|
Gas- Solid flow (absence of solid beside wall)
Hello everybody,
I am facing a problem in modeling a circulating fluidise bed riser. I am using an E-E model with a KTGF for the gas. The problem is everytime I model the flow, the results show a non-phisical absence or very low volume fraction "just" beside the wall for one or two cells beside the wall. other than that everything is ok. Does anyone have any idea why this is happening and how can I fix it. Your help will be highly appreciated and acknowledged in my thesis. Prior thanks for your assistance. |
It probably depends on the boundary conditions you are using. What kind of conditions did you specify? Could you provide some more information about the average particle concentration in your case and the gas mean velocity in the riser?
Best, A. |
Hello Alberto,
The inlet catalyst volume fraction is 11% with flux of 200kg/m2.S and the gas velocity is 2.5m/s. At the walls I am using No slip conditions for the gas and Johnson-JAckson condition for tha catalyst with specularity of 0.001 and restituition of 0.9. Your reply is really appreciated. |
Hi,
is there a specific reason why you are setting the specularity coefficient to 0.001? In Johnson and Jackson boundary conditions, a zero specularity coefficient corresponds to a perfectly specluar reflective condition (meaning the sign of the velocity component normal to the wall is changed), and your value is very close to that. In the literature on riser simulations, you will find that to obtain results comparable with the experiments, the specularity and restitution coefficient at the wall must be tweaked (I know it has no physical meaning, but that's due to the limitations in the kinetic theory closures used in two-fluid models), so that the proper slip velocity and granular temperature profiles are obtained. For example, typical values for the restitution coefficient are 0.9 (with a higher value for the particle-particle collisions, typically 0.95-0.98), and for the specularity coefficient you'll find something around 0.6. See for example the numerous papers of Prof. Gidaspow and his coworkers. This said, are you using any turbulence model? Is the case three-dimensional? And, are you trying to feed fluid and particles from the same inlet, at the bottom, or you're reproducing the real configuration of the system? Best, A. |
First thanks a lot for your concern Alberto,
Yeah, you are right about the sensitivity of the simulations to the restituition and specularity. But I tried to change the specularity to test its effect, but nothing obviuos happened. (Haven't reached 0.6, just tried 0.1) Yeah, I am using turbulence model (K-e) for the gas phase and dispersed solid phase. It's a 2d case. and yeah, I am trying to feed both the gas and the catalyst from the bottom together. But feeding the gas with a developed velocity profile and the solid with a flat velocity profile. Finally, what really worth to be mentioned, is that as soon as the catalyst enters the riser, the value of catalyst velocity just beside the wall quickly reaches zero and the catalyst shifts right away from the wall leading to strange catalyst vol. fraction radial profile (starts from appx. zero then increases then starts to decrease again as exepected). Thanks for your help and support, hoping that you will help me in kicking off my masters. Thanks again |
OK, I suspected it was a 2D case with a common inlet for both the phases, because I met a similar behaviour when I computed risers.
