*Video 43.1 Simulation output video*

Some mail arrived during the tutorial posting, based on that feedback I decided to reduce the calculation power needed to simulate the examples files.

You find all the needed Elmer project files into "Vonkarmanforvideo.zip" archive.

All the required files are contained in the archive, "case.ep" and vtu simulation output files have been excluded to minimize archive dimension.

Mesh has been generated into Elmer GUI using the internal mesher. You can appreciate how coarse is the mesh in the following figure. Simulation is contained in a 1,6mx0.6m rectangular surface, the cylinder is set to 0.14m diameter, geometry dimensions of cylinder have been increase to ease simulation convergence. Of course if quantitative solution is needed the mesh should be refined.

*Figure 43.1 Simulation Mesh, elements have 10 mm side length.*

Simulation is set to transient with 1500 steps of 5e-3 seconds; respect to precedent case the simulation is not any more in an open domain but is now limited by two walls. Simulation have not special configuration issues, you can read all the parameters into "case.sif" ASCII file; Elmer default parameters work fine.

Remember to enable simulation output, in this way simulation steps will be saved in a collection of vtu files that set of files will be used later into Paraview for video production.

Simulation time step should be chose by user. There are not broadly accepted rules to select simulation step size. A rigorous approach can be followed but is neither practical nor easy. Many CFD users rely on the Courant condition. That is a sensitive topic, results are variable in function of simulation equations involved. For a Navier-Stokes equation can be acceptable to impose \(C<1\).

To follow this approach let's set \(C=1=2\frac{tV}{u}=2\frac{t}{10e-3}\) then we get a time step \(t=5e-3s\)

Another approach can be those of reuse results from bibliography, in our particular case we need an approximate evaluation of the phenomenon dominant timescale. On purpose we use and approximation of expected vortex sheed frequency. Strouhal approximate number for our simulation is

Approx \(Re= 1700\) hence \(St=0.2\) and \(f=1.4 Hz\)

As a heuristic rule for every simulation, transport equation dominant, we need to have at least two orders of magnitude or more time samples of the phenomenon. Using our parameters that lead to \(t=7e-3s=\frac{1}{100f}\).

At this level of accuracy is sufficient to have a reasonable initial value. To validate the choice of time step is necessary to run different simulations with different time steps values, that topic will not be treated here. In our case if the time step is to big then we will not see vortex at all in the simulation results.

After the simulation run go to Paraview and load vtu case files then load "Solidmodel.stl"

Set the properties of "Solidmodel.stl" as per following values

Translation 0,5 0 -0,2 Scale 0,009 0,009 0,009 orientation 0 0 90

Now you can save the simulation animation

The video of the Paraview procedure is here below.