[Phicau]

Hi Qi Yang,
Yes, forward means waves and current travel in the X+ direction. Backward means waves travel in X+ and current in X-.
There are 3 places that you need to monitor to set the current: 0/U for the absorption boundary, constant/waveDict for the wave generation boundary and (optional) system/setFields to set the initial condition. All need to be consistent.

A very easy way to proceed is to run the currentWaveFlume tutorial included in olaFlow. Start by running the case conditions that are closer to what you want to obtain (select options 1-4 in the runCase script). Then kill the simulation and study how the files look like. Finally, adapt the case to your particular needs.

Your numerical setup seems to have some issues. Probably you selected a wrong BC or configuration, since the water level seems to increase with time in your simulation. Note that this does not happen if you set everything correctly (as is in the currentWaveFlume tutorial). I have compared the pressure for the cases with waves only (red line) and waves + forward and waves + backward currents (red lines) and the results are perfect.

Best,
Pablo

[qi.yang@polimi.it]

Originally Posted by Phicau

Hi Qi Yang,
Yes, forward means waves and current travel in the X+ direction. Backward means waves travel in X+ and current in X-.
There are 3 places that you need to monitor to set the current: 0/U for the absorption boundary, constant/waveDict for the wave generation boundary and (optional) system/setFields to set the initial condition. All need to be consistent.

A very easy way to proceed is to run the currentWaveFlume tutorial included in olaFlow. Start by running the case conditions that are closer to what you want to obtain (select options 1-4 in the runCase script). Then kill the simulation and study how the files look like. Finally, adapt the case to your particular needs.

Your numerical setup seems to have some issues. Probably you selected a wrong BC or configuration, since the water level seems to increase with time in your simulation. Note that this does not happen if you set everything correctly (as is in the currentWaveFlume tutorial). I have compared the pressure for the cases with waves only (red line) and waves + forward and waves + backward currents (red lines) and the results are perfect.

Best,
Pablo

Thank you for your reply, Pablo. I am simulating wave-current-pile interation. I put my boundary conditions here and also attached the whole simulation files. Could you please give me a look?

alpha.water

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    	"cylinder.*" 
	{
		type	zeroGradient;
		
	}
    
    
    "inlet.*"
    {
        type            waveAlpha;
        waveDictName    waveDict;
        value           uniform 0;
    }
    "sides.*" //frontAndBack
    {
        type            symmetry;//empty;
    }
    "outlet.*"
    {
        type            zeroGradient;
    }
    "ground.*"//bottom
    {
        type            zeroGradient;
    }
    "top.*"//atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
}

p_rgh

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    	"cylinder.*"
	{
	type		fixedFluxPressure;
	value		uniform 0;

	}
    
    
    
    "sides.*"//frontAndBack
    {
        type            symmetry;//empty;
    }
    "outlet.*" 
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }
    "inlet.*" 
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }
    "ground.*"//bottom
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }
    "top.*"//atmosphere 
    {
        type            totalPressure;
        U               U;
        phi             phi;
        rho             rho;
        psi             none;
        gamma           1;
        p0              uniform 0;
        value           uniform 0;
    }
}

U

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

internalField   uniform (0 0 0);

boundaryField
{
        "cylinder.*"
	{
		type	fixedValue;
		value	uniform (0 0 0);


	}  
    
    
    "inlet.*"
    {
        type            waveVelocity;
        uCurrent        (0 0 0);
        value           uniform (0 0 0);
    }
    "outlet.*"
    {
        type            waveAbsorption3DVelocity;
        value           uniform (0 0 0);
    }
    "ground.*"//bottom
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    "top.*"//atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    "sides.*"//frontAndBack
    {
        type    symmetry;//            empty;
    }
}

k

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

internalField   uniform 0.00000001;

boundaryField
{
   	"cylinder.*"
{
type	kqRWallFunction;
value	uniform 1e-8;

}
   
   
    "inlet.*"
    {
        type            inletOutlet;
        inletValue	    uniform 0.00000001;
        value           uniform 0.00000001;
    }
   "outlet.*"
    {
        type            inletOutlet;
        inletValue	    uniform 0.00000001;
        value           uniform 0.00000001;
    }
    "top.*"//atmosphere
    {
        type            inletOutlet;
        inletValue	    uniform 0.00000001;
        value           uniform 0.00000001;
    }
    "sides.*"//frontAndBack
    {
        type      symmetry;//            empty;
    }
    "ground.*"//bottom
    {
        type            kqRWallFunction;
        value           uniform 0.00000001;
    }
}

omega

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

internalField   uniform 0.001;

boundaryField
{
    
    	"cylinder.*"
{
type	omegaWallFunction;
value	uniform 0.001;

