[enry]

after A DAY of searching...i find the command:

you can do it through solve patch as following:

solve initialize initialize-flow
q
solve patch
fluidExt (interface)
fluidInt (interface)

x-velocity
yes
0
q
solve patch
fluidExt
fluidInt

y-velocity
yes
0
q
solve patch
fluidExt
fluidInt

y-velocity
yes
-12 (flow velocity)
q


In your opinion, why I obtain power coefficent > 1 on the blades (from 0 to 6 ) ? My vawt is like savonius, and maybe because the flow around the blades is folly turbulent.... what do u think about that?


Thanks!

[nana]

Hi enry:

You have Cp(power coefficient)>1, I do not have that, my Cp(power coefficient) is very low, I have calcualted the simulation results, it shows me the moment coefficient is around 0.3. However, the average cm = -0.3 at some rpm. I think my turbine is like drag device. I have tried with different rotation also, I mean let the turbine rotate clockwise and counter-clockwise. The result is almost same, i do not think the rotation will give the diffference.

I am doing the experimental set up now. And i need to model the 3D VAWT, Do you have any good suggestion for meshing?

For you problem, I have a good paper for you, i think it might helps. Please google Wind turbine power,energy,and torque. It's a chapter from wind energy system book.

All the best then.

[nana]

Hi Sagarmatha:

I am currently starting doing the 3D VAWT simualtion, I have some problem to make the hex mesh for that domain. Is there any good suggestion for me to do the meshing for 3D VAWT. My blade is straight, there are 4 in total. I need to do the 3D, becasue i need to compare my simualtion results with the tunnel results that I am doing currently.

Thanks a lot.

[esp-m1000]

Hi nana, i suggest you to don't use hex mesh for 3D model, try with t-grid.
I used size function on gambit to have a fine mesh near the blades and a coarse mesh far from turbine.
And Fluent works better with unstructure thetraedral mesh. I have done 2 different volume, one for free stream and one inside the first where is located the turbine, they are separated from interface faces that I set like grid interface on fluent.
Hope this could help.

I have 2 questions for you all guys,

1) On fluent I monitor moment on turbine during my simulation, If I make the turbine rotate in counterclockwise direction I have negative diagram for Cm and in the report forces i have negative moment, on the opposite if i make the turbine rotate in clockwise direction i have positive Cm and positive moment on report forces.
The problem is that my turbine must work with lift becouse it is like a 5-blades H-darrieus VAWT, so to work with lift it has to rotate in counterclockwise direction. I think that negative moment is due to the coordinate system, what do you think about?

2) report forces give to me the value in n-m, how i can get the kW produced?
for example for wind of 7 m/s, on the turbine i have a total moment (pressure moment+viscous moment) of about -7600 n-m, the time step is 0,0055556 s.

Thanks a lot guys....

[nana]

Hi esp:

THe moment that u ahve report from the fluent is consider as torque, as you can see the unit is N-m. It's easy to get the power , just using that N-m multiply with your RPM( rotating speed). That is the power you can extract from the turbine. Thus, you can find the power coefficient CP＝Pturbine/Pwind.

My turbine is 4 straignt blade, like Darrieus VAWT. Almost same as yours. the Cp is around 0.3. However, my Moment seems very low. I think it's becasue of the airfoil profile i am using is not much lift force can be generated. Actually i also try different rotating direction, the result is almost the same, it's only get the negative("-") sign there. But someone told me the negative value tells the turbine is drag device. I also not so sure. But i think should be the coordinate problem since I have try the simulation on that.

Thanks for the suggestion on the meshing. I have try it , it seems the problem is at the blade tip. I will try to figure it out. Thanks a lot.

