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

LES of channel flow: data, case files, technical report.

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

Like Tree14Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 2, 2015, 12:33
Default LES of channel flow: data, case files, technical report.
  #1
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Dear foamers,

I would like to share the results of a simulation campaign that was performed by us here at Uppsala University.
I was supposed to present this at the ongoing OF workshop, but I couldn't make it because of visa issues .

We have performed LES of channel flow using OpenFOAM. In our study we have computed a large amount of statistical quantities, including high-order moments, two-point correlations etc. Also, we have considered three different grids, so one clearly sees how the grid affects the results, and how the results converge towards DNS data as the grid gets better.

We have collected all the acquired profiles in this repository:
https://bitbucket.org/lesituu/channel_flow_data/

A ready-to-run case file can also be found there, so the data should be relatively easily reproduced by others.

A techincal report that documents our study is available for download here:
http://www.it.uu.se/research/publica...orts/2015-014/

This project was basically a way for me to start my Phd and learn about LES and OpenFOAM at the same time, so the starting point was the existing channel flow tutorial. The majority of the setting were left unchanged.
In order to compute most of the statistical quantities we used swak4foam.
Since I think it is quite common for people to start out with channel flow, I hope that the repository we provide will make life a bit easier for future new-commers . In some sense it can also be seen as a swak4foam tutorial.

Any kind of feedback is of course appreciated.

P.S. I was not sure if I should start a new thread or just post this into the existing thread for LES of channel flow. I thought that this thread can serve for discussing the particular resuts/setup/whatever found in our work and the general thread can continue just being general. I leave it to the moderators to decide whether that was a good call .
tiam is offline   Reply With Quote

Old   November 3, 2015, 20:58
Default
  #2
New Member
 
Mohamed Elshahat Ouda
Join Date: May 2010
Posts: 29
Rep Power: 13
me.ouda is on a distinguished road
Hi Timofey,

First of all thanks for this handy report it was very useful for me to read it.
I am trying to validate the k-ε model in openfoam based on the same DNS data.

So far I have one comment regarding your report I am not sure if I misunderstood your point or it is really a mistake. In table 3.2 you put the number of cells along axis and corresponding Y-plus. I have calculated Y-plus based on this information and the equation for the mesh grading used in blockMesh and I found that the the corresponding Y-plus values for this grid should be the double. So I think that these numbers correspond to number of cells in δ not in H, I am I right?
me.ouda is offline   Reply With Quote

Old   November 4, 2015, 03:30
Default
  #3
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by me.ouda View Post
Hi Timofey,

First of all thanks for this handy report it was very useful for me to read it.
I am trying to validate the k-ε model in openfoam based on the same DNS data.

So far I have one comment regarding your report I am not sure if I misunderstood your point or it is really a mistake. In table 3.2 you put the number of cells along axis and corresponding Y-plus. I have calculated Y-plus based on this information and the equation for the mesh grading used in blockMesh and I found that the the corresponding Y-plus values for this grid should be the double. So I think that these numbers correspond to number of cells in δ not in H, I am I right?
Hi Mohamed!

I did a quick test using the UMean profile for mesh M1 and got a a value of 1.74.
We have
y^+ = y_p*sqrt((nu+nuSgs)*U_p/y_p)/nu,
where the _p values are in the cell center closest to the wall.
I ignore the nuSgs, because I don't want to search for the value right now.
Then we get
y^+ = 0.0048*sqrt(2e-5*0.0127449/0.0048)/2e-5 = 1.7489

In the table, the value is 1.9 which is due to the nuSgs I suppose.

In any case, the numbers in the table correspond to h, not delta.
Since you got double values, have you perhaps taken y_p to be the location of the first *point* of the mesh (i.e. the location of the first off-the wall face), not the cell center? Just a guess. Anyhow, please share the values you use and we'll get to the bottom of this .

