|
[Sponsors] |
LTS based Lagrangian particle solver and test cases |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
June 19, 2012, 12:25 |
LTS based Lagrangian particle solver and test cases
|
#1 |
Member
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17 |
Dear FOAMers,
a Lagrangian particle solver for the simulation of evaporative cooling of flue gas in a quenching device is hereby provided to the community. The solver uses the Local Time Stepping (LTS) acceleration technique. Further more a series of test cases is provided along with a short instructions manual in PDF format. The focus of this publication lies on the comparison of the LTS approach with the PISO/PIMPLE based solution method. Solver, test cases and documentation can be found here: http://www.dhcae-tools.com/contributions.htm Feel free to use this thread for remarks, suggestions and questions. Martin Becker and Ulrich Heck |
|
August 1, 2012, 05:07 |
visualization of the Lagrangian particles
|
#2 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Hello Martin, hello Ullrich,
first of all thank you very much for sharing that solver. It seems to work very well. But is it possible to visualize the lagrangian particles in this solver? I did not get it working until now. Thanks in advance! Kind regards Christian |
|
August 1, 2012, 05:17 |
|
#3 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21 |
Hi Christian,
it is not really possible in the cases that we provided. The lagrangian particles evaporate completely within the particle transport iterations, so there is nothing left to be visualized. As we pointed out in the PDF document provided with the test cases and as you can see at these slides presented at the 7th OpenFOAM Workshop (http://www.openfoamworkshop.org/2012.../BeckerMartin/) it is necessary to append another simulation with another solver (for example reactingParcelFoam) to get the particles for visualization purposes. Martin |
|
August 1, 2012, 09:10 |
|
#4 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Hi Martin,
thank you very much for the information. Where should I start working on the solver that not all particles evaporate immediately? Kind regards, Christian |
|
August 3, 2012, 02:37 |
|
#5 |
Member
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17 |
Hi Christian,
there is no need to modify the solver. If you reduce the temperature of the hot gas in the test case, not all of particles should evaporate. Best regards Ulrich |
|
November 8, 2012, 02:11 |
injecting a liquid mixture
|
#6 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Hi,
its me again. Your solver works fine for injecting water. Now I would like to inject a liquid mixture of water and urea. Then the water should evaporate as first fraction from the droplets. Later the urea concentration in the droplets should increase and the evaporation of the second fraction urea should evaporate. I think therefore I have to switch the composition model from "singleMixtureFraction" to "singlePhaseMixture". The only problem is that "singlePhaseMixture" is not available in your solver. Can you please give me a hint, how I can make that composition model available and working in your solver? Thanks in advance! |
|
November 8, 2012, 07:53 |
|
#7 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21 |
Hi Christian,
you can use the "singlePhaseMixture" in the solver this way: In the dhcaeLTSThermoParcelSolver.C switch the cloud classes: Code:
//#include "basicReactingMultiphaseCloud.H" // <--- remove #include "basicReactingCloud.H" // <--- add Code:
//basicReactingMultiphaseCloud parcels // <--- remove basicReactingCloud parcels // <--- add Good luck Martin |
|
November 10, 2012, 09:17 |
|
#8 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Thank you Martin!
I can now use the singlePhaseMixture approach! But it is a pity that the two components of the mixture still do not evaporate one after each other. Both mixture components start evaporating to the same time. Although in real life the lower boiling component should evaporate first before the higher boiling component should evaporate. Do you know how the injected mixture can be really handled as a mixture consisting of two different liquids with differnet boiling points? Kind regards Christian |
|
November 12, 2012, 11:53 |
|
#9 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21 |
Hi Christian,
you can try to add a second cloud by doubling the cloud definition, the source terms etc in the solver sources. Then you can handle two different fluids with there individual Tvap and Tbp etc. Martin |
|
February 4, 2013, 14:38 |
|
#10 |
Senior Member
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16 |
Hi Martin,
by using two clouds I think I can dose two different fluids, but not a mixture of both. I am right? I have now a new idea. Therefore I need the chemical reactions. How can I reintroduce that feature into your solver? Thanks in advance. Kind regards Christian |
|
February 5, 2013, 08:49 |
|
#11 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21 |
Hi Christian,
you should compare the source code files of LTSReactingParcelFoam and dhcaeLTSThermoParcelSolver with each other line by line. For example in hsEqn.H the term "+ combustion->Sh()" must be added and so on. The make/options file must be adjusted, too. Martin |
