4 two-phase gas-solid circulating fluidized bed
 

Hi, everyone:

For a two-phase gas-solid circulating fluidized bed, the predicted solid axial velocity is about 50% of the experimental value(the latter: 10m/s). The modeling framwork is Eulerian-Eulerian approach.

To increase the simulated value, what should I do? I mean, what effect seems to have a great impact on the adjustment?

Could you give me some hints? Thanks in advance.

Re: 4 two-phase gas-solid circulating fluidized be
 

Could you be more specific about your case, i.e. particle size, drag law, solids stress (KT or viscosity input)?

Re: 4 two-phase gas-solid circulating fluidized be
 

Thanks,reza,

The more specific information is provided as follows:

- Particle size= 80E-6 m

- Drag_force_correlation: Gidaspow

- KTGF (partial equation for granular temperature)

Kivam

Re: 4 two-phase gas-solid circulating fluidized be
 

Kivam,

I believe drag is the main contributor but it normally goes the other way and result in higher solids velocity and lower solids volume fraction. Is this true in your case? Gidaspow' drag is OK for GS flows.

Reza

Re: 4 two-phase gas-solid circulating fluidized be
 

Hi,reza,

Actually, I simulated two literature cases and made the comparisons with the corresponding literature experimental data.

It was found from these comparisons simulation that, one case showed higher predicted solid velocity than the experimental one. The other case predicted on the contrary the lower axial solid velocity (this is the case I posted in this Forum). And I also tried different drag correlation available in Fluent software. However, the magnititude o the room for the adjustment is limited.

Therefore, I really want to know: What the main contributing factor is for adjusting the simulation parameter and then matching the experimental data...?

In fact, besides the drag force, I think there might be other important adjustable parameters like the restitution coefficients and specularity coefficient which could play significant role in gas-solid CFB system. However, I am nor sure how to manage those parameters for my purpose.

So, could any one give me some ideas? Thanks.

=== By the way, Reza, I am uncertain whether you are currently working in the field of CFD simulation of gas-solid CFB. If yes, I think we could contact further for debottling together some problems from CFB simulation by using Fluent. I also hope that anyone else who is interested in this topic can join us for intensify the focus on the key subject related to "Circulating Fluidized bed" & "FLUENT".

Re: 4 two-phase gas-solid circulating fluidized be
 

Yes, I agree that those parameters are important, but I think they are more effective in your radial profiles and not the average values. Although some works have shown that the spec. coeff. can effect the slip velocity in very dilute cases for small tubes. I have one more question for you: What kind of solids fraction were you expecting for each? In other words, was one case more dilute than the other, and if yes which is the one with lower than expected solids velocity? (OK two questions)

In reply to your last paragraph, I think by having this open discussion there is a good chance that other CFD experts join in.

Reza

Re: 4 gas-solid CFBs
 

I think that if we are getting the wrong viscosity values for the solids, the solids velocity and consequently the gas velocity would be wrong.

So these other parameters (e,phi,...) could be more important than you think.

Re: 4 gas-solid CFBs
 

In most cases, only the Gs (solid flux,kg/m2 s) and Ug (superficial gas velocity) are known. How to estimate the input paramters of 'solid fraction volume' is also very important for multiphase Eulerian model.

Unfortunately, the method for estimating this parameter is alwalys not mentioned in CFB-CFD simulation literature. According to my experience, I know that in some case the higher 'solid fraction volume' would lead to solid recirculation near the wall region; however, lower one will not.

But I don't know whether there is a unified method to define the inlet solid fraction,which makes 10 persons to get one unique value instead of 10 values. I am sure who has some ideas about this.

Re: 4 gas-solid CFBs
 

Maybe the effect of boundary condition could be avoided if it is defined away from the domain of interest.

Did you define a side entry or an annulus entry for the solids in your model right at the riser wall?

