Fluids

Fluids

SOEC modelling with Fluent

    • Victoria Kurushina
      Subscriber

      Dear All,

      I believe I am not the first person with the questions on how to model electrolysis in ANSYS Fluent using the Add-on models. For the purpose to simulate SOEC at high temperature, I have tried the Add-on Model 3 and Model 4 and encountered a few issues:

      • Model 3 electrolysis (3D) is running and converging, but does not show any change to the H2 fraction (it remains close to the value set at the inlet across the whole gas channel length), as shown in the contour plot below;
      • Model 4 electrolysis (3D) stops working, Fluent closes automatically, right after the model is initialized. (The zones are defined close to the Tutorial on SOFC in the Learning Hub). 
      • Attempts to simulate an electrolysis cell in 2D with Add-on Model 3 have also led to the Fluent shut down.

      It would be great, if you share your experience with the build-in electrolysis models in Fluent.

      Kind regards,

      Victoria

       

    • Aleksey Gerasimov
      Subscriber

      Hello Victoria,

      Please note that our fuel-cell and electrolysis add-on modules are developed and maintained for 3D versions only. Should you, need to perform a quick 2D test, then please consider using a simple 3D model with one single cell in the 3rd direction that have symmetry boundary conditions on either side.

      Please note that a very common mistake that people make when the voltage is set below the OCV voltage in electrolysis module. It must be in excess of OCV. Please check whether this is the case or not. Typically, the thermoneutral voltage (TNV) in SOEC is around 1.3V and most cells require higher values around 1.4-1-5V. Or even more if the internal reforming reaction such as CO2 splitting takes place.

      Regarding initialization for module 4, please ensure that you use the standard initialization and if the problem persists, please consider patching individual variables to specific regions in the cell and this will help us narrow down the problem.

      Hope this helps and best regards,

      Aleksey.

       

      • Victoria Kurushina
        Subscriber

        Dear Aleksey,

        Thank you very much, it is more clear now. I have gone through the SOFC tutorial again (Model 4), to identify possible differences in settings, and I have a few questions to the pp.29-30, where the electrical characteristics are defined for the case. Is this a correct understanding that:

        1) item 5 on p. 29: the 50 iterations run is performed for the Total System Current of 0.01A, as shown earlier in Fig. 7 on p.10? so, there is no other UDS conditions set on any surfaces, like wall_voltage_tap?

        2) when running the cases for 100 iterations each in a sequence, to cover the case matrix in Table 2 on p.30, we set the Total System Current to the value in column 2 and the Electric Potential at the wall_voltage_tap boundary to the value in the 1st column? so that, the first two columns are input, and the three other columns (power, H2 utilization, O2 utilization) are output?

        Or is this just the voltage column value the only input, while the rest is output?

        Kind regards,

        Victoria

    • Victoria Kurushina
      Subscriber

      Is the open circuit voltage the same parameter as the total system voltage (when Converge to Specific Voltage is ticked)? If not, what is the difference? Does the electic potential at wall_voltage_tap have to be higher than the total system voltage, as you mentioned before?

    • Aleksey Gerasimov
      Subscriber

      Hello Victoria,

      Please see answers below.

      1) There are a few ways to specify the potentiostatic or galvanostatic boundary conditions. You can set them on individual walls (taps) or in the SOFC panel. If you set the total current of 0.01A then there is no need to specify anything else on individual boundaries, These inputs on boundarires will be ignored in such case.

      2) You can use either approach, by specifying voltage and getting current or vice versa. I believe either this tutorial or our PEMFC tutorial explain this. The prescribed current (galvanostatic b.c.) is often used, because, it allows us to identify the inlet mass flow rates that are needed for a desired stoicheometry. However, this approach works well if the model include cables or bus bars, where a uniform current density distribution is realistic. However, the potentiostatic boundary conditions are better in those cases, where the electric b.c.'s need to be applied to bipolar plates, A prescribed uniform current over wider surfaces in such cases is neither realistic nor physical, thus causing the additional convergence issues.

      3) No, the specified voltage is the operational voltage e.g. values from column 1 in Table 2 on page 30.

      Best regards,

      Aleksey

    • Victoria Kurushina
      Subscriber

      Dear Aleksey,

      Thank you. I am afraid I have a few more:

      1) So, in the case, when there is an electric potential V1 defined at the wall_voltage_tap, what is the correct relationship of values to be set at the start of the simulation?

      Total System Voltage < Open Circuit Voltage <  V1

      (if defining System Voltage)

      and Open Circuit Voltage <  V1

      (if defining System Current)

      Is this correct?

      And, if I understood well from your reply, the V1 will be accounted for in the simulation, when the System Current is not close to zero?

      2) When running the Model 4 in the Electrolysis mode, I noticed the model itself changes the Total System Current to a negative value of -0.01, while keeping a default +0.01 in the SOFC mode. Is this ok to work with the negative current value, or does it mean there is some mistake in the settings in the electrolysis mode?

