CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Journal

Weber et al. - 2023 - Open-source Computational Model for Polymer Electrolyte Fuel...

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Matt7

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2023, 11:44
Default Weber et al. - 2023 - Open-source Computational Model for Polymer Electrolyte Fuel...
  #1
New Member
 
Miguel Nóbrega
Join Date: Jul 2012
Posts: 21
Rep Power: 13
mnobrega is on a distinguished road
Comments and questions are welcomed on the article Weber et al., Open-source Computational Model for Polymer Electrolyte Fuel Cells, OpenFOAM Journal, February 2023, https://doi.org/10.51560/ofj.v3.50
mnobrega is offline   Reply With Quote

Old   March 7, 2023, 09:30
Default
  #2
New Member
 
Pratik
Join Date: May 2020
Location: Oldenburg, Germany
Posts: 14
Rep Power: 6
Pratik_21 is on a distinguished road
Nice work


I have been working on this model getting to run.Just one observation
In the Makefile, section regionMesh fails because of no constant folder in the subRegions directory.
Its quite easy fix.


My goal is to get this model running for PEM electrolyzers.
I would like to know from developers about possibilities of it.
Pratik_21 is offline   Reply With Quote

Old   March 16, 2023, 15:20
Default
  #3
Member
 
Norbert Weber
Join Date: May 2012
Location: Dresden, Germany
Posts: 37
Rep Power: 14
dl6tud is on a distinguished road
Thank you for this hint. I corrected it.
dl6tud is offline   Reply With Quote

Old   June 15, 2023, 00:43
Default Thank you
  #4
New Member
 
Jose
Join Date: Dec 2020
Posts: 18
Rep Power: 5
jose.ceballos is on a distinguished road
Quote:
Originally Posted by mnobrega View Post
Comments and questions are welcomed on the article Weber et al., Open-source Computational Model for Polymer Electrolyte Fuel Cells, OpenFOAM Journal, February 2023, https://doi.org/10.51560/ofj.v3.50
Thanks for sharing this work, definitely will read it. I'm currently working with the J.P. Kone code and this paper expands my universe about open-source codes for fuel cell simulations.

I'll try to run it hoping to work with this tool in the future.
jose.ceballos is offline   Reply With Quote

Old   July 7, 2023, 04:09
Default Extraordinary PEFC Solver!
  #5
New Member
 
Join Date: Jul 2023
Posts: 2
Rep Power: 0
Matt7 is on a distinguished road
Thank you for sharing the wonderful solver for PEFC! I would definitely like to working with this model!

While I'm still trying to understand the model, I would like to share some of my own opinions.

1. I noticed some disagreement with my understanding in the spices transfer equation in YairEqn.H and YfuelEqn.H. The velocity is the intrinsic velocity, so that it was timed by the porosity. And the diffusion term of the equation was also timed by the porosity and also (1-s). If I understand it correctly, the diffusion coefficient is already renewed (i.e. timed by porosity/tortuosity and (1-s)^1.5) to be the effective diffusivity before you solve the equation. Is there any possibility that you underestimated the diffusivity in your codes?

2. I'm also trying to run your example cases after I fixed the error of constant folder, as mention by Pratik_21. However, I found that the initial residual of the velocity didn't drop, even after I ran thousands of the time steps. I guess it can be fixed by changing the settings in fvScheme and fvSolution. I'm trying to change the PISO control to PIMPLE control in fvSolution of air and fuel regions. Would you mind providing me any suggestion for that?

3. I totally agree with the electrolyte model that you neglected the water transport in the in-plane direction, since it seems to have little impact on the results. Maybe the reason is that the charge transfer can be omitted, and the cathode catalyst layer field can be reduced to a boundary condition consequently, so that we don't need to solve the electrical potential field, which is really a computational sources saver. Please forgive my greed, but do you have any plan to compile the 3D water transfer model in electrolyte and charge transfer model in the future? Since the ohmic resistances may be critical in some other electrochemical system.

I would definitely appreciate your reply!
Thanks in advance!
Matt7 is offline   Reply With Quote

Old   July 22, 2023, 06:19
Default
  #6
Member
 
Norbert Weber
Join Date: May 2012
Location: Dresden, Germany
Posts: 37
Rep Power: 14
dl6tud is on a distinguished road
I am very rarely in this forum, and do not get a message for new posts. In case of comments or questions I am always happy to receive an email.
dl6tud is offline   Reply With Quote

Old   August 31, 2023, 18:00
Default Steps to run
  #7
New Member
 
Jose
Join Date: Dec 2020
Posts: 18
Rep Power: 5
jose.ceballos is on a distinguished road
Greetings;

Could anyone, please, indicate the steps to compile and run the application?

For example, I tried to compile with ./Allwmake inside of the directory .../fuelcellfoam-master/solver but I got errors.

Then at .../fuelcellfoam-master/testcase/ciemat I type make and start to iterate Surface refinement but it never ends.

In the case of the juelich folder, I can run make mesh to visualize the cell in Paraview, but when I type make run it says that there are not enough slots available in the system to satisfy the 16 slots that were requested by the application.

