[mwaqas]

Hello everyone

I am also working with fluidizedBed/RAS (twoPhaseEuler) model. I am using 2.3.0. In my simulation I want to apply partially slip Johanson Jackson boundary condition. My theta.Particles and U.particles boundary conditions (in 0 folder) are as follows

for theeta
walls
{
type zeroGradient;
}

for U.particles
walls
{
type fixedValue;
value uniform (0 0 0);
}

does it mean no slip boundary condition ? If it is so, how can I define partially slip boundary condition. Also where to define "Specularity coefficient"

[RjwV]

Hello,

This is indeed no-slip what you have currently. If you want partial slip then you will either have to implement it yourself in v. 2.3.0 or you can download the development version 2.3.x from the repositories.

In 2.3.x Johnson and Jackson B.C. has been built in already (I am currently testing it).

You can use the following to set your Johnson and Jackson B.C. in U.particles:

wall
{
    type JohnsonJacksonParticleSlip;
    specularityCoefficient 0.50; // Or whatever value you want..
    value $internalField;
}

and in Theta.particles:

wall
{
    type JohnsonJacksonParticleTheta;
    specularityCoefficient 0.50; // Or whatever value you want..
    restitutionCoefficient 0.90;  // Or whatever value you want..
    value $internalField;
}

Hope this helps.

As a side-not: I have been playing around a bit with this B.C. and for now it seems the simulations are crashing. My alpha.particle seems to exceed the maximum packing value which causes my radial distribution function to go haywire. If you notice anything similar please let me/us know.

Kind regards,
Ramon

[mwaqas]

Hello Ramon

Thank you very much. Your comment is very useful. Within a couple of days I will update to V2.3.x, then I will apply partially slip boundary condition. After that I will update my simulation result here.

Regards
mwaqas

[mwaqas]

Hello Ramon

I have updated OpenFOAM-2.3.0 to OpenFOAM-2.3.x. In boundary field, I cant find JohansonJacksonParticalSlip boundary condition. Here is the path where I am looking for it.

home/waqas/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/fields/fvPatchFields/derived

Regards
mwaqas

[RjwV]

Mwaqas, I suggest you look in applications, solver, multiphase, twophaseeulerfoam. It should be there somewhere.

KR.
Ramon

[mwaqas]

Hello Ramon

Thank you for your quick response. I found the boundary condition .
Are you still facing problem of maximum packing limit or your case is working fine. I am running some cases, after completing simulation, I will post my result.

Regards
mwaqas