[waves2Foam] Trying to modify the 3DWaves tutorial to apply to 3D waves incident on a cylinder

arieljeds · October 9, 2015, 06:07

Hi Niels,

I'm trying to modify the 3DWaves tutorial to apply to 3D waves incident on a cylinder using Openfoam version 2.3.0 running on Ubuntu 12.04.

I am using almost the same boundary conditions and also tried to apply the relaxation factor. When I run waveFoam though, I get the following output:

PIMPLE: Operating solver in PISO mode

Reading g

Reading waveProperties

Reading waveProperties
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
Calculating field g.h

No finite volume options present

#0 Foam::error:

rintStack(Foam::Ostream&) in "/home/ariel/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/home/ariel/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::relaxationShapes::relaxationShapeRectangular ::relaxationShapeRectangular(Foam::word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#4 Foam::relaxationShapes::relaxationShape::adddictio naryConstructorToTable<Foam::relaxationShapes::rel axationShapeRectangular>::New(Foam::word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#5 Foam::relaxationShapes::relaxationShape::New(Foam: :word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#6 Foam::relaxationSchemes::relaxationScheme::relaxat ionScheme(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#7 Foam::relaxationSchemes::relaxationSchemeSpatial:: relaxationSchemeSpatial(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#8 Foam::relaxationSchemes::relaxationScheme::adddict ionaryConstructorToTable<Foam::relaxationSchemes:: relaxationSchemeSpatial>::New(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#9 Foam::relaxationSchemes::relaxationScheme::New(Foa m::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#10 Foam::relaxationZone::relaxationZone(Foam::fvMesh const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so"
#11
in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/bin/waveFoam"
#12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13
in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/bin/waveFoam"
Floating point exception

And then it doesn't run from here. I don't understand where the problem would be located or what it applies to. I can send on any other information I'm able, let me know what else I can tell you.

Thanks in advance for any advice

Ariel

ngj · October 9, 2015, 10:57

Hallo,

I am almost sure that the problem relates to your relaxation zones, so try to use relaxationZoneLayout to see, what goes wrong.

Kind regards,

Niels

arieljeds · October 12, 2015, 08:11

Hi Niels,

Thanks for getting back to me. Can you give me any advice on how to use the relaxationZoneLayout?

Thanks again

Ariel

EDIT: Sorry realised this was an extremely stupid question right after asking it! I've managed to get it working, I changed the size of the relaxation zone.

SECONDARY QUESTION:

I have a simulation running but water is only entering from the bottom half of the field (I have a 3D field from -8 < x < 20, -2 < y < 2, -5 < z < 0.5) and the water is only entering for negative y values. I can tell this is happening because if I look at parafoam before running the case, the set up looks correct from one side but from the other there are no waves entering .. Also, when I tried to run the case and then view some results in paraview, paraview shuts down with the error:

Code:

 size 31000 is not equal to the give value of 62000

which also implies that it is only entering half the field. I had a look at the alpha1.org and the alpha.water file and I don't really understand where I went wrong.

Am i looking in the wrong place or can you point me to the file that might help me change my inlet field so that the water enters from -2 < y < 2?

Thanks in advance!

arieljeds · November 11, 2015, 08:06

Hi Niels,

Apologies for not correcting an earlier badly worded question.. I re-read it there and it doesn't make sense!! Sorry about that.. I managed to view the relaxation zone and it looks ok for the moment.

I'm trying to model the free surface flow past/around a surface piercing cylinder. I am currently using relaxation zones. I'm having an issue when I run setWaveParameters after running blockMesh, only half the field (-y only) is being set for alpha.water and p_rgh (see image attached).

I had a look through the source code for the setWaveField and setWaveParameters and I'm not seeing where I can adjust this.

My alpha.water file looks like (without foam header):

Code:

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    top
    {
        type		symmetryPlane;
    }
    
    bottom
    {
        type  		symmetryPlane;
    }
    
    inlet
    {
        type            waveAlpha;
        refValue        uniform 0;
        refGrad         uniform 0;
        valueFraction   uniform 1;
        value           uniform 0;
    }
    
    outlet
    {
        type            zeroGradient;
    }
     
    cylinder
    {
        type            zeroGradient;
    }
    
    seaFloor
    {
        type            zeroGradient;
    }
    
    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
}

And my waveProperties.input file looks like:

Code:

seaLevel 		0.01; 
seaLevelAsReference	false; 

// A list of the relaxation zones in the simulation. The parameters are given
// in a <name>Coeffs below.

