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

gamma-ReTheta turbulence model for predicting transitional flows

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

Like Tree23Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 1, 2016, 05:15
Default
  #101
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Hmm, good to know. I only used the gamma-ReTheta model in application to the T3 cases without pressure gradient and then switched to kkl. Since you mention Cl I assume you're running a case for a foil so it may be that things will be a bit different due to the pressure gradients. Anyhow, thanks for sharing!
Artur is offline   Reply With Quote

Old   July 1, 2016, 05:47
Default
  #102
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
kklomega model implemented in OF presents some iusses ho reported here

Quote:
Originally Posted by malv83 View Post
There are a few problems with the k-kl-omega model in the farfield. One of them is the growth of Laminar Kinetic energy when separation occurs. Lopez and Walters have a paper (have not been published yet) correcting this issue:

Maurin Lopez. D. K. Walters. “A recommended correction to the k-kl-omega transition sensitive eddy-viscosity model”. Journal of Fluid Engineering.

This correction has to be made to the 2008 k-kl-omega model from now on.

Now, Lopez and Walters also developed a new transitional model (k-omega-v2) as an alternative to the k-kl-omega one. This new model has more capabilities (it is more reliable) than the k-kl-omega model, especially in the farfield computations. Fortunately the paper for this new model is already publish.

Maurin Lopez. D. K. Walters. “Prediction of transitional and fully turbulent free shear flows using an alternative to the laminar kinetic energy approach”. Journal of Turbulence, Vol 17, Iss. 3, 2016.

If you see the papers, you will immediately see how the k-kl-omega model is not good for free shear flows, and how the new model corrects all those issues. From now on, k-kl-omega users have to start using the new k-omega-v2 model.

Hope this helps
Artur likes this.
giammy92 is offline   Reply With Quote

Old   July 1, 2016, 05:51
Default
  #103
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Yup, seen that one. Thanks a lot for spreading the word around
Artur is offline   Reply With Quote

Old   July 1, 2016, 06:24
Default
  #104
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
Quote:
Originally Posted by Artur View Post
Hmm, good to know. I only used the gamma-ReTheta model in application to the T3 cases without pressure gradient and then switched to kkl. Since you mention Cl I assume you're running a case for a foil so it may be that things will be a bit different due to the pressure gradients. Anyhow, thanks for sharing!
Why did you switch gamma-ReTheta to kkl ?
giammy92 is offline   Reply With Quote

Old   July 1, 2016, 06:32
Default
  #105
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
In truth, I stopped working on transition for a while but then when I came back to it I had to start getting things done pretty rapidly. By then I had switched to OpenFOAM 3 and had issues compiling the gamma Re theta model so just had to use the built-in one. I'm hoping to get a bit more time to compile the code under new OF soon though when I might go back to it since it seems slightly more robust.
Artur is offline   Reply With Quote

Old   July 1, 2016, 10:43
Default
  #106
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
Might I ask you an advice? I told you that I have an O-Grid so I should use freestream bc for far field...but there is a bc for ReTheta for inlet attached with gammaReTheta in which header file I read:

Note
In the event of reverse flow, a zero-gradient condition is applied

So it means that I could apply it even for far field? I hypothesize this because in freestream header file I read:

Description
This boundary condition provides a free-stream condition. It is a 'mixed'
condition derived from the \c inletOutlet condition, whereby the mode of
operation switches between fixed (free stream) value and zero gradient
based on the sign of the flux.
giammy92 is offline   Reply With Quote

Old   July 2, 2016, 07:22
Default
  #107
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
I would assume you can use that if it's been derived from the inletOutlet BC which works OK with o-grids. I haven't used that BC myself, in the past I would compute the inlet quantities myslef and apply a fixedValue at the inlet but it should be more straightforward with the dedicated BC.
Artur is offline   Reply With Quote

Old   July 4, 2016, 05:18
Default
  #108
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
Thank you Artur but unfortunely my problems don't stop here. I'm performing unsteady simulation with PimpleFoam but I have very high residual of p that i can't able to reduce. How dou you valutate my fvSolution?

solvers
{
p
{
solver PCG;
preconditioner DIC;
tolerance 1e-04;
relTol 0.05;
}

pFinal
{
$p;
tolerance 1e-4;
relTol 0;
}

U
{
solver smoothSolver;
smoother GaussSeidel;
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
nSweeps 2;
}

