[sebastian_vogl]

As I'm not able to compress all files of my case to a size that allows posting them here I'm attaching the files which were changed from the aachenbomb tutorial case. All other files remain are exactly the same as in the aachembomb case.

sprayProperties
injectorProperties
controlDict

[niklas]

So the differences are...

Your pressure and temperature are 50 bar and 800K. With droplets of that size they wont go very far in such high density gas since the influence of the gas is quite high. This is also probably why they dont remain in a straight line.

I reduced mine to 1 bar and 300K to increase the penetration.
Your drops are significantly smaller, increasing the drag even more.

You also have gravity on so the drops reach terminal velocity and hence their distance is kept constant.

[sebastian_vogl]

Thank you for your help, Mr Nordin!

[sebastian_vogl]

So I changed the system properties to Temperatur=300K and pressure=1bar. Furthermore I increased the droplet diameter to 100µm. At first I tried a particle velocity of 100 m/s and then 50 m/s (as in my movie below) to look wether it has any effect. However, whichever particle velocity I take, as you can see in my small movie below, the form of the droplets flow still looks like a snake. For me it seems as if the injector changes its position and that the system properties aren't responsable for the flow behaviour as it can be realized from the time of injection.
The movie doesn't contain all time steps to keep the file size low.



I would be very glad to hear your opinion.
Yours,
Sebastian Vogl

[sebastian_vogl]

Unfortunately I had to realize that the file size is still to big. Would it be all right for you if I sent it you via E-mail?

[edwin_gonzalez]

hi to all, i am new with openfoam and his dieselfoam solver.
i would like to know, how or where i can change the initial ambient density.

I hope you can help me.

[sebastian_vogl]

The dieselFoam solver consists of the following folders:
0, chemkin, constant, system. The "0"-file contains all files that define your initial system properties. There you can vary temperature, pressure, mixture composition etc. So you should be able to specify your initial system conditions.

Yours,
Sebastian Vogl

[edwin_gonzalez]

hi Sebastian,
i am again,
I have other question
¿what does it means (internalField uniform 0.233) in the O2 file ? ¿it doesn't have units?

thanks
Edwin

[sebastian_vogl]

The number 0.233 describes the amount of O2 which is contained in the air. The rest is N2. The "unit" is:
(mol of O2)/(mol of air).
So it doesn't have units as the mol on both sides of the fraction cancel.

[sebastian_vogl]

Hallo everybody,

I want to simulate the injection and evaporation of single drops (C7H16) into a fluid (air). The case is pretty similar to what I wrote in my previous posts above. I have got 5 injectors injecting 10 drops each in a distance of 1e-4 seconds. All drops habe got the same size (50e-6m) and the same start velovity 25m/s. The velocity of the fluid is 0m/s.

My geomitry is a cuboid similar to the aachenBomb tutorial case. The coordinate system is exactly at the same position as in the tutorial, i.e in the middle of the ground wall. The droplets fly in the direction of the positive y-axis (in the tutorial case the spray flies in negative y-direction). The edges have the following length:

x direction=19,75mm
y direction=100mm
z direction=9,75mm

The grid is:

x: 79 zells with each 0,25mm length
y: 400 zells with each 0,25mm length
z: 39 zells with each 0,25mm length

The sense of the geometry and grid size is that every injector has its position in the middle of the face of a zell.
My problem is that, after starting the simulation, I get this error message:

--> FOAM FATAL ERROR : Cannot find injection position (-2 0.001 3.12962e-15)#0 Foam::error::printStack(Foam:stream&) in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::spray::inject() in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libdieselSpray.so"
#3 Foam::spray::evolve() in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libdieselSpray.so"
#4 main in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/dieselFoam "
#5 __libc_start_main in "/lib64/libc.so.6"
#6 Foam::regIOobject::readIfModified() in "/home/singh/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linux64GccDPOpt/dieselFoam "


FOAM aborting


I added my injector properties file and my blockMeshdict file.
Has anyone of you already experienced that problem and knows the solution?
I would be pleased to hear from you.