[esp-m1000]

Thanks nana. Do you mean that you are not able to mesh the blade tip? Try to set an interval size mesh for blade faces tip. For example, I have an airfoil chord for the profile of 1.5m then i set interval size of 0.03.
For your Cp, I don't think that 0.3 is a bad result, Cp=Pturbine/Pwind must be <1, and if u consider Betz limit you know that it can't be >0.5926.
More, HAWT have 0.38<Cp<0.48, drag VAWT (Savonius) 0<Cp<0.16 and HAWT like yours 0.26<Cp<0.37.

I think that there is something wrong to find the kW produced, If I have 7600 Nm and than I multiply for angular velocity the result is unacceptable. i have an angular velocity of 120rpm that means 4π rad/s, if I multiply 7600Nm*4π rad/s=95504W=95,504kW.
I think that this is a too high value....suggestion?

[nana]

Hi esp:

I am sorry to bother u again about the 3D meshing problem. Yeah, I have tried the mesh using size function. But it still not well, there are some questions that i want to share with you.

Have you split the turbine part into different volume? Or you just have 2 volume, the turbine volume and one part is tunnel area.

I also sing size function, how many have you got for the 3D volume meshing? I have tried starting size 0.001-0.03, growth rate from 1.05-1.2, and maxium size 0.1-1. But there are still some bad cell, skewness >0.8. I am using T-grid for the turbine area.

Or have you try to mesh the edge, then face then volume. or you just using size function for the whole turbine volume?

thanks a lot for the sharing.

[esp-m1000]

Hi nana, no problem in ask, when i have some question i will ask too.

I have done many mesh of the turbine, for example structured mesh with hex elements, but in this case the turbine volume was divided in so many volumes, and wasn't so confortable to set on fluent.
More, with thet mesh u will have more element in your mesh (i.e. imagine an hex divided in two parts), moreover you have more cells but fluent works better with thet than hex.
How i have done the mesh: First I did the turbine like volume element, after i done a cylinder, and subtracted the turbine from the cylinder.
I have used a symmetry face, becouse the turbine is symmetrical respect z axis. Then I have done a big volume always symmetrical respect z-axis which include the cylinder-with turbine.
Now i have meshed the faces of the turbine, with interval size of 0.003, but the chord of the airfoils of my tirbine is 1.5 m. So if ur turbine is smaller u have to reduce this factor.
After the mesh of the turbine i have done a size function for the first symmetry face, that is the bottom face of the cylinder, this is a circulare face where there are some holes, that are the airfoil of the blades and the shaft of the turbine (remeber for me this is a symmetry face so there are the same on the opposite).
So for the size function i used

type:fixed
source:edges (i insert the edges of the airfoils and the shaft)
attachment: faces(i insert the symmetry face)
start size:0.003
growth rate:1.1
size limit:0.03.

Then I have meshed the symmetry face. Control if u like the mesh, if not, go to change the value for the size function.

Now i have done a second size function for the cylinder in which is located the turbine.
type:fixed
source: faces (i insert the faces of the turbine)
attachment: volumes(i insert cylinder)
start size:0.003
growth rate:1.1
size limit:0.03.

Than i meshed the volume.

For the end I meshed the external volume that correspond to the free stream.

I used again a size function to have a fine mes near the cylider an a coarse mesh far from it.
I have mesed the surface that are interfaced with cylinder surface (in fluent I used grid interface to use sliding mesh)
and than i used size function from this faces to volume.

Hope this will be helpful. If u have red my last post, can i ask u what do u think about the power i have?

[nana]

Hi esp:

Thanks a lot for the detail explaination. I also try structured mesh with hex elements, but in this case the turbine volume was divided in so many volumes, and i totally agreed with you that wasn't so confortable to set on fluent. I have try the t-grid, it seems the results not that good. But i think it should be no problem after trying.

For the Cp that you mentioned last time.HAWT have 0.38<Cp<0.48, drag VAWT (Savonius) 0<Cp<0.16 and HAWT like yours 0.26<Cp<0.37. I am a bit confused, For my case, i am doing S-VAWT, straight blade vertical turbine like Darrieus types. I have done the 2D simualtion, it seems my trubine is like drag device from the Cm(moment coefficient). For the HAWT(Horizontal) you mean? If yes, the maximum Cp should around 0.5. the VAWT straight blade, the Cp is from 0-0.25. So what is you case? And the Cp for 2D is slways higher than 3D. Let me know what is you case, i might can share some journal papers with you.

