CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Conjugate heat transfer and reactingFoam (chtMultiRegionReactingFoam)

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree16Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 29, 2016, 21:19
Default Conjugate heat transfer and reactingFoam (chtMultiRegionReactingFoam)
  #1
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hello,

If anyone is interested in a solver with conjugate heat transfer + gas phase reaction capabilities, I've posted to github a hybrid of chtMultiRegionFoam and reactingFoam called chtMultiRegionReactingFoam. Steady state and transient solvers for OpenFOAM 4 and the current OpenFOAM-dev version are available (along with tutorials) at:

https://github.com/TonkomoLLC

I hope this is useful for your work. Feel free to contact me if you have any questions or comments.

Best regards,

Eric D.
Tonkomo, LLC
Twitter: @TonkomoLLC,
email: info at tonkomo.com
edaymo is offline   Reply With Quote

Old   August 30, 2016, 11:15
Default Thanks!
  #2
Member
 
Arvind Jay
Join Date: Sep 2012
Posts: 96
Rep Power: 14
arvindpj is on a distinguished road
I was waiting for this feature. I will test and report.
-Jay
arvindpj is offline   Reply With Quote

Old   February 27, 2017, 09:57
Default
  #3
New Member
 
Mohamed el Abbassi
Join Date: Oct 2016
Location: Delft, the Netherlands
Posts: 9
Rep Power: 9
melabbassi is on a distinguished road
Hi Eric,

Thank you for your contribution. I have studied the solver (OpenFOAM 3) this month and benchmarked the implementation of reaction in the cht-version against rhoReactingFoam which is also based on p_rgh. So only 1 region and no conjugate heat transfer. As a test case I modelled the Sandia D flame with 2-step reaction mechanism of Westbrook and Dryer.

With the steady state version I initially couldn't get ignition. Even after adjusting the relaxation factors and setting the initial internal field temperature to 2000 K. The maximum temperature immediately drops to inlet values. I found out that the convention with the SIMPLE algorithm to use a timestep of 1 s was the issue. Unlike the navier stokes equations for steady state problems, the energy and species equations are largely dependent on time, which is probably taken from the 'virtual' timestep. Choosing high timesteps allows little energy release. By adjusting the time step to a much lower value (so that max Courant nr is about 0.2), reaction was finally possible.

Attached you'll find a plot of the temperature progression along the rotation axis. Maximum temperature and temperature rise are similar, but reaction starts a little bit more upstream with chtMultiRegionSimpleFoam. Still, it is a very good result.

The transient version of the solver is less robust. I needed 4 nOuterCorrectors instead of 1 with rhoReactingFoam to get the simulation going, leading to 4 times longer runtime. Can it be due to the pimple algorithm that is implemented differently?

Best,
Mohamed
Attached Images
File Type: png T_plot.png (55.2 KB, 126 views)
arvindpj likes this.
melabbassi is offline   Reply With Quote

Old   February 27, 2017, 15:57
Default
  #4
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hi, Mohamed,

Thank you very much for such a detailed review of chtMultiRegionReactingFoam! This is great feedback, especially on your solution technique for the steady state solver and the benchmark findings.

rhoReactingFoam and chtMultiRegionReactingFoam (directly based on chtMultiRegionFoam for the PIMPLE algorithm) do indeed have different formulations for PEqn, but I do know know offhand if this the root cause of the nOuterCorrectors issue you are report. I am happy to look at your test cases in more detail if you wish to send them to me. To start with, I would want to repeat with OpenFOAM 4.x or OpenFOAM-dev. The OpenFOAM 3.x version you are using is a "beta" version of the chtMultiRegionReactingFoam solver and it was not as thoroughly tested as the versions on github.

I also note that since my initial August 2016 post I have placed on our github site two new solvers: "multiRegionReactingFoam" and "multiRegionReactingPimpleCentralFoam" (the latter based on https://github.com/unicfdlab/hybridCentralSolvers). I have tested multiRegionReactingFoam more extensively against reactingFoam and I would be very curious to know if this solver meets your expectations.

I look forward to further feedback. Thank you again for your insightful reply.

Best regards,

Eric
edaymo is offline   Reply With Quote

Old   March 1, 2017, 09:10
Default
  #5
New Member
 
Mohamed el Abbassi
Join Date: Oct 2016
Location: Delft, the Netherlands
Posts: 9
Rep Power: 9
melabbassi is on a distinguished road
Thanks for the clarity! That explains certain bugs I encountered in your beta version. I should have updated to OF 4 sooner, but it was good training exercise for me to be honest.

