CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Wind turbine simulation in Ansys CFX (http://www.cfd-online.com/Forums/cfx/123310-wind-turbine-simulation-ansys-cfx.html)

aalbanesi September 9, 2013 19:01

Wind turbine simulation in Ansys CFX
 
Hi everyone,

I am going to simulate a horizontal axis wind turbine with Ansys CFX. I have some experience with CFX, in particular with vehicle aerodynamics simulation, and with internal combustion engine simulation.

I have read many posts in this forum regarding wind turbine simulation in CFX, however, i still have some doubts regarding interfaces, frozen rotor and immersed solid approaches.

Does anyone have a CFX-Pre setup to share so I can have a look at it? If not, anyone has a tutorial to share?

Kind regards,

Alejandro

ghorrocks September 10, 2013 05:51

This simulation is quite simple to set up.

First of all - forget immersed solid. That will not be appropriate for a wind turbine model.

For the rotating frame of reference stuff have a look at the rotor/stator tutorial which comes with CFX and other rotating frames of reference examples.

For the "object in a free stream flow" simulation have a look at the Flow around a blunt body simulation.

There are more tutorials on the ANSYS community site, off the ANSYS webpage.

aalbanesi September 10, 2013 17:41

Thank you for your reply. I will get into those tutorials. I am also looking around the Ansys community site.

In case you have any pre files of similar simulations at hand, It would be very helpful.

Kind regards,

Alejandro

er_ijaz September 30, 2013 05:39

Hi r using sliding mesh or MRF analysis?

ghorrocks September 30, 2013 18:25

Sliding mesh allows you to connect two meshes which are sliding past one another and multiple frames of reference allows you to do simulations where different parts of the simulation are in different frames of reference. They are totally different things, but if you are doing a MFR simulation you are probably using sliding mesh as well.

er_ijaz September 30, 2013 23:56

Hi thank u , I have done simulation using sliding mesh analysis. Problem now I'm facing is with post processing ...Do u have any tutorials to work on post processing. I need to do simulation of wake behind the blades or images of wakes

aalbanesi October 10, 2013 11:14

I located the rotor in a Rotating Domain. This rotating domain is immersed in a Stationary Domain, as shown in the next figure. The rotating speed is set manually, and then CFX automatically creates the interfaces.

http://img841.imageshack.us/img841/5904/b01m.jpg

The solver runs normally, but the results are not satisfactory. What am I missing, what is wrong with this configuration?

Also, is there a way to configure the rotating speed as a function of the torque generated by the rotor? (instead of a fixed ideal value, I would like to obtain the real value).

Thanks in advance,

Alejandro

ghorrocks October 10, 2013 17:19

Your domain configuration is fine. You have some other problem causing the inaccuracy - http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Yes, you can set the rotation speed as a function of torque but I do not recommend it in general. It is generally better to run a series of rotational speeds and get the performance curve of the device. Then you can find the rotation speed by interpolation. This means you have a series of simple fixed speed simulations, rather than a tricky variable speed simulation.

aalbanesi October 10, 2013 19:38

Thanks ghorrocks for your quick reply. I will read the Ansys FAQ carefully in order to figure out what is wrong with my simulation. I will follow your advice with regards to the rotation speed.

Perhaps I am not using the correct CEL expression in CFX Pre to compute the torque.

What would you recommend to compute the torque, should I do it in CFX Pre or Post?

If "V" is the wind speed, "Vrot" is the rotation speed, and "rotor" is the part name, can you give me a correct expression of the torque?

Thanks for your help, regards

Alejandro

ghorrocks October 10, 2013 20:28

Torque has nothing to do with wind speed or rotation speed. You can get the torque from an expression like torque_x()@BladeSurface, assuming the rotor is on the x axis and the name of the wall boundary for the rotor is BladeSurface.

aalbanesi October 11, 2013 08:14

Thank you. I assume that the CEL expression of torque is independent of wind speed or rotation speed. I will give it a try, and let you know if it worked.

Btw, do you recommend steady state o transiet simulation?

Kind regards,

Alejandro

ghorrocks October 12, 2013 06:37

That depends on what you are modelling. If you just want the steayd performance then steady state.

Also - you appear to have 1/3 periodicity. Why not model just 1/3 of this?

aalbanesi October 15, 2013 07:53

Your right, one option is to take advantage of the periodicity of the model (perhaps for the firsts simulation).

But for the future, i want to include the support tower in the model, and analyze the interaction between the tower and the rotor.

I will make the firsts simulation with 1/3 of the model, and afterward I will use the complete rotor along with the tower.

Do you think I need to setup an additional interface for this setup (rotor + tower)?

