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

Turbulence model in a simulation with wide spatial range of Reynolds numbers

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2011, 06:37
Default
  #21
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
mesh resolution near wall for laminar flow can be decided based on grid convergence studies.
Correct.

Quote:
Can porous media be a major contributor to non-convergence?
Yes, definitely. In fact I know there is an update in V13 to improve the convergence of porous regions. This may fix your entire problem if you are not using the current version.
ghorrocks is offline   Reply With Quote

Old   September 25, 2011, 18:35
Default
  #22
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
1c) I first of all determine whether a turbulence model is appropriate. In your case it is not. But if it is a turbulent flow then my default option is SST and I would only choose anything else if I had a specific reason to do so - eg anisotropic, bluff body etc. And yes, meshing is very important. The mesh is tailored to the boundary layer I expect to generate.
Quote:
Originally Posted by ghorrocks View Post
No it does not. If you use the k-e model in a laminar flow it will give you more dissipation then is really there, so is a significant source of error. The SST and related models are better here because they degenerate to (almost) laminar flow at low turbulence energies.

@ghorrocks

for the lowest inlet Re of 600, laminar transient model seems to be converging. I am now checking if my main variables of concern (pressure drop and maximum temperature in solid) have stabilised with respect to iteration count i.e. time. Then I can stop the simulation take the result as my evolved steady state solution. I am also trying to see if I can spot any oscillations in velocity pressure etc. by observing them at specific monitor points.

I am also doing the same transient run at higher Re of 1000. Here I am trying with both Laminar and SST model. As you said above , SST model is better than k-epsilon in low Re flow. However, today I came across a publication where the authors argue that even SST model should not be used for low Re and transitional flow. (http://ntrs.nasa.gov/archive/nasa/ca...2008023429.pdf)
In case I find that in my transient simulations, for higher inlet flow Re like 1000-4000, either the laminar model does not work or there is significant difference in results of the laminar and SST models, then do you recommend that I should try using SST model with the transitional model enabled in CFX? I spotted another thread where a model called the gamma-theta transition model has been recommended.( Low Reynolds k-epsilon model )
I personally am sceptical about how good this transitional flow modeling is .
Chander is offline   Reply With Quote

Old   September 25, 2011, 18:38
Default
  #23
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Correct.



Yes, definitely. In fact I know there is an update in V13 to improve the convergence of porous regions. This may fix your entire problem if you are not using the current version.
Oh Ok. Thanks for this important info!
Unfortunately, ver 13 is not available yet at the central cluster where I run my simulations. I'll have to make do with ver12.1 for the moment.
Chander is offline   Reply With Quote

Old   September 25, 2011, 19:29
Default
  #24
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The gamma-theta transitional model was developed for transition on airfoils. Your thing looks nothing like an airfoil so I do not think it will work very well for you.

I agree that the SST model should be avoided for transitional flows without the transition model. It is better to use a laminar model in a slightly turbulent flow - it means you are doing a pseudo-LES simulation but at very low Re the turbulence structures are large so this is OK; rather than use a turbulence model in a laminar flow.

Sounds like you need to lobby your cluster support people. If V13 simply fixes your problem then just imagine how much time you have wasted. And if your support is current you are entitled to this software so the only reason you don't have it is because IT have not installed it..... Multiply your hourly rate by the time wasted and you have a strong case to get it fixed ASAP. If you are a student, well the equation is a bit more tricky
ghorrocks is offline   Reply With Quote

Old   September 25, 2011, 19:48
Default
  #25
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
It is better to use a laminar model in a slightly turbulent flow - it means you are doing a pseudo-LES simulation but at very low Re the turbulence structures are large so this is OK; rather than use a turbulence model in a laminar flow.

If you are a student, well the equation is a bit more tricky
Glen,
I did not get your comment regarding pseudo-LES simulation. Can you elucidate a bit on that?
Yes I am a PhD student
Actually our cluster people had tried to upgrade to ver 13 sometime back but they found some issues with parallalization with ver13. so they decided to stick to ver 12.1
ver 13 would have helped a lot as you said it has non-thermal equilibrium model for porous media also

One thing regarding porous media. I can simulate the pressure loss by modeling porous media simply as fluid domain also by only using the source term for momentum loss. I know this is not accurate as the effect of porosity is not accounted for in other terms of the Navier-Stokes equation. Have you tried with this approach? How good/bad it is in terms of accuracy and convergence?As far as the thermal part is concerned, if I stick to thermal equilibrium assumption, the fluid domain approach should also work. I am not sure though in case of non-thermal equilibrium.
Chander is offline   Reply With Quote

Old   September 25, 2011, 20:26
Default
  #26
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
I did not get your comment regarding pseudo-LES simulation. Can you elucidate a bit on that?
If you are doing it right you will probably get some non-steady turbulent scale fluctuations starting up. This is effectively LES.

