How to find RPM from wind speed in Floworks?
Hi all,
I'm currently simulating a VAWT in CosmosFloworks. I more or less manage to find correct values for the torque that I can expect at a certain amount of wind speed. But I always have to specify the amount of RPM in the global rotating setting. Isn't it possible only to give the wind speed and find out the RPM of the VAWT ? Another question is, I tried to specify a local rotating region but it won't work, I can't define it if it's not a closed area (a cylinder would work but not a open region), any idea someone? I am currently using global rotation which is a bit wrong, I know, but that's the only way I can do for now. if any answers or even questions feel free, I'm running out of imagination ! Thanks in advance, Matco 
The rotating region does not have to be a closed region with solid walls. It is just a region in fluid where the rotating reference system (coordinate system) is applied. It is not a solid body defining some cavity. So you can enclose the area around your turbine with a cylinder and apply a rotating region to it. Don't forget to assign the Stator wall boundary condition to the surfaces of all nonrotating parts within the rotating region. See the CPU Cooler example in Tutorial.

Thanks for replying Ive,
Actually when I put a cylinder around my turbine (and therefore perpendicular to the flow) and define it as the rotating region, it seems like Floworks takes the cylinder as a real solid components (as I am looking in the surface plot in the solver window, the cylinder is visible and represents a border in the velocity plot, a discontinuity that should not be here) even though it is disabled in component control. Therefore I can assume my results are wrong. The computational domain is outside the rotating region, which is not in contact with anything. And the turbine is entirely in the rotating region, the flow is external. Otherwise don't you know how to have the RPM as a goal instead of an input? One of the purpose of my study is to predict how many RPM (or rad/s) we can expect from the turbine and the only thing I can do is defining a rotation by its rotational velocity and not related to the flow velocity. cheers, Matco 
The discontinuity is related to the used model: the rotating region boundaries are split into "slices" or "rings" and all flow parameters are averaged over each slice. So there are some prerequisites for the flow at the rotating region boundaries, e.g. flow velocity vectors should be as much perpendicular to the boundary in each point as possible and the flow parameters should not vary much in circumferential direction near the boundary.
However, in your case it seems that you don't need the rotating region at all. You just need to put your turbine in the flow and find the forces acting on the blades and then calculate rpm from these values. If all blades are identical, you just need to find the forces for one blade. Or you can find the torque acting on the whole turbine. I think that you can find the guidelines in any book on turbine design and probably in the web. 
Sorry for this late reply.
Basically, when I turn off the rotating region option, I don't have any good results (torque close to 0 for any wind speed). However, using the global rotating setting, and a tight computational domain, I got results that confirm our tests for several wind speeds. Therefore, I am going to keep this way of doing, which is moreover quicker. The way that I am calculating the RPM expected is by plotting the torque, and therefore the Power output, versus the RPM of the rotating region. And for a small range of RPM, the Torque is constant and constitutes a threshold whose values are really close to genuine RPM we've mesured. And yet I am not sure about the reliability of this method, why do you think about it? Matco 
This method works if you already know the rpm of your turbine at any wind speed. But if you do not have such data, the most common way is to determine the characteristics of a single blade such as drag, lift and moment using Flow Simulation and then calculate the whole turbine performance from them.

