EXPERIMENTAL AND FINITE ELEMENT ANALYSIS OF A SIMPLIFIED AIRCRAFT WHEEL BOLTED JOINT MODEL

Transcription

1 EXPERIMENTAL AND FINITE ELEMENT ANALYSIS OF A SIMPLIFIED AIRCRAFT WHEEL BOLTED JOINT MODEL A Thesis Presented in Partial Fulfillment of the Requirements for the Degree Masters of Mechanical Engineering in the Graduate School of The Ohio State University By Kathryn J. Belisle ***** The Ohio State University 2009 Thesis Defense Committee: Dr. Anthony Luscher, Adviser Dr. Mark Walter Approved by Adviser Graduate Program in Mechanical Engineering

2 Copyright by Kathryn J. Belisle 2009

3 ABSTRACT The goal of this thesis is to establish a correlation between experimental and finite element strains in key areas of an aircraft wheel bolted joint. The critical location in fatigue is the rounded interface between the bolt-hole and mating face of the joint, called the mating face radius. A previous study considered this area of a bolted joint but only under the influence of bolt preload. The study presented here considered both preload and an external bending moment. This study used a more complete single bolted joint model incorporating the wheel rim flange and the two main loads seen at the bolted joints; bolt preload and the external load created by tire pressure on the wheel rim. A 2x3 full factorial DOE was used to establish the joint s response to various potential load combinations assuming two levels of preload and three levels of external load. The model was analyzed both experimentally and in finite element form. The strain results around the mating face radius were compared between the two analyses. Several parameters were identified that could affect the correlation between the results. The finite element model was modified to incorporate each of these factors and the new results were compared against the original finite element results and the experimental data. The best correlation was found ii

4 when the finite element model preload was adjusted such that the mating face radius strains under only preload matched those of the experimental results. iii

5 This thesis is dedicated to my parents for always encouraging me, for listening when I was frustrated, for picking me up when I was down, for helping me however they could, and for taking pride in my triumphs. iv

6 ACKNOWLEDGMENTS I would like to thank Goodrich Aircraft Wheels and Brakes for allowing me the use of their resources. I would particularly like to acknowledge Bud Runner of Goodrich who was a constant source of expertise, advice, and support. I would like to thank all the faculty and staff of the Ohio State University who helped me throughout the course of my research. I would also like to recognize my fellow graduate students for their support and help. Finally, I would like to acknowledge my family and friends for being constant sources of support and encouragement. v

7 TABLE OF CONTENTS Abstract... ii Acknowledgments... v List of Tables... viii List of Figures... ix CHAPTER 1: Introduction... 1 CHAPTER 2: Background and Literature Review Bolted Joint Models Experimental Setup Finite Element Modeling Comparison of Experimental and Finite Element Results Sensitivity Analysis Summary Torque Free Preload Experiment Literature Review CHAPTER 3: Experimental Analysis Experimental Model Development Experimental Measurement and Data Acquisition System Design of Experiment Test Setup and Procedure CHAPTER 4: Experimental Results Statistical Analysis of Experimental Results Design of Experiment Results Preload Variability Study vi

8 4.4 Bolt Bending Results Experimental Data for Finite Element Comparison CHAPTER 5: Finite Element Modeling Preliminary Model Setup Preliminary Finite Element Analysis Final Finite Element Model Setup CHAPTER 6: Finite Element Results Finite Element Results Acquisition Finite Element Convergence General Finite Element Results CHAPTER 7: Finite Element and Experimental Comparison CHAPTER 8: Summary and Conclusions List of references APPENDICES APPENDIX A: Labview Block Diagrams and Setup APPENDIX B: Bolt Bending Calculations APPENDIX C: Raw Experimental Data APPENDIX D: Statistical Results of the DOE APPENDIX E: Finite Element Data vii

9 LIST OF TABLES Table 3.1: Strain Gage Location Descriptions (*MFR = Mating Face Radius) Table 3.2: Bolt Preload and External Load Values Table 3.3: Loading Conditions Table 4.1: Bolt Bending and Tensile Results Table 4.2: Results at Mating Face Radius Locations for Preload Only (microstrain) Table 4.3: Results at Mating Face Radius Locations (microstrain) Table 5.1: Material Properties Table 5.2: Material Property Combinations Table 5.3: Adjusted External Loads Table 5.4: Adjusted Bolt Preloads Table B.1: Bolt Bending Calculation Spreadsheet Table C.1: Experimental Principal Strains for 12:00 MF Radius Gages Table C.2: Experimental Principal Strains for 3:00 MF Radius Gages Table C.3: Experimental Principal Strains for 6:00 MF Radius Gages Table D.1: Experimental Principal Strains for 6:00 MF Radius Gages Table E.1: Descriptions of Models Table E.2: Finite Element Mating Face Radius Data Table E.3: Finite Element Mating Face Radius Data for Preload Only viii

10 LIST OF FIGURES Figure 1.1: Aircraft Wheel Assembly... 2 Figure 1.2: Bolted Joint Fillet... 3 Figure 2.1: Circular Plate Experimental Model... 6 Figure 2.2: Square Plate Experimental Model... 6 Figure 2.3: Experimental Test Setup... 8 Figure 2.4: Circular Plate Finite Element Model... 9 Figure 2.5: Square Plate Finite Element Model Figure 2.6: Exploded View of Bolted Joint for Torque Free Preload Experiment Figure 2.7: Torque Free Preload Experimental Setup Figure 3.1: Diagram Comparing Actual Nose Wheel with General Model Figure 3.2: Diagram of the Final Experimental Model Design Figure 3.3: Strain Gage Locations Figure 3.4: Mating Face Radius Strain Gage Designations Figure 3.5: Strain Gages Applied to the Mating Face Radii Figure 3.6: Strain Gages Applied to the Rim Flange Figure 3.7: National Instruments Strain Gage Conditioners Figure 3.8: National Instruments Bridge and Bridge Modules Figure 3.9: Final Experimental Assembly Figure 4.1: General Time Series Plot and Statistics Figure 4.2: Worst Case Time Series Plot and Statistics Figure 4.3: Representative Normality Test Figure 4.4: Main Effect DOE Results Figure 4.5: Free Body Diagram of Model Figure 4.6: Results of the Preload Variability Study Figure 5.1: General Preliminary Model Figure 5.2: General Finite Element Boundary Conditions and Loads Figure 5.3: Internal Finite Element Boundary Conditions and Loads Figure 5.4: Mesh Refinement Comparison Figure 5.5: Model with Washers Figure 6.1: Finite Element Strain Measurements Figure 6.2: Mesh Refinement Comparison Figure 6.3: Sample Finite Element Results (Six Load Cases) Figure 7.1: Zoomed Strain Flow Contour of Mating Face Radius ix

11 Figure 7.2: Comparison of Baseline Experimental and Finite Element Results Figure 7.3: Effect of Mesh Refinement on Correlation Figure 7.4: Effect of Bolt Material Stiffness Figure 7.5: Zoomed Plot of Effect of Bolt Material Stiffness Figure 7.6: Effect of Bracket Material Stiffness Figure 7.7: Zoomed Plot of Effect of Bracket Material Stiffness Figure 7.8: Effect of Adjusted External Loads Figure 7.9: Zoomed Plot of Effect of Adjusted External Loads Figure 7.10: Effect of Preload Modifications Figure 7.11: Effect of Solid Washer Figure A.1: Bracket Gage Data Acquisition Block Diagram Figure A.2: Bolt Gage Data Acquisition and Averaging Block Diagram Figure A.3: Data Acquisition Assistant Configuration Figure A.4: Filter Configuration Figure D.1: Detailed Statistical Results for 12 O clock Gage Location Figure D.2: Detailed Statistical Results for 3 O clock Gage Location Figure D.3: Detailed Statistical Results for 6 O clock Gage Location x

12 CHAPTER 1 INTRODUCTION Goodrich Corporation has commissioned the research presented in this thesis to improve the correlation of computer simulated bolted joint models to experimental data as a tool for weight optimization of aircraft wheels, one of their key products. An example of an aircraft wheel assembly is shown in Figure 1.1. The wheel of an aircraft is designed to withstand high loads with minimal weight, so material is removed from the unit wherever possible. Due to the stiffness and size of the tires used in aerospace applications, the wheel must also be made in two halves. The halves are fitted into the tire and then bolted together to form the wheel assembly. Typically, several different tires are specified for a single wheel assembly, and each tire loads the wheel differently. However, these variations in loading are difficult to know without testing. Thus, the wheel must be designed to compensate for various potential load and pressure distributions. This requirement, combined with the weight constraints and multiple bolted joints, render the wheel assembly geometrically complex. 1

13 Figure 1.1: Aircraft Wheel Assembly The complexity of the wheel structure makes the design process extremely difficult. Currently, the process is very reliant on experimentation and testing. This means that new experimental models must be fabricated each time a design change is made to meet weight or performance specifications. Fabrication and testing of multiple models can become very costly and time consuming. Goodrich is interested in reducing the cost and improving the speed of their design process. Computer-aided simulations, such as finite element analyses, can significantly improve this speed and reduce expense. However, a finite element analysis is only valuable if the results correlate to those obtained from physical experimentation. 2

14 A well-correlated finite element model has yet to be established for this particular application. While the wheel structure can be modeled in finite element form, the results do not match experimental results as closely as necessary. In particular, Goodrich has demonstrated large differences between experimental and finite element strain measurements taken in key areas around the wheels bolted joints. These discrepancies are particularly prevalent around fillets around each bolt hole on the mating face of each wheel half. Figure 1.2 shows the fillet around a single bolted joint on the mating face of a wheel half. Mating Face Radius Mating Face Rim Figure 1.2: Bolted Joint Fillet Correction of these discrepancies depends on a thorough understanding of the wheel system. The complexity of the system, particularly the multiple bolted joints, makes this system especially difficult to study as a whole. Thus, the method adopted for this study 3

