HAWT, should we use sliding meshes? or the UDF?
I'm wondering the actual physical mechanism of a wind turbine, HAWT literally. From a basic physics sense, we already knew that the fluid should do work on the turbine to generate the power. That is, despite the start condition of the turbine, if we consider the steady and stable output of the turbine, it should be fluids who accelerates the blades. The resulting torque is balanced with the friction and the resistance of the generator and therefore provides power. However, both the MRF or sliding mesh method are ACTIVE method from my point of view. In specific, they let the blades rotate actively and then the fluid will got disturbed, generating the colorful flow field you've seen on the screen. In other words, this is actually the blades doing work on the fluids, a compressor it is.
Is it the right way to do it?
I have seen a bunch of master thesis and even the official Fluent News (2001 or 2002 Spring) with the analysis on wind turbines utilize these methods. Is there any one who can explain why they did this? How can it be even possible for draining a sensible results? (it actually did...... But I am not comfortable with this weired mechanism..)
Or should I did it another way, applying the UDF and write the governing equation for the rotating motion and let the pressure distribution drives the blade? It is obviously a much more complexmethod, but with a rather sensible physics.
I think I got something wrong in there. Please help me with the confusion. Thank you.
There is really no wrong way about doing this. Yes, you can go write a snazzy UDF and let the fluid pressure rotate the blades. In fact, this would be a great way to do it, you could see exactly how fast the blades would rotate for a given freestream velocity. But, this would only work if you wanted to analyze a single operating condition.
However, it isn't wrong to let the blade work on the fluid and use a sliding grid (for these problems, stay away from SRF or MRF). For my masters thesis I used a sliding grid and it turned out just fine. Now, using this method doesn't allow you to determine the rotation speed for the wind turbine for a given freestream velocity, but what it does do is allow you to build up a performance curve (like efficiency vs. tip speed ratio). When you build up a performance curve for a wind turbine, you usually are searching for efficiency as a function of the tip speed ratio, building on the fact that most wind turbine designs are quantified using dimensionless values. The tip speed ratio can be changed by, you guessed it, either changing the freestream velocity or the rotation speed of the wind turbine!
Therefore, by simply specifying the freestream velocity and allowing the fluid to work on the wind turbine, you can only analyze a single operating condition and cannot build up a performance curve. However, if you want to explore the performance of your wind turbine over several operating tip speed ratios, use a sliding mesh.
Thank you for your reply. You might be a little digress though.
I already knew those. However, I'm more care about the physical implication of this issue. In more specific term, I do care about who does work to whom. It is totally nonsense for me to state that a compressor is equal to a turbine, and they should be using the same method, in this case the sliding mesh technique.
Secondly, I am a little bit confused about "single operating condition". It's kind of ambiguous actually. If you could, please explain it to me. Assume we are now using the UDF approach as I mentioned earlier and assume the turbine was already started up and maintain a specific rotating speed, which simplifies the problem. The pressure distribution on the airfoil cause it to spin due to the lift force generated. The rotor could be accelerated or decelerated, or maintain same rotating speed, it all depends on the capacity of generator I supposed. (which is also the required parameter in the UDF I guess) In this sense, if you suggest the rotor could have various velocity than the problem will no longer stayed in the "single operating condition", but become a more complicated FSI problem. (Yet it might be more realistic) Not to mention the changing pitch angle, it will make the whole simulation a mess. Yet I'm curious about the whole physical process as the turbine rotates. Is there any classical textbook refered to this process? I seldom read a similar discussion on the topic.
What I am asking, is to be more exacting and strict on the examination of the numerical method, and their physical meanings. Otherwise this would turn out to be like "no one knows what others are doing, neither themselves" condition.
Another observation: I notice the quality of the discussion on this forum is getting worse. Some very insightful and inspiring discussions were appearing before 2006, approximately. There are masters and professionals discussing CFD problems on this forum. Yet there are more and more people just want to get some advantages right away, and ruin the atmosphere by posting some of the very meaningless and 'you should read more books' articles on the site. I truly hope myself would never turn out to be one of them.
