[OpenFOAM] Take derivative of mean velocity in paraFoam

hiuluom · January 30, 2014, 01:28

I run LES simulation with pisoFoam and it's finish. And now, I would like to calculate derivative of mean velocity in parafoam also paraview.
$\frac{\partial^2 \langle u_i\rangle}{\partial x_j^2}$
$\frac{\partial \langle u_i\rangle}{\partial x_j}$
<u> it means umean.
I computed umean by fieldAverage in OpenFOAM and now I want to compute derivative above.

Anyone can help me how to get it in parafoam?

Thanks your help.

Bernhard · January 30, 2014, 03:30

Why not using the FOAM framework for this with utilities foamCalc and foamCalcEx?

hiuluom · January 30, 2014, 04:04

Quote:

Originally Posted by Bernhard

Why not using the FOAM framework for this with utilities foamCalc and foamCalcEx?

Hi Bernhard,

I see in command foamCalc has div function.But $\frac{\partial^2 \langle u_i\rangle}{\partial x_j^2}$ is the laplacian, which is div(grad(umean)).
and about first derivative of umean?

I use OpenFOAm 2.1.1, I don't see foamCalcEx as you said. Could you show me clearly?

Thank you,
Thanh

hiuluom · January 30, 2014, 04:43

Hi Bernhard,

I saw your code extended of foamCalcEx on google. Thank you so much your code.

Best regards,
Thanh.

hiuluom · January 30, 2014, 11:07

When I used command foamCalc or foamCalcEx to calculate div(U) and grad(U) but I meet error. Can anyone check help me?

Code:

Selecting calcType div
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : foamCalc div U
Date   : Jan 30 2014
Time   : 23:03:37
Host   : "compeng"
PID    : 7276
Case   : /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.01
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.02
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.03
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.04
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.05
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.06
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.07
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.08
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.09
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.1
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.10001
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.11
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.12
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

Time = 0.13
    Reading U
    Calculating divU
--> FOAM Warning : 
--> FOAM FATAL IO ERROR: 
keyword div(U) is undefined in dictionary "/home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes"

file: /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily/system/fvSchemes::divSchemes from line 36 to line 45.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 400.

End

wyldckat · February 1, 2014, 08:48

Greetings to all!

To answer the original question: there is a filter named "Compute Derivatives", but it doesn't seem to be able to calculate the laplacian.
edit: In the Python Calculator, it does seem possible to use the "laplacian" function: http://www.paraview.org/Wiki/ParaVie...hon_Calculator

As for the latest post: the "div(U)" entry is missing from the file "system/fvSchemes". You can find several examples for such an entry by running this command:

Code:

find $FOAM_TUTORIALS -name "fvSchemes" | xargs grep "div(U)"

If you have a look into the file "compressible/rhoPimpleFoam/ras/cavity/system/fvSchemes" on the tutorials folder, you'll see this block of code:

Code:

divSchemes
{
    default none;
    div(phi,U) Gauss limitedLinearV 1;
    div(phid,p) Gauss limitedLinear 1;
    div(phi,K) Gauss linear;
    div(phi,h) Gauss limitedLinear 1;
    div(phi,k) Gauss limitedLinear 1;
    div(phi,epsilon) Gauss limitedLinear 1;
    div(phi,R) Gauss limitedLinear 1;
    div(phi,omega) Gauss limitedLinear 1;
    div((rho*R)) Gauss linear;
    div(R) Gauss linear;
    div(U) Gauss linear;
    div((muEff*dev2(T(grad(U))))) Gauss linear;
}

If you look carefully, you'll see the line that starts with "div(U)". You need to add that line to the file "system/fvSchemes" in your case, inside the same block "divSchemes".

Best regards,
Bruno

hiuluom · February 2, 2014, 11:42

Hi Bruno,

I thank you so much about this guide, I can calculate div(U) but grad(U) can not compute. In fvscheme has defined grad(U):

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default backward;
}

d2dt2Schemes
{
}

gradSchemes
{
    default         Gauss linear;

    grad(nuTilda)   cellLimited Gauss linear 1;
    grad(U)         cellLimited Gauss linear 1;
}

divSchemes
{
    default         none;

    div(phi,U)      Gauss LUST unlimitedGrad(U);
    //div(phi,U)      Gauss linearUpwind unlimitedGrad(U);
    //div(phi,k)      Gauss limitedLinear 1;
    //div(phi,k)      Gauss upwind;
    div(phi,k)       Gauss SFCD;
    div(phi,nuTilda) Gauss limitedLinear 1;
	div(U)          Gauss linear;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear limited 0.33;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited 0.33;
}

fluxRequired
{
    default         no;
    p;
}

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

And this is error.

