IIRC at least in some version of OpenFOAM it was:

Turbulence off:
Turbulence is not solved but the turbulent viscosity is added to the effective viscosity. Meaning that if there are non-zero k and epsilon fields present the effective viscosity is higher than the laminar viscosity.

"Laminar" turbulence model:
Returns a zero turbulent viscosity -> correct laminar viscosity.

Just a note, as Hrv suggested, to have second order on all meshes, use leastSquares for gradient evaluation. However the use of Gauss should not prevent the vortex shedding.

Imho this is not necessary. As you can see in the case of the cylinder done by Frank Bos, he doesn't perturbate the flow, and the structures start to form immediately.

Yes, icoFoam should do the job if your Re is similar to those considered by Frank Bos. Btw, what is your Re, defined as U*d/nu, where d is the cylinder/sphere diameter?

Regards,

So,

3D simulation is on its way - once it is finished I will post pictures (pressure, velocity plots) and then we can discuss the matter further.

I use the "standard" formulation of the Reynoldsnumber: Re = U*d/nu and I am using air properties for T=20(where the heck is the degree symbol on an American keyboard?) Celcius.

In the meantime I will set up a 2D case for a circular and a square cylinder in low Re(around 100 - that vortex shedding occurs) and will then try to verify the results with a reference. I will probably be able to post the first results in a couple of hours plus pictures of the meshs I used.

-harly

... couple of hours later ...
 

Hi everyone,

so here are some interesting results I'd like to discuss with you:

I took the case Frank Bos offers on his homepage and ran the case with a force configuration in the controldict[1] as presented in the Thread Forces in OF-1.5 and a different viscosity (0.01 instead of 0.0066667) to realize Re = 100.

You can see the C_L / C_D - time - plot for the original(Re=150) here.
http://www.harly.de.vu/www/cylinder_Re150.jpg
You can see the C_L / C_D - time - plot for the Re=100 here.
http://www.harly.de.vu/www/circular_...nk_Bos_50k.jpg
Both were created on the 50k mesh

I took this as my reference for how my cases should look like. The first thing I wanted to change was the parameters Frank used (he sets U to 1 and adapts nu to get the Re) and replace them with "my" standard values for air:

density: 1.204
dynamic viscosity(eta): 1.83692474747684e-5
kinematic viscosity(nu): 1.525684971e-5

with d=1 that would result in U=0.001525....

From here I wanted to reproduce a result I have in a reference[2] for a circular cylinder in 2D at Re = 100.
The results should look as following:
http://www.harly.de.vu/www/reference_Re100.jpg
(I will try to scan the picture, unfortunately I only have a hard copy of my reference - so I took a picture with my camera)

Here is a (bad) picture of the original mesh the results were obtained with:
http://www.harly.de.vu/www/reference_mesh.jpg

Unfortunately I couldn't get any useful results with the "real" air configuration and my question would be WHY? - I figured they would just take longer to get some results but even running them overnight didn't bring useful results, !I could not obtain shedding! - this is very important can someone please comment if she/he had the same experience? Maybe that can solve the problems I am having with my sphere? - What do you think?

I took the cases I had and switched to U=1 and calculated the viscosity with Re = U*d/nu (with U and d always being 1 that means nu = 1/Re).


and here are the competing meshs:

Frank Bos(50k):
http://www.harly.de.vu/www/50k.png
Frank Bos(100k):
http://www.harly.de.vu/www/100k.png
A mesh from me, created in Gambit:
http://www.harly.de.vu/www/mymesh.png
and here are the results:

50k :
http://www.harly.de.vu/www/circular_...nk_Bos_50k.jpg
100k :
http://www.harly.de.vu/www/circular_...k_Bos_100k.jpg
my mesh:
http://www.harly.de.vu/www/circular_Re100_own_mesh.jpg
I packed my case for you to have a look at:

here

I didn't want to repack Frank's stuff so please visit his website and download his testcases:
here

As for the conigurations which were used in all three cases I summed up the most important bits below:

-----------------------------------------------------------------------------------------------------
ddtSchemes
{
default CrankNicholson 0.5;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nu,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(HbyA) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}
--------------------------------------------------------------------------------------------------------------
--------------------------------------------------------------------------------------------------------------
solvers
{
p ICCG 1e-06 0;
U BICCG 1e-05 0;
}

PISO
{
momentumPredictor yes;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}
---------------------------------------------------------------------------------------------------------------

Any suggestions in how I would get my results closer to what it is supposed to be? Please check my controlDict if I am making a stupid mistake while calculating the forces. And Frank if you read this maybe you could tell us if your results were of the same magnitude. Looking forward to your comments.

