# Mesh Independence Problem for Low Reynolds Number (<100) Flow

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 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: 3 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 area-weighted 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 1e-6, I stop the simulation and go to the next case. Typically, to reach my convergence criteria, it takes around 2000-10000 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: 940 Rep Power: 16 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: 3 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: 67 Rep Power: 8 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: 3 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: 940 Rep Power: 16 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 time-scale behavior (the temporal equivalent or long wavelength). devesh.baghel and bgp723 like this. 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: 3 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: 940
Rep Power: 16
Quote:
 Originally Posted by bgp723 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?
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: 3
Quote:
 Originally Posted by LuckyTran 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.
Thank you, this significantly sped up my simulation time and convergence!

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post stru OpenFOAM Pre-Processing 2 August 25, 2015 03:58 Mason liu CFX 18 November 10, 2014 19:37 natty_king OpenFOAM Native Meshers: snappyHexMesh and Others 2 April 17, 2014 01:24 giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 10 August 22, 2012 09:03 chelvistero OpenFOAM 11 January 15, 2010 20:43

All times are GMT -4. The time now is 18:58.

 Contact Us - CFD Online - Top