[30na]

Hi everybody,
I know this problem has been posted by many people but i just can't find an answer for it.
I am trying to simulate a laminar flow over a cylinder using simpleFoam. (re=300)
but i have trouble with Cd and Cl , their magnitudes are not close to the magnitudes in articles and papers.
I use the following code to get Cd and Cl :

forces
{
type forces;
functionObjectLibs ("libforces.so");
outputControl timeStep;
outputInterval 1;

patches ( cylinder );
pName p;
UName U;
rhoName rhoInf;
log true;

CofR (0 0 0);

rhoInf 1;
}
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ( "cylinder.so" );
outputControl timeStep;
outputInterval 1;

patches ( cylinder );
pName p;
UName U;
rhoName rhoInf;
log true;

liftDir (0 1 0);
dragDir (1 0 0);
CofR (0 0 0);
pitchAxis (0 0 1);

magUInf 1.00;
rhoInf 1;
lRef 1;
Aref 1.4;
}

I'm not sure what Aref and LRef should be ? are they the diameter of the cylinder ?
I read somewhere that Aref is diameter*domain length in the z direction ?

Any help would be appreciated !

[alexeym]

Hi,

1. Aref is the front area of the cylinder, Lref is diameter of cylinder.

2. Usually mistake is in CofR, it should be the center of cylinder.

3. If you are trying to compare with published values, make sure you've got more-or-less the same mesh. As it appears values of Cd (especially) and Cl depend on mesh density.

Once I've made a comparison of influence of different parameters on simulation results - http://matveichev.blogspot.fr/2014/0...ex-street.html

[30na]

Thanka for your reply
Does the front area mean diameter*domain in the z direction? I dont really get it, bcuz it's a 2d simulation.

[alexeym]

I've used diameter*(size of domain in Z-direction), results were quite similar to the published ones.

[30na]

Thanks alexeym, how do you determine the size of domain in Z direction?

[alexeym]

If you created mesh with blockMesh, the answer is obvious, look in blockMeshDict. Also you can run checkMesh, it will show sizes of the mesh.

[30na]

No , i have created the mesh using Gambit and then transfered it to a Foam mesh . because it is a 2d mesh , i can't view the 3rd dimension in Gambit

[alexeym]

But when you import the mesh into OpenFOAM you should have a mesh with third dimension.

[30na]

I am starting to think that there might be sth wrong with the solution ,
my case is a laminar one so in RAS properties i changed the RAS model to laminar , should i do sth else or is this the only thing i have to do ?
and for changing the amount of nu, is it enough to just change it's magnitude in the nut and nutilda files or should i change them in some place else ?

[alexeym]

Kinematic viscosity of the fluid is set in constant/transportProperties file.

[30na]

the results seem to be good for Re=40 , but for Re=300 and 1000 , Cd is 1.1 but it should be around 1.5
Any thoughts what the problem might be ?

[alexeym]

1. Mesh can affect Cd greatly.
2. Are you sure solution converges on every time step?

[30na]

thanks again ! I have simulated the same case and mesh with fluent and the results are fine .
But i can't get the same results with openFoam . do you know what Reynolds number is considered turbulent for vortex shedding ?
I have used laminar solver in fluent for all the 3 reynolds number : 40 , 300 , 1000
and the results are close to published results.
But in openFoam i only got a good results for re=40 , using laminar solver? Should i use a turbulent solver for Re=300 and 1000 ?

[alexeym]

Post your case files, tell the meaning of "results are fine". As I'm not sure that your case is set up correctly, I can't suggest you anything.

[30na]

My problem is solved now , I was using SimpleFoam for an unsteady solution ! such a stupid mistake ! I used icoFoam instead and now everything is fine !
Anyways , I want to thanks you for your time and effort to help me get through this, I really appereciate your help !