[aylalisa]

Dear All,

there are some threads about LES where channelOodles solver is mentioned (and used).
I don't find channelOodles in OF2.2.2. Were did it go?

Aylalisa

[alexeym]

Hi,

I guess now it is called channelFoam and it is a part of The OpenFOAM® Extend project (http://www.extend-project.de).

[wyldckat]

Greetings to all!

channelOodles was renamed to channelFoam when OpenFOAM 1.6 was released. This seems to have been because they generalized the "Oodles" modelling - http://openfoamwiki.net/index.php/Oodles - to the generic single-phase incompressible LES modelling we use in OpenFOAM nowadays.

Then when they released OpenFOAM 2.2.0, they dropped channelFoam entirely, because pimpleFoam is now generic enough to contemplate what only channelFoam was be able to do in past versions. This is also hinted by the transfer of the tutorial "incompressible/channelFoam/channel395" to "incompressible/pimpleFoam/channel395".

I have not tested the two tutorial on each version, namely in OpenFOAM 2.1.x vs 2.2.x, to confirm if the results are similar enough.

As for the channelFoam version present in FOAM-Extend 3.0, it's derived from OpenFOAM 1.6.x.

According to the Git history in FOAM-Extend 3.0 and the compilation from the official OpenFOAM git repositories (available here: https://github.com/wyldckat/OpenFOAM-combo/), it seems that the solver has not evolved in either versions/variants.

Honestly, I suggest that you compare the results from the two tutorials on OpenFOAM 2.2.x or 2.3.x vs the one on OpenFOAM 2.1.x or FOAM-Extend 3.0, to ascertain whether it's worth it or not to use channelFoam.

Best regards,
Bruno

[alexeym]

Hi,

wildckat is right, pimpleFoam is more universal as it can handle both LES and RAS turbulence models, and this part of channelFoam:

        // Extract the velocity in the flow direction
        dimensionedScalar magUbarStar =
            (flowDirection & U)().weightedAverage(mesh.V());
    
        // Calculate the pressure gradient increment needed to
        // adjust the average flow-rate to the correct value
        dimensionedScalar gragPplus =
            (magUbar - magUbarStar)/rUA.weightedAverage(mesh.V());
                
        U += flowDirection*rUA*gragPplus;
                
        gradP += gragPplus;

is now implemented as fvOption and described in system/fvOptions like this:

momentumSource
{
    type            pressureGradientExplicitSource;
    active          on;            //on/off switch
    selectionMode   all;       //cellSet // points //cellZone

    pressureGradientExplicitSourceCoeffs
    {
        fieldNames  (U);
        Ubar        ( 0.1335 0 0 );
    }
}

And in fact channelFoam from extended project can be compiled with OpenFOAM 2.2.2 (I've checked only this version) with slight modifications, I've attached archive of the modified solver (from 1.6-ext, modifications are mainly in the name of variables and methods to suit 2.2.2) to the message, if you'd like to compare pimpleFoam and channelFoam.

[aylalisa]

Hello Alexey, Hello Bruno,

does this first code snipet guarantee the constant mass flow rate (as described in OpenFOAM Wiki - ChannelOodles)?

(I still have problems reading the code, partly due to lack of physical understanding and a great deal especially due to the numerous templates and the fact that I am still too much of a beginner. Fight is going on.)


Does this mean that, if I set inlet and outlet to cyclic and activate the momentum source, the flow will not die down and finally (depending on the initial flow field) transit to turbulent flow (because of numerical instabilities)?
I read that it is possible with postChannel to extract these different values (in case of a transient simulation): txx, txy,tyy, txy, eps, prod, vorticity, enstrophy, helicity

I see in the code (calculateFields.H) that txx =sqrt(Txx - (UMeanx*UMeanx))
Is UMean the time-averaged volume field of U? I can't figure out the meanding of Txx
Is txx a statistical moment???

If I create some other perturbations source (U + U') as an inlet boundary condition can I then disclaim the cyclic inlet and outlet boundary conditions? Or is that idea unrealistic because of the demanded channel length (and the necessary number of cells)?

I hope that I did not write to many different questions in this post .


Your answers have already helped really much to improve (at least) my understanding!
Thanks a lot!

