[artkingjw]

Hello all,

I need some advice in diagnosing an issue I have in Fluent, where my problem is converging just fine in transient simulation, but diverging in steady state simulation.

The problem is very simple - just a circular cylinder near a wall. The mesh was produced with ICEM, and sizing is quite fine (see attached). The actual domain is massive, so it shouldn't be the issue.

For BC, I have the circle and bottom wall as wall boundary, the inlet (to the left) as farfield, the top edge as farfield (same direction and magnitude as the left side inlet), the outlet on the right as pressure outlet.

I am using the energy equation, with compressible ideal gas as my fluid, and Sutherland's viscosity model. Mach number is in the order of 0.05-0.1.

So far, for my first few runs, I have gone straight to transient - discarding initial results as the simulation settles down. Transient simulations work just fine for me, converging well within 50 iterations.

The problem is, I now wish to achieve a steady state solution first, which I then feed into the transient calculation. However I cannot seem to achieve any reasonable convergence with the steady state simulation. This happens regardless of my turbulence model choice, choice of PV coupling, discretization scheme, or under relaxation - I haven't tried every possible combination, but most of the common tips I have seen around here, I have tried.

The ONLY thing that I have found to 'help' so far, is Mach number - using a higher Mach number prevents the solution from diverging, but does not cause it to converge, it either oscillates or just stays flat.

I have also tried coarser mesh, and a finer mesh, but they did not help either.

Does anyone have any tips or advice for me? Thank you all in advance.

[CeesH]

Perhaps the issue is that you try to find a steady state velocity, where there is none? I expect that your transient simulations show you shedding behavior of some sort (I don't have experience with compressible flows in this respect though, so don't know exactly what is supposed to happen) - what would you expect your steady state simulation to give you?

And second, why? You already stated that starting transient and discarding the start-up period works fine; what's the benefit of running the simulation again, essentially with a different starting point?

[artkingjw]

Originally Posted by CeesH

Perhaps the issue is that you try to find a steady state velocity, where there is none? I expect that your transient simulations show you shedding behavior of some sort (I don't have experience with compressible flows in this respect though, so don't know exactly what is supposed to happen) - what would you expect your steady state simulation to give you?

Hmm.. True there is vortex shedding, but I'm sure I've seen plenty of SS solutions to cylinder flow before, and in fact the vast majority of problems never reach a steady state anyway?

Originally Posted by CeesH

And second, why? You already stated that starting transient and discarding the start-up period works fine; what's the benefit of running the simulation again, essentially with a different starting point?

I will be doing quite a few cases, so my thinking is that using a steady state solution as a starter will speed up the process - it takes a while for the solution to settle using my previous method. I have also read many recommendations on forums such as this, that it would be ideal to start a transient simulation with a steady state solution.

Thank you.

[CeesH]

The "steady flow past a cylinder" tutorial at the Cornell tutorial page uses a low reynolds number, where no shedding is present - I've never tried a higher Re for that in steady state, but my expectation is that it will oscillate as a transient simulation, only at some false frequency. The divergence you observe may be due to the more complex setup of a compressible flow.

I do agree that in some cases, starting from a steady state solution can help - I do it frequently for stirred tanks (which are not truly steady either, but the periodic flow is only a few percent in magnitude of the mean in many cases), to avoid the lengthy "start up" period. For this particular type of flow, I doubt it would make a huge difference however; you may avoid some of the start-up time, but even if you have a steady-state solution, vortex shedding will be fully undeveloped when you switch to transient. You will still need to discard some of the initial transient solution, representing the development of vortex shedding. In the end, I would not be surprised if the time required to calculate steady flow + shedding development is longer than the time required to directly start from transient. Especially if you take into account the time spent on trying to get the steady state to work in the first case...

[LuckyTran]

The farfield pressure BC is meant to be applied to the freestream boundary (your top boundary) and not at the inlet (and neither at an outlet). You should be using either a pressure inlet or velocity inlet or massflow inlet. You don't have to believe me, just try them.

The farfield BC is a partially non-reflecting BC. That means that the farfield conditions are not strictly imposed. In transient simulations, this gives you some wiggle room. In steady simulations, this is ill-posed. At high Mach numbers, the flow is naturally more reflecting and behaves more like a fixed pressure/velocity BC.

[artkingjw]

Originally Posted by LuckyTran

The farfield pressure BC is meant to be applied to the freestream boundary (your top boundary) and not at the inlet (and neither at an outlet). You should be using either a pressure inlet or velocity inlet or massflow inlet. You don't have to believe me, just try them.

The farfield BC is a partially non-reflecting BC. That means that the farfield conditions are not strictly imposed. In transient simulations, this gives you some wiggle room. In steady simulations, this is ill-posed. At high Mach numbers, the flow is naturally more reflecting and behaves more like a fixed pressure/velocity BC.

Interesting, I never knew that! I will give it a try! Thank you!

[artkingjw]

I changed my inlet to Velocity inlet, and my problem is solved!

Granted the convergence isn't the best, and the values still oscillate, but at least the output pressure and velocity contours look right! The cylinder wake seems to shed as the solution iterates - so it looks like CessH's idea is accurate.

In addition to changing the BC, I also used SIMPLE for PV scheme, and first order schemes everywhere else. Under relaxation was also reduced to 0.15 for Pressure, everything else was reduced by 0.1.