CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Horizontal Axis Wind Turbine (http://www.cfd-online.com/Forums/fluent/86165-horizontal-axis-wind-turbine.html)

CFD XUE March 16, 2011 05:24

Horizontal Axis Wind Turbine
 
I am doing CFD simulation of Horizontal axis wind turbine by using Fluent.
Rotor dia = 6 m
Rotational speed = 20 rad/sec
Air velocity = 10 m/s
I am solving only one blade and using periodic boundary condition. I am using Single Rotating Reference Frame and pressure based solver. Solution is well converged. In fluent, we can write moment about x, y, and z axis.

I think moment about z-axis would be the rotor torque (z-axis is rotor axis). Am I right?

Calculated torque (30 N-m) (moment about z-axis) is around 2.5 time lesser than the torque predicted by BEM (78 N-m). What might be the reason?

I am solving laminar flow. Should I use turbulent flow? Which turbulent model would be appropriate?

Thanks

Kwiaci March 16, 2011 16:06

From my experience with gas turbine blades choosing turbulent model is very important. In case you described it may be neccessary to use one of them. Calculate Reynolds number in critical location for the most severe condition you want to model.
During my master thesis I was obligated to check turbulence model impact on results (mostly on heat transfer). The advice of my lead professor was to use the S-A model. But in a more general case k-e model is more widely used. If you have any verification data compare results for every model and choose the best one.

CFD XUE March 17, 2011 06:13

If I use k-Epsilon model then how to define turbulent boundary condition at velocity inlet?
At velocity inlet, its require to give one of the following:
K and Epsilon or
Intensity and Length scale or
Intensity and viscosity ratio or
Intensity and hydraulic diameter
How to find these turbulent parameters at velocity inlet? Do not have any experimental data.

Kwiaci March 17, 2011 15:29

I used default values for Intensity and Viscosity Ratio (10%/10). But you will have to look in literature for more detailed data.

alxasli March 17, 2011 15:38

your problem is that fluent calculated torque is less than BEM, adding turbulence will even decrease it. BEM results aren't much precise and don't always give correct results

CFD XUE March 18, 2011 06:26

From data I know that one blade of my turbine should produce 85 N-m torque.
Calculated torque by using laminar simulation is 64 N-m while 35 N-m by using k-epsilon turbulence model.

Both are lesser than actual. What might be the reason?
Moreover turbulent calculation gives torque almost half of the laminar calculation. Why????

alxasli March 18, 2011 06:27

how did you obtain 85 ?

CFD XUE March 18, 2011 06:51

from empirical calculation we design a 5 kw power horizontal axis wind turbine. Its rotational speed is 21 rad/sec and have three blades. so one blade should produce around 80 N-m torque.

Torque from laminar calculation is 64 N-m, which is close to empirical calculation but torque calculated from turbulent simulation is very small (34 N-m).

I have not understand that why both (Laminar and Turbulent) torque are lesser than the empirical calculation. What might be the reason?
Moreover turbulent calculation gives torque almost half of the laminar calculation and 2.5 time lesser than empirical calculation. Why????

alxasli March 18, 2011 07:09

if by empirical you mean BEM then it is ok. BEM only gives rough estimation of power and torque. in real life turbine performance will be less than BEM calculation. since CFD is more realistic it gives less performance values. and since in real life there is turbulence which acts like boundary layer separator and contributes to losses, CFD with turbulence gives even less results. it is hard to simulate turbulent flows correctly, so turbulent results may be little exaggerated, in my opinion real turbine performance is somewhere between laminar and turbulent results.
what is the tip speed ratio ? R=3m, w=20r/s, u =10m/s. so, TSR=Rw/u=6
if your turbine was designed for TSR=6 then performance prediction of BEM at lower rotational speeds will be more erroneous

CFD XUE March 21, 2011 04:49

yes, tip speed ratio is 6.

I think boundary layer is more stable in turbulent flow as compared to laminar flow.
So, separation is smaller in Turbulent flow as compared to laminar flow. Since separation is smaller, so, drag would reduce in turbulent flow.
As a result torque should increase in turbulent flow.

What do you think?

cfd_newbie March 21, 2011 04:59

Quote:

Originally Posted by CFD XUE (Post 300302)
yes, tip speed ratio is 6.

I think boundary layer is more stable in turbulent flow as compared to laminar flow.
So, separation is smaller in Turbulent flow as compared to laminar flow. Since separation is smaller, so, drag would reduce in turbulent flow.
As a result torque should increase in turbulent flow.

What do you think?

