How to simulate hot flue with fine dust flows with subsequent quenching?
 

There is an engineering problem which need CFD to analyse.
The hot flue with fine dust flows into a mix chamber and is quenched by the fresh air blowered into the chamber. The mix effect,( the uniformity of temperature at chamber outlet) is critical.
Now I want to analyse it with OF, but I can not find a proper standard solver for it.
Who can give me some hints for it, which standard solver may be modified to meet my case.
I think these models are need:
turbulence model, heat transfer of gas and particle (maybe dig it out form spray model?).

Thanks a lots in advance!

dieselFoam can do this. The
 

dieselFoam can do this.

The only thing you might need to do is to implement
the properties of your particles.

N

Niklas, Thanks! When I compl
 

Niklas,
Thanks!
When I complete it, the result picture will be posted here. It will be my first industry application of OpenFOAM.

Hi Niklas, I fight with diese
 

Hi Niklas,
I fight with dieselFoam whole day, but I have no idea for it.
My case(one industry equipment, so big; it has been done with commercial CFD software.) is that there are two inlets, one for fresh air, another one for hot flue carried dust, no reaction, is steady flow.
I don't know where to change for particle with diameter, density, specific heat as you pointed out.
Would you (or some experienced people) give me more detailed?

Hi FOAMers, Would someone pro
 

Hi FOAMers,
Would someone provide one basic lagrange model application solver?
In Hrv's MFIX training material(in their wiki) there is a tutorial, but I cannot find it in openfoam release.

thanks a lots.

That would be because it has n
 

That would be because it has not been released - it's basically a simple solver for massless particles carried by the incompressible transient flow solution (built into icoFoam). I am a bit anxious of just passing it over because I haev done a number of lagrangian-related bug fixes and until that makes it into the release I cannot guarantee that the thing will work "out-of-box".

However, if you feel adventureous and don't mind getting your hands dirty, I have no objections in passing it over in the current state.

Hrv

Thanks for your kindness. I w
 

Thanks for your kindness.
I wanna fight with it based on your current works for lagrangian solver if you could post it here.

for starters, get the case ru
 

for starters,
get the case running without particles.
THEN try to use a standard liquid to get the case properly set up, for instance water.
Turn off evaporation (in sprayProperties).
That way you will only have energy exchange between particles and gas and no mass transfer.

and you specify initial droplet/particle condition in injectorProperties and sprayProperties (atomizationModel)

You obviously also need to turn off the breakupModel.

Once that is workin you can start modifying the liquid (solid) properties by adding a new liquid
(src/thermophysicalModels/liquids)

N

Hi FOAMers, Sorry for digg
 

Hi FOAMers,

Sorry for digging out this old thread, but it's a 100% relating to what I'm trying to achieve.

My goal is to add some new liquids, but when I look up the .H files of the different already implemented models, I'm confused about the different numbers stated in brackets e.g.

liquid(18.015, 647.13, 2.2055e+7, 0.05595, 0.229, 273.16, 6.113e+2, 373.15, 6.1709e-30, 0.3449, 4.7813e+4).

What do the numbers stand for?

Thanks for any help,
Andreas

The doxygen docs for 'liquid'
 

The doxygen docs for 'liquid' or the corresponding header
src/thermophysicalModels/liquids/liquid/liquid.H
should help you.

There are member functions corresponding to each of the constructor parameters too.

Thank you! Now it's clear w
 

Thank you!

Now it's clear what the numbers in the liquid line mean.

It is also clear that rho_, pv_, etc. refer to the NSRDS functions.
And now it is getting unclear again. What do the scalars in the different NSRDS functions stand for?

OK, OK, obviously these are
 

OK, OK,

obviously these are coefficients for some interpolation functions, aren't they?

Can you please give me a reference, where I can look them up?

Thanks in advance,
Andreas

Assuming you havent been able
 

Assuming you havent been able to execute the command
find $FOAM_SRC -name "NSRDS*"
I suggest you start here
OpenFOAM/OpenFOAM-1.4.1/src/thermophysicalModels/thermophysicalFunctions/NSRDSfu nctions

To find the NSRDS functions wa
 

To find the NSRDS functions wasn't the problem.

"them" related to the coefficients themselves. where can I find them? Am I too dumb to see their description in the NSRDSfunction directories?

from... NSRDSfunc0.H
 

from...
NSRDSfunc0.H
scalar f(scalar, scalar T) const
{
return ((((f_*T + e_)*T + d_)*T + c_)*T + b_)*T + a_;
}

NSRDSfunc1.H
scalar f(scalar, scalar T) const
{
return exp(a_ + b_/T + c_*log(T) + d_*pow(T, e_));
}

NSRDSfunc2.H
scalar f(scalar, scalar T) const
{
return a_*pow(T, b_)/(1.0 + c_/T + d_/sqr(T));
}

NSRDSfunc3.H
scalar f(scalar, scalar T) const
{
return a_ + b_*exp(-c_/pow(T, d_));
}



etc...

