[mm7]

Hi,
I have little experience with OpenFOAM.
My goal is to analyse a hull resistance at speed growing from 0 to Umax, i.e 3 m/s.



I've got openfoam-2212 and started with DTCHull project, I've put my custom hull STL there, decreased volume of "tank" and refinement level to 5.


It worked well, but that was for constant flow velocity.


I've decided to apply linearRamp there.



Currently I am having issues when running runParallel $(getApplication)

error

Creating finite volume options from "constant/fvOptions"

Selecting finite volume options type accelerationSource
[6] [3] [0] 
[6] 
[6] --> FOAM FATAL IO ERROR: (openfoam-2212 patch=230110)
[6] 
[3] 
[3] --> FOAM FATAL IO ERROR: (openfoam-2212 patch=230110)
[3] Unknown fvOption type accelerationSource

Valid fvOption types :

50
(
acousticDampingSource
actuationDiskSource
buoyancyEnergy
buoyancyForce
buoyancyTurbSource
constantHeatTransfer
directionalPressureGradientExplicitSource
explicitPorositySource
fixedTemperatureConstraint
heatExchangerSource
interRegionExplicitPorositySource
jouleHeatingSource
limitTemperature
limitVelocity
meanVelocityForce
multiphaseMangrovesSource
multiphaseMangrovesTurbulenceModel
multiphaseStabilizedTurbulence
patchCellsSource
patchMeanVelocityForce
radialActuationDiskSource
radiation
rotorDisk
scalarCodedSource
scalarFixedValueConstraint
scalarPhaseLimitStabilization
scalarSemiImplicitSource
solidificationMeltingSource
sphericalTensorCodedSource
sphericalTensorFixedValueConstraint
sphericalTensorPhaseLimitStabilization
sphericalTensorSemiImplicitSource
symmTensorCodedSource
symmTensorFixedValueConstraint
symmTensorPhaseLimitStabilization
symmTensorSemiImplicitSource
tabulatedAccelerationSource
tabulatedHeatTransfer
tabulatedNTUHeatTransfer
tensorCodedSource
tensorFixedValueConstraint
tensorPhaseLimitStabilization
tensorSemiImplicitSource
variableHeatTransfer
vectorCodedSource
vectorFixedValueConstraint
vectorPhaseLimitStabilization
vectorSemiImplicitSource
velocityDampingConstraint
viscousDissipation
)

[0] file: constant/fvOptions.velocityRamping at line 21 to 34.

Here is my file constant/fvOptions

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#include    "refValues";

velocityRamping
{
    type        accelerationSource;
    active      on;
    selectionMode all;
    U           U;
    velocity
    {
        type    scale;
        scale
        {
          type        linearRamp;
          start       0;
          duration    $duration;
        }
        value    ($negUmax 0 0);
    }
}

Please advise



The whole project is attached.

[Alczem]

Hey!


Rather than using a fvOptions function, you could try uniformFixedValue as a boundary condition for U. It allows you to specify time-varying boundary conditions, so you can create your ramp

[mm7]

Yes, I've done that as well.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2212                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#include "../constant/refValues";

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

// min flow velocity
internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type uniformFixedValue;
        value $internalField;
        uniformValue {
            value ($negUmax 0 0);
            type scale;
            scale {
              type linearRamp;
              start 0;
              duration $duration;
            }
        }
    }

    outlet
    {
        type            outletPhaseMeanVelocity;
        alpha           alpha.water;
        value           $internalField;
        Umean $Umax;
        UnMean {
            value $Umax;
            type  scale;
            scale {
              type linearRamp;
              start 0;
              duration $duration;
            }
        }
    }

    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    hull
    {
        type            movingWallVelocity;
        value           uniform (0 0 0);
    }
}


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

There was one advise from a developer
"You need to define ramping function for the velocity at three points: inlet (BC type waveVelocity), outlet (BC type outletPhaseMeanVelocity) and you need the velocityRamping fvOption (which was recently renamed to accelerationSource). You need to ensure, that you have same parameters (ramp type, start and duration) for inlet, outlet and fvOption."
I've fount it here Multiphase ramping functionality


I've just changed quarterSineRamp to linearRamp.
But solver shows the error above.

