
[Sponsors] 
October 13, 2015, 12:50 
Mesh Independence Problem for Low Reynolds Number (<100) Flow

#1 
New Member
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 4 
Hello,
I have been trying to study the developing regime of the flow between two infinite plates using FLUENT for very low Reynolds number cases (<100). One parameter that I am interested is the pressure drop along the length of the developing flow. So during fluent cases, I monitor the pressure drop across the entire geometry (by outputting areaweighted average pressure at the inlet since Pout = 0). Once the pressure change per iteration is <0.0001, and rest of the residuals are all below 1e6, I stop the simulation and go to the next case. Typically, to reach my convergence criteria, it takes around 200010000 iterations per case, depending on the mesh. One thing that baffles me is that I cannot seem to get a mesh independent result even though this is a very simple case (2D, infinite plates, laminar flow, etc). Pressure at the inlet changes significantly with different mesh; I have also monitored volume averaged pressure along the entire channel and that's also significantly changing. I have tried meshes ranging from 100 x 100 to 1400 x 1400; due to computation time, I couldn't go higher. I have uploaded my workbench file in the following link: https://drive.google.com/folderview?...nM&usp=sharing If someone could provide some insight, I would really appreciate it! Thank you in advance 

October 14, 2015, 00:25 

#2 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,568
Rep Power: 22 
What are your boundary conditions? Is it a velocity inlet and pressure outlet?


October 14, 2015, 00:32 

#3 
New Member
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 4 
Yes, uniform velocity inlet and pressure outlet.
I have one symmetry condition to cut the computation time/mesh size. 

October 15, 2015, 06:45 

#4 
Member
Devesh Baghel
Join Date: Mar 2009
Posts: 70
Rep Power: 10 
Hi,
1. which pressure parameter you are looking at inlet i.e. static, total ? 2. For low density mesh, can not decide the mesh independency. After some interation of mesh density i.e. abc x abc, only look forward for mesh independent solution. 3. how much difference of pressure values in terms of % you got into your simulaiton. Devesh 

October 16, 2015, 10:36 

#5 
New Member
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 4 
Hello,
1. Static. Since velocity at the inlet is set constant, static or total shouldn't matter, no? 2. I agree. But what is considered low/fine density mesh? I don't want to go much higher than 1000x1000 because of computation time. 3. Previous data looked something like this: Mesh Grid  P @ inlet 100x100 4.16e4 200x200 4.23e4 300x300 4.51e4 400x400 5.02e4 500x500 5.62e4 And the above data was for Re 50 case. But I think I figured out the problem. For higher mesh, I just had to iterate a lot more, around 20000 iterations (why does it take so much for such simple problem?). Previously, I was doing around ~4000 iterations. I guess my initial convergence criteria used before was not great. So now, I'm iterating until all the residuals are below 10^8 or 9 and P does not change more than 0.0001 per 100 iterations or so. The new data looks like below: 100x100: 4.16e4 200x200: 4.21e4 300x300: 4.24e4 400x400: 4.26e4 Thank you for the inputs 

October 16, 2015, 11:33 

#6 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,568
Rep Power: 22 
A low density mesh is one that does not satisfy your grid convergence criteria, but it's still up to you to define what grid convergence is.
Did you use the same initialization for both large and small grids? Faster convergence is possible if you initialize the finer grid with the solution from the coarse grid and vice versa. Since you have already computed the solution on a coarse grid, using that solution as the initial conditions on subsequent runs is preferred to reusing an initial guess of constant velocity. For steady state simulations: The slow convergence is because of the scale disparity between your short wavelengths (grid resolution and long wavelengths (domain size). At each step in the iteration your locally adjusted solution values are local adjustments and affect only the adjacent cells. It takes many iterations for these local adjustments to propagate and fill the entire domain. Even with a good initial guess it can still be slow to converge because of the influence of the multigrid accelerator is limited on larger grids (i.e. the AMG solver). Large grids depends on the multigrid accelerator to accelerate the convergence. However, because of memory constraints, wall time constraints, etc, the multigrid performance is limited so that large grids take relatively more iterations to converge than small grids. Transient problems don't have this issue because there the local effects are definitely local but transient problems are still governed by long timescale behavior (the temporal equivalent or long wavelength). Last edited by LuckyTran; October 22, 2015 at 01:26. 

October 16, 2015, 11:54 

#7 
New Member
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 4 
Thank you for the detailed and quick response LuckyTran!
I initialized large and small grids separately; I did not think about initializing the finer grid with the solution from the coarse grid, but that's a great idea. In order to do that, should I just do: 1) standard initialization 2) compute from inlet 3) initial values: Gauge Pressure, X and Y velocity obtained from course grid 4) initialize? Or is there a way that Fluent can take in the .dat file from course mesh solution and import it somehow to the new mesh and continue iteration from there? About short wave lengths and long wave lengths, that makes a lot of sense. Thank you. 

October 16, 2015, 12:58 

#8 
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,568
Rep Power: 22 
Go to file=>interpolate and write the an interpolate file. Then do read and interpolate on your new simulation. If you write and read all the data then you won't need to do the initialize step on your next simulation. If you are missing some variables then initialize first and then read the interpolate file because when you hit the initialize button it clears all currently existing variables.


October 21, 2015, 12:27 

#9  
New Member
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 4 
Quote:


Tags 
developing flow, infinite parallel plates, low reynolds number, mesh independency, pressure and velocity 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
decomposePar allRegions  stru  OpenFOAM PreProcessing  2  August 25, 2015 03:58 
About the Reynolds Number and Yplus in external flow  Mason liu  CFX  18  November 10, 2014 19:37 
snappyHexMesh sticking point  natty_king  OpenFOAM Native Meshers: snappyHexMesh and Others  2  April 17, 2014 01:24 
Layers:problem with curvature  giulio.topazio  OpenFOAM Native Meshers: snappyHexMesh and Others  10  August 22, 2012 09:03 
external flow with snappyHexMesh  chelvistero  OpenFOAM  11  January 15, 2010 20:43 