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

interFoam VOF is loosing fluid

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

Like Tree2Likes
  • 1 Post By Ivooo
  • 1 Post By flexi182

Reply
 
LinkBack Thread Tools Display Modes
Old   November 2, 2011, 04:59
Default interFoam VOF is loosing fluid
  #1
New Member
 
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 24
Rep Power: 8
wersoe is on a distinguished road
Hello Foamers,

I am running a case with interDyMFoam with OF-2.0.x
It is simulating a shake flask, which is use in bioscience for cultivation of microorganisms and other cells... so, in simple words, its a conical flask fixed at a rotating table. If you look at the flask form one point, you see always the same point at the flask, a little like the movement of the moon... anyway, I manage to change the tankMixer tutorial so that I get the movement rite...

The problem:
With every timestep it looses a certain amount of fluid due to "mathematical diffusion" or something... it became obvious after about 5s simulation time, after 10-15 s no water is in the flask at all!
How can this happen? And can I avoid it?

The mesh is quite good, checkMesh shows no problems at all.
The residues ar quite low, see below...

I attached some of the important configuration files.

Hopefully sb has an idea what could happen here, since I am really stuck here at the moment...


solver.log, just two time step, it looks all time quite the same, time step size will be bigger later on during the simulation...
Code:
Interface Courant Number mean: 0.0066323 max: 0.498321
Courant Number mean: 0.0398762 max: 0.498321
deltaT = 7.7658e-07
Time = 0.000208016105042192333

solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.000208016 transformation: ((0.000163375 2.66915e-07 0) (0.999999 (0 0 0.00163375)))
solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.000208016 transformation: ((0 0 0) (0.999999 (0 0 -0.00163375)))
solidBodyMotionFunctions::multiMotion::transformation(): Time = 0.000208016 transformation: ((0.000163375 2.66915e-07 0) (1 (0 0 0)))
Execution time for mesh.update() = 0.26 s
time step continuity errors : sum local = 1.96807e-13, global = -1.09833e-18, cumulative = -2.77411e-13
GAMGPCG:  Solving for pcorr, Initial residual = 1, Final residual = 6.41289e-07, No Iterations 19
GAMGPCG:  Solving for pcorr, Initial residual = 0.0710413, Final residual = 5.60197e-07, No Iterations 10
GAMGPCG:  Solving for pcorr, Initial residual = 0.00429145, Final residual = 5.82585e-07, No Iterations 7
time step continuity errors : sum local = 3.62563e-18, global = -1.11019e-18, cumulative = -2.77412e-13
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 2.30226e-132  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 3.02039e-132  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 3.96591e-132  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 5.21193e-132  Max(alpha1) = 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.00237312, Final residual = 4.19164e-09, No Iterations 3
DILUPBiCG:  Solving for Uy, Initial residual = 0.00328753, Final residual = 7.49817e-09, No Iterations 3
DILUPBiCG:  Solving for Uz, Initial residual = 0.0020948, Final residual = 3.63414e-09, No Iterations 4
GAMG:  Solving for p_rgh, Initial residual = 0.0253511, Final residual = 0.000118152, No Iterations 3
GAMG:  Solving for p_rgh, Initial residual = 0.00189087, Final residual = 1.84691e-05, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 0.000119528, Final residual = 9.13697e-07, No Iterations 6
time step continuity errors : sum local = 2.13139e-10, global = -7.34516e-19, cumulative = -2.77413e-13
GAMG:  Solving for p_rgh, Initial residual = 0.00091004, Final residual = 2.82139e-06, No Iterations 3
GAMG:  Solving for p_rgh, Initial residual = 4.74559e-05, Final residual = 2.29515e-07, No Iterations 3
GAMGPCG:  Solving for p_rgh, Initial residual = 3.12808e-06, Final residual = 1.99243e-09, No Iterations 4
time step continuity errors : sum local = 4.0557e-13, global = -7.34599e-19, cumulative = -2.77414e-13
DILUPBiCG:  Solving for omega, Initial residual = 0.00892048, Final residual = 7.19565e-09, No Iterations 4
DILUPBiCG:  Solving for k, Initial residual = 0.00479677, Final residual = 1.3686e-10, No Iterations 5
ExecutionTime = 902.75 s  ClockTime = 905 s

