
[Sponsors] 
January 25, 2013, 11:02 
Perfect fluid implementation  interFoam

#1 
New Member
Gaetano
Join Date: Jul 2012
Posts: 18
Rep Power: 6 
Hi all.
This is my first post here, so I'm going to introduce myself: my name's Gaetano and I'm doing a PhD in Chemical Engineering in Naples (Italy). I've been lurking those forums for at least 6 months and I found answers to almost all my questions. This one, however, seems to be a bit more tricky. I'm trying to have interFoam working with one of the two phases being a perfect fluid, i.e. having zero density and viscosity (I'd like to simply put "0" in the dictionary transportProperties). In doing so, I need to avoid all the division by density, if any. I found some in class twoPhasesMixture and I created a new class twoPhaseMixturePerfect with a little (tricky) workaround in it. When I tried to solve the damBreack tutorial with my interPerfectFoam I found this error at the very first step:  Starting time loop Courant Number mean: 0 max: 0 Interface Courant Number mean: 0 max: 0 deltaT = 0.00119048 Time = 0.00119048 MULES: Solving for alpha1 Phase1 volume fraction = 0.130194 Min(alpha1) = 0 Max(alpha1) = 1 MULES: Solving for alpha1 Phase1 volume fraction = 0.130194 Min(alpha1) = 0 Max(alpha1) = 1 #0 Foam::error:rintStack(Foam::Ostream&) in "/share/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/share/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 __restore_rt at sigaction.c:0 #3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) in "/share/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 main in "/local/home/iitcrib3/GaetanoDM/damBreak/interPerfectFoam" #5 __libc_start_main in "/lib64/libc.so.6" #6 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const in "/local/home/iitcrib3/GaetanoDM/damBreak/interPerfectFoam" Floating point exception  It seems that there is a problem with a division (see #3 above) in the p_rgh solver (as the next step should be "DICPCG: Solving for p_rgh ..."), but my insight into the problem ends here. So, here's my question: what does the above error mean? Is there any division with a density in the denominator anywhere in interFoam? But, besides the answers, I'm also looking for advice from expert foamers like many here: is there any chance that my attempt to "hack" interFoam could fit in its "architecture"? I mean: does the algorithm require a division by a density? I'd like to modify only the "shell" and not the "core" of interFoam (sorry for the poor analogy: I can't figure out any better way to make my point). Thanks in advance, Gaetano 

January 25, 2013, 11:20 

#2 
Member
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 8 
Are you sure that the density should be 0?! As far as I know (and can find) the definition of a perfect fluid is only that the viscosity is 0, not that the density is 0.


January 25, 2013, 11:33 

#3 
New Member
Gaetano
Join Date: Jul 2012
Posts: 18
Rep Power: 6 
I think that would be an Euler fluid, but I might have chosen a wrong name for my fluid. I confirm that I'm looking for something with no inertia and no viscosity.


January 25, 2013, 11:44 

#4 
Member
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 8 
Ok, in that case I would suggest using interTrackFoam from the OpenFOAMextend project. If you define a single mesh for fluid 1 and no mesh for fluid 2, you are basically assuming fluid 2 to have 0 density and 0 viscosity.


January 25, 2013, 13:19 

#5 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,740
Rep Power: 29 
And a small detail with respect to the density of the fluid. You will end up dividing by zero, since you create a term, which out of memory, is called rAU in the pEqn.H file. This is essentially an interpolation of your diagonal coefficients in your matrix for the momentum equation. These coefficients scale by rho (density).
The _inverse_ of this field is acting as a diffusion coefficient for the pressure on the Poisson equation, hence you are indeed dividing by zero. Kind regards, Niels 

January 25, 2013, 15:42 

#6 
Member
Nick Gutschow
Join Date: Jan 2013
Posts: 36
Rep Power: 6 
I am not too expereinced in OpenFOAM, but can you do the ol'e 0~ some tiny tiny number? That has worked for me in other modeling programs before.
NG 

January 26, 2013, 06:27 

#7 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,226
Rep Power: 23 
While this is an idea worth trying, I suspect spurious currents to kill you here, as they scale with the density and viscosity ratio between both fluids.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. 

January 26, 2013, 13:54 

#8 
New Member
Gaetano
Join Date: Jul 2012
Posts: 18
Rep Power: 6 
Well, I've already thought about the possibility of rho=eps, but I'm wondering if it would be possible to have it *exactly* zero.
Here's where my evils turn true (bold mine): It seems that I do have to play with the matrix coefficients, and I'd really like to avoid such a task. But still: would it be possible to rewrite the term rAU? And most important: is it worth an attempt? I'm not really a numeric guy... 

Tags 
floating point exception, interfoam, perfect fluid, zero density, zero viscosity 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
Locating and observing a transient fluid phenomena  Chander  CFX  2  September 25, 2011 18:49 
error using combination of step function  xujjun  CFX  1  January 15, 2008 17:46 
What is the total energy for incompressible fluid?  Harry Dong  Main CFD Forum  12  February 4, 2006 01:55 
Help With Modeling A Projectile Fluid In Flight.  Dzeff G.  Main CFD Forum  0  December 10, 1998 22:24 