# Convergence problem

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

 November 19, 2000, 13:45 Convergence problem #1 suthichock Guest   Posts: n/a Hello everybody out there! I have a problem about convergence in my code. My code is FVM with Hybrid (UDS-CDS) differencing scheme and applied to steady flow in ventilated chamber. My problem is when I refine grid the program is not converge (convergence criteria is 1e-4) . It stay at some value depend on number of control volumes used. But it works well when apply to coarse grid. Does anyone have the experence to same problem ? How did you solve it? Any suggestion will please to me. Thank you in advance. Suthichock Nunthasookkasame. Post graduate student, Chulalongkorn University, Thailand.

 November 19, 2000, 20:51 Re: Convergence problem #2 Sebastien Perron Guest   Posts: n/a 1) Is your convergence criteria an absolute norm or a L2 norm? 2) What kind of linear equation solver do you use.

 November 19, 2000, 23:06 Re: Convergence problem #3 arun Guest   Posts: n/a what do you mean by convergence criteria in this case ? is it the non-dimensional mass residue ('b' as per patankar) from the continuity / p' equation ? is it a turbulent flow and accordingly modelled ? please clarify. meanwhile some temporary suggestions : 1. apply double precision throughout - if not applied so far. 2. if uniform grid, pick up the maximum 'b' - if the cv for max 'b' is next to boundary (my guess at this stage - a very common occurence), check equations and program. 3. if non-uniform grid, pick up the max b and min b and (max b/min b)ratio.if the ratio exceeds 1e+03 check if you have ever crossed the ratio of 1.4 (laminar) or 1.2 (turbulent) for any two adjacect cv dimension (for 3d problem in x-y, y-z and x-z directions). modify accordingly. some will argue that with grid refinement, it is a typical problem and has to be compromised for. wanted further discussion then.

 November 20, 2000, 08:46 Re: Convergence problem #4 James Date Guest   Posts: n/a I have also come across this problem when using a commericial FV flow solver, upon carring out successive grid refinement. In my case the problem was turbulent. I found that if the first cell size on any of the wall boundaries was too small, violating the law of the wall Y+ condition (i.e. 30 < Y < 500) the solution failed to converge. I also found that rapid changes in aspect ratio also contributed to non convergence of some solutions.

 November 20, 2000, 12:32 Re: Convergence problem #5 Chidu Guest   Posts: n/a Ofcourse, it could also be that the flow is unsteady and the coarse grid was so dissipative to give a steady solution. So when you refine the grid, it dosent converge. chidu...

 November 20, 2000, 13:36 Re: Convergence problem #6 suthichock Guest   Posts: n/a Hi Sebastien Perron . Thank for your quickly response. First question, My convergence criteria is calculate from sum of absolute resudual normalized by momentum flux at inlet for X and Y Momentum and mass flux from Pressure correction equation (term 'b' in Patankar) normalized by mass flux at inlet. Anyway i know not thing about L2 norm. Could you give me a short explain ation or reference ? Second question, I use 2 kind of linear solver for testing but it gave me the same behavior. They are TDMA and SIP.

 November 20, 2000, 13:47 Re: Convergence problem #7 suthichock Guest   Posts: n/a Hi Arun. Thank for your response. 1) My convergence criteria are the maximum of the residual from X, Y momentum eq. and pressure correction eq. For X,Y momentum, The absolute sum of residual are normalized by momentum flux at the inlet. For prssure correction eq, Yes , as you understand. 2) I did not use any turbulent model in my code. thank again for your suggestion. I will try to work follow your suggestion. Suthichock Nunthasookkasame

 November 20, 2000, 13:57 Re: Convergence problem #8 suthichock Guest   Posts: n/a Hi James Date . Thank for you response. Could you tell me what is Commericial FV code 's name ? Anyway, Do you have any ideas why grid size at the boundary effect the solution convergence ? Suthichock Nunthasookkasame.

 November 20, 2000, 14:06 Re: Convergence problem #9 suthichock Guest   Posts: n/a Hello Chidu. Thank for your comment. Do you know, I really agree with you about this. I ever try to use Upwind differencing scheme to this problem and solution is converged at the same grid used by Hybrid scheme. But when i refine more, It still not converge. So, my assumption is thefaulse diffusion (or numerical diffusion) which generate from UDS can damp some ossilate behavior. Suthichock Nunthasookkasame.

 November 20, 2000, 23:24 Re: Convergence problem #10 arun Guest   Posts: n/a do you mean your convergence criteria are three simultaneously (and not two !! because you have two mom eqs, u and v) viz., u-mom residue, v-mom residue and 'b'? please confirm you are using hybrid and not uds (first order ?). in such case suggest do the following : (1)don't consider u-mom and v-mom eqn residues - consider only 'b'. (2) see if 'b' attaining 1e-04 with coarse grid. (3) if it attains then check u-mom and v-mom res. if 'b' is <=1e-04 but u,v mom res are not, then check cv dimension ratio as i mentioned earlier. it should be <=1.4 (laminar) if using non-uniform grid. increase u-mom and v-mom sweeps. (4) if 'b' not attaining 1e-04, then first increase number of sweeps (just double them and >20) of p' eqn and then u-mom and v-mom eqs (i am against mom sweeps), i hope you have a u-v sequence solving to break the nonlinearity and coupling together.

