Uçak kanat aerodinamiğinin had yöntemi ile analizi ve doğrulama
Analysis and verification of aircraft wing aerodynamics with cfd
Yazar: MEHMET DOĞUKAN KOCABAŞI
Danışman: YRD. DOÇ. DR. HAYRİ ACAR
İstanbul Teknik Üniversitesi / Fen Bilimleri Enstitüsü / Uçak ve Uzay Mühendisliği Ana Bilim Dalı
Derece: Yüksek Lisans, 2018
Konu: Makine Mühendisliği = Mechanical Engineering ; Uçak Mühendisliği = Aircraft Engineering

Özet:
HAD yöntemi 1970' lerin sonunda 2 boyutlu bilgisayar kod ve çeşitli algoritmalarla başlayarak önemli bir atılım gerçekleştirmiştir. HAD yöntemi günümüzde araştırma, geliştirme, optimizasyon, doğrulama vb. gibi işlemler için bir hayli kullanılmaktadır. HAD yönteminin kullanılma amacı varolan veya olmayan bir nesnenin akış karakteristiği hakkında bilgi sahibi olunması isteğidir. Model kompleksliliğiyle doğru orantılı olarak kaynak, yani gerekli olan bilgisayar yatırımı da artmaktadır.
HAD yöntemi teoride hayatı oldukça kolaylaştıran bir alet olsada tecrübeyle sonuç yorumlama olmadan sadece renkli görüntülerden oluşur. Hatanın nerede olduğunun farkedilmesi ve çözülmesi bu yöntemin en önemli parçasıdır.
HAD yöntemi teorik yöntemleri kullanan akademik veya ticari yazılımların numerik hesaplamalar yapması sonucu elde edilmektedir. Teorik hesaplamalarda probleme bağlı olarak Navier-stokes ve süreklilik denklemlerinde bazı parametreler ihmal edildiği gibi aynı şekilde HAD yönteminde de aynı kabulleri girdilere göre yazılım yaparak hesabı numerik olarak çözmektedir.
Bu tez çalışmasında HAD yönteminin günümüzde kullanılma sebeplerinden biri olan sonuç doğrulama hakkında araştırma yapılmıştır. İki adet ayrı geometri bu işleme tabii tutulmuştur. Bunlar NATO' nun birçok deneyinde kullanılan ONERA M6 kanadı ve rüzgâr tünel kalibrasyon modeli AGARD C' dir. 
ONERA M6 kanadı 1972 yılında ONERA S2MA rüzgâr tünelinde transonik hızlarda 30 adet farklı teste maruz bırakılmıştır. Kanat üzerinde 7 adet kesit düzlem oluşturulmuş ve bu düzlemlere ölçüm delikleri yerleştirilmiştir. Ölçüm deliklerinden basınç dağılımı okumaları yapılmıştır. Son olarak basınç katsayıları deliğin konumu bazında hesaplanarak her test için grafikleri çizdirilmiştir.
AGARD C modeli ise, rüzgâr tünel kalibrasyonlarında kullanılan bir modeldir. Transonik hızlarda çeşitli testlere tabi tutulan bu modelin varyasyonları birçok enstitü tarafından ele alınmıştır. Test sonuçları 3 adet hucüm açısı ve enstitülerce oluşturulan farklı modellerin Mach sayıları bazında moment, sürükleme, kaldırma kuvveti katsayıları hesaplanarak her test için grafikleri çizdirilmiştir. 
Bu tezde bilgisayar ortamındaki katı modeli çizilen cisimlerin HAD yöntemiyle akış analizi yapılarak elde edilen sonuçları ile deney sonuçlarının karşılaştırılma yapılması amaçlanmıştır.
Geliştirilmiş çeşitli viskoz modellerinden ikisi ile seçilen testler çözülmüştür. Basınç, sürükleme, kaldırma kuvveti katsayıları karşılaştırılmıştır. Karşılaştırmalar sonucu HAD yöntemi sonuçlarında çeşitli hatalar elde edilmiştir. Bunun nedenleri çözüm ağındaki bozukluk olmasına kanaat getirilmiştir.
Spalart-Almaras viskoz modeli çözümlerinde tek denklem kullanmaktadır. Bu modelin belirli bir transonik hız limitine kadar oldukça doğru çözüm verdiği görülmüştür. Fakat 1.1 Mach sayısından yüksek çözümlerde çözüm ağının hatalarıyla da birlikte çözümdeki hata oranı ciddi şekilde artmaktadır. 
SST (Shear Stress Transport) k-omega modelinde ise girdap ve viskoz etkilerinin daha iyi hesaplandığı bilinmektedir. Yalnız bu yöntem çözüm ağındaki hatalardan oldukça etkilendiği için hesaplamalar yarım olarak yapılabilmiştir.

Abstract:
Computational Fluid Dynamics is used in a wide range for research, development, optimization, validation. Using of CFD started in late 70s with 2D codes. Aim of CFD is assessed about characterics of a flowfield from a new design or existing model. Having a solution form computer system is dependent on complexity of a new design or existing model. Directly proportional to the complexity of the model, the resource required, ie the computer investment, is also increasing.
