CFD Online Discussion Forums - Solution Singularity

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Solution Singularity (https://www.cfd-online.com/Forums/openfoam-solving/197126-solution-singularity.html)

Solution Singularity

Hi Team !

I am facing totally new error. What is Solution Singularity? The solver is SimpleFOAM.

I checked BCs, for any conflicting ones. I checked fluid properties.

Please help.

Code:

Create time



Create mesh for time = 0





SIMPLE: convergence criteria

    field U      tolerance 1e-006

    field epsilon        tolerance 1e-006

    field k      tolerance 1e-006

    field h      tolerance 1e-006

    field p      tolerance 1e-006



Reading field p



Reading field U



Reading/calculating face flux field phi



Selecting incompressible transport model Newtonian

Selecting turbulence model type RAS

Selecting RAS turbulence model kOmegaSST

Selecting patchDistMethod meshWave

kOmegaSSTCoeffs

{

    alphaK1         0.85;

    alphaK2         1;

    alphaOmega1     0.5;

    alphaOmega2     0.856;

    gamma1          0.55555556;

    gamma2          0.44;

    beta1           0.075;

    beta2           0.0828;

    betaStar        0.09;

    a1              0.31;

    b1              1;

    c1              10;

    F3              false;

}



No MRF models present



No finite volume options present





Starting time loop



Time = 1



DILUPBiCCCG:  Solving for Ux:  solution singularity

DILUPBiCCCG:  Solving for Uy:  solution singularity

DILUPBiCCCG:  Solving for Uz:  solution singularity

I think the solver detected a singular matrix. May be all velocities are zero or at least the same and no pressure gradient.

Thanks for the reply in the vacation period. :)

My BCs are,
Inlet Ptotal = 0
Outlet Pstat = 0
And I have a fan source in the domain. I am posting the fan BC from p file here.

Code:

sfan_23_half0

    {

        type            fan;

                patchType                cyclic;

                f List<scalar> 3(111 -222 333);

                value uniform 0;

      }



    sfan_23_half1

    {

        type            fan;

                patchType                cyclic;

                f List<scalar> 3(111 -222 333);

                value uniform 0;

    }

The solution runs on single processor. But problem comes on multi-processor.

I don't know your case en détail, but cyclic boundary conditions may be problematic. You have to ensure that the the inlet measures are identical to the ones at the outlet AND that this is physical realistic.
As far as I understand: You have your fan among the calculated region. Therefore cyclic is not suitable. It is nonphysical too, that the pressure at the one end is the same as at the other. A fan increases the pressure.

Thanks for the reply.

If i have understood you correctly, Fan can not be given like that.

This is the only way I know to give internal fan curve. This is a facezone where I have created this patch.

Before the actual problem I created a test case where I put same fan BC in a pipe and put a porous media cellzone and computed successfully. I have attached the test case picture.

When I actually use the patch in the case, it gives this error.

There is no change only the geometry, mesh and fan equation.

Another interesting observation. It runs on single core, and as soon as I switch to multiple cores it gives singularity error.

Just to close the matter.
The error was due to the singular matrix as mentioned by Piu58. The error vanishes if I initialize it in the U file (Internal field).
Even though, I do not initialize the error vanishes in the second iteration.

As I understand there is no 'excitation' in the field to start the flow, so it gives singular matrix. The pressure jump is dependent on flow and flow is dependent on pressure jump, so it requires initialization.