CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)

 treima September 11, 2012 04:57

1 Attachment(s)
Hello,

I´m trying to solve the onedimensional advection equation

with OpenFOAM.

I took following code:
Code:

    solve     (         fvm::ddt(u) + coeff*fvc::div(u * unitVector_x)     );
But now occours a problem, the solution shows some waves (you can see in the attached picutre). My boundary conditions are

left boundary - fixedValue, uniform 1

Normally there is should be one frontline, all values on the left of the frontline should be 1 and all values on the right 0.

Does anyone have any suggestions concerning my problem?

I had several ideas, why there occure this error. This equation is hyperbolic, another pde of this type is the euler-equation in rhoCentralFoam. Do I have to do some interpolation, too? Or are the numerical errors from OpenFOAM this huge? I´ve tried with a very small timestep (1e-06), too. No improvement occured ;)

regards
treima

 Cyp September 12, 2012 08:40

Hi !

The equation you want to solve is hyperbolic and require a special discretization scheme like flux limiter. For exemple, if you want to solve the equation :

If phi is the flux (F(S)) defined otherwise, you can set a van Leer scheme defining

Code:

surfaceScalarField phiS = fvc::flux(phi/S,S, "div(phi,S)"); solve ( fvm::ddt(S) + fvc::div(phiS) );
and indicate the vanLeer scheme in fvScheme :
Code:

divSchemes {     div(phi,S)  Gauss vanLeer; }
The solution is then much more stable. You can adapt easily this example to your situation.

or

?

Regards,
Cyp

 Hisham September 12, 2012 10:35

Hello,

On a side note: I think you should implement a generic solution (3D) and introduce the one-dimensional condition by defining all side patches (parallel to dimension of interest) as empty!

Regards
Hisham

 treima September 13, 2012 04:37

1 Attachment(s)
Thanks for your advice, it helped me a lot to solve my problem!

The background for solving the onedimensional advection equation was to have a "simple" first step into the world of hypberbolic equations in OpenFOAM.
Of course it is more useful to implement a 3D solution of the problem, so it should be this equation:

My code looks like the following. u is a volScalarField.

Code:

volVectorField uVector (u * normalVector); surfaceScalarField phiU ("phiU", fvc::interpolate(uVector) & mesh.Sf()); surfaceScalarField phiUflux = fvc::flux(phiU, U, "div(phiU,u)"); solve (     fvm::ddt(u) + c*fvc::div(phiUflux) );
Perhaps the first line is not so nice, but you can define a normal vector which fits for the problem, in my case (1,0,0).

I´ve changed my boundary conditions, too. For the upper and the lower boundary I take "empty" and not "zeroGradient".

Dou you have any suggestions for improving my code?

As you can see in the screenshot below, this solution works for the problem shown in my first post. In the next days I´ll do some tests for other geometries and, if this works, I`ll take more complicated hyperbolic equations.

regards
treima

 All times are GMT -4. The time now is 17:26.