Ahmed Body Challenge

Introduction:

In this project, we will be conducting a flow test on the Ahmed body by placing it inside a wind tunnel to the motion of the air over it at 25m/s. This will be done to analyze the drag, lift, and pressure experienced by the body. An Ahmed body is a representation of a car model that is used to study the most basic and simple aerodynamics effect on the designed model. The shape of an Ahmed body is designed to highlight the aerodynamic features of the model. It is also used to check if a self-made CFD code is working correctly.

Solving and Modelling Approach:

The obtained solid part is imported to SpaceClaim and we prepare the model by adding an enclosure around the Ahmed body. We then use a basic mesh and conduct a baseline simulation for the edited geometry using the Reynolds wall stress turbulence model. After executing the simulation, we check the contours and results. The obtained contours will not be that smooth as we have used the basic mesh, as this is a baseline simulation. Now we duplicate the fluent project and go to mesh geometry again. Here we create another enclosure that concentrates on the region around the AHMED body. Then proceed to mesh to create a Hexa mesh for the bigger enclosure and a more refined mesh for the smaller enclosure. Along with that we also add an inflation layer on the car surface using the first layer thickness method. The first layer thickness is calculated according to the appropriate wall Yplis value. Then we use the same setup to execute the simulation and obtain the required results.

Pre-Processing: The following is the preprocessing for the refined case:

Open Ansys fluent and from the different analysis systems in the toolbox drag fluid flow (Fluent) to the project schematic window.

Geometry:

• Right-click on geometry > select open with space claim.
• Now drag the solid part to the space claim window and it gets uploaded.
• Now we need to remove the small wheels in the. Go to design > select split body > click on the bottom surface of the Ahmed body > click the tick mark. From the structure window, delete the parts that have been split.
• Then go to prepare > select enclosure > select the Ahmed body > give the appropriate dimensions > and click the tick mark. This will create a wind tunnel structure.
• To create a smaller enclosure to concentrate on the region around the Ahmed, use the same steps above but the dimensions will be relatively very smaller than the wind tunnel, depending on the length of the wake region.
• Go to prepare > select the interference and click the tick mark to remove the interference.
• Now in the structure select the main structure name and set share topology as share.
• Finally, right-click on the Ahmed body in the structure panel and select suppress for physics.

Mesh:

• Let us start with creating named selection. Select face selection > then select a face and click N and name the selections. Four named selections must be created, namely, inlet, outlet, car wall, and symmetry wall (wind tunnel wall)
• In the mesh > set element size as 100mm > in inflation option used named selections (CAR wall) and the method used for adding inflation layer will be first layer thickness. The first layer height will be 0.43 as the desired yplus in 30.

• As we want Hexa to mesh on the bigger enclosure we add a mesh method. Right-click on mesh > select insert > click on method > then scoping method use geometry selection and select the body > then in method select multizone and mapped mesh type select Hexa.

• Right click on mesh > insert > sizing > scoping method : geometry selection > in geometry : select the smaller enclosure > the mesh size will be 50mm, 40mm and 33mm for three different cases to check for mesh dependency.

• Now click on update > so that the mesh is uploaded in fluent setup.

Setup:

• First, we perform a mesh check. To do so, in domain > select check > and the mesh check is performed.
• Go to general > the solver type is pressure based > and velocity formulation is Absolute > with a steady-state analysis.
• In the turbulence model, we will be using the Reynolds stress (7eqn) model with energy off.

• Now, in the materials, we check for its properties and see if its air.
• In boundary conditions, we set the inlet as a velocity inlet and assign the velocity of 25m/s. And for the outlet, it will be a pressure outlet, with 0 gauge pressure.

• Before we set the reference values we go to reports > select projected areas > then select the direction as x-axis > select the car wall > compute. Note the area. In the reference values compute from inlet > set the area acquired from the projected areas > and length as 1.044m.
• We move on to the method and set the pressure-velocity coupling scheme as simple and second-order pressure and Reynolds stresses discretization.

Solutions:

• Go-to solutions > in reports > select definitions > select force reports > create two reports .ie. for drag and lift coefficients > for both check on report pot and report file.
• In initialization > use hybrid initialization method and initialize.
• Go to results > create > select plane > the method of plane selection is point and normal > the point is 0,0,0 and normal is iZ=0.
• In results > go-to graphics, > select contours > and make a velocity contour on the created plane.
• In solutions > under activities > create > scene animations > select the velocity contour > plot every 10 iterations.
• Set the number of iterations as 500 and click on calculate.

Results and Post Processing

• Let us begin by creating a slicing XY plane. Go to insert > select plane > and give in the details as Z=0.0 and plane as XY plane.
• Now right click in the results outline > select insert > select contours > select the location as created xy plane > select the required variable : pressure and velocity > click apply.
• Now right click in the results outline > select insert > select vector > select the location as created xy plane > select the variable : velocity > click apply.
• We need to create another pressure contour on the car wall.

The following results were obtained for three different element sizes in the body sizing:

Element size = 50mm, No of elements : 149k

Element size = 40mm, No of elements : 272k

Element size = 33mm, No of elements : 464k

Mesh Dependency Test:

No. of elements	Element size (mm)	Coefficient of drag	Lift Force	Drag Force
149895	50	0.384	7.507	17.822
272642	40	0.363	9.294	15.757
465401	33	0.342	9.660	14.680

Conclusion:

The graphical plots and contours for all three types of mesh are almost the same. Small differences are noticed in the appearance of the plots and contours but that is due to the element quality in the. If we notice the velocity contour then we can notice that the velocity around the wake region is high and low at the tail of the Ahmed body. If we connect this observation with the velocity vector plot then we notice that at the wake region the velocity vectors are large which is obvious due to the obstruction offered by the Ahmed body and at the tail of the body there is a circulating flow which is the reason for its low velocity. Whereas, for the pressure contours at the car wall and XY plane, high pressures are observed in the front of the body, and in the wake region we observe negative pressure. Now practically, negative pressure scenarios do not exist. But when we observe analytically, here the negative pressure value makes complete sense because the wake region is the region of low pressure and since the fluid flow model used here is incompressible the pressure gradient enters the Navier stokes equation resulting in the pressure difference that drives the flow. As guage pressure is set as 0Pa to create the pressure difference, the pressure at the wake zone becomes negative, producing higher velocity fluid flow in the region.

When an object moves in a fluid the fluid sticks on the surface of the body and creates a boundary layer over it. Now for certain bodies and type of motion, there is a point on the body where the fluid detaches from its surface, thus breaking the boundary layer, this point at which the fluid detaches from the surface is called the point of separation. This flow separation is caused due to adverse pressure gradient which can be observed at the tail of the Ahmed body.