chtMultiRegionSimpleFoam
 

Dear All,

I am trying to run chtMultiRegionSimpleFoam.

I have prepared a case with 1 fluid region and 6 solid regions.

I have set my case and when I lauch it, I get this error:


I can not understand what it means. Could you help, please?

Thanks a lot,
Samuele

Hi Samuele,

Can you attach the boundary conditions for the "pcm" region, as well as any regions that are in touch with it?

Although, if I have to guess, I think that this sentence:
means that for a certain patch, on one region you have "zeroGradient" and on the other region you have "turbulentTemperatureCoupledBaffleMixed". But the two seem to be incompatible.

Best regards,
Bruno

Dear Bruno,

thanks for answering, first. Also, about your suggestions, I completely agree. The point is that I chacked the boundary conditions twice and I can't find any error. I am attaching to this email all the changeLogDictionary I use. Could you kindly have a look and let me know what's wrong with it?

Thanks a lot,
Samuele

Dear Samuele,

it seems that you put this B.C for a patch in a region (compressible::turbulentTemperatureCoupledBaffleMi xed). then you put zeroGradient to the same patch in the other region which is not applicable. the B.C must be the same for same patch in different regions.

hope it helps.
BR,

I will check it again, then.

Thanks a lot,
Samuele

I have found a first error: I haven't set the right BC in the fluid region.

I ran my case and I get a different error: could you help in solving this, too?

Thanks a lot,
Samuele

The error message is:

Dear Samuele,

this error always appears when there is a problem with three factors: cell size, time step, velocity value. you must compromise the three factors to get smooth run.

hint: adjust dimensions and cell size such that patches boundaries lays on cells boundaries not in middle of it.

hope it helps,

Best Regards,

Ahmed

Do you mean that it could be necessary to remesh my geometry?

no i don't mean so, i only drag your attention to revise it, but you can change your velocity value, or time step. you can go back to the user manual to know how to set time step.

I think that being a steady simulation, the time-step does not influence the solution: is this right?

Greetings to all!

@Samuele:
AFAIK, that is correct. The time step doesn't matter in steady-state simulations... at least not usually.
The unusual example might be LTSInterFoam: http://www.openfoam.org/version2.0.0/steady-vof.php

It gave a SIGSEGV signal (#1) when trying to perform "polyMeshTetDecomposition :: findFaceBasePts" (#3). I'm guessing that this means that there is something very wrong with your mesh. Do a complete check mesh by running:
Best regards,
Bruno

Dear Bruno,

thanks for answering and pardon for the late reply.

This is the output of the command you suggested:

Could you help?

Hi Samuele,

:eek: Oh, this is bad, very bad! Cell determinant values of "0" basically means that there is either a contorted cell that crosses over itself or that it's a cell without volume. This is probably what's triggering the crash!

paraFoam provides you with the ability to also see the sets. Turn on that option and choose to see "underdeterminedCells" that should appear in the same list as the patches. Then try to see where exactly where the problem cells are and try to re-do your mesh.

Another possibility is to follow the example shown here: http://openfoamwiki.net/index.php/SetSet#Usage_example - more specifically, to only remove the cells associated to "underdeterminedCells". But keep in mind that this kind of cell removal strategy has certain limitations, such as possibly and wrongly removing some important cells.

Best regards,
Bruno

Dear Bruno,

I am attaching a picture of the whole volume where it is evident where the underdeterminedCells are.

I can't understand what's wrong with them. Do you have any idea?

First of all, I will try your suggestions.

Thanks a lot,

Samuele

Dear Bruno, Dear All,

after having re-meshed my geometry, I get a very strange result.

First of all, all the mesh checks are ok! Hance I thought that my simulation would have started immediately, but..
..but I got this error:
And trying to open the geometry with paraview, it crashes when I want to view the patches and not the internal mesh. I get a segmentation fault.
And this happens for each region.

Do you have any idea? Could you help?

