[sajad2006]

Hi,
I want to simulate the dispersion and mixing of discrete phase in a domain. The movement of the DP is due to buoyancy, I have activated the gravity. They enter the domain throught the surface at the bottom. The carrying fluid is in case (i) stationary, and in case (ii) moving.

First question is that: is it possible to have the DP with a defined volume ratio and size distribution distributed in all cells in domain? A homogenuos distribution as initial condition is wanted.

Second and more important question: How can I fix the boundary condition at the inlet? I have used injections (multiple ones to create the size distribution), giving the velocity as the theoretical rising Stock velocity. However the results do not make sense. The bubbles are seemed to move much faster into the domain than expected in case 1. For case 2, where the advection is also included, however the bubble movement and rise become very slow and restricted.


Any idea what I am doing wrong?

I prefer to have the inlet surface simply as a boundary conditions which introduces bubbles, and not 'injecting' them into the domain, and leave the movement to be determined by gravity only. Is there any way to do it?

[vinerm]

1. You can use volume or File injection to inject particles throughout the domain. Volume injection is available as a beta option and can only be used with Unsteady Tracking. File option can be used with any setup

2. Suspended particles cannot be simulated with steady-state DPM. The simulation has to be transient. Not just the DPM; well, DPM is always transient but for tracking the suspended particles, even the flow simulation has to be set to transient.

3. For bubbles or particles to rise, the important parameter is the pressure distribution in the fluid. If the pressure is uniform across the particle, in the vertical direction, there is no force on the particle except its weight and then it will not rise up. So, initialize the pressure as it should be in quiescent fluid, i.e., using

[sajad2006]

Originally Posted by vinerm

1. You can use volume or File injection to inject particles throughout the domain. Volume injection is available as a beta option and can only be used with Unsteady Tracking. File option can be used with any setup

2. Suspended particles cannot be simulated with steady-state DPM. The simulation has to be transient. Not just the DPM; well, DPM is always transient but for tracking the suspended particles, even the flow simulation has to be set to transient.

3. For bubbles or particles to rise, the important parameter is the pressure distribution in the fluid. If the pressure is uniform across the particle, in the vertical direction, there is no force on the particle except its weight and then it will not rise up. So, initialize the pressure as it should be in quiescent fluid, i.e., using

Thanks for your reply.
1. I will give it a try.
2. The system was indeed transient. yet The results did not make sense.
3. I will adjust and update.

Thanks,

[vinerm]

If you do not have anything coming from the bottom, set it as wall. The direction of the gravity should be correct, i.e., if it is supposed to be in negative z-direction, then it should be given as -9.81 along z. The reference location for the pressure in the operating conditions should be the highest point of the domain. The operating density must be set to the density of the lightest material. In case particles are lighter, density of particles should be given as operating density. To initialize, do a standard initialization with 0 values for every field. Define a CFF as 9.81*Density*(highest point coordinate - vertical coordinate). If z is vertical coordinate and highest point is 0.291 m, then equation would be 9.81*Density*(0.291 - z). Patch pressure in the domain with this CFF. Then run the simulation.