[stathisk]

Good evening,
I'm trying to validate fvOptions/explicitPorositySource using pimpleFoam but haven't got any success yet.
Specifically, I used pimpleFoam (openFoam versions 3.0.1 and 4) in various validation cases and my results are always deviating from corresponding results of the literature.
I believe that it has to do with the porosity parameter which can not be explicitly defined in explicitPorositySource.
Nevertheless, I modify d and f coefficients by multiplying porosity and porosity^2 respectively.

For example I try to match a driven cavity case taken by:
Yang et al., Analysis of Momentum Transfer in a Lid-Driven Cavity Containing a Brinkman–Forchheimer Medium.
Transp Porous Med (2012) 92:101–118,
DOI 10.1007/s11242-011-9893-8

with the following parameters:
U = 1 [m/s]
L = 1[m]
nu visc = 0.1
Re = 10
porosity =0.1
Da Darcy= 0.001
K permeability = Da * L^2 = 0.001

resulting explicitPorositySource coefficients:
d coeff = porosity/ K= 100
f coeff = porosity^2 * 2 * Fe / sqrt(K) = 2.858
where Fe= 1.75 / sqrt(150*porosity^3)

As you can see in the attached picture (DrivenCavity.png) my results are not accurate enough.
I've also attached a working example (DrivenCavity.zip) for anyone who would like to give it a try.

Any help is highly appreciated.

Thanks!

[Pedro24]

Hi stathisk,

I'm not sure but i think that the D coefficient unit is m^2 and not Darcy (1 Darcy = 0.97.10^-12 m2).

So D = 0.001 Da is equivalent to 0.97e-15 m^2 in OpenFOAM.


Regards,

Pierre

[stathisk]

Hi Pierre and thank you very much for your answer.

I believe you mean that d coefficient units are m^-2.
You're right about that, I forgot to write it in my previous post.

The input parameter in Yang et al. (2012) study is the Darcy number = 0.001 [dimensionless].
Following the definition of Darcy number we get Da=K/L^2,
which gives us the permeability K=Da*L^2 in [m^2] and not in Darcy units.
So I'm not quite sure that I should multiply Openfoam d coefficient = porosity/ K= 100 [m^-2] with 0.97e-15 m^2.


Best regards,
Stathis

[jf_vt]

Hey I am running a simpleReactingParcelFoam case with a porous layer defined with an explicitPorousSource.
In order to setup my case, I initially turned off chemistry, lagrangian & radiation.
The case converge well ( residual in order of .0001 + some other criteria relevant to this case).

In this context, I have been noticing a slight ( ~2%) increase in mass flow through the porous layer. This mass defect decrease if I decrease the darcy coefficient.

Is this normal? ( based on some reading I will tend to think so as people recommend moving to implicit source when porosity effect on the flow increase)
It does not seem that fvOption support semiImplicitPorousSource- is this correct?

I read stuff about implicit and semiImplicit ( nUCorrectors and so forth...) and I tried to mimic the example angledDuctImplicit tutorial (with simplePorousFoam solver)

But for some reasons I cannot make the simpleReactingParcelFoam read the porosityProperties file... ( while reading the source of these solvers, I don't see any difference in their porosity treatment)

Any ideas what I could do to resolve this issue?
Thanks
JF

[jf_vt]

I wil correst my post above
there is a difference in porosity treatment between simplePorousFoam and simpleReactingParcelFoam.
So one way to gofor me will be to try to modify the original simpleReactingParcelFoam solver to add this porosoty treatment.
But my question in my previous post above regarding the lack of mass conservation when using explicitPorousSources in fvOptions still stands...

Thanks
JF

[Pedro24]

Originally Posted by stathisk

Hi Pierre and thank you very much for your answer.

I believe you mean that d coefficient units are m^-2.
You're right about that, I forgot to write it in my previous post.

The input parameter in Yang et al. (2012) study is the Darcy number = 0.001 [dimensionless].
Following the definition of Darcy number we get Da=K/L^2,
which gives us the permeability K=Da*L^2 in [m^2] and not in Darcy units.
So I'm not quite sure that I should multiply Openfoam d coefficient = porosity/ K= 100 [m^-2] with 0.97e-15 m^2.


Best regards,
Stathis

Hi Stathis,

L is the chacteristic length of your porous medium (particle diameter or throat width) and not the length of your computational domain.

Regards,

Pierre

[stathisk]

Hello!

@Pierre
Yes indeed, some authors consider L as the characteristic length of the porous medium, but I've found many cases in the literature that Da number is defined using the characteristic macroscopic length scale. Yang et al. (2012) article (see my 1st post) is an example.

@JF
Sorry for the late response.
I can't tell you much about the lack of mass conservation in simpleReactingParcelFoam since it's a solver that I've never used before.
Concerning porosity treatment, I was able to improve my results by adding the porosity term in the momentum equation using the notation that Nield and Bejan propose in their book (Convection in Porous Media 4th ed., page 17, eq 1.18 , see attachment) and multiple both sides with porosity.


Best regards,
Stathis

[jf_vt]

@Stathis
Thanks it is very helpful

I have digged a little further in it myself and have found that there is also a mesh size issue involved:

The mass conservation deffect is a consequence of unphysical velocity oscillation around a porous/freeflow interface.

These amplitudes create the "mass deffect" I observe when I compute massflow on the porous surface:

-They decrease when the porosity is decreased ( no surprise here...)

-At constant porosity, they decrease when the mesh size around the porous interface is decreased.

I will keep digging... and might try your suggestion.

JF

[rezaeimahdi]

Originally Posted by stathisk

Hello!

@Pierre
Yes indeed, some authors consider L as the characteristic length of the porous medium, but I've found many cases in the literature that Da number is defined using the characteristic macroscopic length scale. Yang et al. (2012) article (see my 1st post) is an example.

@JF
Sorry for the late response.
I can't tell you much about the lack of mass conservation in simpleReactingParcelFoam since it's a solver that I've never used before.
Concerning porosity treatment, I was able to improve my results by adding the porosity term in the momentum equation using the notation that Nield and Bejan propose in their book (Convection in Porous Media 4th ed., page 17, eq 1.18 , see attachment) and multiple both sides with porosity.


Best regards,
Stathis

Hello Stathis

Could you please let me know how you add the porosity term in momentum equation?

In fact, I add porosity in the solver, but pressure cannot converge at all.

I highly appreciated if you can send your modified code to me.

Thanks

[stathisk]

Hi Mahdi,

I'm afraid that I can't share the modified code.

Nonetheless, you can read the relevant information/instructions in my previous posts.

Best regards,
Stathis