[6863523]

Dear all,
I have used the commands below to calculate the volume averaged values for version 3.0.1 and it works fine for me.

functions 
(   

    functionObjects_all_volAverage
    {
        type            cellSource;
        functionObjectLibs ("libfieldFunctionObjects.so");
        enabled         true;
        outputControl   timeStep;
        outputInterval  2000;
        log             false;
        valueOutput     false;
        source          all;
        sourceName      none;
        operation       volAverage;
        fields
        (
            p
	    U
        );
    }

    probes
    {
        // Where to load it from
        functionObjectLibs ( "libsampling.so" );

        type            probes;

        // Name of the directory for probe data
        name            probes;

        // Write at same frequency as fields
        outputControl   timeStep;
        //outputInterval  1;

        // Fields to be probed
        fields
        (

            U
        );

        probeLocations
        (
            ( 0 0.5 0 )   
            ( 1 0.5 0 )


            ( 0.5 0 0 )

        );
    }

);

I know there is a difference between different versions, and I have found one at https://github.com/OpenFOAM/OpenFOAM...es/controlDict.
and modified as

functions 
{   

    cellObj1
    {
        type            volRegion;
        libs ("libfieldFunctionObjects.so");
        enabled         true;
        writeControl   timeStep;
        writeInterval  2000;
        log             false;
        writeFields     false;
        regionType      cellZone;
        name            0();
        operation       volAverage;
        fields
        (
            p
	    U
        );
    }

    probes
    {
        // Where to load it from
        libs ( "libsampling.so" );

        type            probes;

        // Name of the directory for probe data
        name            probes;

        // Write at same frequency as fields
        writeControl   timeStep;
        //outputInterval  1;

        // Fields to be probed
        fields
        (

            U
        );

        probeLocations
        (
            ( 0 0.5 0 )   
            ( 1 0.5 0 )


            ( 0.5 0 0 )

        );
    }

}

But there is always a problem for me as

[11] --> FOAM FATAL IO ERROR:
[11] wrong token type - expected word, found on line 0 the label 0
[11]
[11] file: IOstream.functions.cellObj1.name at line 0.
[11]
[11]     From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::word&)
[11]     in file primitives/strings/word/wordIO.C at line 74.
[11]
FOAM parallel run exiting
[11]

Thank you in advance.
Best Regards,
Bill

[6863523]

BTW: I have found the fieldAverage function. I wonder what is the difference between the fieldAverage and the volume average.

fieldAverage1
     {
     type fieldAverage;
     functionObjectLibs ( "libfieldFunctionObjects.so" );
     enabled true;
     outputControl outputTime;
     outputInterval  100;
     fields
     (
      U
      {
      mean on;
      prime2Mean on;
      base time;
      }

      p
      { 
      mean on;
      prime2Mean on;
      base time;
      }
      );
      }

Thank you in advance.
Any suggestion is appreciated.
Best Regards,
Bill

[Nathanael3]

Hi,

I am working with 1612+ version. Here is a minimal working example to calculate volume averaged value. I tested it over pitzdaily. I works like a charm.

functions
{
    volumeAverage
    {
        type            volFieldValue;
        libs            ("libfieldFunctionObjects.so");

        log             true;
        writeControl    writeTime;
        writeFields     true;

        regionType      all;
        operation       volAverage;

        fields
        (
            p
            U
        );
    }
}

Best regards,
Nathanaël.

[6863523]

Originally Posted by Nathanael3

Hi,

I am working with 1612+ version. Here is a minimal working example to calculate volume averaged value. I tested it over pitzdaily. I works like a charm.

functions
{
    volumeAverage
    {
        type            volFieldValue;
        libs            ("libfieldFunctionObjects.so");

        log             true;
        writeControl    writeTime;
        writeFields     true;

        regionType      all;
        operation       volAverage;

        fields
        (
            p
            U
        );
    }
}

Best regards,
Nathanaël.

Dear Nathanael,
Thank you for the reply.
I have tested the code, but got an error.

