[chicky]

Hello

I use openFoam to create a tutorial for this library. I have to introduce the axissymmetric 2D pipe flow using laminar simpleFoam. But every time i launch the solving it diverged. So I certainly made a mistake somewhere but I cannot find it.

I try to change the relaxation factor and the solver but it don't solve the problem.

can you help me please

you will find my fvschemes and fv solution here with the log :

[Swagga5aur]

Hello Nicky,

I would like to help you and from your log files it seems that you continuity is the issue as well as pressure (due to the high number of iterations).
However, I'm not sure that the issue is your fvSolution or fvSchemes, and would like if you could send your case directory so that I can conduct more testing to determine what the issue is.

My initial thoughts is that it is a boundary condition issue regarding either velocity or pressure fields.

Best regards, Lasse

[chicky]

Thank you it's very kind

I study a pipe with 10mm radius and 60mm length waith air. I use the Reynolds analogie to work with Re=100 so I have a mesh defined for 6m length and 1m radius (axis-symmetric so it is 0.5m). the inlet velocity is 14.61 m/s and the viscosity 0.147 m²/s.

I have put the initial condition for velocity with internalField uniform (14.61 0 0) to help the solver to converge but doesn't matter it diverged anyway.

I put the file with the salome meshing in the gz archive.

thank you very much

[chicky]

Okaye in fact I think I have found my problem.

I add one line in fvSolution that is

consistent yes;

It converged easily after.

[Swagga5aur]

Good to see you found a solution, I also noticed in that the relaxation factors in the fVsolution was defined wrong.

Applying the following in the fVsolution resulted in a converging solution:

SIMPLE
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
        residualControl
    {
        p               1e-2;
        U               1e-3;
    }

}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7; // 0.9 is more stable but 0.95 more convergent
    }
}

This also explains why the consistent yes; solves the issue as simplec does not need any relaxation of the pressure field, according to http://www.openfoam.com/documentatio...fvSolution.php

Have a nice day

[chicky]

Ok I have undedrstand what you mean in your response. The pitzDaily case use consistent yes; (use of SIMPLEC) to solve the problem. But in fact I want to compare with fluent simulation to make a benchmark and fluent is using by default SIMPLE. It is good to know that I need to have a fields relaxation factor for pressure if I am not using SIMPLEC.

You solved my problem. thank you very much