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

interFoam behavior in micro-dimensions

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 23, 2010, 10:13
Default interFoam behavior in micro-dimensions
  #1
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
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
openfoam1 is offline   Reply With Quote

Old   January 25, 2010, 03:54
Default
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,608
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is offline   Reply With Quote

Old   January 25, 2010, 11:04
Default
  #3
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by ngj View Post
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

Code:
    /*--------------------------------*- 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

Code:
    /*--------------------------------*- 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

Code:
    /*--------------------------------*- 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
openfoam1 is offline   Reply With Quote

Old   January 25, 2010, 11:13
Default
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,608
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is offline   Reply With Quote

Old   January 25, 2010, 11:23
Default
  #5
Senior Member
 
Holger Marschall
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 123
Rep Power: 10
holger_marschall is on a distinguished road
Send a message via Skype™ to 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,
__________________
Holger Marschall
web: http://www.holger-marschall.info
mail: holgermarschall@yahoo.de
holger_marschall is offline   Reply With Quote

Old   January 25, 2010, 13:56
Default
  #6
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by ngj View Post
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

Last edited by openfoam1; January 25, 2010 at 14:19.
openfoam1 is offline   Reply With Quote

Old   January 25, 2010, 14:18
Default
  #7
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by holger_marschall View Post
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

Last edited by openfoam1; January 25, 2010 at 14:56.
openfoam1 is offline   Reply With Quote

Old   January 25, 2010, 14:18
Default
  #8
kpm
New Member
 
kpm
Join Date: Jan 2010
Location: Germany
Posts: 9
Rep Power: 7
kpm is on a distinguished road
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.
kpm is offline   Reply With Quote

Old   January 25, 2010, 14:24
Default
  #9
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,608
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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
ngj is offline   Reply With Quote

Old   January 26, 2010, 08:16
Default
  #10
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   January 26, 2010, 08:38
Default
  #11
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by phsieh2005 View Post
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 ..
openfoam1 is offline   Reply With Quote

Old   January 26, 2010, 11:38
Default
  #12
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   January 27, 2010, 04:24
Default
  #13
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by phsieh2005 View Post
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 ..
openfoam1 is offline   Reply With Quote

Old   February 26, 2010, 04:06
Default
  #14
Member
 
Mohammad Zakerzadeh
Join Date: Dec 2009
Location: Aachen, Germany
Posts: 40
Rep Power: 7
moh1367 is on a distinguished road
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?
moh1367 is offline   Reply With Quote

Old   February 26, 2010, 08:20
Default
  #15
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 271
Rep Power: 9
phsieh2005 is on a distinguished road
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
phsieh2005 is offline   Reply With Quote

Old   February 26, 2010, 11:29
Default
  #16
Member
 
Mohammad Zakerzadeh
Join Date: Dec 2009
Location: Aachen, Germany
Posts: 40
Rep Power: 7
moh1367 is on a distinguished road
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.
moh1367 is offline   Reply With Quote

Old   February 26, 2010, 12:11
Default
  #17
New Member
 
Robert Langner
Join Date: Dec 2009
Location: Freiburg, Germany
Posts: 27
Rep Power: 7
Robat is on a distinguished road
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
Robat is offline   Reply With Quote

Old   March 4, 2010, 11:59
Default
  #18
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by moh1367 View Post
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
openfoam1 is offline   Reply With Quote

Old   March 5, 2010, 02:39
Default
  #19
Member
 
Mohammad Zakerzadeh
Join Date: Dec 2009
Location: Aachen, Germany
Posts: 40
Rep Power: 7
moh1367 is on a distinguished road
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!
moh1367 is offline   Reply With Quote

Old   March 5, 2010, 08:41
Default
  #20
Member
 
Join Date: Dec 2009
Posts: 46
Rep Power: 7
openfoam1 is on a distinguished road
Quote:
Originally Posted by moh1367 View Post
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 ..

Last edited by openfoam1; March 5, 2010 at 09:58.
openfoam1 is offline   Reply With Quote

Reply

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
InterFoam stops after deltaT goes to 1e14 francesco_b OpenFOAM Running, Solving & CFD 8 July 31, 2013 02:29
Interfoam... free surface simulation urgent lostin4ever Main CFD Forum 4 October 12, 2010 08:29
Moving from simpleFoam to interFoam with alpha = 0 kjetil OpenFOAM Running, Solving & CFD 1 November 8, 2009 21:04
Open Channel Flow using InterFoam type solver sxhdhi OpenFOAM Running, Solving & CFD 3 May 5, 2009 21:58
Dimensions of laplacian in PISO loop kumar2 OpenFOAM Running, Solving & CFD 2 July 3, 2006 14:34


All times are GMT -4. The time now is 01:41.