Interface Courant Number mean: 0.00666334 max: 0.498319
Courant Number mean: 0.0400127 max: 0.498319
deltaT = 7.79193e-07
Time = 0.000208795297929659983

solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.000208795 transformation: ((0.000163987 2.68919e-07 0) (0.999999 (0 0 0.00163987)))
solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 0.000208795 transformation: ((0 0 0) (0.999999 (0 0 -0.00163987)))
solidBodyMotionFunctions::multiMotion::transformation(): Time = 0.000208795 transformation: ((0.000163987 2.68919e-07 0) (1 (0 0 0)))
Execution time for mesh.update() = 0.26 s
time step continuity errors : sum local = 4.06964e-13, global = 2.12725e-18, cumulative = -2.77411e-13
GAMGPCG:  Solving for pcorr, Initial residual = 1, Final residual = 8.2677e-07, No Iterations 26
GAMGPCG:  Solving for pcorr, Initial residual = 0.0782515, Final residual = 7.38951e-07, No Iterations 21
GAMGPCG:  Solving for pcorr, Initial residual = 0.00468234, Final residual = 3.12732e-07, No Iterations 11
time step continuity errors : sum local = 4.6662e-18, global = 2.12035e-18, cumulative = -2.77409e-13
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 6.8496e-132  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 9.01104e-132  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 1.18666e-131  Max(alpha1) = 1
MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.193844  Min(alpha1) = 1.5643e-131  Max(alpha1) = 1
DILUPBiCG:  Solving for Ux, Initial residual = 0.00237884, Final residual = 3.78435e-09, No Iterations 3
DILUPBiCG:  Solving for Uy, Initial residual = 0.00328912, Final residual = 7.99669e-09, No Iterations 3
DILUPBiCG:  Solving for Uz, Initial residual = 0.00209302, Final residual = 3.10299e-09, No Iterations 4
GAMG:  Solving for p_rgh, Initial residual = 0.0255634, Final residual = 0.000116615, No Iterations 3
GAMG:  Solving for p_rgh, Initial residual = 0.00189883, Final residual = 1.77012e-05, No Iterations 2
GAMG:  Solving for p_rgh, Initial residual = 0.000119078, Final residual = 8.93598e-07, No Iterations 6
time step continuity errors : sum local = 2.10798e-10, global = 2.13129e-19, cumulative = -2.77409e-13
GAMG:  Solving for p_rgh, Initial residual = 0.000931977, Final residual = 2.85761e-06, No Iterations 3
GAMG:  Solving for p_rgh, Initial residual = 4.78142e-05, Final residual = 2.35694e-07, No Iterations 3
GAMGPCG:  Solving for p_rgh, Initial residual = 3.16514e-06, Final residual = 1.28317e-09, No Iterations 4
time step continuity errors : sum local = 2.60862e-13, global = 2.1641e-19, cumulative = -2.77409e-13
DILUPBiCG:  Solving for omega, Initial residual = 0.00886702, Final residual = 5.8744e-09, No Iterations 4
DILUPBiCG:  Solving for k, Initial residual = 0.00479084, Final residual = 1.15469e-10, No Iterations 5
ExecutionTime = 910.15 s  ClockTime = 912 s
Attached Files
File Type: txt controlDict.txt (2.1 KB, 16 views)
File Type: txt dynamicMeshDict.txt (2.0 KB, 44 views)
File Type: txt fvSchemes.txt (1.5 KB, 21 views)
File Type: txt fvSolution.txt (3.0 KB, 15 views)
wersoe is offline   Reply With Quote

Old   November 2, 2011, 06:16
Default
  #2
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Hi Wersoe,

You should send your folder 0, or at least the boundary conditions for alpha1 and U. It would be easier to help you.
Aurelien Thinat is offline   Reply With Quote

Old   November 2, 2011, 08:23
Default
  #3
New Member
 
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 24
Rep Power: 8
wersoe is on a distinguished road
Hi Aurelien,

thanks for trying to help me...

