[DevilX]

Hey Foamers,


i am trying to simulate a part of an air conditioner compressor, where i have the Pressure values of inlet and outlet and the velocity should arrange around this pressure difference. Attached is a picture about the general geometry, in which a valve is implemented, which normally moves up and down, but in this steady state simulation it´s completely fixed.


I checked my boundary conditions thousand times and tried a lot of different setups, also made the mesh finer, tried other solver (buoyantSimpleFoam), made thermophysical simple by regarding all to const, but nothing works.

With Massflow, it runs to a certain extend. For incompressible case with simplefoam, it also worked. But the fluid is very sensible to pressure, so i need to solve this compressible.


I appreciate every help!!


BC´s:
p:

internalField   uniform 1600002;
boundaryField
{
  
      Zylinder_Outlet
            {
               type            fixedValue;
               value        uniform 1600002;
            }
            Zylinder_Upper_Walls
            {
                type            fixedFluxPressure;
                value           uniform 0;
            }
            Zylinder_Plate_Walls
            {
              type            fixedFluxPressure;
                value           uniform 0;
            }
            Zylinder_Limiter
            {
                type            fixedFluxPressure;
                value           uniform 0;
            }
            Zylinder_Zylinder
            {
                type            fixedFluxPressure;
                value           uniform 0;
            }
            Zylinder_Zylinder_Huelle
            {
                 type            fixedFluxPressure;
                value           uniform 0;
            }
    
            Zylinder_Inlet
            {
                type            totalPressure;
                p0                uniform 1700000;
                value            uniform 1700000;
            }

U

internalField   uniform (0 0 0);

boundaryField
{ 
            Zylinder_Outlet
            {
               type pressureInletOutletVelocity;
                value uniform (0 0 0);
            }
            Zylinder_Upper_Walls
            {
               type            noSlip;
            }
            Zylinder_Plate_Walls
            {
               type            noSlip;
            }
            Zylinder_Limiter
            {
                type            noSlip;
            }
            Zylinder_Zylinder
            {
                type            noSlip;
            }
            Zylinder_Zylinder_Huelle
            {
                type            noSlip;
            }
      
            
            Zylinder_Inlet
            {
                type            pressureInletVelocity;
                value uniform (0 0 0);
            )}

T

internalField   uniform 422.15;

boundaryField
{
        Zylinder_Outlet
            {
               type            zeroGradient;
            }
            Zylinder_Upper_Walls
            {
               type            zeroGradient;
            }
            Zylinder_Plate_Walls
            {
               type            zeroGradient;
            }
            Zylinder_Limiter
            {
                type            zeroGradient;
            }
            Zylinder_Zylinder
            {
                type            zeroGradient;
            }
            Zylinder_Zylinder_Huelle
            {
                type            zeroGradient;
            }
     
            Zylinder_Inlet
            {
                type            fixedValue;    
                value           uniform 422.15;
                
            }

[piu58]

I don't understand your case fully. But from my understanding, pressure b.c. at walls should be zero gradient.

[DevilX]

Originally Posted by piu58

I don't understand your case fully. But from my understanding, pressure b.c. at walls should be zero gradient.

Dear Uwe,


thanks for your reply!


It doesn´t matter, if the walls are treated as fixFluxPressure or zeroGradient, the result is the same, sadly.

Edit: it´s used for p_rgh pressure for the buoyantSimpleFoam, so its the same as zeroGradient, see here.



Can i help you in trying to understand the case?

In short: the Inlet is used to represent the pressure, build by a moving cylinder in a compressor. Caused by the high pressure, the fluid moves through the small "pipe" onto the fixed valve, afterwards it flows out to the top.

[Fouch]

Hi DevilX,

Could you share your fvSolution file ?

BR

[DevilX]

Hey Fouch,


of course i can!
You find them below.
With all the BC´s like above, i am at least able to simulate a pressure driven flow, bu only with really low pressure differences.

Is there a way with potentialfoam or seomething else to reduce the rise in pressure peaks that occure at some iterations?
I also treid to use a pressure table, but this doesnt work - OF only recognizes the value in p0, which cant be used for a table..



fvSolution:

solvers
{
p
{
solver GAMG;
tolerance 1e-06;
relTol 0.1;
smoother GaussSeidel;
nCellsInCoarsestLevel 500;

}

"(U|e|k|h|epsilon|)"
{
solver PBiCGStab;
preconditioner DILU;
nSweeps 2;
tolerance 1e-05;



}
}


SIMPLE
{
nNonOrthogonalCorrectors 0;



residualControl
{
p 1e-3;
U 1e-4;
e 1e-3;


// possibly check turbulence fields
"(k|epsilon|omega)" 1e-3;
}
}

relaxationFactors
{
fields
{
p 0.5;
}
equations
{
p 0.5;
U 0.65;
k 0.7;
epsilon 0.7;
h 0.7;
e 0.7;
}
}


fvSchemes:


ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;

div(phi,U) bounded Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
div(phi,epsilon) bounded Gauss upwind;
div(phi,k) bounded Gauss upwind;
div(phid,p) bounded Gauss upwind;
div(phi,e) bounded Gauss upwind;
div(phi,K) bounded Gauss upwind;
div(phi,h) bounded Gauss upwind;
div(phid,p) bounded Gauss upwind;
div(phi,Ekp) bounded Gauss upwind;




}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

[Fouch]

Hi,


I would add pressure limiter in fvSolution just after nNonOrthogonalCorrectors 0; .



pMinFactor 0.1;
pMaxFactor 2;


You have to adjust this value to your case.


Please confirm if it solve you problem.


Best regards,

[DevilX]

Hey,


no it´s not working. It seems that there is still an actual problem with BC´s or Mesh and this brings OF to diverge somehow. If i also try to limit Temperature oder Velocity, it still crashes.

[piu58]

Please try first to get it run with the least complicated physics. That means omit temperature for the first run, only the fluid. If that work you may decide how to add the temperature field. Normally, there is more than one way.

[DevilX]

Hey Uwe,
i think i am not really getting what you want to say, especially the temperature part. I set the thermal properties to constant (idealGas, which it isn´t, turned off the turbulence..) Temperature should be constant in the entire domain. That´s why i am lost somehow. Initilaization with potentialFoam also doesn´t help, because it doesn´t calculate anything.

[piu58]

> f i also try to limit Temperature oder Velocity

That means, you try simulating temperature with the field. I suggest simulating only the compressor.
It is hard to say what happens without the case.

[DevilX]

I try to sum it up, what should happen, with the pictures below. Thats a case for very low pressure difference, in which the simulation runs. Physically, the flow seems right according to the glyphs. Sadly, i can´t provide the whole case.
Temperature ist irrelevant (mostly), the points of interest are:


- pressure/force on valve
- velocity/mass flow around the valve

- pressure difference between flow around valve and cylinder room

[piu58]

I assume that you have a du/dn=0 condition at the upper.

This is not applicable in your case. As you might see in your graphs you have a reflow there. That means that the streaming area after the point where something happens is much too short.

It may be your real geometry, but it does not work this way - it is non-physical.

I recommend defining a much longer region for the outflow.

[DevilX]

Hey Uwe,
thanks for helping me. At the top, its an In/Outlet for velocity and a totalPressure with 16 bar, so that reverse flow is possible. But nevertheless, extending the area can be helpful.


I set the pMin/pMax and run a simulation with 16,2 bar and on round 20 cells at the bottom of the limiter (where no flows goes by normally) these pMin/pMax were reached. Also rho und U had strange values.
in short: I guess the whole setup is really sensitive to the mesh, i refinded it and for now it runs with 17 bar but with Turbulence turend off.


Now the question: Is there some kind of guide, how to get a better Mesh? I found this one and it was helpful, but i still get a ot of problems in checkMesh.

[DevilX]

Hey Folks,


update form my side.



As mentioned, the mesh wasn´t so good, so i customized the .stl a bit and used 50 % more cells in blockmesh. I also used a table based approach for rising the pressure at the Inlet.

So it is running with rhoSimpleFoam up to 17 to 16 bar pressure difference, but i don´t use any wallfunctions. I am now trying to find the highest pressure difference, until it diverges. (simulation time went up of course)

[DevilX]

So, if anyone is still interested in modelling a compressible flow:


- rhoSimple works fine in principle
- mostly it was a problem with the geometry after the valve (as piu suggested) - changing this box to a Cylinder with a small Cylinder on top for Outlet worked
- also apllyng In/Outlet Conditions for omega, k, U and T is useful

- now it works with 17 bar pressure difference with 2nd Order schemes, but the timeStepErrors are to high (0.1-2)
- these errors are directly connected to the residuals of p -lowering them also lowers these timeStepErrors


Hope it helps someone!!

[youknowme]

Originally Posted by DevilX

So, if anyone is still interested in modelling a compressible flow:


- rhoSimple works fine in principle
- mostly it was a problem with the geometry after the valve (as piu suggested) - changing this box to a Cylinder with a small Cylinder on top for Outlet worked
- also apllyng In/Outlet Conditions for omega, k, U and T is useful

- now it works with 17 bar pressure difference with 2nd Order schemes, but the timeStepErrors are to high (0.1-2)
- these errors are directly connected to the residuals of p -lowering them also lowers these timeStepErrors


Hope it helps someone!!

HI.
i found your thread very useful as i am too simulating a pressure driven flow. But i stuck because of bounding of my k/epsilon values. i would like to know if you encountered this problem or not while your simulation.