[FaSe]

Hi
I am ph.D student of mechanical engineering and I am doing my thesis. I’ve read your article about ‘Vertical Axis Wind Turbine’. I am working on a 2D vertical axis wind turbine with two NACA0021 blades. I use Gambit to mesh my model and ANSYS Fluent 16 to run the models. I find the best mesh according to experimental value in a specific TSR (actually highest TSR (2.4), to lower running time). Simulated Domain is a rectangular with a length of 26m and width of 12m. VAWT is located at 6m distance from inlet. In Gambit, I use a boundary layer at blades surfaces and adapt boundaries 4 times in ANSYS Fluent to reach “y plus <1”. I don’t know how to select time step size? Do I have to worry about Courant-Friedrichs-Lewy (CFL) number? When I set time step size as 1 degree revolution of rotor (according to literature articles), I get a good result of Cp (Coefficient of power, according to experimental value) just for the case TSR=2.4 (highest TSR) with y+<1 and CFL>1 (CFL~70). And when I set time step size as 1 degree of revolution for other TSRs, I get wrong results for Cp.
I tried different time step sizes to lower CFL number, but they didn’t reach a good result according to experimental values. Even for CFL<1.
When I want to run the other TSRs to study validation (with y+<1 and CFL>>1), some Cp (Coefficient of power) values are very lower than experimental work and some Cp values are negative. I calculate Cp values with this equation: Cp=Cm*TSR. Which, Cm refers to Coefficient of momentum and I calculate it by taking the average of Cm values for the last one or two revolutions. I’ve written my mesh specifications and numerical procedure below.
I am really confused and don’t know what to do. Because of time lacking, I am under a great pressure. PLEASE HELP ME WITH THIS ISSUE.

Geometry:
Domain Length = 26m
Domain Width = 12m
Rotor Diameter = 2m
Chord Length = 265mm
NACA0021
Mesh specifications:
Number of Cells before adaption = 95298
Number of Cell after adaption = 117978
Numerical procedure in ANSYS Fluent 16:
1. Solver:
Type: Pressure-based
Time: Transient
2. Models: Viscous
Model: k-omega (2 eqn)
k-omega Model: SST
3. Cell Zone Conditions: (select rotating zone)
Check mesh motion box and define rotational velocity according to TSR.
4. Mesh Interfaces:
Create/Edit:
Select “rotating zone” in “Interface Zone 1” column, and “stationary zone” in “Interface Zone 2” column and give a name to the interface.
5. Boundary Conditions:
5-1) Inlet:
Velocity inlet. 8m/s.
Turbulence specification method: Intensity and length scale
Turbulent Intensity = 0.5%
Turbulent Length Scale = 1m
5-2) outlet:
Pressure outlet.
Turbulence specification method: Intensity and length scale
Turbulent Intensity = 0.5%
Turbulent Length Scale = 1m
5-3) Blades (Airfoils):
Moving wall.
Relative to adjacent cell zone. Speed= 0
Rotational.
6. Reference Values:
Area = 2. (Diameter of rotor)
Length=1 (Radius of rotor)
Compute from: inlet
Reference Zone: rotating zone
7. Adapt:
Boundary Zones: select blades
Number of cells = 1
Options: Cell Distance
I adapt 4 times.
8. Solution Method:
Pressure-Velocity Coupling: SIMPLE
Spatial Discretization:
Gradient: Least squares cell based
Pressure: PRESTO!
Momentum: Second Order Upwind
Turbulent Kinetic Energy: Second Order Upwind
Specific Dissipation Rate: Second Order Upwind
Transient Formulation: Second Order Implicit
9. Solution Controls:
Use default values.
10. Monitors:
Residuals…Edit…Convergence Criterion: None
Create…Momentum…select blades
11. Solution Initialization:
Standard initialization
Compute from: all zones
X Velocity = 8m/s
12. Run Calculation:
Time Step Size = time for 1 degree revolution. (0.000909)
Number of Time Steps = time for 6 revolutions.
Check the box for “Data Sampling for Time Statistics”
Max Iterations/Time Step = 20

Appreciate any help

[muhammadshaaban]

Hi,
it was a long time for writing this issue! I have the exactly problem with you! I'm trying to simulate VAWT with MRF and Sliding Mesh. The results are good at the maximum TSR but they are very bad when I used any different TSR.
I expect some solutions for this problem:
1) Taking the steady solution came from MRF method to initialize the transient solution of the sliding mesh.
2) For the sliding mesh method, solve each TSR in a separate fluent file and don't stack the solutions!
3) Be careful during calculating the boundary layer thickness and refine the mesh near the blades with 10 layers times the boundary layer thickness.
4) The turbulence intensity may be the fatal issue since it varies according to the Reynolds number, which varies according to the rotational speed,

If you have reached any solution, please post me!

[satyamshk2]

I think, your reference values are not correct. As per the literature, the reference values will be
Area=swept Area (SPAN*Diameter) or the one you took in the experiment calculation of your geometry
Length= chord of the blade
depth= SPAN in 2D

[satyamshk2]

Corrected values
Depth= 1
Length= radius
ARea= diameter
Cp=cm*lambda