[maddy11]

Hi all,

I'm simulating a supersonic cavity using komega SST model. For Omega BC, I have used turbulentMixingLengthFrequencyInlet. I'm not sure what is the mixing length. Is it simply the cavity depth or length? I'm posting my file here. Kindly look at it and suggest corrections pls!!

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 -1 0 0 0 0];

internalField   uniform 4577132;

boundaryField
{
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            turbulentMixingLengthFrequencyInlet;
	 mixingLength	  0.015;
 	  k 			  k;
          value           uniform 4577132;
    }
    wall
    {
        type            omegaWallFunction;
        value           uniform 4577132;
    }
    top
    {
        type            zeroGradient;
    }
    frontAndBackPlanes
    {
        type            empty;
    }
}

[Tobi]

Hi,

a) please use code tags
b) its the hydraulic diameter multiplied by 0.07.

[maddy11]

Hi Tobias,

Thank you for your kind reply!
Can I take 0.07*cavity depth as the mixing length??

[unilord]

Originally Posted by Tobi

Hi,

a) please use code tags
b) its the hydraulic diameter multiplied by 0.07.

Hey Tobias,

I am writing my thesis, and I need to cite that information. Do you have any reference for it? It would be super useful.

Thank you,
Pedro

[Tobi]

Out of the box ... No. But maybe it's in Wilcox turbulence book.
If this is a reference for you (better than nothing).

https://www.cfd-online.com/Wiki/Turbulence_length_scale

[unilord]

Originally Posted by Tobi

Out of the box ... No. But maybe it's in Wilcox turbulence book.
If this is a reference for you (better than nothing).

https://www.cfd-online.com/Wiki/Turbulence_length_scale

I will have a look. I asked because I saw on CFD direct that it should be 0.07*Diameter (in a circular pipe for fully developed flow). However, I realized that maybe, in OpenFOAM, following what the page you linked says, it is 0.038*Diameter. I was using that before and I had a smaller error comparing to experimental results.

By the way, just to confirm. I am using this setup (for k and epsilon) for a 4 bladed centrifugal pump, with a circular tube as inlet. Would you change anything? It's steady state, with MRF approach.

k

"NCC.*"
    {
        type            zeroGradient;
    }
    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }
    "wall.*"
    {
        type            kqRWallFunction;
        value           uniform 1e-12;
    }
    "blade.*"
    {
        type            kqRWallFunction;
        value           uniform 1e-12;
    }
    inlet
    {
        type            turbulentIntensityKineticEnergyInlet;
        intensity       0.05;
        value           $internalField;
    }

epsilon:

"NCC.*"
    {
        type            zeroGradient;
    }
    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }
    "wall.*"
    {
        type            epsilonWallFunction;
        value           $internalField;
    }
    "blade.*"
    {
        type            epsilonWallFunction;
        value           $internalField;
    }
    inlet
    {
        type            turbulentMixingLengthDissipationRateInlet;
        mixingLength    0.005334;
        value           $internalField; 
    }

[Tobermory]

You can find the value of 0.07 (for mixing layers, pipes and channels) in

H.K. Versteeg and W. Malalasekera, An Introduction to Computational Fluid Dynamics, Prentice Hall, 1995.

Note that it's an empirical value, and varies slightly with case geometry, but is typically always around 10%.

[unilord]

Originally Posted by Tobermory

You can find the value of 0.07 (for mixing layers, pipes and channels) in



Note that it's an empirical value, and varies slightly with case geometry, but is typically always around 10%.

https://www.cfd-online.com/Forums/im...tor/attach.gif
Thank you!

But what about this sentence quoted in CFD Online's thread

For codes using a turbulence length-scale based on the mixing-length (Fluent, Phoenics and CFD-ACE for example) replace 0.038 and 3.8% with 0.07 and 7%.

Should we take that into consideration for OpenFOAM, and apply 0.038 instead of 0.07?

[Tobermory]

That's talking about a specific class of turbulence model, I believe (e.g one equation k-L model?), and is not code specific. You are using kW SST, I think, so you are fine to use the real value, 0.07.

[unilord]

Originally Posted by Tobermory

That's talking about a specific class of turbulence model, I believe (e.g one equation k-L model?), and is not code specific. You are using kW SST, I think, so you are fine to use the real value, 0.07.

I am using k epsilon, is that also fine to use 0.07?

And by any chance, do you know if it is more "correct" to use the eddy viscosity ration instead of the mixing length, let's say, for a centrifugal pump problem? I know that openfoam does have functions that have as input the eddy viscosity ratio. But we could implement it as a fixedValue in inlet.

[Tobermory]

The two methods should be equivalent ... with a two-equation model like k-epsilon, you have 2 degrees of freedom. The simplest is to specify k and L, which have well known empirical behaviour. You could specify k and nut (or nueff/num since you are talking about the viscosity ratio), but this will just give the same data ... providing that you choose the correct nut! They are all interelated by the assumptions in the k-epsilon model.

So, TLDR - if you feel you can specify nut more accurately than L, then my all means use it ... either as a direct boundary condition, or to back-calculate a value of L that you are more confident in.