[stockzahn]

Dear all,

using e.g. the simpleFoam solver I was able to save the residuals and display their evolution during solving by including "#includefunc residuals" in the subdictionary "functions" of the controlDict. However, if I do that with chtMultiRegionFoam, no "postProcessing" folder is created and no residuals are saved.

I also tried to include a function object based on the information here (https://www.openfoam.com/documentati...ieldValue.html) reading several threads here (according to which this should be possible, but they are quite old though). I tried to keep it simple for the first trials:

T0
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
log true;
writeControl writeTime;
writeFields true;
regionType all;
name titanium; //name of the solid region
operation none;
fields ( T );
}

In my understanding this function object should just copy the temperature field and name it "T0". Like with the residuals, there is no output, no error message, no info at all. However, could you tell where my mistake is or if this is not possible in chtMultiRegionFoam ?

Thanks in advance,
stockzahn

[kera]

Hallo stockzahn,

there is a discussion here on how to capture the field residuals for cht solvers. I still do it the old fashioned way by using PyFOAM.

As for your second try with functionObject.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                               |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     chtMultiRegionSimpleFoam;

startFrom       latestTime;

startTime       0;
.
.
.

runTimeModifiable true;


functions
{
    minMax
    {
        type            fieldMinMax;
        functionObjectLibs ("libfieldFunctionObjects.so");
        enabled         true;
        log             false;
        write           true;
        region          air;   // Specify the region
        fields
        (
          T
        );
    }
}

hope this helps!

Regards,
Ricky

PS: I am still using OF-2.3.x, OpenFOAM has come a long way since then.

Originally Posted by stockzahn

Dear all,

using e.g. the simpleFoam solver I was able to save the residuals and display their evolution during solving by including "#includefunc residuals" in the subdictionary "functions" of the controlDict. However, if I do that with chtMultiRegionFoam, no "postProcessing" folder is created and no residuals are saved.

I also tried to include a function object based on the information here (https://www.openfoam.com/documentati...ieldValue.html) reading several threads here (according to which this should be possible, but they are quite old though). I tried to keep it simple for the first trials:

T0
{
type volFieldValue;
libs ("libfieldFunctionObjects.so");
log true;
writeControl writeTime;
writeFields true;
regionType all;
name titanium; //name of the solid region
operation none;
fields ( T );
}

In my understanding this function object should just copy the temperature field and name it "T0". Like with the residuals, there is no output, no error message, no info at all. However, could you tell where my mistake is or if this is not possible in chtMultiRegionFoam ?

Thanks in advance,
stockzahn

[stockzahn]

Thanks Ricky for your help. That's my status:

I tried it with

#includeEtc "caseDicts/postProcessing/numerical/residuals.cfg"

, but this only produced an error message:

--> FOAM FATAL ERROR:
 Cannot open etc file "caseDicts/postProcessing/numerical/residuals.cfg" while reading dictionary "/home/run/InTrCoilQ1/system/controlDict.functions.residualsTitanium"

From function static bool Foam::functionEntries::includeEtcEntry::execute(Foam::dictionary&, Foam::Istream&) in file db/dictionary/functionEntries/includeEtcEntry/includeEtcEntry.C at line 127.

 FOAM exiting

However, I then just copied the lines of "residuals.cfg" into the function subdictionary of the controlDict and it started to work. Key was to insert the lines

writeControl    timeStep;
 writeInterval    1;

also for the function object "T0". The functions of my controlDict now look like this:

functions
{
    residualsTitanium
    {
    type     residuals;
    libs    ("libutilityFunctionObjects.so");
    writeControl    timeStep;
    writeInterval   1;
    regionType      all;
    region titanium;
    fields (T);
    }

    sumT0
    {
    type        volFieldValue;
    libs        ("libfieldFunctionObjects.so"); 
    writeControl    timeStep;    
    writeInterval   1;
     //writeFields          true;
    //regionType      all;
    region         titanium;
     operation    sum;

    fields        (T);
    }
}

for the "sumT0" it works perfectly, but unfortunately in the residuals.dat file in the postProcessing folder displays "N/A" instead of the residuals.



Do you have or does anybody has an idea how to save the residual values in the .dat-file?

[oswald]

You should monitor "h", not T, as chtMultiRegionFoam solves for h.

[stockzahn]

Thanks! So obvious, that wasn't very glorious of me ...