[alexeym]

Here are my results: http://matveichev.blogspot.fr/2014/0...ex-street.html

[Maimouna]

Dear Alexey,

many thanks for your post.

All the best

[Maimouna]

Dear Alexey,

I have one question please,

what's your accurate result in terms of strouhal number?

[alexeym]

You're joking, right?

[Maimouna]

Sorry for that might be silly question, just I would like to know if you checked your convergence in terms of Strouhal number?

[774024952]

hi, Maimouna, I'm new with CFD. And I have a question. What's the meaning of Aref and lRef? And how can I calculate them?
Thanks a lot.

[774024952]

I've found the explain of the Aref and lRef, thanks.

[Maimouna]

Hi. Sorry for late reply. Any question you welcome.

Best wishes

[Maimouna]

Dear Alexey,

did you try free vibration of cylinder in flow in your case about flow past a circular cylinder?

I'm doing that now, but I couldn't fix my problem yet. If you try it, I need your help please.

Many thanks in advanced.

[Shuai_W]

Dear Maimouna, I want to simulate the flow around cylinder, and I do it followed step by step. I use openfoam 2.3.0 and the attached case, I excute it via "./Allprepare".however, when I excute "pimpleFoam",there is an error:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.3.0-f5222ca19ce6
Exec : pimpleFoam
Date : May 08 2014
Time : 13:07:57
Host : "wangshuai-Lenovo-B460"
PID : 6522
Case : /home/wangshuai/OpenFOAM/wangshuai-2.3.0/run/tutorials/incompressible/pimpleFoam/coarse
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



--> FOAM FATAL IO ERROR:
keyword startFace is undefined in dictionary ".defaultFaces"

file: .defaultFaces from line 71 to line 71.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 437.

FOAM exiting

I cannot handle with it, could you help me? Thanks.

[Maimouna]

Dear Shuai,

have you tried my one (attached case). Try that case please, if any problem let me know please.

Regards

[Shuai_W]

Dear Maimouna, I tried the attached case yesterday. Everything is Ok when I typed “./Allprepare” in my terminal. After that, when I typed “pimpleFoam” in my terminal, error appeared like:

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

Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian

Selecting turbulence model type laminar

No finite volume options present

PIMPLE: max iterations = 100

field "(U|p)" : relTol 0, tolerance 0.01

Starting time loop

fieldAverage fieldAverage1:

Starting averaging at time 0

Courant Number mean: 0.0153542679232 max: 0.074259625164

deltaT = 0.00119904076739

Time = 0.00119904076739

PIMPLE: iteration 1

DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00162921759868, No Iterations 1

DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00157520001085, No Iterations 1

--> FOAM FATAL IO ERROR:

keyword laplacian(rAUf,p) is undefined in dictionary "/home/wangshuai/OpenFOAM/wangshuai-2.3.0/run/tutorials/incompressible/pimpleFoam/circularCylinderNew/system/fvSchemes.laplacianSchemes"

file: /home/wangshuai/OpenFOAM/wangshuai-2.3.0/run/tutorials/incompressible/pimpleFoam/circularCylinderNew/system/fvSchemes.laplacianSchemes from line 37 to line 39.

From function dictionary::lookupEntry(const word&, bool, bool) const

in file db/dictionary/dictionary.C at line 437.

FOAM exiting

The error suggested that “keyword laplacian(rAUf,p) is undefined in….”, and therefore, I modified the fvSchemes.laplacianSchemes in my system file.
Before modification:

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss cubic corrected;
laplacian((1|A(U)),p) Gauss cubic corrected;
}

After modification:

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss cubic corrected;
laplacian(rAUf,p) Gauss cubic corrected;
laplacian((1|A(U)),p) Gauss cubic corrected;
}

After that, when I typed “pimpleFoam” in my terminal again, it’s Ok. However, I had three questions as follow:

1. What is the function of changeDictionary? I am very confused with this dictionary.

2. Should it will affect the results when I add “laplacian(rAUf,p) Gauss cubic corrected;” in laplacianSchemes?

3. In your case, I find something like “U~” or “P~”, what does the “~” mean?

My results are in the below (attached case). Thank you for your help.

