[esp-m1000]

Hi nana,
Thanks for help, at moment i'm doing some simulaiton with a mesh with bounday layer, as sagarmatha advised me. He looks one case and data file i sent to him and he found some wrong on y+ function.
Hope this could be the solution.
I have some questions, what do u mean when u said "I also have the negative TSR for my previous simualtion when i mointor the Cm"?
Can u share with me the condition are u using? Like rpm and tsr? and the result u obtained?
and the last one, how do u obtain the average moment after some rotation?
Thanks again.

[nana]

Hi esp:

I do not think bounday layer is suitable for the case, and based on my own experience, y+ value won't affect much even you try the BL. I have tried different y+ value with different set of mesh before, but it seems not much difference. However, if you want to try to prove, jsut try it. I think the msot error is based on the BC set up.

Well, you can give me your email address, i can send my Cm plot to you ok.

[sagarmatha]

Originally Posted by nana

Hi esp:

I do not think bounday layer is suitable for the case, and based on my own experience, y+ value won't affect much even you try the BL. I have tried different y+ value with different set of mesh before, but it seems not much difference. However, if you want to try to prove, jsut try it. I think the msot error is based on the BC set up.

Well, you can give me your email address, i can send my Cm plot to you ok.

i would beg to disagree. i think using a boundary layer (especially the viscous sublayer) is critical to vawt performance prediction. here's why. if you use standard wall functions, you are already assuming a certain shape of the boundary layer. this is ok if you know that what the blade sees is consistently the same. but for a vawt, the flow phenomena is highly unsteady. there is dynamic stall vortex shedding, trailing edge vortex shedding, multiple blade-wake interactions, massive flow separation, etc., etc. gradients parallel and perpendicular to the blade surface are not low. this is not the best candidate to be using standard wall functions. you need to resolve the boundary layer up to the viscous sublayer. you need to have a finer mesh so that the solver can predict the flow field up to the wall, not just assume a certain behavior/shape as what standard wall functions do.

also, y+ is a critical parameter to monitor for good near-wall mesh. if you are using fluent, it suggests a y+ of 30-300 for standard wall functions and y+ average of 1 (with no values exceeding 5) for enhanced wall treatment. the reason why it is important to have a good near-wall mesh is that if you assume a fluid element with shear and pressure forces acting on it, the one responsible for the rotation of the fluid element is the shear. where do you get shear? in may cases, if you have a wall, you will definitely encounter shear forces on the wall that cause your fluid elements to rotate. this is a very important factor in the behavior of the fluid past a wall. this has massive effects on the factors that give lift and drag to a blade. for a static airfoil case, you may not experience significant differences in the results. but for a pitching and plunging airfoil, lift prediction is very sensitive to near wall mesh. even the prediction of flow behavior dramatically changes with different near wall meshes. if you ignore y+, you dont know if your simulation results are sensible or not. also, some turbulence models are sensitive to y+, especially those that try to predict laminar-turbulent transition on walls.

[nana]

Hi Sagarmatha:

I totally agree that y+ is important when chooseing the turbulence model. I also agree that different y+ value need the different turbulence scheme for better and accurate results.

However, I have tried with different Y+ value like Y+=1 using the enhance wall boundary method and also Y+=30~500 using standard wall function to see the difference. The trend is the same, only a bit difference shows in the results. Of course, if you want to see the bounday layer and also the blade interaction, that one is crucial. I jsut say that based on my own simualtion results.

[sohail_27]

Hi all,
I am working on 2D simulation of VAWT using gambit and fluent. I started my work by creating mesh file for single airfoil in vertical motion. I created a central stationary mesh then a circular mesh strip around it which contains airfoil & which would be moving, then i created interface region (again a circular strip) around the moving mesh and finally a big rectangular domain of about 30 times the chord which is stationary mesh. i used velocity inlet for inlet region and pressure outlet for outlet region and pressure farfield for upper and lower edge of rectangular domain and wall for airfoil, but i dont know what BC should i use for interface region in between and in fluent how should i rotate the mesh with some angular velocity so that airfoil would rotate. I read somewhere that we need to write a UDF for that?? Initially i want to compute for flow coming in with Re=10^6 and blades are rotating with 60rpm.
i would be glad if anyone could help me out.
Thanks and Regards.

[sagarmatha]

Originally Posted by sohail_27

Hi all,
I am working on 2D simulation of VAWT using gambit and fluent. I started my work by creating mesh file for single airfoil in vertical motion. I created a central stationary mesh then a circular mesh strip around it which contains airfoil & which would be moving, then i created interface region (again a circular strip) around the moving mesh and finally a big rectangular domain of about 30 times the chord which is stationary mesh. i used velocity inlet for inlet region and pressure outlet for outlet region and pressure farfield for upper and lower edge of rectangular domain and wall for airfoil, but i dont know what BC should i use for interface region in between and in fluent how should i rotate the mesh with some angular velocity so that airfoil would rotate. I read somewhere that we need to write a UDF for that?? Initially i want to compute for flow coming in with Re=10^6 and blades are rotating with 60rpm.
i would be glad if anyone could help me out.
Thanks and Regards.

i dont quite get what you mean. you are simulating a vawt but with a single airfoil in vertical motion?

regarding your mesh, how come you are using more than one interface region (one between the central domain and the rotating mesh and the other one between the rotating mesh and the outer domain)? using interface regions introduces numerical errors and noise in the computation (fluent interpolates values when nodes do not coincide at specific points in time during the sliding). so you must use it only when necessary. why not attach the central domain to the rotating domain and let that rotate as well. put a center post to include the effects of the post on the wake downwind.

regarding BCs, if you are using farfield on two boundaries, why not use farfield on all? specify velocity as a function of mach number. enable energy equation, use ideal gas for air density. see to it you are aware of the temperature setting as speed of sound in dry air is dependent on temperature. if you do this (specifying farfield on all boundaries), you will avoid reverse flow warnings on your fluent run. just be sure your boundaries are far enough. your 30 chord lengths distance does not give us a good picture because you have not told us your vawt diameter, airfoil chord, or vawt solidity.

in defining interface regions, do a back read. it has been posted already. you do not need a udf unless you want variable angular velocity. for constant angular velocity, moving mesh with rotational motion defined is sufficient.

[sohail_27]

Hi sagar,
I am starting my simulations with a smaller VAWT in order to save computation time, My VAWT has diameter of 4. I am searching for posts related to how to move mesh for VAWT in the same thread. I was following fluent tutorial for preparing mesh for sliding mesh, which uses a interface region between stationary grid and moving grid so i did the same, but i experienced some error using interface, when i am actually initializing the problem in fluent it gives a warning that periodicity for interface region is not set. what does that mean? can you help me out? And how can i rotate grid with out using interfaces. Please help me out Buddy.

Thanks for your reply.

[sohail_27]

Hi all,
I am working with VWT 2D simulation, i am using moving mesh method to rotate airfoil, i created stationary mesh for center region and am moving the grid around airfoil, but when im initializing the problem in fluent it gives an error that no periodic zone adjacent to grid interface, i have no clue what does that mean, can anyone help me out please??
Thanks

[nana]

Dear all:

Is there any one doing helical twist blade profile for VAWT. How should i make that turbine blade profile? Anyone can give me some idea? I need to do the numerical simualtion on that trubine and study the turbine performance. I really appreciate that anyone can provide some information on that.


Thanks

[nana]

Hi Sagarmatha:

I am doing validation study for the 3D VAWT with 3 straight blade. I have do the simuation using Fluent to compare the Cp with TSR with one journal paper. The blade profile is NACA 0022 and with chord 100mm and span 400mm. The rotor diameter is arond 600mm. I have tried to mointor the moment coefficient around 10 revoultion using k-e RNG and k-w SST to compare the results with 2 wind speed at 5.07m/s and 5.81m/s from TSR = 2.1 to TSR=2.5. However, i have negative cm when TSR increased to 2.4 and 2.5. I change the time step to 0.001, then i can get the positive cm. Now i am trying to use SA (my prof ask me to try) with the same set up, howver i have negative cm at TSR=2.4 and TSR=2.5. Why it has the negative value. Do you have any suggestion?

I thins the One possibility is becasue the moment will be drop when the turbine rotational speed reach its maximum. However, the SST and RNG turbulence model gives the positive cm. I am a bit lost now. Kindly hope that u can give any suggestion. Really appreciate on yr help.

[grogibear]

Hi all,
for the rotating mesh for VAWT is it similar to the tenth tutorial? I have set up in GAMBIT a NACA 0012. There are the outer and inner regions which is stationary and a denser circular part in which the blade is placed. Do I set up walls in Gambit and then redefine them as interiors like in the tutorial? I have tried simulating in FLUENT once but I think my blade is stationary and the circular fluid is rotating. The tutorial has a small section where one defines the blade as rotating with the surrounding zone but I'm not sure how this works as I never made any relationship between the blade and the rotating section.

