OpenFoam Pressure Inlet Oulet
 

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

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

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

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)

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

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

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

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

I am now using these boundary conditions for velocity/pressure:

velocity:
inlet: fixedValue
outlet: pressureInletOutletVelocity

pressure:(p_rgh)
inlet: fixedFluxPressure
outlet: fixedValue

Should this setting be suitable？I am now using buoyantSimpleFoam. Should we combine totalPressure and pressureInletOutletVelocity?

Thank you.

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?

For me this setting works really well,

Pressure:

Velocity: