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 Tree34Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   May 23, 2012, 05:13
Default
  #101
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Would there be a difference for laminar flow? All we need in the boundary condition is the face normal, which is available for a basic patch. I think the wall-BC is only needed for the turbulence models.
__________________
*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
akidess is offline   Reply With Quote

Old   May 23, 2012, 05:39
Default
  #102
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
i do not understand what you mean, poiseuille flow is something expected even for laminar flow for ex.
i said that i would choose

fixedValue uniform(0 0 0) for the lateral area of the cylinder

and

fixedValue uniform(0 0 0.001) for inlet and outlet.

These are in my opinion the correct (physical) boundary condition for a liquid that moves in a capillary tube. Now the paper is talking about uniform velocity field, so using these BC you will have parabolic profile, at least far from the droplet (not uniform). I do not understand the need of capillary tube, would be more clear for me if the drop moves simply in another liquid with fixed velocity everywhere.

btw the BC you choose are:

zeroGaradient for pressure everywhere
fixedValue for U (0 0 0.001) everywhere

right?

andrea
Andrea_85 is offline   Reply With Quote

Old   May 23, 2012, 07:39
Default
  #103
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Sorry, I totally misunderstood your initial question! You are right that for a real capillary tube, there should be a no-slip on the walls and we'd have a parabolic flow profile if the flow is assumed developed. However, that would introduce shear on the droplet, and they don't want that in this test case. So in the end it is just a droplet with no relative motion to a flowing surrounding liquid. Why they went to the trouble making a cylindric domain instead of a plain box might just be to cut away some cells in the domain which are unnecessary to maintain a minimum distance to the walls.

- 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
akidess is offline   Reply With Quote

Old   May 24, 2012, 05:35
Default
  #104
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
Hi,
my simulation is really bad. the drop starts to move along the z-axis but then, after a while, it diffuses away and the maximum value of alpha goes to 0.6/0.5. How are your results?

andrea
Andrea_85 is offline   Reply With Quote

Old   May 24, 2012, 07:58
Default
  #105
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Andrea, unfortunately I don't have results yet. I'm busy with other things so I don't have much time to play with interFoamSSF these days. I'll report back once I have something. Good luck!
__________________
*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
akidess is offline   Reply With Quote

Old   May 30, 2012, 08:02
Default
  #106
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
I pushed updates to enable the use of adjustable time stepping.
__________________
*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
akidess is offline   Reply With Quote

Old   May 31, 2012, 07:41
Default
  #107
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
I now have results on the moving droplet case with the SSF and CSF formulations - see attachment. As expected, they are both not great.
Attached Images
File Type: jpg movingDropComparison.jpg (31.0 KB, 76 views)
__________________
*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
akidess is offline   Reply With Quote

Old   May 31, 2012, 07:53
Default
  #108
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
Hi Anton,
can you upload the test case with boundary and initial conditions on the repository. just to be sure we are using the same.

thanks

andrea
Andrea_85 is offline   Reply With Quote

Old   May 31, 2012, 08:21
Default
  #109
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Ok, I uploaded the case. What I did was initialize the droplet shape starting from a square droplet of same volume, and then (after 0.0005s) turn on the background velocity field and start doing the real simulation.
__________________
*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
akidess is offline   Reply With Quote

Old   June 1, 2012, 04:13
Default
  #110
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
I noticed something about the Crank-Nicholson scheme - the programmers guide on page 43 states you have to implement a mixing of fvm and fvc terms manually! Is that really up to date, i.e. is it really not enough to modify fvSchemes?
__________________
*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
akidess is offline   Reply With Quote

Old   June 2, 2012, 09:50
Default reducing paracurr on unstructured grids
  #111
New Member
 
Jake
Join Date: May 2012
Posts: 1
Rep Power: 0
nudelsalat is on a distinguished road
Hi guys,

first off its been really interesting to follow your conversation and to see your progress.
I've just started off working on reducing parasitic currents and i was wondering if you have any results or approaches/ideas to reduce these on unstructured grids.

Thx

Jakob
nudelsalat is offline   Reply With Quote

Old   June 3, 2012, 12:18
Default
  #112
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
@Anton
good question. i've never used crank nicholson scheme for my simulations and so i really do not known. My first guess is that it is enough to modify fvScheme but i am not sure.

