[Phicau]

Hi Chen,

olaFlow is written and tested to work in parallel, if you experience any differences in the unmodified version, please report it, as it would most probably be a bug. However, I have never experience such.

Probably there are some glitches in your new implementation that might need to be programmed to be parallel-aware.

Best,

Pablo

[Phicau]

Dear all,

I have just released a library that provides modified versions of k-ε and k-ω SST turbulence models to simulate correctly multiphase systems and mitigate turbulence build-up effect.

You can find all the information in the release post: https://sites.google.com/view/olaflo...ve-simulations

I hope that you find it useful.

Best,

Pablo

[lin]

Originally Posted by Phicau

Dear all,

I have just released a library that provides modified versions of k-ε and k-ω SST turbulence models to simulate correctly multiphase systems and mitigate turbulence build-up effect.

You can find all the information in the release post: https://sites.google.com/view/olaflo...ve-simulations

I hope that you find it useful.

Best,

Pablo

Thanks Phicau for your releasing this contribution. Can you give some explanation how your new implementation of turbulence model mitigate turbulence build-up effect?

[Phicau]

Hi Hua Zen,

Check this reference out:

Application of a buoyancy-modified k-ω SST turbulence model to simulate wave run-up around a monopile subjected to regular waves using OpenFOAM
Brecht Devolder, Pieter Rauwoens & Peter Troch
Coastal Engineering (2017), vol. 125, pp. 81–94
https://doi.org/10.1016/j.coastaleng.2017.04.004

Best,

Pablo

[lin]

Hi Phicau, I've read the paper by Devolder et al. (2017), in which an additional buoyancy term is used to suppress the spurious turbulence generation at the interface. From your blog, two additional turbulence models are implemented(kEpsilonMultiphase, kOmegaSSTMultiphase), what is the difference between these two implementation and that of Devolder et al. (2017)?

[Phicau]

Hi Hua Zen,

the problem in OpenFOAM is that incompressible turbulence models are not prepared for multiphase flows. They assume a constant rho, since under the incompressibility assumption, it will go out of the differential operators. In incompressible multiphase flows, the density of each phase is constant, but the density of the system changes throughout the domain depending on the VOF function value in each cell.

kEpsilonMultiphase and kOmegaSSTMultiphase implementations are exactly the same as provided by OpenFOAM, but the density (rho) has been modified so that the one provided by the multiphase solver (e.g. olaFlow) is used.

Best,

Pablo

[Phicau]

Dear all,

olaFlow is now compatible with OpenFOAM-dev.

I have made some changes in the compilation scripts and added the olaFlow solver. Please note that olaFlow and olaDyMFlow have been merged in the dev version, so olaFlow can handle moving meshes too.

As usual, the latest version is in: https://github.com/phicau/olaFlow

Best,

Pablo

[Aref.shri]

Dear Pablo,
Hi
I am wondering if it is possible to change the waveTheory in the wavemakerFlume tutorial (since it doesn't have any waveDicts)? If yes, how?

[Phicau]

Hi Aref,

the waveDict is generated by the runCase script, in which the linear wave motion of the wavemaker (piston and flap) is programmed. Once you have run the case you can edit the waveDict file as you desire, but runCase only provides the linear wave theory transfer functions.

Best,

Pablo

[Aref.shri]

Hi Pablo,
you mean the waveDict file can be edited while running the case?
thanks for your reply.

[Phicau]

Hi Aref,

no, what I mean is that the waveDict file is generated by the runCase script. Once it has been created you can modify it as you wish and use it in any case. However, the file is only read by olaFlow during the initial time step, therefore, any modifications that you make while the case is running will not have any effects on the simulation that is running.

Best,

Pablo

[Aref.shri]

thanks again Pablo,
it was really helpful.

[dneves]

Hi Pablo, how do I properly reference olaFlow?

I enhance your novelties regarding the turbulence models.

Beste Regards,

Diogo

[Phicau]

Hi Diogo,

it might be too hidden in the website:

https://sites.google.com/view/olaflo...del/references

"If you want to reference the model in your publications it should be called olaFlow, and include any of the following references when citing implementation, validation and applications."

We have used the following example in a recent paper, also adding the GitHub address ( https://github.com/phicau/olaFlow ): The CFD model used in this work is olaFlow (Higuera et al., 2013a,b), developed within the OpenFOAM framework.

We wanted to cite the wave generation and absorption capabilities plus the validation (Higuera et al., 2013a,b), but feel free to change the references. For example, if you would like to cite the porous model and applications it would be (Higuera et al., 2014a,b) or my thesis. For the moving-boundary wavemaker (Higuera et al., 2015)... I think you get the idea.

Don't forget to give credit to Devolder et al. papers for that turbulence models!

Best,

Pablo

[VLima]

Dear all,

I am new to OF and now testing the wavemakerFlume tutorial case, for a piston wavemaker, with olaFlow.

I was wondering if :

1) it is possible (and how) to generate just only one single wave with the piston wavemaker , and not several continuous equal waves, and how to check the profile of the wave generated at some point along the channel;

2) in the case I am running, I got the error:

--> FOAM FATAL ERROR:
The time series is not long enough.

and was wondering why could this be happening. I just changed the wave height and water depth values.

I would appreciate very much any help you could provide with this.

Thank you.

[Phicau]

Hi Vania,

Yes, it is possible, you just need to edit wavemakerMovement.txt so that the wavemaker moves as you wish: one wave and then keep the position.

You can sample free surface elevation, just check how it is done in the breakwater tutorial.

That error indicates that the time series of movement that you provided is no long enough, your simulation time is longer. Select a shorter simulation time or give a longer time series.

Best,

Pablo

[VLima]

Hello Pablo.

Thank you so much for your clarifications.

I did not manage to check the plots for the breakwater case study yet. When running the case (SST and KEpsilon) I come across some errors in the Python scripts, namely concerning names and paths for files/folders I assume:

bash runCaseKEpsilon
blockMesh meshing...
snappyHexMesh meshing...
Preparing 0 folder...
Setting the fields...
Running...
Simulation complete
runCaseKEpsilon: line 44: [: OF_FLAVOUR: integer expression expected
Sampling free surface...
runCaseKEpsilon: line 59: postProcess: command not found
Sampling pressure...
runCaseKEpsilon: line 62: postProcess: command not found
Processing and plotting variables
Traceback (most recent call last):
File "postSensVOF.py", line 21, in <module>
a = os.listdir('./'+postPath)
OSError: [Errno 2] No such file or directory: './postProcessing/sampleDictVOF'
Traceback (most recent call last):
File "postSensPres.py", line 21, in <module>
a = os.listdir('./'+postPath)
OSError: [Errno 2] No such file or directory: './postProcessing/sampleDictPres'


The files sampleDictVOF and sampleDictPres are in the system folder. I tried to change the path but it does not work either.

The errors are common to both SST and KEpsilon. Is anything missing in my installation? Also, is line 44 error relevant for this?

Any suggestions to overcome this are very welcome.

Thank you very much in advance.

[Phicau]

You found a glitch in the code that select the postprocessing tool for your version of OpenFOAM. I should be able to fix it quite easily. Which version are you using?

Please report what the terminal outputs for the following command: echo $WM_PROJECT_VERSION

Pablo

[VLima]

The command "echo $WM_PROJECT_VERSION" outputs "v1606+".

[Phicau]

Hi Vania,

all solved, there was a $ missing in line 44 of the script. All is working now.

You can update the repository to the latest version following the update guide in https://sites.google.com/view/olaflowcfd/source-code

Best,

Pablo