[sagarmatha]

Originally Posted by esp-m1000

Hi sargamatha,
The torque I'm talking on the posts is the moment force fluent give me in report menu.
report->forces->moments.

This moment is in Nm, after to calculate the power i multiply for the angular velocity,
if the turbine rotate at 42rpm, and so moment*42*2*pi/60

I take the value of the last iteration, after about 950 time step and 25000 iteration (for 2D model).
In Cm history diagram i minitor the Cm of each blade, and for each blade the Cm is sinusoidal.

hi esp,

from the looks of it, your moment is indeed negative. but you should not take the last value of the moment because you are doing an unsteady simulation. take the average of the moment for the last full rotation (assuming periodic convergence has been attained) and use that as the torque for computing the power. taking the last value is only valid for a steady simulation like for a horizontal axis wind turbine. the value of the moment acting on a blade for the vawt is not strictly sinusoidal. but it should still be periodically going up and down.

cheers.

[esp-m1000]

amber,
I'm not using mfr, but sliding mesh.
For the interaction between wind and turbine, i think you are right.
I know that the turbine must rotate after the effects of the wind, but i don't know how implement this on fluent.
So i choose a TSR, than the wind speed and found the w.
But doesn't work. As u can see in my last post where there are 2 pic, i obtain negative moment.
Have u suggestions?

Hi sagarmatha,
how can i take the average moment for the last rotation?
For example, my time step correspond to a 2.5° of rotation, so for 1 rotation i have 144 time steps. i must take the report moment for each time step, sum each one and divide for 144?

As u can see in Cm diagram i post, It looks like the Cm are converged, doesn't it?

Thanks for help guys
I must finish this thesis as soon, and don't know how.....

[ambermgupta]

Dontlose hope esp:>
i will discuss this problem with some seniors at my univ on monday[its vacation time here and so its hard to find people with cfd knowhow]
hwevr i know that adina supports fsi and so now evn fluent +ansys cae[though adina is generally accepted to better currently].hwevr reducing tsr value[increase wind speed ,reduce w] will get u into acceptable range for t.do uhave experimental data??

[esp-m1000]

amber thanks so much for help,
i don't know anyone of the software u talked about, exept for fluent and ansys.
I will searh information....
Thanks again

[ambermgupta]

Hey esp check turbine tut at adina website with fsi.seems to be interesting

[esp-m1000]

Thanks amber, I'm watching....

[sagarmatha]

Originally Posted by esp-m1000

amber,
I'm not using mfr, but sliding mesh.
For the interaction between wind and turbine, i think you are right.
I know that the turbine must rotate after the effects of the wind, but i don't know how implement this on fluent.
So i choose a TSR, than the wind speed and found the w.
But doesn't work. As u can see in my last post where there are 2 pic, i obtain negative moment.
Have u suggestions?

Hi sagarmatha,
how can i take the average moment for the last rotation?
For example, my time step correspond to a 2.5° of rotation, so for 1 rotation i have 144 time steps. i must take the report moment for each time step, sum each one and divide for 144?

As u can see in Cm diagram i post, It looks like the Cm are converged, doesn't it?

Thanks for help guys
I must finish this thesis as soon, and don't know how.....

hi esp,

yes, just take a simple average. but you must be careful of how you convert moment coefficient to moment. Cm is computed by fluent using reference values. using default reference values is ok but when you want to compare the values to your "3D" vawt, you must use actual wind velocity, area and length.

your Cm looks periodically converged. but it does look to be in the negative trend. have you done convergence studies to confirm that you are using the appropriate setup parameters? three main things need to be checked: spatial (grid) convergence, temporal (time step) convergence, and iterative convergence.

for spatial convergence, you must be sure you are using a fine enough mesh (also enough points on the blade surface) to capture the flow consistently but not too fine to be computationally expensive. for my blade, i use 1500 points.

for temporal convergence, you must use a small enough time step. i usually use 1° rotation equivalent time step. 5° is a bit too big for me, 2.5° i have not tried.

for iterative convergence, its not recommended to use absolute convergence criteria for residuals. AIAA recommends relative convergence criteria. i am currently doing a study on this and i seem to observe that using 2% relative error as convergence criteria is good already. 5% will just give values that are way too off. 1% takes too long to converge.



hi amber,

for practical reasons, you dont need fsi to simulate wind turbines. if you want to simulate with fsi, you need inertial effects, mass and material properties of your turbine, braking mechanism to prevent overspeed, etc, etc. if you are trying to simulate dynamic stress and deformation effects on the wind turbine, then you have no choice but to use fsi. if you are only interested in performance and the physics of flow, you dont need fsi.

i dont think we should try to make it too realistic. assuming a constant rpm is good enough. even if you assume a rigid wind turbine, one-way or two-way fsi is still "over-the-top" in simulations of VAWTs and HAWTs.

ansys has two-way fsi for years already. i have not tried using it though.

