# Pressure outlet BC help!

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

 November 13, 2012, 10:46 Pressure outlet BC help! #1 Member   Join Date: Jun 2011 Posts: 48 Rep Power: 6 Hey everyone, I posted this earlier on the main forum and no one helped, so I'll try here: I'm trying to run a fairly simple CFD simulation of a box thing in a very basic "windtunnel". My windtunnel is really just a big rectangular domain. Simulation in FLUENT 14.0, mesh made in ANSA 13.2.3. Mesh appears to be great. Skewness all below 0.9 in both solids and shells, no intersections, no negative volume. Made prisms layers for B.L. growth on windtunnel walls, floor, and ceiling, as well as necessary areas of my test object. Hexa-interior mesh. I ran a realizable k-epsilon model (Inlet velocity of 70 m/s is a Re=7x10^6). My boundary conditions were simple: velocity inlet for the inlet of the windtunnel, pressure outlet for the outlet of the tunnel, and walls everywhere else (ceiling/floor/sides/object). Converged (residuals 10-4 or so) just fine in 2000 iterations. Y+ values look fine (between 30 and 250 or so), as do velocity/pressure contours. So we're happy! In real life however, the windtunnel facility is actually an open tunnel, so I changed the sides, and ceiling of the tunnel to pressure outlet conditions to try and simulate the open tunnel scenario. I left the floor as a wall. It stopped working. While most of the residuals look ok, continuity hovered around the 10^-2 or greater area. The velocity contours are clearly wrong. Velocity accelerates out of the back of the domain in the 300 m/s range (remember velocity inlet is 70 m/s), as well as accelerating out of the top, and sides of the domain. So then I tried to keep the top as a wall and only change the sides to pressure outlets, to see what would happen. The velocity contours showing the plane that cuts the top and bottom of the domain still look okay, but on the plane that cuts the sides of the domain looks pretty off. I guess I don't fully understand the pressure outlet BC. Should I be using something else? like a farfield condition or something? Anyone else had this kind of problem before? or should I just leave the top, and sides of the domain as walls and give up on trying to do an "open tunnel" scenario? I'd a appreciate any advice!! I'll also say that for my pressure outlet conditions I have the Gauge pressure as 0 (since in the operating conditions I have the operating pressure as 101325). Doesn't matter anyway cause I tried it with both 0 and 101325. I'm specifying the turbulence parameters using intensity and visocity ratio (.1% and 5 respectively) and the backflow direction specification method as normal to boundary. I'm not using the radial equilibrium pressure distribution, average pressure specification, or targe mass flow rate. In the text output during the solution process, it is currently sensing reversed flow on the sides of the domain when they're turned to outlets...I'm not sure why. It's such a simple problem, I hope someone has some advice! Thanks!

 November 13, 2012, 11:21 #2 Senior Member     Philipp Join Date: Jun 2011 Location: Germany Posts: 1,097 Rep Power: 16 Hi, Pressure outlet means that you set a boundary condition for a fixed pressure at that domain. I am not sure if that's really what you want... If you set a pressure outlet BC at top / sides and outlet this is no tunnel anymore, it's more like a street!? 1) What means "open tunnel"? Can you post pics? 2) Can you post pics of your solution? 3) If you use incompressible flow (I guess you do), changing the absolute pressure does not change anything at all. In incompressible Navier-Stokes equations there is just one place where the pressure appears (gradient of p). That's why the pressure is floating. 4) "reversed flow" is just a warning, no need to worry. Normally, people define a pressure outlet in a way that the flow leaves the volume. Fluent expects that this is allways the case and gives these warnings if flow enters the domain at a pressure outlet. Just to tell people "Hey, there might be a problem here".

 November 13, 2012, 11:54 #3 Member   Join Date: Jun 2011 Posts: 48 Rep Power: 6 Hey, I really appreciate the post! I actually cannot most pics because of confidenciality issues within my company (automotive industry). BUT what I meant by "open" tunnel is that the actual wind tunnel facility is just a contractor, floor, and diffuser (very common in the automotive industry). There are no side walls or ceiling (which sounds weird...no this not and outdoor tunnel) but they are so far away in an enormous room that they're negligible considering the size of my domain. And you're right! this is like a street! So I'm guessing I'm just modeling this wrong and I ought to just keep the sides and top as walls to model more of a, I'll use the term, "closed" test section?

