CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Verification & Validation

Validation: Turbulent Channel Flow, pisoFoam, LES

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

Like Tree4Likes
  • 1 Post By Xiaoyu Yang
  • 1 Post By Xiaoyu Yang
  • 1 Post By Xiaoyu Yang
  • 1 Post By Elyas_Mosibat

Reply
 
LinkBack Thread Tools Display Modes
Old   January 31, 2017, 00:21
Default Validation: Turbulent Channel Flow, pisoFoam, LES
  #1
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Dear All,

First of all, wish you all have a successful year in 2017! I am relatively new to this forum and to OpenFOAM and LES. Thanks for your suggestions in advance!

At the moment, I am trying to validate the code and the LES model via a fully developed incompressible turbulent channel case at Re_tau=180. The pisoFoam solver together with the dynamicKEqn LES model are used. Please I was wondering if anyone could give me some suggestions on how to choose a proper combination of numerical schemes. Instead of the default, I am seeking for higher order schemes for lower dissipation and better accuracy.

The geometry of this rectangular channel is (2\pi\delta, 2\delta, \pi\delta) in the (x, y, z) directions, respectively. For Re_tau=180, the Reynolds number based on the mean centreline velocity is Re_delta=3300, and the kinematic viscosity is scaled such that the half channel height is 1m and the mean centreline velocity is 1m/s. Accordingly, to drive the flow, a corresponding constant x-momentum source term is implemented as a dynamic code through fvOptions. In accordance with this case setup, the periodic boundary conditions (cyclic B.C.) are applied in both the streamwise and spanwise directions.

Comparison results of the mean velocity and the Reynolds stress with DNS (Moser, Kim, and Moin 1999) are attached. As can be seen, the numerical accuracy needs to be improved, and I am struggling with choosing a proper combination of numerical schemes for higher order accuracy. At the moment, the Crank Nicolson scheme with the coefficient 0.9 is used for time integration, and the Gauss cubic scheme is used for the gradient terms. Linear interpolation and Gauss linear corrected Laplacian terms are also used. The used fvSchemes, the fvSolution, and the turbulenceProperties files are also attached for clarity.

Particularly, if the Gauss cubic scheme is used for the divergence terms, the instantaneous flow structures show irregular discontinuities even though the solver could still run.

Besides, at this stage, my primary consideration is about the numerical schemes. To get more familiar with this flow solver, and to save time and get some quick answers, a coarse mesh is used for the current computation. The used grid density is about the half of the standard LES requirements in all the three directions, i.e. dx+=28, dz+=19, dy+_1st=0.36, and dy+_max=37. The noslip wall boundary condition is applied for the top and the bottom walls with the viscous sublayer resolved.

Currently, I am using OpenFOAM-v3.0+ version. It seems that the Crank Nicolson scheme is a good choice for time integration. However, when with the coefficient 1.0, this implementation of the code becomes unstable and the flow diverges. Therefore, I am using the coefficient 0.9. For spatial discretizations, generally, I am trying to find a fourth order combination, preferably with lower dissipation.

Please could anyone give me some suggestions for this.

Thanks for your time!

Xiaoyu
Attached Images
File Type: jpg Fig01_Umean_LogLaw.jpg (65.4 KB, 61 views)
File Type: jpg Fig02_Reynolds.jpg (60.1 KB, 41 views)
Attached Files
File Type: txt fvSchemes.txt (1.4 KB, 11 views)
File Type: txt fvSolution.txt (1.6 KB, 11 views)
File Type: txt turbulenceProperties.txt (1.9 KB, 10 views)
Xiaoyu Yang is offline   Reply With Quote

Old   February 8, 2017, 09:51
Default
  #2
Senior Member
 
ehsan
Join Date: Mar 2009
Posts: 109
Rep Power: 10
ehsan is on a distinguished road
Hello,

We have a similar problem, we tried cubic discretization for channel flow at Re_t=590. We used a relatively coarse grid but used a higher order discretization. The results lasted a lot and we did not get correct but underestimated solution. Would you please give any advice?
Regards
Attached Images
File Type: jpg Schemes.jpg (44.2 KB, 36 views)
ehsan is offline   Reply With Quote

Old   February 8, 2017, 22:28
Default
  #3
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Quote:
Originally Posted by ehsan View Post
Hello,

We have a similar problem, we tried cubic discretization for channel flow at Re_t=590. We used a relatively coarse grid but used a higher order discretization. The results lasted a lot and we did not get correct but underestimated solution. Would you please give any advice?
Regards
Hi Ehsan,

Good to know you are running similar simulations. For me, when the Gauss cubic scheme is used for div() terms, instantaneous flow structures show strange discontinuties. This looks like numerical disorders related to the schemes. Did you get this problem or not please? Do let me know if you get some progress.