relaxationNames (inlet outlet); 

initializationName	outlet; 

inletCoeffs
{
     waveType		stokesFirst;       	// Regular waves
     depth		5.000;			// Water Depth 
     period		6.0; 			// Wave period
     phi		0.00000;		// Phase
     direction		(1.0 0.0 0.0);		// Direction of incoming waves
     height		0.2;			// Wave height in meters
     
     relaxationZone
     {
          relaxationScheme	Spatial; 
          relaxationShape	Rectangular; 
          beachType		Empty; 
          
          relaxType 		INLET; 
          startX		(-8.0 -2.0 -5);
          endX			(-4.0 2.0 0.5);
          orientation		(1.0 0.0 0.0); 
     }
};

outletCoeffs
{
    waveType		potentialCurrent; 
    U			(0 0 0);
    Tsoft		2; 
    
    relaxationZone
    {
    	relaxationScheme	Spatial;
    	relaxationShape		Rectangular; 
    	beachType		Empty; 
    	
    	relaxType		OUTLET;
    	startX			(15 -2 -5);
    	endX			(20 2.0 0.5 );	
        orientation		(1.0 0.0 0.0); 
    }
};

I'm really not seeing where the issue is. I played around with the initial alpha value and had a look and it seemed to distribute it evenly across + and - y values before running setWaveParameters and setWaveField, leading me to believe that the issue is in the direction that my wave is being input.

Hopefully this question makes sense.. Please let me know if there's other info I can give you.

ngj · November 11, 2015, 08:18

Hi Ariel,

Could it be that your gravity vector is still pointing in the y-direction?

Kind regards,

Niels

arieljeds · November 11, 2015, 08:24

Yes that was exactly it! I didn't even think about that.. Thank you for your quick and helpful reply..

arieljeds · November 19, 2015, 13:37

Hi Niels,

I'm trying to construct a case of linear wave flow around a surface piercing cylinder using relaxation zones at the inlet and outlet.

I am very new to CFD and OpenFOAM still so I'm trying to understand the boundary conditions to use with waves2Foam. I managed to set up the case and run it but it is not looking right yet so I have a couple of initial questions..

1) First of all, I am going to be interested in the near-wake only but at the moment, my domain is 2 wavelengths long (38 m). The inlet relaxation zone is 4m long and the outlet is 10m. Is it unnecessary for me to use relaxation zones in this case due to the focus on the near wake?

2) After running waveFoam, the simulation doesn't look right and when I did a vector plot in paraview, the vectors are pointing in the positive z direction instead of the expected x direction. I can't see where this has gone wrong...

My 0/U file is:

Code:

dimensions		[0 1 -1 0 0 0 0];
	
     internalField	uniform (1 0 0);
	
     boundaryField
     {	
     	top
     	{
             type		symmetryPlane;
        }
        
        bottom
        {
             type		symmetryPlane;
        }
        
        inlet
        {
             type		waveVelocity;
             refValue		uniform (0 0 0);
             refGradient	uniform (0 0 0);
             valueFraction	uniform 1; 
             value		uniform (0 0 0);
        }
        
        outlet
        {
             type		fixedValue;
             value		uniform (1 0 0);
        }
        
        cylinder
        {
             type		fixedValue;
             value		uniform (0 0 0);
             
        }
        
        seaFloor
        { 
             type		slip;
        }
        
        atmosphere
        {
             type		pressureInletOutletVelocity; 
             value		uniform (0 0 0);
        }
        
     }

And my waveProperties.input file:

Code:

seaLevel 		0.00; 
seaLevelAsReference	false; 

// A list of the relaxation zones in the simulation. The parameters are given
// in a <name>Coeffs below.

relaxationNames (inlet outlet); 

initializationName	outlet; 

inletCoeffs
{
     waveType		stokesFirst;       	// Regular waves
     depth		5.000;			// Water Depth 
     period		3.58; 			// Wave period
     phi		0.00000;		// Phase
     direction		(1.0 0.0 0.0);		// Direction of incoming waves
     height		0.084;			// Wave height in meters
     
     relaxationZone
     {
          relaxationScheme	Spatial; 
          relaxationShape	Rectangular; 
          beachType		Empty; 
          
          relaxType 		INLET; 
          startX		(-8.0 -2.0 -5);
          endX			(-4.0 2.0 0.5);
          orientation		(1.0 0.0 0.0); 
     }
};

outletCoeffs
{
    waveType		potentialCurrent; 
    U			(0 0 0);
    Tsoft		3.58; 
    
    relaxationZone
    {
    	relaxationScheme	Spatial;
    	relaxationShape		Rectangular; 
    	beachType		Empty; 
    	
    	relaxType		OUTLET;
    	startX			(28 -2 -5);
    	endX			(38 2.0 0.5 );	
        orientation		(1.0 0.0 0.0); 
    }
};

I'd really appreciate any advice on correcting this and can provide the rest of the case files if necessary.

