July 25, 2018 at 9:24 pmsolovievSubscriber
I am working with the wave boundary condition to simulate an internal ocean wave between two layers of seawater with different densities. The velocities produced by Fluent appear to be somewhat different than the theory for these types of waves. In Fluent, the amplitude of the u and w velocities are a bit higher than in the theory. Most notably, in the theory, there is a discontinuity in the u velocity at the location of the internal wave that is not produced by the wave boundary condition. According to Walter Munk (1981) “the vertical displacement has a peak at the transition, and the horizontal velocity changes sign, forming a discontinuity (vortex sheet)" at the location of the internal wave. I have also attached the contour plot showing this issue for the u velocity. Is this something that is missing in Fluent? Or is there a setting that I may be missing?
My current settings for multiphase are VOF – 2 phase, implicit volume fraction, open channel flow and open channel wave BC both checked, implicit body force checked. For the inlet mulitphase, open channel wave BC checked, shallow/intermediate waves, free surface and bottom levels properly set, averaged flow direction, wave theories, 1 wave, 5th order Stokes, and proper height and length. For the outlet multiphase, open channel checked, pressure specification from neighboring cell, and bottom level properly set. I initialize from the inlet and choose Wavy surface.
July 26, 2018 at 10:47 amRobAnsys Employee
The VOF model and waves are designed for phases that don't (and can't mix), and this combination is typically used for water waves with the Airy or Stokes theory. I'm not familiar with Munk's work so can't comment on the reference.
However, for the mixing of two water layers I think you're looking at the Kelvin-Helmholtz effect, https://www.metoffice.gov.uk/learning/learn-about-the-weather/clouds/kelvin-helmholtz shows a nice visual. I'd use species for to model this phenomena.
If I've missed something let me know. Note, as ANSYS staff there are limits on what I and colleagues can discuss/share on public sites.
July 26, 2018 at 10:55 amDrAmineAnsys Employee
Can you clarify more about the expected velocity discontinuity
I guess the theory applied in Fluent is not appropriate here as you are modelling waves between two dense fluids with non-negligible friction (Fenton et al.).
July 26, 2018 at 5:32 pmsolovievSubscriber
rwoolhou and abenhadj,
Thank you for your responses.
We are not interested in mixing of two layers, just the orbital velocities that would be produced by an internal ocean wave of a specified wave height and length.
To clarify what was meant by the expected velocity discontinuity, I have attached a figure from Munk (1981) as well as vertical profiles plots of the u velocity from the simulation compared to the analytical theory. It appears that the discontinuity is not present when Fluent is initialized, it only appears after the model is run for some time steps. After running for a couple of time steps with a very small time step size, the discontinuity in u does appear, however, it is not symmetric across the interface of the two water layers as expected by the analytical theory. I have looked at a case with surface waves (between air and water) and observe the same asymmetry.
Additionally, I have run a test with the internal wave case with almost-zero viscosity (reducing friction) and see no difference in the velocity profiles from the case with normal molecular viscosity.
July 27, 2018 at 7:41 amDrAmineAnsys Employee
I guess with the the one fluid formulation which you are applying will be quite hard to mimic the analytic solution at moderate grid density as you might know VOF does not allow for slip. You will larger grid density in order to approach the reality but you are still facing the formulation limitation.
It is clear that the discontinuity would not appear at the initialization stage. Watch out any reflections at your boundaries, make a time step and grid sensitivity analysis.
Sometimes turbulence damping is required to match the reality especially if Two-Equation models are used (same would apply for RSM too). The coefficient of damping is however not derived from principles. The whole approach is just to dampen the KE from higher density fluid to lower density fluid and this almost the case for gas/liquid systems.
July 27, 2018 at 9:06 pmsolovievSubscriber
- You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Suppress Fluent to open with GUI while performing in journal file
- Floating point exception in Fluent
- What are the differences between CFX and Fluent?
- Heat transfer coefficient
- Getting graph and tabular data from result in workbench mechanical
- The solver failed with a non-zero exit code of : 2
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- Mesh Interfaces in ANSYS FLUENT
- error in cfd post
© 2023 Copyright ANSYS, Inc. All rights reserved.