Thank you , Alejandro

ghorrocks October 15, 2013 19:47

Think frames of reference, not objects. The only rotating thing (which will go in a rotating frame of reference) is the blades. Everything else is stationary. So stick the blades in rotating frame of reference and everything else in a stationary frame. And it is best to stick everything in a SINGLE domain in the stationary frame of reference if possible.

aalbanesi October 16, 2013 08:03

Thank you. It is very clear now.

Regards, Alejandro

aalbanesi October 17, 2013 11:41

Glenn, hi. The simulation is running, but my results are wrong.

I am using in CF-Post the CEL expression you recommended (torque_x()@rotor Default), the rotor is on the x axis and the name of the wall boundary is rotor.

When I compute the power generated (combining torque and rotational speed), the wind turbine is generating more power than the power that is available in the wind, for the same surface (rotor surface). That is impossible.

So, as i figured, it is not a problem of convergence against grid refinement (at least yet). Mesh refinement will eventually come when the simulation works fine (when the power generated by the turbine is below the available power in the wind).

Below I leave a RAR file with the ICEM project (without mesh), a CFX-Pre file with a loaded mesh, and a CFX-Pre file without the mesh.

https://www.dropbox.com/s/lplbmrclkehp5qt/forum.rar

Would you please give a quick look at the CFX-Pre settings, to verify if everything is Ok?

I have also calculated torque as a monitor point in the solver, since I read in another post that sometimes the CFX-Post gives incorrect forces and torques. Since I am getting the same values of torque in the solver as in CFX-Post, I think the problem is in the CFX-Pre settings.

Thank you for your help and patience, regards

Alejandro

ghorrocks October 20, 2013 19:55

I do not have time to check your simulation in detail.

Your assumption that too coarse a mesh cannot result in the generated torque being too high is wrong. It certainly can, so I definitely would check mesh density.

And check out this general FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

aalbanesi October 21, 2013 09:53

No problem Glenn. I know grid refinement affects the results, but I think I have another kind of problem (and I think many other users in the forum have the same problem).

I made several simulations, each one with the same wind speed (V=10 m/s) but with different rotation speeds (increasing from zero to 100 RPM).

Once a specific rotation speed has been reached (above lambda = 5, where labmda is the ratio between the wind speed and the blade tip speed), the blade's aerodynamic coefficient goes up to 70%.

However, Betz limit says it can never be larger than 59.7 %. And, if I increase lambda a bit more, the blade's aerodynamic coefficient CP keeps getting larger until the wind turbine produces more power than the power available in the wind.

Perhaps there is a physical mismatch in the model configuration, as the torque computed by ANSYS depends of the wind speed (fixed value of 10 m/s), and of the rotational speed of the rotating domain (user specified). In the specific literature of wind turbines I found that values of lambda = 7 are quite common, with a CP = 40%. However, for lambda = 7, CFX computes CP = 300%.

Do you have any idea how to make the rotational speed as a function of the torque generated by the blade?

Regards, Alejandro

ghorrocks October 21, 2013 17:27

You can make the rotational speed a function of torque but it significantly complicates the simulation. For most applications it is better to run a sweep of several rotational speeds and interpolate to the steady state speed, and run that speed as a fixed speed run as well. This is a much simpler approach.

drsattar November 8, 2013 03:55

rotational speed
 
Quote:

Originally Posted by aalbanesi (Post 457490)
Glenn, hi. The simulation is running, but my results are wrong.

I am using in CF-Post the CEL expression you recommended (torque_x()@rotor Default), the rotor is on the x axis and the name of the wall boundary is rotor.

When I compute the power generated (combining torque and rotational speed), the wind turbine is generating more power than the power that is available in the wind, for the same surface (rotor surface). That is impossible.

So, as i figured, it is not a problem of convergence against grid refinement (at least yet). Mesh refinement will eventually come when the simulation works fine (when the power generated by the turbine is below the available power in the wind).

Below I leave a RAR file with the ICEM project (without mesh), a CFX-Pre file with a loaded mesh, and a CFX-Pre file without the mesh.

https://www.dropbox.com/s/lplbmrclkehp5qt/forum.rar

Would you please give a quick look at the CFX-Pre settings, to verify if everything is Ok?

I have also calculated torque as a monitor point in the solver, since I read in another post that sometimes the CFX-Post gives incorrect forces and torques. Since I am getting the same values of torque in the solver as in CFX-Post, I think the problem is in the CFX-Pre settings.

Thank you for your help and patience, regards

Alejandro

I take a look on your files and I just doing a simulation for wind turbine using cfx and I notes that you assume that your rotational speed is negative
because your rotation is in clockwise . are you got negative value for torque or not,,, because I have counter-clockwise rotation and i have negative value of torque and I think there is a mistake in my simulation
I hope you can answer me
best regards

best regards


All times are GMT -4. The time now is 03:46.