|September 27, 2012, 07:07||
SOFC with Fluent's Fuel Cell Model
Join Date: Sep 2012
Posts: 1Rep Power: 0
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!
|February 18, 2014, 11:56||
Join Date: Feb 2014
Posts: 1Rep Power: 0
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 : 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?
Last edited by Studen1; February 18, 2014 at 13:04. Reason: fixing
|ansys meshing, fuel cell, sofc, tubular|
|Thread||Thread Starter||Forum||Replies||Last Post|
|2D Fuel Cell Modeling||Nehal||FLUENT||2||August 7, 2012 07:47|
|Charge Transport for Fuel Cell Applications||Jallen13a||FLUENT||1||April 3, 2012 05:32|
|PEM fuel cell modeling||alimech||Main CFD Forum||3||March 3, 2011 07:17|
|Cells with t below lower limit||Purushothama||CD-adapco||2||May 31, 2010 21:58|
|Own turbulence model: cell loop||bastil||OpenFOAM Programming & Development||0||April 7, 2010 17:25|