I hope that my questions make sense!

Thanks,
Ariel

arieljeds · December 2, 2015, 13:10

Hi,

I have been running some cases using Stokes 1st waves in waves2foam based off of the waveFlume case and the 3DWave cases. I am trying to do two things:
1) Simulate regular waves in a wave tank (would like to attempt irregular and possibly 3D ocean waves too but have not attempted this yet)
2) simulate regular wave flow around a cylinder with viscosity but no turbulence

I have set up a case to for the wave tank and run it. First of all, it appears that the relaxation zone is very long because there only seem to be a couple of wavelengths. My domain goes from -5 < x < 150, -10 < y < 10, -5 < z < 2 (z is the vertical direction). The wavelength is L = 30 m (T = 5sec) and the relaxation zone lengths for the inlet and outlet are 1.5*L. Wave height is 0.3 m.

Because it looks as though there are only a couple of wavelengths so I was wondering if the outlet relaxation zone is too long? Also, if I run a vector plot (using glyphs), it appears that there is a lot of reflection. I have been trying to read and understand what is affecting this but am getting stuck. Would really appreciate any help.

Secondly, I used the probeDefinitions to create some data for the free surface but I'm not sure how to plot this data?

Thanks for any help! Please let me know if I can provide you with specific files or anything.

arieljeds · December 7, 2015, 10:33

Quote:

Originally Posted by arieljeds

...

Because it looks as though there are only a couple of wavelengths so I was wondering if the outlet relaxation zone is too long? Also, if I run a vector plot (using glyphs), it appears that there is a lot of reflection. I have been trying to read and understand what is affecting this but am getting stuck. Would really appreciate any help.

Secondly, I used the probeDefinitions to create some data for the free surface but I'm not sure how to plot this data?

Thanks for any help! Please let me know if I can provide you with specific files or anything.

Hi everyone, has anyone had experience with this? I've run the case several times with different wave parameters and then using exactly the same wave set up as in waveFlume and I still have the issue of the wave not travelling the full way down the wave tank. Any advice?

ngj · December 7, 2015, 10:40

Hallo Ariel,

It does not make sense that you say that there is a lot of reflection, but on the other hand the wave does not travel through the entire domain. Your initial question was very hard to understand, which was the reason that I did not answer.

See a guide here to pose "easy to answer" questions:

http://www.cfd-online.com/Forums/ope...-get-help.html

Kind regards,

Niels

arieljeds · December 7, 2015, 10:52

Hi Niels,

Thank you for your quick reply and I apologise for another poorly worded question. I'm extremely new to Openfoam/CFD/programming and sometimes I'm finding it hard to ask a specific question clearly if I'm struggling to understand the relevant area. I hope that this is more specific:

I have set up a wave tank and I would like to begin by simply generating a wave using the relaxation zones and stokes first waves. I have set up the wave tank but when I run the simulation, the wave only appears to reach approximately 1.5 wavelengths (the length of the inlet relaxation zone) and then dissipate, rather than travel down to the outlet. The relaxation zone layout, velocity contour plot at the final time step and my waveProperties.input file are shown here (heading not included to save space):

Code:

seaLevel 		0.00; 
//seaLevelAsReference	false; 

// A list of the relaxation zones in the simulation. The parameters are given
// in a <name>Coeffs below.

relaxationNames (inlet outlet); 

initializationName	outlet; 

inletCoeffs
{
     waveType		stokesFirst;       	// Regular waves
     depth		0.40000;		// Water Depth 
     period		2.0;	 		// Wave period
     phi		0.00000;		// Phase
     direction		(1.0 0.0 0.0);		// Direction of incoming waves
     height		0.1;			// Wave height in meters
     
     // Relaxation zone is where waves are initiated
     relaxationZone
     {
          relaxationScheme	Spatial; 
          relaxationShape	Rectangular; 
          beachType		Empty; 
          
          relaxType 		INLET; 
          startX		(-5.0 -3.0 0);
          endX			( 0.0  3.0 0);
          orientation		(1.0 0.0 0.0); 
     }
};

outletCoeffs
{
    waveType		potentialCurrent; 
    U			(0 0 0);
    Tsoft		2; 
    
    relaxationZone
    {
    	relaxationScheme	Spatial;
    	relaxationShape		Rectangular; 
    	beachType		Empty; 
    	
    	relaxType		OUTLET;
    	startX			(15 -3 0);
    	endX			(20  3 0);	
        orientation		(1.0 0.0 0.0); 
    }
};
     
 
// *************************************************************************//

I have read the paper for wave2Foam and have tried different relaxation layout orientation, starts, finishes and wave properties (depth, period) and have not had success. I am failing to see where the issue lies and would really appreciate any guidance on this.

