[luisfeliperojas95]

Good Morning , My name is Luis Rojas . I am trying to process a mesh with a open atmosphere channel . My enviormental configurations are Velocity in movingWall is 37 on the x-axis else 0 in y and z axis; Preassure in movingWall is 0 , Preassure in frontAndBack is 73120 Pascals. I want to process that mesh on the cavity case. So next I paste my configurations for each variable. The problem is .... Anyway I execute the comand ''icoFoam''. OpenFoam show's me that. I will apreciatte too much if you help me to Know what is happening on my simulation for Future Practices publish a Tutorial Solving this trouble.

$ icoFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.x |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
/* Windows port by CFD support (www.cfdsupport.com) [based on Symscape] *\
\*---------------------------------------------------------------------------*/
Build : 2.3.x-819030ed51bd
Exec : C:\OpenFOAM\cygwin64\opt\OpenFOAM\OpenFOAM-2.3.x\platforms\cygwin64mingw-w64DPOpt\bin\icoFoam.exe
Date : Dec 16 2015
Time : 03:42:33
Host : "EQUIPO2"
PID : 2100
Case : C:/OpenFOAM/cygwin64/opt/OpenFOAM/OpenFOAM-2.3.x/FelipeT/incompressible/icoFoam/SimFelipe/CavityQuebrada/Cavity1
nProcs : 1
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading transportProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.05

Courant Number mean: 0.0595329 max: 121.711
smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 6.45652e-006, No Iterations 12
smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0


--> FOAM FATAL ERROR:
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux : 368.881
Specified mass inflow : 10.4802
Specified mass outflow : 0
Adjustable mass outflow : 0


From function adjustPhi(surfaceScalarField&, const volVectorField&,volScalarField&)
in file cfdTools/general/adjustPhi/adjustPhi.C at line 122.

FOAM exiting

I dont Know why OpenFOAM is showing me an error with the outlet and inlet.

For the Velocity i have this

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
movingWall
{
type fixedValue;
value uniform (37 0 0);
}

fixedWalls
{
type fixedValue;
value uniform (0 0 0);
}

frontAndBack
{
type fixedValue;
value uniform (0 0 0);
}
}

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

For Preassure i have this

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0;

boundaryField
{
movingWall
{
type zeroGradient;
}

fixedWalls
{
type zeroGradient;
}

frontAndBack
{
type fixedFluxPressure;
value uniform 73120;
}
}

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

Next I attached the Mesh Images.

https://drive.google.com/file/d/0B1P...I2R2pMZTg/view

https://drive.google.com/file/d/0B1P...V6SFp6clU/view

https://drive.google.com/file/d/0B1P...E0YU5IMzA/view

https://drive.google.com/file/d/0B1P...VJaFVydTg/view

https://drive.google.com/file/d/0B1P...FKdFNMVFk/view

[wyldckat]

Greetings Luis Rojas,

There are two problems that I can see. The first one:

Originally Posted by luisfeliperojas95

smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 6.45652e-006, No Iterations 12
smoothSolver: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0

This means that the Y and Z directions are of type "empty" and were not solved.
Remember seeing that in the OpenFOAM User Guide, the tutorial for the cavity case tells us that it's using pseudo-2D, by defining the front and back patches as type "empty"? This was also defined in the "blockMeshDict", which consequently means that the same will happen to the resulting file "constant/polyMesh/boundary".
More details in subsection "5.2.1 Specification of patch types in OpenFOAM" of the User Guide: http://cfd.direct/openfoam/user-guide/boundaries/


The second issue is this:

Originally Posted by luisfeliperojas95

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
movingWall
{
type fixedValue;
value uniform (37 0 0);
}

fixedWalls
{
type fixedValue;
value uniform (0 0 0);
}

frontAndBack
{
type fixedValue;
value uniform (0 0 0);
}
}

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

It looks like the fluid is being injected on one end of the geometry, namely through the one named "movingWall". This means that you are asking icoFoam to compress the fluid inside the mesh, because there is no exit defined in any of the other patches. But icoFoam cannot compress fluid, because it's only able to deal with incompressible fluids.

For example, if you want the fluid to exit through the patch "frontAndBack", you need to define the boundary condition like this in the file "U":

frontAndBack
{
   type zeroGradient;
}

Best regards,
Bruno