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

SOFC with Fluent's Fuel Cell Model

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

Like Tree2Likes
  • 1 Post By D Bhardwaj
  • 1 Post By Studen1

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 27, 2012, 07:07
Smile SOFC with Fluent's Fuel Cell Model
  #1
New Member
 
Dhruba Panthi
Join Date: Sep 2012
Posts: 1
Rep Power: 0
D Bhardwaj is on a distinguished road
Hi there,

I already found several unanswered threads on SOFC modeling with Fluent. However, I am posting this thread with a hope to hear from some expert/experienced user in this field.

I am working on modeling a tubular SOFC with Fluent 14.0. I tried with both Fuel Cell and Electrolysis Model, and SOFC Model with Unresolved Electrolyte, but I have not yet been able to reach the expected solutions. Maybe the problem lies with the geometry/mesh itself but being a new user of ANSYS Workbench, I have not been able to identify it properly. Could you please suggest some hints/tricks especially about meshing strategy for the tubular SOFC geomtery?

Thanking you in advance!
sabrina sabi likes this.
D Bhardwaj is offline   Reply With Quote

Old   February 18, 2014, 11:56
Default
  #2
New Member
 
Join Date: Feb 2014
Posts: 3
Rep Power: 10
Studen1 is on a distinguished road
I'm investigating the fuel cell model (only the first one, with resolved electrolyte, SOFC mode) and trying to make it work properly for about a month. This is quite hard due to very poor specifications in the ANSYS help. Just in case somebody faces similar problems I'll write down my experience.
First I encountered an error, which appeared on applying the settings in the SOFC model GUI after all nesessary parameters were set: "GENERAL-CAR-CDR: invalid argument [1]: improper list Error Object: #f". This can happen (at least in version 14.5.7) if you leave the default zone type in the Geometry editor: Solid. Having all zones fluid it works, however some of them can be of both types (wrote in manual).
Then I got a strange error appeared at the calculation start. It was ACCESS_VIOLATION in ANSYS 14.5.7, which turned to "segmentation fault" in 15th version. The most interesting point: no error appeared at first initialization, but if you try to initialize it second time, you got the error. Two days of try-and-error work showed, that the problem can be solved by making the current collector and flow zones porous and applying the setting. After that they can be made non-porous again - the model works without an error. As I understand, this happens because the model solves the potential equations in flow zones too. For that it should get the conductivity of the media and it looks for conductivity property of solid porous material in this zone. And if the zone is not porous, it tries to reach the property, that doesn't exist. After you apply the porous setting, fluent allocates memory for the needed property, so it can be reached even after the "porous" box is unchecked.
After solving these technical problems I began to investigate the model itself. The manual is very superficial, so that even to understand how exactly the UDMs are calculated, some playing with the model is needed. I'll edit this post by adding new unobvious facts.

1) Model shows exactly zero ohmic heat source in the electrolyte. At least, the UDM4 is exactly zero. As I know it should be ionic current density multiplied by the ionic resistance: i_ion*R_ion.
2) The ohmic losses in the catalyst are calculated by the formula W = (i_total)^2/(sigma_ion + sigma_e), where i_total is the sum of ion and electron current densities, "sigma_"s are conductivities. To me that seems a real fail. This should be given by: W = i_ion^2/sigma_ion + i_e^2/sigma_e, and the ratio of these two can reach many orders for poor ionic conductors. This leads to underestimation of joule heating in this model.
3) The open circuit voltage (OCV) is modeled as the difference between the ionic and electronic potentials at the cathode side. By default it is independent from the gas species concentrations and set manually, but the user can edit this value and even calculate it by function. However, as long as we have such a function only at the cathodic side, the local dependence of the transfer current on the species concentration can be modeled only for the cathodic side, while for the anode maximum what can be done is integral dependency. Splitting of the open circuit voltage "jump" in two functions (separate for anode and cathode) could enrich the model functionality.

Unfortunately, I don't see the way to fix these problems withous accessing the source codes, which are not provided. Has anybody ideas: 1) that I'm wrong and the model is right; 2) how to fix it?
DaveD! likes this.