Best,
Timofey
me.ouda likes this.
tiam is offline   Reply With Quote

Old   November 4, 2015, 04:29
Default
  #4
New Member
 
Mohamed Elshahat Ouda
Join Date: May 2010
Posts: 29
Rep Power: 13
me.ouda is on a distinguished road
Hi Timofey,

You are right I am using the height of first cell to calculate Y+, if the value in the table are for the first cell center, then that is perfect.

I have one more question regarding initial and boundary conditions. The value you have used as initial conditions (for U, p, nuSgs and k) seems to be from other simulation (i.e you run for specific time steps to initiate these fields) not calculated based on analytical formula (velocity defect law for example), am I right? if yes can you give some elaboration on this point.

Regarding boundary condition, you are using cyclic B.C., I am not familiar with this B.C. and really I can't understand how it works. for example does it require additional information to define the velocity profile at time step 0?

for my case I am using nonuniform values for U, k and ε at the inlet which I've calculated from the analytical formulas and fix that for all time steps, do you think that this approach is physically correct?
me.ouda is offline   Reply With Quote

Old   November 4, 2015, 10:59
Default
  #5
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by me.ouda View Post
Hi Timofey,

You are right I am using the height of first cell to calculate Y+, if the value in the table are for the first cell center, then that is perfect.

I have one more question regarding initial and boundary conditions. The value you have used as initial conditions (for U, p, nuSgs and k) seems to be from other simulation (i.e you run for specific time steps to initiate these fields) not calculated based on analytical formula (velocity defect law for example), am I right? if yes can you give some elaboration on this point.

Regarding boundary condition, you are using cyclic B.C., I am not familiar with this B.C. and really I can't understand how it works. for example does it require additional information to define the velocity profile at time step 0?

for my case I am using nonuniform values for U, k and ε at the inlet which I've calculated from the analytical formulas and fix that for all time steps, do you think that this approach is physically correct?
Hi!

Regarding the ICs, I used the channel395 tutorial case that is availabnle in openfoam as a starting point. Some initial field is given there, and I did not bother looking deeper into that since, well, it worked for me.
However recently I had to do work initialization and the perturbU utility which you can google for seems to be a great tool. I have successfully used it to initialize an LES.

The cyclic bc is just a periodic boundary condition, so what flows out of the outlet comes back into the inlet. To make this work you have to make sure the domain is sufficiently large.

BUT. You say that you want to verify the k-eps model, so you are doing RANS. Most of this becomes irrelevant to you then. For RANS channel flow is a 1-d problem: you solve for the mean, and the mean only depends on y! You just need a line in the wall-normal direction and that is your mesh .

I think you will benifit from checking out this report:
http://uu.diva-portal.org/smash/reco...89&dswid=-9746
It deals with exactly your problem: testing how different RANS models perform for the channel flow!

Best,
Timofey
me.ouda and ari003 like this.
tiam is offline   Reply With Quote

Old   November 6, 2015, 05:35
Smile
  #6
New Member
 
Mohamed Elshahat Ouda
Join Date: May 2010
Posts: 29
Rep Power: 13
me.ouda is on a distinguished road
Thanks Timofey, that is extremely helpful
me.ouda is offline   Reply With Quote

Old   August 12, 2019, 13:56
Default
  #7
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Dear Timofey,

thank you for your contribution regarding this specific topic.

I have two questions.

1.) You have used oneEqEddy model together with wall damping? Or I missed something?
2.) I tried to perform LES channel flow computations and I cannot get a proper averaged pressure gradient (i.e. wall shear stress or uTau) values. When I compare computed uTau values with DNS, errors are around 20%. These errors seems to be to large as other researchers reported errors below 2% (for same subgrid models and similar mesh resolutions). Did you manage to calculate a proper uTau value?

Best regards!
camel is offline   Reply With Quote

Old   August 12, 2019, 14:08
Default
  #8
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Dear Timofey,

thank you for your contribution regarding this specific topic.

I have two questions.

