Thank you very much Paritosh and Bruno! I understand now the "*.OpenFOAM" file is an empty file for the paraView to know where to read the data. The "paraFoam -builtin" command combines all the "*.OpenFOAM" files into one file, and it works fine for the tutorial case "multiRegionHeater".

As Bruno as said, it is better to start with a simple case for which analytical solution is possible. I still can't get the files "planeWall2D{bottomAir}.OpenFOAM", "planeWall2D{topAir}.OpenFOAM" and "planeWall2D{wall}.OpenFOAM". I continue to compare the "planeWall2D" case with the "multiRegionHeater" to find out the reason.

Try this setup
 

Try this setup. I have made the following changes.

1. The first thing I notice is that the blockMeshDict file is in the system folder. I added following line to Allrun file to copy the file to constant/polymesh folder.
   
   Code:

   ---

   cp system/blockMeshDict constant/polyMesh/blockMeshDict

   ---

2. I combined Allrun and Allrun.pre files. This is personal preference, I like all the commands in one single file.
3. Changed the region name from 'wall' to 'solidWall'. This is do avoid confusion with the boundary type and any other boundary named wall or consisting word 'wall'. I also made corresponding name changes in all the files.

I am using openFoam 2.3 and the case ran without any errors.

If there are errors, don't forget to attach the log files.

Edit:
If you want to learn how things work with Allrun-type files, I advise you to run the case in steps. You can start with Allrun file with one command. Run the case then read and understand the log file. If everything is alright, add the next command and so on.

Quick answer: Check out the "log.<solverName>" file, there you will find the error that occurred!

Dear Paritosh,

Thank you very much for your help! It is very nice of you! Sorry that I couldn't reply earlier, it was too busy these days. I have several questions about fvSchemes in system/topAir.

What is div(Ji,Ii_h) please? I didn't figure it out with google. I understand div(((rho*nuEff)*dev2(T(grad(U))))) the same term as div((muEff*dev2(T(grad(U))))). Am I right? If so, why the both should be written? These two terms do not exist in Bruno's planeWall2D case.

I don't understand the divSchemes completely.
div(phi, U) is the advection of velocity,
what is div(phi, K) please?
div(phi, h) is the advection of enthalpy,
what is div(phi, k) please?
div(phi, K) is advection of the turbulent kinetic energy,
div(phi, epsilon) is advection of the dissipation rate
div(phi, R) is advection of the Reynolds stress,
div(R) is the divergence of the Reynolds stress.

Thank you very much in advance!

Dear Paritosh,

Thank you very much for your help! I have run your "planeWall2D_corr", but it didn't work out completely. "log.blockMesh", "log.topoSet", "log.splitMeshRegions" reported no error. The error began in "log.changeDictionary.solidWall" as

--> FOAM FATAL IO ERROR
cannot find file
file: .../planeWall2D_corr/0/solidWall/dictionaryReplacement at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 72

FOAM exiting

I can run through the tutorial case "multiRegionHeater". I compared the two cases and found that in "mutiRegionHeater" the "changeDictionaryDict" in e.g. "system/bottomWater" begins without "dictionaryReplacement". Why must this function be in planeWall2D please?

I didn't figure out how to attach files and pictures in my Reply in the forum. Could you give me a hint please?

Thank you very much in advance! I really appreciate your help!

Dear Paritosh,

It is quite strange for me that, I got the following error when I ran blockMesh in the original case files of Bruno,

fileName:: stripInvalid() called for invalid fileName Terminaloutput
For debug level (=2) > 1 this is considered fatal
Aborted (core dumped)

But the same blockMeshDict ran successfully in your planeWall_corr case files. I checked the directory, all the folder names are with letters and numbers without spaces. Did you have a similar experience?

I am new in OpenFOAM, I believe I will have quite a few strange mistakes. I would appreciate if you could help me on this. Thank you very much in advance!

Dear Paritosh,

No matter how I rename the folder of Bruno's original case, blockMesh never worked. However, I created a new folder with a valid name as "planeWallTest", and copied all the files of Bruno to this new folder, the blockMesh functioned! Do you have an idea why it is so folder dependent? I suspect whether I have dong something wrong with the installation.

Hey Bruno,
Do you have this CHT tutorial for OpenFOAM v4.1? Or can you suggest what changes is to be made?

Thanks and HNY,
Sandeep

@sandeep.pandey

I am making a short tutorial video for the Planewall2D case with OF 4.1. I will post a link in this thread in a couple of days.

