[dlahaye]

Eric makes a good point. The reverseBurner test case might be good to look into. Our documentation on reserveBurner is at https://mega.nz/file/eBcxWKgJ#CXhpWd...5O3CHRBqIX6XKk

Good luck.

[Alczem]

Hey!



Regarding radiation in the solid, I don't think the solver can handle a participating solid, meaning that there is no radiative field solved in a solid region (I may be mistaken, please correct me if that is the case). So the absorptivity does not matter for a solid region when using the opaqueSolid model.


Having the option to model a solid as a semi-transparent medium would be a great feature to have for CHT applications, but I don't think it is (yet?) implemented

[dlahaye]

What happens is case of switching on the radiation in the solid?

Solid and fluid have distinct settings for density rho, heat capacity Cp and thermal conductivity k.

If radiation does work for fluid, when not for solid? Is this a case of radiation submodes not (yet) being implemented?

Cheers, Domenico.

[Alczem]

Solver-wise, I am not sure what happens, I never took the time to look at the code properly. But there is no radiative field written for solid regions even with the radiation switched on.


My guess is that you have to turn it on to indicate that you expect radiation to happen in the fluid regions, and maybe to use certain boundary conditions such as turbulentTemperatureRadCoupledMixed that refer to neighbouring fluid regions and their associated radiative field. The heat transfer at the interface between the solid and the fluid takes into account the radiation coming from the fluid, but there is only conduction on the solid side.

If radiation does work for fluid, when not for solid? Is this a case of radiation submodes not (yet) being implemented?

I am not experienced enough to know where the differences lie and what it would take to implement radiation in a solid or semitransparent medium Maybe it is really simple and just a matter of not being requested by the userbase.


One trick I have seen and tried myself is to model a solid region as a frozen fluid that still allows radiation to be solved. But one of the main issues is that the rays (if you use fvDOM) are not propagated through the interface between two fluid regions. The radiation is solved separately for each region, if that makes sense. And there is no boundary condition for internal transparent walls or baffles as far as I know.

[edaymo]

Hi Domenico and Alczem,

Thanks for the replies and the helpful discussion.

Going back to sante_junior's original question, he wished to know if absorptivity of zero mean that " refractory wall doesn't absorb any energy." If the turbulentTemperatureRadCoupledMixed (now called coupledTemperature in OF 11) BC is used, radiative heat from the fluid side can be transferred to the solid, even if absorptivity is zero. This is consistent with Alczem's reply, I think.

I believe Alczem is correct that there is no radiative field solved for in the solid. I think this is supported by the comments in the opaqueSolid file in OpenFOAM: https://github.com/OpenFOAM/OpenFOAM.../opaqueSolid.H ... i.e., there is no source term generated for radiation with the opaqueSolid model.

With respect to whether absorptivity and emissivity fields do anything at all in the solid phase, I am not sure. The reverseBurner tutorial, for example, sets an emissivity of 0.1 on the solid side.

Domenico, if I understand the reverseBurner document correctly, you explored the fluid-side absorptionEmission properties, but not the solid side?

The other thing I am now not sure if is if the radiative heat is transferred from the fluid to solid side via the boundary condition, can radiative heat transfer to the solid side if the solid radiationModel is set to 'none'?

Thanks for exploring these matters together.

Best regards,
Eric

[Pablok]

Dear Eric,
Thank you very much for your contribution!
I'm very interested in your solver and would like to know the difference between the standard chtMultiRegionFoam and multiRegionReactingFoam.
I would like to use it for laminar flame heating cold walls, I'm using reduced and detailed chemistry mechanisms. Regarding the thermodynamic package I mostly use the hePsiThermo one.

Regards,

Pablo

[edaymo]

Dear Pablo,

Glad to help.

Firstly, if you are using OpenFOAM 11 or 12 this multiregionReactingFoam contribution is outdated. With the modular solvers, you can choose the thermo model (psi or rho thermo, buoyancy on/off, conjugate heat transfer on/off) with the case configuration.

However, if you are using recent (i.e., within the past few years) version of ESI's OpenFOAM( (openfoam.com) fork, then mutliRegionReactingFoam may be of interest to you for some specific scenarios. This is because the ESI fork has not (yet?) adopted modular solvers from the Foundation fork, and so thermo model (rho vs. psi) and buoyancy (on vs off) are hard coded into the solver itself.

chtMultiRegionFoam is hard coded for rho thermo and buoyancy on. You can of course effectively turn buoyancy off by setting gravity = 0. And for "low speed" flows rho thermo should get you the same answer as psi thermo. Thus, for many gas phase combustion applications with conjugate heat transfer, chtMultiRegionFoam should be just fine.

