L07 NC-programming and Simulation

Transcription

1 Simulation and control of Production Plants L07 NC-programming and Simulation Dipl.-Ing. S. Bauer Tel.: Laboratory for Machine Tools and Production Engineering RWTH Aachen University

2 Overview Introduction What is the purpose of NC-programs? Where are NC-programs used? NC-programs: Formats and dialects Postprocessors: Need and Function Shop floor oriented NC-programming 2

3 Introduction Why do we need NC-programs? Machine-readable and interpretable description of a manufacturing task. Exchange format for automated switching commands and axes-movements. NC-programs can be stored, adapted and reused whenever needed. Complex and large machining operations cannot be controlled manually: Threads, pockets 3D freeform surfaces Parallel acting tools Synchronisation of several aggregates Source: Siemens 3 The NC-program represents the input data of a numerical control (NC). It can be stored and loaded whenever needed to produce the programmed part or execute the specific numerical controlled machining task described by the NC-program. Thus the NC-program contains all information about the job the numerical control has to evaluate (interpret), to pre-process (movements and switching operations) and pass to the executing modules (drives and PLC). The task described by a NC-program can contain the machining of a mechanical part. Therefore the term NC-part program is also used. In addition there exist also NC-programs for simple handling operations. But in general a NC-program is used to describe a machining task in an ASCII format, which can be interpreted by a numerical control. There are different formats and dialects for NC-programming. Depending on the machining task the appropriate NC-programming language is chosen. For several machine tool, control or customer specific functionality the NCprogramming language s codes are extended. They are non-standardised extensions.

4 Numerically Controlled Machine Tools Turning Grinding Drilling Milling Measuring Sawing Cutting, Blanking Sink-, Wire-EDM... 4 NC-programs are used for various technologies and different types of machine tools. The task described in the NC-program has to be adequate to the technology or machine tool, which shall be controlled with this program. Depending on the technology the NC-program can be more or less complex: For co-ordinate measuring machine the path is not as important as the final position. But this final position is matter of measuring and therefore is not exactly predefined by the NC-program. The probe is moved along a path as long as the probe has no contact. For a milling machine tool the path has to be explicitly specified in the NCprogram. The control has the task to exactly execute this tool path.

5 Functions of a NC-program Commands for numerical controls: Tool movement description indirect: workpiece geometry direct: tool movements Technology information Spindle speed, feed, cutting speed Switching commands Spindle clockwise / counter clockwise Tool change Synchronisation Marks for operations with multiple slides Pallet changer, clamping devices, etc. Source: Dassault Systèmes (CATIA V4), EXAPT (EXAPT-Plus) 5 The task to be executed can be described explicitly or implicitly. For instance the NC-program can contain explicit axis values called cutter location curves (CLdata), which are executed without regarding the tool s dimensions. But in modern numerical controls (NC) the tool s dimensions and the tool s wear behaviour can be compensated. Therefore the NC needs commands describing the cutter contact curves (CC-data) to be able to compensate the tool at runtime or even the complete description of the geometry to be machined ( pocket, drill hole,.). In addition the NC-program needs to contain the technological instructions. Milling: feed, spindle speed, clockwise / counterclockwise tool rotation, lubrication on/off, EDM: voltage, maximum charge, relax time, In order to control machine tools with several spindles synchronisation flags and synchronisation information is needed. For instance a lathe machine tool with two slides can only move without the risk of collisions, when the NC-program contains security distances and simultaneously controls the movements of both slides.

6 NC application flow 6 For the process of NC-programming several documents are needed. At first the geometry to be machined needs to be defined as well as the raw part dimensions. The geometry is usually generated in the design department. This department mainly focuses on the shape of the part whereas the way of production is often a secondary aspect. Afterwards this information is passed to the NC-planning. Here the geometry is divided into sections and execution steps, which can be machined successively. These sections are assigned to specific machining technologies. Typical machining technologies are for instance milling, turning, grinding or EDM. Depending on the technology a machine tool to manufacture the part is selected. Based on the machine tool s abilities and depending on the available tools the machining operation including machining strategies and technological parameters (cutting parameters) is defined. This information is stored in a machine tool and NC specific NC-program. Finally the NC-program is executed and the part is produced.

