- **OpenFOAM Running, Solving & CFD**
(*https://www.cfd-online.com/Forums/openfoam-solving/*)

- - **Equilibrium thru Interface**
(*https://www.cfd-online.com/Forums/openfoam-solving/109477-equilibrium-thru-interface.html*)

Equilibrium thru Interface1 Attachment(s)
Hi Foamers!
I'm having a little bit of trouble trying to remake the work done at the work of Waheed et al (2002) (http://www.sciencedirect.com/science...17931002001242), where some axissymetric wedge section of a drop inside a cilinder is taken, this drop containing solute, and the outer phase is solute-free. So, essencially I want to computate the solute transfer. The main problem is that i need to establish a equilibrium of the solute concentration inside and outside the drop, what I believe I could do by phisically stablishing a interface boundary in my domain and using groovyBC to ser the dragient expression. So, essencially, my domain would consist of 2 regions: the drop and the outer phase. By now, the mesh construction is OK, and I could stablish this phisical boundary and the paraFoam recognizes it. But running my case in my own implementation of interfoam (interfoam + solute transport), i noticed that the interface bondary (so called defaultFaces) is not needed. In fact, I can remove it from the boundary listed in the 0 directory with no problem! That's not right, my solver just ignores my equilibrium condition. What should I do? My master depends on this series of simulation :eek: I'm attaching my case files. Thanks in advance, I hope someone out there could help me. PS: In order to save space, after download and extraction please run blockMesh. |

I think you need two domains with non-identical vertices, which you then couple using some sort of a baffle boundary condition. Have a look at the tutorials for chtMultiRegionFoam, where this is done for the temperature equation.
- Anton |

Dear Cyp and Anton,
Thanks for the fast reply. I will check your suggetions, thanks in advance. And yes Cyp, i have a partitioning condition like the one you showed. But how could I implement this on the solver to consider this jump only thru the interface boundary? I will check the reference you suggested. |

I can explain it to you through a simple example. Consider only the diffusion between two phases (beta and gamma for instance) :
In the beta-phase you have and in the gamma-phase Both phases are connected through a flux continuity at the interface and the thermodynamic equilibrium condition reads: What you look for is an partial differential equation that govern where is the phase indicator provided from the VOF solution. With such a formulation, C is defined on the whole domain. In the same manner, you can defined a diffusion field as Now you express the derivative of C : multiplying this relation by D and applying the divergence operator, you get : Just keep in mind that according to the distribution theory you have : . Consequently, the previous equation reduces to: This additional term represents the interfacial jump condition. If there is a continuity, you can get rid of it. However, if you have a partitioning relation, you have to consider it. At the interface, we have . Consequently, more over, So So your diffusion equation becomes : With such a formulation, you will automaticly have a jump condition at the interface between beta and gamma. You can also optimised the solution with I let you adapt this exemple to the advection-diffusion equation. Best regards, Cyp |

Quote:
I don't actually know if you are still following this tread but I have a couple of questions. It came for me too the time to implement the phase jump condition so I came back to this useful thread. In my previous case (a non-volatile tracer) I just had the Laplacian of a bunch of constants and alpha1: no problem in the solution if you insert the explicit laplacian (alpha1 already calculated). But in this case it is different because we have C an alpha1 simultaneously in the laplacian. For what I can see in the other terms OpenFOAM always expects in the laplacian a dimensionedScalar and a volScalarField. So, I gathered all the constant terms in the fraction and calculated them before the C equation: Being this a function of alpha1 I had to define it in the Createfields.H as another volScalarField. Again, no problem. What I actually cannot understand is: how do I formulate this in C++?? should become Code:
`fvm::laplacian(DC, C)` Moreover my low C++ knowledge prevents me for finding an alternative formulation. Do you have any hint? Thanks! |