Last edited by Studen1; February 18, 2014 at 13:04. Reason: fixing
Studen1 is offline   Reply With Quote

Old   October 24, 2014, 03:30
Default Ocv
  #3
New Member
 
Join Date: Feb 2014
Posts: 3
Rep Power: 10
Studen1 is on a distinguished road
Quote:
Originally Posted by Studen1 View Post
3) The open circuit voltage (OCV) is modeled as the difference between the ionic and electronic potentials at the cathode side. By default it is independent from the gas species concentrations and set manually, but the user can edit this value and even calculate it by function. However, as long as we have such a function only at the cathodic side, the local dependence of the transfer current on the species concentration can be modeled only for the cathodic side, while for the anode maximum what can be done is integral dependency. Splitting of the open circuit voltage "jump" in two functions (separate for anode and cathode) could enrich the model functionality
It appears that pem_user.c can be easily modified to add electromotive force corrections on both anode and cathode sides. So now we have right OCV dependence on the fuel and oxygen concentrations! To do this just add your correction to the "eta" expression. Mind the right sign!

Last edited by Studen1; October 24, 2014 at 03:30. Reason: correction
Studen1 is offline   Reply With Quote

Old   January 22, 2015, 09:28
Default i am working with sofc
  #4
New Member
 
manikanta
Join Date: Jan 2015
Location: bangalore
Posts: 4
Rep Power: 9
manikanta is on a distinguished road
hey hi i am working wit unresolved sofc, i completed modelling , meshing, now i am getting problem in specifying input activation problem, in one sentence i cant say where exactly i got stopped. if possible send me a mail with your contact number, we can discuss each other and work together. my email is manikantadevarmani@gmail.com
manikanta is offline   Reply With Quote

Old   January 19, 2018, 15:32
Default
  #5
New Member
 
sabrina
Join Date: Jan 2018
Posts: 18
Rep Power: 6
sabrina sabi is on a distinguished road
I need your help how to draw a tubular fuel cell sofc using ansys(It can be explained in video format) and how to enter the material to study efficiency.please please helping me
I await your answer
thanx
sabrina sabi is offline   Reply With Quote

Old   February 15, 2018, 16:34
Default
  #6
New Member
 
sabrina
Join Date: Jan 2018
Posts: 18
Rep Power: 6
sabrina sabi is on a distinguished road
Quote:
Originally Posted by manikanta View Post
hey hi i am working wit unresolved sofc, i completed modelling , meshing, now i am getting problem in specifying input activation problem, in one sentence i cant say where exactly i got stopped. if possible send me a mail with your contact number, we can discuss each other and work together. my email is manikantadevarmani@gmail.com

Can you help me how draw geometry tubular fuel cell using gambit or know anyone can help me or any tutoriel about this tell me urgent
Please reply
sabrina sabi is offline   Reply With Quote

Old   March 30, 2018, 11:59
Default Electro-refining/Electro-plating
  #7
New Member
 
SAYANTAN BISWAS
Join Date: Mar 2018
Location: Mumbai
Posts: 17
Rep Power: 6
Sayantan Biswas is on a distinguished road
I'm working on Copper Electrorefining process (single Phase) in Fluent.
In 'Species Transport model' Electro-chemistry option is there.

I'm facing problem in Adding material part;

1) How do I add an electrolyte (liquid state) consist of Water+CuSO4+H2SO4 solution (having certain Cu concentration) ?

2) How do I add Cu+2 ions(or any metal ions) and Cu in the reaction mixture (only fluid type materials can be added in reaction Mixture) so that I can define the electro chemistry (cathodic/anodic) reaction in Species Transport model?

Thanks in Advance
Sayantan Biswas is offline   Reply With Quote

Reply

Tags
ansys meshing, fuel cell, sofc, tubular

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
PEM fuel cell modeling alimech Main CFD Forum 4 April 18, 2020 13:15
2D Fuel Cell Modeling Nehal FLUENT 3 April 18, 2020 13:11
Charge Transport for Fuel Cell Applications Jallen13a FLUENT 1 April 3, 2012 05:32
Cells with t below lower limit Purushothama Siemens 2 May 31, 2010 21:58
Own turbulence model: cell loop bastil OpenFOAM Programming & Development 0 April 7, 2010 17:25


All times are GMT -4. The time now is 04:10.