Ahmed Body
The Ahmed Body was first created by S.R. Ahmed in his research “Some Salient Features of the Time-Averaged Ground Vehicle Wake” in 1984. Since then, it has become a benchmark for aerodynamic simulation tools. The simple geometrical shape has a length of 1.044 meters, height of 0.288 meters, and a width of 0.389 meters. It also has 0.05-meter cylindrical legs in height attached to the bottom of the body with diameter of 0.03 meter and the rear surface has a slant of 0.222 meter that falls off at 25, 30 and 35 degrees as shown in Figure 1.
Figure 1. Ahmed Body
Ahmed body is a generic car body (a simplified car model) i.e the flow of air around Ahmed body captures the essential flow features around an automobile.
ANSYS is a general purpose FEA and CFD simulation software. It gives numerical prediction of the behavior of a system. These numerical predictions need to be validated by experimental data. People working in vehicle aerodynamics use Ahmed body to validate their numerical model because the experimental data from wind tunnel testing is available for Ahmed body. Once the numerical model in validated, it is used to design new models of the car.
Grid Independency Test:
Grid independence is a very important issue in numerical simulation, Grid-independent means calculational results change so little along with a denser or looser mesh that the truncation error can be ignored in numerical simulation. Whether the grid is independent directly influences the truncation error or even the rationality of numerical results. The previous research reveals that the grid resolution and time step have a very great effect on the results of unsteady numerical simulation in a certain range. When considering grid-independent issue, in principle a very dense grid can avoid this problem but the calculational resource may be wasted unnecessarily.
In practice, we usually increase the mesh resolution according to a certain ratio and then compare the results of two neighborhood results. If the results tend towards identical, the grid can be considered as grid-independent. Such strategy can utilize computational resource most efficiently as well as obtain reasonable results. The truncation error ɛ caused by grid resolution is defined as the difference between the grid independent result Ø grid independenceand current numerical result Ø :
ɛ= Ø grid independence - Ø
According to previous studies, truncation error ɛ will become smaller and smaller by refined
computational grid. In ANSYS grid independence can be performed by parametric study where the given input is Mesh element size and Body sizing element size and output is drag and lift coefficient as shown in Figure 2.
Figure 2. Parametric Results
From the obtained data, graph between mesh size and output parameter is generated for the observation. As it can be observed from Figure 3. and Figure 4. that after reducing mesh size further from 80 mm there is very less deviation in the values of drag and lift coefficient. Hence, there is no problem in taking 80mm size for meshing as trunacation error is getting reduced significantly.
Figure 3. Graph of Mesh Size vs Drag Coefficient
Figure 4. Graph of Mesh Size vs Lift Coefficient
Geometry Preparation:
Once the CAD Model is ready, it is very important to create a numerically acceptable geometry for the solver to perform CFD Analysis. For performing CFD, computational domain around the Body is required, which obtained by creating enclosure around the body as shown in Figure 5. Height and width of the enclosure from near surface of car is 1 meter. Length of enclosure at front and at rear is 3 meter and 6 meter respectively from the near surface of Ahmed body. The purpose of providing maximum length behind the car is to ensure that the wake behind the car is properly solved before exit plane.
Figure 5. Enclosure around Ahmed body
Meshing:
After the Geometry was reconstructed and became numerically acceptable, the file was imported into ANSYS, to construct the three-dimensional Grid system. Multizone mesh cells were used in the computational Domain.
While creating numerically acceptable geometry, two enclosures were prepared, smaller one to capture wake more accurately with tetrahedral mesh and body sizing of 40mm. The bigger enclosure was meshed with hex dominant elements with element size of 80mm in the far-field where the incoming flow is assumed to be undistributed by the presence of the car. The Grid density is high around the car where the flow gradients can be large which can be observed easily in Figure 6. For the same reason, there are also densely pack mesh near the car surface which can be observed from Figure 7. There are 710126 nodes and 187760 elements in the grid.
