[jovenitta]

Thanks for your quick reply. I will definitely switch to the latest version of OF.

Originally Posted by Phicau

Hi,

this is normal, please check the changelogs. What happens is that there were too many tutorials for different OpenFOAM versions, so I moved the older ones to another repository and just kept the latest version in the main olaFlow repository. You can get them here:

https://github.com/phicau/olaFlow_oldVersionTutorials

and run them normally.

Please, do also note that it is most often recommended to use recent OpenFOAM versions due to bug fixes. Bug fixes and new developments in olaFlow are back-compatible so far.

Best,

Pablo

[AnnaF]

Hi all,


I am using the baseWaveFlume tutorial (OF 5) and am trying to include two internal patches (planar surfaces) to calculate the forces/pressure on. To create the internal patches I am using topoSet -> setsToZones -> createBaffles. My runCase file looks like this:

#!/bin/bash

mkdir 0

echo blockMesh meshing...
blockMesh > blockMesh.log

echo Create internal sets and zones for patches ...
topoSet -dict system/topoSetDict.plateFront
topoSet -dict system/topoSetDict.plateBack
setsToZones -noFlipMap # createBaffles takes zones as input

echo Creating patches for force calculation ...
createBaffles -dict system/createBafflesDict -overwrite #zones as input
##createPatches -dict system/createPatchDict -overwrite #sets as input

echo Preparing 0 folder...
rm -fr 0
cp -r 0.org 0

echo Setting the fields...
setFields > setFields.log

echo Running...
olaFlow > olaFlow.log
#interFoam > interFoam.log

echo Simulation complete.

The createBafflesDict:

internalFacesOnly false; //true; //neither works

baffles
{
plateFrontBaffle
{
type faceZone;
zoneName plateFront;
flip false;

patches
{
master
{
name plateFrontPatch;
type empty;
}
slave
{
${..master}
}
}
}
plateBackBaffle
{
type faceZone;
zoneName plateBack;
flip false;

patches
{
master
{
name plateBackPatch;
type empty;
}
slave
{
${..master}
}
}
}

}

The patches seem to be set up correctly (when I view them with paraView), the simulation runs and finishes. However, the "createBaffles" command messes up the wave generation at the inlet somehow.

I have also tried using createPatch instead of createBaffles - with sets as input; t run it with interFoam and the wave libraries only; internalFacesOnly true/false in the createBafflesDict; when I remove the createBaffles/createPatches command, everything works as usual...

I am not really sure if this is a general OF question, but I was wondering if it might has to do with the wave generation/absorption libraries?

It would be great to get some hints. Thanks.



With kind regards,
Anna

[Phicau]

Hi Anna,

I cannot reproduce this with your information, please send me the case either here or by direct message and I will take a look.

Best,

Pablo

[AnnaF]

Hi Pablo,


thanks for your quick reply.
Please find the case attached.


Regards,
Anna

[Phicau]

Hi Anna,

the problem was setting the baffles to type 'empty', they should be a wall. Also, when they are walls you need to define the BCs in the 0.org folder files.

Find the working case attached. It is a little bit boring now, though, just a standing wave on the left part and still water elsewhere. I guess that you plan not to extend the baffles down to the bottom as a next step.

Best,

Pablo

[AnnaF]

Hi Pablo,

I realized I should have given a more thorough explanation, sorry for that.
Actually, I wanted to have the patches "empty" to just use them to calculate the forces on an internal area (no wall) - in order to evaluate the pressure loss through a porous area in future cases.

Still, your hints pointed me into the right direction and I realized that my baffle setup was wrong and that I need a "cyclic" baffle type. And obviously this has nothing to do with olaFlow...

My case with the cyclic baffle is attached, if anybody else comes across this...

Thanks a lot for your help though, very much appreciated!
Anna

[M.W.G.]

Hi Pablo,

I can see in the manual that the correction velocity Uc is found as follows:
Uc = - sqrt(g/h) * ( eta_measured - eta_target )

Could you kindly let me know what is meant by the targeted elevation (eta_target) ??

To my knowledge, dealing with a pure absorbing wall, the velocity profile should be:
Uc = - sqrt(g/h) * ( eta_measured )

Thanks...

M.W.G

[Phicau]

Hi M.W.G,

you are right in a pure absorption boundary eta_target = 0, meaning that your target is to have no wave, just a fixed water level.

Eta is defined as the free surface elevation and the reference is the still water level, so if you are using active wave absorption at a boundary in which you are also generating waves, eta_target will be your target free surface elevation given by the chosen wave generation theory.