15 was to simplify the system into a series of models that could be easily fabricated, tested, and analyzed in finite element form. The study was completed in two phases. Phase I, completed by Abhijit Dingare [1] of the Ohio State University, considered several aspects of simplified bolted joint modeling. This phase is described more thoroughly in Chapter 2. The study was based on two bolted joint models. The first was an axisymmetric bolted joint with no extraneous geometric features. The second model was a simplified version of the wheel face geometry found immediately surrounding each bolt hole. Experimental and finite element analyses for both models were used to establish the effect of several physical and virtual parameters on the strain in the mating face fillet. Comparisons between experimental and finite element results were also used to understand the correlation, or discrepancies, between testing and simulation. The research presented in this thesis covers Phase II of the study of bolted joint simulation. The goal of this project was to develop and study a new model that more closely represented the actual loading seen in the bolted joints of the wheel structure. Thus, a model was developed to introduce a load due to tire pressure into the bolted joint where the tire pressure acts on the rim of the wheel. Experimental and finite element analyses of this model were intended to shed light on the interactions between bolt preload and external loads and their effect on the strain in the bolt and bolted joint. Again, the correlation between experimental and finite element results was of particular interest. 4

16 CHAPTER 2 BACKGROUND AND LITERATURE REVIEW In a previous study performed in majority by Abhijit Dingare [1], an aircraft wheel single bolted joint was considered under only bolt preload. Two simplified joint models were developed. These models were tested experimentally. Finite element models were then developed for comparison against the experimental results. Based on the initial results, a sensitivity study was performed to further characterize several finite element and experimental parameters. A secondary experiment was also performed to establish the effect of torque on the mating face radius strains. The results of this experiment were compared against the original finite element results. 2.1 Bolted Joint Models Two models were developed to test the effect of bolt preload on an aircraft wheel bolted joint. Both models were single bolted joints made up of two plates. The first model, called the circular plate model, simplified the joint to a set of cylindrical, axisymmetric plates with no face geometry. The second model, referred to as the square plate model, was a pair of square plates. These plates incorporated some wheel face 5

17 geometry into the mating faces of the plates. Both models had a round interface between the plate mating faces and bolt holes referred to as the mating face radius. The circular and square plates are shown in Figure 2.1 and Figure 2.2 respectively. Figure 2.1: Circular Plate Experimental Model Figure 2.2: Square Plate Experimental Model 6

18 2.2 Experimental Setup The experiment was performed using a test setup housed at Goodrich Aircraft Wheels and Brakes. The plates were fitted into a housing that would keep them from rotating. A special bolt, called a Strainsert, was used for testing. A Strainsert is a hollowed bolt with a strain gage applied internally. The Strainsert is calibrated for preload. The head of the Strainsert was held with a wrench plate also made to fit in the housing. A torque tool was then used to tighten the bolt to a specified preload. Strain gages were also applied to the mating face radius of both plates to measure the effect of the preload on the strain in the bolted joint. The strain gages were applied in both the hoop, called horizontal, and axial, called vertical, directions. The symmetry of the two plates with respect to one another was used to apply two gages of opposite orientations at a single location; one on each plate. Figure 2.3 shows the test setup. An example of strain gages on the mating face radius is included in Figure

19 Figure 2.3: Experimental Test Setup 2.3 Finite Element Modeling Finite element models were developed based on the dimensions of the experimental models. Figure 2.4 shows the finite element model of the circular plates. Axisymmetry was used to reduce the model to a 2D model. Symmetry between the plates also served to reduce the model. Figure 2.5 shows the finite element model of the square plates. Symmetry across the yz-plane was used to reduce the model as shown. This model was analyzed in 3D. In both cases, the model was fixed as required by symmetry conditions. The preload was applied as a displacement on the split end (or ends) of the bolt with the displacement being iterated until the desired preload was achieved. 8

20 Figure 2.4: Circular Plate Finite Element Model 9

21 Figure 2.5: Square Plate Finite Element Model 2.4 Comparison of Experimental and Finite Element Results In both cases, the experimental results showed low individual and overall repeatability. Both finite element models tended to under-predict the experimental strains. For the circular plate model, the correlation between finite element and experimental results was reasonable for most gages with strain gage three being an exception. However, this was not considered particularly problematic since this gage was 10

22 measuring in the low strain, or hoop, direction. The correlation was unacceptable, in most cases, for the square plate model. 2.5 Sensitivity Analysis Summary After comparing the initial experimental and finite element results, several potential sources of variation were identified. The parameters that would affect these variations were included in a sensitivity study to see their effect on the joint strains. The finite element parameters included mesh refinement, dimensionality, material modeling, and bolt alignment. Several experimental factors included torque rate, preload control method, and dwell. The first finite element parameter analyzed was mesh refinement. The mesh refinement was increased until the results were no longer affected by the change. It was found that the increased mesh refinement had a significant effect on the results, but at a very high computational expense. Dimensionality was a concern for the circular plate model. A comparison of 2D and 3D models revealed that the 2D axisymmetric model was acceptable. Material property modeling was the next parameter considered. Three material models were available, isotropic, orthotropic, and hypoelastic. The comparison showed that the hypoelastic properties resulted in the best correlation to experimental data. The differences between the three models, however, were minimal, so any model should be acceptable. Finally, the alignment of the bolt within the bolt hole was studied. It was found that a misalignment of the bolt could reduce the overall joint stiffness, thus increasing the strains in all mating face radius locations slightly. 11

23 Several parameters were also tested experimentally. The rate at which torque was applied to the bolt during preloading was tested first. Increasing the torque rate from one to five rpm significantly improved the experimental repeatability. Two methods of controlling the preload were also considered; control of the amount of torque applied and control of the strain in the bolt shaft. The torque control method was found to be more repeatable than the strain control method. Finally, the effect of dwell on the strain output was considered. In the worst case, a 20 microstrain drift was seen over the first 30 seconds of data acquisition. The data tended to stabilize after approximately 30 seconds. 2.6 Torque Free Preload Experiment The application of torque during experimental preloading was identified as a big discrepancy between the experimental and finite element models. A secondary experiment was designed to remove torque from the preload process. To accomplish this, the bolt was cut in two through the bolt shaft. A dowel was used to align the two halves without passing any axial load between them. Figure 2.6 shows the circular plate model with the cut bolt. A similar setup was used for the square plate model. An Instron type testing machine was used to apply the required preload force to the ends of the bolt. Figure 2.7 shows the square plate model setup on the Instron machine. 12

24 Figure 2.6: Exploded View of Bolted Joint for Torque Free Preload Experiment 13

25 Figure 2.7: Torque Free Preload Experimental Setup The original experimental results were generally under-predicted by the finite element models for both the square and circular plates. The results from the torque free experiment were typically over-predicted by the finite element analyses. The correlation between finite element and experimental results worsened when torque was removed from the experiment. One possible reason for this was misalignment of the Instron s test frame. Based on the reduced correlation to finite element results as well as time constraints, this line of research was not pursued further. 2.7 Literature Review A study performed by Jeong Kim, et al. [2] considered four methods of modeling a bolted joint in finite element form. These included a solid bolt preloaded thermally, a 14

26 beam element coupled to nodes on the gripped bodies preloaded by an initial strain on the beam element, a beam element connected to the gripped bodies with 3D element spiders also preloaded by an initial strain on the beam element, and finally a preload pressure applied directly to the contacted bodies with no bolt represented. It was found that the solid bolt model gave the best correlation to experimental results. However, the coupled bolt model significantly improved the computational efficiency of the model. Another study, performed by Gang Shit, et al. [3], incorporated end-plate bolt preload into a finite element model of a beam-to-column connection. The finite element model was compared against an experimental model. The finite element results correlated well to experimental results and gave a more detailed view of the joint response based on results not easily measured during experimentation. Slippage in bolted joint of transmission towers was simulated by finite element analysis in a study by R. Rajapakse, et al. [4]. Bolted joint slippage was found to have a significant, negative effect on the load bearing capacity and displacement of the tower trusses. However, the correlation between finite element analysis and actual results improved when slippage was accounted for under a specific case called frost-heaving. 15

27 CHAPTER 3 EXPERIMENTAL ANALYSIS The first step towards achieving a well correlated finite element model of a bolted joint was the establishment of a baseline for comparison. For this purpose, an experimental analysis was developed. Several criteria were considered in the design of the experimental model and procedure. First, the experiment required the application of two main forces; bolt preload and an external shear load generated by tire pressure on the wheel rim. The model had to allow for the application of both forces with minimal interference to the actual bolted joint. Next, a system was required to measure the effect of these forces at key locations in and around the bolted joint. Third, an experimental design was needed to incorporate the various loading conditions of an aircraft wheel bolted joint. Finally, a test setup and procedure were necessary that would allow for repeatable force application and data acquisition. 3.1 Experimental Model Development An experimental model of an aircraft wheel bolted joint was developed. The model needed to incorporate the two main load sources of an aircraft wheel bolted joint; bolt 16

28 preload and tire pressure on the wheel rim. The model also needed to incorporate the geometry of the aircraft wheel surrounding the joint in order to approximate the appropriate load paths. Boundary conditions were created which allowed the application of simulated loads with minimal interference to the key areas of interest in and around the bolted joint. The first goal of the model design was to simulate the basic geometry of an aircraft wheel bolted joint. The design method adopted was to select an aircraft wheel with certain desirable features and simplify the bolted joint geometry to a feasible set of test brackets. A small wheel was desirable as the proportions of the geometry would be easier to simulate. A wheel with a lower tire pressure rating would reduce the forces required for testing. Symmetry between the joint halves was also desired as this would simplify both the experimental setup and the finite element model. Based on these criteria, the nose wheel of a DeHavilland (DHC-8-400) aircraft was chosen as the basis of the experimental model. This wheel assembly used an eight bolt pattern of 5/16 in. bolts. The bolts were rated for individual bolt torque of 255 in-lbs, which was equivalent to a preload of 6,825 lbs. The rated tire pressure for this wheel was 85 psi. The nose wheel was made of 2014-T6 aluminum. Figure 3.1 shows the cross sectional geometry of a single nose wheel bolted joint (in red) overlaid with the simplified geometry of the experimental model (in green). 17

