CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   simpleFoam - don't know where mass is going (https://www.cfd-online.com/Forums/openfoam-solving/178922-simplefoam-dont-know-where-mass-going.html)

highpressuretube October 19, 2016 10:30

simpleFoam - don't know where mass is going
 
2 Attachment(s)
Hi all,

I am running a simpleFoam k-epsilon flow simulation. Attached is the flow inlet where the inlet diameter of 14,5mm goes down to 3,6mm.

General flow is set to 4l/min so I calculate
0,403722408160178 m/s inlet flow velocity
5,57m/s in the 3,6mm part..

However flow is only reaching 1,78m/s. What is happening there? Where is my mass going?

Problem is continued through the entire model, all steps show reduced velocity.

My p-File:

Code:

{
    version    2.0;
    format      ascii;
    class      volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField  uniform 0;

boundaryField
{
inlet
{
      type            zeroGradient;
}
outlet
{
        type            fixedValue;
        value          uniform 0;
}
walls
{
        type            zeroGradient;
}
SYM
{
      type            empty;
}
}

My U file:
Code:

{
    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            fixedValue;
        value          uniform (0.403722408160178 0.000000 0.000000);
}
outlet
{
      type            zeroGradient;
}
walls
{
        type            fixedValue;
        value          uniform (0. 0. 0.);
}
SYM
{
      type            empty;
}
}

Any suggestions as to where to look for the error is welcome.

Thanks in advance,
highpressuretube

floquation October 19, 2016 11:11

Are you sure your simulation is 3D?

If your simulation is 2D, then you should expect an outlet velocity of (14.5*0.4*L)/(3.6*L)=~1.6 m/s.
Now, looking at your color figure, my eyes would say that the maximum velocity is reached at the beginning of the smaller tube, but it is in fact lower than the maximum value nearby the ending of this smaller tube.
1.6 m/s is slightly lower than 1.78 m/s, and could therefore very well be that value. (Again, I cannot perfectly see the value on a color figure - plot the velocity over a line and you can be sure of the precise value.)

Hence, are you sure your simulation is not in fact 2D?

highpressuretube October 20, 2016 04:15

Hi floquation,

you are soooo right. And I have been spending hours not seeing the woods because of all the trees blocking the view.

But then how would I need to scale my 2D model to be able to compare it to 3D measurements? (I wonder if it makes more sense to reduce to a rotationalsymmetric modell instead of a plane 2D...)

Thanks for the hint,
highpressuretube

floquation October 20, 2016 09:41

Quote:

Originally Posted by highpressuretube (Post 622194)
But then how would I need to scale my 2D model to be able to compare it to 3D measurements? (I wonder if it makes more sense to reduce to a rotationalsymmetric modell instead of a plane 2D...)

That depends on what you'd like to achieve.

If you just want to compare velocities, you should realise that velocities scale with the height of the channel in 2D, whereas they scale with the height squared in 3D.
Using a rotational symmetric model resolves this issue.

If you intend to go for turbulent simulations, you must realise that turbulent flows are not rotationally symmetric, hence a rotationally symmetric model wouldn't be very smart there.
In fact, turbulence is intrinsically 3D, requiring you to use a 3D mesh. If that is too computational intensive for your purposes, then 2D is probably still better than assuming rotational symmetry.
Either way, interpret 2D simulations with caution, as they assume one out of three dimensions to be infinitely long.

highpressuretube October 21, 2016 08:17

Hi floquation,

has to be 3D then.

Thanks for your thoughts,
highpressuretube

highpressuretube October 21, 2016 08:19

How do I mark a thread as solved anyway?


All times are GMT -4. The time now is 10:46.