
[Sponsors] 
February 9, 2007, 15:32 
i am confused about the defini

#1 
Member
Anthony Costa
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
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; 

February 9, 2007, 16:22 
Hi,
Hi Anthony,
Here is quic

#2 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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/OpenFOAM1.3/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 

May 29, 2009, 07:57 
Atomization

#3 
Member
amin
Join Date: May 2009
Posts: 59
Rep Power: 9 
hi
As I know Dr Niklas.Nordin wrote dieselfoam solver by EulerianLagrangian 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. 

June 3, 2009, 07:43 

#4  
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 22 
Quote:
this will answer all of your questions 

June 3, 2009, 08:26 

#5 
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10 
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/UUp/*(UUp)+g Or, How could I check it? Thanks! 

June 3, 2009, 08:55 

#6  
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 22 
Quote:
where is evaluated at the current timestep n. The particle velocity is then updated like this 

June 3, 2009, 10:11 

#7 
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10 
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 

June 10, 2009, 10:32 

#8 
Senior Member

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 

June 11, 2009, 10:29 

#9 
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10 
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? 

June 12, 2009, 02:54 

#10  
Senior Member

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 Quote:


June 12, 2009, 08:19 

#11 
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10 
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. 

July 2, 2009, 03:58 
plot particle trajectory

#12 
Senior Member

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 

July 3, 2009, 09:09 

#13 
Senior Member
xinguang cui
Join Date: Mar 2009
Posts: 116
Rep Power: 10 
Hey zhou:
I didn't solve this problem. I know somebody to use matlab to do postprocessing for particles. If you have any idea, please let me know. 

July 16, 2009, 11:12 

#14  
Member
David P. Schmidt
Join Date: Mar 2009
Posts: 71
Rep Power: 10 
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 LagrangianEulerian Spray Calculations,” Numerical Heat Transfer, Part B: Fundamentals, 48(1), pp. 2544, 2005. The OF method is great for a uniform gas field. For spatially varying gas velocity (which is always the case) a predictorcorrector treatment would be a little bit better. You can get secondorder accuracy by using a trapezoid rule for integrating velocity. David Quote:


July 21, 2009, 05:28 
postprocesse

#15 
New Member
HuangWei
Join Date: Mar 2009
Posts: 8
Rep Power: 10 
Hi zhoubin,
i want to know how to make a vedio in OpenFoam. Thank you. huoyinghw 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
can't mesh an injector  amira  FLUENT  2  December 29, 2008 07:14 
Fuel injector CFD  carno  FLUENT  0  January 28, 2008 05:11 
Multihole GDI injector  Simone  CDadapco  4  September 14, 2007 20:28 
Turbulence in an Injector  Casey  Main CFD Forum  0  April 11, 2005 18:52 
injector with fluent  mehdi icho  FLUENT  1  February 20, 2002 06:56 