Equilibrium thru Interface
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.
Do you have a partitioning relationship between the concentration in both side of the interface ?
Something like :
If it is the case, you can add a transport equation in interFoam solver using the theory of distributions (see Haroun (2012) for exemple)). The concentration jump will be considered as an additional term in your transport equation.
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 .
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.
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++??
Moreover my low C++ knowledge prevents me for finding an alternative formulation.
Do you have any hint?
|All times are GMT -4. The time now is 21:36.|