Flow over Ahmed's Body
The Ahmed body represents a simplified, ground vehicle geometry of a bluff body type. Its shape is simple enough to allow for accurate flow simulation but retains some important practical features relevant to automobile bodies. This model describes how to calculate the turbulent flow field around a simple car-like geometry using the different Turbulent Flow models.
The Ahmed body is a generic car body (a simplified vehicle model). The airflow around the Ahmed body captures the essential flow features around an automobile and was first defined and characterized in the experimental work of S. R. Ahmed in 1984. 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.
In this project, external flow analysis on Ahmed Body in STAR-CCM+ is simulated and results are validated by comparing the velocity profiles at different locations with the experimental results done originally. This is done for two geometries with two different slant angles( 25 degrees and 35 degrees) and for two different turbulent models. Also, to calculate the drag coefficient and lift coefficient for all the configurations.
Objective:
- Create the Ahmed Body slant for both 250 and 350
- Run Steady-state implicit coupled flow simulation
- Use the turbulence models K-OmegsSST and k-epsilon
- Validate the velocity profile along the Ahmed body at different points with the experimental data.
- Calculate the cd and cl using the different turbulence.
1. 3D CAD
Ahmed body dimensions
- The first step is to create the geometry of Ahmed's body in the STAR-CCM+ 3D CAD modeler.
- The coordinates of the Ahmed body are identical to the experimental data.
- Ahmed's body end is at x=0. The front end of the Ahmed body is at -1442 mm in the x-direction.
- The body is symmetrical along the y-axis.
- The simulation procedure is the same for all four cases up to meshing. To change the slant angle we need to change the slant dimension in the sketch.
Sketch :
A 2D sketch is drawn as per the given dimensions and it is extruded for the given width. The sketch is as follows.
now the above 3D CAD body is taken for simulation by creating a new geometry part and the Ahmed body appears in a part list. Now wind tunnel is created around the body.
Wind tunnel dimensions:
Now we have to create a wind tunnel for external flow analysis. While creating a wind tunnel, we will split the road into two parts, we will use the front part of the road as a slip-wall function, and the rest of the road will be taken as no slip-wall function to achieve proper boundary layer thickness. This can be achieved by creating two different blocks and then uniting them. The wind tunnel is ready just name the surfaces as required.
The dimension of the wind tunnel is 1.5m in height, 5m at the front to the end of Ahmed's body, and the back is 3m.
Subtract operation
After creating Ahmed's body and the wind tunnel, we will take a CAD to subtract between Ahmed's body and the wind tunnel to get a nice and clean region for wind flow, without any overlapping surfaces between Ahmed's body legs and the wind tunnel.
Surface repair:
Once the complete geometry is created, new parts are created from them and some boolean manipulations are done to extract the required volume out of the geometry. Then the part is checked for surface issues and if any, it should be repaired.
Boundary Conditions
- Now we have to assign the subtracted part to the region and select the option to create a boundary for each part surface and create one region for each part.
- After assigning parts to regions we will define the boundary types.
- Inlet: velocity inlet.
- Outlet: pressure outlet.
- Environment (side & top surfaces): symmetry plane.
- Road: wall
Meshing
Default controls
- Base size: 30 mm.
- Number of prism layers: 5.
- Prism layer stretching: 1.5
- Prism layer total thickness: 0.0066 m. (33.33% of base size)
Custom controls
- Windtunnel walls = 800% of base Size
- Windtunnel Inlet & Outlet = 400 % of the base size
- Windtunnel base(road) = 200% of base size
Volumetric control is defined on a small block. This block is created to generate a finer mesh near Ahmed's body and to define the wake generated by Ahmed body.
- Volumetric control: Customize isotropic size - Enabled.
- Custome size = 100 % relative to base.
Y+ value:
Y plus is an analytical profile covering the viscous sublayer and the buffer layer. In fact, the boundary layer thickness composed of three regions when going far from the wall, started with viscous sublayer, the buffer layer, and the turbulent layer. Y plus is designed to cover only the first two parts and it is expected to be started from the very beginning of the turbulent layer.
