[feijooos]

Marco, one of my cases has 4 million mesh point. This one is going to take another 2 days. But I should have some results up from some other cases soon.

btw, just to be sure....what are your values for Ubar and nu?

Thanks, Eelco

[zebu83]

My Ubar is the same of "channelOodles" tutorial: Ubar = 0.1335, but I modify nu, I chose nu = 2*10^-5 to have Retau more or less = 180.

The previous pictures are adimensionalized with Retau or Utau, etc. so the results are generic.

Best regards

MT

[zebu83]

Sorry, Eelco, could you post the set of your test case?

In my simulation I use:
dimension (x*y*z): 3.5*2*2
number of cells (nz*ny*nz): 80*180*120

that means, for Retau = 200 (I use Ubar=0.1335, nu=2*10^-5), these adimensional units (x+, y+, z+): 8.75, *, 3.33 [*: means that I have a simple grading in y direction that is 10, so the dimension of the cell in the middle of the channel is 10 time the dimension of the boundary cell, so the range of y+={0.44 - 4.44} more or less].

If I well understand the set of your test case, your situation is more or less this:
dimension (x*y*z): 2pi*1*pi
number of cell (nz*ny*nz): 196*129*160

and if you have a Retau = 400 (that is more or less the same of channelOodles tutorial), you have these adimensional units (x+, y+, z+): 12.81, ?, 7.85 (?: means that I don't know if you put some grading).

I can't use more cell because I have not more computational resource.

bye

MT

[feijooos]

Marco, one of my cases just finished. They are taking longer than I thought. I checked my Retau and it is around 195, a little too high. I want to compare against the paper from Kim (1987) and he uses Retau equal to 180. I have to do some postprocessing now to see how it turned out. I will let you know.

[feijooos]

Marco,

I have the velocity profile, u+ vs. y+ and the results are not good. I think I am missing something..... This profile is not with the fine mesh yet, this is with 96x129x80.

[aldo.iannetti]

Hi All,
Here attached a 1D assial spectra coming from a DNS symulation of a pipe using OF 1.6. Focus your attention on the higher wavenumbers. Is there anyone who knows the meaning of that strange behaviour?
It seems there are some components caracterized by the high wavenumber that do not dissipate.
Please post whatever you think in order to let the investigations go on.

Let me know if something else is needed to understand

[stevenvanharen]

Hi Aldo,

Is this spectrum in space or time?

And what discretization do u use for the convective term?

Regards,

Steven

[aldo.iannetti]

Hi,
It is in space, I used the Gauss linear that I hope corresponds to the CDS schemes, here attached the fvSchemes dict.
Thanks
Aldo

Originally Posted by stevenvanharen

Hi Aldo,

Is this spectrum in space or time?

And what discretization do u use for the convective term?

Regards,

Steven

[stevenvanharen]

ok,

Did you use nyquist's criterion to determine the highest wavelength that you can represent on your mesh? How many cells do you have in the direction you took the spectrum?

If your answer is to the first question is yes and to the second question is at least 200 you can start looking at your schemes.

Do you use a full hex mesh? Do you use stretching? How much? If you use stretching and/or unstructered grids you can try either midPoint CDS or blended.

Steven

[aldo.iannetti]

Yes, 300, full hex unstructured,
how to modify the fv schemes (for exemple)?

Originally Posted by stevenvanharen

ok,

Did you use nyquist's criterion to determine the highest wavelength that you can represent on your mesh? How many cells do you have in the direction you took the spectrum?

If your answer is to the first question is yes and to the second question is at least 200 you can start looking at your schemes.

Do you use a full hex mesh? Do you use stretching? How much? If you use stretching and/or unstructered grids you can try either midPoint CDS or blended.

Steven

[stevenvanharen]

Just change:

div(phi,U)      Gauss linear;

into (for midPoint):

div(phi,U)      Gauss midPoint;

or (for 5 percent upwind):

div(phi,U)      Gauss blended 0.95;

midPoint is kinetic energy conservative on meshes with stretched cells, whereas linear is not (leading to instabilities)

blended supresses instabilities by using a small bit of upwind

A question about physics: What is the smallest wavelength you expect based on your Reynold number and Kolmogorov theory? If your Reynolds number is really low there just might be no smaller eddies.

[aldo.iannetti]

Re_tao=200, Re=5500 I think is not due to the cell shape because I see the same behaviour in a similar simulation of a channel with perfect cells.
is midpoint useful for a perfect channel cells? (I've never used it)
Blending with Upwind will introduce diffusivity....
Aldo

Originally Posted by stevenvanharen

Just change:

div(phi,U)      Gauss linear;

into (for midPoint):

div(phi,U)      Gauss midPoint;

or (for 5 percent upwind):

div(phi,U)      Gauss blended 0.95;

midPoint is kinetic energy conservative on meshes with stretched cells, whereas linear is not (leading to instabilities)

blended supresses instabilities by using a small bit of upwind

A question about physics: What is the smallest wavelength you expect based on your Reynold number and Kolmogorov theory? If your Reynolds number is really low there just might be no smaller eddies.

