[nana]

Hi enry:

Thanks a lot for the detail explanation on the whole thing. However, i think we talk the different Cp at the moment. Your Cp here is the power coefficient, yeah, it should be around 0.3, based on the Bets limit Cp=0.59. The Cp i am refer is the pressure distribution on the blade. Which defines as following:
Cp= P(local)-P(reference)/0.5*rho*v^2*chord length

However, i cannot get the cp lower than 1.

Since you already have the reasonable result on that, can i ask something more in detail. I am doing the 2D and 3D simulation and the wind tunnel experimental also. But I am using SD8020 profile as my blade section, I have the water tunnel test data from my friends which i can compare with. Or which airfoil section have you using? I can help you to look around if i got any relevant paper for you.

Well, I know that y+ is important for the turbulence model. However, for my case i am using stand wall , my y+ is >30 definitely. I am using standard k-epsilon. I have tried to using realizable k-E, however, it seems the residual goes up. I think my solution is not converge, i normally only run 1 0r 2 revolution then stop it to see the result.

Oh, how many blade you have, my VAWT have 4 straight blade. As for the boundary condition, i am using velocity inlet and pressure outlet with sliding mesh. How about your TSR and RPM for the turbine. I am doing TSR=3 with u=3, so the RPM=32.14rad/s=307rpm. I am trying to simulate different TSR with different Wind velocity. Then to obtain the torque curve in order to select the generator for my experimental. How many grid cell have you got for your 2D mesh? Do you refine the mesh? Is there any improvement for the result when you refine the mesh?

Last question, how you set your dt based on free stream velocity and RPM? I am using 60/RPM*1/n, so normally my dt =0.001. I need 300 time steps for one revolution with every 20 inner time step iteration.

Have you checked if your cp solution is converged?(what you mean). The Cm here you mentioned is moment coefficient? How to define that, i know fluent can report the moment.

I have some conference papers just got it today, you may have it.
Numerical simulation of unsteady flow and aerodynamic performance of VAWT with LES

I have another one, but cannot find it now. I will email to you tomorrow when i find it. I also have some experimental data paper if you need it, let me know. Thanks a lot.

[nana]

Hi enry:

Another journal paper. "wind tunnel and numerical study of a small vertical axis wind turbine"

I cannot rem which paper indicate 5% for turbulence viscosity. If i find it out, let u know then

[enry]

Hi nana, thanks for your article, but I'm studying a VAWT like savonius . However I make some 2d simulation with profiled VAWT.

1st. I'm not so sure that pressure coefficient should be less than 1, because profile is rotating and the free stream velocity is not relative velocity, and Pref is based on free stream velocity. What do you think about it?
2nd. I tried to refine my mesh, and results is the same. Pay attention to boundary layer size: keep always the same boundary layer, in order to have desired fine mesh at the blades, than refine other domain. Also build a domain at least 5-6 times bigger than VAWT diameter. My 2d mesh has around 30.000 cells.
3rd. I think that your dt is good. However in fluent manual there is a chapter that describe how to set it. As far as I remember you can set dt in order to have CFL number less than 30-40; check it with fluent postprocessing, there is a gui command on fluent.
4th. Cm is moment coefficent. Fluent can give it to you through gui command: solve-monitor-force. Pay attention to reference value setted in: report-referece value.
5th. I check if solution is converged trough UDF. I wrote a UDF in order to calculate a power coefficient at every time steps, so you can obtain a curve of Cp that can help you to know if solution is converged or not. I think that 2 revolution is not sufficient to have solution converged. However, before to write UDF, try to simulate for 2 and for 5,6 and 7 revolution of the turbine, and compare Cp value. I'm quite sure that 1 revolution is not enough! Use at least 3-4 revolution. However every simulation has different time to converged, even if the VAWT is the same.

I hope that my advice can help you!
Enry.

[nana]

Hi erny:

Thanks a lot for all all the suggestion. I also have some paper on your topic. But it's not 3D simulation. If i got it, i will email to you then. There are some doubts that i want to clarify with you:

1st, How much is the Re number for your case? TSR and Wind speed that you applied for the simulation? The dimension for my blade is with 0.1m chord and 0.4m length. The Re no for my case is from 21k-68k(u=3m/s) up to 10m/s. So the selection of turbulence model should be very careful. Because the standard k-e turbulence is for large Re.

2nd, The Cp(pressure coefficient) I still think should be lower than 1. If using the rotating velocity means the relative velocity. It express as [sqrt*U(free)^2+(wR)^2], it should be large than free stream velocity. What do you think.

3rd, The CFL condition is only applicable for explicit solve, however, for implicit solver, CFL no does not matter for the stability control. Am i right. But in your write up, it also looks reasonable for me.

4th, What kind of UDF that you wrote it for plot Cp(power coefficient). So you mind share with me. I just want to have a look see whether it will helps me out for my problem. My mail address is helenishere30@hotmail.com

Thanks in advance!

