[julienC]

Dear all,

The third release of sedFoam, a two-phase flow model for sediment transport applications, is available on github:
https://github.com/SedFoam/sedfoam

and an open-access article describing the model capabilities is available here:
https://www.geosci-model-dev.net/10/...-4367-2017.pdf

A short introduction and the description of the tutorials can be found here:
http://servforge.legi.grenoble-inp.fr/pub/soft-sedfoam/

This thread is to inform the community about the recent evolutions of the code as well as to gather feedbacks, questions and comments from the community. Don't hesitate!

All the best,

Julien Chauchat

[LeOtTeRz]

Hi Mr. Julien


I'm starting to use sedFoam and I had been run the tutorials but I have some questions about its configuration.


The first one is about of the configuration file "funkySetFieldsDict". What is the function of "field", "expression" and "keepPatches" Keywords in this file?


Is it possible to use the "setFieldDict" file instead of "funkySetFieldDict"? if the answer is yes, Would it work the same as in others solvers?


I know that sedFoam works with two approach for modeling particle stress, kinetic theory of granular flows and dense granular flow rheology, the question is which one needs longer calculation time?


Thank you in advances.

[julienC]

Dear Leandro,


Please find my answers below.

I'm starting to use sedFoam and I had been run the tutorials but I have some questions about its configuration.

The first one is about of the configuration file "funkySetFieldsDict". What is the function of "field", "expression" and "keepPatches" Keywords in this file?

funkySetFieldsDict is used by the command funkySetFields which comes with swak4foam: https://openfoamwiki.net/index.php/Contrib/swak4Foam


It is more general than setFields as it allows to impose "complex" initial conditions.

Very quickly:
"field"= variable to be initialized

"expression" = function to be used for the inital condition
"keepPatches" = keywork that allows to keep the boundary conditions unchanged when writing the new field file.

Is it possible to use the "setFieldDict" file instead of "funkySetFieldDict"? if the answer is yes, Would it work the same as in others solvers?

If you used setFieldsDict/setFields you will only be able to impose step-like initial volume fraction profile. It should work but you might observe stronger oscilations and the code might become less stable.

I know that sedFoam works with two approach for modeling particle stress, kinetic theory of granular flows and dense granular flow rheology, the question is which one needs longer calculation time?

The kinetic theory is more computationally intense as it requires solving for an additional transport equation. There are pros and cons for each model but overall they should provide reasonable solution.


Best regards,


Julien

[Saeid-basu]

Hi Prof. Chauchat

I want to use sedFoam to simulate local bridge sour. My case study contains non-uniform sediments. Is there any possibility to simulate sediment transport in non-uniform sediments with SedFoam? Actually, I have to introduce a sediment mixture with different sizes to the solid phase.

Your kind help and advice are most appreciated.

Best Regards,
Saeid

[julienC]

Dear Saeid,


sedFoam does not model sediment mixtures yet. The best you can do is to use a d50 however you won't reproduce any grain-size sorting mechanisms.



Best regards,


Julien

[Saeid-basu]

Prof. Chauchat

Another question is about the applicability of sedFoam for the morphodynamic module (bed load and suspended load). Can you please tell me more about how sedFoam consider that?

My Best Regards,
Saeid

[julienC]

Dear Saeid,


In two-phase flow models there is no distinction between bed-load and suspended-load, the sediment fluxes comes out from the product of the local velocity times the sediment concentration as a result of the the momentum balance equations for the fluid and the sediment phases. I think it is quite clearly explained in different journal papers on the subject.


Julien

[Jason_Duguay]

Hello Dr. Chauchat,

First, I would like to thank you and your team for putting this solver together

I am applying SedFoam-2.0 to model bed-load transport in a laboratory model. However, before I get too involved in the CFD side of things, would you mind sharing your suggestions on sizing the mesh within the sediment bed (specifically near the water/sediment interface) and in the near wall regions where a sediment/water interface occurs?

Also, does any special care need to be given to choosing wall functions for boundaries where the sediment bed touches the wall?

Any insights on these topics would be greatly appreciated. Thank you for making yourself available to answer questions.

[julienC]

Dear Jason,


Concerning the mesh requirement, it has to be small enough to resolve the thickness of the transport layer (so much smaller than the particle size sometimes). You can perform a sensitivity analysis to the mesh size to check you are converged.



No need to refine too much near the bottom wall if there is a deposited sediment bed as there is no turbulence there. No need for wall functions as well as the additional terms in the two-phase flow turbulence model should play the role of wallfunctions.


I hope this is clear, let me know if you need more informations.


