Hi all

I would like some advice on which commercial cfd code is best for solving microfluidic problems using volume of fluid methods. What is your experiences? The applications are often water-like fluids filling capillaries.

Best regards Lars

I recently completed my PhD on surface tension driven flows in micro channels. I used CFD-ACE, which was a very nice package with good grid gen and post facilities, plus the fortran subroutines are fairly flexible. It even has dynamic contact angle models if you're feeling really brave, but they're empirical parametric as opposed to analytical, so you'll need to do some reading to make the most of them. Another package that is worth a look is Flow3D, but I choose ACE over that one because of the way the meshing works. I tested the usual suspects (PHOENICS, FLUENT, CFX, STAR), and found that for surface tension effects, they either did not provide the model, or it was unstable in an annoying way. Things may have improved since I last tried them (about 3 years ago now), although we've recently had some problems with CFX's VOF model (completely unrelated to MEMS, but still a problem). ACE's VOF model is compatible with particle tracking and isotropically diffusive scalars. Search for ESI-Software, or it might still be under CFDRC. Good luck, and keep your time-steps small.

Thanks for advice!

Did your calculations compare well to experimental results?

Define well. In terms of practical significance, yes the results where perfectly exceptable, but that is obviously going to vary from one application to the next. The problem with surface tension stuff (I'm asssuming you ST will be significant) is that surface defects in microchannels are quite big relative to the overall channel width. Also, surface cleanliness is UBER-IMPORTANT. The substrate surface energy can be completely changed from contaminants. All of this means that real life contact angles are very dynamic, but trying to model dynamic contact angles is a complete arse. The extra source of coupling between theta->U->theta means you need really small timesteps to get a stable solution. I had one set of simulations that took five weeks per simulation to run, and that was with static contact angles. If I'd have introduced dynamic contact angles, I would have need to take the timestep down by an order of magnitude, resulting in a 50 week run. Not good.

It might be interesting to know your application (whether surface tension is significant, what the driving force is, chemistry etc). Mine was all to do with immunoassays and laminar mixing.

One thing I forgot to mention about ACE is that it can't handle multiphase flow in porous media. For that, you'll need something like CFX.

Just courious. Did you get serious problems with parasitic flows in your calculations? Because the interfacial tension is so large in microscale flows. Or you just remedied this by choosing a very small time step? Thanks.

Pete

Sorry, I posted the message in wrong place.

Ahhhh, the joys of Flotsam & Jetsam generation and other annoying phenomena.

OK, let me tell you a story. I tried capturing the torodial vortex (Dussan AIChE 1977 23:131-133) and had a hell of time. I made these lovely butterfly grids and everything, but it just would not remain stable. Gave up in the end, and then it magically appeared in a completely different run where I wasn't trying to capture it. I put it down it the shape of the meniscus (it's convex and pressure driven in the Dussan example, but when I captured it it was concave and surface tension driven). I did however mention that the pressure field in the region of the meniscus was a bit blocky (which would be down to the surface tension algorithm), which would lead to "parasitic" currents.

Basically, there are a number of rules you can follow to avoid this sort of problem. KEEP YOUR GRID ORTHOGONAL!!! If you have to model the flow through a pillar array chamber (like I had to), you are going to end up with some serious skewness. Run this at your bog standard timestep, and you get Flotsam and Jetsam (F&J) everywhere. You can eleviate this problem by reducing the timestep, but as we all now, reduce the timestep by an order of magnitude, and you run time increases by an order of magnitude. DOH!!!

If all you want to do is model the capillary filling of a straight channel, then you're laughing. Even if the channel has a circular cross-section, you can get away with a butterfly mesh with F&J becoming a problem. In MEMS technology, it's a lot easier to make rectangular cross section channels than it is to make circular.

What you'll realise very quickly is that you're not going to model everything correctly (unless you have an uber-cluster). The CFD is going to be an aid to your understanding, but in the end you're going to have to do some serious analysis on your own. Remember, excel is you friend.

Thanks for great advice.

You're right about the surface tension part. The driving force is the surface tension although it might be relevant to do other applications later on (micropumps aso.) I guess I will have a look at ACE, but I can say for sure, that a 5 week run is way too much.

[majid_esi]

the latest ACE is quite good for microfluidics.. few issues that appeared earlier have been cleared off