Citation
Finite Element Analysis and Experimental Verification for Design of a Wind Tunnel Test Stand

Material Information

Title:
Finite Element Analysis and Experimental Verification for Design of a Wind Tunnel Test Stand
Creator:
Buck, Steven
Publication Date:
Language:
English

Subjects

Subjects / Keywords:
Aerodynamic lift ( jstor )
Airfoils ( jstor )
Beams ( jstor )
Design analysis ( jstor )
Inlets ( jstor )
Modeling ( jstor )
Simulations ( jstor )
Streams ( jstor )
Structural deflection ( jstor )
Wedge bodies ( jstor )
Aeroacoustics
Aerodynamic noise
Genre:
Undergraduate Honors Thesis

Notes

Abstract:
The University of Florida Aeroacoustic Flow Facility is designed to acquire acoustic measurements in aerodynamic applications. In taking acoustic data, it is imperative to minimize the noise generation by sources other than the model in question. In the past, a potential source of significant aerodynamic noise and interference was the test stand used to hold models in the open-jet tunnel. The previous test stand had a large portion of its structural components downstream of the inlet. This caused significant aeroacoustic noise generation under certain test conditions, as well as acoustic reflection and scattering. The design task at hand was to create a stand that had all structural members upstream of the inlet plane in order to minimize the surfaces exposed to the flow. An iterative design process was carried out using ProMechanica finite element software to analyze each design. A final design was chosen when no further improvement could be readily achieved, and the predicted deflections were determined to be acceptable. This stand design deflected 0.169” in simulation of estimated maximum loading conditions. After construction of the test stand, an experimental displacement versus load test was conducted, the results of which are compared to simulations. It was found that a discrepancy of 36% was present in the deflection per unit load calculated in the simulations. Future work will be focused on improving results by developing a finite element model of the system that more accurately predicts deflection. ( en )
General Note:
Awarded Bachelor of Science in Aerospace Engineering; Graduated May 3, 2011 magna cum laude. Major: Aerospace Engineering
General Note:
Advisor(s): Dr. Lou Cattafesta
General Note:
College/School: College of Engineering

Record Information

Source Institution:
University of Florida
Holding Location:
University of Florida
Rights Management:
Copyright Steven Buck. Permission granted to the University of Florida to digitize, archive and distribute this item for non-profit research and educational purposes. Any reuse of this item in excess of fair use or other copyright exemptions requires permission of the copyright holder.

Downloads

This item is only available as the following downloads:


Full Text

PAGE 1

1 Finite Element Analysis and Experimental Verification for Design of a Wind Tunnel Test Stand Undergraduate Thesis by Steven Buck University of Florida 2011

PAGE 2

2 Abstract T he University o f Florida Aeroacoustic Fl ow Facility is designed to acquire acoustic measurements in aerodynamic applications. In taking acoustic data, it is imperative to minimize the noise generation by sources other than the model in question. In the pas t, a potential source of significant aerodynamic noise and interference was the test stand used to hold models in the open jet tunnel. The previous test stand had a large portion of its structural components downstream of the inlet. This caused significant aeroacoustic noise generation under certain test conditions as well as acoustic reflection and scattering The design task at hand was to create a stand that had all structural members upstream of the inlet plane in order to minimize the sur faces exposed to the flow An iterative design process was carried out using ProMechanica finite element software to analyze each design A final design was chosen when no further improvement could be readily achieved and the predicted deflections were determined to be acceptable This stand design deflected loading conditions. After construction of the test stand a n experimental displacement versus load test was conducted, the results of which are compared to simulations. It was found that a discrepancy of 36% was present in the deflect ion per unit load calculated in the simulations Future work will be focused on improving results by developing a finite element model of the system that more accurately predicts deflection.

