[openfoam1]

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

[ngj]

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

[openfoam1]

Originally Posted by ngj

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)




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



my boundary condtions

0/U

    /*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    left // patch inlit
    {
        type            fixedValue;
        value           uniform (1e-6 0 0);
    }
    right // patch outlet
    {
        type            fixedValue;
        value           uniform (1e-6 0 0);

    }
    uperWall  // wall uperWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    lowerWall // wall lowerWall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    frontAndBack // empty frontAndBack
    {
        type            empty;
    }
}


// ************************************************************************* //

0/P

    /*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    left
    {
        type           zeroGradient;
    }

    right
    {
        type           zeroGradient;
    }

    lowerWall
    {
        type           zeroGradient;
    }

    uperWall
    {
        type           zeroGradient;
    }

    frontAndBack
    {
        type            empty;
    }
}

// ************************************************************************* //

0/alpha1

    /*--------------------------------*- C++ -*----------------------------------*\
  | =========                 |                                                 |
  | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
  |  \\    /   O peration     | Version:  1.6.x                                 |
  |   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
  |    \\/     M anipulation  |                                                 |
  \*---------------------------------------------------------------------------*/
  FoamFile
  {
      version     2.0;
      format      ascii;
      class       volScalarField;
      location    "0";
      object      alpha1;
  }
  // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
   
  dimensions      [0 0 0 0 0 0 0];
   
  internalField   uniform 0;
   
  boundaryField
  {
      left
      {
          type            zeroGradient;
      }
      right
      {
          type            zeroGradient;
      }
      uperWall
      {
          type            zeroGradient;
      }
      lowerWall
      {
          type            zeroGradient;
      }
      frontAndBack
      {
          type            empty;
      }
  }
   
   
  // ************************************************************************* //

best regards

[ngj]

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

[holger_marschall]

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,

[openfoam1]

Originally Posted by ngj

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 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

[openfoam1]

Originally Posted by holger_marschall

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 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 :



but i think it isn't the problem

regards

[kpm]

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.

[ngj]

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

[phsieh2005]

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

[openfoam1]

Originally Posted by phsieh2005

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 ..

[phsieh2005]

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

[openfoam1]

Originally Posted by phsieh2005

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 ;



for time 0.0002 second ;



for time 0.0003 second ;



for time 0.0004 second ;



for time 0.0005 second ;



can you explain

best regards ..

[moh1367]

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?

[phsieh2005]

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

[moh1367]

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.

[Robat]

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

[openfoam1]

Originally Posted by moh1367

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?

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

[moh1367]

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!

[openfoam1]

Originally Posted by moh1367

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 ..