[kuria]

Hey everyone!

I am new to OpenFoam and I am learning about interFoam. Currently I am trying to write the data for a new variable that can be read in Paraview.
For example: Say I want to write the rho variable data for the user defined writeInterval.
I edited the CreateFields.H file as (the part dealing with rho variable)
volScalarField rho
(
IOobject
(
"rho",
runTime.timeName(),
mesh,
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
alpha1*rho1 + alpha2*rho2
);
rho.oldTime();
// writing a new variable
rho.write();

But this doesnot seem to work, any suggestions on how to address this problem?

Thank you!

[clapointe]

I am not sure why interfoam doesn't automatically write rho, but an easy to understand work around is to define a new field, say rhoWrite, that's written automatically. Then you just need to compute/update rhoWrite with rho before the solver writes data with runTime.write(). So, add

volScalarField rhoWrite
(
    IOobject
    (
        "rhoWrite",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    alpha1*rho1 + alpha2*rho2
);

to createFields.H after alpha/rho are defined. Then add

rhoWrite = alpha1*rho1 + alpha2*rho2;

to interFoam.C before runTime.write() and recompile. Beware that I've not tested the previous suggestions, but I've done similar things in the past.

Caelan.

[kuria]

Hey Caelan

Great! That worked

Thank you

-Kurian

[ARTisticCFD]

Hii Kuria and Clapointe,

Thanks for posting the question and giving a very working answer. I was facing an issue where the scalar field variable was not written at output. Precisely, I just added a variable in a manner given in the wiki page
https://openfoamwiki.net/index.php/H...ure_to_icoFoam

I found out that the new variable is written when I specify fixedValue velocity condition but not when I change it to flowRateInletVelocity. Therefore, I suppose it might have some bug.

Quick fix: Add variable_Name.write() just before runTime.write()

[ARTisticCFD]

Originally Posted by ARTisticCFD

Quick fix: Add variable_Name.write() just before runTime.write()

Adding only this line forces the solver to write the variable at each iteration irrespective of out output controls. Therefore, better to write it in an "if" statement


if(runtime.outputTime())
{
variable_Name.write();
}

Thanks. Hope this helps.

[vishalgarg474]

Hey Guys, is there a possibility where the changes should not be done in the solver but in the controlDict file to write a new variable?


I am trying to write drag coefficients in the multiphaseEulerFoam. I can not make changes in the original solver due to some permission rights. Is there a way that I can add lines in a case directory to write it?


Thank you

[clapointe]

Yep, this is possible via function objects compiled at runtime. You can do something like the following (which is added to controlDict) :

functions
{
    vorticity
    {
       libs ("libutilityFunctionObjects.so");

       type coded;
       name vorticity;

       codeExecute
       #{
          const volVectorField& U = mesh().lookupObject<volVectorField>("U");

          volScalarField enst = 0.5*magSqr(fvc::curl(U));

          static autoPtr<volScalarField> pField;
          if(!pField.valid())
          {
              pField.set
              (
                  new volScalarField
                  (
                      IOobject
                      (
                          "enstrophy",
                          mesh().time().timeName(),
                          U.mesh(),
                          IOobject::NO_READ,
                          IOobject::AUTO_WRITE
                      ),
                      enst
                  )
              );
          }

          volScalarField& enstrophy = pField();

          enstrophy.checkIn();

          enstrophy = enst;
      #};
    }
}

Note that I based this off some thread that I cannot remember, but was asking a similar question -- so this may not be the most efficient way to do it, but it works. Can't remember which version I've used this in... likely 7.

Caelan

[sujata]

Originally Posted by vishalgarg474

Hey Guys, is there a possibility where the changes should not be done in the solver but in the controlDict file to write a new variable?


I am trying to write drag coefficients in the multiphaseEulerFoam. I can not make changes in the original solver due to some permission rights. Is there a way that I can add lines in a case directory to write it?


Thank you

Did your problem resolve? If yes then how have you done it?