[steddy]

Hi all,
Noob here, having a simple question.
Let's take the Motorbike tutorial, that is included in OpenFOAM:

/opt/openfoam7/tutorials/incompressible/simpleFoam/motorBike

How would you modify the files in the '0' folder in order to fully resolve the boundary layer of (both) the motorbike and the floor (Low Reynolds, y+ <= 1)?
I have already seen this post, but it is quite old and I am not sure if it is still valid: k-omega SST and wall functions in OpenFOAM-1.5-dev
I will include for your convenience the code of the k, nut, omega, p, U.orig files.

k

#include        "include/initialConditions"

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform $turbulentKE;

boundaryField
{
    //- Set patchGroups for constraint patches
    #includeEtc "caseDicts/setConstraintTypes"

    //- Define inlet conditions
    #include "include/fixedInlet"

    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }

    lowerWall
    {
        type            kqRWallFunction;
        value           $internalField;
    }

    motorBikeGroup
    {
        type            kqRWallFunction;
        value           $internalField;
    }

    #include "include/frontBackUpperPatches"
}

nut

boundaryField
{
    //- Set patchGroups for constraint patches
    #includeEtc "caseDicts/setConstraintTypes"

    frontAndBack
    {
        type            calculated;
        value           uniform 0;
    }

    inlet
    {
        type            calculated;
        value           uniform 0;
    }

    outlet
    {
        type            calculated;
        value           uniform 0;
    }

    lowerWall
    {
        type            nutkWallFunction;
        value           uniform 0;
    }

    upperWall
    {
        type            calculated;
        value           uniform 0;
    }

    motorBikeGroup
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
}

omega

#include        "include/initialConditions"

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

internalField   uniform $turbulentOmega;

boundaryField
{
    //- Set patchGroups for constraint patches
    #includeEtc "caseDicts/setConstraintTypes"

    #include "include/fixedInlet"

    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }

    lowerWall
    {
        type            omegaWallFunction;
        value           $internalField;
    }

    motorBikeGroup
    {
        type            omegaWallFunction;
        value           $internalField;
    }

    #include "include/frontBackUpperPatches"
}

p

#include        "include/initialConditions"

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform $pressure;

boundaryField
{
    //- Set patchGroups for constraint patches
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           $internalField;
    }

    lowerWall
    {
        type            zeroGradient;
    }

    motorBikeGroup
    {
        type            zeroGradient;
    }

    #include "include/frontBackUpperPatches"
}

U.orig

#include        "include/initialConditions"

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

internalField   uniform $flowVelocity;

boundaryField
{
    //- Set patchGroups for constraint patches
    #includeEtc "caseDicts/setConstraintTypes"

    #include "include/fixedInlet"

    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           $internalField;
    }

    lowerWall
    {
        type            fixedValue;
        value           $internalField;
    }

    motorBikeGroup
    {
        type            noSlip;
    }

    #include "include/frontBackUpperPatches"
}

[openfoamer93]

I assume that the boundary layer is already refined so that y+<1. If not then try to refine the boundary layer using the command:
refineWallLayer 'patchNmae' 0.5

Then

type omegaWallFunction;
value $internalField;

automatically switches to a low Re in case y+<1 and it resolve the boundary layer without using any wall function and switches to wall function when y+ is large.

No need to modify anything

[steddy]

Bassam, thanks for your answer.

I assume that the boundary layer is already refined so that y+<1.

Yes, the average yplus is ~0.04 on the whole surface thanks to tiny layers.

No need to modify anything

Do you have any source to back this up; perhaps an OpenFOAM page I didn't read?

[openfoamer93]

For omega wall function I am sure! You can revise the theory behind this wall function which switch automatically.

However, the k and nut should be:
kLowReWallFunction
nutLowReWallFunction

I just realised that they were not a LowRe

Please revise page 27 from this report that support my claims:
A Thorough Description Of How Wall Functions Are Implemented In OpenFOAM - Chalmers

[steddy]

Thank you very much for your help and time, I will modify accordingly!

[openfoamer93]

So did it work with you? I tried the approach in another case and compared the results to experiment which was satisfactory

[steddy]

Hi, right now I am trying to replicate in OpenFOAM a Simscale case that investigates the Ahmed body, using the boundary conditions that you suggested. I will get back to you as soon as possible and send you the outcomes when the solver will be done; it will take ~ 1 day because the mesh is pretty fine (18M cells and I am using a server with 8 cores only). Thank you again for your dedication
https://www.simscale.com/projects/gs...ni/ahmed_body/

[openfoamer93]

Wow 18M that definitely needs a cluster computer to handle the case. All the best in your simulations!