Hi Samuele,

There seems to be a problem with a patch that is defined to be a symmetry plane:
But without access to the files, I cannot see the actual problem for myself.

Best regards,
Bruno

Here is the case: https://www.dropbox.com/sh/tgdwuqkfodgdffk/zFNdkvUgjH

Could you have a look?

Thanks a lot,
Samuele

This is not a problem of
... if I am not wrong I know this error and I searched long time to find the trivial Problem.
If I am right you have a Problem in the Boundary Conditions of T in packs_2 or in your fluid Region. Maybe your boundary file is wrong (patch type).

Maybe you have no value set.?

Your mesh seems okay.

Regards
Tobi

Dear Tobi,

thanks for answering. Actually, I have solved this very problem (it was due to a bad definition of the boudary conditions) and the simulation's running.
However, the temperature seems to be meaningless: I do have a max temperature of about 740000 K. Too much, I say.

I am going to check this problem, too. Any idea to begin to investigate the issue?

Thanks a lot,
Samuele.

Hi,

write out the first 10 or 20 integrations and have a look at your Domain.
You will be able to see the regions where you get the high temperature values. It could be possible that this Problem occure due to a mesh Problem. otherwise you see if your BC are incorrect or your Settings are wrong.

Good luck

similar problem, but maybe related to some BC
 

Greetings all,

I know this is a very old thread but I'm facing a problem that looks very similar to the one posted here. I'm dealing with a multi region case with the chtMultiRegionFoam solver. My case is made up of some solid regions and a fluid region. It starts solving first the fluid region with no problem but when it starts to solve the first solid region the following error comes up:
Althoug it's not exactly the same message that appeared to the thread's creator (mine seems to be related to some BC, but I don't know exactly which one nor what the problem is...) I followed the steps that Bruno Santos suggested. I check the mesh topology and I found that
Seeing this error I understood that I had exactly the same problem than the creator of the thread, although the message was not exctly the same... Well, first of all I would really like to know what exactly means this error and what an under determined cell is, because the under determined cells in my case belong to some thin regions that are made up of only one column of cells. I actually solved this error by dividing these regions into more columns of cells in the blockMeshDict file.

After I solved the problem with the under determined cells I ran the case again but the same error was shown, so I got stuck because I don't know what it really means and I don't know where to look up.

I attach the changeDictionaryDict file and the T file belonging to the region that crashes so that you can check if there is something wrong in them. In case you need more files or even the entire case, just ask me for it! ;)

Many thanks in advance.

Regards,

Alex

Greetings Alex,

In a case like this, you should apply the good old strategy of "isolate and conquer".

Anyway, from what I can see in the "T" file you provided, there are two major threats:

1. You're using groovyBC. Not that it's dangerous by itself, the problem is that apparently you're not experienced enough with it. Therefore, the first step would be for you to first put aside using groovyBC for now, until you can figure out what is the reason for the problem.
2. You're trying to use variables that are defined only at the end of the file "T". I'm not even sure what to say here... mmm, I guess that this is a good analogy: I'll tell you why this is a problem, after you've spent some time reading a least one good C++ book ;)

Best regards,
Bruno

Dear Bruno,

Thanks for your quick answer!

The wiser advise you could ever give in a case like mine. However, as I am trying to be as wise as you, I already isolated but I'm still waiting for my conquest to come... :(

1. As I mentioned in other posts and you noticed somehow, I'm not an experienced swak user. Nevertheless, finally yesterday I could manage to solve the problem with groovyBC. The problem was that the boundary of the solid region needed a variable coming from a function object I forgot to define in controlDict. I defined it for the fluid region but forgot to do so for the solid region. Thus, I managed to solve my problem! :)
   
   
   Quote:

   Originally Posted by wyldckat (Post 531859) You're trying to use variables that are defined only at the end of the file "T". I'm not even sure what to say here... mmm, I guess that this is a good analogy: I'll tell you why this is a problem, after you've spent some time reading a least one good C++ book ;)

That sentence reminds me of something... Maybe some advice I gave to a novice recently... Are you attacking me with my own weapons? :eek: Well, you are right, my C++ skills are more than weak, but I found no time to learn something about it on my own so far. However, I know something about C language and I know that declaration of variables goes at the top of the file, not at the bottom. I guess that something like that happens in C++... By the way, I didn't put the variable definition at the bottom, the fact that they are in there is because of what we talked about a couple of days ago.

