CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Wind turbine simulation in Ansys CFX

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 9, 2013, 19:01
Default Wind turbine simulation in Ansys CFX
  #1
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   September 10, 2013, 05:51
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   September 10, 2013, 17:41
Default
  #3
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   September 30, 2013, 05:39
Default
  #4
Member
 
ijaz fazil
Join Date: Apr 2013
Posts: 32
Rep Power: 4
er_ijaz is on a distinguished road
Hi r using sliding mesh or MRF analysis?
er_ijaz is offline   Reply With Quote

Old   September 30, 2013, 18:25
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   September 30, 2013, 23:56
Default
  #6
Member
 
ijaz fazil
Join Date: Apr 2013
Posts: 32
Rep Power: 4
er_ijaz is on a distinguished road
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
er_ijaz is offline   Reply With Quote

Old   October 10, 2013, 11:14
Default
  #7
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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.



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
aalbanesi is offline   Reply With Quote

Old   October 10, 2013, 17:19
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
sagarmore likes this.
ghorrocks is online now   Reply With Quote

Old   October 10, 2013, 19:38
Default
  #9
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   October 10, 2013, 20:28
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   October 11, 2013, 08:14
Default
  #11
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   October 12, 2013, 06:37
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is online now   Reply With Quote

Old   October 15, 2013, 07:53
Default
  #13
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   October 15, 2013, 19:47
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   October 16, 2013, 08:03
Default
  #15
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
Thank you. It is very clear now.

Regards, Alejandro
aalbanesi is offline   Reply With Quote

Old   October 17, 2013, 11:41
Default
  #16
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   October 20, 2013, 19:55
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is online now   Reply With Quote

Old   October 21, 2013, 09:53
Default
  #18
New Member
 
Alejandro Albanesi
Join Date: Sep 2013
Posts: 11
Rep Power: 3
aalbanesi is on a distinguished road
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
aalbanesi is offline   Reply With Quote

Old   October 21, 2013, 17:27
Default
  #19
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   November 8, 2013, 03:55
Default rotational speed
  #20
New Member
 
sattar
Join Date: Dec 2011
Posts: 15
Rep Power: 5
drsattar is on a distinguished road
Quote:
Originally Posted by aalbanesi View Post
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
drsattar is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ANSYS Meshing] 3d wind turbine mesh for multiphase simulation mingersai ANSYS Meshing & Geometry 0 January 17, 2012 19:20
2D Simulation of Savonius Wind Turbine ravindersingh FLUENT 4 December 9, 2011 14:00
CFD analysis on wind turbine rotor Ken (Wind Turbine CFD Super Rookie) Main CFD Forum 42 July 18, 2011 22:11
[Other] ANSYS CFX-Meshing problem of a wind turbine blade Zoe ANSYS Meshing & Geometry 1 July 14, 2010 02:02
wind turbine simulation moca CFX 1 July 25, 2009 06:48


All times are GMT -4. The time now is 06:04.