7 Methods for NC-coding Design & Product-Development Planning Production Manual part-drawing knowledge based, manual calculations, look up data in tables and hand-books - geometry evaluation and tool path programming - technology definition Shop floor oriented drawing / CAD file graphical-interactive, problem oriented programming for a specific control and tool - predefined data-masks for programming tasks - dialogs and suggestions for parameters DIN Automated CAD file graphical-interactive for different machine tools - complex geometries - collision-checking routines - calculations of tech. and time optimised tool paths Postprocessor CL Data, APT,... 7 NC-coding can be done manually or assisted by a computer system. The manual coding is generally used for simple parts, which often change and where the use of a computer would be to expensive. The operators generating the NC-programs manually are usually well experienced and know most of the parameters they need to code the program by heart. But still they need to calculate the tool paths based on the given drawings and they need to look up technological cutting parameters depending on the tools available and the given material. A help for the operator is the so called shop floor oriented programming (SFP). The SFP-system is a graphical interactive system running on the human machine interface of the NC or on a separate PC. It offers several data masks to easily program standardised and often used shapes, like pockets, drill holes, planes or contours. The operator does not need to calculate the tool paths. He only types in the necessary parameters. For instance for a drill hole he defines the hole s location and its depth. Then he selects a tool from the SFP-system s tool data base and defines the technological parameters for feed and speed. For more complex and elaborated NC-programs CAM systems are used. Like SFP-systems these systems are able to import CAD files and use a computer to calculate the tool paths. But the automated systems are much more powerful. They are able to automatically recognise contours, geometrical items like features, they can avoid collisions, propose technological parameters and they can generate NC-programs for more than one technology.

8 Input needed for NC-programming Geometry Raw part and final part dimensions Features, tolerances, surface qualities Resources Tools, coolant, clamping devices Workspace, axes dimensions, axes-kinematics Machine Power, type of numerical control Periphery: pallet changer, handling devices,... Technology Workpiece, cutting material, cutting parameters 8 As described before the NC-program passes information concerning a manufacturing task to the numerically controlled machine tool. A NC-program needs to contain information to control the machine tool s axes movements, the technological parameters for feedrate and spindle speed and auxiliary commands to control a pallet changer or the tool magazine. To define all these parameters, the NC-programmer needs adequate input information when he starts to code the NC-program: He needs to know the raw part as well as the final part geometry in order to calculate the volumes to be removed and the tool paths needed to remove this volume. Besides he needs to know, which machining equipment / resources are available: the machine tool with its spindle power and maximum axes range the tools in the tool magazine with their dimensions and their wear status Finally he needs to know the typical technological parameters to machine the given material with the tools he has selected.

9 Geometry Motion commands always programmed with respect to work part geometry, i.e. the work part coordinate system Clamping may block programmed tool paths - clamping devices and positions known at programming time? Raw part geometry determines details of roughing operations 9

10 Technology & Resources Technology parameters must be set according to Cutter shape and material Part material Target surface quality Tools determine machining possibilities high number of blades allows increased feed rate in soft materials, but cannot be used in cutting hard materials robust roughing tools permit higher cutting rates, but cannot deliver finished surfaces optimisation criteria: short machining time (yields high productivity) few different tools (reduce required tool inventory palette) minimised tool wear (lowers cost) Source: Kopp Schleiftechnik, Hilma Spanntechnik 10

11 Influence of the workpiece in NC-programming Prismatic, spherical and planar work pieces (2½ D = 2-D boundary + ½ D for depth) Drill hole, step, slot, pocket, contour, groove,... Constant tool orientation Surfaces, curves interpolation in more than 2 axes (3D geometry) Freeform-surfaces Oriented profiles Tool must be moved and oriented in more than 3 axes simultaneously Source: Open Mind 11 In terms of calculation the geometry of a workpiece usually takes the longest time in NC-coding. For simple holes the calculations are generally limited to positions (x,y,z and sometimes an orientation of the z-axis) and a vertical z-axis movement to achieve the depth of the drill hole. Thus the machining is executed by only one axis, the z-axis.the other axes are only used for positioning. For pockets, planes and simple planar contours generally two axes (e.g. X,Y for milling and X,Z for turning) are moved in parallel. Thus their interaction needs to be controlled by the NC-program. Especially for spherical movements the dependencies between the axes becomes complex. Therefore the NCs and their NC-programming interfaces offer predefined commands to machine circles or sometimes also to machine spirals and hyperbolas. But for more complex shapes all 6 degrees of freedom need to be controlled simultanously. Thus 5 axes are needed: for the translation X,Y,Z and for the rotation A,B (C is the rotating tool). Only by moving all these axes in parallel a freeform surface can be machined with a continuous tool orientation. It is obvious, that the computation of the necessary 5 axes commands is too complex for manual programming. Therefore CAM systems are used to generate these NC-programs.

