This step-by-step exercise aims at providing the user with a hands-on experience using the SimScale Platform for the application of football aerodynamics. The user is enabled to explore the end-to-end (geometry upload to post-processing) approach of the SimScale platform.
In the world of football, it is a known fact that the altitude has a negative impact on the health of players. So much so, that it led to the High Altitude Controversy, where FIFA imposed a ban on countries with stadiums at high altitudes (like Bolivia, Colombia and Ecuador) from hosting the world cup. FIFA’s motive behind this ban was based on the argument that the players from these high altitude countries would have an “unfair advantage”.
In this exercise, we intend to validate/ falsify FIFA’s claim by analyzing the impact of altitude on the aerodynamic forces on a football. The two major forces to be analysed would be the drag, which would impact the velocity of a football, and the side force, which would influence the swerve or swing of a football traversing in air. The aerodynamic forces acting on a football can be split into two parts, pressure forces and viscous forces. Computational Fluid Dynamics is a powerful tool which aids in the quantification of the forces acting on the football.
This example follows the setup for the stadium Estadio Hernando Siles, which stands at an altitude of 3,637 metres (11,932 feet) above sea level. The primary factor which would vary with altitude is the air density. For our example stadium, the air density is 0.85 kg/m3.
For your simulation you are free to select any one stadium from this list:
Your task is to calculate the aerodynamic forces for the football at your choice high altitude stadium to the aerodynamic forces at the sea level (Air Density= 1.226 kg/m3). Following this, a percentage change in the aerodynamic forces is to be reported.
This project can be used as a starting point for your simulation.
Once the geometry has been imported into the platform, we proceed to the mesh generation. In the navigator pane, please select Meshes button and click on New.
The platform now provides you with the option to select the geometry you would like to work with. This option comes in handy when a parametric study with geometric variations is needed. In this homework exercise, we will work with a single geometry. Please assign an appropriate name for your mesh and select the geometry, football.
We will be using the Hex-dominant parametric (only CFD) option for this homework. This approach provides a good user-control over the mesh.
Please enter the number of cells in the x-, y- and z- directions as per the image below. This is done to have a uniform mesh in all directions.
The Background Mesh Box is the domain on which the calculations will be made. It is assigned such that it does not interfere with the physics of the simulation. For example, it is made long enough in the downstream (+x) direction to minimize the influence of wake vortices on the outflow.
Min. Point (x )= -2
Min. Point (y) = -2
Min. Point (z) = -2
Max. Point (x) = 6
Max. Point (y) = 2
Max. Point (z) = 2
The introduction of a Background Mesh Box splits the domain into two parts; inside the football and outside the football. The material point decides the part of domain on which the calculations will be made. This tutorial aims at simulating the external flow around the football, hence the Material point can be placed anywhere outside the football (but within the bounds of the Background Mesh Box). We select our Material Point at the location: (0,1,0).
To create a new geometry primitive, go to Geometry Primitives and please click on New. Then select the option, Cylinder.
The bounds and the radius of the cylinder may then be assigned.
Mesh refinements are crucial to the convergence and accuracy of any CFD simulation. As a next step, we move onto mesh refinements by selecting Mesh Refinements in the Navigation pane and followed by clicking on New.
Region Refinement provides the option to refine your mesh in a pre-specified region. This region may be a solid body or a geometry primitive. We had previously defined a cylinder, which will now serve the purpose of region refinement. Please make sure that the Region refinement mode is set to inside. Select Cylinder from the Geometry Primitives as the region to be refined.
Please Note: After creating a new mesh refinement, select the Type and click on Save.
A Surface Refinement can be created for faces or solids. In both cases, the mesh will be refined near the surface of the selected object. Please implement a surface refinement as shown in the below image.
The Inflate Boundary Layer option enables you to define prism layers on the selected faces in order to efficiently capture the boundary layer. The Inflate Boundary Layer is especially important in this homework assignment since we have strong re-circulation and vortices in the wake of the football, which are consequences of boundary layer separations. The y+ values are limited by this refinement. Please add a new refinement and select the Type as Inflate Boundary Layer. Next, click on Save.
Number of layers = 5
Expansion ratio for layer cell thickness = 1.2
Thickness of the final layer = 0.3
Minimum overall layer thickness = 0.001
Feature Refinement allows you to create a finer mesh close to edges. It extracts the edges from the surfaces and refines the mesh as defined in the “Feature Refinement Levels” panel.
You are now ready to begin the mesh generation. Please select Operation 1 from the Navigation pane and click on Start.
The mesh can now be visualized on the platform:
The more enthusiastic users can also qualitatively and quantitatively analyse the mesh in more detail with mesh clips and the meshing log, respectively.
The mesh now been setup and satisfactorily analysed. The next step in your workflow is to move into the Simulation Designer. To create a new simulation, please click on New.
Please assign a name to your simulation and click Create.
Based on the fact that the maximum speeds attained by the bicylist are well below Mach 0.3 (a thumb-rule for compressibility), Incompressible can be selected as the Analysis Type.