Well, now I could finally make it work I still have a problem. The problem is that the simulation starts running but after some time steps it crashes. Here you can see the last time steps for the fluid region (the one that make it crash):
The problem comes from the inlet patch where the T falls bellow 0 and its value is going down for the last steps. This problem is only coming from one or maybe two cells whose faces belong to the patch, its velocity is raising very fast and its temperature falls. I attach the velocity, temperature and pressure definition at both patches (inlet&outlet)

• T:
  
  Code:

  ---

      up //outlet
    {
        type            inletOutlet;
        value          uniform 311.15;
        inletValue      uniform 311.15;
    }
    down //inlet
    {
        type            fixedValue;
        value          uniform 311.15;
    }

  ---

• P_rgh:
  
  Code:

  ---

      up
    {
        type            fixedValue;
        value          uniform 100000;
    }
    down
    {
        type            fixedValue;
        value          uniform 100000;
    }

  ---

• U:
  
  Code:

  ---

      up
    {
        type            pressureInletOutletVelocity;
        value          uniform ( 0 0 0.001 );
        phi            phi;
        rho            rho;
        tangentialVelocity uniform ( 0 0 0 );
    }
    down
    {
        type            pressureInletOutletVelocity;
        value          uniform ( 0 0 0.001 );
        phi            phi;
        rho            rho;
        tangentialVelocity uniform ( 0 0 0 );

  ---

  }

For more info, the case is about an air chamber that is heated by the solar radiation and the air inside the chamber flows because of the effect of the convection. If you need more info feel free to ask! ;) If I had more time I would have taken some screenshots so that you could see which cells lead to this crash. I will upload them as soon as I can!

Regards,

Alex

Hi Alex,

:eek: temperatures below 0 Kelvin...
It's very much possible that you're triggering an issue related to simulating heat transfer with a steady-state solver. This was addressed sometime ago in another thread... ah, here you go, start reading from here: http://www.cfd-online.com/Forums/ope...tml#post528307 post #60.

And yes, the idea I was trying to give you was exactly about having the variable initializations at the top. And C++ is very similar to C, only just very much more organized... if coded correctly ;)

And I knew that something wouldn't exactly as intended with changeDictionary :( I just couldn't remember what it was exactly.

Either way, the thread I mentioned hopefully will get you in the right direction.

Good luck! Best regards,
Bruno

Hi Bruno,

Thanks for the link but it's not exactly the same problem since my case is a transient one, not steady-state. Now I've had some time I took some screenshots so that you can have an idea about my problem. Here you can see the geometry I used.

http://www.cfd-online.com/Forums/att...1&d=1424098617

As you can see the air region is in the front, and the solid regions are just right behind it (the outline can be seen so that you can have an idea of my geometry). Attached you can find the temperature distribution for the last time step before it crashed. Also the U distribution is attached. As it is shown, the problem comes from the cells near the inlet patch, an extremely high velocity going out of the domain leads to an unphysical temperature distribution in the neighbouring cells, at least this is what it seems to my unexperinced eyes in the field of compressible flow in an opened domain...

I have tried with different discretizations, with a coarser mesh but it allways crashes, sometimes sooner, sometimes later, but it crashes all the time... I don't know if it is a problem of the mesh or a bad definition of the BC's (specification can be seen some posts above!). I need a little help to find the correct way to make it run.

Many thanks in advance.

Regards,

Alex

thread title is chtmultiregionsimplefoamwhich suggests steadystate.
moving on ...
have you checked that the regions are really conformal? (assuming this not AMI) and you havent gained an extra region?

