I tried to create a DieselEngi
I tried to create a DieselEngineFoam case, and it runs from CA=-180 to CA=-100 but then I obtain the usual: FOAM FATAL ERROR: attempt to use janafThermo <equation> out of temperature range 200->5000; T=5017
The mesh was created with k3prep (kiva preprocessor) and converted with kivaToFoam. It is a simple cylinder with polar coordinates (with central axis), 3359 cells, D=0.1m s=0.12m.
I tested it with checkMesh - everything looks o.k.
For the initial conditions I set up the data by combining the dieselFoam and engineFoam tutorials.
I have doubts about several imput data: in constant/injectionProperties, what are Cd and X?
How do I specify the start of injection?
I tried to play with deltaT, nCorectors, nNonOrtogonalCorectors, but it did not help.
I read some threads concerning the topic on this Message Board, but did not find the solution.
Where could I find the answers ( working tutorial, papers, commented code..) to start to use this solver?
are you using fixed temperatur
are you using fixed temperature bc ?
what is about the skewness and the non-orthg. ?
The temperature BC are fixedVa
The temperature BC are fixedValue uniform 373 (like for the kivaTest engineFoam tutorial).
The checkMesh gives me:
Non-ortogonality Max: 0.00127146 average: 0.00028. Non-ortogonality : OK
Max skewness = 72.9826 percent. Skewness OK
try adabatic walls and tell me
try adabatic walls and tell me if the problem still exists.
It works with adiabatic walls
It works with adiabatic walls (zeroGradient)! Thank you for helping me.
I run it to ca=40, with injection and combustion. Then when I wanted to proceed from ca=40 it sais:
FOAM FATAL ERROR: attempt to use janafThermo <equation> out of temperature range 200->5000; T=5.5454e+212 (or such a value). What is the reason (and solution) for that?
I will try some other, more realistic meshes and injection setups with adiabatic walls.
I experienced the same problem
I experienced the same problem with fixed temperature bc (see bugs). I hope there is someone (perhaps Niklas) who can solve this problem. I think this is a bug of the dieselEngineFoam solver!
I did some progress but i stil
I did some progress but i still have many questions.
How can I set up a multiple holes injector or multiple injectors?
-what is X? I found something like molar fraction. Which moles in which?
-what is the unit of the massFlowRateProfile list entries?
>What you usually do is to use
>What you usually do is to use a sector mesh (i.e. 8 injetor holes -> 1/8 sector mesh) and apply cyclic boundary conditions.
> X defines the molecular concentration
> The massFlowRateProfile is a dimensionless profile. It only defines how the profile looks like not the total injected mass!
>> How can I set up a multiple
>> How can I set up a multiple holes injector or multiple injectors?
injectorProperties is just a list of injectors so you can add as many as you want.
X is the liquid volume fraction of the
species defined in liquidFuelComponents in
the unit is dimensionless, it is scaled so that the integrated profile corresponds to the injected mass.
I did some simulations with di
I did some simulations with dieselEngineFoam. The results (total pressure and temperature) are not bad, but I still have many doubts and things to improove.
1. I tried to compare total dQ. I calculated it by dQ.weighedAverage(mesh.V()).value()
The shape is nice, but the value (I supose the unit is J/s) is about 50 x higher than the one obtained with VIBE function in qD simulations. Is it another unit (which?) or I am doing something wrong?
2. What is the difference between atomisation (atomisationModel) and breakup (braeakupModel)? I thaught it was a different word for the same thing, and that there was the difference between primary and secondary breakup/atomisatin.
3. What is the difference between injectorTypes unitInjector and commonRailInjector?
4. The sprayProperties. Which injectorModel is appropriate to simulate the injection (unit injector or common rail) in a big diesel engine (bore x stroke = 0.23 x 0.25 m). And the other sprayProperties (atomisationModel, breakupModel,...)? It would be easiest if someone would show me his sprayProperties file of a succesful simulation.
