
[Sponsors] 
March 1, 2012, 11:29 
bubbleFoam is loosing fluid

#1 
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Dear Foamers,
in the last weeks I tried to successfully use bubbleFoam to simulation multiphase flow inside a steamdrum. After finally getting the simulation more or less stable  the timeStep and maxCo are still very low  yet another problem occurs. I am loosing water. There is one inlet where a steam water mixture is put in. After some time that is 0.05 s in the attached picture it seems like only steam was put in and not a mixture... And I have no idea what BC or scheme or whatever arouses this problem. It seems that steam only pushes away the water level that was initialised with setFields. No separation takes place. The used fvSchemes and fvSolution entries are as follows: fvSchemes Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phia,Ua) Gauss upwind; div(phib,Ub) Gauss upwind; div(phib,k) Gauss upwind; div(phib,epsilon) Gauss upwind; div(phi,alpha) Gauss upwind; div((nuEffa*T(grad(Ua)))) Gauss linear; div((nuEffb*T(grad(Ub)))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } Code:
solvers { p { solver GAMG; tolerance 1e04; relTol 0.1; smoother DIC; nPreSweeps 0; nPostSweeps 2; nFinestSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } pFinal { $p; tolerance 1e04; relTol 0; } "(kepsilon)" { solver PBiCG; preconditioner DILU; tolerance 1e4; relTol 0.0; } "(kepsilon)Final" { solver PBiCG; preconditioner DILU; tolerance 1e4; relTol 0.0; } alpha { solver PBiCG; preconditioner DILU; tolerance 1e5; relTol 0.1; } alphaFinal { solver PBiCG; preconditioner DILU; tolerance 1e5; relTol 0; } } nCorrectors 1; //1 nNonOrthogonalCorrectors 1; nAlphaCorr 1; correctAlpha yes; The problem occurs 2D as well as 3D, laminar and turbulent... The picture that is attached, illustrates the "loosing of the fluid"... (right side / patch) Any idea or help would be very appreciated. Thanks. 

March 2, 2012, 03:50 

#2 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
It would be useful to see a small case that reproduces the problem. Also, what version of OpenFOAM are you using?
Your linear solver tolerances are way too high however. A tolerance of 1.0e8 over p, 10^10 over alpha, and 10^5 for the other variables is what I usually adopt. Also, if your grid is not skewed, set the nonOrthogonalCorrectors to 0, and perform 2 alpha correctors, and 2 nCorrectors. I would say that using upwind should not be necessary, but this depend on the mesh quality :)
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

March 2, 2012, 07:05 

#3 
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Well, if you would send me your email address via this forum I can send you the case. Other users are welcome, too.
Since the grid is generated with ICEM (the snappy grid is not too good) the case directory is about 20 MB. I am using OpenFoam 2.0.1. I used the higher tolerances in order to decrease the computational time. The aim of this 2D case was actually to reproduce a first "quick and dirty" solution to see what problems might occur that could have major influence on the 3D case. With lower tolerances the stability is even worse. And I found out that the picture I attached is the initialisation with setFields. So basically I am not loosing water. It is just that nothing really happens, although I have 4/6 m/s of water/steam that goes in. So after a time of 0.05 seconds (which already took a lot of time on an i7  8GB RAM ... system) multiplied by a speed of 4 or 6 m/s would tend to result in the water moving around 0.2 m and steam around 0.3 m. But as can be seen in the picture neither the first one nor the second one happens. I then realized that the characteristic length is a bit smaller. Thus, epsilon is a lot higher. Now, with the new initialisation the simulation crashes even faster... 

March 2, 2012, 12:43 

#4  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Quote:
Quote:
However, you said you are using meshes generated in ICEM. I recently had a similar problem with a 2D mesh in ICEM, but I did not investigate it too much, and I used another mesh/mesher. To try to understand if it's a mesh conversion problem, is it possible to use another mesh? Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

March 5, 2012, 06:01 

#5 
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Dear alberto,
by using another mesh that is a snappy grid in this case, the solver crashes earlier. So I rather used the finer grid (ICEM) "without" any errors. The mesh is very fine (160k cells) in order to lock out an error due to the mesh. I also setup a small 3D case that only has 100k cells instead of 400k (the "normal" 3D case) to test around... Actually, something happens. But the inlet patches are not meshed appropriate since some cells look "bad". So I might test around with snappy some more time... But I think something is wrong in the setup. Usually, I get problems with "k" rather than anything else. Hopefully, you will find what's wrong... Because compared to interFoam the computational time is like x1000 right now...I tried to act in accordance to the bubbleFoam description inside the OpenFOAM wiki. But it was only partly helpful. I sent you the case along with a few notes a few minutes ago. Thank you very much for your help. 

March 5, 2012, 12:38 

#6  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
Quote:
Two considerations: you are dealing with a system involving phase separation. The implemented kepsilon model is not well defined in such a situation. I have a version of twoPhaseEulerFoam with a turbulence model based on the mixture assumption which I can share if you want. To check if the rest of the setup is OK, switch off the turbulence model. Second consideration: If you are interested in resolving interfaces, you might want to consider multiphaseEulerFoam, which is a multifluid solver, with the capability of reconstructing interfaces too. The algorithm it implements seems to be more robust. The turbulence model is LESbased however (Smagorinsky + vanDriest damping). Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

March 5, 2012, 12:48 

#7  
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Quote:
Quote:
Quote:
Thanks a lot for the information. 

March 5, 2012, 13:25 

#8 
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Well, alberto.
Even when I change the boundaries from "wall" to "patch" nothing really happens at the in or outlets. Could you check my BC's once again? Right now, something happens inside the drum. But the in and out flows are not considered... 

March 6, 2012, 12:22 

#9 
Member
Rob
Join Date: Sep 2011
Posts: 55
Rep Power: 8 
Dear alberto,
finally the case works at least laminar... I therefore set up a small 3D case that has a smaller mesh then the 2D mesh I sent you via email... My problem with the turbulence is the turbulent kinetic energy k... Therefore, I can only use time steps around 1e07 / 1e06... Thus, even the simulation of the small 3D test case would take until 2013... That leads me to two questions... What turbulence model  the one you'd like to share  have you implemented into bubbleFoam? How should I set up k and epsilon to have a stable simulation? The OpenFOAM wiki tells me to set up k and epsilon for the continous phase... But with these values and initialisation I wouldn't get far to a result... Thanks for your help. Best, Rob 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
interFoam VOF is loosing fluid  wersoe  OpenFOAM Running, Solving & CFD  12  June 26, 2013 08:13 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
How to choose the mean diameter value for dispersed fluid?  creddy_trddc  CFX  1  October 30, 2011 05:30 
bubbleFoam solver for nonNewtonian fluid  Benjy  OpenFOAM  0  November 29, 2010 20:25 
Terrible Mistake In Fluid Dynamics History  Abhi  Main CFD Forum  12  July 8, 2002 09:11 