I remember this causing similar issues.

Hello,

Finally I managed to "solve" it. The problem was, I guessed, the Courant number. The fact is that I was solving the case using a fixed time step of, if I'm not wrong, 1s. It was not causing any trouble during the first time steps but after a few time steps the Courant number started raising until the end of the simulation leading this to totally unphysical values. When I found it out I started the run with a deltaT of 0.2s during the first second to get it started and afterwards I switched the parameter adjustTimeStep to yes and maxCo to 0.9 in order to get better values for my simulation. Obviously, I got an improved temperature distribution but they are not totally correct yet. Here you can see the result I got, temperature minimums are not as unphysical as they were, but they are not physical at all yet.

Thanks for your help and time.

Regard,

Alex

Hi foamers,

Is there any kind soul to help me solve this problem? I am getting this error while running. I know the problem is coming from boundary condition but I do not know what should I do further. Please help.



Thanks in advance..................

Quick answer - Follow the instructions given here: http://www.cfd-online.com/Forums/ope...-get-help.html

dear all,
i'm still facing a crach of the chtMultiRegionSimpleFoam after 5 time steps here the end of the log file:
any suggestion will be very welcome, thank by advance ..

Please revise your boundary conditions.

Also, please check user manual for max number of iterations setting, that you may set unintensionally.

hi Ahmed,
thank very much for helping.
i post one of the many BC i have try...
and a little drawing of the physical problem, gaz going through a pipe.
i could not find where to increases the maximum number of iteration...
the solution is may be to run a transient solver first?

Hi Laurant,

I think you have a problem with your air velocity and pressure boundary conditions. Try converting inlet pressure and outlet velocity to zero gradient

the simulation is running only with laminar option, but the velocity of air goes up to 59 m/s ... for 1m./s at inlet
and if i turn kEpsilon option after 4 times step i got:
thank you for helping

Greetings to all!

I had this thread on my to-do list because of laurent98's questions and I finally today managed to take a look into it.

Unfortunately, since almost no information was provided about the case set-up, I'm not able to even try and guess what's wrong :(

@laurent98: If you have not yet solved this problem in your case, then please follow the instructions given on this thread: http://www.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

Bruno,

I know this is an old thread but I am facing the exact problem. I'm trying to solve a heat exchanger problem using chtMultiRegionSimpleFoam and the temperature goes to -90 and then it crashes. I opened a new thread a while ago and didnt get any response over there (http://www.cfd-online.com/Forums/ope...implefoam.html)

Going through different threads I found out maybe if I run my model as transient for a few time steps and then use that data as my IC it would work. Which it didnt and I am getting the following error:

I was wondering if you can take a look at my thread and let me know what am I doing wrong.
(http://www.cfd-online.com/Forums/ope...implefoam.html)

Thanks
Ali

have you changing the values of the
nNonOrthogonalCorrectors or the relaxationFactors in system/fluid_region/fvSolution?
a resource that helped me step up and solve such issues was this
http://www.dicat.unige.it/guerrero/o...sandtricks.pdf

Cheers, derek

Hi Bruno,
thank you very much for your interest, i didn't solve my problem with openfoam yet but i made a simplest computation by hand with classical thermic formulations.
please find attach a general presentation of the problem.
i'am sorry to not be on my computer now, i have not access right now to my OF's files
best regards Laurent

Derek,

Thanks for the response. I actually did play with the relaxation factors a lot!
My last test was that I fixed the temp. every where to see if the solution still explodes which it did! So, now I'm looking different ways to see if I can find some answers for my problem.

Hi Laurent!

As per the little information you provided related to your error some posts above, it seems that you are probably using an excessively high time step. Some time ago I faced a very similar problem to yours and setting adjustTimeStep to yes in controlDict helped me a lot!

Besides that, check that your inlet and outlet BC's are the proper ones.

Hope it helps you a little with your struggle!

Best regards,

Alex