1.) You have used oneEqEddy model together with wall damping? Or I missed something?
2.) I tried to perform LES channel flow computations and I cannot get a proper averaged pressure gradient (i.e. wall shear stress or uTau) values. When I compare computed uTau values with DNS, errors are around 20%. These errors seems to be to large as other researchers reported errors below 2% (for same subgrid models and similar mesh resolutions). Did you manage to calculate a proper uTau value?

Best regards!

1. Yes, see https://bitbucket.org/lesituu/channe.../LESProperties


I'd recommend using WALE though. Or no SGS model at all.



2. You can see the Re_tau that I got in the report. For a fine mesh, you should get good results. I'd recommend delta z+ = 10 and delta x+= 25 as a good start.
tiam is offline   Reply With Quote

Old   August 12, 2019, 14:55
Default
  #9
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Dear Timofey,

thank you.

However, I'm still curious regarding the pressure gradient value in channel395 computations. For instance, when I tried to run channel395 tutorial in of6, the average pressure gradient is still significantly lower than theoretical (i.e. computational is equal to cca 4e-05, whereas theoretical is equal to cca 6.2e-5). These results produce significant error when computational friction coefficient is compared with theoretical value. I've read Phd thesis written by Eugene de Villiers and his results were much better for same setup.

Can you please comment this situation?

Thank you in advance! I appreciate your help.

Best regards!
camel is offline   Reply With Quote

Old   August 12, 2019, 15:00
Default
  #10
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Dear Timofey,

thank you.

However, I'm still curious regarding the pressure gradient value in channel395 computations. For instance, when I tried to run channel395 tutorial in of6, the average pressure gradient is still significantly lower than theoretical (i.e. computational is equal to cca 4e-05, whereas theoretical is equal to cca 6.2e-5). These results produce significant error when computational friction coefficient is compared with theoretical value. I've read Phd thesis written by Eugene de Villiers and his results were much better for same setup.

Can you please comment this situation?

Thank you in advance! I appreciate your help.

Best regards!

How do you measure the pressure gradient? Do you mean the value reported by the fvOption?
tiam is offline   Reply With Quote

Old   August 12, 2019, 15:04
Default
  #11
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Dear Timofey,

I tried to run tutorial case for larger amount of time (i.e. for 7000 s). After that I exported the pressure gradient values from log file and time average it using libreOffice calc.

P.S. I use foam-extend 3.2 so I use channelFoam solver as foam-extend distribution does not have implemented fvOptions.
camel is offline   Reply With Quote

Old   August 12, 2019, 15:09
Default
  #12
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Dear Timofey,

I tried to run tutorial case for larger amount of time (i.e. for 7000 s). After that I exported the pressure gradient values from log file and time average it using libreOffice calc.

P.S. I use foam-extend 3.2 so I use channelFoam solver as foam-extend distribution does not have implemented fvOptions.

OK, I see. I have to say that I've never looked at the pressure gradient values that much, but rather at u_tau, tau_w and Re_tau. How does the error look for those quantities, is it different from what you get for the pressure gradient?
tiam is offline   Reply With Quote

Old   August 12, 2019, 15:15
Default
  #13
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Well, I supposed that uTau can be calculated as sqrt(gradP), where gradP basically represents Tau_w (I've read that in Eugenes PhD). So I used this methodology for calculating uTau, Tau_w and Re_tau. Did I miss something?

How did you calculate these values in your technical report?
camel is offline   Reply With Quote

Old   August 12, 2019, 15:22
Default
  #14
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Well, I supposed that uTau can be calculated as sqrt(gradP), where gradP basically represents Tau_w (I've read that in Eugenes PhD). So I used this methodology for calculating uTau, Tau_w and Re_tau. Did I miss something?

How did you calculate these values in your technical report?

Look at how I compute y+ in a post in this very thread. Basically, you can just compute tau_w by definition as (nu + nuSgs) du/dy, where the gradient is computed using the first off-wall value from the mean velocity profile. Note that nuSgs should be 0 on the wall, but I added it so that you can double check that .
tiam is offline   Reply With Quote

Old   August 12, 2019, 15:28
Default
  #15
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Thank you! I'll check it.

