[mxylondon]

Dear all,
I am struggling with a trouble in pisoFoam using LES for channel flow.

Basically, the velocity curve from experiment has the maximum value of about 1.15 times of inlet uniform velocity, yeah?

But I got much larger max value like 1.4 times of inlet uniform velocity, and it changes sharply from wall to centre.

My question is, what parameters I may make wrong, or anything I can do to develop that?

P.S.
I am using oneEqEddy model. OF version 2.2.0.


Cheers

[itchy]

Hi,

that sounds like to coarse mesh. Which LES Model do you use??? Is your case really turbulent in the LES simulation. Is your case statistically stationary. Have you checked this??

kind regards
Florian

[m.goudarzi]

hi

I have the same problem but with pimple solver. I used oneEqEddy of LES model, and used mapped inlet Method, but the maximum velocity is 1.4 that exceed the experimental data.
yplus of mesh is under 1 and about 162,000 node
please help me ,I am confused

[itchy]

hi m.goudarzi,

do you use Van Driest damping??? The OneEqModel behaves wrong at the wall. You have to use van Driest damping!! Or you can use dynOneEq (without Van Driest damping!), but there is a bug in this model

Is your domain long enough??? Your domain has to be twice the longest turbulent structures (Nyquist criteria) i.e. in a pipe the largest turbulent structures is about 6-7 times the pipe diameter, this leads to a length of your domain of 16 times the diameter.

Is your averaging time long enough?? How have you checked that??

Is your flow statistically statinoary before you start averaging?? How have you checked that?

kind regards
Florian

[m.goudarzi]

Hi dear Florian

Thank you for the quick reply

do you use Van Driest damping??? The OneEqModel behaves wrong at the wall. You have to use van Driest damping!! Or you can use dynOneEq (without Van Driest damping!), but there is a bug in this model

yes! i used " delta vanDriest" in LES properties

Is your domain long enough??? Your domain has to be twice the longest turbulent structures (Nyquist criteria) i.e. in a pipe the largest turbulent structures is about 6-7 times the pipe diameter, this leads to a length of your domain of 16 times the diameter.

I have a channel with 3.33 cm aspect ratio. the length of channel is 20 cm.

Is your averaging time long enough?? How have you checked that??

Is your flow statistically statinoary before you start averaging?? How have you checked that?

I am new user of openfoam, excuse me for this simple question. I dont know about these object, can you explain more?

Thank you
marzieh

[m.goudarzi]

This is my LES properties

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object LESProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

LESModel oneEqEddy;

printCoeffs on;

delta vanDriest;

cubeRootVolCoeffs
{
deltaCoeff 1;
}

PrandtlCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}

Cdelta 0.158;
}

vanDriestCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}

Aplus 26;
Cdelta 0.158;
}

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}

maxDeltaRatio 1.1;
}


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

[itchy]

Hi,

how do you simulate the channel???

I would do it like this:

1. Use pimpleFoam (no relaxation in final iteration, do residualControl with very low values!)
2. use fvOptions with pressureGradientExplicitSource (no mapping method!)
3. initialize your flow with isotropic turbulence (boxTurb) and superimpose a powerlaw profile
4. For LES use Gauss linear (no Upwind!!), corrected (or orthogonal for channel) and backward (ddt)
6. Lets say flowdirection is z and the heigth of the channel is h. As a result of the turbulence structures, the domain has to be: Lz=12h, Lx=4h, Ly=h
7. Run your simulation for 100 flow through domain and then start averaging. (How to average see tutorial channel95)
8. Include a model for your subgrid-stress tensor Tsgs in the oneEq. You need an averaged Tsgs for postprocessing.

How to compare LES data with DNS data:
With LES you simulate a filtered velocity field. The mean value of a filtered signal is equal with the mean value of the unfiltered signal. So you can compare a mean value from a LES with a mean value of a DNS.
This is not true for the RMS value. The RMS value of a LES is smaller then the RMS value of the DNS. To compare this, you have to add the mean subgrid stress tensor TSgs to the covariance matrix of the LES.

Averaging time:
The random error Err of the average depends on the integral time scale Tint. In example, for the mean your random errror is proprtinal:
Err ~ sqrt(2*Tint/tav)
where tav is your averaging time. Tint is a function of space and is much higher near the wall. As a result of this, you have to average much longer at the wall.

You should do a reference simulation with Smagorinsky model. For channel use Smagorinsky parameter Cs=0.05.

kind regards
Florian

[mdallali]

Hi everyone, I model a curved channel with N-S equation in curvilinear coordinates.
I imposed a fix pressure gradient in x- direction which decomposed along the channel in curvilinear coordinate( stream wise and span wise direction) to drive the flow.
So the pressure gradient alter in steam wise and span wise direction along the channel .
But my solution is not stable.
so i Think it s because of unbalance between the body forces.
Does some one has any idea?
Should I use a fixed pressure gradient in stream wise while imposing the centrifugal force as well?

[Gizazu]

Hi everybody, i´ḿ new to openFoam and i´m trying to run pisoFoam for a channel with a pier inside. I received an error (see image) and from that i tried to change somethings in my boundary conditions but still giving the same error.

So, please I need your help to find out what is going wrong, where is my failure and how can I do it right.

it is attached some files (blockMeshDict, U, p, epsilon).

help please.

Kind regards

Gizela

[m.goudarzi]

Hi,

Thank you very much Florian for your answer
I have done all these steps, but the result did not change
I do not know where is the problem