PAGE 3

3 Contents Chapter Page 1. Introduction 4 2. Stand Modification 5 3. Itera tive Design and Analysis 8 3.1. Simulation and Mesh 8 3.2. Loading and Constraints 9 3.3. Equivalent Beams 10 3.4. First Iteration 12 3.5. Second Iteration 14 3.6 Third It eration 15 3.7 Further Atte mpts at Design Improvement 16 3.8. Design Choice 16 4. Physical Testing and Comparison to FEA 18 4.1. Experimental S etup 18 4.2. Comparison of Simulat ion to Experimental Results 20 5. Concluding Statements and Future Work 21 References 23

PAGE 4

4 1. Introduction The University of Florida Aeroacoustic Flow Facility (UFAFF) is an open jet, anechoic wind tunnel designed to take noise data in aerodynamic applications. It is a subsonic wind tunnel facility with a maximum flow speed of 246 ft/sec (75 m/s). The jet dimen s the collector/ walls of the chambe r containing the test section are acoustically treated with fiberglass an echoic wedges in order to attenuate acoustic reflections above 100 Hz and simulate an acoustic free field 1 The tunnel is fitted with a n aeroacoustic silencer in order to filter outside noise and to improve flow uniformity. 2 See Figure 1.1 below. Figure 1.1: UFAFF wind tunnel configuration. Note that several groups of anechoic wedges are hidden for convenience. It was determined that in the testing of certain models, the previous test stand used to secure the models provide s undesirable interaction with the flow field and generate s secondary noise. Specifically, airfoils oriente d at high angles of attack direct the jet flow towards downstream structural members of the stand. In order to mitigate th is effect, a new test stand was designed with all structural members upstream of the inlet plane of the test section. As in the old test stand design, the new, upstream design is constructed of 80/20 6105 T5 aluminum extrusion. This method allows for relative ease of construction and disassembly, as well as Inlet Diffuser Centrifugal Fan Silencer Figure 1.2: Concrete wedge anchors used to secure vertical beams.

PAGE 5

5 allowing alteration of configuration for use with different mod el types. The upstream stand is designed to utilize as many co mponents of the old stand as possible in order to minimize cost of materials. The stand is secured to the concrete floor of the facility via 1/2" diameter, 4" long steel wedge anchors. Four anchors are used to secure each of four vert ical beams as shown in Figure 1.2 The anchors provide a reaction force and moment to prevent deflection of the corners of the stand. The design and experimental procedures are described in more detail in the sections that follow. All results are given and discusse d in depth. Finally, concluding statements contain suggestions for applicability of the new stand and a description of future work to be completed 2. Modification of Test Stand The old structure used to hold models in the stream of the wind tunnel had several large members downstream of the inlet plane of the test section. These members would cause undesirable flow interaction and noise generation, as well as reflecting aerodynamically generated sound. The old s tand design is shown in Figure 2.1 as conf igured for a vertically mounted airfoil (top and bottom bounding plates are not shown for convenience see Figure 2.4 ) This is the model orientation for which the upstream stand is to be primarily utilized. The figure below also depicts the axis directions that will be referenced from this point forth. Figure 2.1: Orientation of old test stand design. Flow Direction Inlet Diffuser 115" 94" 88" x z y 29" 44"

PAGE 6

6 Note the tall vertical beams located downstream of the model These beams are of primary concern when considering flow field disruption and noise generation. Consider the case when the airfoil model shown is oriented a high angle of a ttack as depicted in Figure 2.2 In this scenario, the downwash of the airfoil will potentially interact significantly with the vertical beams This interaction provides unwanted acoustic sources and/or acoustic reflections towards the typical microphone locations shown Figure 2.2: Visual depiction of unwanted flow field interference. Top view. A potential solution to this problem is to utilize a stand with as little structure as possible located in the flow field or acoustically visible to models. The new stand orien tation is depicted in Figure 2.3 below (again without the top and bott om plates shown in Figure 2.4 ) Microphone Location Microphone Location

