[sk11]

Dear FOAMers,
I need a help regarding how to find the pressure across internal faces.
For example, I have a 2D channel flow and a porous block in the flow. how can I find the pressure drop caused by the porous media? (Using functions) Inlet and outlet of the porous media are internal faces. I found there is "pressureDifferencePatch" to find the pressure between two patches. But is there any way I can find the pressure between these internal faces (Since it can not be considered as boundary patches?)
I strongly believe there is some way to get this pressure drop, but I could not find a relevant thread.
Thank you for the help.
Regards,
Sarath

[sk11]

I found a way by using singleGraph function. By plotting the pressure in two different planes. But I had to write a script to do it for two planes and get the pressure drop. I wonder how "pressureDifferenceSurface" works! It can be more easy than this way.

Kind regards,
Sarath

[tomf]

Hi,

I had to do something similar recently. The following works in version 1712:

    deltaTotalPressure_inOutlet
    {
        type            fieldValueDelta;
        libs ("libfieldFunctionObjects.so");
        operation       subtract;

        region1
        {
            type            surfaceFieldValue;
            libs            ("libfieldFunctionObjects.so");
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            inlet;
            operation       areaIntegrate;
            fields          ( p );
        }

        region2
        {
            type            surfaceFieldValue;
            libs            ("libfieldFunctionObjects.so");
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            outlet;
            operation       areaIntegrate;
            fields          ( p );
        }
    }

Regards,
Tom

[jtipton2]

Thanks tomf for your function!

Note that, if you want pressure drop, you should use operation areaAverage. As the code snippet is currently set, operation areaIntegrate will calculate the net force caused by pressure on the patch.

[jtipton2]

Just for the sake of posterity... the original poster was asking how to calculate the pressure drop between internal faces that weren't boundary patches. This can be accomplished with a file as follows:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      sample1;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

        type            fieldValueDelta;
        libs ("libfieldFunctionObjects.so");
        operation       subtract;

        region1
        {
            type            surfaceFieldValue;
            libs            ("libfieldFunctionObjects.so");
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      sampledSurface;
            name            plane300mm;
            sampledSurfaceDict
            {
                type            plane;
                source          cells;
                planeType       pointAndNormal;
                pointAndNormalDict
                {
                        point   (0.3 0.025 0);
                        normal  (0.3 0 0);
                }
            }
            operation       areaAverage;
            fields          ( p );
        }

        region2
        {
            type            surfaceFieldValue;
            libs            ("libfieldFunctionObjects.so");
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      sampledSurface;
            name            plane600mm;
            sampledSurfaceDict
            {
                type            plane;
                source          cells;
                planeType       pointAndNormal;
                pointAndNormalDict
                {
                        point   (0.6 0.025 0);
                        normal  (0.6 0 0);
                }
            }
            operation       areaAverage;
            fields          ( p );
        }



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

The file can then be run using as a postProcess via something akin to:

rhoSimpleFoam -postProcess -func sample1 -latestTime

[Selinus]

Hi jtipton2,
what about if I would like to use this method to compute average properties value on a circle surface?



Thanks for your help

[Alexee]

Originally Posted by Selinus

Hi jtipton2,
what about if I would like to use this method to compute average properties value on a circle surface?



Thanks for your help

I think in case of arbitrary surface you'd need to create a faceZone with topoSet and use

source faceZone;

[CFDanielGER]

Hello everybody,


did something change for the fieldValueDelta function? Because I want to run this code with OpenFOAM v2112 and it gives me following error:

--> FOAM FATAL IO ERROR: (openfoam-2112)
Entry 'type' not found in dictionary "functions.pressureDrop"


file: functions.pressureDrop at line 22 to 49.

    From bool Foam::dictionary::readEntry(const Foam::word&, T&, Foam::keyType::option, bool) const [with T = Foam::word]
    in file lnInclude/dictionaryTemplates.C at line 322.

FOAM exiting

Does anyone know what should be changed or is there another way of calculating the pressure drop between two surfaces?


Many thanks for your help and best regards,
Daniel

[tomf]

For future reference:

multiFieldValue is the name from v2112 onwards.

Cheers,
Tom