For my 3D geometry set up, kindly hope that you can spend few mins to have a look on the pic. I think the geometry should be no problem as I have done the 2D slidng mesh already. If you ahve any question, no problem to pop up. thanks

[esp-m1000]

Hi nana,
sorry, when i wrote "HAWT like yours" i mean VAWT. But the Cp values i gave to u are right. I'm doing simulation on a VAWT similar to yours but i have 5 blades instead of 4 and a non-symmetric airfoil. But this don't mean ur turbine works with drag; Lift is always bigger than drag for airfoil, if they work in normal condition (no-stall).
So your turbine works with lift.
I have looked at your model, i think that cylinder surface are too near blades, and the free stream volume is also too little. I think u must have a bigger cylinder in whinch locate the turbine and a bigger free stream volume. If u can't becouse u have to simulate in a real wind tunnel maybe u have to use a scaled model and so reduce the scale of your model.

For my simulations I have a problem, i had a report moment of 7600 N-m, how i can obtain the power? as i wrote after if i multiply for the time step i obtain a too high value.....

[nana]

Hi esp:

I am doing both simualtion and experimental for my 4blade VAWT. The model I have make for my wind tunnel test with blade dimension 0.1m(chrod) and 0.4m(length). The experimental will carried in the closed loop wind tunnel with square dimension 720mm(Height)X780mm(width). My simualtion geometry set up is based on the tunnel dimension that I am going to used. So I cannot extend as you suggested I think since I have the space constraint. Am I right?

Another question, If i want to compare my results, I need to keep my Re no is the same for both case, then play with the wind velocity.Since I am using chord as 0.1m and 0.4m length for my simualtion turbine blade as well. You have any idea on that?

For the power that you are talking, are you sure you have report the correct one? You need to fix the moment center, in your case, if you set your rotating coordinate (0,0,0), you should set moment center at that point too. And only pay attentation on the torque at the Tz(in z direction) rotating axis. Then you using that value multiply the RPM. This is the mechanical power u got. You need to divide the Wind power as well since the wind velocity is also influence factor, then you can see how much Cp you can obtain. I Think the maximum can obtained is ard 25%.

[esp-m1000]

Hi nana,
If u must use this geometry value i can suggest u to use size function to obtain the mesh but also to mesh cylinder surfaces in the same way of the turbine blade.
So if u use for blades interval size of 0.001 u must use the same value for the cilinder surface.
More if u have too many cells in this way i suggest also to divide on x-y plane ur geometry.
For wind tunnel volume u can use coarse mesh.

But i don't know if this could be a good simulation. Also experimental results in ur wind tunnel maybe will not be so good, u must considerate the interaction between turbine and wind tunnel walls that i think are too close to ur model.

Yes, Reynolds number must be the same for compare results, u can do the sperimantal analysis on a scaled model and operate appropiately to compare the results with CFD in which u will use a full scale model(in this way u can increase the tunnel and the cylinder dimensions). This is an hard way and u will have only an approximative analysis.
Let me know.

For my case, u suggest to multiply for rpm.
Yes I set the rotating center on (0,0,0) and i monitor moment on (0,0,0) and i select the surface turbine. The moment on z-axis is about 7600 N-m, now u suggest to multiply for rpm, but to obtain W i must divide Nm for seconds
W=Nm/s

Can u do a real calculation with my result?
For example I have a moment on z-axis of 7600 Nm, the time step used for unsteady simulation is 0.00555556 s and the turbine has 120 rpm.

Thanks a lot

[nana]

Hi esp:

There are few things I need to clarify with you. No matter how big the geometry i used for my simualtion, I need to make sure the Re number is the same. Even i do the real full scale turbine for my simualtion, but I still need to make sure the Re is the same. So the result will be similar no matter your geometry is big or small.

