Development of a Variational Part Model Using In- Process Dimensional Measurement Error

Transcription

1 Brigham Young University BYU ScholarsArchive All Theses and Dissertations Development of a Variational Part Model Using In- Process Dimensional Measurement Error Shane A. Carlson Brigham Young University - Provo Follow this and additional works at: Part of the Mechanical Engineering Commons BYU ScholarsArchive Citation Carlson, Shane A., "Development of a Variational Part Model Using In-Process Dimensional Measurement Error" (2006). All Theses and Dissertations This Thesis is brought to you for free and open access by BYU ScholarsArchive. It has been accepted for inclusion in All Theses and Dissertations by an authorized administrator of BYU ScholarsArchive. For more information, please contact scholarsarchive@byu.edu.

2 DEVELOPMENT OF A VARIATIONAL PART MODEL USING IN-PROCESS DIMENSIONAL MEASUREMENT ERROR by Shane A. Carlson A thesis submitted to the faculty of Brigham Young University in partial fulfillment of the requirements for the degree of Master of Science Department of Mechanical Engineering Brigham Young University August 2006

3 BRIGHAM YOUNG UNIVERSITY GRADUATE COMMITTEE APPROVAL Of a thesis submitted by Shane A. Carlson This thesis has been read by each member of the following graduate committee and by majority vote has been found to be satisfactory. Date W. Edward Red, Chair Date C. Gregory Jensen Date Carl D. Sorensen

4 BRIGHAM YOUNG UNIVERSITY As chair of the candidate s graduate committee, I have read the dissertation of Shane A. Carlson in its final form and have found that (1) its format, citations, and bibliographical style are consistent and acceptable and fulfill university and department style requirements; (2) its illustrative materials including figures, tables, and charts are in place; and (3) the final manuscript is satisfactory to the graduate committee and is ready for submission to the university library. Date W. Edward Red Chair, Graduate Committee Accepted for the Department Matthew R. Jones Graduate Coordinator Accepted for the College Alan R. Parkinson Dean, Ira A. Fulton College of Engineering and Technology

5 ABSTRACT DEVELOPMENT OF A VARIATIONAL PART MODEL USING IN-PROCESS DIMENSIONAL MEASUREMENT ERROR Shane A. Carlson Department of Mechanical Engineering Masters of Science To improve the geometric accuracy of CNC machined parts, dynamic machining errors due to on-line disturbances (tool deflection, tool wear, heat deformation, etc.) should be accounted for in some manner. Unless these on-line disturbances are properly handled, it is obvious that a high degree of geometric accuracy is difficult to achieve. Many attempts have been made to compensate for these on-line disturbances such as the development of engineering models; however, the models are not adequate enough for reflecting the real phenomenon and are dependent on continuous process monitoring using a variety of sensors. Closed-loop process control is a scheme for manufacturing parts and compensating for on-line disturbances and machine tool inaccuracies using error feedback. The goal has been to develop a system that automatically provides dimensional

6 error feedback to the process machine. Closed-loop process control can be achieved before, during (in-process) or after the machining cycle. In-process control is achieved by measuring the part prior to finishing cuts while the part is fixtured to the machine tool. Although the theory behind an automated closed-loop, in-process control system would significantly reduce manufacturing costs, at the present time, machining errors typically are compensated through manual error feedback. This thesis presents a systematic approach for automatically compensating for dynamic machining errors based on a new closed-looped machining scheme. The new scheme incorporates these errors, found through in-process inspection, into a modified CAD model or Variational Part Model. As a result, the Variational Part Model inherently contains the online disturbances associated with machining. It is important to note that this new scheme assumes the machine tool s static error (ball screw error, joint misalignment, perpendicularity error, etc.) has been addressed by some other compensating method and this scheme only addresses the dynamic machining error. To create the Variational Part Model, the machined part is measured on the machine and compared to the CAD model s theoretical data. The data is then used in conjunction with modeling functions contained in NX s Application Programming Interface (API) to interact with the CAD model and modify its feature geometry. The validity and effectiveness of the methods are presented as well as results from experimental testing. This thesis also presents the methods necessary for automatic CAM process updating to ultimately close the loop between machining and inspection.

7 TABLE OF CONTENTS CHAPTER 1 Introduction Manufacturing Process CAD/CAM development Post Processing Machining Part Inspection Geometric Dimensioning and Tolerancing Form Tolerancing Orientation Tolerancing Profile Tolerancing Runout Tolerancing Location Tolerancing DirectCMM Project In-Process Inspection DMAC Integrating DMAC and PC-DMIS PC-DMIS Measurement Process Plan GD&T Capabilities DirectCAD Interface Inspection Report Development of the Variational Part Model Identifying part features Dimensional Measurement Usage CAM Process Updating...24 CHAPTER 2 Literature Review...25 vi

8 2.1 Closed-Loop Machining Sources of Machining Error Numerical Errors in Part Programming Static Error Dynamic Error Geometrical Feedback Scheme Computer-Integrated Dimensional Inspection The Open C++ API Object Identifiers Consistent Object Identifiers Interfacing with the CAD/CAM Model Conclusion...36 CHAPTER 3 Method VPM Closed-Loop Machining Scheme VPM Methodology Data Comparison VPM Points Creating a Spline Through Points Creating a Through Curves Feature Replacing the Existing Surface Identifying Part Features CAD Modifications Based on GD&T Modifications to Non-Related Features Modifications to Related Features Updating the CAM Process Creating the Operation Creating the Program Group Creating the Method Group Creating the Geometry Group Creating the Tool Group Hardware Configuration for Testing...67 vii

9 3.6.1 Sugino 3-Axis Mill Probing System...68 CHAPTER 4 Results Physical VPM Test Setup Line Profile VPM Results Surface Profile VPM Results...78 CHAPTER 5 Summary and Conclusions New Error Feedback Routine VPM and CAM Process Updating Validation Through Testing Recommendations...85 Bibliography...87 Appendix...89 viii

10 LIST OF FIGURES Figure 1-1 Typical CAD model with tool paths... 3 Figure 1-2 Allowable ranges the tool may deviate... 3 Figure 1-3 Post processing of tool paths... 5 Figure 1-4 Evaluating the flatness of a planar surface [44]... 9 Figure 1-5 Evaluating the cylindricity of a cylindrical feature [4] Figure 1-6 Evaluating the parallelism of a planar surface [4] Figure 1-7 Example showing a surface profile tolerance zone [4] Figure 1-8 Example of evaluating circular and total runout [4] Figure 1-9 Example of the tolerance zone for concentricity [4] Figure 1-10 Example showing the tolerance zone for true position [4] Figure 1-11 DMAC system architecture Figure 1-12 Flow information from PC-DMIS to DMAC Figure 1-13 Graphical User Interface of PC-DMIS Figure 1-14 PC-DMIS feature dialog box Figure 1-15 Typical inspection report output from PC-DMIS Figure 2-1 Closed-loop machining scheme Figure 2-2 Tool path correction method for closed-loop machining Figure 2-3 Test part used for error feedback validation Figure 2-4 Example showing an edge s object identifier Figure 3-1 New closed-loop machining scheme Figure 3-2 Diagram illustrating the VPM methodology Figure 3-3 Paths/levels the probe takes that makes a row of points Figure 3-4 Creating the VPM points Figure 3-5 Bounding box max/min locations Figure 3-6 Adding a VPM point to the edge of a surface Figure 3-7 Periodic and non-periodic splines ix

11 Figure 3-8 Creating splines through points Figure 3-9 Cross product operation calculation Figure 3-10 Copying splines to the outer edges Figure 3-11 Through curves feature showing outlining curves Figure 3-12 Example showing the replace face modeling function Figure 3-13 DirectCAD Graphical User Interface dialog box Figure 3-14 Dialog boxes from NX and PC-DMIS showing CAD ID s Figure 3-15 Calculation of the distance between a line and a plane Figure 3-16 Sugino 3-axis mill used for testing Figure 3-17 Optical transmission probing system Figure 3-18 Optical Machine Module and Machine Interface Unit Figure 4-1 Part used in Variational Part Model test Figure 4-2 Line profile VPM measured error distribution Figure 4-3 Surface profile VPM measured error distribution Figure 4-4 Creation of the Variational Boundary Surface Splines Figure 4-5 Creation of the through curves feature Figure 4-6 Replacing the old surface with the VPM surface x

12 LIST OF TABLES Table 1-1 Application of geometric control symbols... 7 Table 2-1 Error comparison at various manufacturing points Table 2-2 Face types applicable to a NX CAD model Table 3-1 Sugino V9 specifications Table 4-1 Machining parameters used for tool path generation Table 4-2 Line profile measurements versus theoretical values Table 4-3 Line profile VPM measurements versus theoretical values Table A-1 Surface profile measurements versus theoretical values Table A-2 Surface profile VPM measurements versus theoretical values xi

13 CHAPTER 1 INTRODUCTION With the increasing precision of CNC machining centers and CMM technology, in-process part inspection and closed-loop feedback are being realized by using the process machine as an inspection machine. Machining errors found through in-process inspection generally are adjusted through the alteration of NC tool paths by feeding back error offsets to the CNC controller. The research in Direct Machining And Control (DMAC) at BYU has identified a potential application related to process planning, inprocess part inspection and closed-loop dimensional error feedback. This research will utilize previous research that integrated the CMM software package PC-DMIS provided by Wilcox Associates Incorporated with a DMAC motion controller provided by Direct Controls, Inc. (DCI). This integration is called DirectCMM because it directly links the DMAC controller to PC-DMIS without the need for post processing. To prove that closed-loop dimensional error feedback is possible, techniques will be developed to automatically alter part geometry through the feedback of machining errors directly to the CAD model. The techniques will be implemented and tested inside a computer program that utilizes NX s CAD/CAM API to alter CAD geometry, and update CAM process plans. 1