You can test out this hypothesis for your situation by running reactingFoam and chtMultiRegionFoam without conjugate heat transfer (e.g., running chtMultiRegionFoam with just a FLUID region, no SOLID region). If you're happy with chtMultiRegionFoam, then stick with the ESI version of the code.

However, if you think the reactingFoam solver configuration (no buoyancy + psiThermo) is better for your situation, mutliRegionReactingFoam should give the exact same answer as reactingFoam albeit with a solid region included.

If you're wondering now why multiRegionReactingFoam exists since the difference between it and chtMultiRegionFoam is very subtle, it's because this contribution was helpful before chtMultiRegionFoam had the ability to work with species and chemistry (OpenFOAM 5 and earlier). Now that this chemistry + conjugate heat transfer capability is standard in ESI and Foundation forks of OpenFOAM, multiRegionReactingFoam is generally only helpful for those who using the ESI fork who want a solver that's EXACTLY like reactingFoam but with conjugate heat transfer.

I hope this explanation is helpful!

Best regards,

Eric

[Pablok]

Hi Eric,
Thanks for the quick answer.
In my case I'm using the ESI versions of OpenFoam (2106 and above). I also have my own modified version of reactingFoam (mostly working with psiThermo, haven't tried with rhoThermo yet) that I would like to combine with CHT.
multiRegionReactingFoam sounds like the perfect tool for that, I would modify/replace the fluid solver with my own version of reactingFoam and compile it again.
Do you know a simple validation test case for such application? I saw the reverseBurner case but I would like to get rid of turbulence at first.

[edaymo]

Hi Pablo,

Yep - that sounds like a good plan to replace the fluid solver in multiRegionReactingFoam with your own and then compile the new solver.

As to validation cases, here are some ideas:
1. chtMultiRegionFoam has been (I would guess) validated by others. You could create a laminar flow case of your choosing in chtMultiRegionFoam and use that to compare to your solver.
2. Even better, create a case with OpenFOAM 11 or 12 using the modular solver approach, and then compare to your solver.
3. S.M. Mousavi produced a version of multiRegionReactingFoam and has a tutorial case that comes with his work. I have not tried his work. Please see https://www.tfd.chalmers.se/~hani/ku...rteza_Mousavi/.

Meanwhile, there has been some work to validate multiRegionReactingFoam. I don't have the cases, but I have seen the following publications validating mutliRegionReactingFoam.
1. Modeling Turbulent Combustion Coupled with Conjugate Heat Transfer in OpenFOAM https://doi.org/10.1007/978-3-030-55874-1_113

2. J. Toumey has a master's thesis where multiRegionReactingFoam was used for validation cases https://ctdigitalarchive.org/node/3313285


As to my own work -- Most of my validation work with conjugate heat transfer involves surface reactions (as part of the DETCHEM DUO project). I don't have anything that I can think of in my files that both belongs to me and is only for homogeneous reactions but with conjugate heat transfer.

But to recap my main point, I think that OpenFOAM has validated solvers for this purpose, so if you lack data or access to a non-OpenFOAM software solution, you can probably get a good start on your validation case by just running the same case with your custom solver and a standard OpenFOAM solver (or multiRegionReactingFoam) and seeing how they compare.

I hope I have given you some ideas.

Best regards,

Eric

[Pablok]

Hi Eric,
Thanks for your advice, I will try to set-up those cases.
I was able to compile multiRegionReactingFoam with my modified version of reactingFoam.
By curiosity I also tried to use multiRegionReactingFoam without a solid region but would get the error:

--> FOAM FATAL ERROR: (openfoam-2312)
solid not found in table. Valid entries: 1(fluid)

Is it not possible to use the solver with only one (fluid) region?

Best regards,

Pablo

[edaymo]

Hi Pablo,

I am guessing that you did not remove the solid region from the regionProperties file?
See this example regionProperties to run multiRegionReactingFoam (or chtMultiRegionFoam for that matter) with just a fluid region:

https://github.com/TonkomoLLC/multiR...gionProperties

Glad you got things to compile and are moving forward.

Best regards,
Eric

[Pablok]

Yes my bad! I just had to leave the solid entry empty like in your example!
I'll start "validating" and will post some case/results if I have something interesting.

Cheers,

Pablo