Code:

Selecting calcType grad
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec   : foamCalcEx grad U
Date   : Feb 02 2014
Time   : 23:33:44
Host   : "compeng"
PID    : 2674
Case   : /home/huynh/OpenFOAM/huynh-2.1.1/run/pitzDaily
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0


--> FOAM FATAL ERROR: 
Unable to process U
No call to grad for fields of type volVectorField

I really want to calculate $\frac{\partial \langle u_i\rangle}{\partial x_j}= grad(UMean)$ and $\frac{\partial^2 \langle u_i\rangle}{\partial x_j^2} =laplacian(UMean) = div(grad(UMean))$ . I only have computed div(UMean) up to now. Could you show me my error?

wyldckat · February 2, 2014, 13:22

Hi Huynh,

foamCalcEx is missing the ability to handle "grad(U)" and "div(gradU)".
I've finished doing a bug report and respective patch for this here: http://code.google.com/p/foamcalcex/issues/detail?id=2

Download the patch file "changes.patch" from that bug report and place the file inside the folder "foamCalcEx". Then run:

Code:

patch -p1 < changes.patch
./Allwmake

Now go into your case folder and run:

Code:

foamCalcEx grad U
foamCalcEx div gradU

It will likely complain about the missing "div(gradU)", but I think you now know what to do

WARNING: I have not checked if the results given are correct. I simply did what seemed logical in the source code... and the results seemed sane enough.

Best regards,
Bruno

hiuluom · February 3, 2014, 01:03

Hi Bruno,

It worked very good. I thank you so much.

Best regards,
Thanh.

Bernhard · February 3, 2014, 03:54

Quote:

Originally Posted by wyldckat

WARNING: I have not checked if the results given are correct. I simply did you seemed logical in the source code... and the results seemed sane enough.

That's why we didn't include it in the utility up till now, following the Gschaider-philosophy to implement what you need. Anton is working on including your patch.

Thanh, can you let us know your experience with using this patch?

hiuluom · February 3, 2014, 04:54

Quote:

Originally Posted by Bernhard

Thanh, can you let us know your experience with using this patch?

Actually I am proving the variance of pressure equation:
$\begin{split} \frac{1}{2\rho}\frac{\partial\langle p'^2\rangle}{\partial x_i} &=\nu\langle p\frac{\partial^2 u_i}{x_j^2}\rangle -\nu\langle p\rangle\frac{\partial^2\langle u_i\rangle}{\partial x_j^2} \\ & \quad -\langle pu_j\frac{\partial u_i}{\partial x_j}\rangle + \langle p\rangle\langle u_j\rangle\frac{\partial\langle u_i\rangle}{\partial x_j} + \langle p\rangle\frac{\partial\langle u'_iu'_j\rangle}{\partial x_j}\\ & \quad-\langle p\frac{\partial u_i}{\partial t}\rangle \end{split}$
I have average of all these terms above by edit pisoFoam. I only prove left hand side equal to the right hand side of equation by using paraFoam, but gradient and laplacian of mean velocity does not have. So I must calculate it and using parafoam insert equation above.

About the patch of Bruno, I only did following the guide of him. I added command div(U) and div(grad(U)) in fvscheme.

Best regards,
Thanh.

Bernhard · February 3, 2014, 05:04

foamCalcEx was mainly designed for quick and dirty calculation of single operations. If you want to do whole expressions like this, I would recommend funkyDoCalc.

hiuluom · February 4, 2014, 05:46

Quote:

Originally Posted by Bernhard

foamCalcEx was mainly designed for quick and dirty calculation of single operations. If you want to do whole expressions like this, I would recommend funkyDoCalc.

Thanks Bermhard. I will try funkyDoCalc.

FlorisvdBeek · April 26, 2016, 06:44

Hi guys!

[EDIT]: Pffff my bad, lack of reading the error message properly.. It was referring to the multiRegion fvScheme file (in system/FluidRegion1), not the original file (system/fvScheme) which I had not defined at all yet. So, problem solved!

