[Andrea_85]

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

[jens_klostermann]

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

[rcastilla]

Originally Posted by akidess

Andrea, I pushed the testcase to the repository.

Robert, I didn't quite understand which one you think works better now - implicit or explicit?

The negative boundness behaves much better with explicit with my case (liquid-gas). But I am not sure what overall behaviour is better

Robert

[Andrea_85]

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

[jens_klostermann]

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

[akidess]

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.

[phsieh2005]

Hi, Anton,

I retrieved the latest interfoamssf code. Made a couple of changes needed for OpenFOAM-2.1.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!

Pei-Ying
---------------------------/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / 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.x-f1044c880abb
Exec : interFoamSSF
Date : May 13 2012
Time : 20:36:25
Host : "jali"
PID : 6613
Case : /home/hsieh/OpenFOAM/hsieh-2.1.x/solvers/interfoamssf/testCases/staticDroplet
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied 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 = 5e-07

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 = 6.73003e-08, No Iterations 9
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 8.94836e-10, No Iterations 6
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 8.94835e-10, No Iterations 6
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 8.94833e-10, No Iterations 6
GAMG: Solving for p, Initial residual = 1, Final residual = 7.10299e-08, No Iterations 13
time step continuity errors : sum local = 1.23283e-08, global = 2.02179e-20, cumulative = 2.02179e-20
GAMG: Solving for p, Initial residual = 0.103026, Final residual = 7.62369e-08, No Iterations 11
time step continuity errors : sum local = 2.34517e-08, global = 1.13891e-20, cumulative = 3.1607e-20
GAMG: Solving for p, Initial residual = 0.00322057, Final residual = 3.33724e-08, No Iterations 8
time step continuity errors : sum local = 8.882e-09, global = -3.97863e-21, cumulative = 2.76284e-20
PIMPLE: iteration 3
Subcycle 2
DILUPBiCG: Solving for alpha1, Initial residual = 0.00219012, Final residual = 9.7882e-16, No Iterations 3
Liquid phase volume fraction = 0.936 Min(alpha1) = 3.35461e-26 Max(alpha1) = 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/hsieh/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/hsieh/OpenFOAM/OpenFOAM-2.1.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/OpenFOAM-2.1.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#4
at interfaceProperties.C:0
#5
in "/home/hsieh/OpenFOAM/hsieh-2.1.x/platforms/linux64Gcc46DPOpt/bin/interFoamSSF"
#6
in "/home/hsieh/OpenFOAM/hsieh-2.1.x/platforms/linux64Gcc46DPOpt/bin/interFoamSSF"
#7 __libc_start_main in "/lib64/libc.so.6"
#8
at /home/abuild/rpmbuild/BUILD/glibc-2.14.1/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

[Andrea_85]

Hi Anton,
did you just double the domain (200e-6x200e-6x200e-6 and 40x40x40 cells) to get those results? because i got again bad results from my tests. Did you change anything else?

andrea

[akidess]

Andrea, here is the setup I used. Did you remember to change setFieldsDict?

[akidess]

Pei-Ying, the repository version still uses alpha1_ to calculate 'w' in interfaceProperties.C. If unboundedness is larger than 1e-6, 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 time-step (e.g. 1e-7), and then when convergence sets in you can restart with a larger time step.

- Anton

[Andrea_85]

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

[akidess]

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.

[akidess]

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)?

[lindstroem]

I think snappy produces this mesh easily. If you provide and stl-file 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?

[Andrea_85]

i think you are right, just use snappy without "snap" option. It should do the job.

andrea

[Andrea_85]

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 8-9)?

best

andrea

[akidess]

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

[Andrea_85]

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 e-mail i can send you (constant and system dir + stl).


best

andrea

[akidess]

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

[Andrea_85]

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