CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Turbulent wall treatment in multiphase flow regimes

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 10, 2016, 05:19
Question Turbulent wall treatment in multiphase flow regimes
  #1
Member
 
Sebastian W.
Join Date: Nov 2012
Location: Saxony, Germany
Posts: 42
Rep Power: 6
nero235 is on a distinguished road
Send a message via ICQ to nero235
Hello friends,

for quite some time now I am simulating several cases with multiphase flow regimes (3 phases) with openFOAM. I have found that the kEpsilon turbulence model is best for my setup and is easy to validate with a easy water-oil experiment.

We know that the dimensionless wall distance y+ is depending on the velocity, the actual wall distance and the kinematic viscosity of the fluid. Some one can easily calculate this value when it is a single phase system. But what value is the right one, if there is not one but three different values for kinematic viscosities? Problematic was also that I had a block mesh, which meant that I had large blocks on a large diameter shrinking to a very small block on a small diameter. I couldn't control my y+ very well due to the mesh layout and geometry.

I have run many test cases with my multiphase system on different meshes, finer and more coarse at the walls. I tested every different numerical scheme there is: limited, corrected, forward and backward ... I tested every turbulence model: kEpsilon, kOmegaSST ... Every time I received the same error: very high bounding values for the turbulent parameters. Mostly it was epsilon or omega. The result was always a crash of the solver.

I fixed this problem "simply" by not using any wall function for k, epsilon, nut! This is the only way I can run my cases without a crash. My question is now if there is a good value to choose for the turbulent parameters directly on the wall. Right now I am using the "fixedValue" option. Maybe there is a better alternative, I don't know. I still receive a bounding warnings, however this time, the values stay in a normal range.

P.S. If you start your case without a "nut" file and you want to use a "fixedValue" for the turbulent parameters, then openFOAM automatically creates an "nut" with a wall function. OpenFOAM then overwrites the k and epsilon or omega files and uses wall functions for these too. Therefore create a "nut" file with also a "fixedValue" at the wall in order to keep the original files from being overwritten.

Regards, Sebastian
nero235 is offline   Reply With Quote

Old   February 11, 2016, 08:11
Default
  #2
Member
 
Sebastian W.
Join Date: Nov 2012
Location: Saxony, Germany
Posts: 42
Rep Power: 6
nero235 is on a distinguished road
Send a message via ICQ to nero235
Well, changing the BC of k and epsilon from wall functions to fixedValues didn't fix my problem. The crash happens at different physical times, which is weird because this doesn't look like a setup problem. If the BCs or the solver parameters were wrong, the crash would happen always at exactly the same time step. I am using OF 2.3 with MPI version 1.4.3. The error messages change also. I am thinking it maybe a problem with MPI, rather than OF since I could not reproduce the error in serial mode.


Regards, Sebastian


fehler_alt_parallel20_case1.txt

fehler_neu_parallel20_case1.txt
nero235 is offline   Reply With Quote

Old   February 15, 2016, 06:00
Default
  #3
Member
 
Sebastian W.
Join Date: Nov 2012
Location: Saxony, Germany
Posts: 42
Rep Power: 6
nero235 is on a distinguished road
Send a message via ICQ to nero235
So, mpirun wasn't the problem either. Neither was the OF version or any of my BCs or ICs. I've build a smaller case where I had explicit non-orthogonal and skewed cells at the walls. CheckMesh had no problems with the mesh though. The maximum non-orthogonality was 45 and the skewness 1.3. This is more than ok.

This case didn't even run under normal circumstances. The problem was always high bounding epsilon and k values which either caused the iterations to exceed 1000 or caused a FPE which resulted in a solver crash.

I run my cases always with non-orthogonal correction because I always skewed cells in my meshes. I couldn't even believe to run this case turbulent on this mesh with multiphaseInterFoam anymore. Since I tried almost everything without success. However I found the problem in this case. What happened was that the solver tried to correct the epsilon and k values since the correction was higher than 1. The correction is however not limited when using the corrected schemes in laplacianSchemes and snGradSchemes. Using:

Code:
laplacianSchemes
{
    default        Gauss linear limited 0.333;

snGradSchemes
{
    default        limited 0.333;
}
helped by limiting the maximum correction. The 0.333 means that the maximum correction has to be < 0.5 x the orthogonal part of the value. In the contrary the corrected schemes use explicit non-orthogonal correction.

Hope this helps someone Regards,

Sebastian

screen_pv.jpg
nero235 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
Divergence in AMG solver! marina FLUENT 15 August 9, 2016 20:15
Enhanced Wall Treatment paduchev FLUENT 19 April 10, 2016 09:57
Surface Integrals of Species Mass Flow to Wall Incorrect koad FLUENT 4 January 12, 2016 17:38
Difficulty In Setting Boundary Conditions Moinul Haque CFX 4 November 25, 2014 18:30
Enhanced wall treatment and Enhanced wall functions Alina FLUENT 2 January 3, 2012 19:48


All times are GMT -4. The time now is 23:53.