Objective
1) Significance and importance of the Ahmed body.
2) To simulate the Ahmed body and calculate the coefficient of drag and lift also perform the grid dependence test.
Introduction
Two distinct regions created when the air tends to curl downwards at the rear of the vehicle.
(i) High pressure under the vehicle,
(ii) Low pressure on top,
While the airflow passed at the rear of the vehicle, there is a collision or interactions of both pressures results in a wake region. Kinetic energy from these turbulent air interactions tends to act in a direction which is opposite to the direction of travel. Resultant the car engine has to compensate energy losses as a result of the drag. During the flow separation period, vortices are created downstream forming either structured or unstructured wake patterns. Region of recirculation flow immediately behind a body that is caused by viscosity is known as a wake region. The aerodynamic forces created on a vehicle are as a result to various complex interactions between the flow separations and vortex wake’s dynamic behavior.
The Ahmed body is a generic car body or a simplified Automotive vehicle model. The essential flow has been captured by the airflow around the Ahmed body which features around an automobile and was first defined and characterized in the experimental work of S.R. Ahmed. Although it has a very simple shape, the Ahmed body allows us to capture characteristic features that are relevant to bodies in the automobile industry. This model is also used to describe the turbulent flow field around a car-like geometry. Once the numerical model is validated, it is used to design new models of the car.
The main goal of the automotive industry to reduce drag, keeping noise to a minimum, preventing lift (unwanted), and avoiding other unwanted instabilities that can occur at high speeds. Drag is a result of pressure differences between the frontal and the rear end of the vehicle. To reduce drag modifications of the vehicle design or modifications of the airflow around the vehicle. To conduct sufficient aerodynamic analysis in order to observe the behavior of turbulence and pressure, a simplified Ahmed body model will be analyzed. The body is a simplified bluff body that maintains a degree of accuracy when modeling airflow around the vehicle while maintaining great vehicle features.
Modeling: We are using the Ahmed body solid model and first create a solid model of the Ahmed body with help from experimental data. The simple geometrical shape has a length of 1.044 meters, a 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 ha s40 degrees from the top plane.
We can use any cad software for 3D modeling (I prefer for Solidworks) and after import the geometry in the space Claim for different operations.
The outcome for modeling and simulation of Ahmed Body
As we already mention that Ahmed body is the prototype of the automotive car and we run the simulation for calculating the drag and lift force on the Ahmed body. The resistance of an object in a fluid environment is quantified by the drag force. It varies with speed and direction of the flow, Object shape, and size and the density and viscosity of the fluid. The lower the drag coefficient of an object, The less aerodynamics or hydrodynamic drag occurs. In terms of a car, the lower the drag coefficient, the more efficient the car is. The wake flow behind the car is the location at which the flow separates determines the size of the separation zone, and consequently the drag force. So we need to do more exact simulation of the wake flow and of the separation process is essential for the correctness of drag predictions. However, a real-life automobile is a very complex shape to model or to study experimentally. Therefore the Ahmed body is best to use. This also helps to achieve efficient vehicles with minimized fuel consumption, CO2 emissions, and noise, while keeping good driving stability.
Also, Car with low drag is better but decreasing the drag drastically can reduce the downforce and lead to a loss in road traction and a higher and a higher chance of car accidents.
Methodology
1. Modeling of Ahmed Body
2. Meshing
3. Pre-processing
4. Setting-up physics and solving
5. Post-processing
1. Modeling of the Ahmed body:
Step:1 = Create a 3D model using 3d cad software (Solidworks)
Step:2 = Import the geometry in Space Claim ANSYS.
Step :3 Define the enclosure in space claim
Case 1: Baseline Mesh (Using 1 enclosure)
2) Meshing
Start with the baseline Mesh first to check the setup.