[enry]

1st. Re in my case is about 150000, fully turbulent flow. I use both realizable K-E and RNG k-E, and shows the same results. RNG k-E is both for low and high Re, but I think of course that our problem is fully turbulent, and Re is high enough.

2nd. I can't answer to this question... why do you think that Cp must be lower than 1?

3rd. The 1st and 2nd order implicit scheme (if I remember well Implicit Euler and BDF2 ) are stable under no condition. But FLUENT suggests the following advice:

(From:
http://my.fit.edu/itresources/manual...pdf/ug/pdf.htm
chapter 25.17, page 25.113.)


If you have chosen the 1st-Order or 2nd-Order Implicit formulation, the procedure is as follows:
(a) Set the time-dependent solution parameters in the Iterate panel

Solution parameters for the implicit unsteady formulations are as follows:

[...]

To determine a proper choice of Dt, you can plot contours of the
Courant number within the domain. To do so, select Velocity... and
Cell Courant Number from the Contours of drop-down lists in the Contours
panel. For a stable, efficient calculation, the Courant number
should not exceed a value of 20-40 in most sensitive transient regions
of the domain.



4th. Sorry, but I can't share any detail of my work, for privacy. I hope you can understand.... But I can give you any advice if I can.

What do you think about 2nd question? And why do you think that Re=150000 is a low Re ? I think that our problem is very very very fully turbulent ...

[nana]

Hi enry:

1St, I said low Re is based on the normal turbulence flow. In my case, Re is between 21000-68000 because of the small model such as chord length (0.1m).The RNG k-e model with differential viscosity model to account for low-Re effects. However, I have tried Realizable k-e, it seems not work well for my case. Have you try any other discretization besides PRESTO for pressure, and 2nd upwind for momentum? I have tired PISO with PRESTO and standard for pressure and 2nd upwind or QUICK (for quad mesh) for momentum, but It seems the SIMPLE with standard pressure and 2nd upwind for momentum give the best results.

2nd, the dt for my case is 0.001, it needs 314 time step for one revolution. I have check the Courant no for my case, I think it should be fine.

3rd, the Cp (pressure coefficient) I think should be smaller than 1 is based on the theory. Anyway, my cp is always larger than 1. I am not too sure about that. I will clarify the Cp and share with you.

4th, it is totally understanding by without share the things. Do not worry. I just want to know how to write the UDF to define and confirm the solution is converge so that I can ensure that my results are acceptable. Or you have any good suggestion for me?

Lastly, the Re for your case is large, it definitely be turbulent flow. But for mine, I think the model is small for my case. My Re is only 21000 for U=3m/s. But anyway, I do not think I can said that my Re is low since there is no exact definition to define the high and low Re.

Heehee, thanks and really enjoy the time to share all the experience with you.

[nana]

Hi Enry:

I using parallel computing for my current simulation. I have all the data file at different time steps. You have any good suggestion for me to do the post-processing. I try to using Tecplot, but i need to read the data file into Fluent then export as Tec.dat again, which is a bit time consuming. Any other software you recom. Paraview? or Ensight? Should i need to write a script for reading the data files? Thanks a lot.

[enry]

Hi nana!

I set PISO for pressure-velocity coupling, and for Discretization: PRESTO! and 2nd order Upwind. It seems to be the best way to obtain reasonable results, but SIMPLE didn't show me different result obtained from PISO scheme.
I think that Cp may be lower than 1 only on that profile that is at a low angle of attack; if the angle is too large I think that you can't say that; however the flowfield is everywhere turbulent and rot(V) != 0, so I don't know how to predict any results.
To write UDF you have only to calculate the power coefficient at every time steps. If you never write an UDF I advice you to read the UDF manual.
I don't run in parallel...however, why do you want to use an other post-processing program? Why don't you use FLUENT post-processing? Don't you like it?
I used parawiew only when I want to analize OpenFOAM results, but I think that for FLUENT is better FLUENT itself.

Bye!

[tony00]

Hi everyone!
I am still doing 2D simulations of VAWT. Has anyone tried simulating with different meshes and turbulence models (say realizable k-e and k-w SST)? Do you get the same results?
I find the solutions are strongly mesh and turbulence model dependent. Realizable k-e gives considerably higher Cp than k-w SST with the same mesh and same set up!
Is anyone experiencing the same?
How about mesh dependency study? Do you guys have different meshes which give the same results?

Cheers!
Tony

[esp-m1000]

Hi guys, I'm still having problems with my VAWT. I had not time to work on it in the last period, but now I'm starting on it again.
I have done a new mesh of my turbine, I use hexaedral mesh for all the volumes ( I have a 3D model).
When I read the mesh on fluent all work greatly, also if i check the grid, I have done some simulation with steady conditions and the solution converge after about 365 iterations. Now the problem, if i set the solver as unsteady fluent says "Warning: non-positive volume exist". and after starting the iterations it says "Error: divergence detected in AMG solver: pressure correction".
I don't know what to do.
Thanks in advance.