@Jakob
Did you try the drop relaxation on unstructured grid? it would be a good starting point.

best
Andrea_85 is offline   Reply With Quote

Old   June 4, 2012, 05:08
Default
  #113
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
I tried to add changes to use adjustable time step but i got some errors about pimple control. I copied pimpleControl.H/C/I.H from openFoam 2.0.1 in interFoamSSF's folders. This is the error

interFoam.C:215: error: ‘class Foam:impleControl’ has no member named ‘nCorrPISO’
In file included from interFoam.C:217:
pEqn.H:54: error: no matching function for call to ‘Foam:impleControl::finalInnerIter()’
pimpleControlI.H:100: note: candidates are: bool Foam:impleControl::finalInnerIter(Foam::label, Foam::label) const
interFoam.C:100: warning: unused variable ‘cycle’
/home/aferrari/OpenFOAM/OpenFOAM-2.1.0/src/finiteVolume/lnInclude/readTimeControls.H:38: warning: unused variable ‘maxDeltaT’
make: *** [Make/linux64GccDPOpt/interFoam.o] Error 1


i think nCorrPISO has to be changed with nOuterCorr, right?
but i don't know what to do with the other error.
any suggests?

best

andrea
Andrea_85 is offline   Reply With Quote

Old   June 4, 2012, 05:23
Default
  #114
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
ok i solved it. (nCorrPiso is nCorr and in pEqn:h i changed pEqn.solve to match your version). would be great to have the full version compiled with OF 2.1.0.

best
Andrea_85 is offline   Reply With Quote

Old   June 4, 2012, 06:01
Default
  #115
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Quote:
Originally Posted by Andrea_85 View Post
Would be great to have the full version compiled with OF 2.1.0.
I'm going to stick with 2.0.x for now because I have more custom solvers that I'd have to port. However, you can make your life easier by having mercurial do some of the changes for you:
Code:
* Start with Roberto's version for OpenFoam 2.1 (http://code.google.com/r/robertocastillalopez-interfoamssf-210)
* hg pull from my repository (http://code.google.com/p/interfoamssf) in the interfoamssf-210 folder to get my updates
* Run 'hg merge' to combine the two versions into one
* Run 'hg commit' to store the merge changes for the future
Andrea, you have manually already made the changes, so you can skip ahead to the commit step. You can keep on pulling from my repository to get the updates, but after the commit mercurial will remember the changes you made for compatibility to version 2.1.x and leave them untouched.

Good guides on using mercurial are http://hgbook.red-bean.com/read/ or http://hginit.com.
__________________
*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
akidess is offline   Reply With Quote

Old   June 4, 2012, 06:17
Default
  #116
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
Quote:
Originally Posted by nudelsalat View Post
Hi guys,
first off its been really interesting to follow your conversation and to see your progress.
I've just started off working on reducing parasitic currents and i was wondering if you have any results or approaches/ideas to reduce these on unstructured grids.

Thx

Jakob
Jakob, it's been great to share the development experiences and discuss with everyone as well. Feel free to check out this solver and see if it suits your needs, and share your experiences here no matter if good or bad! There's one or two other good threads as well on the forum for working with the standard interfoam solver that I'm sure you've already came across.

Cheers,

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
akidess is offline   Reply With Quote

Old   June 6, 2012, 06:43
Default
  #117
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
Hi Anton,

my simulation is still bad, it is loosing mass. The maximum value of alpha1 drops down to 0.5 after few time steps. Any idea of why?. Do you see the same?

best
andrea
Andrea_85 is offline   Reply With Quote

Old   June 7, 2012, 07:35
Default
  #118
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
In my case the droplet retains it's shape and position until 0.005s (100 time steps), after which it moves off-center and starts diffusing away completely (at this point the volume fraction field isn't conserved any more).
__________________
*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
akidess is offline   Reply With Quote

Old   June 7, 2012, 07:55
Default
  #119
Senior Member
 
Andrea Ferrari
Join Date: Dec 2010
Posts: 296
Rep Power: 8
Andrea_85 is on a distinguished road
i observed exactly the same behavior. I hope this is due to lack of the filtering step. i'll start to think about the implementation as soon i'll have time.

best

andrea
Andrea_85 is offline   Reply With Quote

Old   June 11, 2012, 08:37
Default
  #120
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,121
Rep Power: 20
akidess will become famous soon enough
I started working on the filtering, and I stumbled across an issue with it's formulation. Have a look at the attached image - let's say it's an interface with a slight curvature. 'deltasf' is computed at the faces and will be large in normal to the interface (y) and small in tangential direction (x). Keeping that in mind for equation (22) of the paper, that means we would start filtering in y-direction instead of x. Right?

Further issues: The value of epsilon is undefined, and it is unclear when to apply eq (23)...
Attached Images
File Type: jpg surface_force_filter.jpg (26.9 KB, 37 views)
__________________
*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
akidess 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 56 September 14, 2015 08:11
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 03:44.