 |
 |
 |
|
|
|
[Sponsors] | ||||
channel flow, too large reynolds stress <u'u'> near the wall |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 7, 2020, 03:59
|
channel flow, too large reynolds stress <u'u'> near the wall
|
#1 |
|
Member
niewiemnic
Join Date: Jan 2018
Location: Niemcy
Posts: 80
Rep Power: 8  |
Hallo,
Cuz I could not have answers in OpenFOAM forum, I post this question once more. I simulate channel flow for Re_tau=395 for long time, but I have always really large <u'u'> near the wall. I simulate with pimpleFoam. Inlet, Outlet, left and right are cyclic and walls are wall. My setup is, 1. nu=2,53e-03 (so 1/nu=395) 2. bulk velocity is about 22-23 m/s (patchMeanVelocityForce on inlet), so wallShearStressMean and u_tau are also about 1. Density is supposed to be 1 kg/m^3. 3. turbulence model is WALE-Modell 4. because Re_bulk is low, I use createBoxTurb before the pimpleFoam. (4-1. Or I start my simulation with nu=2,53e-05 and if the flow is turbulent enough, I change viscosity to nu=2.53e-03 again.) 5. Mesh is really coarse, 32*32*32, because I want to make the mesh fine later. 6. After the flow is turbulent enough, I switch on the fieldAverage1. 7. Time steps are with maxCo = 0.99 variable. but I have always <u'u'> about 20-22 m^2/s^2 near the wall. But it should be about 7-8 m^2/s^2 from Reference. What will be the problem? |
|
|
|
|
|
January 7, 2020, 04:17
|
|
#2 | |
|
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Quote:
Because using such coarse grid you capture nothing close to the wall? Plot the rms along y+ |
||
|
|
|
||
|
January 7, 2020, 04:19
|
|
#3 |
|
Member
niewiemnic
Join Date: Jan 2018
Location: Niemcy
Posts: 80
Rep Power: 8 |
thank you for your answer and sorry, in y-direction the number of grids is not 32. y+ are,
Code:
y+ 0 0.441067194 1.040592885 1.855612648 2.963478261 4.469565217 6.516600791 9.299604743 13.0826087 18.22490119 25.21501976 34.7173913 47.63241107 65.19367589 89.06324111 121.5059289 165.6126482 194.3201581 223.0237154 251.7272727 280.4347826 309.1383399 337.8458498 366.5533597 395.256917 423.9525692 452.6482213 481.3833992 510.0790514 538.7747036 567.5098814 596.2055336 624.9011858 669.0118577 701.4624506 725.3359684 742.8853755 755.8102767 765.2964427 772.2924901 777.43083 781.2252964 783.9920949 786.0474308 787.5494071 788.6561265 789.486166 790.0790514 790.513834 |
|
|
|
|
|
|
January 7, 2020, 04:29
|
|
#4 |
|
Member
Join Date: Aug 2018
Posts: 77
Rep Power: 8 |
check your streamwise resolution, having very unbalanced resolutions csn causesuch issues
|
|
|
|
|
|
|
January 7, 2020, 05:04
|
|
#5 | |
|
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Quote:
You have 48 nodes in vertical direction and only 1 node is at y+<1, that is a coarse grid. You first need to improve the wall resolution (at least 3-4 nodes at y+<1) to check the rms at the walls. Of course, I am talking about a wall resolved approach, not a wall modelled one. |
||
|
|
|
||
|
January 7, 2020, 10:48
|
|
#6 |
|
Member
niewiemnic
Join Date: Jan 2018
Location: Niemcy
Posts: 80
Rep Power: 8 |
https://github.com/OpenFOAM/OpenFOAM...LES/channel395
I try simulation newly with this tutorial setup and my max. nondimensional reynolds stress is about yet 13-14... Cuz I use mesh of tutorial file, it should work well. Max. dimensional reynolds stress is about 0.0018 m^2/s^2 and (u_tau)^2 is about 0.00013 m^2/s^2 (Density is 1 kg/m^3). so the max. nondimensional stress is 13.85 [-]...? 
|
|
|
|
|
|
|
January 7, 2020, 11:13
|
|
#7 |
|
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Before continuing the discussion, post here the plot of u+(y+) that you obtained. Post also the three rms plot. I suggest to superimpose the DNS solutions you can get from well known data-base.
