# Spalart-Allmaras model

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

 July 27, 2006, 14:03 Spalart-Allmaras model #1 ganesh Guest   Posts: n/a Dear Friends, I am trying to incorporate S-A turbulence model into an existing NS solver. I am faced with the problem of code blowing up on very strectched meshes, typical of turbulent flows. In this context, I plan to go for wall functions, so as to obtain accurate solutions at expense of less stretched grid(or correspondingly a higher y+). Could anyone point out some references that explain S-A model with wall functions in detail ? Thanks in advance Regards, Ganesh

 July 30, 2006, 22:07 Re: Spalart-Allmaras model #2 Praveen. C Guest   Posts: n/a Are you getting negative turbulent viscosity ? Is that what is causing blow-up ?

 August 1, 2006, 05:11 Re: Spalart-Allmaras model #3 ganesh Guest   Posts: n/a Dear Praveen, Yes, I have problems with negative turbuelnt viscosity, which leads to code blow up. I have improved the convergence a bit using a limit on the lower bound of turbulent viscosity, but from the solution point of view doesnot seem to be helping much. Any comments/suggestions are most welcome Regards, Ganesh

 August 1, 2006, 06:57 Re: Spalart-Allmaras model #4 mar Guest   Posts: n/a I've implemented the S-A model too. here are some suggestions based on my experience. If the eddy viscosity is negative in the wake--> it is normal for S-A model. the problem can be overcame reducing the stretching Another way, which is not so clean, is to perform something like DES using for the parameter d (distance) a mix between the wall-distance and the cell dimension If the eddy viscosity is negative in the wall region --> you have a problem.. In this last case try to inizialize the eddy viscosity with a value different from zero but low. If the problem is still present it can be due to the fact that the flow is laminar in this place and this can be overcame using the tripping function of the turbulent model. Good luck

 August 2, 2006, 03:28 Re: Spalart-Allmaras model #5 Praveen. C Guest   Posts: n/a I have found that if you use an explicit scheme, then the destruction term causes the eddy viscosity to become negative. Try switching off the destruction term to see if this is the case with you. I treat the destruction term in a semi-implicit way: ν2 in the destruction term is replaced with ν(n) ν(n+1). Note that without the destruction term, SA model satisfies a maximum principle; so negative values should not arise if you have a proper descretization. Also, it is recommended to use only a first order upwind scheme for the SA model. Together with a Galerkin discretization of the elliptic terms, you should get a stable scheme.

 August 2, 2006, 13:35 Re: Spalart-Allmaras model #6 ganesh Guest   Posts: n/a Dear Mar and Praveen, I do make use of a first order upwind for SA model. The source terms are linearised, and the destruction terms are treated implcitly. I make use of a diamond path reconstruction procedure for the viscous fluxes. On finer grids, I still end up with a negative viscosity in the vicinity of the leading edge. I am not using the trip term of the model. Could neglecting the trip term lead to such a catastrophic failure of the code as Mar pointed out ? Thanks for your comments Regards, Ganesh

 August 3, 2006, 02:51 Re: Spalart-Allmaras model #7 mar Guest   Posts: n/a In stationary cases I succeed to a stable solution even if for small Reynolds number involving separation bubbles (Re=50000) but in instationary simulations involving relaminarization of the flow-field i have many problems in the leading edge region. If you are performing stationary cases I suggest to properly inizialize the turbulent variables. It MUST works.

 July 2, 2013, 04:14 Spalart Allmaras model #8 New Member   ali Join Date: Feb 2012 Posts: 8 Rep Power: 7 Dear friends, I have also problem with the SA model where the destruction term increases abruptly. I checked the code ans saw that it is because of the negative eddy viscosity nu. I applied it in backward facing and external flows. I neglect the transient terms ft1 and ft2. If the problem is with transient condition please let me know about the trip point and how we should set that term. Thanks

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Margherita Cadorin CFX 0 October 29, 2008 06:24 vandraren OpenFOAM Running, Solving & CFD 3 February 8, 2008 09:42 andimb OpenFOAM Post-Processing 1 April 25, 2006 05:04 andimb OpenFOAM Running, Solving & CFD 0 April 7, 2006 11:31 jj Siemens 0 October 3, 2005 15:31

All times are GMT -4. The time now is 20:59.