[Phicau]

Hi again,
No, I don't believe so. waveAbsorption2DVelocity will certainly reflect more and create more evident partial standing waves, not wave damping.
Using extendedRangeAWA is always preferred in deep water conditions.

Pablo

[erickmartinez]

Hi Dr. Higuera,

I wanted to ask how you achieved only the visualization of the wave surface on the following video on the olaFlow channel: https://www.youtube.com/watch?v=9_SerPY_Mn4
I am trying to achieve something similar for visualization of my simulations but I am not sure how you can only get the surface of the water being visible.

On another hand, I am trying to use olaFlow and I am having some issues with convergence. Do you have any recommendation in terms of an LES model that works well with multiphase or any solver configurations that could help? I would greatly appreciate your input in both matters.

Let me know when you can, thanks!

[Phicau]

Hi Erick,
The free surface is the isosurface of alpha = 0.5, so you just need to set a contour with that parameter to make it visible.

I have limited experience with LES and have never experienced any issues when using it before. I would recommend you to copy the settings from an existing OpenFOAM tutorial and work from there.

Best,
Pablo

[4lix]

Hi Pablo,

First, I want to thank you a lot for your advices and taking time to look at my case. Indeed, the problem was the numerical schemes. I used the fvSchemes file from tutorial and it worked better (no more damping).

But, as you explained, I am now facing reflection problems since we are in deep water conditions and using waveAbsorption2DVelocity.

I am using the master version of olaflow with OF-v2006 and I tried to integrate the extendedRangeAWA theory from dev olaflow.

I met and tried to solve several problems :

1. in genAbs/waveAbsorption/waveAbsorptionVelocity/waveAbsoptionVelocityFvPatchVectorField.C => I changed the arguments of the function subOrEmptyDict line 97 because in OF-v2006 this function now takes 3 arguments instead of 2 in older OF version.

2. in genAbs/waveAbsorption/activeWaveAbsorptionModels/newMemberFun.H => I added the line " Info << "cf " << cf << endl; " under the line 27. Indeed if I don't put this line, it compiles well but when I try to launch the baseWaveFlumeNewAbs tutorial I have this error "*** Error in `olaFlow': munmap_chunk(): invalid pointer: 0x0000000002964b20 ***" [...]. However, with the added line it's working perfectly with the tutorial and my case (no more reflection).

So I wanted to ask you if you already met this kind of problem (2.)? I am not an expert in openfoam developpement and C++ but it seems there is a memory problem. Will you one day integrate the extendedRangeAWA theory to the olaflow master version as I tried ?

Thank you in advance for your help!

Best regards,
Alix

[paulathikalam]

Sorry for crossposting, I had posted this message in the [OLAFLOW] The OLAFOAM Thread without knowing that this is the current active thread for OLAFLOW.

Hii all,

Could you help me out to fix this error.

I am trying to run the tutorial case of baseWaveFlumeNewAbs. I am running it in OpenFoam6. I have not modified anything in the tutorial case, just started the case by executing the runCase script.

The script runs fine till setfields, but when olaflow is executed it pops up an error, i think - related to active wave absoprtion
-----
Active wave absorption BC on patch outlet
"Initial water depths for absorption" 1( 0.4 )

Selecting active wave absorption model extendedRangeAWA
AWA model: patch outlet
Theory: extendedRangeAWA
Number of paddles: 1
Reference water depth: 1(0.4)
Wave period: 3
Updating extendedRangeAWA absorption model for patch outlet
----
full olaflow logfile is also attached.

Is this something to do with the OF version that i am using to run ? or is there something that i should edit ?

Thanks

Paul

[Phicau]

Hi Alix,
I have just solved this issue and check that the case is working for OF-v2012. Download the latest version of the code, and recompile.
The integration will happen in the next major release, but at this stage I cannot offer a tentative date on when it will happen.

Hi Paul,
Which kind of error? I see no errors in the log you sent, did the case get stuck? Anyway, I have tried running the tutorial in OF-6 with the new version and everything works well, so download the latest version of the code, and recompile.

Best,
Pablo

[Stan Zhou]

Originally Posted by Phicau

Hi Stan,
The error is that the outlet patch is dry, which means that the initial water depth for AWA is 0 and the solver ends up dividing by 0 and crashing.

Hi Pablo,

Thanks for your reply. I find that there is a difference between the 2D and 3D wave absorption BCs. As for a 2D case in which a rigid structure higher than water level was close to 'outlet' BC (the outlet patch is dry), when I adopt 2D wave absorption BC, the simulation worked well. However, for a 3D case under a similar situation, the solver crashed. Could you please explain what leads to this phenomenon?

By the way, could you please give some hints on the parameters used in 2D and 3D wave absorption BCs?
For example, as to 'waveAbsorption2DVelocity', there is a parameter 'absorptionDir 666.0' in tutorial case breakwater but there is no such parameter in case 'baseWaveFlume'. Under what circumstances should we add the parameter 'absorption' and how to set its value?
Additionally, in the 3D tutorial case 'irreg45degTank', what are the principles to set values for 'nPaddles' and 'nEdge' ? For example, as for 'front' and 'back' AWA BCs, the value of 'nEdgeMin' is 0 but for the 'outlet' BC, 'nEdgeMin' is 1 in case 'irreg45degTank'.

