icoFoam Courant number growth problem

tdof · September 23, 2016, 10:01

Hello,

I'm new to OpenFOAM 4.0 and only beginning to explore the solver. I want to run a laminar pipe flow case with either icoFoam or pisoFoam, but I've run into some issues. The pipe is 0.1m in diameter and 0.5m in length in the positive y-direction, the fluid is an oil with eta=0.1 Pa*s and rho=900kg/m³. The smallest tetra-element is about 1mm and with an expected u_max of 0.2m/s (inflow u_mean=0.1m/s), the smallest time step shouldn't exceed 0.005s for a Co-number of 1. I know that this issue is a rather common one while getting to know the solver and CFD in general, but I can't seem to find the root of it in my specific case. I've attached the necessary files.

I tried a wide range of time steps, but the Co-number just keeps growing, so I suspect the fv-settings (taken from the icoFoam cavity tutorial) or rather my model setup to be the cause. I also tried to get it to run with pisoFoam, but I didn't know what to write in the turbulenceProperties file after setting the turbulenceModel to laminar.

The boundary conditions for inflow and outflow patches don't seem to be overconstrained, so I don't know what to change there apart from setting the fixed inflow velocity to a mean mass flux, but the keyword for the mass flux doesn't seem to be described in the documentation, although I found some mentionings in older versions of OF via Google but not for recent ones.

Also, how do I know which options to set in fvSchemes ? Especially which types of keywords I need in ddt, d2dt2, grad, div, laplacianSchemes - for examples, when do I need div(phi,U), when do I need more settings and how to choose them?

I'd appreciate any help.

anishtain4 · September 23, 2016, 14:01

Hi,

1. I couldn't find any attached file.
2. If your turbulence model is laminar then you don't need any options there.
3. When using standard solvers which have been used extensively, usually the reason for divergence is the boundary conditions, can you share them with us?
4. If you are trying to use periodic boundary condition with pressure mass flux, try checking $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395
5. For those options I'd suggest to read user manual which gives you a good understanding what every choice will do. To make sure if you need it or not, you can comment it and if OF complains about not finding it you know it's needed, also you can write banana for the options, OF tells you he doesn't know banana, but here's your available keywords.

tdof · September 23, 2016, 14:43

-Oh sorry, I'm new to this forum. I uploaded the files as .txt before posting though, I don't know what went wrong
-Good to know, there was an error message complaining about the missing file. So I recon it must exist, but can be empty?
-See the attachments, I hope you can see them now
-No periodicities, but I might have a look nonetheless
-The keyword trick is a good one, I'll remember that

tdof · September 27, 2016, 17:51

Alright, I revised my BCs and found that the inflow direction was off. My workstation ran into some trouble and I had lost track of my models. The inflow direction is in negative y direction, but it somehow did not change anything. I got pisoFoam to run, but the Courant-number just keeps growing, even with adjustTimeStep activated! And no matter the step size using icoFoam, it's the same. I checked a few setup videos like this one: https://www.youtube.com/watch?v=zDFk0GCZG68 and didn't find any obvious differences concerning the BC setup. Here: http://www.cfd-online.com/Forums/ope...flow-pipe.html is some more input, but no improvement either. I noticed that Hypermesh did not create physicalType keywords in the boundary file, but adding them did'nt change anything. I could really use some advice as I don't know what to look for anymore.

p

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
inflow
{
type zeroGradient;
}

wall
{
type zeroGradient;
}

outflow
{
type fixedValue;
value uniform 0;
}
}

U

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
inflow
{
type fixedValue;
value uniform (0 -0.1 0);
}

wall
{
type fixedValue;
value uniform (0 0 0);
}

outflow
{
type zeroGradient;
}
}

transportProperties

transportModel Newtonian;
nu [0 2 -1 0 0 0 0] 0.1;

controlDict

application pisoFoam;

startFrom startTime;

startTime 0.000;

stopAt endTime;

endTime 0.1;

deltaT 0.00025;

writeControl timeStep;

writeInterval 80;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.8;

fvSchemes

ddtSchemes
{
default Euler;
}

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

divSchemes
{
default none;
div(phi,U) Gauss linear;
div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear orthogonal;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default orthogonal;
}

fvSolution

solvers
{

p
{
solver PCG;
preconditioner DIC;
tolerance 1e-4;
relTol 0;
}

pFinal
{
$p;
relTol 0;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-5;
relTol 0;
}
}

PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
}

turbulenceProperties

simulationType laminar;

tdof · September 28, 2016, 09:27

I succeeded by taking the pipe flow tutorial from FOAMHouse and replacing the mesh with my own one (see http://the-foam-house5.webnode.es/pr...ide-foamcases/). The mesh consists now of 25mm tetras without boundary layer, so it's very rough. deltaT is set to 0.0005s and it runs smoothly, maxCo is 0.021 at the end of the simulation. However, if I set deltaT to 0.005s, Co explodes instantly. How come!? The Courant number should be around 10 times the previous Co, so what is happening there?

anishtain4 · September 28, 2016, 13:41

Hi,

The best way to share your case is to remove all the time directories and constant/polyMesh if you have blockMeshDict so others can download it and run it.
I'm glad you got somewhere, try changing your gradSchemes from "linear" to "limitedLinear 1"

tdof · September 28, 2016, 15:17

Hi,

I use Hypermesh, so no blockMeshDict available. I got some advice in the meantime, my choices in fvSchemes and fvSolution weren't all that great in general. I was just so focused on the BCs that I did not look there more than I thought to be necessary.

Sugajen · June 20, 2017, 20:06

Quote:

Originally Posted by tdof

Hi,

I use Hypermesh, so no blockMeshDict available. I got some advice in the meantime, my choices in fvSchemes and fvSolution weren't all that great in general. I was just so focused on the BCs that I did not look there more than I thought to be necessary.

I am facing a similar issue where the Co number increases due to high pressure gradient. The solver that I am using is icoFoam.
I am able to run the same flow with 0 bar at outlet. But when I include the pressure of 60 bar (which is 6010 sq.m/sq.s in OF units) the Co number increases. Also, I checked my case for a cuboid domain instead of the one with curved edges as seen below. For the cuboid domain with 60 bar, OF solves it perfectly without Co increase. So either it is the mesh or solver. The checkMesh and checkMesh -allGeometry -allTopology yielded no error. So I am pretty sure it is the fvScheme or fvSolution or both. All ideas and suggestions are most welcome!

Do you mind sharing the fvSchemes and fvSolution that fixed your issue ? It would really be of great help.
Thanks in advance!

Currently I am using the following fvSchemes and fvSolution

fvSchemes

Code:

ddtSchemes
{
    default         Euler; // trusted answer
}

gradSchemes
{	
    default	    leastSquares;
}

divSchemes
{
    default         Gauss upwind;
}

laplacianSchemes
{

    default         Gauss linear uncorrected; 
}

interpolationSchemes
{
     default         linear; 
}

snGradSchemes
{
    default         orthogonal; 
}

fvSolution

Code:

solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0.05;
    }
    pFinal
    {
        $p;
        relTol          0;
    }
    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-05;
        relTol          0;
    }
}
PISO
{
    nCorrectors     1;
    nNonOrthogonalCorrectors 2;
    pRefCell        0;
    pRefValue       0;
}

piu58 · June 21, 2017, 01:20

High pressure gradient lead to high local velocity. It is quite normal that the max Co number increases then. I recommend refining the mesh in the areas with the pressure drop or increase.

Sugajen · June 22, 2017, 15:28

Quote:

High pressure gradient lead to high local velocity. It is quite normal that the max Co number increases then. I recommend refining the mesh in the areas with the pressure drop or increase.

