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

Domain format problem on airfoil flow simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 17, 2010, 22:56
Default Domain format problem on airfoil flow simulation
  #1
New Member
 
André H. Nonaka
Join Date: May 2010
Posts: 3
Rep Power: 7
andrenonaka is on a distinguished road
Hello, I'm studying the CFX area for some projects at my university, and I'm having some problems...

I'm doing some tests, and basically I need to simulate the flow over a wing made from an Eppler 423 airfoil. I got the wing dimensions from books, and I got the real results for Lift and Drag of it so I can compare them with the ones I get on the simulation.

First, I tried the rectangular domain with a symmetry wall. After some tries, I got an error of 2~5% for Lift and Drag, not a bad range for our project. But I can't simulate various angles of attack on a rectangular domain, because the flow always leave the domain normal to the outlet and would not represent the true flow of the air, and to create one domain for each angle would be frustrating, so I tried a Cylindrical and Spherical domain approach, then I could vary the cartesian velocity components and the flow would be right.

The results for the Lift in these two kinds of domain were all good, with almost the same error range of the rectangular one. But the drag got a 75% error...
I can't figure out the problem, because the velocity and pressure gradients are fine, and I used the same domain values configuration and same mesh quality for all tests... the only major change I did between the simulations were the domain outlets (I couldn't use outlet for cylindrical and spherical, so I used opening).

What could be the problem? Is this kind of domain unusable for wing flow simulations?

Thanks in advance.

And sorry for the bad english...
Attached Images
File Type: jpg rectangular domain.jpg (25.9 KB, 74 views)
File Type: jpg cylindrical domain.jpg (28.8 KB, 60 views)
File Type: jpg spherical domain.jpg (27.6 KB, 62 views)
andrenonaka is offline   Reply With Quote

Old   May 18, 2010, 03:43
Default
  #2
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Hi,

at the first look I recommend you to use much bigger domains, to avoid the effect of the boundaries. Far from the airfoil you can use bigger elements, so you will get not so more cells. Check the image about the mesh at my post:

NACA 0012 Different Angles of Attack

the little point in the middle is the airfoil

With this setup you can use inlet and outlet, or opening-outlet boundaries.
The accuracy of the cl-cd calculations depends on the near-wall mesh around the airfoil. Of course, you should have a resolved boundary layer, for example for SST: yplus above 2 and at least 15nodes in boundary layer.

Regards
Attesz is offline   Reply With Quote

Old   May 18, 2010, 13:08
Default
  #3
New Member
 
André H. Nonaka
Join Date: May 2010
Posts: 3
Rep Power: 7
andrenonaka is on a distinguished road
Thanks for your help, Attila! I'm trying out the bigger domain, as you suggested, but Im not sure what to do about the size of the elements. I'm creating the mesh in wokbench, and using the patch conforming method with tetraedrons. Im also using an inflation, with 15 layers, altought I cant see it at all in the Spherical domain. What would you recommend for adjusting the elements near the wing? Maybe I should use another method or software for mesh generation?
andrenonaka is offline   Reply With Quote

Old   May 18, 2010, 13:19
Default
  #4
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
15 layer is a good start. Do not go under this value.

Around a simple airfoil a good structured hexahedral C mesh can be easily generated. But CFX mesher is not a professional tool..if you have, try ICEM CFD, I think, there is a tutorial for wing or something like that too. However, an unstructured tetrahedral mesh can be also good in your case. Near the wing use as fine mesh as you can do, and avoid huge expansion ratios. Far from the wing you can use significantly bigger elements, but watch the expansion ratios here too. If you get big size difference between the last boundary layer cell and the first tetra(or pyramid), than use more inflation layers.

Regards
Attesz is offline   Reply With Quote

Old   May 19, 2010, 17:39
Default
  #5
New Member
 
André H. Nonaka
Join Date: May 2010
Posts: 3
Rep Power: 7
andrenonaka is on a distinguished road
Attila, I have ICEM here and I took a look at the tutorials, and it looks like a much better geometry and mesh generator, but it seems a little more complex too... I will need a lot of time to get used to it. And I would like to finish this experiment at CFX mesher first, as soon as possible, cuz everyone is putting pressure on me at the university... the project depends on this step to move on, you see...

About the mesh, I did a lot of tests with bigger domains (the last I tried was 200 times the airfoil chord) and some face sizing, and the error got a lot smaller, but I still get wall interference (I can see velocity and pressure changes near them) and it seems I can't inflate the method anymore, it says that the pre-inflation layer generation are ignored for the faces...

I really needed something else than the face sizing to control the mesh quality around the airfoil. Any suggestions of what could be happening or another kind of method for me to use?

Thanks again!

Last edited by andrenonaka; May 19, 2010 at 17:57.
andrenonaka is offline   Reply With Quote

Old   May 21, 2010, 09:00
Default
  #6
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
I used CFX mesher not too long. Its really simple, but not smart enough.

Search, and ask your problem in http://www.cfd-online.com/Forums/ansys-meshing/ .

Good luck!
Attesz is offline   Reply With Quote

Old   December 4, 2014, 04:57
Default
  #7
New Member
 
Join Date: Oct 2014
Posts: 9
Rep Power: 2
Jayakanth is on a distinguished road
Hi, I am facing a similar problem. I will be using a rectangular domain over a stratosail object. I need to simulate various angle of attacks. What should my domain be for accurate results?
Jayakanth 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
Boundary condition problem for open channel flow Andy CFX 8 October 1, 2012 07:45
Problem in the flow calculation around airfoil swlee OpenFOAM Running, Solving & CFD 3 September 9, 2010 11:51
Residual problem of 2D airfoil simulation caohan FLUENT 9 April 13, 2010 16:03
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
About the invisd flow around an airfoil maximus Main CFD Forum 1 July 16, 2005 15:04


All times are GMT -4. The time now is 19:25.