CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

What is the best "way" to get vortex shedding ?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 1, 2009, 17:48
Default
  #21
Member
 
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 80
Rep Power: 8
juho is on a distinguished road
Quote:
Originally Posted by harly View Post
@albcem:
Which solver would you use ? - so far I was using icoFoam, because I was under the impression I don't need a turbulence model like for the 2D case Frank Bos presents. That explains also, why I used turbulence model switched off in turbFoam. - But maybe that could be the mistake?
-harly
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.
juho is offline   Reply With Quote

Old   April 2, 2009, 02:26
Default
  #22
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by harly View Post
- a switch to complete 2nd order aka backward in time and Gauss linear in space
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.

Quote:
- preturbation of flow
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.

Quote:
Which solver would you use ? - so far I was using icoFoam, because I was under the impression I don't need a turbulence model like for the 2D case Frank Bos presents.
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,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 2, 2009, 13:58
Default
  #23
Member
 
Daniel Harlacher
Join Date: Mar 2009
Location: Davis, CA, United States
Posts: 60
Rep Power: 8
harly is on a distinguished road
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
harly is offline   Reply With Quote

Old   April 3, 2009, 21:47
Default ... couple of hours later ...
  #24
Member
 
Daniel Harlacher
Join Date: Mar 2009
Location: Davis, CA, United States
Posts: 60
Rep Power: 8
harly is on a distinguished road
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.

You can see the C_L / C_D - time - plot for the Re=100 here.

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:

(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:


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):

Frank Bos(100k):

A mesh from me, created in Gambit:

and here are the results:

50k :

100k :

my mesh:

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
harly is offline   Reply With Quote

Old   July 28, 2009, 06:37
Default
  #25
Bob
New Member
 
Bob De Clercq
Join Date: Apr 2009
Location: Belgium
Posts: 17
Rep Power: 8
Bob is on a distinguished road
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
Bob is offline   Reply With Quote

Old   July 29, 2009, 08:15
Default
  #26
Member
 
Markus Weinmann
Join Date: Mar 2009
Location: Stuttgart, Germany
Posts: 77
Rep Power: 8
cfdmarkus is on a distinguished road
I had similar problems when running a LES with wall-functions.
Using a wall-resolved grid helped to get rid of this problem.

Markus
cfdmarkus is offline   Reply With Quote

Old   August 20, 2012, 12:13
Default
  #27
Member
 
Join Date: Jun 2011
Posts: 65
Rep Power: 6
maalan is on a distinguished road
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

Last edited by maalan; September 9, 2012 at 17:38.
maalan is offline   Reply With Quote

Old   April 3, 2014, 03:25
Default
  #28
New Member
 
Join Date: Mar 2009
Location: adelaide, SA, Australia
Posts: 27
Rep Power: 8
mali is on a distinguished road
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
__________________
mali
mali is offline   Reply With Quote

Reply

Tags
laminar, sphere, vortex shedding

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
K-Epsilon for Vortex Shedding Sham FLUENT 30 July 10, 2015 21:13
how can I determine the vortex shedding time step Zhe Liu CFX 3 July 30, 2008 17:16
Vortex shedding? rbel038 CFX 4 April 27, 2008 19:57
Vortex shedding behind cylider in cross flow Muthu FLUENT 0 March 6, 2006 11:29
basic vortex shedding john Main CFD Forum 4 November 6, 2000 14:23


All times are GMT -4. The time now is 22:58.