I looked at the screen shots you posted of your case set up. In line with Mr Salva's above suggestions, you might try turning off the Joule Heating and Reaction Heating for a few iterations when starting a run. (I have made it my standard practice to run 10 iterations with Joule and Reaction Heating models turned off, and then then turning them back on for the remainder of the run.) 

Additionally, you can reduce the relaxation factors on the specific quantities which are diverging in the initial unstable portion of the run, and then increase them later for the sake of faster convergence once the solution stabilizes. 

Here is an example command file that I have used:

/file/rc /home/jdh26c/Fluent/Scaled_Parallel.cas

/solve/initialize initialize-flow

/ssv 0.55 y

/solve/set/under-relaxation mom 0.3

/solve/set/under-relaxation species-0 0.5

/solve/set/under-relaxation species-1 0.5

/solve/set/under-relaxation species-2 0.5

/solve/set/under-relaxation uds-2 0.3

/define/models/resolved-MEA-fuelcells/model-options n n y y y y 0.05 0.04 n n

/solve/iterate 10

/define/models/resolved-MEA-fuelcells/model-options y y y y y y 0.05 0.04 n n

/solve/iterate 990

/solve/set/under-relaxation mom 0.5

/solve/set/under-relaxation species-0 0.7

/solve/set/under-relaxation species-1 0.7

/solve/set/under-relaxation species-2 0.7

/solve/set/under-relaxation uds-2 0.5

/solve/iterate 1000

/solve/set/under-relaxation mom 0.6

/solve/set/under-relaxation species-0 0.8

/solve/set/under-relaxation species-1 0.8

/solve/set/under-relaxation species-2 0.8

/solve/set/under-relaxation uds-2 0.6

/solve/iterate 3000

/file/wd /home/jdh26c/Fluent/Scaled_Parallel_55_5k.dat

This is for a large scale simulation. You may not need to run as many iterations before increasing relaxation factors.

If this run strategy does not help you attain convergence, I can share an example case file with you. (I am running on Ansys Fluent 15.0)

Dear Dmitry

I went through the same process a couple of years back when I was simulating PEMFC but I did it using COMSOL. I can tell you how I went about the process -

After Nguyen's paper, Guvelioglu's really helped me in progressing (https://www.researchgate.net/publication/223083938_Computational_fluid_dynamics_modeling_of_polymer_electrolyte_membrane_fuel_cells).

I hope this helps.

Article Computational fluid dynamics modeling of polymer electrolyte...

Thank you for your detailed answer, Shivesh.

I've created full model, but I have an error while case start to calculate:

  iter continuity x-velocity y-velocity z-velocity energy h2 o2 h2o uds-0 uds-1 uds-2 uds-3 uds-4 time/iter

V_stack = 0.700000 (V) ... V_open = 1.202589 (V) (single cell)

fcu: I_anode = 0.000000 (A/cm^2) ... I_cathode = 513.984313 (A/cm^2) ... dI_mea = -513.984313 (A/cm^2) ... dI_stk = -513.984313 (A/cm^2)

1 1.0000e+00 5.2176e-06 5.2115e-06 1.0626e-01 1.5037e-02 5.2407e-07 1.0161e-06 3.2142e+01 1.2270e-15 2.0960e-02 1.0000e+00 3.3268e+02 6.5911e-03 1:46:08 199

V_stack = 0.700000 (V) ... V_open = 1.188126 (V) (single cell)

fcu: I_anode = 0.000000 (A/cm^2) ... I_cathode = -0.000096 (A/cm^2) ... dI_mea = 0.000096 (A/cm^2) ... dI_stk = 0.000096 (A/cm^2)

# Divergence detected in AMG for species-0, protective actions enabled!

# Divergence detected in AMG for species-0, temporarily solve with BCGSTAB!

# Divergence detected in AMG for species-1, protective actions enabled!

# Divergence detected in AMG for species-1, temporarily solve with BCGSTAB!

# Divergence detected in AMG for species-2, protective actions enabled!

# Divergence detected in AMG for species-2, temporarily solve with BCGSTAB!

Error: Divergence detected in AMG solver: species-2

Error: Divergence detected in AMG solver: species-2

Error Object: #f

No idea what's going on here. But from the cases you've mentioned it looks like the current density is negative for the case of V_open = 1.18 V.

There are 2 ways of simulating PEM fuel cell that I have seen. In one you provide cell voltage and solve for current density in the cell. In the second current density is specified in the cell and you solve for cell voltage. What approach are you following?

In the second approach I guess you can provide an initial value of current density while running the simulations? From what I experienced providing initial value sometimes helps the solver in converging to a solution. Try providing the current density for 1.2 V case as an initial value for the 1.18 V case.

In the first approach I'd try varying V_open to see what is the critical value below which solver stops converging and see if that value is non-realistic. But to be honest this really looks strange. I also faced similar problems and this happened because I did not have an idea of what's going on inside the solver.

Dear Dmitry,

I am trying to answer some of your questions.