Julien

[Yang xiaoyu]

Originally Posted by julienC

Dear all,

The third release of sedFoam, a two-phase flow model for sediment transport applications, is available on github:
https://github.com/SedFoam/sedfoam

and an open-access article describing the model capabilities is available here:
https://www.geosci-model-dev.net/10/...-4367-2017.pdf

A short introduction and the description of the tutorials can be found here:
http://servforge.legi.grenoble-inp.fr/pub/soft-sedfoam/

This thread is to inform the community about the recent evolutions of the code as well as to gather feedbacks, questions and comments from the community. Don't hesitate!

All the best,

Julien Chauchat

Dear julienC,
Hello,I am trying to simulate 3-D scour around a pile on openFOAM. And I saw a vedio of 3-D scour around a pile in github of your SedFoam team. Could you please tell me about the runtime of this tutorial and the number of processor ? I am not sure if I could use SedFoam to run my case because there are only 24 processors in my computer. Is it enouge to run a 3-D scour case using SedFoam? Thank you very much to read my letter. I am looking forward your reply sincerely~

All the Best,
Yangxiaoyu

[rku]

Hi,

I am relatively new to openfoam and need to start a project which will begin with simulating scour under currents first and then move on to including waves in the model as well.

Is it possible to include waves in sedFOAM? I couldn't find any details regarding use of VoF with it or multi-phase simulations with it for that matter? Can it be done? The official papers related to sedFOAM describe it as a two phase solver. Does that mean that it is not a multi-phase solver.?


Thanks in advance!

[julienC]

Dear rku,


You can use an oscilating pressure gradient in sedFoam to mimic waves without free surface or use a combination of interFoam and sedFoam recently published in JGR:
https://agupubs.onlinelibrary.wiley....9/2018JC013930
The code is distributed but we are working on an new version which should be distributed in the coming months


Best regards,


Julien

[neginmondegari]

I'm currently studying for master degree in hydraulic structures at Tehran University.

I'm working on my dissertation project that is" numerical modeling of density current in order to study the effect of bed slope and how to open the bottom outlet ".

May I ask for your expert opinions in regards to the following question please?

Do you think the OpenFOAM solver software “SedFOAM 1” or “SedFOAM 2”, can model turbidity current in two phases with eulerian approach?
If none of these solvers works for this project, please suggest the best solver for modeling this phenomenon.

I would appreciate, if you can please share with me your opinion.

Sincerely,
Negin Mondegari

[julienC]

Dear Negin,

As far as I understand your problem, Sefoam should probably work for your problem. I recommend that you use the latest sedFoam version available on github: https://github.com/SedFoam/sedfoam

Best regards,

Julien CHAUCHAT

[neginmondegari]

thanks for your response i have another question does sedfoam available to model the reservior of the dam and bottom outlet? i aske this question because the modules are not match with each other is it possible to model it or not? is it possible to model labratory flume which lenght is 11 m and the bottom outlet?
is it true that sedfoam has high computation and take along time to solve problems? and is true that sedfoam isn't stable enough?

[julienC]

Hi


I am not sure to fully understand your question and configuration. If you ask wether sedFOAM can solve free surface flows the answer is no but you can use interFOAM to solve this part and use this simulation to force a two-phase sediment transport simulation using sedFOAM.



Concerning the second part, yes sedFoam is computationally intense because the mesh needs to be refined in the near bed layer and the time step is constrained by the coupling between the phases. Both constraints make the simulations expensive. In terms of stability, it can be unstable and you have to have a good background in CFD to perform simulations in new configurations (i.e non existing tutorials).


Best regards,


Julien CHAUCHAT

[neginmondegari]

thanks alot for your response , if i want to model the density current in two-phase in experimental flume which solver in openfoam6, do suggest?
sincerely,
neginmondegari

[neginmondegari]

hello

i have three questions, is it possible to model longterm phenomena with sedfoam? what about interfoam in modeling longterm phenamena?
is it possible to couple sedfoam with interfoam?
regards

negin mondegari

[julienC]

Dear Negin,


You can have a look at Kim et al 2018 in JGR:

https://agupubs.onlinelibrary.wiley....9/2018JC013930


where we coupled sedFOAM with interFOAM.



For long term predictions it is not a suitable method as the computational cost is huge.


Best regards,
Julien

[neginmondegari]

thanks for your response

even i want to model the turbidity current in dam in 2D in sedFOAM and interFOAM , the computational cost is huge if I want to couple them?
I know if i modelthe turbidity current in dam in sedFOAM is wrong , because sedFOAM is for close surface , but if I model it in sedFOAM this fault is it noticable or can be ignore ?