I am sorry Ive but I just can't agree with our method. You can't determine the torque just by extrapolating the results on force acting on the blade in an uniform flow. They are several reasons for this :
 in a rotating flow the blade is not subject to the absolute velocity of the wind but to a relative velocity. Then the angle of attack of the flow on the blade depends of the rotation speed.  This is true in peculiar for vertical axis wind turbine where some of blade move against the wind (for ex. in a darreius turbine).  Most of the time there is some interaction between the blades. With a simple extrapolation the more balde you have, the greater your torque will be. That you can do is a quite complex extrapolation using the Cd vs Cf curve of your profile at different AOA/velocity couples . That's what is done for fan performance extrapolation. The only way to find the right velocity is to make the calculation at several rotation speed and then to trace the curve of the performance coefficient vs the normalized speed. You should have an optimum which gives you your real velocity and torque. 
I completely agree with you. Of course we need to consider blade characteristics at various speed and angles of attack. I thought that it was obvious, because a profile characteristic is not a single point, but a curve. And I didn't mean to simply extrapolate single blade characteristics by multiplying them. Some methods exist that allow to assess efficiency of a turbine from a single blade characteristics, number of blades and rpm range.
My recommendation was related to how to use Flow Simulation for turbine performance calculation. You cannot use it in such straightforward way as Matco tried, so the best way to use it is to determine single blade characteristics and calculate turbine performance from them using widely known methods. 
Just like in real life, putting a wind turbine in the wind and seeing how fast it spins isn't all that useful. I believe you need to pick a wind speed, and spin the turbine at different rates, and measure the average torque at these rates. Then calculate the power by multiplying torque times rpms. (converting the units, of course.) Do this for several different rotational velocities and you will find the peak power point of the turbine for that wind speed. Also the speed where the average torque is near zero is the no load speed.
Having the power curve of your turbine will allow you to intelligently design the alternator or other load you plan to put on it. 
Ive, i don't know if you are familiar with the turbine design method you are talking about but I used to work in the turbomachinery field for years and it is far more complex that it seems at first glance.
Moreover, these methods are almost useless for a VAWT since the angle of attack vary along the rotation path. hansel is right and the only to achieved such calculation is to determine the design point by running several simulations with several rotating speed for each wind speed. 
But you need special calculation models for that, such as freezed rotor. Usually it is very costly.

I can't understand why you are thinking so :confused:.
Frozen rotor is just another name for the MFR approach. Even if the numerical approach is different (there isn't any spatial avering in MFR but local conservation is enforced) it isn't more calculation intensive than the mixing plane approach used by floworks. You can use FW for such calculation. BTW I used it for a HAWT and we obtained very good results (less than 5% error with mesured power output on the whole caracteristic curve) 
It is great that you can achieve good results with Floworks in this kind of simulation. I wasn't so optimistic and I'm happy to know that I was wrong. But the thread starter had some problems with rotating regions, so I tried to propose some way to avoid use of rotating RF. Probably he need to optimize the shape of the rotating region, or to correct stator wall conditions within it.

Actually, I have been using the global rotating option since it was the one that would give me the best results regarding to what we found in reality. However, when I plot Cp versus TSR, instead of giving me a maximum, the curve still continues to increase, whatever high the RPM is.
Thanks a lot for your answers. Cheers, Matco 
Quote:

I realize this is an old thread, but I am modeling something similar (a turbine that rotates perpendicular to the flow axis  cross axial). I am having similar troubles. A rotating reference frame acts almost as though it is a solid wall. This is due to the way floworks assigns boundary conditions over the barrier.
global rotation returns torque values close to what has been found experimentally, but I find it hard to trust the results because the flow trajectories show such interesting motion. 
I'm subscribed to this tread, so it is OK.
Yes, the rotating region is treated as another fluid region, and flow conditions are transferred between the rotating region and the surrounding global flow domain through the rotating region boundaries, and you should consider averaging of flow parameters as described in the Technical Reference document. However, certain efforts were made to improve visualization of flow and particles trajectories at the rotating region boundaries. Which version of FloWorks do you use? Also, in Solidworks Flow Simulation 2010 SP4 a big chapter was added to the Solving Engineering problems document, containing a lot of information and some tips and tricks on the rotation simulation. 
I use 2008 FloWorks.
Just for fun I tried flow along the same axis as the local rotation body, and the flow trajectories look great, the pressure differential is easy to believe, but that's not at all what I want. The problem, I believe, is that the flow needs to be axisymmetrical with the rotating region, and that is inherently impossible with my model because the the flow is perpendicular to the axis of rotation. Has 2010 resolved these problems? 
In 2010 SP2 and later you can choose whether to plot flow trajectories in rotating or nonrotating coordinate system. Plotting flow trajectories in the rotating coordinate system ensures correct interaction of trajectories with the rotating geometry, while plotting trajectories in the nonrotating system provides correct visualization of flow trajectories along all flow path, however the trajectories may intersect with the rotating geometry  but it is only a visual effect.
But I'm afraid that I didn't understand you  do you use the global rotation or local rotating region? The flow parameters averaging applies only to the local rotation. 
Quote:
Local rotation is what I have been referring the remainder of the time. 
All times are GMT 4. The time now is 08:30. 