CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Wind Turbine (VAWT) - Negative Moment in Fluent (http://www.cfd-online.com/Forums/fluent/116999-wind-turbine-vawt-negative-moment-fluent.html)

dalecooper April 30, 2013 08:04

Wind Turbine (VAWT) - Negative Moment in Fluent
 
Hello!

I am doing some research about Vertical Axis Wind Turbine (VAWT) for my master thesis. I have been doing some simulations with Fluent with a 4 bladed turbine. The radius of the turbine is 3 meters.

The main target is to obtain a profile of the Coefficient of Perfomance (Cp) versus the Tip Speed Ratio (TSR). In Fluent I'm using a sliding mesh technique with 1 interface to separate the rotating zone from the stationary zone.

The problem I found is that whatever value of TSR I choose I never get a positive moment coefficient. I have tried to refine the mesh and reduce the time step but that didn't solve the problem.

Any idea or solution would be well received. Thanks in advance!

blackmask April 30, 2013 08:58

You should do the steady simulation with SRF/MRF first. This way you need not warry about the time step size and yet the converged result can be used as a starting point for unsteady sliding-mesh based simulation. If this is a realy turbine, you could ask the designer about the optimal TSR. Do you happen to rotate in the wrong direction?

dalecooper April 30, 2013 10:19

Quote:

Originally Posted by blackmask (Post 424169)
You should do the steady simulation with SRF/MRF first. This way you need not warry about the time step size and yet the converged result can be used as a starting point for unsteady sliding-mesh based simulation. If this is a realy turbine, you could ask the designer about the optimal TSR. Do you happen to rotate in the wrong direction?

Hello blackmask.

I have already used this approach of beginning with a steady simulation with an angular velocity equal to 0 rad/s as my thesis director suggested to me. After that and when the results have converged I move to transient simulation using a constant inlet velocity of 10 m/s and changing the value of the rotational speed in order to simulate different values of the TSR.

I'm using 'Transition SST (4 eqn)' with the default options as a viscous model and I'm not sure if that could be the problem. I have also tried with different solution methods but apart from the covergence velocity no significant changes were detected in Cm.

blackmask April 30, 2013 10:32

No. You should start your simulation with 10m/s inlet velocity and an appropriate rotational speed using the MRF (moving reference frame) technique. You should check the fluent user's guide if you are not familiar with MRF. The default parameters of specifying b.c. for TR-SST could results in an unresonable high turbulent viscosity at the inlet but I do not think it is the reason that you get negtive torque.

CFD_LES May 4, 2013 01:57

Hello dalecooper

I work on a 4-Bladed VAWT with semi-circle blade. I obtain ((Negative)) moment for this VAWT.
You obtained negative moment too. Did you understand the reason?
Could you solve your problem?
Also I have to say, My problem is steady.
Thanks so much

dalecooper July 8, 2013 06:58

Quote:

Originally Posted by CFD_LES (Post 425118)
Hello dalecooper

I work on a 4-Bladed VAWT with semi-circle blade. I obtain ((Negative)) moment for this VAWT.
You obtained negative moment too. Did you understand the reason?
Could you solve your problem?
Also I have to say, My problem is steady.
Thanks so much

Hello CFD_LES,

Finally I was able to solve my problem of negative Cm values in my simulations. All I did was to restart again with the geometry and meshing. So I think there was some problem with the interfaces between the stationary and rotating domains, but I'm not sure if that was the reason. All I can tell you is that after that I began to obtain positive Cm values.

Nowadays I'm doing some simulations in order to obtain the coefficient of performance of the turbine as a function of the tip speed ratio (TSR). The results look pretty good except, for a unique point (TSR=1.5) where the Cm has an abnormal value. I was expecting to obtain an increasing Cm value up to a certain point where the turbine is most efficient, and after that the Cm should begin to decrease.

I have tried with different inlet velocities, but the behavior is exactly the same, and also the critical point is located at TSR=1.5

Best regards

mikebausas October 8, 2013 03:53

hello dale cooper,

I am working with a 2d model VAWT which i simulated using fluent. And now, I generated some results of Cm from the iterations. My question is, what would be my next step in order for me to conclude that the results are acceptable or accurate for the specific turbine I am testing? Where shall I compare my results with? And how did you compute for the other parameters, such as Cp, Torqu, etc? Does Fluent also gives these data? Thanks

Regards,
Mike

dalecooper October 8, 2013 05:06

Quote:

Originally Posted by mikebausas (Post 455631)
hello dale cooper,

I am working with a 2d model VAWT which i simulated using fluent. And now, I generated some results of Cm from the iterations. My question is, what would be my next step in order for me to conclude that the results are acceptable or accurate for the specific turbine I am testing? Where shall I compare my results with? And how did you compute for the other parameters, such as Cp, Torqu, etc? Does Fluent also gives these data? Thanks

Regards,
Mike

Hello mikebausas,

In turbines, one of the most important graphic to obtain is the one that compares the Cp vs TSR (Tip Speed Ratio). From Fluent you can obtain directly the Cm (Coefficient of Moment). Once you get the Cm you must average the values obtained through a number of periods assuring that you have reached a steady solution and use the following equation to obtain the coefficient of performance (Cp):

Cp=Cm*TSR

What I have been doing is simulate for different values of TSR. To do that you have to change the value of the rotational velocity of the sliding mesh zone in which you locate the airfoils for every TSR value.