14 A brief overview of the current methods used in part manufacturing and inspection will be given to more fully understand the DirectCMM project. A short overview of the basic structure of the DMAC motion controller and its integration with PC-DMIS will be discussed. The goals and tasks of this thesis will also be explained. 1.1 Manufacturing Process To take a part from initial design to a finished product requires several steps. They include: CAD/CAM development, post processing, machining, and part inspection. This section will describe how these steps are completed CAD/CAM development Throughout the design process, the design of the part is gradually refined until it is completely defined for manufacturability. To support the development of design, a CAD/CAM (Computer Aided Design/Computer Aided Manufacturing) program such as NX or CATIA is used to create a 3D CAD model. The CAD model contains a theoretical description of the part s form and dimension. In parallel, the CAD model maybe used for functional, structural and thermal analysis using finite element analysis software. Once the CAD model is defined, the manufacturing process plan can be created using the software s CAM application. Inside the CAM application, the machine tool (3- axis, 5-axis, lathe, etc.), proper cutting tools, machining operations (drilling, face milling, etc.), machining methods and geometry to machine are specified and used to generate tool paths (see Figure 1-1). 2

15 Figure 1-1 Typical CAD model with tool paths When a machining method (roughing, semi-finishing, finishing, etc) is chosen, the user enters a couple of machining parameters that are used in calculating the tool paths, feeds and speeds of the chosen geometry. In NX s CAM application, these parameters are called part stock, Intol and Outtol (See Figure 1-2). Figure 1-2 Allowable ranges the tool may deviate Part stock is the amount of material left over after roughing or semi-finishing operations are performed. This parameter is the basic difference between a roughing, semi-finishing, and a finishing operation. Intol and Outtol define an acceptable range the 3

16 tool may use to deviate from the part surfaces (the smaller the values, the more accurate the cut). Intol is the maximum amount by which the tool may penetrate through the surface. Outtol is the maximum amount by which the tool may avoid contacting the surface [1] Post Processing The primary purpose of the CAM application is to generate tool paths and set up the machining parameters needed to manufacture parts. Because there are many different types of machine tools, tool paths generated from the CAM application cannot be sent to a machine to begin cutting. Each machine tool has its own machine controller directing the tool motion and other machining activities. Just as each machine controller differs in hardware, it also differs in software. This means that the tool paths generated in the CAM application must be modified and put in a form in which the machine/controller combination can interpret. This modification of the generated tool paths is called post processing [1]. The post processing of tool paths basically takes two steps. The first step is to convert the tool paths to a list of machine independent commands stored in a CL (cutter location) data file or an APT (Automatic Programmed Tools) data file. These files contain tool path data as well as machining parameters such as feeds and speeds. Even in today s manufacturing industry, APT files are widely used. The next step uses the post processor to convert the APT file to another file format specific to the machine s controller. This newly created file contains machining instructions generally known as M&G code. Figure 1-3 shows the steps involved in post processing. 4

17 Figure 1-3 Post processing of tool paths Machining Once the M&G file is created, it is taken to the specified machine tool for machining. After machining the part, if any errors are discovered in either the process plan or the machined part, the process plan has to be modified. Typically, modifications to the process plan are performed manually at the machine tool by modifying the M&G file, or error offsets are entered into the machine tool s memory to account for tool wear. If any major changes need to be made to the original CAD/CAM model, an entirely new process plan will need to be developed as well as a new M&G file Part Inspection Several new measuring tools have been developed that allow parts to be accurately measured. In the past, when a part was machined, it was either taken to a Coordinate Measuring Machine (CMM) or was measured on the machine tool (in-process part inspection) using a touch probe to check critical dimensions and tolerances. One of the advantages of using a CMM is the ease of inspecting the dimensional and geometrical tolerances of a wide variety of parts. The disadvantage of using a CMM is the fact that the part has to be taken off the machine tool for inspection. Several types of errors found in the machining process can be discovered through the inspection of parts using CMM technology. The errors associated with the machining 5

18 process are categorized in two areas (static and dynamic). Static error is related to the inaccuracy of the machine tool while dynamic error is related to the dynamics of the machining process such as tool deflection, thermal deformation, controller following errors, mechanism compliance, etc. There are many advantages of inspecting parts using a CMM. Tracking trends in the machining process gives the process engineer the ability to make changes when necessary, such as changing the cutting tool or making adjustments for tool wear. Another advantage is being able to perform inspection in a controlled environment conducive to making accurate measurements. These advantages and others are certainly undisputed. The disadvantages associated with the use of CMM s deal mainly with time and energy. When a part is machined it is either inspected before or after the final cut is performed. The part is removed from the machine tool and taken to the CMM. By so doing, the manufacturing process is interrupted and if machining errors are detected, the part will have to either have to be scrapped or re-fixtured on the machine tool again for modifications to be made. This is a major drawback when parts are inspected after final cuts are performed. Additionally, time is spent developing a measurement process plan to measure critical feature dimensions and tolerances. 1.2 Geometric Dimensioning and Tolerancing An important part of inspection is having an understanding Geometric Dimensioning and Tolerancing (GD&T). After a part has been modeled in a CAD system, the CAD model is used in generating an engineering drawing. The engineering drawing is intended to convey the information from the designer to the manufacturer and 6

19 finally to the inspector. It contains all the information necessary to manufacture a part correctly. During inspection, the information contained on an engineering drawing is used to determine if a part is acceptable. A portion of an engineering drawing specifies the permissible deviations of the size and shape of the part. To control these deviations GD&T standards such as the ASME Y standard was developed to provide a system for symbolically defining the geometric tolerance zone within which part features must be contained. The geometric tolerance zones control the features geometric form, orientation, position and size limits. It is suggested that a more in depth understanding of GD&T practices and applications be studied to completely understand the methods used in this research. This section will give a brief introduction to the five basic types of geometric control (form, orientation, profile, runout and location [2]). Table 1-1 shows the five types of geometric control, their respective symbols and applications [3]. 7

20 Table 1-1 Application of geometric control symbols Form Tolerancing Form tolerances control the flatness, straightness, circularity and cylindricity of individual features or elements of individual features. Form tolerances also specify the maximum permissible deviation from the desired form and apply to all points on the surface. A brief description of each form tolerance is given below. [2] Flatness is a condition in which all elements of a planar surface lie in one plane. The tolerance zone for flatness is two parallel planes separated by the specified tolerance as shown in Figure

21 Figure 1-4 Evaluating the flatness of a planar surface [44] Straightness is a condition in which the elements of a surface, median line, or feature axis are a straight line. The tolerance zone for straightness is either two parallel lines, or a cylinder in which the feature axis must lie. Circularity is a condition of a circular line or the surface of a circular feature in which all points on the line or circumference of plane cross section of the feature are the same distance from a common center point or axis. The tolerance zone is specified by two concentric circles surrounding the center point or axis. Cylindricity is a condition in which all points of a surface, radially or longitudinally, are the same distance from a common axis. The tolerance zone is specified as two concentric cylinders surrounding the feature axis as shown in Figure

22 Figure 1-5 Evaluating the cylindricity of a cylindrical feature [4] Orientation Tolerancing Orientation tolerances exist to control the angular relationship between two or more lines, surfaces, or other features. The geometric characteristics include: angularity, parallelism, and perpendicularity. Each of these is briefly discussed below. Angularity is a condition in which a surface or axis is at a specified angle relative to a datum plane or axis. The tolerance zone is made up of two parallel planes at a specified angle from a datum plane or axis. Parallelism is a condition of a surface equidistant at all points from a datum plane. The tolerance zone is defined by two parallel planes, lines or a cylinder parallel to a datum plane or axis as shown in Figure 1-6. Perpendicularity is a condition of a surface at 90 to a datum plane or axis. The tolerance zone is defined by two parallel planes, lines, or a cylinder perpendicular to a datum plane or axis. 10

23 Figure 1-6 Evaluating the parallelism of a planar surface [4] Profile Tolerancing Profile tolerancing describes the outlining shape or form of a line or surface. Two geometric characteristics fall under this category. They are: profile of a line and profile a surface. Each of these is briefly discussed below. Profile of a line is a condition in which line/arc elements follow the true profile (outline) of a given surface. The tolerance zone is composed of two parallel boundaries (lines/arcs) disposed about the true profile of the given surface. Profile of a surface (shown in Figure 1-7) is a condition in which all elements are contained within the true profile (outline) of a given surface. The tolerance zone is composed also of two parallel boundaries disposed about the true profile of the given surface. 11

24 Figure 1-7 Example showing a surface profile tolerance zone [4] Runout Tolerancing Runout tolerances are used to control the functional relationship of one or more features of a part to a datum axis. The features controlled by this type of tolerance include: surfaces constructed around a datum axis and those constructed perpendicular to a datum axis. Typically, when inspected, the part is rotated 360 about the feature s datum axis. There are two types of runout control, circular and total runout. Each of these is briefly discussed below. Circular Runout is a type of control for circular elements of a surface. As the part is rotated, the circular line elements along the surface must be within the specified tolerance. The tolerance zone is specified by two concentric circles separated by the specified tolerance and coaxial with the datum axis as shown in Figure 1-8. Total Runout is concerned with deviation from perfect rotated form. As the part is rotated, all measured elements along the surface must be within the specified tolerance. 12

25 The tolerance zone is specified by two concentric cylinders separated by the specified tolerance and coaxial with the datum axis as shown in Figure 1-8. Figure 1-8 Example of evaluating circular and total runout [4] Location Tolerancing Location tolerances deal primarily with locating geometric features of size relative to datum lines, axes, or planes. The location tolerances are: concentricity, symmetry and true position. Concentricity is a condition in which two or more features have a common center or axis. The tolerance zone is specified by a cylinder with a diameter equal to the tolerance and whose axis coincides with a datum axis as shown in Figure

