CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

issues with multiphaseEulerFoam solver for binary simulation in fluidized beds

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 15, 2023, 21:46
Unhappy issues with multiphaseEulerFoam solver for binary simulation in fluidized beds
  #1
New Member
 
Esmaeel
Join Date: Jul 2012
Location: Melbourne
Posts: 5
Rep Power: 13
Esmaeel is on a distinguished road
Hi everyone, I am trying to study the particle size effects for a binary mixture in a fluidized beds. So the system is particle-fluid but we have three phases: particle1,particle2, and air. The problem that I am facing with multiphaseEulerFoam solver is that the air volume fraction goes below 0.38 and it becomes as low as 0.24. So, each particle volume fraction are around 0.37 for same cells and that leads to the high volume fraction for particle phase. Here is the phaseProperties dictionary. Can anyone please help me understand what is wrong with my phaseProperties which results in high solid concentration? Thanks.



/*--------------------------------*- C++ -*----------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
FoamFile
{
format ascii;
class dictionary;
location "constant";
object phaseProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

type basicMultiphaseSystem;

phases ( particles particles2 air );

//referencePhase particles;

particles
{
type purePhaseModel;

diameterModel constant;
constantCoeffs
{
d 2e-4;
}

alphaMax 0.62;
residualAlpha 1e-6;
}


particles2
{
type purePhaseModel;

diameterModel constant;
constantCoeffs
{
d 2e-4;
}

alphaMax 0.62;
residualAlpha 1e-6;
}


air
{
type purePhaseModel;

diameterModel none;

residualAlpha 0.;
alphaMin 0.38;
}

blending
{
default
{
type continuous;
phase air;
}
}

surfaceTension
{}

interfaceCompression
{}

drag
{
particles_dispersedIn_air
{
type Ergun;
residualRe 1e-3;
}


particles2_dispersedIn_air
{
type Ergun;
residualRe 1e-3;
}

}

virtualMass
{}

heatTransfer
{
particles_dispersedIn_air
{
type RanzMarshall;
residualAlpha 1e-4;
}

particles2_dispersedIn_air
{
type RanzMarshall;
residualAlpha 1e-4;
}

}

phaseTransfer
{}

lift
{}

wallLubrication
{}

turbulentDispersion
{}

// ************************************************** *********************** //
Esmaeel is offline   Reply With Quote

Old   May 16, 2023, 02:20
Default
  #2
Member
 
Utkan Caliskan
Join Date: Aug 2014
Posts: 42
Rep Power: 11
dscian is on a distinguished road
kineticTheoryModel is important for particle dynamics in multiphaseEulerFoam so you need to check that. Furthermore, I don't think current solver can handle two different particle phases properly.
dscian is offline   Reply With Quote

Old   May 16, 2023, 02:38
Default
  #3
New Member
 
Esmaeel
Join Date: Jul 2012
Location: Melbourne
Posts: 5
Rep Power: 13
Esmaeel is on a distinguished road
Quote:
Originally Posted by dscian View Post
kineticTheoryModel is important for particle dynamics in multiphaseEulerFoam so you need to check that. Furthermore, I don't think current solver can handle two different particle phases properly.

Thanks for the reply. The current case is from fluidized bed tutorial and it uses RAS kinetickTheory. I am beginning to accept that two particle systems cannot be modeled with this solver but I might be wrong!
Esmaeel is offline   Reply With Quote

Old   June 5, 2023, 14:28
Default
  #4
Member
 
Mattia de\' Michieli Vitturi
Join Date: Mar 2009
Posts: 50
Rep Power: 17
demichie is on a distinguished road
Quote:
Originally Posted by Esmaeel View Post
Thanks for the reply. The current case is from fluidized bed tutorial and it uses RAS kinetickTheory. I am beginning to accept that two particle systems cannot be modeled with this solver but I might be wrong!
The kineticTheory implementation requires major changes to be able to model multiple solid dispersed phases. In the present state it should be used only with one solid phase.
demichie is offline   Reply With Quote

Old   June 7, 2023, 00:17
Default
  #5
New Member
 
Esmaeel
Join Date: Jul 2012
Location: Melbourne
Posts: 5
Rep Power: 13
Esmaeel is on a distinguished road
Quote:
Originally Posted by demichie View Post
The kineticTheory implementation requires major changes to be able to model multiple solid dispersed phases. In the present state it should be used only with one solid phase.
Thanks. I was wondering if other software like ANSYS-CFX or MFIX can do such modeling of multi-particle systems with euler-euler approach?
Esmaeel is offline   Reply With Quote

Old   June 7, 2023, 01:24
Default
  #6
Member
 
Mattia de\' Michieli Vitturi
Join Date: Mar 2009
Posts: 50
Rep Power: 17
demichie is on a distinguished road
Yes, they can both model multi-particle systems. If you want to do that with OpenFOAM, you have to modify the kinetic class in multiphaseEuler (the main change is the in the radial distribution functions), add a model for a multi-particle maximum packing, and add a solid-solid drag.
demichie is offline   Reply With Quote

Old   June 7, 2023, 01:41
Default
  #7
New Member
 
Esmaeel
Join Date: Jul 2012
Location: Melbourne
Posts: 5
Rep Power: 13
Esmaeel is on a distinguished road
Quote:
Originally Posted by demichie View Post
Yes, they can both model multi-particle systems. If you want to do that with OpenFOAM, you have to modify the kinetic class in multiphaseEuler (the main change is the in the radial distribution functions), add a model for a multi-particle maximum packing, and add a solid-solid drag.
I prefer to stick with OpenfFOAM. I would really appreciate if you could explain more on where/how the changes should be made? I have some experience with modifying solvers/libraries but this multiphaseEulerFoam is complicated/confusing!cheers
Esmaeel 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
Is pressure-based solver adequate for a transient simulation ? y__tb FLUENT 1 May 23, 2022 23:15
solver selection_dynamic mesh_leak simulation nikhil108 OpenFOAM Programming & Development 1 August 13, 2020 17:14
solver selection_dynamic mesh_leak simulation nikhil108 OpenFOAM Running, Solving & CFD 5 August 13, 2020 17:12
How can I use solution from one simulation as initial condition on a remote solver? Dano62 CFX 0 October 21, 2015 17:45
Working directory via command line Luiz CFX 4 March 6, 2011 20:02


All times are GMT -4. The time now is 14:33.