[hammad0252]

Hi, I am working on wind turbine simulation using a rotating reference frame. My aim is to calculate the power generated by the designed turbine. Here is what I have so far.

I have created a fluid domain with the rotor in the middle and a cylinder to simulate the rotating domain. Right now the rotor is subtracted from the domain while the cylinder is whole.





My first question is whether it is fine the way I have it currently configured or should it be some other combination?

Should I subtract the cylinder from the fluid domain and then the rotor from the cylinder?

Any help would be appreciated, Thank You.

[CeesH]

Looks fine, you can indeed subtract the rotor from the cylinder. The cylinder and bulk domain should be separate bodies that do not overlap; is that currently the case?

[hammad0252]

Originally Posted by CeesH

Looks fine, you can indeed subtract the rotor from the cylinder. The cylinder and bulk domain should be separate bodies that do not overlap; is that currently the case?

Currently they overlap as I wasn't sure. I will fix that.

Furthermore as I understand to calculate power I will multiply the rotational velocity given to the moving frame with the torque that is felt on the rotor. Is that correct?

[CeesH]

Ok, if you subtract the cylinder from the box, and keep the cylindrical body with the rotor, all should be fine.

You can calculate the torque using reports > forces and then select moments, setting the right axis origin and direction, and then calculate the torque on the turbine indeed. After that, indeed multiply by the 2*pi*N (rps), and you have the power.

Good luck! Cees

[hammad0252]

Just an update. I made the mesh shown below, used sphere of influence in body sizing so that most of the elements are in the middle.





I feel that the elements might not enough but considering the computer I have access to currently this is the best I can do. I hope to make a finer mesh once I have access to a more powerful computer.

In fluent I set the time to transient, k-w SST for turbulence, frame motion to the cylinder about x-axis at 37.5 rad/s. Inlet velocity set to 5 m/s and pressure outlet. Set the flow time to 5s with 50 intervals each 0.1s. The solution is being calculated as we speak. Hope it works out.

[CeesH]

why is there a very dense mesh region far away from the cylinder? I understand you are limited in the mesh size, so it seems to me it is important to be efficient in refinement - that clump of cells on the upper right does not look very efficient to me. Maybe you can improve the mesh, making sure:

1) the mesh is fine close the the blades, and cruder far away
2) the domain is predominantly filled with hexahedral/polyhedral elements (hexahedral will be though/impossible near the impeller, but surely applicable to the bulk of the domain)

[hammad0252]

I changed the mesh to be a bit more concentrated around the cylinder.

A view of the new mesh


Sliced View Along the XZ Plane



Sliced View Along the YZ Plane



Afterwards I ran the calculations and it came with the following moment report.


But according to this the turbine would generate only 0.090707897*37.5 = 3.40 W
Power available = 0.5*3.1415*(0.4^2)*(5^3)*1.225 ( 1/2 * pi * r^2 * v^3 * rho) = 38.48
Which would correspond to a coefficient of performance of 8.839% which seems quite low. Is this right considering the blade shape and the small size and speed or am I doing something wrong?

[hammad0252]

Looking at the results in CFD-Post I think I might have screwed up the mesh interfacing. I am going to try again this time interfacing each face individually.

[PayarRadfar]

I am doing my final year project (Mechanical engineering, be Hons) on ducted wind tubines. I am mainly interested in increasing the power generation (obviously). I have got also some data from an actual turbine built by a company;such as power generated at each wind speed in the venturi.

I managed to run a cfd model on this and got pretty close results to what the company achieved. Using their data (power generated and power coefficient) and my cfd results, I managed to find the pressure difference caused by the turbine.

The study is a 2d study at first which later on i will be doing also a 3d and instead of the turbine i set a porous region.

My question is even if i do get this right, and lets say i change geometry or some other stuff to increase the mass flow rate, how can I know the new pressure difference caused by the turbine? Because, Based on what I think, turbines would obviously give different pressure difference at different rotational speed (that is how it generates different power at different speed).

Pretty much, I am interested to say that the power generated is increased by certain percentage etc.

Any guides ?

[okinugraha]

Originally Posted by hammad0252

Looking at the results in CFD-Post I think I might have screwed up the mesh interfacing. I am going to try again this time interfacing each face individually.

hammar, why the fluid not flow indeed rotating body or blade ?