[martyn88]

Hello all,

I am trying to simulate a supersonic turbulent free jet but am struggling to get a stable case running.

I think, as is often the case, the problem may lie in the boundary conditions.

Has anyone done a similar simulation that could perhaps advise me on appropriate boundary conditions?

My mesh is effectively a 1/8th section of a converging diverging nozzle surrounded by ambient fluid (atmospheric air)

Here are some images of my mesh:

meshpic.jpg

Foam mesh.jpg

inlet is the small leftmost face (nozzle inlet)
inlet 2 is the leftward facing face
nozzle wall is the horizontal face above inlet
freestream1 is the horizontal face just above the nozzle wall
freestream 2 is the large horizontal face on top
outlet is the rightward facing face
two side boundaries are cyclic AMI


My main concern is the outlet. Initially I defined just inlet, nozzle wall, cyclic boundaries and all other faces were outlet (inlet2, freestream1, freestream2 and outlet) but was unsure if it could handle multiple outlets.


I am using the rhoPimpleFoam solver and below are my 0 files:

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "5e-05";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform (2 0 0);

boundaryField
{
inlet
{
type uniformFixedValue;
uniformValue table
(
(0 (10 0 0))
(0.08 (50 0 0))
(0.1 (50 0 0))
(0.3 (400 0 0))
);
}
inlet2
{
type uniformFixedValue;
uniformValue table
(
(0 (2 0 0))
(0.1 (2 0 0))
(0.4 (0 0 0))
);
}
outlet
{
type pressureInletOutletVelocity;
value uniform (2 0 0);
}
nozzlewall
{
type fixedValue;
value uniform (0 0 0);
}
face1
{
type cyclicAMI;
}
freestream1
{
type slip;
value uniform (0 0 0);
}
freestream2
{
type slip;
value uniform (0 0 0);
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "5e-05";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 300;

boundaryField
{
inlet
{
type totalTemperature;
gamma 1.338;
phi phi;
psi psi;
T0 uniform 973;
value uniform 973;
}
inlet2
{
type zeroGradient;//totalTemperature
//gamma 1.338;
//phi phi;
//psi psi;
//T0 uniform 300;

}
outlet
{
type inletOutletTotalTemperature;
gamma 1.4;
T0 uniform 300;
value uniform 300;
}
nozzlewall
{
type fixedValue;
value uniform 300;
}
face1
{
type cyclicAMI;
}
freestream1
{
type zeroGradient;
}
freestream2
{
type zeroGradient;
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "5e-05";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 101325;

boundaryField
{
inlet
{
type zeroGradient;
}
inlet2
{
type zeroGradient;
}
outlet
{
type totalPressure;
rho rho;
psi none;
gamma 1.4;
p0 uniform 101325;
value uniform 101325;
}
nozzlewall
{
type zeroGradient;
}
face1
{
type cyclicAMI;
}
freestream1
{
type zeroGradient;
}
freestream2
{
type zeroGradient;
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "5e-05";
object muSgs;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
inlet2
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
nozzlewall
{
type muSgsUSpaldingWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
face1
{
type cyclicAMI;
}
freestream1
{
type calculated;
value uniform 0;
}
freestream2
{
type calculated;
value uniform 0;
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "5e-05";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 2e-05;

boundaryField
{
inlet
{
type fixedValue;
value uniform 2e-05;
}
inlet2
{
type zeroGradient;
}
outlet
{
type inletOutlet;
inletValue uniform 2e-05;
value uniform 2e-05;
}
nozzlewall
{
type compressible::kqRWallFunction;
value uniform 2e-05;
}
face1
{
type cyclicAMI;
}
freestream1
{
type zeroGradient;
}
freestream2
{
type zeroGradient;
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volTensorField;
location "5e-05";
object B;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform (0 0 0 0 0 0 0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 0 0 0 0 0 0 0 0);
}
inlet2
{
type fixedValue;
value uniform (0 0 0 0 0 0 0 0 0);
}
outlet
{
type inletOutlet;
inletValue uniform (0 0 0 0 0 0 0 0 0);
value uniform (0 0 0 0 0 0 0 0 0);
}
nozzlewall
{
type zeroGradient;
}
face1
{
type cyclicAMI;
}
freestream1
{
type zeroGradient;
}
freestream2
{
type zeroGradient;
}
FaceGroup8
{
type cyclicAMI;
}
}


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

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "5e-05";
object alphaSgs;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
inlet
{
type calculated;
value uniform 0;
}
inlet2
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
nozzlewall
{
type alphaSgsWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
face1
{
type cyclicAMI;
}
freestream1
{
type calculated;
value uniform 0;
}
freestream2
{
type calculated;
value uniform 0;
}
FaceGroup8
{
type cyclicAMI;
}
}


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


Any help would be greatly appreciated.

