[namsivag]

Hello,
I am trying to write p, T, U values at inlet while solving.
But in surfaceFieldValue.dat, I am seeing headers repeating after every timeStep or deltaT. I would like to stop the repetitive headers.

I am attaching the necessary codes / contents of the files.

I want

# Region type : patch inlet
# Faces       : 174
# Area        : 1.756255e-04
# Scale factor: 1.000000e+00
# Time            areaAverage(p)    areaAverage(T)    areaAverage(phi)    areaAverage(U)
-179.75           9.996845e+04    3.000000e+02    6.017445e-09    (2.330926e-06 -4.596611e-05 1.718942e-02)
-179.5            9.956394e+04    3.000000e+02    1.916559e-07    (-1.352449e-05 -5.353317e-04 5.285954e-01)
:
:
:

I am getting at \postProcessing\velocityInlet\-180\surfaceFieldValue.dat

# Region type : patch inlet
# Faces       : 174
# Area        : 1.756255e-04
# Scale factor: 1.000000e+00
# Time            areaAverage(p)    areaAverage(T)    areaAverage(phi)    areaAverage(U)
-179.75           9.996845e+04    3.000000e+02    6.017445e-09    (2.330926e-06 -4.596611e-05 1.718942e-02)
# Region type : patch inlet
# Faces       : 174
# Area        : 1.756255e-04
# Scale factor: 1.000000e+00
# Time            areaAverage(p)    areaAverage(T)    areaAverage(phi)    areaAverage(U)
-179.5            9.956394e+04    3.000000e+02    1.916559e-07    (-1.352449e-05 -5.353317e-04 5.285954e-01)
# Region type : patch inlet
# Faces       : 174
# Area        : 1.756255e-04
# Scale factor: 1.000000e+00
:
:
:

controlDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1912                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict.1st;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     XiEngineFoam;

startFrom       startTime;

startTime       -180;

stopAt          endTime;

endTime         -160;// 60

deltaT          0.25;

writeControl    runTime;

writeInterval   5;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  no;

maxCo           0.2;

maxDeltaT       1;

functions
{

    timeStep
    {
        name    setDeltaT;
        type    coded;
        libs    (utilityFunctionObjects);

        code
        #{
        #};

        codeExecute
        #{
            const Time& runTime = mesh().time();
            if (runTime.timeToUserTime(runTime.value()) >= -15.0)
            {
                const_cast<Time&>(runTime).setDeltaT
                (
                    runTime.userTimeToTime(0.025)
                );
            }
        #};
    }

    #include "momentum"
    #include "velocityInlet"
}

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

velocityInlet

velocityInlet
{
    // Mandatory entries (unmodifiable)    
    type            surfaceFieldValue;
    libs            (fieldFunctionObjects);
    log             true;        
    // Mandatory entries (runtime modifiable)    
    fields          (p T phi U);
    operation       areaAverage;
    regionType      patch;
    name            inlet;    
    
    // Optional (inherited) entries
    writeFields     false;    

    writeControl    timeStep;
    writeInterval   1;
    writeArea 	false;
}

[mwmalkawi]

Hi


Please have you manged to resolve it as i am having the same problem





Thanks

[tecmul]

This resolves the issue for me on OpenFoam-v2006.

Create a copy of the surfaceFieldValue function object and inside the implementation file, comment out the line

writeFileHeader(file());

Then add the same line to the constructor of the function object.

Foam::functionObjects::fieldValues::surfaceFieldValue::surfaceFieldValue
(
    const word& name,
    const Time& runTime,
    const dictionary& dict
)
:
    fieldValue(name, runTime, dict, typeName),
    regionType_(regionTypeNames_.get("regionType", dict)),
    operation_(operationTypeNames_.get("operation", dict)),
    postOperation_
    (
        postOperationTypeNames_.getOrDefault
        (
            "postOperation",
            dict,
            postOperationType::postOpNone,
            true  // Failsafe behaviour
        )
    ),
    weightFieldName_("none"),
    needsUpdate_(true),
    writeArea_(false),
    totalArea_(0),
    nFaces_(0),
    faceId_(),
    facePatchId_(),
    faceFlip_()
 {
    writeFileHeader(file());
    read(dict);
}

[olesen]

Originally Posted by tecmul

This resolves the issue for me on OpenFoam-v2006.

Create a copy of the surfaceFieldValue function object and inside the implementation file, comment out the line

writeFileHeader(file());

This is horrible. If the problem still occurs with latest maintenance branch of v2006 (currently master) please file a bug report on the issue tracker and let's get it fixed properly.
https://develop.openfoam.com/Develop...nfoam/-/issues

[tecmul]

Originally Posted by olesen

This is horrible. If the problem still occurs with latest maintenance branch of v2006 (currently master) please file a bug report on the issue tracker and let's get it fixed properly.
https://develop.openfoam.com/Develop...nfoam/-/issues

So I searched in the bug reports and came upon this.
https://develop.openfoam.com/Develop.../-/issues/1556
Apparently, this is by design in cases with a dynamic or topologically changing mesh and can be disabled with the "updateHeader" keyword, which defaults to true.

I know user-friendliness is against OpenFoam's design philosophy but it would still be nice if the surfaceFieldValue header file mentioned this.

[olesen]

Originally Posted by tecmul

So I searched in the bug reports and came upon this.
https://develop.openfoam.com/Develop.../-/issues/1556
Apparently, this is by design in cases with a dynamic or topologically changing mesh and can be disabled with the "updateHeader" keyword, which defaults to true.

I know user-friendliness is against OpenFoam's design philosophy but it would still be nice if the surfaceFieldValue header file mentioned this.

Fair enough but sometimes things do get forgotten, or are difficult to find. For these cases it would be best to flag it as an issue. Lamenting about the problem here is perfectly OK, but it increases the probability of things getting fixed if you report them. I've open this issue
https://develop.openfoam.com/Develop...am/issues/1942

[tecmul]

Originally Posted by olesen

Fair enough but sometimes things do get forgotten, or are difficult to find. For these cases it would be best to flag it as an issue.

Alright then, you have inspired me to complai...file reports on some issues I found with the rigid body dynamics library.