|
[Sponsors] |
November 2, 2011, 04:59 |
interFoam VOF is loosing fluid
|
#1 |
Member
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 32
Rep Power: 17 |
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 |
|
November 2, 2011, 06:16 |
|
#2 |
Senior Member
Aurelien Thinat
Join Date: Jul 2010
Posts: 165
Rep Power: 16 |
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. |
|
November 2, 2011, 08:23 |
|
#3 |
Member
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 32
Rep Power: 17 |
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; } } // ************************************************************************* // 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 |
|
November 2, 2011, 09:13 |
|
#4 |
Senior Member
Aurelien Thinat
Join Date: Jul 2010
Posts: 165
Rep Power: 16 |
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. |
|
November 3, 2011, 16:38 |
|
#5 |
Member
angel
Join Date: May 2009
Location: Spain
Posts: 46
Rep Power: 17 |
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 |
|
November 4, 2011, 05:06 |
|
#6 |
Member
Soeren Werner
Join Date: Mar 2009
Location: Wädenswil, Switzerland
Posts: 32
Rep Power: 17 |
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 |
|
February 27, 2012, 08:16 |
|
#7 |
New Member
Ivo
Join Date: Feb 2012
Posts: 26
Rep Power: 14 |
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? |
|
February 27, 2012, 08:22 |
|
#8 |
Senior Member
Aurelien Thinat
Join Date: Jul 2010
Posts: 165
Rep Power: 16 |
Ivooo,
By any chance, do you have any symmetryPlane condition in your case ? |
|
February 27, 2012, 08:37 |
|
#9 |
New Member
Ivo
Join Date: Feb 2012
Posts: 26
Rep Power: 14 |
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.
|
|
February 27, 2012, 08:47 |
|
#10 |
Senior Member
Aurelien Thinat
Join Date: Jul 2010
Posts: 165
Rep Power: 16 |
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. |
|
February 28, 2012, 11:11 |
Check your BCs!
|
#11 |
New Member
Ivo
Join Date: Feb 2012
Posts: 26
Rep Power: 14 |
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] http://www.cfd-online.com/Forums/ope...interfoam.html |
|
June 2, 2012, 18:06 |
|
#12 |
New Member
roberto putzu
Join Date: Mar 2012
Posts: 9
Rep Power: 14 |
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 |
|
June 26, 2013, 09:13 |
|
#13 |
New Member
Felix
Join Date: Aug 2012
Posts: 7
Rep Power: 14 |
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! |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Fluent VOF Volume of Fluid Realistic Solution Problem | wormik | FLUENT | 3 | June 21, 2009 08:04 |
Questions of fluid pairs | fjalil | CFX | 1 | June 10, 2009 18:36 |
Fluid pairs | fjalil | Main CFD Forum | 0 | June 10, 2009 14:47 |
VOF - fluid property problem | weechristo | FLUENT | 1 | April 11, 2009 16:08 |
How to apply negtive pressure to outlet | bioman66 | CFX | 5 | June 3, 2006 02:40 |