In this blog post, I will try to give a description of the governing equation of the ** laplacianFoam** in OpenFOAM that solves a simple Laplace equation, e.g. for thermal diffusion in a solid.

Governing Equation |

The heat conduction equation is given by the following equation:

\begin{align}

\frac{\partial T}{\partial t} = \frac{1}{\rho c_p} \nabla \cdot \left(k \nabla T\right) + \frac{q}{\rho c_p}, \tag{1} \label{eq:conductionEqn}

\end{align}

where \(T\;{\rm [ K]}\) is the absolute temperature field, \(\rho\;{\rm [kg/m^3]}\) is the density field, \(q\;{\rm [W/m^3]}\) is the rate of energy generation per unit volume, \(k\;{\rm [W/(m\cdot K)]}\) is the thermal conductivity and \(c_p\;{\rm [J/(kg\cdot K)]}\) is the specific heat at constant pressure.

If the heat capacity \(\rho c_p\) is spatially uniform, the Eq. \eqref{eq:conductionEqn} can be transformed into the following form irrespective of whether the thermal conductivity \(k\) is spatially uniform or not:

\begin{align}

\frac{\partial T}{\partial t} = \nabla \cdot \left(\alpha \nabla T\right) + \frac{q}{\rho c_p}, \tag{2} \label{eq:conductionEqn2}

\end{align}

where \(\alpha = k/\rho c_p\;{\rm [m^2/s]}\) is the thermal diffusivity.

The ** laplacianFoam** (in OpenFOAM-4.x and earlier versions) doesn’t consider the heat generation and the implemented equation is

\begin{align}

\frac{\partial T}{\partial t} = \nabla \cdot \left(\alpha \nabla T\right), \tag{3} \label{eq:laplacianFoam}

\end{align}

but the solver in the latest development version supports the *fvOptions* so that we can solve \eqref{eq:conductionEqn2} and specify a volumetric heat source.

We can find the Eq. \eqref{eq:conductionEqn2} solved in *laplacianFoam.C*.

58 59 60 61 62 63 64 65 66 67 68 69 70 |
while (simple.correctNonOrthogonal()) { fvScalarMatrix TEqn ( fvm::ddt(T) - fvm::laplacian(DT, T) == fvOptions(T) ); fvOptions.constrain(TEqn); TEqn.solve(); fvOptions.correct(T); } |

The variable *DT* represents the thermal diffusivity \(\alpha\) and it is specified in the *constant/transportProperties* file.

1 2 3 4 5 6 7 8 9 10 11 12 13 14 |
FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // DT DT [0 2 -1 0 0 0 0] 4e-05; // thermal diffusivity m^2/s // ************************************************************************* // |

Comparison with Analytical Solution |

We consider the steady state problem of source-free heat conduction in a concentric cylinder whose inner and outer walls are maintained at constant temperature of 400 K and 300 K respectively. This problem can be analytically solved and the following relation holds for the temperature distribution in the radial direction \(T(r)\):

\begin{align}

\frac{T_1 – T(r)}{T_1 – T_2} = \frac{\ln{(r/r_1)}}{\ln{(r_2/r_1)}}, \tag{4} \label{eq:cylinderT}

\end{align}

where the subscripts 1 and 2 indicate the values at the inner and outer walls respectively shown in Figure 1.

The temperature distribution obtained using * laplacianFoam* is shown in Figure 2 and the comparison between the numerical and analytical solutions is shown in Figure 3. The agreement with the analytical solution is good.

Introduction of Source Term |

In the next post, I’ll deal with a simple example case to introduce how to specify a heat generation source term in * laplacianFoam* using the

*functionality (*

**fvOptions***).*

**scalarSemiImplicitSource**
Thank you.

Thanks! This is helping me with my Thesis!

Actually, the equation (1) is of little wrong. The diffusion term must be

`div(alpha*grad(T))`

rather than simple`alpha*laplacian(T)`

. There is a little difference if alpha is changing with T or spatial coordinate.Thank you for pointing out my mistake. I am going to correct it.

Hi, I am looking into OpenFOAM recently. I am reading , the book of F. Moukalled, L.Mangani and M. Darwish. In the book it is recommended that the thermal conductivity should be interpolated using geometric average rather than algebraic average. However, I cannot find any interpolation implementation of geometric average in OpenFOAM. I think you may be more familiar with it. How to implement one if I want to add an additional interpolation scheme?

Thanks a lot

You might want to try “harmonic” interpolation scheme.

https://github.com/OpenFOAM/OpenFOAM-dev/tree/master/src/finiteVolume/interpolation/surfaceInterpolation/schemes/harmonic

Thanks a lot.

Thank you very much. It is really very much helpful for me. If you allow me I would like to communicate with you.

Excellent contribution for understanding openFOAM.

1000 thanks for your efforts.