manufacturers´ catalogues and in the corresponding norm sheets. A selection of common milling tools are shown below, classified according to their application field: end mill standard types
plain milling cutter face milling cutter counterbore
drills
drill
screw tap
indexable insert drill
reamer
stepped drill
special forms
radius form cutter
angle cutter (form A)
concave cutter
T slot mill
angle cutter (form B)
side mill
Figure 118 Classification of milling tools The above milling tools including all their data are included in the MTS CNC milling simulator and can be called by the user. These tools can be modified or extended to meet the user´s demand. End mill / Slot drill
T-slot cutter
MTS TeachWare • CNC-Grundlagen • Student’s Book
Shell end mill
97
Basic Geometry for CNC Machining
98
Face end cutter
Radius cutter
Angular cutter (type A)
Angular cutter (type B)
Tap drill
Drill
Step drill
Reversible tip drill
Reamer
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Countersink
Concave cutter
Side milling cutter
Cutting edge materials In milling, the cutting edges are not in operation all the time. The milling cut is a discontinuous cut with a changing cutting diameter. Therefore, the cutting edge is exposed to high impact forces. The cutting edge material has to be tough and heat resistant. Today, mostly indexable inserts made of hardmetal are used as milling tools. Only in case of small milling machines soldered hardmetal cutting edges made of high-speed steel or coated high-speed steel tools are used.
High-speed steel
High-speed steel is a high-alloyed tool steel. Due to its high toughness it is able to withstand impact forces. The cutting speed is considerably lower compared with hardmetals or cutting ceramics. It is used for drills, small milling tools and tools with a complicated form (profile cutter). Cutting tools made of high-speed steel are used for cutting less tough materials, for profile cutting and for cutting with low cutting speed.
Hardmetals
Hardmetals are materials which are sintered in form of indexable inserts by using hardening materials and a binding agent. By increasing the binding agent proportion in hardmetal production it is possible to increase the hardness of the material as required. The abrasion resistance of hardmetals can be increased by a titanium nitrid, titanium carbide or aluminium oxide coat. Hardmetal cutting plates are soldered on the milling tool or screwed on it in form of indexable inserts.
Cutting ceramics
Cutting ceramics are rarely used for milling because of their brittleness and sensitivity to fluctuating cutting forces. However, because of the high hardness aluminium oxide is used for machining hardcast materials and hardened steel as well as silicon nitrid for grey cast. Both of these materials are used for cutting without coolant application. Like hardmetal, cutting ceramics are manufactured to be used in form of indexable inserts.
Diamond
Cutting plates made of polycrystalline diamonds are used to cut non-iron metals and plastics. The extraordinary hardness of the diamonds enables double as high cutting speeds with ten times longer cutting edge lifes are achieved as compared with hardmetals. MTS TeachWare • CNC-Grundlagen • Student’s Book
99
Basic Geometry for CNC Machining Diamonds cannot be used for cutting steel. Here they are exposed to high abrasion since the carbon atoms of the diamond are given off to iron atoms (diffusion abrasion).
Cutting geometry Unlike lathe tools milling tools have several cutting edges (see figure 119). Typical of milling is the discontinuous cut as each cutting edge works only for a time.
d
fz
ϕ
d:
diameter of the milling tool
z:
number of teeth
fz:
feed per tooth
ae:
entering point
ϕ S:
entering angle
α0:
clearance angle
β0:
wedge angle
γ0:
angle of rake
λ S:
angle of twist of the edges
ap:
cutting width
s
e
a
β0
0
α0 p
a
λs Figure 119 Cutting geometry milling Clearance angle :
100
The clearance angle is to reduce the friction and consequently the heating of the cutting edge and of the work part. MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Wedge angle :
The size of the wedge angle depends on the hardness of the work part. The smaller the wedge angle the lighter the cutting, however the greater the cutting abrasion and the shorter the cutting edge life.
Angle of rake :
The angle of rake influences cutting chip formation and cutting forces. The larger the angle of rake of the chip the smaller the cutting force, however the risk to breach as well as abrasion of the cutting edge are increased due to erosion.
Entering angle
S:
The entering angle indicates the machining path of the tool with reference to the circumference. It depend on the size of the entering point.
Inclination angle : The size of the inclination angle influences the process of chamfering and cutting-out.
Since the inclined cutting edges are consecutively engaged the milling tool runs with increased quietness.
The configuration of the adjustment angle (see figure 120) is very important in milling. The adjustment angle χ is the angle between the main cutting edge and the surface to be cut.
:
adjustment angle
χ
Figure 120 angle χ of milling tools Adjustment If the adjustment angle is 90°, the highest radial forces are exposed. This angle value is therefore only recommended for right-angled contours. For most milling works an adjustment angle of 75° or 60° is ideal. For long cutting materials the adjustment angle of χ = 45° is ideal. If hardmetal indexable inserts are mostly used, then two cutting angles are available. They can be measured using the reference lines:
• radial cutting angle (reference line through the centerof the milling tool) • axial cutting angle (reference line parallel to milling axis) In case of plain milling with a plain milling cutter the following combinations are mostly used (see figure 121):
• double positive geometry • double negative geometry • positive-negative geometry 2
2
+
1
2
+
-
+
-
-
1 double positive geometry
double negative geometry
1 positive-negative geometry
MTS TeachWare • CNC-Grundlagen • Student’s Book
101
Basic Geometry for CNC Machining radial cutting angle Figure 121 Cutting geometries on plain milling cutter
axial cutting angle
In case of double positive geometry only light driving power is required due to small cutting forces. It is therefore possible to machine thin-walled work parts as well. The spiral-form chips drop off from the tool easily. In case of materials which tend to form built-up edge, for instance aluminium, this geometry is recommended. Double negative geometry is used for machining hard steels and grey cast as well as for roughing. The high cutting forces created hereby require strong driving power and high stability of the machine. Due to the geometry the chips curl on the tool. In case of long-chipping materials this can lead to a chip jam. Positive-negative geometry makes large feeds and big cutting depths possible since the negative radial angle of rake contributes to high breaking strength of the indexable insert. Here the chipping is ideal since the chips flow off from the tool. Tools with a positive-negative geometry are therefore applied for various situations.
Cutting values Milling is a cutting operation with a rotating tool, whereby the cutting edges are not in operation all the time. The cutting movement is caused by the rotation of the tool. Feed direction and cutting direction do not depend on each other. It is realized either by the tool or by the work part or by both of them (see figure 122). The
• cutting speed vc and the • feed speed vf overlap each other and results in a continuous cutting operation. Cutting speed vc The cutting movement is the movement between the tool and the work part, generating only one nonrecurrent chip cut during one rotation without a feed movement. Cutting speed corresponds to circumferential speed of the milling tool on the current cutting edge. It is expressed as v c and m/min. Under consideration of the number of rotations of the spindle n the following formula is received
vc
= π *d * n
in m/min
The cutting speed of a cutting tool depends on the number of the rotations. The direction constantly changes however during cutting operation (see figure 122
vc
vc
n
vc n
vf
d
number of rotation
vf
feed speed
vc
cutting speed
d
vc vc
Figure 122 Cutting values for milling Feed speed vf
102
MTS TeachWare • CNC-Grundlagen • Student’s Book
diameter of the cutting tool
Technological Basics for CNC Machining The feed movement together with the cutting movement enable a constant chip removal during several rotations. In milling, the feed can be indicated in three ways:
• feed speed vf in mm / min • feed per tooth fz in mm • feed per milling rotation f in mm The calculation of the feed speed v f is based on the feed f z , i.e. the feed path per milling tooth. Under consideration ot the number of rotations n and the number or teeth z the formula is as follows:
v f = fn *z z *
in mm / min
The feed speed can be expressed with the following formula as well with reference to the feed per milling rotation.
vf = f *n
in mm / min
Consequently, the following equivalence is valid:
v f = f * nf=
z
*n *z
in mm / min
Cutting width Unlike in turning, a nonuniform chip is cut in milling (see figure 123). The average cutting thickness hm is used as reference.
fz 1
actual chip fz:
feed per tooth
hm:
average cutting thickness
hm Figure 123 Cutting thickness In plain milling, the cutting width ap is the penetration width of the tool into the work part. The working engagement ae is measured on an imagined plane of the working plane. The cutting and feed direction are located on the working plane (see figure 124).
MTS TeachWare • CNC-Grundlagen • Student’s Book
103
Basic Geometry for CNC Machining
1
1
p
ae
a
e
a
ap
working plane
ap: cutting plane ae: entering point
ap: cutting depth ae: entering point
Figure 124 Operating variables in milling In face milling, ap is the cutting depth measured vertically to the working plane. The working engagement a p is identical with the width of the milled surface. The following cutting values must be selected case by case depending on the application and then entered into the milling machine:
• • • •
number of rotations n feed f working engagement ae cutting depth or cutting width ap
This requires extensive experience. As a support standard value tables are therefore available containing cutting values regarding the material to be cut and to the cutting edge material.
Calculation examples of technological values for CNC machining Cutting speed vc
vc
= π *d * n
in m/min
Feed speed vf
v f = f * nf=
z
*n *z
in mm / min
1. Example:
Calculate the cutting speed for milling if the milling tool diameter d = 50 mm and the number of rotations n = 520 1/min. known:
d = 50 mm n = 520 1/min
104
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining unknown:
vc in m/min
it applies :
vc = π *d * n vc = π * 0,05 ⋅ m ⋅ 520 1 min
solution:
vc ≈ 82
m min
2. Example:
Calculate the number of rotations n of an end mill with a diameter of ∅ = 12 mm and cutting speed of vc = 120m/min. known:
d = 12 mm vc = 120 m/min
unknown:
n in 1/min
it applies :
vc = π *d * n n=
n= solution:
, or
vc π *d 120m
π *m in* 0,012m
n = 3183 1 min
MTS TeachWare • CNC-Grundlagen • Student’s Book
105
Basic Geometry for CNC Machining 3. Example:
In plain milling with a face milling cutter a cutting speed of vc = 180 m/min has been scheduled and the number of rotations should not exceed 400 1/min. What is the maximum diameter d of the face milling cutter so that these values are not exceeded? known:
n = 400 1/min vc = 180 m/min
unknown:
d in mm
it applies :
vc = π *d * n d= d=
Solution:
106
, or
vc
π *n 180000mm *min π *min* 400
d = 143mm
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
3.4
Calculation of technological data for CNC machining
Calculation examples of technological data for CNC turning 1. Example:
On a CNC-lathe the sketched bolt is to be roughed as well as finished in four cuts with cutting depths of 6; 6; 5 and 5 mm and a finishing allowance of 0,5 mm. The cutting speed for roughing is vcv = 280 m/min and for finishing vcf = 400 m/min.
0 7
5 4
5 2
Calculate the number of rotations for each cut. 20 50 60
Calculating the number of rotations for roughing (Cut 1-4) and for finishing (Cut 5-6)
datum:
vcv = 280 m/min vcf = 400 m/min
unknown:
n in 1/min
valid :
n=
vc
π *d 1. Cut
2. Cut
∅ = 58mm
n1 = n1
v
= 280 m/min
cv
280m
π *m in* 0,058m
= 1537 1 min
∅ = 46mm
n2 =
v
= 280 m/min
cv
280m
π *m in* 0,046m
n2 = 1938 1 min
3. Cut
4. Cut
∅ = 36mm
v
cv
= 280 m/min
280m π *m in* 0,036m
n3
=
n3
= 2476 1min
n4 =
v
= 280 m/min
cv
280m π *m in* 0,026m
n4 = 3428 1 min
5. Cut
6. Cut
∅= 25 mm
n5 =
∅ = 26mm
v
cf
= 400 m/min
400m π *m in* 0,025m
n5 = 5393 1 min
∅= 45 mm
n6 =
v
cf
= 400 m/min
400m π *m in* 0,045m
n6 = 2830 1 min
MTS TeachWare • CNC-Grundlagen • Student’s Book
107
Basic Geometry for CNC Machining 2. Example:
On a CNC-lathe the sketched bolt is to be roughed in four cuts with cutting depths of 6; 6; 5 and 5 mm, a feed of fv = 0,2 mm and a finishing allowance of 0,5 mm. Because of the various specified roughness heights the ∅ 45 will be finished with a feed of ff1 = 0.07 mm and all other surfaces with a feed of f f2 = 0.12 mm.
0 7
5 4
5 2
The lengths of the approach and retreat movements will each be programmed with 2 mm. 20
The machining time for roughing huv t and for finishing thuf as well as well as the entire machining time thu are to be calculated.
50 60
Calculating the machining time for roughing t huv and for finishing thuf
The machining time for turning is calculated with the following formula:
th =
L *i n *f
in min
The variables are:
• • • •
L i n f
Feed Path Number of Cuts Number of Rotations Feed per Rotation
The feed path L is calculated from the path in which the cutting edge is operating (length l = feed motion in Z and X !) and possible approach / withdrawal paths (length l a or lu) that are traveled in the feed. The following feed paths result for each cut with consideration to 2mm for the approach / withdrawal paths: 1. Cut
L = l + la + lu = 50mm + 6mm + 2mm + 2mm = 60mm
1. Cut
L = l + la + lu = 50mm + 12mm + 2mm + 2mm = 66mm
1. Cut
L = l + la + lu = 20mm + 5mm + 2mm + 2mm = 29mm
1. Cut
L = l + la + lu = 20mm + 10mm + 2mm + 2mm = 34mm
1. Cut
L = l + la + lu = 20mm + 1mm + 2mm + 2mm = 25mm
1. Cut
L = l + la + lu = 30mm + 12mm + 2mm + 2mm = 46mm
datum:
L = Feed Path i =1
108
unknown:
th in min
valid :
th =
L *i n *f
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Calculating the machining time for preturning t huv
1. Cut L = 60mm
2. Cut fv= 0.2 mm
n= 1537 1/min
L = 66mm
fv= 0.2 mm
n= 1938 1/min
L *i n *f 60mm * 1 min th = 1537 * 02 , mm
L *i n *f 66mm * 1 min th = 1938 * 02 , mm
, min t h = 0195
, min t h = 0172
th =
3. Cut L = 29mm
th =
4. Cut fv= 0.2 mm
n= 2476 1/min
L = 34mm
L *i th = n *f 29mm * 1 min th = 2476 * 02 , mm t h = 0,059 min
fv= 0.2 mm
n= 3428 1/min
L *i th = n *f 34mm * 1 min th = 3428 * 02 , mm t h = 0,050 min
0,195 min 0,172 min 0,059 min 0,050 min t huv =+++
t huv = 0,476 min Calculating the machining time t huf f for finishing
5. Cut L = 25mm
6. Cut fv= 0.12 mm
n= 5393 1/min
L = 46mm
L *i n *f 25mm * 1 min th = 5393 * 01 , 2mm t h = 0,039 min th =
fv= 0.07 mm
n= 2830 1/min
L *i n *f 46mm * 1 min th = 2830 * 00 , 7mm t h = 0,232 min th =
t huf = 0,039 min+ 0,232 min t huf = 0,271 min Calculating the entire machining time thug
t hug = t huv + t huf t hug = 0,476 min+ 0,271 min t hug = 0,747 min MTS TeachWare • CNC-Grundlagen • Student’s Book
109
Basic Geometry for CNC Machining 3. Example:
On a CNC-lathe the sketched bolt is to be preturned in four cuts with cutting depths of 6; 6; 5 and 5 mm and with a feed of f v = 0,2 mm. Because of the various specified roughness heights the ∅ 25 will be finish turned with a feed of ff1 = 0.07 mm and all other surfaces with a feed of f f2 = 0.12 mm.
