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

Solid phase average volume fraction

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 10, 2021, 11:12
Default Solid phase average volume fraction
  #1
New Member
 
AJ
Join Date: Feb 2020
Location: United Kingdom
Posts: 20
Rep Power: 4
ajjadhav is on a distinguished road
Dear all,
I am simulating solid-liquid flow using the Eulerian-Lagrangian approach in a closed baffled stirred vessel.
Liquid phase: water, 1150 kg/m3
Solid-phase: Glass bead, 1mm, 2485kg/m3, and volume fraction of 0.024.
I inject same number of Lagrangian particles as in an experiment around 870000, 90 % (798350 particles) of which are one way coupled and 10 % (88703 particles) of which fully coupled with continuous phase. I set the mass flow rate 1.154kg/sec (experimentally in kwon that this is my total solid in the system, I do not know whether I am doing right or not).
I use transient simulation and compare the velocity of liquid and solid phase with experimental data. I solid and liquid velocity are exactly matches with the experimental data.
I have to compare the solid volume fraction.
I have following queries:
1. While set up the model nowhere CFX ask me the solid volume fraction, whereas in fluent this option is available (in initialization), so my question is, did I set up CFX correctly?
2. When I see the particles track, I see particle averaged volume fraction. Why averaged volume fraction is greater than 1. How should I deal with this issue.
If you need more information, please let me know.
Please guide me.
Thank you in advance.
ajjadhav is offline   Reply With Quote

Old   August 10, 2021, 18:52
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,231
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I have no idea if your initial conditions are correct as I have no idea what your initial conditions are.

Volume fraction can be larger than 1 in Lagrangian simulations as there is no limit on the amount of particles which can be at a location. The particles are assumed to have zero size, so an infinite number of them can fit in a finite space. If you are getting large volume fractions like this you should consider whether the Lagrangian approach is appropriate. The Eularian particle models are more appropriate for large volume fractions as you can use models for maximum packing fractions and particle to particle collisions.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   August 10, 2021, 19:25
Default
  #3
New Member
 
AJ
Join Date: Feb 2020
Location: United Kingdom
Posts: 20
Rep Power: 4
ajjadhav is on a distinguished road
Hi Ghorrocks,
Thank you for your reply.
Since, i am using closed stirred vessel, there is no inlet and outlet, so there is no way to set the volume fraction at inlet.
I just set 1.54kg/s mass flow rate in injection region and around 880000 particles.
(In real experiment i use 1.54 kg of solid and remaining water to fill 288 mm tank so the solid is 5.2wt%, i have calculated number of particles in real experiment using size and density, they are around 880000.)
So I donít know this setting will represent the 0.024 volume fraction or 5.2wt%.
If we assume that the setting are correct, do you think 0.024 volume fraction is very high for Lagrangian simulation.
ajjadhav is offline   Reply With Quote

Old   August 10, 2021, 20:12
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,231
Rep Power: 135
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Yes, setting initial conditions for Lagrangian models can be a problem. What you have done is one way to do it, and probably the easiest way.

Is VF=0.024 too high for Lagrangian models? Read the CFX documentation on the available multiphase models to see the list of considerations. If I understand correctly 0.024 is the average VF, the local VF can be much higher than that. For instance at the bottom of the tank where the particles settle could have a very high VF. Whether this is a problem or not depends on what you are doing and whether you want to model the settling at the bottom of the tank accurately.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
lagrangian partices, multiphase flow, particles tracking, stirred vessel, volume fraction

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
how to set periodic boundary conditions Ganesh FLUENT 15 November 18, 2020 07:09
SU2-7.0.1 on ubuntu 18.04 hyunko SU2 Installation 7 March 16, 2020 05:37
Error - Solar absorber - Solar Thermal Radiation MichaelK CFX 12 September 1, 2016 06:15
[swak4Foam] mass conservation of solid phase violated when using groovyBC with twoPhaseEulerFoam xpqiu OpenFOAM Community Contributions 8 June 17, 2015 03:08
interDyMFoam - change in volume fraction gopala OpenFOAM Running, Solving & CFD 0 April 27, 2009 11:46


All times are GMT -4. The time now is 02:08.