[cedric_duprat]

Hi Errico,

have a look on the channelFoam tutorials. That's a good starting point.

OpenFOAM-2.1.x / tutorials / incompressible / channelFoam / channel395 /

Then, this forum page should be interesting too.

Cédric

[turbfoam]

dear cedric,

I read posts in this thread and I facing problems in convergence. It would be nice if you give tips on the fvSchemes and fvSolutions settings for cases involving flow separation like backward facing step, periodic hill etc.

I use periodic BCs for inflow/outflow and spanwise boundaries. my fvSchemes and fvSolutions settings are same to channel395 tutorial, and use smagorinsky model,vanDriest damping with default coefficient.but my simulation residual diverge after few hundred iters. time step is sufficiently less.

Any idea you can give? As to the schemes which can use for cases having separated flow ?

thanking you...

[cedric_duprat]

Dear j.t.

I used a quite old version of OF for these calculations. Details of my numerics can be found on a previous message (July 30, 2008, 11:17)

I did a periodic hill calculation with the same numerics without any problems. Could you give me more details of your case:

What's your configuration? your mesh ? and you initial fields ?

Cédric

[turbfoam]

Originally Posted by cedric_duprat

Dear j.t.

I used a quite old version of OF for these calculations. Details of my numerics can be found on a previous message (July 30, 2008, 11:17)

I did a periodic hill calculation with the same numerics without any problems. Could you give me more details of your case:

What's your configuration? your mesh ? and you initial fields ?

Cédric

dear Cedric,
I read ur previous post.
I want to simulate periodic hill and backward facing step flow. first, im focus on periodic hill., OF 2.1., channelFoam solver.
My mesh is the same as used by Temmerman et. al. in "Highly resolved large-eddy simulation of separated flow in a channel with streamwise periodic constrictions",2004. Its 198 X 128 X 186 cells, and 4.7 million cells total. I'm want to reproduce their results, atleast get reasonable flow field converged solution.

I have attached initial fields "0" folder. (in .zip)

below is LES properties file.I use Euler backward time stepping.nOrthoCorrector=2.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      LESProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

LESModel        Smagorinsky;

delta           vanDriest;

printCoeffs     on;

SmagorinskyCoeffs
{
    ce               1.05;
    ck               0.07;
}


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;
}

Problem is residual diverge after few hundred iters.I also tried much smaller time step,Smag model + cuberootvol delta,smoothdelta etc. but same result.

I calculate yplus value of bottom wall by yplusLES utility, and it shows very high yplus values. Im sure grid is good, so problem is with 'U', I think due to gradients in flow separation. Where am I making mistake?

Thanks very much for interest and help.

[cedric_duprat]

Dear j.t.,

I think your initial field is too far from reality. Uniform velocity is not enough to run a LES calculation. Even if your calculation is running, you will spend days to get converged statistics.

You should improve your initial condition. First, run on a coarse grid (very coarse), and use perturbU tool to initialize the velocity field. When you get a turbulent flows, even if it is not physically correct, use mapField tool to initialise your fine grid quantities.

I think this will help you.

If you have more questions, create a new thread, to keep this one on channel flow calculation only.

Cédric

[turbfoam]

dear Cedric,

I understand the meaning. The flow is not very turbulent enough to be used for LES or any turbulence modeling technique. I will do the same, and will create new thread if I need help.

Thanks so much for your help.

J.T.

[pedroxramos]

Hello...!

I'm a newbie in OF... ANy of you have a tutorial/example for LES open channel?

I want to simulate a open channel flow around a pille to study the scour around it.

Best regards.
Pedro.

[pedroxramos]

Hi!

I'm doing the open channel flow simulation around a pile (LES) and I find an error in the inlet section (too much velocity) wich causes a increment of pressure in the bed of the channel (right up corner of the image: http://d.pr/i/vIcS)

See the video also: http://www.youtube.com/watch?v=G_dtwb8JFD0

Any tips?