For this simulation, it is essential to place the first cell the wall in log-law layer(30 < y+ < 500). So for y+ = 55, the first cell thickness has to be 5 mm for the given velocity, density and viscocity. So the prism layers are generated in a way that the first cell thickness is 5 mm.
Generally when you building grid for RANS model of k-epsilon the target value of y+ should be between 30 and 300. The y+ depends on friction velocity u*=sqrt(Tw/rho) where Tw is wall shear stress, element distance to the nearest wall and local kinematic viscosity.
If your minimum y+ are lower than 30 your grid is to fine in those areas for wall function and you can make it more coarse. On the other hand if your y+ are larger than 300 then you should refine your grid in those areas to fulfill the wall function approach. The average value which openfoam calculates is then simple average of y+ value over whole domain or particular parts.
omega family of turbulence models come with an automatic wall treatment and the omega equation has an elliptic character making this family more suitable for near wall modelling than epsilon based. The mesh requirement for Low Re investigation are the same: boundary condition by yplus not larger than 1 (ideally) or at least in the laminar layer. The BL should be resolved with at least 10 to 15 layers. Bear in mind the relationship between yplus criteria and Pr number.
Physics setup
The Ahmed body is simulated with two different turbulent model i.e. k-e and k-w SST for two different slant angle of 25 deg and 35 deg. Below shows the relevent simulation model required.
For case I & III For Case II & IV
9 probes have been created at different locations on the x-axis to export normalized velocity data.
Case I - Ahmed Body slant 250 for K-e turbulent model
Residuals
Surface Average Inlet Pressure
Surface Average Outlet Velocity
Drag Coefficient
Lift Coefficient
Velocity Contours
Pressure Contours
Streamlines
- From the residual plot, surface average inlet pressure, and surface average outlet velocity we can see that the solution has converged and reached a steady-state condition.
- Coefficient of Drag: 0.35370
- Coefficient of Lift: 0.10562
- From the velocity contour, we can see that the velocity is high at the top region of the Ahmed body at the front of the body. Velocity is low at the back of Ahmed's body at the wake area. Maximum velocity: 61.77 m/s.
- In the pressure contour, we can see that pressure is high at the front face of Ahmed's body due to air impact on the frontal surface of Ahmed's body. The pressure is low at the curved region of the Ahmed body where the velocity is high. Maximum pressure:1003.9 Pa
Comparing Simulation Velocity data with Experimental at y = 0
With the help of probes, the velocity data is compared at the 9 different locations of the region around the ahe Ahmed's body which covers the slant and the wake region of Ahmed's body. Thus for case I - Ahmed's Body slant 250 for the K-e turbulent model, the first four probes' data matches well with the experimental data as it covers the slant of Ahmed's body. The other probes are situated at the wake region formed by Ahmed's body and if we see some velocity data show a higher percentage error.
In all of the 9, we can see that the fast few velocities values and last velocities values match well with the experimental data but the middle values are showing higher % error so this is the effect of selecting a k-e model for defining turbulence.
Case II - Ahmed Body slant 250 for K-w turbulent model
Residuals
Surface Average Inlet Pressure
Surface Average Outlet Velocity
Drag Coefficient
Lift Coefficient
Velocity Contours
Pressure Contours
Streamlines
- From the residual plot, surface average inlet pressure, and surface average outlet velocity we can see that the solution has converged and reached a steady-state condition.
- Coefficient of Drag: 0.3386
- Coefficient of Lift: 0.10234
- From the drag and lift values we can say that for the same geometry drag changes from 0.35 to 0.33 this is the effect of selecting the k-w turbulence model.
- From the velocity contour, we can see that the velocity is high at the top region of the Ahmed body at the front of the body. Velocity is low at the back of Ahmed's body at the wake area. Maximum velocity: 61.68 m/s.