I know that there will be some interaction or wall boundary between my turbine and the tunnel wall. In the real turbine, there is no wall exit, so the experimental results might not that accurate due to all this constraints and some errors. However, i can just compare with my own simualtion and do the optimization for the blade and study the turbine performance. Anyway, this Phd research is a learning period. I have lots of problems for my experimental set up as well. But I can solve it soon.

By the way, do you ahve any idea about the real VAWT turbine size. How much is the Chord and length, how about the Re, you have any idea on that?

For your problem, you want to get the power output and study the power coefficient from the turbine, i think most of people using Cp instead of get power directly. However, based on the value you gived, it seems so large. Are you sure this is the converged solution? If i am not wrong, the Cm should be periodic at different time step. Your time step for unsteady state looks ok for me. I do the roughly calcualtion, but it seems sth it's wrong.

The mechanical power you ahve got for yout turbine Pm=torque * rotating speed (rad/s) = 7200* (120*2*pi/60)

The power that you have obtain from wind Pw=0.5*rho*wind velocity^3*turbine frontal area

The Cp=pm/pw

How about your TSR and velocity for your turbine. I think there are something wrong. Please double check your solution is converged. How many revolution have you set to get the converged solution? Do not worry, you go through your simualtion again and let me know if still have problem. I try my best to help. heehee

[esp-m1000]

Hi nana,
Yes, to have a good simulation to compare with real results the principals adimensional numbers like Re must be the same.
However I think that if u can dispose of wind tunnel and cfd analisys, u can operate also if the wind tunnel walls interact with ur turbine settign the same conditions in both cases. So go on. (I'm really interessed in what are u doing, let me know)
Have u finished the mesh?


I know, there is something wrong on my results, maybe there are some mistake in my simulation but I don't know where.
The chord length is 1.5m, and the Reynolds number calculated as:

Re=(rho*V*c)/mu

the Re number will change with wind speed and with the movement of the blade around the circumference.

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.

Go to mechanical power on the shaft.

Form this calculation I have a Cp=4.5 that is unacceptable.

What do you mean with TSR?
The solutions are converged for each time step, and the revolutions are about 12, because I set 0.00555556s for time step and 1080 time step, so, in 0.00555556s the turbine rotate of 4° and 1080*4°/360=12.

The condition I set are:
define -> model -> solver: pressure based solver, unsteady
define -> model -> viscous: k-epsilon standard
define -> model -> energy equation on

Boundary condition:
Define -> boundary condition
velocity inlet: velocity specification method -> components, reference frame absolute
fluid, in which is located the turbine: motion tipe -> moving mesh, rotational velocity -> 120 rpm
turbine (wall): wall motion -> moving wall, motion -> relative to adjacent cell zone.

Solve:
solve -> control ->solution
URF(under-realaxation factors) the values that fluent gives
pressure-velocity coupling -> SIMPLE
Discretization: Pressure -> PRESTO
All at second order upwind

solve -> monitors -> residuals: i set print and plot and leave the values given
solve -> monitors -> force: options: print, plot and write
wall zones: turbine
coefficient: moment
moment center (0,0,0)

solve -> initialize -> initialize: all zones

solve -> iterate

What's wrong?

[esp-m1000]

Hi nana,
I surfed on the net all these days to find a solution to my big problem concerning the moment on the shaft.
To be honest at first I didn't consider the TSR (i think u mean tip speed ratio) becouse i don't know how to find the optimus TSR for my turbine.
I wanted to do some simulation for different wind velocity, like 3 m/s to 23 m/s with step simulation of 2 m/s, to obtain a power diagram with at the same rpm.
But this approach give me the wrong value for moment and so for the Power.
Now I don't know what to do and what to change.
Do u think i must set a different angular velocity, function of TSR?
and if yes how to calculate the TSR?
Have I to choose one reasonable value?
For example, have I to choose a TSR, 4 for example, and so calculate the angular velocity function of TSR and wind speed?
So if i choose tsr=4=wR/u
w=angular velocity
R=turbine radius=4.5m
u=wind speed
for wind speed of 9m/s
i have w=TSR*u/R=8rad/s=76 rpm.

