Week 3 - External flow simulation over an Ahmed body.

Aim: External flow simulation over an Ahmed body.

Objective: The objective of this project is to determine the aerodynamic forces on the Ahmed body such as drag and lift coefficient and to perform the grid independence test.

The expected results will include

1. Velocity and pressure contours. 

2. The drag coefficient plot for a refined case. ( For a velocity of 25m/sec, the drag coefficient should be around 0.33).

3. The vector plot clearly showing the wake region. 

4. Perform the grid independence test and provide the values of drag and lift with each case. 

Abstract

Ahmed body: The Ahmed body was first created by S.R. Ahmed. It is an important benchmark for aerodynamic simulation tools. It will be clearly shown in the sketch below that it has a length of 1.044 meters, the height of 0.288 meters and the width of 0.389 meters. It also has a 50 millimeter cylindrical legs attached to the bottom of the body and the rear surface which has a slant that falls of at 35 degrees.

The flow for the model is turbulent which is based on velocity and body length. For the default mesh size in ANSYS-FLUENT we will use $k-\epsilon$ model and for the later stage $k-\omega$SST model is used.

Importance of Ahmed body

The drag force is an important factor considering fuel consumption. As the drag force increases the fuel consumption also increases which in turn becomes expensive for the car owners. As the burning of fossil fuels becomes an issue, the manufacturers are pressing for fuel-efficient cars. One of the main factors considering the car is fuel-efficient or not is the car's geometry.

Complex shaped cars are very challenging to model and its difficult to quantify the aerodynamic drag computationally. The Ahmed body is a benchmark model widely used in the automotive industry for validating simulation tools. 

Negative pressure in the wake region 

When the air moving over the vehicle is separated at the rear end, it leaves a large low-pressure turbulent region behind the vehicle which is known as the wake. This contributes to the formation of pressure drag which affects the vehicle performance.

When the vehicle is moving at a certain velocity the fluid imparts viscous force to the vehicle as long as it is in the viscous sublayer of the boundary. When the fluid reaches the rear end of the vehicle it gets detached from the surface of the body causing negative pressure in the wake region. The movement of the fluid around the vehicles depends on the geometry of the car and the Reynolds number.

Significance of point of separation

The point of separation will occur when there is a discontinuity in the surface or a region of the negative pressure gradient (a sharp end or rear portion of the car).

When the flow is attached to the body of the vehicle the viscous force will increase which will increase the pressure and a decrease in velocity before the rear end of the vehicle. As soon as the air encounters the sharp turn causing the velocity to decrease resulting in the negative pressure region which is in the wake region. The recirculation region happens beyond the point of separation.

 the rate of change of pressure is large the mixing process will not occur and the boundary layer flow stops.

The above figure shows that at the point of turning the flow gets separated from the boundary layer and there is a region of recirculation after which the flow attaches itself to the boundary layer.

In order to reduce the separation of fluid from the boundary layer, it is advisable to have a smooth edge to reduce the effect of drag on the vehicle.

Modeling approach

Baseline simulation approach using $k-\epsilon$model.

• Ahmed's body is loaded into the Spaceclaim.
• A single enclosure is drawn across Ahmed's body.
• Now the geometry is loaded for meshing.
• A baseline simulation is set up with the default element size of Ansys (413.6 millimeters).
• A named selection is created for the enclosure viz; inlet, outlet, symmetry.
• To create the named selection for the car the enclosure faces are hidden and box select is selected from the meshing toolbar and (car wall) name is given to it.
• Ansys Fluent window is opened and the geometry is loaded.
• Steady-state, the density-based solver is selected.
• Reference values are updated as per the prescribed conditions.
• In the inlet boundary condition, inlet velocity is 25 $\frac{\mathrm{m/}}{\sec }$ and $300$ $K$ temperature are set.
• Drag-coefficient plot and lift-coefficient plot is created by setting the reference as (car walls).
• Hybrid initialization is selected.
• The solution is initialized by hitting $t=0$
• The cut-plane-z is created along Ahmed's body.
• The velocity contour, pressure contour is created along the cut-plane-z.
• The animation video is created for the velocity contour.
• The simulation is executed for 1000 iteration.

Simulation with a finer mesh using $k-\omega$.

• The first simulation run successfully.
• The geometry is loaded into the SpaceClaim.
• The region of local refinement is created along Ahmed's body.
• As the body is perfectly symmetric, the simulation is executed by considering the only half body. This is the best practice where we can save on the number of cells and get the results faster as well. 
• The geometry is loaded for meshing. The multizone method is selected for the outer enclosure to provide hexahedral mesh which provides accurate results in simulation. 
• The element size for the first enclosure will vary as (100mm, 90mm, 80mm), the element size for the second enclosure will vary as (50mm, 45mm, 40mm), the element size of the leg of Ahmed's body will be 5mm, the first layer thickness, inflation layer, and the maximum thickness will be varied accordingly to imitate the experimental results.
• The rest procedure is the same as above, the necessary contour plot and graphs have been uploaded respectively.

Preprocessing and the solver settings

 Case-1:  External flow simulation over Ahmed body by creating a single closure and using default mesh value of ANSYS-FLUENT

Turbulence model: $k-\epsilon$

 Ahmed body model

 

Creating an enclosure across Ahmed body

Creating a plane section on the origin

The three planes are normal to the x,y,z axes respectively.

As the body is perfectly symmetric, we can simulate by considering only half the body. This is the best practice where we can save on the number of cells and get the results faster as well. 

To get half of Ahmed's body, the section mode is selected in SpaceClaim and the front view plain is selected to yield the desired result accordingly.

Once the geometry part is complete, it is loaded in the meshing window to perform the baseline meshing.