PAGE 7

7 Figure 2.4: Sidewall foam configuration for sideline measurements. Figure 2. 3 : Orientation of the upstream test stand design. As intended, the upstream design greatly reduces the surfaces that are exposed to the flow as well as to sound radiation. Also note that in the stands in both Figure 2.1 and Figure 2 .3 foam sidewalls are implemented for a coustic and aerodynamic purposes b ut are not shown. The sidewall configuration for the ups tream test stand design is illustrated in Figure 2.4 The stand shown in Figure 2 .3 has less exposed scattering surfaces than are depicted, as the 80/20 supports for the model are blocked by the foam. Flow Direction 115" 94" 36"

PAGE 8

8 3. Iterative Design and Analysis The complex geo metry of the stand to be designed calls for computational analysis i n order to determine deflection and strain for expected loading conditions ProMechanica 3 finite element software is therefore used to analyze stand designs under predicted loading conditions The iterative design proc ess is described in this section That is, simulation of a design resulted in a deflection plot, and adjustments of the design were implemented to try to improve results. The process was then repeated until additional significant improvement could not be readily attained. 3.1 Simulation and Mesh: The structure is modeled as a single fused piece of 6105 T5 aluminum. All members are therefore modeled with 4 EM feature is used to create mesh es for each design with resolutions between 13 0 00 and 15 000 elements. The mesh used for the first iteration is shown in Figure 3.1. Figure 3.1: Mesh used for simulation of first design iteration. The mesh shown has a resolution of 14,977 elements. ProMechanica software uses a p method finite element model, which automatically conducts a convergence study d uri ng simulation. A first pass is conducted with all third order elements Subsequently, a second pass is conducted with higher order elements implemented in

PAGE 9

9 high stress gradient regions. 5 The stress error estimate s based on the convergence study in this design process are equal to or below 5% for all simulations 3.2 Loading and Constraints : The highest common loading that can be expected on the stand from a model is from an airfoil at a high angle of attack with the wind tunnel running at full speed This will induce a lift force in the cross stream direction as well as drag and induced drag in the downstream direction. As a n example high lift scenario, a N ACA 4418 p rofile with its flap deflected to 60 and at a 15 angle of attack is considered. According to Abbott and Doenhoff, t he lift and drag coeffic ients at this angle of attack are approximately 1.5 and 0.02 respectively for a Reynolds number of 3 ,000,000 The pit ching moment coefficient is 0.19 Equations 1 ,2, and 3 are used to calculate lift, drag and the pitching moment respectively 6 (1) (2) (3) Here, o freestream velocity, S is the planform area, c is the While previous studies in the facility have used larger models 7 8 f uture work in the UFAFF will use airf oil models with a maximum chord of 12" in o rder to avoid excessive blockage Furthermore, airfoils mounted to this stand will be vertically mounted and therefore have a maximum wetted span of 29", which is the height of the inlet (see Figure 2 .1). Thus, a chord length of 12 and a span of 29" are used in calculations. The spee d used for load calculations is 246 ft/sec, the maximum speed of the tunnel This scenario possesses a Reynolds number of approximately 1,730,000. T he lift generated by the 4418 is therefore 281 lbf and the drag is 3.7 lbf. The pitching moment is approximately 451 inch lbf. The weight of the model is no t considered as it is directly supported by a 3030 beam and is well within the capabability of that beam. Implementing a factor of safety of at least 2.5 the simulations are run with a lift force L of 1000 lbf and a pitching moment M of 1300 inch lbf. A drag force D of 200 lbf is simulated in order to Figure 3.2: Loading conditions for FEA. D/2 D/2 L/2 L/2 M/2 M/2