Any assistance would be appreciated greatly.

Conor, MSc Student

[nana]

Hi Esp:

Have you still working on the VAWT tubrine? I have negative moment coefficient. I think you meet this problem before is it ?
Have you figure it out, is there any suggestion to solve it?

Thanks a lot.

[Anonymized_JL1]

Hello Everyone,

I am working on my Thesis which is basically 2D CFD simulation of Vertical Axis Wind Turbine and comparing my results with "Wind tunnel and numerical study of a small vertical axis wind turbine" by Robert Howell et al. I need to calculate the torque generated by a wind turbine in order to find Cp. In this regard I am running 2D simulation with sliding mesh technique and saving the case/data file after every 10 degrees of rotation hence I have 36 files for one complete revolution. Now I am reporting the value of forces in X and Y direction (Fx and Fy) from each case/data file for all 3 Blades. Then I calculate Torque on each blade using formula
T1 = - Fx1.RcosΘ - Fy1.R.sinΘ
T2 = -Fx2.Rcos(Θ+120) - Fy2.R.sin(Θ+120)
T3 = -Fx3.Rcos(Θ+240) - Fy3.R.sin(Θ+240)
Total Torque T = T1 + T2 + T3 (Total Torque “T” is calculated for every 10 degree of rotations)

Average Torque = Σ T/n (0-360 degrees) where n = 360/10 = 36
Please let me know if the method I am using is correct. I am confused about the sign convention of Torque equations. is there any other way to find out Torque and Cp(Coefficient of performance)?

[/IMG].

[bahruddin]

Originally Posted by nana

Dear all:

Is there any one doing helical twist blade profile for VAWT. How should i make that turbine blade profile? Anyone can give me some idea? I need to do the numerical simualtion on that trubine and study the turbine performance. I really appreciate that anyone can provide some information on that.


Thanks

hai nana,i'm also study helical twist blade profile,i think u need to measure the blade first, in my case, measure the angle twist first, by dividing the blade several sections to help find the points in Gambit, by measuring the height blade twist angle and then measuring the angle helical blade,my blade has same chord so i just need point in several section for help me make turbine blade profile,

hopefully it can help you,sorry for my english

[jakoo123]

Hello,
I am working on a 2D ANSYS simulation for a 3 bladed VAWT. After the solution converges the moment values are totaly wrong and the contours show that the stationary zone is not inter-acting with the moving zone.I would like to ask any one to explain for me what is the problem and provid me with a solution.

Thank you and best regards

[sheikh nasir]

hello
i had the problem in sliding mesh in case of train traveling in tunnel . can any one help me plz. my email is sheikhnasir39@gmail .com
thanks
with regards

[dalecooper]

Hello, I'm a new user of CFX currently working in simulating VAWT in 2D for my master thesis. I have been searching and actually I'm a bit confused trying to put in clear some points.

I've constructed the geometry of the blades in 2D with Ansys Design Modeller and I don't know which is the procedure to simulate a sliding mesh in CFX. I've begun with ICEM CFD, but don't know if that is the best option. One of my doubts consist if this has something to do with the "Rotating Frame of Reference" option in CFX-Pre.

Thanks in advance for any kind of help.

Best regards.

[jwa]

If you're still working on this you may want to have a look at http://www.pdslimited.com/index_file...rbine_VAWT.htm which is a 3D analysis

[p.bhushan2727@gmail.com]

dear frnds plz tell me how to calculate torque in fluent i am working on vertical axis wind turbine H shaped darruis type so for that concern i am doing 2d simulations unsteday for that i am giving cl ,cd cm moniters on blades so will plz tell me how to find out direct torque in fluent or how to co-relate it 2 moment i am attching paper and some images of my mesh so it will clear u problem
plz tell me it needs udf to find torque on blades

[CFD_LES]

Hello
I work on a 4-bladed VAWT (Savonius). My analysis is Steady and 3D. The wind velocity is 10 m/s. this Rotor has 4 blades that each one has a semi-circle section. And the radius of the rotor is 10m (It's very large)
The obtained moment from analysis is negative and low. I don't have any experimental data.
Why the moment is low and negative, while the rotor is very big and wind velocity is 10?????
I'm very anxious, Please help me,
Thanks so much
all the best wishes