[Saikumar Bunni]

Hello,

Am trying a transonic simulation of a supersonic intake, using rhoPimpleFoam and as shown in the figure, top wall (small portion) of the boundaries has to be atmosphere.

For this I tried imposing totalTemperature in 0/T, totalPressure in 0/p and supersonicFreeStream boundary for velocity in 0/U.

But it doesn't work.

So I have used slip boundary condition along with zero gradients of pressure and Temp.

But I eventually want something similar to pressure far-field BC on Fluent. Is there any variant of it for OF?

Find the geometry pic attached. Note that the lines in red represent the shock.

0/U:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (3.53 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (3.53 0 0);
}


outlet
{
type zeroGradient;
}

wall
{
type noSlip;
}

inletOutlet
{
type slip;
}


frontAndBack
{
type empty;
}
}

// ************************************************** *********************** //

0/p:

/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [1 -1 -2 0 0 0 0];

internalField uniform 1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 1;
}

outlet
{
type waveTransmissive;
field p;
psi thermo:psi;
gamma 1.4;
fieldInf 1;
lInf 3;
value uniform 1;
}

inletOutlet
{
type zeroGradient;
}

wall
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

// ************************************************** *********************** //

0/T:
/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 7
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 1;
}

outlet
{
type zeroGradient;
}

wall
{
type zeroGradient;
}

inletOutlet
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

// ************************************************** *********************** //

[ano]

Hi Saikumar,


the equivalent should be the waveTranmissive boundary condition.

I could imagine that rhoCentralFoam or dbnsFoam (from foam-extend) are more suitable for your problem (especially if you are interested in an accurate resolution of the shocks).

[Saikumar Bunni]

Originally Posted by ano

Hi Saikumar,


the equivalent should be the waveTranmissive boundary condition.

I could imagine that rhoCentralFoam or dbnsFoam (from foam-extend) are more suitable for your problem (especially if you are interested in an accurate resolution of the shocks).

Hi I tried the dbnsFoam solver for my supersonic intake case. But I could not capture the Normal shock in my system (figure 2). My free stream Ma was 2.4, and is 1.85, 1.3565 after 1st and 2nd oblique shocks. I expect a Normal shock at the location of Area expansion. Analytical results show my temperature at the end of the duct is roughly 1.93K (scaled) and pressure is 8.8Pa. My simulation, even after 35 seconds couldnt get the Normal shock in it. As shown in the figure 1 and 3, it shows the values I specified at the outlet at the last cells only. My boundary conditions are in simple as follows.

_______________p_______________________T ______________________ U
inlet_______Fixed-value 1Pa_______________ Fixed-value 1Pa_____________supersonic Free-stream 2.4 Ma
outlet______Wave-trans – fieldInf – 8.8Pa_____Fixed-value 1.93K____________zero Grad
inlet Outlet__Wave-trans – fieldInf – 1Pa______inlet Outlet – value 1K_________supersonic Free-stream 2.4m/s
wall________zero Grad___________________zero Grad___________________fixed value – 0 0 0
frontAndBack empty

[ano]

Hi,


Perhaps you could try to use a finer grid (to see whether this gives you the normal shock), decrease fieldInf at the outlet to 3.6 Pa and increase linf (to get rid of the jump at the outlet).


Which schemes did you take?

[Saikumar Bunni]

Originally Posted by ano

Hi,


Perhaps you could try to use a finer grid (to see whether this gives you the normal shock), decrease fieldInf at the outlet to 3.6 Pa and increase linf (to get rid of the jump at the outlet).


Which schemes did you take?

Hi,

I have been struggling with altering b/n schemes and boundary conditions. I read in the literature that for a transonic case with a supersonic inlet, an isolator and a CD nozzle can be used at the downstream end to reduce pressure wave reflections. I have done the same, and the CD nozzle now brings down the pressure at the outlet to 1Pa. But still my case gets crashed. Please find the pdf file (link below) for the geometry and boundary conditions, and also the case files are attached. I have used both rhoCentralFoam and dbnsFoam, but none worked. Please check the readme file to the run the cases.

For the schemes, I haven't changed much from the default one provided on dbnsFoam,
using rusanov flux splitting with BerthJespersen limiter. Tried HLLC which offers greater stability, it didn't work either.

https://drive.google.com/drive/folde...HY?usp=sharing

[ano]

Hi,



Can you try the following Schemes in the dbns case?



flux hllc;
limiter firstOrder;

Making dbnsFoam run comes down to refining the mesh a lot and keeping the Courant number low (<0.3). I could imagine that you need 0.5-1 million cells.