PAGE 10

10 fully view the deflection characteristics of the stand. The loads are distributed equally between the two cross stream beams highlighted in Figure 3.2 At this location the lift force create s the maximum pos sible moment on the stand. The constraints of this finite element model are based on several assumptions of ideality The bottom surfaces of the four large vertical beams in Figure 2 .2 are constrained to zero displacement and zero rotation. This essentially assum e s that the L brackets and wedge anchors do not strain under the expected loading. A parametric study concerning this assumption is to be conducted in order to improve the accuracy of the finite element model. In addition, t he horizontal b eam located below the airfoil model, on the floor in Figure 2 .2 is constrained to zero defle ction in the vertical direction, as it will be blocked by the floor. 3.3 Equivalent Beams: The cross section of an 80/20 beam is extremely complex. In order to reduce the required computing time for simulation a n approximately structurally equivalent beam is utilized with simpler, rect angular cross sections. This is achieved by choosing the beam dimensions such that the cross sectional area and neutral axis moment s of inertia for each equivalent beam are matched to the respective 80/20 beam s Thus, based on simple Euler Bernoulli beam calculations, the beams will strain and deflect equivalently under axial stress and bending moments about their neutral axis 9 The beams, however, are not exactly equivalent un der torsion or moments about axi s other tha n the neutral axis of the beams. However, because of the perpendicularity of most elements in the structure, these loads are expected to be negligible Examination of the simulation deflection results in Figure 3.7 confirms this prediction. The process for derivi ng the equivalent beams involves developing equations for moment of inertia and cross sectional area as a function of the dimensional variabl es depicted in Figures 3. 2 through 3.4 For the 3030 profile shown in Figure 3.2 the two unknown dimensions are the thickness t and the height h of the cross section Two equations are developed from moment of inertia about the neutral axis and the cross sectional area. Both of these values for the actual beams are given by 8020 in their catalogue. 4 The equations are derived from the fundamental equation for moment of inertia for a rectangular profile given below 9 (4) Here, I is the moment of inertia about a specified axis, b is the dimension parallel to the axis, h is the dimension perpendicular to the axis, A is the area of the rectangular section, and d is the distance from the center of the rectangular section to the axis. By analyzing the 3030 equivalent

PAGE 11

11 beam in rectangular portions of its cross section and summing the moments of inertia of each, Equation 5 is derived for the total moment of inertia this profile. Note that I x = I y for this profile. (5) The cross sectional area for the 3030 equivalent beam is given by Equation 6. (6) Equati ons 5 and 6 are used t o solve for the thickness and height of the beam cross section. The resulting di mensions are shown in Figure 3.2 The 1530 equiva lent profile shown in Figure 3.3 is developed in a similar ma nner. However, for this profile the width w of 2.77 inches is used such that the beam will coincide with the 3030 equivalent profile derived above The three unknowns are then the two thicknesses t 1 and t 2 and the height h Three equations are developed from I x I y and A which are used to solve for the three unknowns T his process is again used for the 3060 profile taking the 2.77 inch width from the 3030 equivalent profile. Drawings of the three 80/20 beam cross sections and the derived equivalen t beams are shown in Figures 3.2 through 3.4 Figure 3.2 : 30 30 cross section and equivalent rectangular cross section used for simulation. Units are in inches. 4 Figure 3.3 : 15 30 cross section and equivalent rectangular cross section used for simulation. Units are in inches. 4 A=2.08 0 in 2 I x =0.482 in 4 I Y =1.804 in 4 A=3.448 in 2 I x =3.413 in 4 I Y =3.413 in 4 t 1 =0.42 h=1.38 w=2.77 t 2 =0.21 t=0. 36 h = 2.77 t=0. 36 2 w=h=2.77 x y

PAGE 12

12 Figure 3.4 : 306 0 cross section and equivalent rectangular cross section used for simulation. Units are in inches. 4 3.4 First Iteration : The first iteration test stand is designed based on expectations of relatively large loading in the negative z direction due to high lift models. No reinforcement can be provided by the walls or other components of the building due to the nature of the building and of the chamber itself. Thus, re inforcing diagonal elements are us ed to prevent deflection due to lift Drag forces are expected to be rela tively small so less support is provided for deflection downstream. Figure 3 .5 shows the simulation deflection results for the initial design under the loading and boundary conditions described in Section 3.2 The deflections shown are amplified greatly in the image for visual inspection purposes. The units in the c olorbar are inches. Therefore, the maximu m deflection for this design is deflection is the downstream end of top model support beams. A=3.448 in 2 I x =3.413 in 4 I Y =3.413 in 4 w = 2.77 h = 5.54 t 2 = 0.37 t 1 = 0.46

