interFoam behavior in micro-dimensions
 

hi foamers ;

I'm working with micro-Nano simulations with free surface ,, i chose interFoam solver cause flow in those dimensions considered laminar , i make my mesh in 2D,, but i notice that when the dimensions reduces ( down until 1e-6) the time step approaches zero ( **e-9 or lower) and it takes a horrible time to even write a solution directory ( in 2D!! ) ,, what is the problem with interFoam solver ?!!
any one know what is going on

thanks

Hi

Well, the interFoam solver works (at least for macro-scale) flows, hence I assume their might be an error in your setup.
However as you have given no helpful informations, it is hard to give any help, however I suspect that the problem are in your boundary conditions.

Bests

Niels

Hi Niels ;

that is my case information

that is my mesh

the lower wall have micro craters (0.5 micron X 0.5 micron)


http://img192.imageshack.us/img192/4743/mesh2df.png

that is my alpha initial conditions ,, the flow of water should be from left to right and the micro craters contains air

http://img697.imageshack.us/img697/1882/alpha0.png

my boundary condtions

0/U

0/P

0/alpha1

best regards

Modeling the out-flow velocity distribution is basically the same as specifying the or at least part of the solution, hence try changing the following:

0/U at outlet: type zeroGradient
0/p at outlet: type fixedValue; value uniform 0 or apply hydrostatic pressure. I have not used the new interFoam in 1.6 hence I am not certain of what to use.

Best regards,

Niels

Hi,

you are after simulating the air entrained into the liquid cross-flow. Am I right?

I think in this case it would be wise to initialize the fluid level in the micro craters with some distance to the edges, the local mesh resolution of which should be reconsidered IMO.
Furthermore I think, it is appropriate to incorperate wetting behaviour (i.e. a dynamic contact angle + roughness) and partial slip at these (micro-)scales.

Did you think about adaptive mesh refinement to resolve the interface adequately sharpening the interface to a smaller interfacial width?

best,

Hi Niels ,

i did the changes

0/U at outlet: type zeroGradient
0/p at outlet: type fixedValue; value uniform 0

as you said

the time step for the first interval is 0.048 ,, 2nd interval (**e-7) ,, 3rd interval (**e-9) ,, and it continue with (**e-9) as a time step

,, do you think that is because the cell dimintions is very small (0.05 micron X 0.05 micron ) ?

is that a natural behavior ,, or i did thing wrong

regards

Hi Holger ;


my goal is to compute the lower wall friction coefficient (which have micro craters ) , and compare it with a one don't have any craters ,, and that allow me to calculate the slippage ratio of the wall to use it in another simulation

so the slip (from 0 to 1) should be output from this simulation

i can make my mesh grading towards the water-air interface like that :

http://img402.imageshack.us/img402/5185/grading.png

but i think it isn't the problem

regards

Surface tension effects are dominant in such small scales.
Just simulate a very small cube-shaped drop in such a scale and watch its evolution into a "natural" sphere-shaped drop.
Have a look at the velocities during the transition, compare them to the size of Your mesh, and You will have an explanation for the order of magnitude of Your time step.

Hi

Making an estimate of your Courant number it yields 0.96 based on your results, hence it is very close to one based on your initial conditions. Try lowering your initial time step and I suppose that would help. Say Courant no larger than 0.25 - you can specify that in controlDict, see e.g. damBreak tutorial.
Otherwise Holgers suggestion might be of interest.

Bests,

Niels

Hi,

I was told that interFoam solver is not appropriate for micro-channel flow with surface tension effect.

If you are successful in solving your problem, could you please post your results or finding?

I have tried to solver flow inside a small tube (around 0.2 mm) with strong surface tension effect (air/water). The spurous currents was quite bad.

Thanks

Pei

Hi Pei ;

the case is running till now,, but the problem is that the time step is very small (*.**e-9), so we have to wait horrible time until we get a steady state solution

i have to make order of magnitude analysis to know when i can stop and get steady state solution

when it done ,, it is no problem to share results with you

best regards ..

Hi, openfoam1,

Based on my past experience, the super small detal t is due to spurous currents. Check your velocity field to see if you are getting very high velocity near the air/liquid interface.

Is VOF suitable for micro-channel flow with strong surface tension effect?

