- **OpenFOAM Programming & Development**
(*https://www.cfd-online.com/Forums/openfoam-programming-development/*)

- - **solve equation**
(*https://www.cfd-online.com/Forums/openfoam-programming-development/82606-solve-equation.html*)

solve equationHi all,
I have a stupid question but I don't find the solution. I must solve the following equation: U & grad(eta) - Uz=0 where eta is a scalar field and U is velocity vector and Uz is the z-component of U. How can I write the scalar matrix etaEqn and solve it? Thanks. |

Hi, Is your U field divergence free [div(U)==0]???, in this case you have
U & grad(eta) - Uz=0 -> div(U eta)-Uz=0 so that in FOAM solve(fvm::div(phi,eta)-U.component(vector::Z)==0); where phi is previously defined as phi=U&Sf, like is scalarTransportFoam, icoFoam, etc. Regards. |

One more thing, Is your equation dimensionally consistent?
Best. |

Thank you
Santiago Marquez DamianI solve like you suggest and it works. Info<<"Inizio calcolo Matrice Eta"<<endl; faScalarMatrix etaEqn ( fam::div(phis,eta) ); Info<<"Inizio Relax"<<endl; etaEqn.relax(); Info<<"Inizio Solve"<<endl; solve(etaEqn == (Us & aMesh.faceAreaNormals())); Dimensionally is consistent because eta is a areaSaclarField and U is a areaVectorField. But now I have an other problem, I use as linear solver the eta smoothSolver { smoother DILU; tolerance 1e-06; relTol 0; }; and as boundary condition: in { type fixedValue; value uniform 0; } out { type zeroGradient; } carena { type zeroGradient; } far { type zeroGradient; } but after few iteration the solution explode, do you think I make some macroscopical error? I use also a relax factor of 0.3 for the etaEqn. Thanks. |

I don't know, may be you can post the console output at the exploding moment and some data about the physical problem.
Regards. |

I find the problem is the div shemes, I use a Gauss Linear and all explode, than I change in a Upwind and all works fine!!!
Thank for the help. |

All times are GMT -4. The time now is 07:39. |