PAGE 13

13 Figure 3 .5 : Displacement results for the first design iteration. F x = 200 lbf, F z = 1000, M y = 1300 inch lbf. The colorbar scale is in inches. The simulation provides valuable insight into some of the designs flaws. As stated above, th e maximum deflection point is at the downstream end of the top model support beams. However, inspection of the image reveals that this is in small part due to deformation of these beams, but rather due to deflection of the large vertical beams These vertical beams each have s ignificant deflection in the x or negative x direction direction. It was apparent that though t he lift force acts in the cross stream direction, it causes streamwise deflection due to the moment it creates on the stand. Essentially, the model support beam s pr ovide a moment arm for the lift force This result makes it clear that support for streamwise deflection will i ncrease the structural rigidity of the stand Note the trapezoid based structure used in the first design. That is, the structure illustrated in Figure 3.5 appears as a trapezoid from above. This geometry does not readily allow for reinforcement against downstream deflection. A rectangle based structure is thus employed for the second design iteration. y x z

PAGE 14

14 3.5 Second Iteration: With a rectangle based structure reinforcement in the streamwise direction is possible by are placed between each pair of vertical b ea ms, as can be seen in Figure 3.6 below. This figure shows the results of the simulation for the revised design. Figure 3.6 : Displacement results for the second design iteration. F x = 200 lbf, F z = 1000, M y = 1300 inch lbf. The colorbar scale is in inches. The maximum displacement for the second design iteration is 47%. The implementation of a rectangular profile and the addition of the diagonal trusses are therefore extremely successful. However, significant def l ection in the vertical beams is still pre sent, as can be seen in the image above This deflection in turn causes a n even higher displacement at the downstream end of the upper model support beams. Further reduction in deflection of the se vertical beams is thus considered to be the goal of the next iteration. y x z

PAGE 15

15 3.6 Third Iteration: To further stiffen the main rectangu lar structure, another truss is inserted between each pair of vertical beams. Thus, three diagon al trusses are located between each pair of vertical beams Figure 3. 7 shows the displacement results of the simulation for this design. Figure 3.7 : Displacement results for the third design iteration. F x = 200 lbf, F z = 1000, M y = 1300 inch lbf. The c olorbar scale is in inches. The simulation yields he addition of the third truss res ults in a reduction in maximum deflection of 32%. The point of maximum deflection is still on the top model support beams. Inspection of the above figure shows that the high deflection at this point is due in part to strain in the model support beams themselves, as well as the deflection in the cross stream beam to which they are attached. y x z

PAGE 16

16 3.7 Further Attempts at Design Improvement : Examination of the results shown in Figure 3.7 led to several further attempts a t design improvement. Examination of the image reveals that the model support beams show discernable deformation. One potential method to reduc e deflection of the se model support beams is by reinforcing them with larger diagonal trusses than are present in the structure of Figure 3.6. Simulation of this design alteration shows a reduction of maximum deflection of less than 8 percent. This magnitu de of improvement is unworthy of the cost of the additional materials. Another option that is considered is to brace the top, upstream corners of the structure to the walls of the wind tunne l chamber. However, this method will not be implemented because of the permanent modifications to the chamber that would be required for implementation and the fact that the chamber walls themselves are freestanding 3.8 Design Choice T he stand design shown in Figure 3.7 is chosen for impleme ntation because of its significantly reduced maximum deflection during simulation compared to other designs The stand is shown as orien ted in the UFAFF in Figure s 3.8 and a 3.9 below. All parts required for construction of the stand are listed in Table 3.1. The stand was constructed in the UFAFF and displacement versus loading tests were conducted as described in the next section Figure 3.8 : Final design of the upstream test stand.