[Alczem]

Oh okay, I thought that using uniformFixedValue in a very basic way at the inlet would be enough, like that:

<patchName> {     type            uniformFixedValue;     uniformValue    table     (         (0   (0 0 0))         (5   (10 0 0))     ); }

The ramp is properly defined if I am not mistaken, and you can leave the outlet with a zeroGradient condition? You are using interFoam correct?

[mm7]

Ok. I removed constant/fvOptions

And made 0/U this way

#include "../constant/refValues";

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

// min flow velocity
internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type uniformFixedValue;
        uniformValue table
        ( (0         ( 0 0 0))
          ($duration (10 0 0))
        );
    }

    outlet
    {
        type            zeroGradient;
    }

    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    hull
    {
        type            movingWallVelocity;
        value           uniform (0 0 0);
    }
}

zeroGradient has made outlet like an open side of a fishtank, like a glass has broken there. All water started flow out and level decreased there.


I need a whole body of water (and air) steadily increase velocity from 0 to Umax. In other words - like the boat (with the boundaries) start moving with growing speed in an infinite pond.


Yes, I am using interFoam

[Yann]

Hello Mark,

Just a side note: the link your provided about "accelerationSource" is from the OpenFOAM foundation branch (openfoam.org). You are using the ESI-OpenCFD branch (openfoam.com).

"accelerationSource" does not exist in the OpenCFD branch, and this is why you get the error in your first post.

Regards,
Yann

[mm7]

Originally Posted by Yann

Hello Mark,

Just a side note: the link your provided about "accelerationSource" is from the OpenFOAM foundation branch (openfoam.org). You are using the ESI-OpenCFD branch (openfoam.com).

"accelerationSource" does not exist in the OpenCFD branch, and this is why you get the error in your first post.

Regards,
Yann

Hi Yann,
thank you, I'll try to get the OpenFOAM foundation branch.




thank you Yann,
the OpenFOAM foundation branch works!

[mm7]

Though "accelerationSource" works ok, it is not exactly what I need.
The water coming from the inlet disturbs water in the tank.
I want to model a boat runs with acceleration on undisturbed water.
Like on a pond. So only the boat disturbs it.


One way it would be to create a long block mesh with 0 velocity inlet/outlet, and move the hull along of it. I am afraid it will increase processing time.


Another way is to keep the hull on same position relative to boundary and somehow move whole system - boat and boundary through the calm water.
I hope I explained it well.
Is it possible to define?

[Saralorenzo]

Hello everyone,


I have an error during the runing of my programe that looks like this:


/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 10-e450dce21ea5
Exec : icoFoam
Date : Sep 20 2023
Time : 13:41:42
Host : "adminval-HP-EliteBook-8540w"
PID : 9953
I/O : uncollated
Case : /home/admin-val/Desktop/SARA_CURSO_OPENFOAM/PRUEBA_1/tubo
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0.3

Reading physicalProperties

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.35s

Courant Number mean: 17.0316 max: 253.714
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::symGaussSeidelSmoother::smooth(Foam::word const&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::Field<double> const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, unsigned char, int) at ??:?
#4 Foam::symGaussSeidelSmoother::smooth(Foam::Field<d ouble>&, Foam::Field<double> const&, unsigned char, int) const at ??:?
#5 Foam::smoothSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#6 ? in "/opt/openfoam10/platforms/linux64GccDPInt32Opt/bin/icoFoam"
#7 ? in "/opt/openfoam10/platforms/linux64GccDPInt32Opt/bin/icoFoam"
#8 ? in "/opt/openfoam10/platforms/linux64GccDPInt32Opt/bin/icoFoam"
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10 ? in "/opt/openfoam10/platforms/linux64GccDPInt32Opt/bin/icoFoam"
Floating point exception (core dumped)







And I do not have any idea about where can be the error.


The mesh is ok and I have checked it.


Its about a curved tube where water flows


Could you help me about finding the error?


Thank you in advance, I am learning and I really consider your help