
[Sponsors] 
May 15, 2010, 09:31 

#41 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi nana!
I don't understand that sentence: " When i report the moment, i have 0.01657nm, and the calcualted power coefficient =0.3, by multiply the betz limit Cp=0.18". What do u mean saying "by multiply the betz limit Cp=0.18" ? I investigated sst models too and I think also that is not so good. I think that Std KE sometimes could give us bad results; I tried to use it, but sometimes the simulation braked off. RNG and ENHANCED are the best. In order to understand if my mesh and numerical setup is good I made some simulation at different TSR, and I compared it with other CpTSR curve obtained with tunnel test, and I discovered the same TREND, but not the same results! I have to investigate too in order to understand how can I set the same wind tunnel parameters. you said: "The totoal moment that i Have based on the report data from fluent is around 0.017Nm, however, the ke(RNG)wit hpresto give me 0.072. I also tried the realizable with standard and presto discretization, but the mometum i gained from kerealizablepresto is 0.685 and standard is 0.04." The negative sign have the meaning of the direction of rotation, in order to follow the right hand rules. If your angular velocity is clockwise probably the sign of Moment shoud be negative, because the effective vector moment is "entering in the paper". Have you reproduced THE SAME condition of the paper simulation? Again, are you sure that your timeAVERAGEsolution is timeconverged, and not numericalconverged? In order to discover if your model is correct you have to find the best article you can; it's not so easy, because in the article often there isn't any particular detail of simulation or tunnel test. However, first of all I advice you to make some simulation changing the grid, manteining the same boundary layer at the blades, and increasing the number of cells, and find if the solution is the same. Good luck!!! 

May 15, 2010, 10:58 

#42 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi enry:
thanks for the reply. I have tried different mesh size from 22k to 42k with4 different set of mesh size and running with same boundary conditions. I finally make sure that mesh size 37k for my 2d vertical wind turbine give me the best results. same as you rng with enhance wall give me best results. However, I tried to play with different turbulence specification method, such as k and e, the other one, turbulence intensity=5% and length= 1. However, the results show me large difference. By the way, my rotation is counter clockwise, I get the both positive and negative moment with different turbulence model. Based on the report moment from fluent, I can calculate the powe coefficient. I know the cp should be ard 0.3. What u mean time converge solution v.s numerical converge solution? To ensure the solution is converge, I monitor the velocity at tunnel outlet at every 5 time step. From that output result, I can see very clearly whether the solution is converged. Am I right? Well, have u compare the life and drag coefficient? Any suggestion on that? Thanks a lot 

May 15, 2010, 11:29 

#43 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi nana,
what do you mean saying: " I get the both positive and negative moment with different turbulence model" ? Moment coefficient is sinusoidal, so it's right to obtain positive and negative Cm... probably if you want to build a better vawt is better to obtain all moment positive. Of course the mean moment must be positive! With timeaverage converge solution I mean that timeaverage solution (that is time average Cp , or Cm, or other parameters) should be the same at every time steps, while numerical converge solution is the residual convergence. What do mean saying monitoring velocity at the outlet? Do you have the same mean velocity at the outlet every time steps? I don't understand. I don't monitor the lift or drag because my vawt is like savonius, without airfoil. Solution is very different if you set different turbulent boundary condition at the inlet. To obtain the same resuts choosing for example KE and Turbulence intensity and viscosity ratio you have to set the proper value. There is a relationship with value of K and E, and turbulence intensity and viscosity ratio. Take a look to user manual, chapter 7 Relationships for Deriving Turbulence Quantities Bye 

May 16, 2010, 22:26 

#44 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi enry:
Sorry for my unclear explaination. The positve and negaitve moment I can at same time step with same set up only the turbulence specification are differenct. For example, I got 0.0165718 when i Uisng RNGke, turbulence secification at both inlet and outlet are k and e. However, if i am trying turbulence Intensity and length. The report moment give me 0.04. I have check with the user manual before i change the paramaters. And I know that the Intensity =I=0.16(Re)^1/8, based on my Re, so I =0.05, however, i think i make some mistake on the length scale. For the timeaverage convege soltuion, i am sure that my results are time converaged and not residual converged. I monitor the velocity at the output at each time step, i can ensure my time converged when i check the velocity value are not change any more at each time step a after no.of revolutions. I find it's really annoying for the turbulence model, it has so many parameters and the result are so much different if change some one with the same set up. I have no experimental data to compare, so i cannot ensure that which turbulence model gives me the best results. Really appreciate all the discussion and suggestion that you share with me. Thanks a lot 

