- **OpenFOAM Running, Solving & CFD**
(*https://www.cfd-online.com/Forums/openfoam-solving/*)

- - **twoPhaseEulerFoam - floating point exception (nutb)**
(*https://www.cfd-online.com/Forums/openfoam-solving/63467-twophaseeulerfoam-floating-point-exception-nutb.html*)

twoPhaseEulerFoam - floating point exception (nutb)Hi,
I just started with the twoPhaseEulerFoam Solver. I got while "calculating nutb" a floating point exception. I saw that nutb is turbulent kinematic viscosity of phase b. Where could be the problem? Br |

Quote:
Info<< "Calculating field nutb\n" << endl; volScalarField nutb ( IOobject ( "nutb", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), Cmu*sqr(k)/epsilon ); Most floating point exceptions are divide-by-zeros. As you can see the square of the turbulent kinetic energy, k, is divided by epsilon. I guess you have a zero in your epsilon field? You can eliminate the floating point exception by using a small value such as 1e-13 instead. However, in 1.5.x version this problem is eliminated by using: Cmu*sqr(k)/max(epsilon, dimensionedScalar("smallEps",epsilon.dimensions(), 1e-6)) Where the value of epsilon in the denominator is limited to larger than 1e-6 and thus removing the possibility of a floating point exception caused by a zero in the epsilon field. So another option is to update to 1.5.x or to modify the line yourself and recompile the solver. |

All times are GMT -4. The time now is 23:47. |