[thiago vieira]

Greetings, Dr. Chauchat


I'm currently working on my master thesis investigating the effects of hydrokinetic turbines in live river beds.

The idea is to combine sedFoam with turbinesFoam so as to deploy the Actuator Line Method to represent the turbine at a low computational expense.

Unfortunately, I've been struggling with this case for quite a while. The effects of the turbine are not being computed at all throughout the simulations. Although I've imported the resources from turbinesFoam and all the files related to the turbine, I cannot seem the get the fvOptions right.

I don't really know how to include the source terms related to the turbine in order to compute the effect of energy extracted from the turbine to fluid in the near wake.

Are there any restrictions in sedfoam as to the use of fvOptions?
Is it really possible to combine the Actuator Line Method (turbinesFoam) with sedFoam as I'm trying to do?


I'd very much appreciate your response, professor. Thank you in advance!


Kind regards,
Thiago Vieira

[cyss38]

Dear Tiago,


Are you using the latest version of sedFoam?


We have recently added and validated the fvOptions capabilities.


So i think you can test again, and i'm pretty sure it's possible to combine the actuator line with sedfoam.

Cyrille

[julienC]

Dear Tiago,


As Cyrille said we have recently implemented and validated fvOption in sedFOAM so there is no technical problem to do what you want.

You may be interested by reading this article from French colleagues who coupled Actuator disk model and Blade Element Model with sedFoam :

https://doi.org/10.1016/j.ijsrc.2021.02.003


I also encourage you to contribute to sedFoam by sharing your development with the community.


Best regards,
Julien CHAUCHAT

[thiago vieira]

Dear Dr. Chauchat and Cyrille,


Thank you for your response, I'll try and update sedfoam to its latest version and see if it works.
Also, I'll make sure to take a look at the article you recommended and share my progress with the community.


Regards,
Thiago Vieira

[thiago vieira]

Dear Dr. Chauchat and Cyrille,

First of all, thank you for your help. I've updated sedFoam to its latest version, along with OpenFOAM-v2016 and it seems to be working perfectly. The fvOptions for the Actuator Line Method I'm trying to implement was read successfully.

Even though I can see the model being selected in the log file, my simulations are still illegible. The flow simply goes right past the region of the mesh where the turbine was supposed to be. Also, I'm getting empty files (only zeros) for the forces generated by the turbine as output at each time step.

Would you mind providing me with further assistance?

The fvOptions, controlDict and Ub files follow attached.
Below, the Actuator Line Method selection reads as follows in the log file:

Selecting finite volume options type axialFlowTurbineALSource
Source: turbine
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Source: turbine.blade1
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Source: turbine.blade2
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Source: turbine.blade3
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Frontal area of turbine: 0.636173
Source: turbine.hub
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Source: turbine.tower
- selecting cells using cellSet turbine
- selected 6174 cell(s) with volume 0.594442
Courant Number mean: 8.38152 max: 17.3442
Turbulence suspension term is included
Choice for faceMomentum : false

Starting time loop


Thanks in advance!

[divyathokala01@gmail.com]

Hi,
I would like to do a similar apron scour problem for my case. Could you able to do it? Can I know which version of openfoam you have used? ESI or foundation? Which is the latest version you would suggest? I feel I can get some help from older versions because people have experiences? Can someone help me to get clarified in using latest version or old version.

Divya

[cyss38]

we strongly suggest the latest version of openfoam.com (ESI)

[divyathokala01@gmail.com]

Originally Posted by ajusree

Sir,
I have been trying to modify the sedfoam code of scour downstream of an apron tutorial. I wanted to simulate a river flow in 3D with erodible boundaries. So I kept a rectangular box in blockMeshDict and I gave river geometry as my initial condition in funkySetFieldsDict. But the code got terminated after some time even without reaching 1 sec. When I checked the log file, I found an abrupt rise in the values of some of the variables.

Could you please give me some suggestions to correct this?

Can I know the tutorial name please. only one 3D scour problem is there I couldn't see the results properly

[cyss38]

Originally Posted by divyathokala01@gmail.com

Can I know the tutorial name please. only one 3D scour problem is there I couldn't see the results properly

Indeed there is only one 3D tutorial. The case of @ajusree is a custom case i think, and @ajusree is not part of the sedfoam development team. So we don't have access to this simulation.

[jlpang]

Prof. Chauchat


I am a new openfoamer and I am trying to use sedfoam to simulate a realistic scour case. I have changed many boundary conditions and different input parameters, however, the horse shoe vortex didn't show up. With the same boundary condition and input parameters, the horse shoe vortex emerged in the pimpleFoam. Is there anything I need to take into account in a realistic case?



The parameters in the constant folder are copied from tutorials/3DScour.


Best regards,
Jialin

[julienC]

Dear Jialin,


Most likely you used the default advection schemes (div schemes in system/fvSchemes) and temporal scheme (ddt) which are first order in the tutorial. You need to change to second order for both if you want to see the horseshoe vortex developing.