I am quite new to OpenFOAM (so I hope this is a piece of cake for you guys

) and Im modifying the electrostaticsFoam into a multiRegion solver, but Im running into a similar problem as reported. Im trying to calculate the electric field (just as they do in the original electrostaticsFoam) during createField initialization. Compiling goes well, but when I run a case I get the following error:

Code:

$ electrostaticMultiRegionFoam 

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.1-119cac7e8750
Exec   : electrostaticMultiRegionFoam
Date   : Apr 26 2016
Time   : 12:29:04
Host   : "floris-SATELLITE-L850-184"
PID    : 5875
Case   : /home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create fluid mesh for region Fluid1 for time = 0

Create solid mesh for region Solid1 for time = 0

Reading physicalProperties

*** Reading fluid mesh thermophysical properties for region Fluid1

    Adding to rho

    Adding to phi

    Calculating field magE



--> FOAM FATAL IO ERROR: 
keyword grad(phi) is undefined in dictionary "/home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion/system/Fluid1/fvSchemes.gradSchemes"

file: /home/floris/OpenFOAM/floris-3.0.1/run/dischargeCase/electrostaticFoam/02_opposingConductorsMultiRegion/system/Fluid1/fvSchemes.gradSchemes

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 442.

FOAM exiting

I am calculating the electric field magnitude magE in "createField.H" accordingly:

Code:

// Initialise fluid field pointer lists


PtrList<volScalarField> rhoFluid(fluidRegions.size());
PtrList<volScalarField> phiFluid(fluidRegions.size());
PtrList<surfaceScalarField> rhoFluxFluid(fluidRegions.size());
PtrList<volScalarField> magEFluid(fluidRegions.size());
PtrList<volVectorField> EFluid(fluidRegions.size());
PtrList<dimensionedScalar> kFluid(fluidRegions.size());
PtrList<dimensionedScalar> epsilon0Fluid(fluidRegions.size());


// Populate fluid field pointer lists
forAll(fluidRegions, i)
{
        Info<< "Reading physicalProperties\n" << endl;

    IOdictionary physicalProperties
    (
        IOobject
        (
            "physicalProperties",
            runTime.constant(),
            fluidRegions[i],
            IOobject::MUST_READ_IF_MODIFIED,
            IOobject::NO_WRITE
        )
    );
    
        dimensionedScalar epsilon0
    (
        physicalProperties.lookup("epsilon0")
    );

    dimensionedScalar k
    (
        physicalProperties.lookup("k")
    );
    
    Info<< "*** Reading fluid mesh thermophysical properties for region "
        << fluidRegions[i].name() << nl << endl;
        
    Info<< "    Adding to rho\n" << endl;
        rhoFluid.set
        (
            i,
            new volScalarField
            (
                IOobject
                (
                    "rho",
                    runTime.timeName(),
                    fluidRegions[i],
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                fluidRegions[i]
            )
        );
    
    Info<< "    Adding to phi\n" << endl;
        phiFluid.set
        (
            i,
            new volScalarField
            (
                IOobject
                (
                    "phi",
                    runTime.timeName(),
                    fluidRegions[i],
                    IOobject::MUST_READ,
                    IOobject::AUTO_WRITE
                ),
                fluidRegions[i]
            )
        );
    
    
    Info<< "    Calculating field magE\n" << endl;
        magEFluid.set
        (
            i,
            new volScalarField
            (
                IOobject
                (
                    "magE",
                    runTime.timeName(),
                    fluidRegions[i],
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                mag(fvc::grad(phiFluid[i]))
            )
        );
    
    Info<< "    Calculating field E\n" << endl;
        EFluid.set
        (
            i,
            new volVectorField
            (
                IOobject
                (
                    "E",
                    runTime.timeName(),
                    fluidRegions[i],
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                -fvc::grad(phiFluid[i])
            )
        );
    
    Info<< "    Calculating field rhoFlux\n" << endl;            
    rhoFluxFluid.set
        (
            i,
            new surfaceScalarField
            (
                IOobject
                (
                    "rhoFlux",
                    runTime.timeName(),
                    fluidRegions[i],
                    IOobject::NO_READ,
                    IOobject::NO_WRITE
                ),
         -k*fluidRegions[i].magSf()*fvc::snGrad(phiFluid[i])
            )
        );
}

I should have the grad operator defined properly in fvSchemes:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         leastSquares;
    grad(phi)       leastSquares;
    grad(phiFluid[i])       leastSquares;
    grad(phiFluid)       leastSquares;
}

divSchemes
{
    default         none;
    div(rhoFlux,rho) Gauss upwind;
}

laplacianSchemes
{
    default         none;
    laplacian(phi)  Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
    snGrad(phi)     corrected;
}


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

I have tried playing around with the fvSchemes input, but haven't found a solution yet.

