CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

DNS with openfoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2009, 17:07
Default
  #21
Member
 
Eelco Gehring
Join Date: Mar 2009
Posts: 70
Rep Power: 9
feijooos is on a distinguished road
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
feijooos is offline   Reply With Quote

Old   November 18, 2009, 17:25
Default
  #22
Member
 
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 9
zebu83 is on a distinguished road
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 is offline   Reply With Quote

Old   November 19, 2009, 10:31
Default
  #23
Member
 
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 9
zebu83 is on a distinguished road
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
zebu83 is offline   Reply With Quote

Old   November 19, 2009, 12:00
Default
  #24
Member
 
Eelco Gehring
Join Date: Mar 2009
Posts: 70
Rep Power: 9
feijooos is on a distinguished road
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 is offline   Reply With Quote

Old   November 19, 2009, 12:12
Default
  #25
Member
 
Eelco Gehring
Join Date: Mar 2009
Posts: 70
Rep Power: 9
feijooos is on a distinguished road
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.

feijooos is offline   Reply With Quote

Old   January 20, 2011, 19:42
Default DNS and 1D spectra
  #26
Member
 
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 8
aldo.iannetti is on a distinguished road
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
Attached Images
File Type: jpg Spectra.jpg (26.1 KB, 90 views)
aldo.iannetti is offline   Reply With Quote

Old   January 27, 2011, 10:53
Default
  #27
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 8
stevenvanharen is on a distinguished road
Hi Aldo,

Is this spectrum in space or time?

And what discretization do u use for the convective term?

Regards,

Steven
stevenvanharen is offline   Reply With Quote

Old   January 27, 2011, 16:21
Default
  #28
Member
 
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 8
aldo.iannetti is on a distinguished road
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



Quote:
Originally Posted by stevenvanharen View Post
Hi Aldo,

Is this spectrum in space or time?

And what discretization do u use for the convective term?

Regards,

Steven
aldo.iannetti is offline   Reply With Quote

Old   January 27, 2011, 16:31
Default
  #29
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 8
stevenvanharen is on a distinguished road
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 is offline   Reply With Quote

Old   January 27, 2011, 16:41
Default
  #30
Member
 
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 8
aldo.iannetti is on a distinguished road
Yes, 300, full hex unstructured,
how to modify the fv schemes (for exemple)?



Quote:
Originally Posted by stevenvanharen View Post
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 is offline   Reply With Quote

Old   January 27, 2011, 16:58
Default
  #31
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 8
stevenvanharen is on a distinguished road
Just change:

Code:
div(phi,U)      Gauss linear;
into (for midPoint):

Code:
div(phi,U)      Gauss midPoint;
or (for 5 percent upwind):

Code:
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.
mgg likes this.
stevenvanharen is offline   Reply With Quote

Old   January 27, 2011, 17:10
Default
  #32
Member
 
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 8
aldo.iannetti is on a distinguished road
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





Quote:
Originally Posted by stevenvanharen View Post
Just change:

Code:
div(phi,U)      Gauss linear;
into (for midPoint):

Code:
div(phi,U)      Gauss midPoint;
or (for 5 percent upwind):

Code:
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 is offline   Reply With Quote

Old   January 28, 2011, 03:48
Default
  #33
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 8
stevenvanharen is on a distinguished road
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 is offline   Reply With Quote

Old   January 28, 2011, 03:56
Default
  #34
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 8
stevenvanharen is on a distinguished road
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.
Attached Images
File Type: jpg spectrum.jpg (14.4 KB, 91 views)
stevenvanharen is offline   Reply With Quote

Old   June 8, 2011, 03:29
Default
  #35
New Member
 
Join Date: Oct 2010
Posts: 24
Rep Power: 7
LijieNPIC is on a distinguished road
Quote:
Originally Posted by zebu83 View Post
I have some question about channel DNS simulation with OpenFOAM.

I found in another thread [Channel flow DNS 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.
LijieNPIC is offline   Reply With Quote

Old   September 28, 2011, 18:23
Default
  #36
Member
 
Yong Wang
Join Date: Apr 2009
Posts: 34
Rep Power: 9
ywang is on a distinguished road
Quote:
Originally Posted by LijieNPIC View Post
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.
ywang is offline   Reply With Quote

Old   September 29, 2011, 08:14
Default
  #37
Member
 
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 9
zebu83 is on a distinguished road
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
zebu83 is offline   Reply With Quote

Old   October 6, 2011, 18:47
Default
  #38
Member
 
Yong Wang
Join Date: Apr 2009
Posts: 34
Rep Power: 9
ywang is on a distinguished road
Quote:
Originally Posted by zebu83 View Post
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 is offline   Reply With Quote

Old   October 6, 2011, 21:53
Default
  #39
Member
 
Yong Wang
Join Date: Apr 2009
Posts: 34
Rep Power: 9
ywang is on a distinguished road
Quote:
Originally Posted by aldo.iannetti View Post
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.
ywang is offline   Reply With Quote

Old   October 11, 2011, 03:16
Default
  #40
Member
 
Marco Turchi
Join Date: Jul 2009
Location: Pesaro, Italy
Posts: 31
Rep Power: 9
zebu83 is on a distinguished road
Quote:
Originally Posted by ywang View Post
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
zebu83 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFoam vs CFX5 mass balance in OpenFoam tangd OpenFOAM Running, Solving & CFD 33 May 23, 2010 16:36
CheckMesh error using a tutorial from OpenFOAM 114 with openFOAM 13 martapajon OpenFOAM Native Meshers: blockMesh 7 January 21, 2008 13:52
OpenFOAM users in Munich OpenFOAM benutzer in M%c3%bcnchen jaswi OpenFOAM 0 August 3, 2007 13:11
A new Howto on the OpenFOAM Wiki Compiling OpenFOAM under Unix mbeaudoin OpenFOAM Installation 2 April 28, 2006 08:54
Is GUI there for OpenFoam navaladi OpenFOAM 3 March 28, 2006 09:08


All times are GMT -4. The time now is 11:52.