Study of Aerodynamic Flow Processes Around The Ahmed Body and Validation Against Experimental Data For a 35 Base Slant

Objective:  The shape of a car body in-front of the largest cross-section has only minor influence on the total drag. The main contributions to the drag force originate from the rear part of the body. A drag breakdown reveals that 85% of body drag is pressure drag, most of which occurs at the rear end. The rest 15% is due to friction. Thus, it is very important to design a rear body surface which brings the divided or separated streamlines smoothly together. The Ahmed Body was designed with the intent to characterize this wake region that originates on the rear of an automobile. With Computational Fluid Dynamics (CFD), it is possible to visualise the flow field around the Ahmed Body. This entire project has been divided into four main phases:

• Modelling of the Ahmed Body and Wind Tunnel Geometry
• Case Setup or Pre-Processing
• Post-Processing and Visualisation
• Validation Against Experimental Data

Introduction: Ground vehicles can be termed as bluff bodies moving in close vicinity of the road surface. The shape of such vehicles evolved over the years under the constraints of aesthetics, service, safety etc. With conventional fuels becoming a priced commodity, it becomes imperative to reduce the aerodynamic drag of the vehicle. A salient characteristic of the flow field around an automobile are the regions of separated flow. Separated flow can be defined by those flow streamlines that instead of being parallel to the surface or laminar, get detached and give rise to turbulent flows leading to turbulent friction which in turn increases vehicle drag. Even basic vehicle configurations devoid of any attachment or protrusions and having smooth surfaces generate a variety of complex 2-D and 3-D regions of separated flows.

The Ahmed body represents a simplified, ground vehicle geometry of a bluff body type. Its shape is simple enough to allow for accurate flow simulation but retains some important practical features relevant to automobile bodies. Selection of the configuration of this body is governed by the requirement that it should generate the essential features of a real vehicle flow field except the flow fields that occur due to rotating wheels, engine and passenger compartment, rough underside and surface projections. The model chosen would generate strong 3-D flows in front, relatively uniform flow in the middle and a large structured wake at the rear.

Phase I: Modeling of the Ahmed Body and Wind Tunnel Geometry

The model with a length of 1.044m has a length:height:width ratio of 6.38:2.07:1. For the purpose of this study, only the half car model is simulated to save computational time. This has no bearing on experimental validation. Thus, instead of 389mm, the width considered is 163.5mm. It consists of three parts: a fore body, a mid section and a rear end. Edges of the forebody are rounded as indicated above to achieve a separation free-flow over its surface. Middle section is a box shaped sharp edged body with a rectangular cross section. The rear end has a base slant of 35° (The reason behind selecting this base slant angle has been disucssed later).The rear end has a base slant length of 222mm with sharp edges.

This CAD Model was further split symmetrically for the purpose of simulation. Having the entire Ahmed Body simulated was computationally intensive. It is then imported into Converge to create the wind tunnel around it as well as complete rest of the case setup. There were a number of guidelines that were supposed to be followed while creating the wind tunnel.

• Inlet: This would be the starting point of the airflow which would take place in positive X direction. The flow velocity was chosen as 40 m/s because for a large range of the Reynolds number, both turbulent and laminar flows are possible. In this simulation, turbulent regions are necessary at rear end of the body. Having a turbulent region trips the boundary layer ensuring that a perpendicular momentum transfer takes place that will delay flow separation. This circulation zone is known as laminar bubble, which has been discussed in the post-processing section. Moreover, the friction in laminar flow is considerably lowe which means that for the purpose of drag reduction, laminar flow is preferred.

        Calculation of Reynolds Number, `R_e = (rho*v*L)/mu`

        Where, `rho` is density, 1.225 `(kg)/m^3`

                   `mu` is Dynamic Viscosity, `1.568*10^-5 (kg)/(m*s)`

                    v is free-stream velocity and L is characteristic length, 0.288 m which is the height of ahmed body.

       Thus, `R_e = 768000`. This is the recommended value of Reynolds number to match the experimental data.