Thanks in advance!

Sincerely,
Stan

[paulathikalam]

Originally Posted by Phicau

Hi Alix,
I have just solved this issue and check that the case is working for OF-v2012. Download the latest version of the code, and recompile.
The integration will happen in the next major release, but at this stage I cannot offer a tentative date on when it will happen.

Hi Paul,
Which kind of error? I see no errors in the log you sent, did the case get stuck? Anyway, I have tried running the tutorial in OF-6 with the new version and everything works well, so download the latest version of the code, and recompile.

Best,
Pablo

Thanks for the reply Pablo

Yes, the case got stuck there.

I thought the issue was something related to my OF version, so i removed my older OF6 version and tried with OF7 today. Unfortunately, the dev version of the olaflow fails to compile with OF7.

-----------------
\n\nOlaFlow project wave generation boundary conditions compilation failed
------------------ full log file is attached (dev_log.txt)

but the master version of the olaflow compiles with OF7(master_log.txt)

any idea on how to proceed ? should i revert back to OF6 and see if that works ?


Paul

[Phicau]

Hi Stan,
An absorbing boundary should not be dry initially by definition because AWA needs the water depth to operate.
All of your questions are covered in the PDF document included in the reference materials.

Hi Paul,
Yes, the BCs are not compatible with OF7 yet. If you go back to OF6 they work perfectly, as I reported before.

Best,
Pablo

[paulathikalam]

Originally Posted by Phicau

Hi Stan,
An absorbing boundary should not be dry initially by definition because AWA needs the water depth to operate.
All of your questions are covered in the PDF document included in the reference materials.

Hi Paul,
Yes, the BCs are not compatible with OF7 yet. If you go back to OF6 they work perfectly, as I reported before.

Best,
Pablo

Hi Pablo,


I reverted back to OF6. The dev version of OlaFlow now compiles successfully.


But when i run the tutorial case, baseWaveFlumeNewAbs. It pops up an error and the run stop.


-----------
Running...
munmap_chunk(): invalid pointer
./runCase: line 16: 165208 Aborted (core dumped) olaFlow > olaFlow.log
Simulation complete.
------------- full logfile of blockmesh, sefields and olaflow arre attached.


Thanks


Paul

[Phicau]

Hi Paul,
Have you downloaded the latest version? Note that I pushed some changes 4 days ago. If not, go ahead, download it and compile again.
If this still does not work, it would probably be a good idea to re-compile OpenFOAM and try again.

I have just reconfirmed that everything works perfectly on my computer.

Best,
Pablo

[paulathikalam]

Originally Posted by Phicau

Hi Paul,
Have you downloaded the latest version? Note that I pushed some changes 4 days ago. If not, go ahead, download it and compile again.
If this still does not work, it would probably be a good idea to re-compile OpenFOAM and try again.

I have just reconfirmed that everything works perfectly on my computer.

Best,
Pablo

Hi Pablo,

The problem was with OF6 compilation as you suggested, i corrected everything. Now, olaflow compiles and i am able to run the baseWaveFlumeNewAbs tutorial.

Thanks for the help.

Paul

[victor13165]

Originally Posted by Phicau

Hi again Pibil1,

I have created the olaIsoFlow solver and prepared a tutorial. They can be accessed at:

https://github.com/phicau/olaFlow_supplementary

As I mentioned, olaFlow boundary conditions are fully compatible with isoAdvector scheme.

Best,

Pablo

Hello Pablo,


I think we can all agree that all the tools you created on OpenFOAM for coastal engineering and hydrodynamics are life savers. In my case the porous media flow based on VARANS equations were very useful.


Anyway, I am trying to compile olaFlow_supplementary (olaIsoFlow) for OFv2006, and I have encountered a few problems that I would like to share with the community, hoping that we can solve them together. I have opened an issue on the olaFlow_supplementary GitHub repo (https://github.com/phicau/olaFlow_su...ntary/issues/1) but I don't think it is appropriate/the right place to do that.


Here is an overview of what I managed to solve so far:


Step 1. Change the olaIsoFlow/solver_OFv17xx/Make/options file and add the following lines (in bold):

XE_INC = \
    -I$(LIB_SRC)/transportModels/twoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/transportModels \
    -I$(LIB_SRC)/transportModels/geometricVoF/lnInclude \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/interfaceProperties/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/incompressible/lnInclude \
    -I$(LIB_SRC)/transportModels/immiscibleIncompressibleTwoPhaseMixture/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude \
    -I$(LIB_SRC)/meshTools/lnInclude \
    -I$(LIB_SRC)/sampling/lnInclude \
    -I$(LIB_SRC)/surfMesh/lnInclude

So that the "isoAdvection.H" is properly imported in olaIsoFlow.C. I can't remember why I added the last line but it was so that all header files could be included propery.