Pei

Hi Pei ;

yes this phenomenon happened and a very high velocity appear in the interface see that ;;

for time 0.0001 second ;

http://img8.imageshack.us/img8/7/micro0001.jpg

for time 0.0002 second ;

http://img8.imageshack.us/img8/1667/micro0002.jpg

for time 0.0003 second ;

http://img8.imageshack.us/img8/4025/micro0003.jpg

for time 0.0004 second ;

http://img8.imageshack.us/img8/2118/micro0004.jpg

for time 0.0005 second ;

http://img8.imageshack.us/img8/8716/micro0005.jpg

can you explain

best regards ..

Hi !
I have similar problem with my case which is in nano-scale. By reducing the time step and even using implicit scheme the problem still exist. Are your problem solved?

Hi,

I was told that VOF is not suitable to this type of problem. Several groups have attempted to reduce the parasistic currents problem, but, I have not seem anything that can be implemented in OpenFOAM easily.

Pei

Thanks for your response
So, Whats your suggestion for me? What Should I do now? Is there another solver that is suitable for my case, for example Eulerian? The interface is very important in my case.

Hi Pei,

you said: "interFoam solver is not appropriate for micro-channel flow with surface tension effect."
Could you give us some links/references who told you about that?
The reason might be interesting for me.
(I've got a similar problem.)

Regards,
Robert

unfortunately the problem still exist ,,

those spurious currents still exist even if adopting very high resolution of
the mesh near interface ..

can any one know a solution to that annoying spurious currents near the interface,,

any help will be appreciated ..
best regards

Hi!
My problem is solved now! I found that the steady state time of my case is just about 1e-7 seconds and in this manner there is no need to get to 1s or 2s. Now I set my deltaT to 1e-11 and my courant is about 0.005.
You should examine if it's your case too!

Hello;
this is an encourage news ,, so the problem have a solution exists somewhere ,,
yes me too i don't need to get 1 or 2 seconds ,, but the problem is with that annoying spurious currents near interface ,,

your courant number is very small ,, do you think that when the courant number becomes too small it will solve the problem of spurious currents ?

best regards ..

Hi !

In my opinion, yes!
I check my velocity field and it seemed OK! The courant was about 0.4-0.8 at first and now it reduced so much. Do you resolve your case with very small DeltaT?

Sincerely

Hi
when i reduced the courant number from 0.25 to 0.005 ,, the currents completely disappeared ,, and the problem almost solved ,,

there is another question

i want to enter a boundary condition on the lower wall for alpha1 ,, i want to use alphaContactAngle boundary condition ,, i must enter the following:

1) static contact angle (theta0)
2) the leading and trailing edge dynamic contact angles (thetaA),(thetaR)
3) velocity scaling function for dynamic contact angle (uTheta)

is this important to enter (2) and (3) on my simulation, how can i find those values for water and a given solid

thanks very much ..

Hi openFoam!
I become very glad about your problem is solved now. you can see about the dynamic contact angle in one of the topic in the forum with this title"Dynamic contact angle". unfortunately I haven the link.
Sincerely

Hi,

I am glad to hear that this problem was resolved by reducing delta t. But, I am surprised. What is your channel diameter? What is your surface tension coefficient?

Based on what I read about spurious currents, it can be reduced by some methods, but, they usually work only on very good hex quality meshes.

In my case, I usually have to run the case up to 1 sec - 2 sec. Such a small delta t (< 1e-8) is not practical to me because it will take weeks to complete, even on a cluster with 32 CPUs.

Also, I usually run my case with CFL <= 0.3.

Pei

Hello everybody,
I would like to share my experience on the CFL number limit of interFOAM solvers. I have been using lesInterFOAM to study the breakup of liquid shees in 2D. My nozzle thickness is 50 micrometers. And I have run simulations with a range of CFL numbers on the same geometry and same b.cs. My range of CFL numbers span from 0.2 to 0.005. And I also performed a linear stability analysis in Mathematica for verifying my results. Then I found out that the case with the largest CFL number is 0.2 overpredicted the dominant wavelength when compared to the linear stability analyis. Whereas the case with the lowest CFL number 0.005 predicted the dominant wavelength accurately wwhen compared to the linear stability analysis.

I got into this investigation after looking at the literature "Volume of Fluid methods for immiscible-fluid and free surface flows" Chemical Engineering Journal 141 (2008) 204-221. In this paper it has been specified that the inter-gamma schemes require very small time steps CFL < 0.01 for keeping a sharp interface. But there is no proof given for this condition.
But i think itbecomes infeasible to run simulations on such small time steps.

