CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM News & Announcements > OpenFOAM Announcements from Other Sources

LTS based Lagrangian particle solver and test cases

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree9Likes
  • 3 Post By ulli
  • 1 Post By Chrisi1984
  • 2 Post By MartinB
  • 2 Post By ulli
  • 1 Post By MartinB

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 19, 2012, 12:25
Default LTS based Lagrangian particle solver and test cases
  #1
Member
 
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17
ulli is on a distinguished road
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
phsieh2005, kk2017 and sourav90 like this.
ulli is offline   Reply With Quote

Old   August 1, 2012, 05:07
Default visualization of the Lagrangian particles
  #2
Senior Member
 
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16
Chrisi1984 is on a distinguished road
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
Chrisi1984 is offline   Reply With Quote

Old   August 1, 2012, 05:17
Default
  #3
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21
MartinB will become famous soon enough
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
MartinB is offline   Reply With Quote

Old   August 1, 2012, 09:10
Default
  #4
Senior Member
 
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16
Chrisi1984 is on a distinguished road
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
Chrisi1984 is offline   Reply With Quote

Old   August 3, 2012, 02:37
Default
  #5
Member
 
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17
ulli is on a distinguished road
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
ulli is offline   Reply With Quote

Old   November 8, 2012, 02:11
Default injecting a liquid mixture
  #6
Senior Member
 
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16
Chrisi1984 is on a distinguished road
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!
sourav90 likes this.
Chrisi1984 is offline   Reply With Quote

Old   November 8, 2012, 07:53
Default
  #7
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21
MartinB will become famous soon enough
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
And in createClouds.H change:
Code:
//basicReactingMultiphaseCloud parcels  // <--- remove
basicReactingCloud parcels  // <--- add
Now the solver uses the singlePhaseMixture model selected in the reactingCloud1Properties file.

Good luck

Martin
granzer and sourav90 like this.
MartinB is offline   Reply With Quote

Old   November 10, 2012, 09:17
Default
  #8
Senior Member
 
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16
Chrisi1984 is on a distinguished road
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
Chrisi1984 is offline   Reply With Quote

Old   November 12, 2012, 11:53
Default
  #9
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21
MartinB will become famous soon enough
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
MartinB is offline   Reply With Quote

Old   February 4, 2013, 14:38
Default
  #10
Senior Member
 
Join Date: Jan 2010
Location: Stuttgart
Posts: 150
Rep Power: 16
Chrisi1984 is on a distinguished road
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
Chrisi1984 is offline   Reply With Quote

Old   February 5, 2013, 08:49
Default
  #11
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21
MartinB will become famous soon enough
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
MartinB is offline   Reply With Quote

Old   February 24, 2015, 12:18
Default
  #12
New Member
 
Juan David Rodriguez P
Join Date: Jan 2015
Location: Milano
Posts: 20
Rep Power: 11
JuanRodriguez is on a distinguished road
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.
JuanRodriguez is offline   Reply With Quote

Old   February 26, 2015, 08:05
Default
  #13
Senior Member
 
Elvis
Join Date: Mar 2009
Location: Sindelfingen, Germany
Posts: 620
Blog Entries: 6
Rep Power: 24
elvis will become famous soon enough
Quote:
Originally Posted by JuanRodriguez View Post
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
elvis is offline   Reply With Quote

Old   February 26, 2015, 12:15
Default
  #14
Member
 
Ulrich Heck
Join Date: Mar 2009
Location: Krefeld, Germany
Posts: 41
Rep Power: 17
ulli is on a distinguished road
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
elvis and wyldckat like this.

Last edited by ulli; March 2, 2015 at 11:21.
ulli is offline   Reply With Quote

Old   September 3, 2016, 05:43
Default adding rho file in 0 folder of reactingFoam
  #15
New Member
 
sudhakar singh
Join Date: Jun 2016
Posts: 12
Rep Power: 10
Sud09463 is on a distinguished road
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.
Sud09463 is offline   Reply With Quote

Old   April 12, 2021, 09:10
Default Updating the dhcaeLTSThermoParcelSolver
  #16
Member
 
Sourav Mandal
Join Date: Jul 2019
Posts: 55
Rep Power: 7
sourav90 is on a distinguished road
Quote:
Originally Posted by ulli View Post
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:

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
The compilation with this with OpenFOAM version 8 :
Code:
❯ 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
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file turbulenceModel
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file RASModel
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file compressible
/RAS/RASModel/RASModel.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file mutkWallFunction
/mutkWallFunctionFvPatchScalarField.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file psiChemistryCombustionModel
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file DataEntry
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file basicSpecieMixture
.for source file LTSThermoParcelFoam.C due to No such file or directory
could not open file thermophysicalProperties
.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.-o Make/linux64GccDPInt32Opt/LTSThermoParcelFoam.o
LTSThermoParcelFoam
.C:73:10fatal errorhReactionThermo.HNo such file or directory
   73 
#include "hReactionThermo.H"
      
|          ^~~~~~~~~~~~~~~~~~~
compilation terminated.
make: *** [/opt/OpenFOAM/OpenFOAM-8/wmake/rules/General/transform:26Make/linux64GccDPInt32Opt/LTSThermoParcelFoam.oError 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
sourav90 is offline   Reply With Quote

Old   April 12, 2021, 12:24
Default
  #17
Senior Member
 
Martin
Join Date: Oct 2009
Location: Aachen, Germany
Posts: 255
Rep Power: 21
MartinB will become famous soon enough
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 likes this.
MartinB is offline   Reply With Quote

Old   April 13, 2021, 08:06
Default
  #18
Member
 
Sourav Mandal
Join Date: Jul 2019
Posts: 55
Rep Power: 7
sourav90 is on a distinguished road
Quote:
Originally Posted by MartinB View Post
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.

Last edited by sourav90; April 13, 2021 at 10:36. Reason: rectify link
sourav90 is offline   Reply With Quote

Reply
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 21:54.