# SA model in CFX

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

 August 23, 2018, 13:30 SA model in CFX #1 Member   phd Join Date: Oct 2013 Posts: 76 Rep Power: 12 Hi, there I am trying to use Spalart–Allmaras turbulence model in CFX but haven’t directly found it in the list of turbulence models. On the internet it seems to suggest that SA model is the ‘Eddy Viscosity Transport Equation Model’. But there is no official documents to state that. Moreover the paper that referred by ‘Eddy Viscosity Transport Equation Model’ is from Menter instead of Spalart and Allmaras. Could anyone tell me how can I implement SA model in CFX? Thank you very much!

 August 24, 2018, 03:46 #2 Senior Member     Join Date: Nov 2015 Posts: 244 Rep Power: 11 You can enable SA model by switching beta features ON. CFX Spalart Allmaras turbulence models https://imgur.com/LBiJlw3 https://imgur.com/ipH5Nlm k.vimalakanthan, lostking18 and Kevin Bryant like this.

August 26, 2018, 06:40
#3
Member

phd
Join Date: Oct 2013
Posts: 76
Rep Power: 12
Quote:
 Originally Posted by karachun You can enable SA model by switching beta features ON. CFX Spalart Allmaras turbulence models https://imgur.com/LBiJlw3 https://imgur.com/ipH5Nlm
Hi, Karachun:

Thanks! And I also got some additional info from Ansys technicians about the boundary condition set-up of SA model:

The S-A-Model is still in Beta-Stadium in CFX.
The GUI is not consistent. For this particular boundary condition, the value of TI is simply ignored.

The other options require two values to calculate the turbulent viscosity nu_t at the inlet:
Intensity and Length Scale: nu_t = Cmu * sqrt(k) * length_scale, k = 1.5 * Intensity^2 * Velocity^2
k and epsilon: nu_t = Cmu * k^2 / epsilon
k and omega: nu_t = k / omega
k and Length Scale: nu_t = Cmu * sqrt(k) * length_scale

Hope this will also be helpful.

 August 26, 2018, 07:15 #4 Senior Member     Join Date: Nov 2015 Posts: 244 Rep Power: 11 Thanks for reply!

September 6, 2018, 20:35
#5
New Member

Min Zhang
Join Date: Nov 2017
Location: China
Posts: 22
Rep Power: 8
Quote:
 Originally Posted by lostking18 Hi, Karachun: Thanks! And I also got some additional info from Ansys technicians about the boundary condition set-up of SA model: The S-A-Model is still in Beta-Stadium in CFX. The GUI is not consistent. For this particular boundary condition, the value of TI is simply ignored. The other options require two values to calculate the turbulent viscosity nu_t at the inlet: Intensity and Length Scale: nu_t = Cmu * sqrt(k) * length_scale, k = 1.5 * Intensity^2 * Velocity^2 k and epsilon: nu_t = Cmu * k^2 / epsilon k and omega: nu_t = k / omega k and Length Scale: nu_t = Cmu * sqrt(k) * length_scale Hope this will also be helpful.
Do you know the requirement for the yplus value near the wall? Should the yplus be smaller than 1? There are two options, including default and scalable, for the wall function term.

 Tags turbulence models