Modelling falling solid sphere using interFoam VOF model
1 Attachment(s)
Dear Foamers,
I have been trying to model a falling perspex sphere in water using interFoam. I figured that choosing a large surface tension and dynamic viscosity would allow to represent the perspex sphere by the second liquid phase: the high surface tension should ensure a spherical shape and the high dynamic viscosity should prevent internal fluid circulations in the sphere. With my first attemp I find that the terminal falling velocity is way too small compared to what I expect. I assume a 3 mm sphere (density 2200 kg/m3) in water (1000 kg/m3), hence I expect to find a velocity of about 0.33 m/s However, I find a velocity of about 1 mm/s, which is an order 100 too small. Please find attached a view on the velocity field and pressure distribution over the particle (bubble). My quesions are: 1) Is it in priciple allowed to use VOF for falling object such as small particles? 2) Has anybody simulated solid spheres with VOF ? 3) Could anybody comment on my numerical settings? My impression is that the difficulty is the large pressure inside of the bubble due to the 2*sigma/R bubble pressure. I have choosen sigma as small as possible (0.1 N/m) in order to keep the internal bubble pressure as low as possible. Nevertheless, for R=3 mm this would still lead to a P=2*0.1/3e-3=67 N/m. The hydrostatic pressure over the bubble (which takes care of the buyancy force) is 30 Pa. The pressure I find in the bubble is actually higher than anticipated: about 400 Pa. Perhaps the large pressure drop over the bubble interface give problems ? Well, anyway, in case anybody can say anything sensible about it. Please let me know. I will include a summary of my numerical and physical settings below. Some remarks: I have already varried some things. I checked a different gradScheme interpolation (see fvSchemes): cellMDLimited insteat of Gauss lnear. I have varied the resolution already. This mesh already uses 0.5 mlj cells. The grid was made with blockMesh and some grid refinement in the bubble areay with snappyHexMesh. Also I have tried a large surface tenstion (1 N/m), but none of it leads to a higher falling velocity Well. That's it. Any suggestions appreciated! Regards Eelco constant/transportProperties Code:
Code:
top Code:
boundaryField Code:
boundaryField Code:
application interFoam; Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
hello,
You should try with a smaller viscosity ratio, 1e6 is too much and may give youstrong parasitic current/numerical artefacts ... so try a a viscosity ratio of 1e3. (i.e nu2 ~1e-3) regards, olivier |
viscosity dependence
2 Attachment(s)
Hi Olivier
Thanks for the remark. It indeed appears that the ratio nu_fluid/nu_bubble was choosen too large. I have run a few cases with varying bubble viscosity. Ideally the bubble viscosity is as large as possible (to mimic a solid sphere). For lower viscosities you can anticipate a different drag coefficient of the bubble, given by Cd=(16/Re)*((1+(3mu_p)/(2*mu_f))/(1+mu_p/mu_f)) (analytical solution for Rep<1 by Hadammard,1911) For mu_p<<mu_f this give Cd=16/Re (stokes flow of gas bubble) and for mu_p>>mu_f this gives Cd=24/Re (stokes flow for particle). Clearly, I am not in Stokes regime, nevertheless, if I use this relation I would say that for my choise of nu_p=1e-3 m2/s -> mu_p=rho*nu_p=2.2 Pa s I am in the limit of spherical particles as Cd -> 24/Re. Well, I run a few values of nu_p; attached the graph of the position X_p and velocity U_p of each value, incl the analytical solution for a true spherical particle. As you can see, now indeed I am in the right ball park. My previous value of nu_p (of 0.01 m2/s) gave way too low terminal falling speed, but as soon you go below 2e-3 m2/s for the kinematic viscity (i.e. take nu_p/nu_f < 1000), the terminal rising speed is reasonably well predicted. My only concern now is that the terminal falling velocity is very sensitive to the exact choise of nu_p, whereas the values taken should all be in the limit that Cd-> 24/Re, hence still lead to the same terminal falling velocity. Perhaps this is due to differences in the deformation of the sphere. I will check the influence of the surface tension. But anybody with further suggestions: any comments appreciated:-) Regards Eelco |
Quote:
Quote:
by the way, you sphere is so small, have you ever tried a larger diameter? such as 1cm steel ball? |
Hi Eelco,
There is a group in Sweden performing quite a lot of simulations on settling of solid particles using VOF. Here is one of their paper: A novelmultiphase DNS approach for handling solid particles in a rarefied gas H. Ströma, b, http://cdn.els-cdn.com/sd/entities/REcor.gif, http://cdn.els-cdn.com/sd/entities/REemail.gif, S. Sasicc, http://cdn.els-cdn.com/sd/entities/REemail.gif, B. Anderssona, b, http://cdn.els-cdn.com/sd/entities/REemail.gif http://dx.doi.org/10.1016/j.ijmultip...ow.2011.03.011 Cheers, Duong |
Hey Eelcov,
You mention you perform a grid refinement in the region close to the bubble with snapphyHexMesh. How exactly are you doing this? Thanks! Edit: more infor can be found : http://www.cfd-online.com/Forums/ope...plet-fall.html |
Modelling A solid particle dropping into a Tank
Hello ever one,
Could you please let me know how I can model a solid drop into a tank? Which solver do you recommend? I have three phase of solid gas and liquid. Interfoam works? what about VOF? |
All times are GMT -4. The time now is 23:45. |