Hello Niklas, I'm intereste
 

Hello Niklas,

I'm interested to simulate alternative fuel spray such as vegetable oil spray.
I know from someone who have experience in spray, the spray pattern is depended on surface tension( is it correct?).

So I try to search the dieselFoam and other source file, but I cannot found the input file of surface tension.

where is it located?
and please give a suggestion in modeling spray of alternative fuel.

thank,

Torn

Hi, Yes, surface tension i
 

Hi,

Yes, surface tension is of some importance in sprays http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

all liquids and their properties are located in src/thermophysicalModels/liquids
However, the liquid constructor is one of the ...'largest' ones in OpenFOAM so if you have a look at it I suspect you will have some more questions later.

If you know the name of the oil i can add it for you since i have a script to generate the files.
(If it is a single component liquid that is)

>and please give a suggestion in modeling spray of alternative fuel.
ehh...i dont understand the question.

N

Hi Niklas, Thankyou very muc
 

Hi Niklas,
Thankyou very much for your answer.

Yes after I look at src/thermophysicalModels/liquids , I have so many question. However I will try to learn its in Doxygen.


As you said the name of the oil,
The name of my interesting oil are coconut oil, palm oil and sun flower oil. Do you mean these name or chemical name?

Torn

> The name of my interesting o
 

> The name of my interesting oil are coconut oil, palm oil and sun flower oil.
> Do you mean these name or chemical name?

Yes, but as i said, I can only treat single-component liquids, or mixtures of those.
These oils are not very well-defined are they?
This will make the implementation of the properties a bit tricky.

N

hi all, - how is the liquid
 

hi all,

- how is the liquid volume fraction accomodated in the dieselSpray solvers? ...looking at the gas phase equations I couldn't see any void fraction terms etc to represent the presence of/volume occupied by droplets

thanks,

andy

It isnt, because it is assumed
 

It isnt, because it is assumed that the spray is 'thin'.

N

thanks Niklas, i've been pu
 

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

bubbleFoam I would say, You'l
 

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

thanks - will take a look...
 

thanks - will take a look...

could you put some words aroun
 

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

If you solve for ddt(alpha*rho
 

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 http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

N

many thanks Niklas the fog
 

many thanks Niklas

the fog is slowly lifting http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Dear all, I would like to a
 

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

the viscosity and thermal diff
 

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).

Thank you very much Niklas,
 

Thank you very much Niklas,

David

Dear all, Sorry for such a fr
 

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

You have two constructors, one
 

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

Dear all, I am using diesel
 

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

Hi David, you should try like
 

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

Hi Tommaso, Thank you so mu
 

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