- **FLUENT**
(*https://www.cfd-online.com/Forums/fluent/*)

- - **wall y plus problem**
(*https://www.cfd-online.com/Forums/fluent/75423-wall-y-plus-problem.html*)

wall y plus problemHi, I am doing turbulence modeling of a somewhat complicated tank, and have trouble with the wall y plus value. The wall y plus value ranges from 0 to 200. I tried using yplus/ystar adaption, it says:
0 cells marked for refinement, 47979 cells marked for coarsening Additional cells might have been marked because of the requirements of the adaption algorithms. Dump usage: 1022279 cells, 2203742 faces, 295683 nodes Dump usage: 1022279 cells, 2203742 faces, 295683 nodes Dump usage: 1022279 cells, 2203742 faces, 295683 nodes Grid size ( original / adapted / change) cells ( 1022279 / 1022279 / 0) faces ( 2203742 / 2203742 / 0) nodes ( 295683 / 295683 / 0) How come it calculated 47979 cells to coarsen but at the end nothing change? Can anyone give me some advice? Thanks. Regards, Eric |

Hi
Fluent cant coarsen any mesh beyond the original one I mean that it can only coarsen a mesh that u have alerady refined under Fluent I know it is a very big problem...... If u need advices, write to me |

Hi Karine,
Thank you very much, I really do need advice. I am trying to model a cylindrical tank with a baffle in the middle. I am using the standard k-epsilon model with standard wall functions. However the wall y+ values at the walls ranges from 0 to over 100. I tried adapt->y+/ystar to coarsen the cell so the y+ value is between 30-300, but Fluent didn't coarsen the near wall mesh for me, so I tried adapting to refine the mesh so the y+ value is less than 5 and use the enhanced wall treatment, but then after running the simulation for a while, the y+ values go all over the place again. Thanks for your help. Regards, Eric |

Hi
as i told u, Fluent cannot coarsen the mesh. It can only coarsen a mesh that u have refined, i mean he will give you back ure initial mesh. 1- Are u using an unsteady solver?? 2- Fluent refine the mesh in 2 different ways. u can read about it in Fluent manuel. Roughly speaking , Fluent will divide ure cell (that was marqued for refinement) in 8 cells. So it is not sure that u will get the good size from the first refinmenet. If u do a lot of refinements, u will get a lot of cells...a lot more than u need because u are dividing every cell in 8 parts and not in 2 parts (as u desire). The solution is to do a good mesh in Gambit. U cant know the cell size a priori. I mean u must run a simulation, than see if ure y+ is good or not. If not, u must do another mesh. 3- If ure y+ is so hetregonous, use the k-w turbulence model with enhanced wall functions. It can deal with all y+ ranges (of course, avoid very large y+) 4-If u want absolutely to use standard wall functions , then u must use Gambit. Put coarse mesh where ure y+ is small. The problem is that u must try several times to have a good mesh, where y+ is alway>30. This is a very big limitation in Fluent.....(sometimes u need non conformal grid to do the job) Good luck and write to me again if u still need help ( i hope u are understanding my english) |

Hi Karine,
Thank you very much for your reply again! 1- Yes I am using unsteady solver. 2- I actually don't have Gambit, and I am using Ansys to mesh. It does the meshing automatically and is very hard to manually control the sizing of the mesh, so I have to rely on Fluent to help me refine the mesh near the wall, but as you pointed out, using Fluent to refine causes the mesh to have a lot more cells than I needed and it's using up too much computer resource. If the condition 30<y+<300 is not satisfied, it will only affect the accuracy near the wall right? The flow far away from the walls should still be correct? 4- So if I couldn't get the y+ value within the desireable range, the k-w turbulence model with enhanced wall function is more accurate than the k-e model? Thank you very very much for your help. This is my first time modeling turbulence flow. I really appreciate your advice. Regards, Eric |

Hi
1-as ure flow is unsteady, ure y+ will be varying according to time. U must be sure to keep it in the good range for all time. 2-I never used ANSYS to mesh. it is the new mesh generator for FLuent 12??? friends told me it is very bad (even worse than gambit). I cant help u on this point 3-No. If it was the case, nobody will care about his y+ :) it will affect the accurcy of the whole simulation. 4- k-w and k-epsilon are turbulence models. No one is better than the other. U must compare with experiments to know wich one is better (it will depend on the cases) But k-w with the wall enhanced functions can deal easier with y+ beyond the desired range. See Fluent manual to see the difference between enhanced wall function and enhanced wall treatement. Dont hesitate to write to me if u still facing problems with ure simulation Regards |

Hi Karine,
In my model, there are regions where the main flow is happening and the wall y+ values at those regions satisfy 30<y+<300, but then there are regions the flow is not really moving much, and the y+ value is less than 30 there. Is it fine as long as the y+ value near the region where I am really interest satisfies the condition 30<y+<300, while regions that aren't really relevant, the fluid is not moving much, has y+ value below 30? Thank you very much for your help and advice. Regards, Eric |

Hi
if ure y+ is not good in some places, it may influence the whole solution. We cant know this in details as the N.S equations are non linear, but it is better that ure y+ be fine everywhere. u have 3 possible solutions: 1-use a coarser mesh where the fluid is moving slowly. So ure y+ are in the good range everywhere (30<y+<300). 2-use the k-w model. this model can tolerate more differences in Y+ (anyway, avoid y+ netween 5 and 30, as it will corresponds to the buffer region). 3-Use the k-epsilon with enhanced wall treatement. Ure y+ must be less than 1 (or 5) everywhere. U must generate a fine mesh all over the walls. This solution will consume a lot of calculation time.....(and it is not sure that it will give the best results) Good luck |

Hi Karine,
Thank you so much for your time, help and advice!!! I will try using the kw model first to see if I have similar results. Regards, Eric |

Hi Eric
no problem, u can write to me when u want. Remember that finally, u need to compare with experiments. Perhaps k-w will give u good y+ but a bad result (because the turbulence modeling itself) It is the problem of RANS models: u cant know a priori id ure results will be in a good range of accuracy |

Hi Karine,
I have one more question, does the y+ value need to be between 30 to 300 at the wall where there is separation? The standard wall function is not valid there anyways right? Regards, Eric |

Hi Eric
i have a friend that knows very well how to deal with separated flow. if u have skype or msn, i can give u his adress so u talk with him (i can send it to u in a private message). |

Hi Karine,
Sure thank you very much. How do I send a private message? Regards, Eric |

Hi Eric
i have sent to u his email adress Good luck |

1 Attachment(s)
Hi,
I have a similar problem. I'm simulating, with fluent, the natural ventilation in a building, so I've realized a mesh of a cubic building with a window, which is surrounded by a parallelepiped representing the external air. I've had to refine the mesh in some zones, as those close to the building walls and to the parallelepiped basis. The mesh is that of the attached image. I've a doubt about the near-wall treatment. First I've set k-epsilon RNG with standard wall function. Setting the Yplus of the building walls and the basis of the parallelepiped (which is considered as a rough wall) I've obtained Y+ include between about zero and a 700. Now, I don't know how to proceed, becouse I should coarsen the mesh in those zones where Y+ are less than 30 and refine the mesh whare Y+ are more than 300. Is it right? I know that Fluent can just refine the mesh and not coarsen it. So, what can I do? Thanks a lot. Bests |

All times are GMT -4. The time now is 06:40. |