26 Figure 1-9 Example of the tolerance zone for concentricity [4] Symmetry is a condition in which the median points of two or more opposing surfaces are coincident with the axis or center plane of a datum feature. The tolerance zone is specified by two parallel planes separated by the specified tolerance. True Position is a condition that exactly locates a point, line or plane (usually a feature s center location) in relationship to a datum reference. The tolerance zone is a specified area in which the center, axis, or center plane of a feature is permitted to vary from its theoretical true position as shown in Figure

27 Figure 1-10 Example showing the tolerance zone for true position [4] 1.3 DirectCMM Project The research in Direct Machining and Control (DMAC) at BYU recently proved that the DMAC motion controller can switch from being driven by a machining process to being driven by a measurement process. This allows machine tools to easily be used during the manufacturing process as coordinate measuring machines. This section will discuss the important research developments pertinent to this technology referred to as the DirectCMM project In-Process Inspection While the advantages of using a Coordinate Measuring Machine are undisputed, advances in technology have made it possible to measure parts on the machine tool while it is still fixtured. This type of measurement is called in-process inspection. The most significant advantage of in-process inspection is being able to monitor trends in the 15

28 machining process while the part is fixtured to the machine tool. This ultimately saves money by eliminating the time and labor associated with moving the part to the coordinate measuring machine and back. Other advantages include reduced manufacturing costs, and ultimately being able to directly update process plans when errors are discovered through measurement. The main disadvantage that current in-process machine tools deal with is the issue of machine control. Most current machine tool controllers do not have the capability needed to drive measurement commands. An example of this is the command to move until the controller detects a hit. Machine controllers used today have to be modified to contain this unique capability, which is extremely difficult [5] DMAC An important development of this research project is that of Direct Machining And Control (DMAC). The DMAC controller is an open architecture, software based controller, which controls the motion of target, joint and path moves defined by lines, arcs, or NURBS. The open architecture allows any controlling software package (that can provide suitable motion commands) to connect to the DMAC system (Figure 1-11). 16

29 Figure 1-11 DMAC system architecture The DMAC system is divided into three layers - CAD/CAM/CMM application, Motion Planner, and Servo Controller. Inside the CAD/CAM program, motion commands and settings such as feed rate, spindle speed, etc. are accessed from the CL/APT file and passed to the Motion Planner through the Direct Machine Interface. In short, the Motion Planner uses its own trajectory generator and inverse kinematic routines to generate position, speed, acceleration, and jerk values. These parameters are then converted into torque values and sent to the Servo Controller to perform the functions needed to drive the machine s actuators. A more in depth look at the DMAC Motion Planner architecture and Servo Controller can be found in [6] and [7]. The four main areas of research addressed by the DirectCMM Project are: connecting DMAC to PD-DMIS, development of a standard CMM interface for DMAC, 17

30 handling measurement data, and automatic CAM process updating. These topics are described below Integrating DMAC and PC-DMIS For any controlling software such as PC-DMIS to interface with the DMAC system, a generic interface/driver for controlling any particular CMM had to be created. Previously, Wilcox Associates, Inc. (WAI) had to create an interface for each of their customer s CMM s because each CMM is different. Luckily, the software developers at WAI were willing to work with BYU to create this generic driver. A diagram showing the generic driver, WADriver.dll, as well as the general flow of information from PC- DMIS to DMAC can be seen in Figure 1-12 [8]. Figure 1-12 Flow information from PC-DMIS to DMAC The generic driver interprets the generic commands issued by PC-DMIS and issues the commands expected by any particular CMM. The generic driver provides an open architecture interface that allows the DMAC controller to connect to PC-DMIS. A companion driver, WAILLDriver.dll, was written by a research student at BYU to connect the DMAC controller to the generic driver. This driver exposes certain controlling CMM functions that the generic driver looks for to send back to PC-DMIS. These functions are described by a document provided by Wilcox Associates, Inc. The WAILLDriver.dll also 18

31 exists to account for the differences in the way PC-DMIS and DMAC describe its movements. Each is described in a different format [8]. Once the WAILLDriver receives the movement commands, they are passed to the DMAC controller through a COM interface called icmm. The icmm interface is used for passing motion commands to DMAC and sending and receiving other information [8]. 1.4 PC-DMIS PC-DMIS is the world s leading metrology software produced by Wilcox Associates, Inc. It translates the high-level measuring commands into detailed steps necessary to drive a coordinate measuring machine. These steps are written in a modern machine independent language called DMIS (Dimensional Measurement Interface Specification). PC-DMIS can read, write, and execute a DMIS program in real time or in simulation. The DMIS program (process plan) lists the necessary commands to measure features, create alignments, and define hardware. This section will give an overview of process plans developed within PC-DMIS, the Geometric Dimensioning and Tolerancing (GD&T) capabilities, the DirectCAD interface, and inspection report [9] Measurement Process Plan Two methods are used in creating a measurement process plan. One method is to measure part features by manually moving the CMM around. The other is to use an imported CAD model and interactively select part features to measure. This method allows the user to prepare an automated inspection program. The steps involved are very similar to the development of a manufacturing process plan. They include: importing a part, defining a touch probe, creating a coordinate system (part alignment), and selecting 19

32 features to measure. Figure 1-13 shows the graphical user interface of PC-DMIS and a feature being measured in simulation. [9] Figure 1-13 Graphical User Interface of PC-DMIS GD&T Capabilities PC-DMIS allows the user to measure part features according to Geometric Dimensioning and Tolerancing (GD&T) specifications. The dimensioning possibilities in PC-DMIS include that of calculating distances and angle between features. The types of tolerancing available in PC-DMIS include: form, profile, orientation, location, and runout. The methods used to perform geometric dimensioning and tolerancing in PC- DMIS conform to the principles and guidelines provided in the ASME Y14.5M-1994 national standard. 20

33 1.4.3 DirectCAD Interface PC-DMIS, like most geometric measurement software today can import a graphical representation of the part such as an IGES or STEP file. The software package then uses this file and performs translations to display its geometry. When doing so, the geometric model may lose its feature associativity and also geometric accuracy due to errors in translation. PC-DMIS has a feature called the DirectCAD interface that reduces the errors associated with translation of data from CAD systems into PC-DMIS s internal CAD format. It uses the CAD system's native mathematical routines to obtain requested information. It also uses the CAD system's native Application Programming Interface (API) to access the CAD database to display, and interact with its own geometry. This capability enables PC-DMIS to accurately display and provide necessary information related to the feature model, such as surface topology, feature locations, and object identifiers. Figure 1-14 shows a PC-DMIS dialog box with information related to the feature model [9]. Figure 1-14 PC-DMIS feature dialog box 21

34 The object identifiers (ID) PC-DMIS displays exactly matches the CAD model s object identifiers. This is very useful when implementing NX API functions to change feature parameters. The object identifiers PC-DMIS is able to display are sketch entities (points, lines, circles, arcs, and curves). Currently, PC-DMIS doesn t display the following object identifiers: faces, edges, cylinders, cones, spheres, slots, and bosses. However, this type of capability is just a matter of implementation Inspection Report Once a feature has been measured, the inspection report can be generated. The inspection report is used to print out theoretical and measured values of the measured part features. A graphical report can also be printed out for analysis. The inspection report enables the inspector to visually analyze measurement data in text format. An example of a typical inspection report is shown in Figure Figure 1-15 Typical inspection report output from PC-DMIS 22

35 The first section next to SCN1 describes the measured feature; in this case, a linear-open scanning procedure (shown in red) was performed to measure a line along a surface. The word HIT/VECTOR specifies a point to be measured while scanning the part surface. The first three numbers, to the right, show the theoretical location (x,y,z) of the points. The next three numbers show the orientation (i,j,k) and the last three numbers show the measured location of the points. The section under LIN3 is a best-fit line construction procedure (shown in red) to put the scanned feature in a form that a GD&T routine can understand. The GD&T routine in this case is the straightness of a line. The section next to DIM describes the dimension s name (STRA1), type of dimension (STRAIGHTNESS), and the feature being dimensioned (LIN3). The last line contains the nominal and measured values, tolerances and out-of-tolerance value. 1.5 Development of the Variational Part Model The main objective of this thesis is to automatically update CAM process plans by programmatically creating a Variational Part Model and updating the CAM process when geometric dimensions/tolerances are violated. This section will outline the goals and methods used in accomplishing this task Identifying part features Due to the fact that PC-DMIS is only able to display and identify sketch entities (points, lines, arcs, and curves) in its DirectCAD Interface, an interactive approach to performing this same procedure will be developed inside NX. The NX API functions available for querying features and their respective object identifiers will be used in conjunction with a Graphical User Interface (GUI) developed specifically for this 23

36 research. This will provide a temporary solution to PC-DMIS s shortcomings. If the work performed in this thesis becomes beneficiary to Wilcox Associates, Inc., the implementation could be performed very easily Dimensional Measurement Usage After machining, the part will be inspected for compliance to geometric dimensioning and tolerancing specifications. When geometric dimensions/tolerances are violated, the inspection report will indicate which features need to be modified. This thesis will discuss what the pertinent data needed from the inspection report is and its usage. It also will develop the techniques necessary to create a Variational Part Model by modifying part geometry with the use of the measurement data. These techniques will be implemented in a computer program linked to NX CAM Process Updating After the Variational Part Model is produced, the CAM process plans will be unusable due to the changes in the CAD model. For example, a planar machining operation is no longer valid if its associative geometry is changed to a non-planar surface. The machining operation would have to be modified to reflect the new geometry. The methods used to accomplish CAM process plan updating will be discussed and implemented inside the computer program. 24

