Fluent5.0 technical assistance

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

 October 13, 1999, 14:44 Fluent5.0 technical assistance #1 sangrar Guest   Posts: n/a Hi, I am a Fluent5.0 beginner. Could you help me with a problem ? I am now running a laminar 3-D case with structured grid, segragated solver. It is very easy for me to get the converged results using 1st order momentum. But when I try the 2nd order momentum. It always spends a lot of time and cannot converge. I also try to change the Pressure-Velocity coupling from SIMPLE to SIMPLEC or reduce the under-relaxation factor that mentioned in the manual. But it still doesnot work at all. According to your experiences, Could you give me some other idea to get the 2nd order converged result ? ( Additionally, I find when I try a much lower entrance Re or a much coarse mesh, it can get a 2nd order convergence. ) Thanks a lot for your time. Sangrar

 October 14, 1999, 00:38 Re: Fluent5.0 technical assistance #2 Jin Wook LEE Guest   Posts: n/a 1) It is very natural that 2nd order equation is difficult to converge. 2) Many of my junior engineer says that 'it was not converged because residual is higher than convergence criterion of the code'. Of course, residual is very good indicator to judge the convergency. However, please do not absolutely depend on the default criterion provided by your package. You can judge the convergene by yourself. How about to check 'physical reality of the result', 'degree of the change of the result, iteration by iteration' and/or 'comparison with the experimental data or previously published data'...... Sincerely, Jinwook

 October 14, 1999, 12:29 Re: Fluent5.0 technical assistance #3 John C. Chien Guest   Posts: n/a (1). I do not know what you are trying to achieve. (2). Your experience is fairly typical among CFD users. (3). I do have suggestion that you try something more systematic. (4). First, make the problem 2-D. Then run the code using the first-order method. But, make sure that you set all of the residuals to 1.0E-08. Try to see whether you can get converged solutions. At that point, you should see the the residuals drop to below 1.0E-06 and level-off (flat). (5). Once this is accomplished, increase the mesh density (total number of mesh points or cells) and run the code again. You should do this and plot the results vs the mesh density. You should do this until the result is independent of the mesh density ( increase in mesh density has no effect on the result). (6). The next thing to do is: use the converged solution and the final mesh , set the numerical method to the second-order method and run the code again. At this point, you have a very good initial solution (converged solution) and a fine mesh to begin with, the only change is the numerical method. (7). If you can't get the converged solution with this second-order method, then then it must be a post-doctor research topic. (8). If you can obtain a converged solution with the second-order method, then you can repeat the same processes to solve the 3-D problem. (9). By the way, when eating a hamburger at a fast food shop, you don't have to put everything in it. It is perfectly all right to have a simple hamburger, no cheese, no tomatos, no pickles, no onions. (actually, eating at all-you-can-eat place, you still have to watch your diet or weight. Otherwise, you will have upset stomach .)

 October 14, 1999, 14:58 Re: Fluent5.0 technical assistance #4 Jonas Larsson Guest   Posts: n/a Are you sure that the Re number is low enough to allow a laminar solution? Your description of the problems sounds as if the case is turbulent in reality - when you use a finer grid or a better scheme you get less artificial viscosity to stabilise your flow and you obtain a chaotic or turbulent solution which wont stabilize. That is how it should be if your Re number is high enough.

 October 18, 1999, 02:05 Re: Fluent5.0 technical assistance #5 chris Guest   Posts: n/a Thanks a lot, it is interessting to see how experienced "cfd-people" raelize convergence. But I do not understand point 4.) >But, make sure that you set all of the >residuals to 1.0E-08. scaled residuals ? normalized residuals ? absolut ? How can I scale them ? >Try to see whether you can get converged solutions. >At that point, you should see the the >residuals drop to below 1.0E-06 scaled residuals ? normalized residuals ? absolut ? >and level-off (flat). Thank you

 October 18, 1999, 10:48 Re: Fluent5.0 technical assistance #6 John C. Chien Guest   Posts: n/a (1). It simply says that you should ignore the residual constraint, and set it to a very very small number. (2). If you can not reduce the residuals continuously, the flow is oscillating somewhere. It could be the boundary conditions or the mesh problem. (3). the easiest way to make sure that the flow field has converged is to compare the contour plots at two different times (or iterations). When the solution is converged, you will see only one contour plot instead of two. (4). I have been using FieldView to check the convergence based on this method. That is you look at the computed flow field variables directly using the contour plots from two different times (iterations). It is a practical approach.

 October 19, 1999, 02:06 Re: Fluent5.0 technical assistance #7 chris Guest   Posts: n/a Hy, the idea with the contour-plots is really good. I'll try. But nevertheless: If you take the residuals, do you "scale" or "normalize" them or do you take the absolute values ? I have in the moment the problem that my continuity-res is about 1 whereas the others are about 1e-4 ("scaled"). So what can I do ? I hope it is converged (after 3000 iterations..). But I "feel" that there is something with the different "scaling-features" in fluent, because I never had such high conti-residuals and the solution is nevertheless good if you compare it with measurements. chris

 October 23, 1999, 19:57 Re: Fluent5.0 technical assistance #9 Sung-Eun Kim Guest   Posts: n/a Hi client, Please keep in mind that laminar flow can become unstable at fairly low Re number. Examples are numerous, the most well-known one being symmetry-breaking and subsequent vortex shedding around a circular cylinder. The symmetry-breaking occurs around Re_D = 40. And solving the flow using steady option with full domain (without any imposed symmetry) at higher Reynolds number won't give converged solution. Can you please turn on time-dependent option with time step of roughly 0.001 L/U ?

 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 Lan CFX 5 September 12, 2015 10:09 Martin Bailon Main CFD Forum 3 January 31, 2011 14:39 ck3 FLUENT 1 July 26, 2008 23:42 sheila FLUENT 0 June 14, 2007 21:58 Jonas Larsson Main CFD Forum 0 May 6, 2005 13:35

All times are GMT -4. The time now is 11:56.