sonicfoam nozzle case
 

hi
i am try to simulate aerospike nozzle and examine different bc. when i decrease initial p solving diverge. my bc
for p
dimensions [1 -1 -2 0 0 0 0];

internalField uniform 500000;

boundaryField
{
gasInlet
{
// type fixedValue;
// value uniform 800000;
type totalPressure;
p0 uniform 700000;
U U;
phi phi;
rho none;
psi none;
gamma 1.3;
value uniform 364000;

// type zeroGradient;
}
airInlet
{
// type fixedValue;
// value uniform 100000;

type zeroGradient;
}

outlet
{

type waveTransmissive;
field p;
phi phi;
rho rho;
psi thermo:psi;
gamma 1.3;
fieldInf 14000;
lInf 1;
value uniform 14000;

// type zeroGradient;
}

symPlane
{
type symmetry;
}

freestreem
{
type zeroGradient;
}

spikeWall
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}
for u

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

internalField uniform (100 0 0);

boundaryField
{
gasInlet
{
// type fixedValue;
//value uniform (650 0 0);
type pressureInletOutletVelocity;
phi phi;
rho rho;
value uniform (0 0 0);
}
airInlet
{
// type fixedValue;
// value uniform (10 0 0);
type pressureInletVelocity;
phi phi;
rho rho;
value uniform (0 0 0);
/*
type supersonicFreestream;
pInf 380000;
TInf 300;
UInf (650 0 0);
gamma 1.3;
value uniform (0 0 0);
*/
}

outlet
{
type pressureInletOutletVelocity;
inletValue uniform (0 0 0);
value uniform (0 0 0);
}

symPlane
{
type symmetry;
}

freestreem
{
type supersonicFreestream;
pInf 500000;
TInf 300;
UInf (400 0 0);
gamma 1.3;
value uniform (0 0 0);

// type slip;
}

spikeWall
{
type fixedValue;
value uniform (0 0 0);
}

frontAndBack
{
type empty;
}
}

for T
dimensions [0 0 0 1 0 0 0];

internalField uniform 300;

boundaryField
{
gasInlet
{
type fixedValue;
value uniform 320;
}
airInlet
{
type fixedValue;
value uniform 300;
}

outlet
{
type inletOutlet;
inletValue uniform 300;
value uniform 300;
}

symPlane
{
type symmetry;
}

freestreem
{
type inletOutlet;
inletValue uniform 300;
value uniform 300;
}

spikeWall
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

I want the flow to be induced by the pressure difference between inlet (exit of the nozzle) and the ambient.Attachment 41433

Attachment 41434



With thanks for your attention

no one comment???????

Hi, can you show picture with schematic view of your computational domain - where inlet is located, where outlet and so on.

Can you als share your case directory with 0, constant and system?

thank you for your answer.
please visit this
regards

Hi,

information on the link, that you provided do not gives more about your numerical model.

Problem can be:
- in numeric schemes (fvSchemes, fvSolution)
- in physical properties (constant/thermopysicalProperties)
- in boundary conditions (0/)

The first step, i would recommend is to switch outlet pressure condition to totalPressure.

Can you also upload your case here?

Attachment 41478

thanks a lot for the reply.
i have attached.

Hi,

I would suggest next steps to improve stability

- change pressure "outlet" condition to totalPressure
- change "freestreem" condition for velocity to slip
- change schemes for convection terms to upwind (system/fvSchemes)
- change solution methods for p, U, e (system/fvSolution)
- disable relaxation for all fields (system/fvSolution)
- disable outer corrections, momentum predictor, enable explicit non-orthogonal correction
Maybe, it would be better to switch to rhoPimpleFoam instead of sonicFoam. Because rhoPimpleFoam can work without momentumPredictor and energy conservation, formulated in enthalpy.

Also, you must check that max Courant number (Co) do reach values 0.5 or higher.

Also you can try rhoCentralFoam for your case.

Unfortunately, i can't check this case updated with my changes, because polyMesh folder is missing in tgz

thank you very much for the your exact answer and Attention.
after apply your suggest,i am decrease the ambient pressure and case Converged.:)
i am try rhoCentralFoam but Unfamiliarity with that setup, case diverged.
if i increase the nozzle pressure to supersonic flow, must i change freestreem and outlet BC?
polymesh file i have attached here.


Thanks for all.

hi dear Matvej.
can you check the k,epsilon,alphat,mut files??
thanks a lot.

hi matvej
i am decrease the ambient pressure to 14000 and case diverged.
so i refinement mesh to 109000 cell but diverged.

Hi, mohammad

After inspecting your case i found next issues about computational domain and B.C.:

1) Mesh is too thick in z-direction. Despite the absence of third coordinate (Z) in solution, it is a good practice, to have thickness of cells in Z-direction for 2D simulation in OpenFOAM of order 1/100 of some characteristic length. In your case i would propose to make thickness of mesh 100 or more times smaller then you have now

2) Also, checkMesh tells, that you have some edges, that are not aligned or not perpindicular to empy (Z) direction. This usually means, that mesh is corrupted somewhere. See checkMesh log at the end of my message.

3) For supersonic flows you have to change your boundary conditions at inlet as follow:
- if you know velocity and it is supersonic, then you must supply pressure (p), velocity (U) and temperature (T) at inlet
- if you know only pressure at inlet, then you must extend your inlet in upwind direction to build converging-diverging nozzle to resolve subsonic-supersonic flow correctly

I hope, this will help you

Hi Matvej.
You know what is the reason of diverge case in very low ambient pressure(14000)?

فرستاده شده از GLX G5ِ من با Tapatalk

Don't understand this part, why?

Regards!

I'm sorry, Co do not reach 0.5

Hi, mohammad

Did you fixed your mesh and B.C.?