[sven82]

hi,

I will write out a variable of my own turb. model,
but its doesn't work.
First of all I define a ScalarField in my Header,

volScalarField hybrid_;

for the next step I edit the code file with a new Object

hybrid_
(
IOobject
(
"hybrid_",
runTime_.timeName(),
mesh_,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh_,
dimensionedScalar("hybrid", dimless, 0.0)
),

and follow of the definition in the memberfunction

hybrid_ = tanh ( pow( max( scalar(0) , ( I_ / X_ ) - 1/2 ) , 3) );

// function = tanh( ( max( 0 , l/x - 1/2 ) )³ )

the compile shows now errors and the case run fine for me,
except !!
the code cant write out the values of my defined variable (hybrid_).
When I add the line hybrid_.write() its works,
but for every timestep and not for the defined writecontrol!

Hope everyone got a idea !

Thanks
Sven

[su_junwei]

Hi Sven

you can test the following code

if(runTime_.outputTime())
{
hybrid_.write();
}

Junwei

[sven82]

thanks junwai,

it works

Sven

[samiam1000]

Dear friends,

I am trying to solve the same problem you solved.

Could you help me?

Where should I add that code?

And is it necessary to re-compile the code? Can't I do the same thing in the case-dir, editing the dictionaries (e.g. controlDict)?

Thanks a lot for help,
Samuele

[jhoepken]

First of all, if you would like to change something in the code, you will - of course - have to recompile the respective parts. If you would just like to write a certain field to disk, that is not written automatically, I guess that there is a functionObject to do that.

Otherwise you will have to put something like this in your solver/library

volScalarField foo = mesh.V();
foo.write();

Have a look at the programmer's guide.

[jhoepken]

And it would be great if you could just post your question once!

[samiam1000]

Hi,

thanks for answering and sorry for the double question.

Samuele

[Marshak]

I am having the same problem to solve. Can someone post the correct code because from above posts it is not clear what is the right way to code?

[makaveli_lcf]

Different variants are correct :-)

[dduque]

Hi every one.
I have tried to use these ideas, and other, but right now I am failing to write down a field. I try something as simple as modifying interFoam, and in createFields.H :

    volScalarField surfForce
    (
        IOobject
        (
            "surfForce",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        alpha1
    );

The name "surfForce" makes no sense, I just tried to write down this complicated field and made my request as simple as possible. The thing is, the field is written down correctly in the first time step, and it is identical to the alpha1 field (the one from time step zero, actually). But in subsequent times, it does not change at all, even if it is written. Meanwhile alpha1 keeps changing (where is it told that this field be written, I wonder?).

Thanks in advance. Best,

Daniel

[wyldckat]

Greetings to all!

@Daniel: OpenFOAM's C++ already seems voodoo'ish enough already, so it would be even more complicated if all it took to bind one field to another, would be to reference it only once at construction

In other words, I suggest that you give a quick study to this tutorial: http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam - You'll notice that the "T" field is changed on every iteration, not just at the start.

Best regards,
Bruno

[dduque]

Of course! I know that tutorial almost by heart, but somehow the fact that a whole equation was solved for T had obscured the obvious fact that T is changed. I only have to repeat the field=alpha1 (or whatever) at each iteration then.

Thanks a lot!

Daniel

[ChrisWe]

I actually try to program my own solver and there are some variables that I want to write down in an additional file. When I try this for the turbulent kinetic energy that works fine. Therefore I added in the createFields.H the following code:

volScalarField k_output
(
    IOobject
    (
        "k_output",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    turbulence->k()
);

and in the .c file of my solver the following code:

...
#include "createFields.H"
...
while (runTime.run())
{
...
k_output = turbulence->k();
...
}

All works perfect, OpenFOAM creates a new output-file called k_output where k is stored.


Now I want to do the same with a variable (volTensorField) that I created by myself. In this case the variable is called alphaEff.
Therefore I added the same lines like before in the createField.H file for my own TensorField:

volTensorField alphaEff_output
   (
      IOobject
      (
        "alphaEff_output",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
        ),
        alphaEff       (i also tried alphaEff_output together with (**) )
  );

and in the .c file of my solver:

...
#include "createFields.H"
...
while (runTime.run())
{
...
    volTensorField alphaEff
       (
          IOobject
          (
            "alphaEff",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
            ),
            turbulence->nu()/Pr*I + DT
       );
...
alphaEff_output=alphaEff;  (**) (only when using alphaEff_output)
...
}

Now, I've got some problems, because OpenFOAM doesn't know alphaEff in the createFields.H file.