- In the pressure contour, we can see that pressure is high at the front face of Ahmed's body due to air impact on the frontal surface of Ahmed's body. The pressure is low at the curved region of the Ahmed body where the velocity is high. Maximum pressure:984.84 Pa
Comparing Simulation Velocity data with Experimental at y = 0
From all of the above comparison graphs, we can see that most of the velocity profile of the simulation nearly matches well with the experimental data so from this we can say that the k-w model gives better results than the k-e model of turbulence.
Case III - Ahmed Body slant 350 for K-e turbulent model
Residuals
Surface Average Inlet Pressure
Surface Average Outlet Velocity
Drag Coefficient
Lift Coefficient
Velocity Contours
Pressure Contours
Streamlines
- From the residual plot, surface average inlet pressure, and surface average outlet velocity we can see that the solution has converged and reached a steady-state condition.
- Coefficient of Drag: 0.35491 slightly greater than case I
- Coefficient of Lift: 0.077090 much lesser than case I
- From the velocity contour, we can see that the velocity is high at the top region of the Ahmed body at the front of the body. Velocity is low at the back of Ahmed's body at the wake area. Maximum velocity: 61.73 m/s.
- In the pressure contour, we can see that pressure is high at the front face of Ahmed's body due to air impact on the frontal surface of Ahmed's body. The pressure is low at the curved region of the Ahmed body where the velocity is high. Maximum pressure:1030.7 Pa
Comparing Simulation Velocity data with Experimental at y = 0
From the graphs, we can see that for all the 9 probes or location data simulation velocity data exactly matches for a few starting and for a few ending values. The middle-velocity values show a higher %error for matching with experimental data. The reason is selecting the k-e model.
Case IV - Ahmed Body slant 350 for K-w turbulent model
Residuals
Surface Average Inlet Pressure
Surface Average Outlet Velocity
Drag Coefficient
Lift Coefficient
Velocity Contours
Pressure Contours
Streamlines
Recirculation seen at the end of the body and the vortex is seems detached.
- From the residual plot, surface average inlet pressure, and surface average outlet velocity we can see that the solution has converged and reached a steady-state condition.
- Coefficient of Drag: 0.32159
- Coefficient of Lift: 0.030651
- From the velocity contour, we can see that the velocity is high at the top region of the Ahmed body at the front of the body. Velocity is low at the back of Ahmed's body at the wake area. Maximum velocity: 61.6 m/s.
- In the pressure contour, we can see that pressure is high at the front face of Ahmed's body due to air impact on the frontal surface of Ahmed's body. The pressure is low at the curved region of the Ahmed body where the velocity is high. Maximum pressure:1013.6 Pa
Comparing Simulation Velocity data with Experimental at y = 0
The normalized velocity comparison graphs for case IV show that the k-w model is better for describing the flow profile. The experimental and simulation normalized velocities and flow profiles are in close proximity to each other
Conclusions
The SST k-omega turbulence model is a two-equation eddy-viscosity model that is used for many aerodynamic applications. It is a hybrid model combining the Wilcox k-omega and the k-epsilon models. A blending function, F1, activates the Wilcox model near the wall and the k-epsilon model in the free stream. The k-omega model is well suited for simulating flow in the viscous sub-layer and the k-epsilon model is ideal for predicting flow behavior in regions away from the wall. As we are comparing normalized velocity data of simulation with experimental data, the results obtained out of the k-w SST model will be more accurate.
The slope angle of the slanted surface has significant effects on the characteristics of the wake flow. Like the vorticity contours on the slanted surface with a slant angle = 25 deg is nearly attached to the surface, those which are on the slanted surfaces with a slant angle = of 35 deg are more detached. The vortex formed by slant angle = 35 deg is bigger than slant angle = 25 deg.
For alpha = 35
For alpha = 25
From all of the drag coefficient data, we can say that due to the flow separation, the drag generated at slant angle a= 35 deg is less than a=25 deg.
The velocity profile on the slant shows a straight line as it is taken on the surface of the body and as we move toward positive distance probes we can see a doveloped flow.
The recirculation region was captured more accurately by the K-Omega SST model in both the slant angles. This is again due to the fact, that this algorithm can predict flow separation better than the other 2 equation models.