"(gamma|ReThetatTilda|k)"
{
solver smoothSolver;
smoother GaussSeidel;
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
nSweeps 2;
}

omega
{
$U
tolerance 1e-6;
relTol 0.1;
}

omegaFinal
{
$U
tolerance 1e-7;
relTol 0;
}

UFinal
{
$U;
tolerance 1e-5;
relTol 0;
}

"(ReThetatTilda|gamma|k)Final"
{
$U;
tolerance 1e-6;
relTol 0;
}

}

PIMPLE
{
nOuterCorrectors 20;
nCorrectors 2;
nNonOrthogonalCorrectors 3;
pRefCell 0;
pRefValue 0;

residualControl
{
"(p|U|k|ReThetatTilda|omega|gamma)"
{
tolerance 1e-5;
relTol 1e-2;
}
}
}

potentialFlow
{
nNonOrthogonalCorrectors 10;
}

relaxationFactors
{
fields
{
p 0.3;
}
equations
{
U 0.5;
k 0.5;
ReThetatTilda 0.5;
omega 0.5;
gamma 0.5;
}
}
giammy92 is offline   Reply With Quote

Old   July 4, 2016, 08:17
Default
  #109
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Hi,

Had a quick look and nothing in particular strikes me as wrong. I'd be careful though with the underrelaxation factors you've set, they seem lower than what I'd go with myself. Another possibility is the time step being too large. I'm assuming you're happy with your mesh? Are you initialising your simulation using a steady-state solution or at least potentialFoam first? Otherwise hard to say.

Good luck,

A
Artur is offline   Reply With Quote

Old   July 4, 2016, 12:33
Default
  #110
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
my mesh has max non-orthogonality 88 with 171 non-ortho faces placed near airfoil. About initialization i don't have done anything. Might be non orthogonality of mesh the problem?
giammy92 is offline   Reply With Quote

Old   July 4, 2016, 13:27
Default
  #111
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Yes, 88 sounds quite high. I'd suggest running it with potentialFoam first, then simpleFoam with a standard k-omega SST turbulence model to make sure mesh and settings are ok. Then use the velocity fields from steady-state simulation to initialise the one you're really after. Also, probably best to continue this in a new thread under Running, soling & CFD since we've gone off topic (feel free to send me a private message with a link to the new thread if you end up opening it).

Peace,

A
Artur is offline   Reply With Quote

Old   July 6, 2016, 04:53
Default
  #112
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
Quote:
Originally Posted by Artur View Post
Yup, definitely something fishy going on. Here's the setup I used in the past back when OF was at 2.2.2. This was based on one of the original test cases posted by Felix:
https://www.dropbox.com/s/ly0scvqgdh...3A.tar.gz?dl=0
Maybe have a look and see if there are any major differences between this and your setups.
Artur I haven't understood why for internal field of ReThetatTilda you have set the value calculated for the equation (24) of the paper instead for inlet is set 0.1
The value for internal field, that is just an initialization, shouldn't be same of inlet calculated with (24)? And why the reason of 0.1 at inlet?
giammy92 is offline   Reply With Quote

Old   July 6, 2016, 06:54
Default
  #113
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Hi,

Not entirely sure what you're asking, here's the BC file I used for ReTheta:

Code:
dimensions      [0 0 0 0 0 0 0];

internalField   uniform 1.574098e+02;

boundaryField
{
    flatPlate
    {
        type            zeroGradient;
    
    }
    frontPlate
    {
        type            symmetryPlane;
    }
    top
    {
        type            symmetryPlane;
    }
    inlet
    {
    type        fixedValue;
    value        $internalField;
    }
    outlet
    {
        type            zeroGradient;
    }
}
And yes, I usually set the internal field to the same value as the inlet, it tends to make things more stable. Shouldn't affect the final result though (in an ideal world at least).

Hopefully this addresses your questions.

All the best,

A
Artur is offline   Reply With Quote

Old   July 6, 2016, 07:03
Default
  #114
Senior Member
 
Join Date: Mar 2016
Posts: 133
Rep Power: 10
giammy92 is on a distinguished road
If you see there is a file called initialConditions where the inlet value is 0.1



/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.1 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/

flowVelocity (5.4 0 0);
pressure 0;
turbulentKE 5.668704e-02; // Tu = 3.6%
turbulentOmega 3.149280e+02; // mut/mu = 12
ReThetatTilda 0.1;//1.574098e+02;
#inputMode merge

// ************************************************** *********************** //
giammy92 is offline   Reply With Quote

Old   July 6, 2016, 07:10
Default
  #115
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 20
Artur will become famous soon enough
Oh, I see now. I must have forgotten to delete it when I was experimenting with stuff. Nonetheless, this value doesn't get used in the actual BC file since the inlet value gets specified explicitly. Sorry for the confusion.

