Ahmed Body Challenge
AIR FLOW AROUND AHMED BODY
AIM:-
To perform a CFD analysis on the air flow over a Ahmed body and extracting the important flow parameter like velocity ,pressure and force. Evaluating drag, lift and wake region on Ahmed body.
Introduction:-
Aerodynamics analysis is used in the design of car to reduce drag coefficient. The investigation has obtained the behaviour of newly developed turbulence model for complex geometric cases, a simplified car model known as the Ahmed body, has been tested by Ahmed. The Ahmed body is made up of a round front part, a slant plane at back , a rectangular box which connect the front and the rear part and a wheel base. The flow around road vehicle under normal operating condition is principally turbulent. It is typically characterised by large scale separation and recirculated regions, a complex wake flow, long trailing vortices and interaction of boundary layer flow on vehicle and ground. In developing of a new road vehicle it is essential for the designer to understand thoroughly the structure of flow around the vehicle. This will have influence on such principal feature as the shape of vehicle, aerodynamic drag, fuel consumption , noise production and road handling. Traditionally vehicle designer have gained their understanding of the air flow around a vehicle through extensive wind tunnel testing.
As technology is continuously advancing the CFD has evolves sufficiently to calculate drag and lift on a road vehicle without resort wind tunnel testing. however it take a large resources to gain solution . in order to reduce this to a time scale which is acceptable to vehicle designer ,it is necessary to use a simplified computational technic and adopt a model to describe the mean effect of turbulence. road vehicle aerodynamic design vehicle attributes affected by aerodynamic, typically aerodynamic characteristics and method of calculating road vehicle flow. A road vehicle as being essential a bluff body in a very close ground proximity . the geometry of the vehicle is complex the flow around it is fully three dimensional , the boundary layer are turbulent flow, separation is common and there are large turbulent wake in which longitudinal trailing vortices are common. As is typical for a bluff bodies the principal contribute to drag experience by a road vehicle is pressure drag and major objective of vehicle aerodynamics design is the avoidance , reduction or control separation. Aerodynamically optimized road vehicle still have a flow separation at the rear end.
THEORY:-
Air has a tendency to curl downwards around the ends of a car, travelling upwards from the high pressure region under the car to the low-pressure region on top, at the rear end of the automobile and subsequently collides with moving low-pressure air. The kinetic energy of these turbulent air spirals acts in a direction that is negative relative to the direction of travel intended. Thus, the car engine must compensate for the losses created by this drag. Vortices are released during flow separation and trail downstream to form structured or unstructured wake patterns. A wake is the region of re-circulating flow immediately behind a moving or stationary solid body, caused by the flow of surrounding fluid around the body. The local disturbances in the flow pattern behind the vehicle causes a momentum loss thus causing form drag which extends far behind the bodyworks of a vehicle.
Normally when flow flows over a flat plate we take a pressure gradient to be zero. Due to zero pressure gradient, the free stream velocity over the boundary layer has to be constant according to Prandit integral momentum equation. But when there is pressure gradient over a solid bodies i.e. curved surface , free stream velocity changes. If pressure gradient is negative, then it is favourable condition for flow. But when pressure gradient is positive fluid velocity decrease. Velocity inside boundary layer also decrease . at a certain time fluid attain a zero velocity. This streamline having zero velocity can not move in forward direction so its separates from the path. If a boundary layer encounters a pressure gradient that oppose its flow, it slow down, if this gradient is strong enough ,its stop entirely and start to form a small zone od slowly recirculating fluid. When this happen, not only the fluid layer immediate above the bubble slowed down, but now the streamline must travel a grater distance to cross over the solid object. The slowly recirculating flow applies a considerable amount of retarding shear on the main flow further slow down. The net result of this is that freestream flow effectively sees a thicker object retarding it. In aerodynamics flow separation result in reduce lift and increase pressure drag caused by the pressure difference between the front and rear surface of the object.
The generic Ahmed Body reference model has been chosen as the benchmark for carrying out computations for studying of the aerodynamic parameters. The body was first proposed by Ahmed et al. (1984).The Ahmed body is a very simple bluff body which has its shape simple enough to allow for accurate flow simulation but retains some important practical features relevant to automobile bodies. It has a slant on its rear end, whose angle can be manipulated and the corresponding drag and lift coefficients calculated. This is done to exhibit the air flow over the different geometry sections of an automobile and in its vicinity, at different slant angles. This model portrays how to calculate the turbulent flow field around a simple car-like geometry using the turbulent flow, k-epsilon interface. Ahmed et al. (1984) analysed time averaged wake structure around the Ahmed body at a Reynolds number equal to 1.2*106 by manipulating the rear slant angle in the range of 0-400 in increments of 50. However, the study did not yield information about unsteady flow characteristics of the flow around the Ahmed body.
