
[Sponsors] 
May 11, 2012, 08:49 

#81 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Have a look at the pictures i attached. maybe it might be a boundary effect in case of liquid droplet (first two pictures). i would try to make a bigger surrounding domain to see if performs better.
andrea 

May 11, 2012, 11:21 

#82 
Senior Member
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 9 
Keep in mind that the parasitic currents are more pronounced in the fluid with the lower dynamic viscosity (gas phase). Thus damping the parasitic currents less
Jens 

May 11, 2012, 11:24 

#83  
Member
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 92
Rep Power: 9 
Quote:
Robert 

May 11, 2012, 11:43 

#84 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
hi jens,
thanks to join the discussion. this might explain picture 2 in which is clearly visible that spurious currents are higher in the gas phase but shouldn't we get something similar, but reversed, in the other case? best andrea 

May 11, 2012, 12:14 

#85 
Senior Member
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 9 
Hi Andrea,
It is fun reading your thread and seeing how you progress! In the case 2 (bubble case) the parasitic current are only visible in the bubble (gas drop) and can "cancel out" each other since they are compact in a bubble. In the case 1 (drop case) it is harder for the parsitic currents to "cancel each other" since there are seperated by the liquid drop. Jens 

May 13, 2012, 16:19 

#86 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
Andrea, you were right about the domain size  use a larger domain, and the convergence problems go away The smearing along the mesh direction is somewhat weird, but doesn't seem to be reflected in the force field.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 13, 2012, 20:40 

#87 
Senior Member
PeiYing Hsieh
Join Date: Mar 2009
Posts: 313
Rep Power: 10 
Hi, Anton,
I retrieved the latest interfoamssf code. Made a couple of changes needed for OpenFOAM2.1.x so that interFoamSSF compiled successfully. However, when I ran the staticDroplet test case, the case diverged. I am wondering if I need to make changes for it to run? Thanks! PeiYing /**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.1.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 2.1.xf1044c880abb Exec : interFoamSSF Date : May 13 2012 Time : 20:36:25 Host : "jali" PID : 6613 Case : /home/hsieh/OpenFOAM/hsieh2.1.x/solvers/interfoamssf/testCases/staticDroplet nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 PIMPLE: no residual control data found. Calculations will employ 4 corrector loops Reading field p Reading field alpha1 Reading field U Reading/calculating face flux field phi Reading transportProperties Selecting incompressible transport model Newtonian Selecting incompressible transport model Newtonian Reading g Calculating field g.h time step continuity errors : sum local = 0, global = 0, cumulative = 0 DICPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0, global = 0, cumulative = 0 Courant Number mean: 0 max: 0 Starting time loop Courant Number mean: 0 max: 0 Interface Courant Number mean: 0 max: 0 Time = 5e07 PIMPLE: iteration 1 Subcycle 1 DILUPBiCG: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0 Liquid phase volume fraction = 0.936 Min(alpha1) = 0 Max(alpha1) = 1 PIMPLE: iteration 2 Subcycle 2 DILUPBiCG: Solving for alpha1, Initial residual = 0, Final residual = 0, No Iterations 0 Liquid phase volume fraction = 0.936 Min(alpha1) = 0 Max(alpha1) = 1 GAMG: Solving for pc, Initial residual = 1, Final residual = 6.73003e08, No Iterations 9 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 8.94836e10, No Iterations 6 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 8.94835e10, No Iterations 6 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 8.94833e10, No Iterations 6 GAMG: Solving for p, Initial residual = 1, Final residual = 7.10299e08, No Iterations 13 time step continuity errors : sum local = 1.23283e08, global = 2.02179e20, cumulative = 2.02179e20 GAMG: Solving for p, Initial residual = 0.103026, Final residual = 7.62369e08, No Iterations 11 time step continuity errors : sum local = 2.34517e08, global = 1.13891e20, cumulative = 3.1607e20 GAMG: Solving for p, Initial residual = 0.00322057, Final residual = 3.33724e08, No Iterations 8 time step continuity errors : sum local = 8.882e09, global = 3.97863e21, cumulative = 2.76284e20 PIMPLE: iteration 3 Subcycle 2 DILUPBiCG: Solving for alpha1, Initial residual = 0.00219012, Final residual = 9.7882e16, No Iterations 3 Liquid phase volume fraction = 0.936 Min(alpha1) = 3.35461e26 Max(alpha1) = 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/home/hsieh/OpenFOAM/OpenFOAM2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/hsieh/OpenFOAM/OpenFOAM2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so" #2 in "/lib64/libc.so.6" #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) in "/home/hsieh/OpenFOAM/OpenFOAM2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so" #4 at interfaceProperties.C:0 #5 in "/home/hsieh/OpenFOAM/hsieh2.1.x/platforms/linux64Gcc46DPOpt/bin/interFoamSSF" #6 in "/home/hsieh/OpenFOAM/hsieh2.1.x/platforms/linux64Gcc46DPOpt/bin/interFoamSSF" #7 __libc_start_main in "/lib64/libc.so.6" #8 at /home/abuild/rpmbuild/BUILD/glibc2.14.1/csu/../sysdeps/x86_64/elf/start.S:116 Floating point exception 

