CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

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

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

Like Tree3Likes
  • 2 Post By LuckyTran
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Display Modes
Old   October 13, 2015, 12:50
Default Mesh Independence Problem for Low Reynolds Number (<100) Flow
  #1
New Member
 
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 3
bgp723 is on a distinguished road
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
bgp723 is offline   Reply With Quote

Old   October 14, 2015, 00:25
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 940
Rep Power: 16
LuckyTran will become famous soon enough
What are your boundary conditions? Is it a velocity inlet and pressure outlet?
LuckyTran is offline   Reply With Quote

Old   October 14, 2015, 00:32
Default
  #3
New Member
 
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 3
bgp723 is on a distinguished road
Yes, uniform velocity inlet and pressure outlet.
I have one symmetry condition to cut the computation time/mesh size.
bgp723 is offline   Reply With Quote

Old   October 15, 2015, 06:45
Default
  #4
Member
 
Devesh Baghel
Join Date: Mar 2009
Posts: 67
Rep Power: 8
devesh.baghel is on a distinguished road
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
devesh.baghel is offline   Reply With Quote

Old   October 16, 2015, 10:36
Default
  #5
New Member
 
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 3
bgp723 is on a distinguished road
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
bgp723 is offline   Reply With Quote

Old   October 16, 2015, 11:33
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 940
Rep Power: 16
LuckyTran will become famous soon enough
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.
LuckyTran is offline   Reply With Quote

Old   October 16, 2015, 11:54
Default
  #7
New Member
 
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 3
bgp723 is on a distinguished road
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.
bgp723 is offline   Reply With Quote

Old   October 16, 2015, 12:58
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 940
Rep Power: 16
LuckyTran will become famous soon enough
Quote:
Originally Posted by bgp723 View Post
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.
bgp723 likes this.
LuckyTran is offline   Reply With Quote

Old   October 21, 2015, 12:27
Default
  #9
New Member
 
Daniel B
Join Date: Jul 2014
Posts: 12
Rep Power: 3
bgp723 is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
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!
bgp723 is offline   Reply With Quote

Reply

Tags
developing flow, infinite parallel plates, low reynolds number, mesh independency, pressure and velocity

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
decomposePar -allRegions stru OpenFOAM Pre-Processing 2 August 25, 2015 03:58
About the Reynolds Number and Y-plus 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


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