Relation between k and UPrime2Mean etc in LES
 

Hii,

While doing LES using OF, I found that the value of k and the value of 0.5*(UPrime2Meanxx+UPrime2Meanyy+UPrime2Meanzz) are very different. Can someone please elaborate why is it so? They are supposed to be exactly the same, according to the definition of turbulent kinetic energy.

Thanks,
Tarak

I think the difference is that the k calculated in LES refers to the sub-grid-scale kinetic energy, whereas the 0.5*(u'_ii) refers to the total turbulent kinetic energy

Hii,

Thanks for the reply. But while prescribing the boundary value in k, suppose say at inlet, we set the value of the TKE from k=1.5(I*U)^2. That's not sgs kinetic energy. So doesn't these 2 contradict each other?

Thanks,
Tarak

I'm not sure of that boundary value for k, however, if you take a look at the source codes of the LES models you'll see how the k is calculated.

When using oneEqEddy models the sub-grid kinetic energy is calculated through a transport equation and then used to calculate the subgrid viscocity.

In smagorinsky models the sub-grid kinetic energy is calculated from the velocity gradient.

In LES modeling the SGS quantities are used to close the model. The value of k is an instantaneus value, different from the total turbulent kinetic energy calculated from the Reynolds stress tensor

Thanks a lot. Ya I'm sure that the k is indeed sgs k, but then it becomes difficult to prescribe the inlet condition, as the sgs ke is not known beforehand. So, is it wise to prescribe a relatively low value of k, that is lower than the total turb kinetic energy? I you have some personal experience with this, please do not hesitate to advice.

Thanks,
Tarak

For the problem I'm solving now i'm using a turbulent inlet velocity profile, and for k i'm setting a low value, 2e-5. I'm getting accepable results with this. You should be worried for this condition if using oneEqEddy or kOmega type models, smagorinsky models do not depend on k as it is calculated from the velocity

Thanks a lot.

I am using dynamicOneeqEddy model, that's why I am so concerned about it. I am presently simulating the flow over a circular cylinder for Re=3900, but not managing to get an acceptable recirculation length. So, the way you prescribed now may help. If you had any luck with the flow over a circular cylider please do let me know.

Thanks,
Tarak

k is indeed the turbulent sgs energy (see http://foam.sourceforge.net/doc/Doxy...OneEqEddy.html), but UPrime2Meanxx are the variances of the resolved and time averaged scales http://foam.sourceforge.net/doc/Doxy...0b4d6940d1b9e4.
So your 0.5*tr(UPrime2Mean) is more like kinetic energy of the resolved turbulent scales.

Hi gregor

I am trying to find out how Uprime2Mean is calculated. I went to the source code of fieldaveraging, but still I could not figure out how this parameter is calculated. I am looking for a Reynolds stress definition as below

R=<u'iu'j>+<uiuj>-<ui><uj>

the first trem is unresolved Reynolds stress and the addition of the other two terms are the resolved Reynolds Stress. Is Uprime2Mean the same as above equation?

any comment on the Uprime2Mean calculation will be of great help to me.

Thanks

Uprime2Mean is simply the variance of the resolved scales. Which is the quadratic value of the standard deviation sigma. Standard deviation gives you an idea on how much your values deviate around a mean value.

var = sigma^2 = 1/(N) sum^N(phi - <phi>)^2, where <.> is a time averaged value

So it is the averaged deviation around a mean value ;). The definition of Reynoldstresses has nothing to do with how the variances a calculated.

Gregor

Thanks Gregor

Now, I have an idea on how Uprime2Mean is claculated.
I want to get the time average of Reynolds stress tensor during the run. In Kepsilon Model, R is calculated like this

tmp<volSymmTensorField> kEpsilon::R() const
{
return tmp<volSymmTensorField>
(
new volSymmTensorField
(
IOobject
(
"R",
runTime_.timeName(),
mesh_,
IOobject::NO_READ,
IOobject::NO_WRITE
),
((2.0/3.0)*I)*k_ - nut_*twoSymm(fvc::grad(U_)),
k_.boundaryField().types()
)
);
}

Do you have any idea how I can implement this in OpenFoam?

Since you already have your modelled R field you could just add

to your controlDict to average R over time.

I have already done that. But it gives me the following error

Requested Field R Does not exist in the database

Are you doing LES or RANS and what is your turbulence model ?

Hi,

I think that every field you want to average first has to be created here:

#include "createFields.H"

in your solver. So, go to solver you want to use, and add a new field in createField.H:
something like:

volSymmTensorField R_
...
...
Than, you'll have to add something like this into solver:

R_ = yourTurbulenceModel->R();

And than, field R_ can be averaged...
You'll have to play a little with solver, but this is not a big issue...

