interFoam solver for free surface flow past a circular cylinder
 

Hi All Foamers,

Thanks for taking time to read on.

As the title indicated, I am simulating the flow around a surface piercing cylinder using interFoam (1.7.1). The Re number and the Froude number based on cylinder diameter D is 27000 and 0.8 (Fr = U/sqrt(g*D). The mesh is generated with Gmsh, for all simulations y+ was kept below 1, and mesh sensitivity study was completed. The mesh looks like as attached (stretching in z-direction ),
http://www.cfd-online.com/home/tfuwa/Desktop/mesh.png
The simulations are proceeded with 4-diameters depth of water and 2-diameter depth of air. The LESimulation with oneEqEddy turbulence model is chosen. The results are encouraging but not good enough as simulated in published papers. The lift and drag coefficients are shown below. While the drag is around 1.05 (close to numerical work by others), the lift does not vibrate enough, leading to a Cl rms below 0.1 (should around 0.2). Also, the Strouhal number is away from right.

The average surface elevation is beautiful :), but has a space to be improved compared to experimental results, as illustrated below.

In order to improve and get the force coefficient right, I have tried different turbulence models (LES dynOneEqEddy, Standard k-e), and different convection schemes (limitedLinear, filteredLinear, SFCD, upwind and others), but without success.

Can you please enlighten me on how to improve the simulations and point out where I am wrong?

I attached the fvSchemes, fvSolution and LES coefficients files below, but if more information is needed, do not hesitate to ask for.

Cheers,
Albert

Another two attachment.

Albert

How does your mesh compare to the meshes of the results that you are referring to? I can imagine that the high aspect ratio cells at your inlet will be a problem here. Also, what is the inflow condition in your simulation?

Dear Bernhard,

Thanks a lot for your reply.

The computational domain in my simulation 45D*20D*6D (x*y*z), and I used 60 grids in z-direction. I have two references at hand, and they used 33 grids for 5D (Journal of Fluids Engineering, 2002, Vol. 124, 91-101) and 128 grids for 6D (Journal of Fluids and Structures 27, 2011, 1–22) in z-direction, respectively. And they got similar results. My cell aspect ratio follow between them, but I will try fine mesh in z-direction later on.

The initial conditions are as follows,

inlet
{
U fixed value; p_rgh buoyantPressure; nuSgs zeroGradient; k fixed value 2.354e-2; alpha1 fixed;
}

atmosphere
{
U pressureInletOutletVelocity; p_rgh zeroGradient; nuSgs zeroGradient; k inletOutlet; alpha1 inletOutlet;
}

outlet
{
U zeroGradient; p_rgh totalPressure; nuSgs zeroGradient; k inletOutlet; alpha1 zeroGradient;
}

cylinder
{
U fixedValue uniform (0 0 0); p_rgh zeroGradient; nuSgs zeroGradient; k fixedValue; alpha1 zeroGradient;
}

bottom and sides
{
type symmetryPlane;
}

I appreciate your comments and would like to receive more to get the problem solved.

Cheers,
Albert

With a fixedValue BC for U at the inlet, you will not have velocity fluctuations on the scales larger than the grid scale (since you impose a uniform distribution). In other words, you start with u'_rms = 0, which is not true of course.
Please consult http://www.cfd-online.com/Forums/ope...et-bc-les.html for more information. Maybe you want to use the turbulentInlet boundary condition to impose some random fluctuations on the inflow.

TurbulentInlet, sure, has the potential to improve the result
 

Hi Bernhard,

Thanks for your quick reply. TurbulentInlet, sure, has the potential to improve the result, but it may not be the only reason here. Previously, I simulated one phase flow around a cylinder using pisoFoam combined LES solver with the same inlet and other above mentioned fv conditions, which I should post earlier (sorry for that). That simulation gave a much better prediction on force coefficients, illustrated bellow. This result make me believe there must be other reasons.

Cheers,
Albert

exaggerated free surface elevation - interfoam
 

Hi...

I'm doing the open channel flow simulation with interFoam solver and I got a exaggerated elevation upstream the cylinder http://d.pr/i/Ya1d (http://d.pr/i/Ya1d).



I dont't know why... I use these BC to the atmosphere:

alpha 1
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

U:
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

p_rgh:
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
value uniform 0;
}
k
{
type inletOutlet;
inletValue uniform 0.001;
value uniform 1e-11;
}
nuSgs:
{
type zeroGradient;
}
nuTilda:
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

Help me please!

Best regards!