[ulli]

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

[Chrisi1984]

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

[MartinB]

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

[Chrisi1984]

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

[ulli]

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

[Chrisi1984]

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!

[MartinB]

Hi Christian,

you can use the "singlePhaseMixture" in the solver this way:

In the dhcaeLTSThermoParcelSolver.C switch the cloud classes:

//#include "basicReactingMultiphaseCloud.H"  // <--- remove
#include "basicReactingCloud.H"  // <--- add

And in createClouds.H change:

//basicReactingMultiphaseCloud parcels  // <--- remove
basicReactingCloud parcels  // <--- add

Now the solver uses the singlePhaseMixture model selected in the reactingCloud1Properties file.

Good luck

Martin

[Chrisi1984]

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

[MartinB]

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

[Chrisi1984]

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

[MartinB]

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

[JuanRodriguez]

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.

[elvis]

Originally Posted by JuanRodriguez

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.

I can confirm those links http://www.dhcae-tools.com/Contributions.html are not working

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

[ulli]

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

[Sud09463]

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.

[sourav90]

Originally Posted by ulli

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

Dear Martin & Ulrich,

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:

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

The compilation with this with OpenFOAM version 8 :

❯ wclean all && wmake -j16

yields the following:

PHP Code:

wclean all .
wclean .
Compiling enabled on 16 cores
Making dependency list for source file LTSThermoParcelFoam.C
could not open file hReactionThermo.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file turbulenceModel.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file RASModel.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file compressible/RAS/RASModel/RASModel.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file mutkWallFunction/mutkWallFunctionFvPatchScalarField.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file psiChemistryCombustionModel.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file DataEntry.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file basicSpecieMixture.H for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file thermophysicalProperties.H for source file LTSThermoParcelFoam.C due to No such file or directory
g++ -std=c++11 -m64 -Dlinux64 -DWM_ARCH_OPTION=64 -DWM_DP -DWM_LABEL_SIZE=32 -Wall -Wextra -Wold-style-cast -Wnon-virtual-dtor -Wno-unused-parameter -Wno-invalid-offsetof -Wno-attributes -O3  -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-8/src/finiteVolume/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/meshTools/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/compressible/turbulenceModel -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/compressible/RAS/RASModel -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/incompressible/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/compressible/RAS/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/compressible/RAS/derivedFvPatchFields/wallFunctions/mutWallFunctions -I/opt/OpenFOAM/OpenFOAM-8/src/MomentumTransportModels/incompressible/RAS/derivedFvPatchFields/wallFunctions/nutWallFunctions -I/opt/OpenFOAM/OpenFOAM-8/src/lagrangian/basic/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/lagrangian/intermediate/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/lagrangian/coalCombustion/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/lagrangian/distributionModels/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/specie/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/basic/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/thermophysicalProperties/liquidProperties/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/thermophysicalProperties/solidProperties/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/SLGThermo/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/thermophysicalModels/chemistryModel/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/ODE/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/regionModels/regionModel/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/regionModels/surfaceFilmModels/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/sampling/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/combustionModels/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/applications/solvers/combustion/reactingFoam -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-8/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-8/src/OSspecific/POSIX/lnInclude   -fPIC -c LTSThermoParcelFoam.C -o Make/linux64GccDPInt32Opt/LTSThermoParcelFoam.o
LTSThermoParcelFoam.C:73:10: fatal error: hReactionThermo.H: No such file or directory
   73 | #include "hReactionThermo.H"
      |          ^~~~~~~~~~~~~~~~~~~
compilation terminated.
make: *** [/opt/OpenFOAM/OpenFOAM-8/wmake/rules/General/transform:26: Make/linux64GccDPInt32Opt/LTSThermoParcelFoam.o] Error 1 


Can anyone please help me to make it work?

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

[MartinB]

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

[sourav90]

Originally Posted by MartinB

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

Thanks Martin , for your quick response! I'm trying simpleReactingParcelFoam, however it still needs cutting off much of the functionalities (top down approach), since I do not need evaporation, just passive particle flow. I posted a question here with the opposite approach (bottom up), since I already have a solved flow field and just need to check the particle position as steady state: Confusion: implementing non newtonian viscosity with particle tracking?, but with a non Newtonian model, which is probably not supported by solvers like particleFoam / icoUncoupledKinematicParticleFoam.