Also, provide the boundary names
3) Pre-processing
check the mesh first and after that define the solver. Here we used the density-based solver in steady-state simulation because mach is greater than 0.3 and for this condition, density-based solvers give a much accurate result as compared to the pressure-based solvers. Reynolds number is high so flow is turbulent and here we use the k-epsilon turbulence model with standard wall function. Air is a selected fluid for this simulation.
4) Setting up for physics and solving
providing the boundary conditions
a) inlet- velocity inlet (25 m/s)
b) outlet- pressure outlet (0 pa)
c) car wall and wall- No- slip
d) Symmetry
Also, set up the reference values at the inlet for the calculation of the coefficient of drag and lift.
The current system initialized using hybrid Initialization then run for 1000 iterations.
a) Residual Plot
b) Velocity contour
c) Co-efficient of drag
we get the Co-efficient of drag is 0.4840.
d) Co-efficient of lift
We get the coefficient of lift is 0.4044.
5) Post-processing
a) Velocity contour
b) pressure contour
c) Vector representation of velocity
Since we run the set-up for a baseline mesh we get the expected results as shown above but as we study on the velocity contour and velocity vector, we get some diffused solution because of the unstructured mesh also get the velocity vectors in some unexpected regions. In computational fluid dynamics, we are very sensitive to selecting the correct meshing which mainly depends on the element size. Normally we did a mesh sensitivity study and after getting the appropriate residual graph for convergence we take it for the problem.
The second thing is that we get the coefficient of drag for this baseline mesh is 0.4840 whereas the experimental value was 0.33. So we get a 46.66% error in the coefficient of drag which was not considerable now we need to refine the mesh and run the set up again for getting the appropriate result.
Case 2: Refining the mesh (Using 2 enclosure)
In this case, we set up a two enclosure for more understanding of the behavior of velocity near the Ahmed body and getting the much accurate coefficient of drag and lift values.
For a better understanding of surfaces, we used the midplane and also clean the interferential part so that generated mesh should be more structured and also enable the shared topology so that information will be transferred from one face to another.
Meshing
a) multizone with quad-dominant elements.
Used the element size =100 mm and maximum face size=100 mm.
b) body sizing
For enclosure 2 used the 50 mm element size.
c) face sizing
When we define the element size for enclosure 2 then we get that the shape of the ahmed body leg turns to pentagon type. So here we defined element size=5 mm to stable in their circular shape.
d) inflation
It is a very important phenomenon for refining a mesh because near the wall the center of the elements does not lie in a single line and we don't get the proper information near the walls. So here we used the boundary layer phenomenon. Using the appropriate boundary layer thickness, we can create the boundary layers.
First, calculate the first layer thickness using the Y+ value for a given velocity, area, density, and viscosity value. We can choose y+ value between 30-300 for k-epsilon with standard wall function turbulence model. For getting the correct y+ we should run the simulation and compare the coefficient of drag value from the experimental data. If the error is less than 30% in the coefficient of drag so that we can choose the desired y+ for calculation of the first layer thickness. In our case, we choose y+ 100 to start our simulation.
First layer thickness: 1.47mm
No of inflation layers: 5
Total thickness: 3.65 mm
Provide the boundary names.
3) Pre-processing
check the mesh first and after that define the solver. Here we used the density-based solver in steady-state simulation because mach is greater than 0.3 and for this condition, density-based solvers give a much accurate result as compared to the pressure-based solvers. Reynolds number is high so flow is turbulent and here we use the k-epsilon turbulence model with standard wall function. Air is a selected fluid for this simulation.
4) Set up physics and solving
providing the boundary conditions
a) inlet- velocity inlet (25 m/s)
b) outlet- pressure outlet (0 pa)
c) car wall and wall- No- slip
d) Symmetry
Also, set up the reference values at the inlet for the calculation of the coefficient of drag and lift.
