Hello this is my first post to this forum. I have been experimenting with OpenFOAM 1.5 for about a month now, and am attempting to simulate a wind turbine using a rotating mesh. I believe the tool I need to consider using is either icoDyMFoam or MRFSimpleFoam. (at least as far as I can figure out those two can at least handle the dynamic mesh.) I can't seem to find much information on either program. I appreciate how this group hates stupid quiestions so I've been through the user manaual several times and searched for info on the web and in these forums.
Can anyone point me to a place where I can get more information on these tools? For instance I have no idea what the options are for the dynamicMeshDict. An example that works in OF1.5 would really be great.
Also MRFSimpleFoam doesn't even appear to be compliled in my release. Is that normal or a problem with my installation?
Welcome to OpenFOAM :)
Let me try to answer some questions:
MRFSimpleFOAM - no explicit mesh movement, uses moving reference frame approach to account for the effect of rotation by adding a source term to the momentum equation. Please look for threads by deepBlue and posts on openfoamwiki, he has documented it very well.
Once again welcome to OpenFOAM and I wish you an healthy and productive Foaming.
Thanks jaswi. That was the start I needed. I compiled MRFSimpleFoam and ran the demo. I have much learning to do, but thanks to you, I have some ideas of where you look.
We are also working with wind turbines, and have some comments:
- icoDymfoam (sorry for the mistyping), AFAIK, was written for laminar flows (like icoFoam). I don't think this is your case;
- We've been using the rotationBC utility, for steady state simulations (simpleFoam). It compiles well in both 1.4.1 and 1.5.
Hope that helps,
My wind turbines are VAWTs, and there is so much that is time dependent I'm not sure a steady state solver will be useful. The blade's (wing's) AOA changes with position, one wing diverts the stream toward / away from another wing, etc.
I was hoping icoDyMFoam might do the job. I see there is also a turbDyMFoam that might be better. (Although I don't see any tutorials for it.)
I'm no fluid dynamics expert. Maybe steady state is good enough. I guess it depends if the propagation time for air movement from the front of the VAWT to the back of the VAWT is significant compared to the speed of the blades or not.
I'll check out rotationBC just to keep my options open.
Yes, you are right about VAWTs, I mean that you will have to use transient simulation.
We still didn't try here, but maybe GGI is also a good option for your problem.
I am doing a savonius turbine on turbDyMFoam solver.
I think you turbine should also be run in a turbulent environment, so it is turbdymfoam, not icodymfoam.
and i think MRF is not suitable for a side-blow turbine.
Two dynamic mesh models are possible: Sliding Interface & GGI.
The latter could be run parallelly.
icodymfoam has tutorials for both these two models, they can be modified slightly to fit turbdymfoam.
I don't know what pre-processing software you are using, for me, the mesh conversion process had be a little hard. If it is Gambit or Gmsh, I am now successful.
I am currently using the realizableKE RANS model, it now shows the best fit for Fluent result, but still about 7% difference on Torque.
I hope when you finish, we can discuss a little about the result between turbulent models.
you can also write to me, if you like (*o*) , email@example.com
1) Created the model in solid works and exported the STL file.
2) Created the base mesh (cylinder and surrounding block with hole for cylinder) using blockMesh.
3) Cut the model out out of the cylinder with snappyHexMesh. (very cool program!). Unfortunately snappyHexMesh eliminates the surrounding block.
4) Made another base mesh of only the block with hole with blockMesh.
5) Added it into the cylinder mesh using MergeMesh (which had to be patched to make it work in OF1.5).
You might ask why I bothered to put the block in step 2 if it was just going to be removed. The answer is that the boundary names all get entered at that step. If you don't put it in, when you merge the block back in, then it complains that it had to add boundaries and it refuses to do it.
So now I have my model in a cylinder with a surrounding block ready (i think) for turning and sliding meshes. (I think). I still need to figure that part out.
I did this mostly with trial and error. There is probably a much simpler way to do it, but I haven't found it yet.
do you mean if i want make a unsteady calculation for turbine what i need is
1 turbDyMFoam (make some modification like MRFSimpleFoam to add centrifugal force and Coriolis force and so on)
2 ggi interface
but what is the difference between ggi and slidinginterface?