Proceeding to Domain selection, you can select the mesh on which you want the simulation to be performed. This is particularly productive when you would like to work with different meshes.
Now, we are about to assign our main control parameter, the air density, which varies with altitude. A pre-defined material can be imported from the material library by clicking on Import from Material Library and selecting Air. The density of air is then entered according to the altitude. In this example, we will be working with a density of 0.85 kg/m3. Please select the volumetric region on which the material needs to be assigned, under the tab Topological Mapping.
The initial conditions are assigned to the whole domain at the start of a simulation. During a simulation, the solver tries to converge the solution fields after taking these initial condition values as a starting point. Therefore, it is important to assign best guesses or analytical solutions as initial conditions when possible.
We assume a low turbulence intensity of air (I=5%=0.05) for our simulation. The values of Turbulence Kinetic Energy (K) and Omega (ω) can be calculated (Formulae)*:
Turbulence Kinetic Energy (K) = 1.815
Omega (ω) = 13.71
Please feed in the values of K and omega into their respective positions in the Navigation Pane.
The overview of the physics setup is as follows:
You may now proceed to setup the physics of the simulation. To create a new boundary condition, please select Boundary Conditions in the Navigation plane and click on New.
The inlet boundary condition can be created as follows:
Please create a New Boundary Condition. The outlet boundary condition can be created as follows:
With this boundary condition, we intend to replicate the physics of the football rotation about its axis. A no-slip Rotating wall can be used to fulfill this purpose. Please create a New Boundary Condition. The football boundary condition can be created as follows:
The freestream is modeled as Slip Walls with Zero gradient. Slip walls eliminate the formation of non-physical boundary layers, which would develop if No slip walls were used.
Please create a New Boundary Condition. The freestream boundary condition can be created as follows:
The Numerics on the platform have been optimized and do not need to be changed for this simulation. You could analyse them by selecting Numerics in the Navigation pane :
The Simulation Control provides user-control over the simulation. You can increase the Number of computing cores to 32 and Maximum runtime to 8000s.
Please note: The End time value represents the computation time and Maximum runtime represents the wall clock time (real time!)
For the purpose of accurate verification or validation of the results, additional solution fields need to be post-processed. The platform provides a Result Control panel to serve this purpose. The additional Result Control Items (solution fields) can be setup and exported as follows:
You are now almost ready to start your simulation run. Please navigate to Simulation Runs in the Navigation pane and Check the simulation setup. If there is no error, please create a new run by clicking on New.
Please feed-in the name of your simulation.
Please click on Start to begin your simulation run.
To create the proceeding simulations, you can simply duplicate the simulation setup by right clicking on the simulation you would like to duplicate and press Duplicate.
Please feed-in the name of your new simulation and click on Save.
Please navigate to the Post-Processor in the workflow and select Solution fields.
To add a duplicate of the result, right click on Solution fields and select Load results to viewer. Please ensure that the Mesh Region > internalMesh and all Cell arrays have been selected.
In the second Run 1, select the Mesh Regions: solid_0_Part1 and solid_0_Part1 and the Cell Arrays: wallShearStress and total§_coeff
Please make the first Run 1 invisible by clicking on the eye-symbol. This first Run 1 is the simulation run on which we will be performing the post-processing.
The convergence can be visualized from by selecting the Convergence plot in the Navigation pane.
We now intend to visualize the pressure build up on the football on account of the rotational velocity about its axis. This can be done with the Contour filter. An iso-surface at reasonably low pressure values may be plotted to represent the negative pressure build up due to the rotation.
To create a new filter, select the first Run 1 and click on Add filter.
Then, select Contour as the filter.
The iso-surface contours may be setup as follows:
Slices provide planar representations of Solution fields. We use the slices to analyse the total pressure field around the football and in the wake. Total pressure values represent the energy in the flow and is an ideal field to be analysed in the wake.
To create a new filter, select the first Run 1 and click on Add filter.
Select Slice as the filter.
The Slice may be setup as follows:
Please enable the Colour bar and adjust the Custom data range to suitable values. For this case, a range of [-200Pa,200Pa] has been selected.
The position of the plane can be varied with the tabs Origin and Normal.
Slice in the XY plane:
Streamlines of velocity provide a good qualitative representation of the flow dynamics in the wake region. The streamlines are represented in the Post-processor by a Stream tracer.
To add a Stream tracer, please add a New Filter and select Stream tracer
The Stream tracer may be setup as follows:
If you now make the Contour1 created earlier visible, you can qualitatively analyse the effect of the pressure build up on the velocity.
The aerodynamic forces viz. pressure and viscous forces can be directly visualized from the Force Plot. The unwanted forces can be deselected by simply clicking on them.
As a general best practice for steady state flow problems, it is advisable to average the flow properties, such as Forces, over the final timesteps.
The drag and the side forces may be calculated from the averaged value of the forces as follows:
Drag = Pressure force x + Viscous force x
Side Force = Pressure force z + Viscous force z
The user is also free to analyse the results locally by downloading it to their system. An opensource post-processor, Paraview, can be downloaded here.
Thank you very much for your attention and Happy Simulating.