With kind regards,
Sebastian Vogl

injector properties file:

(
{
injectorType definedInjector;

definedInjectorProps
{
position (0 0.001 0);
direction (0 1 0);
diameter 0.00005;
Cd 0.9;
mass 4.433746186078091663e-10;
temperature 303;
nParcels 10;

X
(
1.0
);

massFlowRateProfile
(
(0.0000e-4 0.0)
(0.0001e-4 1.0)
(0.0002e-4 0.0)

(1.0000e-4 0.0)
(1.0001e-4 1.0)
(1.0002e-4 0.0)

(2.0000e-4 0.0)
(2.0001e-4 1.0)
(2.0002e-4 0.0)

(3.0000e-4 0.0)
(3.0001e-4 1.0)
(3.0002e-4 0.0)

(4.0000e-4 0.0)
(4.0001e-4 1.0)
(4.0002e-4 0.0)

(5.0000e-4 0.0)
(5.0001e-4 1.0)
(5.0002e-4 0.0)

(6.0000e-4 0.0)
(6.0001e-4 1.0)
(6.0002e-4 0.0)

(7.0000e-4 0.0)
(7.0001e-4 1.0)
(7.0002e-4 0.0)

(8.0000e-4 0.0)
(8.0001e-4 1.0)
(8.0002e-4 0.0)

(9.0000e-4 0.0)
(9.0001e-4 1.0)
(9.0002e-4 0.0)
);

velocityProfile
(
(0.0 25.0)
(9.0002e-4 25.0)
);
}
}

{
injectorType definedInjector;

definedInjectorProps
{
position (-2 0.001 0);
direction (0 1 0);
diameter 0.00005;
Cd 0.9;
mass 4.433746186078091663e-10;
temperature 303;
nParcels 10;

X
(
1.0
);

massFlowRateProfile
(
(0.0000e-4 0.0)
(0.0001e-4 1.0)
(0.0002e-4 0.0)

(1.0000e-4 0.0)
(1.0001e-4 1.0)
(1.0002e-4 0.0)

(2.0000e-4 0.0)
(2.0001e-4 1.0)
(2.0002e-4 0.0)

(3.0000e-4 0.0)
(3.0001e-4 1.0)
(3.0002e-4 0.0)

(4.0000e-4 0.0)
(4.0001e-4 1.0)
(4.0002e-4 0.0)

(5.0000e-4 0.0)
(5.0001e-4 1.0)
(5.0002e-4 0.0)

(6.0000e-4 0.0)
(6.0001e-4 1.0)
(6.0002e-4 0.0)

(7.0000e-4 0.0)
(7.0001e-4 1.0)
(7.0002e-4 0.0)

(8.0000e-4 0.0)
(8.0001e-4 1.0)
(8.0002e-4 0.0)

(9.0000e-4 0.0)
(9.0001e-4 1.0)
(9.0002e-4 0.0)
);

velocityProfile
(
(0.0 25.0)
(9.0002e-4 25.0)
);
}
}

{
injectorType definedInjector;

definedInjectorProps
{
position (-4 0.001 0);
direction (0 1 0);
diameter 0.00005;
Cd 0.9;
mass 4.433746186078091663e-10;
temperature 303;
nParcels 10;

X
(
1.0
);

massFlowRateProfile
(
(0.0000e-4 0.0)
(0.0001e-4 1.0)
(0.0002e-4 0.0)

(1.0000e-4 0.0)
(1.0001e-4 1.0)
(1.0002e-4 0.0)

(2.0000e-4 0.0)
(2.0001e-4 1.0)
(2.0002e-4 0.0)

(3.0000e-4 0.0)
(3.0001e-4 1.0)
(3.0002e-4 0.0)

(4.0000e-4 0.0)
(4.0001e-4 1.0)
(4.0002e-4 0.0)

(5.0000e-4 0.0)
(5.0001e-4 1.0)
(5.0002e-4 0.0)

(6.0000e-4 0.0)
(6.0001e-4 1.0)
(6.0002e-4 0.0)

(7.0000e-4 0.0)
(7.0001e-4 1.0)
(7.0002e-4 0.0)

(8.0000e-4 0.0)
(8.0001e-4 1.0)
(8.0002e-4 0.0)

(9.0000e-4 0.0)
(9.0001e-4 1.0)
(9.0002e-4 0.0)
);

velocityProfile
(
(0.0 25.0)
(9.0002e-4 25.0)
);
}
}

{
injectorType definedInjector;

definedInjectorProps
{
position (2 0.001 0);
direction (0 1 0);
diameter 0.00005;
Cd 0.9;
mass 4.433746186078091663e-10;
temperature 303;
nParcels 10;

X
(
1.0
);

massFlowRateProfile
(
(0.0000e-4 0.0)
(0.0001e-4 1.0)
(0.0002e-4 0.0)