12 Influence of the machine tool in NC-programming Number & functionality of the machine tool s axes - Positioning axes (e.g. drilling machine tools) - Orienting axes (e.g. machine table) - Machining axes (e.g. spindle) Kinematics - Serial kinematics - Parallel kinematics Power and ability - Size of the workspace - Length of the machine tool s axes - Accuracy, stiffness - Tools (chuck, number, diameter, length, weight) - Spindle power, maximum feed and acceleration Source: Maho-Deckel, INDEX-Werke 12 The machine tool is another input parameter for the NC-program generation. In general every machine tool has special functionality, which needs to be controlled by individual commands: pallet changer, tool magazine, additional handling axis. Besides machine tools have different axes kinematics. There are 3 axes milling machine tools as well as complex 5 axes machine tools or 6 axes hexapod kinematics. For lathe machine tools the axes kinematics mainly depends on the turrets: The illustrated INDEX-lathe machine tool can be equipped with different turrets and motor driven tools. To control the turrets and motor driven tools it is necessary to know how they are oriented and the possible movements they can execute. The size of the machine, its table or its chuck limits the size of the parts, which can be machined. In addition a machine tool is characterised by its spindle power and the dynamic abilities of its axes.

13 Influence of the control in NC-programming Type of control - Point-Control - Path-Control Interpolation modes - Straight line interpolation - Circular interpolation - Interpolation of simple functions - Spline-Interpolation Auxiliary functions - Number of axes to be controlled simultaneously - Accuracy in positioning - Velocity control - Tool management - PLC functionality 13 As previously explained movements in one or more axes are required to machine a specific geometry. For drill holes the movement is limited to a positioning movement and afterwards an uni-axial movement into the tools axis direction (e.g. z-axis). For the shown pocketing operation up to two axes move in parallel while one pocket level is machined and then a z-movement is required to proceed to the next deeper level. For freeform machining or complex positioning and handling movements, which avoid collisions and minimize path lengths and thus time, several axes are generally moved in parallel. Concerning the NC-coding the type of paths and the number of axes to execute these paths need to be known in the beginning in order to calculate the movement commands.

14 NC-Programs: Formats and Dialects Excerpt of a G-Code program Depending on the task there are different formats for NC-coding G-Code (DIN 66025) One of the first standards and the most popular format Interpolation of arcs, lines Simple statements, primitive switching commands Based on a sequence of lines CLDATA Programming of tool-path (centre or contact point) and orientation APT Task oriented description Raw part description, technology sets, tool description Heidenhain Conversational cycle entry with graphic support simple 2½ D-programming tasks Based on machining cycles (= predefined program elements) StepNC/ ISO Feature-oriented NC-programming Source: EXAPT 14 There are different languages or so called NC-programming interfaces to write a NC-program. The most common one is based on the DIN This so called G-code is probably the oldest standard for NC-coding. Its commands are very simple structured and thus easy to learn. As the G-code is not that powerful and often more complex commands are needed, additional NC-programming languages were and are developed: The cutter location data (CLDATA) is a NC-programming interface to directly control the axes positions. Especially for freeform machining CL-data is used, as all tool radius compensations are computed offline by a CAM system and the machine tool does not perform a cutter contact, but a axis or tool centre point movement. APT (automatically programmed tools) is an interface to program task oriented. The programming task is described in a set of machining operations. APT was developed to store more structured and complete information in the programming systems. Today it is used by NCprogramming systems like EXAPT. APT is not executed by numerical controllers. A postprocessor is used to generate G-code or extended G-code out of the APT program. Heidenhain, a control vendor, has developed his own NC-programming language, which mainly focuses on simple shop floor oriented part programming. Besides there is a standard called ISO (STEP-NC), which still is in a testing phase. The standard s intention is to pass complete geometry and task information to the NC in order to enable more elaborated and autonomous functionality at the NC level: tool correction, wear compensation, path generation.

15 DIN (G-Code) Line: N0005 G00 X20 Y30 Z10 A4 S2600 F0.5 M03 Line Number Command Coordinates Technology Auxiliary functions Path commands: - Interpolation: G0, G1, G3, G2,...G33 - Measuring ref.: G90, G91, - Units: G70, G71, - Zero-offsets: G54,... G59 Coordinate: - Linear main axes: X, Y, Z - Rotational axis: A, B, C - auxiliary axis: U, V, W Interpolation parameters: - I, J, K (for circular interpolation) Technology: - Feed: F - Spindle speed: S - Tool No.: T Auxiliary functions: - Synchronisation: - at the beginning: M03, M04, M07,... - at the end of a line: M00, M02, M05,... - effect: - modal: M03, M04,... - line: M02, The G-code is probably the most frequently used NC-programming language. Its structure is very simple: The G-code is a sequential, line based programming language. Each line consists of an optional line number (a relict of the ancient Computer programming languages) and a set of commands. The commands are divided into technological, geometrical and auxiliary commands. Each command consists of a tag ( G, M, ) and a parameter. This parameter is used to distinguish the commands (M06, M07) or to define a movement command (X100, Y200) or to set the technological parameters (S100, F460). To program loops and to repeat single code segments, the G-code offers subroutines. In addition the G-code is extended by more or less every control and machine tool vendor with their individual commands to control specific auxiliary machine tool functionality or to offer machining cycles to program often used geometries. These extensions are the reason why it is nearly impossible to execute the same NC-program on two different NCs.

16 APT PARTNO/MyWZLPartNo1 MACHDT/30,150,1,10,5,2000,0.8 P1=POINT/80,80,10 C1=CIRCLE/CENTER,P1,RADIUS,40 K1=PATTERN/ARC,C1,90,CCLW,4 A1=REAM/DIAMET,30,DEPTH,25 CLDIST/2 COOLNT/ON WORK/A1 GOTO/K1 FINI Header including the part name General machine data Geometry definition for a list of positions on a circular pattern Command to drill a hole with diameter D=30 mm Sequence of executions End 16 APT (automatically programmed tools) is used on the CAM level. APT is not directly executed on the NC. A postprocessor is needed to translate APT to the NC s programming interface, which generally is G-code. The advantage of APT is it s more complete information. While the G-code only contains movements and commands, APT contains the raw part dimensions, defines geometrical units similar to features and a list of execution commands.

17 Postprocessor Adaptation of Functionality stored in a general way in the CAM or SFP to the commands of the specific CNC. Auxiliary commands e.g. tool change, pallet changer Generate or compile machining cycles Pocket cycles, patterns for drill holes etc. Kinematical transformation Cutter location path (CL) Axis limit Examples BMW is using about 120 Postprocessors DaimlerChrysler: ~300 Postprocessors (worldwide) Source: CNC-online 17 The postprocessor is used to translate and to adapt a more common data format, like for instance APT, to the control and machine specific NCprogramming interface. Especially when several types of numerical controllers are used in parallel, postprocessors become necessary. The CAM is designed to generate a more or less general valid NC-program. It can be used for different types of NCs. A CAM system is also able to handle different technologies (milling, turning, EDM ). But each NC or machine tool requires specific commands. Therefore there are postprocessors, developed by the CAM or external providers. These postprocessors adapt the general NC-program to a specific NC.

18 Manual programming First and traditional method for NC-Programming Limited code productivity and code complexity Fully dependent on programmer Highly flexible, machine operator can change code at the last minute Fully manual, hence error prone 18

19 Manual NC-programming, workflow Machine Tool, Tool catalogue Clamping devices Select machine tool and tools Define clamping position Set-up information Define sequence of execution Work plan Drawing, Technology data, Machine ability Calculate tool paths and technological parameter NC-Program Dry-run / program test Input Information Eventually correct faults Archive Output Information 19 The shown sequence is an example, how a NC-program is generated and tested. First the machining equipment is selected. For this task catalogues are used. Then the clamping position is defined. Based on the available tools and the clamping position the tool paths are calculated. After defining the technological parameters, the program needs to be tested. Errors are likely to occur and therefore a so called dry-run with reduced feed rates and generally without a workpiece is executed. During the dry-run the operator checks if the executed sequence and the executed paths correspond to what he wanted to program. When the program is tested and approved, it is stored. The result of the NCprogramming are several documents: A text describing how to clamp the workpiece, the values of the variable parameters, the zero-offsets and the tools to use. This information is called set-up information. A work plan describing which operations have to be executed in which sequence by the operator and by the machine tool. Finally the NC-program containing the commands to be interpreted and executed by the NC. Depending on the available systems and their functionality, this sequence can look different. For instance a simulation could be added before the dry-run in order to verify the tool paths.

