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

Forces on cylinder in Openfoam

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

Like Tree4Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 15, 2012, 08:50
Default Forces on cylinder in Openfoam
  #1
New Member
 
Join Date: Feb 2012
Posts: 6
Rep Power: 5
krsp is on a distinguished road
Hi everyone,

I am trying to determine the forces and the force coefficients on a cylinder in OpenFoam 1.6-ext. I have typed the following in my controlDict file:

libs ("libmyIncompressibleRASModels.so" "libOpenFOAM.so" "libgroovyBC.so");
application osciTurbFoam;
startFrom latestTime;
deltaT 2.7e-4;
writeControl adjustableRunTime;
startTime 0;
stopAt endTime;
endTime 200.0;
writeInterval 1;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression uncompressed;
timeFormat general;
timePrecision 6;
runTimeModifiable yes;
adjustTimeStep yes;
maxCo 0.5;
maxDeltaT 0.01;

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so");
patches (fixedWall);
pName p;
UName U;
rhoName rhoInf;
rhoInf 1000; // Reference density, fluid
CofR (0 0 0); // Origin for moment calculations
outputControl timeStep;
outputInterval 1;
}
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (fixedWall);
// pName p;
// UName U;
rhoName rhoInf;
rhoInf 1000;
CofR (0 0 0);
liftDir (0 0 1);
dragDir (1 0 0);
pitchAxis (0 0 0);
magUInf 0.05; // Free stream velocity
lRef 0.3; // Diameter of cylinder?
Aref 0.0707; // Ref. Area = cross sectional area?
outputControl timeStep;
outputInterval 1;
}
);


My problem is, that in the two directories "forces" and "forceCoeffs" I only get a 0 directory (only one .dat file for each). Does someone know, why the other timesteps do not generate files for forces and force coefficients?

Thank you in advance
krsp is offline   Reply With Quote

Old   March 17, 2012, 09:54
Default
  #2
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
it is correct. the folder name shows the first time step. but it writes timesteps in the files.
niaz is offline   Reply With Quote

Old   March 20, 2012, 21:32
Default
  #3
New Member
 
Join Date: Mar 2012
Posts: 12
Rep Power: 5
November is on a distinguished road
Hi

If you look at the forceCoeffs.C file, the meaning of magUInf, lRef, Aref are quite clear:

Directions for lift and drag forces, and pitch moment
00073 dict.lookup("liftDir") >> liftDir_;
00074 dict.lookup("dragDir") >> dragDir_;
00075 dict.lookup("pitchAxis") >> pitchAxis_;
00076 00077 // Free stream velocity magnitude
00078 dict.lookup("magUInf") >> magUInf_;
00079 00080 // Reference length and area scales
00081 dict.lookup("lRef") >> lRef_;
00082 dict.lookup("Aref") >> Aref_;
...
00118 scalar pDyn = 0.5*rhoRef_*magUInf_*magUInf_;
...
00127 scalar Cl = liftForce/(Aref_*pDyn);
00128 scalar Cd = dragForce/(Aref_*pDyn);
00129 scalar Cm = pitchMoment/(Aref_*lRef_*pDyn);

in your post, I am wondering if the rhoInf should be 1 rather than 1000 for water??
Please point out if I am wrong...
sunshuai likes this.

Last edited by November; March 21, 2012 at 05:13.
November is offline   Reply With Quote

Old   June 13, 2012, 06:25
Default
  #4
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
hello every1,
i am also new to openfoam. i have done similar sim ulation for flow acrodss a cylinder. i get drag n lift forces correctly, i.e accor ding to vortex shedding i am getting variation in lift forces. but the coeff of drag n lift Cd n Cl, i am getting them constant throughout. i am unable ti digest this contrasting behavour.
please guide me thr this.

thanks n regards malhar.
malhar is offline   Reply With Quote

Old   June 15, 2012, 05:00
Default
  #5
New Member
 
Join Date: Feb 2012
Posts: 6
Rep Power: 5
krsp is on a distinguished road
Hi Malhar,

I'll put my answer to your question here, just in case it could be usefull to others I am also quite new to CFD, but I will try to help as much as I can

Just to understand (please correct me if I'm wrong):
You get oscillating drag and lift forces, corresponding to the expected vortex shedding. But your drag and lift coefficients does not oscillate.