|
February 24, 2015, 12:18 |
|
#12 |
New Member
Juan David Rodriguez P
Join Date: Jan 2015
Location: Milano
Posts: 20
Rep Power: 11 |
Hello Ullrich,
Perhaps I arrived here late, but could you please share again your solver? (The links in the DHCAE Tools page are dead) Thank you. |
|
February 26, 2015, 08:05 |
|
#13 | |
Senior Member
|
Quote:
you do not get the presentation http://www.openfoamworkshop.org/2012.../BeckerMartin/ but you will get the presentation http://sourceforge.net/projects/open...SlidesOFW7.pdf |
||
February 26, 2015, 12:15 |
|
#14 |
Member
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17 |
Dear Juan, dear Elvis
sorry for this. Now it should work again. Best regards Ulli P.S. : I had to update the link: The solver is now here http://www.dhcae-tools.com/Media.html Last edited by ulli; March 2, 2015 at 11:21. |
|
September 3, 2016, 05:43 |
adding rho file in 0 folder of reactingFoam
|
#15 |
New Member
sudhakar singh
Join Date: Jun 2016
Posts: 12
Rep Power: 10 |
hello friends,
I am new to OF, and i want to modify reactingFoam solver to give "rho" values also along with species, temp., pressure and U. how can it be done? can anybody help me. |
|
April 12, 2021, 09:10 |
Updating the dhcaeLTSThermoParcelSolver
|
#16 | |
Member
Sourav Mandal
Join Date: Jul 2019
Posts: 55
Rep Power: 7 |
Quote:
Thanks for sharing your work with the community and providing a excellent documentation (which is not always easy: to find for openFOAM modifications). I could download the source files and the documentation from the links you have mentioned in this thread. However, it was long back since you provided this solver for the community. In this 5 year, the openFOAM codes have changed a lot. The naming schemes especially, changed a lot (like turbulenceModels[/CODE] to momentumTransportModels). I started according to the section 2.1 of the documentation to compile the solver. I am not a C++ programmer at all, but trying to replace the old names with the new ones in the `Make/options` file of the dhcaeLTSThermoParcelSolver. I provide here, the modified `Make/options` file: Code:
EXE_INC = \ -I$(LIB_SRC)/finiteVolume/lnInclude \ -I$(LIB_SRC)/meshTools/lnInclude \ -I$(LIB_SRC)/MomentumTransportModels \ -I$(LIB_SRC)/MomentumTransportModels/compressible/turbulenceModel \ -I$(LIB_SRC)/MomentumTransportModels/compressible/RAS/RASModel \ -I$(LIB_SRC)/MomentumTransportModels/incompressible/lnInclude \ -I$(LIB_SRC)/MomentumTransportModels/compressible/RAS/lnInclude \ -I$(LIB_SRC)/MomentumTransportModels/compressible/RAS/derivedFvPatchFields/wallFunctions/mutWallFunctions \ -I$(LIB_SRC)/MomentumTransportModels/incompressible/RAS/derivedFvPatchFields/wallFunctions/nutWallFunctions \ -I$(LIB_SRC)/lagrangian/basic/lnInclude \ -I$(LIB_SRC)/lagrangian/intermediate/lnInclude \ -I$(LIB_SRC)/lagrangian/coalCombustion/lnInclude \ -I$(LIB_SRC)/lagrangian/distributionModels/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/thermophysicalProperties/liquidProperties/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/thermophysicalProperties/solidProperties/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/SLGThermo/lnInclude \ -I$(LIB_SRC)/thermophysicalModels/chemistryModel/lnInclude \ -I$(LIB_SRC)/ODE/lnInclude \ -I$(LIB_SRC)/regionModels/regionModel/lnInclude \ -I$(LIB_SRC)/regionModels/surfaceFilmModels/lnInclude \ -I$(LIB_SRC)/sampling/lnInclude \ -I$(LIB_SRC)/combustionModels/lnInclude \ -I$(FOAM_SOLVERS)/combustion/reactingFoam EXE_LIBS = \ -lfiniteVolume \ -lmeshTools \ -lcompressibleTurbulenceModel \ -lcompressibleRASModels \ -lcompressibleLESModels \ -llagrangian \ -llagrangianIntermediate \ -lspecie \ -lbasicThermophysicalModels \ -lliquidProperties \ -lliquidMixtureProperties \ -lsolidProperties \ -lsolidMixtureProperties \ -lthermophysicalFunctions \ -lreactionThermophysicalModels \ -lSLGThermo \ -lchemistryModel \ -lradiationModels \ -lODE \ -lregionModels \ -lsurfaceFilmModels \ -lsampling \ -lcombustionModels Code:
❯ wclean all && wmake -j16 PHP Code:
However, it feels that Martin you can update it to make it work much faster, since you are the original author. If you have some time to look into it, I shall be grateful |
||
April 12, 2021, 12:24 |
|
#17 |
Senior Member
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21 |
Dear Sourav,
you can use simpleReactingParcelFoam from OpenFOAM 8 out of the box to do steady state particle transport with evaporation. There is a tutorial provided within OpenFOAM 8, as well. Best regards Martin |
|
April 13, 2021, 08:06 |
|
#18 | |
Member
Sourav Mandal
Join Date: Jul 2019
Posts: 55
Rep Power: 7 |
Quote:
Last edited by sourav90; April 13, 2021 at 10:36. Reason: rectify link |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
dispersion model with lagragian particle tracking model for incompressible flows | eelcovv | OpenFOAM Running, Solving & CFD | 54 | April 10, 2018 09:36 |
OpenCL linear solver for OpenFoam 1.7 (alpha) will come out very soon | qinmaple | OpenFOAM Announcements from Other Sources | 4 | August 10, 2012 11:00 |
test cases | Maciej Matyka | Main CFD Forum | 3 | November 24, 2004 08:27 |
LES - standard test cases? | Mario | Main CFD Forum | 2 | October 14, 2004 02:48 |
compressible two phase flow in CFX4.4 | youngan | CFX | 0 | July 1, 2003 23:32 |