[Maimouna]

Dear Shuai,

that is good news that case working in your OpenFOAM version 2.3.0. Regarding your questions

1. What is the function of changeDictionary? I am very confused with this dictionary.

To get more clarification about change[/QUOTE]Dictionary function look at
http://www.cfd-online.com/Forums/openfoam-pre-processing/101179-how-do-i-use-changedictionary-utility.html

2. Should it will affect the results when I add “laplacian(rAUf,p) Gauss cubic corrected;” in laplacianSchemes?

When you get through the previous link you can get more idea.

3. In your case, I find something like “U~” or “P~”, what does the “~” mean?

I don't know what that two files mean, but I think they are not affected your result.

All the best.

[Maimouna]

Dear Shuai,

recently, I'm using OpenFOAM-2.3.0 because I updated my ubuntu 13.10 to 14.04, which I don't really like. OpenFOAM version that only accompanied with that ubuntu version is 2.3.0. Any way, I tried to work with previous case about circular cylinder that I sent you in the previous post #91, but unfortunately it was gave me the same error that you posted in #92. I solved that problem. It started working and then it stopped by that error

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const at ??:?
#4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const at ??:?
#5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
#7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#8  
 at ??:?
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 at ??:?
Floating point exception (core dumped)

What does that mean? Any Idea please?

Regards

[Shuai_W]

Dear Maimouna:
Did you solve the problem in #93? I am so sorry to say that I have not encountered with that problem, but I think it may be ralated to your OpenFOAM. When you upgrade the version of Ubuntu, and it may have an influence on your OpenFOAM. I used Ubuntu 12.04,and it works well.
I hope you will solve it soon!

[Mehrez]

Hi dear sasanghomi,

Thank you for this interesting reply. However I have 2 main questions in order to understand the changes you have apported to the default icoFoam fvSchemes file:
1- When you switch from: "ddtSchemes { default Euler;" to: "ddtSchemes { default backward;", does the effect on the fluid is that I have less damping ?
2- What does the other modifications (like "limited 0.5") do exactly or how they affect the solution ?
Thank you in advance,

Best regards,

Mehrez

Originally Posted by sasanghomi

Hi ,
I think you use icoFoam as a solver. So I think two parameters have vital role for getting the exact result : 1) discretization method of terms in equations 2)Mesh generation.
So change your fvSchemes and fvSolution as below :

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0;
    };

    U
    {
        solver         BiCG;
        preconditioner   DILU;
        tolerance        1e-05;
        relTol           0;
    };
}


PISO
{
   nCorrectors    2;
   nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
 }

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default backward;
}

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

divSchemes
{
    default         none;
    div(phi,U)      Gauss GammaV 0.5 ;

}

laplacianSchemes
{
    default         Gauss linear limited 0.5;
    laplacian(nu,U) Gauss linear limited 0.5;
    laplacian(rUA,pcorr) Gauss linear limited 0.5;
    laplacian(rAU,p) Gauss linear limited 0.5;
}

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

snGradSchemes
{
    default         limited 0.5;
}

fluxRequired
{
    default         no;
    pcorr;
    p;
}

Hope this helps,
Sasan.

[stephie]

Hello everyone,

at the moment I try to solve a tutorial for channel flow with respect to different LES models which was uploaded for a cours at Chalmers University of technology in 2001. After creating the mesh I wanted to refine the Mesh. I run topoSet. After, I should type in the command : refineMesh -dict -overwrite. And here is the first mistake:

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

Create polyMesh for time = 0

Mesh edge statistics:
x aligned : number:16376 minLen:0.005 maxLen:0.005
y aligned : number:16056 minLen:0.005 maxLen:0.005
z aligned : number:8232 minLen:0.005 maxLen:0.005
other : number:0 minLen:1e+15 maxLen:-1e+15

Refining according to refineMeshDict



--> FOAM FATAL IO ERROR:
cannot open file

file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/-overwrite at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 87.

FOAM exiting

It didn't work. When I typed in <refineMesh> it was okay. Why does this command don't work?

