# Buoyant flow

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 11, 2010, 14:03 Buoyant flow #1 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 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?

 May 11, 2010, 17:20 #2 Senior Member   Join Date: Apr 2009 Posts: 531 Rep Power: 13 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)

 May 17, 2010, 13:11 #3 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 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

 May 17, 2010, 18:41 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 17, 2010, 20:46 #5 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 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.

 May 17, 2010, 22:28 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 If you don't want to suck or blow fluid then why not just use a wall?

 May 18, 2010, 10:15 #7 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 Because it is open to the atmosphere.

 May 18, 2010, 10:35 #8 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 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.

 May 18, 2010, 19:12 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 19, 2010, 13:14 #10 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 Do you mean free slip wall? And what about opening with prescribed velocity (at least for the horizontal boundary?

 May 19, 2010, 18:37 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 25, 2010, 15:46 #12 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 Sorry for the late response, but the link for the CFX-Pre figure is below: http://www.4shared.com/photo/mwkl0X1y/buoyant.html

 May 25, 2010, 19:08 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 26, 2010, 10:05 #14 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 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?

 May 26, 2010, 18:16 #15 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 27, 2010, 13:22 #16 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 Ok, but once I use a more adequate width, why do you recommend a periodic boundary conditions on the side walls?

 May 27, 2010, 19:02 #17 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 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.

 May 28, 2010, 09:37 #18 New Member   Bruno Join Date: Apr 2010 Posts: 16 Rep Power: 8 Ok. I'll try it out. Thanks!

 Tags buoyancy, buoyant flow

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Zhihua Xie CFX 0 September 3, 2007 09:49 ib FLUENT 1 March 26, 2007 13:11 stanley FLUENT 1 February 2, 2007 07:44 curious ... Main CFD Forum 23 July 21, 2006 07:40 Franck Main CFD Forum 3 September 4, 2003 05:57

All times are GMT -4. The time now is 21:41.

 Contact Us - CFD Online - Top