5 4
7
5 2
The cutting speed for preturning is vcv =280 m/min and for finishing vcf =400 m/min. 20
The cutting edge curve for the preturning tool is r v = 0.8 mm and for the finishing tool rf = 0.4 mm.
50 60
The attained roughness height are to be calculated. Calculating the attained roughness heights R t
The roughness height reached by turning is calculated with the following formula:
f2
Rt =
in mm
8* r
The variables are:
• f • r
Feed per Rotation Cutting Edge Radius
datum:
f = 0.07 mm
datum:
f = 0.12 mm
r = 0.4 mm unknown:
in mm Rt
1. Calculating the roughness height the surface ∅ 45
Rt1.6
=
Rt1.6
=
Rt1.6
=
f 2 mm2 = mm 8 ⋅ r 1 ⋅ mm 0. 07
r = 0.8 mm unknown:
Rt1.6
Rt 6.3 = Rt 6.3 = Rt 6.3 =
3. 2
Rt 6.3 = Rt1.6
110
= 0,00153 mm
t
in mm
for 2. Calculating the roughness height the other surfaces
2
8 ⋅ 0. 4 0. 0049
R
f 2 mm2 = mm 8 ⋅ r 1 ⋅ mm 0.12
2
8 ⋅ 0.8 0. 0144 8 ⋅ 0. 8 0. 0144 6. 4
mm
Rt 6.3 = 0,00225 mm
MTS TeachWare • CNC-Grundlagen • Student’s Book
Rt 6.3 for
Technological Basics for CNC Machining
Calculating the cutting forces and the motor power For operating a CNC-machine it is important that the skilled worker understands the relevant mechanisms of the cutting force as well as the machining performance and the drive motor's rated power and actual output.. The multitude of variables influencing the cutting forces do not allow precise calculation with a formula. Some of these factors can only be determined in tests. This has shown, for example, that every material to be machined has a specific cutting force value which varies according to e.g consistency (hard or soft) or machining duration (short or long). Moreover, the tool, its cutting material and its characteristics should be considered. Also important are the programmed operation values, such as feed, number of rotations, cutting speed, chip thickness, chip diameter, machining mechanisms as well as the cutting edge geometry, whereby the angle of rake and the adjustment angle are especially relevant. The cutting edge wear also plays a role.
Example: From a cut.
∅ 60 mm shaft the sketched peg out of Ck 45 is to be preturned and then finish turned in one
Hard-metal corner cutting tools with indexable inserts are available (γ0=90°, κr=90°). The feeds are f v = 0. 2 mm and f f = 0.1mm , cutting speeds are vcv=200m/min and vcf=300m/min. Allowance after preturning is 0.5 mm. The output of the main drive motor is η=0,8. To be calculated: 1. the cutting force Fcv, 1. the cutting performance Pcv and 1. the required power output from the drive Pab .
Datum:
turning length l = 50 mm cutting depth ap = 4.5 mm feed f v = 0.20 mm cutting speed vcv=200m/min
adjustment angle κr=90° output η=0,8
MTS TeachWare • CNC-Grundlagen • Student’s Book
111
Basic Geometry for CNC Machining 1. The cutting force FC
The cutting force FC is calculated with the formula:
f
cutting force = chip diameter * specific cutting force
Fc = b ⋅ h ⋅ kc = a p ⋅ f v ⋅ k c , (with κr=90°) if κr is smaller than 90°, then b is calculated with
b=
ap
sin κ r
,
h = f ⋅ sin κ r kc11⋅ N kc = mc 2 , h mm
h aus
a und
where kcl-1 is the kc-value based on the test conditions and mc is a chip thickness index; kcl-1 and mc can be taken from the following table.
2
Specific Cutting Force k cin N/mm by thickness of cut h in mm
Materials
However, the formula mentioned above is not sufficient for calculating the cutting force. Various compensation factors must first be taken into account. After these compensation factors are considered, the applicable formula is as follows:
Fc = ap v⋅ f c ⋅ k ⋅ K γvo s⋅⋅Kch v Ker ⋅ K
[N ]
The compensation factors in the formula are:
Kγ0 is the angle of rake variation factor. It is calculated from
Kγ o = 1 −
γo
− γ ok
66. 7
, whereby γ0 is the given angle of rake and γok is the angle of rake used for de-
termining the kc-Werte. 112
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Kv is the cutting speed variation factor. The tabular values are only for the area between vc=90...125 m/min. It is taken from the following Kv-vc-Diagram.
Kv- vc - diagram:
The identificated Kv - values are valid for:
v K
v c in m/min Example:
Ksch is the cutting edge variation factor for hard-metal to cutting ceramic, whereby hard-metal is 1 and cutting ceramic is set between 0.9....0.95.
Kver is the cutting edge abrasion factor. It has to be estimated since the kc-values from the table only apply to working sharp tools. For this reason a Kver-value of 1.3...1.5 is used. Solution: The compensation value Ksch conform with the table provisions and can be set with 1. aP and All other values must be determined:
kc = kc =
Kγ o = 1 −
2220
Kγ o == 1 −
0.14
are given.
γ o − γ ok
kc11⋅ N hmc mm2 0.2
fv
66.7 10 − 6 66.7
Kγ o = 0,94
N kc = 2781 2 mm
Selected as the compensation values: Kver=1,3 and taken from the diagram Kv=0,96. For the desired cutting force this yields:
Fc = ap ⋅ f c⋅ k ⋅ Kγ v ⋅⋅Ksch verK K Fcv = 4. 5mm ⋅ 0. 2 mm ⋅ 2781 N / mm 2 ⋅ 0. 96 ⋅ 0. 94 ⋅ 1 ⋅ 1. 3 Fcv = 2936 N 0
MTS TeachWare • CNC-Grundlagen • Student’s Book
113
Basic Geometry for CNC Machining 2. The cutting performancPC
The cutting performance PC is calculated with the equation
m Pc = Fc ⋅ vc N ⋅⋅ min Pcv = 2936 N ⋅ 200
1 min 60 s
=
Nm
60 s
, using the values from the examples yields
m min
Nm , da 1Nm/s = 1W (Watt) ist, sind 9786,7 Nm/s = 9,787 KW s Pcv = 9. 787 KW Pcv = 9786, 7
3. The power output of the drive motorPab
With known cutting performacne the power output of the drive motor Pab is calculated with the formula:
Pab = Pab =
Pcv KW = KW η 1 9787 . 0.8
Pab = 1223 . KW
114
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Calculation examples of technological data for CNC milling Calculating the infeed speed vf
For milling the infeed speed vf is usually calculated in mm per min. However, the feed per tooth f z is just as important, since the skilled worker foremostly knows what feed a cutting edge can endure. This feed must be distinguished from a feed attained in a milling cutter rotation.
• infeed speed vf • feed per tooth
vf in mm / min fz in mm
• feed per rotation
f in mm
The following formulae are available for calculation:
v f = fn *z z *
in mm / min
vf = f *n
in mm / min
v f = f * nf=
z
*n *z
in mm / min
1. Example:
A plate made from C15 is to be milled in one cut using an end-face mill with indexable inserts. The step is 10 mm high. The cutting speed v c is 160 m/min and the feed per cutter edge f z is 0,18 mm. The end-face mill with ∅ = 63 mm has four cutting edges. How high is the infeed speed vf? datum:
vc = 160 m/min d = 63 mm fz = 0,18 mm z =4
unknown:
vf in mm/min
valid :
v f = fz * n * z vc
= π *d * n
n=
solution:
vc
π *d ,
, or
it follows:
vc v f = π * d * fz * z 160000mm vf = π *min* 63mm * 0,18mm * 4 v f = 582mm / min
MTS TeachWare • CNC-Grundlagen • Student’s Book
115
Basic Geometry for CNC Machining 2. Example: Calculating thein feed speed vf
On a CNC-vertical milling cutter the slot of the sketched work part is to be milled in one cut with a two-edged slot boring cutter of 12mm ∅, n = 1800 1/min number of rotations and a feed f z of 0.12 mm. How high is the infeed speed? datum:
n = 1800
1 min
f z = 0.12 mm z=2 unknown:
vf in mm/min
valid :
v f = fz * n * z
,
v f = 0,12mm * 1800 solution:
1 *2 min
v f = 432mm / min
3. Example Calculating the number of rotations n
How high must the number of rotations be when the slot is machined with a boring feed of 0.1 mm per edge and a longitudinal feed of 0.15 mm and with an infeed speed of 200 mm/min ? datum:
f b = 0.10mm f z = 0.15mm mm v f = 200
datum:
valid :
nb in
z=2 unknown:
1 min
nb =
vf
mm fb ⋅ z min⋅ mm
valid :
nl in
1 min
nl = n =
nb =
116
f
200 0.1 ⋅ 2
nb = 1000
1 min
f z = 0.12 mm
min
unknown:
n = 1800
1
vf
mm fzl ⋅ z min⋅ mm 200
1
015 . ⋅ 2 min 1 min
nf = 667
min
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Calculating the cutting force and motor power For calculating the cutting force, the same compensation factors are used for milling as in for turning..
ap cutting depth ae entering point b chip width Fcz cutting force per edge (mean) ϕs entering angle hm middle chip thickness f z feed per edge z number of cutter edges ze number of edges in operation D diameter of milling cutter angle of twist of edges λ adjustment angle of edges κ kc specific cutting force kc1-1 specific cutting force related to chip diameter b ⋅ hm =1 mm mc chip thickness index
ϕs
These are either taken from a book of specifications or, as in the case of the angle of rake variation factor, calculated with the formula
Fc =⋅ Fcz e z N ⋅ 1 = N z ⋅ϕs
ze =
Fcz = b ⋅mh c⋅ k b=
cos λ
66. 7
. For milling, the cutting force is:
. In this formula
and
360°
ae
γ o − γ ok
Kγ o = 1 −
. Herewith are
mm
hm = f z ⋅ sin κ ⋅
and
360°⋅ae mm d ⋅ π ⋅ϕs
.
κ=90°-λ for milling cutters with angle of twist.
Taking into account the compensation factors, the cutting force can be calculated with the formula:
N Fc =e z ⋅ bm⋅ch ⋅k ⋅ Kv γ o ver⋅ K ⋅ K mm ⋅⋅mm = N and with ze , b , hm yields the formula mm2 Fc =
z ⋅ϕs
⋅
ae
⋅
360° cos λ
360°⋅a p
π⋅
ϕs
f⋅
z
⋅ sinkκK⋅ Kc ⋅
γo
⋅
v
⋅ Kver
⋅d
MTS TeachWare • CNC-Grundlagen • Student’s Book
117
3.4
Calculation of technological data for CNC machining
Example:
As shown in the figure, a guide recess should be milled with a 4-edged end-face mill ∅=40 mm into a guide plate made of C35. data :
miller diameter d = 40mm milled width ae = 40mm milled depth ap = 6mm feed f z = 0.12 mm angle of rake γ0 = 10° angle of twist λ = 30° adjustment angle κ = 90° material C35 machine output ηM = 0.82 cutting speed vc=140mm/min
Calculating the cutting force F c
Fc = Fc =
z ⋅ ϕ s a e 360°⋅a p ⋅ ⋅ f⋅ 360° cos λ π ⋅ ϕ s ⋅ d 4 ⋅1
⋅
40
⋅
360°⋅6
360° cos 30° π ⋅ 1 ⋅ 40
z
⋅ sinkκK⋅ cK⋅ Kγ o ⋅
v
⋅
ver
mm N 1mm ⋅ 1 ⋅ mm ⋅⋅mm mm2 ⋅1 = N
⋅ 0.12 ⋅ sin 90°⋅kc ⋅K γ oK⋅ vK ⋅ver
;
the kc-value can not be taken directly from the table. It is calculated as follows:
kc =
kc11⋅ h mc
,
kc11 with 1860 can be taken from the table as well as mc with 0.2. The hm-value is calculated as follows:
hm =
360°⋅a p
π ⋅ϕs ⋅ d
⋅ f z ⋅ sin κ
Consequently,
360 ⋅ 6 = 3. 87mm and π ⋅ 44. 4 ⋅ 40 1860 kc = = 1420 . 0.2 3.87 mm 2 γ −γ 10 − 6 Kγ o = 1 − o ok = 1 − = 0. 94 66. 7 66. 7
hm =
Kv with 0.97 is taken from the diagram. 1.3 is selected for the edge abrasion compensation value Kver. All values for the cutting force are therefore established and can be calculated: Fc = Fc
4 ⋅ 40 ⋅ 6 ⋅ 01 . 2 ⋅1
0.866 ⋅ π ⋅ 40 = 1782 N
⋅⋅⋅⋅ 1420
0. 94 0. 97 13 .
Calculating the cutting performance P c
The following formula is used for calculating the cutting performance Pc:
Pc = Fc *v c
Pc = 1782N * 140 Pc = 1782 * 140
m min
Nm 60s
Pc = 415W
118
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Calculating the required motor output P ab
The following formula is used for calculating the motor output Pab:
Pab = Pab =
Pc
ηM c 0,45KW 0,82
Pab = 055KW Calculating the machining time
In one cut the sketched base sheet made from ST50 (see fig. 1) is to be milled in 12 mm gradations with a three-edged end mill of 32 mm∅ and 16 mm cutting edge lengths. How long is the machining time of the CNC-machine when milled with a feed of 0.12 mm per cutter edge and cutting speed of 120 mm/min? The lenghth of the approach and retreat movements are 22 mm. data:
material: ST50 miller diameter d =32 mm feed per edge f z = 0.12 mm cutting speed
v c = 120
m
min
approach and retreat movements = 22mm cutting depth ap = 12mm work part length Ll = 90mm work part depth Lb = 50mm
The following formula is used for calculating the machining time tnu:
Lges ⋅ i mm ⋅ 1 mm ⋅ min = mm = = min t nu = f vc mm min tnu =
(L2 Ll + 2 AÜ b +2 ;; with
)
f vc
vc 0.12 ⋅ 3 ⋅ 140 = f vc = ⋅π d ⋅π 0032 . 2 ⋅ 110 + 2 ⋅ 70 + 2 ⋅ 22
f vc= f z ⋅ z ⋅ tnu =
=
f vc = 501
mm min
yields:
501
tnu = 0.81 min
3.5
CNC clamping systems
Types of clamping systems A clamping system attaches the work part to the machine tool. It must fulfill two essential functions:
MTS TeachWare • CNC-Grundlagen • Student’s Book
119
3.5
CNC clamping systems 1. It must clearly determine the position of the work part. 1. It must detain all forces from the work part.
The clamping elements constrain the work part and the required force for this is called clamping power. In order to keep the costs for the clamping system as well as for production low, further requirements are made on the clamping system:
• • • •
simple and quick handling versatile usage easy exchangeability of the clamping elements high accuracy with repeated clamping
Clamping power generation Manual clamping is usually used on conventional machine tools. This requires a high energy exertion by the worker. Special clamping systems for individual clamping equipment has been developed to reduce auxiliary times and ease clamping for the worker. Various methods are used for generating clamping power:
• • • •
mechanical clamping power generators hydraulic clamping power generators pneumatic clamping power generators electric clamping systems
Mechanical clamping power generatorsare usually in the form of wedge lever-type or bellcrank lever-type power chucks. These types of force chucks are usually used for turning machines.
