# Convergence

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

 March 7, 2012, 09:58 Convergence #1 New Member   Join Date: Mar 2011 Posts: 11 Rep Power: 8 Sponsored Links hi this may sound crazy. im dealing with modifying an equipment so have simulate more than 50 models to determine the most suitable geometry. some get converged and some models do not converge. the non converged model residuals reach nearly 0.002 and then remain in that value (i was expecting to get a tolerance of 0.001). Since the residual value reamain in a constant value, can i consider them as converged and accurate? do i have to change the cell size and obtain a lesser tolerance value?

 March 8, 2012, 07:53 #2 Member   Narendra Gadwal Join Date: Jul 2010 Location: India Posts: 35 Rep Power: 9 Instead of looking at residuals, better to monitor a quantity like mass flow rate or pressure at any point in the domain .. that would be more appropriate Vorch likes this.

 March 8, 2012, 14:30 #3 New Member   Join Date: Mar 2011 Posts: 11 Rep Power: 8 thanx Naren. you mean monitored values at reference location? well the graphs of moniterd values(u,v,w momentum, presure and temperature) will simply become a straight line after some iterations. does that mean it accurate? or other wise do we have to verify those values experimentally?

 March 8, 2012, 23:24 #4 Member   Narendra Gadwal Join Date: Jul 2010 Location: India Posts: 35 Rep Power: 9 If the curves become straight, (after running in second order also), we can say that the solution is converged and that is the final result. As a second check check the mass balance also. It should be near to zero.

 March 13, 2012, 05:01 #5 Member     Pedram Mojtabavi Join Date: Apr 2011 Location: Iran Posts: 66 Rep Power: 8 Hi, If the residuals remian constant and don get close near the error u determined,then u are gonna have to refine your mesh, decrease the Y+ near walls or change the solver. If you are runing an unsteady simulation, then check the time step. high values of time steps could increas the CFL number and the residuals do not converge. best,

 March 13, 2012, 17:12 #6 Senior Member     Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 741 Blog Entries: 17 Rep Power: 21 There can be several reasons for a simulation not converging. As you are dealing with an optimization (i really hope you are not doing this by hand), the most probable issue is that the configurations not converging are determining some criticalities like the grid getting "weird" or the fluid dynamics becoming intrinsically unstable (i'm assuming you are doing a steady analysis). In the general case is also possible that you need to relax the solver during its trip to convergence. However, i don't see the point in the difference between 1e-3 and 2e-3 in the residuals, they seem both high to me. As someone already did, i suggest you to check on the mass imbalance of your simulation. However, this is not conclusive. Visual inspection of the non converged solution could give additional details. In the very ending, i think that non converged solution shouldn't be used in numerical optimization routines and this usually requires a modification on the limits for the design variables

 March 14, 2012, 21:39 About convergence... #7 Senior Member   Arjun Join Date: Mar 2009 Location: Nurenberg, Germany Posts: 702 Rep Power: 19 Last 2-3 days I have been trying to understand sources of errors on unstructured grids and how to improve their accuracy. Not that it is something new or done for first time but I wish to make my code more accurate and so it was natural to try this. Second reason for looking into this was that I had problems with calculations with very large viscosity. When I say problems I do not mean that it diverges but it seems to be converging to a solution which is not right. This behavior was noticed in some of the meshes but not all of them. So this is what I did. I took a pipe and created various grids on it. Same dimensions but various meshes of different size (few thousands to 1.6 million cells). Further tried all tetra, prisms and hexa meshes (with slight skew since it is pipe ). For this pipe using power law I know theoretical solution. Note that viscosity varies from say 100 till 1E12 in this case. I put theoritical velocity and pressure on cell centers and apply discretization and seek the errors. If someone to say that this solution is converged solution then there shall be no errors. After all this is theorical solution that is present on this grid cells. But it does not work quite this nice. If there is some skew then there exists errors. That is Left hand side NOT EQUAL to right hand side after descretization. If meshes have all well behaved hexa cells then error is very very low. The following are conclusions based on this excersize assuming that there exists some not so nice cells in mesh (which is usually the case): 1. If your solutions converged to machine precision ie 1E-20 or so then it is very likely to be not the correct solution. Strange thing to say but you see when exact solution was descretised on that grid it showed errors so any solution that does not show those errors after discretization shall be other than the correct one. 2. If your solution converged to a state where there exists some errors and residual refuse to fall below certain values. Then it could be better solution than type 1. This is because theoritical solution does show some errors that refuse to go away. But it shall be noted that there is no guarantee of it to be the true solution.

 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 Centurion2011 FLUENT 44 June 20, 2017 09:57 colopolo CFX 13 October 4, 2011 22:03 nasdak CFX 2 June 29, 2009 01:17 tippo CFX 2 May 5, 2009 10:55 ganesh Main CFD Forum 4 June 30, 2006 14:20