29 Figure 3.1: Diagram Comparing Actual Nose Wheel with General Model The actual bolted joint was nearly symmetrical, so the major features could be approximated as such. For the experimental model, the overall thickness of material immediately surrounding the bolted joint was equivalent to that of the actual joint. The geometry in this region was simplified to remove any asymmetry. This was intended to reduce the complexity of the experimental and finite element analyses. The modeled rim flange thickness approximated the thickness of the portion of the actual rim immediately connected to the bolted joint. This was chosen to allow the experimental model to more closely simulate the load path of the aircraft wheel. The width of the experimental model was chosen to be four times the diameter of the bolt plus a quarter inch to insure that no yielding would occur in the rim flange during external load application. See Figure 3.1 for this equation for model width. 18

30 While several dimensions were taken directly from the wheel dimensions, certain dimensions were modified for various purposes. One modification was needed to eliminate a potential source of interference to the desired load path in the rim flange resulting from the method of external load application. In the aircraft wheel, the external load, generated by tire pressure against the rim of the wheel, would be very even along the rim. Thus, an even load distribution across the width of the modeled flange was required. The anticipated loading method for experimentation would not necessarily result in an evenly distributed load at the flange interface to the bolted joint. To remedy this, the flange length of each bracket was extended by three inches. This allowed room to connect the flange to a load source with enough space between the connector and the bolted joint for the load path to spread across the width of the flange. The four holes passing through the rim flanges, shown in Figure 3.2, were designed for the purpose of connecting the brackets to a load source. Another modification to the bolted joint was needed for the measurement system selected for the characterization of the load effects. Strain gages were chosen for measurement. A strain gage would have no effect on the solid material surrounding the bolted joint; however, the wiring required for data acquisition could be problematic given a tight space tolerance. This was recognized as a potential issue inside the bolted joint where key areas of interest included both the bracket mating face radii and the bolt shaft. The diameter of the bolt hole was increased by 0.1 in. and the mating face radius was opened to 0.25 in. to resolve this problem. 19

31 Figure 3.2 shows the final design for the body of the experimental model of the bolted joint. One feature was not included in this diagram; a small runner used to pass strain gage wires out of the bolted joint. The runner was made up of adjoining slots machined into each bracket s mating face to a width of approximately in. and a depth of approximately one half of the width. The slots opened into the mating face radius between the six and three (or nine) o clock positions to avoid interference with the key areas of interest; twelve, three, and six o clock. The wires passed out near a corner of the bolted joint body opposite the rim flange so as to avoid interfering with the joint loading. These runners were considered inconsequential to the stress in the areas of interest in and around the bolted joint. Figure 3.5 shows the wires passing through the slots on the mating faces of both brackets. Based on typical Goodrich practice, the wires running from the strain gages on the bolt shaft were passed through a slot in a special washer, called a shouldered washer. The shouldered washer had a flat face in contact with the bracket face, as would a normal washer. It also incorporated a shoulder that dropped into the bolt-hole. This shoulder served to center both the washer and the bolt which kept the strain gages on the bolt shaft from coming in contact with the sides of the bolt-hole. 20

32 Figure 3.2: Diagram of the Final Experimental Model Design 3.2 Experimental Measurement and Data Acquisition System In order to fully characterize the reaction of the bolted joint to the applied loads, a measurement system was required. Strain gages were chosen as the applicable measurement device. There were three main areas of interest in the bolted joint model. The first was the radius interfacing the bolt-hole and the mating face of each bracket; called the mating face radius. The second was the shaft of the bolt. The third was the rim flange. Figure 3.3 depicts the strain gage locations on the brackets and the bolt shaft. Table 3.1 describes the location intended for each strain gage number of Figure

33 Figure 3.3: Strain Gage Locations Gage # Body/Region Position Description 1 Bracket 1/Rim Flange Upper surface near load source 2 Bracket 1/Rim Flange Lower surface tangent to fillet 3 Bracket 1/MFR* 12 o clock 4 Bracket 1/MFR* 3 o clock 5 Bracket 1/MFR* 6 o clock 6 Bracket 2/MFR* 12 o clock 7 Bracket 2/MFR* 3 o clock 8 Bracket 2/MFR* 6 o clock 9/10/11 Bolt/Shaft 120 o apart Table 3.1: Strain Gage Location Descriptions (*MFR = Mating Face Radius) The mating face radius was the primary area of interest for this experiment. This area has been particularly problematic in Goodrich s past attempts to correlate finite element and experimental data. A good correlation in this region is essential to a valuable finite element model. More specifically, three locations were designated on this radius at intervals around the bolt-hole. These locations were defined as twelve, three, and six 22

34 o clock where twelve o clock was closest to the rim flange (see Figure 3.4). There were also two strain gages placed at each of these locations; one on each bracket. Since the brackets were symmetrical, the stresses around the mating face radii were expected to be equivalent. The gage on one bracket at each location was aligned with the curvature of the radius. These strain gages were referred to as axial gages because they approximately aligned with the axis of the bolt shaft. The second gage at each location, on the opposing bracket, was aligned with the curvature of the bolt-hole. These were referred to as hoop gages because they followed the radius of the bolt-hole, the hoop direction. In future, gage alignments may be shortened to A for axial gages and H for hoop gages. Refer to strain gage numbers three through eight in Figure 3.3 and Table 3.1 for the mating face radius strain gage locations and descriptions. Figure 3.4: Mating Face Radius Strain Gage Designations The bolt shaft was also of interest for two reasons. First, a strain reading on the bolt shaft was directly proportional to the preload being applied by the bolt. Thus, a strain gage on the bolt shaft would allow the operator to apply the required bolt preload based on a direct measurement, as opposed to a less precise torque reading, during testing. This also eliminated test equipment as no torque measurements were required during bolt 23

35 preloading. Furthermore, a strain gage would readily provide information about the change in preload after external load application. Apart from preload measurements, an interest was expressed by Goodrich in the bending of the bolt due to the external loading. For this purpose, a set of three strain gages were placed at 120 degree increments around the center of the bolt shaft. This triad of strain gages could be used to establish bolt bending regardless of the gages orientations with respect to the bending axis. Reference gages nine through eleven in Figure 3.3 and Table 3.1 for the bolt shaft strain gage locations and descriptions. The final area of interest for experimental characterization was the rim flange. The bending in this region was of particular interest. For this purpose, two strain gages were placed on the rim flange (the rim flange is the end pieces of the wheel. We don t have these modeled.); one on the upper surface and one on the lower surface. Both strain gages were placed in the center of the flange width and were aligned to the loading axis. One gage was located tangent to the fillet interfacing the flange to the bolted joint. The second gage was placed on the upper flange surface approximately 2.5 in. from the mating face to capture bending closer to the point of loading. Reference gages one and two in Figure 3.3 and Table 3.1 for the rim flange strain gage locations and descriptions. A total of eleven strain gages were applied to the bolted joint model. All of the gages were Nickel Chromium, 120 ohm, foil strain gages with a gage length of in. Amongst these eleven gages, two different Vishay Micro-Measurements strain gages were used: EA EH-120 and EA DJ-120. However, the only difference between them was the location of the solder pads with respect to the gage grid; all other 24

36 features were equivalent. The strain gages were applied using M-Bond 610, the recommended bonding agent of the strain gage supplier. Figure 3.5 shows the strain gages on the mating face radii of the brackets. Figure 3.6 shows the strain gages on the rim flange. H A A H H A Figure 3.5: Strain Gages Applied to the Mating Face Radii 25

37 (Left: Near Load Application; Right: Fillet Tangency) Figure 3.6: Strain Gages Applied to the Rim Flange A new National Instruments (NI) Compact DAQ series system was selected for acquiring data from the strain gages. The system consisted of four main elements. Each strain gage was connected to a 120 ohm, quarter-bridge strain gage conditioner (part # NI 9944), see Figure 3.7. The conditioners adapted the strain gage wire input to an RJ50 cable output and passed the signal to the channels of a bridge module. Each 24-bit simultaneous bridge module (part # NI 9237) had four channels. The bridge modules connected directly to an NI Compact DAQ chassis (part # 9172) [5]. The bridge could accept up to eight modules, however only three were required in this case. Figure 3.8 shows bridge modules connected to the bridge. 26

38 Labview software was used to acquire and process data retrieved from the NI data acquisition system. This software was used to filter the signal, convert the voltage to a strain output, and write the data to a separate file. Labview was also used in real time to provide feedback for the bolt preload application. The two Labview block diagrams and the associated codes used for the experiment are provided in Appendix A. Figure 3.7: National Instruments Strain Gage Conditioners 27

39 Figure 3.8: National Instruments Bridge and Bridge Modules 3.3 Design of Experiment To properly characterize the bolted joint response to bolt preload and tire pressure, a range of possible load conditions must be considered. For this purpose, a design of experiment (DOE) was proposed. A two by three full factorial DOE was chosen. This design would incorporate two preload values, high and low, and three external loads, high, mid, and low. The actual preload value of the nose wheel bolts for the DeHavilland aircraft was 6,825 lbs. However, this load would produce yielding under the washer in the experimental model. This would make the experiment unrepeatable and the finite element modeling very difficult. Thus, the high preload value was calculated such that no yielding would occur under the washer. The low preload value was chosen to be 10 percent lower than the high preload. The mid value of the external load was calculated 28

40 based on rated tire pressure of the nose wheel and the width of the model. The low and high external loads were 50 percent low and 50 percent high respectively. The calculations were completed and the final values provided by Goodrich. Table 3.2 gives the values of bolt preload and external load for the DOE. DOE Level Preload (lbs) External Load (lbs) Low Mid High Table 3.2: Bolt Preload and External Load Values 3.4 Test Setup and Procedure The final step in the experimental process was the development of the test setup and procedure. Several portions of the test setup have already been discussed, including the experimental model and the measurement system. The external load application method was the final piece of this design. A servo-hydraulic Instron machine (model # 8511) was used as the mechanism for external load application as it was capable of applying varied loads with high repeatability. However, there were several options for connecting the model brackets to the Instron. For example, an extension, such as that seen on the actual wheel rim, could be added to the model s flange and the Instron could apply force to the side of that extension. The more desirable approach was to clamp the ends of the brackets and connect the clamp to the Instron. But again, there were several methods by which to accomplish this goal. In order to conserve the symmetry of the model, it was decided that 29

