Flow Analysis of an airfoil naca- 2412 for low speed

 Good Morning,

This blog is written to give details about the CFD analysis of the naca 2412 airfoil for low speed. Results of which would be compared with the experimental data. It is described step by step procedure to simulate,during this study.

The basic idea of CFD is the analysis of a body, to check how efficient it is in real-world applications. If we take an example of a car, where CFD analysis is frequently used, numerical analysis of it can reveal the features of a  body such as drag coefficient. What would be the steps after analysis to reduce the effect on the body. This was the one example of the application of  CFD in the world of automobiles.

Keeping the above things in mind, we require geometry to analyze. In this case, naca 2412 airfoil with 230 mm chord length was selected, which can be easily found on the internet. The reason was quite obvious as I wanted to validate my results, and experimental datas are readily availaible on the internet. In the present work numerical analysis was done for airfoil with angles of attack 0,2,4,6,8,10,12 and 14 with the flow conditions mentioned below. The aim of the simulations was to acquire a lift coefficient with different AOA, for which incompressible, steady,2D analysis was made except for the case of a 14-degree angle of attack, where 2D, unsteady simulation was performed.

Vinf = 30 m/s ,Re,ch=425905, rho = 1.1555 kg/m^3, mu= 1.87*e-05 kg/m-s., char. length=230mm

GEOMETRY DEFINITION

Star was used for the simulation. As it was the 2D geometry of the airfoil, it was easily imported from the.csv file. After importing the airfoil, it needs to be analyzed in the computational domain. The computational domain is the volume, where the governing differential equations(flow) are solved. This computational domain is discretized, where the governing differential is solved; and this discretized domain is generally called mesh.

As it is evident that g.d.e (governing differential equations) would be solved, which requires boundary conditions. These conditions are given at the boundary of the domain. So if our studied geometry (airfoil) is kept near the boundary, it can influence the results of our geometry. Considering all the above logic, the studied geometry was kept far away from the boundary. Normally, for the external flow analysis boundaries are kept away 10 times the characteristic length from the studied geometry. For this particular study, it was kept 11 times the chord length. it is necessary to note that, all the dimensions are kept either in mm or in the meter as per choice.

Once the geometry is imported and the computational domain is created, different names for the faces of the computational domain can be given. for this study it was analyzed for different angles of attack, there is an option instar, which can be helpful to rotate the airfoil at different angles of attack. This option can be accessed by right-clicking the airfoil body and we can expose this parameter for future changes in the angle of attack.  

Once geometry and computational domain are created, parts can be created for both. These parts are used to subtract the airfoil from the domain(target part) by doing the boolean operation. After doing boolean operations, one new part is generated in the tree of the parts named subtract. This is the part where flow is analyzed. Since this is a 2D analysis, it needs to convert subtracted parts in 2D; Which can be done by operation--> mesh -->badge for 2D meshing. After converting it in 2D, regions can be assigned, it can be done by choosing the substracted domain, right-clicking on the substracted part, and accessing the assigned regions to the parts. In these defining regions, each surface(which means creating boundaries for each part surface) of subtracted parts should be assigned. after the successful creation of the regions, if you check there, there would be the different names of the regions.

After 2D Geometry and regions it , there comes a need to define the physics. since we are simulating 2D flow we can define that  in the continua, physics, and models. steady flow, gas, segregated flow, constant density, and turbulence model. for the turbulence, k-omega sst model was selected(since it is external flow). Once physics is defined there can be reference values and initial conditions options, for reference values everything was kept as it is, and the initial conditions velocity can be changed to 30 m/s, the reason to change the initial velocity is to make convergence quickly.

NOte: it is not to get confused between initial conditions and boundary conditions; initial conditions are those which initialize the solutions, which set the value to all of the flow domain; whereas boundary conditions are defined at the boundary.

so for example, if we had decided to choose the initial conditions as 0 m/s, and our boundary condition is defined at 30 m/s, then the boundary condition has to push the domain to 30m/s, which can delay our solution.   