1. I don't know what you are d
1. I don't know what you are doing in detail. Without providing a detailed information about your calculation of the RoHR we are not able to help you.
To something like this:
loop over all species and cells and use
dQ[celli] -= chemistry.specieThermo()[i].H(T[celli])*RRi[celli]*mesh.V()[celli];
to calculte the rate of heate release due to the chemical reactions.
atomisation -> primary break up
break up -> secondary break up
3. Have look at the different properties in the injector directory
4. The choice of spay sub models depends on the application. In your case I would prefer a commonRailInjector, instead of using a atomisationModel define an initial doplet size distribution and KHRT breakupModel.
I expected the same "strange"
I expected the same "strange" behaviour but I cannot find a solution to get rid of it.
This problem breaks my head http://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif
Yupp, I saw the same problem s
Yupp, I saw the same problem some time ago but I don't find the time to investigate the problem further.
In my case the aspect ratio of the squish was very poor because the cells are squeezed from BTC to TDC. This may impact the spray so this strange behaviour shows up.
Fell free to test some different mesh setups (lower the layers in the squish => better aspect ratio at TDC) to see if my guess becomes true.
Any news releated to this stra
Any news releated to this strange spray behaviour?
I have also experienced this,
I have also experienced this, and I got better behaviour when I moved the injector further into the cylinder (i.e. below the highly compressed mesh in the liner region and away from the cylinderHead wall). I figured it was either the poor aspect ratio that caused the problems, like Stefan says, or the fact that the fuel spray was too close to the wall.
I didn't investigate it further, though.
Hi, How could I define an inj
How could I define an injector with multiple holes?
"injectorProperties is just a list of injectors so you can add as many as you want.
But where do I manifest that I want to 'repeat'
the single hole injector N times and put these
injectors at given positions pointing at given
Hi all, I'm trying to defin
I'm trying to define an injector with multiple holes
but I have thi s ERROR:
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.3.6 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
Exec : dieselFoam . sprayTot
Date : Apr 26 2007
Time : 12:03:33
Host : klunk
PID : 13683
Root : /locals/klunkLoc/sprayCNR25
Case : sprayTot
Nprocs : 1
Create mesh for time = 0.0019835
Selecting thermodynamics package hMixtureThermo<reactingmixture>
Selecting chemistryReader chemkinReader
Reading field U
Reading/calculating face flux field phi
Creating turbulence model.
Selecting turbulence model kEpsilon
Creating field DpDt
Constructing chemical mechanism
Selecting ODE solver SIBS
chemistryModel::chemistryModel: Number of species = 5 and reactions = 1
Selecting sootModel noSootModel
Reading combustion properties
Selecting injectorType commonRailInjector
injectionPressureProfile_.size() = 2, massFlowRateProfile_.size() = 12
end constructor. in commonRail
Selecting atomizationModel off
Selecting dragModel standardDragModel
Selecting evaporationModel saturateEvaporationModel
Selecting heatTransferModel RanzMarshall
Selecting wallModel remove
Selecting breakupModel ReitzKHRT
Selecting collisionModel off
Selecting dispersionModel off
Selecting injectorModel hollowConeInjector
Selecting pdfType RosinRammler
--> FOAM FATAL ERROR : object is not allocated
in file /gamma/dettorre/OpenFOAM/OpenFOAM-1.3.6/src/OpenFOAM/lnInclude/autoPtrI.H at line 165.
I put some info and I found the error in the file:
vector dir = sm.injectors()[i].properties()->direction();
but I can't understand what is the problem.
Can somebody help me?
probably there is something wr
probably there is something wrong in your injector dictionary. Please post the latter.
Hi. I run dieselEngineFoam of
I run dieselEngineFoam of tutorials.
Automatically,injection start 0deg. but I want to change injection timing .
Which file have this parameter??
Please tell me.
You have to modify the massFlo
You have to modify the massFlowRateProfile in constat/injectorProperties
|All times are GMT -4. The time now is 00:45.|