CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Problem in conducting CFD of analysis of wind turbine blade (https://www.cfd-online.com/Forums/cfx/121544-problem-conducting-cfd-analysis-wind-turbine-blade.html)

 atulpat July 31, 2013 05:10

Problem in conducting CFD of analysis of wind turbine blade

3 Attachment(s)
Hello CFX users,
I am working on wind turbine blade analysis with CFX software v11. It is a NACA S809 airfoil with 2 blades. Blade length is 5.32 m. Blade geometry is modeled in solidworks software with proper twist angles as given in research papers. IN CFD analysis, I am getting torque value ≈ 10000 Nm. But in most of the research papers, for the same boundary conditions and blade geometry, the value of torque ≈ 1000 Nm. Here rotating axis of blade is Z-axis. So I am calculating torque about Z-axis. So where I am going wrong?
The boundary conditions are as follows:
For stationary domain:
Fluid domain= Air Ideal Gas
Turbulence model= SST
Air Inlet= 10 m/s velocity
Air Outlet= 0 Pa relative pressure
For rotating domain:
Rotating axis= Global Z
Blade and Hub wall = No slip conditions
Rotating interfaces= frozen rotor model
In CFX results, area average Y+ value for blade wall= 130
Stationary domain size:
Inlet portion length= 3 times of blade length
Outlet portion length= 5 times of blade length
Also mesh quality for rotating domain: Hexa elements (ICEM CFD software)
Angle= 18.27°
Quality= 0.212
Determinant 2x2x2= 0.2012
Eriksson Skewness= 0.308
mesh elements= 3.34 million elements

Here I am using very fine hexa mesh for both stationary and rotating domain . I have changed the angle of attack such as 0 and 12 degree still torque value is 10000 Nm and it is changing only when blade RPM is changing. Also analysis has carried for 1 blade with 180 degree domain (symmetric model) as well as 2 blades domain still results are same. I tried many possibilities such as change in turbulence model, mesh size, turbulence intensity, physical timescale. Here I have attached some images of mesh and CFX pre file. So plz give me the suggestions.

 ghorrocks July 31, 2013 06:08

Your mesh does not look that fine to me.

Have you read the FAQ on accuracy? http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

 atulpat August 1, 2013 06:43

Here mesh size for rotating domain (half domain) is 3432111 elements. My desktop size (47 cm x 27 cm) is bigger due to that it might be looking coarse but it is actually fine mesh. Previously I was tried with 4.2 millions elements but there was no any change in results. If I am going for too fine mesh then it will take too much time to solve the problem.

 ghorrocks August 1, 2013 17:55

I was looking at the mesh on your blades. That looks coarse to me. The absolute number of nodes is a different thing.

 atulpat August 6, 2013 07:39

Now, I have generated very fine mesh with more than one crore elements for rotating domain and beyond that I am not able to refine it due to system constraints. But I think so it will take to much time to solve the model. Previously I was generated fine mesh near to the wall of the blade. Here my another question is that whether coarse mesh will give ten times higher results though we are getting y-plus value near to 127?

 ghorrocks August 6, 2013 19:15

Unfortunately what you have done is not very helpful. So you will get an answer from this mesh - but is it accurate? Did you refine enough? Or not enough? You cannot know.

A better approach is to generate a series of meshes with different densities. Make sure the density difference between each mesh is enough to be worth it - x1.5 on edge lengths is a guide. Then you can look at how the simulations are converging to a value as the mesh is refined. Now you can make an informed decision as to whether your computing power is sufficient to get an answer to the accuracy you require, and how fine a mesh you need for results of the accuracy you want. This is a sensitivity study.

 atulpat August 7, 2013 00:06

1 Attachment(s)
Here I am sure that mesh is accurate and convergence wise there is no any problem. In every case, residual target of 10-6 is achieved. Now for new refined blade, Mesh quality, Eriksson skewness and determinant are more than 0.3 and angle is 18.5. I have attached some images of blade and beyond this I am unable to refine the mesh. Also, I have Intel Xeon workstation with 14 GB of Ram as well as I can simulate the model on another server which has 52 GB of Ram. Yesterday I discussed with my seniors and as per their experience, they informed me that coarse or fine mesh will not give 10 times difference in results. So I am confused that what could be the problem that means whether model is drawn as per research papers or not? Or it may be due to another reason.

 ghorrocks August 7, 2013 00:13

You have not understood my previous post. I was not referring to residual convergence. I was talking about convergence against grid refinement. Please reread the post with the knowledge that it is referring to convergence against mesh size, not residuals.

But your point is valid, it is unlikely a x10 error comes from mesh density. There is probably something more fundamental which is wrong.

How are you calculating your torque values? Using what functions? In the solver or in the CFD-Post or something else?

 atulpat August 7, 2013 02:53

Ok. Though I am changing the mesh size, results are still same for torque and it is changing only when blade RPMs are changing. Here rotating axis is Z. So I am calculating torque about Global Z axis in CFX post.

 ghorrocks August 7, 2013 07:34

What do you get when you calculate the torque as a monitor point in the solver?

 atulpat August 7, 2013 08:16

Actually I dint remember the error. but when I am calculating the torque as monitor point, solver gives the error. I have to always remove it from monitor point then only solver works.

 Armandul August 15, 2013 08:06

Hey, i am not shure, which solver you use, but the thing with the monitor point is quite clear for me. torque is calculatet with surface integral of pressure difference. So the value is for surface, not for a point...

 atulpat August 16, 2013 01:46

Here I am using CFX software to solve the problem. As you have mentioned that we have calculate torque by surface integral of pressure difference but how we can calculate torque by this method? Can you provide details or expressions for the same? Here roting axis of the blade is Z. Also I got some expressions for calculation of torque as follows:
Area X = Area * Normal X
Area Y = Area * Normal Y
ty local = Pressure * Area X * Y
tx local = Pressure * Area Y * X

Using above expression still I am getting 10 times higher torque which is not possible. So are these correct expressions for calculating the torque?

Regards
Atul

 ghorrocks August 16, 2013 01:54

Have you tried using the built in torque functions torque_x/y/z()@ ? Should be no need to write you own expressions, especially when they do not include the viscous contribution to torque.

 atulpat August 16, 2013 07:09

Yes, previously I was calculating the torque by built in functions i.e. function calculator in CFX post. Like, torque about Z axis at blade wall. Hence I tried to used expression as mentioned in previous post but unfortunately it is also giving different results.

 ghorrocks August 16, 2013 07:27

I would try calculating this as a monitor point in the solver again. You said it caused an error, but if properly implemented it should work fine. There is no inherent problem with using this function in the solver to my knowledge.

I have seen it reported by a few people that CFD-Post gives incorrect forces and torques and that the monitor point during a solver run is correct. So I would definitely give it a try.

 atulpat August 17, 2013 04:09

Ok, then I will again try to use this monitor point and after getting result I will come back.

 All times are GMT -4. The time now is 10:01.