[Spacegirl1923]

Hello community! I have been struggling with confidence on some analysis I preformed on an airfoil to be used on an underwater turbine.

A fellow grad student is working the more dynamic motion aspects of the project and I am supporting on the CFD side. He has determined that a particular section of the blade is experiencing a RE of 50,000. Of course wanting to adhere to similarity I have ran my simulations at Re = 50,000 (my airfoil has a chord of 1.0 and I am running 2D analysis in FUN3D, compressible RANS with turbulence defaulted to SA) and then I realized that the Prandlt number defaults to 0.72 (air) and that I believe the Prandtl number for water is 6.99 (roughly depending on temp) trying to ensure I've dotted all my i's and crossed all my t's I reran some angles of attack I get vastly different results. This is also my first time dabbling in hydrodynamics, so I'm wondering what I've missed. I always thought that if you matched RE you could have the same flow results, and I thought Prandtl was more for thermal diffusivity...

[adrin]

The Prandtl number affects your density (and hence pressure variation), so it does have at least an indirect impact. Running a compressible flow code for purely incompressible flow problems is not a very good idea because, I'm assuming, the code uses ideal gas law (or something similar) to couple pressure-temperature-density, whereas this relationship is not valid for liquids (you could theoretically replace the ideal gas law with a more relevant formulation, but, then, I'm not sure how that would affect convergence). Also, depending on how robustly incompressibility is included in the code you may not get a converged solution (or convergence to a correct solution) with a compressible flow code! I had a similar experience a few years ago using a famous compressible flow code, where all the convergence indicators seem to suggest convergence, but the solution was basically garbage! I would strongly suggest that you either use an incompressible flow code (unless you're interested in cavitation), or modify your compressible flow code properly to account for the correct physics (and numerics)

adrin

[Spacegirl1923]

Yes thank you. After posting and not getting an immediate response lol I started looking at the derivation of the non-dimensional equations and realized Pr is there, so obviously the solution will be different not to mention the issues with the equation of state not being valid....duh!!! Live and learn. Thanks for confirming this!!

So for airfoil data for the underwater turbine I can't just grab something off of an airfoil data base then. I would need to run everything for the proper fluid properties. Does Reynolds dynamic similarity even hold between different fluids like air and water?

Once again thank you!!

[adrin]

You can still use air data for water flows, so long as at least the Mach number is very low (clearly, not just barely, in the incompressible flow regime). I would recommend the following:

1) Make sure the data you use for benchmarking is well-respected and referenced by the community at large. Many researchers do not question experimental data, thinking that *that* is the real thing and that CFD is the one that needs validating. This is a misnomer, to say the least. Good experimental data is far more difficult to provide than good CFD results. I have, in fact, demonstrated on quite a few occasions that the data, not CFD results, are wrong (sometimes the research and/or reporting is so sloppy the data fails a basic conservation of mass "smell test").

2) Validate your code and mesh convergence using the physical conditions under which the experiment was conducted. This is your first cut at removing the doubt whether the discrepancies are due to CFD simulation errors or due to the fact that you have water instead of air.

3) Modify your physical properties in small incremental steps and at each step verify that there still is a "good" match with the data. If you see a monotonic change in your benchmark accuracy then you know it's related to the differences in physics.

4) If the differences are indeed large then you need to modify your model (use an equivalent equation of state for water) and repeat everything. Your code may or may not be able to handle these changes

Alternatively, just use a fully incompressible flow code. What is the Reynolds number of your problem and do you need 3-D runs or would 2-D codes suffice, at least initially?

adrin