Re: 4 gas-solid CFBs
 

Hi,Bashu,

In my 2D axi-symmetry simulation, the gas-phase and solid phase are cofed through a single inlet (an INLET edge in Gambit). So, the input parameters for the inlet (VELOCITY-INLET) are: (1) the gas velocity(m/s); (2)the solid velocity; and (3) the inlet SOLID volume fraction.

Therefore, no side entry or annulus entry at the wall is involved in my case.

By the way, do you know how to calculate 'the inlet SOLID volume fraction'? How did you get this input paramater in your simulation?

Re: 4 gas-solid CFBs
 

If starting the BC at the acceleration zone, try 0.5 for solids fraction. In such a case it is probably better to sparate the gas and solids inlets.

If away from acceleration, slip ratio of about 1.2-1.5 for FCC.

I am not really fund of 2d-axi model since it won't let the solids to pass the axis in a transient mode.

Re: 4 gas-solid CFBs
 

Bashu,thanks,

I agree with you arguement: The axi-symmetry model may be problematic,prohibiting particles from crossing the central axial. Actually, a more detailed anaysis on this aspect can be found in a paper by Pain et al.(see sect3.1 of Pain et al.,International Journal of Multiphase Flow,2001,27:527).

Your suggestion for setting the soild fraction might be helpful. One question: Does the 0.5 value for solid fraction come from bubbling fluidized bed in downcomer? How about 0.4?

If choosing one INLET for both gas and solid phases, I think this value may be too big. Therefore, I agree with you that it is probably better to sparate the gas and solids inlets.

Now, my question is: If separating the solid stream with 0.5 for solid fraction, then how to determine the gas veloicty in this 'solid stream' (strictly speaking, a stream with gas+solid mixture,because of the 0.5 value)?

Best regards,

Gromeson

Re: 4 gas-solid CFBs
 

I hope this suggestions are useful:

I choose 0.5 because this way you are not shooting the catalyst into the system by having a non-real high velocity especially if it is a lift zone. I don't have any problem with 0.4 either.

If you have a separate solids inlet, by fixing the solids fraction you get your solids velcoity and a slip ratio 1 will give you gas velocity. Then you put the rest of your gas flow rate in your gas inlet. Although you may also get away with zero velocity for your gas in the solids inlet.

Now probably the best way is to define BC's as far away as you can afford to minimize its effect.

Do you have any suggestions for the wall BC's? What model do you use for solids viscosity?

Thanks

Re: 4 gas-solid CFBs
 

Hi, Bashu,

I understand the method you proposed for the estimation of the inlet solid fraction. For me, there are still two questions or uncertainties:

(1) the different value of inlet solid fraction will bring out different solid velocity, which will result in different solid MOMENTUM input. Therefore, the intial setting of this value as 0.4 and 0.02 will lead to 20 times of solid velocity. Therefore, higher solid-phase MOMENTUM input will be getten for the latter.

(2)Another problem: how to define the length of 'transition zone' or 'the BC far away' to eliminate the effect of the alternative boundary setting. Since the force is not equilibrated at any zone, the 'transition zone' will inevitably contribute to the adjsutment of gas/solid phase velocities(due to the slip effect). As to fully developed zone, this effect seems to be not so remarkable.

Therefore, this two things are still unclear to me. If you have further comment on this, please give your opinion.

Gromeson

(btw, I will give some comment on the wall BC's using another post for clarification purpose. sorry for this separation expression)

Re: 4 gas-solid CFBs
 

Bashu, (....cnted...)

As a response to the question concerning the wall BC's and the model for solids viscosity, the following comment is given:

In most simulations,the KTGF model is used for calculating the solid viscosity. The no slip consdition for the gas phae and partial slip (Johnson Jackson condition) for the particle phase.

However, high attention should be paid to the solid boundary condition due to its complexity. Actually, this BC condition involves three adjustable parameters (the solid-solid restitution coefficient,the solid-wall restitution coefficient, and the specularity coefficient).