[raw17]

Hello
I am to run channel flow with dynSmagorinsky(channel395), but my statistics are not in good agreement with Moser DNS(Retau=395)
Dimesion of my domain is : 4*2*2,80*50*60
I generate initial condition using perturbU utility and run the simulation for long time . After the initial peaks in turbulent kinetic energy the energy fluctuates around a value. After that I run a long simulation and perform average.
using post channel utility
1. vrms , wrms are underestimated.
2. urms is overestimated .
3. Umean is also not matching far from the wall.

the schemes of my channel:


ddtSchemes
{
default backward;
}

gradSchemes
{
default Gauss linear;
grad Gauss linear;
grad Gauss linear;
}

divSchemes
{
default none;
div(phi,U) Gauss linear;
div(phi,k) Gauss limitedLinear 1;
div(phi,B) Gauss limitedLinear 1;
div Gauss linear;
div(phi,nuTilda) Gauss limitedLinear 1;
div((nuEff*dev(grad .T()))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A ),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DBEff,B) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

I use delta cubeRootVol; Same issue I have with static Smagorinsky model also.
Please see my results

Thankyou
Subhendu

[wzx1989221]

Dear Cedric,

I find your posts on LES channel flow very useful. Just one question, how did you deal with the data, in other words, how did you perform the field averaging like getting mean velocity profile and rms plots?

It would be great if you can give me some hints on that. Thank you very much.

Best regards,
Tony

[Arne87]

Hi,

im trying to simulate the Moser channel with LES Turbulence Modelling.
Im using a university code .
Its possible to define a pressure gradient to generate a flow in the channel.
Im trying to implement a dynamic pressure gradient to define a fixed mass flow
through the channel, as Moser et al. and others did.
Atm im using a function

delta_pressure_gradient = (u_soll - uist ) / 10.

Where delta_pressure_gradient is the change in pressure gradient.
u_soll is the velocity calculated by the mass flow of the DNS data and
u_ist the current velocity averaged in space (over the whole channel) and
in time over 1000 time steps.

My problem is that this pressure gradient adjustment need a lot of time unil it
get into some kind of stationary status.

Does anybody know a better function to calculate the pressure gradient for the next time steps ?


Arne

[huangxianbei]

Originally Posted by nzy102

The initial condition of flow was obtained using perturbU.
Ning

Hi:
By the way, I'd like to ask a question about the initial fileds. Yes, perturbU is the best utility to generate a velocity filed, while how about the other fields such as p, nusgs? As we can see from channel395 tutorial, the 0 folder contains 6 files of the initial fields which are all nonuniform list values. How can we generate as these?

Huang Xianbei

[huangxianbei]

Originally Posted by nzy102

I calculated utau based on mean pressure gradient. The utau based on 200 flow through times is 0.0073. The actual value is 0.0079

Ning

Hi, Ning:
I have the same problem as you posted here. Whether the geometry is changed or not , the u_tau is underestimated through the whole calculation, I think it's due to the gradP adjustment during the calculation. However, as you mentioned, the u_tau=0.073 which is only 92.4% of the expected value. This will lead to a lower Re_tau. Have you ever found any solutions up to now?

Xianbei

[GiulioS]

I want to report a question concerned the U_bar used by OpenFoam in the channel flow tutorial, where:
U_bar=0.1335.
If you calculate the Reynolds number as well as Re=2δU_bar/ν you get Re=13350.
But if you want to compare the LES results with the DNS ones (computed at friction Reynolds number 395), as well as Pope suggested, the Reynolds number corresponding to the friction Reynolds number 395 is 13750, where
U_bar_new=0.1375.
That could be a cause of the misleading results.

[HanSolo123]

Hello OFers,

can someone give me a hint concerning the channel395 tutorial with the oneEqEddy LES-turbulence model?
When I run the tutorial without any changes, i get a totally wrong velocity profile. I use the postChannel utility for the latest Times (1000) to get U over y. It gives me the following 25 values due to the symmetry of the geometry with 50 element layers in y-direction:

0.00480001 0.00827117
0.0148983 0.023951
0.026045 0.0374098
0.0383488 0.047655
0.05193 0.0558505
0.066921 0.0635531
0.0834683 0.0714288
0.101734 0.0794559
0.121895 0.0875807
0.144149 0.095728
0.168714 0.103805
0.195829 0.111702
0.225758 0.119296
0.258795 0.126453
0.295262 0.133031
0.335514 0.138891
0.379945 0.143905
0.428988 0.147972
0.483123 0.151042
0.542878 0.153137
0.608836 0.154375
0.681641 0.154972
0.762005 0.155195
0.850711 0.155256
0.948626 0.155269

Then I want to calculate ReTau, which should be around 395, but I only recieve 293.
What I do:

dU/dy @ y=0 : 0,00827117/0,00480001 = 1,72312 which sould be 3,1205
uTau = sqrt(2E-5* 1,72312) = 0,00587 which should be 0,0079
ReTau = uTau/2E-5 = 293 which should be 395

With these wrong values, the dimensionless velocity profile uPlus over yPlus is wrong indeed.
I already refined the mesh, i also tried different SGS Model, but without improvement.
I doubt my calculation of dU/dy is wrong, but I have clue why it is so atm. Probably its just a stupid mistake but I cant find it. Hopefully someone can help me with this issue.

