
[Sponsors] 
November 2, 2012, 00:37 
Nonphysical alpha1 with interFoam and high contact angles

#1 
Member
Adam James
Join Date: Jul 2010
Posts: 36
Rep Power: 7 
Hello all,
I'm using OpenFOAM 2.1.1 (interFoam solver) to model water droplet impacts on superhydrophobic surfaces with very high constantAlphaContactAngle  163 degrees. In short, it's an extension of the dam break tutorial where there's an initialised droplet of water within the domain which, after a period of time, will impact on a superhydrophobic surface. Here are my BC's; Code:
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 { substrate { type fixedValue; value uniform (0 0 0); } atmosphere { type pressureInletOutletVelocity; value uniform (0 0 0); } defaultFaces { type empty; } } Code:
FoamFile { version 2.0; format ascii; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 1 2 0 0 0 0]; internalField uniform 0; boundaryField { substrate { type totalPressure; // zeroGradient; has also been attempted p0 uniform 0; U U; phi phi; rho rho; psi none; gamma 1; value uniform 0; } atmosphere { type totalPressure; p0 uniform 0; U U; phi phi; rho rho; psi none; gamma 1; value uniform 0; } defaultFaces { type empty; } } Code:
FoamFile { version 2.0; format ascii; class volScalarField; object alpha; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 0 0 0 0]; internalField uniform 0; boundaryField { substrate { type constantAlphaContactAngle; gradient uniform 0; limit none; theta0 163; value uniform 0; } atmosphere { type inletOutlet; inletValue uniform 0; value uniform 0; } defaultFaces { type empty; } } Code:
Courant Number mean: 0.00770252 max: 0.487324 Interface Courant Number mean: 0.000653673 max: 0.474258 deltaT = 1.13562e05 Time = 0.0803864 MULES: Solving for alpha1 Phase1 volume fraction = 0.00347786 Min(alpha1) = 0.353626 Max(alpha1) = 1.00404 MULES: Solving for alpha1 Phase1 volume fraction = 0.00347586 Min(alpha1) = 0.350839 Max(alpha1) = 1.00402 MULES: Solving for alpha1 Phase1 volume fraction = 0.00347386 Min(alpha1) = 0.347173 Max(alpha1) = 1.00401 MULES: Solving for alpha1 Phase1 volume fraction = 0.00347187 Min(alpha1) = 0.345021 Max(alpha1) = 1.00399 MULES: Solving for alpha1 Phase1 volume fraction = 0.00346987 Min(alpha1) = 0.346423 Max(alpha1) = 1.00398 DICPCG: Solving for p_rgh, Initial residual = 0.013328, Final residual = 9.31482e13, No Iterations 257 time step continuity errors : sum local = 1.35985e15, global = 4.94506e17, cumulative = 7.33426e11 DICPCG: Solving for p_rgh, Initial residual = 0.0013377, Final residual = 9.42321e13, No Iterations 235 time step continuity errors : sum local = 1.38612e15, global = 2.03524e17, cumulative = 7.33426e11 DICPCG: Solving for p_rgh, Initial residual = 0.00022603, Final residual = 9.38786e10, No Iterations 164 time step continuity errors : sum local = 1.38035e12, global = 3.02764e14, cumulative = 7.33123e11 ExecutionTime = 926.66 s ClockTime = 1033 s Could anyone advise me on what course of action to take? Am I misplaced in thinking that interFoam is suitable for this problem, and if so, is there a better choice of solver for this case? Incidentally, I have tried more diffusive upwind divergence schemes without success either, below are my present schemes; Code:
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { div(rho*phi,U) Gauss limitedLinearV 1; div(phi,alpha) Gauss vanLeer; div(phirb,alpha) Gauss interfaceCompression; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p_rgh; pcorr; alpha1; } // ************************************************************************* // 

November 2, 2012, 04:28 

#2 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,019
Rep Power: 18 
Try this interFoam VOF is loosing fluid
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2 

November 2, 2012, 06:35 

#3 
Member

Hi,
I was noticed some issues related to contact angle boundary condition in openfoam (look at solved: contact angle correction in interFoam). The contact angle boundary conditions which I will use for alpha1 and p are: substrate { type constantAlphaContactAngle; limit gradient; theta0 163; value uniform 0; } and substrate { type fixedFluxPressure; adjoint no; } And they work fine for me for a wide range of contact angle. Duong 

November 3, 2012, 04:12 

#4 
Member
Adam James
Join Date: Jul 2010
Posts: 36
Rep Power: 7 
Thanks for your suggestions. They have shown some promise so far but I will try to get back with firmer conclusions in the near future.
On another note, when saving long animations in paraFoam, the software appears to suffer from a memory leak and crashes when I run out of RAM and swap space respectively. Could anyone point to a solution regarding this additional problem? I can work my way around it manually, in several ways, but that's a last resort. I've seen this issue discussed elsewhere but I haven't come across the solution. Thanks. 

November 3, 2012, 07:44 

#5 
Member
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 7 
I have the same experience as Duong: use the BC's he is suggesting and your problem should go away.
On a side note: I strongly doubt that the constantAlphaContactAngle is the correct BC to be using at all for droplet impact. The main problem is that the velocity dependence of the contact angle will dramatically change the spreading behaviour (see e.g. [1]), which is typically an important aspect of the droplet impact. You could look into the dynamicAlphaContactAngle or even progam your own dynamic model, like the CoxVoinov model. Cheers, Michiel [1] Carlson et al. Phys. Fluids 21, 121701 (2009)  http://link.aip.org/link/doi/10.1063/1.3275853 

November 4, 2012, 00:32 

#6 
Member
Adam James
Join Date: Jul 2010
Posts: 36
Rep Power: 7 
Thanks everybody, I now have some stable results to work with and improve upon, having implemented the boundary conditions first suggested by duongquaphim.
@michielm I have used dynamicAlphaContactAngle previously but that was only from the point of view of attempting to overcome the stability and nonphysical issues I outlined earlier. That said, however, I think it's something I am more than likely to return to. Incidentally, does anyone have a headsup on a viable way to include porous effects on the substrate? Thanks again. 

November 6, 2012, 03:54 

#7 
Member
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 7 
I think this depends a lot on the difference in length scales of your porous structure and your droplet. If e.g. the pores are 200 micron and your droplet is 2000 micron then you might consider to really mesh the pores.
If however the pores are closer to 20 micron then you need some kind of subgrid model/an appropriate BC for it. I know that OF has some libraries/models to work with porous zones so you could look into that. A useful starting point might be this: http://www.tfd.chalmers.se/~hani/kur...ukurReport.pdf 

November 6, 2012, 05:17 

#8  
Member
Adam James
Join Date: Jul 2010
Posts: 36
Rep Power: 7 
Quote:
Previously (in ANSYS Fluent) I just bundled the slot gaps (pores) with my 'atmosphere' BC, I presume that's the logical way to go. I can also break my substrate stems and tips into two patches, with different contact angles respectively. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Artificial high velocities at the interface using interFoam  Arnoldinho  OpenFOAM Running, Solving & CFD  34  November 6, 2015 07:30 
InterFoam Artificially High Velocities  andersson.j  OpenFOAM Running, Solving & CFD  0  February 8, 2011 11:43 
High depression at low alpha inlet (interFoam)  santiagomarquezd  OpenFOAM Running, Solving & CFD  0  June 1, 2010 17:18 
interFoam: strange pressure with high fluid viscosity?  ckroener  OpenFOAM  3  April 7, 2010 12:51 