[Germilly]

Hello;

I'm working in a problem that has gas flowing through porous media. The porous media (solid matrix) has heat source. So, this problem includes heat transfer between the solid matrix and the gas (I'll have two energy equations: Gas and solid matrix).

I'm having problem about which solver should i start to use in OpenFoam to solve this problem.

I've already tried rhoPorousSimpleFoam, but this solver doesn't includes heat transfer between the gas and the solid matrix (It includes only one energy equation).

I think the solver twoPhaseEulerFoam can be an option, because it includes heat transfer between two different fluid phase.

Can anyone tell me which is the best solver which should i start?

Thank you.

Best regards
Germilly Barreto

[dewey]

Hi Germilly

could you find what solver to use?

I think i am doing something related.

[Germilly]

Hello Dewey;

Now, i'm trying to solve the equations presented in the following paper: http://dx.doi.org/10.1016/j.enconman.2016.01.074, by changing the "simpleFoam" Solver, i.e, changing its momentum equation and including the heat transfer equations for porous media.

But, i'm having many problems.

GB

[Cyp]

What about coding your own solver based on Darcy's law? No need to solve Navier-Stokes if you only have a porous domain.

See the tutorials https://web.stanford.edu/~csoulain/O...NG_v5-1-EN.pdf page 68 to 101 (also include a two temperatures model).

Cheers

[Germilly]

Hello Cyp

Thank you for your answer. I have already done the exemple presented in the tutorial you provided (using Darcy's law).

I will need to improve my model (include turbulence ...).

I think to inprove it, i should start using Navier-Stoke equation, or not?

But, for the first version i can use Darcy's law, how you have suggested.

GB

[Cyp]

Hi,

I suggest you first to do some literature review on flow and transport in porous media, so you will have a clear idea of the different scale or representation of physics of flow and transport. The concept of porous media is related to the concept of average: when you represent explicitly the pore-scale structure (I mean you have a full description of the pores) then you solve the flow with Navier-Stokes based solvers. On the other hand, if you represent the porous region by an aggregate of fluid and solid (you don't know the real geometry of the pores), then you have effective properties like permeability and porosity and the flow is governed by a Darcy-like law.

In your case, I guess that you are in the second situation and you want to consider higher flow rate. The best thing is to keep this Darcy-like formulation and to add Forchheimer correction to include inertia terms. We showed in a recent paper that the Forchheimer formalism can also represent turbulence effects.

Some papers:
https://web.stanford.edu/~csoulain/P...hap1_Darcy.pdf
http://oatao.univ-toulouse.fr/11304/...aine_11304.pdf

Cheers,

[Germilly]

Hello Cyp

Thank you for your attention.

Yes, my case is the second one " ... represent the porous region by an aggregate of fluid and solid (you don't know the real geometry of the pores), then you have effective properties like permeability and porosity ... ".

I will see the documents you sent me. If i have some problem, i will come here again.

I can't open the first link, it is not working (error when loading the pdf).


GB

[Germilly]

It is working now.

Thank you

[dewey]

Do you know if for heat transfer and porosu media can works modify chtMultiRegionSimpleFoam or buoyancySimpleFoam instance of SimpleFoam?

[Germilly]

Hello dewey,

I think it is possible if you modify chtMultiRegionSimpleFoam or buoyancySimpleFoam.

I think that the choice of the solver depends of kind of precision you want to include in your model.

I have concluded that it is better to start from an basic solver, and changing it for what you want.

[Adri_12]

Hi Germilly and Cyprien,

In your problem that you solved, was it in steady state ?
Did you have only porous zone or fluid zone coming into porous zone ?
Which start point solver do you advice me to start with?

I am building a case describing heating effects of hot air entering in a porous zone with a inlet velocity, with turbulence, transient and incompressible behaviour of the fluid.

Thanks for your help.

adrià

[Germilly]

Hello,

My approach is steady state. I still have many problems with my model.

In my first approach, I have only porous zone.

Have you seen the following tutorial?

https://web.stanford.edu/~csoulain/O...G_PART_3v5.pdf

Maybe it can help you to choose which solver to start with.

Germilly

[Adri_12]

Hi Germilly,

Sorry for the delay, yes I have seen the tutorial, it is clear that we have 2 choices in OF :
1. Start from a basic solver and implement your equations
2. Explore the fvOptions improving the existent solvers

I thought it would be less time-consuming to profit from 2. option. But I cannot prove it yet .

Let us know if you go on in your work, I am also working on it.

Good luck

Adrià

[Germilly]

Hello,

Ok.
I have not been addressing this issue lately.
I was working in the first part of my work, which is modelling of solar radiation absorption in porous volumetric receivers (porous media). This model give me the heat source of the fluid flow and heat transfer model.

Soon, I will start with the fluid flow and heat transfer modelling using openFoam.

Thank you
Germilly

[Adri_12]

Hi,

As mentionned, I am hardly working on a case of heat transfer dealing with porous media and air (cf attached picture & case)

- I decided to describe all my pipe as a fluid (air)
- and consider the solid aspect of the porous media as another region overlayed on the air region declared as a solid.
regionProperties:

 regions
(
    fluid   (air)
    solid   (solid)
);

- I created a porous cellzone in the air region with topoSet, used in constant/air/fvOptions with explicitPorositySource
- I forced an interregion constantHeatTransfer between air and solid. That has been done with fvOptions in both regions air/solid (porous).