}
    
    
    "inlet.*"
    {
        type            inletOutlet;
        inletValue	    uniform 0.001;
        value           uniform 0.001;
    }
    "outlet.*"
    {
        type            inletOutlet;
        inletValue	    uniform 0.001;
        value           uniform 0.001;
    }
    "top.*"//atmosphere
    {
        type            inletOutlet;
        inletValue	    uniform 0.001;
        value           uniform 0.001;
    }
    "sides.*"//frontAndBack
    {
        type    symmetry;//            empty;
    }
    "ground.*"//bottom
    {
        type            omegaWallFunction;
        value           uniform 0.001;
    }
}

nut

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    
    	"cylinder.*"
	{
	type nutkWallFunction;
	value	uniform 0;
	}
    
    
    "inlet.*"
    {
        type            zeroGradient;
    }
    "outlet.*"
    {
        type            zeroGradient;
    }
    "top.*"//atmosphere
    {
        type            calculated;
        value           uniform 0;
    }
    "sides.*"//frontAndBack
    {
        type     symmetry;//       empty;
    }
    "ground.*"//bottom
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
}

[Phicau]

Hi Qi Yang,
Please follow my advice and start simple. 2D, no structure first, when it works, it is easy to extend to 3D and add the cylinder(s). -> A very easy way to proceed is to run the currentWaveFlume tutorial included in olaFlow. Start by running the case conditions that are closer to what you want to obtain (select options 1-4 in the runCase script). Then kill the simulation and study how the files look like. Finally, adapt the case to your particular needs.

At a first glance:
- The current should not be set to 0 in 0/U/inlet, it will be read from waveDict.
- You should use waveAbsorption2DVelocity instead and set the current at the outlet.

Best,
Pablo

[qi.yang@polimi.it]

Originally Posted by Phicau

Hi Qi Yang,
Please follow my advice and start simple. 2D, no structure first, when it works, it is easy to extend to 3D and add the cylinder(s). -> A very easy way to proceed is to run the currentWaveFlume tutorial included in olaFlow. Start by running the case conditions that are closer to what you want to obtain (select options 1-4 in the runCase script). Then kill the simulation and study how the files look like. Finally, adapt the case to your particular needs.

At a first glance:
- The current should not be set to 0 in 0/U/inlet, it will be read from waveDict.
- You should use waveAbsorption2DVelocity instead and set the current at the outlet.

Best,
Pablo

Dear Pablo,

Thanks for your suggestions. In fact, I reduced the domain length and the cells and I got the logical results. Do you think they are reasonable? The plot is the dynamic wave pressure at the bottom.

Bests,

[AUbuntu]

Dear Pablo,

I am trying to validate the solitary wave generated by olaFlow with theory.
η(t,x)=H 〖sech〗^2 (κ (x-Ct))

In theory we have the below equation.

T= 2h/C √(4h/3H) (3.8+H/h)

for the period of the solitary wave.

So I used T/2 to shift the theory equation to match with the start of the simulation.

η(t,x)=H 〖sech〗^2 (κ (x-Ct-T/2))

but there is a phase difference between the results and I don't know how to justify it!

Could you please let me know how I can fix this.
Kind regards,
Amir

[Phicau]

Hi Kimi,
Please refer to my previous post in which I showed you the time series already.

Hi Amir,
Wave period for a solitary wave is not defined in a universal way. Please check the source code for the definition in olaFlow: 4.0*PII/sqrt(3)*h/sqrt(H/h), that is probably the source of your phase difference.

Best,
Pablo

[pcwang]

Hello Pablo,

I've tried to run the tutorial case 'baseWaveFlumeNewAbs' from 'Dev' branch. I've not change anything of this tutorial case, and only run the './runCase' script.

When this script execute the line 'olaFlow > olaFlow.log', the terminal outputs some errors, and olaFlow couldn't work well:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _7bdb509494-20201222 OPENFOAM=2012 patch=210414
Arch   : "LSB;label=32;scalar=64"
Exec   : olaFlow
Date   : Jun 30 2022
Time   : 23:11:43
Host   : hpws13
PID    : 12794
I/O    : uncollated
Case   : /home/wpc/wpcdata/baseWaveFlumeNewAbs
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Selecting dynamicFvMesh staticFvMesh

PIMPLE: Operating solver in PISO mode

Reading field porosityIndex

Porosity NOT activated

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar
Selecting laminar stress model Stokes

Reading g

Reading hRef
Calculating field g.h

No MRF models present

No finite volume options present
DICPCG:  Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.00119048
Time = 0.00119048

PIMPLE: iteration 1
MULES: Solving for alpha.water
alpha.water BC on patch inlet

Wave Generation BC
Wave theory: StokesI
H: 10
T: 5
h: 130.156
L: 39.0327
Direction: 0?
Generation in: Deep waters.
Relative depth (kh): 20.9515