• Outlet: The far-field outlet is created at a distance such that during simulation, the conditions at the outlet would return to free-stream values of pressure and velocity. This is a good way of validating the simulation. Moreover, creating an outlet which is very near to the rear-end of the ahmed body would lead to interference with the re-circulation zone that is created. So, it\'s a good practice to have the outlet pretty far. The two images below which have been post-processed validate this case.

• Bottom (Free Slip Region): The bottom walls are divided into two portions. One portion which would be near the inlet and extend upto some distance would have free slip condition. This would ensure that the flow takes place without the formation of any boundary layer upto that region. Another guideline to be met during the case setup was the boundary layer thickness would be 30mm at 400mm in front of the body. Using this as reference, the bottom walls were sub-divided accordingly.

       Given that the thickness of the boundary layer, `delta` should be 30mm

       According to the formula, `delta = (0.342*x)/((R_e)^0.2)`

      `delta` is 30mm and `R_e` was calculated as 768000

       `x = (delta*768000^0.2)/0.342` → `x = 1.18 m`

       This is the extra distance that the Bottom (Free Slip) region will end.

• Bottom (Law of Wall): This region extends from the portion where Bottom Free Slip Wall ends upto the outlet. Initially, no slip condition was provided on this portion of the wall. Creating a no-slip region meant zero velocity on the bottom surface which led to a parabolic profile getting developed as we went up.  This led to the simulation results being offset by more than 30% from experimental data during validation phase. Having a law of the wall ensures that the `Y^+` from the bottom wall to the upward regions remain in the turbulent zone thus giving a more accurate velocity prediction.

Phase II: Case-Setup and Pre-Processing:

With the wind-tunnel created and the necessary boundaries labelled, the next step was to proceed with the case setup. The case setup involves choosing Simulation parameters, setting appropriate Boundary conditions to the assigned boundaries, initializing regions, selecting the right turbulence model, choosing grid size and finally selecting the number of files and variables to post-process.

• Run Parameters: Initially, steady-state was selected but it led to extreme difference while validating with experimental data. Thus, transient solver with Full-Hydrodynamic mode was chosen.
• Simulation Time Parameters: The end time is chosen as ~4 times one flow through time. One flow through time is `10.04/40 = 0.251 s` and end time is thus chosen as 1 second.
• Regions and Initialisation: Velocity is also specified here. Temperature is taken as 300K and Pressure as 101325 Pascals. `O_2` with a concentration of 0.23 and `N_2` with a concentration of 0.77 is pulled inside the region. If the velocity is only specified at the inlet and not inside the regions, the solver will take a longer time to run the simulation and compute the velocity and pressure at each cell when the simulation progresses.
• Turbulence Model: Turbulence modelling tries to represent Reynolds stresses in terms of time-averaged velocity components. The common turbulence models are classified on the basis of the number of additional transport equations that need to be seloved along with the RANS equations. For the purpose of this project, `k-omega` model is chosen which solves two extra transport equations to resolve the Reynolds stress tensor. This model is an improvement over the existing `k-epsilon` turbulence model and it addresses some of the key disadvantages associated with `k-epsilon`: Poor predictions for swirling & rotating flows and flows with strong separation, two of the key flow characteristics associated with Ahmed Body simulation. 

• Grid Control: The base grid size is chosen based on the wall-spacing values calculated by taking a desired `Y^+` value. These computations are based on flat-plate boundary layer theory. The inputs required are free-stream velocity, density, characteristic length, desired `Y^+` and dynamic viscosity:http://www.pointwise.com/yplus/ . The following equations are used to arrive at the wall spacing value:

1. Reynolds Number `R_e = (rho*V*L)/mu`.     
2. Skin Friction Co-efficient: It is a non-dimensional number indicating the level of friction between ahmed body and air. `C_f = 0.026/((R_e)^0.142)`.
3. Wall Shear-Stress: It is the surface shear force/unit surface and is given as `tau_w = (C_f*rho*V^2)/2`.
4. Friction Velocity: It gives the rate of increase of turbulent boundary layer. `U_f = (tau_w/rho)^0.2`
5. Wall Spacing, `y = (Y^+*mu)/(U_f*rho)`.