Just a small remark, wave absorption is soon changing in olaFlow, as I will be releasing a new version that works much better and in all relative water depths. You can check the details here: https://sites.google.com/view/olaflo...nts-in-olaflow

Best,

Pablo

[arashghgood]

Dear Pablo
in case of basewaveFlume, I want to have 2 salitory waves moving in the opposite direction. for this, I define a new waveDict file with absdir 180 and wavedir 180 and set the outlet with this file.
unfortunately, it doesn't work. I mean that after running, there is just one wave in one direction in parafoam
could you help me

[Phicau]

Hi Arash,

you have forgotten to change the outlet BC for U. I have decided to include this case in the olaFlow tutorials. You can find a working version here: https://github.com/phicau/olaFlow/tr...olitariesFlume

Best,

Pablo

[ConstanceC]

Hi Pablo,

First of all, thanks a lot for your work and your dedicated help for the users of olaFlow. I am curently simulting Stokes II waves (T=1,265s, H=0.025m, h=2.5m) in order to after work on fluid-structure. When I plot the elevation along time (simulation ran for 150s) at the center of the basin, I observe a non stabilized signal with a kind of temporal reflection. Also, when I plot the mean amplitude along the numerical wave tank, I get a sinusoidale variation of the mean amplitude instead of a constant one. This underlines the spatial reflection happening along the NWT.

I understood reading your PHD thesis that absorption is implemented for shallow waters and that "performance decreases as you move away from the initial assumption of shallow water". Have you any ideas/papers to be able to model Stokes II waves with high depth and improve their absorption ?

Thanks,

Constance

[Phicau]

Hi Constance,

Thanks! You are right, the present absorption model is developed for shallow waters, but I have just developed a general active wave absorption framework that works well in all water depths, take a look at https://sites.google.com/view/olaflo...nts-in-olaflow

Although I will be releasing this soon, feel free to contact me and we can discuss arrangements for a pre-release test for you. You can find my e-mail at the website in the contact tab.

Best,

Pablo

[arashghgood]

In case of baseWaveFlume example (or other OF project), How can I
1) plot surface elevation
2) get numerical data and calculate some physical quantities
3) track particular point of the wave

[arashghgood]

Dear Pablo
Is it possible to change the discretization scheme in OlaFlow? or load a given scheme?

[arashghgood]

Dear Pablo
In case of basicwaveflume example, I design a box with 0.7 m in height and use stock I as a wave type. It works well. After increasing the size of the box to 1.7 m in height, it seems that the wave hit the top boundary at 0.7 m as shown in attachment
could help me to correct it.

[Phicau]

Hi Arash,

to plot free surface elevation please check the breakwater tutorial, you have an example on how to set gauges, process the data and plot them.
You can get data either from sampling functions or from paraview.

I don't understand your last question, I suggest that you read this post and come back with more information: How to give enough info to get help

Best,

Pablo

[arashghgood]

Dear Pablo
in the case of the baseWaveFlume example, I set the wave height to 0.4. when I set the water height in SetField to 0.5 an error happened. when it is greater than 0.6 everything run well.

------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      waveDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

waveType        regular;

waveTheory      cnoidal;

genAbs          0;

absDir          0.0;

nPaddles        1;

waveHeight      0.4;

wavePeriod      1;

waveDir         0.0;

wavePhase       1.57079633;

and

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue alpha.water 0
);

regions
(
    boxToCell
    {
        box (-10 -1 -1) (30 1 0.5);

        fieldValues
        (
            volScalarFieldValue alpha.water 1
        );
    }
);

[Phicau]

Hi Arash,

this is completely normal, the breaking limit is H/h = 0.8 and you are at that point. The cnoidal wave implemented in olaFlow is first order and fails to converge at that large H/h. In the future I may implement some kind of controlled exit and warning to the user when no convergence is obtained.

You may need to use a (very) high order stream function wave to simulate such conditions.

Best,

Pablo

[mleary29]

Hello,

I hope you doing well. I am messaging about the floating object tutorial, for which I can't seem to get a working model. I keep getting floating point errors, and don't know what exactly it is for all I altered was blockmeshdict, 0 folder, fvschemes, and fvsolution to match that of olaFlow.

Thus, I am wondering if anyone has a working floating object tutorial they'd be willing to share. I know this has been asked before, but I do think it will clear up some of the confusion on the exact differences between the interDyMFoam tutorial and this one.

Thanks for the help.

[Phicau]

Hello,

I have modified the floatingObject tutorial in OpenFOAM 5 to make it work with olaFlow. I needed to change the dimensions because with the original values the mesh became very distorted and cells were squeezed beyond limits, so the case blew up.

Mind you, this is a very simple case. Getting a more complex geometry working might prove a real challenge. Maybe the situation has improved now, but I remember reading reports long time ago stating that the 6DoF tutorial was known to fail even for very small changes in the dimensions of the floating box.

Best,

Pablo