Anyone any idea what may go wrong here ?

Thanks,
Floris

January 30, 2014, 01:28	Take derivative of mean velocity in paraFoam	#1
hiuluom Senior Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 105 Rep Power: 12	I run LES simulation with pisoFoam and it's finish. And now, I would like to calculate derivative of mean velocity in parafoam also paraview. $\frac{\partial^2 \langle u_i\rangle}{\partial x_j^2}$ $\frac{\partial \langle u_i\rangle}{\partial x_j}$ <u> it means umean. I computed umean by fieldAverage in OpenFOAM and now I want to compute derivative above. Anyone can help me how to get it in parafoam? Thanks your help.

February 1, 2014, 08:48		#6
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,974 Blog Entries: 45 Rep Power: 128	Greetings to all! To answer the original question: there is a filter named "Compute Derivatives", but it doesn't seem to be able to calculate the laplacian. edit: In the Python Calculator, it does seem possible to use the "laplacian" function: http://www.paraview.org/Wiki/ParaVie...hon_Calculator As for the latest post: the "div(U)" entry is missing from the file "system/fvSchemes". You can find several examples for such an entry by running this command: Code: find $FOAM_TUTORIALS -name "fvSchemes" \| xargs grep "div(U)" If you have a look into the file "compressible/rhoPimpleFoam/ras/cavity/system/fvSchemes" on the tutorials folder, you'll see this block of code: Code: divSchemes { default none; div(phi,U) Gauss limitedLinearV 1; div(phid,p) Gauss limitedLinear 1; div(phi,K) Gauss linear; div(phi,h) Gauss limitedLinear 1; div(phi,k) Gauss limitedLinear 1; div(phi,epsilon) Gauss limitedLinear 1; div(phi,R) Gauss limitedLinear 1; div(phi,omega) Gauss limitedLinear 1; div((rhoR)) Gauss linear; div(R) Gauss linear; div(U) Gauss linear; div((muEffdev2(T(grad(U))))) Gauss linear; } If you look carefully, you'll see the line that starts with "div(U)". You need to add that line to the file "system/fvSchemes" in your case, inside the same block "divSchemes". Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM Last edited by wyldckat; February 1, 2014 at 16:55. Reason: see "edit:"

February 2, 2014, 13:22		#8
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,974 Blog Entries: 45 Rep Power: 128	Hi Huynh, foamCalcEx is missing the ability to handle "grad(U)" and "div(gradU)". I've finished doing a bug report and respective patch for this here: http://code.google.com/p/foamcalcex/issues/detail?id=2 Download the patch file "changes.patch" from that bug report and place the file inside the folder "foamCalcEx". Then run: Code: patch -p1 < changes.patch ./Allwmake Now go into your case folder and run: Code: foamCalcEx grad U foamCalcEx div gradU It will likely complain about the missing "div(gradU)", but I think you now know what to do WARNING: I have not checked if the results given are correct. I simply did what seemed logical in the source code... and the results seemed sane enough. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM Last edited by wyldckat; February 3, 2014 at 05:12. Reason: "I simply did you seemed logical" -> "I simply did what seemed logical"

February 3, 2014, 05:04		#12
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 21	foamCalcEx was mainly designed for quick and dirty calculation of single operations. If you want to do whole expressions like this, I would recommend funkyDoCalc. wyldckat likes this.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
kindly help me .. i have and error at line number 147..	m zubair	Fluent UDF and Scheme Programming	0	February 10, 2019 11:25
derivative definition of velocity IN CFX	aja1345	CFX	9	April 22, 2016 06:21
VELOCITY vs VELOCITY IN STN FRAME vs RELATIVE VELOCITY	everest20	FLUENT	1	July 13, 2015 08:35
WSS and normal velocity gradient for the slanted pipe	wanna88	FLUENT	2	October 1, 2012 22:34
what the result is negatif pressure at inlet	chong chee nan	FLUENT	0	December 29, 2001 05:13

January 30, 2014, 03:30		#2
Bernhard Senior Member Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 21	Why not using the FOAM framework for this with utilities foamCalc and foamCalcEx?

January 30, 2014, 04:43		#4
hiuluom Senior Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 105 Rep Power: 12	Hi Bernhard, I saw your code extended of foamCalcEx on google. Thank you so much your code. Best regards, Thanh.

February 3, 2014, 01:03		#9
hiuluom Senior Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 105 Rep Power: 12	Hi Bruno, It worked very good. I thank you so much. Best regards, Thanh.