I would appreciate the help. Thanks in advanced.
jose.ceballos is offline   Reply With Quote

Old   September 8, 2023, 04:09
Default
  #8
Member
 
Norbert Weber
Join Date: May 2012
Location: Dresden, Germany
Posts: 37
Rep Power: 14
dl6tud is on a distinguished road
Quote:
Originally Posted by Matt7 View Post
Thank you for sharing the wonderful solver for PEFC! I would definitely like to working with this model!

While I'm still trying to understand the model, I would like to share some of my own opinions.

1. I noticed some disagreement with my understanding in the spices transfer equation in YairEqn.H and YfuelEqn.H. The velocity is the intrinsic velocity, so that it was timed by the porosity. And the diffusion term of the equation was also timed by the porosity and also (1-s). If I understand it correctly, the diffusion coefficient is already renewed (i.e. timed by porosity/tortuosity and (1-s)^1.5) to be the effective diffusivity before you solve the equation. Is there any possibility that you underestimated the diffusivity in your codes?

2. I'm also trying to run your example cases after I fixed the error of constant folder, as mention by Pratik_21. However, I found that the initial residual of the velocity didn't drop, even after I ran thousands of the time steps. I guess it can be fixed by changing the settings in fvScheme and fvSolution. I'm trying to change the PISO control to PIMPLE control in fvSolution of air and fuel regions. Would you mind providing me any suggestion for that?

3. I totally agree with the electrolyte model that you neglected the water transport in the in-plane direction, since it seems to have little impact on the results. Maybe the reason is that the charge transfer can be omitted, and the cathode catalyst layer field can be reduced to a boundary condition consequently, so that we don't need to solve the electrical potential field, which is really a computational sources saver. Please forgive my greed, but do you have any plan to compile the 3D water transfer model in electrolyte and charge transfer model in the future? Since the ohmic resistances may be critical in some other electrochemical system.

I would definitely appreciate your reply!
Thanks in advance!

I pushed these bugfixes. Many thanks for pointing out these mistakes!!!
If anyone needs a more detailed documentation than in the article, please feel free to contact me.

dl6tud is offline   Reply With Quote

Old   October 15, 2023, 23:56
Default Suggestion of compiling and running the application
  #9
New Member
 
Join Date: Jul 2023
Posts: 2
Rep Power: 0
Matt7 is on a distinguished road
Dear Jose,

Regards to your question, firstly, I think the code should be run under the environment of OpenFoam v2112. There may be some troubles to run with the different version of OpenFoam and something they are difficult to be fixed.

Then, when I compile the solver, I go to solver/, type the commands below in order
Code:
cd solver/libSrc
wmake libso
cd ../fuelCellFoam
wmake
Running (./Allwmake) in solver/ also works, but the permission to access the files is required, which can be procced by running like
Code:
chmod -777
And some errors can be fixed by running "wclean" before "wamke", if you have previously tried to compile the solver.

Next, when the solver is successfully compiled, I try to run e.g. case/juelich. I go to the case directory, and type (make All). However, (make All) is for parallel run. If your system is not 16 cores, you need edit the file in system/decomposeParDict, change "numberOfSubdomains" and "simpleCoeffs" if "method simple" is employed. For example, I run with 4 cores and my setting is like

Code:
numberOfSubdomains 4;

preserveFaceZones (iFaces);

method          simple;	

simpleCoeffs
{
    n               (2 2 1);
    delta           1e-16;
}
The product of 3 numbers (2 2 1) in simpleCoeffs/n in my case is 2*2*1=4, which should exactly equal to "numberOfSubdomains".

Or if you don't want to run with parallel, you can add a new line in Makefile in case/juelich as below, and run "make Alls" in command window.

Code:
Alls: mesh srun view
meanwhile the "srun" in lines 112-113 should be edited as

Code:
srun:
	(fuelCellFoam | tee log.srun);
p.s. I guess that the author wants to write "fuelCellFoam" instead of "uftFoam" originally.

Matt

Quote:
Originally Posted by jose.ceballos View Post
Greetings;

Could anyone, please, indicate the steps to compile and run the application?

For example, I tried to compile with ./Allwmake inside of the directory .../fuelcellfoam-master/solver but I got errors.

Then at .../fuelcellfoam-master/testcase/ciemat I type make and start to iterate Surface refinement but it never ends.

In the case of the juelich folder, I can run make mesh to visualize the cell in Paraview, but when I type make run it says that there are not enough slots available in the system to satisfy the 16 slots that were requested by the application.

I would appreciate the help. Thanks in advanced.
Feras2020 likes this.
Matt7 is offline   Reply With Quote

Reply
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
polynomial BC srv537 OpenFOAM Pre-Processing 4 December 3, 2016 09:07
what is swap4foam ?? AB08 OpenFOAM 28 February 2, 2016 01:22
Problem compiling a custom Lagrangian library brbbhatti OpenFOAM Programming & Development 2 July 7, 2014 11:32
OpenFOAM without MPI kokizzu OpenFOAM Installation 4 May 26, 2014 09:17
DxFoam reader update hjasak OpenFOAM Post-Processing 69 April 24, 2008 01:24


All times are GMT -4. The time now is 00:34.