I will send you the case files for chtMultiRegionReactingFoam and rhoReactingFoam. Thank you very much for your effort! I will also run them again on OF 4.

The reason I used the p_rgh based solvers was because I wanted to make a consistent comparison and wasn't aware of the psi based multiRegionReactingFoam. Thanks for uploading it!

I'll keep you updated.
melabbassi is offline   Reply With Quote

Old   April 24, 2017, 13:13
Default Hello!
  #6
New Member
 
Jessica Smit
Join Date: Dec 2016
Posts: 1
Rep Power: 0
skibenochek is on a distinguished road
Thank you for your work! Can I use your solver with OpenFoam 2.3.0?
skibenochek is offline   Reply With Quote

Old   April 24, 2017, 14:14
Default Re: Hello!
  #7
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hi,

Thanks for the feedback!

The same programming principles apply for coding a CHT+reaction solver for OpenFOAM 2.3.0, but i think you will find that the solvers on my GitHub page will not compile as-is for OF2.3.

I've got a version of the CHT+reaction solver for OpenFOAM 3.0.x that I haven't gotten around to putting on GitHub yet, but I have not yet created one for OF 2.3/OF2.4.

Please contact me directly (e.g., private message, or info at tonkomo.com) if you would like my assistance to port this CHT+reaction solver to OF2.3. Thanks!

Best regards,

Eric
edaymo is offline   Reply With Quote

Old   October 2, 2017, 11:01
Default OFV5 multiregionsimplereactingfoam error
  #8
Senior Member
 
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 112
Rep Power: 10
Swagga5aur is on a distinguished road
Hello Eric

First of all I would like to thank you for this solver and the continuous work, as I used it for my master thesis concerning modelling a reformation process with external heating.

I noticed an error in the OF 5.0 multiRegionSimpleReactingFoam with respect to the createFluidFields.H dictionary missing the following line

Code:
    reactionFluid[i].setTurbulence(turbulence[i]);
after the following code

Code:
    Info<< "    Adding to turbulence\n" << endl;
    turbulence.set
    (
        i,
        compressible::turbulenceModel::New
        (
            rhoFluid[i],
            UFluid[i],
            phiFluid[i],
            reactionFluid[i].thermo()
        ).ptr()
    );
Prior to this addition I got a turbulence Ptr error when trying to solve a turbulence reaction model.

Just wanted to let you know

Best regards
Lasse
arvindpj and edaymo like this.
Swagga5aur is offline   Reply With Quote

Old   October 2, 2017, 15:48
Default Re: OFV5 multiregionsimplereactingfoam error
  #9
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Dear Lasse,

Thank you very much for the bug report. Indeed, you are correct, and all of the multiRegionSimpleReactingFoam solvers (OF4, 5, dev, 1706, 1612+) have been updated with the reported fix to setTurbulence. I checked the other solvers (e.g., transient multiRegionReactingFoam, chtMultiRegionFoam, etc.) just to be sure, but I didn't find this bug outside of mutliRegionSimpleReactingFoam.

I really appreciate your bringing this matter to my attention. I'm also really happy to learn that this solver helped with your Master's thesis, and that you got good results with it.

Best regards,

Eric
edaymo is offline   Reply With Quote

Old   October 2, 2017, 16:15
Default
  #10
Senior Member
 
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 112
Rep Power: 10
Swagga5aur is on a distinguished road
Hello Eric,

No problem, glad to be of help.

I am experiencing some convergence issues with the multiRegionSimpleReactingFoam compared to the transient solvers multiRegionReactingFoam and reactingFoam.

Not sure if something else is missing in the solver but I'll look into it and post if I find any issues .

I believe the issue may be with the implementation of the OF5.0 EDC combustion model.

Best regards,
Lasse
Swagga5aur is offline   Reply With Quote

Old   October 2, 2017, 16:28
Default
  #11
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hello, Lasse -

I don't typically use the steady state solver, rather, I tend to use the transient solver with LTS.

One idea is to try the same problem with simpleParcelReactingFoam, which is a single region, steady state solver with chemistry, albeit with rhoReactingThermo. Assuming you can come up with reasonable BC's for a non-CHT case, this approach might narrow down whether the problem is with the multiRegion solver, or if the problem is with some other model or the setup.

Good luck and feel free to contact me if I can be of assistance.

