[val46]

Hello,

i have a thermal conduction problem.
I need to modell a cylinder with different conductivity values in x,y and z direction. The cylinder is within a metal tube (isotropic material )

I think i can simply create 3 variables in transportproperties. Let's say lambdaX, lambdaY and lambdaZ. But after that i haven't a glue what to do next. (I'm pretty new to OpenFoam).


Thanks in advance.

Toni

[benk]

You just need to make a volTensorField for your thermal conductivities. In your time=0 directory, create your conductivity field using something like:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volTensorField;
    object      Ds;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -1 0 0 0 0];

internalField   uniform (xx 0 0 0 yy 0 0 0 zz);

boundaryField
{
...
}

where xx yy and zz are the values in the 3 different directions.

[val46]

Hi,

thanks for your reply.

How will the solver recognize the new file?
Don't i have to modify the solver for that?

[benk]

You'll have to add the field by:

volTensorField lambda
(
IOobject
(
"lambda",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

Or you could also just make a tensor in your transportProperties file and read it into your solver using

dimensionedTensor lambda(transportProperties.lookup("lambda"));

[gouravjee]

Originally Posted by benk

You just need to make a volTensorField for your thermal conductivities. In your time=0 directory, create your conductivity field using something like:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volTensorField;
    object      Ds;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -1 0 0 0 0];

internalField   uniform (xx 0 0 0 yy 0 0 0 zz);

boundaryField
{
...
}

where xx yy and zz are the values in the 3 different directions.

can you tell me where to put this code as i am having other properties in transportProperties file which doesnt changes in directions

[pete20r2]

Hi Val,
What solver are you using?
Since it's cylindrical, do you want cartesian defined conductivities (x y z) or cylindrical coordinates (ρ,φ,z).
I can help if you are using multi-region solvers such as cht.

Benk's code goes in you solver source, which would then need to be recompiled, are you at that level?

Regards
Peter

[piu58]

If the temperature distribution outside the cylinder is of lesser interest, or if the conductivity there is much larger than in the cylinder, you may think about a coordinate transformation: Change the cross section of the cylinder for a circle to an ellipse according the proportion of conductivity and change its length too.

This gives you at least a forst idea of the solution.

[mwaqas]

Originally Posted by pete20r2

Hi Val,
What solver are you using?
Since it's cylindrical, do you want cartesian defined conductivities (x y z) or cylindrical coordinates (ρ,φ,z).
I can help if you are using multi-region solvers such as cht.

Benk's code goes in you solver source, which would then need to be recompiled, are you at that level?

Regards
Peter

Hi Peter,


I am using cht to model heat transfer between fluid and solid. suppose I have a cylinder and fluid passing across the cylinder. Could you please help me to define anisotropic thermal conductivity. It would be great, if I don't need to recompile a solver.
I am using Cartesian coordinate system. Along radial direction (x and y coordinate) thermal conductivity is same but it is different along axial direction.
Moreover, in both direction (radial and axial), it is temperature dependent.
Thank you


Regards

[pete20r2]

Hi Muhammad,
My example did not use temperature dependent capacity functions but that shouldn't be too hard to add.
To implement a cylindrical coordinate system edit the thermophysicalProperties file of the domain and make it look like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            heSolidThermo;
    mixture         pureMixture;
    //transport       constIso;
    transport       constAnIso; //<--this bit
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

coordinateSystem //<-- and this bit
{
    type    cartesian;  // global co-ordinate system (redundant)
    origin  (-0.009 0.017861 0);   
    coordinateRotation
    {
        type    cylindrical; // local Cartesian co-ordinates
        //e1      (1 0 0);
        e3      (0 0 1); // axis of rotation
    }
}

mixture
{
    specie
    {
        nMoles      1;
        molWeight   50;
    }

    transport
    {

	kappa   (.1 10 10); //radial tangential longitudinal
    }

    thermodynamics
    {
        Hf      0;
        Cp      50;
    }

    equationOfState
    {
        rho     1000;
    }
}

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

To implement the temperature dependent heat capacity have a look at https://cfd.direct/openfoam/user-guide/thermophysical/
Section 7.1.3, you will probably want janaf or polynomial.

