CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   I need Moving Wall Slip (http://www.cfd-online.com/Forums/openfoam-solving/67862-i-need-moving-wall-slip.html)

hansel August 28, 2009 13:00

I need Moving Wall Slip
 
I'm simulating vertical wind turbines using OF1.5-dev. The boundary condition for U I've been using for the turbine is MovingWallVelocity with a uniform value of (0 0 0). I think this is giving me unrealistic drag on my blades.

Is it possible to have a slip boundary with a MovingWallVelocity?

gocarts September 1, 2009 09:25

Consider MRFSimpleFoam
 
I don't think that the movingWallVelocity is what you want. It assumes that the wall is moving relative to a stationary volume, such as the crown of a piston moving within the confines of a stationary cylinder. Thus the mesh is changing. I'm guessing that you want to keep the entire mesh stationary.

I think you need to consider a moving reference frame (MRF) around your (complete or just a blade?) VAWT, though I don't have any experience with it - have a look at MRFSimpleFoam.

hansel September 1, 2009 10:19

Quote:

Originally Posted by gocarts (Post 228118)
I don't think that the movingWallVelocity is what you want. It assumes that the wall is moving relative to a stationary volume, such as the crown of a piston moving within the confines of a stationary cylinder. Thus the mesh is changing. I'm guessing that you want to keep the entire mesh stationary.

I think you need to consider a moving reference frame (MRF) around your (complete or just a blade?) VAWT, though I don't have any experience with it - have a look at MRFSimpleFoam.

No actually I have my turbine in a round mesh and I'm spinning it. In a VAWT since the blade goes up wind and down wind, and there are blade to blade effects you can't cheat and do it with a stationary mesh and some tricks.

Steve

gocarts September 1, 2009 10:51

More Details
 
Ok, I see.

So you have a rotating (non-conformal) interface on the boundary between the rotating cylinder (containining your VAWT) and the stationary surrounding mesh, and you are running a time dependent simulation, right?

Or are you performing some kind of pseudo MRF with the rotating cylinder as your reference frame and a time dependent, transformed onset velocity?

I don't think I can help much either way, but maybe others can weigh in once they know more about your simulation details.

Good luck.

hansel September 1, 2009 12:31

Quote:

Originally Posted by gocarts (Post 228131)
Ok, I see.

So you have a rotating (non-conformal) interface on the boundary between the rotating cylinder (containining your VAWT) and the stationary surrounding mesh, and you are running a time dependent simulation, right?

Or are you performing some kind of pseudo MRF with the rotating cylinder as your reference frame and a time dependent, transformed onset velocity?

I don't think I can help much either way, but maybe others can weigh in once they know more about your simulation details.

Good luck.

Not being a real CFD person (I'm an EE), I don't know all the terminology. I have a square wind tunnel with a cylindrical hole in the middle. Inside that hole is a second cylindrical mesh that spins. The interface between the two meshes is mated using the ggi extensions of the -dev version so that air, pressure, turb data flows in and out of the spinning mesh. The data in the mesh is also counter rotated as the mesh is rotated. The simulation is time dependent and I try to run it for several rotations which can take days of computer time. I've done this in 3d and 2d.

My problem (and maybe it's not a problem) is that my only option for the boundary condition on the turbine itself is a no slip surface. Since I posted this, people have been telling me that is actually the correct boundary condition to use for modeling the real world and air does not actually slip on a surface no matter how smooth it is. Like I said, I'm not a CFD or fluid dynamics expert so I'm not sure. I just know I'm getting more drag on the blades than I would expect.

gocarts September 1, 2009 17:41

Accurate Drag Prediction is Difficult
 
I think you are performing scenario one that I offered.

No slip is the correct boundary condition for a wall - moving or stationary.

Accurate drag prediction is difficult:
  1. Have you tried increasing/decreasing your mesh resolution to see how the drag prediction trends?
  2. Your turbulence model will influence your drag accuracy - have you tried a different model to see the effect on drag?
  3. Have you tried switching between 'wall functions' (high Reynolds number turbulence models) vs 'integration to the wall' (low Reynolds number turbulence models, high mesh resolution at the wall)?
  4. Have you tried benchmarking a simpler geometry (e.g,. stationary single blade) for which you have known results? Could be another simulation or experiment.
I'm not expecting answers. These are just general thoughts for you to consider.

hansel September 1, 2009 17:48

Quote:

Originally Posted by gocarts (Post 228166)
I think you are performing scenario one that I offered.

No slip is the correct boundary condition for a wall - moving or stationary.

Accurate drag prediction is difficult:
  1. Have you tried increasing/decreasing your mesh resolution to see how the drag prediction trends?
  2. Your turbulence model will influence your drag accuracy - have you tried a different model to see the effect on drag?
  3. Have you tried switching between 'wall functions' (high Reynolds number turbulence models) vs 'integration to the wall' (low Reynolds number turbulence models, high mesh resolution at the wall)?
  4. Have you tried benchmarking a simpler geometry (e.g,. stationary single blade) for which you have known results? Could be another simulation or experiment.
I'm not expecting answers. These are just general thoughts for you to consider.

1) Mesh resolution had little effect, I went as small as 1mm.

2) and 3) I don't know enough to do this, I used values I copied from someone else's turbine experiment, but I don't know that they are good values. However when I run with icoDyMFoam (no turbulance model) the results are fairly close to real life. I suspect I am using a wall function for a very rough wall. I don't even know which parameter that is. Where can I find documentation on turbulance models and TurbFoam (TurbDyMFoam)?

4) I ran a flat plate through air (flat side pushing into the air.) and got a Cd of about 1.8 - 1.9, which I thought was kind of high.
http://www.youtube.com/watch?v=S-ucDIDEbv4

gocarts September 2, 2009 09:05

Turbulence Modeling
 
For general info on turbulence modeling try: http://www.cfd-online.com/Wiki/Turbulence_modeling

Specific to OpenFOAM there is the UserGuide.pdf that is part of the distribution. You might find the lid-driven cavity example useful with the calculation of k/epsilon based on turb. intensity and turb. length scale.

The latest 1.6.x OpenFOAM release has reworked the wall functions (high-Re. Turb. Models) and that might be worth a look, if you haven't already.

liuzhany2000 September 7, 2009 20:55

Cfx
 
I think you'd better use CFX for your problem. There is a special module for turbomachine in CFX.


All times are GMT -4. The time now is 14:31.