37 CHAPTER 2 LITERATURE REVIEW The idea of closed-loop machining has been a critical research topic over the past 15 years. In the past, when a part was machined, it was measured using various gages, taken to a coordinate measuring machine (CMM) or was measured on the machine (inprocess part inspection) using a touch probe to measure critical dimensions and to perform statistical error analysis. This section will discuss key research topics related to closed-loop machining, error compensation techniques and CAD/CAM process updating. 2.1 Closed-Loop Machining Closed-loop machining is basically a system for manufacturing parts with automatic compensation of machining process errors such as worn tools, thermal deformation and other process variations [10]. Figure 2-1 shows the steps involved with the closed-loop machining scheme: 1) to take a part modeled in a CAD/CAM system such as NX, 2) generate tool paths, 3) machine the part, 4) perform inspection, and 5) accept the part or re-machine the part when dimensions become out-of-tolerance. 25

38 Figure 2-1 Closed-loop machining scheme For quite some time now, the closed-loop machining scheme has incorporated the concept of in-process machining and inspection while the part is fixtured on the machine tool. Zhou et al. describes in-process part inspection (in-cycle measuring) and its many advantages [11]: In-cycle measuring (ICM) may be described as the automatic measurement or gauging of a component while it is clamped in the machining position. The on-line measured data are fed back to the machine controller and used as error compensation for workpiece dimensions. ICM has been claimed as a strong tool for automation of the production processes where small to medium batch work is applied. It is, therefore, expected to maximize efficiency and minimize scrap in production. The biggest advantage of the closed-loop machining scheme is being able to monitor process variations and make corrections to the manufacturing process when needed. The ultimate goal is to have 100% machined parts accepted after inspection. The difficulty is that machines are not 100% accurate. Thus process control is extremely important to the success of the company. When in-process machining and inspection is included, closed-loop machining practices allow adjustments to be made dynamically as 26

39 parts are being machined, thus improving part precision and reducing the amount of scrap. 2.2 Sources of Machining Error There are many sources of error in current CNC machining procedures. Various numerical errors occur during CAM part programming procedures such as tool path generation. The machine tool itself has inaccuracies and while machining, errors arise from tool deflection, tool wear etc. These errors cause the machined part to deviate from the desired model. The minimization of these errors has been one of the crucial topics in the CAD/CAM industry. This research deals strictly with compensation of dynamic machining errors for non-thinned walled parts. It assumes parts are left fixtured to the machine tool for inspection and does not compensate for residual stresses that become apparent after parts are removed from their fixtures. This section will discuss previous research related to the various sources of machining error Numerical Errors in Part Programming The accuracy of the finished part is almost entirely dependent on the tool paths generated by the CAM system. The goal of the CAM system is to provide a sufficient number of cutter location data that will produce the part with an allowable amount of error. In general, the greater number of cutter locations, the more precise the part will be manufactured. When tool paths are generated, the cutter location points are provided in a discrete manner. In other words, errors may propagate and are unavoidable due to the point-to- 27

40 point operations of the CNC machine. Some of the errors likely to emerge are interference with the fixture, gouging and under cutting. To compensate for these errors external computer simulation software packages have been developed to check for machining errors developed by other CAD/CAM systems. A CAD/CAM systems simulation module only checks its internal CAM files for verification Static Error All machine tools inherently possess some type of error. A Machine tool s inaccuracy is called static error. Depending on the type (3, 4 or 5 axis) of machine tool, errors in roll, pitch and yaw develop over time and need to be monitored frequently to ensure the quality of manufactured parts. To compensate for static error, researchers have developed an analytic compensation procedure called volumetric error modeling. For a 3- axis machine tool, the compensation procedure corrects for 21 component errors consisting of six error components along each axis and three squareness errors. Measurements of each error are accomplished by using a laser interferometer. To account for the roll errors, an electronic level is used for measurement. This approach is limited however, because the measurements are obtained while the machine tool is load free and does not account for errors occurring during the machining process. [3][12] Dynamic Error Machining process disturbances occurring during the machining process are called dynamic error. Examples of such include: tool deflection, thermal deformation, controller following errors, mechanism compliance, residual stresses, etc. Many 28

41 researchers have attempted methods to compensate for such errors [13-17]. They have also tried to incorporate analytical modeling techniques to model cutting forces, chatter, vibration, heat deformation and tool deflection but have fallen short because the models are not sufficient enough for reflecting the real phenomenon which occurs during machining [12]. In industry today, dynamic error compensation remains a manual process. The technique used mostly is to correct for tool wear. To do so, an operator checks a machined part using various gages or CMM, and then manually enters a tool compensation value into the machine s CNC controller. With higher volumes of parts being produced and even lower volumes, this method takes up too much time and energy. 2.3 Geometrical Feedback Scheme One of the more advanced methods used today for in-process part inspection developed by researchers recently is to make comparisons with the actual CAD model and measured points to update tool paths (Figure 2-2). In the proposed scheme, the machined part is: (1) measured on the machine, (2) compared with the CAD model, and (3) the tool path is corrected repeatedly until the predefined geometric accuracy is obtained. The execution and correction method can be viewed as an iterative approach. The critical steps (2 and 3) involve taking measured data points and adjusting the NC tool paths stored in the nominal CL data file to reflect machining error [12]. The scheme also compensates a machine s static error with continuous monitoring using a laser interferometer and ball bar system. 29

42 Figure 2-2 Tool path correction method for closed-loop machining To illustrate the method, suppose a set of coordinates is obtained by scanning a machined boundary. This data is then compared with the CAD model s surface data. The deviation at each measured point is computed by the distance between a point and a line. This deviation is then used in offsetting the old tool path s closest CL data point. The steps described are calculated as shown below in Equation 2.1. New CL path = Current CL + ( Desired contour Measured profile) (2.1) path Testing of the geometrical error feedback routine was conducted using an aluminum part with the configuration shown in Figure 2-3. The test included the following cutting conditions: HSS end mill, cutting width of 2.5 mm, cutting depth of 4 mm, feed rate of 60 mm/min, and a spindle speed of 900 rpm. Various points along the 30

43 test part were measured as shown in Table 2-1. The results are very significant. The average error (distance between the theoretical and measured values) without compensation measured mm. After compensation (first iteration), the average error measured mm. [18] Figure 2-3 Test part used for error feedback validation Table 2-1 Error comparison at various manufacturing points Theoretical values Measured values without feedback Measured values with feedback X (mm) Y (mm) x (mm) Y (mm) Error (mm) x (mm) y (mm) Error (mm) P P C r P P P P The geometrical error feedback routine showed a significant improvement (79.7% reduction in error) in the precision of the machined part after the first iteration. The results indicate that the approach can be used as a means for correcting both static and dynamic machining process disturbances without having to count on the analytical modeling techniques. The proposed scheme is also meaningful in that it can be 31

44 implemented as a feedback mechanism for geometric control. Although this method compensates for the static and dynamic error, the error adjustments were applied to the NC tool paths instead of the feature model. The problem with this method is the adjusted tool paths are no longer associated with the CAD model s geometry. 2.4 Computer-Integrated Dimensional Inspection Computer-integrated dimensional inspection is a key component in a manufacturing environment. Current development in computer-integrated manufacturing has shown a continuous trend towards achieving higher levels of automation in dimensional inspection. Currently, in a computer-integrated manufacturing (CIM) environment, CAD/CAM systems integrated with CNC machines successfully facilitate the design and manufacturing to a high degree of automation. Dimensional inspection is linked to design and manufacturing through dimensional software programs such as PC- DMIS. Within these software programs, the functionality to analyze geometric dimensions and tolerances is available. [19] Because many geometric tolerance controls involve datums, the programs have integrated the functionality to construct datum reference features based on measured data. The programs compare the measurement data of an actual feature with its nominal design as well as with the constructed datum feature. Four pieces of information are required to make this comparison: geometric information of the nominal design; measurement information of the actual feature; measurement information of the datum feature(s); and the type of geometric tolerance control. To adequately represent a datum feature, a sufficient number of discrete probing points are required. Inspection software programs use best-fitting techniques to construct 32

45 datum features. These techniques use nonlinear least square minimization approaches to best fit the datum features to their discrete measurement data and determine the feature s position, orientation, and/or size. The least squares approximations are applied to the two types of datums (planar and cylindrical). [19] Tolerance zones are also mathematically defined using the same least squares methods. The objective is to provide a definite mathematical form to the tolerance zone so that the computer can automatically make a comparative analysis based on a specified geometric control tolerance. [19] 2.5 The Open C++ API The current technology of CAD/CAM systems allows users to access the system s database and use its application programming interface (API). By programmatically interfacing to the CAD/CAM system, the user is able to perform things not available in its current state. This section discusses some of the concepts surrounding a CAD/CAM systems API (in particular NX) and part model to aid users in accessing and modifying objects embedded within a part file Object Identifiers A CAD/CAM system models its features in a variety of ways, depending on the purpose of the feature and its relationship to other features. The features may be design oriented, drafting oriented, analysis oriented or manufacturing oriented. In each case, the features have a specific object identifier that uniquely identifies the feature when it is loaded into memory. In NX, these object identifiers are called tags. Their physical representation is an integer value. To use any of the user functions available inside a 33

46 particular API, the user needs to have access to these object identifiers. Figure 2-4 shows a part s edge and the edge s respective tag. Figure 2-4 Example showing an edge s object identifier In the case of a NX session, each of the objects have their own unique tag, however, the tag is not consistent between sessions. This means that between sessions, the tags may have different values assigned to them. In addition, the tags can be reused within a session. For example, if a CAD feature was created then deleted, the feature s tag can be reassigned to a different feature at a later point in the same session. The thing to remember is that while the tags may have different values between sessions, the feature associated with the tag is consistent. [1] Consistent Object Identifiers As was mentioned previously, tags are not consistent between sessions nor are they consistent within a session. To overcome this limitation, NX provides what are called handles as an alternate method of consistently referencing features in a session. A handle is simply a string that contains information about the object as well as the objects part (i.e. RMform.prt R ). This enables the feature s tag to be determined in a later session. [1] 34

