[mihir1310]

Originally Posted by Julian K.

.

Mihir, could you also post your fvSchemes? I'd be very interested. Maybe also you rBC setup for P U and T. Thanks.

you mean Bcs of sonicFoam case ?????

As far as schemes are concerned , i used Minmod perfectly , ,However for rhoCentralFoam im not sure, as it is a completely different ballgame ..

[Julian K.]

Originally Posted by mihir1310

you mean Bcs of sonicFoam case ?????

As far as schemes are concerned , i used Minmod perfectly , ,However for rhoCentralFoam im not sure, as it is a completely different ballgame ..

Hi Mihir,

It would be very interesting for me to see your 0/p, 0/U, 0/T files, as well as the system/fvSchemes and maybe also the system/fvSolution dictionary. Perhaps, there is something in, I don't already know.

[mihir1310]

Originally Posted by Julian K.

Hi Mihir,

It would be very interesting for me to see your 0/p, 0/U, 0/T files, as well as the system/fvSchemes and maybe also the system/fvSolution dictionary. Perhaps, there is something in, I don't already know.

Ma

 type            waveTransmissive;
internalField   uniform 1;

boundaryField
{
    inlet
    {
        type            calculated;
        value           uniform 1;
    }
    outlet
    {
        type            calculated;
	//        value           uniform 3;
    }
    
    }

P:

boundaryField
{
    inlet           
    {
         /*type totalPressure; 
	  p0 uniform 1.0135e5; 
         U U; 
	  phi phi; 
	  rho none; 
	  psi none; 
	  gamma 1.4; */
	  type fixedValue;
	  value uniform 54000;     
    }

    outlet          
    {
       type zeroGradient;
	/* type            waveTransmissive;
        value           uniform 8800;
	 field           U;
        gamma           1.4;
	 phi             phi;
        rho             rho;
        psi             psi;
        lInf            0.01;
        fieldInf        8800; */
        
        
    }

T:

internalField   uniform 281;

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform 273;
    }

    outlet          
    {
        type            zeroGradient;
    }

U:

[CODE]internalField   uniform (260.39 0 0);

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform (380 0 0);
    }

    outlet          
    {
		type            inletOutlet;
        inletValue      uniform (10 0 0);
        value           uniform (10 0 0);
        

//type            zeroGradient;
	/*type            waveTransmissive;
        value           uniform (10 0 0 );
	 field           U;
        gamma           1.4;
	 phi             phi;
        rho             rho;
        psi             psi;
        lInf            0.01;
        fieldInf        (10 0 0 ); */
[/CODE]

[mihir1310]

solvers
{
    rho  diagonal {};
    rhoU diagonal {};
    rhoE diagonal {};

    U smoothSolver
    {
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-09;
        relTol           0.01;
    };

    h smoothSolver
    {
        smoother         GaussSeidel;
        nSweeps          2;
        tolerance        1e-10
        relTol           0;
    };
}

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(tauMC) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default          linear;
    reconstruct(rho) vanLeer; 
    reconstruct(U)   vanLeerV;
    reconstruct(T)   vanLeer;

}

snGradSchemes
{
    default         corrected;
}

[Julian K.]

Thanks Mihir!

However, I am a little bit confused, because you said that you use Minmod for the discretization of the divergent terms and backward for the convective terms.

By the way, are you simulating a CD nozzle, as well?

[mihir1310]

Originally Posted by Julian K.

Thanks Mihir!

However, I am a little bit confused, because you said that you use Minmod for the discretization of the divergent terms and backward for the convective terms.

By the way, are you simulating a CD nozzle, as well?

ohh i meant you wanted my rhoCenrtalFoam case [which did not work ]

heres for sonicFoam

ddtSchemes
{
    default backward;           
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss Minmod;
    div(phid,p)     Gauss Minmod;
    div(phi,e)      Gauss Minmod;
}

laplacianSchemes
{
    default         none;
    laplacian(mu,U) Gauss linear corrected;
    laplacian(mu,e) Gauss linear corrected;
    laplacian((rho*(1|A(U))),p) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p;

Im simulating outfield of the nozzle . So my inlet is the "nozzle outlet" ..

[Julian K.]

