
[Sponsors] 
June 12, 2010, 11:07 

#81  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
from the looks of it, your moment is indeed negative. but you should not take the last value of the moment because you are doing an unsteady simulation. take the average of the moment for the last full rotation (assuming periodic convergence has been attained) and use that as the torque for computing the power. taking the last value is only valid for a steady simulation like for a horizontal axis wind turbine. the value of the moment acting on a blade for the vawt is not strictly sinusoidal. but it should still be periodically going up and down. cheers. 

June 12, 2010, 11:27 

#82 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
amber,
I'm not using mfr, but sliding mesh. For the interaction between wind and turbine, i think you are right. I know that the turbine must rotate after the effects of the wind, but i don't know how implement this on fluent. So i choose a TSR, than the wind speed and found the w. But doesn't work. As u can see in my last post where there are 2 pic, i obtain negative moment. Have u suggestions? Hi sagarmatha, how can i take the average moment for the last rotation? For example, my time step correspond to a 2.5° of rotation, so for 1 rotation i have 144 time steps. i must take the report moment for each time step, sum each one and divide for 144? As u can see in Cm diagram i post, It looks like the Cm are converged, doesn't it? Thanks for help guys I must finish this thesis as soon, and don't know how..... 

June 12, 2010, 11:46 

#83 
New Member
amber
Join Date: Jun 2010
Posts: 8
Rep Power: 7 
Dontlose hope esp:>
i will discuss this problem with some seniors at my univ on monday[its vacation time here and so its hard to find people with cfd knowhow] hwevr i know that adina supports fsi and so now evn fluent +ansys cae[though adina is generally accepted to better currently].hwevr reducing tsr value[increase wind speed ,reduce w] will get u into acceptable range for t.do uhave experimental data?? 

June 12, 2010, 11:53 

#84 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
amber thanks so much for help,
i don't know anyone of the software u talked about, exept for fluent and ansys. I will searh information.... Thanks again 

June 12, 2010, 11:58 

#85 
New Member
amber
Join Date: Jun 2010
Posts: 8
Rep Power: 7 
Hey esp check turbine tut at adina website with fsi.seems to be interesting


June 12, 2010, 12:11 

#86 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
Thanks amber, I'm watching....


June 12, 2010, 12:17 

#87  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
yes, just take a simple average. but you must be careful of how you convert moment coefficient to moment. Cm is computed by fluent using reference values. using default reference values is ok but when you want to compare the values to your "3D" vawt, you must use actual wind velocity, area and length. your Cm looks periodically converged. but it does look to be in the negative trend. have you done convergence studies to confirm that you are using the appropriate setup parameters? three main things need to be checked: spatial (grid) convergence, temporal (time step) convergence, and iterative convergence. for spatial convergence, you must be sure you are using a fine enough mesh (also enough points on the blade surface) to capture the flow consistently but not too fine to be computationally expensive. for my blade, i use 1500 points. for temporal convergence, you must use a small enough time step. i usually use 1° rotation equivalent time step. 5° is a bit too big for me, 2.5° i have not tried. for iterative convergence, its not recommended to use absolute convergence criteria for residuals. AIAA recommends relative convergence criteria. i am currently doing a study on this and i seem to observe that using 2% relative error as convergence criteria is good already. 5% will just give values that are way too off. 1% takes too long to converge. hi amber, for practical reasons, you dont need fsi to simulate wind turbines. if you want to simulate with fsi, you need inertial effects, mass and material properties of your turbine, braking mechanism to prevent overspeed, etc, etc. if you are trying to simulate dynamic stress and deformation effects on the wind turbine, then you have no choice but to use fsi. if you are only interested in performance and the physics of flow, you dont need fsi. i dont think we should try to make it too realistic. assuming a constant rpm is good enough. even if you assume a rigid wind turbine, oneway or twoway fsi is still "overthetop" in simulations of VAWTs and HAWTs. ansys has twoway fsi for years already. i have not tried using it though. 

June 12, 2010, 12:24 

#88 
New Member
amber
Join Date: Jun 2010
Posts: 8
Rep Power: 7 
agreed but the way of current modeling [sliding mesh ,mrf] the turbine can rotate even if v=0 isnt it so??


June 12, 2010, 12:38 

#89 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
sargamatha,
for spatial convergence, i have 10056 elements for the upper surface of the blade, and 9080 for the lower surface. To have 12 rotation with 3D model it takes 3 days. But i don't mean, I have 2 pc working on it. For the others kind of convergence, do u think that the errors i have could be due to this? I used 2.5° or rotation per time step, and the absolute convergenze criteria for residuals. But if u say that the erros could be of 5%, my errors i think is very bigger than 5%. 

June 12, 2010, 13:30 

#90 
New Member
amber
Join Date: Jun 2010
Posts: 8
Rep Power: 7 
What the hell even me getting ve momemt[2d savonius ].should be able to clarify till monday,will keep u posted


June 12, 2010, 14:05 

#91 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
Ambermgupta, I hope monday will clarify our problems.
I'm waiting for u becouse i still have negative moment, no matter what i have done. I must finish my thesis as soon as. So your help will be welcome. See u on Monday Have a nice Sunday 

June 12, 2010, 15:05 

#92 
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
right. if you really want to simulate turbine startup, then you need to simulate just about everything including friction and gravity. but most people just want performance optimization and good understanding of flow physics.