My question is is it possible to use higher CFL numbers by increasing the nGammaSubcycles. Any experiences on this matter will be appreciated. I am also studying the influence of nGammaSubcycles on the solution.

bye
with regards
K.Suresh kumar

Probably this tread
http://www.cfd-online.com/Forums/ope...-currents.html
might help those who experiencing high parasitic currents at microscale and as a result a very low time step.

In my case it was a solution.

Hello everybody,
I studied the effect of ngammaSubcycles on the solution. I varied the ngamma Subcycles from 4, 10 ,16,20 while keeping all other parameters constant. The CFL no. was 0.2 and 0.5. There is no difference between these simulations. But i have read in the manual that higher CFL numbers can be used by increaasing this parameter andnot losing the accuracy. I thik this claim is not true.

Then I also modified the pEqn.H and the UEqn.H as specifed in the previous post by SundAERO, I saw that the modification of the surface tension term makes the solution a bit better, but in my case i do not see much improvement. I am still waiting for my simulation to finish and i already see that the simulation without this modification and with the modification are not so different. So i doubt that this modification really does not work for all cases. It always depends on the application that one is studying.

My next question is has anybody tried to use an implicitMULES solver with interFOAM for microdimensions problems. I am planning to compile the implicit MULES with interFOAM and change the fvSchemes files. I just wanted to know if somebody has already tried the implicitMULES solver and seen any improvement in their solution, any comments on comparison between the implicitMULES and explicitMULES solutions for interFOAM are welcome.

Anyhow i will update the findings once i run a implicit case.

bye
with regards
K.Suresh kumar

Hi, kumar,

I ran 2 completely different cases. Both with and without the modifications.

In one case, the modification help, while in the other case, the modification did not help.

So, whether this modification helps or not is case dependent.

Someone told me that this modification was tested few years ago and the conclusion was the following:

it introduces a serious bias in the force
balance of the surface-tension and the results for capillary-rise etc. were
significantly less accurate.

Pei

Hello interFOAM guys

I am happy to inform that after trying every option in the box, i finally found some sucess with the CFL number issue atleast for my case.

I made an implicit solver for solving the alpha equation by calling the MULES::implicitSolve and had to do some more changes to make the solver work.

But the good news is that i already have some initial results from the implicit solver interFoam which i am running for a CFL no. of 0.25 and i see that they match with the case that i ran with the CFL-0.005. I am using the Euler scheem for time integration, in the implciit case which is first order. And the simulation itself is much faster.

So first of all i would thank the guys for making such a code , where i can change the solver as i want.

I would suggest the people who have the problem with the CFL number, where you need small CFL numbers to obtain a reasonably accurate result, you should give a try by implementing the MULES::implicit in interFoam and try it.

But it may work for your case or not. but it is worth giving a try.

bye
K.Suresh kumar

Hi, kumar,

I am excited to hear your good news. I am wondering if you will be willing to share your revised interFoam solver so that I can test it on my case. Or, if you can post the changes you made.

Pei

Hello Pei,
I already got my simulaiton finsished , and i see that the results are much better, but i still have to validate it by extracting the dominant wave information because i am studying breakup of liquid sheets. But i can tell you that they are closer to the case that i ran with a CFL -0.005 with an MULES::explicitsolve. But this does not mean that they are correct unless i compare it with experiments, which i am trying to do.

Anyhow regarding the changes for the solver, here is what i did,

1) cp -riuv --parents --backup applications/solvers/multiphase/interFoam $WM_PROJECT_USER_DIR

2)then i go to the $WM_PROJECT_USER_DIR and change the name to implicit_interFOAM

3)mv interFoam.C implicit_interFoam.C
4)i delete the alphaEqn.H and alphaEqnSubcycle.H
5) I copy the files alphaEqn.H and alphaEqnSubcycle.H from interPhaseChangeFoam to the current directory.

