[Harald]

Hello,

earlier this year, I started using OpenFOAM at work. Now, I reached the point, where I need assistance.

Currently, I got stuck with the correct definition of my problem's outlet boundary conditions.

My test case has the following setup:

• axis-symmetric case (see 1-geom.png):
  • chamber (D = 25 mm) with small high-pressure/temperature region,
  • filter,
  • surrounding area
• initial conditions (see 2-initial-p.png and 2-initial-T.png):
  • air
  • p0 = 1e+05 Pa
  • T0 = 300 K
  • chamber (high temperature/pressure region)
    • air
    • p_region = 20e+05 Pa
    • T_region = 1600 K
  • filter (Darcy-Forchheimer)

• outlet patches
  • front,
  • right
• solver
  • rhoPimpleFoam

Currently, my outlet patches seem to behave like solid walls. This understanding comes from the observation of a reflection from the front-patch (see 3-U.png and 4-U.png). However, that is not what I want. Actually, the outlet patch should be perfectly permeable and, therefore, only cut away everything from the environment, which I do not want to simulate.


Unfortunately, I could not find the solution myself (RAS-tutorials, foamInfo, etc.). Please, take a look at my outlet boundary conditions; can you find an obvious failure?

alphat:


"(front|right)"// outlet
  {
type            calculated;

value           uniform 0;

}

 k:


 "(front|right)"// outlet
 {
type            inletOutlet;
inletValue      uniform 1e-5;
value           uniform 1e-5;
}

 nut:


 "(front|right)"// outlet
 {
type            calculated;
value           uniform 0;
}

omega:


 "(front|right)"// outlet
  {
type            inletOutlet;
value           uniform 1;
inletValue      uniform 1;
}

p:


 "(front|right)"// outlet
  {
type            fixedValue;
value           uniform 1e+5;
}

T:

 "(front|right)"// outlet
  {
type            inletOutlet;
value           uniform 300;
inletValue      uniform 300;
}

 U:


 "(front|right)"// outlet
  {
type            pressureInletOutletVelocity;
value           uniform (0 0 0);
inletValue      uniform (0 0 0);

}

Let me know if I need to provide some additional information.

Harald

[Harald]

Today, I found a solution for my problem with help of foamInfo. It seems that changing the outlet boundary condition of the pressure from fixedValue to waveTransmissive does the job (see 5-U.png,6-U.png).

The new outlet BC reads:

p:

"(right|front)"// outlet
{

type            waveTransmissive;
gamma           1.4;
}