41 the connecting clamps for the two bracket halves should also be symmetrical. The simplest symmetrical design was found to be a double lap joint. Based on the yield strength of the bracket material, the thickness of the rim flange, and the maximum loading conditions, two bolt-holes were added to the experimental model for attaching the lap joint to the rim flange. This bolt pattern was copied on the flange of a steel block threaded to connect to the Instron. The straps of the lap joint were made of aluminum to reduce the rigidity added to the rim flange by the double lap joint. The thickness of the straps was chosen to be equal to the thickness of the rim flange and was verified based on yield parameters. Figure 3.9 shows the model brackets assembled and connected to the Instron machine. 30

42 Figure 3.9: Final Experimental Assembly There were two main aspects of the experimental procedure, loading and data acquisition. Based on the loading cycle of the aircraft wheel, the preload was applied first followed by the external load. Data was acquired at several times during a single 31

43 loading condition to insure a complete understanding of the effect of loading on the joint. A single loading condition referred to a pair of preload and external load values, so there were six loading conditions required by the design of the experiment. Prior to testing, however, the test setup had to be prepared. First, to insure proper alignment, the brackets were clamped on the two sides of the bolted joint. The bolt was then tightened until the joint closed producing an obvious increase in strain in the bolt shaft as shown by the measurement system. The four bolts of the Instron connectors, kept loose to this point, were then tightened and the clamps on the bolted joint were removed. The model was ready for testing. Preload was applied first based on the real time strain feedback from the bolt shaft. Once the appropriate preload value was achieved, two Labview programs were run; one to save 30 seconds of data from the three bolt strain gages and another to save 30 seconds of data from the eight strain gages on the bracket. With the preload data saved, the Instron was used to apply the desired external force for the loading condition being tested. Once the appropriate force was reached, the Labview programs were run again to save data as before. The external load was then reduced to zero and the programs were run a third time to acquire data to show the difference in preload after external loading. Once the data was acquired, the joint was ready for the next loading condition. The order of loading conditions for a full test is given in Table 3.3. The test was repeated seven times to provide enough data for statistical analysis. 32

44 Condition # Preload External Load 1 Low Low 2 Low Mid 3 Low High 4 High Low 5 High Mid 6 High High Table 3.3: Loading Conditions 33

45 CHAPTER 4 EXPERIMENTAL RESULTS Prior to generating a finite element model of the bolted joint, the experimental data was analyzed. A statistical analysis was performed to verify that the experiment was repeatable and that the results were statistically significant. A design of experiment (DOE) analysis was used to establish an understanding of the bolted joint response to loading. A supplemental analysis was performed to show that the method of bolt preloading was repeatable. The bolt bending stress was analyzed to further highlight the joint s response to the various loading conditions. Finally, the experimental results were compiled into a baseline data set for comparison against the finite element results. Initially, the test was only replicated three times. Analysis of this data revealed an anomaly where the third set of data was drastically different from the first two. The test was then repeated four more times to establish the validity of the results. A review of the seven data sets revealed that the first two data sets were different from the last five. Several potential causes of this discrepancy were considered including yielding under the washer, misalignment of the bolt or washers, stretching in the bolt, and the orientation of the bolt strain gages with respect to the bracket flange. The discrepancy could also have 34

46 been caused by slight modifications made as the operator became more familiar with the test setup, equipment, and method. Regardless, the first two runs were considered joint conditioning and were removed from the final data set. This decision was supported by the agreement between the last five data sets. 4.1 Statistical Analysis of Experimental Results The five final data sets were statistically analyzed to verify their validity. The time series stability and the normality of the data signals were validated. Figure 4.1 and Figure 4.2 show representative plots of the general and worst case time series respectively. The maximum, minimum, and mean values are shown by the horizontal lines on each plot with the data values shown on the right axis. The standard deviations are printed on the plots as well. The range of the strain measurement was less than six microstrains for every case. This was considered acceptable since the range was several orders of magnitude smaller than the measured values. In most cases, represented by the general plot, there was little drift in the strain measurement over 40 seconds of data acquisition. Thus, the mean in these cases was readily acceptable. At certain locations under higher loading conditions, more drift was seen as in Figure 4.2. This could have been caused by the method of load application utilized. The ideal method would have used the Instron to directly control the applied load. Due to constraints created by the test setup, a position control method was implemented instead. This control method resulted in a slight downward drift in load over time, which may have translated to the strain results at more sensitive locations. 35

47 Another possible source of drift was relaxation in the bolt or in the joint over time. Given that the overall data range remained within six microstrains, the mean strains were again considered acceptable. Mating Face Radius 6 O'clock Location Strain (microstrains) St. Dev. = Time (seconds) Figure 4.1: General Time Series Plot and Statistics 36

48 Mating Face Radius 3 O'clock Location Strain (microstrains) St. Dev. = Time (seconds) Figure 4.2: Worst Case Time Series Plot and Statistics The strain results were also checked for normality. In general, the strain results were found to be normal, as shown in the representative normality plot of Figure 4.3. The normality test used was the Anderson-Darling method. Thus, a p-value greater than 0.05 was indicative of a normal distribution. There were a couple of cases where the strain results were found to be non-normal. However, the abnormalities were associated with the previously described drift and were considered inconsequential. 37

49 Percent Probability Plot of Mating Face Radius 6 O'clock Location Normal Mean 1386 StDev N 669 AD P-Value Strain (microstrains) Figure 4.3: Representative Normality Test 4.2 Design of Experiment Results A DOE was performed based on the results of the experiment. The intent of the DOE was to provide a statistically based understanding of the bolted joint response to the various loading conditions. The two main factors were preload and external load. External load, applied by an Instron machine, was easily adjusted. The preload level, however, was statistically difficult to adjust as the method required the operator to manually adjust the load using a wrench while monitoring the real time output of the bolt shaft strain gages. Thus, a split plot DOE was applied. The preload level was set and the 38

50 three external loads were tested. The preload level was then adjusted and the three external loads were tested again. This was repeated for a total of five tests. It was expected that the DOE would indicate preload and external load both as main effects at each gage location. It was also expected that preload would have a more drastic effect on the bolted joint. The external load, being of a lower magnitude, was expected to have a lesser effect. Some interaction was expected between preload and external load as well. Figure 4.4 shows the main effect and interaction plots for the three gage locations on the mating face radius. The term column referred to the effect or interaction of effects being considered in that row, while the charts next to the term columns illustrated the magnitudes of the effects. Any effect whose bar fell outside the blue boundary lines was considered statistically meaningful. The magnitude of each effect or interaction is indicated by the contrast value. The individual p-values indicated whether or not a term could be considered a main effect. A low p-value corresponded to a main effect while a high p-value indicated that the term was statistically insignificant. The main effects are highlighted in black in the term column. See Appendix D for more outputs of the DOE analysis. 39

51 Figure 4.4: Main Effect DOE Results As expected, preload, external load, and the interaction between the two were found to be main effects at most gage locations. However, the greater magnitude of the external load effect, indicated by the squared main effect (external load*external load), was not expected. The magnitude of both preloads by comparison to the high external load led to the expectation that the preload would have a greater effect on the bolted joint. Further inspection revealed that the effect of the external load was magnified by the mechanical advantage generated by the lever arm between the rim flange and the bolted joint. The bending moment generated by this lever arm resulted in bending across the three o clock strain gage location. This allowed the external load to overcome the preload, which was 40

52 seen during the experiment in the separation of the joint between the rim flanges. Thus, the statistical insignificance of preload at the three o clock location was caused by the overwhelming effect of this bending moment across the three o clock location. The moment passing through the three o clock location explained the increased strains at this gage location as well as the reduced effect of the preload on those strains. The increased strains spread into the twelve o clock gage location as well, particularly under higher external load conditions. However, the external load did not completely overwhelm the effect of preload at this location. Preload was also a main effect at the six o clock gage location where the external load had the least effect. This was explained by analyzing the joint in terms of the bending moment. The six o clock location was closer to the fulcrum of the bending moment. Thus, the strains in this location were not as drastically affected by the external load as were the other locations. This was supported by the free body diagram of the system shown in Figure 4.5. Looking at the left bracket in the diagram, there were three forces acting on the model: external load, preload, and the reaction force generated by the second bracket. Assuming the three loads were equally spaced from one another at a distance of L, the resulting force and moment equations are shown in the bottom left of the figure. The calculations indicated that the preload could be equated to two times the external load and that the reaction force was equivalent to the external load. The mating face was then viewed as a simply supported beam, shown at the bottom right of the figure. The beam was found to be supported by the external load and the reaction force with the equivalent preload acting at the center. The center load of two times the external load resulted in a moment 41

53 on the beam that was greatest at the location of preload application. Looking back at the free body diagram showed this center location corresponding to the three o clock strain gage location with six o clock being closer to the pin-joint, or fulcrum, and twelve o clock being further from the fulcrum. Thus, the highest strain in the mating face radius was expected to occur at the three o clock location. The twelve and six o clock strains were also expected to be comparable to one another. Figure 4.5: Free Body Diagram of Model 4.3 Preload Variability Study During testing, some variability was noticed in the preload application. The method for preloading the bolt was to torque the bolt with a ratchet. The bolt was tightened until 42

54 the average strain in the bolt shaft reached the strain necessary to produce the desired load. This method was potentially inexact. Thus a study was needed to insure that the variation was within acceptable limits. A very simple method was used for the study. The same basic test setup was used as in the actual experiment, though no external force was applied. The bolt was preloaded to each of the two levels of interest. The preload was applied via the same method as in the actual experiment. Strain measurements were taken at each preload level. The test was repeated three times. Figure 4.6 shows the average equivalent Von Mises strain, in microstrains, for the low and high preload values. All three replicates were included to show the repeatability. The data was also separated by the three bolt shaft strain gages to show any variations between them. The replicates were indicated by colors and the different gages were indicated by symbol shape. 43 Figure 4.6: Results of the Preload Variability Study

