Performing grid dependence study for steady flow over an Ahmed body with slant angle of 20 degrees using ANSYS Fluent
INTRODUCTION:
The Ahmed body is a standard model of a generic car shape used as a reference for wind tunnel testing of road vehicles. The characteristic feature of the structure is the slant plane in the rear side of the body which contributes to flow separation and recirculation in the wake region of the flow. Experimental results have been performed for different slant angles which conclude that the wake region is highly dependent on the slant angle. For slant angles less than `12^0`, the flow mainly remains attached over the slant. Between `12^0` and `30^0` the flow separation increases over the slant and beyond `30^0`, the flow fully separates off the slant. It has also been shown that the aspect ratio of the rear slant can also highly affect the flow separation. Higher aspect ratios lower the critical slant angle. Increasing flow separation leads to an increase in the drag coefficient of the body. Since the body is the generic shape of a car, it can be used for preliminary testings of road vehicles so that the further experiments can be standardized. The structure of the Ahmed body is shown below:
The experimental results from the wind tunnel are also used to compare with the numerical results from a solver to test the accuracy of the numerical model. In this project, we will be testing the Ahmed body with a slant angle of `20^0` in a steady-state turbulent flow with a free stream velocity of `50` `m"/"s` and performing the grid-dependency test. The engineering drawing of the model from different views and dimensions is shown below:
We will be splitting the model into half and creating a fluid domain around the body to perform the flow simulation. Three different meshes with a different number of elements - coarse, fine and very fine, will be used where the "very fine" mesh will reach close to the limit of the student version of ANSYS Fluent which is `512000` elements. We will be comparing the drag coefficient of the model for the three meshes.
COMPUTATIONAL DOMAIN:
A fluid domain is created around the solid body to perform the CFD analysis. The domain should be large enough to capture the flow dynamics. For this problem, a box enclosure is created around the body with a `2` `m` leading region and a `5` `m` wake region. The enclosure extends by `0.5` `m` on either side of the body. This geometry is suitably large but it cannot accommodate the finer cells of a mesh which would significantly increase the computational resources. Hence, a smaller box is generated to implement smaller mesh size. The smaller enclosure extends `1` `m` front and `2` `m` back from the surface of the body and `0.25` `m` on either side. The solid body is subtracted using boolean operation so that it is not a part of the
Named selections are generated on the domain for ease in applying the boundary conditions. The front-most face is named "inlet", the back-most face is named "outlet", the side walls are named symmetry and the bottom faces are named "walls" which would act as a road.
MESHING THE COMPUTATIONAL DOMAIN:
Three different meshes are used to perform the grid dependence study - coarse, fine and very fine. For all the three meshes, `5` prism layers are created with a total thickness of `0.012` `m` around the Ahmed body and `0.02` `m` on the road surface, both with a growth rate of `1.2`. The main parameters affecting the mesh are the size of elements in the inner body (small box) and the outer body (big box). The values of these parameters are listed below.
`{:(ul{text{Mesh}},,ul{text{Outer Body Elements}},ul{text{Inner Body Elements}},,ul{text{No. of Elements}}),(text{Coarse},,0.3\ m,0.2m\ text{(Growth Rate: 1.2)},,154522),(text{Fine},,0.2\ m,0.15m\ text{(Growth Rate: 1.1)},,299108),(text{Very Fine},,0.08\ m,0.05m\ text{(Growth Rate: 1.1)},,467292):}`
The mesh in the inner body is allowed to capture the curvature and proximity which refines the mesh further on the Ahmed body surface. The generated meshes and the zoomed-in prism layers are shown below:
Coarse Mesh
Fine Mesh
Very Fine Mesh
SETUP OF THE FLOW PHYSICS:
Since the inlet velocity is very high, the density-based solver is used. We are solving the Reynolds Averaged Navier Stokes (RANS) turbulent equation. The standard 'k'-'epsilon` turbulence model with standard wall functions is used. The fluid used is air with the following parameters:
Density: `rho = 1.225` `kg"/"m^3`
Dynamic Viscosity: `mu = 1.7894 times 10^{-5}` `kg"/"m-s`
The inlet face is assigned a velocity inlet boundary condition with free-stream velocity magnitude of `50` `m"/"s`. The outlet face is assigned a pressure outlet boundary condition with a gauge pressure of `0` `Pa`. The bottom faces (road) and the surface of the Ahmed body are assigned wall boundary conditions and the remaining sides of the domain are assigned symmetry boundary condition. The frontal area is calculated based on the area of the Ahmed body projected on the y-z plane.
`A = ubrace{(0.39 times 0.29)}_{text{Upper body}} + ubrace{2 times (0.05 times 0.03)}_{text{Legs}} = 0.1161` `m^2`
This value is used as the reference area in the calculation of lift and drag coefficients. The lift and drag coefficient monitors are created to record the respective parameters at each iteration which would allow us to check the convergence of the solution as well. The solution initialization is done using hybrid initialization and then solved for a maximum of `1500` iterations till convergence is achieved.
RESULTS AND DISCUSSION:
Coarse Mesh
Residuals and Monitors
Velocity and Streamlines
Pressure
Fine Mesh
Residuals and Monitors
Velocity and Streamlines
Pressure
Very Fine Mesh
Residuals and Monitors
Velocity and Streamlines
Pressure
The velocity contours for the coarse mesh is more pixelated/blurry than the fine and the very fine mesh. Even though the coarse mesh gives faster results, we can see from the drag and lift coefficient plots that they have still not satisfactorily converged. This is because even though the residuals meet certain convergence criteria, the monitors are still slightly fluctuating. For the fine mesh as well, the drag coefficient does not appear to be fully converged to a fixed value. The very fine mesh can capture the contours and the streamlines in the wake of the Ahmed body showing proper recirculation and flow separation much better than the remaining two mesh. However, ideally we would require much more elements than the very fine mesh to obtain accurate results comparable to the experimental value, but the size of the mesh is limited due to the limit enforced by the academic license of ANSYS Fluent. The lift and drag coefficient values for the different mesh and the number of iterations required for their convergence are compared in the table below:
`{:(ul{text{Mesh Size}},,ul{text{Iterations to Converge}},,ul{text{Lift Coefficient}},,ul{text{Drag Coefficient}}),(text{Coarse},,831,,0.3397,,0.3540),(text{Fine},,1045,,0.2898,,0.3457),(text{Very Fine},,1331,,0.3002,,0.3422):}`
The pressure contours are negative in some areas. This is because CFD-Post displays the pressure contours relative to the reference value which is `101325` `Pa` in this case. The pressure drops are generated because of the flow. At the leading region (head) of the Ahmed body, the flow strikes with the free stream velocity and comes to a halt in the streamwise direction. This leads to the high pressure generated over the head. Due to the curves on the following surface, the flow has to change direction which leads to a pressure drop over the curve. The sidewalls of the Ahmed body are flat, hence we do not see much pressure change in the region and again while entering the slant region, the flow changes direction and leads to the pressure drop. Negative pressures indicate that the pressure of that region is below the atmospheric pressure.