# OpenFoam Pressure Inlet Oulet

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

 June 16, 2015, 07:51 OpenFoam Pressure Inlet Oulet #1 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 10 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, 05:56 #2 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 624 Rep Power: 31 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 amuzeshi, spalartallmaras and Juan Daniel like this.

 June 17, 2015, 08:02 #3 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 10 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, 09:04
#4
New Member

Al_th
Join Date: Apr 2015
Posts: 19
Rep Power: 10
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, 09:12 #5 Senior Member   Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 624 Rep Power: 31 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 EFC likes this.

 June 17, 2015, 10:48 #6 New Member   Jorge Lobera Join Date: Jun 2015 Posts: 6 Rep Power: 10 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, 10:55 #7 New Member   Al_th Join Date: Apr 2015 Posts: 19 Rep Power: 10 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 : http://www.cfd-online.com/Forums/ope...tvelocity.html kaifu, Turin Turambar, calf.Z and 2 others like this.

 March 10, 2019, 05:16 #8 Senior Member   Jianrui Zeng Join Date: May 2018 Location: China Posts: 157 Rep Power: 7 I am now using these boundary conditions for velocity/pressure: velocity: inlet: fixedValue outlet: pressureInletOutletVelocity pressurep_rgh) inlet: fixedFluxPressure outlet: fixedValue Should this setting be suitable？I am now using buoyantSimpleFoam. Should we combine totalPressure and pressureInletOutletVelocity? Thank you.

 March 20, 2019, 11:25 #9 Senior Member   Lukas Fischer Join Date: May 2018 Location: Germany, Munich Posts: 117 Rep Power: 7 I think that you can combine totalPressure for p and pressureInletOutletVelocity for U at the outlet. I think it is a good approach for low compressible or incompressible flows.

March 21, 2019, 00:02
#10
Senior Member

Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 7
Quote:
 Originally Posted by lukasf I think that you can combine totalPressure for p and pressureInletOutletVelocity for U at the outlet. I think it is a good approach for low compressible or incompressible flows.
Thank you, I will have a try.

Should totalPressure be used at outlet to match with pressureInletOutletVelocity which is used at outlet?

 June 6, 2020, 19:08 #11 Member   niewiemnic Join Date: Jan 2018 Location: Niemcy Posts: 80 Rep Power: 7 For me this setting works really well, Pressure: Code: ```inlet { type zeroGradient; } outlet { type totalPressure; rho none; p0 uniform 0; value uniform 0; }``` Velocity: Code: ```inlet { type turbulentInlet; referenceField uniform (38 0 0); fluctuationScale (0.01 0.01 0.01); value uniform (38 0 0); } outlet { type pressureInletOutletVelocity; value uniform (38 0 0); }``` Last edited by spalartallmaras; June 6, 2020 at 20:23.

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