1
4
3 2
chuck drawbar wedge lever jaws Figure 125 wedge lever-type power chuck (mechanical)
chuck drawbar bellcrank lever jaws figure 126 Bellcrank lever-type power chuck (mechanical)
Hydraulic clamping fixtures generate the movement and power needed for clamping with hydraulically powered pistons. These are usually manually controlled by the operator with valves. The clamping power can be accurately controlled and is monitored on a display. Although hydraulic systems require high technical effort, they are quite reliable.
120
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Figure 127 Hydraulic actuating cylinders with through-hole Röhm SZ
Pneumatic clamping fixturesare operated with air pressure and function similiarly to hydraulic clamps. Compressors are used for generating air pressure (compression).
Figure 128 Air actuating cylinders with through hole Röhm LHS
MTS TeachWare • CNC-Grundlagen • Student’s Book
121
3.5
CNC clamping systems
Electric clamps which rotate are used for force chucks with geared scroll systems. They enable a quick adjustment to various work part diameters.
An electromagnetic clutch in the clamp blocks the spindle during the clamping and declamping process, so that the full clamp torque is transmitted to the chuck. Furthermore, there are electric clamps with stroke movements for operating clamping devices and force chucks.
:
thread spindle
:
tie bar
:
clutch
:
epicyclic gears
:
motor
Figure 129 Electric clamp with stroke movement
122
thread nut
:
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
Types and characteristics of clamping devices for turning The different clamping devices for turning will be introduced in this section. In general, the following clamping variations can be distinguished:
• clamping in chucks • clamping with collets • clamping between centers • clamping on mandrels • clamping on faceplates • clamping with turning fixtures • clamping using steady rests Clamping in chucks Chucks are differentiated according to the number of jaws, i.e. two-, three- and four-jaw chucks. Selfcentering three-jaw chucks are most commonly used. They guarantee a quick, secure and centered mounting of round blanks. With a four-jaw chuck, four-, eight- or twelve sided blanks as well as round blanks can be clamped.
Figure 130 Self-centering three-jaw chuck Röhm ZG-ZS
Figure 131 Self-centering four-jaw chuck Röhm ZG-ZS
The jaws are usually hardened and have increments. The jaws can be adjusted so that they can clamp parts with various diameters. By exchanging jaws the turned parts can be either clamped from the inside or outside. Clamping power transmission is usually based on the principal of geared scrolls or key bars.
MTS TeachWare • CNC-Grundlagen • Student’s Book
123
3.5
CNC clamping systems
Clamping power with a geared scroll
Chucks with geared scrolls are for lower clamping power. Only low force can be transmitted since the area between the geared scroll and the jaw is so small.
Figure 132 Geared scroll chuck Röhm EG-ES
Figure 133 Jaw operating mechanism
The disadvantage of chucks with geared scrolls is that changing requires the chucks to be fully dismounted.
:
reversible top jaw
:
adjusting screw spindle
:
base jaw
:
pinion
:
scroll
: :
pinion holder screw operating screw
:
adjusting key
Figure 134 Geared scroll chuck Röhm EG-ES Operation: The rotation of the pinion (4) causes the scroll (5) to turn. The base jaw (3) consequently moves towards the turning axis and clamps the work part.
124
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Clamping power with a key bar
The key bar chuck enables a quick change of jaws and generates higher clamping power than chucks with geared scrolls.
Components: 22
cover
33
indicator pin
51
body
23
drive ring
34
bearing
56
key bar with inner thread
24GB
base jaw
35
thrust ring
57
press pin
24EB
one-piece jaw
36
pressure spring
58
locking slide
25
reversible top jaw
37
pressure spring
76
chip guard
27
operating screw
38
taper key
90
key with toggle
28
slide
39-42
socket head cap screw
29
jaw retaining pin
44
straight pin
Figure 135 Chuck with thrust ring and key bars Röhm Duro Operation The tangentially arranged operating screw (27) engages the internal thread of the actuating key bar (56) to move a slide (28) which in turn moves the drive ring (23). Two further slides in the drive ring (23) transmit the force to the other key bars. The key bars are provided witch helical teeth which engages the teeth of the base jaws (24GB) so that the work part is gripped accurately and concentrically.
MTS TeachWare • CNC-Grundlagen • Student’s Book
125
3.5
CNC clamping systems
Clamping with collets
Collets enable cylindrical work parts to be quickly and accurately clamped. The collet clamps the work part from the outside. Collets are usually only applicable for one work part diameter or a component group since it only has a minimal, radial range of adjustment.
:
work part
:
clamping bocy
:
spindle
:
clamping tube
Figure 136 Collet
Clamping between centers
Clamping between centers is applied for longer parts. The work parts must be cut to length and centered on both sides.
Figure 137 Clamping between centers The following possibilities for clamping between centers can be distinguished based on the maching specifications:
• face drivers with revolving or fixed centers • driver with a vise chuck with clamping ring revolving or fixed centers
126
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Face drivers are generally contained by the main spindle. They are used when the entire surface is to be machined. The work part is clamped between the face driver and the tailstock. A disadvantage is that only low torques are transmitted.
Figure 138 Face driver Röhm 681 The revolving tailstock center is inserted into the tail spindle of the tailstock. Since the center can revolve on its own, higher cutting speeds during turning operation are possible.
Figure 139 Revolving tailstock center Röhm 601
MTS TeachWare • CNC-Grundlagen • Student’s Book
127
3.5
CNC clamping systems
The application area of dead centers is very limited. They only enable minor cutting depths because they warm up and wear too quickly.
Figure 140 Dead center Röhm 667
Figure 141 Dead center with half point Röhm 670
A vise chuck with clamping ring centers the work part and additionally radially clamps it with a clamping bolt. Consequently, larger torques can be transmitted and a higher machining performance is reached.
:
driving disk
:
sleeve with clamping bolt
:
work part
Figure 142 vise chuck with clamping ring
128
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Clamping on mandrels Work parts that have a bore hole, which can be very small, are clamped from the inside with clamping mandrels. Two types can be distinguished: fixed mandrels and expanding mandrels.
Fixed mandrels are minimally conical (cone 1:2000) and are clamped between centers. They are only used for finish turning since only low cutting depths are possible. The rotary accuracy of the centers must be checked before being used. Expanding mandrels are inserted into the inner cone of the main spindle. Clamping is established by the slotted clamping part of the mandrel according to the rotary accuracy as well as by an even grip on the work part. Clamping is enabled by pressing in the taper plug.
Figure 143 Cartridge mandrels Röhm
:
clamping ring
:
clamping sleeve
Figure 144 Cartridge mandrel Röhm MZB Expanding mandrels are clamped between centers and only have a minor clamping area. They operate by expanding a thin-walled, non-slotted sleeve made from a plastic for elastic deformation.
MTS TeachWare • CNC-Grundlagen • Student’s Book
129
3.5
CNC clamping systems
Clamping on face plates
Face plates enable irregularly formed parts to be clamped. The four or more clamping pistons can individually be adjusted as well as be turned. The clamping areas are constructed so that outer and inner clamping is possible. Attaching fixtures and compensating weights is possible with the available clamping slots.
Figure 145 Hydraulically operated 6-jaw pull-down finger chuck Röhm
Clamping with turning fixtures The perforated disk with threaded borings offers a variety of clamping possibilities. However this clamping method requires a careful gyrating mass compensation, because the spindle run will otherwise be imbalanced. This consequently leads to imprecise machining results and in the worst case, damage to the machine tool..
:
work part
:
clamping body
:
clamping bridge
:
gyrating mass compensation
Figure 146 Turning fixture
130
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Clamping with steady rests
Steady rests are used for clamping long, slim work parts in order to withstand work part bending caused by cutting force and own weight.
Figure 147 Self-centering steady rests Röhm SLZ The work part is clamped between centers and additionally supported by steady rests.
Figure 148 Fixed steady rest
MTS TeachWare • CNC-Grundlagen • Student’s Book
131
3.5
CNC clamping systems
Types and characteristics of clamping devices for milling Various possibilities for clamping work parts on milling cutters are introduced in this section. The following clamping variations can be distinguished.
• Jaw Chucking • Magnetic Chucking • Modular Chucking Jaw Chucking
1.
The vise can be turned in steps of 90° on the machine table.
2.
Its position can be changed.
3.
The chucked part can be moved along the x- and z-axes.
Magnetic Chucking
1.
The position of the part on the machine table can be freely defined.
Modular Chucking
1.
The position of the part on the machine table can be changed.
2.
The chuck elements can be defined as modules. The chuck position is specified by the user.
132
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining
The milling cutter machine table with its T-slots is the basis for work part clamping. Depending on how the work part is to be clamped, the following clamping devices can be distinguished:
• • • •
mechanical clamping devices hydraulic clamping devices pneumatic clamping devices electric clamping devices
Mechanical clamping devices Mechanical clamping devices usually consist of various individual components, e.g. clamping iron, clamping board and clamping bolts with T-nuts.
1
3
2
:
work part
:
clamping iron
:
clamping board
:
machine table
:
support element
:
work part
:
clamping iron
:
clamping board
:
machine table
4 Figure 149 Clamping iron and clamping bard For bedding with heavy work parts, alignment and support elements are used.
1 2
3
4
5 Figure 150 Clamping iron, clamping board and support element
MTS TeachWare • CNC-Grundlagen • Student’s Book
133
3.5
CNC clamping systems
Shallow clamps are used for flat work parts whose surfaces need to be kept free for machining.
:
work part
:
shallow clamp
Figure 151 shallow clamp A dividing apparatus with circular table enables work parts to be quickly and symmetrically machined from both sides. It is also possible to flange a chuck to a dividing apparatus which then can be used for accurately dividing and machining round work parts.
Figure 152 Dividing apparatus with circular table
134
MTS TeachWare • CNC-Grundlagen • Student’s Book
Technological Basics for CNC Machining Machine vises
Machine vises are easy to use and reliable. They are used for clamping smaller work parts. Alignment is achieved with a measuring gauge.
Figure 153 Machine vise Röhm UZ The clamping force transmission of machine vises is illustrated in the following figure.
Figure 154 Power transmission Universal machine vises can be horizontally as well as vertically turned. Furthermore, there are also vises that pneumatically generate clamping power.
Figure 155 Precision sine vise Röhm PS-SV
MTS TeachWare • CNC-Grundlagen • Student’s Book
135
3.5
CNC clamping systems
Pneumatic and hydraulic clamping devices
High precision NC vises, that are operated by pneumatic and hydraulic clamping cylinders, are used for CNC-machine tools. Pneumatically operated high precision NC vises allow short opening and closing times. However, the low operating pressure impedes high clamping power. On the other hand, depending on the pressure adjustment, hydraulic clamping elements can exert high clamping power.
Figure 156 High precision NC vice Röhm RBA The construction of a high precision NC vises is illustrated in the following figure.
1
fixed clamping jaw
2
movable clamping jaw
3
hydraulic unit
4
movable jaw
5
spindle
6
spindle nut
7
basic body
8
pneumatic spring
Figure 157 High precision NC vice Röhm RBA Magnetic clamping devices
Work parts made of iron can be clamped with electromagnetic devices. The work part is drawn to the clamping plate after a current is switched on. It can be easily removed after the current is switched off.
Figure 158 Electromagnetic clamping plate
136
MTS TeachWare • CNC-Grundlagen • Student’s Book
Control test „Technological Basics“
7.
Control test „Technological Basics“
1.
What does a tool system on a CNC-lathe consist of?
1.
Why are hard-metal indexable inserts primarily used for tools for CNC-machine tools?
1.
Roughly describe the application areas of hard-metals.
1.
Explain the significance of the clearance angle for machining tools.
1.
What are the advantages of a larger angle of rake for the machining process?
1.
What are the disadvantages of a larger angle of rake for the machining process?
1.
When are negative are negative angles of rake necessary?
1.
What is the significance of the adjustment angle for the machining process?
1.
Exercise: Calculating the number of rotations A shaft with a diameter of d=80mm is to be roughed with vc=120m/min. How high is the number of rotations n?
1.
Exercise: Calculating the cutting speed A disk with a diameter of d=250mm rotates with n=100 /min. How high is the cutting speed vc during turning at the circumference?
1.
Name the functions of a clamping system.
1.
Name the different types of chucks.
1.
What parts are clamped on a faceplate?
1.
When are steady rests used?
1.
Name the different types of clamping power generators.
1.
Name the clamping possibilities on a milling cutter.
1.
What advantages do fixtures have?
MTS TeachWare • CNC-Grundlagen • Student’s Book
137
3.5
138
CNC clamping systems
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
8.
4 Introduction into NC programming
4.1
Work organization and flow of manual NC programming
Comparison of work preparation of conventional and CNC machining CNC-manufacturing has advantages over manufacturing with conventional machine tools, e.g. shorter production times and a higher manufacturing capacity. In order to effectively use these advantages, the work preparation must be accordingly adapted. The objective of manufacturing is to keep the machining time on the machine tool as high as possible. However, to achieve this extensive planning must be done. On conventional machine tools, the skilled worker can only produce or plan. However, on a CNC-machine tool, the worker can concentrate on planning in parallel to the autonomous execution of the NC-program. This consequently leads to much higher machining times on the CNC-machine tool. Using conventional machine tools for production, the workshop drawing, a work plan and work order are available to the worker. Furthermore, the worker must thoroughly plan the work steps and select the tools. Since tool measuring is not possible on conventional machine tools, following each operation the tools must be marked (touched) and then be measured. These steps are redundant when using a CNC-machine tool. However, this does require the tools to be precedingly measured. Many prepatory tasks can be transferred to the machine for CNC-work preparation. The objective is to allocate all documents, tools and clamping devices as well as the blanks so that setting-up and production can immediately begin. The tasks of work preparation can be divided into the following categories:
• creating the required documents, • tool measuring, • managing tools and clamping devices, and • allocating all documents and accessories. The documents required for CNC-manufacturing are much more defined compared with those for manufacturing on conventional machine tools. Creating these documents takes more time, however they are then immediately accessible for repeated orders. In addition to the NC-program, a set-up form is created for setting-up the CNC-machine tool. All information on the used tools and the tool part’s clamping situation is documented in this form. Tool measuring enables the autonomous operation of the CNC-machine tool and easy application of tools on various machines. Tool and clamping device management is more extensive in CNC-work preparation, since they are generally more varied than those for conventional machine tools and accordingly their description is more detailed. The data is stored in tool and clamping device indices. A complete allocation of all documents, preset tools and accessories enables the quick set-up of the CNCmachine tool. The objective is to avoid machining delays and therefore, increase machining time
MTS TeachWare • CNC-Grundlagen • Student’s Book
139
4.1
Work organization and flow of manual NC programming
Organizing the steps of NC programming NC-programs can be generated in different departments. Accordingly, the following forms of NCprogramming can be differentiated:
• programming as part of production organization and • programming in the workshop. The organizational classification of both these forms is illustrated in the following figure.
figure 159 Organizational classification of NC-programming Programming as part of production organization
All planning measures for realizing a manufacturing order are carried out in the department for production planning and precede manufacturing. Programming in this department is termed external programming since the department is outside the workshop area. The NC-programs are written by staffmembers who are specifically trained in NC-programming. They usually work at a programming terminal and create the programs on a computer. Programs are not only generated here but managed as well. The connection to the CNC-machine tool is over a DNC-system. It is practical to generate programs in production planning when
• • • •
extensive NC-programs or NC-programs for complicated work parts are to be created, when many NC-programs need to be managed or when there are many CNC-machine tools.
