[zhxter]

hi, Foamers,

I am now trying to establish a 2D numerical wave tank(NWT) using OpenFOAM.

The left boundary of the rectangular NWT is moving to generate waves. Suppose the name of the patch is set "movingWall", and in the dynamicMeshDict, the contents are as follows,

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh dynamicMotionSolverFvMesh;

motionSolverLibs ("libfvMotionSolvers.so");

solver displacementLaplacian;

displacementLaplacianCoeffs
{
diffusivity inverseDistance 1 (movingWall);
}

My question is : what does the number "1" after the inverseDistance mean?

[dduque]

It's just the number of patches that are listed next. I just found out myself...

[john myce]

Hi guys,

I am also working on dynamic mesh. Does anyone know the meaning of the coefficient set for the following diffusivity methods:

directional (1 200 0);
exponential 5 inverseDistance (...);
motionDirectional (1 1000 0);

I guess they are related to each coordinate axis but I still don't know the meaning of the number setting up.

Cheers,

[john myce]

I'm coming with some updates:

for the coefficient to provide for the exponential method, it is the exponent of the function to calculate the diffusivity:

Foam::exponentialDiffusivity::operator()() const
{
    return exp(-alpha_/basicDiffusivityPtr_->operator()());
}

from /src/fvMotionSolver/motionDiffusivity/manipulators/exponential/exponentialDiffusivity.C

For the directional & motiondirectional methods, I still don't know if it is just the distance in each coordinate axis or the mean non-orthogonality (first coefficient) and mean skewness (second).

References :http://www.tfd.chalmers.se/~hani/kur...h_openfoam.pdf page 23 &
http://www.tfd.chalmers.se/~hani/kur...AM-rapport.pdf from page 11 to 14

Cheers,

[Michael@UW]

Originally Posted by john myce

I'm coming with some updates:

for the coefficient to provide for the exponential method, it is the exponent of the function to calculate the diffusivity:

Foam::exponentialDiffusivity::operator()() const
{
    return exp(-alpha_/basicDiffusivityPtr_->operator()());
}

from /src/fvMotionSolver/motionDiffusivity/manipulators/exponential/exponentialDiffusivity.C

For the directional & motiondirectional methods, I still don't know if it is just the distance in each coordinate axis or the mean non-orthogonality (first coefficient) and mean skewness (second).

References :http://www.tfd.chalmers.se/~hani/kur...h_openfoam.pdf page 23 &
http://www.tfd.chalmers.se/~hani/kur...AM-rapport.pdf from page 11 to 14

Cheers,

Hi John,
Thank you for sharing! I read the reference at http://www.tfd.chalmers.se/~hani/kur...AM-rapport.pdf. It says "the first number determines the mean cell non-orthogonality; while the second number determines the mean cell skewness."

But I doubt the parameters in directional is a vector to control the diffusivity in 3 directions. As I found the code in directionalDiffusivity.C

void Foam::directionalDiffusivity::correct()
{
    const surfaceVectorField n(mesh().Sf()/mesh().magSf());
    faceDiffusivity_ == (n & cmptMultiply(diffusivityVector_, n));
}

Can you confirm that?

Thanks!

Michael

[Michael@UW]

Originally Posted by zhxter

hi, Foamers,

I am now trying to establish a 2D numerical wave tank(NWT) using OpenFOAM.

The left boundary of the rectangular NWT is moving to generate waves. Suppose the name of the patch is set "movingWall", and in the dynamicMeshDict, the contents are as follows,

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dynamicFvMesh dynamicMotionSolverFvMesh;

motionSolverLibs ("libfvMotionSolvers.so");

solver displacementLaplacian;

displacementLaplacianCoeffs
{
diffusivity inverseDistance 1 (movingWall);
}

My question is : what does the number "1" after the inverseDistance mean?

Hi Xintao,
I found the number 1 appears in some tutorials but not in some others. Just wondering if it is optional or not.

Thanks,
Michael

[john myce]

Hi Michael,

I have still a doubt of what we clearly provide as an input for the coefficients.
I tried different values but without any revelation.

Anyway thanks for providing this part of the code.
I have found at this link:
https://www.openfoam.com/documentati...89434350fa0f17

Sf returns cell face area vectors.
magSf returns cell face area magnitudes.
cmptMultiply is scaling two tensors : n which gathers Sf/magSf (cell unit vector) & the one which gathers the user-defined coefficients.

So I definitely think that it does not control the diffusivity in 3 directions but instead (tell me if I am wrong), calculating the diffusivity using the user-defined diffusivity vectors and the unit normal vectors of each face.

Cheers

[john myce]

Originally Posted by Michael@UW

Hi Xintao,
I found the number 1 appears in some tutorials but not in some others. Just wondering if it is optional or not.

Thanks,
Michael

Regarding this question, you don't have to provide this coefficient but if you provide it with the wrong number of patches declared, the meshing process will not running.