Aylalisa

[alexeym]

Hi,

1. About fvOptions. If you compare channelFoam source code with pressureGradientExplicitSource source code:

channelFoam.C:

        // Correct driving force for a constant mass flow rate
            
        // Extract the velocity in the flow direction
        dimensionedScalar magUbarStar =
            (flowDirection & U)().weightedAverage(mesh.V());
    
        // Calculate the pressure gradient increment needed to
        // adjust the average flow-rate to the correct value
        dimensionedScalar gragPplus =
            (magUbar - magUbarStar)/rUA.weightedAverage(mesh.V());

        U += flowDirection*rUA*gragPplus;

        gradP += gragPplus;

pressureGradientExplicitSource.C (correct method)

    const scalarField& rAU = invAPtr_().internalField();

    // Integrate flow variables over cell set
    scalar magUbarAve = 0.0;
    scalar rAUave = 0.0;
    const scalarField& cv = mesh_.V();
    forAll(cells_, i)
    {
        label cellI = cells_[i];
        scalar volCell = cv[cellI];
        magUbarAve += (flowDir_ & U[cellI])*volCell;
        rAUave += rAU[cellI]*volCell;
    }

    // Collect across all processors
    reduce(magUbarAve, sumOp<scalar>());
    reduce(rAUave, sumOp<scalar>());

    // Volume averages
    magUbarAve /= V_;
    rAUave /= V_;

    // Calculate the pressure gradient increment needed to adjust the average
    // flow-rate to the desired value
    dGradP_ = (mag(Ubar_) - magUbarAve)/rAUave;

    // Apply correction to velocity field
    forAll(cells_, i)
    {
        label cellI = cells_[i];
        U[cellI] += flowDir_*rAU[cellI]*dGradP_;
    }
        
    scalar gradP = gradP0_ + dGradP_;

As you can see, they do more-or-less the same. The difference is mainly due to the fact that code from channelFoam is used outside PISO loop, while fvOptions correct method is called inside PIMPLE loop.

2. About calculateFields.H. Well, in fact all the code in this header is commented out, so it is not used in the utility.

3. It depends on the method you'll be using to create perturbations. AFAIK people successfully use cyclic BCs for LES simulations.

[aylalisa]

Hi Alexey,

is it necessary for that 'pressure correction' to be done inside the PIMPLE loop?

The code in calculateFields.H is commented out, but how can I extract the values txx, tyy etc.? Why is it not active anymore?

Do cyclic BCs finally (after enough flows through time) produce turbulence (due to numerical instabilities)with self-similar behaviour?
I've found different methods to create self-similar turbulence, based on superimposing the velocity field with a fluctuation field. Does this proceeding speed up the desired turbulent velocity field?

Best regards,
Aylalisa

[alexeym]

Hi,

1. This way it is implemented in pimpleFoam

        while (pimple.loop())
        {
            #include "UEqn.H"
    
            // --- Pressure corrector loop
            while (pimple.correct())
            {
                #include "pEqn.H"
            }
    
            if (pimple.turbCorr())
            {
                turbulence->correct();
            }
        }

and in the end of pEqn.H

U = HbyA - rAU*fvc::grad(p);
U.correctBoundaryConditions();
fvOptions.correct(U);

Surely you can use fvOptions outside of PIMPLE loop but it will be another solver.

2. I don't know why it's not active. Currently with postChannel you can extract graphs of these values:

    makeGraph(y, UMeanXvalues, "Uf", path, gFormat);
    makeGraph(y, urmsValues, "u", path, gFormat);
    makeGraph(y, vrmsValues, "v", path, gFormat);
    makeGraph(y, wrmsValues, "w", path, gFormat);
    makeGraph(y, RxyValues, "uv", path, gFormat);
    makeGraph(y, kValues, "k", path, gFormat);

    makeGraph(y, pPrime2MeanValues, "pPrime2Mean", path, gFormat);

And I guess old names Txx, Tyy etc are now Rxx, Ryy etc.

3. Yes, it is possible. Sure if you impose right fluctuations (not just white noise), it will speed up generation of the final flow field.

[Alish1984]

Hi Brunoand others

I have some questions that couldnt find a clear answer to them after reading almost all the stuffs about channel or pipe simulation

1. In channelFoam tutorial, what are the contents of the 0 file? how are they produced? are they from a long time run of the simulation without any perturbed initial condition?

2. what is Ubar or magUbar in channelFoam source? I read the source and I guess that it is averaged velocity over entire volume. then what does it mean? if it was averaged velocity over a cross area then ok, it makes sense. but why does channelFoam tend to meet such a weird condition?

