Hello, Looking at the UserG
 

Hello,

Looking at the UserGuide, it's something I should be able to do.
I want to use the linear Upwind scheme for div(phi,U).

Using simpleFoam in Openfoam 1.4.1 on linux 64bit.


div(phi,U) Gauss linear;
div(phi,U) Gauss linear corrected;
div(phi,U) Gauss QUICK;

works fine. But

div(phi,U) Gauss linearUpwind;

does not.



I get:

--> FOAM FATAL IO ERROR : Grad scheme not specified

Valid grad schemes are :

8
(
cellMDLimited
extendedLeastSquares
faceMDLimited
leastSquares
fourth
faceLimited
cellLimited
Gauss
)


file: /home/nr/OpenFOAM/nrousselon-1.4.1/run/ccm2foam4/system/fvSchemes::div(phi,U) at line 40.

From function gradScheme<type>::New(Istream& schemeData)
in file /home/nr/OpenFOAM/OpenFOAM-1.4.1/src/finiteVolume/lnInclude/gradScheme.C at line 65.

FOAM exiting








/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class dictionary;
object fvSchemes;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default steadyState;
}

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

divSchemes
{
default none;
div(phi,U) Gauss linear corrected;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

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

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}


// ************************************************** *********************** //

You need to specify the grad-s
 

You need to specify the grad-scheme used by linearUpwind, e.g.

div(phi,U) Gauss linearUpwind Gauss linear;

or

div(phi,U) Gauss linearUpwind leastSquares;

or if you want to limit the gradient used by the linearUpwind scheme which is often beneficial

div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1;

etc.

Thanks, just what I needed.
 

Thanks,

just what I needed.

Nicolas

I have the same problem and tried to adapte it on my case with the bouyantBoussinesqSimpleFoam, but it didn't work.
This is what I get:
Line 25 is the one with the default gradSchemes. My fvSchemes file is:

You messed up the order: cellLimited is a modifier for a gradient scheme, so it comes first. Think about which class should contain which. :)

div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1;

Enjoy,

Hrv

Hi Hrvoje,

thank you. Stupid mistake. Now it's running! :-)

Regards,
Erik

Hello!

I got a question. Does div(phi,U) Gauss linearUpwind fourth mean that with order fourt the velocity field is approximated?

Cheers

No, it means you use a fourth-order scheme to compute the gradients, but clearly the order of the linearUpwind stays unchanged.

I think I have to learn something. Could you send me a reference which contains the derivation of this kind of scheme?

Could you please have a look at this thread I just created?
http://www.cfd-online.com/Forums/ope...fvschemes.html
thanks!

fvSchemes in OF20
 

"
div(phi,U) Gauss linearUpwind Gauss linear;

or

div(phi,U) Gauss linearUpwind leastSquares;

or if you want to limit the gradient used by the linearUpwind scheme which is often beneficial

div(phi,U) Gauss linearUpwind cellLimited Gauss linear 1;

etc.[/QUOTE]"

Does anyone know, how should the same fvSchemes be set in the 2.0 version of OpenFOAM?

Hi!

My example which I use with pimpleFoam.

Could you help me with this:

Implementing: laplacian(nuEff,U) Gauss linear Gauss fourth;

gives:

[0] --> FOAM FATAL IO ERROR:
[0] Unknown discretisation scheme fourth

Valid schemes are :

3
(
corrected
limited
uncorrected
)

but it should be able to work with fourth...

Thanks

The correct syntax is

Gauss <scheme> <correction option>;

so

Gauss linear corrected;

For fourth-order it is:

Gauss cubic corrected;

Best,

Thanks Alberto for your reply

Now it is running, so I hope my solution will improve.

Thanks

Felipe

Thanks
 

Dear makaveli_lcf,

Thank you for your reply!

Regards,
TKE

Hi again Alberto

Well my simulation ran, but I guess I have not achieved what I wanted.

In the attached graph I have made the simulations from 0 to 20 degrees with a step of 2 degrees with OpenFOAM and another CFD code.

I want to use the QUICK scheme, but I am over predicting my solution with OF in comparison to the other CFD code and both over predict lift in comparison to the measurements (Abbot and Doenhoff).

I have my convection terms with QUICK and the diffusion terms with second order scheme (Gauss linear corrected).

Thus I change my diffusion terms to a fourth interpolation scheme in order to improve my solution (QUICK2), and I can see that the curve is lower, but still it can not capture the separation pretty well. In this case my diffusion terms are Gauss cubic corrected.

Do you have any suggestions for improving my results?

Regards

Felipe

ps: I was going to upload the case but due to the size, it did not let allow me to do it. But I could send you a tar file with it (2.7 MB).

Which OF version do you use?

I use 1.7.1

Ok, because in 20x I noticed strange behavior: viscous terms are under-estimated in my case with equal settings I was simulating in v16 and 17x. I will study it in details and also report here on forum.