[japanese student]

hi

i`m very glad to you if you answer the question.

when i read some articles,i knew about mesh.

to simulate mass transfer from gas to liquid(high schmidt number), we have to refine mesh near the interface.

why do we have to refine mesh?

thanks

[t.teschner]

just imagine what the flow is doing at the interface. you would expect some kind of mixing mechanism present at the interface, so the simplest form would be probably a shear layer, like a jet. at the interface you have increased activities which, physically speaking, are represented by high gradients.
in order to resolve the gradients properly you need to have a fine mesh (ideally also a higher order scheme). so thing of a jet entering a fluid at rest (away from the wall) for example, at the interface your velocity gradient will be higher than everywhere else.

a more mathematical description is that the schmidt number determines your smallest scales locally. you have high velocity gradient and therefore high fluctuations. the dissipation is calculated as epsilon = nu*{du_i/dx_j * du_j/dx_i} where u_i, u_j are the fluctuating velocity components and {} is used to express a mean. hence you would expect a high dissipation near the interface. the kolmogorov scale is calculated as eta = (nu^3 / epsilon)^0.25 ... therefore, the kolmogorov scale scales with one over epsilon, hence, a high value of dissipation means small, local kolmogorov scale. now if you consider the schmidt number than you can use the batchelor scale (or rather you should) which is defined as eta_B = Sc^(-0.5)*eta(x,t). that again tells you that a high schmidt number will further reduce the smallest scale present in your domain.

the last paragraph only needs to be of a concern to you if you are actually doing a DNS, if you are looking at RANS models, than just think about the gradients.

[japanese student]

thank you for your reply!
You've been very helpful.

i understood that i have to refine mesh near the interface in order to resolve the gradients properly.


my teacher who is not a proffesional in numerical simulation teached me that the calculation will diverge if i don`t use fine mesh for high schmidt number.

is it true? why?

if i you answer the question, i`ll be very glad to you.

thanks!

[t.teschner]

if CFD were only that easy ... i am not familiar with the specifics of high schmidt number flows but I would assume that the mechanism present at higher schmidt numbers are acting on such small scales that without mesh refinement the flow would see an extremely coarse mesh. hence, mesh refinement is one thing you should do but also thing about using higher order schemes. they improve accuracy but need a fine enough mesh on the other side to actually see the flow features. not sure if that is answering your question completely, but let me know if you have still some concerns

[cfdivan]

Hi yusuke,

As already pointed out, CFD might be more complicated than that. Trying to find an silver bullet that explains the divergence of simulation is impossible, IMHO. For flows where the mixing process is the king, you real need a very fine mesh in that region (mixing process), not because of the divergence of your solution but of the accuracy. I would say that the turbulence model is one of the most critical topics on this type of flows/simulations. If you consider, for example, combustion problems you may need to simulate length scales that could be pretty close to the kolgomorov scales, which means high mesh resolution. It is strictly related with the scales at which the process happens.

For sure that the mesh is critical, but the most critical I think is the numerical part of the problem, I mean, the discretization schemes. I would suggest to start with a coarse mesh with discretization schemes of 1st order and refine it step by step. Seed the fine simulation with the results of the coarse run...it will help you out to avoid high divergence/instabilities as soon as you refine. You can also try high order schemes. Bear in mind that high order schemes does not mean high accuracy sometimes.

Try to explore a bit more the numerical methods for PDE and fluid dynamics. It may help you a lot.

Regards,

[japanese student]

thank you so much for your reply.

your advice will help me to do my project.



i`m deeply grateful to you(t.teschner,cfdivan)!