CFD Online Discussion Forums

CFD Online Discussion Forums (
-   FLUENT (
-   -   2D Simulation of Savonius Wind Turbine (

ravindersingh December 5, 2011 11:11

2D Simulation of Savonius Wind Turbine

I need to simulate the 2D savonius wind turbine in fluent.

For this I created a mesh in Gambit. In Gambit there is one domain that contains the wind turbine domain, i.e a large rectangle containig a circle enclosing thw wind turbine. An interface is added so as to connect the mesh in Fluent.

In Fluent, I use Define->Grid Interfaces to set up the interface. As there are two domains: the one enclosing the the turbine is the rotating fluid which I set it to Moving Mesh and give it a certain rpm. The blade walls are aslo set to rotational motion. Standard k-e model is used and the inlet is velocity inlet and the outlet is pressure outlet.

Using the above process I try to iterate but i never achieve convergence of 1e-3.

Please tell me what I am doing wrong.

Thanks in advance

Far December 5, 2011 12:49

1e-3 is very hard to achieve in Fluent. I recently saw the Comparison of fluent 12 (convergence behaviour of 6.3 and 12 are same) and 13. In which fluent 12 converged to 1e-2 and fluent 13 converged to 1e-4 to 1e-5.

Well this is one aspect. However it also depends on your mesh quality. Some times if problem is unsteady and then you can not solve it as steady state.

ravindersingh December 8, 2011 13:21

Finally Solved it.
I did unsteady simulation, with blade walls as moving wrt the rotating domain. Also the rotational speed should be correct, I set it to a negative value and the solution converged to 1e-5.

Far December 8, 2011 14:40

well done. If possible please briefly describe your approach with some results here so that it be useful for the future

ravindersingh December 9, 2011 14:00

1 Attachment(s)
Meshing in Gambit
Two domain basically two faces.
First face is a big rectangle with a circular hole. Second face is the circle that fits into the hole in fist face. The second face contains the blades and is the one to be modelled as moving mesh. Interface is to be added in the gambit boundary conditions.

Unsteady Fluent simulation with k-e model
Read the mesh. Then create the Grid Interface from Define menu. (Uncheck both Coupled & Periodic)
Boudary Conditions:
Inlet -> Velocity type
Outlet -> Pressure Outlet.
The fluid domain containing the blades -> Moving mesh ->Set rotational speed.
The bladewalls-> Set to Moving->Rotational (relative to adjacent cell zone)

Thats it. You solve it. The important is that the inlet velocity and the rotational speed.
You must monitor the Cm history curve from Solve->Monitors->Force
The Cm history curve wrt time must be periodic.
I have attached one pic.

All times are GMT -4. The time now is 12:20.