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

Problem in simpleFoam airFoil2D forceCoeffs

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 10, 2013, 08:24
Default
  #21
New Member
 
reza sadeghi
Join Date: May 2013
Posts: 16
Rep Power: 5
reza1111 is on a distinguished road
Hi.
I'am going to simulate a flow around NACA0009 at 5 degree AOA. I used simpleFoam solver and my setup is same as the airfoil2D tutorial. when i get the result, the forces and forceCoeffs are too less than I expected. the ratio of the forces compare with Fluent results are 1:25. I know this is weird. and I guess I did something wrong. I have done the case using Fluent and the results were good.
Please give me some hints.
Thanks
reza1111 is offline   Reply With Quote

Old   July 22, 2013, 17:28
Default
  #22
New Member
 
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 6
Rafael_Coelho is on a distinguished road
I just re-installed Openfoam and will run the airfoil case as a benchmark. Will post some results late this week.
Rafael_Coelho is offline   Reply With Quote

Old   July 28, 2013, 04:33
Default
  #23
New Member
 
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 6
Rafael_Coelho is on a distinguished road
I just ran the airFoil2D case and I got the following results:

forceCoeffs output:
Cm = -15.2719
Cd = -0.231827
Cl = 1.85603
Cl(f) = -14.3439
Cl(r) = 16.2

After 350 interactions.
Rafael_Coelho is offline   Reply With Quote

Old   July 28, 2013, 04:52
Default
  #24
New Member
 
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 6
Rafael_Coelho is on a distinguished road
Changing the liftDir and dragDir as suggested by tcarrigan:

functions
{
forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;

patches ( wall );
pName p;
UName U;
rhoName rhoInf;
log true;
rhoInf 1.225;
liftDir (-0.139173 0.990268 0);
dragDir (0.990268 0.139173 0);
pitchAxis (0 0 1);
magUInf 26;
lRef 1;
Aref 1;
}
}


I got the following Cl and Cd:

forceCoeffs output:
Cm = -15.2719
Cd = 0.0287385
Cl = 1.87023
Cl(f) = -14.3368
Cl(r) = 16.2071

My question now is: How did you (tcarrigan) get those values for liftDir and dragDir?????
Rafael_Coelho is offline   Reply With Quote

Old   October 14, 2013, 03:46
Default hi all
  #25
New Member
 
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 5
wes1204 is on a distinguished road
hi all

I am also facing to same problem.

my case is 2d wind flow around bridge deck.

experimental data is
Cd = 0.245
Cl = 0.028

but my openfoam results were calculated as 0.002, 0.001...
the order of coefficients is quite different to experimental data.

so I did it myself using pressure field.

I extracted pressure value from paraview after slicing mesh to obtain 2d value.
then, I got Force components,generating Normal component of surface and integrating.

this values are almost similar to experimental data
Cd : 0.224
Cl : 0.001

but to do this, I should waste my time and large storage since Values should be 1000Hz.

I dont know why openfoam output is wrong.

my code is same to yours.

functions
{
forces
{
type forces;
functionObjectLibs ( "libforces.so" ); // lib to load
outputControl timeStep;
outputInterval 1;
patches
( bridge ); // change to your patch name

// name of fields
pName p;
UName U;
log true; // dump to file
rhoName rhoInf;
rhoInf 1.25;
CofR ( 2.3 0.7569 0 );
log on;
}
forcesCoeffs
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches
(
bridge );

pName p;
UName U;
log true;
rhoName rhoInf;
rhoInf 1.25;
CofR ( 2.3 0.7569 0 );
liftDir ( 0 1 0 );
dragDir ( 1 0 0 );
pitchAxis ( 0 0 1 );
magUInf 10;
lRef 0.353;
Aref 0.353;
}
}

If you guys solved this problem, please help me
wes1204 is offline   Reply With Quote

Old   October 14, 2013, 04:10
Default
  #26
New Member
 
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 6
Rafael_Coelho is on a distinguished road
Check your liftdir and dragdir axis. It depends on your geometry.
wes1204 likes this.
Rafael_Coelho is offline   Reply With Quote

Old   October 14, 2013, 05:50
Default thanks
  #27
New Member
 
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 5
wes1204 is on a distinguished road
Quote:
Originally Posted by Rafael_Coelho View Post
Check your liftdir and dragdir axis. It depends on your geometry.
Rafael Coelho
thank you for reply

in my case, inlet is left side, outlet is right side and top and bottom is wall,
of course, front and back is empty for 2d.

the object is a deck of bridge so I think directions of drag and lift is right.