[ambermgupta]

agreed but the way of current modeling [sliding mesh ,mrf] the turbine can rotate even if v=0 isnt it so??

[esp-m1000]

sargamatha,
for spatial convergence, i have 10056 elements for the upper surface of the blade, and 9080 for the lower surface. To have 12 rotation with 3D model it takes 3 days. But i don't mean, I have 2 pc working on it.

For the others kind of convergence, do u think that the errors i have could be due to this? I used 2.5° or rotation per time step, and the absolute convergenze criteria for residuals. But if u say that the erros could be of 5%, my errors i think is very bigger than 5%.

[ambermgupta]

What the hell even me getting -ve momemt[2d savonius ].should be able to clarify till monday,will keep u posted

[esp-m1000]

Ambermgupta, I hope monday will clarify our problems.
I'm waiting for u becouse i still have negative moment, no matter what i have done.
I must finish my thesis as soon as. So your help will be welcome.
See u on Monday
Have a nice Sunday

[sagarmatha]

Originally Posted by ambermgupta

agreed but the way of current modeling [sliding mesh ,mrf] the turbine can rotate even if v=0 isnt it so??

right. if you really want to simulate turbine start-up, then you need to simulate just about everything including friction and gravity. but most people just want performance optimization and good understanding of flow physics.

[sagarmatha]

Originally Posted by esp-m1000

sargamatha,
for spatial convergence, i have 10056 elements for the upper surface of the blade, and 9080 for the lower surface. To have 12 rotation with 3D model it takes 3 days. But i don't mean, I have 2 pc working on it.

For the others kind of convergence, do u think that the errors i have could be due to this? I used 2.5° or rotation per time step, and the absolute convergenze criteria for residuals. But if u say that the erros could be of 5%, my errors i think is very bigger than 5%.

the negative moment you get is probably due to a very high tsr. for a savonius, tsr should be around 1 for max power coefficient. the rahai blade had around 0.4 power coefficient for a tsr of 1.6, much better than the benesh. and everyone knows the benesh is better than the standard S-type savonius (even with overlap).

for temporal convergence, try 1° equiv time step. compare results to your 2.5°. if they match closely, then 2.5° is enough. if they dont, you dont have a time-independent simulation (meaning your time step is a bit too large).

for iterative convergence, i find that a relative convergence criteria of 5% usually means a residual of not lower than 1e-04 for at least one of the monitored parameters (usually continuity or turbulent kinetic energy). but for 2% and 1%, residuals are of the range of 1e-04 or lower.

[esp-m1000]

Hi sargamatha,
First of all I would say thanks to u and to all guys for the help.
I set a TSR=4 becouse i'm not modelling a savonius turbine or a drag device, but a darrieus like turbine. So I found that for Darrieus turbine TSR is usually 4÷7, do u think i have to choose a lower TSR?
Thanks again...

[sagarmatha]

Originally Posted by esp-m1000

Hi sargamatha,
First of all I would say thanks to u and to all guys for the help.
I set a TSR=4 becouse i'm not modelling a savonius turbine or a drag device, but a darrieus like turbine. So I found that for Darrieus turbine TSR is usually 4÷7, do u think i have to choose a lower TSR?
Thanks again...

sorry for my mistake. tsr of 4 is ok for darrieus.

[esp-m1000]

Hi sagarmatha,
don't u worry, because i have done some simulation for TSR 1.6, 1.7, 1.8, 1.9, 2, 2.5 and also for TSR=4 at 5m/s.
The results are not so good because for:
1)TSR=1.6, ω=17RPM, finally I have a positive moment about 50 Nm, it is positive but very poor, because

Pw=1/2*rho*V^3*D=689W

and

Pe=50Nm*ω=89.01W

so

Cp=89.01/689=0,129

2)TSR=1.7, ω=18 RPM, positive moment about 57 Nm, always positive but very poor,

Pe=57Nm*ω=107.44W

so

Cp=107.44/689=0,156

3)TSR=1.8, ω=19 RPM, positive moment about 53 Nm, always positive but very poor,

Pe=53Nm*ω=105.45W

so

Cp=105.45/689=0,153

4)TSR=1.9, ω=20 RPM, positive moment about 30 Nm, always positive but very poor,

Pe=30Nm*ω=62.83W

so

Cp=62.83/689=0,091

5)TSR=2.5, ω=27 RPM, negative moment about -20 Nm.