(1.0000e-4 0.0)
(1.0001e-4 1.0)
(1.0002e-4 0.0)

(2.0000e-4 0.0)
(2.0001e-4 1.0)
(2.0002e-4 0.0)

(3.0000e-4 0.0)
(3.0001e-4 1.0)
(3.0002e-4 0.0)

(4.0000e-4 0.0)
(4.0001e-4 1.0)
(4.0002e-4 0.0)

(5.0000e-4 0.0)
(5.0001e-4 1.0)
(5.0002e-4 0.0)

(6.0000e-4 0.0)
(6.0001e-4 1.0)
(6.0002e-4 0.0)

(7.0000e-4 0.0)
(7.0001e-4 1.0)
(7.0002e-4 0.0)

(8.0000e-4 0.0)
(8.0001e-4 1.0)
(8.0002e-4 0.0)

(9.0000e-4 0.0)
(9.0001e-4 1.0)
(9.0002e-4 0.0)
);

velocityProfile
(
(0.0 25.0)
(9.0002e-4 25.0)
);
}
}

{
injectorType definedInjector;

definedInjectorProps
{
position (4 0.001 0);
direction (0 1 0);
diameter 0.00005;
Cd 0.9;
mass 4.433746186078091663e-10;
temperature 303;
nParcels 10;

X
(
1.0
);

massFlowRateProfile
(
(0.0000e-4 0.0)
(0.0001e-4 1.0)
(0.0002e-4 0.0)

(1.0000e-4 0.0)
(1.0001e-4 1.0)
(1.0002e-4 0.0)

(2.0000e-4 0.0)
(2.0001e-4 1.0)
(2.0002e-4 0.0)

(3.0000e-4 0.0)
(3.0001e-4 1.0)
(3.0002e-4 0.0)

(4.0000e-4 0.0)
(4.0001e-4 1.0)
(4.0002e-4 0.0)

(5.0000e-4 0.0)
(5.0001e-4 1.0)
(5.0002e-4 0.0)

(6.0000e-4 0.0)
(6.0001e-4 1.0)
(6.0002e-4 0.0)

(7.0000e-4 0.0)
(7.0001e-4 1.0)
(7.0002e-4 0.0)

(8.0000e-4 0.0)
(8.0001e-4 1.0)
(8.0002e-4 0.0)

(9.0000e-4 0.0)
(9.0001e-4 1.0)
(9.0002e-4 0.0)
);

velocityProfile
(
(0.0 25.0)
(9.0002e-4 25.0)
);
}
}
)


blockMeshdict file:

convertToMeters 0.001;

vertices
(
(-9.875 0 -4.875)
(-9.875 0 4.875)
(9.875 0 5.875)
(9.875 0 -4.875)
(-9.875 100 -4.875)
(-9.875 100 4.875)
(9.875 100 4.875)
(9.875 100 -4.875)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (39 79 400) simpleGrading (1 1 1)
);

edges
(
);

patches
(
wall walls
(
(2 6 5 1)
(0 4 7 3)
(0 1 5 4)
(4 5 6 7)
(7 6 2 3)
(3 2 1 0)
)
);

mergePatchPairs
(
);

[sebastian_vogl]

Hallo everybody,

I recently found my mistake on my own. It was as simple as stupid:
I wanted to place 4 injectors in a region of 4mm in x-axis around the central positioned injector. However I wrote e.g (-2 0.001 0) in the injectorprops-file instead of (-0.002 0.001 0).I simply mixed up meters and millimeters. So the program couldn't find the position because it was outside the geometry. The problem was probably to simple to be seen by me.
Hopefully I didn't waste your time. Nevertheless I want to thank everyone who reflected about the problem.

Yours,
Sebastian

[haghajani]

Hello everybody!

Is dieselFoam, the proper solver, to model High Pressurized Liquid Hydrogen spill from a pipeline?

The pressure is 15-20 Mpa and the hole side is in the order of 1 cm.
The matter which made my interest to think to dieslfoam, is LH2's atomization after releasing to atmosphere;

Thanks in advance,
Hamed

[haghajani]

Dear Foamers,

Please elaborate,

if the "dieselFoam", is the right/proper solver to be implemented in problems such as "High Pressurized Liquid Hydrogen (LH2) spill" from a pipeline?
The Pressure is in the Range of "15-20" Mpa and the Hole in the Pipe is in the order of "1" Cm.