Simulating with a default mesh size of Ansys-Fluent

Creating named selection to set up physics and boundary conditions.

Inlet boundary condition (velocity inlet).

Outlet boundary condition (pressure outlet)

Symmetry boundary condition

Creating named selection for car walls

To create the named selection for car walls we need to hide the faces of the enclosure by hitting function key f8.

Performing meshing with default mesh size in ANSYS-FLUENT

The geometry is cut into two halves by using a section plane

Thus the mesh is created inside Ahmed's body which is not good for simulation because the flow outside Ahmed's body is taken into account. It can be fixed by going back to Spaceclaim, one of the copies should be suppressed for physics.

The required geometry is then loaded into the ANSYS-FLUENT window.

Simulation procedure

Setting up of physics

 

Reference values

The frontal area of Ahmed body

Material properties

Viscous model

 

 

 

Hybrid initialization is selected and the solution is initialized by hitting $=$

Creating a cut plane to see the velocity change along Ahmed's body.

Creating contour plot along cut plane z

Results

Residual plot

After 700 iterations, the same repeating trends are observed.

Drag-coefficient plot

Lift-coefficient plot

 

Velocity contour

Pressure contour

 

Drag-coefficient	0.7253
Lift-coefficient	0.5865

 

It can be inferred from the following figure that the results of the base simulation are distorted and do not capture the turbulent flow behind the body perfectly. This simulation captures the wake length, high velocity, low-velocity areas which can be used to further refine the mesh value around the Ahmed body and add a local refinement around.

Case-2 (a)  External flow simulation over Ahmed body with finer mesh in a double enclosure.

Turbulence model: $k-\omega$ .

First refinement

A region of local refinement is added to the Ahmed body.

Share Topology: It is set to share. It is used for sharing the information between the two enclosures and also to make the mesh uniform.

The geometry is loaded into the meshing window.

Meshing

The meshing involves the following steps

Method

Outside the box, the hexahedral mesh is used. The mesh is of the highest quality and gives higher accuracy.

Multizone method:  It is used to create hexahedral meshes wherever possible and for other regions where different mesh types are used it will connect it properly.

 

 

Sizing: It is defined as increasing the number of elements by decreasing the element size. The element size of the second closure is $\mathrm{0.05mm}$

Element size for the first enclosure: $100$$mm$ 

Maximum size for the first enclosure: $100$ 

Element size for the second enclosure:  $50$$\mathrm{mm}$

Element size of pillars of Ahmed body: $5$   

Inflation layer: It is the process of adding layers to the boundary to cover the boundary layer thickness fully.

The first cell height predicted value is $5$

Inflation layer: $5$

Last layer thickness: $15$ 

Y+ value : 345

 

Residual plot

After 1750 iteration the same repeating trends are observed

Drag-coefficient plot

Lift coefficient plot

Velocity contour

Wake region

Pressure contour

Wake region

The vector plot showing the wake region

 

Drag coefficient	0.38361
Lift coefficient	0.30305

Case 2(b) : Second refinement

Turbulence model: $k-\omega$.

The multizone was used for the second area. The number of element size for the outer enclosure is taken as $90$ whereas the element size for the inner closure is taken as $45$. Face sizing was implemented for the pillars of Ahmed's body ( $5mm$).

Inflation layer

First layer thickness: $3$

Number of layers: $10$

Last layer  thickness:  $15.4793$

The value of y+ is around 207.

Residual plot

After 1600 iterations the same repeating trends are observed.

Drag coefficient

Lift coefficient

Velocity contour

Wake region

Pressure contour

 

Wake region

Vector plot showing the wake region

Drag coefficient	0.3512
Lift coefficient	0.2889

 

Case 2(c): Third refinement

Turbulence model: $k-\omega$.

Element size in the first enclosure: $80mm$ 

Element size in the second enclosure: $40mm$

Element size of the bottom leg of Ahmed body: $5mm$

Number of inflation layer: $10$

First layer thickness: $0.15mm$

Last layer thickness: $0.77mm$

Number of elements: $348448$

Y+ : $10$

Residual plot

After 1200 iteration the repeating trends are observed.

Drag coefficient plot

Lift coefficient plot

Wake region

Pressure contour

Wake region

Vector plot near the wake region

 

 

Drag coefficient	0.3498
Lift coefficient	0.2884

 

Demonstration of grid independence test

Comparison of all cases

Steady-state, Turbulent flow, Density-based, Fluid material-Air
Grid Independence Test	Turbulence-model	Number of elements	Lift-Coefficient	Drag-Coefficient
Baseline mesh	$k-\epsilon$	$83781$	$0.5865$	$0.7253$
First refinement	$k-\omega$	$192628$	$0.3030$	$0.3836$
Second refinement	$k-\omega$		$0.2889$	$0.3512$
Third refinement	$k-\omega$	$348448$	$0.2884$	$0.3498$

 

It can be inferred that the imitation of the experimental result is obtained during the second refinement. Thus the grid independence test saves a lot of computational time and convergence can be achieved by using smaller cell sizes for calculation.

Conclusion

• It can be inferred that the grid independence test is performed to know the smaller cell size for convergence.
• Apart from mesh refinement, convergence depends on the Y+ value, inflation layer, it is advisable to use $k-\omega$ as the turbulence value because it calculates the values well near the wall.
• As the setup is refined drag coefficient, lift coefficient decreases.
• Y+ plays an important role in determining the value of drag.
• The negative pressure in the wake region is primarily because there is no flow in that region. This can be further attributed to various factors such as separation and recirculation which is evident from the vector plot near the wake region.
• The point of separation occurs at the rear end of the vehicle, the separation occurs beyond this point where it can be observed that the flow recirculates and attaches it to the boundary layer.