[stevenvanharen]

midPoint will be exactly the same as linear if you use cells without stretching

blended will indeed introduce diffusion

I use sometimes either of these for DNS but that is on unstructured grids
(polyhedral cells).

Based on your Reynolds number you would expect physics at these wavelengths. What I find strange is that you have already dropped 6 orders of magnitude before the strange behavior in the at the high wavelengths start. Imagine where you would end up if the energy would keep dropping after say k = 45?

About your mesh, how did you mesh a pipe with perfect hex cells? And where did you extract the spectrum? In the center of at the wall?

[stevenvanharen]

This is one of my spectra for a DNS of a channel flow at Re_tau = 180.
Spectra extracted over the plane in the center of the channel.

As you can see my mesh is 128 cells in streamwise direction so I have less information than you. Drop in magnitude almost the same.

[LijieNPIC]

Originally Posted by zebu83

I have some question about channel DNS simulation with OpenFOAM.

I found in another thread [http://www.cfd-online.com/Forums/ope...flow-dns.html] channelDNS program (that Alberto post long time ago), I compiled it and it work perfectly!
Then I created a new directory (channelDNS) and in this directory I run my simulation of a channel with this parameter:
L*H*W: 3.5*2*1
nx*ny*nz: 80*130*60
nu=4*10-5 (to have a Re_tau=180 more or less)

I use:

that is like fvSchemes of boxTurb tutorial, except of temporal schemes (CrankNicholson 0.5 instead of euler).

When I visualized the results I notice that in the middle of the channel there are some strange bubble, but they don't come from the wall streaks!

This cause a bed Umean and u_rms profile.

Where/what are the errors?
Probably interpolation schemes or resolution?

Thank you very much in advance.

Best regard
MT

Hello, Marco, can you post the channel DNS code in the forum again, I cannot download it. Thank you very much.

[ywang]

Originally Posted by LijieNPIC

Hello, Marco, can you post the channel DNS code in the forum again, I cannot download it. Thank you very much.

It's strange,,,I can download it.

[zebu83]

Lijie here this is the link to the file that I wrote about:
http://www.cfd-online.com/OpenFOAM_D...S_tar-3861.unk

I'm sorry for the late.

MT

[ywang]

Originally Posted by zebu83

Lijie here this is the link to the file that I wrote about:
http://www.cfd-online.com/OpenFOAM_D...S_tar-3861.unk

I'm sorry for the late.

MT

Marco, have you ever tried to use some other div schemes?

I am using my own solver in the frame of OpenFOAM. The size of the channel is 4pi*2*(4pi/3), and the mesh is 128*128*128 (uniform in the x and z directions, simpleGrading=10 in the y direction).

My solver will crash when I use linear and midpoint as the div scheme. So, I am using Gamma0.1 and the solver works. Based on Jasak's paper about Gamma scheme, it should be similar with the central(linear) scheme. However, the velocity in the sublayer is smaller than Moser's DNS results. That means more dissipation has been introduced.....

[ywang]

Originally Posted by aldo.iannetti

Re_tao=200, Re=5500 I think is not due to the cell shape because I see the same behaviour in a similar simulation of a channel with perfect cells.
is midpoint useful for a perfect channel cells? (I've never used it)
Blending with Upwind will introduce diffusivity....
Aldo

Steven, I am simulating the turb channel flow with Re_tau=180. I found your master thesis

My solver will crash with linear/midpoint.....but works with blended0.995. hope I can get good result with it.

[zebu83]

Originally Posted by ywang

Marco, have you ever tried to use some other div schemes?

I am using my own solver in the frame of OpenFOAM. The size of the channel is 4pi*2*(4pi/3), and the mesh is 128*128*128 (uniform in the x and z directions, simpleGrading=10 in the y direction).

My solver will crash when I use linear and midpoint as the div scheme. So, I am using Gamma0.1 and the solver works. Based on Jasak's paper about Gamma scheme, it should be similar with the central(linear) scheme. However, the velocity in the sublayer is smaller than Moser's DNS results. That means more dissipation has been introduced.....

Hi Ywang,
my set case was: 3,5h*2h*2h; mesh: 80*180*120 (like you uniform the in x and the z direction, simpleGrading = 10 in the y direction); Re_tau=200 (more or less).

I changed "fvSchemes" like this:
ddtShemes: Euler;
gradSchemes: Gauss linear (for all)
divSchemes: default-none / div(phi,U)-Gauss cubic
laplacianSchemes: default-none / laplacian(nu,U)-Gauss linear corrected / laplacian((1|a(U)),p)-Gauss linear corrected

I hope this is useful.

Marco