# interFoam algorithm

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

 February 18, 2013, 06:46 interFoam algorithm #1 New Member   Pierre HORGUE Join Date: May 2009 Posts: 24 Rep Power: 9 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

 February 19, 2013, 07:20 #2 New Member   Pierre HORGUE Join Date: May 2009 Posts: 24 Rep Power: 9 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

 February 19, 2013, 08:51 #3 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 1,139 Rep Power: 20 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. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2

 February 19, 2013, 08:58 #4 New Member   Pierre HORGUE Join Date: May 2009 Posts: 24 Rep Power: 9 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.

 February 19, 2013, 10:50 #5 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 1,139 Rep Power: 20 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. *Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2

 February 19, 2013, 11:03 #6 New Member   Pierre HORGUE Join Date: May 2009 Posts: 24 Rep Power: 9 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

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post DanM OpenFOAM Running, Solving & CFD 11 January 5, 2013 07:21 Krishna Sandeep OpenFOAM Running, Solving & CFD 3 June 14, 2012 01:32 sxhdhi OpenFOAM Running, Solving & CFD 3 May 5, 2009 21:58 Yan Kai Main CFD Forum 0 April 18, 2007 03:48 Yan Kai FLUENT 0 April 13, 2007 23:17

All times are GMT -4. The time now is 13:05.