Thank you again for your time

ngj · December 7, 2015, 11:33

Hallo Ariel,

My only guesses are that you have either way too few cells per wave length or your specification of the water depth does not match that given by your geometry.

Kimd regards,

Niels

arieljeds · December 10, 2015, 08:22

Hi Niels,

Thanks again for getting back to me. Ok, this did seem to be the problem. I realised I only had a few cells per wavelength so I have increased that to approx. 75 cells per wavelength. Is there a general value of cell per wavelength that should be followed? I am also attempting to run a case with flow over a cylinder using an extension of the same mesh set up from the potentialFoam cylinder tutorial (the entire field is set up instead of just a quarter). As the mesh is slightly more complicated than a simple wave tank, I have only managed to have 25 cells per wavelength at the inlet. I haven't yet run the case to see the effect it has.

I have a secondary question in regards to the transportProperties dictionary that is used in each tutorial (I think that the same ones are used in interFoam as well). I noticed that in the github versions of the tutorials, there is no transportProperties file. Why is this file missing in the tutorials?

ngj · December 10, 2015, 11:18

Good afternoon,

@Ariel: The transportProperties are copied to the correct location at the time of execution of the tutorial. This procedure was needed in order to preserve cross version compatibility of waves2Foam.

With respect to the discretisation of the computational domain, then 25 cells per wave length is definitely too little and so might 75 be. The correct answer will rely on your actual problem and I recommend you to perform some testing on your own.

Kind regards,

Niels

October 9, 2015, 06:07	Trying to modify the 3DWaves tutorial to apply to 3D waves incident on a cylinder	#1
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi Niels, I'm trying to modify the 3DWaves tutorial to apply to 3D waves incident on a cylinder using Openfoam version 2.3.0 running on Ubuntu 12.04. I am using almost the same boundary conditions and also tried to apply the relaxation factor. When I run waveFoam though, I get the following output: PIMPLE: Operating solver in PISO mode Reading g Reading waveProperties Reading waveProperties 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 Calculating field g.h No finite volume options present #0 Foam::error:rintStack(Foam::Ostream&) in "/home/ariel/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/ariel/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64-linux-gnu/libc.so.6" #3 Foam::relaxationShapes::relaxationShapeRectangular ::relaxationShapeRectangular(Foam::word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #4 Foam::relaxationShapes::relaxationShape::adddictio naryConstructorToTable<Foam::relaxationShapes::rel axationShapeRectangular>::New(Foam::word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #5 Foam::relaxationShapes::relaxationShape::New(Foam: :word const&, Foam::fvMesh const&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #6 Foam::relaxationSchemes::relaxationScheme::relaxat ionScheme(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #7 Foam::relaxationSchemes::relaxationSchemeSpatial:: relaxationSchemeSpatial(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #8 Foam::relaxationSchemes::relaxationScheme::adddict ionaryConstructorToTable<Foam::relaxationSchemes:: relaxationSchemeSpatial>::New(Foam::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #9 Foam::relaxationSchemes::relaxationScheme::New(Foa m::word const&, Foam::fvMesh const&, Foam::Field<Foam::Vector<double> >&, Foam::Field<double>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #10 Foam::relaxationZone::relaxationZone(Foam::fvMesh const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/lib/libwaves2Foam.so" #11 in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/bin/waveFoam" #12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #13 in "/home/ariel/OpenFOAM/ariel-2.3.0/platforms/linux64GccDPOpt/bin/waveFoam" Floating point exception And then it doesn't run from here. I don't understand where the problem would be located or what it applies to. I can send on any other information I'm able, let me know what else I can tell you. Thanks in advance for any advice Ariel

December 10, 2015, 11:18		#14
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Good afternoon, @Ariel: The transportProperties are copied to the correct location at the time of execution of the tutorial. This procedure was needed in order to preserve cross version compatibility of waves2Foam. With respect to the discretisation of the computational domain, then 25 cells per wave length is definitely too little and so might 75 be. The correct answer will rely on your actual problem and I recommend you to perform some testing on your own. Kind regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request. Last edited by wyldckat; August 25, 2018 at 12:13. Reason: removed answers to other posts that were on the main thread

