[clarinha]

Hi everyone,

I am trying to simulate free-surface flow over a river. The riverbed is very detailed, obtained from high-resolution topographic data. The mesh resolution is 2 mm across the domain. The idea is to run a range of velocities and flow depths, with which I will obtain drag and friction factor exerted by the riverbed. I would like to simulate the river reach only, without adding a channel upstream to allow flow development. I am also interested in capturing the free surface distortions caused by the bed topography once the flow is stabilised.

For this purpose, I am using interFoam and cyclicAMI at the inlet and outlet. The turbulence model is RNG k-epsilon. For the sake of the simulation, the bed slope is 2 degrees.

The issue with the simulation is that water (alpha.water > 0.5) and, thus, the free surface are not being correctly “mapped” from outlet to inlet, though the patches show similar values of the variables, which is strange. As a result, the water level is near zero near the inlet because water does not recycle from the outlet. I have tried both createPatchDict and the manual editing of the boundary file to implement cyclicAMI. I use setFieldsDict to define the initial water volume. Please find attached some relevant files. If it’s something related to the implementation of the cyclicAMI or another misstep, I’d be happy if you could help me identify the possible cause, and I’m also happy to provide further details of the model.

Cheers,
Clarinha

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2306                                  |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    arch        "LSB;label=32;scalar=64";
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

6
(
    inlet
    {
        type            cyclicAMI;
	neighbourPatch	outlet;
	transform	translational;
	separationVector	(2.01876947 0 -0.07049698);
        nFaces          1596;
        startFace       1923927;
    }
    outlet
    {
        type            cyclicAMI;
	neighbourPatch	inlet;
	transform	translational;
	separationVector	(-2.01876947 0 0.07049698);
        nFaces          1560;
        startFace       1925523;
    }
    top
    {
        type            patch;
        nFaces          46056;
        startFace       1927083;
    }
    leftWall
    {
        type            wall;
        inGroups        1(wall);
        nFaces          5633;
        startFace       1973139;
    }
    rightWall
    {
        type            wall;
        inGroups        1(wall);
        nFaces          5797;
        startFace       1978772;
    }
    bed
    {
        type            wall;
        inGroups        1(wall);
        nFaces          46288;
        startFace       1984569;
    }
)

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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2306                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0.001;

boundaryField
{
    "(inlet|outlet)"
    {
	type		cyclicAMI;
    }
    top
    {
	type		totalPressure;
	p0		uniform 0;
    }
    "(leftWall|rightWall|bed)"
    {
	type		fixedFluxPressure;
    }

}


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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2306                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    "(leftWall|rightWall|bed)"
    {
        type            zeroGradient;
    }
    top
    {
        type            inletOutlet;
	inletValue	uniform 0;
	value		uniform 0;		
    }
    "(inlet|outlet)"
    {
	type		cyclicAMI;
    }

}

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

[VRN]

Hello Clarinha,

This is unfortunately a know shortcoming in the formulation of the interFoam solver. The problem arises because the solver uses a single pressure system for simplicity; combining the static and hydrostatic pressure to give the modified pressure (p_rgh). In the solver algorithm, the modified pressure equation is solved.

When you have a cyclic boundary where the two boundaries are at different heights (physically) there is a pressure jump across the boundaries due to the different values of h at either sides of the boundary, leading to unphysical behaviours.

Some workarounds have been suggested in previous discussions in the community forums (Ref thread https://www.cfd-online.com/Forums/sh...d.php?p=335817.), but I have not tried to implement them so cannot comment on their accuracy.

Good luck!