[Wesley]

would like to create apply a fully developed velocity profile at the inlet to my simulation.

I am currently using OpenFOAM 12 and I have not yet found how to do this.

I have tried several approaches without success.

For comparison, in OpenFOAM 9, applying this inlet condition:

    Inlet
    {
        type                flowRateInletVelocity;
        volumetricFlowRate  3.39e-5;
        extrapolateProfile  yes;
        value               uniform (0 0 0);
    }

would result in this inlet velocity profile (scaled to the velocity profile of the inlet):




This same information in OpenFOAM 12 results in a uniform inlet velocity (scale is from 0 to the average velocity across the inlet):



I have not yet found how to create a fully developed velocity profile at the inlet.

Thank you for any help you can give to me to get a fully developed velocity profile with OpenFOAM 12.

Edited to add: Until I can get a developed velocity profile at the inlet, I will be using an added length of flow with the slip boundary condition. This will deliver a somewhat developed velocity profile and will not result in very high pressures at the outer circumference of the inlet where the flow is in contact with the walls (noSlip) of the simulation.

[rmoerland]

Not sure if you found the solution, but it appears what you're looking for is the 'profile' option to flowRateInletVelocity. This was committed by Henry on Jan 24, 2022. So, it should be in version 10 and later.


From the documentation:


Example of the boundary condition specification for a volumetric flow rate:
<patchName>
{

type flowRateInletVelocity;
volumetricFlowRate 0.2;
profile laminarBL;

}


Example of the boundary condition specification for a mass flow rate:


<patchName>
{

type flowRateInletVelocity;
massFlowRate 0.2;
profile turbulentBL;
rho rho;
rhoInlet 1.0;

}

[Wesley]

Thank you for the suggestion, but it does not appear to give me the expected results. There is still not a developed flow at the inlet.


It is always possible I am overlooking something, so here is what I have for the U file at time 0:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  12
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    Inlet
    {
        type    flowRateInletVelocity;
        volumetricFlowRate  3.39E-05;
        profile laminarBL;
    }

    Outlet
    {
        type            zeroGradient;
    }

    Walls
    {
        type            noSlip;
    }

}

// ************************************************************************* //

Inlet velocity results for time = 0



Inlet velocity results for time = final (steady-state solution reached)

Originally Posted by rmoerland

Not sure if you found the solution, but it appears what you're looking for is the 'profile' option to flowRateInletVelocity. This was committed by Henry on Jan 24, 2022. So, it should be in version 10 and later.


From the documentation:


Example of the boundary condition specification for a volumetric flow rate:
<patchName>
{

type flowRateInletVelocity;
volumetricFlowRate 0.2;
profile laminarBL;

}


Example of the boundary condition specification for a mass flow rate:


<patchName>
{

type flowRateInletVelocity;
massFlowRate 0.2;
profile turbulentBL;
rho rho;
rhoInlet 1.0;

}

[michael_h]

There are several tutorial which use flowRateInletVelocity successfully.
They are listed with foamInfo -a flowRateInletVelocity.

It is important that your "Walls" are "type wall" and not "type patch" in blockMeshDict or snappyHexMeshDict.

[Wesley]

michael_h, thank you for the guidance.


I followed your comment on the "Walls" allowed the inlet velocity profile to create the developed velocity profile at the inlet.

I use Salome to generate the geometries I am simulating. To change the type, I went to the /constant/polyMesh directory and modified the type from what had been "patch" to "wall".

    Walls
    {
        type            wall;
        nFaces          3248;
        startFace       64940;
    }

There is now a developed velocity profile at the inlet, as shown below.

Originally Posted by michael_h

There are several tutorial which use flowRateInletVelocity successfully.
They are listed with foamInfo -a flowRateInletVelocity.

It is important that your "Walls" are "type wall" and not "type patch" in blockMeshDict or snappyHexMeshDict.