May 14, 2012, 03:14 

#88 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
Hi Anton,
did you just double the domain (200e6x200e6x200e6 and 40x40x40 cells) to get those results? because i got again bad results from my tests. Did you change anything else? andrea 

May 14, 2012, 04:41 

#89 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
Andrea, here is the setup I used. Did you remember to change setFieldsDict?
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 14, 2012, 05:06 

#90 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
PeiYing, the repository version still uses alpha1_ to calculate 'w' in interfaceProperties.C. If unboundedness is larger than 1e6, then that can lead to problems. If you change line 131 to use alpha1c_, all should be well.
Alternatively, initialize the simulation with a smaller timestep (e.g. 1e7), and then when convergence sets in you can restart with a larger time step.  Anton
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 14, 2012, 08:45 

#91 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
After some attempts I realized why I had different results. The issue seems to lie in the smoothing of the gradient, so i decided to comment it out for the moment. I think more tests in this direction are needed before push it in the repository.
Without the smoothing of gradAlpha i got really nice results (see attached picture). andrea 

May 14, 2012, 09:00 

#92 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
Indeed already after seeing your first results with smoothing I've been thinking about the smoothing and the inclusion of an on/off switch. It would be interesting to see how the performance is on dynamic problems.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 21, 2012, 10:40 

#93 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
I started thinking about the moving droplet test case. Does any one have suggestions how to best build the mesh in fig 6a (see attachment)?
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 21, 2012, 10:47 

#94 
Senior Member
Join Date: Nov 2010
Posts: 113
Rep Power: 7 
I think snappy produces this mesh easily. If you provide and stlfile with the outer cylinder, the first step of snappy would be to delete the cells cutting the boundary and produce that mesh  or am I wrong?


May 21, 2012, 10:56 

#95 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
i think you are right, just use snappy without "snap" option. It should do the job.
andrea 

May 22, 2012, 10:20 

#96 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
This is what i have obtained with snappyHexMesh. The mesh seems the same as in the paper. Did you already think about how to implement filter of capillary forces and capillary fluxes (pag 89)?
best andrea 

May 22, 2012, 10:46 

#97 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
Looks better than what I got with Gambit Which software did you use to generate the STL file? And can you upload your snappyHexDict?
I thought I'd try the test case without filtering, see what comes out and then add it.  Anton
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 22, 2012, 10:58 

#98 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
i used gmsh, http://www.geuz.org/gmsh/,it is a really easy software if you need simple geometry. The case is too big to be uploaded here. If you give me your email i can send you (constant and system dir + stl).
best andrea 

May 22, 2012, 11:17 

#99 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,139
Rep Power: 20 
I actually already had an STL file generated with Salome (also trivial), I was just curious about what else can be used. Together with your dict file I also have a mesh now I did however turn off the snap feature  I think it's unnecessary here.
 Anton
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

May 23, 2012, 04:49 

#100 
Senior Member
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8 
What boundary conditions did you choose? They write fixed velocity and zeroGradient for pressure everywhere, but on the jagged cylinder the correct condition should be wall BC, or not?
andrea 

Tags 
capillary flows, interfoam, parasitic currents 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
how to monitor free surface elevation vs time in OF?  ozgur  OpenFOAM PostProcessing  56  September 14, 2015 08:11 
parasitic currents  PeiYing Hsieh  Main CFD Forum  0  January 13, 2009 20:58 
Parasitic currents reduction  hsieh  OpenFOAM Running, Solving & CFD  0  January 13, 2009 16:44 
Parasitic currents reduction  hsieh  OpenFOAM Running, Solving & CFD  0  January 13, 2009 16:37 
Modelling ocean currents of the past Earth  pgm  Main CFD Forum  3  March 2, 2005 09:45 