3. I compared results of a channel395 case solving by the pisoFoam and channelFoam for some different conditions
a) channelFoam with initial conditions in 0.org file: no turbulence
b) channelFoam without cyclic BC (turbulentInlet velocity replaced) with IC in 0 file (perturbed IC): turbulence decays

c) pisoFoam with initial conditions in 0.org file without cyclic BC (turbulentInlet velocity replaced): no turbulence
d) pisoFoam without cyclic BC (turbulentInlet velocity replaced) with IC in 0 file (perturbed IC): turbulence decays

then I have this question, it seems that these are cyclic BC and perturbed initial condition both that run the turbulence, is it right?
if it is right then what can we do if we dont want to use cyclic BC in a case?

[wyldckat]

Greetings to all!

@Ali: I've had your post in my to-do list for some time now and I finally managed to look into this today:

Originally Posted by Alish1984

1. In channelFoam tutorial, what are the contents of the 0 file? how are they produced? are they from a long time run of the simulation without any perturbed initial condition?

Possibly used a utility similar to PerturbU: http://www.cfd-online.com/Forums/ope...-perturbu.html - more specifically, the one on this post: http://www.cfd-online.com/Forums/ope...tml#post187619 post #34
Coincidentally, someone else also named Ali asked a similar question back in 2005 and got this answer: http://www.cfd-online.com/Forums/ope...tml#post187629 post #44

Originally Posted by Alish1984

2. what is Ubar or magUbar in channelFoam source? I read the source and I guess that it is averaged velocity over entire volume. then what does it mean? if it was averaged velocity over a cross area then ok, it makes sense. but why does channelFoam tend to meet such a weird condition?

In OpenFOAM 2.1.x, file applications/solvers/incompressible/channelFoam/readTransportProperties.H
has this code:

    //  Read centerline velocity for channel simulations
    dimensionedVector Ubar
    (
        transportProperties.lookup("Ubar")
    );

    dimensionedScalar magUbar = mag(Ubar);
    vector flowDirection = (Ubar/magUbar).value();

Therefore, "Ubar" is the "centerline velocity for channel simulations". The likely reason: if a channel was filled with a fluid going at laminar flow speeds, almost the whole flow speed would be identical; if it's in the turbulent regime, then the speed at the centerline should be the on average similar to the laminar speed... for example, similar to a parabolic flow profile.

Originally Posted by Alish1984

3. I compared results of a channel395 case solving by the pisoFoam and channelFoam for some different conditions
a) channelFoam with initial conditions in 0.org file: no turbulence
b) channelFoam without cyclic BC (turbulentInlet velocity replaced) with IC in 0 file (perturbed IC): turbulence decays

c) pisoFoam with initial conditions in 0.org file without cyclic BC (turbulentInlet velocity replaced): no turbulence
d) pisoFoam without cyclic BC (turbulentInlet velocity replaced) with IC in 0 file (perturbed IC): turbulence decays

then I have this question, it seems that these are cyclic BC and perturbed initial condition both that run the turbulence, is it right?
if it is right then what can we do if we dont want to use cyclic BC in a case?

I think I found a paper a few minutes ago that state that pimpleFoam or channelFoam modified to use PIMPLE would give the best results... ah, it's this one: http://congress.cimne.com/eccomas/cf...pers/01454.pdf
Just in case the link gets broken in the future, the paper specifics:

• OPENFOAM SIMULATION OF MASS TRANSFER IN SPACER-FILLED CHANNELS
• José L.C. Santos, João G. Crespo, Vítor Geraldes
• V European Conference on Computational Fluid Dynamics, ECCOMAS CFD 2010

As for the tests and questions you made on this point:

1. cyclic BCs were used with an initial field value, because it's trying to quickly simulate how a section of fluid inside a channel would behave. For example, if the channel is as big as 10km by 500m, and you only want to study how 100m x 100m section of fluid behaves over a period of time, it's not necessary to mesh the whole channel of 10km by 500m, it's just a matter of meshing only the 100m by 100m and using cyclic BCs.
2. I'm not sure I understood your 2 questions. I say this because if I understood you correctly, it seems you have not tried/studied any other tutorial example in OpenFOAM's "tutorials" folder, which many exemplify how to set-up and use turbulence modelling. Perhaps you can detail a bit more what you're asking?

Best regards,
Bruno