
[Sponsors] 
February 4, 2010, 04:54 
Setting condition on a VAWT

#1 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 9 
Hi to all,
This is my first topic but I read the forum for some years... I'm doing CFD analisys for my thesis at university on a Vertical Axis Wind Turbine. I have designed and meshed a 3D vertical axis wind turbine with 5 blade on gambit. I have done two different fluid zones in the mesh one for free flow and one in agreement with the turbine . Now I have done some simulation on fluent, but the first problem is that after about 2500 iterations the residuals don't converge but become flat (can i assume the the solution is good?), maybe this is caused from the contidions I set. The second problem is that I use a Multiple rotating reference frames, so I must set the angular velocity of blades and mesh. I want to know how to let that the wind makes move the turbine, and if I am on good way or there are some mistakes. Sorry for my bad english and thakns in advance for your precious help. Last edited by espm1000; February 9, 2010 at 05:02. 

February 9, 2010, 05:04 

#2 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 9 
Is there someone that can help me?
Please.... 

March 1, 2010, 13:58 
Use moving mesh

#3 
New Member
Join Date: Nov 2009
Posts: 22
Rep Power: 9 
Hi
for VAWT you must use sliding mesh (or moving mesh as Fluent calls it) and run an unsteady simulation. Regards 

March 1, 2010, 14:31 

#4 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 9 
hi tony, thanks for your answer.
Can I ask you how to make sliding mesh on gambit? As I said in my mesh I have done 2 different fluid zone, one for free stream and other in agreement with the turbine blades. What Can I do to use sliding mesh? Thanks 

March 1, 2010, 14:59 
Mesh for VAWT

#5 
New Member
Join Date: Nov 2009
Posts: 22
Rep Power: 9 
Hi
Check out the tutorial of compressor vane and the one of axial turbine. Google Fluent tutorials and check the sliding mesh tutorials. Anyway you will find that: you need to define an interface between the rotating and the stationary part of your domain. The two parts of the domain should not be connected. Once you imported the mesh in Fluent you define the interface by coupling the stationary one with the rotating one. Define solver unsteady. Define the rotating domain as moving mesh (rotating) with the turbine angular speed. Define the turbine blades (walls) as stationary (with respect to the rotating domain). Run the simulation Regards 

March 1, 2010, 15:10 

#6 
New Member
Join Date: Jan 2010
Posts: 28
Rep Power: 9 
Ok I will try, thanks.
I hope you will help me again if I will need... 

March 10, 2010, 12:31 

#7 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi, I'm also doing a master thesis on a VAWT.
How have you interpreted the new wall that Fluent create after the interface is setting up ? Have you changed the boundary conditions that FLUENT give to the new walls? What kind of turbulence model have you choose? What about PV coupling? And discretization? My setup is the following, but I'm trying to change it: >PV coupling: SIMPLE >Discretization: Pressure: Standard Momentum, Turb Kin Energy, Turb Diss Rate : 2nd order Upwind > KEpsilon Realizable Enhanced Wall Treatment > Unsteady 1st order Thanks, and I hope that we can help togheter! 

March 10, 2010, 14:32 

#8 
New Member
Join Date: Nov 2009
Posts: 22
Rep Power: 9 
Hi Enrico,
In my case I am obtaining very high torque and as a consequence an amazing Cp of 1.2. Since I believe my setup is correct, I have narrowed down the varaibles to investigate to:


March 10, 2010, 15:01 

#9 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi tony.
At this stage i'm simulating on a 2D blades. I choose EWT because on FLUENT's user guide advice to use it when the problem involves rotating flows. My y+ is in buffer layer, from 1 to 30, but for your Standard wall threatment you should have y+>30. What is your Cp? In my case I find a Cp = (w <T(t)>)/(0.5 rho V^3 D) where : w = angular velocity <T(t)> = time average torque, based on one complete rotation of the turbine, after achieved convergence of <T(t)> D = turbine diameter (2D! you should have Frontal Area) There is a limit on Cp, from Betz law Cpmax = 0.59. How do you impose Turbulent viscosity ratio and Turbulence Intensity at inlet and outlet? I leave 10%. Last edited by enry; March 11, 2010 at 05:16. 