47 As can be seen in the example above, the handle is composed of a part called form.prt. The preceding two letters, RM, refer to the type of object being referenced and the numbers at the end are unique to the feature. A feature s handle is determined using the user function UF_TAG_ask_handle_of_tag(). The handle is also used to determine the feature s current tag using the user function UF_TAG_ask_tag_of_handle(). [20] Interfacing with the CAD/CAM Model The major CAD/CAM systems of today have recognized the benefits of an open architecture API. They allow users to programmatically interface with a CAD/CAM model. Each of the system s APIs provide the functionality that allows custom built programs to access information from the CAD/CAM model. The following modeling function from NX s Open C++ API is a good example of the functionality available to interact with a CAD/CAM model [20]. UF_MODL_ask_face_type ( tag_t face, int * type ) This user function has the specific purpose of asking the type of a NX face. The first object in the function is the face s object identifier, specified by face, and the second object is the face s type. When this function is utilized, the specific type of face is returned in type as an integer value. The user function would return one of the following types [1] listed in Table 2-2. The respective integer value is also shown for clarification. Table 2-2 Face types applicable to a NX CAD model Type of face Integer value UF_MODL_CYLINDRICAL_FACE 16 UF_MODL_CONICAL_FACE 17 UF_MODL_SPHERICAL_FACE 18 UF_MODL_TOROIDAL_FACE 19 UF_MODL_SWEPT_FACE 20 UF_MODL_PLANAR_FACE 22 35

48 Table 2-2 (continued) UF_MODL_BLENDING_FACE 23 UF_MODL_PARAMETRIC_FACE 43 UF_MODL_OFFSET_FACE 65 UF_MODL_FOREIGN_FACE 66 An example of using a CAD system s Open C++ API is that of PC-DMIS. As was mentioned in the Section 1.4.3, PC-DMIS s DirectCAD interface uses the CAD system's API to request information pertaining to the CAD model. In particular, the information focused on in this research is the object identifiers which PC-DMIS displays in its feature dialog boxes. 2.6 Conclusion While the need for a fully automated closed-loop machining scheme is real, industry is still performing manual feedback routines. After machining errors such as tool wear are discovered, machine operators manually enter tool compensation values into the machine s CNC controller. The inability to compensate for machining error generated during the manufacturing aspect of the closed-loop machining scheme have driven researchers to develop new compensation techniques. One such researcher developed an iterative feedback routine to adjust tool paths by comparing the measured profile with the tool path profile. Although this method showed improvements, by changing the tool paths, the associativity of the CAD/CAM model no longer exists. The advancements of CAD/CAM technology have made it possible for users to access the CAD/CAM system s database by allowing free access to the systems API. This enables users to make modifications to a CAD/CAM model. The critical component 36

49 needed to do so is the object s identifier or tag. With the appropriate identifier, user functions can be used to query the CAD database and make modifications. With this knowledge, and the developments of PC-DMIS with its DirectCAD interface, the direct link to obtaining these identifiers has been made possible. 37

50 38

51 CHAPTER 3 METHOD To automatically correct machining errors through closed-loop feedback, techniques were developed and implemented in a NX plug-in (computer program run from inside NX). The techniques developed take measurement information from PC- DMIS s inspection report and use them to create the Variational Part Model (VPM). Development was performed using a computer program running inside NX with hypothetical measurement data. Final testing was performed on a 3-axis machine tool that performed both the machining and measurement tasks. This chapter will describe in detail the method and techniques used to automatically create the VPM and update the CAM process plan. 3.1 VPM Closed-Loop Machining Scheme A new closed-loop machining scheme was developed with the addition of the VPM. The VPM is basically a copy of the original CAD model with slight modifications made to its geometry to account for dynamic machining error. Thus any changes made to the original CAD model would have to be made prior to machining. The following in-process machining, inspection and error feedback routine shown in Figure 3-1 shows where the VPM fits into the closed-loop machining scheme. After machining, the part is inspected and its geometric dimensions and tolerances are 39

52 evaluated. In so doing, when the CMM software reports errors, modifications are automatically made to a VPM and the process plan updated. The newly created VPM inherently possesses the machine s dynamic machining error. When the part is remachined, a more accurate part is manufactured, thus eliminating scrap. Figure 3-1 New closed-loop machining scheme 3.2 VPM Methodology The goal of this research is to develop the methods and techniques to modify part geometry by using measurement data. The modifications are made possible by using a CAD/CAM system s API. The API contains the modeling functions available to users to write customizable software programs. Examples of modeling functions include: creating points, lines, arcs, cylinders, blocks etc. Even the more advanced operations are available like creating surfaces with the through curves function. This section discusses the methodology used to create the VPM and describes each of the modeling functions used in this research provided by NX [20]. Figure 3-2 illustrates the VPM methodology. 40

53 Figure 3-2 Diagram illustrating the VPM methodology The general idea is to first take the part s measured data and compare it to the part s theoretical data. This is accomplished by measuring part surfaces with an inspection software program such as PCDMIS. The data is then fed into a software program created in this research and stored in a usable format. The second task is to take the data and create points that represent the new VPM surface. Third, a series of splines are created through the VPM points. The splines are then used in conjunction with a through-curves feature operation. This feature is called a sheet body- a body with zero thickness, made up of a collection of one or more faces that do not enclose a volume. The final task is to replace the existing surface with the new, through-curves sheet body. 41

54 3.2.1 Data Comparison When PCDMIS reports a dimensional or geometric out-of-tolerance condition, the inspection report is fed into the software program created for this research. The software program is executed inside a NX plug-in. As NX is opened, the plug-in is loaded and placed on the menu bar. The plug-in contains an interactive Graphical User Interface (GUI) called DirectCMM that allows the user to select the inspection report and run the program. The actual data comparison is performed inside this program. The first part of the program searches the inspection report for data, stores the data and then compares the data. Comparisons between the measured and theoretical values are made to determine what the VPM should look like. At each measured data point, the distance between each of the measured points and their corresponding theoretical points is calculated. This calculation (Equation 3.1) describes how far each point along the surface deviates from its intended location. ( x x ) + ( y y ) 2 + ( z z ) 2 meas 2 theo meas theo meas theo Distance = (3.1) When a part is measured, the probe usually is programmed to travel along a straight path to take a series of hits. Each straight path taken by the probe is considered a row. When circular objects are measured, the probe is positioned at a certain height/level and moves around the object taking a series of hits. In this instance, at a certain level, a series of hits is considered a row. Most of the time, multiple paths/levels are taken by the probe to measure a surface. Figure 3-3 shows the path the probe takes to measure different surfaces. 42

55 Figure 3-3 Paths/levels the probe takes that makes a row of points VPM Points To create the VPM points, an offset (distance calculated in Section 3.2.1) is applied to each of the theoretical points. The directions of the applied offset are the directions the probe travels to take hits. These directions are also the surface normals at each point. The inspection report contains the surface normals. The software program searches for these values as well and are stored for later use. These offset points become the VPM points. The software program doesn t actually create points, however, the point s locations are calculated and stored for later use. Figure 3-4 illustrates how the VPM points are created. 43

56 Figure 3-4 Creating the VPM points After the VPM points are calculated, two additional points are added to each row of points. One point is added to the beginning and another to the end. These points are calculated to ultimately be located on the edges of the surface. They are intended to make sure the entire surface is modeled and appropriately represented. To create these points, the theoretical locations on the edges as well as the surface normals are needed. To obtain the needed information a few API modeling functions are accessed. The first function called obtains the surface s maximum and minimum locations that bound the surface. These locations theoretically construct a box wherein the surface resides. Figure 3-5 shows a surface s bounding box. Figure 3-5 Bounding box max/min locations 44

57 The API modeling function used to obtain these max/min locations is called UF_MODL_ask_bounding_box( ). The function has one input, object, which is the object identifier. The output, bounding_box[6], contains the max/min locations. The minimum x,y,z location is the first 3 values and the maximum x,y,z location is the last 3 values. The function is shown below. UF_MODL_ask_bounding_box ( tag_t object, double bounding_box[ 6 ] ) The second API modeling function used returns a point on a surface given a reference point. The point on the surface is actually expressed as a u,v parameter. This parameter describes the point s location on the surface. The function is called UF_MODL_ask_face_parm( ) and is shown below. UF_MODL_ask_face_parm ( tag_t face_id, double * ref_pnt, double * parm, double * face_pnt) The function has two inputs (face_id, and ref_pnt). The face_id is the surface s object identifier and ref_pnt is a reference point. The reference point is used to locate the u,v parameter (parm), an output. The u,v parameter is the closest location on the surface to the reference point. The calculation of the reference point will be discussed later. The other output (face_pnt) contains the x,y,z location of the point on the surface described by the u,v parameter. The calculation of the reference point involves using the row s first and last theoretical points, the max/min locations of the bounding box and a dot product operation. To be simplistic, the row s first and last theoretical points will be referred to as 45

