Pressure driven cd nozzle flow
 

hello,
i am trying to simulate a pressure driven flow through a convergent divergent nozzle using rhoCentralFoam
conditions given to me are:
nozzle inlet-Po-1.028 bar
ambient inflow-Po-1.007 bar
total temperature-300k
outflow-p-1 bar.
pressure-
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 1.01325;

boundaryField
{

inlet
{
type totalPressure;
p0 uniform 1.028;
U U;
phi phi;
rho rho;
psi none;
gamma 1.4;
}
ambientinlet
{
type totalPressure;
p0 uniform 1.007;
U U;
phi phi;
rho rho;
psi none;
gamma 1.4;
}


outlet
{
type waveTransmissive;
field p;
phi phi;
rho rho;
psi thermo:psi;
gamma 1.4;
fieldInf 1;
lInf 50;
value uniform 1;
}
bottom
{
type symmetryPlane;
}

obstacle
{
type zeroGradient;
}
top
{
type zeroGradient;
}
defaultFaces
{
type empty;
}
}
Velocity-
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type zeroGradient;
}
ambientinlet
{
type zeroGradient;
}

outlet
{
type zeroGradient;

}

bottom
{
type symmetryPlane;
}
obstacle
{
type fixedValue;
value uniform (0 0 0);
}
top
{
type zeroGradient;
}

defaultFaces
{
type empty;
}
}
Temperature-
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 300;

boundaryField
{
inlet
{
type totalTemperature;
gamma 1.4;
T0 uniform 300;
value uniform 300;
}
ambientinlet
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}


obstacle
{
type zeroGradient;
}
top
{
type zeroGradient;
}
bottom
{
type symmetryPlane;
}
defaultFaces
{
type empty;
}
}
inlet-nozzle inlet
ambientinlet-ambient inflow
obstacle-nozzle profile
bottom-bottom of the whole domain
top-top boundary
outlet-outlet for the whole domain.

i have attached the geometry, grid and Mach plot for the above described case.I am not able to understand the strange flow pattern in the nozzle region( if i increase the nozzle pressure to 2 bar or above , this problem doesn't exist) . I think there is some problem with the boundary conditions but i am not able to figure it out.Kindly, help me solve this issue.
thank you
srikanth

To me, it looks like you are generating pressure waves at the sharp corner where the fluid exits into the big rectangular section. Those pressure waves travel downstream (you can see them slightly in the blue region of your Mach-number field). For low pressure differences they also manage to travel upstream into the nozzle where they get reflected from the inlet and interact on the way back with incoming waves. For Mach>1 this can't happen, of course. Does anyone else have a thought?

hey thanks for the reply.So, what do you think i should do??

Since there are no non-reflecting inlet BCs (that I know of), i would extend your inlet into a big box. In that box you can apply your pressure BC. Within that box, you can either coarsen the mesh towards the inlet boundary so that the short wavelength pressure waves are filtered out or use a small porous medium right after the inlet boundary which also damps the pressure waves and should prevent reflections.

Hi Srikanth,
Ive been working on nozzle simulation with similar condition for a good while now (i.e. totalTemp totalPress inlet with waveTrans BC) with Pressure Ratios around 25-250.

what is the scale on the Mach image you posted?
It almost looks like mach waves from surface roughness but with the pressure ratio you have it should be safely subsonic (i.e. no mach waves)?

First thing that jumps out at me: in the images you posted it looks like there is a fairly large jump in your mesh's cell size in the axial direction near the throat. Sharp changes in cell size can definitely cause local oscillations in simulations.
Maybe try smoothing out the mesh a bit in key regions (throat and nozzle lip)?

Also numerical scheme can have a pretty significant impact I typically use TVD vanLeer with good results. I've also heard NVD work well with rhoCentralFoam.

depending on how the sim is initialized rhoCentralFoam can take a while to reach steady state with a lot of pressure waves bouncing around especially in the converging section. Idk if your looking at steady-state or transient results.

the LINF value can cause oscillations too for the waveTransmissive boundary condition (but thats usually in the quiescent medium around the plume)


Just a couple thoughts apologies if this is old news to you. I just recalled banging my head against a wall on some similar problems not too long ago

cheers,
Jason