Thankyou in advance

[martyn88]

Could anyone please help me with this problem? I still can't get a stable simulation to run.

Thanks

[kalle]

First of all, these kind of flows are quite tricky to calculate accurately. Normally, literature would suggest a density based runge kutta solver for this case. There is no such solver in official openfoam distribution. The closest you get is the rhoCentralFoam solver, but it is to my knowledge too dissipative for LES.

The rhoPimpleFoam solver is OK at low Mach number, though it can be stable for your case as well. You should however not trust shock prediction too much. You have not posted your whole case so I cannot say what is wrong directly, but it looks a bit strange to have zeroGradient on T and k on the inlet. You might try changing that. Else, closely monitoring all fields timestep by timestep might point out what is going wrong.

K

[ville]

Hi,
I wrote such a density based RK4 LES solver, a picture of a supersonic jet is found in http://users.tkk.fi/~vavuorin/
Best,
Ville

[pg22]

Ville,

That's a great picture of a supersonic jet.

The picture shows shock waves, acoustic waves and turbulent structures all at once. Can you give more detail of your method? Is it described in your submitted paper?

Also, on the subject of the original question, the solution will be sensitive to reflections from the boundaries. A non-reflective boundary condition will be required to prevent non-physical waves disturbing the flow field.

I have developed one such suitable boundary condition. Please see 'Modelling shock wave phenomena in over-expanded jets using OpenFOAM--P. L. Garlick', available at http://www.opensourcecfd.com/conference2010/en/proceedings.html

The method solves the one-dimensional Euler equations at each boundary cell, allowing waves to pass out of the domain but not to enter.

Paul.

[ville]

Hi,
Could you send me the paper via email ville.vuorinen at aalto.fi ?
The method I'm using is the explicit density based RK4 method.
The convection terms are discretized by a new method called
"Scale-Selective Discretization"
http://www.sciencedirect.com/science...45793012003799
which provides artificial dissipation in the spirit of ILES but by focusing
the dissipative effects truly only to the small scales via a filtering procedure.
The bulk viscosity by Cook and Cabot is applied in the OF code I implemented
to stabilize weak shocks and gradients.
Additionally, I'm using a simple shock sensor to detect the normal shocks (Mach disk).
At the normal shocks an additional (local) low-pass filtering of the solution is
carried out for numerical stability. I don't need any non-reflecting BC's because
the domain is very large and the mesh is very coarse at the boundaries.
Actually, the whole injection system is closed and there is no inflow or outflow either.
Inflow is modeled by actually meshing a large pressurized "bottle" from which a converging nozzle starts and enters the chamber. This is quite nice since a) this extra stage takes only <1% of all the cells and no approximate bcs are required b) more realism.
No outflow bc is needed either since the domain a) is closed in reality (cylinder of
a combustion engine) b) is very large.
I will post more details in couple of days..
Best,
Ville

[pg22]

Sure, the paper is on its way.

Paul.

[noridk_14]

Check this. You should use a open source code; it always works.

http://cfdosc.wordpress.com/2012/07/...upersonic-jet/

[ville]

Hi,
as mentioned, I implemented the density based RK4 solver with OpenFOAM.
Our paper (based on the OpenFOAM solver) on "Large-Eddy Simulation of Highly Underexpanded Transient Jets"
will appear in Physics of Fluids soon. If you want a preprint please contact
me ville.vuorinen@aalto.fi .
Best,
Ville

[halowine]

hi everybody,

I'm trying to do a LES freestream Jet with rhoCentralFoam for my internship. I found some good results for RANS model compared to some PIV data and now I want to compare with LES simulation.

I found some strange behavior with my first simulation...
here's the contour plot for velocity for k-omega SST RANS

and here's the contour plot for oneEq LES


It's like there is no turbulent viscosity at all... The solution is static through the time, that's something we don't expect for LES case.
My flow is controlled by pressure ratio between the inlet and the outlet, my Mach number is around 0.5 at the throat.

Does anybody already try a LES case with rhoCentralFoam ?
Does that come from the inlet BCs (maybe turbulentInlet instead of totalPressureInlet) ?

ps : I put the 2 folder (LES/RANS) with the solution.
https://drive.google.com/folderview?...0k&usp=sharing

Thanks all