CFD Online Discussion Forums - [waves2Foam] IO error when running waveIsoFoam with OF1812: Dictionary entry not found

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Community Contributions (https://www.cfd-online.com/Forums/openfoam-community-contributions/)

- - [waves2Foam] IO error when running waveIsoFoam with OF1812: Dictionary entry not found (https://www.cfd-online.com/Forums/openfoam-community-contributions/225271-io-error-when-running-waveisofoam-of1812-dictionary-entry-not-found.html)

IO error when running waveIsoFoam with OF1812: Dictionary entry not found

Hi all,

I am currently trying to run waveIsoFoam, one of the new solver from waves2Foam, with OF1812. However, when I tested a case that I have successfully run with waveFoam on OF1712, I got the following error message:

Code:

[31] --> FOAM FATAL IO ERROR: 

[31] Dictionary entry for patch inlet not found

[31] 

[31] file: IOstream

[31] 

[31]     From function static Foam::autoPtr<Foam::waveModel> Foam::waveModel::New(const Foam::word&, const Foam::fvMesh&, const Foam::polyPatch&)

[31]     in file waveModel/waveModelNew.C at line 58.

Some times it would include a path in the error

Code:

[0] --> FOAM FATAL IO ERROR: 

[0] Dictionary entry for patch inlet not found

[0] 

[0] file: /vortexfs1/scratch/jinshichen/waveFlume_rand_kostab_topo_parallel_iso_run/processor0/constant/waveProperties

[0] 

[0]     From function static Foam::autoPtr<Foam::waveModel> Foam::waveModel::New(const Foam::word&, const Foam::fvMesh&, const Foam::polyPatch&)

[0]     in file waveModel/waveModelNew.C at line 58.

However, I do include the inlet properties in the waveProperties file, which is shown below:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  v1712                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version        2.0;

    format        ascii;

    class        dictionary;

    object        waveProperties;

}

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



seaLevel            4.5;

seaLevelAsReference true;



relaxationNames     ( inlet outlet );



initializationName  outlet;



inletCoeffs

{

    waveType            irregular;

    N                   50;       //Number of sampling frequencies

    Tsoft               30;        //Ramp time



    // Define the phases

    phaseMethod         randomPhase;



    // Define the spectrum

    spectrum            JONSWAP; 

    Hs                  0.8;      // Significant wave height

    Tp                  7;        // Peak wave period   

    gamma               3.3;      // Peak enhancement factor

    depth               4.5;      // Water depth

    direction           (1 0 0);

    

    frequencyAxis

    {

       discretisation       equidistantFrequencyAxis;



       lowerFrequencyCutoff 0.1;

       upperFrequencyCutoff 0.3;



       writeSpectrum        false;

    }



    relaxationZone

    {

        relaxationScheme    Spatial;

        relaxationShape     Rectangular;

        beachType           Empty;

        relaxType           INLET;

        startX              ( 0 0 0 );

        endX                ( 30 1 0 );

        orientation         ( 1 0 0 );

    }

}



outletCoeffs

{

    waveType            potentialCurrent;

    U                   ( 0 0 0 );

    Tsoft               2;



    relaxationZone

    {

        relaxationScheme    Spatial;

        relaxationShape     Rectangular;

        beachType           Empty;

        relaxType           OUTLET;

        startX              ( 350.907 0 0 );

        endX                ( 370.907 1 0 );

        orientation         ( 1 0 0 );

    }

}







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

Thus, I am wondering what is wrong with this code. Since I have successfully run the identical case with wavefoam solver on OF1712, I am wondering that whether there are some required syntax change when converting this to waveIsoFoam and OF1812? (I have changed the setting for isosurface part in the fvSolution, but I didn't change the rest).

My controlDict looks like the following:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  1.5                                   |

|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    object      controlDict;

}

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



application     interFoam;



startFrom       startTime;



startTime       0;



stopAt          endTime;



endTime         10;



deltaT          0.001;



writeControl    adjustableRunTime;



writeInterval   0.05;



purgeWrite      6;



writeFormat     ascii;



writePrecision  6;



writeCompression uncompressed;



timeFormat      general;



timePrecision   6;



runTimeModifiable yes;



adjustTimeStep  yes;



maxCo           0.05;



maxAlphaCo      0.25;



maxDeltaT       1;







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

Thank you in advance for all of your input on this!

Hi all,

I have found a temporary fix: If you delete the "waveModel" library from EXE_LIB list in file "/waves2Foam/applications/solvers/solvers1812_PLUS/waveIsoFoam/Make/options" and recompile it, it should fix the problem. However I am still looking for a more thorough solution.

Thank you!

Best,
Jinshi

Hi Jinshi,

Thank you for reporting the bug. I have removed waveModels in Make/options and updated the repository. It is indeed a bug, because waveModels relate to the OpenFoam-ESI wave models and not waves2Foam.

Kind regards

Niels

‘g’ was not declared in this scope

Quote:

Originally Posted by JinshiC (Post 762489)

Hello Jinshi
I try to combine interfoam and wavefoam in OF1812, but i got error when i wmake for new solver as:
/home/leqt/OpenFOAM/leqt-v1812/applications/utilities/waves2Foam/src/waves2Foam/lnInclude/readWaveProperties.H:27:38: error: ‘g’ was not declared in this scope
referencePoint.value() = g.value()/Foam::mag(g.value());
^

Could you tell me how to fix it, please.
Many thanks

Hi Le,

I am not entirely sure what you did, and I didn't make a new solver my own (just using Niels' waveIsoFoam solver). However, it does seem to me that you have missed defining g (gravitational acceleration) somewhere in your model but have included it in the back end equation. I'd personally like to refer your question to other people who are more experienced that me.

Thank you!

Best,
Jinshi

Quote:

Originally Posted by JinshiC (Post 762489)

Perhaps a silly question.. But can you elaborate on how to peform the recompilation? I don't really know where to start...

Hello everyone, I am using the OF2012 and I am facing the same problem as you. Do you know if the solution is the same as what you did for your OF version?
Did anyone face this problem with the OF2012?

Thank you in advance.

Quote:

Originally Posted by ngj (Post 762578)

Hi Niels,

First of all I would like to thank you for you great work with waves2Foam.

I guess you were talking about /solvers1812_PLUS/. I have realized that in the next version solvers (2012, 2106 and 2206) the "wave model" library is still in the options file. I was having the same error " Dictionary entry for patch inlet not found". Once I recompile without it, there is no error.

It is still a bug or am I missing something?

Kind regards,

Manuel

Quote:

Originally Posted by MFS (Post 856387)

Hi Seoane,

Could you elaborate the recompile process after you deleted the wavemodel library please? Thank you.

Hi Zhang,

Once I deleted the file, I just executed "wmake" command in ~/waves2Foam/applications/solvers/solvers2206_PLUS/my_new_solver/

I followed the instructions given in the waves2Foam manual.

I don't know if I have already solve your doubt...

Kind regards,

Manuel