[bharadwaz]

Originally Posted by pete20r2

Hi Muhammad,
My example did not use temperature dependent capacity functions but that shouldn't be too hard to add.
To implement a cylindrical coordinate system edit the thermophysicalProperties file of the domain and make it look like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            heSolidThermo;
    mixture         pureMixture;
    //transport       constIso;
    transport       constAnIso; //<--this bit
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

coordinateSystem //<-- and this bit
{
    type    cartesian;  // global co-ordinate system (redundant)
    origin  (-0.009 0.017861 0);   
    coordinateRotation
    {
        type    cylindrical; // local Cartesian co-ordinates
        //e1      (1 0 0);
        e3      (0 0 1); // axis of rotation
    }
}

mixture
{
    specie
    {
        nMoles      1;
        molWeight   50;
    }

    transport
    {

	kappa   (.1 10 10); //radial tangential longitudinal
    }

    thermodynamics
    {
        Hf      0;
        Cp      50;
    }

    equationOfState
    {
        rho     1000;
    }
}

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

To implement the temperature dependent heat capacity have a look at https://cfd.direct/openfoam/user-guide/thermophysical/
Section 7.1.3, you will probably want janaf or polynomial.

what to take as origin
is it center of the cylinder

Thank you

[eugenioS]

Dear all,

I'm trying to verify the chtMultiRegionFoam (v1706) for the case of anisotropic conductivity (kappa). I'm comparing the results obtained with the following two configurations:

1. Isotropic mode, where I set the following:

thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

mixture
{
...
transport
{
kappa 170;
}
...
}

2. Anisotropic mode:

thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constAnIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}

mixture
{
...
transport
{
kappa (170 170 170);
}
...
}

For some reason, the results are different (the isotropic case is correct). Anyone here knows why the anisotropic case doesn't replicate the results? Do you see something that is wrongly set in thermophysical properties?

Thank you in advance,

Eugenio

[shach934]

Hi,
just a hint, when you are using constAnIso solid, be sure at the boundary condition T you are using directionalSolidThermo at kappaMethod. Also add a aniAlpha. The names I am not very sure, you may google it. Maybe this is the reason.

Originally Posted by eugenioS

Dear all,

I'm trying to verify the chtMultiRegionFoam (v1706) for the case of anisotropic conductivity (kappa). I'm comparing the results obtained with the following two configurations:

1. Isotropic mode, where I set the following:

thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

mixture
{
...
transport
{
kappa 170;
}
...
}

2. Anisotropic mode:

thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constAnIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}

coordinateSystem
{
type cartesian;
origin (0 0 0);
coordinateRotation
{
type axesRotation;
e1 (1 0 0);
e2 (0 1 0);
}

mixture
{
...
transport
{
kappa (170 170 170);
}
...
}

For some reason, the results are different (the isotropic case is correct). Anyone here knows why the anisotropic case doesn't replicate the results? Do you see something that is wrongly set in thermophysical properties?

Thank you in advance,

Eugenio

[eugenioS]

Originally Posted by shach934

Hi,
just a hint, when you are using constAnIso solid, be sure at the boundary condition T you are using directionalSolidThermo at kappaMethod. Also add a aniAlpha. The names I am not very sure, you may google it. Maybe this is the reason.

Thank you! This was actually the problem..

I needed to define the boundary condition in internal walls (between solids) in the following way:

nonIsotropicWall
{
...
kappaMethod directionalSolidThermo;
alphaAni Anialpha;
...
}

[shach934]

Good to hear that!
However, I remember I had a problem about this directionalSolidThermo function. Though the result is correct, the wall heat flux calculated by wallHeatFlux function is not correct. I am not sure if its due to my setting or the function itself. So, be careful if you are using wallHeatFlux to calculate the heat flux.

Originally Posted by eugenioS

Thank you! This was actually the problem..

I needed to define the boundary condition in internal walls (between solids) in the following way:

nonIsotropicWall
{
...
kappaMethod directionalSolidThermo;
alphaAni Anialpha;
...
}

[mikulo]

Originally Posted by shach934

Good to hear that!
However, I remember I had a problem about this directionalSolidThermo function. Though the result is correct, the wall heat flux calculated by wallHeatFlux function is not correct. I am not sure if its due to my setting or the function itself. So, be careful if you are using wallHeatFlux to calculate the heat flux.

Hey,

May I ask, what do you mean by the wall heat flux function? Are you referring to externalWallHeatFluxTemperature boundary condition?

Regards,
Mike

[eugenioS]

Hello,

I think he is referring to the post process that evaluates the heat flux at boundaries, not to the boundary condition.

Regards

[mikulo]

Originally Posted by eugenioS

Hello,

I think he is referring to the post process that evaluates the heat flux at boundaries, not to the boundary condition.

Regards

Hey,

Thanks for your response. However, I do found a problem with regard to the boundary condition as well. If you have tried and tested it well, please share your thoughts. Thanks!

Regards,
Mike

[bikooo3878]

Thank you, sir! I've been looking for the reason of the unphysical results for a couple of days and thought it had something to do with the coordinate system or a numerics issue. directionalSolidThermo solved it!