First of all, to obtain the proper segregation you have to specify quite a high value of the granular temperature (see for example J. De Wilde papers, where he clearly shows it). This might lead to unphysical results in the bottom zone of the risers and some numerical instability, so you need to find the right value for your case. Second, what you see (particle concentration higher a bit far from the wall) is not necessarily wrong. Check the granular temperature profiles at the same height, and you should notice that the temperature is higher at the wall and lower where you see the maximum concentration. This has a physical explanation: particles hit the wall, and are reflected, as a consequence the velocity variance is high, even though the mean flux accross the wall is zero due to the impermeability condition. A high velocity variance leads to a high granular temperature, and a lower particle concentration. One way to lower the temperature there is to increase the dissipation (lower rest. coeff.) or lower it elsewhere in the system (increase rest. coeff.). Btw, what is the value of the restitution coefficient for collisions between particles? Third, if you use the "per-phase" k-eps model, you might want to try the RNG model with differential equation for the viscosity in the low-Re zones.It will be a bit harder to converge, but in some cases it provides better results. I hope this helps :) Alberto |
Yeah this was really helpful, but as usual I still have some SHORT :D questions. 1- I tried to initialize the solution with a granular temperature of "10" but as the solution starts to converge it returns to its low values again all over the riser. 2- The analysis you mentioned is right theoretically, but do u think that this result is physically soundable. I haven't see in the literature any experiment that supports this absence of catalyst near the wall. 3- I am using 0.9 for wall restituition and 0.95 for particle-particle restitution. So to what extent do you suggest to lower the wall restituition. 4- You said that you met similar behaviuors before, so what was the solution you decided at the end. Have you just accepted the theoretical analysis (of granular temperature and so). or have u done any changes. Really I appreciate your efforts, you are of great support to me in my masters, I can say the best support. Thanks again and waiting for your preciuos replies. |
Quote:
Yes, that's normal. What has to be "high" is the granular temperature imposed at the boundary. The value of 10 seems pretty high to me, but something in the range 0.1 - 1 (m/s)^2 might work. Quote:
Of course this might not agree with experiments, and the reasons are different: first it might depend on the operating conditions, the nature of the particles and the effects you do not consider in the model (electrostatics for example), second during the experiments was the concentration measured exactly at the wall or at a small distance from it? Quote:
Quote:
This said, I find the approach not exactly scientific and physically sound, because you actually force the model to obtain what you want instead than putting the right physical parameters into it and see if it works. ;) It has also to be said that a major difference is played by the 2D geometry in my experience. A three dimensional simulation is a lot more expensive, but it usually provides better results. |
Alberto, I am speachless and don't know how to thank you for your preciuos replies.
- I am using a catalyst of particle size 100micro and density of 1990kg/m3. - Do you mean that I can impose granular temperature at boundary condition? can you tell me how I can do so in FLUENT. - May I ask what is your experience with CFD modeling of CFBs (Circulating Fluidised Beds). Do you have any experience in modeling a FF(Fast Fluidisation) regime in a dense flow. I am focusing on how to reach FF in dense risers and not a DSU (Desnse Suspension Upflow). Again and Again and Again, thanks a million for your help |
Hi,
yes, you can specify the granular temperature at the boundary conditions. For the inlet, it should be in the tab where you specify the boundary condition for the particle phase. Btw, you should use the partial differential equation for the granular temperature (set it in the phases dialog box), which I assume you are actually already using, considering you use Johnson and Jackson wall conditions. About my experience, I did my master degree and PhD on gas-particle flow CFD simulations. The test case I used for the densest case I considered was the riser of Knowlton (see for example Prof. Arastoopour work on it in his Fluor-Daniel lecture, but also the extensive work of the MFIX team ( www.mfix.org ) and Prof. Hjertager). Best, |
I couldn't find the granular temperature in the phases dialog box. Is granular conductivity the same as granular temperature :S.
When you simulated Knowlton case, what regime you got. Fast Fluidisation (falling catalyst near walls) or DSU (Dense Suspension Upflow). Have you ever met a case with upward moving solids at the walls or in all of them the solids were falling at the wall. |
Hi,
in FLUENT 6.3, you can set the granular temperature at the boundary condition in the boundary condition panel, selecting the corresnponding granular phase. In the phases panel, when you select a granular phase, and show its properties, you can decide if you want to use the algebraic model or the partial differential equation for the granular temperature. In Knowlton riser I had particle downfall at the walls (core-annular structure). I run a test-case where particles do not fall along the wall. You find an example of this in Tartan and Gidaspow paper about granular temperature measurements (if I remember right, it is published on AIChE Journal). Best, |
Hi Alberto,
Do you have some reference or work done where RNG k-epsilon gives better results? If you have them, can you give me? Thanks in advance! Quote:
|
| All times are GMT -4. The time now is 22:27. |