[mohammad]

Hi guys,
I'm simulating the NREL wind turbine with CFX.
my model contains about 4 million nodes.
I decided to check the node sensitivity analysis to see the effects of node density near the blade....
As I increased the number of nodes inside the boundary layer( say roughly from 14 to 19 nodes) and also as an other time I increased the number of nodes in chordwise direction ( form 37 to 50), the results deviated from the first set of the results and they went far away ( say about 40%) from Experimental result....

*Experiment ( v=4.5): Thrust force=552.91
*model 1 ( 37 chordwise , 14 node inside boundary layer) :Thrust force=754
*model 2 ( 37 chordwise , 19 node inside boundary layer) :Thrust force=874
*model 3 ( 50 chordwise , 19 node inside boundary layer) :Thrust force=917

I tried to keep the quality of mesh constant during the changes and I'm wondering why the results are diverging like this???

can everybody help me please?

[ghorrocks]

Looks like you are miles away from an appropriate mesh density. I suspect you will have to be far finer than these models.

[juliom]

I do agree with ghorrocks, the mesh quality is very poor, since you have different results qith each one!!!

[ghorrocks]

Mesh quality does not necessarily mean different results. It can, but a good quality mesh with an inadequate resolution will also do this. It could be either (or both) quality or resolution.

[mohammad]

Hi
Now I have 2 other questions...
I'm trying to increase the no. of nodes near my blade...two times more, and it will make my model HUGE for my PC to run it...then I MUST reduce no. nodes somewhere else.
Question1: Do you think the mesh density away form the balde( say one span length away) is of the same importance as the near-blade node density....I don't think so...then to lower No. nodes, do you think I can reduce the mesh density one blade span length away from the blade. What can be the largest ,but safe, distance between two successive nodes in axial direction?

Question2: Which part is less influential for my case to change the mesh density within that par...[far away in upstream or Downstream]?

Regards

[mohammad]

Originally Posted by ghorrocks

Mesh quality does not necessarily mean different results. It can, but a good quality mesh with an inadequate resolution will also do this. It could be either (or both) quality or resolution.

Hi ghorrocks;
to give some more information, the quality of my model is 0.41 and the smallest angle is 24 deg.
I think the matter of my model should be resolution....I will try some more runs and i will write the results for more clarity ASAP.

Regards

[cfd_newbie]

Originally Posted by mohammad

Hi
Now I have 2 other questions...
I'm trying to increase the no. of nodes near my blade...two times more, and it will make my model HUGE for my PC to run it...then I MUST reduce no. nodes somewhere else.
Question1: Do you think the mesh density away form the balde( say one span length away) is of the same importance as the near-blade node density....I don't think so...then to lower No. nodes, do you think I can reduce the mesh density one blade span length away from the blade. What can be the largest ,but safe, distance between two successive nodes in axial direction?

Question2: Which part is less influential for my case to change the mesh density within that par...[far away in upstream or Downstream]?

Regards

ASAK Mohammad,
The cold heart truth about the NREL's Phase VI validation is that till now nobody has been able to solve this problem accurately and consistently using RANS. I have been advised by some very senior paper in this field (and also pointed out in many papers) is that LES or DES is the way forward. Other researchers have tried much better grids than what you are using and are still unable to to get good results. Regions both near and in the wake region are important.
My suggestion is that you should have a very good mesh and fine mesh (so that there is no doubt about the mesh quality) and see how good RANS results are and then you should move to DES or LES.
If the computational resources are a constraint than you should have better access to computational resources for this problem.
Raashid

[ghorrocks]

Nice answer Raashid. I am sorry Mohammad, but if your computer is unable to take larger meshes then it is quite likely you will never get a good answer to your simulation. That is why people make super computers to run CFD simulations - because you have to if you want accurate answers in many classes of simulation.

[mohammad]

Thank you,both of you, for your good guidelines

[mohammad]

Hi Raashid, Glenn.

Just to add more information to this thread for more clarity, here I present the values of Yplus on my blades which I got( Up-blade and Down-blade in 4 pictures ).
As its obvious except at the "tip section" of both blades, the value of "Yplus " for nodes on the surface are good enough( PLEASE INFORM ME IF I'M EXAGGERATING). But still thsose changes of results happens when i change no of mesh in far-blade zone( see the opening of this thread).

The only matter remains unsolved is a proper choice turbulent model and MOST PROBABLY Raashid's suggestion about LES or DES is true...

I will run my model in transient mode with LES or DES and I will add more info to this thread.

Anybody, please correct me and give me more of your knowledge and experiences.

Regards

[ghorrocks]

To establish if your mesh is fine enough you really should do a sensitivity analysis.