Simulation of air flow over Ahmed body using Ansys Fluent

1. Introduction

External car aerodynamics plays a significant role in reduction of fuel consumption, noise and driver stability. With manufacturers subjected to stringent limitations of carbon dioxide, NOx emissions and market demand to continually improve the efficiency and mileage, immense resources are expended in studying the flow of air over the body of the vehicle. With the rising computational processing power through research and innovation, more and more focus on studying these parameters have shifted to computational simulations rather than the conventional wind tunnel physical experiments.

• Ahmed\'s body and its importance

One of the drawbacks of computational simulations of fluid flow is the poor confidence levels in the results obtained. Hence, there is a need to validate the results using physical experiments. Considering the complexities involved in a modern day automobile, the expenses of simulating the fluid flow with realistic prototype would be enormous. To solve this issue, a generic car body called Ahmed body was proposed by S. R. Ahmed in 1984.

Fig 1- Ahmed body drawing

The figure describes the simplicity of the car body which upon simulation gives the desired characteristics with ease. Due to its simplicity, a relatively coarse mesh or a scaled down physical model can be used to reduce the expenses incurred during simulation without compromising on the results of accuracy. The simulation results successfully capture the recirculation regions in the wake of the body, formed due to flow separations. The model can be used to compute the forces in the wake region and establish the coefficients of drag and lift.

Ahmed body has found its importance in validating the numerical models used to simulate the fluid flow. As a standard aerodynamic model for simulation, the proposed numerical model is studied for different slant angles and Reynolds numbers and the results are validated through physical experiments. The accuracy in measurements establishes a significant confidence level in the numerical model which is then used to simulate complex vehicle models.

1. Geometry

For this case, we consider the Ahmed body with slant angle 20 degrees. Due to its symmetry, we can consider splitting the body via the mid-plane. This gives additional computational capacity of refining mesh maintaining the accuracy of the results. The split body is created using Spaceclaim.

Fig 2 – Splitting of Ahmed body

To simulate the wind tunnel, we create an enclosure surrounding the body for which the dimensions are displayed in the below figure.

Fig 3- Dimensions of enclosure

Fig 4- Isometric view of geometry for simulation

1. Baseline mesh

We run the case by using baseline mesh or default grid size as calculated in Ansys Fluent.

Nodes= 8672

Elements= 42983

Fig 5- Baseline mesh

3.1 Initial and boundary conditions

For the fluid flow, the fluid under consideration is air with velocity at the inlet boundary condition being 25 m/s. The boundary conditions for other boundaries are shown in the table below:

Table 1 Boundary conditions

Boundary	Type	Parameter
Bottom_wall	Wall	-
Car_wall	Wall	-
inlet	velocity-inlet	25 m/s
interior-enclosure_enclosure	interior	-
outlet	pressure-outlet	0 (gauge)
symmetry	symmetry	-

3.2 Solver

The simulation is run using density based type of solver. Density based solver may give you better accuracy over the pressure based solver for compressible flows. The pressure based solvers are preferred for problems with low Mach numbers and incompressible flows (less than 0.3) as the simulation time is considerably low. Since the case under study is relatively simple, density based solver can be used.

Time: Steady

Turbulence model: K-Ɛ Realizable

3.3 Results

The steady simulation is run for 2000 iterations.

3.3.1 Residuals

Fig 6- Residuals for simulation using baseline mesh

A brief study of the residuals suggest the convergence of the simulation at iteration= 1050

3.3.2 Velocity plot for wake region

The solution is post processed to obtain the velocity contour plot and vector plot.

Fig 7- Velocity contour and vector plot

As can be clearly seen in the above figure, due to coarse mesh, the wake region is not captured in the simulation. Hence, the next logical step is to refine the mesh using optimization techniques

1. Mesh refinement

The baseline is modified by reducing the element size, introducing inner enclosure around the body and incorporating inflation layer at the boundary walls. The study is divided into three sub-divisions with moderate mesh, fine mesh, finer mesh

4.1 Geometry

Another enclosure is introduced of relatively smaller size around the body using Spaceclaim.

Fig 8- Inner enclosure dimensions

4.2 Interference check

Fig 9- Section view (a) With interference (b) After interference check

The generated geometry is checked for interference in Spaceclaim. The double hatch lines in the inner enclosure indicated the interference present. This is resolved using the interference check command to obtain the updated geometry as shown in figure.

Note that to introduce different mesh element sizes for the inner and outer enclosures, it is mandatory to allow topology share feature in Spaceclaim.

4.3 y+ calculation

In order to ensure that the first wall thickness at the boundary walls of the body is beyond the laminar viscous region, we calculate the y+ value for the given case.

The equations based on skin friction on the boundary walls are:

Re=ρ.U_∞L/μ

Cf= 0.026/Re^1/7

τ= Cf.ρ.U_∞²/2

U_fric = √(τ.ρ)

y = y+.μ /U_fric.ρ

In this case, U_∞ = free stream velocity = 25 m/s.