Best regards,
Julien Chauchat

Originally Posted by jlpang

Prof. Chauchat


I am a new openfoamer and I am trying to use sedfoam to simulate a realistic scour case. I have changed many boundary conditions and different input parameters, however, the horse shoe vortex didn't show up. With the same boundary condition and input parameters, the horse shoe vortex emerged in the pimpleFoam. Is there anything I need to take into account in a realistic case?



The parameters in the constant folder are copied from tutorials/3DScour.


Best regards,
Jialin

[jlpang]

Dear sir,
Thank you for the response. I will try to change the schemes and see if it works.


Best regards,
Jiali

[jlpang]

Dear sir,
Thanks again for your useful suggestion, after I changed div schemes and ddt schemes to second order, the horseshoe vortex emerged. But when I check the scour around the cylinder, the alpha_a in paraview barely changed. It is not getting better after I refined the mesh. Could you please give me some suggestions to correct this?
Best regards,
Jialin

[zjy]

Dear Professor：It was a great honor to read your article published on JFM（A finite-size correction model for two-fluid large-eddy simulation of particle-laden boundary layer flow）.And I have some questions to consult with you:

Is the finite-size correction model included in your open-source case（3Dchannel560)？If so, can you tell me in which file to open it，If not, how can I get it？

In the 0 file in 3Dchannel560, flm, alphaPlastic,Theta file appears. Can you explain to me what it represents

Can this code be used to calculate a flow with a high sediment content, such as a sediment volume fraction around 0.2？

[mathiant]

Originally Posted by zjy

Dear Professor：It was a great honor to read your article published on JFM（A finite-size correction model for two-fluid large-eddy simulation of particle-laden boundary layer flow）.And I have some questions to consult with you:

Is the finite-size correction model included in your open-source case（3Dchannel560)？If so, can you tell me in which file to open it，If not, how can I get it？

Thank you for the interest in our publication. The finite-size correction model is not available in the latest sedFoam release but the 3DChannel560 tutorial corresponds to the configuration "GB" investigated in the paper. The source code with the finite-size correction model is available upon request. I can send you a link to download it through private message.

In the 0 file in 3Dchannel560, flm, alphaPlastic,Theta file appears. Can you explain to me what it represents

The flm* and fmm* files correspond to variables used to compute the eddy viscosity in the dynamic Largrangian LES model, alphaPlastic is a field used in the dilatancy model (not used in this configuration) and Theta is the granular temperature in the kinetic theory.

Can this code be used to calculate a flow with a high sediment content, such as a sediment volume fraction around 0.2？

SedFoam can be used to simulate flows with sediment concentration ranging from dense (close to maximum packing fraction) to dilute regimes. However, the finite-size correction model has only been validated for dilute configurations.

Regards,

Antoine MATHIEU

[zjy]

Thank you for your reply, I have sent you a private message, please share the source code with the finite-size correction model with me, you can also send it to me via email 22034146@zju.edu.cn. Thank you again for sharing this highly innovative code

[zjy]

Originally Posted by mathiant

Thank you for the interest in our publication. The finite-size correction model is not available in the latest sedFoam release but the 3DChannel560 tutorial corresponds to the configuration "GB" investigated in the paper. The source code with the finite-size correction model is available upon request. I can send you a link to download it through private message.


The flm* and fmm* files correspond to variables used to compute the eddy viscosity in the dynamic Largrangian LES model, alphaPlastic is a field used in the dilatancy model (not used in this configuration) and Theta is the granular temperature in the kinetic theory.


SedFoam can be used to simulate flows with sediment concentration ranging from dense (close to maximum packing fraction) to dilute regimes. However, the finite-size correction model has only been validated for dilute configurations.

Regards,

Antoine MATHIEU

Dear sir:

Sorry to bother you again, but I don't seem to have received your private message or email. Could you please send it again?

Regards,

yang

[Feras2020]

Prof. Chauchat

Hello, I'm relatively new to the open-form software, and I've been attempting to run the 2DPipelineScour tutorial. However, I encountered an issue where the simulation stopped after only four seconds. When I checked the simulation, I noticed some unusual behaviour at the inlet boundary condition for alpha.a. To resolve this, I switched the inlet boundary condition from a coded fixed value to a zero gradient, allowing me to complete the simulation successfully.

I aim to conduct multiple simulations for this tutorial using different shear rates. The objective is to achieve diverse velocity profiles through these simulations. In the fluid velocity file (0-org/U.b), I adjusted the bottom friction velocity, starting with 0.04318, and then tried both 0.4318 and 0.004318, but found that the simulation remained unchanged from the original with a bottom friction velocity of 0.04318.



Best regards,
Feras Algafary

[eduard.puig.montella]

Hi Feras,


I checked the 2DPipelineScour tutorial and I noticed that both Kinetic theory and mu(I) rheology are on. I turned the kinetic theory off and the case works smoothly without any change at the boundary conditions.

Concerning the friction velocity I made the changes in 0_org/U.a and 0_org/U.b, and the results seem sound (see figures below. For a friction velocity of 0.0043 the bed remains horizontal) . Make sure you change both the fluid and solid frictional velocity.

Eduard


bed_profiles_0.0043.jpg

bed_profiles_0.043.jpg