CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

"libforces.so" reporting too low values for forces on airfoil.

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

Like Tree3Likes
  • 1 Post By haakon
  • 1 Post By hakonbar
  • 1 Post By hakonbar

Reply
 
LinkBack Thread Tools Display Modes
Old   March 8, 2013, 10:43
Default "libforces.so" reporting too low values for forces on airfoil.
  #1
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 4
hakonbar is on a distinguished road
Hi everyone!

My name is Håkon Line, and I'm a mechanical engineering student at the NTNU, Trondheim. I started using OpenFOAM about half a year ago, and am now using it for my Master's thesis. I'm posting here because I've recently hit upon a problem which at first I thought would be trivial, but which has me completely stumped. Any help would be immensely appreciated, as I still have a long way to go and my deadline is fast approaching =)

I'm simulating a classical benchmark case, the naca0012 foil at Ma = 0.15, Re = 6*10⁶ (http://turbmodels.larc.nasa.gov/naca0012_val.html). I'm using simpleFoam with the SA-model and 2nd order upwind convection schemes. The mesh is generated with SHM. The airfoil is generated from the equation given at the previously linked-to webpage, and converted to stl-format by the utility "points2stl" developed by Alejandro Roger.

Now, my problem is that the forces on the wing, as calculated by the utilities in 'libforces.so' are way too low:
(Cl = 0, 0.104 and 0.193 for alpha = 0, 5 and 10 degrees, respectively)
(Cd = 0.0019, 0.0023 and 0.0041 for alpha = 0, 5 and 10 degrees, respectively)

As these values are several times smaller than they should be, I suspect a multiplying factor is off somewhere, but I've no idea where that may be. The values for the lift and drag coefficients are consistent with the forces reported in forces.dat, so the error doesn't lie with the non-dimensionalization.

Furthermore, when I retrieve the surface normals and the surface pressure from paraView, and use that to find the pressure distribution and lift on the wing, my results closely match the validation data.

Since my pressure distribution is ok, I guess I could ignore the bad data produced by libforces, but I'm going to simulate this and similar shapes in pimpleDyMFoam, and I want to make sure that the forces "seen" by the wing are correct before I proceed. Where should I start looking?

best regards,
Håkon Line

I'm attaching a dropbox-link to one of my run cases:

http://dl.dropbox.com/u/21618777/12a10simpleSA.zip
hakonbar is offline   Reply With Quote

Old   March 15, 2013, 13:14
Default
  #2
Senior Member
 
Håkon Strandenes
Join Date: Dec 2011
Location: Norway
Posts: 111
Rep Power: 10
haakon will become famous soon enough
Ok, Håkon, I have had a quick look at the case you provided and think I might have spotted your mistake:

The first thing I did was to check your mesh and patches. This seemed OK, and I found that your arifoil had a chord of 1 m and span of 0.2 m. This gives a reference area of 0.2 m^2. Please be aware of the fact that your STL-file has a span of 1 meter, but your mesh is only 0.2 meter thick. This is due to the thickness setting in extrudeMeshDict.

Then I found the freestream velocity to be 51 m/s, and the density to be 1 kg/m^3. By looking the output from the forces command I found that at the last step, the force in the lift direction (y) was 251.4 N.

By using the usual formula for lift coefficient, C_L = F_L / (0.5*rho*U^2*A) I calculated your lift coefficient to be 0.967. This seems to be approximately in agreement with the numbers predicted by http://turbmodels.larc.nasa.gov/naca0012_val.html for alpha = 10 degrees (quick graphical readout). You have however not given (and I can't find) what the exact angle of attack is, but from the file name I assume it's 10 degrees.

So the conclusion is that you have used wrong area in the forceCoeffs-definition. You have specified Aref 1.0, while you should have specified Aref 0.2. This is the reason for your low lift and drag coefficients.