As you suggested I refined the mesh but it didn't make much of a difference. Finally solved with the following fvSchemes

Code:

ddtSchemes
{
    default         Euler;
}

gradSchemes
{	
    default         cellLimited Gauss linear 1;
}

divSchemes
{
    default         Gauss upwind; 
}

laplacianSchemes
{
    default	    Gauss linear corrected;
}

interpolationSchemes
{
     default         linear; 
}

piu58 · June 23, 2017, 01:21

> As you suggested I refined the mesh but it didn't make much of a difference

If you want to control the Co number you need to refine the mesh only in the areas of fast changes and high velocity (areas where the high Co occurs). This way you minimize the required wall time for a simulation. Or, in other words , you may use a coarser mesh in areas with low CO number.

tdof · June 27, 2017, 08:19

Hi Sugajen, I'm using the settings set by HelyxOS (I tried it once, unfortunately no longer supported by newer versions of OF). They're working quite well and I've used them ever since. However, I don't know if there are possibilities to improve the settings manually since I didn't change much except the usage of GAMG:

fvSchemes:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
|       o          |                                                          |
|    o     o       | HELYX-OS                                                  |
|   o   O   o      | Version: v2.3.1                                           |
|    o     o       | Web:     http://www.engys.com                            |
|       o          |                                                          |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version 2.0;
    format ascii;
    class dictionary;
    location system;
    object fvSchemes;
}

    ddtSchemes
    {
        default Euler;
    }


    gradSchemes
    {
        default Gauss linear;
        grad(nuTilda) cellLimited Gauss linear 1;
        grad(k) cellLimited Gauss linear 1;
        grad(kl) cellLimited Gauss linear 1;
        grad(omega) cellLimited Gauss linear 1;
        grad(epsilon) cellLimited Gauss linear 1;
        grad(q) cellLimited Gauss linear 1;
        grad(zeta) cellLimited Gauss linear 1;
        grad(v2) cellLimited Gauss linear 1;
        grad(f) cellLimited Gauss linear 1;
        grad(sqrt(kt)) cellLimited Gauss linear 1;
        grad(kt) cellLimited Gauss linear 1;
        grad(sqrt(kl)) cellLimited Gauss linear 1;
    }

    divSchemes
    {
        //default Gauss linear;
        div(phi,U) bounded Gauss linearUpwindV grad(U);
		div(phi,U) Gauss linear grad(U);
        div(phi,k) bounded Gauss linearUpwind grad(k);
        div(phi,epsilon) bounded Gauss linearUpwind grad(epsilon);
        div(phi,zeta) bounded Gauss linearUpwind grad(zeta);
        div(phi,q) bounded Gauss linearUpwind grad(q);
        div(phi,omega) bounded Gauss linearUpwind grad(omega);
        div(phi,nuTilda) bounded Gauss linearUpwind grad(nuTilda);
        div(phi,T) bounded Gauss limitedLinear 1;
        div(phi,kl) Gauss limitedLinear 1;
        div(phi,kt) Gauss limitedLinear 1;
        div(phi,R) Gauss upwind;
        div(R) Gauss linear;
        div((nuEff*dev(grad(U).T()))) Gauss linear;
	div((nuEff*dev2(T(grad(U))))) Gauss linear;
        div(phi,v2) bounded Gauss linearUpwind grad(v2);
        div(phi,f) bounded Gauss linearUpwind grad(f);
    }

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

    laplacianSchemes
    {
        default Gauss linear limited 0.333;
    }

    snGradSchemes
    {
        default limited 0.333;
    }

    fluxRequired
    {
        default no;
        p ;
    }

fvSolution

Code:

/*--------------------------------*- C++ -*----------------------------------*\
|       o          |                                                          |
|    o     o       | HELYX-OS                                                  |
|   o   O   o      | Version: v2.3.1                                           |
|    o     o       | Web:     http://www.engys.com                            |
|       o          |                                                          |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version 2.0;
    format ascii;
    class dictionary;
    location system;
    object fvSolution;
}