CFD is a tool that makes life easier in theory, but it is only made up of color images without experiential interpretation. It is the most important part of this method of recognizing and resolving where the error is.
CFD is the result of performing numerical calculations of academic or commercial software using theoretical methods. In the theoretical calculations, some parameters in Navier-Stokes and continuity equations are neglected depending on the problem, and in the same way in the CFD, the same arguments are numerically solved by performing software according to the inputs.
In this thesis study, a result validation study which is one of the reasons of use of CFD is done. Two separate geometries are involved in this process. These are the ONERA M6 wing and the wind tunnel calibration model AGARD C used in many NATO experiments.
The ONERA M6 wing was subjected to 30 different tests at transonic speeds in ONERA S2MA wind tunnel in 1972. Seven cross-sectional planes were formed on the wing and measurement holes were placed in these planes. Pressure distribution readings were made through the measurement holes. Finally, the pressure coefficients are plotted on a per-hole basis and plotted for each test.
The ONERA M6 geometry, modeled on the surface, is available on the NASA website in the verification archive. Here the coordinates were corrected in the Solidworks solid model program. To avoid a problem caused by scaling when transfering to the CFD, the drawing tolerances were preserved by converting it to the model "igs" format. However, there are some situations such as the union of some surfaces.
In ANSYS Spaceclaim program, these conditions were re-edited to give the geometry an angle of attack (3.06°) for the test conditions and the mold was made for flow volume. The wing is located right in the middle of the test section and is positioned at the origin to detect distance differences in coordinate system. Flow volume test was created with circumstantial to stay connected to the dimensions of the cross section. Although there are 6 surfaces, 3 boundary conditions are determined. 
Each surface in the translated model is named in detail and ANSYS Meshing provides a meshing by giving the appropriate parameters.
The patch conforming algorithm, which is used to knit the volume mesh starting from model, is used. The skewness and orthogonal quality values of the mesh, which indicate the number and the number of nodes and the quality, are important values to be examined.
For body sizing, a rectangular prism is drawn which can fit into the wing into the flow volume. As shown in Figure 2.6, the dimensions are 500x2000x1500 mm3. The reason for this volume formation is to define a reference for the solution network in that region. It is aimed at establishing a mesh more frequently than the remaining volume.
The more often the face sizing is dimensioned, the better the resolution on the surface to be measured. Therefore, the thickness value has been entered to create a mesh of as good quality as possible on the surface.
Inflation is an important parameter in determining how viscous flow effects affect the values above the surface. There are several methods of participating in the mesh of the inflation method. (eg. maximum thickness, first thickness).
There are a few equations that must be calculated to give the distance of the first thickness. The value of the y+ coefficient is important in first thickness of inflation. The y+ coefficient varies according to viscous methods. However, the optimal default value to use when calculating which viscous model is unknown is 1. 
The method defined for the inflation parameter in our flow volume is to give the maximum thickness. Maximum thickness is how many pieces of inflation are given to give the distance of the surface of the last layer from the surface to the surface. In this case, inflation of 10 units is defined within 1.2 times for 1 mm. Expected skewness and orthogonal quality are not inflated by a small amount depending on the situation.
Commercial software of ANSYS is used for solution for CFD. The solution was performed in the Fluent solver program. Firstly, the single-equation Spalart-Almaras turbulence viscous model is used. The solution is 1000 iterations with this model. Secondly, 1000 iterations were carried out in the same solution with the SST k-omega turbulence viscous method, which has higher accuracy and gives better results in the vortex model.
The properties of the air in the material section were compressible flow due to the large Mach number over 0.3, and the density was chosen as the ideal gas. In this way, both the temperature and the pressure values of the cooling air are added into the calculation. If the incompressible ideal gas was selected, only the temperature value solver will participate. Other features are left by default. The wall defined surfaces and the wing are defined as aluminum, which is the material found in the program's default.
From the boundary conditions, the pressure far-field are passed in the first solution of input and output, and Mach number is 0.8395. The input and output pressure values are given as 0 because the ambient operating condition is 101325 Pa. If so, the program will recognize it as calibrated value and add it to the ambient condition. The second solution is also defined velocity inlet as inlet and pressure outlet as outlet. The input speed is defined as 285.67 m/s. The pressure values at the inlet and outlet are set to 0 Pa in the same way due to the operating condition value. The wing and test section wall sections are defined as wall in the program.
In the solution methods, it is selected as coupled in the Spalart-Almaras single-equation turbulence model solution. Residuals are the second order, except for the corrected turbulence viscosity. In the SST k-omega viscous model solution, the scheme is again defined as coupled and the residuals are all second-order. The solution was evaluated as steady state, but the pseudo transient option was opened to solve the flow volume transient and tried to obtain a better solution. There is no initialization between solutions to determine how different solutions will show each other. Both solutions start with their default values. In the conclusion section, the differences between the two solutions can be seen. 
The AGARD C model is a model used for wind tunnel calibrations. Variations of this model subjected to various tests at transonic speeds are handled by many institutes. The test results are plotted for each test by calculating the moment, drag, lift force coefficients of 3 different angles of attack and Mach numbers of different models created by the institutes.
