CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   Setting condition on a VAWT (

esp-m1000 February 4, 2010 04:54

Setting condition on a VAWT
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.

esp-m1000 February 9, 2010 05:04

Is there someone that can help me?

tony00 March 1, 2010 13:58

Use moving mesh
for VAWT you must use sliding mesh (or moving mesh as Fluent calls it) and run an unsteady simulation.


esp-m1000 March 1, 2010 14:31

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?

tony00 March 1, 2010 14:59

Mesh for VAWT
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


esp-m1000 March 1, 2010 15:10

Ok I will try, thanks.
I hope you will help me again if I will need...

enry March 10, 2010 12:31

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 P-V coupling? And discretization? My set-up is the following, but I'm trying to change it:

->P-V coupling: SIMPLE
Pressure: Standard
Momentum, Turb Kin Energy, Turb Diss Rate : 2nd order Upwind
-> K-Epsilon Realizable Enhanced Wall Treatment
-> Unsteady 1st order

Thanks, and I hope that we can help togheter!

tony00 March 10, 2010 14:32

Hi Enrico,
  • you do not need to do anything to the new walls that Fluent sets up: leave them as they are.
  • p-v coupling should only change the convergence speed, and should not affect the actual solution so I would not investigate different coupling scheme at this stage (maybe someone else could send his suggestion on this point).
  • Your set up parameters look OK to me.
  • I am also using Realizable k-epsilon but, I am using STD wall functions rather than EWT. Have you checked your y+?
You do not specify if your simulation is 2D or 3D.
In my case I am obtaining very high torque and as a consequence an amazing Cp of 1.2. Since I believe my set-up is correct, I have narrowed down the varaibles to investigate to:
  • mesh quality (mesh independent soution)
  • 2D/3D model: I would check if a 2D gives the same results as a 3D
  • Turbulence model. Maybe it is possible to make a mesh for a LES simul and to compare the results to RANS.
What are your thoughts?

enry March 10, 2010 15:01

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%.

enry March 10, 2010 15:05

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.


tony00 March 10, 2010 19:55

Torque calculation
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:
  • I saw you are getting the torque with a UDF. Why is that? You can get the moment coefficient from the GUI very easily (Solve->monitors->force->Cm) and you can get Fluent to dump it in a txt file which you can then use to plot, calculate torque etc. That's the way I am doing it. Would the two values of the torque compare in your case?
  • in the Cp formula you use (Cp = (w <T(t)>)/(0.5 rho V^3 D) ~ 0.3) is the torque per unit area?

enry March 11, 2010 04:53

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.

nana April 22, 2010 03:54

Hi esp-m 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 :)

sagarmatha April 27, 2010 17:58

high torque?
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 k-e 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)

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.

nana April 27, 2010 21:48

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.:)

nana May 5, 2010 03:12

Boundary set up on VAWT
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

enry May 5, 2010 10:40

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?

nana May 5, 2010 23:00

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 k-epsilon and k-omega. 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.

enry May 6, 2010 03:17

Hi nana,
I'm studying both 2D and 3D VAWT. My cp is around 0.2-0.3. I use realizable K-E 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!!! :p
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?


enry May 6, 2010 03:41

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.

All times are GMT -4. The time now is 02:53.