Strange behaviour of the water flume

Dear forum

I am currently modeling on a water flume. But the calculation shows a strange behaviour. To get to the reason for this, I built a physical 1:6 model and simulated the "numerical experiment". I know my physical model is not perfect, because of the friction an it's also not totally horizontal... But for me I thought it would be good to see if the two model gave me results in the same direction.

In the physical model the flume is filled over the whole width. In the numerical model everything comes together in the middle!?

Does anyone have an idea where the error in my case definition could be?

Many thanks in advance

Raphael


Comments

  • Hi,

    That seems like a viscosity problem.

    I've seen that you are using artificial viscosity with values (0.000001 and 0 for bound). Those values are very strange in my experience. They need to be calibrated.

    Have you tried more conventional values like (0.1 for both ?)

    Regards,

  • Could you also try using the SPS-LES model instead?

    Could be quite interesting to see if it produces better results while being stable.

    If you stick with artificial viscosity, you would probably have to tune alpha a bit. 0.01 is usual SUGGESTED (but not necesarily correct!) for wave tanks.

    Kind regards

  • @TPouzol Now I make a new calculation with 0.1 for both. I hope this will fix the problem.

    @Asalih3d I tried SPS-LES with the values  (0.000001 and 0 for bound). For this I get the same results. May I try SPS - LES with 0.1 for both?

    Is there a formula to get a proper value for artificial viscosity or do I have to choose it by try and error?

    Kind regards

  • In SPS-LES the viscosity value should be set to the actual physical viscosity.

    For artificial viscosity I asked the question you posted yesterday: https://forums.dual.sphysics.org/discussion/1897/can-artificial-viscosity-model-real-viscosity#latest

    Please read the post, it might help you.

    Perhaps a next step would be to test with multi-phase simulation?

    Generally looking at your picture I feel that the simulation catches the physics roughly. It widens at top and converges at the end. Perhaps increasing particle count will help even more. Another suggestion would be adding a very thin layer of fluid particles on the slope before you open for the lid in your simulation.

    Kind regards

  • Another thing, You are using a dp=0.01 and don't use the mDBC. Have taken in consideration the gap that is formed around boundaries ( https://dual.sphysics.org/index.php/faq/#Q_13 ) If not, that means there is a gap around boundaries of approx 0.026m, And thus the opening of the box is smaller than you think.

    Please keep us informed of your results

    Regards

  • Thanks for the hints.

    I will try several modifications an post the results here.

    Probably this will take a while ...

    Regards

  • edited November 7

    I have now done some experiments with different parameter configurations. Especially the value for the parameter "visco" has a big influence. If you change the parameter "viscoboundfactor" the collision of the lateral waves shifts downwards (see blue arrows in the attached PDF). With SPS - LES I made only two passes. The viscosity of water should be 10^-6 m2/s. Probably there would be better results, the bigger the parameter "viscoboundfactor" is chosen !? Unfortunately I could not make more tests due to time constraints. 

    All in all, the result with visco = 0.01 and viscoboundfactor = 1.0 looks almost like the physical experiment. dp is still 0.01 Meters.

    Regarding mDBC: For the flume this would have been an option.

    But the goal of my work is to use a real terrain as STL. When I look at the mDBC tutorial and examples, I don't find any hints how to do this with such geometries. But overall the gap is relatively small (especially in a real terrain).

    Thanks again for the hints and the help! Without them I probably would have looked for the error for weeks.


    Regards

    Raphael


  • edited November 8

    Thanks! happy that you could make it work!

    There is not much difference between the three values for boundaries and that seems right since the flow if very turbulent and as such rugosity of the boundaries don't play a huge role.

    Regards

  • Dear Raphael,

    choosing the right value of alpha led to results very similar to the experimental ones. In the other cases, your flow was too viscous or too noisy.

    I see that the viscobound factor does not play a significant role when the proper alpha value is chosen. Thanks for your interesting application!

    Regards

    Corrado

  • edited November 29

    @raphael_zueger

    Late addition. As long as you play with artificial viscosity recall that

    simulated kinematic viscosity ~ artificial viscosity x artificial speed of sound x smoothing length

    (see https://en.wikipedia.org/wiki/Smoothed-particlehydrodynamics#Viscosity_modelling for the formulation). Of course this simulated kinematic viscosity will not be close to the material kinematic viscosity. Too much of artificial stuff at play. As order of magnitudes 0.01 x 10 x 0.001 is already hundredfold larger than the material kinematic viscosity of water.

    However, that tells us the direction things change across different settings. So each time you touch a quantity at the right hand side, you are going to see an effect looking like a change of viscosity. For example, if you halve the particle spacing, you halve the smoothing length, and the simulated flow will behave half as viscous. So there is more than just that artificial viscosity alone that determines viscous-looking outcomes.

    Thanks for sharing and illustrating your work.

Sign In or Register to comment.