May 17, 2010, 05:44 

#45 
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Hi nana:
time converged solution means your monitored parameters are behaving in a steady, consistent pattern. if you are monitoring the moment coefficient, the ripple of the "wave" pattern of the moment coefficient is consistently following a pattern. this means that the peaks of each wave is in the same or close value to the ones of the adjacent waves. this sometimes can be as long as 10 VAWT revolutions. i've read a thesis where the author claims that convergence is attained after 30 revolutions. for some of my simulations, i have not had convergence after 20 revolutions, the peak of a wave is always lower than that of the previous wave. that being said, its up to you if you think the behavior is already in "dynamic steadiness". i would not count on the velocity being constant at the outlet. monitor something that is inherent in the turbine, not away from it. regarding selection of the turbulence model, there is really no perfect model for all types of problems. that is the reason why this "turbulence" thing has not been solved up to today. nobody can claim their turbulence model is "the model" of all models. this brings me to the next important point: you need experimental data to validate your model. without that, your "guess simulations" may be as good as any other person doing similar simulations. and they may all be far from the actual thing. remember, doing a 2D simulation overestimates the moment coefficient and subsequently the power coefficient of the VAWT. you now need to attribute the difference of your values from actual data to many reasons. but not being able to quantify the difference of your model from actual data is a big problem. i've had some runs using different turbulence models. the main thing i observe when using the ke models (fully turbulent) is that the torque ripple is very smooth. but if you compare that to the kw, kw SST, kklw, even the laminar model, all the other models show some form of irregularity in the wave, some form of randomness as a natural phenomena of turbulence. i believe the ke model is not really the best model for VAWT simulations because the flows near the wall are critical as their interaction with the wall is the main factor for the development of vorticity. if there are no shear forces as a result of "wall resistance", you will not have rotation of any fluid element. so modeling near wall fluid elements is really critical and using a turbulence model appropriate for wall bounded flows is important. ke is good with farfromwall problems, not with wallbounded flows. Last edited by sagarmatha; May 17, 2010 at 06:18. 

May 17, 2010, 08:00 

#46 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi sagarmatha.
I agree with u saying KE is not accurate for wall problem, but I think that modified KE ( enhanced or RNG) work well for VAWT problems. From fluent manual I can read that RNGKE is more accurate for rapidly strained flow or swirling flows than KE std. Probably RSM is better than other models; I tried to solve my problem (vawt) with RSM and I compared it with RNGKE, and they show me the same results; my conclusion is that maybe KE and modified KE ( enhanced or RNG) is not accurate for swirling flow, but only if the rotating velocity is very high! Fluent manual recommends you to use RSM model in cyclone flows, high swirling flows in combustor, rotating flow passages, problems that involves very high rotating velocity. What do u think abuot that? 

May 17, 2010, 08:30 

#47 
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Hi enry:
i agree with you that up to a certain extent ke is applicable to VAWT problems. especially if the expected Reynolds numbers are really high. i've seen simulations where ke RNG gave very good results compared to experimental data. when this happens, ke RNG is the better model to use because it converges faster and gives good results. but for low Re problems, differential viscosity ke RNG may be an option but i have not tried using it. and i have observed that kw, kw SST (with transitional flows activated) and up to a certain extent kklw can give realistic results for low Re situations. that is why what ever simulation is being done, validation with experimental data is critical. otherwise you can never be sure of the accuracy of the results. 

May 17, 2010, 08:46 

#48 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Thanks for your reply!
Do you have some articles (wind tunnel test or numerical results) that I can use to validate my mesh? I found a lot of article, but only few of that can give me some details about turbulent intensity and viscosity ratio at the outlet of the wind tunnel (and distance between outlet and vawt) or at the inlet of numerical domain. I'm studying a savonius vawt. Thanks! 

May 17, 2010, 09:46 

#49 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi nana,
have you investigated the reason of Cp>1 on your blades? Sagarmatha, have you any idea about that? Nana says that her pressure coefficient on the blades is bigger than 1 in some position... do u think that Cp should be less than 1? I'm not so sure that Cp must be <1 ... maybe because flowfield is not irrotationally... What do u think? 

May 17, 2010, 17:24 

#50  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
i'm sorry but i dont have articles with the outlet conditions as you mentioned. regarding the distance of the outlet from the VAWT, you can just do an analysis on that independent of experimental data at first. see if up to what point the outlet can be considered as farfield already. that goes true to the sides and the inlet as well. but from my readings and simulations, 10 VAWT diameters is a good place to start. then again, i am doing HVAWT with low solidity, not Savonius. i can imagine huge vortices generated by the huge blades of the Savonius. a collegue of mine (who is on the other side of the planet from where i am) did a study on Savonius with twisted and untwisted blades (full 3D but static, not rotating). i think i can try to get in touch with him and see if he has some literature that he can point us to. for the pressure coefficient that nana is having problems with, i have never encountered such high values as was mentioned. i sometimes get values greater than 1 but they can still be considered within the incompressible theory as they are around 1.001 to 1.005, not that high. maybe checking on the reference values for could be a start but that i assume nana already did. 