As a sidenote: have you seen this tutorial/webpage: https://www.hpc.ntnu.no/display/hpc/...l+Calculations ? It is by no means a perfect airfoil setup or simulation, but it includes some nice features, especially on the meshing part. On that page you can find generators for both STL-solids and C-meshes for common NACA 4-digit airfoils. Be aware that the case is made for OpenFOAM 2.1, and not 2.2. Some modifications are needed to have it working in 2.2.
s.m likes this.
haakon is offline   Reply With Quote

Old   March 16, 2013, 07:03
Default
  #3
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 4
hakonbar is on a distinguished road
Thanks a lot! Man, I can't believe I overlooked that bit. It really helps with a fresh pair of eyes when you've stared yourself blind at a problem. =)

EDIT: I've also been made aware of a bug in 2.2.0 - if the body on which you'd like to measure the forces consists of several patches, only the force on the last patch will be written to file (http://www.openfoam.org/mantisbt/view.php?id=773). This bug has been ironed out in the latest git release (http://www.openfoam.org/download/git.php).

Last edited by hakonbar; March 18, 2013 at 09:48.
hakonbar is offline   Reply With Quote

Old   July 12, 2013, 06:42
Default
  #4
New Member
 
Julio Silveira
Join Date: Feb 2013
Location: London
Posts: 15
Rep Power: 4
biau is on a distinguished road
You should change this lines on your controDict for every angle of attack

liftDir (0 1 0);
dragDir (1 0 0);

e.g.

liftDir (0.05233 0.99863 0)
dragDir (0.99863 0.05233) 0)
biau is offline   Reply With Quote

Old   July 16, 2013, 13:16
Default
  #5
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 4
hakonbar is on a distinguished road
Hi biau,

In this case, the foil was at an angle, and the incoming flow was in the positive x-direction, so there was no need to change the reference directions away from the default.
s.m likes this.
hakonbar is offline   Reply With Quote

Old   August 13, 2013, 14:59
Default
  #6
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 6
s.m is on a distinguished road
Quote:
Originally Posted by hakonbar View Post
Hi biau,

In this case, the foil was at an angle, and the incoming flow was in the positive x-direction, so there was no need to change the reference directions away from the default.
Dear hakonbar, for applying the angle of attack to our simulation, is it true to write the velocity of flow over an airfoil e.g (50 0 0),and use the "transformPoints" utility to rotate the domain and the airfoil e.g 15 deg?
instead of writing the velocity (50cos(alpha=15) 50sin(alpha=15)) we write the velocity (50 0 0) and rotate the domain 15 degree by "transformPoints" utility.
i attach the pictures clarifying my question.
Thank you
Attached Images
File Type: jpg angle-of-attack-15.jpg (10.1 KB, 19 views)
File Type: jpg angle-of-attack-0.jpg (8.8 KB, 14 views)
s.m is offline   Reply With Quote

Old   August 14, 2013, 06:12
Default
  #7
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 4
hakonbar is on a distinguished road
Yep, that's correct! If your foil is a 4-digit NACA foil, you can use Håkon Strandenes' foil generator (link further up in the thread). This one lets you set the angle of attack of the foil when you create it, so you don't have to rotate the whole domain.
s.m likes this.
hakonbar is offline   Reply With Quote

Old   August 14, 2013, 07:30
Default
  #8
s.m
Senior Member
 
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 6
s.m is on a distinguished road
Quote:
Originally Posted by hakonbar View Post
Yep, that's correct! If your foil is a 4-digit NACA foil, you can use Håkon Strandenes' foil generator (link further up in the thread). This one lets you set the angle of attack of the foil when you create it, so you don't have to rotate the whole domain.
Thank you very much, actually i have multi element airfoil for my analysis, now i am working on one element airfoil.
any way, i understand from your explanation that there is no difference between rotating domain and applying the alpha to our initial velocity,
do i get it right?
s.m is offline   Reply With Quote

Old   August 15, 2013, 08:38
Default
  #9
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 4
hakonbar is on a distinguished road
Exactly. The drag component of the force is parallel with the flow direction, and the lift component is normal to it, pointing upwards for positive lift, and downwards for negative.
hakonbar is offline   Reply With Quote

Reply

Tags
airfoil2d, lift and drag

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
cl,cd data for pitching/plunging airfoil at low Re Quarkz Main CFD Forum 1 August 9, 2011 03:11
what defines a low Re number for airfoil flows? Rif Main CFD Forum 1 January 13, 2008 02:07
Low Speed Airfoil Max Main CFD Forum 1 March 13, 2007 18:24
About low Reynolds number airfoil experiment data. zqnwpu Main CFD Forum 5 December 25, 2004 04:52
Low Reynolds number for airfoil Richard Main CFD Forum 1 March 20, 2000 08:24


All times are GMT -4. The time now is 03:07.