March 10, 2010, 15:05 

#10 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Sorry
I think that LES is very expensive.... Cp for 3D is always less then 2D ... I choose my mesh doing a finer mesh and comparing results... I try to simulate with PRESTO! and PISO, but results is the same of the standard options. User manual advice to use PRESTO and PISO for our problem. Enry Last edited by enry; March 11, 2010 at 06:31. 

March 10, 2010, 19:55 
Torque calculation

#11 
New Member
Join Date: Nov 2009
Posts: 22
Rep Power: 9 
Hi Enrico,
turbulent intensity 10% I think is plausible. I know BEtz limit is Cp=0.59. I am getting Cp=1.2. I was joking when I called it an amazing Cp. I am trying to spot where the error is. I have two questions on the torque:


March 11, 2010, 04:53 

#12 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi,
yes, of course, T is torque per unit area. I wrote a UDF in order to get the time average torque, that FLUENT can't give you. Bye. 

April 22, 2010, 03:54 

#13 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 10 
Hi espm 1000:
I am doing the same thing as you currently. I have finish the 2D model with sliding mesh and also the dynamic motion, you can see that the blade part is rotating. However, i have problem to do the Hex mesh for 3D. Which software are u using? I am using gambit, and i have 4 straight blade for my VAWT. I am doing the simulation inside wind tunnel. I have problem to get a good mesh on that. Any suggestion, thanks a lot 

April 27, 2010, 17:58 
high torque?

#14 
New Member
sagarmatha
Join Date: Apr 2010
Posts: 19
Rep Power: 9 
high values of torque could mean a few things.
for one, a fully turbulent assumption causes delayed dynamic stall and higher torque due to late onset of flow separation (separation drops lift dramatically). this should be checked with the actual flow that is being simulated. does the Reynolds number indicate fully turbulent flow? if not, then ke is not realistic. but if there is tripping of flow at the leading edge, then fully turbulent assumption is safe even if free stream conditions indicate laminar flow. then again, torque values should be validated and checked properly. another reason for high torque is having erroneous computation. from the torque coefficient (Cm), you can compute for the torque easily but keep in mind the frontal area of the VAWT. always go back to the actual geometric dimensions of the turbine that is being simulated. this can be used as a guide: Cm = T/(0.5 x v^2 x rho x A x L) where v = fluid velocity rho = fluid density A = rotor projected area L = rotor radius solve for T to get the torque. then power is just P = T x w, where w is the turbine angular velocity. always keep consistent units when doing computations and comparisons. lastly, 2D results always overpredict actual 3D values. if simulation is done in 2D and compared directly to 3D, then losses should be used to explain the differences. some losses could come from blade tip vortices, support arm drag, and post shading effect. one more note (but this one i have not fully checked). if mesh within the VAWT domain is not refined enough, the wakes generated by the blade as it passes the upwind part gets unnecessarily dissipated, faster than wanted. when this wake interacts with the other blades (or with the same blade that generated it), the flow could be a lot smoother (although still turbulent). this could mean higher lift generated and consequently higher torque. 

April 27, 2010, 21:48 

#15 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 10 
HI Sagarmatha:
Thanks a lot for the detail explanation for the difference between 2D and 3D VAWT. I have some idea on that. But the current problem for me is hard to get the good mesh for the 3D VAWT inside wind tunnel. I have make the 3D domain with 4 straight blade inside wind tunnel. I have subtract the blade part from the tunnel, I have difficulties to mesh the whole thing as I have tried a lot to mesh it , but i still cannot make it. You have any good suggestion , or can i get your mail as i can send the .dbs file for your review. Thanks alot. 

