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

bubblefoam totally failed on unstructured mesh.

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 6, 2012, 02:34
Smile bubblefoam totally failed on unstructured mesh.
  #1
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
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.
sharonyue is offline   Reply With Quote

Old   December 6, 2012, 04:14
Default
  #2
Member
 
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 6
michielm is on a distinguished road
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.
michielm is offline   Reply With Quote

Old   December 6, 2012, 04:28
Default
  #3
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
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.




MRFzone problem in ICEM,
in this thread I tried use structured mesh on bubblefoam but failed, so I have to use unstructured mesh.then....

same geometry,structured and unstructured mesh,different behaviour.
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.
Attached Images
File Type: png ff.png (34.9 KB, 77 views)
Attached Files
File Type: zip unstructuredmeshbubblefoam.zip (15.7 KB, 17 views)
sharonyue is offline   Reply With Quote

Old   December 10, 2012, 02:29
Default
  #4
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Thats quite weird, is there anyone tried an unstructured mesh on bubblefoam?
sharonyue is offline   Reply With Quote

Old   December 14, 2012, 07:32
Default
  #5
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
nobody is here?...
sharonyue is offline   Reply With Quote

Old   December 14, 2012, 08:34
Default
  #6
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
get a dropbox account and put the mesh there.

why do you have different inlet velocities for the phases?
niklas is offline   Reply With Quote

Old   December 14, 2012, 09:25
Default
  #7
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by niklas View Post
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.
sharonyue is offline   Reply With Quote

Old   December 14, 2012, 10:49
Default
  #8
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
doesnt work. hotfile is terrible.
cant download and now it says im downloading and I can only download 1 at a time.
niklas is offline   Reply With Quote

Old   December 15, 2012, 00:08
Smile
  #9
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by niklas View Post
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 is offline   Reply With Quote

Old   December 18, 2012, 01:52
Default
  #10
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Looks like only FOAM developers can tackle this problem?...
sharonyue is offline   Reply With Quote

Old   December 18, 2012, 02:41
Default
  #11
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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.
niklas is offline   Reply With Quote

Old   December 18, 2012, 04:37
Default
  #12
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by niklas View Post
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.....
sharonyue is offline   Reply With Quote

Old   December 18, 2012, 04:49
Default
  #13
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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 likes this.
niklas is offline   Reply With Quote

Old   December 24, 2012, 23:42
Default
  #14
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
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.
sharonyue is offline   Reply With Quote

Old   December 26, 2012, 10:12
Default
  #15
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
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 :-)
Attached Files
File Type: txt controlDict.txt (1.3 KB, 39 views)
File Type: txt fvSchemes.txt (1.9 KB, 51 views)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 26, 2012, 10:16
Default
  #16
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post
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 is offline   Reply With Quote

Old   December 26, 2012, 11:34
Default
  #17
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post
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.
Attached Images
File Type: jpg 2.jpg (33.5 KB, 49 views)
sharonyue is offline   Reply With Quote

Old   December 26, 2012, 11:45
Default
  #18
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
You should improve your mesh resolution if you want to obtain reliable results.

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

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 26, 2012, 11:48
Default
  #19
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 676
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post
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~
sharonyue is offline   Reply With Quote

Old   December 26, 2012, 11:50
Default
  #20
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
May I know why you are trying to use a tetrahedral mesh?
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
Mesh motion with Translation & Rotation Doginal CFX 2 January 12, 2014 07:21
Unstructured Mesh ICEM on a cube jerome_ ANSYS 0 May 30, 2012 05:34
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11


All times are GMT -4. The time now is 14:04.