The next step should be to run the simulation by <pyFoamPlotRunner.py pimpleFoam >& log and it also do not work.
There is still the mistake: pyFoamPlotRunner command not found

I had a look in a lot of discussions, but I couldn't find an answer.. because pyFoam is alreay installed.

So i tried to type in <pimpleFoam> to start the simulation and here ist the next mistake:

--> FOAM FATAL IO ERROR: keyword laplacian(rAUf,p) is undefined in dictionary "/home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes" file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes from line 45 to line 51. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 437. FOAM exiting

I would be grateful if anyone might help me to solve this tutorial.

Thank you so much, nice regards,

Stephie

[Mehrez]

Hi dear Stephie,
After refining the mesh you should interpolate your fields (U, p... for example) from the old mesh to the new fine mesh. Then, you can start your simulation.
There is a function in OpenFoam to perform interpolation.
Regards,

Mhrz

Originally Posted by stephie

Hello everyone,

at the moment I try to solve a tutorial for channel flow with respect to different LES models which was uploaded for a cours at Chalmers University of technology in 2001. After creating the mesh I wanted to refine the Mesh. I run topoSet. After, I should type in the command : refineMesh -dict -overwrite. And here is the first mistake:

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

Create polyMesh for time = 0

Mesh edge statistics:
x aligned : number:16376 minLen:0.005 maxLen:0.005
y aligned : number:16056 minLen:0.005 maxLen:0.005
z aligned : number:8232 minLen:0.005 maxLen:0.005
other : number:0 minLen:1e+15 maxLen:-1e+15

Refining according to refineMeshDict



--> FOAM FATAL IO ERROR:
cannot open file

file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/-overwrite at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 87.

FOAM exiting

It didn't work. When I typed in <refineMesh> it was okay. Why does this command don't work?

The next step should be to run the simulation by <pyFoamPlotRunner.py pimpleFoam >& log and it also do not work.
There is still the mistake: pyFoamPlotRunner command not found

I had a look in a lot of discussions, but I couldn't find an answer.. because pyFoam is alreay installed.

So i tried to type in <pimpleFoam> to start the simulation and here ist the next mistake:

--> FOAM FATAL IO ERROR: keyword laplacian(rAUf,p) is undefined in dictionary "/home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes" file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes from line 45 to line 51. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 437. FOAM exiting

I would be grateful if anyone might help me to solve this tutorial.

Thank you so much, nice regards,

Stephie

[alexeym]

Hi,

Originally Posted by stephie

After, I should type in the command : refineMesh -dict -overwrite. And here is the first mistake:
...
--> FOAM FATAL IO ERROR:
cannot open file

file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/-overwrite at line 0.

The command in fact should be

refineMesh -dict system/refineMeshDict -overwrite

Guess this is again due to OpenFOAM's version incompatibility.

So i tried to type in <pimpleFoam> to start the simulation and here ist the next mistake:

--> FOAM FATAL IO ERROR: keyword laplacian(rAUf,p) is undefined in dictionary "/home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes" file: /home/stephanie/OpenFOAM/stephanie-2.3.1/run/smagorinsky_mini/system/fvSchemes.laplacianSchemes from line 45 to line 51. From function dictionary::lookupEntry(const word&, bool, bool) const in file db/dictionary/dictionary.C at line 437. FOAM exiting

And this again is due to modification in 2.3.1. You have this line in fvSchemes:

laplacian((1|A(U)),p) Gauss linear corrected;

now it should be written as

laplacian(rAUf,p)  Gauss linear corrected;

And finally about pyFoamPlotRunner error, it is not pyFoamPlotRunner, it is pyFoamPlotRunner.py.

[stephie]

Good morning Alexey,

you are amazing - thank you so much. After typing in the correct command to refine the Mesh it worked. Now it looks like the image in the description

Also the second hint was right, I changed this line in fvSchemes and the simulation run.
The only thing, which did not work is pyFoamPlotRunner.py. There is still the mistake command not found. Maybe I miss something when I installed OpenFoam...do you have any idea?
But it doesn't matter... I'm happy, the simulation run.

Thank you so much for your help