June 12, 2010, 15:11 

#93  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
for temporal convergence, try 1° equiv time step. compare results to your 2.5°. if they match closely, then 2.5° is enough. if they dont, you dont have a timeindependent simulation (meaning your time step is a bit too large). for iterative convergence, i find that a relative convergence criteria of 5% usually means a residual of not lower than 1e04 for at least one of the monitored parameters (usually continuity or turbulent kinetic energy). but for 2% and 1%, residuals are of the range of 1e04 or lower. Last edited by sagarmatha; June 12, 2010 at 17:27. 

June 12, 2010, 18:31 

#94 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
Hi sargamatha,
First of all I would say thanks to u and to all guys for the help. I set a TSR=4 becouse i'm not modelling a savonius turbine or a drag device, but a darrieus like turbine. So I found that for Darrieus turbine TSR is usually 4÷7, do u think i have to choose a lower TSR? Thanks again... 

June 13, 2010, 07:04 

#95  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:


June 14, 2010, 05:16 

#96 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
Hi sagarmatha,
don't u worry, because i have done some simulation for TSR 1.6, 1.7, 1.8, 1.9, 2, 2.5 and also for TSR=4 at 5m/s. The results are not so good because for: 1)TSR=1.6, ω=17RPM, finally I have a positive moment about 50 Nm, it is positive but very poor, because Pw=1/2*rho*V^3*D=689W and Pe=50Nm*ω=89.01W so Cp=89.01/689=0,129 2)TSR=1.7, ω=18 RPM, positive moment about 57 Nm, always positive but very poor, Pe=57Nm*ω=107.44W so Cp=107.44/689=0,156 3)TSR=1.8, ω=19 RPM, positive moment about 53 Nm, always positive but very poor, Pe=53Nm*ω=105.45W so Cp=105.45/689=0,153 4)TSR=1.9, ω=20 RPM, positive moment about 30 Nm, always positive but very poor, Pe=30Nm*ω=62.83W so Cp=62.83/689=0,091 5)TSR=2.5, ω=27 RPM, negative moment about 20 Nm. What do you think about those results? 

June 14, 2010, 07:10 

#97  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:


June 14, 2010, 07:36 

#98 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 7 
sagarmatha I sent a private message to you.


June 14, 2010, 23:17 

#99 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi esp:
Sorry for the late reply as I am sick for the last few days. Yeah, there are some doubts that i want to clear with u. First, you need to run a different set of simualtion in order to get the optimum RPM and TSR. The real turbine need TSR=2 to let it self rotating first. So my suggestion is to set TSR=2, and play with different wind velocity like U=3,4, 5 m/s for example. (Starting from the lower wind speed). But you should know what is your cutin wind speed (it means the shaft can be generated power from that wind speed onwards). Second, I am using ke, RNG solve, as my Re is relatively low. However, I am a bit confused about your setting. What you mean if the turbine doesn't move the Re is about 929073, for a wind of 9 m/s. If the turbine rotate with 120 rpm and with 9 m/s wind speed Re=6700000. Why you saying like that. For the real turbine, 9m/s is really high wind speed. are you sure this one is the correct value? I think you statement is wrong (for a wind of 9m/s, the turbine doesn't move, the Re is about 929073). It is impossible, how come the turbien cannot move since the speed is really hight nearly the optimum wind speed. My suggestion is : set for the fix TSP starting from 2, you need to search what is the cutin speed for your turbine, like Sandia 17m darrieus turbine the cut in speed is at 5m/s. However, you can do the simualtion from U =2 or 3m/s, by fix TSR, you can calculate the RPM. Then do the simualtion. Since you are doing the 5 blade turbine, you can find a paper try to do the validation study to ensure the current Fluent solver that you are using is correct. Which I am doing currently, it seems my simualtion works well. The Cm will give the periodic function like sine wave. REmember, you can also compare with the 3 or 4 straight blade, it's only the turbine solidity is different. For higher solidity, the performance should be lower than the lower one. So actually you can comapre your Cp with the 3 or 4 blade. You also can comapre with my case if you blade is straight. All the best then 

June 14, 2010, 23:25 

#100 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi esp:
I just go through the previous post, I also have the negative TSR for my previous simualtion when i mointor the Cm. The first thing I thought there should be something wrong, or maybe the rotation is worng, or the coordination is wrong. Now i got the periodic Cm after i change the BC set up. I think for you BC, you should using the turbulence viscosity and length scale. Then using outflow at the BC outlet, however, the pressure outlet seems give me the same results compare to the outflow. the rest BCs looks ok for me. I am uisng PISO for pv coupling. As I said previously, my Re is realatively low, i am using ke RNG. For you case, i think ke standard should be ok. Or you can try kw sst model as well if you have enough time. All the best 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Help for setting 3D boundary condition in compressing water vapor  sogolf  FLUENT  0  September 27, 2009 15:05 
Boundary condition setting for water hammer proble  yizhou  FLUENT  1  October 12, 2007 12:16 
Need help setting a boundary condition...  HSeldon  FLUENT  2  August 28, 2006 14:10 
Warning 097  AB  CDadapco  6  November 15, 2004 05:41 
setting a body force as a boundary condition  blair  CFX  1  April 5, 2003 15:36 