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

bounding of k and epsilon diverges solution

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 10, 2017, 00:58
Default bounding of k and epsilon diverges solution
  #1
New Member
 
Sagar
Join Date: Sep 2017
Location: Surat, India
Posts: 8
Rep Power: 3
Dave110 is on a distinguished road
Hello,

I am using multiphaseInterFoam to simulate one case. For this case i am using k-epsilon turbulence model.

I have created unstructured mesh and quality of mesh seems to be right. CheckMesh report is as given below.

Checking geometry...
Overall domain bounding box (-3.65028 0 -3.91767e-016) (6.37721 4.4 3.6496)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-3.1831e-017 1.41703e-015 8.34435e-017) OK.
Max cell openness = 3.08743e-016 OK.
Max aspect ratio = 8.96002 OK.
Minimum face area = 4.24312e-007. Maximum face area = 0.108377. Face area magnitudes OK.
Min volume = 1.50115e-010. Max volume = 0.0121032. Total volume = 90.7938. Cell volumes OK.
Mesh non-orthogonality Max: 68.5635 average: 17.1285
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.983603 OK.
Coupled point location match (average 0) OK.

Mesh OK.


When i run my case using laminar model it works well but when i switch to k-epsilon it diverges due to bounding of epsilon followed by bounding of k after some iteration.

My fvScheme and fvSolution files are attached with this thread.

For initialization of k and epsilon, i have calculated their values using standard formulas and their values are in the order of 10^-10(for k) and 10^-15 (for epsilon) at the inlet and at outlet zeroGradient condition is used.(I have also tried with different values but still diverge the solution)

So my Question is "What is the reason for divergence by adding turbulence model only and how to resolve it?"

Thanks for the help in advance.
Attached Images
File Type: jpg Residuals.jpg (41.0 KB, 37 views)
Attached Files
File Type: zip fvScheme_and_fvSolution.zip (1.3 KB, 14 views)
Dave110 is offline   Reply With Quote

Old   October 10, 2017, 06:24
Default
  #2
New Member
 
Join Date: Aug 2017
Location: Milan Area, Italy
Posts: 10
Rep Power: 3
Teosim is on a distinguished road
Hi,
you could first try to reduce the max non-orthogonality of the mesh (at least below 60).

If that is not an option you could start by adding non-ortho correctors to your solver (set nNonOrthogonalCorrectors to 2 or 3).

When I have to work with max non-ortho around 70 I also change the schemes to something like this (and stick with first order accuracy for divSchemes of turbulence terms):

Code:
gradSchemes
{
    default       cellLimited Gauss linear 0.5;  // or cellLimited leastSquares 1.0;
    grad(U)        cellLimited Gauss linear 0.5;  // or cellLimited leastSquares 1.0;
}

laplacianSchemes
{
    default         Gauss linear limited 0.5;
}

snGradSchemes
{
    default         limited 0.5;
}
If BC are consistent you should achieve stability. Please also consider uploading your log file for more info.
Teosim is offline   Reply With Quote

Old   October 12, 2017, 23:43
Default
  #3
New Member
 
Sagar
Join Date: Sep 2017
Location: Surat, India
Posts: 8
Rep Power: 3
Dave110 is on a distinguished road
Hi Teosim,

Thanks for your reply. I have incorporated your suggestions and try to simulate the case But it still diverges.

I am attaching residuals plot as well as log file after changing fvSchemes and fvSolution files as per your suggestions.

Main thing i have observed is that this case works well with laminar model and it diverges with k-epsilon model. It can also be seen from log file that initiation of divergence starts from k and epsilon which ultimately leads to divergence of velocity and pressure fields. Am I right ?

I have tried different values of k and epsilon in "0" directory but it not works. So what should be the bottleneck ?

I have tried to simulate same case with Fluent with same mesh and k-epsilon model. It works.

So, other question is "Is there any difference in convergence criteria or treatment of k and epsilon in Fluent and OpenFOAM ?"


All suggestion are welcome.
Attached Images
File Type: jpg Residuals_2.jpg (41.3 KB, 23 views)
Attached Files
File Type: zip log.zip (11.1 KB, 3 views)
Dave110 is offline   Reply With Quote

Old   October 13, 2017, 01:19
Default
  #4
New Member
 
CFDfreak
Join Date: Dec 2016
Posts: 15
Rep Power: 3
nandhakumar is on a distinguished road
Hello

For your case it seems your initialization of k and epsilon seems very small. What is the velocity of your model. For high velocity flow your initial k and epsilon should be more realistic. Also you said you are using unstructured grid, it needs your schemes should be properly selected. Try using bounded gauss upwind (stable but less accurate) for divergence. Try modeling with structured grid.

You can also add nOuterCorrector value between 50 to 100 based on your simulation time. Because PIMPLE algorithm is not properly utilized. while using unsteady solution it is always better to use outer correctors. If you want to know more about how using PIMPLE algorithm try reading Mathematics, Numerics, Derivations and OpenFOAMŪ. Full-text available · Book · Dec 2016. Tobias Holzmann.

kindly specify what you are modeling that will be helpful.

Thank you
nandhakumar is offline   Reply With Quote

Reply

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
SimpleFoam k and epsilon bounded nedved OpenFOAM Running, Solving & CFD 16 March 4, 2017 08:30
Bounding k and epsilon & coldEngineFoam sasanghomi OpenFOAM 1 September 13, 2013 12:12
Problem with SimpleFoam for a solution around an OneraM6 wing gara1988 OpenFOAM Running, Solving & CFD 3 November 13, 2012 05:47
epsilon and K blowing up. sivakumar OpenFOAM Running, Solving & CFD 1 October 25, 2012 04:50
SimpleFoam k and epsilon bounded nedved OpenFOAM Running, Solving & CFD 1 November 25, 2008 20:21


All times are GMT -4. The time now is 04:22.