Hello. I have been working
I have been working with OpenFOAM for nearly have a year, been posting and discussing in this board, but I'm still struggeling with a particular problem: the testcases about surface tension. Let me give you a summary.
Onno Ubbink gives a small overwiev of the problem in his Ph.D thesis (Chapter 5.3.5).
The setup is a "square" bubble in zero-gravity conditions, which should gain an equilibrium shape of a circle - induced by surface tension.
In the thesis there are some references to previous works, namly these:
- Brackbill (1992) - A continuum method for modelling surface tension
- Lafaurie (1994) - Modelling merging and fragmentation in multiphase flow with SURFER
I tried to simulate the two models described in the above publications and a third one from 2005: Vincent - Parasitic currents induced by surface tension (http://test.interface.free.fr/Case10.pdf)
Brackbill is dealing with an inviscid fluid. So there is no kinematic viscosity for both phases. Furthermore the bubble is initialized with circular shape already.
As I have experienced OpenFOAM (1.4.1) is not able to simulate this situation. Due to the absense of viscosity there is no damping between the both phases. The well known parasite currents are beginning to move the interface and even to move the bubble away from its initial position. Have a look at this video which is the result obtained with the values of Brackbill on a rather coarse mesh (30x30):
Lafaurie is computing with 'artificial' properties. He set all the applicable properties (density, viscosity, surface tension coefficient) equal to 1, which will not represent any natural combination of fluids.
The simulation is running, but the results obtained are rather 'slow' - I had to simulate at least 100 seconds to get round about 80% of the analytic pressure-jump inside the bubble.
Vincent is in between the both cases described above. He is using a real combination of water and glycerin. Due to the small values of the kinematic viscosity (~10^-6) the simulation is behaving like the case from Brackbill. The bubble is eventually moving away from its centered position.
So it looks like the simulation parameters from Lafaurie can produce satisfing results. At least at first glance.
In addition to compare the pressure inside the bubble with the results from the laplace-equation Lafaurie introduced a dimensionless constant which should be a characteristic value of the 'quality' of the surface tension model used in the calculations.
Its mainly a ratio between the applying surface tension coefficient, the viscosity and the magnitude of the parasite currents. The smaller the value of this number, the better the surface tension model.
Unfortunately the results obtained with the Lafaurie-properties yield to a dimensionless number in the magnitude of 10^-1. Lafaurie himself found the number of about 10^-2 15 years ago. Currents implementations result in 10^-5 to 10^-7, if you want to believe in Vincent.
So the results found with OpenFOAM yield to parasite currents which magnitudes are too high.
OpenFOAM is regarded as a very potential software - but can't deal with such a simple testcase?
So, I hope I made my point in what I'm struggeling with. I have discussed part of this problem in older threads, now you have a rather complete overwiev.
Anyone how mad the effort to read the whole text is welcome to let me know what he is thinking about this problem.
Any help is appreciated.
Thanks in advance.
Thanks to history posts of yours I came to know a lot about the interFoam solver, so now I'll try to do something back:
You have to be very careful with spurious currents; also with implementing a reduction factor, like 2phi(x)/(phi1+phi2), with the speed at 0; there are still some problems remaining, leading to velocity vectors.
It is strange that the square is moving in your case, since it should be axisymmetrical, so the sum of all velocities should cancel each other out.
If you read carefully through Brackbill, you might notice that another possibility is to model the surface tension as (in OpenFoam code):
At the moment I am reading
E. shirani et al./Journal of Computational Physics 203 (2005) 154-175.
Where a new interface pressure model is layed out (PLIC method) Once I though it out, I'll implemented it in the interFoam solver and discuss the results.
I am also working with interFoam. Recently, I tested interFoam with Brackbill case (which I made a post here http://www.cfd-online.com/Forums/ope...bill-work.html) and found there is a very strange result of curvature. If the correct curvature is K = 1/R, the computed curvature varies from +30K till -30K which is unbelievable for me.
Do you have an experience on that? Could you please comment on my test case?
|All times are GMT -4. The time now is 14:53.|