Hi guys, I am simulating a 2D flow over a savonius turbine where the turbine rotor was locked at a particular angle relative to the flow(I'm looking for a validation with a paper). When I run a steady simulation I can't reach convergence: the moment coefficient oscillate around a fixed value so I believed that does not really exist a steady solution because of vortex shedding phenomena. Now I'am interested to the value of the moment coefficient to check validation with the paper, so i believed to run an unsteady analysis so i can get this value after time averaging. Is my reasoning good?

If my reasoning is ok,i will use,in the unsteady simulation a segregated flow solver+ the implicit unsteady time model; Do I make any check on the courant number before starting the simulation to prevent low accuracy?

regards rob

ps:Sorry for my english...

Hi Rob, I'm simulating a 2D savonius rotor also. I've perform several analysis in Fluent (segregated solver, implicit, unsteady/steady) with Moving reference frame (MRF) and moving mesh (MM). With MRF (steady analysis) you can obtain an average torque of the rotor at X rad/s, but i have obtain different values at different rotor's angle, i think it must be unsteady. With MM (unsteady) i have obtain some results of efficiency that are close to the Sandia wind tunnel tests, but when I analyze the Benesh 1988 (Pat. 4784568) and 1996 (Pat. 5494407) or the Rahai (Pat.Ap. 20070104582) i obtain different values that does not match. So I think i'm doing something wrong. I have used the k-e-RNG, S-A, and Reynolds Stress Model for viscosity. - k-e-RNG: torque value close to Sandia values (at TipSpeedRatio = 0.9) - S-A: lower torque than RNG - RSM: divergence Hope it helps I have one question, How the courant can prevent low accuracy? César Also:Sorry for my english There are some papers: - Wind Tunnel Performance Data for Two- & Three-Bucket Savonius Rotors, Sandia Laboratories 1977, SAND79-0131 - A THREE-TIERED APPROACH FOR DESIGNING AND EVALUATING PERFORMANCE CHARACTERISTICS OF NOVEL WECS Analysis and comparison of CFD results with wind tunnel results of savonius rotor. By the way it didnt specify the CFD setup.

Hi Guys,

i am happy to meet you guys working on Savonius.. i have performed several simulations on 2-D Savonius using sliding mesh in fluent. i have used K-e std and K-e Realisable..but the torque coefficient differing from sandia report by giving more negative torque..

I am doing some thing wrong..but i couldn't able to find. Sandia report told by Cesar is good one to look for comparision.

I kept courant number less than 1 since i got some error message regarding turbulent viscosity..

Hi Saravanan, It is great to hear from more people working in this, this is a great way to colaborate Are you having a lower values than Sandia? I've obtained Cp=0.235 at TSR=0.85 using: *Model - 1m diameter - area of air 10 radius for the inlet (inlet to rotor) and both sides, 14 radius for the outlet *Boundary conditions - Velocity inlet 10m/s, Pressure otulet 0Pa, Symetry (2 faces), moving mesh (rotational velocity 17rad/s = TSR=0.85) - Working conditions Pressure = 0 *Solver - Pressure based - Unsteady 2nd order *Viscosity model = K-e RNG (I dont know if it is OK) *Solution control - P-V = coupled - Momentum, pressure, etc = 2nd order *Iterations - time step size = 0.001 - iterations per time step = 10 - analisys time = arround 5 sec. This configuration gives good results for the savonius, but for the benesh profile i'm not having good results. For the benesh 1996 i'm obtaining Cp=0.27 at TSR=1 I have the same problem regarding the turbulent viscosity, it takes very high values. If I use a courant number less than 1 it will work? (I imagine that you are talking about the courant number that appears when you use the Pressure-Velocity Solution Control = coupled) Why it solves this issue? I have increased the turbulent viscosity limit to avoid that issue. May be it isn´t the best way to do it. I've posted some videos taken from fluent in youtube - Savonius wind turbine CFD 2D - Savonius wind turbine CFD 2D - benesh rotor

Ok, i've checked about the courant number, I think you are using a density based solver. And when the changes in the solution are highly nonlinear it is better to use a lower value. (default values, for explicit=1 for implicit=5) Are you using the implicit or explicit formulation? I haven't use the density based solver but i will check how does it perform

Here's another tip, The moment coefficient (Cm) is calculated by Fluent dividing the moment by ( 0.5 RHO V^2 A L ) Cm = M / ( 0.5 RHO V^2 A L ) , So in the analysis, Fluent obtain the the moment and then it calcules the Cm and present it in the Cm plot, but we need the Moment to calcule the power multiplying it by the rotational speed Or may be we can obtain the Cp directly with the Cm Cp = TSR Cm Note: RHO, V, A, and L are the density, velocity, area, and length (Radius in this case) this values needs to be ADDED to the Reference Values panel. Fluent menu: Report - Reference Panel

[javadshahbazi]

Hi all people:
I want to simulate Savonius rotor as you , but there is a problem:
we don't have angular velocity of rotor? actually we have wind velocity and first we must get rotor speed? how we can do this?

[mutata]

hello guys...i am trying to perform CFD analysis of a simple savonius wind turbine .made a CAd model in solid edge.have made the mesh in gambit and imported it to FLUENT for analysis..there is a problem.fluent is NOT analysing the blades.it is skipping it.

solution?

[sheikh nasir]

hello,
i am using fluent for my work , i.e unsteady , sliding mesh , for train moving in tunnel . can any body help me. my email is sheikhnasir39@gmail.com
thanks

[fragomar]

Hi guys

I am also simulating a turbine Savonius but I use the a helical model (Windside). I work in Phoenics and now I am trying to use Star ccm+ to compare results. If someone wants to contact me to share information would very helpful, my email is balam_6666@hotmail.com

Excuse my english is not good.
I speak spanish.