when set a pressure boundary a
when set a pressure boundary as
F1 { type timeVaryingUniformFixedValue; timeDataFileName "inlet.dat"; value uniform 1e+5; } When I run sonicLiquidFoam, I got errors: --> FOAM FATAL IO ERROR : file "" does not exist file: at line 1. From function IFstream::operator() in file db/IOstreams/Fstreams/IFstream.C at line 171. FOAM exiting Fixes: Please enter the folder $WM_PROJECT_DIR/applications/solvers/compressible/sonicLiquidFoam/, and edit the file createFields.H, then delete the line 41: 30 volScalarField rho 31 ( 32 IOobject 33 ( 34 "rho", 35 runTime.timeName(), 36 mesh, 37 IOobject::NO_READ, 38 IOobject::AUTO_WRITE 39 ), 40 rho0 + psi*(p-p0), 41 p.boundaryField().types() 42 ); and also delete the comma at the end of the previous line (line 40). In addition, in file sonicLiquidFoam.C, I think rho0 + psi*p in line 105 should corrected as rho0 + psi*(p-p0) in order to compute the density rightly. P.S. I post this bug and fix in my blog, www.durun.cn/?p=364 |
The transfer of the p BCs is a
The transfer of the p BCs is a problem for complex BCs and your fix means that rho would get BCs of type "calculated" which should be OK. I will make this change in 1.5.
> In addition, in file sonicLiquidFoam.C, I think rho0 + psi*p in line 105 should corrected as rho0 + psi*(p-p0) in order to compute the density rightly. I don't agree; note the difference between rho0 and rhoO. However for consistency rhoO + psi*p should be used on line 40 of createFields.H. Henry |
All times are GMT -4. The time now is 20:09. |