CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

parasitic currents

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

Like Tree22Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 11, 2012, 08:49
Default
  #81
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Attached Images
File Type: jpg liquidDrop_alpha.jpg (13.9 KB, 50 views)
File Type: jpg liquidDrop_U.jpg (16.3 KB, 47 views)
File Type: jpg gasDrop_alpha.jpg (10.7 KB, 44 views)
File Type: jpg gasDrop_U.jpg (12.4 KB, 36 views)
Andrea_85 is offline   Reply With Quote

Old   May 11, 2012, 11:21
Default
  #82
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
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
jens_klostermann is offline   Reply With Quote

Old   May 11, 2012, 11:24
Default
  #83
Member
 
Robert Castilla
Join Date: Apr 2009
Location: Spain
Posts: 80
Rep Power: 8
rcastilla is on a distinguished road
Quote:
Originally Posted by akidess View Post
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
rcastilla is offline   Reply With Quote

Old   May 11, 2012, 11:43
Default
  #84
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Andrea_85 is offline   Reply With Quote

Old   May 11, 2012, 12:14
Default
  #85
Senior Member
 
Jens Klostermann
Join Date: Mar 2009
Posts: 117
Rep Power: 8
jens_klostermann is on a distinguished road
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
jens_klostermann is offline   Reply With Quote

Old   May 13, 2012, 16:19
Default
  #86
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
Attached Images
File Type: png maxu.png (5.0 KB, 50 views)
File Type: jpg liquid_drop_alpha1_fc.jpg (16.6 KB, 62 views)
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 13, 2012, 20:40
Default
  #87
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   May 14, 2012, 03:14
Default
  #88
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Andrea_85 is offline   Reply With Quote

Old   May 14, 2012, 04:41
Default
  #89
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
Andrea, here is the setup I used. Did you remember to change setFieldsDict?
Attached Files
File Type: gz liquid_droplet.tar.gz (4.2 KB, 17 views)
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 14, 2012, 05:06
Default
  #90
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 14, 2012, 08:45
Default
  #91
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Attached Images
File Type: jpg maxU_liquidDrop.jpg (13.9 KB, 50 views)
Andrea_85 is offline   Reply With Quote

Old   May 14, 2012, 09:00
Default
  #92
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 21, 2012, 10:40
Default
  #93
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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)?
Attached Images
File Type: jpg ssf_fig6a.jpg (20.7 KB, 44 views)
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 21, 2012, 10:47
Default
  #94
Senior Member
 
Join Date: Nov 2010
Posts: 113
Rep Power: 6
lindstroem is on a distinguished road
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?
lindstroem is offline   Reply With Quote

Old   May 21, 2012, 10:56
Default
  #95
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
i think you are right, just use snappy without "snap" option. It should do the job.

andrea
Andrea_85 is offline   Reply With Quote

Old   May 22, 2012, 10:20
Default
  #96
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Attached Images
File Type: jpg cylinder.jpg (56.0 KB, 54 views)
Andrea_85 is offline   Reply With Quote

Old   May 22, 2012, 10:46
Default
  #97
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 22, 2012, 10:58
Default
  #98
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Attached Files
File Type: txt snappyHexMeshDict.txt (10.2 KB, 8 views)
Andrea_85 is offline   Reply With Quote

Old   May 22, 2012, 11:17
Default
  #99
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   May 23, 2012, 04:49
Default
  #100
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 275
Rep Power: 7
Andrea_85 is on a distinguished road
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
Andrea_85 is offline   Reply With Quote

Reply

Tags
capillary flows, interfoam, parasitic currents

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 monitor free surface elevation vs time in OF? ozgur OpenFOAM Post-Processing 55 October 31, 2013 10:33
parasitic currents Pei-Ying 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


All times are GMT -4. The time now is 21:52.