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

Fluid-Solid Domain

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 15, 2011, 13:12
Default Fluid-Solid Domain
  #1
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
Hi, I am currently using CFX to model the movement of a sand particle through a water channel.

I have 2 domains, a fluid domain for water, and a solid domain for a sand particle. Can I check how what setting can I use so that I can see the solid domain follow the flow of the fluid domain? So far, the only option I have found is the boundary detail under the Fluid Solid interface which allows me to change the Mesh Motion options.

Thanks in advance.
arien009 is offline   Reply With Quote

Old   October 16, 2011, 17:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Can you explain what you are trying to do? Most people model stuff like sand with a particle tracking model. So why are you using a solid domain? Are you trying to model the motion of the sand particle on the individual grain level?
ghorrocks is offline   Reply With Quote

Old   October 16, 2011, 17:35
Default Fluid-Solid Domain
  #3
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Can you explain what you are trying to do? Most people model stuff like sand with a particle tracking model. So why are you using a solid domain? Are you trying to model the motion of the sand particle on the individual grain level?
Yes, I am trying to model the sand particle at the grain level. I am now starting with just 1 grain to see the interaction, and will proceed on to more. What must I do to the settings such that the solid domain (sand particle) will move responding to the flow I have applied to the fluid domain (water)?

Thanks.
arien009 is offline   Reply With Quote

Old   October 16, 2011, 17:41
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Any of the rigid body approaches should make the sand grain move as fluid flows over it.

But before we go any further we will need to understand what you intend to get out of this work. Why are you interested in the flow over a single grain? What is wrong is existing drag models, packing factors and other particle models already present?
ghorrocks is offline   Reply With Quote

Old   October 16, 2011, 17:53
Default Fluid-Solid Domain
  #5
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
I am studying the behavior of a non-newtonian fluid in particlular the interactions of each individual particles subjected to a transient pressure loading and then the behavior after the pressure is relaxed. I need to measure the displacement of the particles when subjected to a pressure applied to the fluid body.

Thanks.
arien009 is offline   Reply With Quote

Old   October 16, 2011, 18:11
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I see. If you only have one particle and no collisions this can be done using immersed solid (although the immersed solid approach may have accuracy issues with non-newtonian flow, depending on exactly what sort of non-newtonian model you have). The other rigid body approaches with moving mesh are move accurate but harder to implement - and extremely hard to implement if you have multiple particles.

What type of non-newtonian fluid is it? Non-newtonian in shear, time or something else?
ghorrocks is offline   Reply With Quote

Old   October 16, 2011, 18:27
Default
  #7
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
It's Shear Thickening Fluid.

I have tried modeling the sand particle using 'Transient Structural' while the water using 'Fluid Flow (CFX)', similar to the oscillating Plate with 2-way FSI tutorial but I keep encountering the error below, which I think might be due to meshing?

Which method is recommended to handle my problem?
1. using purely CFX (my original question in this thread)
2. using the Transient Structural and Fluid Flow (CFX) method
3. any others?


+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| CFX encountered the error: Read. Fatal error occurred when reque- |
| sting Total Mesh Displacement for Interface. |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| cplg_SendCommand failed to send the command: ERROR -- CFX encount- |
| ered the error: Read. Fatal error occurred when requesting Total |
| Mesh Displacement for Interface. |
| |
| |
| |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine cplg_SendCommand |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+
End of solution stage.
+--------------------------------------------------------------------+
| The following transient and backup files written by the ANSYS CFX |
| solver have been saved in the directory C:/Documents and |
| Settings/wzhu/Local |
| Settings/Temp/161011_5020_Working/dp0/CFX/CFX/Work1/Fluid Flow |
| CFX_002: |
| |
| 0_CS.trn |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| ANSYS Solver terminated with return code 256 |
+--------------------------------------------------------------------+
arien009 is offline   Reply With Quote

Old   October 17, 2011, 06:47
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Looks like you are using a moving mesh approach. This is the most difficult approach to do so I would not use this unless you have good reason to do so.

Firstly, as this is a shear thickening fluid then it has no transient component (or does the non-newt fluid generate its own transient flows?). Then can you so a series of steady state runs at various relative flow rates and generate a drag versus slip velocity curve, then you can use a simple solver to integrate up the motion of the sand grain.

Secondly, if this approach is too simplistic for you then the easiest approach to model it directly is using immersed solids. As the flow is very low Re number this should work fine.

And finally, why are you modelling an individual grain of sand? Are you trying to develop a drag law for your fluid to apply in a lagrangian particle tracking model with lots of grains? Or something else? People do not usually care where a single grain of sand ends up
ghorrocks is offline   Reply With Quote

Old   October 19, 2011, 20:05
Default
  #9
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
Can I check whether should I use the Rigid Body Modeling to simulate my problem (see below)?

http://www.edr.no/blogg/ansys_blogge..._body_modeling

I am also wondering what is the size of the 'subdomain' I should choose to 'wrap around' the the rigid body. Any good rule of thumb?
arien009 is offline   Reply With Quote

Old   October 20, 2011, 06:28
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That tutorial only shows a few of the available methods. If you explain what you are doing more fully we might be able to help you choose the best method. Specifically:

Quote:
why are you modelling an individual grain of sand? Are you trying to develop a drag law for your fluid to apply in a lagrangian particle tracking model with lots of grains? Or something else? People do not usually care where a single grain of sand ends up
ghorrocks is offline   Reply With Quote

Old   October 20, 2011, 08:50
Default
  #11
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 104
Rep Power: 8
juliom is on a distinguished road
Send a message via Skype™ to juliom
I think you should think about using the multiphase model lagrange or discrte model.
I thin you just want to knoe how is the path of your sands particle, am I right?
juliom is offline   Reply With Quote

Old   October 20, 2011, 11:37
Default
  #12
New Member
 
Join Date: May 2011
Posts: 15
Rep Power: 6
arien009 is on a distinguished road
I need to model the position of each sand particle in the fluid (assume all the same size and shape) when subjected to an impact loading on the overall fluid domain. To see how they align and after that see how they realign after the impact loading is dispersed.
arien009 is offline   Reply With Quote

Old   October 20, 2011, 12:39
Default
  #13
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 104
Rep Power: 8
juliom is on a distinguished road
Send a message via Skype™ to juliom
So, I am almost sure you should use teh lagrange model (particle model), it is a kinf of multiphase model..
Your problem is a multiphase problem indeed.
juliom is offline   Reply With Quote

Old   October 20, 2011, 17:22
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,807
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you want to model grain packing then you will need to do a DEM model. CFX cannot do this itself, you will need to couple CFX to something like EDEM to do that.
ghorrocks 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
CFX domain comparison Kiat110616 CFX 4 April 3, 2011 22:43
Fluid - Solid Domain Interface Daniel CFX 6 February 15, 2009 19:09
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11
UDF Scalar Code: HT 1 Greg Perkins FLUENT 8 October 20, 2000 12:40


All times are GMT -4. The time now is 03:48.