Disadvantageous is that
• the NC-programs must be optimized on the CNC-machine tools and • there is little contact with the workshop. 140
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Programming in the workshop
Generating NC-programs in the workshop is known as machine-based programming. The NC-programs can either be directly created on a machine or at a programming terminal near the machines. The NC-programs written in the workshop and in production planning are directly controlled and optimized on the CNC-machine tool by the operator during set-up. It is practical to generate programs in production planning when:
• • • • •
the experience of the workshop staff is to be considered, short NC-programs or NC-programs for simple tool parts are to be created, there are only few CNC-machine tools, or available NC-programs are to be quickly accessed.
Disadvantageous is that
• the workshop personnel needs to specially trained and • lengthy programming time can possibly result in machining standstill.
Differences between the programming types
For manual programming, the programmer formulates the NC-program so that it can be directly understood by the CNC-control. Every step that a CNC-machine tool is to execute must be individually programmed. Extensive geometric calculations must be made with respect to the CNC-control efficiency and the geometric complexity of the work part. Possible errors or collisions with e.g. clamping devices can not be automatically detected. Simulations, which illustrate the tool movements, are integrated into most CNC-controls for testing the NC-program. For computer-aided (automatic) programming, the programmer is supported by a programming system. This system takes over routine work that is susceptible to error when programming manually, such as calculating coordinates and cutting data. The fundamental difference to manual programming is that not the tool path is defined step-by-step, but rather how the tool part is meant to look after machining. The geometric and technological data is herewith strictly separated. For automatic programming the sequence of operations for generating a NC-program is as follows: 1. First the work part must be geometrically defined. A representation of the finished part as well as the blank is necessary. 1. Subsequently, the individual machining operations are specified. The programming system assists the programmer in selecting the appropriate tool and automatically calculates the necessary cutting data. 1. Finally a NC-program for a specific CNC-machine tool with a specific CNC-control is generated and can then be transferred to the machine.
MTS TeachWare • CNC-Grundlagen • Student’s Book
141
4.1
Work organization and flow of manual NC programming
CNC-programming can be done with different procedures and at different places. An overview of these possibilities is given in the following figure.
figure 160 Overview of NC-programming procedures and systems
142
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Programming procedure for manual NC programming at programming seat Manufacturing on CNC-machine tools requires thorough planning and production preparation. All operations that are executed by a skilled worker on a customary turning or milling machine must be well thought-out and defined by the programmer in advance. In manual NC-programming, the programmer formulates the machining task in an NC-program without assistance from a programming system. The subsequent steps are herewith followed: 1. definition of machining steps 1. definition of necessary tools 1. calculation of technological data 1. calculation of geometric data 1. generating NC programs for individual machining processes 1. control of NC programs The partial tasks to be executed are illustrated in fig. 3 and are subsequently explained.
MTS TeachWare • CNC-Grundlagen • Student’s Book
143
4.1
Work organization and flow of manual NC programming
figure 161 NC Programming Phases
Definition of machining steps Specifying the machining sequence structures the NC-program to be generated. The programmer defines the individual operations based on the production drawing. Furthermore, the necessary clampings and the applicable clamping devices are registered in a clamping plan. Similarly, the individual machining steps are registered in an operation sheet. Definition of necessary tools The programmer specifies the tools needed for each machining step. The tools are selected from a tool in-
dex. Calculation of technological data The cutting data with respect to the material and the used tool must be specified for each machining step. Calculation of geometric data The coordinates needed for programming traverse are taken from the production drawing or are specified by calculating known coordinates. Generating NC programs for individual machining processes With respect to the previously determined geometric and technological data, the programming steps are registered on a programming sheet. Control of NC programs The travel movements are simulated on a CNC-machine tool in order to detect and control programming errors.
144
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Quality assurance during CNC production The quality of parts manufactured on conventional machine tools is especially dependent upon the machine operator’s training and constancy. In contrast, identical work parts of consistent quality can be repeatedly manufactured on CNC-machines over a long period of time. The following factors can affect the quality of the manufactured work part:
• the created NC-program, • tool abrasion (cutting-edge life of the tool edge), • the work part material (characteristics and form), • the CNC-machine (precision and non-oscillating installation), • environmental factors (temperature effects) and • the operator’s behavior (error recognition with respect to quality). Possibilities for regulating quality How can the factors influencing quality be minimized?
• Test, optimize and carefully run the program for the first work part as well as make necessary corrections with respect to accurate dimensioning.
• Tool wear can be monitored on a CNC-machine. This monitoring function is done by the CNC-control, e.g. when the maximum machining duration for the tool has been reached, the tool is automatically replaced by an identical one. Another possibility for determining abrasion is with a modern CNCmachine equipped with a cutting force gauge. Herewith a tool is automatically changed as soon as the cutting force increases beyond a set limit. Deviations in dimension can be detected with integrated measuring systems. For internal toolfig. measur• ing, e.g. a probe is incorporated in a collision-free position in the turret of a CNC-lathe (see 4). In the cyclical sequence of part manufacturing, a measuring process is included and automatically implemented. This process is executed by a CNC-measuring program accessed by the CNC-control.
1 probe tool
3
turret
2 Figure 162 Internal tool measuring
• Calibrated measurement and test techniques for precise measuring and verification. • Operator training. • Air-conditioning the workshop rooms. • Observing quality when purchasing and installing a machine.
Workshop
MTS TeachWare • CNC-Grundlagen • Student’s Book
145
4.2
NC programming basics
The different programming procedures, the NC-program management as well as the clamp and tool indices should be demonstrated.
4.2
NC programming basics
A NC-program comprises a series of commands with which the CNC-machine tool is instructed to manufacture a certain tool. For each machining process on a CNC-machine tool, the NC-program has a command with relevant information. These commands are alphanumerically coded, i.e. they consist of letters, numbers and characters.
NC programming standards (ISO) The ISO-Norm 6983 strives for standardizing the NC-programming of machines in the production area. This is however limited to standardizing certain commands as well the general structure of a NC-program. CNCcontrol manufacturers have considerable liberty for incorporating their own NC-commands in their controls. Subsequently, the general structure of an NC-program according to ISO 6983 is illustrated.
Structure of an NC program Structure of an NC program: A complete NC-program consists of the following elements: % TP0147
NC-program beginning,
N10 G54 X80 Y100...
a series of NC-blocks
...
with the information for machining and
N75 G01 Z-10 F0.3 S1800 T03 M08 ...
a command for ending the program.
N435 M30
figure 163 Structure of an NC-program The program beginning consists of a character or a command (ex. %) which informs the CNC-control that a NC-program will follow. Additionally, the first line of the NC-program also contains the program name (ex. TP0147). Furthermore, both characteristics are also important for the NC-program manager as well as for calling the NC-programs in the CNC-control. NC-program names can contain alphanumerical or numerical characters. For most CNC-controls 2-6 digit character sequences are used for identification. An NC-program consists of a chronological sequence of blocks. They contain the relevant geometric and technical information that the CNC-control requires for each machining step. The program end is commanded with M30 or M02. Everything that stands before the character % for commenting the program is ignored by the control. This enables any explanations on the program or tool to be attached preceding the actual program. Comments are also allowed within a program, e.g. for identifying particular blocks. These, however, must be set in brackets.
146
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Structure of a program block Every NC-block consists of a block number, a number of words as well as a specific control character which informs the CNC-control that the NC-block has ended. This control character is called LF for line feed. It is automatically generated in NC-programming when the enter-key of the CNC-control or the enter-key on the PC-keyboard is pressed. N75
G01
Z-10.75
F0.3
S1800
T03
M08
LF
Number of the NC-block
Word
Word
Word
Word
Word
Word
invisible block ending character
figure 164 Structure of a program block
Structure of a program word A word consists of address letters and a number with a plus/minus sign. The definition and sequence are designated in the programming instructions of the CNC-control systems. Depending on the address letter, the number either pertains to a code or a value. Example
Address
Number
Definition
N75
N
75
For the address N, 75 is the number of the NC-block.
G01
G
01
For the address G, 01 is a code. The NC-command G01 is "Moving
Z-10.75
Z
-10.75
the tool along a straight line at infeed speed". For the address Z, -10.75 is a value. Corresponding to the NCcommand G01 of the preceding NC-block example, this means that the tool is to be moved to the position Z=-10.75 in the current tool coordinate system.
figure 165 Structure of a program word The form of numerical entry depends on the CNC-control: Z-35.5 is equivalent to e.g. the same target coordinates as Z-035.500. For most CNC-controls the positive sign "+" can be excluded in the NC-program. Generally, three groups of words in an NC-block can be differentiated: G-Functions
Coordinates
Additional and Switching Functions
G00
X
F
G01
Y
S
G02
Z
T
G54
M
figure 166 Groups of program words
MTS TeachWare • CNC-Grundlagen • Student’s Book
147
4.2
NC programming basics
The sequence of the words in an NC-block is designated as follows: Address
Definition
1.
N
block number
2.
G
G-functions
3.
X, Y, Z
coordinates
4.
I, J, K
interpolation parameter
5.
F
feed
6.
S
speed
7.
T
tool position
8.
M
additional functions
figure 167 Sequence of program words Words that are not needed by a block can be excluded. Block number N The block number is the first word in a block and designates it. It can only be conferred once. The block number has no influence on the execution of the individual blocks since they are invoked following the order in which they were entered into the control. G-function Together with the words for the coordinates, this word essentially determines the geometric part of the NCprogram. It consists of the address letter G and a two-digit code. Coordinates X, Y, Z The coordinates X, Y, Z define the target points that are needed for travel. Interpolation parameters I, J, K The interpolation parameters I, J, K are e.g. used to define the center of a circle for circular movements. They are usually entered incrementally. Feed F The speed at which the tool is to be moved is programmed with the function F. The infeed speed is usually entered in mm/min. For turning, the unit mm/U pertaining to spindle rotation can also be used. Spindle speed S The function S is for entering the spindle speed. It can be directly programmed in rotations per minute. Tool position T The address T together with a numerical code designates a specific tool. The definition of this address differs according to the control and can have the following functions: • Saving the tool dimensions in the tool offset table • Loading the tool from the tool magazine. Additional functions M The additional functions, also known as auxiliary functions, primarily contain technical data that is not programmed in the words with address letters F, S, T. These functions are entered with the address letter M and a two-digit code.
148
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Comparison of programming codes/keys of various CNC controls The basic commands are standardized in ISO 6983. CNC-control manufacturers add their own extensions or commands to these basic ones. Subsequently, a comparison of commands in different controls is given
Description
MTS
OKUMA
FANUC 16M
rapid traverse linear interpolation in slow feed motion
G00 G01
G00 G01
G00 G01
circular interpolation clockwise
G02
G02
G02
circular interpolation counter-clockwise
G03
G03
G03
Dwell Time
G04
G04
G04
cancel Cutter or tool nose compensation
G40
G40
G40
Cutter or tool nose compensation: left
G41
G41
G41
Cutter or tool nose compensation: right
G42
G42
G42
Maximum spindle speed designation
G50
Select work cordinate system one
G54
Activate absolute dimensioning
G90
G90
G90
Activate incremental dimensioning
G91
G91
G91
feedrate in mm per min
G94
G94
G94
feedrate in mm per revolution
G95
G95
G95
Constant Speed Cutting ON
G96
Constant Speed Cutting OFF
G97
X-coordinate of the target point
X
X
X
Y-coordinate of the target point
Y
Z-coordinate of the target point
Z
Z
Z
Distance between starting position and circle center in X
I
I
I
Y
Distance between starting position and circle center in Y
J
Distance between starting position and circle center in Z
K
K
K
J
spindle speed
S
S
S
Feedrate
F
F
F
Tool Changing
T
T
T
activate the spindle in clockwise rotation activate the spindle in counter-clockwise rotation
M3 M4
M3 M4
M3 M4
deactivate the spindle
M5
M5
Mounting the tool
M5 M6
Activate coolant
M8
M8
M8
deactivate coolant
M9
M9
M9
Program hold
M00
M00
M00
program end and backspacing
M30
M30
M30
MTS TeachWare • CNC-Grundlagen • Student’s Book
149
4.2
NC programming basics
Select the higher spindle speed Range
M42
ignoring spindle rotation M code answer
M63
150
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming CNC Exercise
In the following NC-program, the contour of a pre-turned part is finished. For each command give the corresponding definition. Block No. N05
Commands
Description
O 0300
0300 program name
T040404
select the tool from the turret position 4
M3 M42 M63 G96 S140 N10
G50 S3000
N15
spindle speed (revolution per minute)
G0 X20 Z2 M8
N20
G1 X20 Z0 G42
N25
G3 X28 Z-4 I0 K-4
N30
G1
N35
G2
Z-28 X34 Z-31 I3 K0 N40
G1 X38
N45
Z-33 G1
N50
G1
Z-53 X44
MTS TeachWare • CNC-Grundlagen • Student’s Book
151
4.2 Block No. N55
NC programming basics Commands
Description
G3 X50 Z-56 I0 K-3
N60
G1 Z-64
N65
G2 X62 Z-70 I6 K0
N70
G1 X66
N75
G1 X71 Z-72
N80
G1 X76
N85
G40
N90
G0 X500 Z500 M5 M9
N95
152
M30
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming CNC Exercise
In the following NC-program, the contour of a work part is milled. For each command, give the corresponding definition. Block No.
Commands FX100
N05 N10
Description program name
G54 G90 G49
cancel tool length compensation
G80
cancel canned cycle
G40
N20
G17
select the X-Y-plane
G21
metric input
G91 G28
reference point return
Z0. M9 N25
G91 G28
reference point return
X0. Y0. N30
T01
select the tool number 1 from the magazine
M06 N35
G90 S1600 M03
N40
G0 G43
tool length compensation
Z20. H17 N45
X-20.
N50
Z-6.
N55
G1
offset number for the tool length
Y-20. M08 G41
N60
X10. D1
offset number for the cutter radius
F250.
feedrate (in mm per min)
G1 Y82.
MTS TeachWare • CNC-Grundlagen • Student’s Book
153
4.2
Block No. N65
NC programming basics
Commands
Description
G2 X18. Y90. R8.
N70
radius of the circle
G1 X82.
N75
G2 X90. Y82. R8.
N80
G1 Y18.
N85
G2 X82. Y10. R8.
N90
G1 X18.
N95
G2 X10. Y18. R8.
N100
G3 X-10. Y38. R20.
N105
G0 G40. X-20. Y-20.
N110
G0 Z40. M5
154
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block No. N115
Commands
Description
G91
activate incremental dimensioning
G28
reference point return
Z0. M9 N120
G90 G80
cancel canned cycle
G49
cancel tool length compensation
G40 N125
M30
Workshop
On the CNC-machine tools, available NC-programs are to be loaded and be executed step-by-step. Special attention should be paid to the respective control panels with the manufacturer-specific pictograms.
MTS TeachWare • CNC-Grundlagen • Student’s Book
155
4.3
Introduction to manual NC programming
4.3
Introduction to manual NC programming
Procedure for manual NC programming The procedure for manual programming can be divided into four steps: 1. 1. 1. 1.
analysis of workshop drawings definition of work plans choice of clamping devices and necessary tools (set-up sheet) generating the NC program (program sheet)
Various documents must be analyzed and plans for production execution must be created. (see fig. 168). study
study
work order
workshop drawing
tools
programmer
work plan
clamping devices
set-up form
program sheet
figure 168 Procedure for manual programming Analysis of workshop drawings
The workshop drawing (see fig. 169) contains the geometric and technical information for the finished part. The dimensions, the surface specifications as well as information on the machining procedure to be used (e.g. cutting, threading, hardening) are taken from the drawing. Information on the work to be executed as well as on the number of work parts and the deadlines is specified in the work order.
figure 169 Workshop drawing turning
156
figure 170 Workshop drawing milling
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming Definition of work plans
The workshop drawing and the work order determine the machining operation sequence. Basic type No..: 4711
Standard work plan No.: 007
Sketch for basic type: Gear wheel
Maximum ratings:
Work piece material:
90 <= Da < 150 35 <= Di < 80 10 <= NB < 20 2 <= Z < 20
Round bar Dr = 1.05 x Da Lr = L + 5 Material: C45
Da: = External diameter Di: = Internal diameter
N.
