# OpenFoam Pressure Inlet Oulet

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

 June 16, 2015, 06:51 OpenFoam Pressure Inlet Oulet #1 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 3 Hi all, I'm new in CFD world; I have been working for three months with OpenFoam doing tutorials and some simple cases. Now I´m working in my first real case. I´m trying to simulate flow and temperatura in the interior of a wind turbine using buoyantSimpleFoam solver. The problem is that we have one outlet where we know the pressure but we don't know if the flow is going to enter or to go out. We have tried several BC but we don't find the correct one. There are some InletOutlet Bc where you have to specify the velocity in the case of the flow entering; and we don´t know this value. Anyone knows any solution or suggest to my problem? There are any BC where you shouldn´t specify the velocity value? Thank you so much

 June 17, 2015, 04:56 #2 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Delft, Netherlands Posts: 328 Rep Power: 12 Hi, It would probably be best ot use a combination of totalPressure for the pressure (equal to your environment pressure) and a pressureInletOutletVelocity boundary condition on the velocity. Regards, Tom

 June 17, 2015, 07:02 #3 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 3 Thanks Tom, pressureInletOutletVelocity is one of the BC that i have already tested, but I have used it with fixedFluxPressure for 0/p_rgh. The problem with pressureInletOutletVelocity is that you should specify the value for the velocity if the flow is entering: myPatch { type pressureInletOutletVelocity; phi phi; tangentialVelocity uniform (0 0 0); value uniform 0; } When i have used this BC with this values, the flow is not able to enter. I know that there are zones in my surface where the flow should enter and other zones where the flow should go out. Thanks

June 17, 2015, 08:04
#4
New Member

Al_th
Join Date: Apr 2015
Posts: 19
Rep Power: 3
Hi jlobera,

I am currently doing a simulation where I have an outlet that can let flow in or out.

If I remember correctly I am using the following BC at inlet and outlet (I specify fixed pressure at inlet/outlet)

Quote:
 Inlet { type pressureInletVelocity; value uniform (0 0 0); } Outlet { type pressureInletVelocity; value uniform (0 0 0); }
I do not have any problem so far and flow looks physically correct.

You could also look at the BC "pressureInletOutletVelocityFvPatchVectorField " :
https://github.com/OpenFOAM/OpenFOAM...hVectorField.H
Quote:
 Velocity inlet/outlet boundary condition patches for where the pressure is specified. zero-gradient is applied for outflow (as defined by the flux) and for inflow the velocity is obtained from the patch-face normal component of the internal-cell value.

 June 17, 2015, 08:12 #5 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Delft, Netherlands Posts: 328 Rep Power: 12 Hi jlobera, You do not have to specify the tangential velocity part and the "value" entry is just a placeholder for the first time-step. I agree with al_th, it should work. I do believe the fixedFluxPressure would mess things up since that one would need the flux over your patch, which you do not know. Regards, Tom

 June 17, 2015, 09:48 #6 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 3 Thank you so much tomf and al_th, You are right, the problem was the fixedFluxPressure BC. I have tried using inletOutlet BC for velocity and fixedValue for pressure and it works well. Can you explain me what's the difference between inletOutlet and pressureInletOutlet? And what is more correct to use in this case? Regards

 June 17, 2015, 09:55 #7 New Member   Al_th Join Date: Apr 2015 Posts: 19 Rep Power: 3 As far as I can tell with my (poor) understanding of Openfoam : - inletOutlet BC : You either have zero-gradient (when flow goes out) or a user specified velocity value (when flow goes in) - pressureInletOutlet BC : You either have zero-gradient (when flow goes out) or a value that depends on the user specified pressure If you want to set the pressure at the boundary, then using pressureInletOutlet can let you have a velocity vectorfield that is well defined according to the specified pressure. Edit : This link can maybe give you additional insight into the pressureInletOutlet BC : pressureInletOutletVelocity

 Tags air flow simulation, outlet bc, pressure bc, pressure boundary

 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 Tanjina FLUENT 0 November 3, 2013 12:34 joshi20h FLUENT 0 September 26, 2012 12:41 beastieboys6 FLUENT 3 April 10, 2012 22:46 Alina FLUENT 1 November 30, 2007 08:39 Antech Main CFD Forum 0 April 25, 2006 02:15

All times are GMT -4. The time now is 23:53.

 Contact Us - CFD Online - Top