I had never seen this kind of approach but seems to work

some questions to help me to continue to improve it :

• Can someone check my case and confirm that I'm using well the interregionHeatTransfer function ?
• What does it mean in fvOptions fields, semiImplicit ? :

constantHeatTransferCoeffs
    {
        interpolationMethod cellVolumeWeight;
        nbrRegionName   solid;
        master          true;

        nbrModel        solidToAir;
        fields          (h);
        semiImplicit    no;
    }

• Why can we know who is the master true/false the air or solid ?
• I'd like to use a Nusselt number as an input instead of an htcConst x AoV ? I've seen that variableHeatTransfer is available but I don't managed to use it.
• I am still using chtMultiRegionSimpleFoam, even if my heat propagation depends on time, so should I switch to chtMultiRegionFoam ? I think my case does not work in transient, but I go on step by step... If you have any ideas do not hesitate.

Anyway I think it is a good start and I hope people will find it useful.



regards,



Adrià

[deepbandivadekar]

Originally Posted by Adri_12

Hi,

As mentionned, I am hardly working on a case of heat transfer dealing with porous media and air (cf attached picture & case)

- I decided to describe all my pipe as a fluid (air)
- and consider the solid aspect of the porous media as another region overlayed on the air region declared as a solid.
regionProperties:

 regions
(
    fluid   (air)
    solid   (solid)
);

- I created a porous cellzone in the air region with topoSet, used in constant/air/fvOptions with explicitPorositySource
- I forced an interregion constantHeatTransfer between air and solid. That has been done with fvOptions in both regions air/solid (porous).

I had never seen this kind of approach but seems to work

some questions to help me to continue to improve it :

• Can someone check my case and confirm that I'm using well the interregionHeatTransfer function ?
• What does it mean in fvOptions fields, semiImplicit ? :

constantHeatTransferCoeffs
    {
        interpolationMethod cellVolumeWeight;
        nbrRegionName   solid;
        master          true;

        nbrModel        solidToAir;
        fields          (h);
        semiImplicit    no;
    }

• Why can we know who is the master true/false the air or solid ?
• I'd like to use a Nusselt number as an input instead of an htcConst x AoV ? I've seen that variableHeatTransfer is available but I don't managed to use it.
• I am still using chtMultiRegionSimpleFoam, even if my heat propagation depends on time, so should I switch to chtMultiRegionFoam ? I think my case does not work in transient, but I go on step by step... If you have any ideas do not hesitate.

Anyway I think it is a good start and I hope people will find it useful.



regards,



Adrià

Hi,

I was able to run your case without any issues. However, I am not sure the results are correct.
e.g. check the attached velocity plot. Those bumps on two ends of the porous zone look spurious. The temperature drop within the porous zone also appears rather quickly (before the zone ends); am not sure if that's physically correct.


I'd like to get your feedback on this or if you've any updates.

[deepbandivadekar]

Originally Posted by Adri_12

I had never seen this kind of approach but seems to work

Just realised, the solution doesn't converge in 1000 steps. I'm running it again for more number of steps. I will update. However, do you have any feedback at this point?

[Germilly]

Hello,

I want to share with you some updates I have achieved regarding to modelling of fluid flow and heat transfer in porous media.


First of all:

1) The physical model and the methods used in the development of the solver are described in detail in the following paper: Three-dimensional CFD modelling and thermal performance analysis of porous volumetric receivers coupled to solar concentration systems. This paper can also be found in my ResearchGate.

2) Part of the solver coding was presented in the 3rd Iberian Meeting of OpenFOAM technology users. The presentation file, which has parts of the code, can be found in my ResearchGate: OpenFOAM solver for 3d modelling of solar thermal volumetric receivers coupled to concentration systems or in the following link.


Model development:

To start, I have programmed a basic solver that simulates fluid flow in a circular pipe. This was performed solving the 3D Navier-Stokes equations for steady state conditions using the simple algorithm. Another option is to start with the simpleFoam solver.

After the basic solver was working correctly, I started to change the Navier-Stokes equations for the case of fluid flow in porous media. I have used continuous scale approach (volume averaged mass and momentum conservation equations). Next, I have added the energy conservation equations of the solid matrix structure and heat transfer fluid to the solver. For this part, the following tutorial was very useful. The governing equations (mass, momentum and energy conservation equations) are presented in the paper I referred above.

Attached are the following source files of my solver:

createFields.H
UEqn.H
pEqn.H
TsEqn.H (Energy conservation equation of the solid matrix structure)
TfEqn.H (Energy conservation equation of the heat transfer fluid)

Parts of the code need to be improved.
I hope this can help.

Regards,
Germilly Barreto

[Raghul13]

Hello Germilly,

I am currently working on developing a conjugate heat and mass transfer model to characterize a convective drying process of food substance treated as porous medium. Can you give me some suggestions on treating the boundary between the fluid and the porous media interface. Can I use the conventional no slip boundary condition or should I use the Beavers B.C

[Germilly]

Originally Posted by Raghul13

Hello Germilly,

I am currently working on developing a conjugate heat and mass transfer model to characterize a convective drying process of food substance treated as porous medium. Can you give me some suggestions on treating the boundary between the fluid and the porous media interface. Can I use the conventional no slip boundary condition or should I use the Beavers B.C

Hello Raghul,

Which approach are you using for modelling the porous media? Is it pore-scale or continuous-scale approach?

Regarding to boundary conditions when continuous-scale approach is used, please see the sections 2.5 and 4.1.1 of the following paper:

Three-dimensional CFD modelling and thermal performance analysis of porous volumetric receivers coupled to solar concentration systems

GB