Based on these calculations, wall spacing came out to be 0.26mm. Having such a fine grid will lead to the simulation running indefinitely. Since, this mesh size is only required at the Ahmed Body, so a top-down approach was used to arrive at the values of base grid. Thus a base mesh of 0.02m was used across X,Y and Z.

Phase III: Post-Processing and Visualisation: The key objectives of this phase is to calculate lift and drag force using the pressure force plots, obtain velocity and pressure contours to visualise the flow around Ahmed Body and visualise wake structure at the rear end of the ahmed body.

→Calculation of Lift and Drag Force Using Paraview:

Drag force acts parallel to the wind flow and opposes the relative motion of the object. A high drag force is an undesirable phenomenon that can lead to the car working to overcome the drag force thus ending up spending fuel.The aerodynamic design of a car is a very big contributor to how much the drag force would oppose the motion of the object. Drag Co-efficient, which is normalized using the drag force gives an indication of how much aerodynamic a certain object is. Drag Co-efficient is calculated as:

`C_d= (2*F_d)/(rho*V^2*A)`,  

`C_d` is the drag coefficient,
`F_d` is the drag force
`rho` is density of the fluid in which the object is moving
`V`    is freestream velocity
`A`    is Frontal Area of the object

Lift force acts perpendicular to the wind flow and is what helps to generate downforce on an object. Cars, on the other hand, are designed in such a way that they produce a negative lift or downforce. This negative lift force helps the car to maintain contact with ground surface even at very high speeds. The lift coefficient is normalized using the lift force formula:                                        

`C_l = (2*L)/(rho*V^2*A)`,

`C_l` is the lift co-efficient

`L` is the lift force  

→As can be seen below, the drag force generated by wheels is 1.34N and the drag force generated by Ahmed Body is 14.8N 

→ Wheels generate 0 downforce because there is no place for the air to pass under the wheels so as to get a pressure differential. The Ahmed Body generates downforce of -132.9 N.

The lift and drag forces and the frontal area of the body were computed using a post-processing tool known as Paraview. For doing this, the first thing that needs to be done is convert the post-processed files using Ensight. A test.case file is generated which can be opened using paraview. Next, the steps below should be followed:

1) Go to \'Filters\' and select \'Extract Block\'. Choose Ahmed Body and Ahmed Body Wheels as the the blocks since this is where lift and drag co-efficients will be calculated.

2) Next, the surface needs to be extracted from the generated block so that normals can be generated. To do this, go to \'Filters\', select \'Extract Surface\' and then click on Apply.

3) After the surface has been generated, the next thing would be to generate surface normals using which drag and lift will be calculated. Again, go to \'Filters\', select \'Generate Surface Normals\' and then check the box \'Compute Cell Normals\'.

4) To compute Lift or Downforce, bring up calculator in Paraview. In the Result Array Name Box, type \'Downforce\', then change the attribute mode to \'Cell Data\'. After that select Pressure from the scalars drop-down menu and multiply it with NormalsY.

5) To compute Drag, bring up calculator in Paraview. In the Result Array Name Box, type \'Drag\', then change the attribute mode to \'Cell Data\'. After that select Pressure from the scalars drop-down menu and multiply it with NormalsX. Notice how most of the drag force is concentrated towards the rear end. This re-affirms the statement that was made in the Objective section of the Project: \"The shape of a car body in-front of the largest cross-section has only minor influence on the total drag. The main contributions to the drag force originate from the rear part of the body. A drag breakdown reveals that 85% of body drag is pressure drag, most of which occurs at the rear end.\"

6) Lastly, the drag and lift forces need to be integrated over the entire body using \'Integrate Variables\' Feature. Thus, the following values for drag and lift force were calculated:

Downforce : 131.693 N

Drag : -19.0154 N

7) To calculate the drag co-efficient, the frontal area of ahmed body will have to be extracted. For doing this import the post-processed file and check the box Camera Parallel Projection. Select Points On in the front view of the body. Extract selection based on the points selected. Apply the Delaunay 2D filter and set alpha value so that the ahmed body is properly selected and ensure that best fitting plane is selected here. Finally, Integrate Variables to get the Frontal Area as: `0.5289 m^2`.

