CFD Online Discussion Forums - Outlet BC with Interfoam

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

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

- - Outlet BC with Interfoam (https://www.cfd-online.com/Forums/openfoam-solving/99268-outlet-bc-interfoam.html)

Outlet BC with Interfoam

I'm simulating a waterfall device using Interfoam. Everything's fine but the outlet.

If you look at the picture you'll see the water at the end of the domain that seems reflected by the outlet surface. Isn't supposed to just disappear as soon as it touchs the surface ?

Here is my BC:

Code:

FoamFile

{

    version     2.0;

    format      ascii;

    class       volScalarField;

    location    "0";

    object      alpha1;

}

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

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField

{

    inlet

    {

        type            fixedValue;

        value           uniform 1;

    }

    outlet

    {

        type            inletOutlet;

        inletValue      uniform 0;

        value           uniform 0;

    }

    walls

    {

        type            zeroGradient;

    }

    defaultFaces

    {

        type            zeroGradient;

    }

}

 

FoamFile

{

    version     2.0;

    format      ascii;

    class       volScalarField;

    object      p_rgh;

}

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

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField

{

    inlet

    {

        type            buoyantPressure;

        value           uniform 0;

    }

 

    outlet

    {

        type            totalPressure;

        p0              uniform 0;

        U               U;

        phi             phi;

        rho             rho;

        psi             none;

        gamma           1;

        value           uniform 0;

    }

    walls

    {

        type            buoyantPressure;

        value           uniform 0;

    }

 

    defaultFaces

    {

        type            buoyantPressure;

        value           uniform 0;

    }

}

 

 

FoamFile

{

    version     2.0;

    format      ascii;

    class       volVectorField;

    location    "0";

    object      U;

}

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

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField

{

    outlet

    {

        type            pressureInletOutletVelocity;

        value           uniform (0 0 0);

    }

 

    inlet

    {

        type            fixedValue;

        value           uniform (0 1 0);

 

    }

 

    walls

    {

        type            fixedValue;

        value           uniform (0 0 0);

    }

 

    defaultFaces

    {

        type            fixedValue;

        value           uniform (0 0 0);

    }

}

Any comment ?

I would rather go with zeroGradient instead of buoyantPressure for the "inlet"...
Furthermore, could you provide some more information?
Such as velocities / grid and maybe schemes and solution algorithms?
Do you have a laminar or turbulent case?

I usually have defaultFaces set to "empty" for everything. But I do not know what "faces" are inside your defaultFaces "class"...

As already mentioned, some more information would be useful for me and others to help you.

I think it is perfectly fine. I have used that exactly outlet condition with a standing plunging wave crossing the boundary and I did not get any reflections or disturbances.

May that water come from the first time steps when the waterfall develops? Maybe due to air movement on the first time steps the falling water may not reach so far, leading to what you see (there's a wall on the bottom, right?)

Sorry for the lack of information.

At the moment I'm working with a sample case so laminar model only.

DefaultFaces BC is there but there are no faces assigned to it (I have to remove it).

The grid is quite coarse, but good for its purpose.

Here is the checkmesh result:

Code:

/*---------------------------------------------------------------------------*\

| ========= | |

| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |

| \\ / O peration | Version: 2.1 |

| \\ / A nd | Web: www.OpenFOAM.org |

| \\/ M anipulation | |

\*---------------------------------------------------------------------------*/

/* Windows 32 and 64 bit porting by blueCAPE: http://www.bluecape.com.pt *\

| Based on Windows porting (2.0.x v4) by Symscape: http://www.symscape.com |

\*---------------------------------------------------------------------------*/

Build : 2.1-c62f134541ee

Exec : checkmesh

Date : Mar 30 2012

Time : 12:09:17

Host : "UFFTECNICO7"

PID : 2072

Case : C:/TAPS/CFD/cascmurotest

nProcs : 1

SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

fileModificationChecking : Monitoring run-time modified files using timeStampMaster

allowSystemOperations : Disallowing user-supplied system call operations

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

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats

points: 406885

faces: 1140167

internal faces: 1080679

cells: 367648

boundary patches: 4

point zones: 0

face zones: 0

cell zones: 0

Overall number of cells of each type:

hexahedra: 356140

prisms: 2740

wedges: 0

pyramids: 0

tet wedges: 18

tetrahedra: 0

polyhedra: 8750

Checking topology...

Boundary definition OK.

Cell to face addressing OK.

Point usage OK.

Upper triangular ordering OK.

Face vertices OK.

Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...

Patch Faces Points Surface topology 

defaultFaces 0 0 ok (empty) 

inlet 262 318 ok (non-closed singly connected) 

outlet 48316 49856 ok (non-closed singly connected) 

walls 10910 11571 ok (non-closed singly connected) 

Checking geometry...

Overall domain bounding box (-0.035 -0.03 -0.03) (0.035 0.36 0.2)

Mesh (non-empty, non-wedge) directions (1 1 1)

Mesh (non-empty) directions (1 1 1)

Boundary openness (-3.8139e-015 6.38513e-016 8.69605e-016) OK.

Max cell openness = 3.55749e-016 OK.

Max aspect ratio = 7.29527 OK.

Minumum face area = 1.76004e-007. Maximum face area = 6.04908e-006. Face area magnitudes OK.

Min volume = 9.94385e-011. Max volume = 1.2288e-008. Total volume = 0.00265921. Cell volumes OK.

Mesh non-orthogonality Max: 47.0849 average: 4.61111

Non-orthogonality check OK.

Face pyramids OK.

Max skewness = 1.94815 OK.

Coupled point location match (average 0) OK.

Mesh OK.

End

I quite agree with Phicau, maybe it's nothing to be worried.

I just needed a confirmation that my BC were reasonables.

Just in case, here is a small movie of what's happening: http://www.box.com/s/8c79ad85af98d9405da9

Anyway I'm testing the case using a bigger domain...

Daniele

Dear all, my cases with an outlet worked fine in OF 1.7.1 but now with OF 2.1.x there is no outflow anymore, alpha1 gets reflected at the outflow. Is there a change in the versions? otherwise it must be due to some changes i did in the fvSchemes and fvSolution files...

using PISO instead of PIMPLE solves the problem

Ok turning old searching the cause of alpha1 being reflected at the outflow, I finally got it (its not about PISO or PIMPLE). Maybe this is a bug dependent on ubuntu version, but it is quite relevant. The difference between the two pictures below showing an outflow of a channel is only that I moved the grid from positive x quadrant to negative x quadrant. When the whol gid lies at a position that the x-coordinates are smaller than 0 the outflow works! Maybe this should be reported.

I changed p_rgh from type outletInlet outletValue uniform 0 to zeroGradient and the reflection of alpha1 at the outlet vanishes. Anyway I'd be happy for any explanation why a shift of the grid from negative to positive coordinate system quadrant can cause such behavior when outletValue uniform 0 is used for p_rgh.