Machining description
01
saw LR mm long and deburr
02
turning and main drilling
Production aids
sketch
Date 13.03.91
Machining alternatives Decision criteria
120 <= Da < 240 and 30 <= L < 80
Z: = Counter value NB: = Slot width
Machine group
Cost center
Dr: = Work piece diameter Lr: = Work piece length
tr [min]
Calculation formula for time per piece te [min/piece]
55/1
1101
3
te = 0,5 x Dr
66/1
1212
12
te = 1,5 x (Dr - Da) + 0,1 x Lr
1300
0
te = 0,5 x number of drillings
03
sketching
axial drillings available
04
auxiliary drillings
axial drillings available and drilling-Ø <= 10 mm
71/1
1217
2
te = 0,5 x number of drillings
axial drillings available and drilling-Ø > 10 mm
72/2
1217
2
te = 0,05 x number of drillings x drilling depth
figure 171 Work order This sequence is then registered in a work plan. The clamping situation must already be considered at this time. Clamping must be sketched for complicated situations or reclamping.
figure 172 Work plan
MTS TeachWare • CNC-Grundlagen • Student’s Book
157
4.3
Introduction to manual NC programming
Choice of clamping devices and necessary tools
In this phase, all data needed for executing the individual machining operations, i.e. for high-quality production, is entered into the work plan (see fig. 14). After selecting the required clamping elements, the necessary tools are chosen and the pertinent cutting data for each operation is calculated.
figure 173 Set-up form All data that is needed for setting up the CNC-machine tool is listed in the set-up form (see fig. 15). Especially the information on the program number and drawing number as well as the work part name identifies all documents required for the order. For repeated orders, information on the position of the work part enables an easier set-up of the clamping situation. Generating the NC program
The programmer creates the NC-program based on the workshop drawing and work plan, and enters the individual program blocks into a program sheet (see fig. 16). This program sheet supplements the documents at hand. For a repeated order, the machine can then immediately be set-up. Program Sheet
Programming
N G
XZI
K F MT
figure 174 Program Sheet
158
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Manual NC programming Turning CNC exercise
Instructed generation of NC-programs for CNC-turning operations Task: An NC-program is to be generated for manufacturing the following part.
figure 175
Follow the subsequent steps for generating the NC-program: 1. 1. 1. 1.
definition of the work plan choice of clamping devices and necessary tools generating the NC program simulating the NC program
MTS TeachWare • CNC-Grundlagen • Student’s Book
159
4.3
Introduction to manual NC programming
Definition of the work plan
Work plan for machining the first side: Machining Sequence
Tool
Turret Position
Cutting Values
Outline
1 check blank
1
dimensions 2 clamp work part 1.side 3 define work part zero point
3 2
4 Face Turning
Left Corner Tool
T04
CL-SCLCL-2020/R/1208
G96 F0.15
4
S140
5 Centering
Center Drill
T09
CD-03.15/050/R/HSS
G97 F0.16 S1800
6 Drilling
Twist Drill Ø 14mm
T07
DR-18.00/130/R/HSS
G97 F0.22 S1000
7 Outside contour roughing
Left Corner Tool
5
T04
CL-SCLCL-2020/R/1208
G96 F0.1
6
7
S140
8 Outside contour finish- Left Corner Tool ing
CL-SVJCL-2020/R/1604
T02
G96 F0.1 S280
160
MTS TeachWare • CNC-Grundlagen • Student’s Book
8
Introduction into NC programming Work plan for machining the second side:
Machining Sequence
Tool
Turret Position
Cutting Values
Outline
1 check work part
2
2 clamp work part 2.side
1 3
3 define work part zero point
4 Face Turning with offset 0.2mm
Left Corner Tool
T04
CL-SCLCL-2020/R/1208
G96 F0.28
4
S140
5 Outside contour roughing
Left Corner Tool
T04
CL-SCLCL-2020/R/1208
G96 F0.28
5
S140
6 Predrilling
Reversible Tip Drill Ø 22mm DI-22.00/051/R/HMT
T12
G97 F0.2 S850
MTS TeachWare • CNC-Grundlagen • Student’s Book
6
161
4.3
Introduction to manual NC programming
Machining Sequence 7 Inside contour roughing with offset
Tool Inside Turning Tool Post
Turret Position T05
Inside Turning Tool Post
S120
T10
9 Outside contour finish- Left Corner Tool ing
CL-SVJCL-2020/R/1604
T02
G96 F0.1 S280
162
7
G96 F0.1 S220
BI-SVQJCL-2020/R/1604
Outline
G96 F0.2
BI-SDQCL-1616/R1104
8 Inside contour finishing
Cutting Values
MTS TeachWare • CNC-Grundlagen • Student’s Book
8
9
Introduction into NC programming Setting-up the CNC machine (set-up sheet)
After start, the MTS-simulator is automatically set-up with blank, clamping and turret allocation. If the following set-up data does not conform with the current set-up data, then it must be changed in the set-up operation.
figure 176 Setup Dialog
figure 177 Interactivmod
Set-up sheet for machining the first side:
CONFIGURATION MACHINE MTS01 TM-016_-R1_-060x0646x0920 CONTROL MTS TM01 PART CYLINDER D075.000 L100.000 MATERIAL AlMg 1::Aluminium DENSITY 002.70 MAIN SPINDLE WITH WORKPART CHUCK "Chuck Turning\Jaw chuck\KFD-HS 160" STEP JAW "Jaw\Step jaw\HM-160_200-02.001" TYPE OF CHUCK EXTERNAL CHUCK OUTSIDE STEP JAW CHUCKING DEPTH E18.000 TAILSTOCK TAILSTOCK POSITION Z+1095.000 CURRENT TOOL T01 TOOLS T02 "DIN69880 V 30\ T04 "DIN69880 V 30\ T05 "DIN69880 V 30\ T07 "DIN69880 V 30\
Left corner tool\CL-SVACL-2020 L 1604 ISO30" Left corner tool\CL-SCLCL-2020 L 1208 ISO30" Inside turning tool postaxial\BI-SDQCL-1212 L 0704 ISO30" Twist drill\DR-14.00 108 R HSS ISO30"
T09 "DIN69880 V 30\ T12 "DIN69880 V 30\ T14 "DIN69880 V 30\
Center drill\CD-04.00 056 R HSS ISO30" Reversible tip drill\DI-22.00 051 R HMT ISO30" Inside turning tool postaxial\BI-SDQCL-1212 L 0704 ISO30"
TOOL COMPENSATION D02 T02 Q3 D04 T04 Q3 D05 T05 Q2 D07 T07 Q7 D09 T09 Q7 D12 T12 Q7 D14 T14 Q2
R0.4 X+70.0 Z+45.0 R0.8 X+70.0 Z+45.0 R0.4 X-8.364 Z+160.0 R0.0 X+0.0 Z+180.0 R0. 0 X+0. 0 Z+70.0 R0.0 X+0.0 Z+180.0 R0.4 X-8.364 Z+160.0
G0.0 E52.393 I-0.4 K-0.4 A+2.372 L16.178 N01 G0.0 E05.005 I-0.8 K-0.8 A+4.375 L11.855 N01 G0.0 E18.027 I+0.4 K-0.4 A+16.744 L7.029 N01 G14.0 E59.0 I+0.0 K+0.0 A+0.0 L0.0 N01 G04.0 E0.0 I+0.0 K+0.0 A+0.0 L0.0 N01 G22.0 E0.0 I+0.0 K+0.0 A+0.0 L0.0 N01 G0.0 E18.027 I+0.4 K-0.4 A+16.744 L7.029 N01
MTS TeachWare • CNC-Grundlagen • Student’s Book
163
4.3
Introduction to manual NC programming
Set-up sheet for machining the second side:
For machining the second side, the work part is reclamped, i.e. no blank is clamped! The work part is clamped after the first side is machined. The current form is defined in part GEOMETRY.
File Selection Window
figure 178 Diagram of the menu sequence for the Work part Manager.
figure 179 File information for loading a preproduced work part.
CONFIGURATION MACHINE MTS01 TM-016_-R1_-060x0646x0920 CONTROL MTS TM01 PART GEOMETRY X+071.331 Z+0165.500 G01 X+075.000 Z+0165.500 G01 X+075.000 Z+0191.000 G01 X+014.000 Z+0191.000 G01 X+014.000 Z+0093.000 G01 X+020.000 Z+0093.000 G02 X+028.000 Z+0097.000 G01 X+028.000 Z+0121.000 G03 X+034.000 Z+0124.000 G01 X+034.000 Z+0145.600 G03 X+034.800 Z+0146.000 G01 X+044.000 Z+0146.000 G02 X+050.000 Z+0149.000 G01 X+050.000 Z+0157.000 G03 X+062.000 Z+0163.000 G01 X+066.000 Z+0163.000 G01 X+070.766 Z+0165.383 G03 X+071.331 Z+0165.500 M30
I+000.000 K+004.000 I+003.000 K+000.000 I+000.400 K+000.000 I+000.000 K+003.000 I+006.000 K+000.000
I+000.283 K-000.283
MAIN SPINDLE WITH CHUCK "Chuck Turning\Jaw chuck\KFD-HS 160" WORKPART STEP JAW "Jaw\Step jaw\HM-160_200-02.001" CHUCKING DEPTH E53.000 Right side of the part: Z+0191.000 CHUCK "Chuck Turning\Jaw chuck\KFD-HS 160"
164
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming NC programming NC program for the first side
Block Commands No.
Description
%200
Program name
4) Plandrehen N010 G54 Z+226.000
G54 set absolute zero Z+226.000 Z- coodinate of the current workpart zero
N015 G96 S0140 T0404 M03
G96 Constant speed cutting ON S140 Spindle speed T0404 Selection of the tool from turret position 4 M3 activate the spindle in clockwise rotation
N020 G92 S3000
G92 Speed limit S3000 Spindle speed
N025 G00 X+078.000 Z+000.200
G00 Rapid traverse X+078.000 X- Coordinate of the target point Z+000.200 Z- Coordinate of the target point
N030 G01 X-001.000 F000.150 M08
G01 Linear interpolation in slow speed motion X-001.000 X- Coordinate of the target point F000.150 feedrate in mm per revolution M8 activate coolant
N035 G00 Z+002.000
G00 Rapid traverse Z+002.000Z- Coordinate of the target point
N040 X+200.000 Y+200.000 M5 M9
X200.000 X- Coordinate of the target point Z200.000 Z- Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
MTS TeachWare • CNC-Grundlagen • Student’s Book
165
4.3
Introduction to manual NC programming
Block Commands No.
Description
5) Centering
5) Zentrieren N045 G97 S1800 T0909 M03
G97 Constant Speed Cutting OFF S1800 Spindle speed T0909 Selection of the tool from turret position 9 M3 activate the spindle in clockwise rotation
N050 G00 Z+002.000
G00 Rapid traverse Z2 Z- Coordinate of the target point
N055 X+000.000
X+000.000 X- Coordinate of the target point
N060 G01 Z-005.800 F000.160 M08
G01 Linear interpolation of slow feed motion Z-005.800 Z- Coordinate of the target point F000.160 feedrate in mm per revolution M08 activate coolant
N065 G00 Z+002.000
G00 Rapid traverse Z002.000 Z- Coordinate of the target point
N070 X+200.000 Z+200.000 M5 M9
X200.000 X- Coordinate of the target point Z200.000 Z- Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
166
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
N075 F000.220 T0707 M03
F000.220 feedrate in mm per revolution
6) Drilling T0707 Selection of the tool from turret position 7 M3 activate the spindle in clockwise rotation N080 G97 S1000
G97 Constant Speed Cutting OFF S1000 Spindle speed
N085 G00 Z+002.000
G00 Rapid traverse Z+002.000Z-Coordinate of the targer point
N090 X+000.000 M08
X000.000 X- Coordinate of the target point M08 activate coolant
N095 G84 Z-105.000 A+001.000 B+001.000 D+005.000 K+025.000
G84 Drilling cycle Z-105.000 Z-coordinae of the target point A+001.000 Dwell time after retraction B+001.000 Dwell time when target point is reached for chip breaking D+005.000 Digression (reduction of drilling depth) K+025.000 first depth of cut
N100 G00 X+200.000
G00 Rapid traverse
N105 Z+070.000 M5 M9
X200.000 X- Coordinate of the target point Z070 Z- Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
MTS TeachWare • CNC-Grundlagen • Student’s Book
167
4.3
Introduction to manual NC programming
Block Commands No.
Description
7) Outside contour roughing N110 G96 S0140 T0404 M03
G96 Constant speed cutting ON S0140 Spindle speed T0404 Selection of the tool from turret position 4 M3 activate the spindle in clockwise rotation
N115 G92 S3000
G92 Maximum spindle speed
N120 G00 X+075.000 Z+002.000
S3000 Spindle speed G00 Rapid traverse X+075.000 X- Coordinate of the target point Z+002.000 Z- Coordinate of the target point
N125 G57 X+000.600 Z+000.200
G57 finishing allowance activation X+000.600 finishing allowance activation in X-Richtung (durchmesserbezogen) Z+000.200 finishing allowance activation in Z-Richtung
N130 G81 X+018.000 Z+002.000 I+004.000
G81 straight roughing cycle X+018.000 X- Coordinate of contour start point Z+002.000 Z- Coordinate of contour start point I+004.000 Infeed
N135 G42
G42 tool nose compensation: right of the contour
N140 G01 X+018.000 Z+000.000
G01 Linear interpolation of slow feed motion X+018.000 X- Coordinate of the target point Z+000.000 Z- Coordinate of the target point
N145 X+020.000
X+018.000 X- Coordinate of the target point
N150 G03 X+028.000 Z-004.000 I+000.000 K-004.000
G03 circular interpolation counter-clockwise X+028.000 X- Coordinate of the target point Z-004.000 Z- Coordinate of the target point I+000.000 Distance between starting position and circle center in X K-004.000 Distance between starting position and circle center in Z
N155 G01 Z-028.000
G01 Linear interpolation of slow feed motion Z-028.000 Z- Coordinate of the target point
N160 G01 X+018.000 Z+000.000
G01 Linear interpolation of slow feed motion X+018.000 X- Coordinate of the target point Z+000.000 Z- Coordinate of the target point
168
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
N165 G02 X+034.000 Z-031.000 I+003.000 K+000.000
G02 Circular interpolation counter-clockwise X+034.000 X- Coordinate of the target point Z-031.000 Z- Coordinate of the target point I+003.000 Distance between starting position and circle center in X K-000.000 Distance between starting position and circle center in Z
Block Commands No.
