CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   How to simulate hot flue with fine dust flows with subsequent quenching? (http://www.cfd-online.com/Forums/openfoam-solving/58759-how-simulate-hot-flue-fine-dust-flows-subsequent-quenching.html)

leosding December 2, 2005 07:15

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!

niklas December 2, 2005 07:26

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

leosding December 2, 2005 09:30

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.

leosding December 3, 2005 10:50

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?

leosding December 8, 2005 01:29

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.

hjasak December 8, 2005 15:29

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

leosding December 8, 2005 22:26

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.

niklas December 9, 2005 07:54

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

lord_kossity June 11, 2008 07:16

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

olesen June 11, 2008 08:03

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.

lord_kossity June 11, 2008 09:04

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?

lord_kossity June 11, 2008 10:50

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

niklas June 12, 2008 10:19

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

lord_kossity June 12, 2008 10:54

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?

niklas June 13, 2008 01:58

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...

lord_kossity June 13, 2008 02:40

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

niklas June 13, 2008 03:36

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...

niklas June 13, 2008 04:14

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

lord_kossity June 13, 2008 04:42

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!

niklas June 13, 2008 04:45

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?


All times are GMT -4. The time now is 22:23.