[heather]

thanks Niklas,

i've been putting together an eulerian-eulerian moment-based spray model library, and am looking to add its functionality into one of the distributed solvers - rhoTurbFoam looks like a good candidate... i would like to include the void fraction field into the gas phase equation set - what would be the most appropriate way to do this?

many thanks,

andy

[niklas]

bubbleFoam I would say,
You'll end up with alot of problems near the nozzle if you dont do it 'old Henry's' way.

You should take a look at how he eliminates the void-fraction from the momentum-eq.

N

[heather]

thanks - will take a look...

[heather]

could you put some words around how the void fraction has been eliminated? - looking through the code i'm struggling to see what's going on...

many thanks,

andy

[niklas]

If you solve for ddt(alpha*rhoa*Ua) = ...
you'll end up with numerical problems as alpha->0, since you essentially will be solving a system 0=0.
Usually this is delt with by just setting alpha to something SMALL if it is lower than SMALL.
However, numerically this will give you major stability problems, especially in this situation.
What can be done is to use the continuity equation and derive an equation for ddt(rhoa*Ua) instead, which will be better numerically. You'll get some extra terms because of this and if you look at the momentum equations in bubbleFoam Im sure you can spot them.

Henry has written a nice report on how to derive all of this stuff.
Maybe he can send it to you if you ask him nicely

N

[heather]

many thanks Niklas

the fog is slowly lifting

[davidpalko]

Dear all,

I would like to ask you about setting up properties for Eulerian phase in DieselFoam solver. More concretly, from discussion forum I found out that liquid fuel componet (lagr. particles) physical properties are defined in /src/thermophysicalModels/liquids and enthalpy calculation from temperature is through NASA polynomials specified in therm.dat file within in case.
However, how can be (speaking about dieselFoam) set the properties for Eulerian fluid (properties like viscosity etc...)?

Thank you so much.

Regards,

David

[niklas]

the viscosity and thermal diffusivity is calculating using sutherland's law,

take a look in src/thermophysicalModels/specie/transport/...

Mass diffusion is calculated using a Schmidt number (atm same for all species)

effective properties are all really functions of the turbulent viscosity and the effective enthalpy diffusion is calculated using the Prandtl number (alphah in turbulenceProperties dictionary).

[davidpalko]

Thank you very much Niklas,

David

[davidpalko]

Dear all,
Sorry for such a frequent messaging, but I 've got one more question. According to Nikas's post above viscosity is calculated using sutherland's law. However, these files (in src/thermophysicalModels/specie/transport/...) still needs to read constants mu1, T1, mu2, T2. Wherefrom do they read them? Is this the file where you specify mu1 for temperature T1 and mu2 for T2?

Thank you so much in advance.

Regards,

David

[niklas]

You have two constructors, one where the
As and Ts are given, the other where they are
calculated using 2 viscosities and temperatures.

However, for the chemkin reader, all the transport property constants have been hardcoded, (check chemkinLexer.L) and
are the same for all species.

As = 1.67212e-6
Ts = 170.672

Niklas

[dhebert]

Dear all,

I am using dieselFoam and would like to have the simulation output the gas phase of fuel at a certain boundary "on the fly". Can someone tell me where the fuel field is created, and how I can reference it? For example, when I try C7H16.boundaryField[outletpatch] I get an error saying C7H16 is not defined.

Thanks,

David

[lucchini]

Hi David,
you should try like this:

- composition.Y("C7H16").boundaryField()[outletPatch].

This should work. However, have a look at the implementation of the following classes to better understand the thermodynamic approach:

$FOAM_SRC/thermophysicalModels/combustion/hCombustionThermo
$FOAM_SRC/thermophysicalModels/combustion/mixtures/multiComponentMixture
$FOAM_SRC/thermophysicalModels/combustion/mixtures/reactingMixture
$FOAM_SRC/thermophysicalModels/combustion/mixtureThermo/hMixtureThermo

bye,
Tommaso

[dhebert]

Hi Tommaso,

Thank you so much for your help. What you suggested works great. Thanks also for pointing out where to find implementations in the code, it is a big help.

David

[dhebert]

Hello everyone,

When I insert an injector with a specified diameter, do the droplets get injected from the center or edge of injector. For example, say I set a hollow cone injector with diameter 1mm and angle of 30 degrees. Will the droplets be injected with a 30 degree angle from the center or at 1mm from center?

Thanks,

David

[ville]

Hi David,
In sprayInject.C (/OpenFOAM/OpenFOAM-1.3/src/lagrangian/dieselSpray/spray/)
there is a variable called
injectionPosition which determines the place
where the drop is created (around line 100).
To my understanding the drop is created to this
position initially which would be the nozzle center. You can change this variable here to take into account that your nozzle has a 1mm diameter.
I hope I answered your question.
-Ville

[dhebert]

Ville,

Thanks for pointing this out, it was a big help to know where to start looking. It looks like in the injector definitions the initial droplet position is specified by the position() function. For example, near line 223 of /OpenFOAM/OpenFOAM-1.3/src/lagrangian/dieselSpray/injector/swirlInjector.C there exists:

scalar iRadius = d_*rndGen.scalar01();
scalar iAngle = 2.0*mathematicalConstant::pi*rndGen.scalar01();

return
(
position_
+ iRadius
* (
tangentialInjectionVector1_*cos(iAngle)
+ tangentialInjectionVector2_*sin(iAngle)
)
);

.
.
.

which, if I am not mistaken, randomly selects the radial and angular position of the droplet to be injected. Similar defitions exist for other injector types. If my interpretation is not correct, could someone clarify?

Thanks,

David

[niklas]

That is correct.
The position of the injection point is randomly chosen within the circle defined by injector position and diameter of injector.

[aderliner]

Hi everyone:

I am working on the project about fuel spray,the fuel I am interested is DME, it is C2H6O. I find that there is a folder named C2H6O in /src/thermophysicalmodels/liquids/, I wonder if it is DME. Also, I want to know how to use the fuel.

Thanks a lot~~~!

Best regards~~~!

Bobby

[niklas]

Yes, it is DME.