Best regards,

Eric
edaymo is offline   Reply With Quote

Old   April 1, 2023, 01:36
Default
  #12
New Member
 
BISSAI NKAA
Join Date: Feb 2022
Posts: 16
Rep Power: 4
sante_junior is on a distinguished road
Hi Mr. El Abbassi
I read with great attention your exchanges with Eric Daymo and your work on conjugate heat transfer through a rotary kiln. I was very impressed with your results. I am looking to reproduce a work almost identical to yours in a cement kiln using local refractory materials where I will use biogas and LES as a turbulence model.

Please can you share your test cases with me so that I can use them as a tutorial?

Sincerely Sante Junior BISSAĻ
sante_junior is offline   Reply With Quote

Old   April 2, 2023, 16:33
Default
  #13
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 723
Blog Entries: 1
Rep Power: 17
dlahaye is on a distinguished road
We documented the reverseBurner tutorial test case and made our report available at https://mega.nz/file/eBcxWKgJ#CXhpWd...5O3CHRBqIX6XKk . Possibly there is valuable information here.

Kind wishes, Domenico.
dlahaye is online now   Reply With Quote

Old   April 4, 2023, 01:13
Default
  #14
New Member
 
BISSAI NKAA
Join Date: Feb 2022
Posts: 16
Rep Power: 4
sante_junior is on a distinguished road
Quote:
Originally Posted by dlahaye View Post
We documented the reverseBurner tutorial test case and made our report available at https://mega.nz/file/eBcxWKgJ#CXhpWd...5O3CHRBqIX6XKk . Possibly there is valuable information here.

Kind wishes, Domenico.
Hi Domenico
Thank you for your quick reply. I will take a closer look.
Sincerely, Sante Junior BISSAI
sante_junior is offline   Reply With Quote

Old   April 23, 2023, 03:58
Default
  #15
New Member
 
BISSAI NKAA
Join Date: Feb 2022
Posts: 16
Rep Power: 4
sante_junior is on a distinguished road
Quote:
Originally Posted by sante_junior View Post
Hi Domenico
Thank you for your quick reply. I will take a closer look.
Sincerely, Sante Junior BISSAI
Hi Domenico Lahaye
Your document has helped me a lot. But I am facing a new dilemma. I have two regions (fluid and solid) but when I run my case, the second region is not read and my calculation spits out and generates me errors.
I attach the image of the error to my message.

I really need your help
Attached Images
File Type: jpg solide region error.jpg (115.1 KB, 14 views)
sante_junior is offline   Reply With Quote

Old   April 23, 2023, 17:24
Default
  #16
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hi,
If I read your printStack correctly, it seems the problem is with one of your patches, and the exact reason fo the solver crash is that there is no field named phi (phi is the mass flux, kg/m2/s). For a solid we do not expect convection and thus it is not surprising that there is no field named phi. The printStack also refers to the inletOutlet BC, which is not a good BC for a solid region, since inletOutlet requires the surfaceScalarField phi... that as mentioned does not exist in a solid region.
I hope this analysis is helpful.
Best regards,
Eric
edaymo is offline   Reply With Quote

Old   June 19, 2023, 22:25
Default
  #17
Member
 
mactone hsieh
Join Date: Apr 2012
Location: Taiwan
Posts: 31
Blog Entries: 1
Rep Power: 14
mactone is on a distinguished road
Hi Eric,

Thank you for sharing the code. In the reverseBurner case, simple burner interacting with wall can be solved. I wonder what's the difference between this chtMultiRegionReactingFoam with official openfoam9 chtMultiRegionFoam?

If the solid is composed of multiple layers of materials, how to set it? Any tutorial or examples?

Thank you.
mactone is offline   Reply With Quote

Old   June 19, 2023, 23:22
Default
  #18
Member
 
Eric Daymo
Join Date: Feb 2015
Location: Gilbert, Arizona, USA
Posts: 48
Rep Power: 12
edaymo is on a distinguished road
Hi Mactone,

chtMultiregionReacting foam is outdated: it really only served a purpose through OpenFOAM 5.x. In OpenFOAM 6 chemical reaction capability was added to chtMultiRegonFoam and it's capability is the same as chtMultiRegionReactingFoam.

I also maintained multiRegionReactingFoam also at TonkomoLLC's GitHub site until this year (psiReactionThermo, p instead of p_rgh equation). However, now OpenFOAM-dev (what I presume will be called OpenFOAM 11 in a month or two) has the ability to mix and match conjugate heat transfer, chemical reactions, buoyancy and so much more through the use of modules. Thus, OpenFOAM "11" will surely have the same capabilities as multiRegionReactingFoam.

