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

laminar simplefoam diverged (axissymmetric)

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 26, 2017, 08:36
Unhappy laminar simplefoam diverged (axissymmetric)
  #1
New Member
 
nicky chaigneau
Join Date: Jun 2017
Posts: 12
Rep Power: 5
chicky is on a distinguished road
Hello

I use openFoam to create a tutorial for this library. I have to introduce the axissymmetric 2D pipe flow using laminar simpleFoam. But every time i launch the solving it diverged. So I certainly made a mistake somewhere but I cannot find it.

I try to change the relaxation factor and the solver but it don't solve the problem.

can you help me please

you will find my fvschemes and fv solution here with the log :
Attached Files
File Type: txt fvSolution.txt (1.6 KB, 30 views)
File Type: txt fvSchemes.txt (1.3 KB, 13 views)
File Type: txt log.txt (5.0 KB, 9 views)
chicky is offline   Reply With Quote

Old   June 26, 2017, 08:45
Post
  #2
Member
 
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 97
Rep Power: 7
Swagga5aur is on a distinguished road
Hello Nicky,

I would like to help you and from your log files it seems that you continuity is the issue as well as pressure (due to the high number of iterations).
However, I'm not sure that the issue is your fvSolution or fvSchemes, and would like if you could send your case directory so that I can conduct more testing to determine what the issue is.

My initial thoughts is that it is a boundary condition issue regarding either velocity or pressure fields.

Best regards, Lasse

Last edited by Swagga5aur; June 26, 2017 at 14:02.
Swagga5aur is offline   Reply With Quote

Old   June 27, 2017, 04:24
Default
  #3
New Member
 
nicky chaigneau
Join Date: Jun 2017
Posts: 12
Rep Power: 5
chicky is on a distinguished road
Thank you it's very kind

I study a pipe with 10mm radius and 60mm length waith air. I use the Reynolds analogie to work with Re=100 so I have a mesh defined for 6m length and 1m radius (axis-symmetric so it is 0.5m). the inlet velocity is 14.61 m/s and the viscosity 0.147 mē/s.

I have put the initial condition for velocity with internalField uniform (14.61 0 0) to help the solver to converge but doesn't matter it diverged anyway.

I put the file with the salome meshing in the gz archive.

thank you very much
Attached Files
File Type: gz poiseuille.tar.gz (138.5 KB, 11 views)
chicky is offline   Reply With Quote

Old   June 27, 2017, 05:21
Default
  #4
New Member
 
nicky chaigneau
Join Date: Jun 2017
Posts: 12
Rep Power: 5
chicky is on a distinguished road
Okaye in fact I think I have found my problem.

I add one line in fvSolution that is

consistent yes;

It converged easily after.
chicky is offline   Reply With Quote

Old   June 27, 2017, 07:28
Post
  #5
Member
 
Lasse Brams Vinther
Join Date: Oct 2015
Posts: 97
Rep Power: 7
Swagga5aur is on a distinguished road
Good to see you found a solution, I also noticed in that the relaxation factors in the fVsolution was defined wrong.

Applying the following in the fVsolution resulted in a converging solution:
Code:
SIMPLE
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
        residualControl
    {
        p               1e-2;
        U               1e-3;
    }

}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7; // 0.9 is more stable but 0.95 more convergent
    }
}
This also explains why the consistent yes; solves the issue as simplec does not need any relaxation of the pressure field, according to http://www.openfoam.com/documentatio...fvSolution.php

Have a nice day
Swagga5aur is offline   Reply With Quote

Old   June 27, 2017, 08:31
Default
  #6
New Member
 
nicky chaigneau
Join Date: Jun 2017
Posts: 12
Rep Power: 5
chicky is on a distinguished road
Ok I have undedrstand what you mean in your response. The pitzDaily case use consistent yes; (use of SIMPLEC) to solve the problem. But in fact I want to compare with fluent simulation to make a benchmark and fluent is using by default SIMPLE. It is good to know that I need to have a fields relaxation factor for pressure if I am not using SIMPLEC.

You solved my problem. thank you very much
chicky is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with simpleFoam, laminar pipeCyclic fantaste OpenFOAM Running, Solving & CFD 0 January 14, 2015 04:37
NonNewtonian, steady state, Laminar, Incompressible for simpleFoam. ngjaeho OpenFOAM Pre-Processing 1 December 19, 2014 07:08
SimpleFOAM issues solving laminar and Kepsilon AndrewMortimer OpenFOAM Running, Solving & CFD 1 November 4, 2013 05:28
Laminar simpleFoam and inviscid simpleFoam herenger OpenFOAM Running, Solving & CFD 7 July 11, 2013 07:27
SimpleFoam: Laminar vs. Turbulent Convergence JasonG OpenFOAM 0 June 2, 2011 09:29


All times are GMT -4. The time now is 08:14.