Hi Frank, I needed the mean
 

Hi Frank,

I needed the mean fixed pressure boundary condition for some other stuff... so I've now implemented one. For the case I'm looking at it behaves pretty well. If you'd like to re-visit your vortex shedding simulations with the new outlet b.c. please give me a shout and I'll pass over the code.

It bothers me a little bit that OpenFOAM did not perform the way I've expected (pride is a sin, I know) :-) and this may bring some closure to the problem...

Hrv

That would be very nice. I wil
 

That would be very nice. I will just see how the new BC behaves for my problem.

While finishing a paper on previous work, I am still working on these cylinder flows using OpenFOAM, I varied grid and time step size. My main issues at this time are:

* I did not succeed in getting a grid independent solution.
* I like to verify if the bahaviour of the solver is indeed second order accurate (in space and time).

Possibly the new BC could shed some light on these problems. As soon as I get some fruitfull results I will post them on a website.

Regards, Frank

Hi Frank, Can you please po
 

Hi Frank,

Can you please post the source code you used to obtain the frequency of the flow. I'm trying a similar problem using Openfoam and since I'm not too good in C++, I'm looking for some help. I don't know exactly how to compile and use the probe, so some instructions should be useful.

Thanks very much for your help!

Just after the runTime.write()
 

Just after the runTime.write() call in the icoFoam.C file, I put the following header file

#include "computeForces.H"

This file includes some code to calculate the lift, drag and moment and output the values to screen. This code is taken from the liftDrag utility.

When the lift/drag are written to screen, the foamLog routine is used to write the lift/drag histories to files. Finally these files are read into matlab for post-processing, the frequencies is only one thing I am looking at.

If you still got some difficulties with this, I could send you the source code by mail, if you want.

Regards, Frank

Fantastic! Thanks a lot. I'll
 

Fantastic! Thanks a lot. I'll give it a try as soon as I can.

Hi Frank, So all I need to
 

Hi Frank,

So all I need to do is edit icoFoam.C in the ~/OpenFOAM/OpenFOAM-1.3/applications/solvers/incompressible/icoFoam directory and include a reference to the computeForces header file?

Do I have to recompile OpenFoam to get this to work? Also, how does the foamLog routine work? Do I have to run it after the case has converged or before?

Thanks for your help!

You have to create your own cr
 

You have to create your own createForces.H file. I simply took some stuff from the liftDrag utility, the part where the force are being calculated.

Furthermore I would create your own solver, for example: icoMySolverFoam in your user application directory. Try not to change the original code, instead create your own solvers, utilities and libraries. As a start copy and rename icoFoam to you user's application directory. Then try the stuff I mentioned before involving createForces.H etc...

Frank

Does anybody know why the Cour
 

Does anybody know why the Courant number is still significant. Isn't Crank Nicholson supposed to be an implicit scheme which is unconditionally stable (as Frank mentioned)?

I think both stability and acc
 

I think both stability and accuracy should be noticed.
Though I am little confused why Frank said,

"The max courant number which corresponds to the chosen time step (0.02) was between 1.7 and 1.9. I also performed computations with half of the time step (0.01) such that the max Courant = 0.8 - 0.9. In that case the vortex wake was also similar."

It should be a little little different in someplaces that may have not been awared of.

http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Daniel

What?
 

What?

Hello Frank and hello Foamers,
 

Hello Frank and hello Foamers,

I have trouble in the flow over circular cylinder case, could you give me some advice?

1. May I know which reference are you reading for Re=150?
2. How did you set the inlet velocity profile?
3. Are you sure that the ddtSchemes with "CrankNicholson 0.5" is good for the case? I have compared the following
a) CrankNicholson 0.5;
b) CrankNicholson 0.9;
c) Euler;
d) backward;
and I found:
1) Courant number does not change the solution significantly as you said;
2) The Cd values of CrankNicholson are higher than those of Euler and backward, I don't know which are more accurate?

Not only that, my geometry is exactly as the one in Ferziger's book, see the pic below, but my average Cd (3.415) is higher than the book's (3.228)!
What might go wrong?
http://www.cfd-online.com/OpenFOAM_D...your_image.gif
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

Thanks...

\Daniel

http://www.cfd-online.com/Open
 

http://www.cfd-online.com/OpenFOAM_D...your_image.gif
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

Thanks...

\Daniel

http://www.cfd-online.com/Open
 

http://www.cfd-online.com/OpenFOAM_D...ges/1/9201.jpg
http://www.cfd-online.com/OpenFOAM_D...ges/1/9202.jpg

Thanks...

\Daniel

Sorry for that, Chrome is stil
 

Sorry for that, Chrome is still green, I have to use IE. \Daniel

Hi all, I'm currently using
 

Hi all,

I'm currently using openFoam on the flow around
a cylinder in order to better understand the code
parameters and post-processing functionalities.
I see that some of you are using a lift/drag utility. That would be a very useful tool which
doesn't seem to be implemented in the version I have (1.4).
Could someone tell me where I could find an updated version of the lift/drag utility?
(and possibly a short guide or description of
what it does).

Thanks very much for your help

Seb

Look at this link, http://www
 

Look at this link,
http://www.cfd-online.com/OpenFOAM_D...tml?1212507143

Good luck, Seb!

\Daniel

Thanks Daniel, I am testing
 

Thanks Daniel,

I am testing a similar case,flow around a cylinder at Re=100.
I'm using icoFoam, and I'm looking at the drag coefficient and vortex shedding frequency.
After checking that the results are time step independent, I varied the divScheme.
I found that the best results (providing my experimental results that I'm using as a reference are accurate enough) are obtained using
Gauss Linear, and not the upwind scheme. For the moment, I only tried these two, and I just find a bit strange that Gauss Linear gives me better results. Is this scheme centered?

Thanks for any comment you could make on this,
it will be helpful.

Hi Sebastien, Try also the
 

Hi Sebastien,

Try also the vanLeerV scheme for convection. This gives nice vortex preserving results for me.

Frank

Hi Frank! I want to do a si
 

Hi Frank!

I want to do a simulation of FSI of a bridge deck (A very high Re), could you recommend me some papers on FSI.

{I have paid a lot of focuses on DES and DDES tech for the last several months, but I'm afraid they are still unaffordable. http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif}

Thank you very much.

Daniel

Hi Sebastien, Gauss Linear i
 

Hi Sebastien,
Gauss Linear is simply central differencing. If it does not result in any numerical instability for you then why not keep it. 2nd order is all good.
Frank recommends vanLeer, which simply blends with upwind, for stability's sake, in which case limitedlinearV is not bad either...

Ciao

Pierre