Regards.

mct90 April 3, 2014 04:42

1 Attachment(s)
Quote:

Originally Posted by dalecooper (Post 455642)
Hello mikebausas,

In turbines, one of the most important graphic to obtain is the one that compares the Cp vs TSR (Tip Speed Ratio). From Fluent you can obtain directly the Cm (Coefficient of Moment). Once you get the Cm you must average the values obtained through a number of periods assuring that you have reached a steady solution and use the following equation to obtain the coefficient of performance (Cp):

Cp=Cm*TSR

What I have been doing is simulate for different values of TSR. To do that you have to change the value of the rotational velocity of the sliding mesh zone in which you locate the airfoils for every TSR value.

Regards.

Hi Dalecooper. i am also studying similar project.
I want to know, to obtain a CP-TSR graph like the image, does the cm decrease at a value of rotational velocity(w).

For ex; w=1,tsr=1 cm=0.12 ---w=2,tsr=2 cm=0.20---- w=3 trsr=3 cm=0.18 ---.
Attachment 29809

shahizare April 6, 2014 22:56

Quote:

Originally Posted by mct90 (Post 483622)
Hi Dalecooper. i am also studying similar project.
I want to know, to obtain a CP-TSR graph like the image, does the cm decrease at a value of rotational velocity(w).

For ex; w=1,tsr=1 cm=0.12 ---w=2,tsr=2 cm=0.20---- w=3 trsr=3 cm=0.18 ---.
Attachment 29809


Hi Dalecooper
kindly please help me . i simulate vawt in fluent in 2d and 3d model . i have problem with a reference numbers in fluent , what do you think how much i should put for area and length . and after getting results (cm) how can i convert it to Cp?

shafqat May 5, 2014 14:03

hi i just want to know why my Cm keeps on increasing at high tsr..i mean it has to decrease after optimal tsr

mct90 May 14, 2014 06:32

Quote:

Originally Posted by shahizare (Post 484255)
Hi Dalecooper
kindly please help me . i simulate vawt in fluent in 2d and 3d model . i have problem with a reference numbers in fluent , what do you think how much i should put for area and length . and after getting results (cm) how can i convert it to Cp?

Hi,

I am working 2d vawt. In reference values i took length=R (rotor radius) and Area= 2*R*h .(h=1 because of 2D). references are below;

http://www.iaa.ncku.edu.tw/~aeromems...%20control.pdf (page 341 )

Impacts of solidity and hybrid system in small wind turbines
performance M.H. Mohamed (page 497)

shahizare May 15, 2014 02:46

Quote:

Originally Posted by mct90 (Post 491724)
Hi,

I am working 2d vawt. In reference values i took length=R (rotor radius) and Area= 2*R*h .(h=1 because of 2D). references are below;

http://www.iaa.ncku.edu.tw/~aeromems...%20control.pdf (page 341 )

Impacts of solidity and hybrid system in small wind turbines
performance M.H. Mohamed (page 497)



abi nasilsin :)


this is link of my work https://www.dropbox.com/sh/c2hl306cm...Tm6mI8i8xX2T8a

actually in what reason i dont know why i can not get good validation with my reference . is it possible for you to check my case file?

tasakor lar :)

aalisha May 30, 2014 00:05

Hello CFD Mates!!

I am a Masters student working on a vertical axis marine current turbine. I am using Fluent for the required simulations. To calculate the Cp, I have monitored the value of Cm, Cl and Cd.

However, the value obtained for Cm is very high ( 85, 70 etc). If anyone can guide me what is the reason for this. It will be a great help. Thanks.

amin_veysi August 7, 2014 10:19

Quote:

Originally Posted by aalisha (Post 494773)
Hello CFD Mates!!

I am a Masters student working on a vertical axis marine current turbine. I am using Fluent for the required simulations. To calculate the Cp, I have monitored the value of Cm, Cl and Cd.

However, the value obtained for Cm is very high ( 85, 70 etc). If anyone can guide me what is the reason for this. It will be a great help. Thanks.

hi aalisha change the reference value,
reference value panel, change the velocity, area and length

aalisha August 11, 2014 22:56

Hey Amin,

Thanks for your kind reply. I tried it and its working now.

JUDASHU January 20, 2015 22:30

Quote:

Originally Posted by mct90 (Post 491724)
Hi,

I am working 2d vawt. In reference values i took length=R (rotor radius) and Area= 2*R*h .(h=1 because of 2D). references are below;

http://www.iaa.ncku.edu.tw/~aeromems...%20control.pdf (page 341 )

Impacts of solidity and hybrid system in small wind turbines
performance M.H. Mohamed (page 497)

hi
I am doing a 2D VAWT CFD simulation with Fluent, and I have my reference valus as you suggested, I still wonder what the "compute from" and "reference area" should be, and I have got a CM curve in my attachment, it seems fluctuates drastic, so is this a normal case or did I have something wrong in my case?http://www.cfd-online.com/Forums/mem...121-092339.jpg


All times are GMT -4. The time now is 12:25.