The current system initialized using hybrid Initialization then run for 1500 iterations and do 1000 iterations more for finding convergence accurately.
a) Residual Plot
b) Velocity contour
c) Co-efficient of drag
we get the Co-efficient of drag is 0.406
d) Co-efficient of lift
We get the co-efficient of lift is 0.287286
5) Post-processing
a) Velocity contour
b) pressure contour
c) Vector representation of velocity
d) Line position for the velocity and pressure plots
e) Velocity plots for 3 different positions
f) Pressure plots for 3 different positions
As we can see in the above figure,
I) The problem is converged near the 1250 iterations.
II) We defined the bottom face as a wall so no-slip boundary conditions applied, that's why we get the zero velocity near in the bottom and also get some reduction in velocity as velocity passed over Ahmed body due to the boundary layer separation and friction forces.
III) The coefficient of drag is 0.406. ( less than 30% error while comparing to the experimental data.
IV) The coefficient of lift is 0.287286
V) For a better understanding of velocity flow, we create a vector plot for velocity and get some wake region behind the Ahmed body.
VI) Create a velocity plot in three different positions after the Ahmed body for better understanding. We get some velocity reduction near the wall after the Ahmed body and when we go further (from bottom to top), there is a constant velocity.
VII) Also, create a pressure plot for three different positions after the Ahmed body. We can see that it starts with some positive pressure near the wall and when it goes up in a vertical direction, there is a negative pressure that occurs in the wake region.
This simulation is done on taking y+ value 100, as we are using the k-epsilon turbulent model with standard wall function. So we can choose the y+ from 30-300. But we assure the error in the coefficient of drag value not more than 30% then refined the mesh for getting the appropriate results.
| Y+ |
Ist layer thickness |
Total thickness (5 inflation layers) |
co-efficient of drag |
% error in Cd |
| 70 |
1.028 |
2.5579 |
0.4120 |
24.84 |
| 100 |
1.47 |
3.65 |
0.406 |
23.03 |
| 140 |
2.344 |
5.845 |
0.40316 |
22.16 |
Grid Independence Test
As we get the result from taking the desired y+ value, we need to perform the grid independence test for getting the coefficient of drag values approx to the exact values.
Refine 1:
Meshing
a) multizone with quad-dominant elements.
Used the element size =85 mm and maximum face size=85 mm.
b) body sizing
For enclosure 2 used the 45 mm element size.
c) face sizing
When we define the element size for enclosure 2 then we get that the shape of the ahmed body leg turns to pentagon type. So here we defined element size=4 mm to stable in their circular shape.
d) inflation
First layer thickness: 1.47mm (Y+ 100)
No of inflation layers: 8
Total thickness: 6.32 mm
Provide the boundary names.
3) Pre-processing
check the mesh first and after that define the solver. Here we used the density-based solver in steady-state simulation because mach is greater than 0.3 and for this condition, density-based solvers give a much accurate result as compared to the pressure-based solvers. Reynolds number is high so flow is turbulent and here we use the k-epsilon turbulence model with standard wall function. Air is a selected fluid for this simulation.
4) Setting up physics and solving
providing the boundary conditions
a) inlet- velocity inlet (25 m/s)
b) outlet- pressure outlet (0 pa)
c) car wall and wall- No- slip
d) Symmetry
Also, set up the reference values at the inlet for the calculation of the coefficient of drag and lift.
The current system initialized using hybrid Initialization then run for 1500 iterations.
b) Velocity contour
c) Co-efficient of drag
We get the Co-efficient of drag is 0.4004
d) Co-efficient of lift
We get the value of lift is 0.28995
5) Post-processing:
a) Velocity contour
b) pressure contour
c) Vector representation of velocity
d) Line position for the velocity and pressure plots
e) Velocity plots for 3 different positions
f) Pressure plots for 3 different positions
Refine 2:
Meshing
a) multizone with quad-dominant elements.
Used the element size =70 mm and maximum face size=70 mm.
b) body sizing
For enclosure 2 used the 37 mm element size.
c) face sizing
When we define the element size for enclosure 2 then we get that the shape of the ahmed body leg turns to pentagon type. So here we defined element size=3 mm to stable in their circular shape.
d) inflation
First layer thickness: 1.47mm (Y+ 100)
No of inflation layers: 10
Total thickness: 9.1018 mm
Provide the boundary names.
