Problems with thermal profiles of chemical reactor
 

Good morning,

I am simulating the fluid dynamics of a packed bed reactor for methanol production and comparing them with some previous results I have obtained with simplified models. My CFD model (cfx) comprises a "slice" (30°) of the tubular reactor; the mixture (mainly CO, H2, CO2 and small amounts of inerts) enters the unit at 473K and reacts along the reactor. The cooling medium is vapour at a constant temperature of 240°C (I have just put the wall temperature equal to 240°C). The unit has been modelled as a porous domain (made of Aluminium).

The simple CFD model I have implemented seems to work with no problem, and predicts the productivity of methanol well (if compared to the previous models I have used). In spite of this, the predictions of the thermal profiles along the reactor are absolutely not reliable: I would expect a strong increase of temperature in proximity of the entrance of the reactor (due to the exothermic reaction involved) up to a peak, and then a progressive decrease of temperature up to a plateau (i.e., cooling medium temperature, 240°C). In other words, I would expect a steep augmentation of T in the first 10% of reactor length, mainly due to the exothermicity of the chemical reaction and then a milder thermal decrement of T, as the reaction reaches the chemical equilibrium and no reaction heat is produced any longer (but the cooling effect of vapour prevails).

In my simulations, though, it seems that the fluid is progressively heated up to the cooling medium temperature (i.e., it goes from 473 K to 240°C = 513 K), with no temperature peaks, as if no reaction heat were released (but the reaction occurs!!). I have implemented the kinetics through a series of expressions, that I have then utilized as "Sources" in a subdomain (called "Reaction Domain"). Similarly, I have put the reaction heat as energy source inside the aforementioned subdomain. Even after many checks, it seems that the reactions and the expression for reaction heat are properly written. The strange thing is that the reaction kinetics are properly predicting my system behaviour (and their values are in line with those of my previous models), and, similarly, the value of reaction heat is comparable with that obtained in simpler models, but in the CFD model the released heat somehow "disappears" from the thermal profile of the reactor.
I have also tried to change the turbolence model, with no appreciable differences in the final results.

Has anybody suggestions on where the problem could be?
I have attached the CFX-pre ccl file ("PBR.ccl", in the attached zip folder), but I also use an "Initial Value" file, to make the simulation quickly converge ("export"). I hope the latter file can be easily introduced in the main simulation (I was not sure on how to properly export a .res file). Please, let me know in case of any problem with the files.

Let me thanks you a lot,
Riccardo

- Did you check the imbalances during the calculation?

- At the end of the output-file there is an overview of all contributions in the energy equation. It should tell you where the energy goes. Can you share the output file of your calculation here?

- I have no experience with this option:
FLUID SOLID HEAT TRANSFER:
Heat Transfer Coefficient = 457.007 [W m^-2 K^-1]
Option = Heat Transfer Coefficient
END

Does this mean that the energy is going into the aluminium porous material? Does this have such a high conductivity that it becomes invisible as the heat is transferred to the outer wall?

I would recommend that you pick a simple exothermic chemical reaction which you have high quality data for the temperature field for and simulate that as a validation of your method of modelling heat in exo/endo-thermic reactions.

This is, in general how I recommend you approach all simulations with complex and multi-layered physics. You have to be sure you can model all the physical effects on a simple and well-validated case before you can combine them all together into a complex case.

Solution
 

Good afternoon,
Thanks a lot for both answers.
I solved the problem: the energy was simply going into the solid phase and in this way no thermal peak could be observed (as Gert-Jan suggested).
I have simply replaced the option "adiabatic" for the solid phase with something more reliable (the solid temperature is now assumed to be equal to the fluid one).

I am now having a problem with diffusivities, but, as it is a completely different topic, I should post it in another thread.

Thanks again,
Riccardo