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

- - **IcoFoam Is it a NavierStokesEquation**
(*https://www.cfd-online.com/Forums/openfoam/60735-icofoam-navierstokesequation.html*)

Hi,
I try to analyse the icHi,
I try to analyse the icoFoam Solver. The Solver solves the Equation: ddt(U)+div(phi,U)-Laplacian(nu,U)=-grad(p) this themes seems to be a Navier-Stokes-Equation but I miss an U at div(phi,U). The Navier-Stokes Equation I know sould be: ddt(U)+U*div(phi,U)-Laplacian(nu,U)=-grad(p) Does the U appear later in the discretisation or is it a variation of the Navier-Stokes-Equation? Thx, Jörn |

No: the N-S equation that _youNo: the N-S equation that _you_ know is
ddt(U)+U*div(U)-Laplacian(nu,U)=-grad(p) Since div(u)=0 we can rearrange this as ddt(U)+div(U*U)-Laplacian(nu,U)=-grad(p) The finite volume discretisation however linearises this by representing one of the U terms in div(U*U) as the flux phi, hence ddt(U)+div(phi,U)-Laplacian(nu,U)=-grad(p) We then need to iterate around a bit to take account of the fact that when U changes from this solution, phi must be updated... Clear now? Gavin |

Thanks for the fast help.
ThiThanks for the fast help.
This helps a lot. I didn't see the step: ddt(U)+U*div(U)-Laplacian(nu,U)=-grad(p) to ddt(U)+div(U*U)-Laplacian(nu,U)=-grad(p) Joern |

Here it is, with subscript x,yHere it is, with subscript x,y,z meaning differentiation and u,v,w being velocity components and U the vector:
In the x-direction div(U * U) reads: (u * u)_x + (u * v)_y + (u * w)_z = u_x u + u u_x + u_x u + u v_y + u_z w + u w_z = u_x u + u_x u + u_z w + u*(u_x + v_y + w_z) = u_x u + u_x u + u_z w where the term in the bracket are identical to zero for incompressible flows, as it is your continuity equation. The same can be done for the other directions and you will have understood the step above. Best regards, Niels |

Thx for your Help.
I think Thx for your Help.
I think I now understand the solver algorithm. Now I have to understand the discretisation ;) Joern |

Hallo,
i have a new problemHallo,
i have a new problem with the same topic http://www.cfd-online.com/OpenFOAM_D...part/happy.gif I try to understand the sover sonicFoam. This solver solves the Equations: ddt(rho, U)+div(phi, U)-laplacian(mu, U)=-grad(p) and ddt(rho, e)+div(phi, e)-laplacian(mu, e)=-div(phi/rho)+mu*magSqr(symm(grad(U))) For me it looks like some kind of impulse and energy equation from the compressible Navier Stokes equations. Does someone know which equations sonicFoam solves or where i can find some literature about the algorithm an his mathematic roots? sorry for posting nearly the same question again, but i need the infos for my further work and i don't see it alone. thx, Joern |

sonicfoam is a solver for compsonicfoam is a solver for compressible ideal gas flow. That why the solver use the continuity-,momentum-, energy-, and ideal gas equation in its algorithm.
look in the programmer's guide ! there is an nice tutorial named: "Supersonic flow over a forward-facing step" on page 58 ! http://foam.sourceforge.net/doc/Guid...mmersGuide.pdf |

I reactivate this old thread, cause i have a question about the sonicFoam solver.
sonicFoam is a solver with PISO loop for the compressible Navier-Stokes equations. I think i understand most of the solver but one think is not clear: if i set mu=0 in sonicFoam it solves the Euler Equations for a compressible, inviscid, perfect gas. (thats what i want to simulate) But there is a little difference. sonicFoam just looks at the inner energy e=T*Cv (just thermal energy). The Euler Equations (and also the Navier-Stokes) work with the energy e=T*Cv+1/2*mag(v)^2 (thermal energy + kinetic energy). why can the kinetic energy be ignored? And why is the the solver still consisten to the Euler-/Navier-Stokes Equations? thx for help, Joern |

All times are GMT -4. The time now is 15:07. |