CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

DPM initial and boundary conditions

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 27, 2020, 04:36
Default DPM initial and boundary conditions
  #1
New Member
 
Sadjad
Join Date: Aug 2016
Posts: 4
Rep Power: 9
sajad2006 is on a distinguished road
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?
sajad2006 is offline   Reply With Quote

Old   February 27, 2020, 05:02
Default Dpm
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 35
vinerm will become famous soon enough
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 \rho g h
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   February 27, 2020, 05:34
Default
  #3
New Member
 
Sadjad
Join Date: Aug 2016
Posts: 4
Rep Power: 9
sajad2006 is on a distinguished road
Quote:
Originally Posted by vinerm View Post
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 \rho g h
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,
sajad2006 is offline   Reply With Quote

Old   February 27, 2020, 10:41
Default Pressure Profile
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 35
vinerm will become famous soon enough
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.
sajad2006 likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

Tags
buyoancy, discrete phase, dpm fluent, gravity flow, injection

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Suppress twoPhaseEulerFoam energy AlmostSurelyRob OpenFOAM Running, Solving & CFD 33 September 25, 2018 17:45
HeatSource BC to the whole region in chtMultiRegionHeater xsa OpenFOAM Running, Solving & CFD 3 November 7, 2016 05:07
simpleFoam error - "Floating point exception" mbcx4jc2 OpenFOAM Running, Solving & CFD 12 August 4, 2015 02:20
Micro Scale Pore, icoFoam gooya_kabir OpenFOAM Running, Solving & CFD 2 November 2, 2013 13:58
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00


All times are GMT -4. The time now is 18:45.