[Eren10]

Originally Posted by boger

I just pasted your entry (with the modifications I already mentioned) into my controlDict and I got the desired output in forces/0/forceCoeffs.dat.

this is really strange, there happens nothing at mine case ( the case is running well)

this is mine controlDict. ( i am using 1.7.1 version )

FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application icoFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 0.5;

deltaT 0.0005;

writeControl timeStep;

writeInterval 20;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

functions
(
forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches
(
AirFoil
);
pName p;
UName U;
log true;
rhoInf 1;
CofR ( 0 0 0 );
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis ( 0 0 1 );
magUInf 25;
lRef 1;
Aref 1;
}
);

[boger]

I'm using 1.6-ext, so if there's a difference caused by 1.7.x, I'm not familiar with it.

[Eren10]

how can I see the content of libforces.so (any lib file ) ?

If someone here uses 1.7x version please check for me if the libforces.so works as I have cited here .

[boger]

Content of the library? Do you mean the source code? You can see it here. Go to "classes" and then pick "forces" from the list.

[Eren10]

Originally Posted by boger

Content of the library? Do you mean the source code? You can see it here. Go to "classes" and then pick "forces" from the list.

Thank you. I am trying to understand how the calculations are programmed and I am looking what the possibilities are. maybe after this I can use the abilities of OpenFOAM much better

[aerothermal]

Dear foamers,

the sampleDict sent by velezisaza worked well for me.
i am working to get Cp from a cylinder in a tunnel.
however, the sample tool provided me all data on patch.

How can I extract pressure information in a line, i.e., in the patch intersection with a plane (like normal to Z and at 0,0,0) ? Should I do it by hand? Does openfoam have a tool for this?

regards,

[Akuji]

Hello!

I've got a question about
liftDir (0 1 0);
dragDir (0 0 1);
pitchAxis (0 0 0);

liftDir and dragDir : Lift and Drag direction vectors are specified

. But, if I ser liftDir (0 0.1 0) I have another result of Cd. So, how is right to set lift and drag Dir?


And, what is pitchAxis? I blow on a box, Did I need it?

[jms]

Dear all,

I am using this function that it is needed in controlDict in orer to get the lift, drag and moment coefficients for a computation of the flow around an airfoil. The results I get for the lift and drag coefficients are very good compared to the reference I am using for both lift and drag coefficients but they are very bad for the moment coefficients. I use CofR=0.25*chord.
Any idea why I am getting this bad results?

Thanks,

José

[anijdon]

hello.
I want to figure drag coefficient on walls of a cube which is located in a flat plane in 3D. I put

·rhoInf : the density of fluid.

·MagUinf : uniform velocity in the upstream of cube.

·Aref : the area of each cube's surface

· lref :the length of each cube's edge

· dragDir : flow direction (Uinlet=(1,0,0) in 0 directory)

but this result is not true. would you tell me my mistakes?

thanks.

[Eren10]

Hi,

I have only replaced the mesh on the tutorial incom/simplefoam/airfoil2D. I want to check the Cl , Cd values. the airfoil size is the real size on the mesh.

But I get nonsense values. I am using openfoam 1.7.1, with the following function:

functions
{
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (UpperCamber LowerCamber TrailingEdge);
log true
pName p;
Uname U;
rhoName rhoInf;
rhoInf 1.225;
magUInf 25;
CofR (0.25 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 -1);
lRef 1;
Aref 1;

outputControl timeStep;
outputInterval 1;
}
}


How can I solve this issue . Because I am using the tutorials I assume that the flow is correct.

[Eren10]

Can someone please obtain the Cl, Cd, Cm values for the tutorial case , incompressible/simpleFoam/airFoil2D

I am using 1.7.1 version, I can't get the right values. I am almost thinking of a bug

[Akuji]

Originally Posted by Eren10

Can someone please obtain the Cl, Cd, Cm values for the tutorial case , incompressible/simpleFoam/airFoil2D

I am using 1.7.1 version, I can't get the right values. I am almost thinking of a bug

Did you try to change patches?

[Eren10]

Originally Posted by Akuji

Did you try to change patches?

I have tried to get the coefficients for the given mesh in the tutorial (airFoil2D) as well as the mesh that I have drawn, both failed

Can someone maybe write here the obtained coefficients of tutorial airFoil2D case ? I will compare it with obtained value of the 1.71 version.

[Eren10]

can someone help me about this issue ?

[Eren10]

I have obtained lift and drag from forceCoefficients. I have also calculated lift and the drag using the data of wallShearStress and the pressure distribution.

The results are:


Cd Cl
forceCoeff: 0.0113219 0.339877

calculatedMatlab: 0.009311 0.33927


Cl value is close, but the discrepancy of the Cd value is too big. From the experiments the Cd value should be around 0.00889 (airfoil).
Am I doing something wrong ? or is it the forceCoeffs ??????


*if someone wants to test it I can send mine matlab file.

[Eren10]

Originally Posted by Eren10

I have obtained lift and drag from forceCoefficients. I have also calculated lift and the drag using the data of wallShearStress and the pressure distribution.

The results are:


Cd Cl
forceCoeff: 0.0113219 0.339877

calculatedMatlab: 0.009311 0.33927


Cl value is close, but the discrepancy of the Cd value is too big. From the experiments the Cd value should be around 0.00889 (airfoil).
Am I doing something wrong ? or is it the forceCoeffs ??????


*if someone wants to test it I can send mine matlab file.

When I multiply the value of the calculatedMatlab with the density 1.225, I get 0.0114, almost the same value from forceCoeffs.

Can someone please explain why I have to multiply the " skin friction coefficient ( obtained from the wallShearStress" with the density to get the same value ? ( incompressible flow)

[Akuji]

Originally Posted by Eren10

When I multiply the value of the calculatedMatlab with the density 1.225, I get 0.0114, almost the same value from forceCoeffs.

Can someone please explain why I have to multiply the " skin friction coefficient ( obtained from the wallShearStress" with the density to get the same value ? ( incompressible flow)

Can you send main matlab file? (attach to the post)

[Eren10]

Originally Posted by Akuji

Can you send main matlab file? (attach to the post)

I get now the same values. Sorry

[Fransje]

To all users using version 1.7.*, and having the dreaded:

Could not find U, p or rho in database

error, here is a work around to get the test case running.

Simply add, in the function definitions:

rhoName rhoInf;

To have something like:

functions
{
forces
{
type forceCoeffs;
functionObjectLibs ( "libforces.so" );
outputControl timeStep;
outputInterval 1;
patches
(
wall
);
pName p;
UName U;
log true;
rhoName rhoInf;
rhoInf 1;
CofR ( 0 0 0 );
liftDir ( 0 1 0 );
dragDir ( 1 0 0 );
pitchAxis ( 0 0 1 );
magUInf 30;
lRef 1;
Aref 1;
}
}

Kind regards,

Francois.

[hfs]

Originally Posted by aerothermal

Dear foamers,

the sampleDict sent by velezisaza worked well for me.
i am working to get Cp from a cylinder in a tunnel.
however, the sample tool provided me all data on patch.

How can I extract pressure information in a line, i.e., in the patch intersection with a plane (like normal to Z and at 0,0,0) ? Should I do it by hand? Does openfoam have a tool for this?

regards,

Hello!
Did you figure this out?!

I need the same. I need the Cp values on a point on the patch, i.e., in the patch intersection with a line (with given y, z and parallel to x for example)

Could you please let me know how can I get that?

Thanks!