Ok, seems you are digging pretty deep here. It isn't really nonsense to think of a turbine and a compressor as the same. Work is work, energy is energy. Whether the fluid works on the turbine or the turbine works on the fluid doesn't necessarily matter (Think of the energy equation, energy in=energy out). This is why we can allow the wind turbine to work on the fluid in a CFD simulation and still achieve accurate results.
When I say single operating condition, I'm referring to a single tip speed ratio (if you are unfamiliar with the term tip speed ratio you can find it pretty much anywhere online). Once a HAWT achieves a quasi-steady state, it is operating at a single tip speed ratio. The rotor isn't being accelerated or decelerated anymore by the fluid, hence the term quasi-steady. This is not an over simplification, this is actually what happens for HAWTs. Now VAWTs are a little different, but I won't get into that.
Now, if you were studying the startup behavior of a wind turbine, that would be much different. In that case the turbine would be accelerating through several tip speed ratios, however, it seems you are only interested in the steady state behavior.
Just so you know, I don't believe the generator needs to be involved. Typically, the CFD process is purely aerodynamic. If you were using a UDF you would allow the fluid to act on the blades, accelerate the wind turbine to a steady-state, and determine the rotation speed. Then, post-CFD, you could determine if the generator could handle the rotation speed achieved by the blades and determine if you need any aerodynamic breaking or something similar.
So like I mentioned before, if you were to allow the wind turbine to work on the fluid, you could examine various operating conditions and analyze the performance characteristics of the rotor. Ideally, this is what most people would like to accomplish.
And one more thing. Typically when modeling a compressor you would use a SRF (single reference frame) or MRF, and this reference frame would a moving reference frame. Hence, the fluid looks as if it is rotating while the blades are stationary.
Think of the alternate approach. Allow the blades to rotate in a sliding grid. Now the blades are working on the fluid. What's the difference? The only difference is the frame of reference.
In the first SRF case, you can imagine that you are rotating with the blades, hence, the blades look as if they are stationary. In the second case where the blades are working on the fluid in a sliding mesh approach, you are now in the global reference frame watching the blades rotate. This is why both methods are pretty much equivalent. The only difference is the frame of reference.
I think this should answer your question. I've attached a link to the FLUENT user guide for rotating reference frames, hope it helps.
Thanks to the discussion. Yet you have made some clear mistakes in the difference between turbine and compressor.
The two resulting flow field should be different. As you know the work equals to force times displacement, it implies that the tangential force component of the blade is in the direction of the blade motion (a pump) or opposite to it (a turbine). You are confusing with the concept of reference frame since the fluid will get accelerated by the compressor and decelerated by the turbine, no matter which reference frame are you using. Furthermore, the rotation direction of the wake flow for a turbine and a compressor are also opposite considering the same rotating direction of these two machines. (Is it even a wake flow for a compressor?) The former is caused by the reacting force exerted by the turbine blade, while the latter is the result of momentum transfer. There are totally different mechanism driving the flow pattern. Don't you care about that? Is it really doesn't matter when you are calculating the pressure distribution and the velocity field, and the resulting drag, lift and moment? I doubt that.
There are definitely some tricks in there, and I would like to find it out. Or I couldn't apply the method comfortably.
I should have clarified, I was talking about a centrifugal compressor and vertical axis wind turbine (my thesis project), kinda got carried a way :) Seems your case would be comparing an axial compressor and horizontal axis wind turbine. But it doesn't really make a difference in the end.
In any case, let me put one thing to rest...the tangential force component of a turbine blade is in the direction of the rotation, that's how the blade rotates! As a fluid works on a blade, the blade produces both lift and drag, these force components can be further broken down to a normal and tangential force component and it's this tangential force component that drives the rotation of the turbine.
Furthermore, both a compressor and a turbine would have a wake rotating in the same direction. However, compressors such as those found in gas turbine engines typically use stators to straighten the flow, eliminating the rotating wake (a secondary loss mechanism). If no stators existed, the flow would be rotating just like the flow leaving a turbine.
