CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Problems with simulating an airfoil (http://www.cfd-online.com/Forums/star-ccm/94666-problems-simulating-airfoil.html)

 flo-b November 22, 2011 10:45

Problems with simulating an airfoil

Hi guys,

i have some major problems with simulating a wind turbine. The biggest problem is that i don't get the right torque. I found out that this is due to a wrong calculated lift coefficient.
That's why i tried to simulate an easy shaped blade and see if i can get the right coefficient at this one, but i failed too.
I am supposed to get a lift coefficient of 0.594 using Naca0012 at wind velocity 20 m/s and an angle of attack of 5 degree. My result is sadly about 0.22.

I put my blade (chord: 1m; width 2m) in an ashlar-formed domain (length: 10m; width: 3m; height: 4m) and meshed it with a trimmer getting a approx. 1.7 million cells. My front is a velocity-inlet with 20 m/s, my top, bottom and rear are pressure-outlets and my both sides have the symmetry-boundary-condition.

I'm using a steady-state case with segregated flow, constant density and the SST (Menter) K-Omega model (Gamma ReTheta treatment). I read some papers which used the same set up, so I think this should be appropriate.

I also read somewhere at this forum that I have to look at my boundary layer. Well, the thickness is 6mm and inhibits 12 layers. My y+ scalar field says that my blade is in the range of 0 to 1.98. The values above 1 are only near the very beginning of my blade and at the sides. I also know that there is a y+ wall distance estimation tool on this webpage. But my english is not my first language and so i totaly don't know what to do with this estimated wall distance (which I think is very important).

So, if anyone of you can improve my simulation, I'd be very grateful.

Greetings, Flo

 sail November 22, 2011 14:17

gamma re theta is not so easy to use. have you at least tried with the standar k-omega sst? the advantage of the transitional model should be more about the drag.

first of all, your domain looks a little bit small. i usually keep at least 30 cordlenght in front and on the top and bottom, and about 60 downstram of the blade to prevent that the imposed b-c infuences the solution.

also, i would reccomand checking the inlet turbulent quantities, to see if they are reasonable.

 abdul099 November 23, 2011 16:46

The mesh resolution is very bad. I got about 35 million cells for a 4.5m section of a glider wing, and that was just acceptable but not a perfect mesh (it was the maximum I was able to handle at this time).

When using a transition model, you need to resolve your boundary layer much better than you do. 12 prism layers are not enough for that. To get a good drag value, you should use about 20 to 25 prism layers and even more for a transition model. And as sail said, that has a bigger impact on the drag but not that much on the lift.

And most important: Your setup sucks! You compare two completely different values!
The lift coefficient of 0.594@5deg is the lift coefficient for a 2-dimensional flow around the airfoil. You would get this value with an infinite wing, or when you've got some large endplates.
In your case, your domain is 3m wide while the span of the "wing" is 2m. So you allow air to pass the wingtip, and it will do this! There will be air flowing from the pressure side around the tip to the suction side. This causes a vortex behind the wing (also known as wake turbulence) and significantly reduces lift (and increases drag). This is the reason why gliders or long-haul commercial planes have very long wings and short-haul planes are using winglets.
Especially when your setup is symmetrical, the largest distance of any point to the next wingtip is only 1m, therefore the flow is highly 3-dimensional.
Comparing values of this highly 3-dimensional flow to a 2-dimensional case is just crap. Either modify your domain and don't allow any air to pass the wingtip, or compare it to experimental data gained with the same setup. And when you decide to go the first way and modify your domain, I recommend to use a shorter section with a span of just a few inches. That will save a lot of cells and allow you to resolve your boundary layer much better without increasing computational effort too much.

 flo-b November 24, 2011 08:39

Hi guys.
First of all, like abdul099 mentioned, the major problem was the downwash of the blade. Yesterday, I changed the width of my domain ending in the same size of my blade section. This resulted in a lift coefficient of about 0.543. Afterwards, like sail proposed, I increased the length of my domain to 100m and the height to 60m. This gave my a result of about 0.531.

@sail: On my wind turbine I didn't try the standard k-omega model. Instead, I formerly used Spalart-Allmaras and the standard k-epsilon model of star-ccm+. The results didn't change much. For my turbulent conditions, I only changed the turbulent intensity to 0.001. Do you have any suggestions for my viscosity ratio? I only know that my intensity is ought to be low.

@abdul099: I read about some wind turbine simulations calculating the model with approx. 2.0 million mesh. The results aren't that bad. So I thought using an 1.7 million mesh should be enough for an easy shaped blade profile. But yes, as you wrote my setup wasn't really good. I changed it as mentioned above. I still have a difference of about 10%. I'll try some more layers and a higher mesh. Do you think this will eliminate my 10% difference?

Thanks for the answers, does anyone have some tips for simulating a whole turbine reliable?

 All times are GMT -4. The time now is 22:18.