[ngj]

Hi Alessandro

You could try something like this in the command line:

grep -v "<word in header>" forces.dat | tr -d '(' | tr -d ')' > forces.dat.modified

I do not have a forces.dat file available, hence just replace <word in header> with a word from the header. Then it should work without any problems.

Best regards,

Niels

[83_Ale_83]

Originally Posted by ngj

Hi Alessandro

You could try something like this in the command line:

grep -v "<word in header>" forces.dat | tr -d '(' | tr -d ')' > forces.dat.modified

I do not have a forces.dat file available, hence just replace <word in header> with a word from the header. Then it should work without any problems.

Best regards,

Niels

Thank you very much, it does exactly what I was looking for

[AirS]

You should try this:

sed 's/(/ /g' forces.dat > forcesi
sed 's/)/ /g' forcesi > forces

where forces is the same file as forces.dat without the brackets.
Hope it helps!

[jploz]

Hi,

you can use any text postprocessing tool you like (e.g. sed, awk, a perl script) and modify the file (described above).

If you want to remove it directly from the output you will have to create your own version of the forces function object and remove the according lines of source code and recompile it.

HTH.

[83_Ale_83]

Thank a lot for your advises, I take in consideration all of them

[rubenparedes]

Hi,

You can do it in a different way, please check [1]. They recommend to add some lines in the foamLog script.

Ruben

[1] http://www.cfd-online.com/Forums/ope...rces-of15.html

[83_Ale_83]

Hi Ruben,

thank you for the advice but I have changed che controlDict in order to obtain the forces values...I don't know how to obtain forces and coeffs from a log file

functions
{
forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (ala); // change to your patch name
rhoName rhoInf;
rhoInf 1.184; //Reference density for fluid
CofR (1 0 0); //Origin for moment calculations
outputControl timeStep;
outputInterval 1;
}
forceCoeffs
{
// rhoInf - reference density
// CofR - Centre of rotation
// dragDir - Direction of drag coefficient
// liftDir - Direction of lift coefficient
// pitchAxis - Pitching moment axis
// magUinf - free stream velocity magnitude
// lRef - reference length
// Aref - reference area
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (ala);
rhoName rhoInf;
rhoInf 1.184;
CofR (1 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 1);
magUInf 25;
lRef 1; // sphere diameter
Aref 0.1; //1/2 * projected area = pi*r²/2

outputControl timeStep;
outputInterval 1;
}
}

[rubenparedes]

Hi Ale,

I use 1.5 version, but I assume that 1.6 version generates a forces directory where the forces.dat file is saved. Check reply # 19 in [1]

good luck,

R

[SD@TUB]

..., but I assume that 1.6 version generates a forces directory where the forces.dat file is saved.

That's correct.
I'm facing some problems of forces output for several patches. Entering all patch names within

patches (patch1 patch2 patch3 ...);

i get summarized forces and moment for the given patches. But i want to distinguish the forces/moments of each patch. When i repeat

forces
{
...
}

for every patch, the data are seperated but mixed together within ./forces/<firstTimeStep>/forces.dat! I prefer a solution of creating directories for everey patch, like ./forces/patch1/forces.dat, ./forces/patch2/forces.dat and so on. Any advise of handling several patches in functions -> forces is much appreciated...


/Stefan

[rubenparedes]

Hi Stefan,

I am new to OpenFoam and Cpp, so maybe I will say something stupid. Also, I have never worked with multiple patches, what do you mean when you say "for every patch, the data are separated but mixed together within ./forces/<firstTimeStep>/forces.dat"?

I was reading the force.C file, and it looks like in the makeFile() function the force directory is set as:
forcesDir = obr_.time().path()/name_/obr_.time().timeName();

So, I think that changing the "/obr_.time().timeName()" part with a kind of "/patchSet_()[# ID of patch in list?]" could work to get a directory <#IDpatch>/forces.dat.

That makes sense?,

R.

[SD@TUB]

Hello Ruben,

that could be a solution (i didn't try it).
What i did to fix it, is some way easier. Ich changed

forces
{
...
}

in

patchname
{
...
}

within functions{...} and i get different directories for the included patches!

/Stefan

[83_Ale_83]

Hello,
I need to look inside the code of libforces...How I can do it? I would like to know in which way openfoam compute the forces...

[SD@TUB]

In case of 64-bit setup, libforces.so is located at

/usr/local/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libforces.so

In Doxygen the dependencies of forces treatment are listed, see here:
http://foam.sourceforge.net/doc/Doxy...1_1forces.html

Forces are integrated over given walls with patchIntegrate[patchI]. Viscous forces depends on shear stress, pressure forces are related to the pressure field on the wall.

[alexisespinosa]

Following the indications in this thread, I was able to set the force calculation for a flow past a cylinder.

But I have done a lot of runs in the past days without these settings and i want to calculate the forces from the result files that I already have, because running again the cases will be very time consuming. Obvioulsly, it is possible. I just need to read the U and p files for every saved time and use the force functions to calculate forces.

But how can I do that???

Thanks a lot.
Alexis

[rubenparedes]

Hi Alexi,

I think that you can use the "execFlowFunctionObjects" utility, but first you need to include in the controlDict file the forceObject as described above.

R.

[alexisespinosa]

Thanks Ruben,

The execFlowFunctionObjects is working, BUT it creates a result file for every saved time step! That is a problem, but the biggest problem is that it overwrites it each time step. So, at the end I get just one file with the forces for the latest time step that i have saved.

Do you know how to avoid overwriting?? It would be wonderful if execFlowFunctionObjects could work with all the saved timesteps just as if they were being generated in runtime. In that way it would output just one file at the end but with one line per processed time, instead of overwriting.

Thanks,
Alexis

[rubenparedes]

Hi Alexi,

I am not sure about it, but it sounds to me like you are using:
outputControl timeStep;
outputInterval 1;

Maybe you can try using outputTime instead.

Good luck,

R.

[alexisespinosa]

When I use
outputControl outputTime;
Then the utility processes every time directory I have with saved results, but it does not create any file. Nothing!!
When I use
outputControl timeStep;
outputInterval 1;
Then again, execFlowFunctionObjects process every time directory and creates a forces.dat file for every time, but it always overwrite the old one, so it keeps overwriting files and at the end i finish with just one file. The problem is that in every file there is only one line with the calculated forces for that specific time. So, at the end I finish with just the calculated forces for the last time.

Thank you very much.

I also started a thread in OpenFoam_bugs about the execFlowFunctionObjects, I hope that we can also get some hints over there.

Thanks again,

Alexis

[sandy]

Originally Posted by ronaldo

could someone tell me the best way to simulate the Flow over a Cylinder?
Laminare, k-epsilon and k-omega!

k-omegaSST

[83_Ale_83]

We are a little bit off topic, but why you think k-omega SST?