[chnrdu]

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

[henry]

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