Firstly, the module of the Electrolysis and the PEMFC are not the same. I strongly recommend reading Fuel Cell Modules Manual (you can find it in Internet). Of course, if you want to solve a PEMFC, you have to select PEMFC model.

Secondly, you can change the pemfc.model.c but not for the boundaty conditions. In this program you can change, for example, the properties of the membrane (as you know, Fluent only has the properties for Nafion 117).

On the other hand, there is a tutorial of Fluent for modeling a PEMFC. You can find it in Internet without problem. The tutorial is easy to do and there are a lot of advises.

About your problem of divergence, try to do the tutorial. Maybe, you can detect your problem!

The fuel cells model in fluent is very touchy when it come to getting a convergent solution. First off, you need a very high quality mesh. Try to stay away from tet-elements if at all possible, and use a structured mesh. 

Secondly, you are going to need to change some of the advanced solution controls to get a stable solution. If you go under Solution Controls (same place you set relaxation factors) then click on  >Advanced

Thanks for your answers! 

Shivesh, it is good idea following to the second method specified the current density. Earlier I provide cell voltage. I think this error can be connected with the first order scheme which I use. I will try another options.

Antonio, in the Electrolysis module we can find option - PEMFC (as well as SOEC and SOFC). Reading manual I don't find any critical differences between this module and PEMFC module. 

Also I have tutorial for fluent 6.3. Following it I have the same error.

I did file with screenshots: https://yadi.sk/i/_oLMVuzbsq6YX

It seems  I've tried all model's setting, but result is the same - error. Can someone share your own correct fluent model of pem or model from tutorial? I couldn't understand what is wrong in my model.

Dear Dmitry,

I am going to give you some advices according to my experience using Fluent in PEMFC.

1- First Step: Simulate only the fluids (Air+Water in cathode and H2+Water in anode). The idea is to obtain an initial point.

2- According to your error, I have checked that your input is the voltage so you want to obtain the current density. Try to solve step by step, I mean,try to solve V=1.15, V=1.05.... V=0.7. With this strategies is easier to reach a solution.

3- If you have the same error, you should deactivate some models such as Butler-Valmer Rate, Membrane Water transport or Multiphase until you will reach an initial solution. Once you have an initial solution, you can activate the models step by step.

Good Luck!

I looked at the screen shots you posted of your case set up. In line with Mr Salva's above suggestions, you might try turning off the Joule Heating and Reaction Heating for a few iterations when starting a run. (I have made it my standard practice to run 10 iterations with Joule and Reaction Heating models turned off, and then then turning them back on for the remainder of the run.) 

Additionally, you can reduce the relaxation factors on the specific quantities which are diverging in the initial unstable portion of the run, and then increase them later for the sake of faster convergence once the solution stabilizes. 

Here is an example command file that I have used:

/file/rc /home/jdh26c/Fluent/Scaled_Parallel.cas

/solve/initialize initialize-flow

/ssv 0.55 y

/solve/set/under-relaxation mom 0.3

/solve/set/under-relaxation species-0 0.5

/solve/set/under-relaxation species-1 0.5

/solve/set/under-relaxation species-2 0.5

/solve/set/under-relaxation uds-2 0.3

/define/models/resolved-MEA-fuelcells/model-options n n y y y y 0.05 0.04 n n

/solve/iterate 10

/define/models/resolved-MEA-fuelcells/model-options y y y y y y 0.05 0.04 n n

/solve/iterate 990

/solve/set/under-relaxation mom 0.5

/solve/set/under-relaxation species-0 0.7

/solve/set/under-relaxation species-1 0.7

/solve/set/under-relaxation species-2 0.7

/solve/set/under-relaxation uds-2 0.5

/solve/iterate 1000

/solve/set/under-relaxation mom 0.6

/solve/set/under-relaxation species-0 0.8

/solve/set/under-relaxation species-1 0.8

/solve/set/under-relaxation species-2 0.8

/solve/set/under-relaxation uds-2 0.6

/solve/iterate 3000

/file/wd /home/jdh26c/Fluent/Scaled_Parallel_55_5k.dat

This is for a large scale simulation. You may not need to run as many iterations before increasing relaxation factors.

If this run strategy does not help you attain convergence, I can share an example case file with you. (I am running on Ansys Fluent 15.0)

I have tried to switch on equations consequentially: flow, then energy and so on,  after every 200-300 iterations (step by step). But the calculation is interrupted by error: divergence detected in amg solver: temperature. And as a result, floating point exemption.  Please, send me your case, I would like to calculate it on my workstation. I guess that some error could be in fluent 17.

Dear colleagues,

Can anyone explain how to compile basic or customized UDF code for PEMFC simulation?

I compiled lots of simple UDF, but now I have an error compiling even basic UDF for fuelcell module. In general, I use VS 2012 Professional x64 and Fluent 17.1.