55 The maximum range across the three replicates for any of the gage locations was only about 30 microstrains. The difference between the averages of the two levels was 106 microstrains. Dividing the variance of the group means (106 microstrains) by the mean of the within-group variances (30 microstrains) resulted in an F-value of approximately 3.5. A higher F-value indicates better statistical repeatability. The F-value of 3.5 indicated that the repeatability was adequate, however improvements to the preload application method would be desirable if the testing were repeated. Thus, the results validated the method of preload application. 4.4 Bolt Bending Results The bending stress in the bolt was calculated from the average strain results of the three gages on the bolt shaft for each load condition. See Appendix B for the spreadsheet setup and equations used for the calculation of bolt bending based on three strain gages positioned 120 o apart around the bolt shaft. Table 4.1 shows the bolt bending strain for each of the six loading conditions. The tensile and total strains are included as well. The last row shows the percent of bolt bending strain over total strain. 44

56 Preload Low High External Load Low Mid High Low Mid High Strain (bend) Strain (tensile) 1,460 1,954 2,715 1,617 2,024 2,756 Strain (total) 1,591 2,282 3,520 1,757 2,279 3,492 % Bend/Total 8% 14% 23% 8% 11% 21% Table 4.1: Bolt Bending and Tensile Results The trend across the load cases was expected. The bending increased as the external load increased. This supported the conclusion that the lever arm between the bolted joint and rim flange magnified the effect of the external load on the bolted joint. At the mid and high external loads, the bolt bending stress was greater for the low preload cases. This was expected because the external load had less force to overcome at the lower preload level. At the low external load, the bolt bending stress was greater for the high preload case, which indicated that the low external load did not overcome the bolt preload as overwhelmingly as the higher external loads. This trend was supported by the fact that the low external load did not visibly separate the bolted joint during testing. 4.5 Experimental Data for Finite Element Comparison Table 4.2 presents the average strain results, in microstrains, for the various gage locations around the mating face radius when only preload was applied to the bolted joint. The preload conditions were included in the rows of the table and the external load conditions were included in the columns. Table 4.3 presents the final set of data taken for 45

57 the six loading conditions at each mating face radius strain gage location. Both data sets were taken from the average of the last five replicates. The values of each replicate were assumed to be the mean of all data points taken during the appropriate run. The values presented here were used as the baseline for comparison against the finite element analyses. See Appendix C for tables of raw experimental data. Table 4.2: Results at Mating Face Radius Locations for Preload Only (microstrain) Table 4.3: Results at Mating Face Radius Locations (microstrain) 46

58 CHAPTER 5 FINITE ELEMENT MODELING Once the experimental baseline was established, a finite element model was needed for comparison. A preliminary model was developed based on the experimental design. An iterative process was used to establish the effect of various parameters on the results. The parameters included contact area, mesh symmetry, contact friction, boundary conditions, and rigid body elements (RBE). The model was then updated to incorporate the knowledge gained from the preliminary analysis as well as more accurate geometry. The updated geometry was based on the dimensions of the actual experimental brackets which were not exactly the same as those defined by the design. The model was then used to investigate the effects of other parameters on the bolted joint finite element results. These included mesh refinement, material properties, load accuracy, and the inclusion of washers in the assembly. 47

59 5.1 Preliminary Model Setup Initially, MSC.Patran and MSC.Marc were used to mesh and analyze the bolted joint with HEX8 isoparametric (brick) elements. However, the meshing method and computation time required for even the simple single bolted joint made this model infeasible. The results of research with this model would not have been readily related to Goodrich s more complex models either, as the modeling method and software were drastically different from Goodrich s methods. A new approach was needed to improve the relationship between the FE model of the single bolted joint and the actual multi-joint models required by Goodrich. Thus, the preliminary model was developed in UG NX 5.0, the FE package employed by Goodrich. This model was meshed with ten node tetrahedral elements as the geometry of an actual wheel model would require. Figure 5.1 shows the general model and mesh used in the preliminary finite element analysis. Both brackets were included in the model; however the rim flanges were shortened to exclude the Instron connectors. The assumption was made that the stiffness of these connectors could be adequately modeled by boundary conditions such as fixed surfaces or sliders. The washers and bolt were also excluded from the preliminary model to simplify the development process. The simplified model was used to understand and verify boundary conditions, contact application, and other finite element parameters with a readily modifiable model and a low computation time. 48

60 49 Figure 5.1: General Preliminary Model 49

61 As previously mentioned, the model was meshed with 10-noded tetrahedral elements. A 1D beam element was used to represent the bolt because a bolt preloading tool was available in UG NX for use on this element type. The beam element, centered on the axis of the bolt shaft, was connected to the bracket body using an array of 1D rigid body elements of class three (RBE3 s). These elements were connected to every node within the projected washer contact area on the surface of the bracket. Table 5.1 gives the material properties applied to the brackets and to the bolt element. 0D spring elements with unit stiffness in all six degrees of freedom, called c-bush spring-to-ground elements, were applied to four nodes on each rim flange. These elements were intended to prevent potential unconstrained rigid body modes. Part Material Young s Poisson s Density Modulus (psi) Ratio (lbm/in 3 ) Bracket Aluminum 10.2e Bolt Steel 29e Washer Steel 29e Table 5.1: Material Properties Once the mesh was generated, boundary conditions and loads were applied to simulate the conditions of the experimental setup as shown in Table 5.2. To remove the potential for rigid body motion, the end of one rim flange was fixed in the three translational degrees of freedom (shown in bright green). The external force was applied evenly to the end of the other bracket (shown in orange) under the assumption that the law of equal and opposite reaction would supply the load on the fixed bracket. Rigid 50

62 sliders were applied to the sides of the unfixed rim flange to simulate the motion constraints of the Instron in testing (shown in bright pink). Figure 5.3 illustrates the mating face contact area and the bolt preload. Contact was applied between the mating faces of the two brackets (shown in blue). Though the contact is shown by spots in the figure, the actual contact is made evenly across the entire surface area. The initial model utilized linear contact with an arbitrary friction coefficient of The bolt preload (shown in red) was applied to the beam element (shown in yellow) via the bolt preload tool in UG NX. This tool applied the preload before the external load during the analysis process. Rigid body element spiders (shown in deep green) were used to connect the ends of the bolt beam to every node in the washer contact area on each bracket. 51

63 Long Slider Length Mid Slider Length Short Slider Length 52 Figure 5.2: General Finite Element Boundary Conditions and Loads 52

64 Figure 5.3: Internal Finite Element Boundary Conditions and Loads 5.2 Preliminary Finite Element Analysis An iterative process was then used to establish the effect of certain finite element model parameters on the preliminary analysis. The first parameter considered was the contact area at the mating face. The initial model included both the flat surface of the mating faces and a portion of the mating face radii. The principal maximum strain results were analyzed at the strain gage locations around the mating face radius of each bracket. A comparison of the results for the two brackets showed an interesting phenomenon. While results for the bracket with the force applied to it were on the same order as the 53

65 experimental strains, the results taken from the bracket with the fixed end were drastically lower. An investigation of the cause of this issue revealed that the contact area was at fault. When the contact area was reduced to include only the flat surfaces of the mating faces, the results were found to be much more closely related. Though the modified contact area resolved the drastic differences between the two brackets, slight discrepancies were still found in the results. Differences between the strains at the three and nine o clock mating face radius gage locations for a single bracket were of particular interest. Since the boundary conditions and loads were applied symmetrically to the system, the results should have been equivalent. The results at a single gage location for both plates demonstrated a similar error. It was found that asymmetry in the mesh, though minor, would affect the symmetry of the results. The asymmetry resulted from the meshing method which used a 2D paved surface mesh to seed, or enforce a mesh distribution, in the 3D mesh. The order in which surfaces were paved, the number of surfaces paved, and the built-in paving tool used could affect the symmetry of the resulting 3D mesh. This issue was resolved by improving the symmetry of the 2D seed meshes. Using the model with the improved contact area and mesh symmetry, the effect of changing the coefficient of contact friction was analyzed. The initial coefficient of 0.05 was chosen arbitrarily to minimize friction. The modified friction coefficient was chosen based on the aluminum-to-aluminum contact to be The model was analyzed with this value and the results were equivalent to those of the initial model. Friction coefficient did not affect the response of the bolted joint. 54

66 The next adjustments to the model focused on the boundary conditions. First, the fixed constraint was moved from the end surface of the rim flange to the upper and lower surfaces of the end partition. Refer to Figure 5.2 for visual definition of the end partition. This change did not affect the results. Next, the length of the flange included in the slider constraint was considered. Both longer and shorter sliders were used with the initial slider being of a middle length. Figure 5.2 shows the three slider lengths along the edge of one flange. It was found that increasing the slider length increased the bending in the rim flange unrealistically and reduced the correlation to the experimental results. However, the shorter slider had no appreciable effect on the results. Thus, it was concluded that the slider length in the initial model, the mid length, was acceptable. Finally, the model was analyzed with the sliders and external force applied on both rim flanges instead of fixing one end. This version resulted in equivalent strains to those of the initial model. The last parameter changed in the preliminary analysis was the class of the rigid body elements (RBE s) used to connect the bolt beam to the washer contact area. The two available classes were RBE2 and RBE3. Both element types can be used to distribute a load between two bodies. The RBE2 s are typically applied to mitigate solution errors caused by large discrepancies between the stiffness of two adjoining bodies. While this might be necessary in some cases, it ultimately adds stiffness to the overall model. RBE3 s are not intended to mitigate stiffness differences, and thus do not add stiffness to the model. The RBE3 s were chosen for the initial model because these elements would not affect the overall model stiffness as would the RBE2 s. No large variations in 55