According to my tests, I often found that there are some overshoots in velocity near the wall. So, the near wall treatment is also complicated in Fluent. The possible reasons might be related to:

(1) Grid meshing (Yplus control for the coarse grid and/or the fine grid) in the near-wall region. Especially the distance of the first grid close to the wall for the turbulence or even for the laminar viscous flow;

(2) Choice of grid discretization (first-order or second order);

(3) The proper choices of the combination of the above-mentioned three adjustable parameters.

So, to get a satifactory results, it seems that a large amount of tries should be done for the hydrodynamics of gas-riser when using Fluent software.

What is your testing experience? Could you make some comment on this.

Gromeson

Re: 4 gas-solid CFBs
 

I just started working on Flow analysis in a CFB riser. You guys seem to be far ahead in this research and was wondering if you could help me some. I'm currently having trouble loading the tutorial UDF for the Eulerian-granular-heat file. I need to change the directory to the working directory where the source file (.c) and data file are located on the Visual Studio 2005 Command Prompt. How can I create the path?

Re: 4 gas-solid CFBs
 

Yes the KINETIC ENERGY (rho*eps_s*vel^2) will be higher if one prescribes lower solids fraction for a given solids mass flow rate. That's the point. The results will not be the same with different BC's. For example see Chemical Engineering Education J. (vol. 32, n.2, spring 1998, CFD Case Studies in Fluid-Particle Flow, Jennifer L. Sinclair). The solids inlet velocity seems too high.

I guess by "FAR AWAY" I mean a location where the BC has less effect. For acceleration zone, one can bring the solids as a side entry not attached to the riser, but probably 3-4 diameter away and size the solids inlet to have a low velocity and a 0.4-0.5 solids fraction.

Re: 4 gas-solid CFBs
 

Unfortunately I am also testing the parameters to get some reasonable results.

I was using no slip for the walls, but it seems more people are suggesting JJ BC for the wall. I am not sure what kind of granular temperature and viscosity profiles should I expect though.

Re: 4 gas-solid CFBs
 

Bashu,

At least, from simulation viewpoit, NoSlip BC condition is relatively simper and reduces one adjsutable parameter (i.e. the parameter for solid-wall restitution coefficient).

For high velocity CFB, the interation between particle and wall seems to become more remarkable compared to other caes such as bubbling fluidized bed. Anyway, like you, I am not very sure whether the NoSlip is an adequate choice or not.

In the literature, there are some persons adopted this BC condition for CFB. However,as you mentioned, a lot of people prefer to using the JJ B.C., albeit it is of complex nature in model setting. The comercial software,Fluent, has recently been used in simulating CFB systems. But the succesful examples are few in the literature, and the simulation details were seldom reported. On the contrary, the simulation using in-house code simulations have been reported in the past 25 years.

Re: 4 gas-solid CFBs
 

Yes, the NO SLIP may have its advantages , but I am not sure if it does good when you are using a ktgf model where the viscosity in not an input to the model.

Just a note that even if you use a no-slip for velocity at the wall, when you have ktgf model you will still need the particle-wall restitution coeff. as input.

Re: 4 gas-solid CFBs
 

Hi, bashu,

Sorry, it is my mistake.

It should say that the adjustable parameter of 'specularity coefficient' can be avoided, instead of 'the particle-wall restitution coefficient'. The latter is still needed in No-Slip BC condition.

Re: 4 gas-solid CFBs
 

There is a paper published recently by NETL/Fluent people related to wall BC. Although the paper is focused on Simonin turbulent model, they show the effect of the BC on the profiles.

By using ktgf, it is believed that the gt values affect the density profile. It maybe the egg-chicken story though.

A good expertiment and a good mesh independent model could help in systematically identifying the three parameters (p-p and p-w restitution coefficients and specularity coefficient) needed to match the experimental values or at least figure out their effect on the maesurable variables like density, pressure and velocity.

Re: 4 gas-solid CFBs
 

Hi,Bashu,

I agree with you. For the grid geration,do you have any idea or principle on producing a mesh-independent model? I mean, from the viewpoint of the distribution of grid points, how to generally assign the non-uniform grids?

