CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Fluent :- turbulence Model

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   May 22, 2012, 08:15
Default Fluent :- turbulence Model
  #1
Member
 
prince
Join Date: Jun 2011
Posts: 56
Rep Power: 6
prince_pahariaa is on a distinguished road
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.
prince_pahariaa is offline   Reply With Quote

Old   May 23, 2012, 03:30
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
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! You have to live with it . CFD is not meant to be easy!!!
mohammad hossein likes this.
Far is offline   Reply With Quote

Old   May 23, 2012, 07:23
Default
  #3
Member
 
prince
Join Date: Jun 2011
Posts: 56
Rep Power: 6
prince_pahariaa is on a distinguished road
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..
prince_pahariaa is offline   Reply With Quote

Old   May 23, 2012, 09:05
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
which mesher you are using? you may go for the local refinement/mesh adaptation in fluent for the critical areas
Far is offline   Reply With Quote

Old   May 24, 2012, 01:09
Default
  #5
Member
 
prince
Join Date: Jun 2011
Posts: 56
Rep Power: 6
prince_pahariaa is on a distinguished road
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 Mesh quality 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..
prince_pahariaa is offline   Reply With Quote

Old   May 24, 2012, 01:22
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
In tgrid there are very good options for the boundary layer meshing. You can ask ANSYS support for help.
Far is offline   Reply With Quote

Old   November 25, 2014, 13:22
Default
  #7
New Member
 
azna
Join Date: Nov 2012
Posts: 19
Rep Power: 4
azna is on a distinguished road
Hi,

I was wondering that are the equations for k- epsilon turbulence model different for simulation using Eulerian dispersed multiphase model or VOf multiphase model?

Thanks
azna is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
gamma-ReTheta turbulence model for predicting transitional flows FelixL OpenFOAM Programming & Development 77 June 20, 2015 10:20
How to create a 3Ds Car Model importing to FLUENT? spysunny Main CFD Forum 1 January 11, 2012 00:40
Fluent 12 k-w SST turbulence model DarrenC FLUENT 0 December 13, 2009 09:33
two turbulence model in fluent duaiduaihu FLUENT 1 August 26, 2009 19:39
FLuent CAvitation Model requires Turbulence? CFDtoy FLUENT 2 January 12, 2007 11:27


All times are GMT -4. The time now is 02:37.