I think that the answer is extremely easy, but I'm sitting now about two days in front of my PC without any progress. Maybe one of you knows the answer for my little problem



(the idea of

if(runTime_.outputTime())
   {
    alphaEff.write();
  }

works, but then the probes-function doesn't work for alphaEff).

[alexeym]

Hi,

Why would you like to define alphaEff inside 'while (runTime.run())' loop and not outside?

Also you can define it just like:

volTensorField alphaEff
(
    IOobject
    (
        "alphaEff",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    mesh,
    <dimensions of alphaEff>
);

as anyway you recalculate it every time step (if my guess is correct).

It will be automatically written every write time.

[ChrisWe]

Thank you very much for your rapid answer, but this solution doesn't work at all.

When I tried your idea, OpenFoam needed an INPUT-File in the 0-folder and a MUST_READ in the IOobject because of the <mesh> entry. After changing this, all worked.

So for all who have the same problem, this was my solution:

In the solver-folder, I added the following IOobject into the <createfields.H> file:

volTensorField alphaEff
   (
      IOobject
      (
        "alphaEff",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
      ),
      mesh
);

This file requires an additional INPUT-File in the boundary 0-folder that is called alphaEff and looks like the other boundary-files.

In the .c file of the solver, I only have to update alphaEff in the time-loop, in my case:

alphaEff=turbulence->nu()/Pr*I + DT;

With this solution, its possible to take probes from alphaEff.
The only ugly part of this solution is the one, that you have to create an additional Input-File for alphaEff.

Maybe someone knows a solution, where I don't need this file.
When I try to create an IOobject with NO_READ, OpenFoam doesn't work anymore.

[alexeym]

I don't know what modifications you've done to proposed solution (I guess you've ignored the line with dimensions), but here's a piece of working code:

...
    flux_
    (
        IOobject
        (
            "heatFlux",
            mesh.time().timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimEnergy/dimTime/dimVolume
    )
...

or we can use another way to initialize field to zero:

...
    flux_
    (
        IOobject
        (
            "heatFlux",
            mesh.time().timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("flux", dimEnergy/dimTime/dimVolume, 0.0)
    )
...

There's no heatFlux file in 0 folder and field flux_ is written every writeInterval.

In your case it should be tensor, not scalar.

[ChrisWe]

Ahhhh, now its working without defining an Input-File for alphaEff. Thank you very much for your patience and your helpfulness!!!

In my version before, I had to replace your NO_READ with MUST_READ because I thought, that the dimensions aren't necessary at all. But I was wrong, NO_READ only works together with the dimensions in this case:

      mesh,
      dimensionedTensor("alphaEff", dimArea/dimTime, tensor::zero)

[vigneshTG]

Dear All,

I am working on VOF method and using interFoam solver. I would like to write the whole surface tension term in UEqn.H (fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1)) to the output. I tried creating a volVectorField in CreateFields.H as below

//*******************************************************************************//
volVectorField ST
    (
        IOobject
        (
            "ST",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1)
    );
//*******************************************************************************//

But I get error as below

In file included from interFoam.C:60:0:
createFields.H: In function 'int main(int, char**)':
createFields.H:40:26: error: 'interface' was not declared in this scope
createFields.H:40:58: error: 'alpha1' was not declared in this scope
/opt/openfoam222/src/finiteVolume/lnInclude/readTimeControls.H:38:8: warning: unused variable 'maxDeltaT' [-Wunused-variable]
make: *** [Make/linux64GccDPOpt/interFoam.o] Error 1

Can anyone help me how to rectify this Or is there any other way to write the surface tension term to the output.

[alexeym]

Hi,

where exactly did you put the code? Obviously it should be placed after definition of alpha1 (line 36) and interface (line 76).

From error output I can see that expression with alpha1 and interface is at the line 40, so I guess definition of volScalarField started before definition of alpha1 and interface (hence the error). Also

fvc::interpolate(interface.sigmaK())*fvc::snGrad(alpha1)

will give you surface field, you need to reconstruct it (see fvc::reconstruct in UEqn.H) to get volume field.

[vigneshTG]

Thanks Alex !! You pointed it out, i wrote the definition of surface tension term before alpha definition. Now i corrected it and it works !!

Thank you very much !!