58 row-end-points. The dot product is used to find the perpendicular distance from the rowend-points to the max/min locations. Two vectors are needed in the dot product calculation. The first is a unit vector that describes the probe s direction of travel as it moves along the row of points. It is calculated by subtracting the two row-end-points. The second is the vector from one of the row-end-points to the max/min location. A reference point is calculated by offsetting one of the row-end-points by the smallest calculated distance obtained through the dot product operation. The direction of the offset is the unit vector describing the probe s direction of travel. Offsetting in this direction allows the entire row of points to be aligned in the same direction. With the surface point (face_pnt) acquired, the next step is to obtain the point s surface normal. The API modeling function used to accomplish this is called UF_MODL_evaluate_face( ). The function output is a pointer to the data structure containing the needed surface normal. The function is as follows: UF_MODL_evaluate_face( tag_t face_tag, int deriv_request, double parms[2], UF_MODL_SRF_VALUE_p_t eval_result) The function has three inputs (face_tag, deriv_request, and parms[2]). The first input, face_tag, is the object identifier. The second input is used to specify what type of derivative is to be computed. In this case, the desired derivative is the unit normal. To specify this, deriv_request is set equal to UF_MODL_EVAL_UNIT_NORMAL. The third input, parms[2], is the u,v parameter value that was obtained previously. With all the needed information, the two additional points can be calculated and added to the series of VPM points. To calculate the new points, the same offset applied to 46

59 the row-end-points is applied to the new points as shown in Equation 3.2. This research assumes points are measured close (within.05 mm) to the edges, thus supporting the idea that the offsets would be equal. Figure 3-6 shows the addition of a VPM point to the edge of a surface. new_pnt = (3.2) x, y,z face_pnt x,y,z ± dist surf_normi, j,k Figure 3-6 Adding a VPM point to the edge of a surface Creating a Spline Through Points The next step is to create a spline through each row of VPM points. The API modeling function, UF_CURVE_create_spline_ thru_pts( ), allows the user to create a spline, which passes through a number of points specified by the user. The function call has a number of necessary inputs and outputs the object identifier. The function call is specified as follows: UF_CURVE_create_spline_thru_pts ( int degree, int periodicity, 47

60 int num_points, UF_CURVE_pt_slope_crvatr_t point_data[ ], double parameters[ ], int save_def_data, tag_t * spline_tag) As can be seen, the spline s degree, periodicity (periodic or non-periodic), and number of points are inputs to this function. Figure 3-7 shows the two types of splines (periodic and non-periodic). Figure 3-7 Periodic and non-periodic splines The next input, point_data[ ], is specified inside the data structure UF_CURVE_pt_slope_crvatr_t and contains the point s x,y,z locations, and the slope and curvature of the spline. The input, parameters[ ], is used to parameterize the spline. The input, save_def_data, is used to save the defining data with the spline and finally the last part of the function is an output, spline_tag, which is the object identifier. Example I located in the Appendix shows the coding used to create a series of splines as well as the values used for the functions inputs. Figure 3-8 shows the creation of three splines through their corresponding row of points. 48

61 Figure 3-8 Creating splines through points Since the goal is to completely represent the entire surface, two additional splines are created at the outer edges. The splines created at the outer edges are actually copies of the edges nearest splines. This operation is carried out first by performing a dot product operation to calculate the distance from each edge to the nearest spline. Each of the spline s points are copied and translated to the edge s border. The dot product calculation uses the vector from the max/min location to a row-end-point and the unit vector perpendicular to the probe s direction of travel. The unit vector is calculated using a cross product operation and the right-hand rule. The cross product uses the probe s direction of travel along the path and the probe s orientation (see Figure 3-9). The cross product gives the vector perpendicular to the other two vectors. Figure 3-10 shows the two additional splines translated to each edge. 49

62 Figure 3-9 Cross product operation calculation Figure 3-10 Copying splines to the outer edges Creating a Through Curves Feature The next step is to create a surface that encompasses each of the splines created in the previous step. The API modeling function used to perform this step is called 50

63 UF_MODL_create_thru curves( ). This function allows the user to create a sheet body through a collection of curve outlines. The curve outlines are called section strings. The section strings can either be a curve, edge, or a face. The function call is shown below. UF_MODL_create_thru_curves ( UF_STRING_p_t s_section, UF_STRING_p_t s_spine, int * patch, int * alignment, double value[ 6 ], int * vdegree, int * vstatus, int * body_type, UF_FEATURE_SIGN boolean, double tol[ 3 ], tag_t c_face_id[ 2 ], int c_flag[ 2 ], tag_t * body_obj_id ) The first two inputs, s_section and s_spine are associated with data structures that contain the curve outlines. The curve outlines in this research are the splines created in the previous step. The other defining inputs include: the type of patch, alignment, alignment data (value[6]), degree of surface, periodic status of surface, type of body, boolean operation, tolerances, neighboring surface identifiers, constraint flags, and the object identifier of the through curves feature. Example I located in the Appendix contains the coding used to create the feature as well as the values for the function inputs. Figure 3-11 shows the creation of the through curves feature. 51

64 Figure 3-11 Through curves feature showing outlining curves Replacing the Existing Surface The final step is to replace the old surface with the new surface. The UF_MODL_create_replace_ face( ) modeling function allows the user to replace a set of faces with another face. The function call is as follows: UF_MODL_create_replace_face ( tag_t * target_faces, int num_target, tag_t * non_blend_faces, int num_non_blend, tag_t tool_face, logical reverse_direction, tag_t * feature_tag ) The critical inputs are the target_ faces, which represent the faces that will be replaced and the tool_face, which represents the new face. The other inputs include: the number of target faces, the non-blended faces, the number of non-blended faces, the direction of the operation and the object identifier. Example II in the Appendix shows the actual coding used to implement the function. Figure 3-12 gives an illustration of a face being replaced by another. 52

65 Figure 3-12 Example showing the replace face modeling function 3.3 Identifying Part Features One of the key issues regarding the development of the VPM is automatically identifying part features such as lines, arcs, curves, faces and other CAD features. To use API modeling functions such as UF_MODL_create_replace_face ( ), the user has to know the target_face s object identifier. As was touched on in the Section 1.4.3, PC- DMIS has a feature called the DirectCAD Interface, which allows it to obtain object identifiers. Because PC-DMIS currently has not implemented this functionality, an interactive, Graphical User Interface (GUI) built in NX was created to provide the needed functionality. Figure 3-13 shows the GUI s dialog box with the different features available to choose from. 53

66 Figure 3-13 DirectCAD Graphical User Interface dialog box The Graphical User Interface (GUI) was entitled DirectCAD Interface because of its relation to PC-DMIS. This interface enables the user to select the desired feature and obtain the feature s object identifier (CAD ID), geometry type and handle. When the user selects one of the interface buttons, the user is prompted to select the desired feature on the CAD model after which the blank fields are then filled in as shown in Figure This research uses the feature s handle because its identity never changes (see Section 2.5.2). The user copies the handle and pastes it in the ID field (located in the PC-DMIS 54

67 dialog box) also shown in Figure From that point on, the appropriate object identifier will be linked to the feature being measured. Figure 3-14 Dialog boxes from NX and PC-DMIS showing CAD ID s Once again, this type of functionality could easily be integrated into PC-DMIS, because PCDMIS has access to the CAD systems API. The NX API functions used in identifying the feature s object identifier, feature type and handle are listed below. UF_UI_select_with_single_dialog ( char * message, char * title, int scope, UF_UI_sel_init_fn_t init_proc, void * user_data, int * response, tag_t * object, double cursor[ 3 ], tag_t * view ) UF_MODL_ask_feat_type (tag_t object, char **feat_type) UF_TAG_ask_handle_of_tag(tag_t object) The first function, UF_UI_select_with_single_dialog( ), is used when a button is pushed on the DirectCMM GUI. When a button is pushed this function is called and it automatically displays a dialog box that prompts the user to select a feature. The important output of this function is the object identifier (object). The object identifier is then passed into the function called UF_TAG_ask_handle_of_tag( ). This function 55

68 returns the persistent handle of the object identifier in the form of a character string. The feature s type is obtained with the function called UF_MODL_ask_feat_type( ). It uses the object identifier and returns the feature s type in the form of a character string. 3.4 CAD Modifications Based on GD&T The methodology described in this research was developed to modify any measurable surface as long as it can be compared to its theoretical surface. The methodology can also be used with Geometric Dimensioning and Tolerancing (GD&T) principles. The GD&T principles are mathematically defined and thus very applicable to this research. The objective is to be able to create a VPM based on a surface s measured data and its dimensions and tolerances. As was described in Section 1.2, there are five classifications of Geometric Tolerancing (form, orientation, location, profile, and runout). Each classification either pertains to individual features (meaning datums are never used), or is related in some way to another feature (meaning datums are used). This section discusses how the VPM methods described in Section 3.2 are applied to surfaces when GD&T principles are utilized. This section will also discuss how the methods are applied to periodic features like cylinders and cones Modifications to Non-Related Features The GD&T classifications pertaining to non-related features are Profile and Form. The geometric characteristics of Profile include profile of a line and profile of a surface and can either be applied to related or non-related features. The geometric characteristics of Form include straightness, circularity, flatness and cylindricity. These characteristic tolerances are applied to either rotational objects or planar objects. Since Form tolerances 56

69 are specified to control how far actual surfaces are permitted to vary from the perfect geometric form, the general method described in Section 3.2 is used. This holds true for flatness, circularity, and cylindricity, however an additional method was developed for tolerances dealing with straightness of line elements on rotational surfaces. Occasionally, a rotational surface will be inspected for the surface s straightness. The difference between the general method and this method is that instead of creating a thru curves feature, a revolved feature is created. To create the revolved feature, a spline is created through the single row of points and revolved about the surface s axis. To create the revolved face, the API modeling function, UF_MODL_create_revolved( ) is used. The function is as follows: UF_MODL_create_revolved ( uf_list_p_t obj_id_list, char **limit, double point[ 3 ], double direction[ 3 ], UF_FEATURE_SIGN sign, uf_list_p_t *feature_list) The function inputs the list of objects (obj_id_list) that are to be revolved. In this instance, the list contains a single spline. The other inputs are the limits of revolution (limit). This value is set to a 360 revolution. The point[3] and direction[3] are specified to represent the point and axis of revolution. The feature sign is set so a new target solid is created. The output of the function is a list of features created from this operation. The values of point[3] and direction[3] are obtained from the modeling function called UF_MODL_ask_face_data( ), shown below. UF_MODL_ask_face_data ( tag_t face, int * type, double point[ ], 57