Hey Jaydeep,
Thanks for taking this initiative, eagerly waiting!:)

planeWall2D case for OpenFOAM4.0
 

Happy New Year everybody,

I have made a more simplified version of the planeWall2D. I would appreciate if anyone would like to comment on the resulting temperature and velocity fields. Are they correct?

I wonder how to display the velocity in the solid domain as 0 instead of red in my image?

When I plot the velocity vector field with Glyph in paraView, there are always two arrows in one cell. I attached my state file, any suggestions would be very helpful for me.

I wonder how can I monitor the residuals during computing. I tried
and add
below the "runApplication 'getApplication' " in "Allrun", but it was unsuccessful with the following text in the terminal:
Does anyone know how to manage it?

Thank you very much in advance,

All the best,

Sitajeje

Happy New Year Alex,

your master thesis is really impressive! I learned a lot from your descriptions and case files, especially about the fvOption! Thank you very much for sharing your master thesis with the public!

Best,

Sitajeje

Happy New Year,

I'm glad you find my site useful, Sitajeje, and I really appreciate your thoughts about it. I hope more people can find a little help in my web site.

Best regards,

Alex

Hallo Alex,

I am struggling with adding a heat source to chtMultiRegionSimpleFoam with fvOption. I divided my computation domain into 2 blocks and gave name to them. I found that topoSet is then not necessary. Am I right?

I copy your fvOption file into constant/heater and set cellZone to heater. blockMesh, splitMeshRegions, changeDictionary ran through till chtMultiRegionSimpleFoam. The error appears as

keyword selectionMode ist undefined in ..../fvOption.volumetricHeatSource.scalarSemiImplicitSo urceCoeffs

The same error occurred when I added selectionMode into the dictionary scalarSemiImplicitSourceCoeffs.

I found quite a few your comments and questions on chutMultiRegionSimpleFoam. You mentioned in a thread in 2014 that the source term is of no effect in the new chtMultiRegionSimpleFoam solver. Is it true? I would appreciate greatly if you would share your experience with me.

Thank you very much in advance!

Best regards,

sitajeje

adding heat source to chtMultiRegionSimpleFoam with fvOptions
 

Dear Foamers,

I want to add heat source to the solid domain while calculating with the chtMultiRegionSimpleFoam solver. I followed the following link which is a discussion of Bruno with another problem reporter on adding heat source with fvOptions.

https://bugs.openfoam.org/view.php?id=1266

The test case is the same as my post #91, except that fvOptions is added in system/heater and the bottom face of the heater is changed to zeroGradient instead of fixedValue in temperature.

I met a strange error as

I would appreciate greatly if someone can help me!

Best regards,

sitajeje

got it done. It was a version problem. The case from Bruno is excellent!

Hi sitajeje,
I want to use chtMultiRegionFoam for a problem. But I thought it is better to start with chtMultiRegionSimpleFoam. Since the old files are not compatible, I don't know how to modify them. Did you apply it on OF v 4.0? Do you know whether it is compatible with v 4.1 or not?
Is it possible for you to share your file?

mom

Dear Jaydeep,
I am eagerly waiting for your tutorial video ;)
Thank you all for allocating time and sharing your knowledge

mom :)

reversal flow at the outlet in a free convection
 

Dear OpenFOAMers,

I met a problem with chtMultiRegionFoam while simulation natural convection. I believe I am not the only person who met this difficulty. I would appreciate if anyone can help me. It is going to be helpful for our community.

Please find my computation domain in the attached image. It is a 2D simulation. The domain is 25mm wide and 135mm long. The Grashof number is roughly 1e6 < 1e9, so the flow should stay laminar. The left border is an insulated wall. A rectangular solid with a heat source of 1W locates next to the wall. The other three sides are atmosphere with totalPressure, p0=1e5 for p_rgh and pressureInletOutletVelocity, value uniform (0 0 0) for u.

I would expect a thermal boundary layer next to the wall, which extends out of the domain with a weak scattering after passing the heating solid. However the boundary layer decreases its speed pretty far away from the outlet and becomes reversal flow next to the right border. I doubled the width of the computation domain, and the same result occurs: the flow reverses and turn down next to the right border. This indicates that the simulation is wrong because of the boundary condition.

I wonder whether anyone has experience with setting the boundary conditions of atmosphere for free convection? Any suggestions, comments would be very helpful for me. Thank you very much in advance!

Best regards,

Sitajeje

Dear Foamers,

Problem is solved. The temperature should be zeroGradient at the upper border instead of inletOutlet.

Thank you all the same!

Best regards,

Sitajeje