Description
N170 G01 Z-053.000
G01 Linear interpolation of slow feed motion Z-053.000 Z- Coordinate of the target point
N175 G01 X+044.000
G01 Linear interpolation of slow feed motion X+044.000 X- Coordinate of the target point
N180 G03 X+050.000 Z-056.000 I+000.000 K-003.000
G03 Circular interpolation counter-clockwise X+050.000 X- Coordinate of the target point Z-056.000 Z- Coordinate of the target point I+000.000 Distance between starting position and circle center in X K-003.000 Distance between starting position and circle center in Z
N185 G01 Z-064.000
G01 Linear interpolation of slow feed motion Z-064.000 Z-Coordinate of the target point
N190 G02 X+062.000 Z-070.000 I+006.000 K+000.000
G02 Circular interpolation counter-clockwise X+062.000 X-Coordinate of the target point Z-070.000 Z-Coordinate of the target point I+006.000 Distance between starting position and circle center in X K-000.000 Distance between starting position and circle center in Z
N195 G01 X+066.000
G01 Linear interpolation of slow feed motion X+066.000 X- Coordinate of the target point
N200 G01 X+071.000 Z-072.500
G01 Linear interpolation of slow feed motion X+071.000 X- Coordinate of the target point Z-072.500 Z- Coordinate of the target point
N205 G01 X+076.000
G01 Linear interpolation of slow feed motion X+076.000 X-Coordinate of the target point
N210 G40
G40 cancel tool nose compensation
N215 G80
G80 End of contour definition for straight roughing cycle
MTS TeachWare • CNC-Grundlagen • Student’s Book
169
4.3
Introduction to manual NC programming
N220 G00 X+200.000 Z+200.000 M5 G0 Rapid traverse M9 X200.000 X-Coordinate of the target point Z200.000 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
8) Outside contour finishing N225 G96 F000.100 S0280 T0202 M03
G96 Constant speed cutting ON F000.100 feedrate in mm per revolution S0280 Spindle speed T0202 Selection of the tool from turret position 2 M03 activate the spindle in clockwise rotation
N230 G92 S4000
G92 Speed limit S4000 Spindle speed
N235 G00 X+010.000 Z+002.000
G00 Rapid traverse X+010.000 X- Coordinate of the target point Z+002.000 Z- Coordinate of the target point
N240 G42
G42 tool nose compensation: right of the contour
N245 G01 X+013.000 Z+000.000
G01 Linear interpolation of slow feed motion X+013.000 X- Coordinate of the target point Z+000.000 Z- Coordinate of the target point
N250 G23 O135 Q210
G23 Programmteilwiderholung O135 Start block number Q210 End block number
170
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
N255 G00 X+200.000 Z+200.000 M5 G00 Rapid traverse M0 X200.000 X-Coordinate of the target point Z200.000 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant N260 M30
M30 End of program
MTS TeachWare • CNC-Grundlagen • Student’s Book
171
4.3
Introduction to manual NC programming
NC program for the second side
Block Commands No.
Description
%201
Program name
4) Face Turning N005 G54 Z+188.000
G54 set absolute zero Z+188.000 Z-Coordinate of the current workpart zero
N010 G96 S0140 T0404 M03
G96 Constant Speed Cutting ON S140 Cutting Speed T0404 Selection of the tool from turret position 4 M3 activate the spindle in clockwise rotation M42 Select the higher spindle speed range
N015 G92 S3000
G92 Spindle speed limitation S3000 Maximum spindle speed
N020 G00 X+078.000 Z+001.5 0
G00 Rapid traverse X+078.000 X-Coordinate of the target point Z+001.500 Z-Coordinae of the target point
N025 G01 X-001.000 F000.280 M08
G01 linear interpolation in slow feed motion X-001.000 X-Coordinate of the target point F000.280 feedrate in mm per revolution M8 activate coolant
N030 G00 Z+002.000
172
G00 Rapid traverse Z+002.000 Z-Coordinate of the target point
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
5) Outside contour roughing N035 G00 X+078.000
G00 Rapid traverse X+078.000 X-Coordinate of the target point
N040 G00 Z+000.200
G00 Rapid traverse Z+000.2000 Z-Coordinate of the target point
N045 G01 X+012.000
G01 Linear interpolation of slow feed motion
N050 G88 X+070.400 Z+000.200 R+004.000
X+012.000 X-Coordinate of the target point G88 Cycle radius X+070.400 X-Coordinate of the target point Z+000.200 Z-Coordinate of the target point R+004.000 Rounding radius
N055 G01 Z-025.000
G01 Linear interpolation of slow feed motion Z-025.000 Z-Coordinate of the target point
N060 G00 X+200.000 Z+200.000 M5 G00 Rapid traverse M9 X200.000 X-Coordinate of the target point Z200.000 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
MTS TeachWare • CNC-Grundlagen • Student’s Book
173
4.3
Introduction to manual NC programming
Block Commands No.
Description
N065 G97 S0850 T1212 M03
G97 Constant Speed Cutting OFF
6) Predrilling S0850 Spindle speed T1212 Selection of the tool from turret positiion 12 M3 activate the spindle in clockwise rotation N070 G92 S1500
G92 Speed limit
N075 G00 Z+002.000
S1500 Spindle speed G00 Rapid traverse Z+002.000 Z-Coordinate of the target point M8 activate coolant
N080 X+000.000 F000.200 M08
X+000.000 X-Coordinate of the target point F000.200 feedrate in mm per revolution M08 activate coolant
N085 G84 Z-034.800 A+001.000 B+001.000 D+004.000 K+020.000
G84 Drilling cycle Z-034.800 Z Coordinate of the target point A+001.000 Dwell time after retraction B+001.000 Dwell time when target point is reached for chip breaking D+004.000 Digression (reduction of drilling depth) K+020.000 first depth of cut
N090 G00 X+200.000
G00 Rapid traverse X200.000 X-Coordinate of the target point
N095 Z+070.000 M5 M9
Z70 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
174
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
7) Inside contour roughing N100 G96 F000.200 S0120 T0505 M04
G96 Constant speed cutting ON F000.200 feedrate in mm per revolution S0120 Spindle speed T0505 Selection of the tool form turret positin 5 M4 activate the spindle counter clockwise
N105 G92 S3000
G92 Speed limit S3000 Spindle speed
N110 G00 X+021.000 Z+002.000
G00 Rapid traverse X+021.000 X-Coordinate of the target point Z+002.000 Z-Coordinate of the target point
N115 G57 X-000.600 Z+000.200
G57 finishing allowance activation X+000.600 Finshingin X allowance Z+000.200 Finishing in Z allowance
N120 G81 X+040.000 Z+002.000 I+002.500
G81 straight roughing cycle X+040.000 X-Coordinate of contour start point Z+002.000 Z-Coordinate of contour start point I+002.500 Infeed
N125 G41
G41 Tool nose compensation: left of the contour
N130 M08 G01 X+038.000 Z+000.000
G01 Linear interpolation of slow feed motion X+038.000 X-Coordinate of the target point Z+000.000 Z-Coordinate of the target point M8 activate coolant
N135 X+034.000 Z-002.000
X+034.000 X-Coordinate of the target point Z-002.000 Z-Coordinate of the target point
N140 G88 X+034.000 Z-015.000 R+002.000
G88 Cycle radius X+034.000 X-Coordinate of the target point Z-015.000 Z-Coordinate of the target point R+002.000 Rounding radius
N145 G01 X+026.000
G1 Linear interpolation of slow feed motion X+026.000 X-Coordinate of the target point
N150 Z-035.000
Z-035.000 Z-Coordinate of the target point
N155 X+013.000 N160 G40
X+013.000 X-Coordinate of the target point G40 cancel tool nose compensation
N165 G80
G80 End of contour definition
N170 G00 X+200.000
G00 Rapid traverse X200.000 X-Coordinate of the target point
N175 Z+070.000 M5 M9
Z+070.000 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
MTS TeachWare • CNC-Grundlagen • Student’s Book
175
4.3
Introduction to manual NC programming
Block Commands No.
Description
8) Inside contour finishing N180 G96 F000.100 S0220 T1010 M04
G96 Constant speed cutting ON F000.1000 feedrate in mm per revolution S0220 Spindle speed T1010 Selection of the tool from turret position 10 M4 activate the spindle counter-clockwise
N185 G92 S4000
G92 Speed limit S4000 Spindle speed
N190 G00 X+040.000 Z+002.000
G00 Rapid traverse X+040.000 X-Coordinate of the target point Z+002.000 Z-Coordinate of the target point
N195 G23 O125 Q160
G23 program part repetition O125 Start block number Q160 End block number
N200 G00 Z+002.000
G00 Rapid traverse X+002.000 Z-Coordinate of the target point
N205 X+200.000
X+200.000 X-Coordinate of the target point
N210 Z+070.000 M5 M9
Z+070.000 Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
176
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
9) Outside contour finishing N215 G96 F000.100 S0280 T0202 M03
G96 Constant speed cutting ON F000.100 feedrate in mm per revolution S0280 Spindle speed T0202 Selection of the tool from turret position 2 M3 activate the spindle in clockwise rotation
N220 G92 S4000
G92 Speed limit S4000 Spindle speed
N225 G00 X+034.000 Z+001.000
G00 Rapid traverse X+034.000 X-Coordinate of the target point Z+001.000 Z-Coordinate of the target point
N230 G42
G42 tool nose compensation: right of the contour
N235 G01 Z+000.000 M8
G01 Linear interpolation of slow feed motion Z+000.000 Z-Coordinate of the target point M8 activate coolant
N240 G88 X+070.000 Z+000.000 R+004.000
G88 Cycle radius X+070.000 X-Coordinate of the target point Z+000.000 Z-Coordinate of the target point R+004.000 Rounding radius G01 Linear interpolation of slow feed motion
N245 G01 Z-026.000
Z-026.000 Z-Coordinate of the target point N250 X+072.000
X+072.000 X-Coordinate of the target point
N255 G40
G40 cancel tool nose compensation
N260 X+200.000 Z+200.000 M5 M9
X+200.000 X-Coordinate of the target point Z+200.000Z-Coordinate of the target point M5 deactivate spindle M9 deactivate coolant
N240 M30
M30 End of program
MTS TeachWare • CNC-Grundlagen • Student’s Book
177
4.3
Introduction to manual NC programming
Simulation of the NC program and Quality control by measuring work results
In automatic mode, the generated NC-programs are simulated in real-time and with respect to possible collisions.
figure 180 Automatic Mode menu diagram.
figure 181 Automatic Mode menu.
To start an NC program in Automatic Mode, two procedural steps are required: 1. As a first step after starting Automatic Mode, the main menu is loaded, allowing you to enter the name of the NC program (par example: %200) to be simulated. Accept program: Use F1 or to confirm the program name appearing in the information line. If the program is available, it is subsequently loaded into program memory; if not, an appropriate error message is displayed.
1. Continue by selecting the desired simulation mode for program execution Automatic: Select F1 to execute the program specified in the dialogue line under continuous automatic control. Single NC block: Use F2 to activate single block operation.
figure 182 Menu during continuous automatic run.
178
figure 183 CNC Turning, 3D Display, Optional section.
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming Quality control by measuring work results
A work part can be measured after machining (automatic mode) or during machining after every operation (single block) and can be compared with the values in the drawing. Procedure: Description
Entry
1. Call CNC turning in the main menu.
F1 (turning)
2. Select menu automatic mode.
F2
3. Call a present NC program, par example %200. 4. Select the simulation type „automatic mode“.
(automatic mode) Using the keyboard type in„%200“ and confirm.
F1 (Automatic mode) On the screen the simulation of the machining starts.
5. Select menu measurement.
F6
(Dimension 3D)
6. Select menu point dimension.
F6
(Point dimension)
7. Select the point for measurement.
F1 (next point) or F2
(previous point) For the selected point the data are shown on the screen
8. Quit the menu measurement.
F8
(Abort)
F8
(Quit)
MTS TeachWare • CNC-Grundlagen • Student’s Book
179
4.3
Introduction to manual NC programming
Manual NC programming Milling CNC Exercise
Instructed generation of NC-programs for CNC-milling Task: An NC-program is to be generated for manufacturing the following part:
figure 184
Follow the subsequent steps for generating the NC-program: 1. 1. 1. 1.
180
definition of the work plan choice of clamping devices and necessary tools generating the NC program simulating the NC program
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming Work plan
Machining Sequence
Tool
Magazine Position
Cutting Values
1 check blank
Outline Y
dimensions 2 clamp work part 3 define work part zero point
1
2
3
X
4 Contour left side
SLOT MILLING TOOL
T01
mill 8mm deep
5 Contour right side
SLOT MILLING TOOL
T01
mill 8mm deep
6 Contour octagon
F250 S1600
4
F250 S1600
SLOT MILLING TOOL
T01
mill 4mm deep
5
F250 S1600
6 7 Contour with arcs mill 6mm deep
SLOT MILLING TOOL
T01
F250 S1600
7
MTS TeachWare • CNC-Grundlagen • Student’s Book
181
4.3
Introduction to manual NC programming
8 Contour Circle r=25mm
SLOT MILLING TOOL
T01
F250 S1600
mill 2mm deep
8
9 Circular Pocket r=15mm
SLOT MILLING TOOL
T02
F50 S1800
mill 4mm deep
9
10 4 x Centering
CORE DRILL
T03
F80 S2000
11 Drill 4 x core hole
DRILL
T04
M6
12 4 x tapping M6
182
F50 S1500
TAP
T05
10
F150 S150
MTS TeachWare • CNC-Grundlagen • Student’s Book
11
12
Introduction into NC programming Setting-up the CNC machine (set-up sheet)
After start, the MTS-simulator is automatically set-up with blank, clamping and turret allocation. If the following set-up data does not conform with the current set-up data, then it must be changed in the set-up operation
figure 185 SetupDialog
figure 186 Set-up Mode; „Work part and clamping fixture definition" menu.
CONFIGURATION MACHINE MTS VMC-024_ISO30_-0500-0400x0450 CONTROL FANUC SERIE 16M BLANK DIMENSIONS X+100.000 Y+100.000 Z+025.000 VISE "Chuck Milling\Vise\RS 110" CHUCKING DEPTH E+010.000 SHIFT V+000.000 ORIENTATION A0° PART POSITION X+150.000 Y+150.000 left corner of the part: X+150.000 Y+150.000 Z+105.000 CURRENT TOOL T01 TOOLS T01 T02 T03 T04 T05
"ISO SK 30\ "ISO SK 30\ "ISO SK 30\ "ISO SK 30\ "ISO SK 30\
Slot Milling tool\MS-20.0 038K HSS ISO 1641" Slot Milling tool\MS-20.0 038K HSS ISO 1641" Core drill\DC-08.0 090 HSS ISO 3294" Drill\DR-05.00 052 HSS ISO 235 Tap\TA-M06.0 1.00 HSS ISO 2857"
TOOL COMPENSATION D01 D02 D03 D04 D05
T01 R010.000 Z+119.000 N01 T02 R010.000 Z+119.000 N01 T03 R000.000 Z+065.000 N01 T04 R002.500 Z+097.900 N01 T01 R010.000 Z+119.000 N01
WORKPART ZEROPOINTS G54 X150.000 Y+150.000 Z+105.000
MTS TeachWare • CNC-Grundlagen • Student’s Book
183
4.3
Introduction to manual NC programming
NC programming
Block Commands No.