Alright, now on to the good stuff! Let me begin by simplifying our problem a bit, this tends to reduce the confusion and we can get more out of it. Let's assume an ideal case (no losses), not realistic, but it will help with the explanation. Assume a fluid is approaching a turbine with some kinetic energy (energy in). This fluid then works on the turbine, rotating its blades and transforming the energy from kinetic energy in the wind to the mechanical energy in the rotating blades (energy generated/energy out). Therefore, for this ideal case, energy in=energy out (now for a wind turbine you can imagine the next step would convert the mechanical energy into electricity, however, this is CFD and we are not concerned with electricity, just aerodynamic efficiency).
Next, assume just the opposite. Assume we have a compressor, blades that work on a fluid. These blades require energy to rotate and hence have some mechanical energy while rotating. In the ideal case, these blades act on the fluid and convert 100% of the mechanical energy into the kinetic energy of the fluid. And there you go! Both cases are equivalent.
Differences will arise however for the non-ideal case, but aren't as drastic as you might think. In CFD analysis, we are concerned with the aerodynamics, so loss mechanisms like the generator efficiency of a turbine or a motor efficiency for a compressor are not our concern until after the CFD analysis. What we are concerned with is the loss due to the aerodynamic design of the wind turbine. Losses such as viscous effects, wakes, tip leakage, etc. These are losses inherent in both turbines and compressors, they are not unique to just one or the other. Yes the use of stators after a compressor works to eliminate rotation in the wake, but again, not important for this explaination.
Ok, now for a real world example that actually works. Think of a computer fan. A computer fan works on a fluid to cool a device like a processor. Now take this computer fan and blow air past it, let the fluid work on the fan. What happens? The blades of the computer fan will rotate. Again, this is evident in the energy equation. The amount of work it takes to drive a fan blade to a certian rotational velocity is roughly equivalent to the amount of work a rotating fan blade will impart on a fluid. And this is why we can model a wind turbine either way and get the same result.
Lastly, instead of listening to me ramble, you should try it in Fluent. It won't take that long to set up. Let some wind speed start up and drive the rotation of a wind turbine, record the rotation speed and wind turbine efficiency. Next, use a sliding domain approach and set up the case for the same tip speed ratio (some blade RPM and inlet velocity to achieve the same tip speed ratio) and record the efficiency. They should be the same. And again, the reason people use this approach is so they can simply specify a tip speed ratio and record the wind turbine efficiency (coefficient of performance), because in the end, this is what a wind turbine designer is really looking for.
I will simplify my question. An idealistic household fan and an idealistic windwill. You are saying that the flow field at the back of the windmill will be approxiamtely identical to the one blows from the fan (in front)? Is this what you are saying?
So far an excellent discussion. I think we are deviating from the original question to much. Your original question was regarding the way in which to simulate a horizontal axis wind turbine. There are two ways of doing this:
Method 1. SPECIFY ONLY AN INLET VELOCITY and allow the fluid to work on the blades. This will in turn start up the wind turbine and the rotor will eventually reach a steady state and you can extract the true performance and efficiency for a given wind speed. This is definitely a great way to do this, but again, you're only looking at a single tip speed ratio.
Method 2. SPECIFY BOTH THE INLET VELOCITY AND THE ROTATION SPEED OF THE WIND TURBINE. In this approach you are directly specifying the tip speed ratio of the wind turbine. Keep in mind, we aren't just allowing the blades to work on the fluid (we also have an inlet velocity), we are tricking the simulation into thinking it is the fluid that is rotating the blades. The biggest advantage of this approach is that it allows us to determine the wind turbine efficiency at various tip speed ratios, because now all we have to do is adjust either the inlet velocity or the rotation speed of the wind turbine, both of which we now have control. Again, the efficiency is the most important aspect in wind turbine design.
You may think the second method is unrealistic because we are forcing the wind turbine to rotate at a given speed regardless of the inlet velocity. The way you can tell if the results aren't making sense is if you find the efficiency of the wind turbine to be NEGATIVE. If the efficiency is POSITIVE, then the operating condition is realistic. Also, rather than trying to spend time convincing yourself through discussion try experimenting using both methods, that should really convince you that both methods work. Use both methods to determine the EFFICIENCY (dimensionless value) of your wind turbine for the SAME TIP SPEED RATIO. You should come up with very similar values.
