[wyldckat]

Originally Posted by ksfbangbangda

Now, there are 2 porosity zones with different parameters in my case, how can I define porosityProperties/constant ?

Quick request: Please provide more details, because at least I cannot see what exactly are referring to.

In addition, I advise you to follow the instructions given here: http://www.cfd-online.com/Forums/ope...-get-help.html

[Pedro24]

Originally Posted by ksfbangbangda

Now, there are 2 porosity zones with different parameters in my case, how can I define porosityProperties/constant ?

The toolbox has been updated and now accept heterogeneous porosity field "eps" for the two solvers impesFoam and anisoImpesFoam.

1) As before, you can define porosity as a scalar (eps is defined in transportProperties)
2) If you put a volScalarField "eps" in the time directory, it will be used by the solver to compute the two flows. Use setFields to generate your heterogeneous porosity field.

I update the tutorial "injectionAniso_case2" to give an example.

Regards,

Pierre

PS: Please note that porosity time derivative is not included in the conservation equations and must be constant.

[Ingmar]

Hey,

I have different zones in my geometry with different porosity and pore diameter. Different pore diameter leads to different capillary pressure. Is it possible to define different pc_max (for the linear model) or different pc0 (for brooks and corey) in different regions?

Thanks for your help!

Ingmar

[Pedro24]

Hi Ingmar,

Currently, the parameters of capillary pressure models are defined as scalar so you can not simulate what you need directly. You should modify the files:

porousModels/capillarityModels/BrooksAndCorey/pcBrooksAndCorey.H
porousModels/capillarityModels/BrooksAndCorey/pcBrooksAndCorey.C

to indicate that parameters (alpha, pc0, Sminpc, Smaxpc in that case) are volScalarField and not dimensionedScalar anymore (you should read these files in timeDirectory or, better, in constant).
Note that you will have probably some errors in compilation (due to the fact that BrooksAndCorey use "pow" function which has some issues when dealing with VolScalarFields).

I think that even if it is not a big change in the toolbox, you should know correctly openfoam to implement it.

Good luck :-)

Pierre

[Pedro24]

Hi,

I had several foamers having similar requests so i just updated the toolbox to allow heterogeneous model parameters.

The Kr and Pc models now look in the folder "constant/porousModels" to see if parameters are present (for example a pc0 file for the Brooks and Corey model).

Case 1: file is present so the parameter is heterogeneous (define for each computation cell)
Case 2: file is not present so it reads "BrooksAndCoreyCoeffs_" in transportProperties if it is present
Case 3: set a default value (0 for most cases).

Each parameters is independent so you can define a partly heterogeneous model. Example is given in tutorials (BuckleyLeverett/BrooksAndCorey and 1Dinfiltration)

You should use the setFields function to correctly initialize your parameters in the time directory and then move parameters-files to the "constant/porousModels" folder (I don't want parameter fields in the time directory because they are constant).

Please let me know if you find bugs in the code so that I can improve/correct it .

Sincerely,

Pierre

Source code : https://github.com/phorgue/porousMultiphaseFoam.git

[Ingmar]

Hi Pierre,

thanks for the update its working fine in 1D and 2D cases.
Currently I'm trying to calculate a 3D case and I'm always getting a saturation higher than 1. I created a wedge for a cylinder and I'm using the linear solver for a flow of Ub through the pipe (so basically its flow through a pipe filled with porous media). Any Ideas what the problem might be?

Ingmar

[Pedro24]

Originally Posted by Ingmar

Hi Pierre,

thanks for the update its working fine in 1D and 2D cases.
Currently I'm trying to calculate a 3D case and I'm always getting a saturation higher than 1. I created a wedge for a cylinder and I'm using the linear solver for a flow of Ub through the pipe (so basically its flow through a pipe filled with porous media). Any Ideas what the problem might be?

Ingmar

This issue is generally related to the timestep which may be too big (explicit computation of the saturation equation). Maybe you should try to reduce the maxCo in your 3D case.

Pierre

[chemcfd]

Hi,

I tried to compile the solvers using standard OF-3.0.1 version but compilation was not successful. Could you please help me to fix the issue in compilation? Thank you in advance.

Please find below the compilation errors:

[Pedro24]

Hi CHiller,

The message :

C:/BLUECF~1/ofuser-of4/platforms/mingw_w64GccDPInt32Opt/bin/impesFoam.exe: error while loading shared libraries: libporousModels.dll: cannot open shared object file: No such file or directory

means that the library libporousModels.so does not compile correctly in the toolbox (the file is not present).

I do not know precisely the c++ structure of dynamic meshes in openfoam and probably there are some deep changes to implement in the toolbox to use it. Probably you should not only change solver "impesFoam" but also the associated libraries (porousModels and maybe porousBoundaryConditions).

Sincerely,

Pierre

[us7]

Hello,
I am new to openFoam and using twoPhaseEulerfoam (two phase flow or air in the water). I added a porous baffle in the (air-water) path using fvOptions. Is it possible to add relative permeability into DarcyForchheimer model. I am using explicitPorositySource by using fvOptions but trying to add relative permeabuility or (K=kkr where kr can be alpha - phase fraction) in it.

I also tried this model but i don't understand how impesFoam will work when there is no porous media e.g. gas dispersion through sediments into water column (no porous media). it would be really great if you can give me any idea how can i do this or your solver (impesFoam) ok to use in my case?

Kind Regards
Umer

[Cyp]

Hi Ulmer,

In impesFoam, you solve generalized Darcy laws. Which means that by construction, there are always solid in the cells. This is a prerequisite.

Cheers,
Cyprien

[us7]

Thanks Cyprien. Can you recommend me any solver related to this case?

Regards,
Umer

[Cyp]

You can probably customize twoPhaseEulerFoam to add relative permeability in the porous regions.

[us7]

Thanks. Yes i am already trying that solver but i have few questions related to that if you may like to give some suggestion. I am using twophaseEulerfoam and using explicitPorosity source term in fvOptions. Currently i am using two phase air and water. The source term in openfoam just let me to put values for D and F.

-Currently source term is Si = -(μ D + 1/2ρ|u|F)ui where D = 1/K , K= intrinsic permeability but in case of two fluids how is it calculating K.

-is K=KKre in case of two phase or its taking absolute permeability which is mentioned in fvOption "d d [0 -2 0 0 0 0 0] (2e11 2e11 2e11)"?

-if yes, then is it ok to use this explicit porosity source term for two phases because this source term is not calculating relative permeability for each phase.

Here, i am struggling to add relative permeability into this explicitPorositySource term like

Si = -(μ D/kre + 1/2ρ|u|F)ui

so it will start taking effect of both phases where Kre is a function of saturation or volume fraction alpha. and for this what i could understand so far is, i have to modify DarcyForchheimer.C and all related files. Please correct if i am wrong here.

Regards,
Umer

[Cyp]

Actually, what I am suggesting is that you give up with this fvOption feature. Instead you clone twoPhaseEulerFoam and you implement your own source term with the dependency you want.

[Faiz498]

I downloaded the toolbox from git link

After running ./Allwmake command inside porousMultiphaseFoam directory, I got a long error. I am attaching initial part of the error. Can anyone help me how to proceed from here?
The error says it is could not open x.H files for y.C files
I am using Foam-extend4.0 in Ubuntu16Screenshot from 2019-06-25 18-54-14.jpgScreenshot from 2019-06-25 18-54-42.jpg

[PRATBHARAT]

hi,
I am using OpenFOAM 6. I have a case in which porosity is varying along width and length having empirical relation found by using DEM. Can anyone help me?
Thanks in Advance.

Regards,
Pratyush