[Elham]

Dear all,

I have checked the log file and I knew that the final residuals for Ux, Uy, Uz , k and p are much better. The ones that I've reported in the last post were initial residuals. The final ones are as following:
Ux, Uy and Uz ~ O(10^-6)
p~ O(10^-5) in first loop and p~O(10^-10) in the second loop of correction
k~ O(10^-6)

Is there any way to plot the final residuals instead of initial ones?

Cheers,

Elham

[tiam]

Originally Posted by dradenkovic

I will describe my problem better.

Real dimensions of channel that I am studying are 6 meters length, 35 mm is height and 350mm is width. In my LES simulation, I was watching only part of domain, 6m x 35mm x 35mm. Mesh was dense, 830 x 108 x 52 elements. Mean velocity was 20 m/s.
For flow initialization I used perturbUChannel utility. I used Smagorinsky with vanDriest damping. I did this simulation for 4.5 seconds, that is about 15 flow through times, formed with mean velocity and length of channel.
After using postChannel utility, there is no big difference in velocity profile after 0.5 s and 4.5 s.
https://www.dropbox.com/s/vpzz8rlaud...rison.eps?dl=0

What criterion should I use in order to know when simulation has converged, when there is no big change in velocity during this small time length? Perhaps it would be bigger difference in velocity if I waited for 50 seconds or more?

Now I am doing simulation in 2m x 35 mm x 52.5 mm channel. Mesh is finer, I have 926x114x82 elements in x,y and z direction. However, I am doing 0.1 seconds per day, which is slow if I need around 100 flow through times, that is around 10 s.

Please don't tell me to use RANS.

http://www.cfd-online.com/Forums/ope...nnel-flow.html

My final goal is modeling of pneumatic conveying of dilute particle flow, but I have problems with verification of pure channel flow for relatively long time.

Any advice is highly appreciated.

Regards,
Darko

Hi Darko,

In principle, the higher the order of the statistics you want, the longer it takes to converge them. I've never used any formal criteria but relied on just seening that things "don't change anymore".
One thing you can look at is the behvaiour of the average (in space) u_\tau.
Mostly this is useful for looking whether the initial transients have been flushed out. These can affect the average for a long time, so you should restart the simulation at that point and only then start the field averaging.

If 4.5 sec is 15 flow-through times, it is a bit surpising that you get the same profile after 0.5 sec --- seems way too fast for convergence.
The results in the figure you attach don't look too good either. Maybe you can upoad the case to Dropbox, I might have some time to take a quick look at it.

Best,
Timofey

[tiam]

Originally Posted by Elham

Dear all,

I have checked the log file and I knew that the final residuals for Ux, Uy, Uz , k and p are much better. The ones that I've reported in the last post were initial residuals. The final ones are as following:
Ux, Uy and Uz ~ O(10^-6)
p~ O(10^-5) in first loop and p~O(10^-10) in the second loop of correction
k~ O(10^-6)

Is there any way to plot the final residuals instead of initial ones?

Cheers,

Elham

Ok this is much more reasonable. Regarding the solver, multigrid is probably the better option.

You should definitely be able to plot the residuals. If nothing else works, you can use PyFoam, it allows you to plot everything you see in the logfile by specifying a regular expression. Takes some time to get a hang of it, but it is worth it.

Best,
Timofey

[Elham]

Dear Timofey,

Since I couldn't get to my desired Retau with a very small channel area, I run the channel that you have used with all your settings including the channel size, mesh, solvers,...
But after more than 12000 sec I still could not get to Reb=13300 and Retau=395. My results with M2 mesh of your case are as followings:
Reb=15072
yPlus1=4.27
Retau=1764
delxPlus=88
delzPlus=58

What is your idea about my case. I have read your report "Large_Eddy Simulation of Turbulent Channel Flow" and set everything like yours.

Cheers,

Elham

[tiam]

Originally Posted by Elham

Dear Timofey,

Since I couldn't get to my desired Retau with a very small channel area, I run the channel that you have used with all your settings including the channel size, mesh, solvers,...
But after more than 12000 sec I still could not get to Reb=13300 and Retau=395. My results with M2 mesh of your case are as followings:
Reb=15072
yPlus1=4.27
Retau=1764
delxPlus=88
delzPlus=58

What is your idea about my case. I have read your report "Large_Eddy Simulation of Turbulent Channel Flow" and set everything like yours.

Cheers,

Elham

Hi!
I don't know, it is hard to tell just like that. The thing is that Reb is enforced by the solver, since you prescribe Ub, delta and nu as input parameters, so that should really not be off whatever else happens . You should get 13350!