PAGE 17

17 Figure 3.9 : Key dimensions of the upstream stand design. Units are in inches. Table 3.1: Parts list for final test stand design. Part Description Quantity Qty. in Stock 3060 115" 4 4 3030 20" 4 anchors per end 1 0 3030 82" 4 anchors per end 5 5 3030 30" 4 anchors per end 2 0 3030 46" 4 anchors at one end 5 0 3030 46" 4 anchors per end 1 0 3030 12" 4 anchors per end 1 0 1530 24" 45 deg. (trap) 15 15 1530 43.93" 45 deg. (par) 8 0 1530 29" 4 4 1010 29" 2 0 1010 34" 2 anchors per end 6 6 Bolt/anchor assembly 88 88 Bolt/T nut assembly 132 132 Base L brackets 8 8 Concrete wedge anchors 16 16

PAGE 18

18 4. Physical Testing and Comparison to FEA A particular goal of the design process for the upstream test stand is to determine the capabilities of the stand under various loading conditions. In order to d etermine the limits of the stand, the FEA result s must be verified so that predictions could be considered valid. In order to accompl ish this, the physical stand is subjected to various loadings, and the displace ment at a point on the stand is measured for each. The same load ing conditions are then simulated in ProMechanica. A plot of displacement versus load is then developed for both the physi cal and simulated displ acement tests, and comparisons are made. 4.1 Experimental Setup: The load is applied to the stand via the two pulley system shown in Figures 4.1 and 4.2 By applying the tension in the steel cable to the stand twice, t he two pulley system effectively causes a load equal to double the applied weight. The logic behind doubling the load is that a higher deflection allow s for lower error in deflection measurement. The load is applied in the downstream direction The weights applied to the cable are in the form of several improvised objects readily available in t he lab, including a 58 lb. paint can, two 26 lb. lead bricks, and a 13 lb. lead brick. The loads are based on measurements with a ConAIR digital household scale with a resolution of 0.2 lb. Note that this loading configuration is arbitrary, as the same load is implemented in the simulations in order to compare results

PAGE 19

19 Figure 4.1: Schematic of displacement test. Figure 4.2 : Two pulley system implemented for load application. The deflecti on measurements are taken with a Keyence LK G32 non contact laser displacement sensor (LDS) The LG Q32 is rated at an accuracy of + 0.05%. 10 Measurements are able to be read to a resolution of 0.001 mm (3.94e 4 in.). The sensor is placed on a tripod and This setup is shown in Figure 4.3 below. Figure 4.3 : Laser displaceme nt sensor configuration. Pulley 1 Pulley 2 Load Application

PAGE 20

20 4.2 Comparison of Simulation to Experimental Results Simulations are run replicating the load conditions from the physical displacement tests. In the simulations the boundary conditions are the same as described in Section 3.2. The load is applied in the downstream d irection and acts on the cross stream beam that Pulley 2 in Figure 4.2 is attached to The simulation results are analyzed in order to find the displacement s of the same point measured by the LDS The resulting plot of deflection versus load for both simulated and physical displacement test is shown in Figure 10 below. Figure 4.4 : Comparison of simulation results to physical stress tests. Table 4.1: Displacement results for both experimenta l and simulated cases. Load (lbf.) Physical (in.) Simulated (in.) % Error 115.6 0.0046 0.0027 41.4 167.6 0.0069 0.0037 46.0 219.6 0.0089 0.0051 42.7 245.6 0.0100 0.0057 43.0 T he data acquired for the physical displacement test has a regression coefficient of 4.1e 5 in/lbf and an R 2 value of 99.96 The deflections are therefore very nearly linear with load. The simulation data are linear with a regression coefficient of 2.6e 5 in/lfb and a R 2 value of 99.5%. The percent error in stiffness between simulation and the physical experiment is then 36%. The