67 stiffness were expected between bodies, so RBE2 s were not necessary. It was also expected that the less rigid RBE3 s would more realistically simulate the interaction between the bolt, washer, and bracket. It was found that the class 2 elements reduced the correlation between the finite element and experimental models significantly. The reduced correlation coupled with the expectation that the class 3 RBE s would better represent the actual stiffness of the bolt led to the decision to use RBE3 s in the final model. 5.3 Final Finite Element Model Setup Upon completion of the preliminary analysis, the assembly parts were updated to incorporate the exact geometry of the experimental brackets still excluding the Instron connectors. While the majority of the bracket dimensions matched the design, the grip length of the brackets, the width of material through which the bolt passes in the bolted joint, had been shortened in the actual unit do to a machining error. With the updated geometry, the finite element model was developed to incorporate some of the lessons learned from the preliminary analysis. Specifically, the model was developed with attention to the mesh symmetry around the bolt hole and between the two brackets. The contact area between the brackets included only the flat surfaces and the coefficient of friction was held at The boundary conditions included the external force and sliders on both rim flanges to improve the symmetry of the model. Finally, the class 3 rigid body elements were used to connect the bolt to the brackets as these seemed to more closely simulate an actual bolt. 56

68 Once the final model was developed, it was used to test the effect of several parameters on the correlation to the experimental baseline. The first of these was the refinement of the mesh. Specifically, the mesh refinement was only considered potentially significant in the contact area and where measurements were needed. Thus, the mesh was refined at the mating faces and around the mating face radii. The mesh remained less refined throughout the remainder of the model to improve the computational efficiency. The initial mating face and mating face radius meshes were based on an element size of 0.1 in. To achieve a relatively refined mesh, the element size in these areas was decreased to approximately 0.05 in. Figure 5.4 illustrates the difference between the refined and unrefined meshes at the mating face and mating face radius. 57

69 58 Unrefined Refined Figure 5.4: Mesh Refinement Comparison 58

70 Next, several potential discrepancies were identified in the material properties, specifically the modulus of elasticity, of both the bracket and bolt materials. First, the modulus of elasticity of the bracket aluminum (7050-T7351) was called into question. It was discovered that the manufacturer s specification of 10.3e6 psi differed from the specification typically used by Goodrich, 10.2e6 psi. A value of 10.0e6 psi was also chosen arbitrarily to further the understanding of this parameter. The modulus of elasticity of the bolt was also varied based on a different concept. It was recommended that the reduced bolt length due to the exclusion of the bolt head, the nut, and the washers could affect the resulting stiffness of the bolt in the model. The inclusion of threads in the loaded section of the bolt shaft could also serve to reduce the stiffness of the bolt. Based on the knowledge of Goodrich s bolt structures expert, the modulus of elasticity was reduced by four percent, to a value of 27.9e6 psi, as a way to counter the effect of threads in the loaded portion of the bolt shaft. The model was also analyzed with the bolt modulus reduced by 40 percent. This represented the worst case scenario; taking into account the difference in bolt length, the exclusion of stiffening material in the bolt head and nut, and the inclusion of threads in the loaded section of the shaft. The resulting worst case modulus of elasticity was 17.4e6 psi. Table 5.2 shows the various combinations of material properties used to characterize the effect of varying the modulus of elasticity of the bracket and of the bolt on the resulting mating face radius strains. 59

71 Modulus of Elasticity (psi) Bracket Bolt 10.2e6 17.4e6 10.2e6 27.9e6 10.2e6 29.0e6 10.3e6 29.0e6 10.0e6 29.0e6 Table 5.2: Material Property Combinations Another potential source of error between the finite element and experimental models was the accuracy of the loads applied during experimentation. This possible inaccuracy applied to both the external load and bolt preload. To characterize this parameter, the external load was first increased and then decreased by 50 lbs for each load case. The preload values were maintained for these analyses. The new external load values are given in Table 5.3. The preload values also offered some potential discrepancies. First, it was recognized that the experimental preload was slightly decreased after the external load was removed. The average experimental bolt preloads were calculated for the high and low preloads after the external load had been applied and removed. These values were then used in the six load cases with the original external loads. It was also noted that the original preloads applied in the finite element model resulted in significantly lower strains than the experiment at the mating face radius strain gage locations. The preloads were increased until the mating face radius finite element results matched the average results from the experiment within one percent. The six load cases were repeated with the increased preloads and the original external loads. Table 5.4 provides the new preload values analyzed. 60

72 Model External Load (lbs) Case Low Mid High Original lbs lbs Table 5.3: Adjusted External Loads Bolt Preload Model Case (lbs) Low High Original Post-External Load Matching Experimental MFR Table 5.4: Adjusted Bolt Preloads The final step was to analyze the model with washers incorporated into the assembly. To accomplish this, the model was regenerated from scratch with two shouldered washers, one on each side of the bolted joint. The bolt beam and RBE3 s were adjusted such that the bolt length included the washers and the RBE3 s connected the bolt to the faces of the washers instead of to the bracket. Contact was applied between the washer and the bracket face as well as between the shoulder of the washer and the inside of the bolt hole. The friction coefficient of 0.05 was used in this case as well. Figure 5.5 illustrates the meshed model with the washers. 61

73 Figure 5.5: Model with Washers 62

74 CHAPTER 6 FINITE ELEMENT RESULTS 6.1 Finite Element Results Acquisition Strain results were extracted from the finite element models at the three experimental strain gage locations around the mating face radius; twelve, three, and six o clock. These locations are identified in Figure 6.1. Two methods were available for extracting strain data. The first was to take the value of the single node corresponding to the center of the experimental strain gage. This is shown at the top of Figure 6.1. The second method was to take an average of the strains for several nodes immediately surrounding the center of the strain gage location. This method was tested using a refined mesh such that the area covered by the averaged nodes would more closely represent the dimensions of the strain gage. See the bottom of Figure 6.1 for a representation of the averaging method. Ultimately, it was found that the results of both methods were comparable. Thus, the single node method was used to simplify the data acquisition process. The single node results for each gage location were averaged between the two brackets to obtain the final data values. See Appendix E for data values for all strain gage locations and models. 63

75 12:00 3:00 6:00 Figure 6.1: Finite Element Strain Measurements 6.2 Finite Element Convergence A brief study was performed to verify that the selected mesh refinement represented a fully converged solution. The initial mesh is illustrated at the top of Figure 6.3 while a 64

76 doubly refined mesh is shown at the bottom. Both meshes show the principal maximum strain contours. The general trends in the strain results were found to be comparable between the two meshes. The less refined mesh did not appear to disrupt the flow of the strain distribution. Individual nodal results showed a slight, one to two percent, variation in strain between the two refinements. Thus, the mesh was further refined and analyzed. The second refinement showed no appreciable change to the strain results. Thus, the results had converged. Furthermore, the difference between the strains in the first two meshes was found to be negligible by comparison to the 500+ percent change in computation time. Thus, the mesh shown at the top of Figure 6.2 was acceptable for this study. 65

77 Figure 6.2: Mesh Refinement Comparison 66

78 6.3 General Finite Element Results Figure 6.3 illustrates the strain trends around the mating face radii across the various load conditions for the general finite element model. All six plots use the same fringe plot color scale. The top three renderings depict the three external load cases under low preload. The bottom plots show the three external load cases under high preload. In all cases, the highest strains occurred across the three o clock gage location. This is expected as the joint bends through this region. The strain appeared to spread into the twelve o clock location at higher external loads. The results also showed that the external loading had a greater effect on the results than the change from low to high preload. Overall, the trends represented in the finite element results correlated to the experimental trends. However, there were discrepancies between the strain values. 67

79 68 Figure 6.3: Sample Finite Element Results (Six Load Cases) 68

80 CHAPTER 7 FINITE ELEMENT AND EXPERIMENTAL COMPARISON Prior to modeling the bolted joint in finite element form, several parameters were identified that could have an effect on the correlation between the model and the experimental baseline. Several of these parameters were tested during the development of the finite element model. These included mesh symmetry, boundary conditions, contact area, contact friction, and RBE class. Based on the new understanding, an improved model was developed to investigate several key factors. These included mesh refinement, material properties, load accuracy, and the inclusion of solid washers in the assembly. The average maximum principal strains were taken for each analysis at the three mating face radius strain gage locations and were recorded in units of microstrains. A vector field plot, shown in Figure 7.1, was used to verify that the principal maximum strain flow around each mating face radius gage location was in the direction of the appropriate experimental strain gage. The results of the analyses were then compared against the experimental baseline to highlight the effects of the parameters on the correlation and, ultimately, on the bolted joint. 69

81 Figure 7.1: Zoomed Strain Flow Contour of Mating Face Radius The first step in the analysis process was to establish a base correlation. Thus, the results of the base finite element model were compared against the experimental data. Figure 7.2 is a set of plots showing the maximum principal strains from the experimental and finite element analyses. The three plots show the results for each of the mating face radius gage locations and include all six load cases. The percent difference between the finite element and experimental results are included for each data set. 70

82 71 Figure 7.2: Comparison of Baseline Experimental and Finite Element Results 71

83 The three o clock gage location showed the best correlation with less than ten percent difference for all load cases. The correlation at all three gage locations appeared to be the worst when the low external load was applied regardless of the value of preload. The correlation improved as the external load increased leading to more acceptable correlations when the high external load was applied. One possible explanation for this external loading trend increased noise passed to the strain gages under lower loading. However, it was also considered possible that this trend was created by an inadequacy in the setup of the finite element model. Thus, a modification to the finite element model that would improve the correlation would need to affect the bolted joint more under lower external loading. The first factor considered was the refinement of the mesh in the mating faces and mating face radii. Since less separation occurred in the bolted joint under lower external loads, more contact would be maintained between the mating faces for the low external load cases. Thus, the refinement of the mesh had the potential to affect the lower external load cases more than the mid or high cases. It was also important to verify that the coarse mesh was not distorting the strain results. Thus, the refinement of the mesh was doubled in the mating faces and mating face radii of both brackets. The results and percent differences were added to the baseline plot with the experimental and unrefined data. The new plot is shown in Figure

