CFD Online Discussion Forums - PressureInletOutletVelocity BC

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)

- - PressureInletOutletVelocity BC (https://www.cfd-online.com/Forums/openfoam-pre-processing/116039-pressureinletoutletvelocity-bc.html)

PressureInletOutletVelocity BC

Hi to all
Someone know how velocity is obtained from pressure in pressureInletOutletVelocity?

thank to all

its like zeroGradient when fluid flows out of domain and is the inletValue specified when fluid flows into the domain.it only says that we have a specified pressure in its folder and doesn't use it to calculate velocity.

I think you are wrong because for example I set this boundary condition and for inflow I have a U different from the fixed value that I set ( (0,0,0) in my case). In some forum I find that the velocity of the flow inflow into the domain is calculated from the flux, but I don't understand how...Any suggestion?

see description in pressureInletOutletVelocityFvPatchVectorField.H
in opt folder->src->finiteVolume->fields->fvPatchFields_>derived:

Code:

Description

    This velocity inlet/outlet boundary condition is applied to pressure

    boundaries where the pressure is specified.  A zero-gradient condtion is

    applied for outflow (as defined by the flux); for inflow, the velocity is

    obtained from the patch-face normal component of the internal-cell value.



    The tangential patch velocity can be optionally specified.



    \heading Patch usage



    \table

        Property     | Description             | Required    | Default value

        phi          | flux field name         | no          | phi

        tangentialVelocity | tangential velocity field | no  |

    \endtable



    Example of the boundary condition specification:

    \verbatim

    myPatch

    {

        type            pressureInletOutletVelocity;

        phi             phi;

        tangentialVelocity uniform (0 0 0);

        value           uniform 0;

    }

    \endverbatim



Note

    Sign conventions:

    - positive flux (out of domain): apply zero-gradient condition

    - negative flux (into of domain): derive from the flux in the patch-normal

      direction

and see .C file of it.
this of code I found in pressureDirectedInletOutletVelocity.C that is like pressureInletOutletVelocity:

Code:

refValue() = inletDir_*phip/(rhop*ndmagS);

that is phi/(rho*area_of_cellface) that is same internalField(U) normal to ilet patch and is what I said you.

I see the file .H e .C but I not familiar with C language so it's difficult for me understand these files. My BC is:
pressureInletOutletVelocity
value uniform (0,0,0)
so U must be zero in portion of patch in which there is inflow? But my U is different from zero.Why?
For this reason i previously give reason to the user that say that U is calculated from the flux for inflow.

thank you very much for you replies

no.it seems that both inflow and outflow uses internalField value of velocity even in inflow situation.I correct myself your value is not important in inflow case.as I saw in the code phi/(rho*area) is used as you know phi=rho*patch_ area*U_normal then above expression is equal to U_normal at neghbour patch.
it seems correct because when you specify a value for pressure you shouln't specify velocity concurrent with that for well-posedness of cfd problem.
(p and T or U and T)

I didn't find the code lines that you write in my .C file, probably because the implementation of the BC is changed from two different version but I think that meaning is the same.
thank you very much for your help

for completeness it seems that in outlet velocity is implicitly calculated and in inlet just explicitly.
I think its because outflow is more likely to be unstable and inflow is more stable(from my experiences and what have read so far.somebody help me why is it so?)
And in inflow because maybe pressure is set such that involves velocity(like totalPressure) it should use velocity at that same time(explicit) not at later time after matrix calculation (implicit)
I think its the cause or soneone correct me.

hi
i want to simulate flow around airfoil.can i use pressureInletOutletVelocity for in or out boundary condition?
this boundary condition use for external flow?

Hi,
is present an inverse flow near Bc? if yes you can use pressureInletOutletVelocity.
See post 18 of this link
http://www.cfd-online.com/Forums/ope...tvelocity.html

dear diack very very thank you for your riply:)

In what part of software the boundary condition equations are written ?
for example i need the equation of inletoutlet boundary condition

here you find code for all inletOutlet conditions
http://www.openfoam.org/docs/cpp/

Hi,
Someone please help me to obtain inlet velocity profile where the flow is fully developed channel flow and the flow is 2D,steady and incompressible. I have used inlet velocity equation as U(1,J)=((4.0*(YV(J)))*(5.0-(YV(J))))/25.0 where the height of the channel is 5 unit.All the velocity vector is not parallel and the SHI profile is slightly curved . Original velocity equation is U=4Y(1-Y).

I will be grateful. Thank you.

Quote:

welcome forum Shamim

1- this question is not related to this post, so open new thread, unrelated post make forum mess

2- you should describe your question more precisely then other users can help you easier