Regards,
Dejan

Quote:

Originally Posted by morard (Post 341034) Hi, I think that every field you want to average first has to be created here:

It doesn't matter where you create it, as long as it is registred in the object registry.

Quote:

Originally Posted by morard (Post 341034) R_ = yourTurbulenceModel->R();

Depending on if he is doing RANS or LES it could be

yourTurbulenceModel->B() (for LES)

aswell

Gregor

Ufff, sorry, my mistake. It's LES about (from the first post).
So, it's definitely:

yourTurbulenceModel->B() (for LES)

Ok i just wondered, because its not the original guy asking anymore.

And if its LES then you have to create the field first (i.e. in #include createFields.H) and then assign it like B_ = yourLESturbMod->B().

I was just confused by his RANS example, where the R field gets created by default from the turbulence model.

hi

I am using RANS and KEpsilon Model to solve my problem and the error still exists. I went through KEpsilon.C to find how R is calculated and saved. I see that in this file, k and epsilon are written in a file by using


k_
(
IOobject
(
"k",
runTime_.timeName(),
mesh_,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
autoCreateK("k", mesh_)

but for R, it is

tmp<volSymmTensorField> kEpsilon::R() const
{
return tmp<volSymmTensorField>
(
new volSymmTensorField
(
IOobject
(
"R",
runTime_.timeName(),
mesh_,
IOobject::NO_READ,
IOobject::NO_WRITE
),
((2.0/3.0)*I)*k_ - nut_*twoSymm(fvc::grad(U_)),
k_.boundaryField().types()
)
);
}

by Looking at the above file, I see that R is created but it is not written anywhere. I changed NO_WRITE to AUTO_WRITE, but nothing happened. Do you still believe that R is created and can be averaged?!

Thanks for your time. I do appreciate your help

Ok i guess the reason is that you R field is only created as a tmp field if you are calling the R() function. So you should try what morad suggested and create a separate R field inside your createFields.H

as




and make sure that you update it every time step by

R_ = turbulence->R()

Gregor

my Solver is pisoFoam. So, Should I add these new lines to the createFields.H inside the pisoFoam Directory?! Do I need to compile these codes when I add those terms?

in createFields.H inside pisoFoam Directory, I see that it reads U and P fields rather than writing them

Info<< "Reading field U\n" << endl;
volVectorField U
(
IOobject
(
"U",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

are you sure this is the place to create R field?

Yes you would have to recompile your code.


It reads the fields and creates an entry in the object registry, which is needed for the sampling. So its nothing wrong with putting it in there, but you can place it anywhere else where it fits ;)

Gregor

...and don't forget to change the name of the solver :)

Ok, thanks guys.

to compile a code, As far as I remember, I should use wmake libso. do I need to make a new library for my new solver let's say pisoFoam2?!
I do not want to change pisoFoam.C. I want to make a copy of that somewhere and then change it.

by the way, by the following command, do you mean that I should use this inside pisoFoam solver?! and what is turbulence?! do you mean RASModel ->R()?!

R_ = turbulence->R()

Hi,

first, just copy original pisoFoam and change name to, as you said, pisoFoam2 (but, my suggestion is to choose something other like pisoRFoam, because after some tome you will have pisoFoam2, pisoFoam3,... and you will definitely forget what did you change in each of those..). So, you have to change pisoFoam.C to pisoFoam2.C. Than, open Make folder and inside files, you also have to change:

pisoFoam2.C

EXE = $(FOAM_APPBIN)/pisoFoam2

Then navigate your terminal to pisoFoam2 folder and execute:

wclean
wmake

now you have your own solver pisoFoam2. Now do the changes mentioned by Gregor and me.

If you take a look into createFields.H, you will see how pointer is created. At the end of the file it is written:

autoPtr<incompressible::turbulenceModel> turbulence
(
incompressible::turbulenceModel::New(U, phi, laminarTransport)
);

so, you'll have to put inside pisoFoam2.C

R_ = turbulence->R();

Put this inside while loop. Between the lines: turbulence->correct(); and runTime.write(); might be a good position. So, at the end you'll have:

turbulence->correct();

R_ = turbulence->R();

runTime.write();

This should wor.

Check this page:
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

There you can find a lot of useful things.

Thanks Morad. So nice!
I will try it out!

Hi

I compiled the new pisoFoam solver and I added the following line to the code:

createField.H


Info<< "Reading field R\n" << endl;
volSymmTensorField R
(
IOobject
(
"R",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh
);

and to the pisoFoam2 solver,



volSymmTensorField R
(
IOobject
(
"R",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
turbulence->R()
);

R.write();


This way, the solver reads R field from time 0 and it writes and updates the R field every time step to a directory.