    PISO
    {
        nCorrectors 1;
		nOuterCorrectors 1;
        nNonOrthogonalCorrectors 1;
		nOuterCorrectors 1;
    }


    solvers
    {
        p
        {
            solver GAMG;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.001;
            smoother GaussSeidel;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }
        U
        {
            solver GAMG;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.001;
            smoother GaussSeidel;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }
		
       UFinal
        {
            solver GAMG;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.001;
            smoother GaussSeidel;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }
		
		 pFinal
        {
            solver GAMG;
            smoother GaussSeidel;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.001;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }
		
		
        p_rgh
        {
            solver GAMG;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-10;
            relTol 0.01;
            smoother GaussSeidel;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }

        f
        {
            solver GAMG;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-10;
            relTol 0.01;
            smoother GaussSeidel;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }



        p_rghFinal
        {
            solver GAMG;
            smoother GaussSeidel;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.0001;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }

        fFinal
        {
            solver GAMG;
            smoother GaussSeidel;
            agglomerator faceAreaPair;
            mergeLevels 1;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 200;
            tolerance 1e-6;
            relTol 0.0001;
            nPreSweeps 0;
            nPostSweeps 2;
            nFinestSweeps 2;
            minIter 1;
        }



        k
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        kl
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        kt
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        q
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        zeta
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        epsilon
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        R
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        nuTilda
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        omega
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        h
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        T
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        v2
        {
            solver smoothSolver;
            smoother GaussSeidel;
            tolerance 1e-6;
            relTol 0;
            minIter 1;
        }

        rho
        {
            solver PCG;
            preconditioner DIC;
            tolerance 0;
            relTol 0;
            minIter 1;
        }

        rhoFinal
        {
            solver PCG;
            preconditioner DIC;
            tolerance 0;
            relTol 0;
            minIter 1;
        }

        e
        {
            solver PBiCG;
            preconditioner DILU;
            tolerance 1e-06;
            relTol 0;
            minIter 1;
        }

    }

    relaxationFactors
    {
        fields
        {
            p 1;
            p_rgh 1;
            rho 1;
        }

        equations
        {
            epsilon 1;
            f 1;
            h 1;
            k 1;
            kl 1;
            kt 1;
            nuTilda 1;
            omega 1;
            q 1;
            R 1;
            T 1;
            U 0.3;
            v2 1;
            zeta 1;
            "alpha.*" 1;
            epsilonFinal 1;
            fFinal 1;
            hFinal 1;
            kFinal 1;
            klFinal 1;
            ktFinal 1;
            nuTildaFinal 1;
            omegaFinal 1;
            qFinal 1;
            RFinal 1;
            TFinal 1;
            UFinal 1;
            v2Final 1;
            zetaFinal 1;
            "alpha.*Final" 1;
        }

    }

andrenel · May 24, 2023, 15:00

I had the same problem. I finally figured out that it might be the numerical scheme might be the problem.

So I outlined the problem to chatGPT4 and asked it to write a fvScheme. It did and I copied the text into the fvScheme. Worked. I am using icoFoam.

Below is the fvShemes entry that the AI provided:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}

ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
limited cellLimited Gauss linear 1;
}

divSchemes
{
default none;
div(phi,U) Gauss linearUpwind grad(U);
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(phi,omega) Gauss linearUpwind grad(omega);
div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p ;
}

