Week 3 - External flow simulation over an Ahmed body.

Hello this is Shlok here in this we are going to discuss about the Ahmed bodyCimulation in CFD Ansys Fluent So beofre going furthur lets get a few details about Ahmed Body

Ahmed body is a simplified vehicle body used for capturing basic yet charecteristic features seen in objects used in the automobile industry. It is used for testing new CFD solvers or testing one's ability to perform simulations as there are a pleothra of experimental data available about the ahmed body to compare simulation data to.

In this project, I will be performing an analysis on an Ahmed Body in ANSYS using the Fluent solver.

Geometry

This is the sketch drawing:

n this project, the angle of bend ($\phi$

) is 20 degrees. The geometry can be imported from another CAD software or it can be created in ANSYS. I imported a .STEP file for this project in SpaceClaim.

Since this is a complex simulation and the ahmed body is symmetrical along the z axis, the geometry was split into two along the z axis using ANSYS's split tool.

This is the geometry after the spliting:

A wind tunnel has to be created around the ahmed body, there are multiple methods to achieve this, but the easiest is using the enclosure tool in ANSYS to generate the tunnel. The inlet of the wind tunnel is 2 metres from the front of the ahmed body, the outlet is 5 metres from the back of the body. The height and of the enclousure is 1 metre above the ahmed body while the width is 0.5m from the side of the body. The enclousure is checked for Interference and it is repaired as well.

Further enclousures may be created for mesh refinement.

This is the final geometry with three enclousures:

Make sure the original extrusion is suppressed before closing SpaceClaim.

Meshing

The base size is 0.1m. There are multiple mesh controls used to generate the mesh for this geometry, they are:

1. Mesh -> Inflation

This option is used to accurately capture the boundary layers on the surface of the body.

 

2. Method -> Multizone

This option is used to generate mesh in the outer region which is primarily hexahedral

3. Sizing -> Body Sizing

This option is used to refine the larger inner enclousure of the wind tunnel. The increased size gives us more accurate results near the ahmed body. Element size is 0.05m.

4. Sizing -> Face Sizing

This method is used to ensure that the legs of the ahmed body are circular and not polyhedral.

5. Sizing -> Body Sizing

This option is used to refine the smaller inner enclousure of the wind tunnel. The increased size gives us more accurate results near the wake region. Element size is 0.02m.

After all these controls are applied, this is the resultant base mesh:

Zooming in,

These are the mesh metrics:

As seen, most elements have their quality >0.6, hence it can be said that the mesh quality is satisfactory.

Setup

Boundaries

inlet - inlet

outlet - pressure outlet

wall-car - wall (no-slip)

back, top and bottom - symmetry

symmetry zplane - symmetry

A separate boundary was created for the symmetry plane to make post processing easier.

Reference Values

The most important values here are: Area, Density, Length and Velocity.

The area was calculated using ANSYS Fluent, Results -> Reports -> Projected Areas:

This is the cross sectional area for the half ahmed body

Materials

The existing materials (air) properties were used and were left unchanged.

We know, Reynold's Number

$Re=\frac{\rho \cdot u\cdot D}{\mu }$

 

where, $\rho$

is density ($kg/m^3$), $u$ is inlet freestream velocity ($m/s$), $D$ is charesteristic length of the ahmed body ($m$) and $\mu$ is kinematic viscosity $kg/(m.s)$

.

In this case, $\mu =1.78\cdot {10}^{-5}kg/(m.s),D=1m,u=25m/s\text{and}\rho =1.225kg/m^3$

 

$Re=\frac{1.225\cdot 25\cdot 1}{1.78\cdot {10}^{-5}}$

 

$\Rightarrow Re=1711467$

or $Re=1.7\cdot {10}^6$

 

Viscous

k-omega SST was used for all simulations for this project due to its excellence in solving external flows and wake regions.

Reports

Two reports were created.

1. Lift Coefficient of wall-car

2. Drag Coefficient of wall-car

 

Solution - Methods

Simulation of the base setup

The simulation ran for 100 iterations and the results are below:

Residuals

Drag Coefficient

The final value of drag coefficient is 0.29310978, which is in agreement with experimental and simulation data.

This data is from Moghimi et al. [1]

 

 

Lift Coefficient

The final value of lift coefficient is 0.24969179, the discrepancy is due to variation in reynold's number and low mesh resolution near some regions of the ahmed body.

Contours, Plots and Vectors

Note: All plots, contours and vectors were obtained from the finer mesh, due to its higher solution clarity.

1. Velocity contours

These were taken in CFD - Post.

Zooming in,

Zooming in further,

The wake is clearly visible.

2. Pressure Contour

These were taken in CFD - Post.

Zooming in,

There is a high pressure region at the front of the body due to how flowing air is acculumated at the front.

The pressure is negative in some regions, this is not an error in the simulation but rather how ANSYS and Fluent functions. The "pressure" displayed in ANSYS is actually gauge pressure, the gauge pressure is 0 when the total pressure is the atmospheric pressure. In this case, the "pressure" being negative is merely the pressure dropping below atmospheric in some regions.

3. Vector Plot

These were taken in CFD - Post. The background contour is the velocity contour.

Zooming in,

Zooming in further near the wake region,

Switching the type of arrow to see the lines more clearly,

Two distinct regions can be spotted behind the ahmed body with two vortices (seen from this view) or recirculating regions behind the ahmed body.

4. Animation

This was taken in Fluent.

Initially the wake regions has some disturbances but they are eventually ironed out the solution reaches steady state.

Grid Dependence Test

A Grid Dependence Test is used to ascertain whether the final values of the solution are dependent on the mesh or not. This is an important test to ensure the simulation results are correct.

In this test, the test will involve 2 different simulations - one where the mesh becomes more finer and other where the mesh becomes more coarser.

Coarser Mesh

For this test, the smaller inner enclousure is removed (point 5 under Meshing) and the simulation is ran for the same parameters.

These are mesh statistics:

The values of drag and lift coefficient are below:

Lift Coefficient: 0.22592755

Drag Coefficient: 0.35537949

Finer Mesh

For this test, a spherical region centered at x=1.2, y=0.1 and z=0 is created and the mesh size in this region is decreased.

It was added going to Mesh -> Controls -> Sizing

 

This is the region seen in ANSYS:

The details of the regions are below:

This is the resultant mesh seen in ANSYS:

These are mesh statistics:

Other simulation parameters were kept the same as the baseline simulation and the simulation was ran:

The values of drag and lift coefficient are below:

Lift Coefficient: 0.22918563

Drag Coefficient: 0.28130557

Summary of Grid Dependence Test

 

	Lift Coefficient	Drag Coefficient	Nodes	Elements
Coarser Mesh	0.22592755	0.35537949	37033	104163
Base Mesh	0.24969179	0.29310978	83137	309948
Finer Mesh	0.22918563	0.28130557	110583	455282

 

Drag coeffcient decreases as number of elements increase, this claim is substantiated by the work of Jie Tian et al [2]

 

 

The important takeaway is that drag coeffcient does not vary significantly when the mesh is made more finer. While the drag coefficient does vary when the mesh is made more coarse. This means that the grid dependence test has passed.

 

Conclusion and Observations

 

1. The simulation of the Ahmed Body runs well and is in some agreement with experimental and empirical data on the body.
2. There are regions behind the body where wakes are formed, circling regions of low velocity which induce a considerable amount of velocity drag on the body. This is seen in the simulation and experimental data by Gilliéron et al.[3]