Since CD = FD/(1/2*rho*g*D*U^2) and CL = FL/(1/2*rho*g*D*U^2), a quick guess could be, that you have puttet the reference values for either rho, D or U equal to 0 in the controlDict file. (D corresponds to Aref).

And to your other question, you're right, that the total force on the cylinder comes from both pressure differences around the cylinder and from friction. The drag force (also called the in-line force) acts in the direction of the flow, while the lift force acts in the transverse direction.

Regards..
krsp is offline   Reply With Quote

Old   June 15, 2012, 05:04
Default
  #6
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
dear krsp,
thanks for the reply. well u got my problem correctly. i wil post the control dict file which i have employed for this case. then u can easily find out the fault in it.

thanks n regards,
malhar
malhar is offline   Reply With Quote

Old   June 15, 2012, 05:04
Default controldict
  #7
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application icoFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 200;

deltaT 0.01;

writeControl timeStep;

writeInterval 50;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so");
patches (cylinder);
pName p;
UName U;
rhoName rhoInf;
rhoInf 1000; // Reference density, fluid
CofR (-2.5 0 0); // Origin for moment calculations
outputControl timeStep;
outputInterval 50;
}
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (cylinder);
// pName p;
// UName U;
rhoName rhoInf;
rhoInf 1000;
CofR (-2.5 0 0);
liftDir (-2.5 0.5 0);
dragDir (-2 0 0);
pitchAxis (-2.5 0 0);
magUInf 1; // Free stream velocity
lRef 1; // Diameter of cylinder?
Aref 3.142; // Ref. Area = cross sectional area?
outputControl timeStep;
outputInterval 50;
}
);

// ************************************************** *********************** //
malhar is offline   Reply With Quote

Old   June 15, 2012, 05:10
Default
  #8
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
forcesMoments fm = forces::calcForcesMoment();

scalar pDyn = 0.5*rhoRef_*magUInf_*magUInf_;

vector totForce = fm.first().first() + fm.first().second();
vector totMoment = fm.second().first() + fm.second().second();

scalar liftForce = totForce & liftDir_;
scalar dragForce = totForce & dragDir_;
scalar pitchMoment = totMoment & pitchAxis_;

scalar Cl = liftForce/(Aref_*pDyn);
scalar Cd = dragForce/(Aref_*pDyn);
scalar Cm = pitchMoment/(Aref_*lRef_*pDyn);



above is the code written in the forceCoeffs.C file for calculating the Cl, Cd,Cm. i am not understanding what are time(), first(), second()

malhar
malhar is offline   Reply With Quote

Old   June 15, 2012, 05:49
Default
  #9
New Member
 
Join Date: Feb 2012
Posts: 6
Rep Power: 5
krsp is on a distinguished road
I don't understand the directions you typed for drag and lift. If your steady flow runs parallel to the x-axis, I think they should be something like:

liftDir (0 0 1); (OR (0 1 0); if the y-axis is your vertical axis)
dragDir (1 0 0);

Also I think your outputInterval is quite high. If your time step is 0.01s, you only get the results for every 0.5s. Just make sure, that it is often enough to capture the vortex shedding frequency.
To your reference area I would put it equal to the cylinder diameter. (Of course that depends on which formula you refer to, but that is what is done in the book "Hydrodynamics around cylindrical structures" by B. Mutlu Sumer and Jørgen Fredsøe)

Finally as posted above, I think that if you solve an incompressible problem rhoInf should be 1 instead of 1000, because the value is already included in the pressure..

Hopefully this will help a bit
krsp is offline   Reply With Quote

Old   June 15, 2012, 05:56
Default
  #10
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
dear krsp.....
it may be co-incidental... there u found out the fault n here me too:-)...i got dat prob. i have set the code to run. wil msg u the results once i get them.

thank you very very much.

wishes,
malhar
krsp likes this.
malhar is offline   Reply With Quote

Old   July 2, 2012, 18:03
Default
  #11
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
i've just done the simulation around cylinder and use above controlDict. in Re=150 experiment data says Cd=1.5 but i get Cd=1.6 that is not accurate. i changed my mesh(gambit) better(more resolution) and used smaller time step(0.01) but the result became worse! Cd=2.7 ??!!!
i dont know what did happen? with a better mesh and smaller time step and similar other conditions my result became worse!
please help what maybe happened that i got this bad result!??
amin66 is offline   Reply With Quote

