[Cornelia]

I am trying to set up a model with several hundred of porous membranes of size 1.3m² each. Their thickness is 0.003m and their Darcy's coefficient is 10e+10 m^(-2) - quite high!

My first idea was to use a porousBafflePressure BC inside the simpleFoam solver. But I found out that this BC is really unstable: it is already quite hard to get converged a simple test case, and it seems to be impossible for my real model.

So I had a deeper look into porousSimpleFoam solver. With a test case I found out that I have to use a very fine mesh inside my porous media and also next to my porous media in order to predict the pressure loss through the membrane accurately. If I use only 1-2 cell layers inside my membranes, the pressure drop is computed much too low. For my real model I would get a crazy amount of cells...


So I wonder if somebody can share some experiences or ideas on how I can set up my model efficiently:
- How do you usually model your porous membranes? As porous baffle or as porous media?
- Is there a good way to converge the porousBafflePressure BC?
- How fine is your mesh?
- etc.

[giack]

Hi,

I have a similar problem (simulation of pressure drop through a membrane). Did you find the answer to your questions? How did you proceed in your simulations?

Many thanks

[Cornelia]

Hi Giack,

Unfortunately there is still no working solution inside the official version of OpenFoam. At the moment I still have to use a commercial solver for such cases.

But there is a small company in Germany that has developed an extended porousBafffle boundary condition. Their name is www.dhcae-tools.com. If you are interested and willing to spend some money, just have a look.

That is also my plan at the moment, to find out more about it.

[Ahmed Khattab]

Originally Posted by Cornelia

I am trying to set up a model with several hundred of porous membranes of size 1.3m² each. Their thickness is 0.003m and their Darcy's coefficient is 10e+10 m^(-2) - quite high!

My first idea was to use a porousBafflePressure BC inside the simpleFoam solver. But I found out that this BC is really unstable: it is already quite hard to get converged a simple test case, and it seems to be impossible for my real model.

So I had a deeper look into porousSimpleFoam solver. With a test case I found out that I have to use a very fine mesh inside my porous media and also next to my porous media in order to predict the pressure loss through the membrane accurately. If I use only 1-2 cell layers inside my membranes, the pressure drop is computed much too low. For my real model I would get a crazy amount of cells...


So I wonder if somebody can share some experiences or ideas on how I can set up my model efficiently:
- How do you usually model your porous membranes? As porous baffle or as porous media?
- Is there a good way to converge the porousBafflePressure BC?
- How fine is your mesh?
- etc.

Hi Cornelia,

could you tell me how did you set membrane properties in transportProperties file?

[giack]

Hi to all,

I solved the problem using the fan boundary condition. You can create an internal patch (zero tichkness) with createBaffle and then use the fan boundary condition for the pressure field.

In this way you essentially create two coincident patches with cyclic behavior and impose a pressure drop through them.

I attached an example of the files p and createBaffleDict.

I hope it will be useful to you

createBafflesDict.txt

p.txt

[JanoVR]

Good day,

I am really new to CFD modelling.
I am trying to model an organic solvent nanoflitration system; ie a membrane system separating an organic compound and a homogeneous catalyst.
The catalyst must be rejected by the membrane.

I am not sure how to go about simulating a membrane?
I have read about porous mediums, but I am not sure if this will be suffice for my system?
Is there maybe a tutorial on membrane filtration I can study?

Any advice will be much appreciated.

Thank you

[giack]

Hi to all,

I have to correct my previous statement. Indeed the fan BC is used for pressure rise, while for pressure drop the porousBafflePressure bc can be used.
I had the same problems described by Cornelia in the first post only for high values of the pressure drop. In these cases a stable solution can be reached decreasing the relaxation factors. I didn't experience any problem with this boundary condition till a pressure drop of the order of 700 Pa.

[giack]

Hi to all,

I have to correct my previous statement. Indeed the fan BC is used for pressure rise, while for pressure drop the porousBafflePressure bc can be used.
I had the same problems described by Cornelia in the first post only for high values of the pressure drop. In these cases a stable solution can be reached decreasing the relaxation factors. I didn't experience any problem with this boundary condition till a pressure drop of the order of 700 Pa.

[sk11]

Hey giack,
Are you still working on this? I am using porousBafflePressure BC as well for obtaining pressure drop through a porous baffle. But I experience a problem in obtaining the surface as it is while meshing. How do you manage to get the net_135.stl as it is? Is this geometry (surface) curved? I tried using regionwise meshing aroud the geometry using snappyHexMesh, but I still couldnot snap the mesh to the surface of the geomtry to obtain the original shape. It would be nice to know how you managed to tackle this.
Many thanks.
Sarath

[giack]

Hi,

the geometry of my net is in attachment. I had problems with the mesh of the net too.

I solved in the following way:

- create the stl net_closed (in attachment)
- mesh the internal part with snappy
net_closed
{
// Surface-wise min and max refinement level

level (6 6);
faceType internal;
faceZone net_closed;
cellZone net_closed;
cellZoneInside inside;

}
- apply the createBaffle

If the cell zone is meshed properly than the net will be represented in good way, since it corresponds to an internal surface that already exists. I also added a refinement region around the net_closed geometry

Giacomo

[sk11]

Thanks alot Giacomo.

I believe this will work for me. My net is already a closed one.

They are able to mesh to the surface with out creating the patch becuase of the face type 'internal' isn't it?


Regards,
sarath

[giack]

Yes, exact