Best,
Timofey

[Elham]

Dear Timofey,

By reading your report carefully, I understood that your Uc which is the centre line velocity is very near to mine, let's say, 0.1497 comparing to yours 0.15210, consequently our Re_c are near. by using your yPlus function that you have used in controlDict and calculating utau, my utau is 0.0066 and yours is 0.00746. My results are based on averaging after 50 flow through (channel width over ub) and until 20000 sec. My first yplus is 0.7371 and I have more than 10 cells in y+<5.
1. I suppose your Ub is based on your initial settings and you didn't read it anymore, I am right?
My u versus y in global coordinate when I put u_c for y-axis (ave(streamwise u)/0.1335) is much near to DNS rather than (ave(streamwise u)/u_c).
2. What is your idea about my results? Is it correct to put y-axis (ave(streamwise u)/0.1335) for global coordinates plot?
I have attached my results based on y-axis (ave(streamwise u)/0.1335) for global coordinates plot.

Thanks for your kind attention.

Cheers,

Elham

[tiam]

Originally Posted by Elham

Dear Timofey,

By reading your report carefully, I understood that your Uc which is the centre line velocity is very near to mine, let's say, 0.1497 comparing to yours 0.15210, consequently our Re_c are near. by using your yPlus function that you have used in controlDict and calculating utau, my utau is 0.0066 and yours is 0.00746. My results are based on averaging after 50 flow through (channel width over ub) and until 20000 sec. My first yplus is 0.7371 and I have more than 10 cells in y+<5.
1. I suppose your Ub is based on your initial settings and you didn't read it anymore, I am right?
My u versus y in global coordinate when I put u_c for y-axis (ave(streamwise u)/0.1335) is much near to DNS rather than (ave(streamwise u)/u_c).
2. What is your idea about my results? Is it correct to put y-axis (ave(streamwise u)/0.1335) for global coordinates plot?
I have attached my results based on y-axis (ave(streamwise u)/0.1335) for global coordinates plot.

Thanks for your kind attention.

Cheers,

Elham

Hi,
Ub is enforced by the solver by a varying pressure gradient. So whatever value you put in fvOptions should be enforced and your Re_b should be very accurate.
Yes, scaling with U_b is common practice when plotting in outer coordinates.

Your result is a bit weird since you have some jiggling in the core of the channel. Both for the line and the stars -- I don't know which represent ehat though.

[Elham]

Dear Timofe,

The star data are the DNS ones. Sorry I forgot to mention that. The jiggling may be because of the lack of enough points of probe.

Thanks for all your helps.

Cheers,

Elham

[dradenkovic]

Timofey,

I see now that you replied to my question about ten days ago.

In the meantime, I solved problem. Instead of larger domain from my above post, I used smaller part of domain (similar approach was in Eugen's PhD, page 162), with dimensions 140 mm x 35 mm x 52.5 mm. Comparing to my above case, mesh was much finer. Flow through time was around 200.

Here is velocity comparison

https://www.dropbox.com/s/vpzz8rlaud4rug6/LogLawComparison.eps?dl=0


Thank you for replying.

Regards,
Darko

[dradenkovic]

If we say, that 200 flow through times, if we use postChannel utility, is enough for obtaining converged velocity profile in channel (i.e velocity profile that is symmetric with very negligible differences, which can be a criterion, as I read somewhere), how many time steps is expected in order to obtain converged two-point velocity correlations?

I ask this because I think that two-point correlations that I have calculated are still time - dependent or I have error in Matlab code. Here is complete Matlab code and all necessary data, so that anybody can run program.

https://www.dropbox.com/s/cdc9w5aa63...tions.zip?dl=0

Velocity in channel is 20 m/s. Dimensions of channel are 140 mm x 35 mm x 52.5 mm. If I forgot something important to say, please ask.

Regards,
Darko

[Elham]

Originally Posted by cedric_duprat

Hi Eugene,

euh ....not really )

As I told, the geometry and the grid are different. it's the same geometry as the DNS calculation. So streaks are shorter than the box and there is (should be) no effect from the outlet on the inlet.

the time discretisation is Crank-Nicholson. (I think it's backward in the tutorial).
For the numerical scheme I using only central diffential scheme (to keep second order accurate).
so there is no limitedLinear 1 for these terms (div(phi,k), div(phi,B))
Then, the time step is different to keep Co number less than 0.4.
For the solver, I'm using ICCG to solve the pressure (and the same PISO as the tutorial) and BICCG for the other quantities, which is quite different from the tutorial also.

Can these settings bring me some over diffusive terms, because, it should not, contrary to the tutorial (convective scheme view).

Thank you for giving advise,... I hope it's not a stupid question. But, because the results are not so "bad" (but also not so good ) ), I think it's just a small things.