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

September 23, 2016, 10:01	icoFoam Courant number growth problem	#1
tdof Member Join Date: Jun 2016 Posts: 31 Rep Power: 10	Hello, I'm new to OpenFOAM 4.0 and only beginning to explore the solver. I want to run a laminar pipe flow case with either icoFoam or pisoFoam, but I've run into some issues. The pipe is 0.1m in diameter and 0.5m in length in the positive y-direction, the fluid is an oil with eta=0.1 Pa*s and rho=900kg/m³. The smallest tetra-element is about 1mm and with an expected u_max of 0.2m/s (inflow u_mean=0.1m/s), the smallest time step shouldn't exceed 0.005s for a Co-number of 1. I know that this issue is a rather common one while getting to know the solver and CFD in general, but I can't seem to find the root of it in my specific case. I've attached the necessary files. I tried a wide range of time steps, but the Co-number just keeps growing, so I suspect the fv-settings (taken from the icoFoam cavity tutorial) or rather my model setup to be the cause. I also tried to get it to run with pisoFoam, but I didn't know what to write in the turbulenceProperties file after setting the turbulenceModel to laminar. The boundary conditions for inflow and outflow patches don't seem to be overconstrained, so I don't know what to change there apart from setting the fixed inflow velocity to a mean mass flux, but the keyword for the mass flux doesn't seem to be described in the documentation, although I found some mentionings in older versions of OF via Google but not for recent ones. Also, how do I know which options to set in fvSchemes ? Especially which types of keywords I need in ddt, d2dt2, grad, div, laplacianSchemes - for examples, when do I need div(phi,U), when do I need more settings and how to choose them? I'd appreciate any help.

June 21, 2017, 01:20		#9
piu58 Senior Member Uwe Pilz Join Date: Feb 2017 Location: Leipzig, Germany Posts: 744 Rep Power: 15	High pressure gradient lead to high local velocity. It is quite normal that the max Co number increases then. I recommend refining the mesh in the areas with the pressure drop or increase. Sugajen likes this. __________________ Uwe Pilz -- Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)

June 23, 2017, 01:21		#11
piu58 Senior Member Uwe Pilz Join Date: Feb 2017 Location: Leipzig, Germany Posts: 744 Rep Power: 15	> As you suggested I refined the mesh but it didn't make much of a difference If you want to control the Co number you need to refine the mesh only in the areas of fast changes and high velocity (areas where the high Co occurs). This way you minimize the required wall time for a simulation. Or, in other words , you may use a coarser mesh in areas with low CO number. __________________ Uwe Pilz -- Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)

May 24, 2023, 15:00	Courant Number and Residual Exponential Growth icoFoam	#13
andrenel New Member Andre Nel Join Date: Sep 2022 Location: Skippack PA Posts: 2 Rep Power: 0	I had the same problem. I finally figured out that it might be the numerical scheme might be the problem. So I outlined the problem to chatGPT4 and asked it to write a fvScheme. It did and I copied the text into the fvScheme. Worked. I am using icoFoam. Below is the fvShemes entry that the AI provided: /--------------------------------- C++ -----------------------------------\ \| ========= \| \| \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \| \| \\ / O peration \| Version: v2012 \| \| \\ / A nd \| Website: www.openfoam.com \| \| \\/ M anipulation \| \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } ddtSchemes { default Euler; } gradSchemes { default Gauss linear; limited cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss linearUpwind grad(U); 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(phi,omega) Gauss linearUpwind grad(omega); div((nuEffdev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } // *********************************************** ********************* //

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Other] Can't Shake Erros: patch type 'patch' not constraint type 'empty'	BrendaEM	OpenFOAM Meshing & Mesh Conversion	12	April 3, 2022 19:32
SigFpe when running ANY application in parallel	Pj.	OpenFOAM Running, Solving & CFD	3	April 23, 2015 15:53
decomposePar pointfield	flying	OpenFOAM Running, Solving & CFD	28	December 30, 2013 16:05
same geometry,structured and unstructured mesh,different behaviour.	sharonyue	OpenFOAM Running, Solving & CFD	13	January 2, 2013 23:40
IcoFoam parallel woes	msrinath80	OpenFOAM Running, Solving & CFD	9	July 22, 2007 03:58