Yeah, but which values do I se
 

Yeah, but which values do I set for a, b, c, ...?

lets look at C7H16.H vapor
 

lets look at C7H16.H

vapor pressure is declared as
NSRDSfunc1 pv_;

and in the constructor we have

pv_(87.829, -6996.4, -9.8802, 7.2099e-06, 2),

and the constructor for NSRDSfunc1 is
NSRDSfunc1(scalar a, scalar b, scalar c, scalar d, scalar e)

i.e. a=87.829, b=-6996.4, etc...

aha, well thats from the .H he
 

aha, well thats from the .H headers

Source:
NSRDS - AICHE
Data Compilation Tables
of Properties of
Pure Compounds

Design Institute for Physical Property Data
American Institute of Chemical Engineers
345 East 47th Street
New York, New York 10017

National Standard Reference Data System
American Institute of Chemical Engineers

T.E. Daubert - R.P. Danner

Department of Chemical Engineering
The Pennsylvania State University
University Park, PA 16802

Well, yesterday I googled for
 

Well, yesterday I googled for some of these key words but I did not find any tables.

Don't you have any other references, preferably some books?

btw, thanks for the patient iteration of the question!

those are books, I think 7 of
 

those are books, I think 7 of them,
thick like @$"! and just full of tables.

what liquid are you interested in?

Ah, ok. Right now I finally fo
 

Ah, ok. Right now I finally found these books in our University Library. So I'm now going to see if they exist also in reality :-)

I have a small perl-script to
 

I have a small perl-script to help me in this that
you might want to use

http://files.nequam.se/liquidProperties.tgz

the units in the NSRDS tables are per mole and not per kg, so some coefficients needs to be recalculated.

there is an example file for water that shows you how its done.
to create the foam .C and .H files just run
./nsrds2foam.pl props.water

Thank you very much. I'll s
 

Thank you very much.

I'll soon have a look at it!

Hi Niklas, Another thing...
 

Hi Niklas,

Another thing...
Since you are still into combustion research (as far as I know/imagine) I have another question to you; in your PhD you mention that "a practical Eulerian treatment of the spray [...] will not be realizable for some time." According to another thread (http://www.cfd-online.com/OpenFOAM_D...tml?1213613536),
I'm interested if it is now possible to simulate combustion using Euler-Euler methods?

Best regards,
Andreas

In openfoam - not at the momen
 

In openfoam - not at the moment afaik, but im working on it http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Im currently looking into the ELSA approach.

Sounds quite interesting to me
 

Sounds quite interesting to me http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Could you share some of your literature with me?

Back to the original topic of
 

Back to the original topic of NSRDS functions and adding liquids...

Today I managed to order the "Data compilation tables of properties of pure compounds" to our TU library http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

What I'm thinking about now is:
Will it be possible to add solid molecules instead of liquid ones or am I then going to run into conflicts concerning atomization an break up for example?

SAE 2005-01-0213 Coupling Vap
 

SAE 2005-01-0213
Coupling Vaporization Model with the Eulerian ....
Lebas, et al.

SAE 2003-01-0005
A 3D Eulerian Model to Improve the Primary Breakup of Atomizing Jet
Blokkeel, et al.

Numerically, its all about Reynolds and Weber numbers so it doesnt matter if its solid or liquid, as long as surface tension, density, viscosity exist and produce usable number.
And you can always turn off any model you dont need.

Thank you very much for the re
 

Thank you very much for the references!

The reason for me asking if it is possible to include solid molecules is that in your example of H2O and the according "props.water" file all the coefficients for the solid properties are omitted (e.g. solid heat capacity).

How can I add these values for example if I want to create the foam .C and .H files for NaCl?

solid properties have been omi
 

solid properties have been omitted from the 'liquids'.

If you still would like to use it I suggest you just replace the heat capacity with the solid heat capacity. etc.

It doesn't seem to be that eas
 

It doesn't seem to be that easy to implement solids using your pearl script...

I'm running into the error "Equation for latent heat of evaporation is not implemented yet."
Could you please help me out!?

which equation is it.
 

which equation is it.

It's the equation for Heat of
 

It's the equation for Heat of Vaporization.
For water it is "solved" using NSRDS function 106 (4 coeeficients).
For NaCl it is "solved" using NSRDS function 100 (only 1 coefficient given).

It seems like that's the problem...

Now that the problem is solved
 

Now that the problem is solved, I add NACL to the liquids directory and run "wmake libso".
At first it looks quite promising;
'dependency list for source file NACL/NACL.C' is made and '~/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libliquids.so' is updated.

But when I try to run my case a FATAL ERROR occurs: Unknown liquid type NACL

why is that???

You need to add NACL/NACL.C
 

You need to add
NACL/NACL.C
to the src/liquids/Make/files file

then you can run 'wmake libso'

Well, I already added that "NA
 

Well, I already added that "NACL/NACL.C" line in any file in the Make directory. - Without any success...

try recompiling the lagrangian
 

try recompiling the lagrangian stuff and the dieselFoam application.

anyhow, that doesn't work eith
 

anyhow, that doesn't work either.
I recompiled the three directories in the lagrangian subdirectory and also the dieselFoam solver.
But NACL is still unknown.

Do you have any further hints?

Hi Niklas,

did you have success with the ELSA approach??
I would be very interested...

Thanks a lot Mr. Nordin for this post, I'm using Perry's handbook for determine the properties, did you have any other suggest?
Thanks a lot
Kind regards