20 Motivation for automated NC-programming 20

21 Shop-Floor oriented programming Shop-floor oriented programming is a concept, a way of getting programming tasks done Software systems may support this concept, the benefits depend on whether the concept as a whole is implemented Core idea is about empowering the machine operator to flexibly adapt the program according to workshop conditions - and unforeseen challenges Goal: Provide automated programming support without the complexity of a CAM-system, and provide for feeding back the machine operators changes 21

22 Motivation for shop floor oriented NC-coding 22

23 Shop floor oriented programming (SFP) Idea: Source: Heidenhain SFP supports the operator to easily program recurring machining tasks. Even Geometry, such as contours or complex pockets, can be generated with a SFP system. In dialogues the SFP systematically asks for all parameters the operator can look up in the drawing or in his tool data base. As a result the SFP generates the NC-program with the machine specific commands. 23

24 Functionality of SFP Systems Primary goal: support the operator in generating and editing NC-programs as well as set-up activities Program visualisation Simulation of the machining process (offline, online) Raw part, finished part, tool information, tool paths, Adapt the NC-program, select or modify tools Zero offsets, tool geometry data Generate NC-programs Predefined, parameterised elements (drill holes, pockets, planes, taps...) Safety Definition of safety distances / areas Tool path generation with collision avoidance Tangential approach and retract movements Source: Heidenhain, dcade 24

25 Machining cycles in SFP Systems Turning cycles Based on raw part definition and a final contour the volume to be machined is divided into single cuts Uni- and bi-directional strategies Backside, front machining Detection of rest material Drilling Deep holes Holes located on patterns Tapping Threading Outer- / inner thread Planar or spherical threads Multiple threading Finishing operations for precision threads Grove cycles Grooves Chamfers, edge round Milling cycles Sets of parameterised contours Slots Pockets with islands / bosses Cylinders Tool path Tool measuring Laser Touch probing Raw part measuring Touch probing 25 Machining cycles are used to parameterise machining tasks. They are either directly executed by the NC or a postprocessor is needed to translate them to simple standard commands. Machining cycles make NC-coding less complicated. For instance the NC-coding to drill a deep hole can be very time consuming, as several retract movements are needed to get rid of the chips. A machining cycle for a deep hole drilling operation would simply have some parameters, describing the overall depth and the maximum depth for one drill action until a retract is necessary. The series of drill and retract movements then is computed by the postprocessor or the NC itself. The operator is effectively assisted and boring as well as error-prone activities are effectively reduced.

26 Trends in shop floor oriented NC-programming (SFP) 26 The shop floor oriented programming aims to support the operator at the machine tool or in the shop floor. Therefore menus and dialogues are used, which describe the machining task and ask for parameters to program the machining task. Besides theses systems need to be attached to the more complex programming systems of the planning department. This attachment is necessary to ensure, that NC-programs can be exchanged and that common data bases for technology parameters or tools can be used. The import of CAD geometry data becomes necessary, when drawings are handled in the shop floor. Today there are still a lot of paper drawings, but as CAD systems become more easy to use, geometry information is stored digitally and can be accessed by computer based systems.

27 1) SFP Systems for specific technologies Used to control machines which manufacture a typical type of parts Example: Milling of crankshaft (typical Orbital geometry) Advantages No NC-coding knowledge required Easy to understand and to learn dialogues Programming effort is reduced to few parameters Illustrations of the part explain the parameters Preset data masks with proposed values support the operator when generating a new program Source: andron 27

28 Examples Tool grinding Camshaft Gear grinding (Zahnradschleifen) Gear grinding (Zahnradschleifen) Source: andron 28 There are machine tools, which are designed and used for only a specific type of workpieces. For instance tools to mill or grind gears can be programmed by simply defining technology and geometry specific parameters. The complex axes movements can be calculated by the NC itself. For these machine tools the human machine interface looks different than for a conventional milling or turning machine tool. The data masks are adapted to the specific task and all irrelevant information is left out. Images describing the machining operation and the relevant parameters assist the operator while he generates the parameter set to control the machine tool. Operating becomes more easy. A conventional NC-program is not needed any more. The parameters are stored in a parameter table and can be loaded, whenever needed.

