Flow Over Ahmed Body (Steady Analysis)

Project Title: Study the flow over the Ahmed Body.

Objective:

1. Study the negative pressure gradient in the wake region.

2. Study the significance of point of separation.

3. Study the Drag and Lift coefficient at a various rear slant angle.

4. mesh independence study.

Introduction

The flow around road vehicle (car, buses, trucks) under normal operating condition is principally turbulent. It is typically characterized by large-scale separation and recirculation regions, a complex wake flow, long trailing vortices and interaction of boundary layer flow on vehicle and ground. In developing a new road vehicle it is essential for the designer to understand thoroughly the structure of flow around the vehicle. This will have an influence on such principal feature as the shape of the vehicle, aerodynamic drag, fuel consumption, noise production and road handling. Traditionally, vehicle designer has gained their understanding of the airflow around a vehicle through extensive wind tunnel testing.

What is an 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, the height of 0.288 meters, and a width of 0.389 meters. It also has 0.5-meter cylindrical legs attached to the bottom of the body and the rear surface has a slant that falls off at 40 degrees.

fig 1 2D diagram of Ahmed Body.

fig 2 3D model of Ahmed Body for CFD simulation.

Aerodynamic Design of Ahmad Body

Aerodynamics analysis is used in the design of the car to reduce the drag coefficient. The investigation has obtained the behaviour of newly developed turbulence models for complex geometry cases, a simplified car model, known as the Ahmed body, has been tested by Ahmed. The Ahmed body is made up of around front part, a moveable slant plane placed at back part of the body to study the coefficient of drag and separation phenomena at different angles, and a rectangular box, which connects the front part and the rear slant plane. As the wake separation flow behind the Ahmed body is the main contributor to the drag force, accurate prediction of the separation process and the wake flow are the keys to the successful modelling of this case.

Many researchers have made use of CFD techniques to perform numerical simulations related to an automobile. Several numerical simulations were performed to analyse the pressure field, velocity vector field, and aerodynamic force prediction related to a passenger car. The external surface of the car is very important in aerodynamics aspects of vehicles such as stability, comfort and fuel consumption at high speeds. The total weight and modification of the external surfaces of the car are the most important to improve the aerodynamics characteristics of the car. These characteristics are helpful to improve the cruising conditions, greater stability of navigation, and lower fuel consumption. This is possible only when a redesign of car and frame and use of electronic devices in the car.

Modelling Airflow Over The Ahmed Body.

In the Airflow Over the Ahmed Body verification model, our Ahmed body has a 20-degree slant and is placed in the following domain, measuring 8.044-by-1.261-by-0.761 meters, to compute the flow field. The front of the body is placed at a distance of 2 car lengths (2L) from the flow inlet. To reduce the computational cost, the asymmetry plane is introduced to model half of the model. To capture the wake region another small encloser is created around the body.

The flow for this model is turbulent, which is based on the Reynolds number determined by the body length and inlet velocity. The simulation solves for the turbulent kinetic energy in addition to the velocity field. For this simulation, we need a larger mesh size than what is usually common to resolve the turbulent flow. More specifically, we use a finer mesh downstream of the model to capture the wake zone.

The flow for this model is turbulent, which is based on the Reynolds number determined by the body length and inlet velocity. The simulation solves for the turbulent kinetic energy and dissipation in addition to the velocity and pressure fields.

fig 3 Enclosure Model

Meshing

fog 4 Meshing of an enclosure model

The structural hexahedral mesh is used in some part of enclosure to reduce the overall mesh count. The unstructured tetrahedral mesh is used near the Ahmed body for better flow physics study.

.

fig 5 Operations used during meshing.

to add boundary condition we need to give an appropriate name to the body part like inlet-outlet wall symmetry etc.

fig 6 Inflation layer addition over car wall.

to capture the boundary layer over the car wall we need to add prism layer in the flow direction. for external flow simulation, I am considered y+ value 100.

fig 7 First layer height calculation

for first layer height calculation, I am considered inlet velocity 25m/s density of air 1.225kg/m3 dynamic viscosity 0.000017984kg/m*s characteristic length of car body 1.044m and y+ value 100.

first layer height thickness has come around 0.0014396m and Reynolds number 1777830.29

total no of prism layer is 5

growth ratio of the prism layer is 1.2

fig 8 Total no of Element and Nodes

fig 9 Orthogonal quality of the mesh

Orthogonal mesh quality should be greater than 0.1

Setup

• The density-based solver is used because it solves the coupled set of the equation such as continuity, momentum, and energy in a coupled manner. it\'s slower and memory intensive to solve because it solves all equation in one iteration. Density base solver may give better accuracy over the pressure base solver for compressible flow.
• Steady-state simulation is done.
• Viscous Model: k-epsilon Realizable Enhanced Wall Treatment model is used.

