Unstable transient analysis

[Anonymous]

I'm having some trouble setting up a transient analysis for a station I'm modelling. The platform doors have a varying flow rate through them, whilst the upper opening to the concourse has a zero pressure set to it, as well as a large diffuser supplying cool air. The simulation appears to run smoothly for the first 27 steps (seconds) when the doors have similar values. After this though, some doors have been set to experience a large increase in flow rate (about 4 times larger), whilst other doors down the opposite end of the platform reverse their flow (infiltration instead of exfiltration). At this point the model becomes unstable and the velocity rapidly increases by orders of magnitude with each step.

Attached a screenshot of the plot showing it go wild. Also has what the station looks like after 25 seconds before the instability.

How can I resolve this?

Cheers

[marwan_azzam · Accepted solution]

I would restart the solution from 27 seconds and use a smaller time step size to see if this helps.

Marwan

[frederic.gaillard.7]

Hello Dr Tomato, 

Based on your description, your problem seems to be a recirculation problem : you have an inward and an outward throught the same boundary condition (Pstatic=0).  If you add  vector perpendicular to this boundary you will be able to see this behavior. For the sake of the continuity equation, vector need to be uniformly distributed and oriented in the same direction. 

Several thing could help in this case : 

1. activate the flag adv5_no_dtime, turning it to 1 
2. Refine the mesh near this outlet
3. As Marwan pointed out TimeStepSize had to be smaller.

Hope It Helps

Fred

[Anonymous]

Thank you both @marwan_azzam and @frederic.gaillard.7 ,

When you say I should increase the time steps at 27 seconds, what do I do with the values at the boundary conditions. For e.g, the doors that receive a flow rate of 4m3/s at 27 seconds and then 16m3/s at 28 seconds, would I need to manually introduce a gradual increase? Like 10m3/s at 27.5 seconds?

@frederic.gaillard.7  this model should experience some recirculation at the 0 pressure boundary condition, with the other boundary conditions changing between inlets and outlets, but you say that recirculation cannot happen? Or that the model needs to be more rigorous to handle this? I will try your suggestions.

I also found a bit more on transient model instability (https://forums.autodesk.com/t5/cfd-forum/solver-becomes-unstable-in-transient-analysis/m-p/8951180). It sounds like I might even need to extend the area where the 0 pressure boundary sits. 

Thanks again.

[frederic.gaillard.7]

Hello @Anonymous , 

Thank you for the clarification.

If the surface where you applied the boundary condition (Pstatic=0) the flow constantly change direction, extend your outlet. (Outlet_lenght = 10xoutlet_diameter)

Adding a tip next to this surface might be, also, a good idea. This way the flow, will be free to circulate as it please. An outlet must be added at the end of the tip. 

The important thing, here, is the flow who is leaving the model must be equal to the flow who is entering in your model. This remain true at any time of your simulation : mass conservation principle,  mass can not appear or vanish in your model. In the summary file you can keep track of your mass balance. 

Hope it answers your question. 

Fred

[Anonymous]

So I extended the zero pressure BC area, not quite by 10x diameter, but nonetheless there seems to be no recirculation and looks to be fairly uniform (see screenshot).  The adv5 flag may have helped with this too.

A new issue has emerged in one end of the model with velocity rapidly increasing. There is no BC here, but one outlet nearby. I think I may have to refine the mesh a bit more in this region, unless you have any other ideas?

Thanks @frederic.gaillard.7  for your help, I will update you on how I go.

[frederic.gaillard.7 · Accepted solution]

Hello @Anonymous , 

refine your mesh, and if unrealistic velocity persist reduce your time step as Marwan pointed out. 

Make sure that every strong gradient and high velocity stream are adequately meshed 

Hope it help 

Fred

[Anonymous]

Just to update, refining the mesh, extending the zero pressure BC region, and using a smaller step size (1s to 0.25s) all worked. Now I just need to handle the results which will take some time because the file is so massive!

Thanks again