Okay, thanks. I think I'll try your settings. Let's see what it produce.

By the way:
With rhoCentralFoam I noticed that a change of the lInf value (of the waveTransmissive BC) from 0.01, over 0.05, 0.5, 5, 50, 500 and finally 5000 does not have any effect on the result of my simulation. Which is, that the pressure waves are not transmitted across the outlet. Thus, I assume that rhoCentralFoam is (by any reason) not capable to apply the waveTransmissive BC. However, sonicFoam does apply the waveTransmissive BC, and changes of lInf resulted in very different behaviours.

Does anyone know, why a certain BC does not work with a certain solver?

[bephi]

hi at all!
i read all the comments concerning the growing courant nr. problem because mine is the same

i set up a case with the icoFoam solver to achieve a first solution which i can improve later with other solver that display the reality better. i took the controlDict, fvSchemes and fvSolutions from the "icoFoam cavity tutorial".
unfortunately not even this simplified calculation works because after round about 8 to 10 time steps the courant nr. is increased to something over e+100 (well i'd say this is a bit more than 1 )

first i tried to decrease the time step to 3.5e-6 and change the writeControl to "adjustableRunTime"... but when looked at the runlogs, the timestep didn't change and remained constant.

then i tried to limit the courant number with "maxCo 1", but i read that it doesn't work for "icoFoam", because its a simple solver. is this correct?

do you have any idea, what i can do to achieve a solution that doesn't abort?

[joern]

hi bephi,

try to use bounded schemes like "upwind" or a TVD-Scheme for the div-schemes.

i think the convective terms produce an unbounded solution so you have to limit them.
icofoam solves the NS-Eqs. I haven't testet this solver but i tested simplefoam and there its nearly the same problem.


Joern

[bephi]

hi joern!
thanks a lot for the quick reply!
so you say I should change this:

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linear;                            // change into "Gauss upwind"
}
laplacianSchemes
{
    default         none;
    laplacian(nu,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
}
interpolationSchemes
{
    default         linear;
    interpolate(HbyA) linear;
}
snGradSchemes
{
    default         corrected;
}
fluxRequired
{
    default         no;
    p;
}

EDIT: i changed it and first my max.Co-Nr. doesn't get over 7! but unfortunately the Co-Nr. increases again after round about 20 timesteps until the calculation ends... an improvement was achieved but what can be changed too?

would it be okay when the mean value of the co-nr. is <1 or should the max Co-Nr <1 as well?


if also needed, here are my files:
p and U starting files:

dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.000000;
boundaryField
{
symmetry
{
type symmetryPlane;
}
inlet
{
type fixedValue;
value uniform 452.38;
}
outlet
{
type zeroGradient;
}

dimensions [0 1 -1 0 0 0 0];
internalField uniform ( 0.000000 0.000000 -1.000000 );
boundaryField
{
symmetry
{
type symmetryPlane;
}
inlet
{
type fixedValue;
value uniform ( 0.000000 0.000000 -1.000000 );
}
outlet
{
type zeroGradient;
}

controlDict

application icoFoam;
startFrom       startTime;
startTime       0;
stopAt          endTime;
endTime         1e-3;
deltaT          3.5e-6;
writeControl    adjustableRunTime;
writeInterval   10;
purgeWrite      0;
writeFormat     ascii;
writePrecision  6;
writeCompression uncompressed;
timeFormat      general;
timePrecision   6;
runTimeModifiable yes;
adjustTimeStep    yes;
maxCo        1.0;

fvSchemes

ddtSchemes
{
    default         Euler;
}
gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
}
divSchemes
{
    default         none;
    div(phi,U)      Gauss upwind;
}
laplacianSchemes
{
    default         none;
    laplacian(nu,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
}
interpolationSchemes
{
    default         linear;
    interpolate(U) linear;
}
snGradSchemes
{
    default         corrected;
}
fluxRequired
{
    default         no;
    p;
}

fvSolver

solvers
{
    p PCG
    {
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0;
    };
    U PBiCG
    {
        preconditioner   DILU;
        tolerance        1e-05;
        relTol           0;
    };
}
PISO
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
}

[joern]

the max-conum should not be much larger than 1 because the discretisation of OF ist just semi implicit.
the decoupling in OF causes explicit factors.

