# Problem with Convergence!!

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

 February 20, 2008, 03:49 Problem with Convergence!! #1 Elleana Guest   Posts: n/a Hi all, Could some one please tell me what are the general causes of convergence problems. Iam doing simple heat transfer analysis the continuity equation seems to oscillate up and down along with the x, y and Z velocities. Reducing the resuduals does not seem change the situation much. Can some one please lend their thoughts on this. I have checked the boundary condition and mesh seems to be fine. Cheers Elleana

 February 20, 2008, 07:01 Re: Problem with Convergence!! #2 Amit Guest   Posts: n/a Check the order of scheme you r using, first try with first order scheme than after sufficient convergence switch to higher order scheme.

 February 20, 2008, 07:20 Re: Problem with Convergence!! #3 Elleana Guest   Posts: n/a Hi, Iam working on first order. i havent turned the second order yet. Cheers Elleana

 February 20, 2008, 07:34 Re: Problem with Convergence!! #4 Armin Guest   Posts: n/a hi,if you are solving this problem employing Segregated Method it is some time helpful to make some changes to the under relaxation factors, in case of heat transfer temperature and energy under relaxation factors are important, other relaxation factors have a second level of importance, be careful although you might be able to make the solutions converge they might be inaccurate, changing momentum under relaxation factor is effective, moreover if you are using coupled method changing the Courant number and also implementing adaptive grid might help the solution converge, it is a lot more helpful if you can specify the conditions of your problem, thereby I can help you better.

 February 20, 2008, 09:01 Re: Problem with Convergence!! #5 Elleana Guest   Posts: n/a HI Armin, Thanks for your reply. There is a louvre on the left hand side of the building which is 8m * 27m *2.8m. there are thermal mazes placed at eaqual distances on the path of the flowing air on both sides of the 8m width. the air inturn flows in a zig zag way around these obstructions. the idea is to cool down the external air to an extet to reduce the work of the air handling by a factor. i have declared a velocity inlet and a pressure outlet with temperature boundary condition for the walls of the thermal maze. From what iam witnesing it is creating excess turbulence inside. is it a good idea to solve the flow and energy equations first. use them as a initial solution and solve the turbulence equations. Cheers Elleana

 February 23, 2008, 06:53 Re: Problem with Convergence!! #6 armin Guest   Posts: n/a Dear Ellena solving the flow and energy at first can be useful especially when you are working with high speeds, on the other side if the method of your solution is segregated you can change the relaxation factors especially momentum, and also you can gradually change the boundary condition without the necessity to initialize the solution ,decreasing the momentum coefficient can converge your solution.

 February 23, 2008, 16:31 Re: Problem with Convergence!! #7 Carlos Guest   Posts: n/a Hi Elleana, You need to check these things in this order to solve convergence problems: 1) Check you have scaled you grid! Sounds obvious but SO MANY students I help don't do this. They create cad and mesh files in mm then just run in fluent which of course uses the SI unit metres. 2) Next, check the quality of your mesh. What is the worst skew like? Anything above 0.85 equiangle skew is not good but certainly, 0.9 should be a maximum. This is most common problem with convergence problems. Even just 10 highly skewed cells in a 5 million cell domain can cause massive problems - This is probably you problem. Therefore, re-mesh in the problem areas but changing the cell distribution, maybe one edge has a significantly larger spacing that an adjacent one - again this is a common mistake and all part of mastering CFD. 3) From you description you have flow which has high velocity and pressure gardients. You MUST have enough cells in these regions e.g. in the vicinity of sharp corners. To reduce this problem, either cluster more cells in those regions - this will reduce the 'jump' in flow variables from iteration to iteration, or re-model sharp corners with radii to reduce high gradients in the variables. 4) If you have a problem after all that with a 1st order solution, then and ONLY then, reduce the under relaxation factors (URF's). There is no point relaxing a solution on a badly posed problem - get the cad and mesh right first THEN alter the solution controls to help you. In my experience, you can reduce the pressure URF from 0.3 to 0.2 (not much lower) and momentum from 0.7 to 0.5 but no lower than 0.3. Doing this will make convergence times longer so be sure to iterate for longer. 5) Finally make sure you run to convergence - NOT the default of 10^-3, this is rubbish! Reduce the residual convergence limit for say continuity to 10^-9. Your solution will never reach this but it is designed to eliminate 'convergence error'. When the residuals are level (or oscillate about a common point) then you have true convergence. Its also good practice to monitor a drag force or a pressure and apply the same method - wait until it is level. Doing this does take longer but why analyse an unconverged solution! Get it right first then no messing about later... Good luck, Carlos.

 February 23, 2008, 16:37 Re: Problem with Convergence!! #8 Carlos Guest   Posts: n/a P.S. Run isothermal simulations first and then use those to initialize thermal simulations, this is good practice at first. However, with more confidence and experience you can get a converged solution for a 2nd order/Quick model with heat transfer, species transport and get convergence - from scratch! Its all down to the quality of the mesh and model set up. Carlos.

 February 28, 2008, 02:44 Re: Problem with Convergence!! #9 Elleana Guest   Posts: n/a Hi Carlos & Armin, Thank you very much for the valuable tips. My apologies for sending a delayed email as i was on a break. I have followed the steps and its working fine now. Thanks Kind regards Elleana

 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 Forrest_Lei OpenFOAM 3 July 19, 2011 06:00 commonyue Main CFD Forum 1 December 1, 2009 04:54 nasdak CFX 2 June 29, 2009 01:17 Emily FLUENT 2 March 21, 2007 23:18 Balraj Main CFD Forum 3 December 9, 2004 01:24

All times are GMT -4. The time now is 20:19.

 Contact Us - CFD Online - Privacy Statement - Top