Fluidized bed modeling
I have been trying modeling a fluidized bed. Up to now I run into some problems. One of these is that the vertical tube gets an inflow at the top where an outflow is expected; because of the water that enters from the bottom through the bed. The BC at the top is set to outflow, but CFX puts a temporary wall at the top. The simulation stops with errors because of thermodynamic properties going out of range, like a steep pressure drop in the domain.
The fluidum is water and the solids are glass beads. the reactor is a 1mm wide and 1m long tube with a bed height of 0.1m. I created two domains, 0.1m in height for the initial bed with a maximum packing of 0.74 and a domain for the rest of the tube with only water in it. In both domains the same multiphase parameters are applied.
I use the eularian approach with the kinetic theory applied and drag correlations of Wen Yu. I set the buoyancy to an appropriate level in relation to the fluidum.
Inflow is set as a velocity
Outflow is set as static pressure 0 Pa
Wall is set to no-slip
Where the two domains meet, the BCs are set to opening at 0 Pa
- The velocities in the domain are set to 0
- The bottom domain, the bed, is packed with solids set to 0.74
- The top domain is set to 1.0 fluidum, so not solids initially
- The relative pressure is set at 0 Pa
My questions are:
- Is a domain packed with solids (Seen as a fluid by CFX because of the Eulerian approach) and a domain with just one phase above it a good approach? Or is there another way of setting an initial bed height?
- What could cause the unexpected inflow of fluidum and particles at the top of the tube? How can I prevent this from happening?
Thanks in advance for any help!
You should not need two domains for this. A single domain with properly described physics should be OK. You can define maximum packing factors for the model. The initial bed height is just set as an initial condition.
I think if you do this as a single domain your back flow problem will disappear.
Thank you for your response.
If I'm correct, I can best use an expression for the bed height?
I read some tutorials on CEL expressions, the best option is to use a step function. Is there a more detailed guide how to program these expressions as I have no experience with this?
I understand the concept of the step function:
step(f) with f<0 returns 0
step(f) with f=0 returns 0.5
step(f) with f>0 returns 1
But I don't know how to use it, any help is very much appreciated!
I also found this thread but it didn't add to my understanding of the programming part:
You could use the step function, or you could use a 1D interpolation function. Interpolation functions are a bit easier to understand.
Thanks! The interpolation function seems to be a good option :)
I have managed to include an expression for the bed height in a single domain. This is going well. So far so good.
But the inflow at the outlet still occurs, and the temporary wall at the outflow hasn't disappeared. There are a few things happening at the start of the simulation:
- The maximum packing is set to 0.74 and the bed has the same value. But when the simulation starts, the bed gets denser than the maximum packing allows it to be.
- This movement of the particles (I think) induces a flow of the fluid downwards approximately ten times the velocity of the inflow. I set the fluid to be incompressible, in short there is an inflow from the bottom; the particles and fluid are moving downwards towards the inflow.
What am I doing wrong? How do I prevent the fluid and the particles from initially flowing downward to being influenced by the inflow and eventually going up?
Please advice, it is appreciated a lot!
Clearly you have not implemented the packing factor correctly.
I have to agree, but I don't have a clue how to set the packing factor anywhere else then at the maximum packing factor option for particles. It is also stated in the help file that this maximum packing value can not be numerically guaranteed.
I found some info in the manuals and help files. I am using another solid pressure model then the kinetic theory. Hopefully this is the way to go...
I have no experience in fluidised bed simulations so cannot help you much - but I am pretty sure CFX support will have some example simulations to get you started.
My model seems to work, but it takes a while to calculate 1s in real time. For completeness I'll put some findings here for others struggling with an FB in CFX.
- In the modelling guide a lot best practice guidelines are given for two phase solid-liquid flows, but they are a bit scattered across the document.
- Use a transient simulation with adaptive time stepping, not a steady-state
- Use very small time steps, maximum order of magnitude of e-5
- Use a coarse grid to reduce computational time, or be so lucky to have a super computer ready. This is only for the lucky few...
- Use the kinetic theory, this is the main reason for the very small time step...
- Use an expression for setting an initial bed height. Do not use multiple domains for this, it is far to complicated and not necessary.
- Begin with First order Euler backward and low resolution turbulence. When you have a solution use those initial values for higher order calculations.
- Begin with an incompressible flow.
- Check, check and double check every setting as this is a very sensitive model...
|All times are GMT -4. The time now is 09:12.|