Reynolds number, Re = 1.74 e006

Considering a high y+ model with y+ more than 30 ( to avoid simulation of laminar sub layer near the boundary) , the first boundary layer wall thickness,

y= 0.00044 m = 0.44 mm

4.4 Mesh

The mesh is refined by reducing the element size of the outer enclosure and selecting multizone method to incorporate hexahedral meshes. The inner enclosure is subjected to body sizing with finer grid size. The bottom cylindrical regions of the car body are meshed with face sizing to ensure smooth fluid flow along the circular walls. Furthermore, the faces of the car body is subjected to inflation layer of several layers of the type- total wall thickness,

Fig 10-Multizone meshing for outer enclosure

Fig 11- Body sizing for inner enclosure

Fig 12- Face sizing on cylindrical extruded boss

Fig 13- Inflation layer on named selection- Car-wall

The case is divided to three different mesh patterns details of which are shown in the table below

Table-2 Different cases of Mesh refinement

Mesh	Inner enclosure
Case 1	Case 2	Case 3
Element size- Enclosure 1	0.1	0.1	0.1
Element size- Enclosure 2	0.05	0.035	0.025
Face sizing	0.005	0.004	0.003
Inflation layers	5	6	8
Total layer thickness	0.0124	0.0075	0.0025
Number of nodes	26157	47979	110913
Number of elements	87180	199037	501958

4.5 Solver

The same settings are used to run the simulation.

4.6 Results

4.6.1 Residuals

Fig 14 –Residuals for three different cases of mesh refinement

The brief study of the residuals for the three cases suggest convergence of solution at 1400, 850 and 800 iterations

4.3.2 Velocity plot

Fig 15 –Velocity contour for three different cases of mesh refinement

Fig 16 –Velocity vector plot for three different cases of mesh refinement

From the velocity contour plot and vector plots, we can observe the wake region with backflow, the length of the wake region, the flow separation and recirculation regions around the Ahmed body. A brief comparison of the plots for the three cases suggests the best results for the case-3 with highest level of mesh refinement.

4.3.4 Force coefficients

To quantify the forces in wake region, we calculate the drag and lift coefficients for all three cases.

Fig 17- Reference values for simulation

Fig 18- Drag and lift coefficients for case-2

Table-3 Comparison of results for the three cases

Mesh	Baseline	Inner enclosure
Case 1	Case 2	Case 3
Element size- Enclosure 1	0.31146	0.1	0.1	0.1
Element size- Enclosure 2	Nil	0.05	0.035	0.025
Face sizing	Nil	0.005	0.004	0.003
Inflation layers	Nil	5	6	8
Total layer thickness	Nil	0.0124	0.0075	0.0025
Number of nodes	8672	26157	47979	110913
Number of elements	42983	87180	199037	501958
Cd	0.3913	0.246	0.3662	0.3662
Cl	0.2407	0.1899	0.2773	0.3043

Using the experimental results performed in the research work carried out by Meile et al https://www.researchgate.net/publication/330383775, the drag coefficient for Re=1.74 e006 was 0.33.

Thus, the given simulation study is able to calculate Cd=0.366 with an error of 10% with experimental results.

1. Grid dependency

A comparison of the drag coefficient calculated in the different cases indicates that the results are very similar for case-2 and case-3. The same can be observed in a velocity line plot at a short distance from the back of the body along the y-axis.

Fig 19 Velocity line plot at wake region along y-axis

Thus, it can be concluded that the solution obtained for case-2 is a grid independent solution.

1. Pressure contour plot

The study is further extended to plot the pressure contour plot as shown below:

Fig 20 –Pressure contour plot

6.1 Negative pressure in the wake region.

It can be observed from the pressure contour plot that pressure at the rear end of the Ahmed body is negative. As the air flows over the body, the velocity increases to avoid separation of the flow. This increase in the velocity results in decrease of the pressure. At the wake region, the recirculation and backflow results in significant drop in velocity profile and in turn results in negative pressure in the region.

Due to the negative pressure at the wake region, a force is exerted from the front wall to the back wall. This force is the drag force, which the vehicle has to overcome by expending fuel.

1. Significance of the point of separation.

The point of separation of flow in the car body determines the size of the wake region. An early flow separation would results in a large wake region and higher drag forces. This would significantly affect the fuel efficiency of the vehicle. On the other hand, optimization of the aerodynamic design in order to shift the point of flow separation is one of the most influential parameter in achieving low drag coefficients. In case of Ahmed body the flow separation can be controlled by adjusting the slant angle φ.

1. Conclusion

Thus, the study successfully simulates the air flow over Ahmed body to determine the velocity, pressure contours, wake region and the force coefficients by performing a grid independency test.