Cedric

Dear Cedric,

Would you please let me know why you kept Co number less than 0.4? Is it based on your own experience and cause better results?
I had a relatively good results with rough mesh but not with a finer mesh. The time steps for both of them were the same. Is it because of the time step? Co number for the finer mesh is about 1.0.


Cheers,

Elham

[cedric_duprat]

Elham,

Well, as you can see on the forum, I ran these calculations in 2008 (with an old version of OpenFOAM) so .... I don't remember every settings.

What I remember is that if I increased the CFL to much, calculation crashed (which make sence). 0.4 was kind of optimum for my case.

The size of your mesh and your time-step (if it has been fixed) give you the CFL. If you refine your mesh and you keep the same time-step, you'll get a higher CFL value. Why don't you reduce the time step in such a way that the same CFL is used in both calculations ?

What are your results for coarse and fine mesh ? could you give us more details on these meshes ?

Cédric

[tiam]

Originally Posted by cedric_duprat

Elham,

Well, as you can see on the forum, I ran these calculations in 2008 (with an old version of OpenFOAM) so .... I don't remember every settings.

What I remember is that if I increased the CFL to much, calculation crashed (which make sence). 0.4 was kind of optimum for my case.

The size of your mesh and your time-step (if it has been fixed) give you the CFL. If you refine your mesh and you keep the same time-step, you'll get a higher CFL value. Why don't you reduce the time step in such a way that the same CFL is used in both calculations ?

What are your results for coarse and fine mesh ? could you give us more details on these meshes ?

Cédric

This is a good question though. I have no problem running at CFL around 1, but many papers mention 0.4-0.5, is there are a particular reason for these choices?

Also, protip -- to know what time-step to pick for a certain CFL you can use the adjustableTimeStep option during the simulation phase where you dump the transients. Then, you can check out the max time-step you had in the log and use that as a constant time-step value in the part of the simulation where you collect the statistics.

[Elham]

Originally Posted by tiam

This is a good question though. I have no problem running at CFL around 1, but many papers mention 0.4-0.5, is there are a particular reason for these choices?

Also, protip -- to know what time-step to pick for a certain CFL you can use the adjustableTimeStep option during the simulation phase where you dump the transients. Then, you can check out the max time-step you had in the log and use that as a constant time-step value in the part of the simulation where you collect the statistics.

Thanks.

Elham

[Elham]

Dear all,

My results for Re_tau=330, target Re_tau=395, with 5 cells in y+<5 and the first y+=0.73 and Re_b=13350 has been attached. As you see the profile in global coordinate is near to DNS results but in wall coordinate is so far from DNS. I suppose I am doing something wrong in drawing the plots. I let the flow to pass around 90 flow throughs and then averaged just for 8 flow throughs. I know the averaging time is not enough but the difference between DNS results and mine is so big that I think the problem will exist after passing more and more time.
I would appreciate if anyone can give me some clues.
PS: The problem may be come from the spatial averaging as I just do time averaging in a specified plane and no spatial averaging. If I want to use fieldAverage function in ControlDict, I need to keep data of every time step which demands high storage capacity.

Cheers,

Elham

[anishtain4]

Elham,

How are you calculating the wall shear stress? It seems your wall scaled plots are off by a scale, use wallGradU utility to read the velocity gradient at the wall rather than calculating it by matlab or anything else.

[Elham]

Dear Mahdi,

I calculated utau by means of wallGradU and wallShearStress utility but the big gap between mine and DNS exists. Actually, the utau in all of the methods are nearly the same. You can have a look at my calculation process. I will appreciate if you can correct me:


yPlus=dist()/nu*sqrt((nu+nuSgs)*mag(snGrad(U))) %in controlDict (Timofey code))
yPlus1=time_averaged of yPlus
Y1=dist() % in controlDict
utau=yPlus1(:,2)*nu/Y1;

Cheers,

Elham

[tiam]

Originally Posted by Elham

If I want to use fieldAverage function in ControlDict, I need to keep data of every time step which demands high storage capacity.

Cheers,

Elham

Hm? Why? You just have to keep the UMean field in the memory, that is it. It updates the average at every time-step without storing anything extra.

Best,
Timofey

[cedric_duprat]

Elham,

What is U in your yPlus calculation ? instanteneous or averaged velocity ?
Have you try to calculated utau from the averaged velocity profiles you send us ?
I mean from the mean velocity profile you can calculate tauw
from tauw you get utau. Is this value coherent with the one you already have ?

Cedric

[Elham]

Originally Posted by tiam

Hm? Why? You just have to keep the UMean field in the memory, that is it. It updates the average at every time-step without storing anything extra.

Best,
Timofey

Dear Timofey,
When I use fieldAverage to have UMean in each outputTime, I just have UMean in the outputTime directory. So I need to keep output time directory which is demands big memory space.