Learning Forum

[ucla278924569]

[Karthik Remella]

Hello,nThese are two different ways of modeling surface tension force at the interface of the two fluids. Having said that, they are completely different mathematical formulations. On one hand this force is modeled as a volumetric source term in the momentum equation and in the other, the surface tension force is modeled as a surface stress tensor. nThe results you obtain also will depend on the type of grid you use. nI'd say this - if CSF works for you and you are satisfied by the results, I'd say continue using the CSF formulation.nIf you have not looked into the theory guide on the mathematical formulation: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v202/en/flu_th/flu_th_vof_surf_tens.htmlnThanks.nKarthikn

[ucla278924569]

Thank you, Kremell. nFor my first picture, I didn't use either one model. When I use either CSS or CSF, the parasitic current always exist and the water penetrate the interface and get into the air region. However, when I only set up a constant surface tension without these models, it works well. Thus, I wonder if it is necessary to enable one of the model to say modelling the surface tension. The guide seems to say that it is necessary so i am confused.nAlso, is what you mean the type of gird the shape of the mesh cell?.BestnJianhuan

[Karthik Remella]

Hello,nModeling surface tension or not depends on the problem you are trying to model. If you are modeling a capillary flow, then surface tension is extremely important. However, if the flow you are modeling is very macroscopic and the surface tension does not feature in your flow, you don't really need to model.nHaving said that, what are the dimensions of your problem? Can you please post a screenshot of your computational mesh? Also, are you converging every single time-step? What is the Courant number when you run the simulation (each time-step)?nThanks.nKarthik

[ucla278924569]

Thank you so much, KarthiknHere is my dimension and how I set it up. Water initially fill up the upper part and air is in the groove. Without the CSS or CSF, it converges (1e-3) very well. After a few time step, It takes just around 5 trails then converges. The Courant number is around 0.9 and seems decreases slowly.nnWith CSF, the Courant number is like around 90. It takes much longer to converge.nnI just tried to set the surface tension coefficient to be none. And I run it for the same time, then I got a similar result (not sure if the same). nI am confused how the interface sustains if no surface tension is modeled.nBestnJianhuan

[Karthik Remella]

Hello,nCan you please try and reduce the time-step in your CSF simulation? This would reduce your Courant number in the simultion.nPlease let me know if this works.nThanks.nKarthikn

[ucla278924569]

Time step was 1e-6 and i ran the calculation for 20 steps (2e-5 s). I changed to 1e-8 and then run it for ~1700 steps (1.7e-5 s). Volume fraction, stream function and velocity vector are shown below.nThe weird current did not happen on the interface so far, but the velocity field near the interface is quite strange and velocity there is quite big compared to the case without CSF.Thanks for your help, KarthiknBestnJianhuann

[Karthik Remella]

These are spurious parasitic currents and are quite common in VoF models. One way is to reduce these currents is to reduce the time-step. There are of course other ways of reducing these. I'd strongly recommend looking them up in the literature if you wish to learn more. nI hope this helps.nThanks.nKarthikn

[Amine Ben Hadj Ali]

What you can do apart from reducing time step is to use Viscous Dissipation (look for that under beta feature). It might (only might not should) as parasitic currents will always be there: in 2D more than in 3D. Based on qucik estimation your time step size cannot be larger than 1e-8[s] even lower.n