|
[Sponsors] |
How to simulate hot flue with fine dust flows with subsequent quenching? |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
December 2, 2005, 07:15 |
How to simulate hot flue with fine dust flows with subsequent quenching?
|
#1 |
Member
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 17 |
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! |
|
December 2, 2005, 07:26 |
dieselFoam can do this.
The
|
#2 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
dieselFoam can do this.
The only thing you might need to do is to implement the properties of your particles. N |
|
December 2, 2005, 09:30 |
Niklas,
Thanks!
When I compl
|
#3 |
Member
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 17 |
Niklas,
Thanks! When I complete it, the result picture will be posted here. It will be my first industry application of OpenFOAM. |
|
December 3, 2005, 10:50 |
Hi Niklas,
I fight with diese
|
#4 |
Member
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 17 |
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? |
|
December 8, 2005, 01:29 |
Hi FOAMers,
Would someone pro
|
#5 |
Member
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 17 |
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. |
|
December 8, 2005, 15:29 |
That would be because it has n
|
#6 |
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,904
Rep Power: 33 |
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk |
|
December 8, 2005, 22:26 |
Thanks for your kindness.
I w
|
#7 |
Member
Leosding
Join Date: Mar 2009
Posts: 51
Rep Power: 17 |
Thanks for your kindness.
I wanna fight with it based on your current works for lagrangian solver if you could post it here. |
|
December 9, 2005, 07:54 |
for starters,
get the case ru
|
#8 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
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 |
|
June 11, 2008, 08:16 |
Hi FOAMers,
Sorry for digg
|
#9 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
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 |
|
June 11, 2008, 09:03 |
The doxygen docs for 'liquid'
|
#10 |
Senior Member
Mark Olesen
Join Date: Mar 2009
Location: https://olesenm.github.io/
Posts: 1,679
Rep Power: 40 |
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. |
|
June 11, 2008, 10:04 |
Thank you!
Now it's clear w
|
#11 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
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? |
|
June 11, 2008, 11:50 |
OK, OK,
obviously these are
|
#12 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
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 |
|
June 12, 2008, 11:19 |
Assuming you havent been able
|
#13 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
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 |
|
June 12, 2008, 11:54 |
To find the NSRDS functions wa
|
#14 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
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? |
|
June 13, 2008, 02:58 |
from...
NSRDSfunc0.H
|
#15 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
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... |
|
June 13, 2008, 03:40 |
Yeah, but which values do I se
|
#16 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
Yeah, but which values do I set for a, b, c, ...?
|
|
June 13, 2008, 04:36 |
lets look at C7H16.H
vapor
|
#17 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
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... |
|
June 13, 2008, 05:14 |
aha, well thats from the .H he
|
#18 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
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 |
|
June 13, 2008, 05:42 |
Well, yesterday I googled for
|
#19 |
Member
Andreas Dietz
Join Date: Mar 2009
Location: Munich
Posts: 79
Rep Power: 17 |
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! |
|
June 13, 2008, 05:45 |
those are books, I think 7 of
|
#20 |
Super Moderator
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 29 |
those are books, I think 7 of them,
thick like @$"! and just full of tables. what liquid are you interested in? |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|