[Tobi]

Hi together,

i am working on a testcase in which water vaporizes on a heated wire (diameter = 0,1 mm)

The case is working well but i 've problems with my BC couse my steam don't get out of my integration area. In the video i added you can see that its circulating in the case but i wanna let it out.

VIDEO : http://ww3.cad.de/foren/ubb/uploads/...eWater.mpg.zip

So my Boundary-File looks like that:

top
{
    type            patch;
    nFaces          100;
    startFace       42335;
}bottom
{
    type            patch;
    nFaces          100;
    startFace       42435;
}
right
{
    type            slip;
    nFaces          170;
    startFace       42535;
}
symmetryZY
{
    type            symmetryPlane;
    nFaces          300;
    startFace       42705;
}
heat
{
    type            wall;
    nFaces          60;
    startFace       43005;
}
empty
{
    type            empty;
    nFaces          42700;
    startFace       43065;
}

my U and p_rgh files are:

dimensions      [ 0 1 -1 0 0 ];internalField   uniform ( 0 0 0 );
boundaryField
{
    symmetryZY
    {
        type            symmetryPlane;
    }
    heat
    {
        type            fixedValue;
        value           uniform ( 0 0 0 );
    }
    empty
    {
        type            empty;
    }
    right
    {
        type            slip;
    }
    bottom
    {
        type            outletInlet;
        value           $internalField;
        outletValue     $internalField;
    }
    top
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }
}

and the p_rgh file is:

dimensions      [ 1 -1 -2 0 0 ];internalField   uniform 101325;
boundaryField
{
    symmetryZY
    {
        type            symmetryPlane;
    }
    heat
    {
        type            buoyantPressure;
        value           $internalField;
    }
    empty
    {
        type            empty;
    }
    right
    {
        type            slip;
    }
    top
    {
        type            totalPressure;
        phi             phi;
        U               U;
        gamma           1;
        rho             rho;
        psi             none;
        p0              $internalField;
        value           $internalField;
    }
    bottom
    {
        type            buoyantPressure;
        value           $internalField;
    }
}

Any tricks or suggestions?
Thx in advance,
Tobi

[nimasam]

hi
first of All, what is your solver?
second i may try inletOutlet or zeroGradient for bottom in U

[Tobi]

Originally Posted by nimasam

hi
first of All, what is your solver?
second i may try inletOutlet or zeroGradient for bottom in U

Hey nimasam,

my Solver is interPhaseChangeFoam with implement temperatur field and temperatur depended pSat.


Okay i ll try inletOutlet/zeroGradient for the bottom.
I 've tryed to use pressureInletOutletVelocity for the top BC like in the tutorial "breakdam" but the steam can not get out.

okay i ll change the bottom BC and ll tell you if its working.

Thx for replaying
Tobi

[Tobi]

Hi,

i 've solved the case with your advice to change the bottom to zeroGradient or inletOutlet (refer to U).

The steam doesn#t get out of the boundarys

[egp]

Hi Tobi,

Do you have a reference for the temperature dependent Psat model that you are using?

Thanks, Eric

[Tobi]

Originally Posted by egp

Hi Tobi,

Do you have a reference for the temperature dependent Psat model that you are using?

Thanks, Eric

Hi Eric, yes i have the temperature dependent Psat correlation from August-Roche-Magnus.

My simulation is working now and the solution seeems very good.
But i am waiting for experimental values.

I am still trying to get a good solution and handle the BC for that case.
Hope i could help you.

Tobi

[egp]

Hi Tobi,

Thanks. Can you give me a citation for August-Roche-Magnus?

There is a student in our group who is looking at laser-induced vaporization for creating a bubble. Very high-temperature, short duration pulse of energy. She has the heat-transfer and energy absorption modeled, and is now working on the vaporization.

Eric

Originally Posted by Tobi

Hi Eric, yes i have the temperature dependent Psat correlation from August-Roche-Magnus.

My simulation is working now and the solution seeems very good.
But i am waiting for experimental values.

I am still trying to get a good solution and handle the BC for that case.
Hope i could help you.

Tobi

[Tobi]

Originally Posted by egp

Hi Tobi,

Thanks. Can you give me a citation for August-Roche-Magnus?

There is a student in our group who is looking at laser-induced vaporization for creating a bubble. Very high-temperature, short duration pulse of energy. She has the heat-transfer and energy absorption modeled, and is now working on the vaporization.

Eric

Hi Eric,

i used the equation from http://www.tfd.chalmers.se
I ve no citation for that - exept google and wiki

and you can implement it with that code:

{
const dimensionedScalar t30_11("30.11", dimensionSet(0,0,0,1,0,0,0), 30.11);
const dimensionedScalar t273_15("273.15", dimensionSet(0,0,0,1,0,0,0), 273.15);
const dimensionedScalar t1("1", dimensionSet(0,0,0,1,0,0,0), 1);
const dimensionedScalar p610_94("610.94", dimensionSet(1,-1,-2,0,0,0,0), 610.94);
// dimensionSet( [kg], [m], [s], [K], [kg*mol], [A], [cd]), [kg/(m*S^2)]=[Pa]
// August-Roche-Magnus formula
pSat = p610_94 * exp( 17.625*(T-t273_15) / max(t1, T-t30_11) );
//max(1,...) is included to avoid problems with devision by 0
}

Tobi


PS: I am interested to get the bubbles involved in my solver couse i wanna simulate the heat transfer from a heated wire.

Like -
free convection
bubble convection
and film convection

i am not sure if thats correct translated but in my case i don 't get bubbles.