Hi all. With your help we got the turbine simulation working, and it is giving very accurate results (in steady state it matches perfectly measures from a wind tunnel). We are now solving transient simulations, and testing other turbulence models such as SAS-SST.

However, we would like to make the rotational speed a function of torque in CFX CEL, and compare the final rotational speed with our data. Given the inertia value (known to us), how could we make such function?

I know Glenn does not recommend this, but we would like to try it anyway to compare.

Thank you and regards,

Alejandro

Yes, I do not recommend this. It is much easier to run a series of fixed rotation speeds then interpolate to find the operating speed based on the torque output of each rotation speed.

But if you insist on doing it that way:
It would be nice to use the rotating frame of reference model to do the rotor and use an expression to control the speed, factoring in the torque, load and inertia. The problem is that the inertia requires knowledge of the previous speed and that can be tricky to get in CEL. You might be able to use tricks like areaAve(omega)@rotor as these callback functions return the valve from the previous time step. There are also some pretty horrible tricks to get additional variables retain values from previous iterations. Or you could just jump right in and write a fortran user routine to do it, then you can properly account for everything.

Then you can go the 6DOF solver approach. This can account for inertia easily, but the generalised motion model in this model will be far slower than the rotation only one in rotating frames of reference and your run time will be immense.

Thank you Glenn for your reply. At this moment we are doing what you recommend: running series of fixed rotation speeds. How can I find the operating speed with this method?

As the rotating speed rises so does the torque, until we reach a certain rotation speed where the torque starts to diminish. I suppose the correct rotation speed is the point where maximum torque is achieved, right?

I am not familiar with the rest of the options, but I will look into it. Regards,

Alejandro

No - have a think about what determines the steady state operating speed.

The rotor will not accelerate or decelerate when there is no net torque on the rotor. There will be zero net torque when the torque produced by the turbine equals the torque absorbed by the generator and other losses. So you need to know what your load is doing, as well as the rotor.

Then you plot a chart of net torque versus speed. Interpolate to where the net torque equals zero and that is your operating speed.

Dynamic Stability of projectile
 

Dear All
I am new to CFD. I want to calculate stability derivative of projectile using 6-dof analysis in CFX or FLuent or any other software. my basic aim is to calculate the derivative of pitching moment and magnus coefficient.
can anybody help me or have some tutorial files

Try the fluent forum for help on this.

But if you are looking for derivatives of pitching moments and similar coefficients it does not sound like you want to do a 6DOF simulation. This sounds like you want to do a series of stationary simulations at a range of angles of attack so you can determine the coefficients you are looking for. This is a straight forward set of simulations as no 6DOF is required.

Hey guys, I got a question that fits really fine in here, hope you are okay with that.

My topology is quite close to the one of aalbanesi and I'm already working with 1/3 and everything works fine, almost.

I got a realistic torque at the shaft and and a cp of approx 0.4, which sounds great to me. But I got the following problem:

The velocity of the fluid is not getting smaller, I gave a velocity of 12.5m/s at the inlet and it's almost constant until the outlet, which is about 10x of the height of my blade far (according to ansys).

So I think that the Simulation does not know, that the blades take power out of the wind and the shaft is braked by the Generator and so on.

So I thought of creating a subdomain to drop the velocity to 2/3 in the rotorplane and to 1/3 behind (not sure where exactly), according to Betz. I tryed different setups in the subdomain/sources/loss model.

I do not understand the meaning of the streamwise direction and the Options of the streamwise loss, also the ansys help did not clear that for me.

Are any other recommendable pdf, tutorials or hints by you guys?

Thank you very much for your Patience. Peace.

Looking at the pic earlier, and you say it is similiar. Are your side boundaries walls? Or, is the blade in an enclosed tunnel in your model?

Almost similiar, I have three domains axial, a stationary inlet-domain, a rotational domain, and a stationary outlet-domain. I do not have radial to my rotating domain a stationary one.

So the blade does not have an extra enclosure. Which side? At the top is a counterrotating wall and at the side is symmetry with rotational periodicity.

But how to define a velocity loss according to Betz?

There is no need to define a velocity loss. It will be part of the solution when the solver conserves mass and momentum so an accurate simulation will already have it.

What is your solver momentum imbalance? If that is small than the imbalance from the inlet to outlet is what the rotor is absorbing - and that is what you are looking for, isn't it?

Glenn is right. Velocity loss is part of solution, but you have to model it correctly to get that.

If you have walls on the side of your entire domain, with a fixed inlet velocity, by nature of conservation of mass/momentum, your exit velocity (average) will be the same (assuming incompressible fluid).

Okay, I think I see what you mean. I force the velocity with use of walls because of the conservation of mass/momentum... Mh. So I'll concidere to use an opening at the top of the outlet-domain. Mh, I'll have a try.

As far as good, thank you both. You'll hear from me ;)

Hey guys, me again.

The simulation is on a good way. I almost miss her at night ;)

I have a question which was sometimes already clear to me and than weird again. The value of my torque which comes out of the torque function around my rotational axis (z) with location on my blade via named selection is sometimes quite different.

Now my question: As I simulate "just" a 120° part of my real modell with only a single blade instead of three, do I have to multiplicate the torque with"3" or should it have according to the symmetry the right amount of torque?

And: I tryed to define my angular velocity on several ways. When I define it as an Expression with the value of e.g. 300[min^-1] and set the turbine power as an Expression too with P=2*PI*M*n. P has the dimension [degree]... :( Although M has the right dimension of Joule. Weird.

Thanks for your time!

If you model 120° of the full thing you will then have to multiply the torque by 3 to get the total torque of the device.

Okay thanks!

Hey Glenn, hey guys.

Deadline is coming close and I got a new massive problem yesterday.

I'm checking the convergence of the grid at the moment and there five were single steps:

• the radius
• inlet_interface1 - distance
• interface1_rotorplane - distance
• rotorplane_interface2 - distance
• interface2_outlet - distance

FYI: I have three domains in direction of stream, a stationary (inlet), a rotating (including the blade) and a stationary again (outlet).


I recognized that I did not got a convergence for the inlet_interface1 - distance. So I decided to run the simulation again with all values extremely high. So I definetly could suspend the influence of the frames (walls, inlet, outlet, interface) and now comes the big prob: I got an huge torque at the blade which can surely not be right, its almost 5 times higher then the torque of the existing construction...


I have no ideas.


Can I do a mistake by choosing the values "too" high?
Any ideas?
Need more input from me?


Thanks for your time!

There are many things other than bonuary proximity which can affect accuracy:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Hi Alejandro,

What have you changed in your model? How did you managed to get accurate/suitable results for your wind turbine? At the moment, I have the same problem with my analysis and don't know what is the reason. For low roational speed and lower velocities it gives correct results, but design wind speed and rotational speed I get Cp around 300%. Could you please help me?

Thanks in advance.

Best Regards,
Kutan

Have you looked at the accuracy FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

There is not a single thing required for accurate results, many things need to be correct for the results to be accurate. The FAQ lists most of them.

I know the list and did all the steps. I just wonder how and/or what Allejandro did so that he got the correct results.

Regards,
Kutan