# simpleFOAM not giving steadystate solution

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

July 18, 2012, 07:51
#1
Senior Member

aerospain
Join Date: Sep 2009
Posts: 125
Rep Power: 9
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.

Thanks!
Attached Images
 slice_m04.png (30.6 KB, 32 views) slice_m05.png (41.2 KB, 34 views)

 July 18, 2012, 08:15 #2 Senior Member     Niels Nielsen Join Date: Mar 2009 Location: NJ - Denmark Posts: 472 Rep Power: 16 We probably need a little more info such as schemes for example. Depending on the Re the flow around a square will rarely be steady-state 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: 9 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
Senior Member

aerospain
Join Date: Sep 2009
Posts: 125
Rep Power: 9
Quote:
 Originally Posted by linnemann We probably need a little more info such as schemes for example. Depending on the Re the flow around a square will rarely be steady-state 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
Dear linnemann,

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 time-averaged (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: 9
Quote:
Aerospain,
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 time-dependent! From that point of view, I think your approach is (might be) not O.K.
1. perform the numerical modelling of time-dependent flow;
2. do some "premature" modelling to get the impression on the time-step and mesh-size scale;
3. choose fine enough time-step, fix it and do the grid dependence study (for a given/fine enough time-step) using three consistently refined meshes;
4. once the "optimal" mesh (giving the mesh-size independent reults) is determined, use three (or more, if needed) consistently refined time-steps 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 start-up and pulsating test case problems, Journal of Non-Newtonian Fluid Mechanics, 154 (2008), pp. 153-169.

where the similar "issue" is resolved.

Cheers,
Primoz

 August 6, 2012, 07:50 #6 Senior Member   aerospain Join Date: Sep 2009 Location: Madrid, Spain Posts: 125 Rep Power: 9 Thank you Ternik, Your step-by-step 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 Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post gueynard a. Main CFD Forum 19 June 27, 2014 21:22 mgdenno OpenFOAM 4 September 13, 2011 12:58 prapanj Main CFD Forum 2 July 30, 2011 19:07 nakor FloEFD, FloWorks & FloTHERM 0 April 22, 2011 04:34 Abhijit Tilak Main CFD Forum 6 February 5, 1999 02:16

All times are GMT -4. The time now is 08:02.