[AMR96]

Hello,

I'm trying to run a steady state simulation for a 7 serpentine channel PEM fuel cell using ANSYS Fluent's PEMFC module. Currently I can run simulations but I can never achieve convergence as the residuals become constant after around 300 iterations and they stay that way with very little change. I also looked at the contours and none of them make sense when compared to the contours found in literature. For example the Hydrogen mass fraction contour presented below shows the H2 mass fraction decreasing initially but then it starts to increase again when reaching the out let. The same goes for the Oxygen contour on the cathode side. (The inlet is on the right side in all images)




For boundary conditions I have the following:

At the anode I have a mass flow velocity and a constant temperature of 80C. The mass fraction of H2 is 0.6 and mass fraction of H2O is 0.4.

At the cathode inlets I have mass flow velocity and constant temperature of 80C. The O2 mass fraction is 0.21 and H2O mass fraction is 0.15.

For outlets I have pressure outlets. The voltage at cathode terminal is also set to 0.6 V. The rest of the boundary conditions are set as stated in ANSYS user guide.

I really don't understand where the problem is and any help is greatly appreciated. Below is the residual curve that I obtained after 600 iterations.

[edwardsh]

Hey, I believe I can help a bit.

First off, the H2 graph may not be as unrealistic as you think. H20 is drawn from the anode to the cathode by electro-osmotic drag, so it's mass fraction is also falling. This in turn raises the mass fraction of H2, simply because there is a lower fraction of H2O, not because the amount of H2 molecules is rising. There are no source terms in the governing equations for H2, so it should not be possible for it to come out of nowhere. A similar thing is likely happening with O2 due to water being used for membrane hydration. A good idea might be to compare the species balance of the inlet and outlets (ie, does the amount of O2 and H2 consumed equal the ammount of H2O produced)

As for convergence, the PEMFC model can be a pain to get right. I've found that I get good convergence by following these steps:
1. Use least squares cell based as the discretisation method for gradient (methods tab)
2. Set the URFs for pressure to 0.7, Momentum to 0.3 and species, energy, both potentials and the three water equations to 0.95 (controls tab). You can raise the water content and electric and protonic potential back to 1 once the model is decently converged
3. In advanced in solution controls, set the cycle type of all equations to f-cycle, add BCG-STAB to the species, energy, potential and multiphase equations and lower their termination criteria to 0.001

In general, if you're seeing oscillatory behaviour in a residual, lowing the corresponding URF usually helps. Finally, depending on the mesh size, the solution my take several thousand iterations to converge rather than a few hundred

[vahid7333]

Hello
I simulated a tubular SOFC with unsolved electrolyte
inlet boundary conditions of mass flow inlet with mole fraction h2=0.475 and h2o=0.525 for the fuel channel and o2=0.298 for the air channel, but after convergence the mass fraction at the beginning of the fuel cell becomes zero and It does not reach the end, what is the problem?
thanks for your help

[lavendar12]

Hi edwardsh, may I know what is the criteria for convergence, ie residual falls below 1e-6? I tried to simulate soec with addon module 3 but for h2 the residuals fail to fall below 1e-1 no matter how many iterations I did.

[edwardsh]

Hey @lavendar12. Generally high residuals are either a symptom of a mesh that's too coarse, or due to the numerical methods. For PEMFCs you generally need at least 3-5 vertical layers in the mesh for the GDLs and CLs. As for the numerical methods, the model generally has a hard time solving the species balance equauation. You can help this by using BCG stabilisation and lowering the species URFs to 0.95. Also, you can set all the descritidation methods to first order upwind, which is a low accuracy but highly stable method. Once that's got a decent solution, you can change it to second order upwind.

[amin_u50]

Hello everyone,
I am kind of new to PEM FC simulation, I am trying to simulate a single channel using Ansys. I do see an issue when I start initialization. It gives me an error of "It is highly likey that the Anode CAT/GDL are not setup correctly"

I appreciate your guidance.

[edwardsh]

I can't say I've ever seen that error before. All you need to do to set up the Anode GDL and CL is to assign the correct zone in the PEMFC model UI. Assuming you've done this and double checked everything, what happens when you run the model?

[amin_u50]

Thanks for your quick reply,

Yes I did define the zone for each layer in UI. When I click on the run it, the simulation start the iterations and after 2-3 steps it diverges.

Hybrid initialization is done.

Warning: It is highly likely that the Cathode CAT/GDL are not set up correctly!

Warning: It is highly likely that the Anode Collector and GDL are not connected!