May 5, 2010, 03:12 
Boundary set up on VAWT

#16 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 10 
Hi tony:
I would like to know how you set up for the time step size and no.of Time steps for your simulation on VAWT? I am doing almost the same thing. As i have tried different set of simulations with different solver set up to get the most accurate results. How much RPM have you used for your sliding mesh? I also have some weird cp on the airfoil, it is all greater than 1. I was wondering to find out why the Cp like that. But currently, no good news yet. Kindly hope that you can share the experience with me. thanks a lot 

May 5, 2010, 10:40 

#17 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi nana,
I'm studying 3D VAWT, and I create the mesh with cooper scheme in Gambit. > I create first the mesh for 2D model, and then create the 3D volume through surface translation "with mesh". >Gambit create a volume with mesh, then I delete the VOLUME mesh,maintaining only the face mesh of the originally 2D blades,but at the bottom and the top of the turbine! > I set the edge mesh on the third dimension ( the axis of the VAWT) > Now you can set the cooper scheme and mesh volume. I think that Gambit can't create a cooper mesh without THE SAME originally mesh on the 2 side of the VAWT, even if you mesh these part in the same way. So you should create the 2d model with mesh first. I hope that my advice can help you. I have a problem: how can I set the turbulent viscosity ratio in the boundary conditions? I'm trying to compare my results with wind tunnel results from some article. I found only an article that indicate the turbulent intensity, but not the turbulent viscosity ratio. Any ideas? 

May 5, 2010, 23:00 

#18 
Member
Join Date: Jul 2009
Posts: 43
Rep Power: 10 
Hi enry:
I have no problem with the mesh. I just want to know what kind of B.Cs that you have set up for the 2D VAWT. Well, you might not study the 2D, only 3D. For the viscosity ratio, i just leave as default. But i have trying the different RANS, like kepsilon and komega. I have try to using the turbulence viscosity at 10% and length at 1, it seems acceptable for the simulation. I have read a journal, it set viscosity at 5% with length @1. I will try it out. Well, how much the pressure coefficient cp that you have obtained? My cp always larger than 1. You have any idea? I used velocity inlet as my inflow and pressure outlet at exit. I even try using outflow as exit boundary condition. But the very strange things is that when i using the same BCs with finer mesh, the residual goes up for epsilon. I also try different discretization for momentum, based on the fluent user guide and my 2D mesh is quad mesh. The QUICk scheme is well suitable. 2nd order upwind is more for tri/hybrid mesh, however, with SIMPLE scheme, it not works well also. Only SIMPLE with standard pressure and 2nd order upwind for momentum works well. I will try the 3D later as 2D can predict the aerodynamics performance. keep in mind, if you want to compare your simulation results wit experimental, the flow condition must be the same. 

May 6, 2010, 03:17 

#19 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi nana,
I'm studying both 2D and 3D VAWT. My cp is around 0.20.3. I use realizable KE with enhanced wall treatment. Do you set a boundary layer at the blades? Set it in order to obtain y+>30 if you use a std wall treatment, otherwise if you set enhanced wall treatment try to obtain lower value of y+ . I set the 2nd order discretization, and PRESTO! for pressure, but it isn't so important to obtain a good solution. Do you make an unsteady simulation? how do you compute Cp? Cp = w <T(t)> / ( 0.5* rho * V^3 D ) in 2D simulation, where <T(t)> is the mean torque on the vawt, based on a rotational period of vawt at least; w is the angular velocity in rad/sec; V is the free stream speed; D is the vawt diameter (in 3D simulation you have to replace D with A=frontal area). Pay attention to Cm file that fluent write at iteration, because Cm adimensionalized as you set in fluent. Have you checked if your cp solution is converged? My solution converge after at least 10 revolution of the vawt. Set properly your Dt, based on free stream velocity and angular velocity of the vawt. My vawt makes a revolution after 200 time steps, and every time steps fluent makes 20 iteration. However, I know that I have to set the same parameter of a tunnel test, and it's so difficult to find every value!!!! but I think that it isn't useful to check my mesh with another fluent mesh... I think my mesh is better than others!!! I compare also fluent results with OF results and they are the same, but I'm interesting in comparing my result with real wind tunnel experiment. Have you found any articles that says every tunnel value? Regards. Enry. 

May 6, 2010, 03:41 

#20 
Senior Member
Herman
Join Date: Nov 2009
Posts: 122
Rep Power: 9 
Hi nana, I have a question for you: have you found any article that simulate 3D vawt with CFD? I'm not... can you post me title and author of the article that you found, the article that sets viscosity at 5% ? thanks a lot.
Enry. 

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  Siemens  6  November 15, 2004 05:41 
setting a body force as a boundary condition  blair  CFX  1  April 5, 2003 15:36 