CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   bubblefoam totally failed on unstructured mesh. (http://www.cfd-online.com/Forums/openfoam-solving/110206-bubblefoam-totally-failed-unstructured-mesh.html)

sharonyue December 6, 2012 02:34

bubblefoam totally failed on unstructured mesh.
 
Sorry, but yes, I have to concede that bubblefoam totally cant run on an unstructured mesh.
I even dont need to attach my case.
Just generate any simple cyclinder with an inlet,wall,outlet with an unstructured mesh. and run bubblefoam or twophaseeulerfoam.


bang!!......blowing up!


anyway,Thats is not my expected,I want a plausible suggestion how to prevent blowing up.

michielm December 6, 2012 04:14

If you want people to solve a problem for you, you should provide much much more details.

So you DO have to upload your case, because nobody is going to take the effort of making a mesh and running a simulation just to see what you mean.

If you show that you have put some effort into thinking about the issue and trying to solve it and share this information, then somebody might be willing (and be able) to help you.

sharonyue December 6, 2012 04:28

2 Attachment(s)
Hi Michiel:

Thank you very much for my consideration. actually I have done lots of works about bubblefoam, even all of them are extremely simple ones.




http://www.cfd-online.com/Forums/ope...tml#post396032
in this thread I tried use structured mesh on bubblefoam but failed, so I have to use unstructured mesh.then....

http://www.cfd-online.com/Forums/ope...behaviour.html
in this thread I have tried unstructured mesh on twoPhaseEulerFoam,or bubblefoam,it cant get convergence.

untill now I dont know if bubblefoam can handle unstructured mesh...

I cant upload my case because the fluent.msh is large.... but I can upload a image.
its a very simple case. if anyone can generate a mesh then just put it in mycase folder,the fluentMeshToFoam fluent.msh, setFields . bubbleFoam..
you will see the result.


everytime I receive an Email, I would be more closer to my success...thats exciting.

sharonyue December 10, 2012 02:29

Thats quite weird, is there anyone tried an unstructured mesh on bubblefoam?

sharonyue December 14, 2012 07:32

nobody is here?...

niklas December 14, 2012 08:34

get a dropbox account and put the mesh there.

why do you have different inlet velocities for the phases?

sharonyue December 14, 2012 09:25

Quote:

Originally Posted by niklas (Post 397539)
get a dropbox account and put the mesh there.

why do you have different inlet velocities for the phases?

Thank you for reminding me the dropbox Niklas. I upload my case on hotfire. you can chekc it out there.
https://hotfile.com/dl/184355810/d49...p.html?lang=en
https://hotfile.com/dl/184356440/5e7...p.html?lang=en


you can run it directly as of I have set the alpha field and generated the mesh.:

twoPhaseEulerFoam


U1 is the gas velocity , U2 is the liquid velocity, there is only air get in the column,so U2 inlet is zero.

If you can give me any assistance I would be very appreciated.

niklas December 14, 2012 10:49

doesnt work. hotfile is terrible.
cant download and now it says im downloading and I can only download 1 at a time.

sharonyue December 15, 2012 00:08

Quote:

Originally Posted by niklas (Post 397567)
doesnt work. hotfile is terrible.
cant download and now it says im downloading and I can only download 1 at a time.

here is a link on dropbox~

https://www.dropbox.com/s/1v6n8cf39n...structured.zip
https://www.dropbox.com/s/mguy6w6gm9...structured.zip

sharonyue December 18, 2012 01:52

Looks like only FOAM developers can tackle this problem?...

niklas December 18, 2012 02:41

the main problem is the mesh-quality at the interface. I would try to remake the mesh, slightly finer and also to add some outer corrections instead of running in piso mode.

I dont know if that is sufficient, but its impossible to get it working with that mesh.

sharonyue December 18, 2012 04:37

Quote:

Originally Posted by niklas (Post 398013)
the main problem is the mesh-quality at the interface. I would try to remake the mesh, slightly finer and also to add some outer corrections instead of running in piso mode.

I dont know if that is sufficient, but its impossible to get it working with that mesh.

Thank you very very much. although this problem has not been handled.I would be very thankful for your assistance.

um...maybe twophaseeulerfoam in next edition of OpenFOAM would be better on dealing with this mesh problem.? But I dont have much time to wait.....

niklas December 18, 2012 04:49

add this to controlDict and watch what happens to the velocities

Code:

functions
{
    extraInfo
    {
        type              coded;
        functionObjectLibs ( "libutilityFunctionObjects.so" );
        redirectType      average;
        code
              #{
            const volVectorField& U1 = mesh().lookupObject<volVectorField>("U1");
            const volVectorField& U2 = mesh().lookupObject<volVectorField>("U2");
            Info << "max U1 = " << max(mag(U1)).value() << ", U2 = " << max(mag(U2)).value() << endl;
            const volScalarField& p = mesh().lookupObject<volScalarField>("p");
            Info << "p min/max = " << min(p).value() << ", " << max(p).value() << endl;
        #};
    }
}


sharonyue December 24, 2012 23:42

Dear Niklas,
yeah, thats help, somthing wired about velocity fields. but finally,I dont know how to run bubblefoam or twophaseeulerfoam on that mesh. is this regarding to the model itself? if its ture. that is far beyond my ability.

alberto December 26, 2012 10:12

2 Attachment(s)
Use the "upwind" scheme for the divergence term of U1 and U2, and use the "uncorrected" option for Laplacians and snGrad. Also, fix the maximum time step to a much lower value than 1s, to avoid too strong fluctuations in the time-step.

I attach the files I used, and it ran up to 0.18s, then I stopped.

P.S. There is no reason to use an unstructured mesh with such a simple geometry :-)

sharonyue December 26, 2012 10:16

Quote:

Originally Posted by alberto (Post 399089)
Use the "upwind" scheme for the divergence term of U1 and U2, and use the "uncorrected" option for Laplacians and snGrad. Also, fix the maximum time step to a much lower value than 1s, to avoid too strong fluctuations in the time-step.

I attach the files I used, and it ran up to 0.18s, then I stopped.

P.S. There is no reason to use an unstructured mesh with such a simple geometry :-)

Oh my GOD! Thank you so very much Prof. alberto. I have been waiting for your reply. coz I know you can handle this question. I will try this . and update this thread if its necessary.

sharonyue December 26, 2012 11:34

1 Attachment(s)
Quote:

Originally Posted by alberto (Post 399089)
Use the "upwind" scheme for the divergence term of U1 and U2, and use the "uncorrected" option for Laplacians and snGrad. Also, fix the maximum time step to a much lower value than 1s, to avoid too strong fluctuations in the time-step.

I attach the files I used, and it ran up to 0.18s, then I stopped.

P.S. There is no reason to use an unstructured mesh with such a simple geometry :-)

Well~Prof.Alberto, I have tried, but the result looks...unsatisfactory.the image has been attached.If you have time,could you do me a favor check this thing out again please? Thank you.
BTW,I really admire what you have done in CFD research.

alberto December 26, 2012 11:45

You should improve your mesh resolution if you want to obtain reliable results.

P.S. Alberto works just fine, no need of titles ;-)

sharonyue December 26, 2012 11:48

Quote:

Originally Posted by alberto (Post 399100)
You should improve your mesh resolution if you want to obtain reliable results.

P.S. Alberto works just fine, no need of titles ;-)

Okay! I will remesh and try it, and update the result! Thanks alberto~

alberto December 26, 2012 11:50

May I know why you are trying to use a tetrahedral mesh?


All times are GMT -4. The time now is 21:39.