CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

simpleFOAM not giving steadystate solution

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2012, 07:51
Default simpleFOAM not giving steadystate solution
  #1
Member
 
aerospain
Join Date: Sep 2009
Location: Madrid, Spain
Posts: 84
Rep Power: 7
aerospain is on a distinguished road
Send a message via Skype™ to aerospain
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!
Attached Images
File Type: png slice_m04.png (30.6 KB, 29 views)
File Type: png slice_m05.png (41.2 KB, 32 views)
aerospain is offline   Reply With Quote

Old   July 18, 2012, 08:15
Default
  #2
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 445
Rep Power: 14
linnemann will become famous soon enough
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.
linnemann is offline   Reply With Quote

Old   July 18, 2012, 09:16
Default
  #3
Senior Member
 
niaz's Avatar
 
A_R
Join Date: Jun 2009
Posts: 118
Rep Power: 8
niaz is on a distinguished road
Dear aerospain
you solved a case not steady state. simplefoam does not have problem. your test case physically is unsteady.
niaz is offline   Reply With Quote

Old   July 18, 2012, 09:43
Default
  #4
Member
 
aerospain
Join Date: Sep 2009
Location: Madrid, Spain
Posts: 84
Rep Power: 7
aerospain is on a distinguished road
Send a message via Skype™ to aerospain
Quote:
Originally Posted by linnemann View Post
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!
aerospain is offline   Reply With Quote

Old   August 1, 2012, 06:54
Default
  #5
Member
 
Primoz Ternik
Join Date: Apr 2009
Location: Maribor, Slovenia
Posts: 65
Rep Power: 8
ternik is on a distinguished road
Quote:
Originally Posted by aerospain View Post
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!
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.
In your case, I would:
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
ternik is offline   Reply With Quote

Old   August 6, 2012, 07:50
Default
  #6
Member
 
aerospain
Join Date: Sep 2009
Location: Madrid, Spain
Posts: 84
Rep Power: 7
aerospain is on a distinguished road
Send a message via Skype™ to aerospain
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.
aerospain is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 09:31.