[alberto]

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

Regards,
Alberto

[hjasak]

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

Hrv

[hjasak]

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

Hrv

[alberto]

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

[hjasak]

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

[alberto]

Thanks Hrv. It works! :-)

[lr103476]

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

[alberto]

Check your mail :-)

A.

[ehsanyasari]

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

[alberto]

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

[ehsanyasari]

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

[ehsanyasari]

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

[alberto]

You're welcome :-)

Happy new year,
Alberto

[ehsanyasari]

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.

[asaha]

Hello Alberto,

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

Thanks.

[johndeas]

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

runTime++;
    
mesh.write();

Unfortunately, at runtime I get:

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 ?

[johndeas]

To be more accurate, here is my new 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.

[henrik]

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

Henrik

[johndeas]

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

functionObjectlist::off()

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

[henrik]

Dear John,

the keyword is "active_" ...

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

Henrik