[rekap]

Hello,

I am using the interMixingFoam solver for a tri-phase case. From the User Guide, I know that interMixingFoam : "Solver for 3 incompressible fluids, two of which are miscible, using a VOF method to capture the interface".

Alpha1 is the immiscible fluid while alpha2 and alpha3 are the miscible fluids.

The simulation run well but in post-processing I see that alpha1 and alpha2 mix which it should not happen.

Does anyone know why?

[dzordz]

There is a mistake in the code and it only has to do with one command line being executed too late in the loop (it took me way too long to figure this one out )

The way it works is in alphaEqns.H you have a for loop which does following things:

for loop:

1. create the complete convective flux for alpha 1
2. create the bounded (upwind) flux for alpha 1
3. calculate the flux correction for alpha 1
4. calculate the limiter for alpha 1 [this calculates lambda coefficients]
5. create the complete convective flux for alpha 2
6. create the bounded (upwind) flux for alpha 2
7. calculate the flux correction for alpha 2
8. calculate the limiter for alpha 2 [this calculates lambda coefficients]
9. construct the limited flux for alpha 1
10. construct the limited flux for alpha 2

...

Now as you can see the step 9 should be earlier, between steps 4 and 5. The reason is step 4 calculated you coefficients for bounding your phase 1, but those are not actually used for construction of the limited flux of phase 1 and are overwritten by coefficients calculated for bounding of phase 2 (step 8). In a sense you are using the same lambdas for construction of both fluxes, which is incorrect.

Correct the mistake, recompile and you should be fine.

P.S. also the tolerance for alphas in fvSolutions should be smaller then in tutorial (at least for my case)


This solves the problem of mixing of phases 1 and 2, but I also think there is a problem with the way diffusion is written into the program, because I keep getting the same result no matter what diffusion constant I use. Still trying to figure that one out.


Hope it still helps

[MrFyzzix]

Originally Posted by dzordz

..., but I also think there is a problem with the way diffusion is written into the program, because I keep getting the same result no matter what diffusion constant I use. Still trying to figure that one out.

Any updates on this? Does it have to do with numerical diffusion?