•Drag Co-efficient Using Paraview Drag Force, `C_d = (2*F_d)/(rho*V^2*A)`

→ `C_d = (2*-19)/(1.225*40^2*0.5289)` → `C_d = -0.0366`

•Drag Co-efficied Using Converge Drag Force, `C_d = (2*16.14)/(1.225*40^2*0.5289)` → `C_d = 0.0311`

→`Y^+`Visualization: For Law of the Wall Model, `Y^+` should be between `30`-`100` which would indicate that the first cell is in the log-law region. A value lower than that would mean that the cell is in the viscous sub-layer or transition region. The below image shows that `Y^+` isn\'t uniform throughout the ahmed body. It is pretty high on the front side. However, the value is in the log-law range at the rear of the body. Moreover, the rear side is of a greater interest since velocities will be probed around that location. 

→Pressure and Velocity Contours Visualisation of Rear Side:   In this project, a right-half car model was simulated, so the cut-outs visible below is actually the centerline of AHmed Body. The concept of vortex-dominated flows is utilised by first relating it to a low aspect ratio flat-plate lifting surface placed at an angle of attack greater than 10°. This configuration leads to the development of two concentrated side edge vortices which dominate the nearby flow field creating strong suction forces that help increasing lift of the flat plate wing. A similar situation is developed when the rear, upper-surface of the Ahmed body is slanted. This vortex dominated flow dicussed above is present in the range of `10°<theta``<30°`. At angles greater than `30°` however, the flow over the whole rear base gets separated. This fully separated case is shown below as blue coloured recirculation zones and the corresponding pressure distribution is even as can be seen from the pressure contour. This re-circulation zone is also created due to the perpendicular momentum transfer that takes place in the turbulent region. Because of the large base slant angle the Coanda effect suddenly loses power which goes on creating this vaccuum that is rushed to fill by air thereby creating a strong re-circulation zone.

For angles greater than `30` degrees, a slight negative lift or downforce gets developed and the vortex structure breaks down thereby decreasing the effect of rear, upper-surface slant on drag and lift. This fact has a bearing on the design of hatchbacks where rear window inclination angle should be more than `35°` or less than `25°`. Thus it can be said that `30°` is the bracket angle for rear slant. At `35°` the vortex dominated flow structure breaks down. 

→Pressure and Velocity Contours Visualisation of Front Side:  As shown by the drag-force contours above, the front side barely generates any drag. Thus the discussion will only be limited to the velocity and pressure changes happening at the forebody. As the front side interacts with the oncoming flow, a stagnation region develops where the pressure suddenly increases to a large value leading to a consequential decrease in velocity as per Bernoulli Effect. As the flow moves towards the top the fluid particles start to accelerate and since the upper surface is curved upwards a region of low-pressure occcurs. The point where the forebody is curved the most, experiences a considerable drop in pressure and a subsequent increase in velocity. This region is known as the Suction Peak. Moreover, the moving stream of surface will tend to follow the curvature of the surface according to the Coanda Effect. The pressure right above the curved surface of ahmed body is lower than the free stream pressure far above it. This exerts a centrifugal force on the flow particle and keeps the flow particles attached to the curved surface.

Finally, after visualising the front, middle and rear end, the statement made in the introduction section is proved: \"The model chosen would generate strong 3-D flows in front, relatively uniform flow in the middle and a large structured wake at the rear.\"

→Wake Structure at the Rear End: As illustrated below by the left oval which is the centerline of the Ahmed Body, flow in middle part of the slant surface separates at the upstream edge (represented by blue arrows just at the tip of slant). This separation region eventually joins the separation bubble (recirculation zone) of the base. The merging of these two regions fuelled by zero disturbances in the oncoming flow leads to an absence or a sudden reduction in the strong side-edge vortices (see right side oval) that were being generated at lower base slant angles.This separation region also lowers the pressure which is present on the complete surface of base slant which is accompanied by the increase in pressure drag or drag force as shown above. 

Detached flow can also be visualised in the entire base and upper surface of the Ahmed Body. The flow detaches along the slant surface and develops a single, significantly large recirculation region within the wake.