Here are the contents, its quite simple, since it is all around just wall, the same like in the tankMixer tutorial...

One more thing: I use the k-o SST turbulence model instead of laminar...


U:
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0);

boundaryField
{
    Deckel
    {
        type            movingWallVelocity;
        value           uniform (0 0 0);
    }
    Wand
    {
        type            movingWallVelocity;
        value           uniform (0 0 0);
    }
}

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

alpha1 before setFields:
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    Deckel
    {
        type            zeroGradient;
    }
    
    Wand
    {
        type            zeroGradient;
    }
}

// ************************************************************************* //
setFieldsDict:
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue alpha1 0
);

regions
( 
    boxToCell
    {
        box ( -0.1 -0.1 0 ) ( 0.1 0.1 0.02725 ); //10mL
//        box ( -0.1 -0.1 0 ) ( 0.1 0.1 0.04525 ); //20mL
        fieldValues
        (
            volScalarFieldValue alpha1 1
        );
    }
);

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

Any idea?

Your help is much appreciated...

Best, Sören
wersoe is offline   Reply With Quote

Old   November 2, 2011, 09:13
Default
  #4
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
I don't see any problem in your files.

Did you try to run your case on several meshes with different cell's size ?
You can divide by 2 your reference cell size at each step and see if you are stabilizing the volume of fluid
.
I have run the tutorial and there is the same problem, obviously because of the cell size.
Aurelien Thinat is offline   Reply With Quote

Old   November 3, 2011, 16:38
Default
  #5
Member
 
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 8
anmartin is on a distinguished road
Hello,
I have the same ploblem since of1.6 but i do not have any solution. I have tried with different mesh size with same results.
Regards
anmartin is offline   Reply With Quote

Old   November 4, 2011, 05:06
Default
  #6
New Member
 
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 24
Rep Power: 8
wersoe is on a distinguished road
Hello,

thanks for your replies...

I use a polyeder mesh create with following steps:
1: Salome for geometry and surface mesh
2: enGrid for boundary layer and volume mesh with tetraeder
3: polyDualMesh for conversion to polymesh

The size of the domain is about 500mL.
The mesh is about 2mm in edge lenght, which gives about 800 k cells with tetra and about 200k with poly...

I run the case with single processor, and with 4 and 8 processors...

The main thing I dont understand is that the time step continuity error is very small, about 1e-18, even after many thousands time steps the cumulative error is just about 1e-15.
So what happens here?

@Aurelien: Could you give me a hint how you reduce the mesh size by 2? Which tool do you use for it?

@anmartin: Thanks for the hint, anyway, I cant use it. For the motion I use the multiMotion class, which was introduced in OF 2.0.


Any help would be much appreciated.

Best, Sören
wersoe is offline   Reply With Quote

Old   February 27, 2012, 08:16
Default
  #7
New Member
 
Ivo
Join Date: Feb 2012
Posts: 22
Rep Power: 5
Ivooo is on a distinguished road
Hi Wersoe,

For what it's worth, after 3 months; refining the mesh can be done using the 'refineMesh' tool. But of course you can also change the blockMeshDict to change the cell size.