PAGE 21

21 magnitude of error shows th at the simulation model requir e s refinement before further predictions can be considered valid Specific recommendations are outlined below. 5 Fut ure Work The results of the displacement test display a significant dis crepancy between simulation results and experimental data. Despite the fact that both sets of data are linear, the displacement per unit load calculated during simulation differs by a margin of 36% from experimental data. Under the assumption that accurate data was taken during the displacement test, the simulatio n model must be adjusted in order to more accurately coincide with experimental data. Several areas of interest in the finite element model will be explored. An assumption made in modeling the test stand system was the bottom surfaces of the four main ver tical beams remained very close to the floor such that deflections of these surfaces are negligible. These surfaces are therefore constrained to zero translation in any directi on. However, the steel anchor bolts and aluminum L brackets securing these beams to the floor would have undergone finite strain during the physical d isplacement test. As a parametric study this boundary condition will be explored by attempting to include the L bracket and anchors in the finite element model The test stand will then be constrain ed by means of these components and d eflections will be compared to the experimental data. This model can be simplified by performing a preliminary analysis on the securing system and eliminating components from the model that do not contribute significantly to deflection. For example, it would be unnecessary to model the steel anchor bolts if their change in length is negligible compare d to deflection of the L brackets. Primary sources of deflection in the L bracket/anchor system must therefore be identified and analyzed using basic mechanics of materials equations Another area of interest is a comparison of the results obtained using the full solid element simulation model described in Section 3 to results using a beam element model The reason for this investigation is due to the cross sectional geometry of the equivalent beams used in analysis. It was proposed that the thin, hollow cross section might have caused error in the model because of the low resolution of elements in the t hickness direction as evident in Figure 3.1 A simple beam element model may therefore be able to predict the deflection with relative accuracy with a much lower computation al requirement. To further the refine the finite element model developed by the process just described it would be beneficial to conduct further displacement test s under loading directions other than downstream. With a finite element model that is able to predict both downstream and cross stream deflections, it would be possi ble to predict deflections before experimentation with e ven greater accuracy than can be attained without further physical displacement testing. Howe ver, the

PAGE 22

22 finite element models that will be developed based on t he load configurations used thus far will s till be very valuable tools for the UFAFF. 6. Concluding Statements The stand that has been designed and that currently stands in the UFAFF was designed based on an iterative optimization process. In physical experimentation, the stand deflected one hun dredth of an inch under a downstream loading of 245.6 lbf. Simulation of the same loading condition results in a deflection that was 43% less. This discrepancy can be largely attributed to two assumptions used during simulation: ideally fixed boundary cond itions, and perfectly fused interfaces between structural members. In reality, the non ideality of both of these conditions contributes to the reduced stiffness of the physical test stand. Utilization of the finite element model devel oped and used as described in this paper will require implementation of a factor of safety This will ensure that the excess stiffness evident in the simulation model does not result in underestimation of deformation and, in turn, error during physical exp erimentation. The average ratio of experimental deflection to simulation was 1.77 with a maximum ratio of 1.86. Based on these r esults, it is recommended that, in use of this finite element model, a factor of safety of at least 2 is applied to the predicted deflections. Wi thout the model improvements described in Section 5, simulation results should not be used to predict exact deflections. However, use of this finite element model for obtaining an order of magnitude of deflections and for carrying out trend based design is still practical.

PAGE 23

23 References 1 3052, May 2005. 2 The Aeroacoustic Corporation, Retrieved April 28, 2011. http://www.aeroacoustic.com/ 3 Parametric Technology Corporation, Creo Elements/Pro, Retrieved April, 2011, http://www.p tc.com/products/creo elements pro/ 4 80/20 Catalog 16 pp. 74 78, Retrieved January, 2011, URL: http://www.8020.net/interactive catalog.html 5 Pro Mechanica How It Works Retrieved April, 2011 http://www.elite consulting.com/how_mechanica_works.htm 6 Abbott, H. and Doenhoff, A., Theory of Wing Sections Dover Publications, Inc., New York, 1959. 7 B ahr, C., Yardibi, T., Lui, F., and 2957, May 2008. 8 udy of a 4576, July 2010. 9 Sun, C. T., Mechanics of Aircraft Structures John Wiley and Sons, New York, 2006. 10 Keyence Corporation, LK G Series CCD Laser Displacement Sensor, Retrieved April, 2011, URL: http://www.keyence.com/products/measure/laser/lkg/lkg_applications_5_1.p hp