CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Fluent :- turbulence Model (http://www.cfd-online.com/Forums/main/102103-fluent-turbulence-model.html)

prince_pahariaa May 22, 2012 08:15

Fluent :- turbulence Model
 
Friends,

I have read many threads in this forum regarding turbulence models. Still i am not very clear with it. I would like to put some thoughts of mine which is making me confused. I will really appreciate any help here..

1) Can we apply standard k-epsilon or RNG or Relizable turbulence model when Y+ = 1 in Fluent ?? I guess we can not apply any variance of k-epsilon model when mesh is too fine near the wall. But still would appreciate any comment on this..

2) Variance of K-omega model, as per ANSYS theory guide, uses wall function when coarse grid is used and switch to low Reynolds number model when mesh is very fine near the wall (Y+=1). Which wall function it used ?? In the GUI interface of FLUENT, i can not observe any wall function like i did while using K-epsilon model. As values of Y+ is available to fluent after only few iteration. How does the FLUENT decide whether to use wall function or low Reynolds number model for initial iterations ??

3) To tackle heat transfer problem, where temperature gradient near the wall is important which model will you suggest. With my logic K-epsilon should ruled out automatically as it does not handle near wall region well.

4) Also, in my opinion low Reynolds number model is the best bet we have for heat transfer problem. But requirement of very fine grid is very much problematic. And i am not able to generate such fine mesh for my complicated geometry involving many solid objects in path of flow and holes in those solid objects for the passage of fluid.

Far May 23, 2012 03:30

Quote:

1) Can we apply standard k-epsilon or RNG or Relizable turbulence model when Y+ = 1 in Fluent ?? I guess we can not apply any variance of k-epsilon model when mesh is too fine near the wall. But still would appreciate any comment on this..
Yes you can. Turn on the low-Reynolds number treatment in TUI. But you should keep in mind that the LRN K-epsilon requires Y+ ~ 0.2 and on the other hand LRN K-omega requires Y+~ 2

Quote:

2) How does the FLUENT decide whether to use standard wall function (SWF) or low Reynolds number (LRN) model for initial iterations ??
It is decided based on y+. These are the values I get from "Dr. Florian Menter"
Y+ <= 6 near wall treatment. LRN
Y+ > 6 and Y+ < 30 : mix of both through some function. details are given in help
Y+ > 30 : SWF


Quote:

3) To tackle heat transfer problem, where temperature gradient near the wall is important which model will you suggest. With my logic K-epsilon should ruled out automatically as it does not handle near wall region well.
I tend to prefer V2f model, this is LRN model and can be turned on through TUI. 2nd option would be the SST model. For heat transfer Y+<0.1 is recommend. Please note that reducing Y+ further (less than 0.1) may introduce round off errors so be careful.

4)
Quote:

Also, in my opinion low Reynolds number model is the best bet we have for heat transfer problem. But requirement of very fine grid is very much problematic. And i am not able to generate such fine mesh for my complicated geometry involving many solid objects in path of flow and holes in those solid objects for the passage of fluid.
Alas! :eek: You have to live with it ;). CFD is not meant to be easy!!!

prince_pahariaa May 23, 2012 07:23

Thanks Far

You did help a lot.. Although it did not fix my current problem but it will help in long run..

I will try and see what can i do with what i have.. I may post more related to these turbulence model.. Please reply if u can..

Regards..

Far May 23, 2012 09:05

which mesher you are using? you may go for the local refinement/mesh adaptation in fluent for the critical areas

prince_pahariaa May 24, 2012 01:09

I am using GAMBIT for meshing and solving it in FLUENT.

I am trying to adapt the grid where Y+ is large in Fluent but till now with not much success. As geometry is so complex, I have very little control over meshing. I am using unstructured T/Grid mesh in Gambit and doing Volume mesh directly. I have divided my volumes in many small parts and i can mesh them properly, But there is one big volume which contain all other volumes (other volumes are wall and solid objects with holes) is creating problem. This big cylindrical volume i made by using split operation and i do not have any control on meshing this particular volume. I have posted the detail of my geometry in this link http://www.cfd-online.com/Forums/ans...h-quality.html and there also i get help from you. But with renew problem of Y+, i am stuck again.

If u can provide any suggestion on how to mesh that big volume, it will help a lot. In mean time, i will keep trying.

Thanks for all the help..

Far May 24, 2012 01:22

In tgrid there are very good options for the boundary layer meshing. You can ask ANSYS support for help.


All times are GMT -4. The time now is 11:23.