[FluidViscosity]

Hello!

I am modelling free surface flow around a surface-piercing strut with a blunt trailing edge and I have a problem with some unwanted (unphysical) standing waves in the domain.

I am currently doing a time sensitivity analysis and this phenomenon seems related to the timestep. Estimated courant numbers of 20, 10, 5, 2 and 1 are being tested as 'physical timesteps' from 0.013 to 0.00068 seconds.

I am using the best practice advice found in the CFX documentation .

A colleague passed on some expert parameters he found helpful in the past for similar issues:
EXPERT PARAMETERS:
linearly exact numerics = t (default f)
overlap relaxation fluids = 0.9 (default 1.0)

These made no noticeable change!

Additionally he mentioned that changing the discretisation of the advection interpolation from tri-linear to linear-linear would be beneficial, though I haven't yet tried it.
"By default, linear-linear interpolation is used unless the flow involves buoyancy, in which case tri-linear interpolation is used for improved accuracy." - CFX documentation.
This change can be implemented by modifying the local RULES file, which may not be an option for me as I tend to use HPC clusters rather than a local machine.

I am using a structured mesh from ICEM of approx. 9 million nodes. The waves seem to begin after block change in which cell size is slowly increased into the far field. The attached photo of the mesh is at the (nominal) free surface height. I have improved the sharp change in volume for subsequent runs, however, despite this large change in mesh size, the standing waves are across the entire domain so I'm not sure it is a mesh problem.

What are your recommendations to debug this problem?

NR5_CFL_Y25_C5.txt
Standing wave.png
Standing wave2.jpg

[FluidViscosity]

A few more lessons learnt:

I have since tried a few more things to no avail.

• Changing the Body Force Averaging Type to harmonic from volume-weighted(more robust, and recommended for free surface flows) did not have an effect.
• Changing the advection scheme to upwind from high resolution(has more numerical dissipation) did not have an effect.
• Changing to a less fine mesh (~5 million nodes) with no sharp volume changes did not have an effect.

Next on my list to try

• Reduce the Interface Compression Level to 1 (default 2)
• Change the Froude number of the simulation (previous tests with the at Fr=3 did not have the spurious waves. Current test at Fr=2.5)
• Try set the Volume of Fractions option to coupled.
• Experiment with different VoF equation class timesteps (currently 1/10th of simulation timestep)

Would appreciate any feedback!

[ghorrocks]

I have modelled similar surface piercing struts in a past life and had no problems like this.

My comments (highest priority first):
* Are you sure you have run for long enough? This is probably a startup transient which just needs to convect out the outlet boundary. Residuals are not a good way of detecting this type of convergence.
* You might find adding imbalances as a convergence criteria will help here.
* I do not like your automatic time step changing thing. My recommendation is you start with a small enough time step that it starts to converge, then you observe to convergence. If it is converging slowly but monotonically then you increase the time step by maybe a factor of 10 using "change run in progress". If the residuals are going spiky and starting to diverge then decrease the time step by a factor of 10. Repeat this everytime you are confident you can see a monotonic convergence or signs of divergence. This way you quickly find the actual time step size this simulation can handle. Once you have worked out the time step is like to run at, then you write a function like you have to automate it for future simulations.
* Don't use those expert parameters unless you know you need them. It looks like you don't need them so don't complicate things by using them. I did not use these parameters in my work on struts.
* I would not have the vf equation on a different time step size to the other equations unless you have shown that it helps. Again, don't complicate things unless you know you need it.
* Why have you got max iteration 1460, min 300? This looks like a kludge because the residuals are not picking up convergence (and I don't think you are converged anyway). If you use imbalances as an additional convergence criteria I suspect it will fix this and you won't need this term.
* Coupled and segregated vf equations will make a big difference. They did for me, and not always for the better

[FluidViscosity]

Hi Glen!

Many thanks for your response.

In these steady state runs I have been running for 5 seconds of pseudo time [1-2]. In other words 1460 iterations multiplied by my specified physical timestep gives 5 seconds. At the Froude number of my tests (2-4) that equates to ~two pass throughs of the domain. I chose 5 seconds as a means to to compare simulations at different timesteps and to give any vortical structures time to develop. I have found that force convergence can occur before cavity structure is finalised, and so I have ceased to use an interrupt control based on the std deviation on the lift coefficient as my main way to halt a run. Instead I rely on the (still imperfect) method of running for the same amount of pseudo-time.

Imbalance criteria:
I've just read a little on imbalance convergence criteria including your discussion here. My imbalances have been fairly consistent at different timesteps, mesh sizes and number of iterations. Somewhere in the vicinity of:
U = ~0.4%
V = ~0.04%
W = ~-0.02%
P = 2-3%
Mass-water = 2-3 %
Do you think I should chase tighter imbalances than that or are those values typical for free surface flows?

Timestep:
I'll give this a go. I can certainly achieve monotonic convergence for some runs, so there might be scope to increase timestep.

Expert parameters:
Yes if they are not helping I will remove them. For completeness one of my earlier comments stated that to force the solver to use linear-linear interpolation (rather than the default trilinear) one needed to change the RULES file. Instead, the setting may be found in Solver Control/Advanced/Interpolation Scheme/Pressure Interpolation Type -> Linear-linear.

VoF Timestep:
Thanks for the comment. I was using the CFX modelling guide for free surface flows which recommends changing the VoF timestep to be an order of magnitude lower than the other transport equations. I can say that for my simulation, there is no difference between Vof timestep being 0.1*regular timestep and 0.025*regular timestep.

To report back on some of the tests that ran over the weekend:

• Reducing Interface Compression Level to 1 reduces spurious wave amplitude.
• Vof coupling also helps a lot in reducing the spurious wave I had behind the strut, but accentuated a wave near one of my inlets. I have also found some unhealthy looking checker-boarding (although magnitude is small). Images: left coupled, right segregated VoF equations.
• This phenomenon changes with Froude number. The faster the inlet flow, the more numerically stable the run is (smaller and fewer spurious waves)

I guess my next steps are to keep playing with timesteps until I get a successful run with correct looking results, after which I can resume my time sensitivity analysis.

VoF_couple-segregated_iso.jpg
VoF_couple-segregated_pressure.jpg

Both references below do state that length of simulation is critical for accuracy. They recommend between 5-10 seconds.
[1]
Casey Harwood, Kyle Brucker, Francisco Miguel Montero, Yin Lu Young, and Steven L. Ceccio, "Experimental and Numerical Investigation of Ventilation Inception and Washout Mechanisms of a Surface-Piercing Hydrofoil", in 30th Symposium on Naval Hydrodynamics, At Hobart, Australia (, 2014).

[2]
Andrea Califano and Sverre Steen, "Analysis of Different Propeller Ventilation Mechanisms by means of RANS Simulations", in Proceedings of The First International Symposium on Marine Propulsors (, 2009).

[ghorrocks]

It looks like you are being quite thorough in your analysis. You are testing the options and seeing what works.

My only comment is on the imbalances - a 2-3% imbalance on pressure and vf equation is a little high, usually you try to get below 1%. But a sensitivity analysis will confirm or deny this in your case, which is what you have done plenty of so far with the other options.