[11] --> FOAM FATAL ERROR:
[11] Unknown function type volFieldValue

Then I modified the volFieldValue to volRegion. There is no such error any more.
Thank you.
Best Regards,
Bill

[Nathanael3]

Hi,

Nice to hear that you found a solution.
The discrepancy may arise from the differences between our OpenFOAM versions.

Best regards,
Nathanaël.

[6863523]

Originally Posted by Nathanael3

Hi,

Nice to hear that you found a solution.
The discrepancy may arise from the differences between our OpenFOAM versions.

Best regards,
Nathanaël.

Dear Nathanaël,
Thank you very much for your professional reply. It is really helpful and saved me a lot of time.
I wonder if you have experience with the bash script execution to start the case running.
I have posted the problem here #13-#18
error when compile a new solver on version 4.1
Forget about the "functions" problem, because you just solved it.
Thank you for your time and kind help.
Best Regards,
Bill

[6863523]

Dear Nathanaël,
I wonder if you have any experience of calculating the volume averaged values only in a part of the domain, say, the values averaged in a 1/3 of the fluid domain?
Thank you in advance.
Best Regards,
Bill

[sitajeje]

Dear Foamers,

I cannot excute volRegion in chtMultiRegionSimpleFoam, although this functionObject works fine for pimpleDyMFoam. In the controlDict I wrote almost the same, except field "p" for pimpleDyMFoam and field "T" for chtMultiRegionSimpleFoam.

functions
{
  volRegion1
    {
        type             volRegion;
        libs               ("libfieldFunctionObjects.so");
        writeFields     true;
        regionType    cellZone;
        name            heater;
        operation       volAverage;
        fields
        (
            T
        );
    }
}

I would appreciate if anyone can help me to execute volRegion in chtMultiRegionSimpleFoam.

Thank you very much in advance!

Best regards,
sitajeje

[bineet_aero]

Originally Posted by sitajeje

Dear Foamers,

I cannot excute volRegion in chtMultiRegionSimpleFoam, although this functionObject works fine for pimpleDyMFoam. In the controlDict I wrote almost the same, except field "p" for pimpleDyMFoam and field "T" for chtMultiRegionSimpleFoam.

functions
{
  volRegion1
    {
        type             volRegion;
        libs               ("libfieldFunctionObjects.so");
        writeFields     true;
        regionType    cellZone;
        name            heater;
        operation       volAverage;
        fields
        (
            T
        );
    }
}

I would appreciate if anyone can help me to execute volRegion in chtMultiRegionSimpleFoam.

Thank you very much in advance!

Best regards,
sitajeje

Hii i am having similar problem, were you able to solve it ? thanks

[Krapf]

This is working in OpenFOAM 8:

volAverage
{
    libs              ("libfieldFunctionObjects.so");
    type            volFieldValue;
    operation      volAverage;
    region          fluid;
    fields           (T);
    writeFields    false;
}

[Rustralia]

I have the same issue. Did anyone find a solution?

Originally Posted by bineet_aero

Hii i am having similar problem, were you able to solve it ? thanks

[CarCin]

Originally Posted by Krapf

This is working in OpenFOAM 8:

volAverage
{
    libs              ("libfieldFunctionObjects.so");
    type            volFieldValue;
    operation      volAverage;
    region          fluid;
    fields           (T);
    writeFields    false;
}

Dear Krapf,

I'm trying to use the same function but it does not work for me in OpenFOAM 8.
I have added the lines you report in my controlDict, like this:

functions
{
    volAverage
    {
        libs              ("libfieldFunctionObjects.so");
        type             volFieldValue;
        operation     volAverage;
        //region        fluid;
        fields           (T);
        writeFields   false;
    }
}

and then run by typing "pimpleFoam -postProcess -func volFieldValue". The error is the following:

--> FOAM FATAL IO ERROR: 
keyword type is undefined in dictionary "controlDict/functions/volFieldValue"

file: controlDict/functions/volFieldValue from line 6 to line 15.

    From function const Foam::entry& Foam::dictionary::lookupEntry(const Foam::word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 797.

Do you have any suggestion? How do you make it work?
Thank you in advance,
Best
Carlo