I don't know what the problem is.....

anyway thank you for your reply
wes1204 is offline   Reply With Quote

Old   October 14, 2013, 14:51
Default
  #28
New Member
 
reza sadeghi
Join Date: May 2013
Posts: 16
Rep Power: 5
reza1111 is on a distinguished road
Hi Baek

with using checkMesh check the depth of your geometry.
using with fluent in 2d cases the depth be considered a unite. while in OF cases it depends on the depth of your 3d geometry . so the length of the cell in z direction will affect the reference values.

good luck!
reza1111 is offline   Reply With Quote

Old   October 17, 2013, 08:03
Default Thanks
  #29
New Member
 
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 5
wes1204 is on a distinguished road
Quote:
Originally Posted by reza1111 View Post
Hi Baek

with using checkMesh check the depth of your geometry.
using with fluent in 2d cases the depth be considered a unite. while in OF cases it depends on the depth of your 3d geometry . so the length of the cell in z direction will affect the reference values.

good luck!
Hi reza

Thank you for your advise.

I think that this problem is almost sloved.

my case is 2D on x-y plane and z direction has 0.01 length. (5x1.5x0.01)

first, I divided force by z length(0.01).
after that, I calculated Cd,Cl directly using F/(1/2)*rho*U^2*L
finally I got
Cd : 0.29
Cl : 0.1853

observation data in experiment is
Cd: 0.21
Cl: 0.028

Cd is almost similar to observation data but Cl is quite differnt.
I guess that the reason why Cl is quite diffent is due to geometry.

My geometry was simplified quite much.

Thank you for your advise
and I appreciate for Rafael_Coelho's advise
wes1204 is offline   Reply With Quote

Old   March 18, 2016, 09:01
Default
  #30
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 2
giammy92 is on a distinguished road
Quote:
Originally Posted by tcarrigan View Post
You have the x-component of the lift direction backwards, should be -sin(alpha). And the y-component of drag should be sin(alpha).

For the airfoil2D example I get the following results:
Cd = 0.0288648
Cl = 1.86931

Sorry but for airfoil2D example I have U (25.75 3.62 0) and therfore an angle of attack of 8. So, i have liftdir (-sin8 cos8 0) but because the direction of drag is the opposite of flux i think that dragdir (-cos8 -sin8 0). What do you think about?
giammy92 is offline   Reply With Quote

Old   March 18, 2016, 09:04
Default
  #31
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 2
giammy92 is on a distinguished road
Quote:
Originally Posted by tcarrigan View Post
lRef is a reference length and Aref is a reference area. These values are used to compute the coefficients of lift, drag, and pitching moment. Because this is a 2D case and the airfoil has a unit length, therefore, lRef=1 and Aref=1. If this were a 3D calculation, lRef would be something like the mean chord length and Aref could be wing area.

To get Cl there is no need to extract Cp and sum them up for a total lift coefficient. By setting up the appropriate reference values in the forceCoeffs (like below), OpenFOAM will compute Cl for you.

I believe the AOA for the airfoil2D exampel is 8deg. Here are the reference values I used:

forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;

patches ( wall );
pName p;
UName U;
rhoName rhoInf;
log true;
rhoInf 1.225;
liftDir (-0.139173 0.990268 0);
dragDir (0.990268 0.139173 0);
pitchAxis (0 0 1);
magUInf 26;
lRef 1;
Aref 1;
}
Sorry but for airfoil2D example I have U (25.75 3.62 0) and therfore an angle of attack of 8. So, i have liftdir (-sin8 cos8 0) but because the direction of drag is the opposite of flux i think that dragdir (-cos8 -sin8 0). What do you think about?
giammy92 is offline   Reply With Quote

Reply

Tags
airfoil2d, forcecoefficient, simplefoam

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
Trying to run a benchmark case with simpleFoam spsb OpenFOAM 3 February 24, 2012 10:07
SimpleFOAM + SST-Model + problem with convergence A.Devesa OpenFOAM Running, Solving & CFD 0 November 9, 2010 05:43
Can I solve this problem by Fluent? Kai_kc FLUENT 1 October 27, 2010 05:29
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13


All times are GMT -4. The time now is 15:51.