CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   conditional solving of transport equation (http://www.cfd-online.com/Forums/openfoam-solving/96367-conditional-solving-transport-equation.html)

 dzi January 20, 2012 09:41

conditional solving of transport equation

hi people,
I would like to set up a solver for a solidification process with solving a transport equation for a species only in the liquid phase of the sytem.
There is a volScalarField alpha which defines the state of phase (0<alpha<1). alpha is the liquid fraction, alpha = 0 -> complete solid.

How can I define a solver which works only in the non solid part of the domain like:

// definition of eq.
{liqEqn = ....}
// conditional solving of liqEqn
if (alpha != 0) liqEqn.solve();

Is there somewhere a similar case/tutorial/documentation reference?
dzi

(I use OF 2.01)

 marupio January 22, 2012 14:10

It is very difficult to only use portions of the mesh for the matrix solution in OpenFOAM. You'd probably have to create a new temporary mesh, and create new variables on it - then you'd have to create new boundaries where it is cut-off... Rather than that, you probably want to work with the full mesh, and modify the matrix so that the portion from the solid cells reduce to a trivial equation.

I'm thinking you could create a custom preconditioner for your matrix. I don't know exactly what you want to do to the matrix to achieve this, though.

 akidess January 23, 2012 04:35

I think the easiest solution is to multiply all terms in the equation with alpha.

 alberto January 24, 2012 11:51

Quote:
 Originally Posted by dzi (Post 340306) hi people, I would like to set up a solver for a solidification process with solving a transport equation for a species only in the liquid phase of the sytem. There is a volScalarField alpha which defines the state of phase (0 complete solid. How can I define a solver which works only in the non solid part of the domain like: // definition of eq. {liqEqn = ....} // conditional solving of liqEqn if (alpha != 0) liqEqn.solve(); Is there somewhere a similar case/tutorial/documentation reference? thank you for advice, dzi (I use OF 2.01)
You can simply define a flag in this way:

volScalarField solveEq(pos(alpha-alphaCutOff));
volScalarField doNotEq(1-solveEq);

which is 1 when alpha > alphaCutOff, and 0 elsewhere. Then there are two possible solutions, depending on what you are trying to do (momentum equation or scalar equation?)

- Momentum equation:

Code:

```fvMatrix UEqn (   solveAlpha*   (       //Put your equation here   )+   doNotSolve*   (       fvm::Sp(coeff,yourVariable)  // Set the variable to zero or to a value here   ) );```
- Scalar equations: you can use what done above, or drop elements from the matrix and fix the value of the solution directly using
Code:

`myEqn.setValues(...)`
See for example OpenFOAM/OpenFOAM-2.1.x/applications/solvers/multiphase/bubbleFoam/wallDissipation.H for an example.

Best,

 dzi January 25, 2012 04:47

thank you for the replies,
for me the easiest solution is the suggestion from akidess to multiply all, or parts of the equation with alpha. Looks like it can be solved and I get something out which makes sense.

The other suggestions also sound interesting. I will try if I come to a limit with the first solution, but on the first glance they seem to be more sophisticated.

Thank you again for helping on this topic!
dzi

 alberto January 25, 2012 11:19

Quote:
 Originally Posted by dzi (Post 341024) thank you for the replies, for me the easiest solution is the suggestion from akidess to multiply all, or parts of the equation with alpha. Looks like it can be solved and I get something out which makes sense.
This depends on what you are solving for, but in general, multiplying by zero both sides of the equation without doing anything else will introduce a (0 = 0) equation and make the linear system singular.

If you are solving the momentum equation, you will also have to deal with the problem of the central coefficient going to zero, which will lead to a segmentation fault when you calculate H/A. You can check how this problem is addressed in compressibleTwoPhaseEulerFoam.

Best,

 hawkeye321 January 30, 2013 02:57

Solidification in OpenFOAM

Hi
I am solving a binary alloy solidification problem with OpenFOAM. For the species equation, which seems to be the most critical equation especially at the region where channels form, I have used zero grad boundary conditions; which causes a flow into the wall. Have you guys also used grad(CL) = 0, and grad(C) = 0 at the boundaries?

 Neka December 3, 2015 09:04

conditional solving of transport equation

Hello dear foamers,
I want to revive this old thread with a new question.
I wonder if it is possible in OpenFOAM to solve a transport equation only for cells whose variable values are larger than a certain value.
Like: solve Eqn. only for values >0…
Let me explain:
I simulate a fluid consisting of two gas fractions gas1 and gas2. Gas2 does not cover the whole simulation domain but is present in places. So, basically, there are regions where the concentration of gas2 is zero. Consequently, the partial density rho of gas2 in those regions is zero too.
In order to simulate a thermal non-equilibrium I need to solve the energy equation for both gases separately. I want to solve the energy equation for gas2 only for regions, where the density of gas2 is larger than a certain value (e.g. 10e-9 or something…). My energy equation is taken from rhoCentralFoam, where the internal energy is solved in two steps:
Step1: the predictor step without diffusion term:
solve
(
fvm::ddt(rhoE)
+ fvc::div(phiEp)
);

Than calculating internal energy and correcting boundary conditions:

e = rhoE/rho - 0.5*magSqr(U);
e.correctBoundaryConditions();
thermo.correct();
rhoE.boundaryField() =
rho.boundaryField()*
(
e.boundaryField() + 0.5*magSqr(U.boundaryField())
);

Step2: the diffusion correction equation.

if (!inviscid)
{
solve
(
fvm::ddt(rho, e) - fvc::ddt(rho, e)
- fvm::laplacian(turbulence->alphaEff(), e)
);
thermo.correct();
rhoE = rho*(e + 0.5*magSqr(U));
}

The predictor step is working just fine, but since I have to divide rhoE by rho of gas2 I understandably get the error, because there are cells in the simulation domain with rho = 0.
What I did is:

forAll(e, celli)
{
if (rho [celli] > 0.000001)
{
e [celli] = rhoE [celli]/rho [celli] - 0.5*magSqr(U[celli]);
}
else
{
e [celli] = e [celli]*0.0;
}
}

But I have my suspicion, that this technique is highly inefficient concerning the computational speed.

The next problems occur by executing:
e.correctBoundaryConditions();
and
thermo.correct();

When executing the command “correctBoundaryConditions” the solver crashes with the following report:

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
...

...
Floating point exception (core dumped)

I took a look at “src/OpenFOAM/</SPAN>fields/</SPAN>GeometricFields/</SPAN>SlicedGeometricField/</SPAN>SlicedGeometricField.C</SPAN>”, where I suppose the function “correctBoundaryConditions” is defined, but my OpenFOAM knowledge is too little to understand the file.

My questions are:
- Is there a better way than using the “forAll” loop, like I did?
- How could I handle the printStack -error coming up by calling the correctBoundaryConditions-function?

</SPAN>

 olivierG December 3, 2015 10:43

Hello,

I guess you should also loop over boundaryMesh, not only (internal) cells.

regards,
olivier

 Neka December 3, 2015 11:31

Hello Olivier, hello all.

Olivier, thank you for the quick reply.

I just did it like this:

Code:

```                 forAll(e.boundaryField(), patchi)                 {                     fvPatchScalarField& ePatch = e.boundaryField()[patchi];                     forAll(ePatch, facei)                     {                               if (rho[facei] > 0.000001)                               {                                   e.correctBoundaryConditions();                               }                               else                               {                                   e[facei] = e[facei]*0.0;                               }                     }                 }```

It compiles just fine.

The same problem appears with the command thermo.correct(). What I did there is:

Code:

```                 forAll(e, celli)                 {                     if (e[celli] > 0.000001)                     {                               thermo.correct();                     }                 }```

It compiles also fine.
I guess, that the function e.correctBoundaryConditions() is only executed for the particular cell “I” at each forAll-loop and not over all boundary cells.
Is it right?
Because otherwise I would get the same error as without using forAll.

The next challenge is the corrector step:

Code:

```             solve             (                 fvm::ddt(rho, e) - fvc::ddt(rho, e)               - fvm::laplacian(turbulence->alphaEff(), e)             );```

Here I have the same error as with the correctBoundaryConditions()-function, namely:

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
...

...
Floating point exception (core dumped)

Is there some technique to solve this equation conditionally (for e > 0.00...)?

Regards
Alex

 All times are GMT -4. The time now is 14:14.