6) Then i modify the alphaEqn.H file. The modofoed file is shown below

{
word alphaScheme("div(phi,alpha1)");
word alpharScheme("div(phirb,alpha1)");

surfaceScalarField phir("phir", phic*interface.nHatf());

for (int gCorr=0; gCorr<nAlphaCorr; gCorr++)
{
surfaceScalarField phiAlpha =
fvc::flux
(
phi,
alpha1,
alphaScheme
)
+ fvc::flux
(
-fvc::flux(-phir, scalar(1) - alpha1, alpharScheme),
alpha1,
alpharScheme
);

// Pair<tmp<volScalarField> > vDotAlphal =
// twoPhaseProperties->vDotAlphal();
// const volScalarField& vDotcAlphal = vDotAlphal[0]();
// const volScalarField& vDotvAlphal = vDotAlphal[1]();

// volScalarField Sp
// (
// IOobject
// (
// "Sp",
// runTime.timeName(),
// mesh
// ),
// vDotvAlphal - vDotcAlphal
// );

// volScalarField Su
// (
// IOobject
// (
// "Su",
// runTime.timeName(),
// mesh
// ),
// Divergence term is handled explicitly to be
// consistent with the explicit transport solution
// divU*alpha1
// + vDotcAlphal
// );

//MULES::explicitSolve(alpha1, phi, phiAlpha, 1, 0);
//MULES::explicitSolve(oneField(), alpha1, phi, phiAlpha, Sp, Su, 1, 0);
MULES::implicitSolve(oneField(), alpha1, phi, phiAlpha, zeroField(), zeroField(), 1, 0);

rhoPhi +=
(runTime.deltaT()/totalDeltaT)
*(phiAlpha*(rho1 - rho2) + phi*rho2);
}

Info<< "Liquid phase volume fraction = "
<< alpha1.weightedAverage(mesh.V()).value()
<< " Min(alpha1) = " << min(alpha1).value()
<< " Max(alpha1) = " << max(alpha1).value()
<< endl;
}
And then i compile by changing the Make/files.

But to tun the case sucessfully i had to add the following lines to my fvSolution file
{
alpha1
{
maxUnboundedness 1e-5;
CoCoeff 2;
maxIter 5;
nLimiterIter 2;

solver PBiCG;
preconditioner DILU;
tolerance 1e-12;
relTol 0.1;
};
which i took from the cavitating bullet tutorial. I still have to look in to the tolerance and relTol.

I also changed the ddt schemes in the fvSchemes by setting default Euler


bye
with regards
K.Suresh kumar

Thanks kumar!

I will give it a try to see if this helps with my two different cases.

Pei

Hi Kumar,
Have you got any news?. I'm trying to simulate a two fluid system in a microchannel (dimension of the order of micron). Using MULES::explicit i got delta t =1e-7 s and the simulation takes a lot of time. In my opinion, the problem is that at the interface the parasite velocity are too big (up to 0.5 m/s!! when the inlet velocity is 1e-4 m/s) and so the time step remains small (dt=Co*dx/U).
I tried to implement the MULES::implicit, following your suggestions. The time step is still of the order of 1e-7 s and the simulation is very slow. I'm using OF 1.7.1.
Any idea why i can not increase the time step as in your case?

Thanks

andrea

Hi Andrea,
I would first like to ask you, what method are you using for the time discretization, are you using Crank-Nicholson or Euler implicit.

My experience with using MULES::implicit was not satisfactory, so i did not use it for my further study.

Also do you use adjustimestep for your simulation.


regards
K.Suresh kumar

Hi Kumar, thanks for the answer.
I'm using Euler scheme for ddt and yes, i'm also using adjustable time step.
I have not tried using a fix time step and force the solver to go faster, but i guess it would crash!

andrea

Do you have any idea to speed up my simulation? How did you solve your problem with the CFL number?

I tried to run exactly the same case as before but now with the dimension of millimiters instead of micron. Everythink is ok, the simulation time is good using Co=0.3.

Any help is appreciated

andrea

Hi Andrea, I was wondering If you found any solution to increase the speed of the simulation. I am facing the same issue.

Hello All,


It is a very interesting thread (even thought old). I am also doing simulations using interFoam for rally low capillary numbers (10^(-5) - 10^(-4)).


The issue , is for me to respect the Brackbill condition (or Galusinski and Vigneaux criterion to take into account the viscosity) with my current meshing (1-2 micrometer/cell), I need to have a courant number of 0.005 at the very least.



However, this lead to excessive waiting time to get enough time steps. Did anyone find a solution to get accurate solutions (avoiding spurious currents) for low capillary numbers problems in interFoam without blowing up the computational time ?


Thanks for any hints or suggestions!




Sincerely,
Santhosh