What do you think about those results?

[sagarmatha]

Originally Posted by esp-m1000

Hi sagarmatha,
don't u worry, because i have done some simulation for TSR 1.6, 1.7, 1.8, 1.9, 2, 2.5 and also for TSR=4 at 5m/s.
The results are not so good because for:
1)TSR=1.6, ω=17RPM, finally I have a positive moment about 50 Nm, it is positive but very poor, because

Pw=1/2*rho*V^3*D=689W

and

Pe=50Nm*ω=89.01W

so

Cp=89.01/689=0,129

2)TSR=1.7, ω=18 RPM, positive moment about 57 Nm, always positive but very poor,

Pe=57Nm*ω=107.44W

so

Cp=107.44/689=0,156

3)TSR=1.8, ω=19 RPM, positive moment about 53 Nm, always positive but very poor,

Pe=53Nm*ω=105.45W

so

Cp=105.45/689=0,153

4)TSR=1.9, ω=20 RPM, positive moment about 30 Nm, always positive but very poor,

Pe=30Nm*ω=62.83W

so

Cp=62.83/689=0,091

5)TSR=2.5, ω=27 RPM, negative moment about -20 Nm.


What do you think about those results?

how large is your case file? maybe you can send it to me and i try to run it. lets exchange emails via private message.

[esp-m1000]

sagarmatha I sent a private message to you.

[nana]

Hi esp:

Sorry for the late reply as I am sick for the last few days. Yeah, there are some doubts that i want to clear with u.

First, you need to run a different set of simualtion in order to get the optimum RPM and TSR. The real turbine need TSR=2 to let it self rotating first. So my suggestion is to set TSR=2, and play with different wind velocity like U=3,4, 5 m/s for example. (Starting from the lower wind speed). But you should know what is your cut-in wind speed (it means the shaft can be generated power from that wind speed onwards).

Second, I am using k-e, RNG solve, as my Re is relatively low. However, I am a bit confused about your setting. What you mean
if the turbine doesn't move the Re is about 929073, for a wind of 9 m/s.

If the turbine rotate with 120 rpm and with 9 m/s wind speed Re=6700000.

Why you saying like that. For the real turbine, 9m/s is really high wind speed. are you sure this one is the correct value? I think you statement is wrong (for a wind of 9m/s, the turbine doesn't move, the Re is about 929073). It is impossible, how come the turbien cannot move since the speed is really hight nearly the optimum wind speed.

My suggestion is : set for the fix TSP starting from 2, you need to search what is the cut-in speed for your turbine, like Sandia 17m darrieus turbine the cut in speed is at 5m/s. However, you can do the simualtion from U =2 or 3m/s, by fix TSR, you can calculate the RPM. Then do the simualtion.

Since you are doing the 5 blade turbine, you can find a paper try to do the validation study to ensure the current Fluent solver that you are using is correct. Which I am doing currently, it seems my simualtion works well. The Cm will give the periodic function like sine wave.

REmember, you can also compare with the 3 or 4 straight blade, it's only the turbine solidity is different. For higher solidity, the performance should be lower than the lower one. So actually you can comapre your Cp with the 3 or 4 blade. You also can comapre with my case if you blade is straight. All the best then

[nana]

Hi esp:

I just go through the previous post, I also have the negative TSR for my previous simualtion when i mointor the Cm. The first thing I thought there should be something wrong, or maybe the rotation is worng, or the coordination is wrong. Now i got the periodic Cm after i change the BC set up.

I think for you BC, you should using the turbulence viscosity and length scale. Then using outflow at the BC outlet, however, the pressure outlet seems give me the same results compare to the outflow. the rest BCs looks ok for me. I am uisng PISO for p-v coupling. As I said previously, my Re is realatively low, i am using k-e RNG. For you case, i think k-e standard should be ok. Or you can try k-w sst model as well if you have enough time. All the best