[CFDanielGER]

Hello everyone,


I want to calculate the pressure difference between the inlet and outlet of my domain with the following code:

      Druckdifferenz
      {
        type                      fieldValueDelta;
        functionObjectLibs         ("libfieldFunctionObjects.so");
        enabled                   true;
        writeControl            timeStep;
        writeInterval            1;
        log                        true;
        writeFields                false;
        operation                subtract;

        region1
        {
              type                    surfaceFieldValue;
              libs                    ("libfieldFunctionObjects.so");
              log                     false;
              writeControl            timeStep;
              writeFields             false;
              regionType              patch;
              name                    inlet;
              operation               areaAverage;
              fields                  ( total(p) );
              writeArea             true;
        }
        region2
        {
              type                    surfaceFieldValue;
              libs                    ("libfieldFunctionObjects.so");
              log                     false;
              writeControl            timeStep;
              writeFields             false;
              regionType              patch;
              name                    outlet;
              operation               areaAverage;
              fields                  ( total(p) );
              writeArea             true;
        }
        }

I didn't put it in the controlDict file, more precisely I have a seperate file in the system directory with some other functions I am postprocessing. I call this file with the following code:


simpleFoam -postProcess -dict "system/PostProcess_Werte" -latestTime


For older versions the code works without problems but now it gives me the following error:


--> FOAM IOWarning :
Found [v1612] 'functionObjectLibs' entry instead of 'libs' in dictionary "functions.Druckdifferenz"

This keyword is 60 months old.

--> FOAM Warning :
Unknown function type fieldValueDelta


Is someone aware of this problem and knows what I have to change?


Many thanks for your help and best regards,
Daniel

[tomf]

Hi Daniel,

They changed the name to multiFieldValue for version 2112.

The warning just means you can use libs instead of functionObjectLibs in the controlDict.

Best Regards,
Tom

[CFDanielGER]

Many thanks for your answer Tom. My complete code looks now like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2112                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      functionObject;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

functions
{
    pressureDropInletOutlet
    {
        type            multiFieldValue;
        libs             (fieldFunctionObjects);
        operation       subtract;

        region1
        {
            type            surfaceFieldValue;
            libs            (fieldFunctionObjects);
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            inlet;
            operation       areaAverage;
            fields          (total(p));
        }

        region2
        {
            type            surfaceFieldValue;
            libs            (fieldFunctionObjects);
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            outlet;
            operation       areaAverage;
            fields          (total(p));
        }
    }
}

But there is still an error:

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


file: functions.pressureDrop at line 21 to 48.

    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

Am I missing something?

[tomf]

Hi,

It is a bit weird that is says functions.pressureDrop instead of functions.pressureDropInletOutlet, so maybe the issue is in the controlDict, or the naming of the file when you issue the command? Or it is because you have the call to the functions in there? I can only guess based on the information you share.

I Hope that some of these questions help you find your issue, I do not see any obvious syntax error in the example you provide.

Cheers,
Tom

[s1291]

Originally Posted by tomf

Hi,

It is a bit weird that is says functions.pressureDrop instead of functions.pressureDropInletOutlet, so maybe the issue is in the controlDict, or the naming of the file when you issue the command? Or it is because you have the call to the functions in there? I can only guess based on the information you share.

I Hope that some of these questions help you find your issue, I do not see any obvious syntax error in the example you provide.

Cheers,
Tom

This might be irrelevant to the error above but the multiFieldValue function object requires that the regions' dictionaries be included within "another" functions dictionary.

This is the syntax according to the documentation:

multiFieldValue1
{
    // Mandatory entries
    type        multiFieldValue;
    libs        (fieldFunctionObjects);
    operation   average;

    // List of fieldValue function objects as dictionaries
    functions
    {
        region1
        {
            ...
            // Optional
            resultFields        (field1 field2);
        }
        region2
        {
            ...
            // Optional
            resultFields        (field1 field2);
        }

        ...

        regionN
        {
            ...
            // Optional
            resultFields        (field1 field2);
        }
    }
}

[CFDanielGER]

Sorry for not updating this post. I got it working. I created a file called pressureDrop in the system directory and the code looks now like this:

        type            multiFieldValue; //fieldValueDelta; multiFieldValue;
        libs             (fieldFunctionObjects);
        operation       subtract;
        
        functions
        {
        region1
        {
            type            surfaceFieldValue;
            libs            (fieldFunctionObjects);
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            inlet;
            operation       areaAverage;
            fields          (total(p));
        }

        region2
        {
            type            surfaceFieldValue;
            libs            (fieldFunctionObjects);
            log             false;
            writeControl    timeStep;
            writeFields     false;
            regionType      patch;
            name            outlet;
            operation       areaAverage;
            fields          (total(p));
        }
        }

I call it in the controlDict file by:

#includeFunc pressureDrop