What value shall I set for the Convergence criteria?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 February 25, 2010, 08:07 What value shall I set for the Convergence criteria? #1 New Member   Steven Tay Join Date: Jan 2010 Posts: 28 Rep Power: 8 I am currently working on the sensitivity analysis on the meshes and time steps. However, I have a question on the convergence criteria. According to the Ansys training notes, we need to set the convergence criteria of minimum of 1e-4, if we need it to be more accurate, we have to reduce it. The question is, for my application, it is enough to set it at 1e-4? If it is not enough, which value should I set and how to decide which value is the most suitable value? Is it correct that we should set the default value first (1e-4) and after getting the best mesh and time step, run this setting and compare results with my experiment results? If the results tally, then the convergence criteria set was ok, if it does not tally, then I should reduce the convergence criteria till I get the best results. Does that make sense?

February 25, 2010, 08:12
#2
New Member

Arvind
Join Date: Mar 2009
Posts: 15
Rep Power: 9
Quote:
 Is it correct that we should set the default value first (1e-4) and after getting the best mesh and time step, run this setting and compare results with my experiment results? If the results tally, then the convergence criteria set was ok, if it does not tally, then I should reduce the convergence criteria till I get the best results. Does that make sense?

U r absolutely correct!!!! The convergence criteria is specific for a particular problem.For better accuracy u can set it to 1e-6.

 February 25, 2010, 08:25 #3 Member   SanS Join Date: Mar 2009 Posts: 41 Rep Power: 9 Apart from residuals alone, its a good practice to ensure that your variables of interest have also converged. You could do this by monitoring your variables using monitor points.

 February 25, 2010, 08:48 #4 New Member   Steven Tay Join Date: Jan 2010 Posts: 28 Rep Power: 8 Thanks for the prompt respond! I have a clearer directions now!

 February 25, 2010, 08:48 #5 New Member   Arvind Join Date: Mar 2009 Posts: 15 Rep Power: 9 @ sans Pls can u explain hw can we monitor the variable using monitor points

 February 25, 2010, 08:54 #6 New Member   Steven Tay Join Date: Jan 2010 Posts: 28 Rep Power: 8 I think sans is referring to adding user define monitor points, like inlet and outlet temperatures, pressures and so on, depending on which variables you are interested in. I hope I am right.

 May 14, 2010, 12:39 Solution Accuracy #7 Senior Member   Join Date: Feb 2010 Posts: 145 Rep Power: 9 ANSYS technical help responded with below when I asked for general comments about ensuring the accuracy of a solution: You ask a lot of good questions! Basically errors in CFD can be categorized as follows: 1) Geometric Representation - make sure relevant features in the geometry are included - ensure that your inlets/outlet are not too close to the area of interest 2) Specificiation of Boundary Conditions - ensure the boundary conditions are correct (for example if you have a pressure profile, but assume an average pressure at a boundary it will affect your results) - ensure that the boundary conditions are well posed (for example for an incompressible case, don't specify a mass flow rate in and a different mass flow rate out, or the solver will be sure to get the wrong answer) 3) Discretisation Errors - ensure that your mesh is fine enough to minimze these errors. This is easier said than done. You may want to perform a mesh sensitivity study to check this. For example, run the same geometry with a mesh size of "N" nodes, "2*N" nodes, "4*N" nodes, and "8*N" nodes, where "N" is some number of nodes that you think is reasonable. Check your solution - at some point you will find that the changes in solutions when you double the number of nodes in the solution will become negligible. - ensure you accurate resolve areas of high gradients (for example the boundary layer around walls) - ensure the timestep you have selected is suitable. - ensure that you use higher order numerics where possible. Most of the numerics are bounded second order in CFX (ex. High Resolution Advection Scheme), so you probably don't need to worry about this too much. 4) Numerical/Roundoff Errors - ensure the case is well converged to reduce these errors - a well converged case will have: * low residual values - RMS residuals machine roundoff for single precision is roughly 1e-6, and for double precision it is 1e-8. These should not be able to get residuals lower than these values, but you might not even need to go this low. You could do a residual sensitivity study - run the case to 1e-4, 1e-5, 1e-6 and see how the results change. Maybe 1e-4 is accurate enough. I typically use 1e-5 as a starting point. * small global imbalances - generally speaking, if residuals are small, global imbalances should be small as well, but it's not always the case. I like to ensure global imbalance are less than 0.1%. * solution variables no longer change with each iteration - typically you should monitor values in the solver manager that you are interested in knowing. Maybe for your case it is average outlet temperature, or maximum heat transfer coefficient on the fin surface. Whatever you thin is important, add a monitor point for it, and ensure it has reached a fairly consistent value. 5) Modelling Errors - make sure that you are modelling all relevant physics (i.e. is the correct turbulence model being used, is radiation important, are the walls being modelled as being smooth when they are rough in reality) Those are the main things to consider - the CFX help documentation will go into more details about these topics if you are interested. krisipanikou, dreamz, alireza1941 and 2 others like this.

 May 14, 2010, 12:44 #8 Senior Member   Join Date: Feb 2010 Posts: 145 Rep Power: 9 Arvind, In CFX-Pre, right click on Output Control and select Edit. Click Monitor tab. Under Monitor Points and Expressions, click Add New Item. Enter expressions like massFlow()@Inlet or areaAve(Pressure)@Inlet or areaAve(Temperature)@Outlet, where Inlet and Outlet are Named Selections which have been created in Mesh. See manuals for syntax on additional expressions.

 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 swarley FLUENT 3 June 24, 2009 11:18 star CD-adapco 2 January 14, 2009 05:57 edwin FLUENT 1 February 14, 2008 20:24 Renato. Main CFD Forum 6 June 6, 2007 19:51 maoasis FLUENT 3 May 14, 2006 13:55

All times are GMT -4. The time now is 10:06.

 Contact Us - CFD Online - Top