A
Artur is offline   Reply With Quote

Old   January 24, 2018, 22:56
Default Help Me
  #116
Member
 
ESI
Join Date: Sep 2017
Posts: 46
Rep Power: 8
ht2017 is on a distinguished road
Quote:
Originally Posted by klausb View Post
Hello,

how are the values for /0/ReThetatTilda and gamma calculated?

Case: Airfoil, Re=1e6, Tu=0.06, U=14.6

Klaus
Hi you. did you Know setting up for Airfoil for KomegaSSTLM? If you know You can teach me. Thank you very much
ht2017 is offline   Reply With Quote

Old   January 25, 2018, 10:23
Default
  #117
Senior Member
 
Klaus
Join Date: Mar 2009
Posts: 259
Rep Power: 22
klausb will become famous soon enough
Hello,

please describe the simulation you are planning (airfoil, Reynolds number, Tu...) and your setup problems.

In general, it's a good idea to use a working case which uses a similar turbulence model as a starting point and make adjustments rather than creating a new setup from scratch. You could use a steady state (simpleFoam) case which uses e.g. kOmegaSST if you have one and you should look at the tutorials maybe there's a case using the model you want to use.

To get an idea about calculating the model specific initial values (specific 0 folder content for gammaInt and ReThetat) read the academic papers describing the model:

Langtry, R. B., & Menter, F. R. (2009).
Correlation-based transition modeling for unstructured parallelized
computational fluid dynamics codes.
AIAA journal, 47(12), 2894-2906.

Menter, F. R., Langtry, R., & Volker, S. (2006).
Transition modelling for general purpose CFD codes.
Flow, turbulence and combustion, 77(1-4), 277-303.

Langtry, R. B. (2006).
A correlation-based transition model using local variables for
unstructured parallelized CFD codes.
Phd. Thesis, Universität Stuttgart.

Klaus
ht2017 likes this.

Last edited by klausb; January 25, 2018 at 15:02.
klausb is offline   Reply With Quote

Old   January 25, 2018, 20:38
Default
  #118
Member
 
ESI
Join Date: Sep 2017
Posts: 46
Rep Power: 8
ht2017 is on a distinguished road
Quote:
Originally Posted by klausb View Post
Hello,

please describe the simulation you are planning (airfoil, Reynolds number, Tu...) and your setup problems.

In general, it's a good idea to use a working case which uses a similar turbulence model as a starting point and make adjustments rather than creating a new setup from scratch. You could use a steady state (simpleFoam) case which uses e.g. kOmegaSST if you have one and you should look at the tutorials maybe there's a case using the model you want to use.

To get an idea about calculating the model specific initial values (specific 0 folder content for gammaInt and ReThetat) read the academic papers describing the model:

Langtry, R. B., & Menter, F. R. (2009).
Correlation-based transition modeling for unstructured parallelized
computational fluid dynamics codes.
AIAA journal, 47(12), 2894-2906.

Menter, F. R., Langtry, R., & Volker, S. (2006).
Transition modelling for general purpose CFD codes.
Flow, turbulence and combustion, 77(1-4), 277-303.

Langtry, R. B. (2006).
A correlation-based transition model using local variables for
unstructured parallelized CFD codes.
Phd. Thesis, Universität Stuttgart.

Klaus
Hi klausb,
I am using KomegaSSTLM for my simulation. But I don't know the reason why my result incorrect?
this is my case:
I run the simulation for A-airfoil with inlet condition is M = 0.15,Re = 2.1e6, alpha =13.1,Tu = 0.1%,μ_t/μ =2.
I calculate the coefficients:
K =3/2(UI)^2 = 3/2 (51.9*0.1%)^2=0.00404; ω = ρ* k/μ*(μ_t/μ)^-1
ω = 1.225*0.00404/(1.846*10^-5)*(2)^-1=134.05;
gamma I choose 1. gama = 1;
Re_thetat = (1173.51-589.428*Tu+0.2196/(Tu^2))*F(λθ) if Tu<= 1.3;
Re_thetat = 331.50*(Tu-0.5658)^-0.671*F(λθ) if Tu >1.3;
F(λθ) =1-1(-12.986*λθ-123.66*λθ^2-405.689*λθ^3)*e^(Tu/1.5)^1.5 if λθ<=0;
F(λθ) =1+0.275*(1-e^(-35.*λθ))*e^(Tu/0.5) if λθ>0;

From this function: I choose λθ = 0 ( I not sure it is correct I only think Du/Ds = 0 Inferred λθ = 0) then I calculate Re_thetat = 1.365e+3.