Step 2. In "alphaEqn.H", change:

advector.advect();

to:

#include "alphaSuSp.H"
 advector.advect(Sp, Su);

And copy the file "alphaSuSp.H" from $FOAM_APP/solvers/multiphase/interFoam/alphaSuSp.H to the olaIsoFlow/solver_OFv17xx directory. From memory I think alphaSuSp.H is also in olaFlow/solvers/olaFlowOFv19xx-20xx if one would like to copy it from there.

Step 3. This is the one I'm stuck on. Basically, I get a bunch of messages like:

Make/linux64GccDPInt32Opt/olaIsoFlow.o : In function « void Foam::isoAdvection::limitFluxes<Foam::zeroField, Foam::zeroField>(Foam::zeroField const&, Foam::zeroField const&) » :
olaIsoFlow.C: undefined reference to « Foam::isoAdvection::debug »

or even (and this is the first error message in the list)

Make/linux64GccDPInt32Opt/olaIsoFlow.o : In function « Foam::isoAdvection::type() const » :
 olaIsoFlow.C: undefined reference to « Foam::isoAdvection::typeName »

I have attached the full error message in a log file, if somebody is brave enough to read it.

I have read that the "undefined reference" message can appear for several reasons, such as bad object files linking, or that certain functions aren't explicitly defined (i.e. only have prototypes).

Does anyone have any suggestions on what I can try? Also, is it more likely that this problem arises from my own OpenFOAM installation/environment or simply because olaIsoFlow for v17xx is too old?

Thanks in advance for any help, guidance or advice.

Cheers,
Victor

error_message_log.txt

PS: I don't really know which files to attach to give more info. Please let me know what you need and I will make sure to include them. The olaIsoFlow files can be viewed on GitHub at https://github.com/phicau/olaFlow_su...solver_OFv17xx

[erickmartinez]

Good morning,

Is olaFlow compatible yet with OpenFOAM 2106? Let me know at your convenience in case an update is yet to be released and if you have any idea of when it would be available! Thanks

[Phicau]

Hi Victor,
That code was produced long time ago. In the meantime, isoAdvector has been integrated into the OpenFOAM.com version, and it should be easier to start from there. Right now I have limited spare time, so I cannot offer a time frame in which I will be able to look at it.

Hi Erick,
I believe so, I believe that the latest release has not made any changes in the VOF solvers and the solver compiles automatically. If you find any compatibility issues just let me know.

Best,
Pablo

[yannaixiao]

Dear all,
I have established a three-dimensional model to simulate the impact of waves on structures. From the results, I found that there seems to be some problems in the wave height time history curve. The wave height monitoring points in the figure below are near the wave making boundary. It can be seen that serious wave attenuation has occurred since the second cycle.(The wave height time history curve is shown in the figure uploaded below)I don't know what the reason is.
Here is some information about the model:
1.The wave making model adopts the regular wave stokes Ⅲ, with a wave height of 10 meters, a period of 12 seconds and a wavelength of about 200 meters.More detailed wave setting information is in the waveDict below.
2.The whole calculation domain is 730m long, 4.8m wide, 65.8m high and 55m deep. The structure in the model is 450 meters away from the wave making boundary. The structure is 50 meters high, 4.4 meters wide and 270 meters long. The structure is in the middle of the calculation domain in the Y direction, and the surface is irregular.
3.As for the boundary conditions, the left side of the model is the wave making boundary, the front, rear and right sides are the wave absorption boundary, and the bottom and structure are the wall boundary. The following U file has detailed boundary condition settings.

[Phicau]

Hi,
The wave dissipation issues has been treated several times in this thread and in The OLAFOAM Thread , please look for the relevant posts to get some ideas on how to fix it.

As a recap, wave dissipation is usually caused by: the choice of numerical schemes, inadequate mesh, turbulence buildup (see https://olaflow.github.io/blog/turbu...ons-revisited/ )

A quick tip: always start in 2D before moving into 3D, and only do so when the case is working.

Best,
Pablo

[philiplu]

Hello, Phicau and OLAers,
great, if you can help me:

for irregular waves
- in OLA, there's an easy way to verify wave field? (never doubt OLA, but for regular waves, WS i.e. eta of OLA can be compared with theoretical solution, how irregular waves?)
- in OLA, how to estimate the reflection coefficient, if waves are breaking/broken due to sloping?

thank you in advance
Philip

[GrivalszkiP]

Hi!
In my olaFlow simulation I would like to produce water surface - time diagrams in pre-defined coordinates. For example in a known X and Y, what is the depth of water in every time.
If I use the "Paraview method" (plot over line, integrate variables, plot selection over time) it works, but only if I apply really coarse mesh. However, I would like to do a mesh sensitivity analysis, and If I refine my mesh - in this case Paraview can't handle the task within a reasonable runtime.

Is there a simple method to write the depth in pre-defined coordinates over time under olaFlow simulation run?

Thank you in advance!

Peter

[Phicau]

Hi Philip,
Close to the wavemaker you can compare against the theoretical solution too. Elsewhere you are better off comparing the spectrum instead.

Hi Peter,
The breakwater tutorial includes all the files that you need to set and process the free surface elevation gauges. The results can be generated at runtime.

Best,
Pablo