The aerodynamically unfavourable wheels are exposed to airflow of relatively high velocity. It has been observed by means of experimental investigation that the addition of wheels and wheelbase to it leads to an increase of around 30% drag and 40% lift, respectively . another effect of the car body that influence significantly the drag caused by the wheel is its usually short longitudinal extension. This result in a strong impact of the frontal part of the vehicle o the direction of the flow of the wheels. if the distance between the front of the body and the wheel axis is decreased the yaw angle of the flow increase. It has been found that the wheel angle is very sensitive to yaw angle of attack. It has been found that the major part of the drag coefficient increase due to the addition of the wheel and the wheelhouse generated on the lower portion of the wheels which are exposed to the flow in the ground clearance of body. This lower portion of the wheels is very important source of large pressure force together with the flow inside the wheelhouses also has significant value on the over all flow field. The present case the Ahmed body is investigate with wheels.
Geometrical details:-
The following Figure 1, shows the Standard Ahmed Body. Among a number of design requirements, the reduction of both drag and aerodynamic heating is the major challenge in the design of supersonic and hypersonic vehicles. Reducing the aerodynamic drag on these vehicles ensures reaching the desired range (or altitude) and, in the same time, enables economizing the fuel usage, simplifying the
Figure 1, Ahmed body Figure 2, Dimensions
propulsion system requirements, and maximizing the ratio of payload to take-off gross weight. The reference Ahmed Body is 1044mm long, 389mm wide and 288mm high front radius is 100m, the slant angle is 20 degree and slant length is 222mm, wheel radius 30mm with ground distance to body bottom is 50mm as shown Figure 2. In ANSYS 2019 R3 Space claim, a single body domain of air is created surrounding the Ahmed body walls after subtracting it from the air enclosure. The dimension of enclosure in +X axis is 5m,in -X axis is 2m,in +Y axis is 1m, -Y axis is 0m, +Z axis is 0 and in -Z axis is 0.5m as shown in Figure 3.The refinement must be given to successfully examine the
Figure 3, Domain Enclosure Figure 4, Refinement enclosure
Figure 5, Simulation Model
wake region . For refinement an enclosure is created with dimension with +X axis 1m ,-X axis 0.5m, +Y axis 0.5m, -Y axis 0m,+Z axis0 and in -Z axis 0.26m as shown Figure 4. As the body is perfectly symmetrical so in present case we take only half of Ahmed body to reduce the mesh count. For this we have a option called split body in Space claim with this tool we split body in to two half and active only one half for physics. This will lead to reduce a mesh count and lower computation time then we use mirror command to reflect the same as shown Figure 5.
MESH:-
On the outer air domain the hex mesh is generated with Multizone mesh technique . In global setting maximum and minimum size is defined so that mesh will be uniform in outer domain . To create a good face mesh between outer domain and refinement area the interference with enabled share topology option must be generated in Space claim so mesh would not we overlap and connected uniformly as shown in figure 6 and 7. For refinement region tetra mesh is generated with using Face sizing option. For wheel the face mesh is generated. To evaluate a turbulent flow and implement the near wall treatment ,refined mesh near the wall is given, for this 8 layers of inflation layer is created with transition ration of 1.2 and wall distance is calculated with Y+ value of 100 so first cell height is 1.4mm as shown in Figure 8 and 9.
Figure 6, Final Mesh
Figure 7, Refinement mesh Figure 8, Inflation layer
Figure 9, Trimetric view of mesh
Grid independency study:-
In order to obtain a CFD simulation, independent of grid size, a set of three simulations with different grid size were carried out with
Grid – A: 117304 element
Grid – B: 281344 element
Grid – C: 504330 element
The drag and lift coefficient estimated from these three grids at flow condition correspond to inlet velocity of 25 m/s. number of iteration take to converge the solution is also described.
|
GRID |
Element number |
Drag coefficient |
Lift coefficient |
Iteration |
|
Grid A |
117304 |
0.33 |
0.21 |
576 |
|
Grid B |
281344 |
0.29 |
0.25 |
791 |
|
Grid C |
504330 |
0.28 |
0.24 |
818 |
From the table it is shown that the between grid A and Grid B the difference between drag coefficient is 0.04 and also the difference between Grid B and Grid C ,difference between drag coefficient is .01 so Grid C give a more appropriate value of drag coefficient also we can go for more element number but it take much more time to simulate and due limitation of computing power it be maximum number of element we can support for simulation. From some of the research paper experimental value of Drag coefficient on Standard Ahmed Body for Grid C seems much closer than any other grid size therefore we choose Grid C for all remaining calculation. The graph showing variation with size is shown in Figure 10.