Phase IV: Validation Against Experimental Data: In this phase, velocities at different Y-locations in Paraview will be plotted and then compared against experimental data: https://drive.google.com/file/d/1Jtr6SxhutNNEwCFPWbp2Jp7dpiSRNdzT/view?usp=sharing . In order to probe the velocities, points at distince X locations either halfway towards the rear side, at the rear side or away from the rear side where re-circulation zones occur were selected. Then by using the plot over line command the starting and ending X,Y,Z co-ordinates were entered. Points Y was selected to lie on the X-axis and Velocity_X was selected to lie on the Y-axis.

The line plots were saved in .csv format from which velocity:0, Points:0 and Points:1 were extracted and then compiled into one sheet for plotting against experimental data. The sheet can be accessed using this link:  https://drive.google.com/file/d/1WRz-Ut1FaHR2DKINgCIWU8925k6ED9B2/view?usp=sharing. The simulation does a pretty good job in capturing the physical properties of the flow field. There are slight deviations from the experimental data, especially in regions of high drag. A common feature observed in all the overlay plots is that beyond a Y-distance of approximately `0.33` metres, the value of velocity becomes somewhat uniform. The height of the Ahmed Body excluding wheels is `288 mm` suggesting that the flow variations are happening around the Ahmed Body. The flow streams at `0.33` metres and beyond start returning to free-stream velocity of `40 m/s`. 

•At `-13 mm`: This probe was made at the slant surface of the Ahmed Body where flow separations appear. The first probe is made at 0.236m which is slightly lesser than the maximum height of the body. A negative value of velocity appears between 0.236 and 0.3 metres suggesting that the flow velocity has considerably reduced and separation regions have begun forming. Right after 0.3 metres which is away from Ahmed Body in Y-direction velocity of the flow particles increases suddenly where it then reaches near free-stream velocity.

• At `-263 mm`: This is the only plot which is extremely deviating from the experimental data because `Y^+` isn\'t resolved sufficiently in these areas. The first probe has been made considerably far from the Ahmed Body where free-stream conditions are observed.   

•At `37 mm`: This probe has been made in the region where flow re-circulation is the strongest. The first point has been taken as `0.02m`, the region occuring just below the re-circulation or vaccuum zone where free-stream conditions are present as suggested below. As we start moving above, the velocity suddenly dips below `0 m/s` suggesting that this is the vaccuum zone. Beyond `0.25 m` the flow velocity suddenly increases to nearly `40m/s`.

•At `87 mm`: The flow pattern observed here is similar to the patterns at 37 mm which means that strong re-circulation is still present. 

• At `-113 mm`: This line plot was created in middle section of the Ahmed Body. The first point was plotted right above the body where the velocity suddenly increases from 0 to 40 as we move beyond towards 0.33 metres.

•At `-63 mm`: This plot was created right where the upper surface starts to slant. It is also the region where the flow suddenly separates from the surface of ahmed body which can be suggested by the negative velocities at that point.

•At `137 mm`: This plot has been created from `0.028m` which is reght below the re-circulation zone upto the point where free-stream conditions are present. The high negative velocities present seen below suggest that flow reversal is still taking place even this far from the body and is also stronger than the flow at `37mm` and `87mm`. Inspite of the absence of side-edge vortices which shape the flow mechanisms in the wake, a cross-flow field is thus observed in the far-field. A strong downwash creating vortex with a narrow core is prevalent here.

•At `187mm`: The flow pattern observed here is similar as above.

References:

[1] Race Car Aerodynamics By Joseph Katz, `2^(nd)` edition

[2] Flow and Turbulence Structures in the Wake of a Simplified Car Model (Ahmed Model) By H.Lienhart, C.Stoots, S.Becker (2003)

[3] Some Salient Features of the Time-Averaged Ground Vehicle Wake By S.R Ahmed, G.Ramm and G.Faltin (1984).

[4] https://youtu.be/VEe7NxB5Vo8

[5] NPTEL CFD Lectures By Dr.Suman Chakraborty

[6] Aerodynamics of Road Vehicles, Wolf Heinrich Hucho