I have yet to get reasonable numbers with turbDyMFoam. (Probably because I have no idea what to use for turbulence parameters.) I suggest starting with icoDyMFoam and see what you get. I find I get pretty reasonable results on a lot of VAWTs.

Hi hansel, thanks for your quikly reply.
Sorry but, icoDyMFoam is a solver for LAMINAR flows, isn't it? I can't understand how can I get reasonable results...

Hi enry

I'm fairly new to this but is magUInf the right value?

Hi Nick,
I found my error...
Since the mesh is 2D, OF tranform it into 3D mesh, even if it solve with 2D solver. So to compare 2D FLUENT's results with pseudo-3D OF's results I have to divide OF results by thickness that OF create. :)

enry

So how did they compare? Mostly I'm simulating vertical axis marine current turbines and also use CFX while I explore this option.

Hi Nick,

the curves overlap! Results is very very similar. I haven't done any error percentage until now, but I'm satisfied.

Enry, would you post what you used for transport properties and RASProperties? I've never manage to get good numbers form turbDyMFoam.

Hi again Enry

Sounds good. How did the processing times compare?

Another question Enry!

Are you using parallel? Can you get forces etc. in parallel? If so how?!

Cheers
Nick

@Nick: Sorry, not yet, but I think that I will run calculation in parallel untill next month.

@Hansel:

RASProperties:

RASModel RNGkEpsilon;

You can use also realizable K-E. Standard K-E don't work.


TransportProperties:

transportModel Newtonian;

nu nu [0 2 -1 0 0 0 0] 1.46e-05;

CrossPowerLawCoeffs
{
nu0 nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf nuInf [0 2 -1 0 0 0 0] 1e-06;
m m [0 0 1 0 0 0 0] 1;
n n [0 0 0 0 0 0 0] 1;
}

BirdCarreauCoeffs
{
nu0 nu0 [0 2 -1 0 0 0 0] 1e-06;
nuInf nuInf [0 2 -1 0 0 0 0] 1e-06;
k k [0 0 1 0 0 0 0] 0;
n n [0 0 0 0 0 0 0] 1;
}


ControlDict:

applicationClass turbDyMFoam;

startFrom latestTime;

startTime 0;

stopAt endTime;

endTime 8;

deltaT 0.0001;

writeControl adjustableRunTime;

writeInterval 0.5;

cycleWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.3;

maxDeltaT 1.0;

functions
(



forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (blades); // change to your patch name
rhoName rhoInf;
rhoInf 1.225; //Reference density for fluid
CofR (0 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 (blades);
rhoName rhoInf;
rhoInf 1.225;
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 1);
magUInf 6;
lRef 1;
Aref 1;

outputControl timeStep;
outputInterval 1;
}


ggiCheck
{
// Type of functionObject
type ggiCheck;

phi phi;

// Where to load it from (if not already in solver)
functionObjectLibs ("libsampling.so");
}





);

// ************************************************** *********************** //

Fv schemes and Fv solutions are those imposed into turbFoam cavity tutorial.

Hi nick, sorry, I read only your last reply ;).

FLUENT is faster than OF, because In FLUENT I impose a time step, wile in OF I set adjustTimeStep in order to have CFL<0.3-0.4.
I can say that FLUENT is maybe three - four times faster than OF.

Thanks for the info, Enrico. One last question (I think). How fine was your mesh at the turbine's surface?

Hi hansel,
I create a mesh that can give me a value of mean y+ about 30. Mesh resolution so depend of course on simulation set up. My first cell is about 1/800 turbine diameter.
I advice you to get some simulation in order to establish your mesh resolution near the blades.

Wind Turbine
 

Hey guys,
I've read this thread and some others and its been helpful. I am trying to simulate a wind turbine at a high rpm in OF1.7. Now, I read online that simpleSRFFoam is not good for this. So my options are pimpleDymFoam or MRFSimpleFoam. I gather that pimpleDymFoam moves the mesh whereas MRFSimpleFoam does not (it adds a source term).

I guess when I think of a wind turbine simulation, I usually imagine just creating a mesh for a single blade and then using periodic boundary conditions but from the looks of it none of you guys are doing that - why is that? And I'm still not sure which one is better - MRFSimpleFoam or pimpleDymFoam. If anyone has plots of results from these versus experimental data, I would love to see it.

Thanks!

I've been trying to simulate VAWTs, and since the air flows from one side to the other it's not symmetric about the center.

Will OF1.7 rotate meshes?

If you used pimpleDymFoam, i think that moves the mesh doesnt it?

Hi Foamers,

I inserted an obstacle in the icoFoam/cavity case and to see what happens when it rotates I've included dynamic mesh effects on icoFoam.

The thing is: The square rotates correctly, but the problem is that the mesh rotates with it, and that produces an invalid mesh (severe non-orthogonality). I would like the mesh to just stretch and contract as the square rotates. I mean, I don't want the points attached to the square to rotate.
To better explain: When you look at the mesh in the wireframe form on paraView, I want the horizontal wires to keep their y(vertical) position and move (expand or contract) horizontally as the square rotates, and I want the vertical wires to keep their x (horizontal) position and move (expand or contract) vertically as the square rotates.

How can I implement this?

I'm on OpenFoam 171 and had to modify icoFoam to create icoDyMFoam. How can I install the 1.5-dev? There I believe lives icoDyMFoam and the GGI utility.

Thanks and regards!

All the best

Hi all,

I made a 2D mesh using the blockMeshDict and now I wish to rotate producing a half geometry. For example, rotating (180 degree) 2D cylinder we obtain a half 3D cylinder.

There is a tool called rotateMesh (http://www.openfoam.com/features/mesh-manipulation.php) but how can I use it ? Any idea ?

Thanks.