K epsilon (k-ε) turbulence model is the most common model used in Computational Fluid Dynamics (CFD) to simulate mean flow characteristics for turbulent flow conditions. It is a two-equation model that gives a general description of turbulence by means of two transport equations (PDEs). The original impetus for the K-epsilon model was to improve the mixing-length model, as well as to find an alternative to algebraically prescribing turbulent length scales in moderate to high complexity flows.

1. The first transported variable is the turbulent kinetic energy (k).

2. The second transported variable is the rate of dissipation of turbulent kinetic energy (ε).

The enhanced wall treatment is a blended wall model or wall function. It blends the separate models in the two-layer approach by use of a damping function so that the transition between the two is smoother.

• Fluid Material: Air Density 1.225kg/m^3, Viscosity 1.7894e-5 kg/m*s

Boundary Condition

• Car Wall: No-slip boundary condition
• Ground Wall: No-slip boundary condition
• Inlet: Velocity 25m/s
• Outlet: Pressure outlet 0 pa (gauge)
• Symmetry: Symmetry

Solution Method

fig 10 Solution Method

Implicit Least Square Cell-Based method is used. For Flow, Turbulent Kinetic Energy, Turbulent Dissipation Rate Second-Order Upwind Scheme is used.

A pseudo transient is a form of implicit under-relaxation for steady-state cases. It helps in stabilizing the case and at the same time gives faster convergence.

Solution Control

fig 11 Solution control

Result

1. At velocity 25m/s and rear slant angle 20-degree

fig 11 Residuals plot

As we see the pattern of residuals is constant from 1200 iteration to 2000 iteration so we can conclude that solution is converged.

fig 12 Drag coefficient plot

the mean value of the drag coefficient is 0.32718 and experimental is 0.33 so the error is 0.8545%

fig 13 Lift coefficient plot

fig 14 pressure contour on the symmetry plane

As we see in front of Ahmed body pressure is high because the whole kinetic energy of air converted into pressure energy (stagnation point). as the air move over the body pressure start reducing and velocity start increasing. in some part, negative pressure is created.

fig 15 Pressure contour on Ahmed body

The air becomes almost stagnant as it strikes the vehicle which results in air exerting very high pressure on the front-engine grill of the vehicle represented by the red area. The airflow then gets divided between the upper and lower surface of the vehicle. The higher pressure air on front surface accelerates as it travels over the curved nose surface of Ahmed body, causing the pressure to drop. This lower pressure creates lifts over the roof 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 creates lift that then acts upon the surface area of the rear slant.

fig 16 Velocity contour on the symmetry plane

Velocity contour is exactly opposite to pressure contour. in front of body velocity is zero. velocity is minimum at the rear slant side due to formation of vortices.

fig 17 Recirculation velocity vector at the rear end

fig 18 Path line of velocity at rear end

fig 18 Velocity contour at the various rear angle

Gives us the velocity of air along different geometry sections of the Ahmed body. The yellow area corresponds to the velocity 25m/sec, while the blue area shows low velocity and high-pressure region and red area gives high-velocity low-pressure region.

The velocity contours clearly indicate that the wake region, and consequently the form drag, continually decreases as the rear slant angle is increased from 20-30 degree and thereafter, boundary layer separation occurs on the rear slant. However, there is an increase in a lift with an increase in rear slant angle due to a larger pressure difference generated between the top and bottom surfaces of the vehicle, and this results in larger lift-induced drag. So, a trade-off between these two drag mechanisms is done to determine the optimum angle giving minimum drag coefficient.

As the wake area is reduced, the drag-causing eddies (vortices), generated due to the pressure difference between the top and bottom of the Ahmed body at the rear trailing end, come closer together. This results in less kinetic energy being dissipated due to these smaller eddies and consequently less compensation power required by the engine to propel the vehicle forward. It results in higher pressure being applied at the rear surface of the body and consequently less form drag.

Conclusion

• Critical rear angle is 3 degree.
• At 25m/s with 20 degrees rear slant angle, the mean value of the drag coefficient is 0.32718 and experimental is 0.33 so the error is 0.8545%
• The drag and lift coefficient becomes randomly dispersed after the flow becomes unattached after increasing rear slant angle to 30 degrees and beyond.
• Flow circulation rake place at rear end of the body.

Reference

• Ahmed, S.R. and Ramm G., “Some salient features of the time-averaged ground vehicle wake,” SAE Technical Paper 840300, 1984
• C. M. E. Robinson, “Advanced CFD modelling of road-vehicle aerodynamics,” PhD. Thesis, University of Manchester Institute of Science and Technology, May 2001.
• R. B. Sharma and R. Bansal, “CFD simulation for flow over passenger car using tail plates for aerodynamic drag reduction,” IOSR-JMCE, vol. 7(5), pp. 28-35, 2013.
• S. Yongling, W. Guangqiang and Xieshuo, “Numerical simulation of the external flow field around a bluff car,” Shanghai Tongji University Shanghai, China.