There are cross-section images given in AGARDograph 64 and wikipedia. Sketches were drawn, and the solid model was extracted from the Solidworks program. For the K1 test theme, dimension of 70 mm for diameter was taken and the drawing tolerances were preserved by converting the model to the "igs" picture format to avoid a geometrical problem when switching to the CFD. In ANSYS Spaceclaim program, it is divided into halves for the symmetrical solution which is more suitable for the computer features and the mold is made for the flow volume. The modeler is located right in the middle of the flow volume and is originally positioned to sense the distance differences. It was determined as half sphere to give only 3 surface boundary conditions. The hemisphere oval surface is divided into two parts to obtain the inlet and outlet surfaces required for boundary conditions. The flat part is used for symmetry axis and surface. The radius of half a circle is 8 meters.
Each surface in the translated model is named in detail and ANSYS Meshing provides a network of solutions by giving the appropriate parameters.
Patch conforming algortm can not be applied, especially because the wing and tail geometries can not be wrapped with a neat mesh due to the tapering of the tip parts. Therefore, the "Patch Independent" method, which is the method of creating the correct meshing from the volume, has been chosen. 
To catch the boundary layer at the high Mach numbers, it is necessary to create very small boundary layer sections because there is no inflation in our flow volume. The distance from the nearest surface to the surface, ie the first layer of the boundary layer, can be incorporated into the mesh depending on the computer characteristics. The grid size is set to "coarse".
In general, with CFD, there is a great importance in reaching the solution of the first result in a fast and healthy way. It is generally calculated using viscous single-equation solutions. Therefore, the Spalart-Almaras viscous method, which is mostly successful at high speeds, was used as the first solution. The solution is 1000 iterations like this. Then 1000 iterations were carried out with the same solution with the SST k-omega viscose method reaching solution with equations of second order, which is more accurate and better in vortex modeling.
The properties of the air in the material section were compressible flow due to the large Mach number in the solutions of 0.3, and the ideal gas was chosen as the ideal gas. In this way, both the temperature and the pressure values of the cooling air are added. If the incompressible ideal gas was selected, only the temperature value solver will participate. Sutherland was chosen because the viscosity variant changed the viscosity value depending on the temperature to better effect the dissolution. The solid part of the wall that is defined remains in the default aluminum of the program.
From the boundary conditions, the Mach number 0.7 was entered by passing the pressure distant field in the first solution of inlet and outlet. The input and output pressure values are given as 0 because the ambient operating condition is 101325 Pa. If so, the program will recognize it as calibrated value and add it to the ambient condition. The second solution is also defined as input speed input and output pressure output. The input speed is defined as 238.2 m/s. The pressure values at the inlet and outlet are set to 0 Pa in the same way due to the operating condition value. The solid model parts (wing, fuselage, tail) are defined as walls. The common surface interrupted due to the division of the flow volume into two is defined as symmetry in the sense that the solution of the same hemisphere flow volume is repeated. The above values are valid for the solution with M = 0.7.
The solution was evaluated as continuous flow, but the pseudo discontinuous option was opened to solve the flow volume discontinuity and tried to obtain a better solution.
Priming was carried out using the Spalart-Almaras viscous method with reference to the conditions at the beginning. The second solution is to take the result of the SST k-omega, Spalart-Almaras single-equation viscous model as the first solution and make iterations on it.
During the simulation of the SST k-omega model, which is the second solution in the solution methods, reverse flow occurred in some regions and absolute pressure limitation was experienced.
In this thesis, it is aimed to compare the experimental results with the results obtained by flow analysis of solid objects drawn in computer environment by CFD.
Selected tests have been solved with two of the various improved viscous models. Pressure, drag, lift force coefficients are compared. A number of mistakes were made in the results of the CFD. The reason for this is the disorder of the case mesh.
Spalart-Almaras uses a single equation in viscous model solutions. It has been shown that this model provides an accurate solution to a certain transonic speed limit. However, in the case of higher Mach numbers than 1.1 Mach, the error rate of the solution increases repeatedly as well as the errors of the mesh.
In the Shear Stress Transport (SST) k-omega model, the vorticity and viscous effects are more accurate than others. However, since this method is highly influenced by the errors in the mesh, calculations could be halfly missing.
Lancer 200 aircraft without copyright complaint were selected. Cold flow through the CFD method has been applied to various aircraft parts and combinations in a single dimension. In this study, it was aimed to observe the effects of aerodynamic force and coefficient values on the wing and fairing as a result of the simulations. In the following 9 cases, it is stated which solid geometry is used. Case 1: Body only, Case 2: Wing only, Case 3: Tail only, Case 4: Only Wing Tail, Case 5: Body Wing Only, Case 6: Full Body Wing Tail, Case 7: Half Body Wing Tail, Case 8: Half Guns Wing Tail + Fairing (NACA 4412), Case 9: Half Body Wing Tail + Fairing (NACA 4412) + α = 8 °, Case 10: Half Body Wing Tail + Fairing (NACA 4412) + α = 12 °, Case 11: Half Body Wing Tail + Fairing (NACA 4412) + α = 16 °