May 17, 2010, 17:52 

#51 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
ok sagarmatha, thanks a lot.
Do you know a method to estimate turbulence intensity at the inlet, having turbunece intensity at the blades? I'm going mad to find some DETAILED reference!!!!!! 

May 18, 2010, 00:10 

#52 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi enry and sagarmatha, thanks a lot for the sharing and suggestion regarding on the problem. Really appreciate so much on that.
I agree that different turbulence model gives the different results. So it is curical that we need to compare the results with experiment results to ensure which model is more accurate for the particular problem. I have using keRNGdifferential viscosity with enhance wall to test my 2D VAWT again. I have monitor the Cm with 10 revolution. my dt=0.001 and rpm=191, with u=3m/s and tsr =2. it takes 315 time step for one revolution. I have observed my Cm data, it's like Sin wave, however, the mean Cm is negative around 0.015. I remembet enry told me, if it's negative it's mean my rotation is wrong, i do not think so. My current rotation is counterclockwise, i think my VAWT is more like drag device. The Cm i ahve mointor is include the 4 airfoil blade and shaft, only the rotating zone, or whould i include the tunnel wall. I trying to upload the image, but I am jsut using linux system, not so familar with the function. So you guys mind to pass me the mail address that i can mail to you about the image about cm. I have calcualted the power coefficient based on the Cm, it's roughly ard Cp=0.15.but should be negative. Or do u think that my results are wrong , any suggestion? The pressure coefficeint for my case is still bigger than 1, i could not get the value lower than 1. I also lost my idea now. Any suggestion, thanks a lot 

May 18, 2010, 00:28 

#53 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi enry and sagarmatha:
Here is the Cm plot, kindly hope you have alook on that. 

May 18, 2010, 03:56 

#54 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
mmm....
I don't know nana.... are u sure that 4 blades is better than 3? Have u tried to build a 3blades vawt? If u put the 4 airfoil so closer togheter, maybe mean Cm could be negative... It's the only suggestion that come to mind... Does your vawt have the airfoil like the following picture? Surely yes... sorry but I also lost my idea ... Last edited by enry; July 30, 2011 at 18:34. 

May 18, 2010, 06:34 

#55 
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Hi nana:
try to monitor the Cm for one blade. you can do a phase shift (90 degrees) for the other blades and just sum up all four to get the total torque for the VAWT. no need to monitor the Cm for the post (shaft) as there should be negligible values there. do not also include the walls. the reason why i am suggesting that you monitor the Cm for just one blade is that you can analyze the behavior of one blade as it goes around one complete revolution. you can precisely pinpoint the position of dynamic stall, loss of lift and positive lift again as the blade moves through the upwind and downwind portions of the domain. you will then see where the "drag" is happening for just one blade. if the solution is timeconverged, this approach can be considered valid for all blades. it is no surprise that you can get negative mean Cm. that is a possibility. you are right when you said that your VAWT seems to be "dragging" instead of producing torque. try to use a different tsr (say 4). have you done this simulation using a standard symmetric airfoil (NACA0015 perhaps). see if you get the same negative torque. consider also a farfield approach to the walls (sides of the wind tunnel). will you get the same results if the walls are sufficiently far away? maybe there are blockage issues there that cause your VAWT to not produce positive torque. 

May 18, 2010, 06:44 

#56  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
try to look for data from meteorological/atmospheric journals. maybe they have some info. for me, currently i just use freestream farfield assumptions on the Tu and length scale (less than 0.1% Tu and 0.1L for the length scale). 

May 18, 2010, 23:45 

#57 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 8 
Hi enry:
Yes, my VAWT is looks like the pic you have showed. But it has 4 blade instead, and the airfoil profile is sd8020. I need to do the simulation for a company, they have 4 blade for the design, so i cannot change the design, but i can do the optimatization by changing the blade profile, liek the airfoil shape, chord length and so on. This is the later stage of my work. I also cannot extend my moment arm as i need to compare with the tunnel experiment results. The tunnel have dimension constraint, the longest dimenison for the turbine i can put is only 0.6m. Haha, this is Research work, full of challenges and stones along the road. Thanks a lot. 

May 27, 2010, 06:59 

#58 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi nana, Hi sagarmatha.
A simple question, but I can't find the command. How can I initialize flow setting: absolute, under reference frame, THROUGH COMMAND LINE??? I can't find the command... if I write: solve initialize initializeflow Fluent sets relative to cell zone under reference frame in solution initialization control pannel. Can you help me? Thanks a lot! 

May 28, 2010, 13:10 

#59 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 7 
Hi nana,
have you solved your problem with Cp>1 (pressure coefficient) ? my cp is also >1 ( even if my vawt is like savonius...) . What do you think about it? thanks! 

May 30, 2010, 03:34 

#60  
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 7 
Quote:
sorry no idea, too. i tried to figure it out but cant seem to find it. 

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 