29 2) SFP Systems for milling Prismatic parts Limited to 2 ½ D elements / shapes Drill holes, slots, planes, pockets, steps,... Calibration of tools and raw part clamping positions Nesting for blank parts SIEMENS Vendors: (CAD/)CAM system provider: Gibbs CAM, EXAPT (EXAPTplus), Keller (CNCplus), MTS-CNC, UGS (dcade),... Control vendors: Heidenhain, Siemens (ShopMill), andron, BOSCH,... 29

30 Machine specific set-up (MTS-CNC) Working space & security distances and areas Dimensions Traversing range Clamping devices Vise Clamping kit / set of clamping blocks etc. Vacuum clamping systems Tool magazine Offset definition of the chuck Menu based tool geometry offset definition Spurce: MTS-CNC 30 The shop floor based programming needs to follow the steps already described before. But contrary to the manual programming the operator is guided by the SFP system throughout the whole programming process. First the machine tool is selected and its work space is defined. In general this has to be done only once for a machine tool. Then the raw part is defined and the clamping devices are selected. There are even SFP systems, which can display and partly consider the clamping devices within the collision avoidance. The tool magazine can generally be displayed and edited by the SFP systems.

31 Set-up (MTS-CNC) Define the raw part Dimensions of the raw part Clamping positions for multi axes machining Select clamping kit and the devices positions Automatic calibrate the raw part position by touch probing Set-up of the tool magazine Magazine position Tool geometry Lifetime Substitute tools Source: MTS-CNC 31

32 Path programming (MTS-CNC) Programming a sequence of machining commands Identify geometric items (drill hole, slot, pocket,...) Determine the sequence of execution Select strategies and tools Define the technological parameters Simulation Verify the tool path Detect and avoid collisions Get an idea about the sequence of execution and the result to be expected Source: MTS-CNC 32 The geometry to be machined, respectively the tool paths are programmed interactively. The SFP offers different types of contours (lines, arcs) which can be selected and added to each other in order to define contours. At the end there are simulation routines, which display the tool path and show the removed material depending on the tool path and the tool s dimensions (length, radius). This helps the operator to verify if a collision might occur. Testing and simulation are very important. Even if a dry-run or a computer based simulation are time consuming, they help to avoid serious crashes.

33 Siemens ShopMill Tools Raw part Raw part probing Geometry Technology Simulation 33 The systems ShopMill and ShopTurn are distributed by Siemens and can be bought as an option for the Siemens controllers. The given images are screenshots from the SFP-system for milling, called ShopMill. As shown in the upper left screenshot the system directly uses the Siemens tool data base and therefore offers an easy to use tool to assign tools to previously programmed machining geometries (lower left image). The set-up is also assisted by the system (upper-right image). The operator can shift (X,Y,Z) and rotate the clamping position (A,B). Besides routines are offered to touch probe the raw part and copy the measured positions into the set-up s zero-offsets. Finally the systems can simulate the machining. This helps the operator to detect collisions and to verify that he has programmed the right geometry.

34 3) SFP Systems for turning technology Rotational parts Contours (in xz-plane) Groves Threads Drill holes Systems: CAD/CAM vendors: EXAPT (EXAPTplus), Keller (CNCplus Drehen), MTS-CNC (CNC-Drehen), CNC Control vendors: Siemens (ShopTurn, AutoTurn, WOP 840C), INDEX, Traub,... Source: Keller (top), Siemens (bottom) 34

35 CAD/CAM toolchain automates programming tasks to relieve programmer extends the limits of program complexity, hence enables the machining of complex parts always consists of a software system which provides programming automation through algorithms software complexity requires training different from machine operation skills; This often results in establishing a separate process planning department one-way programming, i.e. changes at the machine are difficult to perform and must be reported back to process planning 35

36 Geometry import Source: EXAPT 36 The EXAPTplus system offers several data bases and routines to support the NC-programmer. There are interfaces to import technological data sets, tool data and CAD drawings. The operator does not need to type in all data, but he can easily load the data form other systems. 1) Geometry recognition by EXAPTplus In an interactive programming system the CAM data set can be imported from an existing geometrical information, a CAD drawing or the geometry has to be generated interactively. In the given example we use the import functionality of EXAPTplus in order to read in an AUTO- CAD drawing. After the import routine has been carried out the final part geometry is available in the CAM system. Now the raw part has to be defined. Raw part information is usually not available in CAD systems as the design does focus on the finished part. Therefore the raw part geometry is defined interactively in EXAPTplus. Based on the raw and final part the EXAPT system starts a geometry recognition routine in order to compute the parts contour and in order to find typical shapes, which are assigned to specific machining operations, like: -drilling, tapping, circular or linear cutting movements,... The recognised contour is displayed in the upper right image. The original CAD data is shown in the lower left image.

