i am confused about the defini
 

i am confused about the definitions and uses of the configuration of both the unitInjector and the commonRailInjector in the dieselFoam/dieselEngineFoam cases. position and direction are self explanatory, but ...

assuming i start with some diameter of particle injected, increasing the mass drastically increases the amount of injected material per unit time in the simulation -- the definition of mass also seems to limit the total amount of mass injected into the system before the injector is turned "off". what am i really defining here? shouldn't the mass of each particle be nicely defined by its radius and the density of the species being tracked? (C7H16 here ...)

nparcels also confuses me ... an increase there increases the number of parcels injected per unit time in the simulation, but has no effect whatsoever on the mass injected per unit time.

i assume Cd refers to the stokes law correction term in the lagrangian? what is X?

how is massFlowRateProfile defined?

sorry to as so much at once ... i just can't seem to find the appropriate documentation.

thanks,
ac;

Hi, Hi Anthony, Here is quic
 

Hi,
Hi Anthony,
Here is quick answer to start with...
for instance in injectorProperties, if you
pick a simple unitInjector you can vary the mass flux by changing the Cd value. If you go to
the spray library the explanation will become
clear to you
(see unitInjector.C:
scalar v = massFlowRateProfile_[i][1]/(Cd_*rho*A);
). The unitInjector.C will be found in
/OpenFOAM/OpenFOAM-1.3/src/lagrangian/dieselSpray/injector/unitInjector

The mass flow rate profile is just a list of
flow rates. The left column is the time and
the right column the flow rate in unitless
quantities. So if you have a constant rate you
could say e.g.

massFlowRateProfile
(
(0 8.0)
(0.010 8.0)
(0.040 8.0)
(0.060 8.0)
(0.070 8.0)
);

(or any positive number instead of 8.0)
for a 70 ms injection. I've always kept X at
the value 1 but don't remember what the meaning
of it was.

nparcels is the nof parcels (about) injected during your simulation. So if mass is kept as
constant then you will only increase the nof
parcels.

In my opinion some of the parameters are related just to the implementation and you will have
to read the code to understand and make sure what they mean.
Best regards,
-Ville

Atomization
 

hi
As I know Dr Niklas.Nordin wrote dieselfoam solver by Eulerian-Lagrangian approach(discrete droplet method (DDM) ).If you want to use this method you face to droplet in dense spray instead of liquid core,then why did he create an atomization model like LISA ,....?How can I use these atomization models when I have droplet in start of injection?
I think that atomization already done in DDM method.
It sounds strange.

http://openfoamwiki.net/index.php/Co...ctorProperties

this will answer all of your questions

Hey foamers!

I would like to inquire something about the evolution of the particle velocity.
I have checked the standard drag model and solidParticle about the question. There are only difference for the computing of some parameter. I guess both of them use the same numerical method to difference the particle motion equation.But it is very pity that I really don't know what the numerical method is.
who could tell me the numerical method to difference the following equation in foam?
d(Up)/dt=Cd/U-Up/*(U-Up)+g
Or, How could I check it?

Thanks!

for the dieselSpray you re-write the equation so it reads like this


where is evaluated at the current timestep n.
The particle velocity is then updated like this

Thanks! It is great answer. And it is what I need.
If you like, please answer my another question.
I would like to observe trajectory of separate parcel or particle. It means that the trajectory of the particle is showed in a line during the time in the computing domain.

Do you think the trajectory of particle could be depicted in the paraview?

Do you know how to generate the particle trajectory?

Thanks a lot

Hi Cui,

After your simulation, you could do in this way:
1. foamToVTK;
2. paraview;
3. File/Open/VTK, and select lagrangian, then select sphere instead of arrow, change the scale as you want.
Then you can see the particle.

Hope it works.

Bin

Hey zhoubin:

Thanks for your reply. I have done as your method. However, it is not really what I would like to do.
I care about the position of one particle changing with the time. I would like to know the trajectory of the particle with time. I need to show it as a line for the whole life after one particle entering into the geometry and before it goes out the geometry.

Do you have some experience about it?

Hi Cui,

I do not fully understand your purpose. Do you want to plot them as the streamline?

If yes, I do not have this experience, and it is interesting if some one could tell us. I will also investigate this postprocessor ability.

Bin

Hey zhoubin!

It is almost. I think it is not correct for ` ji xian` because it is the particle position changing with time.

I wish there are other people to care this problem.

plot particle trajectory
 

Hi Cui,

Have you solved your problem about plotting particle trajectory with time?

I remember in Fluent, we can plot this. In OpenFOAM, I only know make a video.

If some friends have any experience, welcome for advice.

Bin

Hey zhou:

I didn't solve this problem. I know somebody to use matlab to do post-processing for particles. If you have any idea, please let me know.

Foamers,

If you are curious about the accuracy of particle integration schemes, I looked at the error in this paper. My tests were with a different code, but it still might be helpful.

Sasanka Are, Shuhai Hou, David P. Schmidt, “Second Order Spatial Accuracy in Lagrangian-Eulerian Spray Calculations,” Numerical Heat Transfer, Part B: Fundamentals, 48(1), pp. 25-44, 2005.

The OF method is great for a uniform gas field. For spatially varying gas velocity (which is always the case) a predictor-corrector treatment would be a little bit better. You can get second-order accuracy by using a trapezoid rule for integrating velocity.

-David

postprocesse
 

Hi zhoubin,:)
i want to know how to make a vedio in OpenFoam. Thank you.
huoyinghw