BOUNDARY CONDITIONS

Once , physics is set , regions can be modified and assign boundary conditions as well.For this study the shape of the computational domain was chosen which has three inlet surface boundary conditions and one outlet condition. So, in the region, it is normal to find three regions, one is for the inlet, one for the outlet, and the last one for the airfoil.For the inlet region, the velocity inlet condition was applied, once applied it requires to choose the flow direction since we want our flow in a particular direction, it was not recommended to choose the normal to the boundary.once flow direction is defined, velocity value can also be defined at the boundary as 30 m/s.another boundary was outlet where pressure outlet was selected, and for the airfoil, it was chosen as the wall.  

MESH

Once boundary conditions are defiened , mesh generations can be started. which can be done by accessing the operations-->new -->automated mesh 2D,where polygonal  mesher and  prismatic layer can be selected.after doing it,a new options names automated mesh2D appears under the operation; where various options regarding the mesh can be adjusted. There are options to select the base size, in this case it was 0.002 m, target surafce size, and minimum surface size can be adjusted furthermore.simualating this kind of flow, it is necessary to capture the effect of boundary layer,to capture the effect of the boundary layer,it is necessary to define the numbers of  prisam layer and thickness of the prisam layers.since we are capturing the boundary layer, the thickness of boundary layer must  encompassing the prism layer or in other sense, prism layer thickness should be such that it can capture the boundary layer. For this study, turbulent B.L( boundary layer) over flat plate helped to estimate the thickess of B.L.for this it was calculated around 6.36e-03m. so, thickness of the boundary layer is estimated, but it  is required to calculate the prism layer thickness and first cell thickness (which is y) and stretching of the first cell which can encompassess B.L. which can be calculated as below in shown fig.0 

fig.0 y calculations.

Once y is calculated, it can be stretched with appropriate stretching factor of 1.1 & consequetly deriving the numbers of prism layer required.once entered all the details, meshing can be executed.
since it does not require very fine mesh & prisam layer at the boundary of the domain , it can be controlled by accessing custom control -->surface control. wake refinement can also be created by choosing the volume control and creating the required shape for mesh refinement.Once executed it creates mesh, the mesh did for this study is shown below.

                         fig. 1   Domain                                                                       fig. 2 Prism layer

Once, meshing is finished, it can be simulated for different angle of attack and can obtain the lift coefficient for it. As it was discussed earlier, in the current study angle of attack ranging from 0-14, with interval of 2 were analyzed. After changeing various AOA and each time value of the cl was taken at the convergence.These results were compared with the experimental data. The experimental data were taken from the experiment conduted at oral roberts university, which i have linked below in the reference.

Simulation was done, and the coefficient of the lift was taken for different AOA. These datas were compared with experimental data which is shown below in the graph.

fig. 3 Cl Vs Alpha

 In the above graph fig.3 which estimates the lift coefficient, it is clear that for AOA of 0-12 it predicts a good lift coefficient; whereas for AOA 14 it deviates from the experimental data. The reason for that is in the turbulence modeling; a fully turbulent assumption is made in the kw-sst model, which assumes higher eddy viscosity(causes turbulent momentum transfer) and which higher estimation increases momentum transfer consequently delaying the separation. This delayed separation creates low-pressure regions on the suction side than the real one; which gives a higher value of lift coefficient.

Along with the lift and drag coefficient, some of the images were also capture for velocity vectors and pressure contours which is shown as below.

        fig. 4 pressure contour AOA 2                                        fig. 5 velocity vectors AOA 2

Along with this it seems necessary to see the how the lift coefficient converges for higher AOA 14.

    fig. 6 cl convergence AOA 14                                               fig. 7 cp for AOA 14

Moreover, it was also captured how for different angle of attack velocity profile varies past the airfoils.

AOA =0

 AOA=2

 AOA=12

The main objective of this independent study was to acquire the life coefficient ; analyse how far it can approximates the data.

Note:- this study was conducted independently by me, comments are welcomed.

Reference:-https://www.researchgate.net/publication/319271205_Aerodynamic_Performance_of_the_NACA_2412_Airfoil_at_Low_Reynolds_Number