Liquid Hydrogen jet's spray breakup and atomization (in to air) and vaporization (to gas Hydrogen), shortly after its spill from an unintended damage to a carrier pipeline, and formation of combustible clouds due to its dispersion and buoyancy(which may brings a fire, if ignition sources be available), are the key parameters of this problem, and It seems all this capabilities are gathered in "dieselFoam".

Isn't the above mentioned problem, similar to spray through a simple orifice?
How, liquid jet at inlet for studying its probable droplet formation/breakup, is defined?

Looking forward to have your kind comments,

Thank you in advance,
Hamed Aghajani

[tsencic]

Hello everybody,
I have problems with the shape of diesel sprays, with the spray angle in particular:
Whichever injectorModel and sprayAngle I select I obtain a thin jet. Only the top of it seem to follow the sprayAngle setting, while for the rest, the droplets seem to fly paralel. I even tried to modify some injector submodels, but I did not get wider sprays from the nozzle. Example: ConstInjector, sprayAngle 50:

From the arrow directions it is visible that the velocities are oriented as it is set, but the dropplets do not fly in that direction. In other words, the dropplet path is not aligned with the droplet velocity vector.
I tried to reproduce something like this:

What could be the reason for that? How could I solve it?
Do I interprete results badly? How could I reproduce the spray angles that are reported by experiments reports?

[niklas]

your initial drop-size is too small.

[ville]

Hi,

I guess I should begin by thanking Niklas for writing an excellent Lagrangian particle tracking
code for OpenFOAM. I'm happy to announce that
after running and running with big meshes, parallel, big clouds etc I'm not able to report
on any problem in the particle tracking algorithm so far.


Then to the question.. I think that the question of spray shape is really good. If you are doing RANS you need to specify the spray opening angle since you won't be resolving the
flow field and shear layer correctly.

In the experimental picture the spray opening
angle is formed by two factors 1) initial phenomena near the nozzle and 2) shear layer vorticity of the jet. The problem is that with the huge cell sizes of your simulation + RANS turbulence model you won't get images like in experiments and you
have strange phenomena such as particles going
in a line, not really forming a 'physical' looking cloud etc .

With LES in very fine grids you get similar spray shapes as in experiments (like the one above) but you need lots of cells. I'm making a phd on LES of sprays on grids as fine as 40-100 microns and then you can reproduce quite reasonably some of the experimental phenomena. And the small grid size is not a problem if particles are say 10 microns which is e.g. in diesel type situation - to my understanding - quite common further away from the nozzle, depends on injector details for example.


Regards,
Ville

[tsencic]

Ok. Thank You for the answers.
I increased droplet size, turned off breakup, and reduced cell size.
Experiment settings are:
fuel: NHPT (C7H16)
O2: 0% (I turned chemistry off)
Ambient temperature: 1000 K
Ambient pressure: 4.33 MPa
Ambient density: 14.8 kg/m3
nozzle diameter: 0.1 mm
injection pressure: 150 MPa
fuel temp: 373 K
experimental liquid length: 9.2 mm

I attach the sprayProperties and injectorProperties, I would be glad If You find the time to take a look:


The turbulence model is kEpsilon, cell size is about 0.4 mm around the nozzle.

Here is the result:


It looks a bit better but I am still not satisfied. It is normal that the cone angle decreases after the first moment, but here it falls to almost 0. Hence I do not obtain a conical spray but more a mushroom shape spray. The direction velocities point to 50deg, but the droplets fly downstream.

My final goal is soot simulation on large engines (bore abot 0.5 m), but I supposed that I should start from obtaining a reasonable spray. Perhaps it is not a god aproach, since If I need such a fine grid in a huge mesh I will need a computer power that is not available to me. I would apreciate an opinion on this.

Where is my mistake? Is there a guidance for cell size to obtain a more phisical looking spray, using RANS and kEpsilon?

Best regards,
Tomislav

[tsencic]

Sorry,
here are the files:
sprayProperties

injectorProperties


Here is the image


Tomislav

[tsencic]

I try again:
sprayProperties
injectorProperties

[ville]

Hi,
How many cells does the domain above contain i.e.
how many cells are there to resolve the spray width?
I would put at least 20-30-40 to resolve the region above the x-z plane. The droplet momentum relaxation
timescale is probably also very high. Since that scale is proportional to d^2 you can stop the droplets earlier (if that is what you want) if you decrease d by some factor. BTW, in your input files
I'd turn the includeOscillation to "no". You should also make the mesh finer in x direction accordingly and add more parcels (how many drops
do you now have in one parcel?).
-Ville