Phase-1 volume fraction = 0.765625  Min(alpha.water) = 0  Max(alpha.water) = 1
alpha.water BC on patch inlet
MULES: Solving for alpha.water
alpha.water BC on patch inlet
Phase-1 volume fraction = 0.765625  Min(alpha.water) = 0  Max(alpha.water) = 1
DICPCG:  Solving for p_rgh, Initial residual = 1, Final residual = 0.0281341, No Iterations 2
time step continuity errors : sum local = 6.76728e-07, global = 1.09967e-19, cumulative = 1.09967e-19
DICPCG:  Solving for p_rgh, Initial residual = 0.013655, Final residual = 0.000664405, No Iterations 20
Velocity BC on patch inlet

Wave Generation BC
Wave theory: StokesI
H: 10
T: 5
h: 130.156
L: 39.0327
Direction: 0?
Generation in: Deep waters.
Relative depth (kh): 20.9515


Active wave absorption BC on patch outlet
"Initial water depths for absorption" 1( 130.156 )

Selecting active wave absorption model extendedRangeAWA
AWA model: patch outlet
    Theory: extendedRangeAWA
    Number of paddles: 1
    Reference water depth: 1(130.156)
    Wave period: 5
Updating extendedRangeAWA absorption model for patch outlet
double free or corruption (out)

My OpenFOAM version is v2012, and my system version is Ubuntu 20.04. It is puzzling that when I ran this tutorial in my VMware virtual machine, everything went well. In my virtual machine, the OpenFOAM version is also v2012, but the system version is Ubuntu 18.04.

Then I tested the tutorial 'baseWaveFlume' which was not using the extendedRangeAWA model in Ubuntu 20.04 system(OpenFOAM-v2012). And olaFlow worked very well. So I think there are no errors when I compiled the olaFlow codes.

This error confused me a few days. Is this something to do with the system version that I am using to run ?

Hope for your answer.

Thanks

Peicen

Updated in July 1st 2022, 10:30 :

This morning, I tried the tutorial case 'baseWaveFlumeNewAbs' in other work station whose system version is CentOS 7.9.2009 and OpenFOAM version is also v2012, and this tutorial runs very well. So I think there must be some difference between these work stations.

[Tianqi Ma]

Originally Posted by abas.rahmani86

hi pablo
I have a problem with simulating wave with period less than 3 sec by olafoam
I try to simulate a flume without any structure and get a regular wave in it
but after 30 second i see irregularity in wave.the photo show wave gage at 3,8 and 12 meter from begining of flume(wave maker).I attach source file too.
wave period=1.67 sec
wave height=0.175 m
water depth=0.8 m
I really confuse because i change every parameter for it.
do you meet this ever?
many thanks for your reply Pablo.
abas rahmani
[/IMG]
[/IMG]
[/IMG]

Hi Abas,

Did you solve the problem? I also have the same problem as you posted. The wave elevations at some locations are irregular.

Thanks

[Sarah_Ag]

Hey everyone, I'm in a bit of a situation now. I created a mesh using blockmesh and basewaveflume tutorial like base, BUT my simulation goes crazy, it's like the wave created displace all the water of the ocean and become a tsuname. I'm sending the pics so you guys can understand better. I'm putting below my wave dict, fvschemes, and fvsolution here.



Dis you guys already saw something like this? Can help me or give me any tips? Thanks in advance.


FVSCHEMES


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
div(rhoPhi,U) Gauss limitedLinearV 1;
div(U) Gauss linear;
div((rhoPhi|interpolate(porosity)),U) Gauss upwind 1;
div(rhoPhiPor,UPor) Gauss upwind 1;
div(rhoPhi,UPor) Gauss upwind 1;
div(rhoPhiPor,U) Gauss upwind 1;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
div((muEff*dev(T(grad(U))))) Gauss linear;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div((phi|interpolate(porosity)),k) Gauss upwind;
div((phi|interpolate(porosity)),epsilon) Gauss upwind;
div(phi,omega) Gauss upwind;
div((phi|interpolate(porosity)),omega) Gauss upwind;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p_rgh;
pcorr;
alpha.water;
}


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









FVSOLUTION





/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
"alpha.water.*"
{
nAlphaCorr 1;
nAlphaSubCycles 2;
alphaOuterCorrectors yes;
cAlpha 1;

MULESCorr no;
nLimiterIter 3;

solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0.05;
}

"pcorr.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-5;
relTol 0;
}

p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0.05;
}

p_rghFinal
{
$p_rgh;
relTol 0;
}

U
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0.05;
}
}

PIMPLE
{
momentumPredictor no;
nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
fields
{
}
equations
{
".*" 1;
}
}


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









WAVE DICT


/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.3 |
| \\ / A nd | Web: http://www.openfoam.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object waveDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

waveType regular;

waveTheory StokesII;

genAbs 1;

absDir 0.0;

nPaddles 1;

waveHeight 1.0;

wavePeriod 4.05;

waveDir 0.0;

wavePhase 1.57079633;

// Change both entries to true to re-read this dictionary upon restart.
rereadAlpha false;
rereadU false;

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