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

Buoyant flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 11, 2010, 14:03
Default Buoyant flow
  #1
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Hi,
anyone know the correct way to set up a buoyant flow simulation with static pressure boundary conditions? The problem is how to set the correct pressure profile along a boundary, since (if the fluid is compressible) it will depend on height and on fluid state equation.
In case of air ideal gas, I tried p(z)=k*(z-z_ref)+p0 (z is the coordinate parallel to the gravity vector) as the CFX manual recommends, but I was not able to figure out how to chose the constant k.
Any idea of whats happening?
brunorgs is offline   Reply With Quote

Old   May 11, 2010, 17:20
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 516
Rep Power: 12
stumpy is on a distinguished road
I have used the following in the past for compressible fluids:
Zref = 2 [m]
Tref = 300 [K]
Pref = 101325 [Pa]
mwair = 28.96 [kg kmol^-1]
Denref = Pref*mwair/(R*Tref)
Phydrostatic = Pref*exp(mwair*g*(Zref-z)/(R*Tref)) - Pref - Denref*g*(Zref-z)
stumpy is offline   Reply With Quote

Old   May 17, 2010, 13:11
Default
  #3
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Hi,
I just tested it, and it worked fine for the vertical boundaries. But I'd like to use an opening condition on the superior boundary as well (perpendicular to gravity), but the flow (over a flat plate) that should run paralel to x, "falls" from the top and then leaves the control volume by the lateral and frontal faces of it.
In this case, should I apply a velocity profile on the top boundary?

Thanks,
Bruno
brunorgs is offline   Reply With Quote

Old   May 17, 2010, 18:41
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
You cannot define both the pressure and velocity at a boundary. This is over-defining the boundary.

If the opening is perpendicular to gravity then it just has a constant pressure applied. No need for hydrostatic. Alternately if you know the velocity/flow rate then you can apply a velocity/flow rate boundary.
ghorrocks is offline   Reply With Quote

Old   May 17, 2010, 20:46
Default
  #5
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
I have one vertical and one horizontal opening boundaries (it is intentional, for testing). I appied the relation that the guy stumpy suggested on both boundaries. Of course in the horizontal, constant z boundary, it results in a constant pressure, so I could directly set a value for the pressure there, but the big question, I think, is what's the right pressure value, at the vertical boundary, that will keep the flow horizontal, instead of sucking the fluid out or blowing fluid in. That is why I'm wondering if it is better to set a velocity profile instead of a pressure profile.
brunorgs is offline   Reply With Quote

Old   May 17, 2010, 22:28
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you don't want to suck or blow fluid then why not just use a wall?
ghorrocks is offline   Reply With Quote

Old   May 18, 2010, 10:15
Default
  #7
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Because it is open to the atmosphere.
brunorgs is offline   Reply With Quote

Old   May 18, 2010, 10:35
Default
  #8
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
In short, I'm running a test simulation of flow over a flat plate. I'd like to set correctly a simulation using openings with static pressure condition on the left, right, top and forward boundaries (wall on the bottom and inlet with prescribed velocity on the backward boundary), and buoyant air ideal gas.
It must be buoyant because later I'll release heavy gas at some point in the domain.
brunorgs is offline   Reply With Quote

Old   May 18, 2010, 19:12
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I would still recommend you consider using walls on the sides, or making the inlet include the side walls. Pressure boundaries where the flow goes tangent to the boundary are always convergence nightmares.
ghorrocks is offline   Reply With Quote

Old   May 19, 2010, 13:14
Default
  #10
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Do you mean free slip wall? And what about opening with prescribed velocity (at least for the horizontal boundary?
brunorgs is offline   Reply With Quote

Old   May 19, 2010, 18:37
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Slip walls are better than no slip, but as long as the outer walls are far enough away it probably won't matter much.

Can you post an image of what you are trying to do? Otherwise I will be guessing.
ghorrocks is offline   Reply With Quote

Old   May 25, 2010, 15:46
Default
  #12
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Sorry for the late response, but the link for the CFX-Pre figure is below:
http://www.4shared.com/photo/mwkl0X1y/buoyant.html
brunorgs is offline   Reply With Quote

Old   May 25, 2010, 19:08
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Consider making the side walls periodic boundaries. Also be aware this simulation is almost certainly transient and 3D and if you want to model it correctly you will have to get adequate width to capture these features.
ghorrocks is offline   Reply With Quote

Old   May 26, 2010, 10:05
Default
  #14
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
For now I don't wanna capture the 3D effects of the flow, only to chose the most adequate boundary conditions. So, why should I use a periodic boundary condition in the side walls instead of, for example, outlet or opening conditions?
brunorgs is offline   Reply With Quote

Old   May 26, 2010, 18:16
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
But if the flow is 3D then there is no valid 2D model of it. You are over constraining the model into an incorrect solution.
ghorrocks is offline   Reply With Quote

Old   May 27, 2010, 13:22
Default
  #16
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Ok, but once I use a more adequate width, why do you recommend a periodic boundary conditions on the side walls?
brunorgs is offline   Reply With Quote

Old   May 27, 2010, 19:02
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,923
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Because a periodic side boundary is the least constraining. It is also very simple to do (no need to specify anything) and very numerically stable.
ghorrocks is offline   Reply With Quote

Old   May 28, 2010, 09:37
Default
  #18
New Member
 
Bruno
Join Date: Apr 2010
Posts: 16
Rep Power: 7
brunorgs is on a distinguished road
Ok. I'll try it out. Thanks!
brunorgs is offline   Reply With Quote

Reply

Tags
buoyancy, buoyant flow

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
Mass flow and U-Mom flow in CFX Zhihua Xie CFX 0 September 3, 2007 09:49
reversed flow at velocity inlet / mass flow inlet ib FLUENT 1 March 26, 2007 13:11
How to change from mass flow to volume flow rate stanley FLUENT 1 February 2, 2007 07:44
potential flow vs. Euler flow curious ... Main CFD Forum 23 July 21, 2006 07:40
Plug Flow Franck Main CFD Forum 3 September 4, 2003 05:57


All times are GMT -4. The time now is 18:07.