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

How to set phases with different velocity

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 2, 2012, 03:42
Default How to set phases with different velocity
  #1
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
Hello I am want to implement stratified two-phase flow by CFX. The phases are (Oil and Water) the oil flowing at the lower part of the pipe and water at the upper part. The two phases flows at different superficial velocities I need to ask how I can set the velocity of each phase in this case in CFX-Pre?
In Bump tutorial I saw they set only one velocity for both phases? Furthermore reference to my case which it better the segregated solved or the coupled solver?

Thanks a lot
Kbaker
kbaker is offline   Reply With Quote

Old   May 2, 2012, 13:01
Default
  #2
Senior Member
 
Julio Mendez
Join Date: Apr 2009
Location: Greensboro, U.S.A
Posts: 108
Rep Power: 8
juliom is on a distinguished road
Send a message via Skype™ to juliom
Dear colleague,
You do this, jsut defining to phases, and using the Euler-Euler model, specifically particle model.
At the inlet you define each velocity..
Good luck!
juliom is offline   Reply With Quote

Old   May 2, 2012, 16:11
Default
  #3
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
Hi thanks for the answer. Is Euler-Euler model is same as homogeneous model with free surface model available in Multiphase menu? How can I select particle model I think it not appropriate to my case cause I have continuous fluids (not have particles anymore within the domain of solution)?
kbaker is offline   Reply With Quote

Old   May 2, 2012, 18:09
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot see the phase velocities in the bump tutorial as it is a homongenous model - both phases share a single velocity field and this is appropriate for free surface models where you have one phase or the other and they do not mix. If you run an inhomogenous model then velocities will be available for both phases.
ghorrocks is offline   Reply With Quote

Old   May 3, 2012, 06:44
Default
  #5
Senior Member
 
Join Date: Jan 2011
Posts: 178
Rep Power: 6
mariam.sara is on a distinguished road
?????????????????????
mariam.sara is offline   Reply With Quote

Old   May 3, 2012, 06:52
Default
  #6
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
Thanks ghorrocks for the reply. In my case the phases not mixed (I have stratified flow case) and there is a clear interface between them. If I use in-homogeneous model I think CFX will force the phases to be mixed and I not want this occurs? I want the phases flows within the pipe with different velocities separately? so is the in-homogeneous model ensure this thing?
kbaker is offline   Reply With Quote

Old   May 3, 2012, 07:22
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Looks like I have confused mariam. At least I have achieved something today

If the phases never mix then use the homogenous model. You only use inhomogenous when interphase slip happens. In your case you define a boundary with the velocity defined by its position, but still using the homogenous model.
ghorrocks is offline   Reply With Quote

Old   May 3, 2012, 09:04
Default
  #8
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
may you clear to me pls how I can apply what mentioned in your phrase (you define a boundary with the velocity defined by its position) in CFX-Pre?
kbaker is offline   Reply With Quote

Old   May 3, 2012, 09:08
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If the surface is at z=0, then for z<0 you define velocity=0 [m/s], and where z>0 you define velocity=1[m/s].
ghorrocks is offline   Reply With Quote

Old   May 3, 2012, 12:08
Default
  #10
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
You mean I need write CEL expression at inlet for the velocity? if it a CEL expression may you write it for the same conditions you mentioned me above in your example with surface at z=0 ?
kbaker is offline   Reply With Quote

Old   May 3, 2012, 17:23
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Yes, a CEL expression. Have a look inthe documentation and tutorials on CEL, it is quite a simple language.
ghorrocks is offline   Reply With Quote

Old   May 4, 2012, 03:17
Default
  #12
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
Well in Bump tutorial at inlet boundary they set the turbulent length scale as UpH is this the value for the height above the interface or the full channel height?
Another thing in Bump tutorial too at outlet boundary they define static pressure as equation represented by DownPres ? should I set the same relation to my case? As I know from the tutorial guide this relation depends on the expected height of free surface at outlet in my simulation the height of the free surface unknown at outlet (at inlet it known and I tried CEL expression for it) and I want it computed from the downstream flow reference to the boundary at inlet?
kbaker is offline   Reply With Quote

Old   May 4, 2012, 06:36
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You should choose your boundary conditions to match what you are modelling.

Also boundaries which only see a single phase are much simpler. If you can make use of this it will be simpler.
ghorrocks is offline   Reply With Quote

Old   May 4, 2012, 06:56
Default
  #14
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
1) You not answer my question about UpH at inlet boundary in Bump tutorial is it represent the height above the interface (air level above the interface)?

2) Another thing what you advice me to use at the outlet boundary? pressure outlet or opening boundary?
kbaker is offline   Reply With Quote

Old   May 4, 2012, 08:23
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I have not looked at thtat tutorial in detail for a while. But if you understand the tutorial you will be able to work it out. So you better look at it a bit closer.

Use an outlet when you do not expect back flow as it is a more numerically stable boundary. Use openings when back flow is possible, but be aware that it will be less numerically stable. If you are putting a boundary near a separation it is probably better the move the boundary down stream to avoid it.
ghorrocks is offline   Reply With Quote

Old   May 4, 2012, 14:27
Default
  #16
Senior Member
 
kbaker's Avatar
 
Khalid Baker
Join Date: Mar 2009
Location: IRAQ
Posts: 118
Rep Power: 8
kbaker is on a distinguished road
Thanks a lot ghorrocks for the valuable information. I have some doubts hope you explain it for me:
1) Reference to my case which it is better to use the segregated solver or coupled solver?
2) When I select homogeneous model>free surface model>standard should I select interface compression level or leave it clear? If yes how many interface level should I select?

Thanks
kbaker
kbaker is offline   Reply With Quote

Old   May 5, 2012, 07:25
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,945
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
1. Depends which side of bed you got out of this morning. They both have sterngths and weaknesses and I don't have time to describe them all.
2) The default settings are usually good. But if you have some time I recommend trying all the options and seeing what ones work well for your simulation.
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
why shroud velocity can't be set myleader CFX 6 October 18, 2011 04:12
can i set the velocity and pressure at the inlet at the same time by UDF minyang.cau FLUENT 0 July 14, 2009 23:14
How to set up the velocity in the let boudary changing with time. flying OpenFOAM Running, Solving & CFD 7 June 5, 2009 09:26
udf inlet velocity is not set correctly, why ? GaoGe FLUENT 0 June 17, 2008 08:33
How to set transient ang velocity? edi ghirardi FLUENT 0 April 12, 2005 09:34


All times are GMT -4. The time now is 09:34.