[antonio_ing]

Hi everybody and happy 2009
I have started today working with a darrieus VAWT geometry. I did a first simulation without any rotation with simpleFoam but now I have to add the rotation of the profiles. Since the vortices will interact in a unsteady way, i guess that the best solver should be turbDyMFoam, but i have no experience with this solver (or equivalently icoDyMFoam).
Can anyone give me some details?

thanks in advance

[antonio_ing]

can anyone give me some help?

[mparodi]

Hi Antonio,

did you manage to get some basic material on turbDyMFoam?

I am also trying to set up a case, but without success.

Mauro.

[NickG]

Hi

This is what I do starting from separate inner and outer meshses:

-> mergeMeshes /home/nick/OpenFOAM/nick-1.5-dev/Turbine/2degGgi/ 600mm2degTunnel /home/nick/OpenFOAM/nick-1.5-dev/Turbine/2degGgi/ 600mm2degRotor
[That has 4 arguments: master root ; master case; slave root; slave case]

To set up case from combined mesh in new folder:

copy to new case folder from tutorials/IcoDyMFoam/mixerGgi: 0, constant, system

replace /constant/polymesh with mergeMeshes polymesh (inside the folder named from the value of your timestep in mergeMeshes controlDict)

change type for inside and outside sliding interface to ggi and paste underneath startFace:

shadowPatch outsideSlider;
zone insideZone;
bridgeOverlap false;

for insideSlider and:

shadowPatch insideSlider;
zone outsideZone;
bridgeOverlap false;

for outsideSlider. Your sliding faces maybe named differently so replace insideSlider and outsideSlider accordingly. e.g. mine read:

InterT
{
type ggi;
nFaces 180;
startFace 7782;
shadowPatch InterR;
zone outsideZone;
bridgeOverlap off; //relates to consistency of mesh size across interface: can be true, false, on, off
}
InterR
{
type ggi;
nFaces 180;
startFace 15482;
shadowPatch InterT;
zone insideZone;
bridgeOverlap off;
}

change names of slider moving and static arguments in dynamicMeshDict to correspond to your interface boundary names (e.g. from insideSlider to InterR for my case)
change rpm and coordinateSystem if necessary.

write k, epsilon, etc. depending upon turbulence model. Use example from turbFoam as an example for interface patches: type ggi; e.g. from my k file:

InterT
{
type ggi;
value uniform 25; // you don't need to include this line
}

[if you want to run in parallel: add to decomposeParDict: globalFaceZones ( insideZone outsideZone );]

write "setBatch" file: faceSet insideZone new patchToFace InterR
faceSet outsideZone new patchToFace InterT
quit
place in case folder

-> setSet -batch setBatch

-> setsToZones -noFlipMap

-> turbDyMFoam

Hopefully it runs!

[mparodi]

Hi Nick,

I really appreciate your help .

The model looks to be running now!

Many Thanks,

Mauro.

[lordvon]

You did not have to replace the fvsolution or fvscheme files under /system/ in the icoDyMFoam tutroial?

[NickG]

If you're using turbDyMFoam but starting from IcoDyMFoam then you need equations for the turbulence. Check fvsolution or fvschemes in turbFoam tutorial for examples