Figure 10, Grid Independency
Solver setup:-
For the present work the solver used was Fluent 2019 R3. The solving technique is solver for 3D, steady state, compressible flow using double precision and serial processing technique. For present case we choose a compressible flow . its seem that for a velocity of nearly 100m/s or above Mach number 0.3 the compressible flow is preferred but in our case we have a free stream velocity of 25 m/s which is less than 100 m/s but to implement the effect of compressibility of fluid in simulation equation we choose Flow as a Compressible flow. In fluent we choose density based solver. Defining models such as viscous model Standard K-e model is done. A standard wall function with non equilibrium wall function is opted for near wall treatment. It takes in to account the effect of pressure gradients o the distortion of the velocity profile and by that account for some non-equilibrium effect. The fluid is taken as Air and it’s property is taken as density =1.225 kg/m^3, viscosity = 1.7894 e-05 kg/m-s, .
The input boundary condition needed for the simulation has been taken as , Input is velocity input of 25 m/s, outlet is taken as pressure outlet at zero gauge pressure, outer wall is taken as symmetry and car wall is also taken as wall with wall condition no slip and adiabatic wall condition then for half symmetry is taken as symmetry.
Solution method is implicit and in reference value for area is calculated from command called projected area under result the frontal area is calculated which project along the X axis. The reference length is 1.044m and velocity of 25m/s. to calculate the drag and lift coefficient on car wall we create a plot in report definition for both drag and lift coefficient. Solution is initialized with Hybrid initialization. Number of iteration is set to 1000 to get converge solution.
Results:-
The drag and lift coefficient is calculated on a Standard Ahmed body and plot is extracted as shown in Figure11 and 12 . From the velocity contour on figure14 and 15 it is clear that flow become unattached at rear slant. In figure ,at given velocity of 25 m/s air the green area correspond to the velocity at 25 m/s, while blue area show low velocity and high pressure region and red area gives the highest velocity at low pressure region as shown in Figure 18. The velocity contour clearly indicate that the wake region. The boundary layer separation occur at the rear slant.
Figure 11, Drag Coefficient Figure 12, Lift Coefficient
Figure 13, Convergence plot Figure 14, Velocity Contour
Due to the wake region the drag causing eddies are generated and cause a pressure difference between top and bottom result in much higher kinetic energy being dissipated and more power is required by the engine to propel the vehicle forward. The air becomes almost stagnant as it strikes the vehicle which result in air exerting very high pressure on front engine grill of the vehicle represented by the red area. The flow area gets divided between the upper and lower surface of the vehicle. The higher pressure air on front surface accelerate as its travels over the curved nose surface of Ahmed body, causing the pressure drop. This lower pressure create lift over the roof
Figure 15, Velocity contour in refined area
surface as the air passes over it. As the air continues to flow and make its way to the rear a notch is created by the rear slant owing to flow separation, leaving a vacuum or low pressure space which the air is not able to fill properly. The resulting lower pressure create lifts that then act upon the surface area of the rear slant. From the convergence plot all variables are continue to decrease showing good criteria for convergence and all variables oscillate with same frequency and continue to show decreasing trend as shown in Figure 13.
Figure 16, Vector plot
Figure 17, Vector plot showing wake region Figure 18, Pressure contour
Another goal is to visualization of velocity on the wake region n downstream of Ahmed body with plotting a line in two different region where wake is generated. In figure 19 the line placed just behind the Ahmed body the velocity along the height is calculated and we see that velocity first decrease and then oscillate showing the region of recirculated air then as flow goes downstream is stabilize to final velocity and on Line 2 which is placed further away show a less oscillation means wake region is dispersed as shown in Figure 20. Vector plot is shown in Figure 16 and 17, which clearly illustrate the wake region behind the Ahmed body.
Figure 19, Line behind Ahmed body Figure 20, Velocity chart on line
Conclusion:-
The good CFD analysis of Ahmed body using Fluent is performed successfully. It has been shown that simulation provide a good agreement with the Standard data, in terms of drag and lift coefficient ,velocity profile and wake region.
The drag coefficient of Ahmed body is calculated as Cd= 0.28 and lift coefficient Cl= 0.24. overall the velocity profile from simulation show good agreement and the wake region generation as what we expected . the recirculated region on downstream side of Ahmed body is clearly defined in both velocity contour and velocity vector plot.