However, I am still curious regarding that pressure gradient. Eugene noted in his PhD (page 163):

To ensure consistency, the streamwise bulk velocity, Ub, through the channel is adjusted to be equal to the average DNS value by varying an imposed streamwise constant pressure gradient, ∂P/∂x. - this basically means Eugene used something similar (or same) to the channelFoam solver.
The time averaged value of this quantity is equivalent to the mean wall shear stress and can be compared to the corresponding DNS value. - Regarding to this statement, the tau_w should be calculated as sqrt(gradP), where gradP is value given in simulation log file.
camel is offline   Reply With Quote

Old   August 12, 2019, 15:36
Default
  #16
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Thank you! I'll check it.

However, I am still curious regarding that pressure gradient. Eugene noted in his PhD (page 163):

To ensure consistency, the streamwise bulk velocity, Ub, through the channel is adjusted to be equal to the average DNS value by varying an imposed streamwise constant pressure gradient, ∂P/∂x. - this basically means Eugene used something similar (or same) to the channelFoam solver.
The time averaged value of this quantity is equivalent to the mean wall shear stress and can be compared to the corresponding DNS value. - Regarding to this statement, the tau_w should be calculated as sqrt(gradP), where gradP is value given in simulation log file.

I mean, yes, the gradP and tau_w are trivially connected in the case of channel flow, so in principle you should get similar results using the two methods. I prefer computing it by definition because


- It works for all flows and not only channel flow.
- It uses a field that is readily available without the need to parse the log.
tiam is offline   Reply With Quote

Old   August 12, 2019, 15:41
Default
  #17
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
I agree with your statements.

I'll try to investigate this topic a little bit more and give you some feedback as soon as I find some solution.

One more question. What procedure did you use to calculate the vorticity fluctuations that you compared with available DNS results (i.e. https://turbulence.oden.utexas.edu/d...han395.vortvar )?
camel is offline   Reply With Quote

Old   August 12, 2019, 15:44
Default
  #18
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
I agree with your statements.

I'll try to investigate this topic a little bit more and give you some feedback as soon as I find some solution.

One more question. What procedure did you use to calculate the vorticity fluctuations that you compared with available DNS results (i.e. https://turbulence.oden.utexas.edu/d...han395.vortvar )?

I use swak4foam for these type of things, see

https://bitbucket.org/lesituu/channe...em/controlDict


Basically, I create a field defined as curl(U) and then add it to the fieldAverage. I am pretty sure there is a native function object for vorticity as well.
tiam is offline   Reply With Quote

Old   August 12, 2019, 15:47
Default
  #19
New Member
 
Join Date: Jan 2014
Posts: 19
Rep Power: 9
camel is on a distinguished road
Great. Thank you for all comments.

P.S. I've seen your paper "A Library for Wall-Modelled LES Based on OpenFOAM Technology". Really nice paper. Will this library be available (or perhaps it is already available?) to OpenFoam community soon?
camel is offline   Reply With Quote

Old   August 13, 2019, 04:11
Default
  #20
Senior Member
 
Timofey Mukha
Join Date: Mar 2012
Location: Stockholm, Sweden
Posts: 116
Rep Power: 11
tiam is on a distinguished road
Quote:
Originally Posted by camel View Post
Great. Thank you for all comments.

P.S. I've seen your paper "A Library for Wall-Modelled LES Based on OpenFOAM Technology". Really nice paper. Will this library be available (or perhaps it is already available?) to OpenFoam community soon?

https://bitbucket.org/lesituu/libwallmodelledles


Enjoy
tiam is offline   Reply With Quote

Reply

Tags
channel flow, les, swak4foam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
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 9 February 5, 2021 10:15
UDF issue MASOUD Fluent UDF and Scheme Programming 14 December 6, 2012 13:39
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 07:21
PhD in turbulence Hans Main CFD Forum 14 October 8, 2001 03:03
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 05:23.