Simulation of NREL UAE Phase VI turbine
 

Hi,

I'm trying to simulate the wind turbine in fluent using MRF. Basically, I'm tyring to recreate the whole experiment (wind tunnel included). However, the problem is that the torque produced on my simulation is about half that of the experiment. I'm not sure what could have gone wrong. I'm using a k- SST model with transition. My inlet is 3 diameters upstream while the outlet is 7 diameters downstream of the turbine. Are there any details I need to especially take note of to ensure an accurate simulation, or has anyone faced such a problem before?:confused:
Thanks in advance!

Hello,

I am working on the same project. I haven't got any torque values out but as soon as I do I will let you know.

Did you get good Cp's?

Thanks,
Fred

One more thing,

I remember reading this problem happening to other people. Maybe you should multiply the value by 2 since you have two blades.

Thanks for your help. While the values are around half of the experimental ones, I don't think it's a matter of multiplying by two, since the cm is about the axis of rotation, and my simulation is not periodic.

Once I've analysed the cp values I'll get back to you.

Well, I've analysed the cp distribution, and integrated the forces along the blade jut to ensure I've got the right torque, and the torque is still about half of what it should be. Checking the force coefficients, the normal force coefficient is much higher in my simulation, while the tangential force coefficient is much lower. I'm not sure what else I can do.

To anyone who reads this, I have changed the turbulence model to k-ω SST without transition to better match the wall y+ of the simulation (with transition requires a y+ of 1 and without requires a y+ of 30 to 300). However, the simulation results have not differed significantly. Inlet TI was 0.5% and viscosity was 10, to match the conditions of the NASA-Ames wind tunnel. outlet condition was outflow, and the wind tunnel walls are wall condition, to match the experiment.

I am now in the process of refining the mesh, to bring the y+ closer to 30. To reduce computational time, I'm cutting it down to half a rotor with periodic condition. If this works, I'll post here so that others having the same problem can try it out.

Hey what documentations have you been using for simulating the NREL? How did you determine the TI at the inlet?
What meshing software are you using?

Fred

I'm using Gambit to mesh (I just imported all the blade cross-sections based on the data given in the NREL UAE Phase VI document). I used the TI that's typical of the NASA-Ames wind tunnel. The TI was stated in http://www.nrel.gov/docs/fy01osti/29494.pdf.

I'm now running several different turbulence models besides k-ω SST to see if those work. The periodic simulations seem to converge faster.

Thanks for the info,

I had that PDF, I must have missed that bit.

I have been trying to remesh my mesh because I get problems when I switch to viscous solutions. I am using ICEM CFD. So far I have used a whole 360 domain but as soon as i can i will do a periodic simulation.

i also could not find the the atmosperic conditions. What are you using for the atm pressure?

Fred

Hey Fred,

I'm just using normal atmospheric pressure. I doubt that there was any specific pressure control in the wind tunnel, and the pressure will not matter that much since it's the gauge pressure that's important. Unfortunately, all the turbulence models came up with similarly inaccurate results. I'm now trying to refine my mesh around the blade, and hopefully not have too many cells. I have read literature that used 11m cells to successfully do a steady-state simulation, but this would require more juice than I have. http://yrc.utcb.ro/2010/p/YRC_2010_THCE_Razvan_Mahu.pdf

also, just to let you know, I've made a new mesh with a prismatic boundary layer. The y+ of the simulation is less than 5, so it will work well in k-ω SST with transitional flows. The results look slightly better, but still far off from experimental. I'm now attempting to incrementally increase the speed to 72rpm (run 100 iterations at incremental values of rpm), and see if it makes any difference at all.

Well, I've got zilch. If there's anyone who could help me, I'd really appreciate it.

Hey thanks for the papers,

how many elements have you got with the last mesh?

I have now been trying to improve my mesh before doing other simulations. What's the height of the first prismatic layer?

fred

my prismatic boundary layer is uniform (not aspect ratio based). The first height is 0.0000675. 20 layers, growth rate of 1.25. I think it's quite a good boundary layer. From studies I've done previously, it's about 3% of chord, so good enough to capture important features of the boundary layer.

my meshes are generally 2.5-3 million cells, with at least 2-2.5 million within the rotor zone alone (the cylindrical volume with the rotor within it). Most of these are concentrated around the rotor.

I have an inkling my usage of the dimensions of the NASA-Ames wind tunnel might be bamboozling the solver, as the sides are only 2-4 rotor diameters in length. Even with a transient, sliding mesh solver, the solution diverges (after about the same number of iterations as the steady state solution. Interesting?)

I have now changed the sides to a circular boundary, with a diameter of 5 rotor diameters. Also, I have changes the upstream and downstream (inlet and outlet) boundaries to 7 diameters from the centre. Let's see if these changes work. I'm attempting different combinations of BCs for the inlet, side and outlet, to see which gives the best result. I'll let you know.

also I cannot exceed by much more than 3m cells, as my computer won't be able to solve it. That's why I'm doing a periodic simulation, which means I have an equivalent of 6 million cells for a full rotor.

This is my setup I have been using now,

Periodic mesh with 4 radius upstream, 5 downstream and 3 on the side.

I am around 1 millionf of elements with 10 prismatic layers with the same parameters as yours.

I am using a single moving reference frame with k-w sst.

As you see in the pic I set inlet velocity, outlet outflow (1), far field as wall, blade as wall (zero velocity at the wall), symmetry for the semi cylinder in the middle and periodic for the two sides.

I first start with low rotational velocity as 1 rpm, then to 3, then to 7.54 at 7 m/s. So far, it has been converging. Before I was using symmetry for the farfield and could not converge and was also getting reversed flow and 'turbulent viscosity ratio limited to....'. So with farfield set as wall it got a lot better.

Now I have been looking at the cp's, but they are well off, they get up to 30-40......the simulatin has not converged properly yet, but I don't think it's going to change a lot. What could the problem be? Maybe the setup for the single moving reference frame or the mesh is not accurate enough...

You know when you setup the inlet velocity, do you leave zero for initial gauge pressure?

Hows are you doing with your problem with the torque?

Fred

Right.....just changed the outlet bc from outflow to pressure-outlet at 0 pa and the cp's are much much better. what turbulence specs did you use for this bc? I just left default, i.e. backflow turb kin energy 1 and backflow specific dissipation rate 1 as well. do you think it's ok.

So i was having a look at the torque, I put moment center 0 0 0 (my origin) and mom axis 0 1 0 (rotation axis is y), select moments and and the blade and get the following (see pic), is the circled valued the one I am looking for right?

Yes, that's the one you are looking for. But the value looks rather low, doesn't it?

Oh yeah it does. So that's the final value evethough I am using periodic?

For periodic you have to multiply by 2, since it will only compute the moment for one blade. Even then the value is low, no? At 7m/s the experimental torque is about 800Nm