[AUN]

Dear All,

I'm trying to simulate a fully coupled two-way FSI Simulation of a wind turbine. The objective is to achieve the pressure distribution on the blade surface during steady-state operation and import the loads on the same structure in the Mechanical APDL Environment and get the resulting deformations and stresses in the internal structure of the blades.

The approach that has been followed is similiar to Tutorial No. 23 Oscillating Plate.

The blade has been modelled as a solid body in DM. The fluid domain is a rectangular cuboid. By appling Boolean Operations the two volumes were subtracted.

The real problematic part lies in constraining the structure and applying the appropriate boundary conditions.

Wind Turbines are essentially rotating structures that are excited by the wind. I tried to perform the CFD analysis through MFR however, the issue was that the wind turbine actually started behaving like a Fan. Rather than extracting energy from the flow and decelerating it, the wind turbine now was adding energy to the flow and accelerating it. With regards to MFR I applied the following BC's: Frozen Rotor on BOTH sides of the Turbine, Counter-Rotating Wall, an inlet, an outlet and walls (no slip). I therefore ruled out MFR for the fluid analysis portion as this is not the intended function of the machine and I on my part could not get any other way of getting this done. This is my first question: How to apply MFR to simulate a wind turbine?

Next, the other option was that of 6-DOF which would capture the transient and steady state behaviour of the turbine but at the same time with very big disadvantage. I am interested in a flexible structure and not a rigid one.

The last option remaining with me in this case was that of constraining the hub in rotation ONLY and letting the flow rotate the blades. I applied a REMOTE DISPLACEMENT to the hub, constraining it in all DOF's except Rotation in X. The blades were declared as interface. The blades were set into motion at a simulation time of 0.3s however later, the ANSYS Interface Loads (Structural) would 'diverge'.
I even tried changing the BC's at the hub i.e. letting all degrees of freedom as free and constraining axial displacement in X only however, the effort was futile.

Therefore I next created a cylindrical support at the center of the hub and letting it free in the Tangential Direction only. After a simulation time of 13.45 s , there was no observable rotation achieved just out-of-plane bending.
Next Question: How to constrain this wind turbine, which has been modelled as a single solid body in DM such that I get only flapwise deflections (edge-wise and torsional suppressed) and the blades rotate by the action of the wind.

Any help will be very much appreciated. Thanks in advance.

AUN

[stumpy]

Hi Aun,
using MFR is certainly the correct way to simulate this. You should have two fluid domains; one will be a cylindrical region surrounding the blades, the second will be the box representing the far field with the cylindrical region cut out. Using 3 frozen rotor interfaces for the connections between the cylinder and outer box is fine. The cylindrical domain will be a rotating domain. The blades will be stationary walls, since this means stationary in the rotating domain.
If you end up with energy added to the flow then it just means that for the imposed wind speed the turbine is moving too fast. This may be physically correct, or it may be that mesh refinement is needed to get a better answer, or some additional physics need to be modeled (e.g. using the transition model to account for laminar to turbulent boundary layer transition). It's important to get the fluid simulation correct before starting any FSI work.
On the structural side the root of the blades or the hub can be a fixed support. You would then apply a rotational velocity on the whole model. Note that this models the rotational forces, but it does not actually rotate the structure. The same thing happens on the CFX side - the rotating domain accounts for the rotating forces on the fluid, but it does not physically rotate the mesh. So you should expect the blades to not move in CFD-Post, but that's just because you are viewing the results in a rotating frame of reference.
Hope this helps.

[Atze]

Dear AUN,

I'm trying to simulate a case similar to your. A vertical axes wind turbine. My problem is the non linear ansys solver diverge ("crit" quantities). What can i do? How the meshes (fluid and solid) are supposed to be for a good solution? Time step?

Thanks in advice

[AUN]

Dear Atze,

I myself am very new to this work to be very honest.
However, I can, based on your problem say with much assurity that there is something wrong with your BC's for the structure part. My suggestion would be that leave the FSI part completely, model the structure, constrain it, apply loads, solve it and see what happens. I am currently following stumpys suggestion; because it sounds very logical to me.
Maybe what we are trying to do involves constraint equations, maybe some additional vital Commands both of which I have'nt been able to sort out yet.
DOF's are the major problem.

Regards,
Aun

[Atze]

Hi AUN,

thanks for your answer. I think there's something wrong with BC's too. Just a question: Looking your photos i suppose blades are setted as Fluid/Structure interface. What about the central support? It's just a Fixed support or also a interface?

Regards.

[AUN]

Hey Atze,

It is a cylindrical support. The photos represent just one of the thousand tries that I have done changing the loads and supports each time.
P.S. Check your element type too. SOLID 186 has three DOF's. Model the blade as SHELL 181 and see the outcome. Maybe that is of some help. Keep me updated. I still am quite eager to model the 'rotation' and not just the 'rotational effect'! ;-)

Regards,

AUN

[AUN]

All issues resolved. Thanks alot.

[AUN]

Some of the simulation results . . .

[AUN]

Dear Mike,

With regards to the far-field boundaries, which option would be better: Outlet/Opening?
I tried keeping an outlet type boundary condition first at the farfield walls and the in the Solver run got the message that 'a wall has been placed at portions of an outlet to prevent fluid from flowing into the domain at xyz% of the areas and pqr% of the faces.
With regards to CFD-Post, how can we post-process the wake region?


Thanks in advance,

Aun

[ghorrocks]

If the back flow at the outlet is small then I would not worry about it. In fact if your outlet is far enough away from the blades to not be affecting the results it will almost certainly be small or zero.

So unless there is a gross recirculation in the domain - and that should not be the case for a wind turbine - then use an outlet.

[AUN]

Dear Glenn,

I was able to make some modifications to what I had been doing earlier and here is the outcome.
I now have the far-field walls around more than three rotor diameters from the rotor. BC - Static Pressure Rel Pressure: 0 Pa. But that message in the solver about the a wall being placed at portions of an outlet persists.
I have an inlet at 6 m/s, outlet [Static Pressure: Rel. P 0 Pa] and ground in the stationary domain.
I have the HAWT in the rotating domain. The wall in the rotating domain has not been specified any velocity.
I have three domain interfaces with frozen rotor, normal GGI connections.
The mesh size is +4 million. With reasonable resolution in proximity of the blade walls.
The Gamma Theta option for transitional turbulence is being used. Automatic wall scaling and Inlet turbulence was given the default values. I'm using the SST k-omega turbulence model.
At first, given an inlet velocity of 6 m/s, I was able to match the load on the generator at 214 rpm. The power output was 434.21 W.
Now, with the modifications, 6 m/s, 210 rpm, power output: 524.36 W. I will still match the power by reducing the rpm but what I really cannot comprehend is that whether what I have modelled is it even correct or not.
I plotted the Velocity is Stn Frame streamlines and yes they have now curved up behind the blades but I was sort of assuming that I'd be able to see that 'helix'. Although I can see the flow decelerating.
Also, with regards to the pressure drop, I am making contour plots on planes that slice the entire domain. I donot see a pressure drop there, regardless of the plot variable, Abs Pressure, Pressure, Tot Pressure etc etc.

Any suggestions?

Thanks in advance,

Aun

[AUN]

. . . .

Got it! . . . Finally! :-)

. . . .

[AUN]

RFR/MFR

Frozen Rotor

[tranchitam]

Hi AUN

How can you get this result?

I've a problem with pathlines. The pathlines does not continue to spin when it goes out of the interface behind wind turbine. I also using CFX and the setting for interface is similar to your setting.

Could you give me some advices?

Thanks alot