Dear CFD XUE,
From my experiences in last 3 years of performing validation of NREL Phase VI experiments I have learned this lessen - predicting aerodynamics loads and power curve of wind turbine through CFD is a tough nut to crack.
See my post in the following section -
http://www.cfd-online.com/Forums/mai...irfoils-3.html
You can ask more for further clarification.
Raashid

cfd_newbie March 21, 2011 06:36

Quote:

Originally Posted by CFD XUE
1. For validation of NREL Phase VI experiments you performed steady state or transient simulation?

2. Please send me this paper, "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit.

3. What do you think about my statement that:
I think boundary layer is more stable in turbulent flow as compared to laminar flow.
So, separation is smaller in Turbulent flow as compared to laminar flow. Since separation is smaller, so, drag would reduce in turbulent flow.
As a result torque should increase in turbulent flow.

1. We performed both the steady state and transient simulations but the results were under predicted and disappointing in most of the case.
We have used SST, Real KE and KERT turbulence model. All fail to consistently produce accurate results.

2. Since we don't have access to CFX we cannot independently verify the new transitional model by Dr. Menter. (may you can ?)

3. Regarding your statement I think that for a particular free stream velocity if the flow is facing a fixed pressure gradient the turbulent boundary layer will be more stable but not by a significant margin. This is my understanding, it may be wrong and I haven't performed experiments the validate this.

cfd_newbie March 21, 2011 06:39

One more query. What tool are you using to perform the BEM analysis of your blade ?

mohammad April 16, 2011 00:57

Quote:

Originally Posted by cfd_newbie (Post 300305)
Dear CFD XUE,
From my experiences in last 3 years of performing validation of NREL Phase VI experiments I have learned this lessen - predicting aerodynamics loads and power curve of wind turbine through CFD is a tough nut to crack.
See my post in the following section -
http://www.cfd-online.com/Forums/mai...irfoils-3.html
You can ask more for further clarification.
Raashid

Hi..I'm working on the same report of NREL..as you say you have good experience, can you send me some good results or reports or papers of your work or others you found useful.

I would be really grateful...

mohammad April 16, 2011 01:20

Quote:

Originally Posted by CFD XUE (Post 299611)
I am doing CFD simulation of Horizontal axis wind turbine by using Fluent.
Rotor dia = 6 m
Rotational speed = 20 rad/sec
Air velocity = 10 m/s
I am solving only one blade .....

Calculated torque (30 N-m) (moment about z-axis) is around 2.5 time lesser than the torque predicted by BEM (78 N-m). What might be the reason?
....

Dear all...
I'm working on the somewhat the same project and I hope my experiences may be useful.
I use double domain, (3.1 million node rotary domain+ 1 million node stationary doamin) in CFX .
PLZ pay attention to these notes if you haven't already done:
1-For accurate results I would like to say you must choose a good Turb. model which run well in separation..I found SST...
2- Try to satisfy number of nodes is the boundary layer and try to satisfy the Yplus criterion for your meshing .

One more Question for CFD XUE; are you sure that you have multiplied the value of moment for one blade by number of blades? 30 N.m is for one or after multiplication?

Cheers

cfd_newbie April 16, 2011 02:54

Quote:

Originally Posted by mohammad (Post 303845)
Hi..I'm working on the same report of NREL..as you say you have good experience, can you send me some good results or reports or papers of your work or others you found useful.

I would be really grateful...

Dear Mohammed,
Nice to know that you are working on the same problems.

I suggest you should take a look at the following papers for NREL, which will give you valuable information about wind turbine simulations.

"Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes",
R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA-2006-0395 44th AIAA Aerospace Sciences Meeting and Exhibit

and

http://wwweng.uwyo.edu/mechanical/fa...-2009-1221-908

I will be very happy to help you in anyway possible.

mohammad April 16, 2011 03:25

Dear Raashid,

Thanks a lot friend

cfd_newbie April 16, 2011 03:40

Quote:

Originally Posted by mohammad (Post 303854)
Dear Raashid,

Thanks a lot friend

No need for any thanks. Just inform me if you are bale to get correct and consistent results. I will be happy if you be able to do it.

monaya flower June 2, 2012 11:34

what about boundary condition for HAWT

s.q May 28, 2013 11:22

Quote:

Originally Posted by cfd_newbie (Post 300305)
Dear CFD XUE,
From my experiences in last 3 years of performing validation of NREL Phase VI experiments I have learned this lessen - predicting aerodynamics loads and power curve of wind turbine through CFD is a tough nut to crack.
See my post in the following section -
http://www.cfd-online.com/Forums/mai...irfoils-3.html
You can ask more for further clarification.
Raashid

hi raashid
i had simulated a wind turbine in fluent.
and now i want to calculate the output power using torque(report-forces-moment)
but this output power is 10 times bigger than real amount.


would you plz help me????


All times are GMT -4. The time now is 05:02.