what does it look like if you change the contour plot from temperature to velocity? is it purely the downdraft and the viscosity of the fluid forcing your ambient to move downward? I would expect it to circulate within your cut-plot (depending on dimensions).
Did you use symmetry for this? There is actually an updraft on the right edge (central axis assuming symmetry). This would suggest that perhaps a boundary condition isn't quite right.
There also seems to be some base structure or floor shown in the 1st figure which isn't present in the 2nd. This could alter the overall flow.
Thanks for getting back to me. Here's the a velocity contour plot:
I would expect a circulation pattern as well; the downdraught certainly isn't intentional. This is a quarter model with symmetry conditions at the cut planes. This plot is through one of those planes. All other domain boundaries have the default boundary condition. I hadn't noticed the updraught above the flask but that is an interesting point. I originally ran this study with a domain that was about half the size (in each principal direction) and experienced similar results.
You are correct about the floor that has been removed in the second plot. This has been done as part of the test requirement I'm trying to represent. I am looking into the effect of adding this back in at the moment but the transient is taking a while to run. I wouldn't expect it to cause the effect I'm seeing though.
Some other points of note:
- For each study I have run the peak velocity has been located between the upper and lower plates of the pallet the flask is standing on (typically in the XZ plane). In some studies this has been in the region of 500m/s.
- I am running periodic flow freezing to achieve modest run times. I have experimented a little with the parameters and 100 iterations on/20 off, starting after 60 iterations seems to work okay, although I don't have a benchmark to check against as the non-flow freezing study I set up ran 11 seconds of physical time in 11 days over Christmas.
Thank you for your assistance.
The elimination of that floor would have some effect by allowing the ambient to move vertically as opposed to requiring a 90deg turn at the floor - but not as drastic an impact on velocity as you've seen.
My #1 concern would be the use of flow freezing with natural convection. Because flow freezing suspends changes in velocity but continues to calculate temperatures it might mess things up by creating runaway conditions.
What do you truly need to calculate here? Can you force the calculation time (physical time per step) to be larger to prevent long solve times? I don't do much transient and I know it comments if the specified time step is longer than its default time step, but does it produce an error?
I could see this type of overall velocity profile (minus the center updraft) for a small structure in a large space. If you actually have a floor and ceiling this would reduce the size of the convection currents (if this is the case I would either add walls or put this in a hollow cube and run it as an internal). But if you are getting 500m/s from free convection something is obviously wrong.
Flow freezing is a bit of a black box to me at the moment. I have yet to establish a consistent rationale for selecting the parameters and achieving a given reduction in run time. That aside, I'll give what you have suggested a go. I think I did this before Christmas but can't recall what the outcome was. Typically I have found that the automatic time-step starts off small and gradually increases as the changes to the flow field settle down. However, as it was of the order of microseconds on the study I ran over the holidays I had to abandon it and seek an alternative.
Due to the nature of what I am doing I am unable to enclose the flask. The study is simulating a pool fire caused by a fuel spillage. The floor has been removed in order to allow free upwards flow of air, although in most previous studies (by external contractors and using other CFD codes) a forced updraught has been applied to achieve peak velocities next to the flask of around 10m/s. The purpose of the study is to determine the peak temperatures at different points within the flask before and after the fire. A lot of the model setup is in accordance with the regulatory guidance material I am working to.
Studies are running and I'll let you know the outcome.
I've made some progress on this using a greatly simplified model and experimenting with Calculation Control Options. I'm still not sure what is causing the downdraft, but it's definitely not flow freezing. However, I have established that flow freezing was indeed causing some runaway conditions between the pallet plates (supersonic flow and high temperatures (2000K+) that were causing the solver to fall over). Therefore I have experimented with fixed time-steps and time-steps that increase linearly and these seem to be achieving consistent results. I still don't have a benchmark using automatic settings as even on the simplified model the run time is estimated at many hundreds of hours.
Regarding the downdraft, my current thinking is that it could be something to do with the steady-state results that are being used as the initial conditions for the transient. There's nothing wrong with the results themselves, but maybe something weird is happening in translation.