37 Tool selection Source: EXAPT 37 2) Tool selection: select tools and assign them to the different places in the turret In order to be able to call tools for the machining operation, we need to define tools and their position in the turret. As for all operations in an interactive programming system there are also data masks and menus to do so. These masks already provide pre-defined data sets for the most common shapes of tools and tool holders. By simply selecting these items the tool can be defined and then only the specific values have to be typed in. All tools and tool holders are then stored in a database, which manages all equipment and the machining resources of the machine tool. In German this database is called BMV (Betriebsmittel Verwaltung).

38 Programming of the tool path Source: EXAPT 38 3) NC-programming: selection of operation, tool, starting and end point The tool path generation and the definition of the operations sequence is the most important part of the NC-programming. There are two ways this can be done. a) Automatically The system recognises the final parts contour and calculates the volumes that have to be removed based on the raw part s geometry. Then the tools and technological values are chosen to remove this volume. Depending on the tool and its cutting parameters (cutting depth,...) the tool paths are generated. b) Interactive The user still has the choice, which tool, technology, starting position etc. suggested by the system he wants to use. Based on his selections the system calculates the machining sequence and the tool paths. The EXAPT system offers the combination of both methods. The operation planning can be done automatically and then be optimised by the operator. He can select single geometrical elements and define different operations for each of them. Thus the advantage of an interactive programming method depends on the knowledge stored in the system s database and the worker s know-how. If the database is powerful and the system s algorithms can consider various machining operations and technological options, the automatically generated NC-program can be considered to be optimised. But in general the user s experience is not stored in databases and can only be used, by involving him into the programming process. He often knows better which tool to use or which cutting direction to apply. => The operator s know-how is only included by interactive systems

39 Technology definition Source: EXAPT 39 4) Technology selection The technology as part of the operation is defined by a set of values: -feed, speed, cutting depth,... For different materials and depending on the selected tool these values have been calculated and evaluated for former NC-programs and are stored in a database. The EXAPT system uses this data when generating a new NCprogram. Thus the operator does not have to look-up what he did the last time, but is supported by the systems proposal. In case the technology is not adequate, the operator can adapt the parameters and store the data set for the current NC-program and for future use.

40 Simulation of the NC-program Source: EXAPT 40 4) Simulation of the NC-program after operations have been synchronised Especially in lathe machine tools it is very common to use more than one tool at the same time and to use tools, which are fixed on different turrets that are synchronously moving. Generating a NC-program these simultaneous movements have to be considered in order to avoid collisions while optimising the tool paths. As the operator always wants to finally check the computed results, the CAM and SFP systems usually offer a simulation. Especially collisions can be detected by observing the simulation. The simulation is also needed to show the machine operator what will be machined in which way. The operations sequence is shown by the movement of the tools and a time scale.

41 Generated NC-program Source: EXAPT 41 5) NC-program generated by EXAPTplus Finally EXAPTplus generates different documents: -NC-program -tool list -set-up information -raw part information The shown NC-program contains all switching commands, movements and synchronisation information needed to machine the example part on a specific machine tool. Therefore the EXAPT system offers postprocessors which generate specific NC-programs or generate a CLDATA file based on the APT data stored inside the EXAPT system. The given NC-program lists the commands for both slides in one file. This format does help the operator to understand the synchronisation of the two slides movements.

42 Generated set-up information Source: EXAPT 42 6) Set-up information The set-up information contains instructions for the operator who wants to execute the NC-program. He needs to know how to clamp the raw part, where to define the zero-offsets and where to move the axes in order to start the NCprogram. Additionally the set-up information contains a list of tools required to machine the part. The operator has to ensure, that the tools are available and that they match the requirements concerning wear criteria and tool geometry.

43 Conclusion Control technology is not limited to the control of machine tools. The algorithms used for tool-path and axes movement generation can also be used for simulation and visualisation. The benefit of the algorithms and software modules highly depends on the possibility to reuse them in various applications: two different pocket-milling-algorithms will probably not compute the same tool-paths. Thus for a reliable simulation it is necessary that the NC internal algorithm is the same as the one used for simulation. Source: Siemens 43