Are you fixing the pressure or mass driving force? Explain how are you forcing the flow in streamwise direction. Have you tried to get a solution without any model? Generally, the peak in the rms close to the wall is obtained in LES at a greater value than DNS, see here https://www.researchgate.net/publica...mulation_codes |
|
|
|
|
|
|
January 8, 2020, 01:05
|
|
#8 |
|
Member
niewiemnic
Join Date: Jan 2018
Location: Niemcy
Posts: 80
Rep Power: 8 |
Sorry that I dont know how can I upload images here.
https://drive.google.com/open?id=1v-...jZ_mh-UebgWSXF Here you can download graphs for u+ and uu+ If vv+ and ww+ help to give me advices, I will upload also the graphs soon. I let velocity constant in domain with Code:
momentumSource
{
type meanVelocityForce;
selectionMode all;
fields (U);
Ubar (0.1335 0 0);
}
The meanVelocityForce fvOptions calculates a momentum source so that the volume averaged velocity (1) in the whole computational domain (all) or a part of domain specified using cellSet or cellZone reaches the desired mean velocity Ubar. p.s. I try to simulate with nu=2e-05. Calculated (estimated) Re_tau is unfortunately about 350, not 395. |
|
|
|
|
|
|
January 8, 2020, 03:58
|
|
#9 | |
|
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Quote:
You can clearly observe that your computed flow rate is quite greater than the DNS one. This effect is common in a LES solution with excessive turbulent viscosity and coarse grid resolution. I suggest You: 1) compute a solution without any SGS model 2) try to use the dynamic model 3) refine the grid doubling the number of nodes |
||
|
|
|
||
|
January 9, 2020, 08:27
|
|
#10 |
|
Member
niewiemnic
Join Date: Jan 2018
Location: Niemcy
Posts: 80
Rep Power: 8 |
I am really thankful for your advices.
https://drive.google.com/open?id=1hU...IDrcl_sAICyrt0 There are two new graphs for u+ and uu+ with dynamic smagorinsky sgs model. First, I made mesh finer in every direction, expecially in the direction of height doubled, Code:
y+ 0.000 0.375 0.787 1.240 1.738 2.284 2.884 3.544 4.268 5.064 5.938 6.899 7.954 9.113 10.386 ... And I used dynamic smagorinsky sgs model. Finally the max. value of <u'u'> is reasonable, but still there are error in coordinates. Can you help me a little bit more? p.s. sorry that I didnt try DNS myself cuz I never used DNS till now. The DNS-Values in the graphs are from a reference. |
|
|
|
|
|
|
January 9, 2020, 08:34
|
|
#11 | |
|
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,849
Rep Power: 73 |
Quote:
100 nodes in vertical direction are now good but, as you can see from the plot of u+ (I suggest to use a semi-log plot as it is a standard in literature), your solution is wrong, very different from the DNS but also from similar LES solutions obtained using OF. I suppose you have some problem in the setting of your case. Just to be sure, how long do you wait before to start sampling the data for the statistical averaging of the velocity? Have you assessed to get only the fields after a statistically steady state is reached? |
||
|
|
|
||
|
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| Wall shear stress in channel flow | sreeyuth | OpenFOAM Running, Solving & CFD | 2 | September 5, 2014 11:02 |
| UDF for wall slipping | HFLUENT | Fluent UDF and Scheme Programming | 0 | April 27, 2011 13:03 |
| Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug | unoder | OpenFOAM Installation | 11 | January 30, 2008 21:30 |
| what the result is negatif pressure at inlet | chong chee nan | FLUENT | 0 | December 29, 2001 06:13 |
| X-Y plot of Yplus in Fluent 5.3 | Luo | FLUENT | 24 | April 11, 2000 07:07 |
Linear Mode
