[akidess]

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.

[Andrea_85]

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

[akidess]

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

[Andrea_85]

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

[akidess]

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!

[akidess]

I pushed updates to enable the use of adjustable time stepping.

[akidess]

I now have results on the moving droplet case with the SSF and CSF formulations - see attachment. As expected, they are both not great.

[Andrea_85]

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

[akidess]

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.

[akidess]

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?

[nudelsalat]

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

[Andrea_85]

@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]

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]

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

[akidess]

Originally Posted by Andrea_85

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:

* 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.

[akidess]

Originally Posted by nudelsalat

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

[Andrea_85]

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

[akidess]

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).

[Andrea_85]

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

[akidess]

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)...