
[Sponsors] 
November 17, 2012, 19:09 
pEqn.flux()

#1 
Member
Charlie
Join Date: Dec 2010
Location: USA
Posts: 82
Rep Power: 8 
Hi Foamers,
I've got a little confusion here about the pEqn.flux(). So, what does it really mean, say we want to solve the following momentum equation: ddt(voidfraction*U) + convection_terms == voidfraction * grad(p) + Other terms. As the first step, in OpenFOAM, the following UEqn is solved: ddt(voidfraction*U) + convection_terms == Other terms. and discretise this equation into linear system, we could obtain the following form, that is: A() *[U] = H(). and we can define phi = fvc::interpolate (U) & mesh.Sf(); which is the surface mass flux. and the "real" velocity field should be : A() *U = H() voidfraction * grad(p) . To satisfy the continuity equation, we have: ddt(voidfraction) + div(voidfraction*U) = 0 Thus the pressure equation becomes: pEqn == { laplacian(voidfraction*voidfraction/A(), p) = ddt(voidfraction) + div(voidfraction*phi) } then, my question is, pEqn.flux() = SnGrad(p) or pEqn.flux() = (voidfraction*voidfraction/A())*SnGrad(p) how could we update the phi after we solved the pressure equation, which of the following is right? (1) phi = pEqn.flux(); (2) phi = (1/A()) * (voidfraction*pEqn.flux()/(voidfraction*voidfraction/A())); this could make a big difference is we want to model the flow through a porous media, and I still don't quite get the exact meaning of pEqn.flux(), though it is stated in the following link that The .flux method includes contributions from all implicit terms of the pEqn (the Laplacian) http://openfoamwiki.net/index.php/IcoFoam Could anybody help me with this problem? Thanks! 

November 21, 2012, 09:46 

#2 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 438
Rep Power: 17 
Hi, the pEqn you're assembling is:
Code:
fvScalarMatrix pEqn ( fvm::laplacian(rUA, p) == fvc::div(phi) ); so that the method pEqn.flux() gives you the discrete version of the flux of p, which is this is not calculated by explicit operators like fvc::grad but directly using the matrix's coefficients. Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar Last edited by santiagomarquezd; November 21, 2012 at 16:16. 

November 21, 2012, 15:08 
That's great, Thanks!

#3 
Member
Charlie
Join Date: Dec 2010
Location: USA
Posts: 82
Rep Power: 8 
Hi, Santiago,
Thanks very much for your kind reply. That's great, it really helps me a lot to understand the code. According to your explaination, then I guess, my option (2) should be the right way to correct the phi, right? (2) phi = (1/A()) * (voidfraction*pEqn.flux()/(voidfraction*voidfraction/A())); Regards, Charlie 

November 21, 2012, 15:51 

#4 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 438
Rep Power: 17 
Looking at the equation you want to solve it seems to be (2), please check lines 7893 of
https://github.com/OpenFOAM/OpenFOAM...lerFoam/pEqn.H which is the code for pEqn.H in twoPhaseEulerFoam. This solver has the kind of momentum equations that you dealing with. Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar Last edited by santiagomarquezd; November 21, 2012 at 16:16. 

November 21, 2012, 16:08 
Thanks!

#5 
Member
Charlie
Join Date: Dec 2010
Location: USA
Posts: 82
Rep Power: 8 
Thanks!
My first clue of my doubt also comes from the twoPhaseEulerFoam, I think, right now, I have a clear understanding of how the pressure is corrected, Thanks again! Regards, Charlie 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
phi = pEqn.flux() vs. linearInterpolate(U) & mesh.Sf()  santiagomarquezd  OpenFOAM Programming & Development  32  June 12, 2014 01:50 
pEqn.flux()  ata  OpenFOAM  6  August 25, 2013 22:31 
pEqn.flux()  ata  OpenFOAM  2  January 24, 2011 23:31 