November 13, 2012, 19:38
#4
Senior Member

Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 141
Rep Power: 4
Quote:
 Originally Posted by eishinsnsayshin Hey, I really appreciate the post! I actually cannot most pics because of confidenciality issues within my company (automotive industry). BUT what I meant by "open" tunnel is that the actual wind tunnel facility is just a contractor, floor, and diffuser (very common in the automotive industry). There are no side walls or ceiling (which sounds weird...no this not and outdoor tunnel) but they are so far away in an enormous room that they're negligible considering the size of my domain. And you're right! this is like a street! So I'm guessing I'm just modeling this wrong and I ought to just keep the sides and top as walls to model more of a, I'll use the term, "closed" test section?
From your descriptions it sounds like we are working on similar flow domains. I selected a free-shear wall at the sides and the top surfaces and this provided good agreement with the velocity profiles from a benchmark study.

In Fluent you can set the pressure outlet at the end with 0 relative pressure to the 'reference' pressure which is your domain at 1 atm for example. I have encountered similar 'reverse flow' warnings but that is simply because the application expects the boundary to behave as an outlet and any recirculation or backwash will trigger this warning.

The only time I ever actually worried about this was when the continuity equation residuals were simply diverging to values in the order of 10^3 or 10^4 and clearly my setup was invalid. This gave me maximal eddy viscosity ratio warnings and I think the backflow was so strong that the entire flow in the domain was in the opposite direction to my inlet haha.

The only setting I am unsure about is the Backflow direction specification method which allows the 'normal to boundary setting'. Is it good or recommended for this to be turned on or off when attempting to capture flow recirculation?

Just my 2 cents based on limited knowledge and experience.
__________________
--
Mechanical Engineering
Sydney, Australia

 November 14, 2012, 15:05 #5 Member   Join Date: Jun 2011 Posts: 48 Rep Power: 6 Thanks for the reply!! I'll give that B.C. a shot. As for the Backflow Method, I have always left the Backflow direction specification method to Normal to Boundary for my pressure outlets. I guess I've never had a reason to change it. I don't know any more about it besides that when backflow occurs, the direction of the flow will be normal to the boundary and the total pressure used will be the Gauge Pressure you set (zero). I dont think there's a way to turn it off...you just have to pick a method in FLUENT.

 November 16, 2012, 11:03 #6 Member   Join Date: Jun 2011 Posts: 48 Rep Power: 6 Related to this, would it be OK to use a symmetry condition for the sides and top of the domain? This would just force all normal components of the flow variables to zero which wouldn't hurt anything since I'm not doing a thermal model right? And the flow is leaving the domain anyway. I tried it and the results look okay....

 November 16, 2012, 20:04 #7 New Member   Join Date: Oct 2012 Posts: 27 Rep Power: 4 I was solving a similar model and used symmetry BC! i would suggest you to do the same. Pressure outlet is being interpreted from FLUENT as a real oytelt of you flow (backflow phenomena could also appear). Symmetry is a good choise for open space because you do not have the no slip condition(walls).

 December 4, 2012, 00:36 #8 Senior Member     Ovi Join Date: Oct 2012 Location: Sydney, Australia Posts: 141 Rep Power: 4 That sounds like a good idea but, I also was thinking about the main differences between the zero-shear walls and the symmetry boundary condition and this raised a few questions. Based on my understanding, the symmetry condition will set the normal gradients to zero and provide no additional resistance to flow in the parallel direction (zero-shear). This is also true for the zero-shear wall boundaries however they are likely to block the flow in the wall-normal direction. Hence, it seems that the symmetry condition would be much more suitable near regions which contain recirculation and separated flows. I think it would also be valid to use a zero-shear wall however, it should be sufficient far away from the flow features to minimise any influence on them. Please discuss whether this idea is valid. __________________ -- Mechanical Engineering Sydney, Australia

 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 joshi20h FLUENT 0 September 26, 2012 12:41 kino Main CFD Forum 5 April 13, 2011 11:03 CoG STAR-CCM+ 4 June 9, 2010 21:47 Dave FLUENT 1 August 12, 2004 17:39 DS & HB Main CFD Forum 0 January 8, 2000 16:00

All times are GMT -4. The time now is 02:50.