More specifically, taking 2-D CFB as example, I have the follwoing questions:

(1)Should the grids be uniformly-distributed along axial direction or non-uniformly-distributed specially at the inlet accerelation zone? Generally, how to treat this matter?

(2)In some literature, some people assigned the uniform grids to the radial direction. But I am uncertain how to balance the grid requirement in near wall zone (e.g in case of using turbulent model)? Do you think it is necessary to give more grid consideration over the near-wall zone? How about the grid consideration on the central zone?

Hope to get some general ideas as guidance. Thanks.

Re: 4 gas-solid CFBs
 

Before replying to your questions let me just remind you that a lot of research is going on in this area and all of what I mentioned should be just considered as one idea in million ideas. With that in mind, read on:

I think since in our multiphase models at least the TIME AVERAGE gradients are not very sharp near the wall (or almost anywhere in the domain) we may not need a lot of cells there.

If you have a turn or a change of flow direction (core and annulus interface, catalyst pick up from a downflow pipe) you need more mesh density.

But in the instantaneous world, we have all these boundaries (read gradients, clusters, bubbles, ...) moving. So what can we do to capture correctly these moving gradients?

I think the core-annulus interface is difficult to identify upfront so maybe for a very accurate answer you need to use the adapt mesh feature. Is it realistic for unsteady multiphase? I don't think so, since probably you end up with the whole domain refined.

I think you don't need a lot of mesh near the wall and so a unifrom radial mesh should be good and may be more mesh in the acceleration zone is not a bad idea.

I hope some other experts in this field jump into the discussion and let us know their idea.

Re: 4 gas-solid CFBs
 

I'm getting a Floating pointer error on my solid-gas riser model? Please what do you think i'm doing wrong?

Re: 4 gas-solid CFBs
 

Femi,

Can you provide more detail about your case?

Re: 4 gas-solid CFBs
 

I'm modelling 2DDP gas-solid flow in a riser section with dimensions 1.2m X 0.17m. I've created the mesh and trying to analyse in Fluent. particle density - 7800Kg/m3, gas density - 1.2Kg/m3, gas velocity - 1.0m/s

When iterating i get intermittent commands that, "solution is converged" but the iteration still keeps going on until it gets to the number of time steps that I set for it. How do I define the residence time so it will stop on convergence?

Also, at the end of iteration it gives me an Error: cx-dialog-done: wta[1](widget) Error Object: *the-non-printing-object*

Please what do these imply?

Re: 4 gas-solid CFBs
 

For a transient model, the solution needs to be converged at each time step and that's what you are seeing.

But the gas-solids flows normally do not reach a steady state and you should continue the simulation until you are in a quasi-steady state. Then you turn on the time-averaging feature of fluent and let the simulation run for some time. The time average results are what you are after.

I am not sure about the error you are getting.

Re: 4 gas-solid CFBs
 

Thanks alot.

How do I then make my simulation to stop on convergence?

Re: 4 gas-solid CFBs (also......)
 

Please also can you tell me how I can view the my data at different time sets?

For example, my volume fraction at 0.1sec, 0.5sec and 1sec?

Re: 4 gas-solid CFBs (also......)
 

You need to use "file, auto save" and save your data files at a certain interval. This way you can go back to different files and view the results at the desired times.

There is no convergence criteria for multiphase cases (especially dense cases) and you need to decide when to stop the model.

Re: 4 gas-solid CFBs (also......)
 

Thanks alot, you confirm things for me pretty well.

Okay I'm trying to evaluate how my solid holds up will change over time at different heights and with variations in the mesh and riser geometry (diameter).

How do I obtain numeric values for my X-Y plots and contours?

Can I use the K-epsilon (2eqns) or Renolds stress (5eqns) in my model and how does this affect it?

Re: 4 gas-solid CFBs
 

I want to create tables and graphs to analyse my data. Do you know if I can do that on the Eulerian because for some reason, I dont have the PDF table on Display. And if I was required to generate and read one how do I do that?