[sharonyue]

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]

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]

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]

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

[sharonyue]

nobody is here?...

[niklas]

get a dropbox account and put the mesh there.

why do you have different inlet velocities for the phases?

[sharonyue]

Originally Posted by niklas

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]

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

[sharonyue]

Originally Posted by niklas

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]

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

[niklas]

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]

Originally Posted by niklas

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]

add this to controlDict and watch what happens to the velocities

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]

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]

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]

Originally Posted by alberto

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]

Originally Posted by alberto

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]

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

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

[sharonyue]

Originally Posted by alberto

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]

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