Horizontal Axis Wind Turbine
I am doing CFD simulation of Horizontal axis wind turbine by using Fluent.
Rotor dia = 6 m Rotational speed = 20 rad/sec Air velocity = 10 m/s I am solving only one blade and using periodic boundary condition. I am using Single Rotating Reference Frame and pressure based solver. Solution is well converged. In fluent, we can write moment about x, y, and z axis. I think moment about zaxis would be the rotor torque (zaxis is rotor axis). Am I right? Calculated torque (30 Nm) (moment about zaxis) is around 2.5 time lesser than the torque predicted by BEM (78 Nm). What might be the reason? I am solving laminar flow. Should I use turbulent flow? Which turbulent model would be appropriate? Thanks 
From my experience with gas turbine blades choosing turbulent model is very important. In case you described it may be neccessary to use one of them. Calculate Reynolds number in critical location for the most severe condition you want to model.
During my master thesis I was obligated to check turbulence model impact on results (mostly on heat transfer). The advice of my lead professor was to use the SA model. But in a more general case ke model is more widely used. If you have any verification data compare results for every model and choose the best one. 
If I use kEpsilon model then how to define turbulent boundary condition at velocity inlet?
At velocity inlet, its require to give one of the following: K and Epsilon or Intensity and Length scale or Intensity and viscosity ratio or Intensity and hydraulic diameter How to find these turbulent parameters at velocity inlet? Do not have any experimental data. 
I used default values for Intensity and Viscosity Ratio (10%/10). But you will have to look in literature for more detailed data.

your problem is that fluent calculated torque is less than BEM, adding turbulence will even decrease it. BEM results aren't much precise and don't always give correct results

From data I know that one blade of my turbine should produce 85 Nm torque.
Calculated torque by using laminar simulation is 64 Nm while 35 Nm by using kepsilon turbulence model. Both are lesser than actual. What might be the reason? Moreover turbulent calculation gives torque almost half of the laminar calculation. Why???? 
how did you obtain 85 ?

from empirical calculation we design a 5 kw power horizontal axis wind turbine. Its rotational speed is 21 rad/sec and have three blades. so one blade should produce around 80 Nm torque.
Torque from laminar calculation is 64 Nm, which is close to empirical calculation but torque calculated from turbulent simulation is very small (34 Nm). I have not understand that why both (Laminar and Turbulent) torque are lesser than the empirical calculation. What might be the reason? Moreover turbulent calculation gives torque almost half of the laminar calculation and 2.5 time lesser than empirical calculation. Why???? 
if by empirical you mean BEM then it is ok. BEM only gives rough estimation of power and torque. in real life turbine performance will be less than BEM calculation. since CFD is more realistic it gives less performance values. and since in real life there is turbulence which acts like boundary layer separator and contributes to losses, CFD with turbulence gives even less results. it is hard to simulate turbulent flows correctly, so turbulent results may be little exaggerated, in my opinion real turbine performance is somewhere between laminar and turbulent results.
what is the tip speed ratio ? R=3m, w=20r/s, u =10m/s. so, TSR=Rw/u=6 if your turbine was designed for TSR=6 then performance prediction of BEM at lower rotational speeds will be more erroneous 
yes, tip speed ratio is 6.
I think boundary layer is more stable in turbulent flow as compared to laminar flow. So, separation is smaller in Turbulent flow as compared to laminar flow. Since separation is smaller, so, drag would reduce in turbulent flow. As a result torque should increase in turbulent flow. What do you think? 
Quote:
From my experiences in last 3 years of performing validation of NREL Phase VI experiments I have learned this lessen  predicting aerodynamics loads and power curve of wind turbine through CFD is a tough nut to crack. See my post in the following section  http://www.cfdonline.com/Forums/mai...irfoils3.html You can ask more for further clarification. Raashid 
Quote:
We have used SST, Real KE and KERT turbulence model. All fail to consistently produce accurate results. 2. Since we don't have access to CFX we cannot independently verify the new transitional model by Dr. Menter. (may you can ?) 3. Regarding your statement I think that for a particular free stream velocity if the flow is facing a fixed pressure gradient the turbulent boundary layer will be more stable but not by a significant margin. This is my understanding, it may be wrong and I haven't performed experiments the validate this. 
One more query. What tool are you using to perform the BEM analysis of your blade ?

Quote:
I would be really grateful... 
Quote:
I'm working on the somewhat the same project and I hope my experiences may be useful. I use double domain, (3.1 million node rotary domain+ 1 million node stationary doamin) in CFX . PLZ pay attention to these notes if you haven't already done: 1For accurate results I would like to say you must choose a good Turb. model which run well in separation..I found SST... 2 Try to satisfy number of nodes is the boundary layer and try to satisfy the Yplus criterion for your meshing . One more Question for CFD XUE; are you sure that you have multiplied the value of moment for one blade by number of blades? 30 N.m is for one or after multiplication? Cheers 
Quote:
Nice to know that you are working on the same problems. I suggest you should take a look at the following papers for NREL, which will give you valuable information about wind turbine simulations. "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes", R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA20060395 44th AIAA Aerospace Sciences Meeting and Exhibit and http://wwweng.uwyo.edu/mechanical/fa...20091221908 I will be very happy to help you in anyway possible. 
Dear Raashid,
Thanks a lot friend 
Quote:

what about boundary condition for HAWT

Quote:
i had simulated a wind turbine in fluent. and now i want to calculate the output power using torque(reportforcesmoment) but this output power is 10 times bigger than real amount. would you plz help me???? 
All times are GMT 4. The time now is 01:18. 