Quote:
Kind Regards Rimsha |

@Article{Haroun2010,
Title = {Volume of fluid method for interfacial reactive mass transfer: Application to stable liquid film }, Author = {Y. Haroun and D. Legendre and L. Raynal}, Journal = {Chemical Engineering Science }, Year = {2010}, Number = {10}, Pages = {2896 - 2909}, Volume = {65}, Abstract = {A volume of fluid method is developed in order to simulate reactive mass transfer in two-phase flows and is applied to study reactive laminar liquid film. The thermodynamic equilibrium of chemical species at the interface is considered using Henry's law. The chemical species concentration equation is solved using primitive variables and local fluxes are locally directly calculated at the interface. The present treatment of jump discontinuity of chemical concentration is consistent with a volume of fluid approach and the difficulty to calculate accurate local mass flux across interface is overcome. For plane interface, the precision of the numerical simulation is found to be very satisfactory while for curved interface a special procedure has been developed to reduce the development of spurious fluxes at the interface. The algorithm is validated for different cases by comparison with available solutions. The method is then applied to study non-reactive and reactive mass transfer in a falling liquid film. The results show that the liquid side mass transfer is well predicted by the Higbie (1935) theory when the transfer is controlled by the film advection provided that adequate parameters are considered, i.e. the actual velocity at interface and not the average liquid film velocity. For situations controlled by diffusion, the Sherwood number tends to a constant value characteristic of purely diffusive situations. For the reactive mass transfer, first and second order irreversible chemical reactions in the liquid phase are considered. The numerical results are compared respectively, with Danckwerts (1970) and Brian et al. (1961) solutions and good agreement is observed. The proposed Volume of Fluid method is shown to be well adapted to deal with interfacial reactive mass transfer problems. }, DOI = {http://dx.doi.org/10.1016/j.ces.2010.01.012}, File = {Haroun2010.pdf:ARTICLES/Haroun2010.pdf:PDF}, ISSN = {0009-2509}, Keywords = {\{CFD\}}, URL = {http://www.sciencedirect.com/science/article/pii/S0009250910000291} } Cheers, |

Quote:
Rimsha |

Note that although it was ages ago there is a mistake in the derivation done by Cyp:
is wrong, it should be leading to the result of which, by the way, describes the view from "the other phase" compared to Haroun, who ends up at which would be equal to assuming (which in fact is just ). Note that Cyps answer was a mixup of both solutions of nominator and denominator. Edit: Thanks anyway Cyp, this was generally a great help. And while at it, has anyone here managed to reproduce the calculations in the paper with OpenFOAM? I kind of struggle with different Henry coefficients (some work, some produce an exception). |

3 Attachment(s)
Finally my solver works now the way it was supposed to be. For anyone who cares I will attach my modified solver as well as two testcases. All modifications were made by made, but based on the publication by Haroun et al (2010), cited above, as well as Nieves-Remacha et al (2015):
The Attachements: interHarounFoam:This is the solver. it is a modified version of interFoam, implementing both Equations found in Nieves-Remacha (2015), Supplemental. This means it implements as well the Haroun approach, as an approach by Marshall et al. (2012). It is merely for testing purpose, the diffusion coefficients are fixed to in the createFields.H, and the fields used are named H (for NievesRemacha2015:This is a sample case for the first example in the supplemental by Nieves-Remacha et al. It contains all relevant data to run interHarounFoam and generate one set of the results. Haroun2010:A sample case to reproduce the example shown in Figure 1 a/b of Haroun et al. (2010). This case can be run as it is, too.A couple of further notes: - Both sample cases contain a visual.pvsm, which can be loaded in paraview (either using File > Load State) or starting paraview with the parameter --state=visual.pvsm.
You will have to fix the path to your case, though. - Since diffusion coefficients and Herny coefficient are fixed in the solver, you will need to modify the createFields.H and re-compile the solver every time you want to try other values. Sorry about that. I am working on a library, which does the same thing, only better, which I intend to "publish" here soon.
- In the fvSchemes make sure to use a
*Gauss linear*scheme (or*Gauss cubic*, for what it matters) to solve div(phi,C). Most other schemes will fail, somewhere between extremely wrong results to crashing the solver. - Nieves-Remacha implement both equations as balances using the cellSurface (surfaceScalarField phiC), calculating first phiC ~ snGrad(alpha) and then div(phiC). Mathematically, the same could be achieved by having a laplacian(c, alpha) (something like that). Here OF allows to use a volScalarField c, which can also be created based on Harouns equation. However, this doesn't work either. I couldn't be bothered with the numerics or maybe even a simpler, mathematical reason for this, but you might care about this if you ever want to implement it on your own. Took me some days..
May the foam be with you, Timm |

All times are GMT -4. The time now is 19:50. |