Dear Foamers,

I'm trying to simulate a gas flow through an injector at high pressure levels up to p=400-500 bar and pressure ratios around pi=3-4. Attached you can find a picture of the involving mesh with the inlet on the left side and the three outlets on the right side which was created with cfMesh, cartesianMesh.
The problem I'm dealing with is the edge at the nozzle. Some cells have very high values (U,p,ptot,rho), others that are very close have very low values. These skips are leading to the divergence after a few hundred iterations depending on the operating point and the initialization. Are there any smoothing operations for my fvSchemes? Or would you suggest another meshing-strategy?
It's not a problem of the boundary conditions, I already figured that out...

Here are my current fvSchemes:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         localEuler rDeltaT;
}

gradSchemes
{
    default 	    Gauss linear;
    grad(p)	    faceLimited Gauss linear 1.0;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss upwind;

    div(phid,p)     Gauss upwind;
    div(phi,h)      Gauss upwind;

    div(phi,K)      Gauss upwind;
    div(phi,k)      Gauss upwind;
    div(phi,omega)  Gauss upwind;

    div((muEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss upwind phi corrected;
}

interpolationSchemes
{
    default         skewCorrected linear;
    reconstruct(U)  GammaV 1.0;
    reconstruct(p)  Gamma 1.0;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


// ************************************************************************* //

Thanks in advance!

[betakv]

Hi Matzbanni,

please can you specify used solvers and folder with initial conditions

VB

Originally Posted by betakv

Hi Matzbanni,

please can you specify used solvers and folder with initial conditions

VB

I'm using a own compressible solver based on rhoPimpleFoam (implemented Peng-Robinson EoS, chung viscosity, janaf specific heats). Please find attached my initial conditions...

Regards!

[franjo_j]

Hello,

By looking into provided information, I suggest the following:
1. Set the mut and alphat to slightly larger values that you expect in the final solution. Increased diffusion in the first couple of iterations could help stabilise the solution.
2. What is the maximum Co number in your case? It may beneficial to reduce it in the first couple of iteration while the solution changes rapidly.
3. What is the maximum non-orthogonality in the mesh, and where is it located? You could also improve convergence by switching on a few non-orthogonal corrector during the first couple of time steps.

I hope this helps you a bit.

Regards,

Franjo

Originally Posted by franjo_j

Hello,

By looking into provided information, I suggest the following:
1. Set the mut and alphat to slightly larger values that you expect in the final solution. Increased diffusion in the first couple of iterations could help stabilise the solution.
2. What is the maximum Co number in your case? It may beneficial to reduce it in the first couple of iteration while the solution changes rapidly.
3. What is the maximum non-orthogonality in the mesh, and where is it located? You could also improve convergence by switching on a few non-orthogonal corrector during the first couple of time steps.

I hope this helps you a bit.

Regards,

Franjo

Thanks Franjo for your input! I played a little with the meshing settings, here's the thing: if I use no or one boundary layer, there's no problem with the simulation, it converges perfectly. If I use more than one, I get the mistakes i described.
The maximal Courant number for my simulation is fixed at 0.4 (with local time stepping), the non-orthogonality is not an issue. Any ideas?

[franjo_j]

Originally Posted by matzbanni

Thanks Franjo for your input! I played a little with the meshing settings, here's the thing: if I use no or one boundary layer, there's no problem with the simulation, it converges perfectly. If I use more than one, I get the mistakes i described.
The maximal Courant number for my simulation is fixed at 0.4 (with local time stepping), the non-orthogonality is not an issue. Any ideas?

What is the size ratio between the last cell in the boundary layer and the rest of the mesh? This ratio grows when the number of boundary layers is increased, and can be problematic in case of high gradient variation.
Do you use optimiseLayer option for boundary layers? It is implemented to improve the smoothness and orthogonality of cells in the boundary layers, and out tests have shown beneficial impact on convergence and accuracy.

Originally Posted by franjo_j

What is the size ratio between the last cell in the boundary layer and the rest of the mesh? This ratio grows when the number of boundary layers is increased, and can be problematic in case of high gradient variation.
Do you use optimiseLayer option for boundary layers? It is implemented to improve the smoothness and orthogonality of cells in the boundary layers, and out tests have shown beneficial impact on convergence and accuracy.

Hello Franjo,
due to the really high gradients in my setup that could have a major influence, you're right. I'll try to reduce the size ratio and will report tomorrow... There's no such option that I can define the (fixed) size of the first layer?

Regards!

[franjo_j]

Originally Posted by matzbanni

Hello Franjo,
due to the really high gradients in my setup that could have a major influence, you're right. I'll try to reduce the size ratio and will report tomorrow... There's no such option that I can define the (fixed) size of the first layer?

Regards!

Hi,

You can specify the upper bound on the thickness of the first layer by setting the maxFirstLayerThickness where appropriate.

Regards,

Franjo

Originally Posted by franjo_j

Hi,

You can specify the upper bound on the thickness of the first layer by setting the maxFirstLayerThickness where appropriate.

Regards,

Franjo

I've seen that in the user guide, the other way round would be also great (maybe in the next release )...