I am using OF2.3.0 with pimpleFoam solver and standard settings from the /tutorials/incompressible/pimpleFoam/channel395/ dict.

PS: in this thread it was mentioned to calculate uTau with the pressure gradient, but in my case it is zero from x=0 to x=4m. Dont know how I can handle with this information.

[GiulioS]

I think you have wrong to calculate du/dy. However, how many iterations have you done?

Originally Posted by HanSolo123

Hello OFers,

can someone give me a hint concerning the channel395 tutorial with the oneEqEddy LES-turbulence model?
When I run the tutorial without any changes, i get a totally wrong velocity profile. I use the postChannel utility for the latest Times (1000) to get U over y. It gives me the following 25 values due to the symmetry of the geometry with 50 element layers in y-direction:

0.00480001 0.00827117
0.0148983 0.023951
0.026045 0.0374098
0.0383488 0.047655
0.05193 0.0558505
0.066921 0.0635531
0.0834683 0.0714288
0.101734 0.0794559
0.121895 0.0875807
0.144149 0.095728
0.168714 0.103805
0.195829 0.111702
0.225758 0.119296
0.258795 0.126453
0.295262 0.133031
0.335514 0.138891
0.379945 0.143905
0.428988 0.147972
0.483123 0.151042
0.542878 0.153137
0.608836 0.154375
0.681641 0.154972
0.762005 0.155195
0.850711 0.155256
0.948626 0.155269

Then I want to calculate ReTau, which should be around 395, but I only recieve 293.
What I do:

dU/dy @ y=0 : 0,00827117/0,00480001 = 1,72312 which sould be 3,1205
uTau = sqrt(2E-5* 1,72312) = 0,00587 which should be 0,0079
ReTau = uTau/2E-5 = 293 which should be 395

With these wrong values, the dimensionless velocity profile uPlus over yPlus is wrong indeed.
I already refined the mesh, i also tried different SGS Model, but without improvement.
I doubt my calculation of dU/dy is wrong, but I have clue why it is so atm. Probably its just a stupid mistake but I cant find it. Hopefully someone can help me with this issue.

I am using OF2.3.0 with pimpleFoam solver and standard settings from the /tutorials/incompressible/pimpleFoam/channel395/ dict.

PS: in this thread it was mentioned to calculate uTau with the pressure gradient, but in my case it is zero from x=0 to x=4m. Dont know how I can handle with this information.

[tiam]

Dear Foamers, I'm also doing some channel flow computations, using the DNS data from Moser et al as reference. I am currently trying to compare the two-point correlations and I can't figure out how they are scaled in the DNS data.

I mean, the correlations are already normalized by definition, so why the need for a new scale? It says in the files that it is scaled by U_tau and h, but I can't figure out how . Maybe those that worked with this data could give me a hint?

[tiam]

Originally Posted by GiulioS

I want to report a question concerned the U_bar used by OpenFoam in the channel flow tutorial, where:
U_bar=0.1335.
If you calculate the Reynolds number as well as Re=2δU_bar/ν you get Re=13350.
But if you want to compare the LES results with the DNS ones (computed at friction Reynolds number 395), as well as Pope suggested, the Reynolds number corresponding to the friction Reynolds number 395 is 13750, where
U_bar_new=0.1375.
That could be a cause of the misleading results.

Yes, I have been wondering about this too..

[killsecond]

Originally Posted by lakeat

from my post " June 16, 2009, 03:26", you will see how to get wallshearstress;
then I do an average of wallshearstress;
then sqrt(wallshearstress);

Hi, Daniel
How did you do the average of wallshearstress?

[infinity]

Hi
Im trying to validate results for One-Equation LES model and I also used MapField utility for grid study purpose but getting unacceptable results after mapping. How should I initialize the flow to get correct answers in channel flow case?