CFD Online Discussion Forums - [mesh manipulation] Generating nonuniform meshes with sizefunction

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

- OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)

- - [mesh manipulation] Generating nonuniform meshes with sizefunction (https://www.cfd-online.com/Forums/openfoam-meshing/61812-generating-nonuniform-meshes-sizefunction.html)

Generating nonuniform meshes with sizefunction

Is it possible to generate non-uniform grids with nodes positioned following a distribution expressed by an analitical function?

Regards,
Alberto

Yes. Generate a uniform mesh

Yes. Generate a uniform mesh and then move the points :-)

Hrv

Yes. Generate a uniform mesh

Yes. Generate a uniform mesh and then move the points :-)

Hrv

Do you mean with the moveMesh

Do you mean with the moveMesh solver?
I gave a look, but it doesn't seem I can use a user defined function but only linear, quadratic and exponential (I need an hyperbolic tangent).

Alberto

How about just doing a little

How about just doing a little custom code like this:

pointField newPoints = mesh.points();

forAll (newPoints, i)
{
// Your code here, calculate the point position
}

mesh.movePoints(newPoints);

mesh.write();

Hrv

Thanks Hrv. It works! :-)

Thanks Hrv. It works! :-)

Hi Alberto, Could you possi

Hi Alberto,

Could you possibly give an example of how to move the internal points of a uniform mesh? (Just the few lines within the forAll(newPoints,i){} )

Thanks, Frank

Check your mail :-) A.

Check your mail :-)

A.

Hi I want to solve channel f

Hi
I want to solve channel flow with hyperbolic mesh in one direction. i am new in O-F, how can i generate hyperbolic mesh in O-F?
Regards
Thanks for your help

Hello Ehsan, the trick is exa

Hello Ehsan,
the trick is exactly the one explained by Hrvoje in this thread.

Create a uniform mesh, with the number of nodes you need in the three directions. Then write a small utility which:

- Reads the mesh (see how this is done in all solvers or mesh manipulation utilities).

- Does

pointField newPoints = mesh.points();

forAll (newPoints, i)
{
// Your code here, calculate the point position
}

mesh.movePoints(newPoints);

mesh.write();

using an analytical expression to relate the position of a node in a uniform grid to the new position (this is commonly done to generate grids for channel flow simulations).

Regards,
Alberto

Hello Alberto Thank you very

Hello Alberto
Thank you very much for your guide.
Could you possibly give your code? And tell me where should I add this code?
Excuse me for my basic question because I am new in O_F.
Best regards

hello Alberto Thank you very

hello Alberto
Thank you very much for your help,it works well.
Best Regards.

You're welcome :-) Happy ne

You're welcome :-)

Happy new year,
Alberto

Happw new year Alberto I am

Happw new year Alberto

I am going to run a channel395 with channel oodles solver, when i choose mixedsmagorinskey model and laplace filter, after some iteration, courant number diverged. but when i used simple filter it works,and also when i changed the mesh into uniform mesh, it works.

Do you have any idea about this problem?
Best Regards.

Hello Alberto, Thanks for y

Hello Alberto,

Thanks for your hyperbolicSpacingChannel code. It works well with the given channel395 case.

Thanks.

Hi, I would like to output the polyMesh in a new time directory. I tried to add

Code:

runTime++;

    

mesh.write();

Unfortunately, at runtime I get:

Code:

Requested field U does not exist in the database





    From function Foam::fieldAverage::initialise()

    in file fieldAverage/fieldAverage.C at line 108.



FOAM exiting

So how can I output in a new time directory, the same way renumberMesh or snappyHexMesh do ?

To be more accurate, here is my new code

Code:

#include "argList.H"

#include "Time.H"

#include "polyMesh.H"

#include "transformField.H"



#include "fvMesh.H"



using namespace Foam;



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

//  Main program:



int main(int argc, char *argv[])

{

#   include "setRootCase.H"

#   include "createTime.H"

#   include "createMesh.H"



    pointField points=mesh.points();

    

    // Reading non-uniform grid parameters



    Info<< "Reading hyperbolicSpacingProperties\n" << endl;



    IOdictionary hyperbolicSpacingProperties

    (

        IOobject

        (

            "hyperbolicSpacingProperties",

            runTime.constant(),

            polyMesh::meshSubDir,

            runTime,

            IOobject::MUST_READ,

            IOobject::NO_WRITE,

            false

        )

    );



    Info<< "Reading A coefficient\n" << endl;



    dimensionedScalar A

    (

        hyperbolicSpacingProperties.lookup("A")

    );



    Info<< "A = " << A.value() << endl << endl;

    

    Info<< "Reading B coefficient\n" << endl;

    

    dimensionedScalar B

    (

        hyperbolicSpacingProperties.lookup("B")

    );

    

    Info<< "B = " << B.value() << endl << endl;

    

    // Adapting the grid

    

    points.replace(vector::Y, A.value()*points.component(vector::Y) + 

                (1.0 - A.value())*(1.0 - Foam::tanh(B.value()*(1.0 - 

                points.component(vector::Y)))/(Foam::tanh(B.value()))));



    

    // Setting the default precision of the points data to 10

    IOstream::defaultPrecision(10);

    

    mesh.movePoints(points);

    

    runTime++;

    

    mesh.write();

    

    //Writing points

    // Info << "Writing points into directory " << points.path() << nl << endl;

    // points.write();



    return(0);

}

It might be very naive, but I have still not completely grasped how data is organized in OpenFOAM.

Dear John,

this error is not at all obvious ;-)

My bet is that you have a functionObject (fieldAverage to be precise) which I asking for U, but cannot find it.

Comment it and all will be fine - I hope :o

Henrik

I think one day I saw a piece of code which deactivated functionObjects, but I can not find it again. Do you see what I am refering to ?

-EDIT-

Just found it, it seems to be the

Code:

functionObjectlist::off()

method. I'll try this next time I have a grip on a work station.

Dear John,

the keyword is "active_" ...

$FOAM_SRC/postProcessing/forces/lnInclude/forces.H

Henrik