Water turbine drag calculation
 

Hi everybody,
I'm doing an analysis on an axial water turbine, similar to the one that you can see in the attached picture. I set the simulation using CFX and the results are good compared to the experimental tests I've done on this turbine.

Now I'm trying to make a good analytical model to predict the negative torque caused by the rotation of the three hubs in calm water. The water flows only in the turbine channel, whereas it is calm in the hub's region.

The hubs are NACA 0012 at 0 deg angle of attack. The drag coefficient Cd is approximately 0.008 (extracted from Xfoil), the density of the water is around 1000 kg/m3 and the turbine's speed is 1750 rpm.
From the formula D=0.5*rho*S*(ω*r)^2*Cd , I obtain a really small drag force (and small torque obviously) compared to the one obtained from the simulation (0.15 Nm in theory, 8 Nm in CFX). Is there something wrong in the simulation or the analytical approach is wrong somehow?

Thanks!

The theoretical approach you are using assumes the airfoil is moving through still fluid in a far field. The hub of the device will have neither still fluid nor a far field.

But there is also the general question of CFD accuracy - have a look at this FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

First of all, thanks for your answer.
I thought that the different results could have been given by accuracy problems, but the difference between analytical results and CFD results are too big (0.15 Nm vs 8 Nm).. do you think that this difference is compatible with accuracy problem?

A seriously inaccurate simulation will produce seriously inaccurate results.

But also inappropriate application of empirical results will also be misleading - as I said, I don't think your use of free field airfoil drag coefficients is appropriate. Your "theoretical" calculation is likely to be very inaccurate as well.

I assume you're taking the frozen rotor approach? That's good to get the simulation going. For highly accurate simulations of a rotor and stator you should then continue the simulation using a sliding mesh approach. I.e.

1. Perform a steady frozen rotor simulation and stop when your monitored values do not change (torque, velocity etc.,)
2. Continue from point 1 using sliding mesh (simulating one revolution should be enough)

Also beware: CFX computes torque relative to a local coordinate system. If your geometry is not centered at (0, 0, 0) then you need to create a new coordinate system which has its origin on the axis of rotation. Also please note new coordinate systems created in CFX Pre aren't passed on CFD Post.

As part of my job I simulate a large number of mix tanks driven by rotor stators; I get better results using the EARSM and RSM turbulence models over the standard SST turbulence model.