I am too seeing this problem, also with interDyMFoam... The alpha1 fraction in the domain should not change if there's no inflow or outflow, but it does. As far as I know, the VoF scheme should be fully conservative, no matter what the cell size is. I just cannot really pinpoint the problem, in some simulations I can see it happening immediately, in other simulations it doesn't happen or only after a long time. Could it have something to do with large-small cell transitions?
Ivooo is offline   Reply With Quote

Old   February 27, 2012, 08:22
Default
  #8
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Ivooo,

By any chance, do you have any symmetryPlane condition in your case ?
Aurelien Thinat is offline   Reply With Quote

Old   February 27, 2012, 08:37
Default
  #9
New Member
 
Ivo
Join Date: Feb 2012
Posts: 22
Rep Power: 5
Ivooo is on a distinguished road
Quote:
Originally Posted by Aurelien Thinat View Post
Ivooo,

By any chance, do you have any symmetryPlane condition in your case ?
No, but I do use the constantAlphaContactAngle BC condition. I simulate a droplet around a fibre, and I set the contact angle of the fibre to some high value so that the liquid moves to find its lowest energy state. While it looks ok, I can check the volume fraction of alpha1 in the domain, and it decreases. Some snapshots and volume vs time evolution are given in the Figures attached.
Attached Images
File Type: png scrshot_t0.png (68.8 KB, 63 views)
File Type: png scrshot_t_last.png (65.5 KB, 58 views)
File Type: png volumeloss.png (21.3 KB, 58 views)
Ivooo is offline   Reply With Quote

Old   February 27, 2012, 08:47
Default
  #10
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Well, for what it's worth :
I had some issues with the conservation of the fluid volume fraction in my simulations. It was linked to the pressure condition over a symmetryPlane. The gradient was not defined correctly. I switched for a slip wall with buoyant Presssure condition to fix it.
Aurelien Thinat is offline   Reply With Quote

Old   February 28, 2012, 11:11
Default Check your BCs!
  #11
New Member
 
Ivo
Join Date: Feb 2012
Posts: 22
Rep Power: 5
Ivooo is on a distinguished road
Hi,

Just to follow-up the volume loss problems using constantAlphaContactAngle; be sure to set the 'limit' parameter to 'zeroGradient', otherwise a flux through the interface will emerge. Another option is to change the pressure boundary conditions, as outlined in the post of phsieh2005 in [1].

[1] how to specify wall contact angle for compressibleInterFoam?
farazarbabi likes this.
Ivooo is offline   Reply With Quote

Old   May 21, 2012, 04:51
Default
  #12
New Member
 
Join Date: May 2012
Posts: 3
Rep Power: 5
masterblaster is on a distinguished road
Aurelien,
I had symmetryPlanes and replaced them with slip conditions and buoyantPressure but see the same loss of fluid that i had before...
masterblaster is offline   Reply With Quote

Old   June 2, 2012, 17:06
Default
  #13
New Member
 
roberto putzu
Join Date: Mar 2012
Posts: 9
Rep Power: 5
roby is on a distinguished road
Hello,

This is maybe just a silly idea coming to my mind: What if you reduce the tolerances in the fvSolution? (i particular for U) If you have a continuity problem, maybe it's because the equation is not sufficiently well approximated.

Roby
roby is offline   Reply With Quote

Old   June 26, 2013, 08:13
Default
  #14
New Member
 
Felix
Join Date: Aug 2012
Posts: 7
Rep Power: 5
flexi182 is on a distinguished road
For constantAlphaContactAngle
you must use
fixedFluxPressure

-> Calculates the pressure gradient in that way that the velocity bc is fullfilled
Velocity*Area is Flux! and the flux is at the wall then zero!
jhmoon9 likes this.
flexi182 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
Fluent VOF Volume of Fluid Realistic Solution Problem wormik FLUENT 3 June 21, 2009 07:04
Questions of fluid pairs fjalil CFX 1 June 10, 2009 17:36
Fluid pairs fjalil Main CFD Forum 0 June 10, 2009 13:47
VOF - fluid property problem weechristo FLUENT 1 April 11, 2009 15:08
How to apply negtive pressure to outlet bioman66 CFX 5 June 3, 2006 01:40


All times are GMT -4. The time now is 10:25.