My problem is two things:

1- I want to have R field written in time directories specified in controlDict (specified write intervals). My new solver writes R in each time step and gives it as an output every time.

2- When I do field averaging, I do not receive the old error which was "the Requested R field does not exist". Now, R field is created. But, it seems that for field averaging, the algorithm gets the initial R field and average that during runtime which always gives the same thing for all times.


I would be happy if you can suggest a way to overcome any of the above issues.

Thanks,

there you made a mistake


In the pisoFoam2.C a simple

should be sufficient. You just want to get the R-field every timestep not create it every timestep. Furthermore you don't need a
since you have told the objectRegistry to handle it by IOobject::AUTO_WRITE

Gregor

I also tried adding this line instead of R.write(). But, I received an error when compiling the code. I will post the error in an hour or so.

Thanks

hi,

Thanks to your comments, I could get field average of R over time.

I also want to calculate U*U and get the average of this field over time. U is given by OpenFoam. I just need to add some lines to calculate U*U. if U=[1 2 3;4 5 6], by U*U, I mean the result is [1 4 9;16 25 36]. I do not know how openfoam writes U field so that I can write a "for loop" to calculate U*U. do you have any suggestions?

Hi Gregor

I guess Uprime2Mean(0) is also equivalent to the following equation

<UU>-<U><U>, where <> is time averaged value.
since 1/n sum^N (U-<U>)^2= <UU>-2<U><U>+<U><U>=<UU>-<U><U>.
Am I right?

correct see http://en.wikipedia.org/wiki/Computa...r_the_variance

but i am a bit confussed by your vector definition in the above post ( U=[1 2 3; 4 5 6] ??)

Gregor

You guys are making a mistake. Calling "R()" for an SGS model will not return the total Reynolds stress. It will just return the SGS stress. The only reason it is called "R()" is for compatibility with the RANS model nomenclature.

UPrime2Mean is calculated as:

UPrime2Mean_new = alpha*UPrime2Mean_old + (1-alpha) * sqr(U) - sqr(Umean);

with alpha = (Time - dTime) / Time

If you work it out, this is identical to the definition for Reynolds stress when averaged over a long time (<UU>-<U><U>).

To get the full stresses (resolved + SGS) you thus need UPrime2Mean + RMean. Unfortunately, you will still have to modify a solver to create RMean since the R field is not available by default as noted below.

I know its confusing to discuss RANs matters in a LES thread but sam1364 is using kEpsilon (according to http://www.cfd-online.com/Forums/ope...tml#post340914).

Gregor

Hi guys,

I have done UPrime2Mean + RMean to get the total Reynolds Stress for RANS simulation. I could get RMean thanks to Gregor suggestions. But I see a big problem when calculating R or Rmean and that is the values of R or RMean at the walls of cavity which are not zero (I am solving the lid driven cavity flow). I am using kqrwallfunction for R but I do not understand why I get non zero values of Reynolds stress at fixed walls. Am I using the right wall function, Should I set the values of R zero at the fixed wall?

I would assume that you are looking at R in the first cell next to the wall (which isnt zero). R exactly at the wall is zero since your k should be zero.

Gregor

No, I am looking at wall and I am using this initial set up for R

dimensions [0 2 -2 0 0 0 0];

internalField uniform (0 0 0 0 0 0);

boundaryField
{
movingWall
{
type kqRWallFunction;
value uniform (0 0 0 0 0 0);
}
fixedWalls
{
type kqRWallFunction;
value uniform (0 0 0 0 0 0);
}
front
{
type symmetryPlane;
}
}

I guess based on the equation given in Kepsilon.C for R, the values at wall can be non zero.

Nice to meet you , Tarak.
Now I have the same question of you had last year. I am confusing about how to set the k. I had done some work in backward step simulation with oneeqEddy and dynamicOneeqEddy model at the same grid and the same condition. I set k as 1*10-5 in both simulaiton, but the dynamicOneeqEddy model diverge after about 15s, but can go on to compute.Would you please give me some suggestion on it？

Hi Gregor

In my URANS simulation k is not equal to 0.5*(Uprime2MeanXX+Uprime2MeanYY+Uprime2MeanZZ). This is probably because k and epsilon are calculated using evolution equation and R is computed using boussinesq approximation. whereas UPrime2Mean is computed using postprocessing of U field. So I doubt Reynolds stress is UPrime2Mean in URANS simulations.
I will appreciate your comment.