I am using CFD with mass transfer to investigate a 2-D internal flow that is laminar but has some recirculation zones. I'm looking at the convection and diffusion of a trace component that has a very low diffusivity in the mixture. The Schmidt number (analogous to the Prandtl number in heat transfer) is about 700 for this component. The surface mass transfer coefficients continue to decrease as I refine the grid, and there appears to be no end in sight. What are the special tricks to modeling high Sc (Pr) flows?

(1). I don't have any idea about what you are trying to do. And I don't have time to figure out your problem. (2). But I think you are talking about three things,: one is the high Schmidt number ( similar to Pr) =700 for that component, the other is the mesh refinement, and the last is the decreasing surface mass transfer coefficients. (3). I think, before you start the computation, you need to define your problem first. Then size your computational domain. Then estimate your final flow field distributions, before creating your mesh. (4). What I am saying is, you need to identify the areas such as the boundary layer first so that you can arrange your mesh to properly capture the solution and the wall properties. You have to know something about your flow field before attempting the mesh generation. Sorry, I can only give you this very general hint.

Hi,

I think;

For problems involving very small diffusivity hence negligible diffusion, numerical (false) diffusion can be much larger than physical diffusion. The numerical solutions then are much more sensitive to mesh and discretization scheme you use. Perhaps that's why the solutions keep changing as you refine the mesh.

Dear Jon Johnson

I had nearly similar situation more than ten years ago. My problem was so called double diffusive natural convection with Pr=7.0 and Sc=700. Reminding my old experience, there was no trick except concentrating grid in the boundary layer. Only what I could was to increase grid number and to use supercomputer. It was crazying computation for 2D unsteady problem.

Following is for your reference for laminar natural convection in the cavity. Ratio of thermal and solutal(mass) boundary layer is, approximately,

delta thermal / delta solutal = [(Ras/Rat)*(Sc/Pr)]**(0.25)

Rat : thermal Rayleigh number, Ras : solutal(mass) Rayleigh number

Considering, in general, Ras is much larger than Rat, mass boundary layer is very very thin. For forced convection, I can not remember exactly but mass boundary layer is more thin, maybe, power of 0.5 rather than 0.25(not clear value).

Sincerely, Jinwook

Hi, Jon,

I believe I understand this problem quite well, since I have been working on related problems for many years (may be, 20 years? Cannot even remember).

And your question is relevant to a lot of staff which really should be clearly understood by all who work on steady small-diffusion-term problems, like, say, high-Re steady flows.

First, this problem can be solved by asymptotic methods, assuming Sc tending to infinity. Quite probably, you can obtain the result relatively easy, from a computational viewpoint, but the background theory is complicated. If you are interested in this approach, contact me by e-mail: sergei@chernyshenko.dnntm.rssi.ru or chernysh@ma.man.ac.uk, and we will discuss what can be done and how you could use, for example, some of my results.

Without asymptotic methods, this is very tricky indeed. The reason is that you have the recirculating region. Diffusion effects in it are of order 1/Sc, unlike the boundary layer where they are 1/sqrt(Sc) >> 1/Sc. However, this weak diffusivity affects the result by on order of unity. Sure, all this is explained by asymptotic theory. Practical consequences for pure numerical approach are quite serious. In a similar problems the following behaviour was anticipated and was partially (too long to explain why partially) demonstrated by numerical experiments.

Suppose, you choose a particular mesh structure and start to perform calculations on a sequence of more and more fine meshes. Eventually, the solution ceases to change, and you believe you have a grid-independent solution. If, then, you create a mesh of different structure, and do the same, you obtain again what seems to be a grid-independent solution but it turns out to be different from the first one! Really, if you continue to refine the mesh, both solutions eventually start to change again, and on a very fine mesh they will be the same. But the probability of obtaining a wrong answer is high. The reason for this behaviour is simple. If you neglect the diffusion term completely, then all that the equations tell you is that the concentration of the admixture is constant along streamlines. It is all right for streamlines crossing the boundary since you can determine the concentration on them from the boundary conditions. For closed streamlines, however, the admixture distribution over streamlines is determined by the diffusion, HOWEVER SMALL IT IS! In a numerical simulation, you have a numerical error. Let, for simplicity, assume that you are using first-order upstream differencing for convective terms. Then this numerical error can be more or less described as an effect of some additional diffusivity, which is then characterised by its own Schmidt number, say, Sc_num. This numerical diffusivity will then compete with the physical diffusivity. If, for example, your Sc_num is about 70 and Sc is 700, then the numerical diffusivity will determine the concentration on closed streamlines. On the other hand, 1/Sc_num is a measure of numerical error, and if you are satisfied with, say, 2% accuracy, you would conclude that you obtained a grid-independent result. Note now, that numerical diffusivity differs from phisical one not only in magnitude but also in structure: physical diffusion coefficient is a constant scalar while numerical one is a tensor with spatial variation. This is why the solution seems to be independent of the grid step but still depends on the grid structure. Only when you refine you grid so that Sc_Num >> Sc, you can expect to obtain the correct result. This, however, may indeed require a supercomputer.

It might be, of course, that your difficulties are due to something less subtle, but it is hard to tell without looking further into the details. Well, indeed, you may contact me by e-mail, I do not mind. It might be even interesting for me. Anyway, hope this can help you.

Yours Sergei

Jon and Jin, sorry, I posted an answer in a wrong bracnh, it was meant for Jon.

Sergei