CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Convergence in Transient; Divergence in Steady State

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By CeesH
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 23, 2018, 03:34
Default Convergence in Transient; Divergence in Steady State
  #1
New Member
 
Arthur
Join Date: Apr 2015
Posts: 10
Rep Power: 6
artkingjw is on a distinguished road
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.
Attached Images
File Type: jpg mesh.jpg (186.5 KB, 19 views)
artkingjw is offline   Reply With Quote

Old   May 23, 2018, 04:06
Default
  #2
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
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?
CeesH is offline   Reply With Quote

Old   May 23, 2018, 04:28
Default
  #3
New Member
 
Arthur
Join Date: Apr 2015
Posts: 10
Rep Power: 6
artkingjw is on a distinguished road
Quote:
Originally Posted by CeesH View Post
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?


Quote:
Originally Posted by CeesH View Post
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.
artkingjw is offline   Reply With Quote

Old   May 23, 2018, 05:31
Default
  #4
Senior Member
 
Cees Haringa
Join Date: May 2013
Location: Delft
Posts: 607
Rep Power: 13
CeesH is on a distinguished road
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...
artkingjw likes this.
CeesH is offline   Reply With Quote

Old   May 23, 2018, 09:17
Default
  #5
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 3,571
Rep Power: 44
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
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 likes this.
LuckyTran is offline   Reply With Quote

Old   May 23, 2018, 20:53
Default
  #6
New Member
 
Arthur
Join Date: Apr 2015
Posts: 10
Rep Power: 6
artkingjw is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
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 is offline   Reply With Quote

Old   May 24, 2018, 03:51
Default
  #7
New Member
 
Arthur
Join Date: Apr 2015
Posts: 10
Rep Power: 6
artkingjw is on a distinguished road
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.
artkingjw is offline   Reply With Quote

Reply

Tags
convergance, ideal gas, steady state, transient

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Laminar transient or Turbulent steady state? zippostyle Main CFD Forum 21 February 13, 2019 15:13
DPM steady state or transient Danial1992 FLUENT 0 June 25, 2017 20:30
Transient & steady simulation DIVYA P SOMAN ANSYS 0 September 3, 2016 15:09
error message cuteapathy CFX 14 March 20, 2012 07:45
About the difference between steady and unsteady problems Lisa Main CFD Forum 11 July 5, 2000 15:37


All times are GMT -4. The time now is 20:13.