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

Initial solution for Turbulence models

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 29, 2005, 04:39
Default Initial solution for Turbulence models
  #1
Madhukar Rapaka
Guest
 
Posts: n/a
Hi

to start a simulation one should initialize the solution first. For turbulence models in FLUENT like RS model, it is necessary to have a good initial guess(initial solution). how to get a god initial guess. Is there any standard method.

Thanks in advance
  Reply With Quote

Old   November 29, 2005, 07:20
Default Re: Initial solution for Turbulence models
  #2
John
Guest
 
Posts: n/a
Madhukar, You can use the "Initialize" feature in the "Solve" Menu to intialize the solution. This then allows use to use the "Iterate" panel. If you would like to initiate a solution that may have convergence issues, I believe it can be useful to set the viscosity model to "inviscid," then initialize it, then iterate it for a while (or until convergence), then reset the viscosity model to your desired setting, and continue with more iterations (without re-initializing). The inviscid solution will therefore be a useful starting point for a more complex viscous modeling effort. - John

  Reply With Quote

Old   November 29, 2005, 08:19
Default Re: Initial solution for Turbulence models
  #3
D.Pavitran
Guest
 
Posts: n/a
Hi,

You can also run your case with K-epsilon model for some iterations for good intial guess,and then u can change the viscous model to RSM.

regards/

Pavitran D
  Reply With Quote

Old   November 29, 2005, 10:12
Default Re: Initial solution for Turbulence models
  #4
RoM
Guest
 
Posts: n/a
Starting with ke wont help you with RSM because ke does not provide an inital solution for the reynolds stress terms. Although the manual states it is good to start a RSM calculation with ke i have some doubts about this. I talked with a fluent engineer and his opinion was to go all the way RSM if you have to use it and forget about the ke start. I dont use RSM so i cant comment on it very deeply but it would be good if someone with some more experience could give some advice if its good (or not) to start RSM with ke.

RoM
  Reply With Quote

Old   November 29, 2005, 14:56
Default Re: Initial solution for Turbulence models
  #5
Anindya
Guest
 
Posts: n/a
For external aerodynamics fluent advises not to use other rans models to initialize the flow (I believe RoM already stated this in the previous email.

Start with the rsm model directly. Use first order schemes for some time and then shift to second order ones.

There is a short manual on external aerodynamics provided by fluent on their user service website. You can look at that to see the steps to be followed to use rsm.

Anindya

  Reply With Quote

Old   November 30, 2005, 02:43
Default Re: Initial solution for Turbulence models
  #6
D.pavitran
Guest
 
Posts: n/a
Hi rom,

I am not sure about this, but think over it and if i am wrong please reply me back

In Fluent the production terms in normal stress tranport equations of RSM are modelled with boussinesq assumption. So, dont u think we have a good approximation of turbulent viscosity (since turbulent viscosity = cmu*k*k/epsilon in RSM) and also the corresponding velocity gradients (ex:du/dy, dv/dy of P11 for uu transport equation and P12 for uv transport equation).

regards/

Pavitran D
  Reply With Quote

Old   November 30, 2005, 05:11
Default Re: Initial solution for Turbulence models
  #7
Vagelis
Guest
 
Posts: n/a
Hi All!

There are two ways to impose an initial solution for this problem.

1)From initialization panel, where sb imposes constant values for entire flow field.

2)Step by step solution process. At the beginning sb can start from a solution which approximates the final solution and then use the 'approximate solution' as initial guess for the final.

Using the RSM,I think it's better to have an 'approximate solution' which is closer to the final (start with inviscid flow, k-e model) than impose constant values for entire flow field (to start directly with RSM) which is farther away from reality even from the previous 'approximate solution'. My experience is that: I simulated an external (low Reynolds,turbulent)flow around a 2D circular cylinder using RSM .To get solution I was compelled to use as initial guess an 'approximate solution' otherwise my problem didn't converge! I used as initial solution the k-e model and the final results were excellent.

  Reply With Quote

Old   December 5, 2005, 00:12
Default Re: Initial solution for Turbulence models
  #8
Murthy
Guest
 
Posts: n/a
Hi Madhu,

Actually in InHouse coding Practise it's recommended to approximate Reynolds Stresses to nuti and strain-rate. where nuti is obtained from Mixing Length Hypothis. Once you start getting Approximate solution feild for mean flow, Reynolds stresses are calculated by solving all RS transport equations. In FLuent, I don't know how exactly it works.

My Experiance with RSM in Fluent is You first start your simulations with K-Epsilon model where you can specify Turbulent Intensity and Hydrolic diamter. These two parameters are used to get initial guess. But in reality your initial guess should always be close to your final solution for that you must have some priori knowledge on your system you r studying.

Murthy

  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
Darcy-Forchheimer law for specifying Porous Zones Ger_US OpenFOAM 17 August 30, 2013 09:30
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 05:15
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
TurbFoam problemlarge Co number sunnysun OpenFOAM Running, Solving & CFD 6 March 10, 2009 09:05
On the damBreak4phaseFine cases paean OpenFOAM Running, Solving & CFD 0 November 14, 2008 21:14


All times are GMT -4. The time now is 11:26.