- **OpenFOAM**
(*https://www.cfd-online.com/Forums/openfoam/*)

- - **fvc::div(phi,rho) vs fvc::div(phi)**
(*https://www.cfd-online.com/Forums/openfoam/84642-fvc-div-phi-rho-vs-fvc-div-phi.html*)

fvc::div(phi,rho) vs fvc::div(phi)hello
could you tell me whats the difference between fvc::div(phi,rho) vs fvc::div(phi) ? thank in advance |

Quote:
phi is rho*U so div(phi)=divergence of ((rho)U) and div (phi,U)=divergence of ((rho)UU) I haven't seen div(phi,rho) but it should be divergence of ((rho)(rho)U). Read user guide for more information: http://www.openfoam.com/docs/user/fv...20-1120004.4.5 Regards,:) |

Hi, may I also ask, in icoFoam I noticed that
fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(nu, U) why is phi used in convective div() term when nu (I suppose kinematic viscosity) is used in the laplacian term? shouldn't left hand side be divided by rho? |

phi = Uf & Sf, which Sf is face area , and Uf is velocity at face center
so its a volume flux {m.s} and nu = mu/rho :) |

Please correct me if I am wrong.
ddt(U) [m/s2] laplacian(nu,U) [m/s2] I assume nu here = mu/rho grad(p) [m/s2] I assume pressure here has been divided by rho as well? However, div(phi, U) If phi = rho * U, then the unit will be different? |

Hi,
You should realise that the definition of phi is different for an incompressible flow solver (e.g. icoFoam) than for an compressible flow solver. For an incompressible flow solver phi = U, for a compressible flow solver phi = rho*U. Thus, the face flux for an incompressible flow solver is (S_f · phi_f) = (S_f · U_f), which is exactly what Nima was trying to tell you. To be honest, the notation in OpenFOAM is a bit sloppy. The face flux is given the name phi, which is confusing if you write fvm::ddt(U) + fvm::div(phi, U) - fvm::laplacian(nu, U). I suggest you have a look at section 2.4 of the Programmer's Guide, which is located in the $WM_PROJECT_DIR/doc/Guides-a4 directory. |

Hello and thank you for the precision .
I am actually trying to run a poiseuille case in channel with cyclic conditions. I don't know If I have to choose icoFoam or channelFoam solver. Actually in the channelFoam code I don't know what represents sgsModel->divDevBeff(U) in the equation? see http://foam.sourceforge.net/docs/cpp/a02641_source.html on line 63 Thank tou for your answer. Camille |

Hi Camille,
First, I think it would have been more appropriate to open a new thread for this. My guess is that a little searching on the forum would have gotten you a long way as well. To answer your question, go with the channelFoam solver. It has been developed to do exactly what you want. Have a look at the chan395 tutorial. The definition of divDevBeff depends on the particular subgrid-scale model that you use. For most subgrid-scale models this term is defined in GenEddyVisc.C. http://foam.sourceforge.net/docs/cpp...ce.html#l00096 Use Doxygen to find out more about the different subgrid-scale models. Doxygen is there for a reason. |

Thank you for your answer actually I also have to kearn how to search correctly on the help guide ^^
but so , what s the difference between nuEff and nu? and what does the temperature T have to do here? it because the problem is coupled? in laminar case we don't care? thank you sorry it s not so easy to come from nowhere .. I have then introduced a new subject for other questions about Poiseuille. here: http://www.cfd-online.com/Forums/ope...tml#post387650 |

If alpha = 0.5*Foam::erf(4.0*(T-Tmelt)/(Tl-Ts))+scalar(0.5);
Are fvc::div(phi,alpha) and 4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*(U & fvc::grad(T)) the same? From the results, they are not quite the same. Why? Is there anything different other than a simple algebraic transformation? |

Hi Chad,
No, those are not the same. The most important difference is the location at which the expressions are evaluated. If fvc::div(phi,alpha) is used, alpha is evaluated at the cell face according to equation (2.16) in the Programmer's Guide. For a central difference scheme this value is obtained by linear interpolation of the cell center values. If 4.0*exp(-pow(4.0*(T-Tmelt)/(Tl-Ts),2))/Foam::sqrt(pi)/(Tl-Ts)*(U & fvc::grad(T)) is used, the whole expression is evaluated at the cell center. You could write out the seperate discretisations and you will see that they are not the same. I would recommend you to use fvc::div(phi,alpha), since it maintains the conservative form of the convection term. |

Quote:
But at t=120s, temperature field is: ( 309.228 306.009 302.865 303.179 . . . ) As you can see, the temperature field is not monotone which is not correct. |

Hi Chad,
It is hard to tell what the source of your problem is, because you are not giving any details about the simulation itself. I suggest you open a new thread about your problem, so we stay on-topic here. Try to give as much details about your simulation as possible. You could think of boundary conditions, grid resolution, numerical schemes, etc. Perhaps it is a good idea to post a part of the solver output aswell. |

Maysam,
Do you know if does exist a tutorial or guide that list side to side the mathematical equations on one side and on the other side how they are written in the openFoam code. I have found something here http://www.foamcfd.org/Nabla/guides/UserGuidese14.html, but I was searching for something with some practical examples for a newbie. |

All times are GMT -4. The time now is 20:56. |