To answer your other question... If the solid is comprised of multiple thin layers you can use the kappaLayers feature in the conjugate heat transfer boundary condition. If the layers are thicker and you wish to model the solid domain, then I think the old OpenFOAM 6 multiRegionHeater tutorial can show you how to setup multiple adjacent solid layers. I don't think this tutorial has been included in newer versions of OpenFOAM.

Happy foaming!

Best regards,
Eric
edaymo is offline   Reply With Quote

Old   June 20, 2023, 04:41
Default
  #19
Member
 
mactone hsieh
Join Date: Apr 2012
Location: Taiwan
Posts: 31
Blog Entries: 1
Rep Power: 14
mactone is on a distinguished road
Hi, Eric,

Great appreciated for the lightening speed reply.

It looks the OpenFOAM is becoming better and better with your support. Really looking forward OpenFOAM 11, though I use OpenFOAM-v2206 now.

Meanwhile, I can use multiRegionReactingFoam at TonkomoLLC's GitHub site to solve mix and match conjugate heat transfer, chemical reactions, buoyancy problems. Is that correct? It seems the chtMultiRegionFoam could also solve reactingFlow, I still don't know the difference between chtMultiRegionFoam and multiRegionReactingFoam.


Last, for the kappaLayers, I've used the boundary below for the furnace wall in the reactingFoam, though using the externalWallHeatFluxTemperature will change the combustion chamber temperature, the simulation results only show the fluid temperature. If I use multiRegionReactingFoam, I could get the transient temperature change of the furnace wall?

Code:
Walls
{
        type            externalWallHeatFluxTemperature;

        mode            coefficient;

        Ta              constant 300.0; // ambient temperature [K]
        h               constant 10.0; // Heat transfer coefficient [W/m^2/K]
        thicknessLayers (0.05 0.02); // Layer thicknesses [m]
        kappaLayers     (0.04  50); //Layer thermal conductivities [W/m/K]
       // It's isowool-1260 5cm (0.04 W/m/K) + steel plate 2cm (50 W/m/K)

        kappaMethod     fluidThermo;

        value           $internalField;
    }
mactone is offline   Reply With Quote

Old   June 20, 2023, 05:17
Default
  #20
Member
 
mactone hsieh
Join Date: Apr 2012
Location: Taiwan
Posts: 31
Blog Entries: 1
Rep Power: 14
mactone is on a distinguished road
Quote:
Originally Posted by edaymo View Post
Hi Mactone,

chtMultiregionReacting foam is outdated: it really only served a purpose through OpenFOAM 5.x. In OpenFOAM 6 chemical reaction capability was added to chtMultiRegonFoam and it's capability is the same as chtMultiRegionReactingFoam.

I also maintained multiRegionReactingFoam also at TonkomoLLC's GitHub site until this year (psiReactionThermo, p instead of p_rgh equation). However, now OpenFOAM-dev (what I presume will be called OpenFOAM 11 in a month or two) has the ability to mix and match conjugate heat transfer, chemical reactions, buoyancy and so much more through the use of modules. Thus, OpenFOAM "11" will surely have the same capabilities as multiRegionReactingFoam.

To answer your other question... If the solid is comprised of multiple thin layers you can use the kappaLayers feature in the conjugate heat transfer boundary condition. If the layers are thicker and you wish to model the solid domain, then I think the old OpenFOAM 6 multiRegionHeater tutorial can show you how to setup multiple adjacent solid layers. I don't think this tutorial has been included in newer versions of OpenFOAM.

Happy foaming!

Best regards,
Eric

Hi, Eric,

I try to use the reverseBurner case in tutorial with multiRegionReactingFoam.
It showed FOAM FATAL ERROR:
Code:
Unknown patchField type compressible::turbulentTemperatureRadCoupledMixed for patch type mappedWall
It's the error due to T boundary condition, I am not sure it gas or solid side error.

I wonder if you could provide me a sample case file for multiRegionReactingFoam and multiRegionSimpleReactingFoam respectively.

Great appreciated.

Best,
Mactone
mactone is offline   Reply With Quote

Reply

Tags
chtmultiregionfoam, conjugate heat transfer, openfoam, reactingfoam, reaction

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[swak4Foam] how can use Cp and Cv in Swak variables? immortality OpenFOAM Community Contributions 18 December 9, 2016 01:04
Multiregion heat transfer Habibfateh OpenFOAM Programming & Development 0 February 18, 2014 15:53


All times are GMT -4. The time now is 03:21.