Description
O 200
O Program number O and program name
N005 G90 G80 G40 G49 G17 G21
G90 Absolute Dimensioning G80 Canned cycle cancel G40 Tool radius compensation cancel G49 Tool length compensation cancel G17 XY plane G21 Metric input
N010 G91 G28 Z0
G91 Incremental dimensioning G28 Reference point return Z0 Z-Coordinate of the Intermediate Point
N015 G91 G28 X0 Y0
G91 Incremental dimensioning G28 Reference point return X0 X-Coordinate of the Intermediate Point Y0 Y-Coordinate of the Intermediate Point
N020 G54
G54 Work coordinate system 1 selection
4) Contour left side mill 8mm deep N025 T01 M06
T01 Select the tool 1 M06 Mounting the tool 1
N030 G90 G00 X-20 Y-20
G90 Absolute dimensioning G00 rapid traverse X-20 X-Coordinate of the target point Y-20 Y-Coordinate of the target point
N035 G43 Z20 H17
G43 Tool length compensation + Z20 Z-Coordinate of the target point H17 Select the compensation offset 1
N040 S1600 M03
S1600 spindle speed M03 activate the spindle in clockwise rotation
N045 Z-8 M08
Z-8 Z-Coordinate of the target point M08 activate coolant
N050 G41 G1 X5 D1 F250
G41 Tool radius compensation left G1 linear interpolation in slow feed motion X5 X-Coordinate of the target point D1 Select the compensation offset 1 F250 feedrate in mm/min
N055 Y110
184
Y110 Y-Coordinate of the target point
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
5) Contour right side mill 8mm deep N060 G0 X95
G0 rapid traverse X95 X-Coordinate of the target point
N065 G1 Y-10
G1 linear interpolation in slow feed motion Y-10 Y-Coordinate of the target point
N070 G40 G0 X-20 Y-20
G40 Tool radius compensation cancel G0 rapid traverse X-20 X-Coordinate of the target point Y-20 Y-Coordinate of the target point
6) Octagon mill 4mm deep N075 Z-4
Z-4 Z-Coordinate of the target point
N080 G41 G0 X15 D1
G41 Tool radius compensation left G0 rapid traverse X15 X-Coordinate of the target point D1 Select the compensation offset 1
N085 G1 Y65
G1 linear interpolation in slow feed motion Y65 Y-Coordinate of the target point
N090 X35 Y85
X35 X-Coordinate of the target point Y85 Y-Coordinate of the target point
N095 X65 N100 X85 Y65
X65 X-Coordinate of the target point X85 X-Coordinate of the target point Y65 Y-Coordinate of the target point
N105 Y35
Y35 Y-Coordinate of the target point
MTS TeachWare • CNC-Grundlagen • Student’s Book
185
4.3
Introduction to manual NC programming
Block Commands No.
Description
N110 X65 Y15
X65 X-Coordinate of the target point Y15 Y-Coordinate of the target point
N115 X35
X35 X-Coordinate of the target point
N120 X5 Y45
X5 X-Coordinate of the target point Y45 Y-Coordinate of the target point
N125 G40 G0 X-20 Y-20
G40 Tool radius compensation cancel G0 rapid traverse X-20 X-Coordinate of the target point Y-20 Y-Coordinate of the target point
7) Contour with arcs mill 6mm deep N130 Z-6 N135 G41 G1 X10 D1
Z-6 Z-Coordinate of the target point G41 Tool radius compensation left G1 linear interpolation in slow feed motion X10 X-Coordinate of the target point D1 Select the compensation offset 1
N140 G1 Y82
G1 linear interpolation in slow feed motion Y82 Y-Coordinate of the target point
N145 G2 X18 Y90 R8
G2 circular interpolation clockwise X18 X-Coordinate of the target point Y90 Y-Coordinate of the target point R8 radius r=8 of the circular arc
N150 G1 X82
G1 linear interpolation in slow feed motion X82 X-Coordinate of the target point
N155 G2 X90 Y82 R8
G2 circular interpolation clockwise X90 X-Coordinate of the target point Y82 Y-Coordinate of the target point R8 radius r=8 of the circular arc
N160 G1 Y18
G1 linear interpolation in slow feed motion Y18 Y-Coordinate of the target point
N165 G2 X82 Y10 R8
G2 circular interpolation clockwise X82 X-Coordinate of the target point Y10 Y-Coordinate of the target point R8 radius r=8 of the circular arc
N170 G1 X18
G1 linear interpolation in slow feed motion X18 X-Coordinate of the target point
186
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
N175 G2 X10 Y18 R8
G2 circular interpolation clockwise X10 X-Coordinate of the target point Y18 Y-Coordinate of the target point R8 radius r=8 of the circular arc
N180 G3 X-10 Y38 R20
G2 circular interpolation counter-clockwise X-10 X-Coordinate of the target point Y38 Y-Coordinate of the target point R8 radius r=8 of the circular arc
N185 G40 G0 X-20 Y-20
G40 Tool radius compensation cancel G0 rapid traverse X-20 X-Coordinate of the target point Y-20 Y-Coordinate of the target point
8) Contour circle r=25mm mill 2mm deep N190 Z-2
Z-2 Z-Coordinate of the target point
N195 G41 X25 D1
G41 Tool radius compensation left X25 X-Coordinate of the target point D1 Select the compensation offset 1
N200 G1 Y50
G1 linear interpolation in slow feed motion
N205 G2 X25 Y50 I25
Y50 Y-Coordinate of the target point G2 circular interpolation clockwise X25 X-Coordinate of the target point Y50 Y-Coordinate of the target point I25 X-Coordinate of the center of circular arc
N210 G40 G1 Y65
G40 Tool radius compensation cancel G1 linear interpolation in slow feed motion Y65 Y-Coordinate of the target point
N215 Z5
Z5 Z-Coordinate of the target point
N220 G91 G28 Z0 M5
G91 Incremental dimensioning G28 Reference point return Z0 Z-Coordinate of the Intermediate Point M5 deactivate spindle
N225 G91 G28 X0 Y0 M9
G91 Incremental dimensioning G28 Reference point return X0 X-Coordinate of the Intermediate Point Y0 Y-Coordinate of the Intermediate Point M9 deactivate coolant
MTS TeachWare • CNC-Grundlagen • Student’s Book
187
4.3
Introduction to manual NC programming
Block Commands No.
Description
9) Circular pocket r=15mm mill 4mm deep N230 T02 M06
T02 Select the tool 2 M06 Mounting the tool 2
N235 G90 G0 X50 Y50
G90 Absolute dimensioning G00 rapid traverse X50 X-Cordinate of the target point Y50 Y-Coordinate of the target point G43 Tool length compensation +
N240 G43 Z20 H18
Z20 Z-Coordinate of the target point H18 Select the compensation offset 2 N245 S1800 M3
S1800 spindle speed M03 activate the spindle in clockwise rotation
N250 Z2 M8
Z2 Z-Coordinate of the target point M8 activate coolant
N255 G1 Z-4 F50
G1 linear interpolation in slow feed motion Z-4 Z-Coordinate of the target point F50 feedrate in mm/min
N260 G42 G1 X38 Y53 D2
G42 Tool radius compensation right G1 linear interpolation in slow feed motion X38 X-Coordinate of the target point Y53 Y-Coordinate of the target point (Starting point of the quarter-round starting move r=12) D2 Select the compensation offset 2
188
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
N265 G2 X50 Y65 R12 F200
G2 circular interpolation clockwise X10 X-Coordinate of the target point Y18 Y-Coordinate of the target point (Target point of the quarter-round remove r=12) R12 radius r=12 of the circular arc F200 feedrate in mm/min
N270 G2 J-15
G2 circular interpolation clockwise (full circle milling r=15) J-15 Y-Coordinate of the center of circular arc
N275 G2 X62 Y62 R12
G2 circular interpolation clockwise X62 X-Coordinate of the target point Y62 Y-Coordinate of the target point (Target point of the quarter-round remove r=12) R12 radius r=12 of the circular arc
N280 G40 G1 X50 Y50
G40 Tool compensation cancel G1 linear interpolation in slow feed motion X50 X-Coordinate of the target point Y50 Y-Coordinate of the target point
N285 G0 Z50 M9
G0 rapid traverse Z50 Z-Coordinate of the target point M9 deactivate coolant
N290 G91 G28 Z0 M5
G91 Incremental dimensioning G28 Reference point return Z0 Z-Coordinate of the Intermediate Point M5 deactivate spindle
N295 G91 G28 X0 Y0
G91 Incremental dimensioning G28 Reference point return X0 X-Coordinate of the Intermediate Point Y0 Y-Coordinate of the Intermediate Point
MTS TeachWare • CNC-Grundlagen • Student’s Book
189
4.3
Introduction to manual NC programming
Block Commands No.
Description
N300 T03 M06
T03 Select the tool 3
10) 4x centering M06 Mounting the tool 3 N305 G90
G90 Absolute dimensioning
N310 G43 Z20 H19
G43 Tool length compensation + Z20 Z-Coordinate of the target point H19 Select the compensation offset 3 S2200 spindle speed
N315 S2200 M03
M03 activate the spindle in clockwise rotation N320 G0 Z1
G0 rapid traverse Z1 Z-Coordinate of the target point
N325 G98 G81 Z-5 R-3 F80 L0
G98 Return to the initial point G81 Drilling cycle, spot boring R-3 Z-Coordinate of the safety plane Z-5 Coordinate at the bottom of the hole F80 feedrate in mm/min L0 The Drilling cycle is only stored!
N330 M98 P1910
M98 P Subprogram call 1910 Subprogram number
190
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
Block Commands No.
Description
11) 4x Core hole drilling N335 T04 M06
T04 Select the tool 4 M06 Mounting the tool 4
N340 G90 G0 X0 Y0
G90 Absolute dimensioning G0 rapid traverse X0 X-Coordinate of the target point Y0 Y-Coordinate of the target point G43 Tool length compensation +
N345 G43 Z20 H20
Z20 Z-Coordinate of the target point H20 Select the compensation offset 4 N350 S1500 M03
S1500 spindle speed M03 activate the spindle in clockwise rotation
N355 G0 Z1
G0 rapid traverse
N360 G98 G83 Z-10 Q6 R-3 F50 L0
G98 Return to the initial point
Z1 Z-Coordinate of the target point
G83 Peck drilling cycle Z-10 Coordinate at the bottom of the hole Q6 Digression R-3 Z-Coordinate of the safety plane F50 feedrate in mm/min L0 The Peck drilling cycle is only stored! N365 M98 P1910
M98 P Subprogram call 1910 Subprogram number
MTS TeachWare • CNC-Grundlagen • Student’s Book
191
4.3
Introduction to manual NC programming
Block Commands No.
Description
N370 T05 M06
T05 Select the tool 5
12) 4x Tapping M06 Mounting the tool 5 N375 G90 G0 X0 Y0
G90 Absolute dimensioning G0 rapid traverse X0 X-Coordinate of the target point Y0 Y-Coordinate of the target point G43 Tool length compensation +
N380 G43 Z20 H21
Z20 Z-Coordinate of the target point H21 Select the compensation offset 5 N385 S150 M3
S150 spindle speed M03 activate the spindle in clockwise rotation
N390 G00 Z1
G00 rapid traverse
N395 G98 G84 Z-8 R-3 F150 L0
G98 Return to the initial point
Z1 Z-Coordinate of the target point
G84 Tapping cycle Z-8 Coordinate at the bottom of the hole R-3 Z-Coordinate of the safety plane F150 feedrate in mm/min L0 The Tapping cycle is only stored!! N400 M98 P1910
M98 P Subprogram call 1910 Subprogram number
N405 G90 G49 G80 G40 M30
192
M30 program end and backspacing
MTS TeachWare • CNC-Grundlagen • Student’s Book
Introduction into NC programming
NC subprogram
Block Commands No.
N10
Description
O 1910
O Program name
G90 X18 Y18 M8
First drilling position: G90 Absolute dimensioning X18 X-Coordinate of the drilling position Y18 Y-Coordinate of the drilling position
N15
Y82
N20
X82
N25
G98 Y18
M8 activate coolant Second drilling position: Y82 Y-Coordinate of the drilling position Third drilling position: X82 X-Coordinate of the drilling position Fourth drilling position: G98 Return to the initial point Y18 Y-Coordinate of the drilling position
N30
G00 G90 G80 Z50. M9
G00 Rapid Traverse G90 Absolute dimensioning G80 Canned cycle cancel Z50 Z-Coordinate
N35
G91 G28 Z0 M5
M9 deactivate coolant G91 Incremental dimensioning G28 Reference point return Z0 Z-Coordinate of the Intermediate Point M5 deactivate spindle
N40
G91 G28 X0 Y0
G91 Incremental dimensioning G28 Reference point return X0 X-Coordinate of the Intermediate Point Y0 Y-Coordinate of the Intermediate Point
N45
M99
M99 subprogram end
MTS TeachWare • CNC-Grundlagen • Student’s Book
193
4.3
Introduction to manual NC programming
Simulation of the NC program
In automatic mode, the generated NC-programs are simulated in real-time and with respect to possible collisions.
figure 187 Automatic Mode menu Diagram.
figure 188 Automatic Mode menu.
To start an NC program in Automatic Mode, two procedural steps are required: 1. As a first step after starting Automatic Mode, the main menu is loaded, allowing you to enter the name of the NC program (par example: 1909) to be simulated. Accept program: Use F1 or to confirm the program name appearing in the information Line. If the program is available, it is subsequently loaded into program memory; if not, an appropriate error message is displayed. 1. Continue by selecting the desired simulation mode for program execution Automatic: Select F1 to execute the program specified in the dialogue line under continuous automatic control. Single NC block: Use F2 to activate single block operation.
figure 189 Menu during continuous automatic run.
figure 190 CNC Milling, 3D Display, Optional section.
Workshop
The students are to manufacture the programmed part on the CNC-milling machine.
194
MTS TeachWare • CNC-Grundlagen • Student’s Book
9.
Control test „Introduction into NC programming“
1.
List the steps for manual programming.
2.
What is the difference between a work plan and a programming sheet?
3.
Explain the meaning of "switching information".
4.
Name and explain five commands for a CNC-machine.
5.
Explain the structure of an NC-program.
6.
Explain the structure of a program block.
7.
Explain the structure of a program word.
8.
Explain the address letters F, S, T, M, X, Y, Z.
9.
Explain the following program words for a) absolute programming (G90) b) incremental programming (G91)! X 53, Z 184.005
10.
What do the address letters I, J, K express?
11.
Define the following functions with the corresponding program words (G-command or M-command) clockwise circular interpolation activate activate coolant spindle in clockwise rotation
12.
For which cases are constant cutting speeds required? Explain why.
13.
With which G-function is constant cutting speed programmed?
14.
Read and explain the following program block. Illustrate the sequence of motions. G01 G95 X100 Z-5 F0.25 S600 T0101
15.
Read and explain the following program block. Illustrate the sequence of motions. G02 G96 X30 Z-30 I30 K-15 F0.2 S180
16.
Read and explain the following program section! N5 N10
G90 G0
G96 X133
T0101 Z2
N20 N30 N40 N50 N60 N70
G1 G0
Z-395 X135 X123 Z-269.8 X133 Z2
F0.3 Z2
G1 G2 G0
Z-274.8
S100
M3
M8
I133
K-269.8
O70
MTS TeachWare • CNC-Grundlagen • Student’s Book
195
4.3
Introduction to manual NC programming
Solution of the CNC exercise on page 151
In the following NC-program, the contour of a pre-turned part is finished. For each command give the corresponding definition. Block No.
