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

interFoam algorithm

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 18, 2013, 06:46
Default interFoam algorithm
  #1
New Member
 
Pierre HORGUE
Join Date: May 2009
Posts: 17
Rep Power: 8
Pedro24 is on a distinguished road
Hi ,

For each time step, I found that the order of the computations is a little bit strange.

1) It computes the new surface force term using the alpha field at the time "n"
Code:
       twoPhaseProperties.correct();
2) Compute the alpha field "n+1" using the velocity field U at the time "n"
Code:
        #include "alphaEqnSubCycle.H"
3) Compute the pressure-velocity field at the time "n+1" using the surface term force at the time "n"
Code:
        // --- Pressure-velocity PIMPLE corrector loop
        while (pimple.loop())
        {
            #include "UEqn.H"

            // --- Pressure corrector loop
            while (pimple.correct())
            {
                #include "pEqn.H"
            }

            if (pimple.turbCorr())
            {
                turbulence->correct();
            }
        }
Why don't we inverse the step 1 and 2. It will allows to use the surface term force at the time "n+1" in the navier-stokes equations ?

It seems more logical to update the surface force term (step 1) just after computing the new alpha field. In my mind, the algorithm should be :

1) update properties time "n"
2) compute implicitly velocity-pressure field "n+1"
3) compute alpha field "n+1" using the velocity-pressure previously computed

Am I wrong ?

Thank You,

Pierre
Pedro24 is offline   Reply With Quote

Old   February 19, 2013, 07:20
Default
  #2
New Member
 
Pierre HORGUE
Join Date: May 2009
Posts: 17
Rep Power: 8
Pedro24 is on a distinguished road
I confirm what I said before, this is an error in the "interFoam" solver (and the derivated solvers).

In the H. Rusche thesis, page 162, we can see the following solution procedure :

steps 1-4 : refer to the moving frame

step 5 : transport "alpha1"

step 6 : update properties (smooth gamma => curvature computation => surface force term)

step 7 and 8 : PISO-loop to compute pressure-velocity fields.


Maybe this error should be reported to the OpenFOAM Foundation to correct it for the following versions.


Pierre
Pedro24 is offline   Reply With Quote

Old   February 19, 2013, 08:51
Default
  #3
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
How are step 5-8 different than what is already implemented?
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   February 19, 2013, 08:58
Default
  #4
New Member
 
Pierre HORGUE
Join Date: May 2009
Posts: 17
Rep Power: 8
Pedro24 is on a distinguished road
In the current version of "interFoam", the step 6 is computed before the step 5.

First it computes the surface force term :

Code:
twoPhaseProperties.correct();
and then it computes the new alpha1 field :

Code:
#include "alphaEqnSubCycle.H"
So, the surface force term used in the PISO loop is computed using the old-time alpha field, which is different from the usual solution procedure.
Pedro24 is offline   Reply With Quote

Old   February 19, 2013, 10:50
Default
  #5
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
The interface curvature for the surface force term is calculated by calling interface.correct() after the alphaEqnSubCycle.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   February 19, 2013, 11:03
Default
  #6
New Member
 
Pierre HORGUE
Join Date: May 2009
Posts: 17
Rep Power: 8
Pedro24 is on a distinguished road
Ok, I had inverted the "correct" function of twoPhaseMixture for the viscosity with the "correct" function of interfaceProperties for the curvature.

Thank you for your reply
Pedro24 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
interFoam vs. simpleFoam channel flow comparison DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21
Does PISO algorithm work with interfoam in openFOAM 2.1.0? Krishna Sandeep OpenFOAM Running, Solving & CFD 3 June 14, 2012 01:32
Open Channel Flow using InterFoam type solver sxhdhi OpenFOAM Running, Solving & CFD 3 May 5, 2009 21:58
About Phase Coupled SIMPLE (PC-SIMPLE) algorithm Yan Kai Main CFD Forum 0 April 18, 2007 03:48
About Phase Coupled SIMPLE (PC-SIMPLE) algorithm Yan Kai FLUENT 0 April 13, 2007 23:17


All times are GMT -4. The time now is 01:11.