3) Pre-processing
check the mesh first and after that define the solver. Here we used the density-based solver in steady-state simulation because mach is greater than 0.3 and for this condition, density-based solvers give a much accurate result as compared to the pressure-based solvers. Reynolds number is high so flow is turbulent and here we use the k-epsilon turbulence model with standard wall function. Air is a selected fluid for this simulation.
4) Setting up the physics and solving
providing the boundary conditions
a) inlet- velocity inlet (25 m/s)
b) outlet- pressure outlet (0 pa)
c) car wall and wall- No- slip
d) Symmetry
Also, set up the reference values at the inlet for the calculation of the coefficient of drag and lift.
The current system initialized using hybrid Initialization then run for 1500 iterations.
b) Velocity contour
c) Co-efficient of drag
we get the Co-efficient of drag is 0.4004
d) Co-efficient of lift
we get the coefficient of lift is 0.287577
5) Post-processing
a) Velocity contour
b) pressure contour
c) Vector representation of velocity
d) Line position for the velocity and pressure plots
e) Velocity plots for 3 different positions
f) Pressure plots for 3 different positions
Some observations are made on the basis of the above hypothesis
| |
Main case |
Refine 1 |
Refine 2 |
|
Enclosure 1 element size
|
100 mm |
85 mm |
70 mm |
|
Enclosure 2 element size
|
50 mm |
45 mm |
37 mm |
|
Ahmed body leg face sizing
|
5 mm |
4 mm |
3 mm |
|
Y + value
|
100 |
100 |
100 |
|
Inflation Layers
|
5 |
8 |
10 |
|
Total thickness
|
3.65 |
6.32 |
9.1018 |
|
Nodes quantity
|
57530 |
90877 |
157031 |
|
Elements
|
191051 |
279043 |
476042 |
|
Coefficient of drag
|
0.406 |
0.4004 |
0.386132 |
|
Coefficient of lift
|
0.287286 |
0.28995 |
0.287577 |
Reason for the negative pressure in the wake region
When velocity flow is higher, there should be low pressure. And in Ahmed body simulation case, the pressure is high enough to detach layer from the body while velocity and shear stress becomes zero and create a wake region There is a negative velocity gradient and shear stress due to the flow circulation which causes reversible highly turbulent flow as shown in velocity vector contour. But fluid has to move against the adverse pressure gradient resultant there should be low pressure inside the wake reason which responsible for drag force.
Significance of point of separation
The point of separation in turbulent flow is the detachment of a boundary layer from a surface into a wake in an external flow problem. Due to the friction forces, velocity starts decreasing and also gets an increase in pressure. Flowing against an increasing pressure is known as flowing in an adverse pressure gradient. The boundary layer separation starts when it has traveled far enough in an adverse pressure gradient so that the speed of the boundary layer relative to the surface has stopped and reversed direction. So the flow separation occurs and takes the forms of eddies and vortices. After separation, the fluid exerts only constant pressure. In other words, Flow separation occurs due to the pressure difference on the front and rear surface of the body.
Due to flow separation, an increase in pressure drag, and a reduction in lift occur.
Inference
1) Ahmed body is used as an automotive prototype. Once we calibrate this simulation from the experimental data, we can use the solver for complex automotive structures.
2) Mesh refinement gives more accurate results (Coefficient of drag and lift). But we should care about it and without proper justification don't take too many cells because it increases the computational time.
3) For selecting a y+ value, it should be noted that the error in the drag coefficient should not more than 30% for a normal refined mesh. After getting a proper y+ we should be refined our mesh for getting accurate results.
4) Negative pressure rises in the wake due to reversible highly turbulent flow which will be responsible for the drag force.
5) Flow separation occurs due to the pressure difference on the front and rear surface of the body.
Post Graduate Program in Hybrid Electric Vehicle Design and Analysis
