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

convergence of solution question

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 11, 2005, 09:50
Default convergence of solution question
  #1
julie
Guest
 
Posts: n/a
Hello all sorry but I have a very simple question to ask. How do we decide if the solution is reasonable?

When I plotted the residuals, it shows a relatively horizontal line with small fluctuations and is of the order of 10^-2. Is this acceptable since it did not decrease exponentially?

Also my other velocities have pretty low values 10^-6 but continuity convergence is much higher at 10^-2. How?

Thanks a lot julie
  Reply With Quote

Old   November 11, 2005, 10:36
Default Re: convergence of solution question
  #2
Jeremy
Guest
 
Posts: n/a
Hi Julie,

In order to determine if a solution has converged and if it is reasonable requires one to look at several aspects. The fact that the residuals have leveled out is an indication that the solution has converged, but is not always the case. Some problems are numerically stiff and require changes to relaxation factors to get better convergence. Some cases, like natural convection, sometimes (not always) benfit from running an steady case as an unsteady case to get things to converge properly.

Residuals of 10^-2 for the continuity equation (CE) may or may not be good. The residuals do depend on the initialization. For example, if you do a simulation of a laminar flow in a straight pipe, with an initial guess of 0 for the flow velocities, the solution may converge with CE residuals of 10^-4 or 10^-5, or even lower. However, if you were to start the same case, but initialized the flow based on the average velocity, or from a converged or close to converged solution from another run, you may find that the residuals might only drop to 10^-2. The residuals are based on the initial error, therefore in this second case you do not see the residuals drop that much, as there was very little error to start off with. For this reason, the convergence monitoring with all residuals set to converge at 10^-3 is not necessaerily applicable to every case.

But even if the residuals level out, and the solution converges, it may not be a reasonable solution. You need to compare the results to either literature values or experimental values. Plot numerical versus experimental velocity profiles and see if they match. Calculate the fRe and see if it matches with literature values.

Also, have you performed an grid independance test? Solutions will converge on course meshes, but there may be significant errors in the solution compared to finer meshes.

Hope that helps.

  Reply With Quote

Old   November 11, 2005, 12:07
Default Re: convergence of solution question
  #3
Jason
Guest
 
Posts: n/a
You should also be monitoring your values of interest. You can monitor forces, or averaged flow properties (like average pressure or mass flow rate), or flow properties at a point (all these are available under Solve=>Monitors). You should be monitoring anything you plan on reporting. Your specific solution isn't converged if those monitors are still drifting. Then once you're convinced that these values aren't changing, and your residuals aren't changing, then you can call that specific case converged. Once you have that case converged, then you validate the solution by comparing it to experimental or literature values like Jeremy was saying.

Hope this helps, and good luck, Jason
  Reply With Quote

Old   November 13, 2005, 04:06
Default Re: convergence of solution question
  #4
julie
Guest
 
Posts: n/a
Hello,

I have defined monitors for the values I want to monitor. However, I do not understand what do you mean by drifting? Because my monitors will show a trend depicting the flow. They will not remain steady rite?

Thanks a lot to both jason and jeremy.

julie
  Reply With Quote

Old   November 14, 2005, 09:35
Default Re: convergence of solution question
  #5
Jason
Guest
 
Posts: n/a
For a steady state solution, you should get a constant value. If you're running an unsteady case, then you're right, they will change with the flow, but a steady state case implies that the values throughout your domain are constant over time (and therefore once convergence is reached they will be constant over iterations). When I say drifting... sometimes what ends up happening is that the residuals may look level, but if you're looking at the monitor data you'll see that the values are slowing rising or falling.

Hope this helps, Jason
  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
Force can not converge colopolo CFX 13 October 4, 2011 22:03
Convergence question with regards to discretization karananand FLUENT 8 July 16, 2010 14:49
Do you know of any tweaks of the solver parameters to accelerate solution convergence sek OpenFOAM Running, Solving & CFD 0 September 15, 2006 13:45
General Unsteady solution convergence Freeman Main CFD Forum 0 December 7, 2005 18:08
problems with solution convergence Roberto Ciardulli CD-adapco 12 October 29, 2000 04:36


All times are GMT -4. The time now is 15:24.