84 73 Figure 7.3: Effect of Mesh Refinement on Correlation 73

85 In most cases, the refined mesh only improved the correlation by one or two percent. The greatest improvement, three or four percent difference, was seen at the three o clock gage location. However, the correlation at this location was already within ten percent of the experimental results. Further, it was found that the refined mesh improved each load case similarly at a given strain gage location. Finally, while the refined mesh led to a slight improvement in the correlation to the experimental model, the computational expense was great. The unrefined model ran in about seven minutes where the model with the refined mesh took around 40 minutes. Though this was feasible for the single bolted joint model, it would not be as reasonable in a large, multi-joint model. Thus, it was decided that the element size of 0.1 in. used for the base finite element model was allowable for a bolted joint analysis. The next parameter modified was the material stiffness (young s modulus of elasticity) applied to the bolt. The method of modeling the bolt in the finite element model was to generate a round beam element with the cross-section of the actual bolt and length equivalent to the grip length of the joint. The beam was connected to the bracket via rigid body elements and a preload was applied using the bolt preload tool. The base finite element model assumed the stiffness of the beam was equivalent to the material stiffness of the steel bolt (E = 29.0e6 psi). However, this did not account for the shortened bolt length, the exclusion of the bolt head, washers, and nut, or the inclusion of threads in the loaded region of the bolt shaft. Each of these factors would serve to reduce the stiffness of the bolt. Thus, the modulus was reduced to 27.9e6 psi to represent the best case stiffness reduction accounting only for the inclusion of threads in the loaded length of the shaft. Another analysis, with a modulus of 17.4e6 psi represented the 74

86 worst case taking into account the change in length, the threaded region of the shaft, and the reduction in mass due to the exclusion of the bolt head, washers, and nut. Figure 7.4 compares the resulting strains of the three finite element analyses against the experimental baseline. 75

87 76 Figure 7.4: Effect of Bolt Material Stiffness 76

88 The four percent reduction from 29.0e6 to 27.9e6 psi had no appreciable effect on the resulting strains in the mating face radius. The 40 percent reduction to 17.4e6 psi also had no appreciable effect at the low external load. However, there was a slight effect when the high external load was applied. Figure 7.5 shows the bolt stiffness plots zoomed on the high external load cases. Interestingly, the reduced bolt stiffness improved the correlation at the three and six o clock gage locations by about 50 microstrains, but worsened that of the 12 o clock location by the same amount. The modified bolt stiffness seemed to degrade the response of the bolted joint by comparison to the experimental response. Thus, the original material property of E = 29.0e6 psi was found to be the most feasible. 77

89 78 Figure 7.5: Zoomed Plot of Effect of Bolt Material Stiffness 78

90 The bracket material stiffness was another potential source of error between the finite element and experimental models. The base finite element model used a young s modulus of 10.2e6 psi, the value typically employed by Goodrich for that type of aluminum. The material supplier, however, specified a modulus of 10.3e6 psi. In order to fully characterize the effect of bracket material stiffness, a lower modulus of 10.0e6 psi was analyzed as well. The results of these three analyses are provided in Figure

91 80 Figure 7.6: Effect of Bracket Material Stiffness 80

92 Increasing the modulus by 100 ksi had only a slight effect, if any, on the strains in the mating face radius. The effect, though minimal, reduced the correlation to the experimental results. Thus, it was decided that Goodrich s typical material property specifications were more reasonable for the bracket aluminum. In general, the reducing the stiffness by 200 ksi served to improve the correlation by only one or two percent. The change in bracket material properties affected all the load cases similarly. Thus, it was not found to be the factor causing the discrepancies between low and high external load cases. The results gave no justification for modifying the bracket modulus from the original specification. Figure 7.7 shows a zoomed view of the bracket modulus comparison plot for clarification. 81

93 82 Figure 7.7: Zoomed Plot of Effect of Bracket Material Stiffness 82

94 The next parameter that might affect the bolted joint strains was the accuracy of the external loads applied during experimentation. Specifically, the indirect method of controlling the Instron load via displacement control left some room for experimental error. However, based on the digital load read-out of the Instron, it was not expected that the load would fluctuate more than a few pounds. For the initial characterization, a much higher load fluctuation was chosen to highlight any potential effects on the correlation to the finite element results. Thus, analyses were performed with 50 lbs added to and subtracted from the original external load values. Figure 7.8 shows the results from the adjusted external loads compared against the experimental results and those of the base finite element model. 83

95 84 Figure 7.8: Effect of Adjusted External Loads 84

96 In general, the results showed a very low sensitivity to the accuracy of the external load. The three o clock strain gage location showed a slightly higher sensitivity. This was expected since the external load caused bending across this gage location which increased the magnitude of the strains in this region as compared to the other two gage locations. The variations created by the adjusted external loads were also expected. The decreased external loads resulted in lower strains everywhere in the model which reduced the correlation. Increasing the load resulted in the reverse. The external load adjustments affected each load case similarly indicating that inaccuracies in the external loads were not the cause of the discrepancies between the low and high external load cases. Figure 7.9 highlights the variations caused by the external load modifications. 85

97 86 Figure 7.9: Zoomed Plot of Effect of Adjusted External Loads 86

98 The next factor of interest was the value of the bolt preload. The base model used the original values of preload that were applied to the experimental model at the beginning of each load case. However, the value of preload applied was different from that measured after the external load was applied during experimentation. The preload values were reduced to the average preloads measured after external loading. During the finite element analysis process, it was recognized that the strains resulting around the mating face radius from preload with no external loading were 22 to 23 percent lower than those measured during experimentation. Thus, a finite element model was analyzed with the preloads increased such that the strains in the mating face radius more closely approximated those of the experimental results. Figure 7.10 compares the results of the two modified preload cases to the experimental and base finite element results. 87

99 88 Figure 7.10: Effect of Preload Modifications 88

100 The reduced preload had little to no effect on the resulting strains in the mating face radius for most cases, particularly at the three o clock gage location. The correlations for the low external load cases at the twelve and six o clock locations were slightly reduced. This indicated that the low external load cases might be more affected by modifications to the preload than the mid and high cases, which was the desired trend for improvement of the overall correlation to the experimental data. This theory was corroborated by the increased preload results. When the preloads were increased by 22 percent to match the experimental preload results, the correlations improved drastically, particularly for the low external load cases. All of the correlations were found to be within ten percent difference of the experimental results. Looking at the two most important locations, twelve and three o clock, the correlations are within six percent. Thus, the finite element model appeared to be very sensitive to the preload values. Finally, the finite element model was adjusted to incorporate solid washers into the assembly. The bolt beam was then connected to the outer surface of the washers with rigid body elements. Contact was generated between the washers and the bracket faces. Contact was also utilized between the washer shoulders and the inside surface of the bolt holes to prevent the washers from translating. Spring-to-ground elements prevented the washers from rotating. Figure 7.11 shows the results of this model compared against those of the experimental and original finite element models. The inclusion of solid washers reduced the correlation to the experimental results at the twelve and six o clock locations. The three o clock gage location was not significantly impacted. It was inferred from this result that the inclusion of solid bolts would generate a similar response. 89

101 90 Figure 7.11: Effect of Solid Washer 90

102 CHAPTER 8 SUMMARY AND CONCLUSIONS An experiment was performed to establish a baseline data set for use in the study. This baseline was considered during both the finite element model development and the finite element results analysis. Several basic finite element parameters were tested during the development phase. These included mesh symmetry, boundary conditions, contact area, contact friction, and rigid body element class. A final model was developed based on these results. The model was used to understand the effect of mesh refinement, material properties, load accuracy, and the inclusion of solid washers in the assembly on the correlation to the experimental baseline. The experiment was conducted such that a total of seven data sets were collected. Anomalies were noticed in the first two data sets collected as compared to the last five. Based on their relative agreement, the last five data sets were averaged to form the experimental baseline. The data was verified statistically. A design of experiment analysis was performed to provide an understanding of the bolted joint. It was found that both preload and external load had significant effects on the bolted joint. However, the effect of the external load was drastically greater than that of the preload. This was 91

103 explained by the lever arm created by the location of the external load application. Bolt bending for the various load conditions was also considered to further the understanding of the bolted joint. During the finite element model development phase, analyses were performed to identify the effect of certain parameters on the strain results. Mesh symmetry and contact area were found to be of particular importance to the model. The mesh needed to be symmetric both across the interfacing brackets and around the bolt holes of each bracket. Mesh seeding, enforcing a symmetric mesh by mapping a surface with 2D element prior to 3D meshing, was used to achieve this symmetry. The strain results were also negatively affected by the curvature of surfaces included in the contact area. It was found that a flat contact area significantly improved the correlation of the results to the experimental baseline. Thus, the mating face radius was excluded from the contact area. Another parameter of importance was the rigid body element class. A comparison of the class two and three elements revealed that the class three elements resulted in a better correlation to the experimental results. Several variations were made to the boundary conditions to verify that the chosen boundary conditions were the best for this study. It was found that the boundary conditions had little effect on the results in the mating face radius so long as they were applied far enough away from the bolted joint. A half inch of the end of the rim flange was found to be an acceptable region for boundary condition application. The spring-to-ground elements were found to reduce the potential for rigid body motion in the analysis without affecting the strain results in the bolted joint. Finally, the coefficient of contact friction had no effect on the results of the analysis. 92

104 The final finite element model was created using knowledge from the developmental analyses. A couple of changes were then made in relation to the mesh. First, the mesh was refined from an element size of 0.1 in. to 0.05 in. in the mating faces and mating face radii. While the refinement did improve the correlation to the experimental results by two to four percent, the computational efficiency of the model was drastically reduced. The 570+ percent increase in computation time would be unacceptable for a multi-joint model. Thus, the element size of 0.1 in. was deemed acceptable for finite element modeling of a bolted joint. The other change to the mesh was the inclusion of solid washers in the model. This change increased the number of contact areas required and the length of the bolt beam. The analysis showed that the inclusion of solid washers in the assembly significantly reduced the correlation to the experimental results at twelve and six o clock. The simpler model had better results and was more computationally efficient. The effect of varying the modulus of elasticity of both the bolt and bracket materials was also characterized via a series of analyses. The reduction of the bolt material stiffness by four percent had no appreciable effect on the resulting strains in the mating face radius. A more drastic reduction, 40 percent, improved the correlation in some cases and reduced the correlation in others. Thus, the overall response to variation in the bolt material stiffness was a degraded response of the bolted joint as compared to the experimental results. Increasing the modulus of elasticity of the bracket material from 10.2e6 to 10.3e6 psi had no appreciable effect on the results. Reducing the modulus by 200 ksi served to improve the correlation for each case by one to two percent. However, 93