70 double dir[ ], double box[ ], double * radius, double * rad_data, int * norm_dir ) The only input to this function is the object identifier (face). The function outputs the face s type, point, direction, bounding box, its radius (if it has one), other data pertaining to its radius and the face s normal direction Modifications to Related Features The GD&T classifications pertaining to related features are orientation, location, profile, and runout. Orientation tolerances include angularity, perpendicularity, and parallelism. Location tolerances include position, concentricity, and symmetry. Runout tolerances include circular runout and total runout. Each of these types of tolerances is related to another feature (datum). To prove that the VPM methodology can be applied to GD&T principles, the methods based on a parallelism tolerance will be discussed. The methods described in this section are applicable to each of the other tolerance characteristics. The general idea is to compare the surface s measured data to the surface s geometric tolerance zone established by a datum feature. Planes and cylinders mathematically describe a parallelism tolerance zone. The first step is to establish the tolerance zone s orientation. This is accomplished by creating a best-fit plane or cylinder through the datum features measured data points. The plane s orientation is described by its normal direction and the cylinder s orientation is described by its axis. The method used to construct a best-fit plane in this research uses a least squares, orthogonal regression approach. For a complete derivation of the orthogonal regression 58

71 approach it is recommended to obtain copies of the articles referenced in [21][22]. This approach measures the least squares errors orthogonally to the proposed plane. The necessary elements to construct a plane are a point and a direction. The constructed plane will pass through the average of a set of points. We will let ),, ( i i i i z y x X = v represent the set of all measured points and = = m i i X m A 1 ) (1/ v v represents the average of the set of points. With calculated, the direction of the plane is calculated by setting up the following matrix : ),, ( c b a A = v M (A) = = = = = = = = = = m i i m i i i m i i i m i i i m i i m i i i m i i i m i i i m i i c z c z b y c z a x c z b y b y b y a x c z a x b y a x a x A M ) ( ) )( ( ) )( ( ) )( ( ) ( ) )( ( ) )( ( ) )( ( ) ( ) ( (3.3) When the matrix is filled, its eigenvalues are calculated. The eigenvalues of the matrix are directly related to the plane s normal direction. As it turns out, when the smallest eigenvalue of Equation 3.3 is determined, the direction (unit length normal) of the plane is the corresponding eigenvector N v. These values can be found with any standard eigensystem solver or can be calculated using a method such as the Jacobi method [23]. The basic elements of a cylinder are a center point, C, an axis direction, W, a height, h and a radius, r. We will let { } n i i X 1 = represent the set of all measured points, which approximately models a cylinder. The equation defining cylinder points X is a quadratic equation and is written in standard form as: ( ) ( ) ( ) 1 2 = C X r WW I C X i T T i (3.4) where I is the identity matrix. The derivation of the above equation can be found in [24]. The goal of finding the least squares fit cylinder is to minimize the total squared error. 59

72 The total squared error, defined by the energy equation below (Equation 3.5) is used for minimization: E n T I WW, i i 1 (3.5) 2 i= 1 r T ( ) ( ) ( ) C W, r = X C ( X C ) This research accomplishes the minimization of the above equation by starting out with an initial guess of the center point and axis direction. With the guesses, an initial parameter vector is formed. Afterwards, a line containing the initial parameter vector is searched to obtain the minimum of E along the line. The parameter vector at which the minimum occurs is used as the starting point for the next linear search using a line of different direction than the first. A few general methods such as the conjugate gradient method or the method of steepest descent are suitable for the minimization technique described above. After each iteration, a confidence interval is calculated. If the confidence interval is satisfied, a solution is found. When the datum s orientations have been established, the next step is to locate the measured data point furthest from the datum. This point establishes the tolerance zone s outer boundary. This is accomplished by using the API vector function UF_VEC3_distance_to_plane( ), shown below. The four inputs to this function include the point to calculate the distance from (pnt1[3]), the point located on the plane (pnt_on_plane[3]), the plane s normal direction (plane_normal[3]), and a tolerance value used for checking (tolerance). The functional output is the normal distance from the point to the plane (distance). UF_VEC3_distance_to_plane ( const double pnt1[ 3 ], const double pnt_on_plane[ 3 ], const double plane_normal[ 3 ], double tolerance, 2 60

73 double * distance) After the furthest measured data point is found, a reference plane or cylinder is created half way between the outer and inner tolerance zones. The reference plane or cylinder in this research contains the same orientation as its datum. Most of the time, this is the case with parallelism tolerances; however, the time when this isn t the case is when the tangency symbol is applied to the parallelism tolerance. For demonstration purposes, this research uses the same orientations of the datums. To calculate the location of the plane, a point (ref_plane_pnt) is calculated using the equation below (Equation 3.6). The reference cylinder s radius is established by subtracting ½ of the tolerance from the furthest point s radius. ref_plane_ pnt x, y,z = max_pnt x,y,z -1 2 tol diri, j, k (3.6) The next step is to calculate the VPM points. For the parallelism of a plane-plane situation, the distance (along the surface s normal direction) from the measured points to the reference plane is calculated. Figure 3-15 shows how the distance is calculated. The distances are then used to offset each of the theoretical points along the theoretical surface s normal direction. After the VPM points are created, splines are created through the VPM points, the through curves feature is made and the old surface is replaced with the VPM surface. 61

74 Figure 3-15 Calculation of the distance between a line and a plane To consider the parallelism of an axis-axis situation, the reference cylinder s axis is placed (hypothetically speaking) in the center of the theoretical cylindrical feature. The NX API function UF_MODL_ask_face_data( ) is used to find the cylindrical feature s properties. Since several levels of points are measured on the cylindrical feature, the location (ref_pnt) where each level (plane) intersects the reference cylinder s axis is computed. The same computation shown in Figure 3-15 is made to determine these ref_pnts. To calculate the VPM points the offset distance is computed. The offset distance is the difference between the reference cylinder s radius and the distance from the measured points to the ref_pnts. The calculated distances are then used to offset the theoretical points. The direction of the offset is the surface s normal direction at that point. To finish creating the new surface, splines are created through each level of VPM points, a through curves feature is made and the old surface is replaced with the VPM surface. 62

75 3.5 Updating the CAM Process One of the objectives of this research is to develop methods to automatically update the manufacturing process plan that corresponds to the changes made to the VPM. When any change is made to part geometry, the associated tool paths are no longer valid and need to be updated. After researching how a manufacturing process plan is setup in NX, a few problems arose which make automatically updating a CAM process plan slightly more difficult. One of the problems relates to when planar surfaces are modified and become non-planar. Planar milling operations such as FACE_MILLING are only associated to planar surfaces. If a planar milling operation is specified to a planar surface, and the corresponding VPM surface is non-planar, the milling operation is no longer valid and cannot be used. Some other type of milling operation such as CONTOUR_AREA would have to be specified that is capable of machining non-planar surfaces. The other problem relates to NX s current capabilities. A user can manually interact with a CAD/CAM model and update tool paths by selecting a tool path regeneration menu option, however, NX currently does not contain the programmatic capability of automatically regenerating tool paths. The only way to automatically update tool paths is to start over and create the tool paths from scratch. This way, both problems are resolved; the type of machining operation can be specified and can be automated. The difficulty is automatically determining the appropriate type of machining operation. This section will discuss the methods used to programmatically setup a new manufacturing process, and generate new tool paths for the VPM surfaces. To demonstrate these methods, the steps involved in creating a non-planar milling operation 63

76 (CONTOUR_AREA) will be discussed. In short, the milling operation is programmatically added to a series of groups (program, method, geometry and tool) and the tool paths are finally generated. Example III in the Appendix gives a complete coding example showing how this is performed Creating the Operation The first step is to create the milling operation. To do this, the milling operation s type and subtype have to be specified. The following function is used to create the operation. UF_OPER_create ( char * type_name, char * subtype_name, tag_t * new_operation ) The operation s type_name and subtype_name are set equal to MILL_CONTOUR and CONTOUR_AREA respectively to machine a non-planar surface. The function s output is the operation s object identifier (new_operation) Creating the Program Group Once the operation is specified, it can be placed inside a program group. A program group can be seen as a container for various operations and is created using the function UF_NCPROG_create( ) as is shown below: UF_NCPROG_create ( char * type_name, char * subtype_name, tag_t * new_prog_group ) 64

77 The names of the program s type and subtype are inputs to this function and can be any particular character string. The function s output is the program group s object identifier (new_prog_group). Once the program group is created, it is placed inside the CAM Setup. NX refers to the NC machining environment as a Setup, which allows the user to organize and logically group all the information related to the operation. To accomplish this, the object identifier of the Setup is queried using the function UF_SETUP_ask_setup (tag_t * setup_tag ) and used in conjunction with the following function to obtain the Setup s root program. UF_SETUP_ask_program_root ( tag_t setup_tag, tag_t * root_prog_group ) The function s output (root_prog_group) is the Setup s root program and is used to add the program group (new_prog_group) to the Setup s root program. The function UF_NCGROUP_accept_member( ) shown below is used to add new program group to the root program group. UF_NCGROUP_accept_member ( tag_t parent, tag_t member ) The parent is the root program group (root_prog_group) and the member is the new program group (new_prog_group). The last step is to add the operation (new_operation) to the new program group using the same function Creating the Method Group The machining method specifies the type of cut to be made (rough, semi-or finish). Since the roughing and semi-finishing cuts have been completed, the finishing 65