In my test cases (for my diploma thesis) the solver simplefoam was only stable with maxCoNum<1.5.

Try maxCoNum<1. 7 is too much for OF, i think. That would just work with a full implicit solver.


Add:
If you use "Gauss linear" for all discretisations you get an central that is instable for ALL Delta t.

[alberto]

Add:
If you use "Gauss linear" for all discretisations you get an central that is instable for ALL Delta t.

A bit too broad as statement. Central schemes, largely used in LES also for the convective term, are unstable only if the local Péclet number is larger than 2.

Best,

[mohsenkh599]

hi everyone
I have a new solver for two-phase modeling. but there is a problem while running any case (dam break for instance). when in ControlDict I put the write interval one second the solution diverge quickly but if I put it .05 second the solution converges. I could not understand how the write interval affects the convergence of the system.
please help as soon as possible

[alberto]

Originally Posted by bephi

if also needed, here are my files:
p and U starting files:

dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.000000;
boundaryField
{
symmetry
{
type symmetryPlane;
}
inlet
{
type fixedValue;
value uniform 452.38;
}
outlet
{
type zeroGradient;
}

dimensions [0 1 -1 0 0 0 0];
internalField uniform ( 0.000000 0.000000 -1.000000 );
boundaryField
{
symmetry
{
type symmetryPlane;
}
inlet
{
type fixedValue;
value uniform ( 0.000000 0.000000 -1.000000 );
}
outlet
{
type zeroGradient;
}

You are fixing both velocity and pressure and velocity at the inlet for an incompressible flow (you use icoFoam). Let the inlet as is, but fix the pressure at the outlet, and set it to zeroGradient at the inlet.

Best,

[alberto]

Originally Posted by mohsenkh599

hi everyone
I have a new solver for two-phase modeling. but there is a problem while running any case (dam break for instance). when in ControlDict I put the write interval one second the solution diverge quickly but if I put it .05 second the solution converges. I could not understand how the write interval affects the convergence of the system.
please help as soon as possible

It doesn't :-)

Please open a new thread, and provide more information to increase the chances someone can help.

Best,

[bephi]

Originally Posted by alberto

You are fixing both velocity and pressure and velocity at the inlet for an incompressible flow (you use icoFoam). Let the inlet as is, but fix the pressure at the outlet, and set it to zeroGradient at the inlet.

Best,

hello alberto! thanks for your hint!

you are right that it doesn't make sense to fix pressure and velocity at the inlet! i changed it but now my max. Co-No is increasing again to around about 7... is this a problem?

greets!

[joern]

Originally Posted by alberto

A bit too broad as statement. Central schemes, largely used in LES also for the convective term, are unstable only if the local Péclet number is larger than 2.

Best,

ok, you'r right. but for icoFoam (like simplefoam) a use of Central Schemes lead to da central method.

@bephi:
a maxconum of 7 is now problem as long as your solution is ok ^^
take a look at the results (paraview) if they look physical ok.
or try to calculate a bit longer to look if the solver stays stable.

have you tried smaller timesteps to see if the maxconum stays smaller?

[bephi]

hi!
at the moment my problem is the following:
i calculated a time step of 3.5e-6 s because my highest velocity is 26.83 m/s² and the smalest element lenght is 0.0001m
the fluid needs round about 0.3 to 0.5 s to flow through the model so it would take 100000 steps which is too much in my in opinion.. so i increased the timestep to 0.0003 and after that to 0.00003 but then the co-number increases again until the calculation crashes...

i didn't thought that a simple laminar calculation would be so difficult?!

[joern]

if it takes to many steps, try a coarser mesh.
but if your mesh is too fine you need smaller timesteps, thats normal.

are you sure about your max. velocity?
i dont know the eigenvalues of the NS-eqs but for the euler-equations the max. velocity isnt just the max. u, its max.(u+c) with the speed of sound c.

my tip:
try smaller timesteps, you will see if the solver stays stable.


btw: how many cells does your testcase have?

[bephi]

now a calculation with 100 timesteps was successful...i think i'll set up 100 additional steps and look what happens...
when do i know that the solution is converged?

my model has 116112 trias, 622697 tetras and 198870 pentas