# Problem with alphas of interMixingFoam

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 4, 2016, 08:41 Problem with alphas of interMixingFoam #1 New Member   Join Date: Apr 2016 Posts: 6 Rep Power: 7 Hello, I am using the interMixingFoam solver for a tri-phase case. From the User Guide, I know that interMixingFoam : "Solver for 3 incompressible fluids, two of which are miscible, using a VOF method to capture the interface". Alpha1 is the immiscible fluid while alpha2 and alpha3 are the miscible fluids. The simulation run well but in post-processing I see that alpha1 and alpha2 mix which it should not happen. Does anyone know why?

 September 7, 2016, 04:00 #2 Member   Join Date: May 2016 Posts: 39 Rep Power: 7 There is a mistake in the code and it only has to do with one command line being executed too late in the loop (it took me way too long to figure this one out ) The way it works is in alphaEqns.H you have a for loop which does following things: for loop: create the complete convective flux for alpha 1 create the bounded (upwind) flux for alpha 1 calculate the flux correction for alpha 1 calculate the limiter for alpha 1 [this calculates lambda coefficients] create the complete convective flux for alpha 2 create the bounded (upwind) flux for alpha 2 calculate the flux correction for alpha 2 calculate the limiter for alpha 2 [this calculates lambda coefficients] construct the limited flux for alpha 1 construct the limited flux for alpha 2 ... Now as you can see the step 9 should be earlier, between steps 4 and 5. The reason is step 4 calculated you coefficients for bounding your phase 1, but those are not actually used for construction of the limited flux of phase 1 and are overwritten by coefficients calculated for bounding of phase 2 (step 8). In a sense you are using the same lambdas for construction of both fluxes, which is incorrect. Correct the mistake, recompile and you should be fine. P.S. also the tolerance for alphas in fvSolutions should be smaller then in tutorial (at least for my case) This solves the problem of mixing of phases 1 and 2, but I also think there is a problem with the way diffusion is written into the program, because I keep getting the same result no matter what diffusion constant I use. Still trying to figure that one out. Hope it still helps

October 10, 2017, 10:26
#3
New Member

Gary
Join Date: Oct 2017
Posts: 4
Rep Power: 5
Quote:
 Originally Posted by dzordz ..., but I also think there is a problem with the way diffusion is written into the program, because I keep getting the same result no matter what diffusion constant I use. Still trying to figure that one out.
Any updates on this? Does it have to do with numerical diffusion?

 Tags alphas, immiscible fluid flow, intermixingfoam, simflow

 Thread Tools Search this Thread Search this Thread: Advanced Search 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 Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [Other] engineFoam new mesh problem ayhan515 OpenFOAM Meshing & Mesh Conversion 5 August 10, 2015 08:45 Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43 JFDC FLUENT 1 July 11, 2011 05:59 Se-Hee CFX 2 June 10, 2007 06:29 ParodDav CFX 5 April 29, 2007 19:13

All times are GMT -4. The time now is 19:27.

 Contact Us - CFD Online - Privacy Statement - Top