[ege.koseoglu]

Hello dear Foamers, excuse me if my question is misplaced or already answered in a different thread but I swear I have searched for this question everywhere I could think of, alas without a definitive answer.


The project in my mind is to model the mass and heat transport processes in my laboratory catalytic fixed-bed reactor. So the question is; is it possible to simulate a catalytic packed bed in it's most basic form. I know that this is possible in Fluent and Comsol. The system I have in mind is very basic, imagine a tubular reactor with three axial sections. In all sections there is the particle bed with a given porosity (i.e. eps = 0.4). But only in the middle section, reaction is defined. I don't require the particles to be spatially resolved or anything like that. I'm aware that compressible flows through porous media is handled in rhoPorousSimpleFoam and reacting flows on rhoReactingFoam, but how to combine reactions with porosity?


I have already experience with OpenFOAM. As I said, I couldn't find this case study anywhere in the internet although I know that it's one of the most frequent cases for reaction engineering. I would be very grateful if someone could point in the direction.

[edaymo]

Hi,

There are a few resources out there to help with the simulation of a catalytic fixed bed reactor.

To your initial question, how do you combine reactions with porous regions? The most basic answer is that you can define two porous regions with topoSet. The first porous region can be called inert and is located in the top and bottom section of your bed. The second porous region can be called catalyst and is the zone where reactions take place. Again, the location of this second porous region can be defined with topoSet. Now with two cell zones created (inert and catalyst), you can setup Darcy's law for both regions via fvOptions or fvConstraints (depending on the OpenFOAM version you are using). The zoneCombustion model can be used to only have reactions occur within the defined catalyst zone.

If your reactions are simple and fall into one of the predefined OpenFOAM rate equations (e.g., Arrhenius, LangmuirHinshelwood, and so on) and the reactor is isothermal or adiabatic, then this is probably good enough to allow you to solve your problem.

If on the other hand you need to use a more complicated reaction mechanism or account for realistic packed bed heat transfer, you may need to look at other tools.

catchyFoam https://github.com/lavdwall/catchyFOAM
can be used to model fixed bed reactors with kinetics handled by Cantera. As far as I know their packed bed porous media models do not account for "realistic" packed bed heat transfer for non-isothermal, non-adiabatic heat transfer.

With respect to porous media heat transfer, Tobias Holzmann has an absolutely brilliant example of porous media heat transfer in OpenFOAM at his website https://holzmann-cfd.com/community/t...talyst-heat-up. In this particular case there are no reactions but in modern versions of OpenFOAM chtMultiRegionFoam can run with chemical reactions. But again, in standard OpenFOAM you are limited to just a few kinetic forms (or you can program your own).

I personally do a lot of catalytic fixed bed reactor simulations with DUO, which couples OpenFOAM and DETCHEM. Our OpenFOAM Workshop 18 paper was recently published: https://link.springer.com/article/10...12-024-01764-8. In this case I used a single energy equation for the solid and fluid phases and validated the fixed bed reactor against experimental data for an steam methane reforming (SMR) reactor. You are welcome to private message me for more information on DUO. My OFW 18 slides and the source code for heat transfer in a single porous region (OpenFOAM 10) is found at https://github.com/TonkomoLLC/OFW18

One final note: you can also consider if you need CFD for your simulation work. There are good non-CFD tools that can predict reactor performance with reasonable accuracy in many circumstances. As an example, you can check out DETCHEM PBR: https://www.omegadot.software/software/detchem/


Between all of these options I hope that you find a solution that works for you.

Best regards,

Eric

[ege.koseoglu]

Well, that's is far more helpful and detailed than I could wish for, so thank you a lot edaymo. I will try out the tutorial and your other suggestions


To name a few details, I'm working on ammonia reforming and would like to see how far isothermal and non-mass-transport-limited we might get with the kinetic parameters we have determined. I actually measure no significant drop in the T but the spatial resolution is not that great. I will be using a modified power-law so that should not be that hard. Still the concentration dependencies on multiple species make it hard to use analytic solutions such as postulated by Mears. Still, I will require to figure out a way to get down to a Thiele modulus for this reaction which accounts both NH3 and H2 concentrations. If you have any suggestion there as well, would be most welcome.

[edaymo]

Hello,

Glad the reply is helpful. DUO can model porous mass transfer resistances either with an effectiveness factor model (i.e., I think the effectiveness factor is what you're getting at with the Thiele modulus calculation) or a 1D reaction-diffusion equation model. This is discussed in the paper I referenced above from last year's OpenFOAM Workshop. As far as I know DUO (DETCHEM+OpenFOAM) is the only CFD solution that can solve for the local (i.e. at every cell for porous media, or face for wall reaction) effectiveness factor to adjust the reaction rate.

Most of the time, though, people will estimate a global effectiveness factor for the entire reactor and then just apply it as a factor that multiplies the pre-exponential in the rate expression.

Hopefully some hint in my earlier reply will get you moving forward. Otherwise feel free to ask further questions.

Thanks and best regards,
Eric