September 23, 2016, 14:01		#2
anishtain4 Senior Member Mahdi Hosseinali Join Date: Apr 2009 Location: NB, Canada Posts: 273 Rep Power: 18	Hi, 1. I couldn't find any attached file. 2. If your turbulence model is laminar then you don't need any options there. 3. When using standard solvers which have been used extensively, usually the reason for divergence is the boundary conditions, can you share them with us? 4. If you are trying to use periodic boundary condition with pressure mass flux, try checking $FOAM_TUTORIALS/incompressible/pimpleFoam/LES/channel395 5. For those options I'd suggest to read user manual which gives you a good understanding what every choice will do. To make sure if you need it or not, you can comment it and if OF complains about not finding it you know it's needed, also you can write banana for the options, OF tells you he doesn't know banana, but here's your available keywords.

September 27, 2016, 17:51		#4
tdof Member Join Date: Jun 2016 Posts: 31 Rep Power: 10	Alright, I revised my BCs and found that the inflow direction was off. My workstation ran into some trouble and I had lost track of my models. The inflow direction is in negative y direction, but it somehow did not change anything. I got pisoFoam to run, but the Courant-number just keeps growing, even with adjustTimeStep activated! And no matter the step size using icoFoam, it's the same. I checked a few setup videos like this one: https://www.youtube.com/watch?v=zDFk0GCZG68 and didn't find any obvious differences concerning the BC setup. Here: http://www.cfd-online.com/Forums/ope...flow-pipe.html is some more input, but no improvement either. I noticed that Hypermesh did not create physicalType keywords in the boundary file, but adding them did'nt change anything. I could really use some advice as I don't know what to look for anymore. p dimensions [0 2 -2 0 0 0 0]; internalField uniform 0; boundaryField { inflow { type zeroGradient; } wall { type zeroGradient; } outflow { type fixedValue; value uniform 0; } } U dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { inflow { type fixedValue; value uniform (0 -0.1 0); } wall { type fixedValue; value uniform (0 0 0); } outflow { type zeroGradient; } } transportProperties transportModel Newtonian; nu [0 2 -1 0 0 0 0] 0.1; controlDict application pisoFoam; startFrom startTime; startTime 0.000; stopAt endTime; endTime 0.1; deltaT 0.00025; writeControl timeStep; writeInterval 80; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 0.8; fvSchemes ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; div((nuEffdev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear orthogonal; } interpolationSchemes { default linear; } snGradSchemes { default orthogonal; } fvSolution* solvers { p { solver PCG; preconditioner DIC; tolerance 1e-4; relTol 0; } pFinal { $p; relTol 0; } U { solver PBiCG; preconditioner DILU; tolerance 1e-5; relTol 0; } } PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; } turbulenceProperties simulationType laminar;

September 28, 2016, 09:27		#5
tdof Member Join Date: Jun 2016 Posts: 31 Rep Power: 10	I succeeded by taking the pipe flow tutorial from FOAMHouse and replacing the mesh with my own one (see http://the-foam-house5.webnode.es/pr...ide-foamcases/). The mesh consists now of 25mm tetras without boundary layer, so it's very rough. deltaT is set to 0.0005s and it runs smoothly, maxCo is 0.021 at the end of the simulation. However, if I set deltaT to 0.005s, Co explodes instantly. How come!? The Courant number should be around 10 times the previous Co, so what is happening there?

September 28, 2016, 13:41		#6
anishtain4 Senior Member Mahdi Hosseinali Join Date: Apr 2009 Location: NB, Canada Posts: 273 Rep Power: 18	Hi, The best way to share your case is to remove all the time directories and constant/polyMesh if you have blockMeshDict so others can download it and run it. I'm glad you got somewhere, try changing your gradSchemes from "linear" to "limitedLinear 1"

September 28, 2016, 15:17		#7
tdof Member Join Date: Jun 2016 Posts: 31 Rep Power: 10	Hi, I use Hypermesh, so no blockMeshDict available. I got some advice in the meantime, my choices in fvSchemes and fvSolution weren't all that great in general. I was just so focused on the BCs that I did not look there more than I thought to be necessary.