Thanks in advance,

Xiaoyu
Xiaoyu Yang is offline   Reply With Quote

Old   February 9, 2017, 00:22
Default
  #4
Senior Member
 
ehsan
Join Date: Mar 2009
Posts: 109
Rep Power: 10
ehsan is on a distinguished road
Hello,

Thank you, no, we did not have this problem but our run time was really increased compared to the default setting of OpenFOAM. Another point: we used PIMPLEFoam solver for our simulation.

Best Regards
ehsan is offline   Reply With Quote

Old   February 9, 2017, 04:06
Default
  #5
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Quote:
Originally Posted by ehsan View Post
Hello,

Thank you, no, we did not have this problem but our run time was really increased compared to the default setting of OpenFOAM. Another point: we used PIMPLEFoam solver for our simulation.

Best Regards
Hi Ehsan,

Thanks for your suggestions. Let me try the pimpleFoam solver shortly.

At the moment, with a combination of the backward time integration and Gauss linear spatial discretizations, I am getting some improved results using a fine mesh (81 x 161 x 81). For this, the mean velocity profile and the Reynolds stresses are attached in the following.
Xiaoyu Yang is offline   Reply With Quote

Old   February 9, 2017, 04:24
Default
  #6
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

Total Reynolds Stress and Turbulence Energy Spectrum of LES

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu
Attached Files
File Type: pdf Fig01_Umean_LogLaw.pdf (28.0 KB, 24 views)
File Type: pdf Fig02_Reynolds.pdf (41.1 KB, 18 views)
Bashar likes this.
Xiaoyu Yang is offline   Reply With Quote

Old   February 28, 2017, 20:04
Default
  #7
Member
 
Bashar
Join Date: Jul 2015
Posts: 61
Rep Power: 3
Bashar is on a distinguished road
Quote:
Originally Posted by Xiaoyu Yang View Post
Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

Total Reynolds Stress and Turbulence Energy Spectrum of LES

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu
Hi,
So sorry to bother you ,but is it possible to share how you plot these results in your attachment? I am looking for away to post-process the results of my LES case . I have the data for UPrime2Mean and R and I want to extract it from the files in OpenFoam and then draw it.
Sorry again to ask you in your post.
Bashar is offline   Reply With Quote

Old   March 1, 2017, 05:15
Default
  #8
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Quote:
Originally Posted by Bashar View Post
Hi,
So sorry to bother you ,but is it possible to share how you plot these results in your attachment? I am looking for away to post-process the results of my LES case . I have the data for UPrime2Mean and R and I want to extract it from the files in OpenFoam and then draw it.
Sorry again to ask you in your post.
Hi Bashar,

I assume that you got your Umean, UPrime2Mean, and RMean files from the solver. Then, for the channel case, you can use the tool --- postChannel to collapse the data down to single-line profiles. By default, this tool does not calculate the sub-grid-scale stresses, i.e. the RMean part. Therefore, you need to modify it a little bit. This should be straight-forward. Look for the way how the resolved Reynolds stresses are calculated. Then, copy paste and change to RMean values.

Let me know if you need further assistance.

Good luck......

Xiaoyu
Bashar likes this.
Xiaoyu Yang is offline   Reply With Quote

Old   March 2, 2017, 12:35
Default
  #9
Member
 
Jingchang.Shi
Join Date: Aug 2012
Location: Xi'an, China
Posts: 62
Rep Power: 6
aerosjc is on a distinguished road
Hi!

I'm also trying to validate my DNS results of channel flow at Re_tau = 180, but with codes in Flux Reconstruction method. There are 2 problems I want to discuss with you.

1. How to specify Re_tau = 180? The way I'm using is illustrated in http://desperadoshi.github.io/Notes/...del/index.html. Bother you to check if it's correct. Basically it's using Dean's law.

