Iam working in GAS/SOLID flow in fluidized bed, iam using kinetic theory of ganular flow,in this method we have to give two different restitution coefficients for particle-particle interactions,and particle -wall interactions.The software fluent is asking only for particle-particle interactions,then how can give to the software the resititution coefficient for particle-wall interactions.

IF i want to plot the time averaged flux or solid density at any point in the fluidized bed horizontally in the X-direction, how can we enable the software to give such a time averaged plot.

Hi Hariharnath, I will try to answer with my understanding and you are always welcome to debate on this.

Particle-Wall Restitution coefficient:

It is defined at the wall boundary conditions when solving solid phase granular temp. equation. If you are using PDE in Fluent6.2, open wall boundary condition panel where you find granular tab. When you open that granular tab, you will find a place to define this coefficient.

In the case when you solve only algebraic equation, you suply wall boundary conditions for gran. temp. and vel. through UDF.

Time averaged data: When solving unsteady flow, select the Data sampling tab on the iterate panel to get time averaging.

Hope this helps -US

thank you a lot, but iam having one doubt,iam selcting the option of DATA SAMPLING in the iteration panel,by selecting this option,iam getting mean avgerage values for voluem fraction and velocity, but what i need is to plot the CUSTOM FIELD FUNCTION of SOLID-DENSITY along the x -direction, the solid density should be time averaged at all the locations.

Is Solid-density you mean, (Particle_density)*(Solid_Fraction)? In this case, it should be simple. You know the Particle_density. You get time averaged solid_fraction. Based on these two, you should easily get time averaged solid-density through out the domain.

I work on Gas-solid circulating fluidized bed, and we use above definition for solid_density. Are you using something different than this?

Regards, -US

thanks alot, iam just now into this field. what you said abt solid density is absolutely correct, i will try in that manner. one more doubt is that in ur earlier message u said that you have to use PDE to get granular tab, but iam using the GT equation, what the solver is providing,then how can i switch over into 1)PDE OF GT 2)linear equation of GT

hello! i'm working on fluidized bed dryer,but first i want to simulate a fluidized bed. i have some problem in convergence.would you help me please? i want to give you my case file or step by step definition of problem in fluent and ask you what i must do? king regards

Do the following: Define --> Phase

Select Solid phase, and open its boundary condition panel.

It is the same panel where you set granular phase conditions, such as diameter, solid viscosity, conductivity, pressure etc.

Just below the tab where you select 'Granular', you will find PDE option. If you want to solve Full PDE equation for GT, select that option. Otherwise, leave that and it would solve just algebreic eqn for GT.

ps: PDE option for GT is available only in FLUENT 6.2. Earlier version solves algebreic eqn only neglective diffusive and convective term.

Regards -US

hi Masood, i want to know the exact problem ur facing.

The problem what ur facing regarding convergence, me too facing the same. by nature of the fluidized it seems that we will never get the convergence,as i was told by my professor, so what iam doing is iam simulating it for real fluidization time of 40sec.

hi us, we r using 6.1.2 version, so iam not getting the PDE, under granular option, so what can i do, here we r even having CFX 5.1 version, would this version of CFX supports this PDE option? thanknig you US HARI

You can implement PDE using UDF. But should be taking more time. However, in many cases, Algebreic eqn gives satisfactory results and you may not really need PDE. In this case, u should be implementing wall boundary conditions for Gran Temp and particle vel. using UDF.

I do not have any experience with CFX. I only know that CFX also provides kinetic theory use for granular particles. But don't really know about its modeling capabilities. Somebody told that implementation is the same in both CFX and FLUENT.

-US

Hello Hari,

A question. If you dont get convergence, how would it help simulating for 40s of real time?

-US

in my case what it is happening is that, i was asked by my PROF, to produce the result published in one paper, in that he gave all his results for some intermediate times in 40sec of real fluidization time, so i didnt concentrate more on convergence,

so what i have to do for convergence.

For which paper you are trying to reproduce the data?

To have good convergence is always important to make sure that the continuity is satisfied in the domain. For multiphase problems, to get good covergence is always be a problem but different things to be tried to get the best. What kind of convergence you do get? In terms of residue. Ofcourse, convergece should be judged based on other important solution parameters too.

In general, you can improve convergence, reducing mesh size or reducing time step size or both. Many other factors too.

By the way, if you get the comparable results then u shouldn't worry. Bcs that is the thing you require.

-US

the way u said is correct,in his paper he gave the boundary conditions too,and the results iam getting are comparable with his results, iam getting convergence in terms of residue, i kept the residual convergece limit to 10^(-6),so it didnt get converge, but if i reduce the convergence limit ,it gets converged.

hari and us! as i said before,i work on fluidized bed but i have convergency problem.residual for continuity dont become to 10-1.i use unsteady,eulerian,segragated,k-e turbulence with standard and per phase,solid vof=0.5,d(particle)=0.0003m,velocity inlet,pressure outlet,wall BC's.time step=0.0005s. geometry:a vertical cylinder,d=0.4m,H=2m. what should i do? regards

If you can afford, reduce the timestep size or mesh size or both. That should improve convergence.

Try using more conservative Under relaxation factor. In my case, reducing URF for momentum to 0.4 or 0.5 slightly improved convergence.

Try yr best to use hex or Quad mesh only.

Try solving laminar flow for both solids and gas. Start from there to introduce turbulence. That might help. Per phase turbulence model,with my experience, give trouble converging well. But should be best to use.(I model fast fluidization, not conventional fluidization, which is yr case)

Otherwise, for such kind of twophase flow, my experience so far is that it's difficult to converge.

Do you encounter 'reversed flow' warning at the pressure outlet?

Hope this helps. -US

Dear us! it is converged!i solved the problem with step by step solution!1st,steady state without vof of solid equation and turbulence,2nd,with vof of...and 3rd,unsteasy solution of that! but i had reverse flow error.what means that?is it a problem? regards

It's good. I thought u r using Eulerian model. But it's vof. I don't hv much of exp. with its num. behavior/stability. Good to share ur experience.

Ideally, there shouldn't be any reverseflow warning. It is not there when we define very accurate boundary conditions especially at outlet(with proper backflow values). Generally, it is difficult to know backflow values in my case. However, if yr results are ok , then u shouldn't worry.

-US

Hi US! my case is not vof!vof of solid means volume fraction of secandary phase(solid) in eulerian multiphase flow! it means i use eulerian model! regards

[Kanarya]

hi,

I am simulating on CFB reactors and using E-E model.I am using k-epsilon model and Enhenced Wall treatment in fluent14. yplus value is 3.
So, I can get convergence with Algebric Granular temperature but not with PDE one. I tried to give also inital values like 1e-10 as well but it doesnt work.
do you have any idea?

thanks in advance!