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

ASM-bottom variation

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   December 19, 2011, 12:50
Default ASM-bottom variation
  #1
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Dear all,
I am modeling a density current composed of a mixture of water plus sediments using the algebraic slip model (ASM).
I would like to compute the bottom variation (due to the settling of the particles). Is there any way of doing this using ASM (or at least to infer this)?
Regards
antonio is offline   Reply With Quote

Old   December 19, 2011, 18:05
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Just for clarification - due you mean the ASM turbulence model or a particle slip model?
ghorrocks is offline   Reply With Quote

Old   December 19, 2011, 18:09
Default
  #3
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
I mean algebraic slip model.
antonio is offline   Reply With Quote

Old   December 19, 2011, 18:17
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
OK, thanks. What do you mean by the "bottom variation"? Are you trying to work out how the particle settle at the bottom of the thing?

What type of particles are they?
ghorrocks is offline   Reply With Quote

Old   December 19, 2011, 19:02
Default
  #5
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Please imagine a mixture of water and sediments (by definition the algebraic slip model uses spherical particles) entering in a smooth flume with "clean water". You will have a wave of sediments that will "travel" along the flume and some of these sediments will settle in the bottom. This rate of deposition will be different along the flume.My main purpose is to see how the bottom longitudinal configuration has changed along the flume from time t=0 (where the bottom was smooth) to a certain time (where some sediments have settled in the bottom).
antonio is offline   Reply With Quote

Old   December 19, 2011, 19:33
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX does not have good models for what you want to do.

If you consider the lagrangian particle approach - CFX can model particles falling out of the flow, but does not have deposition models or scouring models. So the particles will fall out of the flow and hit the bottom wall, but will disappear and not build up a bed.

If you consider the eularian approach (which appears to be what you are looking at) - you can use maximum packing fractions to build up something which looks like a "bed", but it does not have the proper physics of particle bedding and scouring so would not be very accurate in many applications.

I think Fluent has some recent stuff on this area in the V14 release. Also other codes such as Flow3D have some models here. But if you want to use CFX then I would consider linking it to a DEM code (eg EDEM) so the DEM code handles the bedding and scouring models and CFX does the fluid flow.
Flowdy likes this.
ghorrocks is offline   Reply With Quote

Old   December 19, 2011, 19:46
Default
  #7
Senior Member
 
Join Date: Jan 2010
Posts: 110
Rep Power: 7
antonio is on a distinguished road
Please can you explain in more detail what you mean by "you can use maximum packing fractions to build up something which looks like a "bed""?Are you saying to consider a certain upper limit of the sediments mass fraction in order to "predict" the "new" bed configuration?
antonio is offline   Reply With Quote

Old   December 19, 2011, 19:50
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It depends on what you are trying to do. If you only want to see where the particles drop out of the flow then do not worry about it and what you have described is fine. But if you want to form a bed or a bed which then can be scoured then it is more complex.

The issue is that there is no limit to the volume fraction of particles by default. The particles will keep building up assuming they take no space until the volume fraction reaches 1. But in reality there is a maximum packing fraction where all the particles are packed together, but the fluid exists in the gaps between the particles. This maximum packing fraction is a volume fraction less than 1.
ghorrocks is offline   Reply With Quote

Old   October 9, 2012, 08:34
Default
  #9
New Member
 
Jop Jansen
Join Date: Jan 2012
Location: Holland
Posts: 1
Rep Power: 0
jjansen is on a distinguished road
I am currently trying to tackle a similar problem using cfx 14.
I decided to try a mesh displacement method using ASM to simulate the settled sand as a bed. Simultaneously I remove the mass of the settled sand using a sink term in the bottom boundary. This seems to work for simple settling colum cases, however when I swith to a case with a "flow component" (for instance a bucket with inlet (0.1 volconc. particle mixture) and an outlet (stat.pr. boundary) the model crashes after a certain amount of time. Did anybody gain any more knowledge on this topic so far, with perhaps related tips and tricks?

Thanks in advance!
jjansen is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Variation of gravity with time Whyman OpenFOAM Programming & Development 36 March 30, 2015 13:35
Pressure variation in a heating channel gRomK13 Main CFD Forum 0 August 6, 2009 12:18
xy plot help -- large variation in results alemenchaca Main CFD Forum 0 May 17, 2009 13:45
Compiling OpenFOAM13 on AMD64 with OpenSUSE 101 silent_missile OpenFOAM Installation 5 August 10, 2007 07:31
DISH BOTTOM RUSHTON TURBINE Anne FLUENT 0 September 26, 2005 12:45


All times are GMT -4. The time now is 11:14.