2. How to prove the results are DNS? Of course, we can compare with published results from well-known paper. However, how can we prove it's DNS with our own framework. Do you think the convergence of the FFT of time history of pressure or velocity could prove it's indeed DNS? Maybe there is somewhat connection between turbulence energy spectra and such spectra I described above, but I guess the convergence of turbulence energy spectra should be used to prove it's DNS, instead of FFT of time history, is that true? Apart from FFT way or turbulence energy spectra way, how do you prove your results are DNS?
aerosjc is offline   Reply With Quote

Old   March 2, 2017, 22:33
Default Validation: Turbulent Channel Flow, pisoFoam, LES
  #10
Member
 
Bashar
Join Date: Jul 2015
Posts: 61
Rep Power: 3
Bashar is on a distinguished road
Quote:
Originally Posted by Xiaoyu Yang View Post
Hi Bashar,



I assume that you got your Umean, UPrime2Mean, and RMean files from the solver. Then, for the channel case, you can use the tool --- postChannel to collapse the data down to single-line profiles. By default, this tool does not calculate the sub-grid-scale stresses, i.e. the RMean part. Therefore, you need to modify it a little bit. This should be straight-forward. Look for the way how the resolved Reynolds stresses are calculated. Then, copy paste and change to RMean values.



Let me know if you need further assistance.



Good luck......



Xiaoyu


Thanks a lot for your input. So , to clarify, I need to execute this tool in my case directory, then it will print the data , which I can plot it using any program of my choice?
Regarding, the part that I need to modify the tool , that I did not understand how to do it. I will search to see how to do that since I never did such thing.
Best wishes and many thanks .
Bashar


Sent from my iPhone using CFD Online Forum mobile app
Bashar is offline   Reply With Quote

Old   March 3, 2017, 09:24
Default
  #11
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Quote:
Originally Posted by aerosjc View Post
Hi!

I'm also trying to validate my DNS results of channel flow at Re_tau = 180, but with codes in Flux Reconstruction method. There are 2 problems I want to discuss with you.

1. How to specify Re_tau = 180? The way I'm using is illustrated in http://desperadoshi.github.io/Notes/...del/index.html. Bother you to check if it's correct. Basically it's using Dean's law.

2. How to prove the results are DNS? Of course, we can compare with published results from well-known paper. However, how can we prove it's DNS with our own framework. Do you think the convergence of the FFT of time history of pressure or velocity could prove it's indeed DNS? Maybe there is somewhat connection between turbulence energy spectra and such spectra I described above, but I guess the convergence of turbulence energy spectra should be used to prove it's DNS, instead of FFT of time history, is that true? Apart from FFT way or turbulence energy spectra way, how do you prove your results are DNS?
Hi Jingchang,

Good to know you are running similar cases.....

For DNS case setup, the Dean's correlation is ok. I feel probably the key thing is to determine the correlation between the inner and outer scales, or equivalently the corresponding Reynolds numbers. For Retau=180, the centreline Reynolds number Remax = Umax*delta/nu is about 3300. This gives fairly accurate inner and outer scales with relative error less than 2%. For a given combination of the half channel height "delta" and the kinematic viscosity "nu", than the friction velocity "u_tau" and and the centreline velocity "Umax" may be determined. Then, the channel model should be while defined, based on Reynolds number similarity. For higher friction Reynolds number cases, I guess you need to find the corresponding "Remax".

For DNS results, I guess it depends on the way how they are computed. In my mind, by definition, DNS means that the N-S equations are solved directly without any extra turbulence models, such as RANS models or LES SGS models. So I feel basically in a DNS simulation, all scales of turbulent motions are resolved directly, rather than modelled. So far this is still limited to relatively low Reynolds number flows, due to heavy computational intensity. On the other hand, once discretized, numerical issues arise such as stability, dissipation and dispersion of a particular scheme, etc. Therefore, special treatment may be needed to get a set of accurate converged solutions. But this should be a different topic. Then, for validation or benchmark purpose, I guess you might want to compare your DNS results with other available datasets, such as the mean statistics, the Reynolds stress budgets, and the spectrum, etc......

Not quite sure, but hopefully these answer your questions......

