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

Dam break

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

Like Tree3Likes
  • 1 Post By Jack_Landis
  • 2 Post By Artur

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 9, 2016, 13:21
Question Dam break
  #1
Member
 
Jack_Landis's Avatar
 
Join Date: Feb 2016
Posts: 32
Rep Power: 10
Jack_Landis is on a distinguished road
Hi everyone,

I'm quite new at using openFoam and in general CFD. I can't understand a part of he fvSolution file.

Code:
solvers
{
    "alpha.water.*"
    {
        nAlphaCorr      2;
        nAlphaSubCycles 1;
        cAlpha          1;

        MULESCorr       yes;
        nLimiterIter    3;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-8;
        relTol          0;
    }

    pcorr
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-5;
        relTol          0;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-07;
        relTol          0.05;
    }

    p_rghFinal
    {
        $p_rgh;
        relTol          0;
    }

    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-06;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor   no;
    nOuterCorrectors    1;
    nCorrectors         3;
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    equations
    {
        ".*" 1;
    }
}
1) Why alpha.water is posed between apices?
2) Why is it needed to use p_rgh instead of p?
3) Why is it needed to specify p_rghFinal and how is it defined here?
4) What is pcorr?
5) Does ".*" in relaxation factors mean that 1 is applied to each field?

I know these are probably trivial questions, but I really don't know where to find information about that...

Can someone help me?
Can you also suggest me a way to get a deeper understanding than that given by the guide?

Thank you very much!
xoitx likes this.
Jack_Landis is offline   Reply With Quote

Old   March 12, 2016, 14:20
Default
  #2
Senior Member
 
Artur's Avatar
 
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 372
Rep Power: 19
Artur will become famous soon enough
Hi,

1. It needs the "" because otherwise the dot in the line would make the reader cough
2. Multiphase solvers in OpenFOAM tend to solve for pressure less the hydrostatic component rho*g*z, i.e. the p_rgz, or dynamic pressure. This makes some tricks with setting the BCs easier. Note that the solver still computes total pressure and saves it as p based on the gravity field you specify in constant/g
3. p_rghFinal describes settings used for the final iteration within the time step. Whether it's needed depends on whether you're using pimple or piso and on other things. If you look at the PIMPLE tutorials all of the cases have *Final defined for all the fields because the solver needs those.
4. pcorr is the pressure correction, see e.g. here: https://en.wikipedia.org/wiki/Pressu...rection_method ; in short, it's a standard way of coupling pressure and velocity for incompressible flows, or from fvSolution perspective yet another field that needs to be solved for.
5. you are correct, the ".*" is an OpenFOAM wildcard

I suggest having a look here for some basic background on CFD, will explain what pressure corrections are, what do the schemes and solvers actually do and more; totally recommend to anyone new to CFD:
https://engineering.purdue.edu/ME608/webpage/main.pdf

All the best,

A
Jack_Landis and xoitx like this.
Artur is offline   Reply With Quote

Old   March 16, 2016, 06:56
Default
  #3
Member
 
Jack_Landis's Avatar
 
Join Date: Feb 2016
Posts: 32
Rep Power: 10
Jack_Landis is on a distinguished road
Hi Artur!

Thank you very much for the explanation and the suggestions! I think that book is very well explained!
Jack_Landis 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
[DesignModeler] DesignModeler Scripting: How to get Full Command Access ANT ANSYS Meshing & Geometry 53 February 16, 2020 16:13
Dam break simulation water level decreases over time aarratia FLUENT 1 May 9, 2014 11:25
compressible dam break simulation smsanth OpenFOAM Running, Solving & CFD 0 September 2, 2013 03:51
3D dam break modeling(earthen dam) yasharif FLUENT 0 December 11, 2011 02:25
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 13:24


All times are GMT -4. The time now is 08:49.