Quote:
Actually our cluster people had tried to upgrade to ver 13 sometime back but they found some issues with parallalization with ver13. so they decided to stick to ver 12.1
My preferred approach would be to fix the problem. You have paid for the software, so install it and use it. Not installing it is just making things hard for yourself for no reason.

Quote:
I can simulate the pressure loss by modeling porous media simply as fluid domain also by only using the source term for momentum loss.
Correct.

Quote:
I know this is not accurate as the effect of porosity is not accounted for in other terms of the Navier-Stokes equation.
The porous model in CFX (to my knowledge) just applies a source term. So it is no different to applying the source term yourself. I do not expect it to be any more accurate.
ghorrocks is offline   Reply With Quote

Old   September 25, 2011, 20:35
Default
  #27
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The porous model in CFX (to my knowledge) just applies a source term. So it is no different to applying the source term yourself. I do not expect it to be any more accurate.
Actually the CFX manual mentions that the difference between full porous media model and fluid model with momentum loss terms is that in the former porosity affects all the terms of Navier-stokes equation and not only the source term as in the latter approach. It also states the modified equations for the full porous model.
I was thinking what difference will using a fluid model with momentum source term make in my simulations in terms of convergence and accuracy.
Regarding ver13, I`ll continue to try and get it
Chander is offline   Reply With Quote

Old   September 25, 2011, 20:39
Default
  #28
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I was not aware of the difference in porosity models. You learn something evey day.

If I was you I would trial the momenum source approach anyway. Maybe set up a simple benchmark simulation and compare if they are any different for flows similar to what you are looking at. If there is not difference then use whatever is easiest to get working properly.
ghorrocks is offline   Reply With Quote

Old   September 25, 2011, 20:45
Default
  #29
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Yes, I should probably try that.
Thanks again for your quick and patient replies
Chander is offline   Reply With Quote

Old   September 27, 2011, 12:48
Default
  #30
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
@ghorrocks

Hi Glen,
I am attaching here a cross-section of my mesh along with yplus plotted in that cross-section. Can you have a look at this and advise any changes if required?

Meanwhile transient simulations are showing promise. Thanks again for guiding in that direction.
Attached Images
File Type: jpg Mesh.jpg (62.8 KB, 14 views)
Chander is offline   Reply With Quote

Old   September 28, 2011, 07:11
Default
  #31
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
As I said in the other post you do not need to make porous domains different domains. You can make them sub-domains of the entire fluid domain. It probably won't make any difference but it is worth a try.
ghorrocks is offline   Reply With Quote

Old   September 28, 2011, 08:04
Default
  #32
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Yes, I will try that.
I just wanted to check with you about the nature of mesh (uniform) and the y+ at the wall . Is this kind of mesh and this much resolution good enough/ overkill or nit sufficient if I have to use k-omega based models for flow Re in the range of 1000-4000.
Chander is offline   Reply With Quote

Old   September 28, 2011, 08:45
Default
  #33
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,094
Rep Power: 94
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You need to do a mesh refinement study to determine if your mesh is adequate. You cannot tell by simply looking at it.

Lots more detail is here:
http://www.cfd-online.com/Wiki/Ansys...publishable.3F
ghorrocks is offline   Reply With Quote

Old   September 28, 2011, 08:48
Default
  #34
Senior Member
 
Join Date: Oct 2010
Location: Zurich
Posts: 176
Rep Power: 7
Chander is on a distinguished road
Ok.

Certainly, I will do a mesh refinement study.
I am familiar with GCI method and have used it before. You might recall , I had discussed that with you a few months back here
Chander is offline   Reply With Quote

Reply

Tags
cfx, reynolds number, turbulence model

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
Turbulence model for low Reynolds number flow? Nokadu Main CFD Forum 3 May 26, 2013 11:42
Fan heater model: what turbulence source to use? andy20 CFX 7 March 3, 2008 17:42
Turbulence Models for very low Reynolds Numbers Sudhi CFX 1 March 2, 2007 19:03
turbulence model simulation in unsteady flow Chang Main CFD Forum 2 February 12, 2005 07:28
Large Eddy simulation Andreas Hauser Main CFD Forum 1 May 20, 2000 20:33


All times are GMT -4. The time now is 11:25.