I have the coefficients:
K =0.00404;ω =134.05,gamma = 1,Re_theta = 1.365e+3 this is the coefficient value for inlet condition.

And Then I set up following the tutorial incompressible/simpleFoam/T3A. I change the geometry to A-airfoil and set up the value coefficient and I run it.
The finally, I run with comment line "simpleFoam -postProcess -func 'wallShearStress' and paraFoam. In the paraview I load out the data in the surface top-Airfoil. I plot the wallshearstress following the x-axis. But my result incorrect.

If you have experienced run with KomegaSSTLM for airfoil Please teache me. I really hope anyone who can help me resolve it.
Thank you very much
ht2017 is offline   Reply With Quote

Old   January 25, 2018, 22:09
Default
  #119
Member
 
ESI
Join Date: Sep 2017
Posts: 46
Rep Power: 8
ht2017 is on a distinguished road
Quote:
Originally Posted by klausb View Post
Hello,

please describe the simulation you are planning (airfoil, Reynolds number, Tu...) and your setup problems.

In general, it's a good idea to use a working case which uses a similar turbulence model as a starting point and make adjustments rather than creating a new setup from scratch. You could use a steady state (simpleFoam) case which uses e.g. kOmegaSST if you have one and you should look at the tutorials maybe there's a case using the model you want to use.

To get an idea about calculating the model specific initial values (specific 0 folder content for gammaInt and ReThetat) read the academic papers describing the model:

Langtry, R. B., & Menter, F. R. (2009).
Correlation-based transition modeling for unstructured parallelized
computational fluid dynamics codes.
AIAA journal, 47(12), 2894-2906.

Menter, F. R., Langtry, R., & Volker, S. (2006).
Transition modelling for general purpose CFD codes.
Flow, turbulence and combustion, 77(1-4), 277-303.

Langtry, R. B. (2006).
A correlation-based transition model using local variables for
unstructured parallelized CFD codes.
Phd. Thesis, Universität Stuttgart.

Klaus
Hi Klaus,
Could you teach me to set up on the airfoil with KomegaSSTLM turbulence.
This is my set up:


ht2017 is offline   Reply With Quote

Old   January 25, 2018, 22:13
Default
  #120
Member
 
ESI
Join Date: Sep 2017
Posts: 46
Rep Power: 8
ht2017 is on a distinguished road
Quote:
Originally Posted by klausb View Post
Hello,

please describe the simulation you are planning (airfoil, Reynolds number, Tu...) and your setup problems.

In general, it's a good idea to use a working case which uses a similar turbulence model as a starting point and make adjustments rather than creating a new setup from scratch. You could use a steady state (simpleFoam) case which uses e.g. kOmegaSST if you have one and you should look at the tutorials maybe there's a case using the model you want to use.

To get an idea about calculating the model specific initial values (specific 0 folder content for gammaInt and ReThetat) read the academic papers describing the model:

Langtry, R. B., & Menter, F. R. (2009).
Correlation-based transition modeling for unstructured parallelized
computational fluid dynamics codes.
AIAA journal, 47(12), 2894-2906.

Menter, F. R., Langtry, R., & Volker, S. (2006).
Transition modelling for general purpose CFD codes.
Flow, turbulence and combustion, 77(1-4), 277-303.

Langtry, R. B. (2006).
A correlation-based transition model using local variables for
unstructured parallelized CFD codes.
Phd. Thesis, Universität Stuttgart.

Klaus
Hi you,
I want to plot the graph similar it. but I don't konw How to do it in paraview?
https://www.cfd-online.com/Forums/me...re900-you2.jpg
ht2017 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
Low Reynolds k-epsilon model YJZ ANSYS 1 August 20, 2010 13:57
Centrifugal Pump and Turbulence Model Michiel CFX 12 January 25, 2010 03:20
RSM & Transitional Flows!!! Erika FLUENT 0 March 31, 2006 10:56
Turbulence model Herry Phoenics 1 May 29, 2003 13:19
turbulent separated flows Yin Fidelity CFD 9 February 19, 2003 11:50


All times are GMT -4. The time now is 17:44.