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!

kklomega model implemented in OF presents some iusses ho reported here

Yup, seen that one. Thanks a lot for spreading the word around :)

Why did you switch gamma-ReTheta to kkl ?

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.

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.

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.

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;
}
}

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

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?

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 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:confused:
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?

Hi,

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

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

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

// ************************************************** *********************** //

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

Help Me
 

Hi you. did you Know setting up for Airfoil for KomegaSSTLM? If you know You can teach me. Thank you very much

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

Hi Klaus,
Could you teach me to set up on the airfoil with KomegaSSTLM turbulence.
This is my set up:
https://www.cfd-online.com/Forums/me...903-myset2.jpg
https://www.cfd-online.com/Forums/me...902-myset1.jpg
https://www.cfd-online.com/Forums/me...e901-myset.jpg

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