
[Sponsors] 
Convergence in Transient; Divergence in Steady State 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 23, 2018, 02:34 
Convergence in Transient; Divergence in Steady State

#1 
Member
Arthur
Join Date: Apr 2015
Posts: 34
Rep Power: 10 
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 0.050.1. 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. 

May 23, 2018, 03:06 

#2 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
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 startup period works fine; what's the benefit of running the simulation again, essentially with a different starting point? 

May 23, 2018, 03:28 

#3  
Member
Arthur
Join Date: Apr 2015
Posts: 34
Rep Power: 10 
Quote:
Quote:
Thank you. 

May 23, 2018, 04:31 

#4 
Senior Member
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 0 
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 startup time, but even if you have a steadystate 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... 

May 23, 2018, 08:17 

#5 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,665
Rep Power: 65 
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 nonreflecting 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 illposed. At high Mach numbers, the flow is naturally more reflecting and behaves more like a fixed pressure/velocity BC. 

May 23, 2018, 19:53 

#6  
Member
Arthur
Join Date: Apr 2015
Posts: 34
Rep Power: 10 
Quote:


May 24, 2018, 02:51 

#7 
Member
Arthur
Join Date: Apr 2015
Posts: 34
Rep Power: 10 
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. 

Tags 
convergance, ideal gas, steady state, transient 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Laminar transient or Turbulent steady state?  zippostyle  Main CFD Forum  21  February 13, 2019 14:13 
DPM steady state or transient  Danial1992  FLUENT  0  June 25, 2017 19:30 
Transient & steady simulation  DIVYA P SOMAN  ANSYS  0  September 3, 2016 14:09 
error message  cuteapathy  CFX  14  March 20, 2012 06:45 
About the difference between steady and unsteady problems  Lisa  Main CFD Forum  11  July 5, 2000 14:37 