[cute]

Hi All,

I am using scalarTransportFoam tutorial with some modification, i.e two PDEs with no flow. I have 3D domain 1 x 1 x 1 m^3 and I set internal mesh with initial value C=1 uniformly. When I run this solver on one processor, it works fine. But when I run it on 4 processors, I don't get the similar result. When i visualize in paraview, I observed that at time t=0 the value is C=1 everywhere (correct) but at the next time step say t=1 it turns to ZERO. I don't know why? Do I need to do something else before running in parallel. Application runs, but does not produce the correct result.

Do you have any suggestion?

Thanks.

[cute]

I fixed my previous problem by increasing allocated memory. By default it was 1G.

Now I am facing another problem. I divided my domain on 4 processors as (2 2 1). As initial setup, I placed biomass in processor 0, 1, and 2 leaving 3 as empty. I am expecting the biomass should spread in all directions and should occupy space in empty slot. But it is not. Please see figures (contour surface).

Why is it happening? and how to fix? Any suggestion.

Thanks.

[cute]

Anyone has any suggestion. I am stuck.
Thanks.

[hk318i]

Have you tried the same case on single processor? Just to confirm your expectations.

[cute]

Yes, it is working good on single processor. I mentioned it in my first post.

[hk318i]

I run quick few cases to try to reproduce the problem but I could not. Attached here a image for a case with zero velocity (no flow), pure diffusion. As you can see there is diffusion through the processor interface. Also I run ``laplacianFoam`` for the same case to double check and I get the same behaviour. Moreover, I tried to start with zero inside and one at the inlet and it worked as well. Probably we need to know more about your code and case setup to help.

[cute]

Thanks. Here is my decomposeParDict

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

numberOfSubdomains 4;

method          simple;
//method          scotch;

simpleCoeffs
{
    n               (2 2 1);
    delta           0.001;
}

hierarchicalCoeffs
{
    n               (2 2 1);
    delta           0.001;
    order           xyz;
}

manualCoeffs
{
    dataFile        "";
}

distributed     no;

roots           ( );

Let me know, what else you need to know.

[hk318i]

``decomposeParDict`` looks fine. You may try to decompose in Z direction as well (2 1 2). It could give an indicator where is the problem come from. Are you currently using ``scalarTransport`` or your solver?

[cute]

Thanks Hassan Kassem.

I used (2 1 2) partition, and still the same result. That is one of the region is completely empty. I am using my solver which is modified version of scalar transport equation. Here is my code snippet

while (simple.loop())
    {
        Info<< "Time = " << runTime.timeName() << nl << endl;

        while (simple.correctNonOrthogonal())
        {
            forAll(DX, cellI) {
                DX[cellI] = alpha.value()*X[cellI]*X[cellI];
            }
            
            solve(fvm::ddt(X) == fvm::laplacian(DX, X) + k*X);
            
        }

        runTime.write();
    }

[alexeym]

Hi,

1. What is wrong with DX = alpha*sqr(X) (or DX = alpha*X*X)? Why do you need loop?

2. Since you are using loop, DX values at processor boundaries are not updated. Try inserting DX.correctBoundaryConditions() after loop.

[hk318i]

I can't see the point of the loop as well but what worries me here why this behaviour is consistent even when he changes the decomposition. 🤔

[cute]

Thanks for the reply.

(1) If I don't use loop, I get dimension problem. In my case DX is m^2/s, X is kg and alpha is dimensionless. If I use alpha*sqr(X), I get dimension problem, i.e. m^2/s = kg^2. The only way, I could figured out is to use loop. If you have some suggestion to fix this error, that would be easy solution.

(2) I tested DX.correctBoundaryConditions() on a quick run and it seems to worked out on initial testing.

(3) Since this solution works, I need to extend my model by adding another PDE. I don't know how to incorporate both equations. Is there any tutorial or test-case to solve coupled PDE? Please suggest. My preference is to add both discritized equation in a matrix and then solve. I don't want to solve using segregated way.

[alexeym]

1. Why can't you set dimensions of alpha to m2*s^-1*kg^-2? Why not use non-dimensioning coefficient X1 with dimensions kg and value 1 so you can calculate DX as alpha*sqr(X/X1)? If you still afraid of dimensions, you can use internalField() that is dimensionless, so DX.internalField() = alpha.value()*sqr(X.internalField()).

3. As you can see, nobody wants to answer "abstract" questions. Solution to your parallel run problem was proposed as soon as you posted your snippet. Post your equations.

[cute]

Thanks, I will try your solution and I did not think that way (feeling stupid).

Here are my equations that I want to solve:

ddt(C) = laplacian(d, C) - alpha*F(C)*X
ddt(X) = laplacian(DX, X) + F(C)*X - beta*X

where F(C) = C/(0.5+C) and d, alpha and beta are some real numbers.

[alexeym]

Well, guess, if you would like to solve your equations in coupled manner, you have to write them in coupled manner, i.e. q = ||C, X||, and then write your equations in terms of q. Then you introduce volVector2DField and solve equation as usual, or just use volVectorField assuming third component as 0. For solution of vector equations, you can refer to any UEqn.H in incompressible solvers.

If you would like someone to rewrite your equations in vector form (and then post corresponding code), you have to explicitly ask for this. Also I think separate post could attract more interested persons.

[cute]

Thanks, I will post it separately.