N05
N10
N15
N20
N25
N30
N35
N40
N45
196
Commands
Description
O 0300
0300 program name
T040404
select the tool from the turret position 4
M3
activate the spindle in clockwise rotation
M42
select the higher spindle speed range
M63 G96
ignoring spindle rotation M code answer Constant speed cutting ON
S140
spindle speed
G50
maximum spindle speed designation of
S3000
revolution per minute
G0
rapid traverse
X20
X-Coordinate of the target point
Z2
Z-Coordinate of the target point
M8
activate coolant
G1
linear interpolation in slow feed motion
X20
X-Coordinate of the Target Point
Z0
Z-Coordinate of the Target Point
G42
tool nose compensation: right
G3
circular interpolation counter-clockwise
X28
X-Coordinate of the target point
Z-4
Z-Coordinate of the target point
I0
Distance between starting position and circle center in X
K-4
Distance between starting position and circle center in Z
G1
linear interpolation in slow feed motion
Z-28
Z-Coordinate of the target point
G2
circular interpolation clockwise
X34
X-Coordinate of the target point
Z-31
Z-Coordinate of the target point
I3
Distance between starting position and circle center in X
K0
Distance between starting position and circle center in Z
G1
linear interpolation in slow feed motion
X38
X-Coordinate of the target point
Z-33
Z-Coordinate of the target point
G1
linear interpolation in slow feed motion
Z-53
Z-Coordinate of the target point
MTS TeachWare • CNC-Grundlagen • Student’s Book
Solution of the CNC exercise on page 162
Block No.
Commands
Description
N50
G1
linear interpolation in slow feed motion
X44
X-Coordinate of the target point
N55
G3
circular interpolation counter-clockwise
X50
X-Coordinate of the target point
Z-56
Z-Coordinate of the target point
I0
distance between starting position and circle center in X
K-3
distance between starting position and circle center in Z
G1
linear interpolation in slow feed motion
Z-64
Z-Coordinate of the target point
G2
circular interpolation clockwise
X62
X-Coordinate of the target point
Z-70
Z-Coordinate of the target point
I6
distance between starting position and circle center in X
N60
N65
K0
distance between starting position and circle center in Z
G1
linear interpolation in slow feed motion
X66
X-Coordinate of the target point
G1
linear interpolation in slow feed motion
X71 Z-72
X-Coordinate of the target point Z-Coordinate of the target point
G1
linear interpolation in slow feed motion
X76
X-Coordinate of the target point
N85
G40
cancel tool nose compensation
N90
G0
rapid traverse
X500
X-Coordinate of the target point
Z500
Z-Coordinate of the target point
M5
deactivate the spindle
M9
deactivate coolant
M30
program end and backspacing
N70
N75
N80
N95
MTS TeachWare • CNC-Grundlagen • Student’s Book
197
4.3
198
Introduction to manual NC programming
MTS TeachWare • CNC-Grundlagen • Student’s Book
Solution for the CNC exercise on page 164 Solution for the CNC exercise on page153
In the following NC-program, the contour of a work part is milled. For each command, give the corresponding definition. Block No.
Commands
Description
FX100
program name
N05
G54
select work cordinate system one
N10
G90
activate absolute dimensioning
G49
cancel tool length compensation
G80 G40
cancel canned cycle cancel tool radius compensation
G17
select the X-Y-plane
N20
N25
N30 N35
N40
N45
N50
N55
G21
metric input
G91
activate incremental dimensioning
G28
reference point return
Z0.
Z-Coordinate of the target point
M9
deactivate coolant
G91
activate incremental dimensioning
G28
reference point return
X0.
X-Coordinate of the target point
Y0.
Y-Coordinate of the target point
T01
select the tool number 1 from the magazine
M06
mounting the tool
G90
activate absolute dimensioning
S1600
spindle speed
M03
activate the spindle in clockwise rotation
G0
rapid traverse
G43
tool length compensation
Z20.
Z-Coordinate of the target point
H17
offset number for the tool length
X-20.
Z-Coordinate of the target point
Y-20.
Z-Coordinate of the target point
Z-6.
Z-Coordinate of the target poin
M08
activate coolant
G1
linear interpolation in slow feed motion
G41
cutter compensation: left
X10.
X-Coordinate of the target point
D1
offset number for the cutter radius
F250.
feedrate in mm per min
MTS TeachWare • CNC-Grundlagen • Student’s Book
199
4.3 Block No.
Introduction to manual NC programming Commands
Description
N60
G1
linear interpolation in slow feed motion
Y82.
Y-Coordinate of the target point
N65
G2
circular interpolation clockwise
X18.
X-Coordinate of the target point
Y90.
Y-Coordinate of the target point
R8.
radius of the circle
N70
G1
linear interpolation in slow feed motion
X82.
X-Coordinate of the target point
N75
G2
circular interpolation clockwise
X90.
X-Coordinate of the target point
Y82.
Y-Coordinate of the target point
R8.
radius of the circle
N80
G1
linear interpolation in slow feed motion
Y18.
Y-Coordinate of the target point
N85
G2
circular interpolation clockwise
X82.
X-Coordinate of the target point
Y10.
Y-Coordinate of the target point
R8.
radius of the circle
N90
G1
linear interpolation in slow feed motion
X18.
X-Coordinate of the target point
N95
G2
circular interpolation clockwise
X10.
X-Coordinate of the target point
Y18.
Y-Coordinate of the target point
R8.
radius of the circle
G3
circular interpolation counter-clockwise
X-10.
X-Coordinate of the target point
Y38.
Y-Coordinate of the target point
R20.
radius of the circle
G0
rapid traverse
G40.
cancel cutter compensation
X-20. Y-20.
X-Coordinate of the target point Y-Coordinate of the target point
G0
rapid traverse
Z40.
Z-Coordinate of the target point
M5
deactivate spindle
N100
N105
N110
200
MTS TeachWare • CNC-Grundlagen • Student’s Book
Solution for the CNC exercise on page 164
Block No. N115
N120
N125
Commands
Description
G91
activate incremental dimensioning
G28
reference point return
Z0.
Z-Coordinate of the target point
M9
deactivate coolant
G90
activate absolute dimensioning
G80
cancel canned cycle
G49
cancel tool length compensation
G40
cancel tool radius compensation
M30
program end and backspacing
MTS TeachWare • CNC-Grundlagen • Student’s Book
201
4.3
Introduction to manual NC programming
Answers for the control test „CNC Basics“:
1. - The CNC machine tool is not operated manually but programmed. It then automatically processes the entered NC program. - The CNC machine has adjustable axle drives. - The CNC machine has a path measuring system for each travel axis. 2. - All information necessary for machining the work part is entered as commands. -The computer, integrated in the CNC control, controls all functions and adjusts all travel movements. 3. - CNC machine tools work with higher machining speeds. - CNC machine tools work with constant quality. - CNC machine tools work with higher precision. - CNC machine tools lead to shorter transit times. 4. - The feed axes must be controllable to enable the tool to be moved into the exact position desired. 5. - motor - mechanical clutch to avoid overload as well as electronic control - ball thread drive for play-free power transmission - sensor as a travel path measuring system - power amplifier with analog or digital interfaces to the CNC control 6. - two axes minimum 7. - the X axis (face rotating axis) - the Z axis (longitudinal axis) 8. - three axes minimum 9. - the X axis - the Y axis - the Z axis 10. - The controllable spindle axis C on the CNC lathe. - The rotation axis C of a rotary table on a CNC milling machine. 11. - Driven tools enable milling and boring on a CNC lathe.12. - The rotary table enables turning on a CNC milling machine. - The work part can be machined from various sides. 13. - It enables playfree movement of the feed axes - Both halves of the ball thread nut are clamped to each other. The power is transmitted between the spindle and the nut without friction by the balls. 14. - In case of direct position measuring the position is measured directly on the slide. - In case of indirect position measuring the position is defined based on the rotation of the spindle. 15. - In case of absolute position measuring the position can be directly defined on the measuring scale. - In case of indirect position measuring only movements are added together. Therefore the position must be constantly re-calculated. 16. - To keep the cutting speed constant. - To control the start and the halt. 17. - Tool turret - Tool magazine with tool change device 18. - chain magazine - line magazine - ring magazine - plate magazine - cassette magazine
202
MTS TeachWare • CNC-Grundlagen • Student’s Book
Answers for the control test „Basic Geometry“ Answers for the control test „Basic Geometry“:
1. - Turning :
+X
C
+Z
2. - Milling :
Y
X
Z
3. - If points are dimensioned using an angle and a distance, example: drilling hole circle. 4. - Point control - Line control - Path control 5. - 2 ½D path control on the X/Y plane - 2 ½D path control on the X/Z plane - 2 ½D path control on the Y/Z plane 6. - In case of a 2 ½D path control all three axes can be traveled to one by one, only two at one time however. Therefore, the plane on which the travel movement is to take place has to be selected first. 7. - The machine zero point M is the srcin of the machine coordinate system. - The work part zero point W is the srcin of the work part referenced coordinate system. It is set so as to enable the drawing dimensions to be taken directly from it. - The reference point R is required for machines with incremental path measuring system to indicate the control first an absolute position. - The tool reference point E is used to measure the applied tools. 8. - The work part zero point W should be positioned so that the drawing dimensions can be directly taken over for programming. - In turning, in the rotation axis and in most cases on the front face of the work part. - In milling, in most cases on the left lower corner point of the work part surface. 9. - Dimension tolerances do not cumulate. - Single incorrect dimensions do not lead to subsequent errors. - In turning work parts the diameter values can be directly entered as X value.
MTS TeachWare • CNC-Grundlagen • Student’s Book
203
4.3
Introduction to manual NC programming
10. - When incrementally dimensioning points. - When identical contours or boring patterns as well as recesses are to be machined repeatedly. 11.
5 1 0 2 0 3 0 2 5 1
15 2 0
30
20 15
12. - A control chain is open - a feedback loop is closed! - In case of a control chain machines are affected without controlling the consequences. Resulting from internal or external influences deviations from the desired set values are possible. - In case of a feedback loop these deviations are corrected by measuring the actual values and adjusting them to the set values by the feedback loop. 13. - Example: Position feedback loop: When the tool moves, the desired position is transferred to the position feedback loop as a set value.The path measuring system measures the actual position and returns the value to the feedback control. If these values are not identical, also as a result of internal and external influences (disturbance entities), the corresponding movement is initiated until the desired position (set value) has been reached. 14. - As milling tools with various diameters are eventually used. If only the milling machine center point path were considered deviations would appear on the work part. 15. - The length of the milling tool L. - The radius of the milling tool R. 16. - In travel movements, which do not run parallel to the X and Z axis, dimension deviations are created. 17. - The length of the turning tool L. - The measurement of Q. - The tool tip radius R. 18. - To enable the control to calculate the tool tip radius in the correct direction. 19. - Measuring with a tool setup device. - Measuring with zero tools. - Direct measuring when machining a work part. - Optical measuring on a CNC machine tool.
204
MTS TeachWare • CNC-Grundlagen • Student’s Book
Answers for the control test „Technological Basics“
Answers for the control test „Technological Basics“:
1.
- Tool carriers - Tool holders - Indexable inserts
2.
- higher cutting speeds and higher cutting-edge life compared with high-speed steels - quick and simple exchange of indexable inserts
3.
- P (blue) für long shipping material - M (yellow) for materials which are difficult to be machined - K (rot) for short shipping materials
4.
- The clearance angle influences friction on the work part and consequently, the heating-up of the cutting edge.
5.
- A larger angle of rake improves the machining flow. - A larger angle of rake reduces the cutting forces.
6.
- A larger angle of rake increases the cutting edge breach. - A larger angle of rake increases the decarburization.
7.
- Negative angles of rake are necessary for machining hard and brittle material.
8.
- The adjustment angle influences the feed power, the forces against the work part, the cutting width and the cutting depth.
9.
vc = π *d * n ,
or
n=
vc π *d
n=
120m π *m in* 0,08m
n = 477 1 min 10.
vc
= π *d * n
vc = π * 0,25 ⋅ m ⋅ 100 1 min vc = 78
m min
MTS TeachWare • CNC-Grundlagen • Student’s Book
205
4.3
Introduction to manual NC programming
11. - It must clearly determine the position of the work part. - It must detain all forces from the work part. 12. - keybar chucks - jaw chucks with scrolls possibly
two-jaw chucks three-jaw chucks four-jaw chucks
13. - large work parts - irregularly formed work parts 14. - For clamping long, slim work parts 15. - mechanical power generation - pneumatic power generation - hydraulic power generation - electric power generation 16. - clamping with clamping elements - machine vises - fixtures 17. - quick work part exchange - accurate clamping of work part
206
MTS TeachWare • CNC-Grundlagen • Student’s Book
Instroduction into CNC technology
Answers for the control test „Introduction into NC programming“:
1. The programmer must determine all necessary information required for the NC-program. The steps are: 1. defining machining steps 2. defining necessary tools 3. calculating technological data 4. calculating geometric data 5. generating the NC-program 6. controlling the NC-program 2. The work plan contains all machining operations, clamping devices and technological data that was calculated in the production drawing. 3. Switching information relates to commands that switch machining functions on or off. Example: spindle rotation coolant tool change 4. see Comparison of programming codes/keys of various CNC-controls 5. An NC-program consists of a beginning (Ex. %), an end (Ex. M30) and a chronological sequence of NC-blocks. 6. An NC-block consists of a block number and series of words. 7. A program word consists of an address letter and a number with +/-sign. 8. F S T M X Y Z
feed speed tool position in tool storage or turret additional or switching information target coordinates in X-direction target coordinates in Y-direction target coordinates in Z-direction
9. a) Travel to a diameter of 53mm and to target coordinate Z 184.005. b) Travel incrementally from the present tool position 53mm in +X-direction and 184.005 in +Zdirection. 10. The address letters I, J, K are interpolation parameters. For example, when programming circular movements they incrementally define the coordinates of the circle center with respect to the starting point of the circular movement. 11. clockwise circular interpolation: G02 activate coolant: M8 activate spindle in clockwise rotation: M3 12. A constant cutting speed is used for face and form turning. A constant surface quality is obtained since the number of rotations adapts to the changing diameters. 13. With the command G96 and starting speed S Ex.: G96 S2000 14. G01 G95 X100 Z-5 F0.25 S600 T0101 Travel tool Nr. 1 considering the tool compensation value in storage Nr. 1 in a linear movement with a feed of 0,25mm per rotation towards target coordinates X100 (diameter) and Z-5.
MTS TeachWare • CNC-Grundlagen • Student’s Book
207
4.3
Introduction to manual NC programming
15. G02 G96 X30 Z-30 I15 K-15 F0.2 S180 Travel clockwise in a circular movement with constant cutting speed and a feed of 0,2mm per rotation towards the target coordinates X30 and Z-30. The circle center is incrementally located 15mm in +X-direction and 15mm in +Z-direction from the starting point. 16. N5 G90 G96 T0101 S100 M3 M8 Absolute programming call, constant cutting speed with starting speed of 100 rotations per minute, the tool Nr. 1 with the compensation value in storage Nr. 1. Activate the spindle in clockwise rotation and coolant. N10 X133 The toolG0 moves in rapid Z2 traverse to the coordinates X133 and Z2. N20 G1 Z-395 F0.3 The tool travels with a feed of 0,3mm per rotation to the target point X133 and Z-395. N30 G0 X135 Z2 The tool moves in rapid traverse to the coordinates X135 and Z2. N40 X123 The tool moves in rapid traverse to the coordinates X123 and Z2. N50 G1 Z-269.8 The tool travels with a feed of 0,3mm per rotation to the target point X123 and Z-269.8. N60 G2 X133 Z-274.8 I5 K0 The tool travels clockwise with a feed of 0,3mm per rotation in a circular movement to the target point X133 and Z-274.8. The circle center is incrementally located 5mm in +X-direction from the starting point. N70
G0
Z2
The tool moves in rapid traverse to the target point X133 and Z2.
208
MTS TeachWare • CNC-Grundlagen • Student’s Book