[enry]

Hi esp-m1000.
The answer is simple. You have to change your mesh for unsteady simulation. You have to use sliding interface. Read the manual to understand how to set it .

Bye.

[esp-m1000]

Hi Enry, and thanks for your quick help.
I will try soon.
But, where I must use sliding interface?
And if I can ask, where can I find it in the manual?

[tony00]

Hi esp1000,
in Sect. 11 of the User's guide and in Tutorial 11 you'll find the explanations for setting up an unsteady sliding mesh simulation. You might also be worth having a look at Tutorial 9 which is Multiple Ref. Frame for steady simulations (but you should not need it).

Regards

[nana]

Hi enry:

I have try different turbulence k-e with RNG and Realizable model for my problem with Presto and standard for pressure discretization.

I have compare the results about the pressure distribution on one blade, i also calculate the Power coefficeint (Cp) based on the moment that report from fluent. Cp=Torqure(momentum)*omega/0.5*rho.v^3*dia, it seems the ke-RNG-with standard pressure discretization give me the best results compare to the Presto. The totoal moment that i Have based on the report data from fluent is around 0.017Nm, however, the k-e(RNG)wit hpresto give me -0.072. I also tried the realizable with standard and presto discretization, but the mometum i gained from ke-realizable-presto is 0.685 and standard is -0.04.

My question is : is the negive sign does not matter is it? I do not have experimental results to compare as i need to compare with my own experimental results which i Have not done yet. I also try k-w sst, but it give me error with the same set up. i think sst is not for my case. So i think RNG-standrd or RNG-presto gives me the best and reasonable results. But i still want to compare which one is the best. But i do not have dat to compare.

How u compare your results? Any suggestion for me ? I have try to monitor the velocity at the outlet of the tunnel in order to get the converge results after no.of revolutions. It seems with lower rpm, it converge ard 6 revolution and higher rpm need more revoltuion to converge. Is my way to solve the problem correct? any commence? Thanks a lot.

[sagarmatha]

Originally Posted by esp-m1000

Hi Enry, and thanks for your quick help.
I will try soon.
But, where I must use sliding interface?
And if I can ask, where can I find it in the manual?

hi esp-m1000,

to use the sliding mesh technique, first you need two meshes. one is for the fixed mesh, other one is for the rotating mesh (circular mesh). these two must fit perfectly re: diameter of circular rotating mesh must be equal to the diameter of the "hole" in the fixed (stationary) mesh.

then you have to read one of the meshes first (File>Read>Case). it doesnt matter which you choose first. then, to add the other mesh you have to go to Grid>Zones>Append Case File.

dont forget to define the grid interface. also dont forget to do a grid check.

hope this helps.

[nana]

Hi Sagarmatha:

I have some doubts about my simualtion results for my 2D vertical axis wind turbine. I am using both k-e RNG and realizable turbulence model with k and e turbulence specification, it seems RNG with standard pressure discretization give me the good and reasonable results. When i report the moment, i have 0.01657nm, and the calcualted power coefficient =0.3, by multiply the betz limit Cp=0.18. However, when i try to use the same condition, by change the turbulence specification to turbulence inensity=5%, and length scale =1. I have report moment = -0.044. The rpm=191 and freestream velocity=3, chord length=0.1m for this case.

My question is why the difference so large. Why have negative sign? Do u have any experience about the Cl and Cd value for this case.

thanks a lot for the reply and help.

[sagarmatha]

Hi nana:

you might want to compare what the values of k and e are when you specify turbulent intensity and length scale. if they are a lot different from your original k and e specifications, then that could be a reason.

how come your length scale is so large? its 10 times bigger than your chord length. do you expect the eddys generated to be really big? the negative moment coefficient could mean drag is dominating in your experiment (very much like what happens when you set a TSR that is really high, say 10).

what you set as an inlet condition is not what the VAWT sees as there is turbulent intensity decay from the inlet to the point where the flow hits the VAWT. try to plot the turbulent intensity contours for both simulations and compare the values of Tu at the point very close to the VAWT.

[esp-m1000]

Hi sagarmatha, I have meshed again my model with two separate fluid zones, the surfaces are not connected, but when I check the grid on fluent it says:


WARNING: Unassigned interface zone detected for interface 6
WARNING: Unassigned interface zone detected for interface 7
Checking storage.
Done.

WARNING: Check grid failed.

On gambit I set the surfaces as "interface" what's wrong?


EDIT: solved following tutorial 11

[nana]

Hi esp:
you need to go fluent>solve>grid interface, then set interface 1 and 2 from each zone. Then creat the common interface , after that u check the grid again. It should be no problem.

[sagarmatha]

hi esp:

in my version of fluent, its Define>Grid Interface. type a name for the interface, select one interface on the left column, select the other interface on the right column. do not tick periodic and coupled. then click create.

as nana suggested, do a grid check. there should be no problem after this.

do not forget to define the moving mesh rotational velocity in the boundary conditions. mind the units (rpm or rad/s, depending on your units setup).