CFD Online Logo CFD Online URL
Home > Forums > STAR-CCM+

Influence of initial conditions in SteadyState

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

Like Tree5Likes
  • 4 Post By kyle
  • 1 Post By abdul099

LinkBack Thread Tools Display Modes
Old   March 29, 2012, 09:14
Default Influence of initial conditions in SteadyState
Senior Member
Join Date: Dec 2011
Posts: 121
Rep Power: 7
fshak92 is on a distinguished road
If i am right,the initial condition should not have any influence if our solution is converged.
In my Conjugate Heat Transfer simulation,After about 10 iteration i get the residual about 10^-5 and this residual isn't changed anymore... .
Therefor i expect that the results aren't changed by continuing iteration.But by each iteration(in spite of no changes in residual) my results are changed.
Also the initial condition has huge influence on my results(in spite of having the same residual about 10^-5)

Do you know why?
Thank you in advance.
fshak92 is offline   Reply With Quote

Old   March 29, 2012, 12:40
Senior Member
Join Date: Mar 2009
Location: Austin, TX
Posts: 147
Rep Power: 11
kyle is on a distinguished road
You are correct that in a valid steady state simulation that you should end up with the same solution regardless of initial conditions. Your problem is your interpretation of what is being presented to you as "Residuals". In commercial CFD software, residuals are of absolutely no use in determining convergence. They may help in determining reasons for divergence, but that is about it.

The residual values provided by Star-CCM+ are normalized to 1 in the first iteration*. So, if you start your simulation with initial conditions wildly different than the steady state solution, the residuals will rapidly fall and appear to level off long before the simulation has actually converged. This is likely the behavior you are seeing. At the other end of the spectrum, if you use initial conditions that are very near the steady state solution, the residuals will never fall very far, and you may get a valid converged solution with residuals above 1e-1. This is why it is a very bad idea to have a convergence rule based on residual values.

To properly gauge convergence, you need to monitor other values. For a CHT simulation such as yours, I would monitor the heat transfer rates at each of your solid-fluid and solid-solid interfaces, the temperature of the flow at the outlet (assuming you have an outlet), and possibly the temperatures of a few individual solid cells that you expect to converge last. Once all of those values have stopped changing, or at least begin osculating about a constant value, then your simulation is converged.

* This is a terrible design. It is only done so that the residual plots look pretty for the manager that CD-adapco is selling the software to. For all the fantastic meshing and solving algorithms in Star-CCM+, their design decisions do a fantastic job of obstructing natural workflow, inhibiting flexibility, and somehow simultaneously confusing users and treating them as if they are idiots.
Pauli, siara817, fshak92 and 1 others like this.
kyle is offline   Reply With Quote

Old   April 1, 2012, 16:09
Senior Member
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 15
abdul099 is on a distinguished road
the residuals are normalised to the highest residual within the first 5 iterations. And I assume this is not done to better sell the software but for better judgement about a simulation. When a simulation converges very slowly, residuals will show a completely wrong picture without normalisation.
fshak92 likes this.
abdul099 is offline   Reply With Quote


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
alphaEqn.H in twoPhaseEulerFoam cheng1988sjtu OpenFOAM Bugs 15 May 1, 2016 16:12
lift and drag on ship superstructures vaina74 OpenFOAM Running, Solving & CFD 3 June 8, 2010 12:30
Error log OpenFOAM 6 August 7, 2009 05:44
Negative value of k causing simulation to stop velan OpenFOAM Running, Solving & CFD 1 October 17, 2008 05:36
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07

All times are GMT -4. The time now is 22:52.