Old   July 3, 2012, 00:35
Default
  #12
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
dear amin,
wat is ur domain size?? is ur cylinder in a confined channel??? wat inlet boiundary condition have you taken???

regards Malhar.
malhar is offline   Reply With Quote

Old   July 3, 2012, 10:11
Default
  #13
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
dear malhar

1. for curved mesh and time step=0.1 taken this result for Cd:
fluent:1.484 , Openfoam:1.6 , experiment:1.5

2. for rectangular domain mesh and timestep=0.001 taken this result for Cd:
fluent:1.32 , Openfoam:2.55 , experiment:1.5

velocity inlet condition for inlet
Attached Images
File Type: png Untitled1.png (26.2 KB, 125 views)
File Type: jpg Untitled.jpg (65.2 KB, 178 views)
File Type: jpg Untitled3.jpg (70.0 KB, 162 views)
File Type: jpg Untitled4.jpg (94.2 KB, 152 views)
sunshuai likes this.
amin66 is offline   Reply With Quote

Old   July 3, 2012, 13:15
Default
  #14
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
dear Amin
i wanted to know your type of boundary conditin. have you taken fully developed flow condition i.e parabolic for your prob at inlet???? if nt den its necessary if ur upstream length is nt enough long for the flow to get developed. most probably the incorrectness in Cd Cl is because of dat.
regards,
Malhar
malhar is offline   Reply With Quote

Old   July 3, 2012, 13:15
Default
  #15
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Dear amin
your solution does not converge change the number of correction in cvsolution text.
but i am sure that the openfoam predict drag more than real value.
it may occure because of pressure calculation
niaz is offline   Reply With Quote

Old   July 3, 2012, 14:24
Default
  #16
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
dear malhar, i attached my case study.

dear niaz, how can i know that my solution has converged or not? and how can plot the residuals like fluent?
Attached Files
File Type: zip cylinder.zip (5.5 KB, 138 views)
amin66 is offline   Reply With Quote

Old   July 3, 2012, 14:42
Default
  #17
New Member
 
Malhar Malushte
Join Date: May 2012
Posts: 16
Rep Power: 5
malhar is on a distinguished road
dear Amin,
i am too new to OF...even i dont know how to know that solution has converged or nt and to plot residuals.....in fact i am nt understanding wat u meant by convergence in ur case n how it may be related to ur prob.
malhar is offline   Reply With Quote

Old   July 3, 2012, 15:18
Default
  #18
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Dear amin
I check it by saving it in a text file. and check it by eye.
secondly, It is a point which I catch it by experiment. if you import meshes from other sources, you need to do more loops for convergance of solution. try it

Quote:
Originally Posted by amin66 View Post
dear malhar, i attached my case study.

dear niaz, how can i know that my solution has converged or not? and how can plot the residuals like fluent?
niaz is offline   Reply With Quote

Old   July 3, 2012, 15:22
Default
  #19
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
other points, your mesh shows that your blockage ratio is not enough. so don`t compare your result with one which has wider blockage ratios.
it is important point. you can find this point in a paper from sanjey mittal.
only search it. it is in his site
niaz is offline   Reply With Quote

Old   July 3, 2012, 16:53
Default
  #20
Member
 
Amin
Join Date: Mar 2012
Posts: 60
Rep Power: 5
amin66 is on a distinguished road
Dear A_R, tnx for your attention. i just say in rectangular domain mesh i have wider blockage ratio and more node numbers than the curved domain mesh.(as you can see up the pictures) but the result became worse.
amin66 is offline   Reply With Quote

Reply

Tags
forces and force coeff.

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
forces in interFoam Svensson OpenFOAM Post-Processing 2 May 9, 2012 13:31
New OpenFOAM Forum Structure jola OpenFOAM 2 October 19, 2011 06:55
FORCES don't run! C12Carbon OpenFOAM 0 September 10, 2011 07:34
Summer School on Numerical Modelling and OpenFOAM hjasak OpenFOAM 5 October 12, 2008 13:14
OpenFOAM Training and Workshop Hrvoje Jasak Main CFD Forum 0 October 7, 2005 07:14


All times are GMT -4. The time now is 08:07.