Lastly, you really need to keep in mind that wind turbine analysis is done using DIMENSIONLESS quantities like the tip speed ratio and coefficient of performance. I can't stress this enough, and if you don't understand this you can find it in any paper discussing wind turbine CFD.
If this discussion, reading papers, and doing your own research hasn't convinced you that either method will yield the same results, than I'm sorry, but I really don't know how to explain this further. I've attached the links to two videos. The first video shows the flow field for a vertical axis wind turbine simulation using Method 1 described above, look at the flow field. The second video is my vertical axis wind turbine simulation using Method 2 described above. Again, observe the flow fields, they are very similar even though two different techniques were used to determine the performance.
I hope this helps.
And to answer your simplified question. Yes for an idealistic windmill (no losses) the velocity behind the rotor would be zero, as the windmill has extracted all the energy available in the wind (ideal case). And the velocity in front of a fan would be zero as well in the ideal case because the electricity driving the mechanical motion of the fan is being 100% converted into the kinetic energy of the air behind the fan.
Also, forgot to mention, seems you are a little confused with the ideal case. For an ideal windmill, it extracts all the energy in the wind approaching the rotor and therefore the velocity behind the windmill is zero.
I'm glad to have you discuss this with me. I have gained a lot from you.
However, I would still have to point out your misunderstood about this process. First, the pump(compressor, fan, whatever) is no way equaled to a turbine. The basic physics foundation are different. Turbines extract energy from fluid, while compressor deliver energy to the fluid. The wake flow of a turbine and the flow pass fan will never be the same. This is because the rotating wake flow of the turbine is caused by the reacting force (as the result of acting force on the blade) while the flow caused by fan is simply the momentum transfer from blade to fluid. You can identify them by the simple physics:
work=force * variation of displacement
Two ways to explain this situation:
1. Apply this rule to the blade (it is simpler for this case): then if the direction of the force exerted by fluid (lift, in this case) and the direction of blade motion are identical. This is a turbine. I supposed you are familiar with the Cl plot with attack angle. If the attack angle is keep decreasing (This can be done by increasing the TSR in reality) and finally it would become a fan because the negative lift force is opposed to the blade motion. If we can assure the lift is positive and the rotating direction is correct, then it is a turbine indeed.
2. Apply this rule to the fluid: it is the complete opposite of above, and I think you could figure it out by the direction of velocity change and the fluid motion. It is applicable if you examined the flow field.
This is the case.
Please don't say we let the blade rotate actively because a turbine is similar to a fan. That is ridiculous actually.
To my knowledge, the control strategy of the turbine (electrically, maybe?) could help the turbine remain a constant rotating speed and maintain the operation in the optimal operating point to extract the torque from the fluid. In a given free stream velocity, the simulation will be true only if in reality the turbine could balance on this operating condition, or omega specifically. If there isn't a mechanism working like this, then the torque acting on the turbine axis will accelerate the rotating motion and therefore in reality you would measure another TSR. The simulation will then be nonsense. I would like to know more on this mechanism if you have had some references.
For another thing, to me it is of vital importance to understand the physics completely before you get into a simulation. Otherwise it would be throwing some junks into some junks and get another set of junks, wouldn't it?
For your reference, I fully understand the mechanism of SRF, MRF and sliding mesh method and I have done many simulations. I didn't respond to all your materials given is because I already know them well. Thanks anyway.
In addition, although you have provided a set of flow field movie. It is too assertive to state the flow field are similar by simply look at those colorful contours moving around. The quality may be right but the quantitive is what we care. You didn't specify the flow condition, the rotating condition, the foil data and other vital, causing-difference parameters to this comparison. I cannot accept that the two methods are similar based on the "observation", nor your explanation of the difference between turbine and compressor. It is just not the way we verify something.
i am using sliding mesh for train moving through tunnel, but i am not able to make it work . can any body help me . my email is sheikhnasir39@gmail .com
|All times are GMT -4. The time now is 06:28.|