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Tutorial - Heave and Pitch Simulation of Ship hull moving through head sea waves	Cam	FLUENT	6	February 13, 2019 18:12
Cylinder tutorial	robbo	OpenFOAM Running, Solving & CFD	39	June 7, 2018 07:07
[OpenFOAM.org] Compile OF 2.3 on Mac OS X .... the patch	gschaider	OpenFOAM Installation	225	August 25, 2015 19:43
how to apply an sudden displacement or Force of a cylinder with solid solver?	allenfieldin	OpenFOAM Running, Solving & CFD	11	February 15, 2015 20:37
tutorial for solving oscillating cylinder problem	CH	FLUENT	8	April 2, 2014 10:56

October 9, 2015, 10:57		#2
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hallo, I am almost sure that the problem relates to your relaxation zones, so try to use relaxationZoneLayout to see, what goes wrong. Kind regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

October 12, 2015, 08:11		#3
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi Niels, Thanks for getting back to me. Can you give me any advice on how to use the relaxationZoneLayout? Thanks again Ariel EDIT: Sorry realised this was an extremely stupid question right after asking it! I've managed to get it working, I changed the size of the relaxation zone. SECONDARY QUESTION: I have a simulation running but water is only entering from the bottom half of the field (I have a 3D field from -8 < x < 20, -2 < y < 2, -5 < z < 0.5) and the water is only entering for negative y values. I can tell this is happening because if I look at parafoam before running the case, the set up looks correct from one side but from the other there are no waves entering .. Also, when I tried to run the case and then view some results in paraview, paraview shuts down with the error: Code: size 31000 is not equal to the give value of 62000 which also implies that it is only entering half the field. I had a look at the alpha1.org and the alpha.water file and I don't really understand where I went wrong. Am i looking in the wrong place or can you point me to the file that might help me change my inlet field so that the water enters from -2 < y < 2? Thanks in advance! Last edited by arieljeds; October 12, 2015 at 10:52.

November 11, 2015, 08:18		#5
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hi Ariel, Could it be that your gravity vector is still pointing in the y-direction? Kind regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

November 11, 2015, 08:24		#6
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Yes that was exactly it! I didn't even think about that.. Thank you for your quick and helpful reply..

December 2, 2015, 13:10		#8
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi, I have been running some cases using Stokes 1st waves in waves2foam based off of the waveFlume case and the 3DWave cases. I am trying to do two things: 1) Simulate regular waves in a wave tank (would like to attempt irregular and possibly 3D ocean waves too but have not attempted this yet) 2) simulate regular wave flow around a cylinder with viscosity but no turbulence I have set up a case to for the wave tank and run it. First of all, it appears that the relaxation zone is very long because there only seem to be a couple of wavelengths. My domain goes from -5 < x < 150, -10 < y < 10, -5 < z < 2 (z is the vertical direction). The wavelength is L = 30 m (T = 5sec) and the relaxation zone lengths for the inlet and outlet are 1.5*L. Wave height is 0.3 m. Because it looks as though there are only a couple of wavelengths so I was wondering if the outlet relaxation zone is too long? Also, if I run a vector plot (using glyphs), it appears that there is a lot of reflection. I have been trying to read and understand what is affecting this but am getting stuck. Would really appreciate any help. Secondly, I used the probeDefinitions to create some data for the free surface but I'm not sure how to plot this data? Thanks for any help! Please let me know if I can provide you with specific files or anything.

December 7, 2015, 10:40		#10
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hallo Ariel, It does not make sense that you say that there is a lot of reflection, but on the other hand the wave does not travel through the entire domain. Your initial question was very hard to understand, which was the reason that I did not answer. See a guide here to pose "easy to answer" questions: http://www.cfd-online.com/Forums/ope...-get-help.html Kind regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

December 7, 2015, 11:33		#12
ngj Senior Member Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Copenhagen, Denmark Posts: 1,900 Rep Power: 37	Hallo Ariel, My only guesses are that you have either way too few cells per wave length or your specification of the water depth does not match that given by your geometry. Kimd regards, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

December 10, 2015, 08:22		#13
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi Niels, Thanks again for getting back to me. Ok, this did seem to be the problem. I realised I only had a few cells per wavelength so I have increased that to approx. 75 cells per wavelength. Is there a general value of cell per wavelength that should be followed? I am also attempting to run a case with flow over a cylinder using an extension of the same mesh set up from the potentialFoam cylinder tutorial (the entire field is set up instead of just a quarter). As the mesh is slightly more complicated than a simple wave tank, I have only managed to have 25 cells per wavelength at the inlet. I haven't yet run the case to see the effect it has. I have a secondary question in regards to the transportProperties dictionary that is used in each tutorial (I think that the same ones are used in interFoam as well). I noticed that in the github versions of the tutorials, there is no transportProperties file. Why is this file missing in the tutorials?