Figure 6. Meshing of Enclosure
Figure 7. Enlarged view of Mesh
For the geometry, inflation feature has been setup to utilize the growth of 5 layers from the surface of car boundary with total thickness of 12.5 mm and 1.2 growth rate from the first layer. In addition to capturing the boundary layer effect accurately, inflation also contributes to lesser element count and computational time. Inflation layer are clearly visible in Figure 8. around the surface of solar vehicle.
Figure 8. Inflation Layers around Ahmed Body
Boundary Conditions:
The front plane was given the “velocity-inlet” boundary condition. The bottom of the domain and ahmed body was set as “No slip wall” and the top and the sides of the domain are set as “Symmetry” so that these surfaces would not bring any effects on the simulation. The outlet boundary condition is set to “Pressure-outlet” with gauge pressure of 0 Pascal. All the boundaries can be observed in Figure 9.
Figure 9. Boundary Condition for Enclosure
In Fluent, the three dimensional, segregated, steady state solver is used. Air was selected as working fluid with density of 1.225 kg/m3.Reference values for area, length, velocity and viscosity were given as 0.131482 m2, 1.044 m, 25 m/s and 1.7894e-05kg/m-sec respectively. In addition to the Residuals of numerically solved governing equations, monitoring of the lift coefficient Cl and the drag coefficient Cd to determine the convergence of the computations has been done.
Simulation Result:
The numerical simulation was converged for 124 iterations displaying message in the console as shown in Figure 10.
Figure 10. Converged Solution
The residual is the difference between the previous result and the current result. As these errors are decreasing the equation results are reaching values that are changing less and less. This is what is known as convergence. The residual plot for the Ahmed body is shown ib Figure 11.
Figure 11. Residuals Plot
The numerical drag coefficient evolutions during the iterations can be observed in Figure 12. The final value of drag coefficient computed is 0.3364.
Figure 12. Drag Coefficient Plot
The graphical change in lift coefficient during the iterations can be observed in Figure13. The positive value of ‘coefficient of lift’ means an upward force is exerted on the body. The value of lift coefficient after simulation is 0.28782.
Figure 13. Lift Coefficient Plot
The pressure distributions on the surfaces of the ahmed body has been examined and presented in Figure 14. The regions of high pressure appear at the frontal area of the body. The airflow experiences resistance at these locations, hence it is expected that the pressure increases when velocity drops. Also, we can see that the flow field around the whole car surfaces develops in a relatively smooth manner expect for the frontal area.
Figure 14. Pressure Contours
Velocity vectors and contours can be observed in Figure 15. and Figure 16. respectively at mid-plane of vehicle. They provide an excellent visualization of the flow around the ahmed body depicting details of wake region. Wake region is the most important thing to analyze in order to determine amount of drag and lift experienced by the body which can be observed clearly behind ahmed body.
Figure 15. Velocity Vectors
Figure 16. Velocity Contours
Negative Pressure in Wake Region:
Consider a fluid particle flows within the boundary layer around the ahmed body. From the pressure distribution measured in Pressur Contour, the pressure is a maximum at the frontal area and gradually decreases along the body. Due to gradual decrease in pressure, fluid particle accelerates and results in increase in its flow velocity. The flow stays attached in this favorable pressure region as expected.
However, the fluid particle at rear of the ahmed body experiences flow separation generated by slope present at rear of the ahmed body, leaving a highly turbulent region behind the body called the wake. Wake region is produced because fluid particle is not able to fill the region generated by slope responsible for low pressure (or negative pressure) space.
Significance of Point of Separation:
The point of separation is the point where the air stops "sticking" to an object that is moving through the air. When an object is moving through the air, the air molecules push back on it and resist the object's movement - this resistance is called pressure drag. As the air flows around the object, it "sticks" to the object, forming what is known as the boundary layer. This "attached flow" is flowing very smoothly. The point on the body where the boundary layer lifts off the surface is called the point of separation. When the air flow separates off the surface, the pressure drag usually increases.