
[Sponsors] 
July 18, 2012, 07:51 
simpleFOAM not giving steadystate solution

#1 
Member

Hi everyone,
I am running a grid convergence study on a 2D square cylinder by refining four times an initial coarse grid (by refineMesh). All grids have been run by 5000 iterations and each of them, besides the first one, start from a mapped solution of the final iteration (5000) of the previous coarser grid (done by mapFields). My surprise came when opening in paraView the last two solutions (pictures attached) and the finest grid gave an "unsteady" looking solution. Mesh04 the first picture and Mesh05 the other one. Any hints, please? Thanks! 

July 18, 2012, 08:15 

#2 
Senior Member
Niels Nielsen
Join Date: Mar 2009
Location: NJ  Denmark
Posts: 445
Rep Power: 14 
We probably need a little more info such as schemes for example.
Depending on the Re the flow around a square will rarely be steadystate and you could simply have refined the mesh to such a degree that the numerics start behaving more transient since the fluxes wont be "damped" as much. Its just an idea
__________________
Linnemann PS. I do not do personal support, so please post in the forums. 

July 18, 2012, 09:16 

#3 
Senior Member
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8 
Dear aerospain
you solved a case not steady state. simplefoam does not have problem. your test case physically is unsteady. 

July 18, 2012, 09:43 

#4  
Member

Quote:
Thank your for your help. I was aware from the beginning that my "physical" problem is unsteady and the "computational" one as not capturing the whole extent of the physics. But, as it is usually done in grid convergence studies, you first run a steady solution to define your mesh size, and the you run unsteady solutions to define your time step. Besides, I will need to compare steady solutions and timeaveraged (unsteady) solutions in a couple of months. What you mention about the fluxes goes along the lines of what I've been talking to some colleagues during lunch break. I've decided to run two meshes in unsteady mode to check how the turbulence behaves and if I can observe anything "going wild". cheers! 

August 1, 2012, 06:54 

#5  
Member
Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8 
Quote:
defining the mesh size based on a steady state solution results is O.K., but as you said, you do not achieve steady state solution (results) because your case is timedependent! From that point of view, I think your approach is (might be) not O.K. In your case, I would: 1. perform the numerical modelling of timedependent flow; 2. do some "premature" modelling to get the impression on the timestep and meshsize scale; 3. choose fine enough timestep, fix it and do the grid dependence study (for a given/fine enough timestep) using three consistently refined meshes; 4. once the "optimal" mesh (giving the meshsize independent reults) is determined, use three (or more, if needed) consistently refined timesteps to show (prove) that the solution obtained on a chosen mesh size is time independent. In addition, I suggest to go through the following paper A.S.R. Duarte, A.I.P. Miranda, P.J. Oliveira. Numerical and analytical modeling of unsteady viscoelastic flows: The startup and pulsating test case problems, Journal of NonNewtonian Fluid Mechanics, 154 (2008), pp. 153169. where the similar "issue" is resolved. Cheers, Primoz 

August 6, 2012, 07:50 

#6 
Member

Thank you Ternik,
Your stepbystep explanation asserts me on what I had in mind. Just one comment, I've been able to produce (numerical) steady results by starting from zero time all the grids. Before, I was using the results of each coarser mesh as a restart point for the following finer mesh. This allowed for the disturbances present in the solution to build up and show the physical unsteadiness after the third finer grid. Have a great summer! C. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
grid dependancy  gueynard a.  Main CFD Forum  19  June 27, 2014 21:22 
interFoam solution tolerances  mgdenno  OpenFOAM  4  September 13, 2011 12:58 
Neumann Boundary Condition for Poisson Equation solution in Polar Coordinates  prapanj  Main CFD Forum  2  July 30, 2011 19:07 
Transient, initial variables from a previous solution  nakor  FloEFD, FloWorks & FloTHERM  0  April 22, 2011 04:34 
Wall functions  Abhijit Tilak  Main CFD Forum  6  February 5, 1999 02:16 