In the last post I write the conditions i set on fluent. Do u see something wrong?

Thanks so much……

[ambermgupta]

hi esp.reading yours and nanas post for a while now,for i am too simulating vawt.
in fluent there is explicitly no fsi module and so you have to input w.
now according to certain articles published[can mail them if u like],optimum tsr for savonius is near about 7 i.e for tsr =7 u will get the highest T.
SO THE BEST WE CAN DO ,I BELIEVE IS ASSUME TSR=7 AND PLOT T VS V[WIND SPEED].
NOW HERE IS MY QUESTION R U CALCULATING T THROUGH MOMENT COEFFICIENT OR UDF.JUST TO BE SURE ,IS THE T SO OBTAINED IS AT CENTRE OF MASS .[T=1/2DENSITY*A*V[2]*C]

[esp-m1000]

Hi ambergupta,
I don't understand what do u mean for "no fsi module".
Now i'm doing a simulation with TSR=4 with wind of 5m/s.
I'm not working on a savonius but with a darrieus.

I don't calculate the T with a UDF, but I obtain moment from fluent report.
I think the T obtained should be given from the relationship you worte, but the problem is that V change repedeatly with the rotation of the turbine becouse is given by the sum of wind velocity and the angular velocity of the turbine, so it isn't so easy to calculate.

As i have said above I'm doing right now a simulation with TSR=4 and wind velocity
=5m/s on 2D model.
But there is always something wrong, becouse I have a Moment of 225Nm (the report moment is negative),
that gives me a Power of Pe=225Nm*42RPM*2*pi/60=989W.

But wind energy is less Pw=1/2*rho*V^3*D(diameter)=1/2*1.225*5^3*9=689W

so Cp=Pe/Pw=1.43

I'm becoming mad about this.

[sagarmatha]

hi ambergupta,

can you give me the titles of the articles regarding savonius turbines running at tsr=7? i am a bit confused as to how these vawts can run at high tsr when they are drag machines. if they used the Rahai profile then maybe they can have some lift properties that increase torque at high tsr. otherwise, max power coefficient for ordinary savonius (S-type) is at tsr=1. with overlap it may be higher.


high esp,

how do you compute back the torque from the moment coefficient report of fluent? do you multiply the average by 0.5 x rho? i assume you get the average of the last few rotations of your simulation (assuming periodicity is attained).


thanks.

[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.

[ambermgupta]

hi sagar
my bad,i incorrectly mentioned 7 instead of 1 lol 7 is just too high!!!!
now regarding torque issue f=force on blade=k*[v-wr][2] k is some constant.so if f is varying t will vary . u r right esp it is not apt to measure t through measuring cm.

esp r u using mrf??if so here is the problem with ur method
fsi means fluid structure interaction,ie turbine rotating because of air falling on it,in our case we mention w beforehand.
therefore i could mention w =1000rpm for v=1m/s and get ambiguous reading.
in MRF case T*W=CP*K*V^3 DOES NOT HOLD AS I CAN VARY W AND V INDEPENDENTLY .THIS METHOD IS ONLY GOOD ENOUGH TO STUDY FLOW PATTERN AND COMPARE DIFFERENT GEOMETRIES [LIKE SHAFTLESS VS ONE WITH SHAFT] IN WHICH CASE WE R MORE CONCERNED ABOUT COMPARITIVE READINGS THAN ABSOLUTE .IF YOU HAVE EXPERIMENTAL DATA U CAN INCREASE V FOR A GIVEN TSR VALUE TO GET CP<1.LET ME KNOW IF MY RESONING IS WRONG.