Porosity and permeability in PorousInterFoam
 

Dear all,

I'm trying to understand how to set porosity and permeability in porousInterFoam solver.

For example:
- porosity = 0.8
- permeability = 1.e-9 m2
and defining D = 0.8/1.e-9

I'm using the following in the porousZones dictionary for a isotropic media.

{
note "Reinforced Media";
porosity 0.8;
Darcy
{
d d [ 0 -2 0 0 0 0 0 ] ( -1 D -1 );
f f [ 0 -1 0 0 0 0 0 ] ( 0 0 0 );
}
}

Is this correct?

Which is the mathematical formulation for continuity, momentum and volume fraction equations used in porousInterFoam? Does porosity appears in all equations?

thanks,

hi,

a difinition of porous zone and f,d is introduced in source file of porous zon

Hi Khattab,

Thanks for your reply.

I took a look at the porousZone.H file.

In the definition of the the S (line 50), there is no reference for the porosity. It seems that if the media has a porosity different than one all you need to do is to explicitly specify it at the "constant/porousZones" dictionary, however I've been solving some problems with the porousInterFoam solver and I only get reasonable (actually corrected) results when I multiply S by the porosity.

I'm getting the results I need, however this "little trick" is bothering me, since I'm not sure about the correct formulation and I may be doing something wrong.

Did you have this problem (or something like this) before?

Thanks,

Hi,

i think this PDF will be helpful.

http://www.tfd.chalmers.se/~hani/kur...ukurReport.pdf

GOOD LUCK

Hi,

thanks again for your reply.

Actually, I've got the idea of multiplying the source term by the porosity when I was reading this tutorial for the first time. I saw in Eq. (1) of the tutorial that gamma (porosity) is used only for the transient term, than I did

D = porosity/permeability instead of D = 1./permeability

and got reasonable results (actually results are good).

I understand that this is an approximation since all terms of the momentum equation should be multiplied by the porosity. Am I right?

I can not understand why only the transient term is multiplied by the porosity in the porous media model.

Hello Jeferson,

I have actually the same kind of Problem.
Even if the porosity does not have anything to do with D and F. It does not occur in openfoam native porous media library.

You had a good idea about your little trick, I have to test it.
But are you sure about the formula : D = porosity/permeability?

Because bigger is D, slower the fluid runs through the porouszone right?
And technically smaller is the porosity, slower the fluid runs through the porouszone?

So It´s quite wrong if you do D = porosity/permeability?

It´s not better to do : D = 1/(permeability*porosity) ?

Thanks for your reply.

Cheers

Hi,

I really never understood why my "trick" works. However, I have tested it many times and it works. At least in version 2.1.1 (also in older 2.* versions).

I know that version 2.3 has a problem, and as long as I know, the porous media model does not work well in this version. I've tried to upgrade to version 2.3 once and had to return to the old 2.1.1.

Thanks,

Jeferson

Hi all,


For real two-phase flow in porous media solver, you can have a look at this thread: http://www.cfd-online.com/Forums/ope...-openfoam.html

And keep in mind that porousInterFoam can be used only when very strong assumptions are satisfied (no capillarity, sharp interface...)...

Best,

Hello Jeferson,

I tested your trick on OF 2.2 and :
IT´s WORKING !

I don´t know why too but results still really similar with PAM RTM about resin injection.

The problem still, I cant explain that.

Well, thanks a lot for your messages.

Best regards and Happy New Year !

Dear All,

I'm a new user of OpenFoam, I want to modelling water flow in porous media.
Not clear for me how to calculate D and F numbers.
D=porosity/permeability, am I right? But this is only 1 number. d (0 0 0) how can I calculate all three coordinates?
Sorry for the stupid question.

Thanks for your reply.

Hello,

the permeability is a tensor. The 3 components that you have to specify go on the diagonal of the tensor D, have a look at the source code to see how D is constructed. If your porous media is isotropic the x-y-z entries are equal, for anisotropic media they are not.

Hope this help!

Andrea

hello Oruzeaz !
This is not a stupid question !

I´m using OpenFOAM since September ! So I know how complicated it is to try to understand all the little tricks of this Software.
And not everything is clear ! So it´s a pleasure to try to help you.

about F, I´ve never touch it, It´s might be for really special cases.
about D, if you check it is in m^-2 so it looks like 1/permeability (because of permeability is in m² of course)

about the question of introducing the porosity, if you check the porousInterFoam solver, this latter dont support the "porosity" parameter.
As said the devellopers here : http://openfoam.org/mantisbt/view.php?id=477

Just saying : find it how to set up by your self! lol

Here Jeferson tried to introduce the porosity into D by doing :
D = porosity/permeability
and it seems it´s work, I did it by my self and the results are similar to PAM-RTM (for me about resin injection) not exactly perfect but really near to!!

As said Andrea, permeability is a Tensor, because the permeability can be different depends on the direction of the fluid. It means in your porous media, your fluid can move faster in X than in Y or Z direction. Just depends the settings of your porous media. Then to Quote Andrea : If your porous media is isotropic the x-y-z entries are equal, for anisotropic media they are not.

I hope what I said was helpful for you!
Good luck about your work!

Hallo Andrea,

thank you for your answer, it was helpful. I have another question. How can I calculate f?
When I use it?

Eszter

Hello,

take a look at the source code:

src/finiteVolume/cfdTools/general/porosityModel/DarcyForchheimer/DarcyForchheimer.H

you 'll find a small description of the coefficients.

f is the Forchheimer coefficient [1/m] and should be use when inertial effects are not negligible. Both d and f are case-dependent coefficients that are usually calculated from experimental data (or simulations), so you should know them for your case.

Hope this help!

Andrea

hi foamers,
i gonna set the darcy number 10e-5, but i don't know how to use d and f in porosityproperties,
if anyone knows please help me!
thanks