 November 20, 2000, 23:45 Re: Convergence problem #11 Mukhopadhyay Guest   Posts: n/a 1. Grid aspect ratio is a very important 'aspect', which we very often neglect and/or ignore and then land up in mess. Any one can look at the book by Anderson et.al. 2. y+ <50 is also not a problem provided one uses the proper formulation and incorporates IT. In a commercial software I do not know how you do it. However, target should be to maintain 300 > y+ > 50. In reality the code should have the provision for checking the same. One can look at the publications of Rodi, Nallasamy and others for 2-layer , 3-layer models.

 November 21, 2000, 00:06 Re: Convergence problem #12 Mukhopadhyay Guest   Posts: n/a One question here : Is the steady state solution being attempted thru the solution of elliptic equation or parabolic equation with so-called 'false transient' approach ? If the second one is true, then how is the adequacy of calculation of residuals for momentum equations being taken care of ? Will Suthichock please let us know ? I believe there is the clue. Where is our friend, philosopher and guide John.C.Chien ?

 November 21, 2000, 04:51 Re: Convergence problem #13 Fred Uckfield Guest   Posts: n/a I get this behaviour all the time in my applications. If you have discrete jets interacting with solid walls or plumes interacting with a stratified environment then natural instabilities can make it difficult to obtain the steady state solution. Diffusion (real or numerical) will always help the jets to settle down as will damping down the velocities either by underrelaxation or reducing 'virtual' time steps (if you are using that approach). Actually using a pseudo time stepping approach in systems that are inherently unstable wil lead to periodic variations in the residuals that itself is a good indication that there is no steady state solution (or at least you are in or near a transitional state). The N/S equations know what should be going on and comprehend how they are being solved, they will react according to how you treat them (just like women). Fred.

 November 21, 2000, 06:41 Re: Convergence problem #14 suthichock Guest   Posts: n/a Hello Arun. Normally , I uses Hybrid in my code. I thought that it quite stable. But some time I try the other scheme to compare the results. When i read the response massages most of these talk about CV ratio. Could you explain to me how the grid ratio effect the solution? Suthichock Nunthasookkasame

 November 21, 2000, 08:48 Re: Convergence problem #15 Sebastien Perron Guest   Posts: n/a 1) I have read the other messages concerning your problem. I had the same problems using an hybrid scheme. My problem would converge with an upwind sheme but wouldn't with the hybrid sheme. If you want to get rid of some of the false diffusion with the upwind sheme I suggest using the power law sheme. You'll will obtain better results and it is far more stable. 2) The L2 norm of function f is : sqrt( integral (on domain) f^2 dV ) For a discrete problem it is similar to the norm you use. 3) The norm you use is a sum, if you increase the numer of unknows this norm will get bigger. In order to avoid this, It is better to sum over the residuals which can be multiply by their associated volume (or surface in 2D) i.e. |r| = sum_i r_i*dv_i 4) What kind of scheme do you use to solve the incompresible flow (Simple, Simple, Simplec, Chorin'a algorithm or derivative)

 November 21, 2000, 09:51 Re: Convergence problem #16 James Date Guest   Posts: n/a The code is CFX-4.3. I'm note sure which boundary you are referring to? If you are referring to the outer boundary, the grid should be as smooth as possible, however if the boundary is placed far enough away from the major distrubances in the flow, hence the flow gradients are small, rapid changes in aspect ratio, cell size, etc can often be got away with. I hope this helps.

 November 22, 2000, 00:20 Re: Convergence problem #17 Mukhopadhyay Guest   Posts: n/a Suthichock Sorry to intrude. I refer to your posting addressed to Arun re : 'how the grid ratio effect the solution ?'. 1. Suggest consult 'Computational Fluid Mechanics and Heat Transfer' by Dale.A.Anderson, John.C.Tannehill and Richard.H.Pletcher (Hemisphere,1984), p.358 and chap.3.[John.C.Chien, you agree I hope !] . Additionally you may consult the book 'Applied Numerical Methods in Engineering' by B.Carnahan,et.al. You will get a feel of consistency, stability, convergence and various kinds of errors in solving PDE thru FDE. 2. In our working group, with whatever little experience we have, we observe that dimension ratio for two adjacent cvs [delta-y(i)/delta-y(i+1)] should be 1.2 max (tur) and 1.4 max (lam) for majority of the problems we have handled. We also ensure that the aspect ratio of any one cv (delta-y/delta-x) does not exceed 1.4 in critical regions. 3. I tend to look at the problem this way, I wish I had mathematics to support (any help by anyone please ?): We estimate the acceleration thru the mom eqns and hence the speed at which the information gets transmitted should depend on the constrain we impose thru the cv dimension (time step apart). In first order upwind, this is partly taken care of because only the upstream is considered. In central diff or hybrid (cd+ud) scheme we incorporate the downstream also while the estimate is to be arrived at thru 'our' imposition of cv dimension. Hence we are putting a binding on the speed of transmission of the information (e.g., the BCs). This leads to problems.

 November 22, 2000, 17:23 Re: Convergence problem #19 Chidu Guest   Posts: n/a dude! I hope you are aware of a literary construct known as a paragraph!! If yes, please try to use it. The intention is not to be rude here, your posting did take me by surprise. I have never seen such a mass of words. regards, chidu...

 November 22, 2000, 18:40 Re: Convergence problem #20 John C. Chien Guest   Posts: n/a (1). That is because we are all having convergence problem! (2). Thank you very much for your patience to read the long message. I can assure that when I run a commercial cfd code, it takes much longer to converge, several days to a couple of weeks to converge. I had to run the same case several times because it normally would diverge several times. (3). Everyone would be very happy to use CFD if someone could show us the 1-2-3 step 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 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 16:04.