CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Turbulence kinetic energy not defined for incompressible SA model

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

Like Tree2Likes
  • 1 Post By ndev
  • 1 Post By ndev

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 17, 2015, 12:21
Default Turbulence kinetic energy not defined for incompressible SA model
  #1
New Member
 
Fernando Soares Alves
Join Date: Oct 2013
Posts: 16
Rep Power: 10
FernandoSoares is on a distinguished road
Hi Foamers,

I was attempting to run simpleFoam using Spalart-Allmaras model for incompressible flow over a backward facing step in current OF240. The simulation starts normally, but I get the following warning:

Code:
--> FOAM Warning : 
    From function tmp<volScalarField> SpalartAllmaras::k() const
    in file SpalartAllmaras/SpalartAllmaras.C at line 280
    Turbulence kinetic energy not defined for Spalart-Allmaras model. 
    Returning zero field
As far as I knew, SA model variables were actually only nut and nuTilda (am I right?). And for the matter my original directory was mapped from a kOmegaSST solution obtained earlier and I used createTurbulenceFields to generate the remaining fields of interest. So my starting directory actually contains a k file.

I tried to find out why I was getting such a message by taking a look in the code. A similar message would also be displayed for the epsilon field, which does not happen in my simulation.

Has anyone ever had such issue with incompressible SA? Is it really meaningful in terms of solution for the model to get always zero field for k and epsilon? I'm asking this because I'm getting ~steady residuals way above the accuracy desired.
FernandoSoares is offline   Reply With Quote

Old   November 6, 2015, 10:32
Default
  #2
New Member
 
Join Date: Sep 2015
Posts: 15
Rep Power: 8
dappe is on a distinguished road
Hi Fernando
I'm having the same issue while simulating an Impinging Jet with a compressible solver. Also in my case I already have k folder because I ran the same case with kOmegaSSt. It is very strange and I d like to know if this affects the results: in fact I have oscillating residuals, the solution does not converge and I m trying to find out which could be the problem.
Let me know if you will solve this problem.
Alessandro
dappe is offline   Reply With Quote

Old   November 6, 2015, 14:54
Default
  #3
New Member
 
Nate
Join Date: Oct 2013
Location: Amherst, MA
Posts: 13
Rep Power: 10
ndev is on a distinguished road
In my experience, a "Foam Warning" can be taken as an informational, but not significant, message about your simulation...though there could be some exceptions. In this case it is true that the SA equations cannot return a turbulent kinetic energy field...but having k in your zero directory shouldn't do anything. Alessandro, this in no way should produce oscillating results, or affect the solution in any way, so you can definitely start looking elsewhere for issues!
dappe likes this.
ndev is offline   Reply With Quote

Old   November 9, 2015, 04:02
Default
  #4
New Member
 
Join Date: Sep 2015
Posts: 15
Rep Power: 8
dappe is on a distinguished road
Thank you ndev!
dappe is offline   Reply With Quote

Old   February 28, 2018, 11:09
Default
  #5
Member
 
Join Date: Mar 2009
Posts: 89
Rep Power: 14
aerogt3 is on a distinguished road
Does anyone know where this could come from? I am getting the error despite not having k in any of the timesteps (or constant) folders in any of my processor folders. I have scoured controlDict and the function objects (like fieldaverage, etc.) looking for k but cannot find anything.

Really curious where this message comes from and eager to get rid of it!
aerogt3 is offline   Reply With Quote

Old   February 28, 2018, 12:12
Default
  #6
New Member
 
Nate
Join Date: Oct 2013
Location: Amherst, MA
Posts: 13
Rep Power: 10
ndev is on a distinguished road
You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

Code:
const tmp<volScalarField> tk = turbModel.k();
If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.
aerogt3 likes this.
ndev is offline   Reply With Quote

Old   March 1, 2018, 06:46
Default
  #7
Member
 
Join Date: Mar 2009
Posts: 89
Rep Power: 14
aerogt3 is on a distinguished road
Quote:
Originally Posted by ndev View Post
You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

Code:
const tmp<volScalarField> tk = turbModel.k();
If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.
Good catch! That was the issue. I had been looking at my BCs, and all my wall functions were nutUSpalding wall function. BUT, on one zone, which had a roughness, I was using nutkRoughWallFunction. I've switched that out for nutURoughWallFunction. Thanks a lot!
aerogt3 is offline   Reply With Quote

Old   October 24, 2019, 12:07
Default
  #8
New Member
 
Join Date: Oct 2019
Posts: 2
Rep Power: 0
Leslie Lee is on a distinguished road
Quote:
Originally Posted by ndev View Post
You want to be looking for things that will call the k() method in Spalart-Allmaras. What boundary condition are you using on nut? I ask because if you are using "nutkWallFunction" you're calling in the BC:

Code:
const tmp<volScalarField> tk = turbModel.k();
If so, you may want to switch to "nutUSpaldingWallFunction" or "nutUWallFunction" as these really only use the velocity gradients and viscosity.
Hi foamers,

I have the same issues while simulating an Impinging Jet with BuoyantBoussinesqSimpleFoam. So I try to use "nutUSpaldingWallFunction" and "nutUWallFunction", as you suggested. But, it didn't work out. Please let me know if you have other solutions to fix this. Thanks~

Lee
Leslie Lee is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Overflow Error in Multiphase Modelling with Two Continuous Fluids ashtonJ CFX 6 August 11, 2014 15:32
Turbulent kinetic energy in k-epsilon model khunyeu FLUENT 0 October 7, 2013 02:31
Wall Treatment of User defined Turbulence Model Yang Chung FLUENT 0 August 23, 2008 12:31
Average turbulence kinetic energy / intensity tucker FLUENT 2 January 11, 2006 21:40
turbulence kinetic energy? Eric FLUENT 1 December 3, 2000 11:41


All times are GMT -4. The time now is 13:24.