105 these results offered no justification for permanently modifying the modulus from the original Goodrich specification. Thus, the modulus of elasticity of the bracket material was kept at 10.2e6 psi. Finally, several adjustments were made to characterize the joint s response to variations in the external load and preload. The external load was characterized by increasing and decreasing the loads by 50 lbs. The results were as expected. Decreasing the load decreased the resulting strains in the mating face radius which corresponded to a decrease in the correlation to the experimental baseline. Increasing the external load resulted in the opposite reaction. However, since each load case and gage location was affected evenly, it was established that the accuracy of the experimental external load was not the cause of the major discrepancies between the finite element and experimental models. The preload characterization was based on preload values reduced to the average experimental preloads measured after external loading and values increased by approximately 22 percent such that the mating face radius strains matched those of the experiment prior to external loading. The reduced preloads had no appreciable effect on the strains in the mating face radius. The increased preloads, however, resulted in a drastic improvement in the overall correlation to the experimental baseline. The correlations for each load case and gage location were within 10 percent difference. More importantly, the correlations were within six percent at the twelve and three o clock gage locations; the locations of greatest import. Thus, the finite element model appeared to be very sensitive to the correlation mating face radius strains under only preload. 94

106 Several conclusions were drawn and verified throughout the course of this research. First, it was found that the external load generated the greatest main effect response. This was corroborated by the simplified free body diagram of the brackets. The external load was also found to have a strong nonlinear effect. This was seen by the drastic increase in strains moving from the mid to high external load by comparison to the much smaller increase moving from the low to mid external load. The DOE also highlighted this effect. While the work performed for this model was verified, it was also possible that the modified joint geometry affected the overall response. Specifically, the increased bolt-hole radius and the broadened mating face could affect the relationship of this model to the aircraft wheel. Analysis of the response in an aircraft wheel bolted joint could resolve this concern. Analysis of actual aircraft wheel bolted joints could also corroborate the preload matching technique that led to the best correlation between experimental and finite element results. This matching technique was introduced for a couple of reasons. First, the finite element model response to preload, with no external load applied, did not appear to adequately represent the experimental response in the mating face radius. Specifically, the strains in the mating face radius were significantly lower at each location in the finite element analysis. Matching these mating face radius strains would lead to a more accurate representation of the experimental bolted joint under both preload and external load. It was also established that the UG NX bolt preloading tool was not clearly understood and that it may not adequately represent an actual bolt preload under the conditions of the model used. Finally, it was known that the preload would have a 95

107 greater effect on the results for the low external loads as opposed to the high external loads. This type of effect was of particular interest since the correlations were much worse under low external loading than under higher external loading. Finally, various best practices were established for finite element modeling of aircraft wheel bolted joints. First, a tetrahedral element size of 0.1 inch gave reasonable accuracy for this application. This mesh density should be verified for wheels of different dimensions and loading. Maintenance of mesh symmetry between the mating faces and around the bolt holes could also significantly improve the model response. When using linear tetrahedral elements, contact areas should be restricted to flat surfaces. The coefficient of contact friction did not appear to be significant for this model; however, it may become significant under torsion loads. Next, it was found that the rigid body elements of class three gave the best correlation to the actual bolted joint given the finite element configuration of the bolt. This might change for different bolt modeling techniques. Furthermore, a reduction in strain should be anticipated when solid bolt or washer elements are introduced into the model. Finally, matching the finite element mating face radius strains to experimental results under the influence of only preload may serve to improve the correlation between simulated and actual results. However, this technique should be verified against experimental results from bolted joint preloading in actual aircraft wheels. Furthermore, the technique should be analyzed for the numerous potential methods of modeling the bolt in finite element form. A set of finite element modeling best practices were developed throughout the course of this research as well. 96

108 This study considered the effect of numerous major finite element parameters on the correlation to experimental results. However, several factors remain that could be included in future studies to improve the understanding of bolted joint finite element modeling. First, the increase in preload to match mating face radius strains needs to be studied further as a potential solution to discrepancies in multi-joint models. Characterization of this phenomenon could lead to improved bolt preload modeling techniques. Along the same lines, comparisons could be made between various methods of applying preload to bolted joints. Some potential preloading methods include the beam element and rigid body elements used in this study, solid bolt ends connected by a beam element in the center with a bolt preload applied to the beam element, and a solid bolt with thermal preloading. Different methods could be used to model the solid bolt. A study could also be performed to understand and validate the UG NX bolt preload tool. Finally, nonlinear finite element modeling in UG NX 6.0 could be compared against the linear modeling used for this study. Nonlinear models could incorporate nonlinear contact and/or material properties. 97

109 LIST OF REFERENCES [1] Dingare, A. D. (2007).Advanced Analysis of Aircraft Bolted Joints. The Ohio State University Master's Thesis. [2] Kim, J, Yoon, J. C., & Kang, B. S. (2007). Finite element analysis and modeling of structure with bolted joints. Applied Mathematical Modelling. 31, [3] Shi, G, Shi, Y. J., Wang, Y. Q., & Bradford, M. A. (2008). Numerical simulation of steel pretensioned bolted end-plate connections of different types and details. Engineering Structures, 30, [4] Ahmed, K. I. E., Rajapakse, R. K. N. D., & Gadala, M. S. (2009). Influence of bolted-joint slippage on the response of transmission towers subjected to frostheave. Advances in Structural Engineering. 12. [5] (2009). National Instruments: NI CompactDAQ. Retrieved January 17, 2009, from National Instruments Web site: 98

110 APPENDICES 99

111 APPENDIX A LABVIEW BLOCK DIAGRAMS AND SETUP 100

112 Figure A.1: Bracket Gage Data Acquisition Block Diagram 101

113 Figure A.2: Bolt Gage Data Acquisition and Averaging Block Diagram 102

114 Figure A.3: Data Acquisition Assistant Configuration 103

115 Figure A.4: Filter Configuration 104

116 APPENDIX B BOLT BENDING CALCULATIONS 105

117 Three (3) Strain Gages Installed 120 Apart on a Shank Strains INPUT ε 1 ε 2 ε 3 Ø ε t ε b Max ε ε b / ε t μ in/in μ in/in μ in/in to NA from μ in/in μ in/in μ in/in ε max =MAX(B7:D7) =B7+C7+D7- B9-D9 =MIN(B7:D7) =ATAN( *(2*B9-C9- D9)/(C9-D9))*180/PI() =(B9+C9+D9)/3 =(2*B9-C9- D9)/(3*SIN(E9*PI()/180)) =F9+G9 =G9/F9 106 Table B.1: Bolt Bending Calculation Spreadsheet 106

118 The yellow cells above indicate the input data. This data was taken from average strain readings for the three strain gages on the bolt shaft. The cells immediately below the highlighted cells sort the three strain gage readings from maximum to minimum. The next five cells use the equations shown to output certain desired values. First, the angle from the maximum gage reading to the neutral axis is calculated. The equation is based on the geometry indicated in the diagram shown at the bottom of the table. Next, the average tensile strain is calculated in column five based on the strain readings. Column six calculates the average bending strain based on the strain readings and the angle to the neutral axis from column four. The total strain (bending plus tensile) is found in column eight. Finally, column nine establishes the ratio of bending to tensile strains. 107

119 APPENDIX C RAW EXPERIMENTAL DATA 108

120 Rep 1 Rep 2 Rep 3 Rep 4 Rep 5 Rep 6 Rep 7 Ave. Reps 3 7 Preload MF Rad. 12:00 Principal Strains (Gage 3 = Min; Gage 7 = Max) (microstrains) Low Mid High SG 3 SG 7 SG 3 SG 7 SG 3 SG 7 Low High Low High Low High Low High Low High Low High Low High Low High Table C.1: Experimental Principal Strains for 12:00 MF Radius Gages 109

121 Rep 1 Rep 2 Rep 3 Rep 4 Rep 5 Rep 6 Rep 7 Ave. Reps 3 7 Preload MF Rad. 3:00 Principal Strains (Gage 4 = Max; Gage 8 = Min) (microstrains) Low Mid High SG 4 SG 8 SG 4 SG 8 SG 4 SG 8 Low High Low High Low High Low High Low High Low High Low High Low High Table C.2: Experimental Principal Strains for 3:00 MF Radius Gages 110

122 MF Rad. 6:00 Principal Strains (Gage 5 = Min; Gage 6 = Max) (microstrains) Low Mid High SG 5 SG 6 SG 5 SG 6 SG 5 SG 6 Rep 1 Rep 2 Rep 3 Rep 4 Rep 5 Rep 6 Rep 7 Ave. Reps 3 7 Preload Low High Low High Low High Low High Low High Low High Low High Low High Table C.3: Experimental Principal Strains for 6:00 MF Radius Gages 111

123 APPENDIX D STATISTICAL RESULTS OF THE DOE 112

124 Run Pattern Preload External Load Microstrain 12 o clock Microstrain 3 o clock Microstrain 6 o clock Table D.1: Experimental Principal Strains for 6:00 MF Radius Gages 113

125 Note: The preload was not randomized due to the method of preload application. Randomization of the order would have introduced too much variability into the experiment. A split-plot design was used where the preload was non-random for each replicate and the external load was random. 114

126 Figure D.1: Detailed Statistical Results for 12 O clock Gage Location 115

127 Figure D.2: Detailed Statistical Results for 3 O clock Gage Location 116

128 Figure D.3: Detailed Statistical Results for 6 O clock Gage Location 117