So,

I have done all steps as wrote in Solutions#2024479 (ANSYS Customer portal):

ANSYS Inc\v140\fluent\fluent14.0.0\addons\fuelcells

(Please note that folders "v140" & "fluent14.0.0" are valid for Release 14.0 and are slightly different for other releases. It is advised to find the exact location of the "fuelcells" folder using Windows Explorer)

3) Copy the above "fuelcells" directory from its standard location to your local directory where your case( and data) files are. For example, D:\Data\PEM_example.*

4) Enter the fuelcells/src folder, in our example: D:\Data\PEM_example\fuelcells\src. This folder contains a customizable pem_user.c file which you can modify. Please make a cosmetic change to this file so that you know and can check if the desired local pem_user.c is used (i.e. from your local directory) and not the one from the standard ANSYS installation directory. For, example you can modify one of the User-Defined Memories slightly. Upon loading the library into ANSYS FLUENT you are able to see the list and naming for all used User-Defined Memories and User-Defined Scalars.

For example, replace the line:

strncpy(udm[ 0], "X Current Flux Density", STRING_SIZE-1);

with:

strncpy(udm[ 0], "X CURRENT FLUX DENSITY", STRING_SIZE-1);

and then it will be very easy to spot which file/library is used.

5) Make sure that the FLUENT_INC environment variable is set correctly to the current ANSYS FLUENT installation directory i.e.:*

C:\Program Files\ANSYS Inc\v140\fluent*

The above path can be different for a different release of ANSYS Software or if the installation of ANSYS Software has been carried out in a non-default location.

6) Define the FLUENT_ADDONS environment variable to correspond to your customized version of the Fuel Cell and Electrolysis module, i.e FLUENT_ADDONS should point to your local directory that contains your case file and the customized "fuelcells" directory, i.e. D:\Data\PEM_Example in our case.

NOTE: In order to define the environment variables in Steps 5 & 6 above please go to:

Start -> Control Panel -> System -> Advanced System Settings -> Environment Variables:

Under "System variables" please press "New" to create "FLUENT_INC" & "FLUENT_ADDONS" variables.

7) Modify the "Path" environment variable by appending:

;C:\Program Files\ANSYS Inc\v140\fluent\ntbin\win64

to the existing Path.

8) Return to your local "fuelcells" folder.

9) Open a new DOS command prompt and issue the following command:

nmake -f makefile_master-client.nt clean

This will clean all old libraries.

10) Issue another command to build a new library so that the changes you've made can become active:

nmake -f makefile_master-client.nt

But when I check makelog file in my local fuelcells\win64\3ddp, I see some error.

I attached pem.c and makelog files to this question.

Any suggestions?

Dear Dmitry, 

I would like to know if you have solved this problem.

I am not able to initialize in fluent and it gives received a fatal signal (segmentation fault).

Sometimes it says couldnt find "nmake". When I try to compile the pem_user file. It says "cannot find localize.h" . 

Regards,

Manoj

Dear Dmitry

i am using GAMBIT for mesh and boundary condition , according to the given in  tutorial ,but how to define all the boundary condition like any interface between membrane.

Regards

Ramakant

Dmitry and Manoj, these are questions that are best addressed to your Fluent technical representative and they have PEM trial cases which they can share with you.  Outside of that, this Fluent presentation may shed some light on how you setup a PEMFC problem. 

if you are already interested in the topic I can share some results I've obatined with fluent add on module...

regards

Yes, Giosue, please, share your results. I'd like to see it. 

Thank you. 

dear Dmitry, 

If you are using the add-on module model you don't need to use and compile any udf.

Obviously if you want make changes in the "standard" model you have to do it.

To my experience most of the issue are due to the poor mesh or bad defined zones in the model, or bad initialization of the model.

I've find usefull to start with the the appended thesis, hope will help you

Thank you for this thesis. 

I almost haven't restrictions in computing resources, I can calculate cases up to 1 billion volume cells. But my main purpose is to create my own udf file and some model constant to functions. And here I've faced with problem of comailing of udf file by VS. 

Dear All

How to calculate the mass flow rate(Anode) & (cathode) inlet in PEM fuel cell.

Thank you

the inlet flow rate for a fuel cell can be calculated trhough the following relation 

N=I/nF * S

where N is the molar flow (mol/s) I the current (A) n the number of equivalent (2 for hydrogen and 4 for Oxygen) and F is the Faraday constant (96485 C/mol) S the stoichiometric factor (

if you need the flow rate in terms of mass simply multiply the N by the molar mass of the hydrogen or Oxygen or Air.

If you use Air instead of Oxygen as oxidant consider the Oxygen content in the Air is approx 1/5 then you must multiply Noxygen *5 to obtain the Nair

Refer to recent publication on the same topic in sciencedirect.com . I found few papers which describe the simulation in detail. Hope that will be useful for your simulations.

ALL THE BEST

Can you please share your finds?

I had a glance through those abstracts and methodologies while reviewing/refereeing a paper. I did not save the results. Kindly search in Science Direct, you will get the recent ones.

ALL THE BEST

How to do PEM fuel cell modeling without using Addon module in ANSYS Fluent ?

I am simulating PEMFC Module in fluent. But facing w

Problems of Divergence detected in AMG solver:species 0,1,2,3

Please help me how to I remove this problem