[Zomzzz]

hi i was doing some analysis and the residual curve doesn't look so optimistic as all ux and uy uz are horizontal and they didn't reach 1 e-6
so i am not sure that the results are trusted and in para view they flow doesn't go as i expected.
any suggestion and thought what should be revised in pre processing ?

[unilord]

Originally Posted by Zomzzz

hi i was doing some analysis and the residual curve doesn't look so optimistic as all ux and uy uz are horizontal and they didn't reach 1 e-6
so i am not sure that the results are trusted and in para view they flow doesn't go as i expected.
any suggestion and thought what should be revised in pre processing ?

Please provide more information:


- Give a general view of what case you are trying to simulate. Turbomachinery, external flow around a car, etc...

- Is the problem steady or transient? By the results I assume it's steady but still. Incompressible or not.

- If possible show the fvSchemes.


- Show the checkMesh log

[yomn]

the cae is baically a room where i blow hot air from some diffuser, i already checked the check mesh all is ok and all within the limits,

here is the fvscheme file:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}

ddtSchemes
{

default steadyState;

}

gradSchemes
{

default cellLimited leastSquares 1;

}

divSchemes
{

default none;

div(phi,omega) bounded Gauss upwind default;

div(phi,T) bounded Gauss upwind default;

div(phi,U) bounded Gauss upwind grad(U);

div((nuEff*dev2(T(grad(U))))) Gauss linear;

div(phi,k) bounded Gauss upwind grad(k);

}

laplacianSchemes
{

default Gauss linear limited corrected 0.333;

}

interpolationSchemes
{

default linear;

}

snGradSchemes
{

default limited corrected 0.333;

}

fluxRequired
{

default no;

}
wallDist
{
method meshWave;
}

[unilord]

Originally Posted by yomn

the cae is baically a room where i blow hot air from some diffuser, i already checked the check mesh all is ok and all within the limits,

here is the fvscheme file:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}

ddtSchemes
{

default steadyState;

}

gradSchemes
{

default cellLimited leastSquares 1;

}

divSchemes
{

default none;

div(phi,omega) bounded Gauss upwind default;

div(phi,T) bounded Gauss upwind default;

div(phi,U) bounded Gauss upwind grad(U);

div((nuEff*dev2(T(grad(U))))) Gauss linear;

div(phi,k) bounded Gauss upwind grad(k);

}

laplacianSchemes
{

default Gauss linear limited corrected 0.333;

}

interpolationSchemes
{

default linear;

}

snGradSchemes
{

default limited corrected 0.333;

}

fluxRequired
{

default no;

}
wallDist
{
method meshWave;
}

From the fvSchemes solely, I can tell that you should use a second order scheme for the convective term "grad(U)". linearUpwind is a good choice.

Again, I would like to see the checkMesh in order to evaluate two main things: If you have more tetrahedrals than hexahedrals, I would sugest swapping the leastSquares to Gauss linear, since I have found that it is more suitable in cells with less faces. Other, the maximum non orthogonality, in order to understand the snGradScheme. If it is lower than 60 you can go with corrected.


With this said, I do believe the problem you have might be due to the boundary conditions. Can you show them?

[Zomzzz]

here is the text file and i copied U/p file and check mesh output as well, thanks in advance.

[unilord]

Originally Posted by Zomzzz

here is the text file and i copied U/p file and check mesh output as well, thanks in advance.

Well,

To be honest, I don't find anything to be wrong with this setup. The only things I would say are:

- You really have 252 million cells? I never saw something like that in Openfoam. Just out of curiosity, how much time did it take to do 1000 iterations?

- I have worked with static pressure outlet/total pressure inlet bc's and I have found that they can be quite unstable. Can't you swap to a flow rate outlet and static pressure outlet or vice versa?

- I would also sugest you to try and work with full upwind schemes and cellLimited Gauss Linear 1, just for a first approximation to see if the
pressure residuals are that high because of the schemes.

- I haven't had a look at th fvSolution but that also affects the solver. Are you using GAMG for the pressure? Try and use "nCellsInCoarsestLevel = 1000". For initial iterations I always use relTol=0.01 and tolerance = 1e-8. If the GAMG solver doesn't work you can try another one (PBiCGStab).

Other than this, I wouldn't be able to give you any other tips. If anyone more experienced than me could have a look at this that would be great.