BTW..would you mind add to our online group..firstname.lastname@example.org.
hi~, I am not familar with solid works, but I am sure Gambit can do it, and doesn't need MergeMesh.
Only you have to pay attention to the treatment of the interface.
there is a utility for it, and you can find the script for it in the forum.
btw,you mesh is in 3D?
sorry, I am not quite well understanded you first question?
for the second, GGI uses a aglorism on the interface, and SI remeshes the interface, the result on my experience is the same. the only differece is that SI doesn't support parallel running.
not in parallel, the speed is also quite alike.
My geometry is in 2D, and GGI gives the fastest speed on 8-way parallel;
And for SI, you can use GAMG linear solver to speed up to like GGI 2-way parallel. And GAMG performs not well on parallel on GGI.
I am not sure about all the remarks, it is only my experience.
My mesh is 3d.
I'll have to check out Gambt sometime.
for the first question.i mean the MRFSimpleFOAM in OF is a steady solver. I am not quiet sure what i will do if i want to do a unsteady simulation. i guess first thing is to add "ddt" term and then rotating mesh with time steps..but is that ok or need more??
BTW. when you adding to us it is time to have dinner.so. :) ..i am sorry.
if you only want to get the thing rotation without any unsteady irregulary effect, you also can use SRFSimpleFOAM. this is the rotation version of SimpleFOAM that makes the illusion of rotation. in MRF you have 2 zones. But if you only want to get like wing aerodynamics in a rotation system of a mono-wing, SRFSimpleFOAM is perfect. and it runs faster.
Well, I think not only the ddt item.
Suppose you get a turbine which rotates around the z-axis.
if the wind is from exactly z-axis, it would be OK, without ddt for steady, and with ddt for unsteady.
if the wind is from x direction, I guess the the interface treatment method of MRF will counter trouble, both steady and unsteady.
am I right? ................I am not sure.
Does MRF with GGI have a "jumping mapping" ability?
Hi wolle and Yuhai
thanks for your reply! for "unsteay" i don`t mean irregular effect of turbulence.i mean the relative position change of rotor and stator.it need the dynamic mesh dictionary i guess .
you may find something in tutorial of MRFSimpleFOAM
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
origin (0 0 0);
axis (0 0 1);
direction (1 0 0);
// ************************************************** *********************** //
but it is useless now. i think it need support in MRFSimpleFoam code.
that is i wish some want to tell me how to.
i add MRF to turbFoam like what MRFSimpleFoam do ,i want to do the unsteady calculation of pump.but i face the error messages like:
Time = 0
Courant Number mean: 0.0502405 max: 0.5
deltaT = 0.000246692
//after add coriolis
smoothSolver: Solving for Ux, Initial residual = 8.88095e-06, Final residual = 6.33714e-08, No Iterations 2
smoothSolver: Solving for Uy, Initial residual = 9.06538e-06, Final residual = 6.39123e-08, No Iterations 2
From function T& tmp<T>::operator()()
in file /root/OpenFOAM/OpenFOAM-1.5-dev/src/OpenFOAM/lnInclude/tmpI.H at line 164.
is there anyone can help me
Hi yuhai, I'm trying to simulate a flow around a VAWT in order to comprare OF results with FLUENT results, but OF Torque in three times less than FLUENT one. Could you help me? I set realizablekE model, Ggi and to obtain force on the blades I add this function in controlDict:
functionObjectLibs ("libforces.so"); //Lib to load
patches (blades); // change to your patch name
rhoInf 1.225; //Reference density for fluid
CofR (0 0 0); //Origin for moment calculations
// 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
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 1);
// Type of functionObject
// Where to load it from (if not already in solver)
I use turbDyMFoam solver, and all the fvScheme and fvSolution I used is the same used in turbFoam tutorial. I think that I set up well the interface because postprocessing the solution I can see the blade rotate, and the flow go through interface.
Thanks in advance!
|All times are GMT -4. The time now is 18:45.|