Keep in touch,

Xiaoyu
Xiaoyu Yang is offline   Reply With Quote

Old   March 3, 2017, 09:34
Default
  #12
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
[QUOTE=Bashar;639260]Thanks a lot for your input. So , to clarify, I need to execute this tool in my case directory, then it will print the data , which I can plot it using any program of my choice?
Regarding, the part that I need to modify the tool , that I did not understand how to do it. I will search to see how to do that since I never did such thing.
Best wishes and many thanks .
Bashar


Hi Bashar,

Yes, in your case directory, execute the "postChannel" command, this tool will look for your time averaged datasets and collapse the data down to a single-line profile. Then, you could plot your results using other software packages, such as Tecplot or MatLAB.

To modify this tool, probably, you could search for some suggestions on how to modify an application under the OpenFOAM framework. Then, look through my previous posts to see how to add in the Rmean part.

Good luck,

Xiaoyu
Bashar likes this.
Xiaoyu Yang is offline   Reply With Quote

Old   March 6, 2017, 17:27
Default
  #13
Member
 
Jingchang.Shi
Join Date: Aug 2012
Location: Xi'an, China
Posts: 62
Rep Power: 6
aerosjc is on a distinguished road
Sorry for late reply.

Now, I modify the method I described and I'm sure it's correct.

Thank you for the reply.
aerosjc is offline   Reply With Quote

Old   March 7, 2017, 03:58
Default
  #14
New Member
 
Elyas
Join Date: Dec 2015
Location: Iran
Posts: 3
Rep Power: 3
Elyas_Mosibat is on a distinguished road
Quote:
Originally Posted by Xiaoyu Yang View Post
Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

Total Reynolds Stress and Turbulence Energy Spectrum of LES

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu
Hi Xiaoyu
If your turbulence model is Eddy viscosity , the GenEddyVisc is used to calculate the SGS part;
tmp<volSymmTensorField> GenEddyVisc::B() const
{
return ((2.0/3.0)*I)*k() - nuSgs_*twoSymm(fvc::grad(U()));
}
and if you are using another type of LES model , the GenSGSStress is used, and the SGS stress tensor will computed from your model
Xiaoyu Yang likes this.
Elyas_Mosibat is offline   Reply With Quote

Old   March 7, 2017, 09:20
Default
  #15
New Member
 
Xiaoyu Yang
Join Date: Jan 2017
Location: China
Posts: 8
Rep Power: 2
Xiaoyu Yang is on a distinguished road
Quote:
Originally Posted by Elyas_Mosibat View Post
Hi Xiaoyu
If your turbulence model is Eddy viscosity , the GenEddyVisc is used to calculate the SGS part;
tmp<volSymmTensorField> GenEddyVisc::B() const
{
return ((2.0/3.0)*I)*k() - nuSgs_*twoSymm(fvc::grad(U()));
}
and if you are using another type of LES model , the GenSGSStress is used, and the SGS stress tensor will computed from your model
Hi Elyas,

Thanks a lot! Let me check this......

Regards,

Xiaoyu
Xiaoyu Yang is offline   Reply With Quote

Old   March 24, 2017, 15:30
Default
  #16
New Member
 
kokab
Join Date: Mar 2017
Posts: 1
Rep Power: 0
kokab is on a distinguished road
hello everybody
I also have a problem in validating my channel for Re_tau=395.
my channel is (2pi,2,pi) and LES model is WALE, all the set up are the same as channel395 in openFOAM tutorial.
I have attached my plots, can anyone tell me how to improve my result?
- mesh (60,60,60)
- openFOAM 3.0.1
- solver algorithm pimpleFoam
thanks all
Attached Images
File Type: jpg 1.jpg (94.0 KB, 14 views)
kokab is offline   Reply With Quote

Reply

Tags
incompressible, les, pisofoam, turbulent channel flow, validation

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
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 8 October 25, 2016 19:48
Problems with validation of LES for turbulent annular flow fgarita OpenFOAM Verification & Validation 0 October 12, 2016 05:37
Velocity curve in channel flow by pisoFoam and LES mxylondon OpenFOAM Verification & Validation 9 June 21, 2015 07:28
Serious problems to perform LES of the channel flow LB76 OpenFOAM Verification & Validation 5 June 21, 2012 07:40
Initial conditionfor turbulent channel flow in LES pankaj saha Main CFD Forum 0 November 30, 2007 13:04


All times are GMT -4. The time now is 00:09.