CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

DieselFoam spray

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 14, 2005, 02:48
Default Hello Niklas, I'm intereste
  #1
New Member
 
Chalothon Thumthae
Join Date: Mar 2009
Posts: 13
Rep Power: 8
thumthae is on a distinguished road
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
thumthae is offline   Reply With Quote

Old   June 14, 2005, 03:53
Default Hi, Yes, surface tension i
  #2
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
Hi,

Yes, surface tension is of some importance in sprays

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
niklas is offline   Reply With Quote

Old   June 14, 2005, 07:31
Default Hi Niklas, Thankyou very muc
  #3
New Member
 
Chalothon Thumthae
Join Date: Mar 2009
Posts: 13
Rep Power: 8
thumthae is on a distinguished road
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
thumthae is offline   Reply With Quote

Old   June 14, 2005, 08:36
Default > The name of my interesting o
  #4
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
> 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
amolrajan likes this.
niklas is offline   Reply With Quote

Old   September 22, 2005, 05:58
Default hi all, - how is the liquid
  #5
New Member
 
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 8
heather is on a distinguished road
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
heather is offline   Reply With Quote

Old   September 22, 2005, 06:02
Default It isnt, because it is assumed
  #6
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
It isnt, because it is assumed that the spray is 'thin'.

N
niklas is offline   Reply With Quote

Old   September 22, 2005, 06:29
Default thanks Niklas, i've been pu
  #7
New Member
 
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 8
heather is on a distinguished road
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
heather is offline   Reply With Quote

Old   September 22, 2005, 06:42
Default bubbleFoam I would say, You'l
  #8
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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
niklas is offline   Reply With Quote

Old   September 22, 2005, 06:53
Default thanks - will take a look...
  #9
New Member
 
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 8
heather is on a distinguished road
thanks - will take a look...
heather is offline   Reply With Quote

Old   September 22, 2005, 09:48
Default could you put some words aroun
  #10
New Member
 
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 8
heather is on a distinguished road
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
heather is offline   Reply With Quote

Old   September 22, 2005, 10:23
Default If you solve for ddt(alpha*rho
  #11
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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

N
niklas is offline   Reply With Quote

Old   September 22, 2005, 10:46
Default many thanks Niklas the fog
  #12
New Member
 
Andrew Heather
Join Date: Mar 2009
Posts: 16
Rep Power: 8
heather is on a distinguished road
many thanks Niklas

the fog is slowly lifting
heather is offline   Reply With Quote

Old   September 8, 2006, 04:50
Default Dear all, I would like to a
  #13
New Member
 
David Palko
Join Date: Mar 2009
Posts: 9
Rep Power: 8
davidpalko is on a distinguished road
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
davidpalko is offline   Reply With Quote

Old   September 8, 2006, 05:42
Default the viscosity and thermal diff
  #14
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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).
niklas is offline   Reply With Quote

Old   September 8, 2006, 06:24
Default Thank you very much Niklas,
  #15
New Member
 
David Palko
Join Date: Mar 2009
Posts: 9
Rep Power: 8
davidpalko is on a distinguished road
Thank you very much Niklas,

David
davidpalko is offline   Reply With Quote

Old   September 11, 2006, 03:25
Default Dear all, Sorry for such a fr
  #16
New Member
 
David Palko
Join Date: Mar 2009
Posts: 9
Rep Power: 8
davidpalko is on a distinguished road
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
davidpalko is offline   Reply With Quote

Old   September 11, 2006, 07:22
Default You have two constructors, one
  #17
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
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
sushant likes this.
niklas is offline   Reply With Quote

Old   November 16, 2006, 10:00
Default Dear all, I am using diesel
  #18
Member
 
David Hebert
Join Date: Mar 2009
Posts: 31
Rep Power: 8
dhebert is on a distinguished road
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
dhebert is offline   Reply With Quote

Old   November 16, 2006, 16:04
Default Hi David, you should try like
  #19
Member
 
Tommaso Lucchini
Join Date: Mar 2009
Posts: 82
Rep Power: 8
lucchini is on a distinguished road
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
lucchini is offline   Reply With Quote

Old   November 16, 2006, 22:04
Default Hi Tommaso, Thank you so mu
  #20
Member
 
David Hebert
Join Date: Mar 2009
Posts: 31
Rep Power: 8
dhebert is on a distinguished road
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
dhebert is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
DieselFoam Spray Evaporation Continuity Error spv24 OpenFOAM Running, Solving & CFD 14 December 30, 2010 11:50
DieselFoam and ReactingFoam matteo_rosa_sentinella OpenFOAM Pre-Processing 4 September 28, 2009 10:35
Problem in dieselFoam skherad OpenFOAM Running, Solving & CFD 0 July 6, 2006 04:48
Problem in dieselFoam skherad OpenFOAM Running, Solving & CFD 0 July 6, 2006 04:45
About dieselFoam tsjb00 OpenFOAM Running, Solving & CFD 3 August 16, 2005 16:59


All times are GMT -4. The time now is 20:43.