4
$\begingroup$

I am studying the performance of volumetric solar receivers (specifically ceramic foams) versus the change of many parameters: solar flux, surface temperature, porosity, pore diameter, flow pressure and flow velocity. I have seen two ways in the literature to model porous media:

  1. Drawing a complex 3D structure that is analogous to the porous zone.

While this might be a very-problem-specific solution, but turbulence modelling in that case is not a problem.

  1. Averaging the governing partial differential equations to account for the nature of porous media and introducing new terms to the equations (porosity $\epsilon$ and superficial velocity).

And this is the approach I am taking which is used in porous models in many CFD solvers.

However, while reading about the treatment of turbulence in porous media in the FLUENT user guide I found that turbulence is not exactly modelled:

turbulence in the medium is treated as though the solid medium has no effect on the turbulence generation or dissipation rates. This assumption may be reasonable if the medium's permeability is quite large and the geometric scale of the medium does not interact with the scale of the turbulent eddies. In other instances, however, you may want to suppress the effect of turbulence in the medium.

I find "medium's permeability is quite large" quite ambiguous (What values are considered large?) and don't know whether my model will be badly affected by this treatment or not and to what extent?

So has anyone came through this before? or am I overcomplicating things for a parametric study?

$\endgroup$
4
$\begingroup$

It is just saying that since there is no turbulence or dissipation being computed; your solution will be less accurate for lower and lower permeability. As I read it; eddy currents in this model will cross the medium. For a thin wire fence this would match reality; for a furnace filter it would not because the air is laminar as it exits the filter. The extent to which this assumption affects your solution depends on your geometry and how much the turbulence affects your measured results.

I recommend you post on the CFD-Online Fluent Forum.

Here are some existing forums that may be of use: Porous Fluent CFD-Online search

You may want to consider an opensource solver for this situation as opposed to closed source fluent that has undesirable assumptions:

OpenFOAM Website
A Porous Media in OpenFOAM Forum
Porous Media in OpenFOAM
Porous Media and Heat Transfer In OpenFOAM

$\endgroup$
  • $\begingroup$ Thanks for the useful links Eric, Do you have any idea if turbulence is treated differently in OpenFOAM? $\endgroup$ – Algo Jan 3 '16 at 5:52
  • $\begingroup$ I am not an expert in this, but it does support porous multiphase so there is a good possibility it would support turbulence modeling inside the porous medium. Here is a paper on it: sourceforge.net/projects/openfoam-extend/files/… $\endgroup$ – ericnutsch Jan 4 '16 at 1:26
1
$\begingroup$

Short answer: The FLUENT approach is trivial.

Many information are lost due to the space-averaging process - over a representative elementary volume - of the governing equations (which is the essence of every porous model that tries to avoid the complexity of the real geometry of the porous media), So any turbulence model is not to "reproduce the fine structure dynamics of the flow but to take into account information embedded in smaller scale for large scale modelization."[1]. The FLUENT approach simply ignores this fact or even assumes that there is no turbulence energy dissipation or generation due to the porous zone (similar approach was taken by Antohe and Lage to develop a new turbulence model that lead to trivial solutions ($k = 0$ or $\epsilon = 0$)).

I found that STAR-CCM+ code follows a similar way in turbulence treatment:

The effect of a porous region on turbulent flow depends on the internal structure of the porous medium. Where turbulence is present, the turbulence scales are determined from the geometric structure of the porous medium. As it is not possible for STAR-CCM+ to predict the turbulence scales directly, you specify the appropriate values on the porous region. Turbulence quantities in fluid leaving the porous region are constructed from the user-defined values; they are not transported from the upstream side of the porous region.

So, I think if you are pragmatic enough to have a model that can sacrifice the accuracy of results of the turbulence model you use, these assumptions are the best you can get.

[1] $k–\epsilon$ Macro-scale modeling of turbulence based on a two scale analysis in porous media - Francois Pinson, Olivier Gregoire, and Olivier Simonin.

[2] A new turbulence model for porous media flows. Part I: Constitutive equations and model closure - Federico E. Teruel and Rizwan-uddin.

$\endgroup$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.