78 machining method is chosen. Parameters such as Intol, Outol, and Part Stock are also defined in this step. Example III in the Appendix shows how these parameters are specified. To create the machining method, the same steps (with a few exceptions) are taken to create a method group and also to add the milling operation. One difference is the function (shown below) to create the method group. UF_NCMTHD_create ( char * type_name, char * subtype_name, tag_t * new_mthd_group) The other difference is the function used to ask the CAM Setup s root method group. The function is shown below. UF_SETUP_ask_mthd_root ( tag_t setup_tag, tag_t * root_mthd_group ) Creating the Geometry Group The geometry group defines the machining geometry and other parameters such as Part, Blank, and Check geometry, MCS orientation, and clearance planes. Once again, Example III in the Appendix shows how these parameters are specified. The following functions are used to create the geometry group and obtain the CAM Setup s root geometry group. UF_NCGEOM_create ( char * type_name, char * subtype_name, tag_t * new_geom_group ) UF_SETUP_ask_geom_root ( tag_t setup_tag, tag_t * root_geom_group ) 66

79 3.5.5 Creating the Tool Group The tool group defines which cutting tools are to be used and defines the tools attributes such as diameter, lower radius, length, taper angle, etc. To create a tool group and obtain the CAM Setup s tool group the following functions are used. Example III in the Appendix demonstrates how tool parameters are specified. UF_CUTTER_create ( char * type_name, char * subtype_name, tag_t * new_tool_group ) UF_SETUP_ask_mct_root ( tag_t setup_tag, tag_t * root_mct_group ) 3.6 Hardware Configuration for Testing The methods described throughout this research are all software oriented. To completely verify the VPM methodology, the methods need to be physically tested. A description of the hardware used for testing will be presented in this section Sugino 3-Axis Mill The physical mill used for this research made available by Direct Controls, Inc. (DCI) is a Sugino V9 (3-axis mill). This mill was originally donated to DCI for research and development purposes by Sugino Machine, Inc. located in Japan. The mill was retrofitted with a DMAC controller (first of its kind) by DCI and with the help of the DMAC research team at BYU. While the mill s workspace is limited to smaller parts, its speed and precision capabilities are impressive. Figure 3-16 shows a picture of the mill and the physical specifications are listed in Table

80 Figure 3-16 Sugino 3-axis mill used for testing Table 3-1 Sugino V9 specifications Stroke X axis mm 200 Y axis mm 200 Z axis mm 250 Table Working area mm 300 x 500 Allowable load kg 300 Distance from table to spindle mm 150 ~ 395 Spindle Speed Standard rpm 17, kW High Speed rpm 22, kW Feed Rate Rapid feed rate m/min 30 Cutting feed rate m/min 10 Min. programmable unit mm Accuracy Positioning mm Repeatability mm ± Probing System The probing system consists of three parts (Probe, Optical Machine Module, and Machine Interface Unit) and is developed by Renishaw. Special thanks go to BYU s Precision Machine Shop and Wilcox Associates, Inc for providing the necessary probing hardware for completion of this research. 68

81 The probe used for testing is a Renishaw MP7. The probe is an old generation touch trigger probe that is used for workpiece setup and inspection on CNC machining centers. The probe measures approximately 150 mm with the stylus and tool shank connected. Because it is quite large, the Sugino mill s workable volume is limited to only smaller parts. Figure 3-17 shows the MP7 probe and the other probing devices. Figure 3-17 Optical transmission probing system The probe communicates with the CNC machine controller through an optical transmission system using infrared technology. The probe transmits signals to the Optical Machine Module (OMM), which interprets the signals. The OMM receives signals from the probe whenever the probe turns on or off, or if the stylus is deflected. The OMM in turn conveys the signal to the Machine Interface Unit (MI12). The OMM is mounted to the machining center and is hardwired into the MI12. The MI12 converts the signal to a form compatible with the machine controller. The MI12 also has an audible indicator 69

82 signifying when the probe has taken a hit. Figure 3-21 shows the OMM and MI12 components. Figure 3-18 Optical Machine Module and Machine Interface Unit 70

83 CHAPTER 4 RESULTS The best methods for automatically creating the Variational Part Model (VPM) were sought throughout this research to compensate for dynamic machining error. To validate these methods, physical testing was performed. It should be noted that the testing performed did not compensate for the machine s static error (ball screw error, joint misalignment, perpendicularity error, etc). This chapter will discuss how the tests were performed as well as present the results obtained through measurement. In particular, two parts were machined and measured. The measurements were used to create the VPM and then the parts were remachined and measured. The first test was based on a single row of measured points and evaluated to a line profile tolerance. The second test was based on several rows of measured points and evaluated to a surface profile tolerance. 4.1 Physical VPM Test Setup The Sugino 3-axis machining center described in Section was used to perform both the machining and inspection tasks. The two parts used were made out of Aluminum and measured x x 30 mm. The CAD/CAM model (shown in Figure 4-1) was created in NX and PCDMIS was used for inspection planning. The part s non-planar surface was tested to validate the methods described in this research. 71

84 Figure 4-1 Part used in Variational Part Model test To bias some error into the system, a radial offset of 0.1 mm was applied to the part s non-planar surface. The biased error was applied to the part to represent the semifinished surface and to allow material to be removed during the finish machining step. A radial offset was chosen to appropriately compare theoretical and measured values. With this offset, the values correlate with each other; meaning the surface normals are identical along either surface. In theory, after machining, the surface would be 0.1 mm above its originally intended location and still have material overstock to correct for the radial offset and machine the intended profile. Each part was directly machined from NX using the generated tool paths and measured on the machine with the MP7 touch trigger probe described in Section 0. The radial offset CAD/CAM model was used for machining and the original CAD model was used inside PCDMIS to compare theoretical and measured values. To create the VPM, the radial offset CAD/CAM model s surface was modified and its tool paths regenerated. Table 4-1 lists the machining parameters used for tool path generation. 72

85 Table 4-1 Machining parameters used for tool path generation Rough Cut Semi-Finish Cut Finish Cut Part Intol 0.03 mm 0.03 mm mm Part Outol 0.12 mm 0.03 mm mm Part Stock 1.0 mm 0.3 mm mm Tool Type Flat End Mill Ball End Mill Ball End Mill Tool Diameter mm mm mm % Step Over 30% 30% 10% The two tests used scanning procedures to measure the two surface profiles. The first test considered verifying the methods for updating for a single row of measurements taken along the surface. PCDMIS calls this type of measurement routine a Linear Open Scanning procedure. The inspection process plan was created to include this scanning procedure; composed of a single row of 75 points spaced evenly along the surface. The second test was setup to verify that an entire surface could be measured and corrected. To accomplish this, a UV Scanning Procedure was included in the process plan that included 10 rows of 50 points. Because scanning procedures have not yet been implemented into the Wilcox Associates, Inc. generic driver (WADriver.dll, see Section 1.3.3), the process plan had to be modified to convert the scanning procedures into individually measured points. Although more time consuming, the result is the same. The inspection reports created by PCDMIS containing the measured results were used to create each of the VPM s. The NX software program developed in this research read in the inspection reports and automatically generated the new VPM surfaces. After the VPM s were created, the tool paths were regenerated and the parts were re-machined. 73

86 4.2 Line Profile VPM Results After machining the first part, the theoretical and measured values of the part were compared. Table 4-2 shows the theoretical and measured values prior to VPM creation. The measured error, calculated as the distance between the theoretical and measured values is also shown. Table 4-2 Line profile measurements versus theoretical values Original Inspection (Line Profile Test) Theoretical Values Measured Values Error X Y Z X Y Z

87 Table 4-2 (continued) * units shown in mm 75

88 As can be seen, the error values ranged from mm to mm. The average error was mm. After the VPM was created, the tool paths were regenerated and the part was re-machined. After re-machining, the part was measured and the theoretical and measured values were compared. Table 4-3 shows the measurements taken as well as a comparison to the theoretical values. Table 4-3 Line profile VPM measurements versus theoretical values Variational Part Model Inspection (Line Profile Test) Theoretical Values Measured Values Error X Y Z X Y Z

89 Table 4-3 (continued) * units shown in mm 77

90 As can be seen, the 0.1 mm error offset was corrected. The smallest error measured on the VPM was mm ( in) and largest error measured was mm ( in). The average error measured was mm ( in). Figure 4-2 shows a histogram illustrating how the measured error was distributed. Figure 4-2 Line profile VPM measured error distribution 4.3 Surface Profile VPM Results As was mentioned before, the same CAD/CAM model and error offset used in the line profile test was used to verify that an entire surface could be measured and corrected. As the amount of data is too large to be included in this Section, the results of the first and last measurements can be seen in the Appendix (Table A-1, Table A-2). The error values of the non-compensated part ranged from mm to mm. The average error measured was mm. After creating the VPM and re-machining, the part was measured and the theoretical and measured values were compared. Figure 4-3 shows a histogram illustrating how the measured error was distributed. 78

91 As can be seen, the smallest error measured on the VPM was mm ( in) and the largest error measured on the Variational Part Model was mm ( in). The average error measured was mm ( in). Figure 4-3 Surface profile VPM measured error distribution The following figures are shown to illustrate how the VPM for this test was created and what the final VPM looks like. The figures were exported from NX and show the splines and surface geometry from the VPM presented in this test. Figure 4-4 Creation of the Variational Boundary Surface Splines 79

92 Figure 4-5 Creation of the through curves feature Figure 4-6 Replacing the old surface with the VPM surface In conclusion, the two tests demonstrate the validity of the Variational Part Model concept and prove that automatic closed-loop machining is possible. The tests show that dynamic machining error can be compensated. The results indicate that the VPM s measured error was approximately equal to what was measured prior, thus indicating that any dynamic error was accounted for and that the majority of the measured error left was caused by the machine s static error. Although none of the methods to compensate for a 80