
[Sponsors] 
October 22, 2008, 00:39 
What is phi in simpleFoam

#1 
New Member
ehsan vaghefi
Join Date: Mar 2009
Posts: 9
Rep Power: 17 
Hi there
I have been using simpleFoam to solve my problem, I was wondering the what is the "phi" file that openFoam is calculating ? a more general question , can calculate fluxes (as vectors) on each of nodes ? Cheers. Ehsan 

October 22, 2008, 08:14 
As this phi question creeps up

#2 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,225
Rep Power: 51 
As this phi question creeps up every 2 weeks or so, I thought it might be a good candidate for the FAQ: http://openfoamwiki.net/index.php/Main_FAQ#What_is_the_field_phi_that_the_solver _is_writing
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

September 7, 2011, 12:31 
phi Field in Momentum and Eenrgy Equations

#3 
Member
,...
Join Date: Apr 2011
Posts: 92
Rep Power: 14 
Hi Everybody
I have added temperature equation to icoFoam in the manner that has been described in http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam The main part is fvScalarMatrix TEqn ( fvm::ddt(T) + fvm::div(phi, T)  fvm::laplacian(DT, T) );From a mathematical manipulation i founded out that phi should be "ui + vj" here. And this vector form for phi is in complete disagreement with what has been described for the field phi in the following page  "http://openfoamwiki.net/index.php/Main_FAQ" in section "3.1.3 What is the field phi that the solver is writing" "3.1.3 What is the field phi that the solver is writing " The answer in this file is the mass flow through the cell faces ( with the area of the face).  In Summary: Do you guys know whether phi is different in the vector form of the momentum equation and scalar temperature equation! What I had founded out is that YES, it should be different. But I am NOT sure! I would appreciate if someone helps me!! 

September 7, 2011, 19:25 

#4  
Senior Member
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 621
Rep Power: 0 
Quote:
Dan 

July 22, 2013, 12:10 
The units do not seem to match

#5 
New Member
Sri
Join Date: Nov 2012
Posts: 10
Rep Power: 13 
Hi,
Is Phi just U dotted on to A or rhoU dotted on to A as you have described on the page. The table has units cu.m/s which would fit the first description of Phi (U dotted on to A). Thanks, Sri 

September 28, 2013, 03:21 

#6 
New Member
eric
Join Date: Nov 2010
Location: Vancouver, Canada
Posts: 16
Rep Power: 16 
I just start learning FOAM and also have the same question about phi.
In the equation of motion UEqn, phi seems to be rho*U. But in the equation of energy TEqn, phi is U. This phi bothers me a lot. Can anyone explain it please. Thanks in advance. 

September 29, 2013, 07:37 

#7 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,982
Blog Entries: 45
Rep Power: 128 
Greetings to all!
openfoamwiki.net is undergoing some changes on the FAQ section. I've updated the FAQ associated to this thread's topic: http://openfoamwiki.net/index.php/FA..._is_writing.3F @Eric: You didn't mention which solver you were looking at, but the answer should be simple: compressible solvers use the rho field; incompressible solvers do not use the rho field. If look at the user guide, section "2.1.1.3 Physical properties", you'll see that the fluid density is implied when using "kinematic viscosity nu": http://www.openfoam.org/docs/user/cavity.php Best regards, Bruno PS: I also merged the two threads where Eric had posted, because it made sense to keep the two threads in a single discussion.
__________________


September 29, 2013, 12:00 

#8 
New Member
eric
Join Date: Nov 2010
Location: Vancouver, Canada
Posts: 16
Rep Power: 16 
Thank you very much for the explanation. I am now much clearer with this little guy phi.


July 19, 2024, 17:01 

#9  
New Member
Masoud Rvn
Join Date: Sep 2023
Posts: 9
Rep Power: 3 
Quote:


October 5, 2024, 08:49 

#10 
New Member
Pouya Namakshenas
Join Date: Oct 2024
Posts: 1
Rep Power: 0 
If you look at the solver code for instance in $FOAM_SOLVERS/basic/scalarTransportFoam/createFields.H, you can see that it reads createPhi.H, and if you refer to $FOAM_SRC/finiteVolume/cfdTools/incompressible/createPhi.H, you see
surfaceScalarField phi ( IOobject ( "phi", runTime.timeName(), mesh, IOobject::READ_IF_PRESENT, IOobject::AUTO_WRITE ), linearInterpolate(U) & mesh.Sf() ); so for the solvers such as scalarTransport and the ones consider incompressible fluid phi = U*Sf [m³/s] However, for compressible solvers like rhoPimpleFoam it reads compressibleCreatePhi.H instead of createPhi.H and if you refer to that you can see surfaceScalarField phi ( IOobject ( "phi", runTime.timeName(), mesh, IOobject::READ_IF_PRESENT, IOobject::AUTO_WRITE ), linearInterpolate(rho*U) & mesh.Sf() ); hence, phi = rho*U*Sf [kg/s] for compressible solvers. I hope it helps 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SimpleFoam nutilda an R  linnemann  OpenFOAM Running, Solving & CFD  13  October 9, 2014 09:14 
Problems with the RSM in simpleFoam  sberg  OpenFOAM Running, Solving & CFD  10  February 25, 2014 20:39 
NACA0012 with simpleFOAM  nuovodna  OpenFOAM Running, Solving & CFD  7  May 19, 2010 05:58 
Using simpleFoam with water  nico765  OpenFOAM Running, Solving & CFD  7  October 23, 2007 06:39 
SimpleFoam woes  msrinath80  OpenFOAM Bugs  2  April 13, 2007 11:15 