-harly

[1]: link to the used controlDict
[2]: Computational Modelling of vortex shedding flows by Vlado Przulj

Hi Daniel,

I encounter the same problems as you with respect to the absence of any vortex shedding behind the sphere. Did you already solve the problem with the hints of your last message?

At the moment, I am running a case with a perturbated inital velocity field, but I am pessimistic about the result...

Many thanks.

Regards,
Bob

I had similar problems when running a LES with wall-functions.
Using a wall-resolved grid helped to get rid of this problem.

Markus

I am in the same point as you with a cube centered in the domain by using RANS models...
did you find the solution???

Antonio

Hi Harly and All,

Thanks for the posting, it's a good discussion. I'm also doing about the same simulation, flow over a square, 2d at Re= 22k. I have three grid resolution, course:30cells x 4 edges, medium:50 cells x 4 edges and fine: 80 cells x 4 edges. The course and medium have wall function and the fine without wall function.

The results for coarse and medium are about the same for experiments, but for fine grid is not.

Any comment why the fine grid gives the 'wrong' results? The y+ for fine grid is less than 3, so I don't use wall function.

Thanks,
Mali

Dear harly,
Did you figured out why you sometimes cannot obtain shedding?

I'm doing simulation around rectangular prism with Re 1e5 and I can't get oscillations of Cd and Cl and vortex shedding using RANS.
The results of LES calculations are ok.

Regards,
Paulina

Paulina, can you post some of your log output?

I'm a little bit out of topic, my calculations were made in Fluent.

I've tried to recreate simulation from an article (http://www.sciencedirect.com/science...43974X06001593) were they used same grid for LES and RANS, and enhanced wall funcion for Kato Launder k-epsilon.
Using above mentioned configuration my Cd and Cl were completely flat (as if it was laminar flow).

Yesterday I run simulation for standard wall function for a grid with higher y+. I've got oscillations of Cl, but after 2s it went flat.

I still don't know what is missing in the calculations (grid? set up?).

How long did you let it running after the decay of the initial oscillations? It sometimes took a really long time in Fluent until the actual von Karman street started.

The longest time was about 4 seconds. I assumed that nothing new will happen later. The period of one oscillation (from the article and my LES simulation) is about 0,13s.

While using same grid as for LES initial oscillations were quite small and ended even before 1s.

Do you think that 10s would be enough for vortex shedding to occur?

I'll run simulations few more hours and let you know about the results.

How long is your time step and did you switch all the numerical settings to 2nd order?

Yes, all numerical settings are in 2nd order (And Fluent 15 run in double precision). BC are velocity inlet and outflow.

The time step is 0.002s or 0.001s. I used even 0.0005s but haven't seen difference in the results.
As a convergence criteria I set up epslion equal to 1e-7, so now it is 5 iterations per 1 time step.

You can see settings and how Cd and Cl look after few more seconds of calculations.

I can not guarantee that, but I once had this behavior and after a long time of waiting the vortex street started. If you have time, give it a try ;)

10 seconds passed and nothing happened. The flow field looks like after steady flow calculations.

I think this is a matter of bad lack, or rather bad mesh.

I'm out of ideas what to change to get right results.

I've tried few more things but the situation is still the same.
Initial oscillations are gone after few seconds and nothing else happens.

If you would like to try and check here you can find my mesh and inlet profiles:
https://www.dropbox.com/sh/5hui9t2vk...toMth-SJa?dl=0

Hi all,
Did you solve your problems? I was actually solving flow past acylinder with D/H=0.3 and Re=100. I am getting correct strouhal number but getting very low drag co-efficient. Can you tell me why? I am really stuck at this for relly long time. I am using openFoam 3.0.1 and ubuntu 16.04. i have attached my case.

Thanks in advance...

regards
Subhankar

Subhankar,

Have u try higher order scheme?