      3) Another question that comes is about the H2 fraction at the outlet for either SOFC or SOEC steady-state simulation. The SOFC tutorial (Model 4), I think, considers the situation when this fraction is somehow known or guessed. But if you have a goal to learn the H2 fraction at the outlet, should this value be set to 0 or sort of the best guess?

       

      Kind regards,

      Victoria

    • Aleksey Gerasimov
      Subscriber

      Hello Victoria,

      I am not sure I understood your questions correctly, therefore, please see my answers below. Please do not hesitate to clarify any aspects if you feel that I misunderstood something.

      1) The electric potential in a fuel cell operation = V_cathode_tap - V_anode_tap and this value is always lower than the open circuit voltage (OCV) in fuel cells, In electrolysis mode the applied voltage must exceed the OCV value, regardless of the type of the electric boundary conditions.

      2) It is normal to see the negative current, it is just a sign that the module works in Electrolysis module.

      3) This is for reversed flow only, that might take place in the initial stages of the simulation or if the outlets are located close to the active zone. It is best to avoid a situation where you have reversed flow at the outlets of your domain.

      Best regards,

      Aleksey

    • Victoria Kurushina
      Subscriber

       

      Dear Aleksey,

      Thank you for the replies, it is very helpful.

      Could you explain, please, how to avoid the sigsegv error when working with my own geometry?

      I have tried the SOFC tutorial geometry in the electrolysis mode, and it is possible to initialize the solution and get some results. However, when I draw my own simple planar cell geometry (CC-GC-CAT-ELE-CAT-GC-CC) and set the electrolysis mode, following all tutorial steps, except loading the user expressions (because they are for SOFC), what I get is sigsegv error after the initialization, and Fluent shuts down. If this is Standard initialization, it is just the error code in the consol and shut down. If this is the Hybrid initialization, Fluent spells in the consol “Hybrid initialization is done.”, then SIGSEGV error and shut down.

      I understand this likely means that some physics is defined incorrectly, but it is not apparent, unfortunately. The last thing I tried: I followed the meshing guidance, specified in details in the PEMFC tutorial, so this is not the mesh accuracy problem. It would be good to have your perspective on this.

      Kind regards,

      Victoria

       

    • Aleksey Gerasimov
      Subscriber

      Hello Victoria,

      Please let me know what was the error message with the standard initialization. If you patch each solved variable individually, do you have the same error? If so, at which point?

      For the hybrid initialization, SIGSEGV is a segmentation violation error and it means that something is either missing or being specified inconsistently. I presume you are using the "Fuel Cell & Electrolysis" module. The first thing that catches the eye is the  (CC-GC-CAT-ELE-CAT-GC-CC)  sequence. I'd assume that CC stands for Current Collector, GC - Gas Channel, CAT - catalyst and ELE is the Electrolyte. Where is the porous gas diffusion layer that connects the current collector and the reaction zone (catalyst)? Can the current flow through it?

      Best regards,

      Aleksey.

    • Victoria Kurushina
      Subscriber

      Dear Aleksey,

      I am trying to use the Model 4 in Electrolysis mode. I can add GDL, but in the Model 4 tabs there is nowhere to put it (at least, if following the SOFC sequence, there is no place where GDL or any other layers between CC and CAT would have any settings).

      With standard initialization, it does not finish. Just SIGSEGV, and the next thing is Fluent shuts down.

      Patch should be applied to all variables?

      Kind regards,

      Victoria

    • Aleksey Gerasimov
      Subscriber

      Hello Victoria,

      Ok, if the Unresolved Electrolyte SOFC module is used then the catalysts and electrolyte cannot be specified as designated separate cell zones. This is the simplification of the module. This is likely to be the source of the problem. There should be a way for the electric current to flow from the reaction zone to the terminals.

      Best regards,

      Aleksey.

    • Victoria Kurushina
      Subscriber

       

       

       

      Dear Aleksey,

      Could you, please, reiterate about the cell zones? Currently, at the Mesh, I make the Named Selections for the planar cell, as in the image below. Do you mean that some of them should be deleted from Mesh for the Model 4 to work?

      Currently, the list of cell zones (in the other image below) appears to be consistent with the SOFC tutorial, except there is an extra “electrolyte” layer. I have tried not to name-select the electrolyte body at Mesh, but the Model 4 in this case will create this layer on its own in Fluent, so I am trying to keep naming everything myself, just not to be lost in names.

      About the electric current: do you mean that there should be definitely a surface of contact between the CC and the CAT on both sides, for the Model 4 to work? This is what is done in the tubular geometry from tutorial.

      Added: when running my own geometry in Fluent, outside the Workbench, the initialization works ok, but the start of the Solution gives the SIGSEGV error, followed by the message in red: "The f1 process could not be started". 

      Kind regards,

      Victoria

       

       

       

       

Viewing 10 reply threads
  • You must be logged in to reply to this topic.