Continuity convergence issue on a 3d wing
Hi all,
I'm modelling a section of a 3d wing with a cgrid topology using the kklw transitional model in Fluent. I have velocityinlet and pressureoutlet BCs and the side planes are periodic. I'm using Simple Quick as the solution method. Starting off with a steady solver, the residuals of continuity go down to 10^3 and then they remain in this neighbourhood. I then switch to the unsteady solver with a time step of 10^6 and residuals go down to 5*10^5 however this is not a good convergence level for me as the lift and drag do not stabilize and the flow is not developed. My main issue is with the continuity equation, although the same mesh works well in terms of convergence in CFX, I struggle in Fluent. My mesh quality is decent and I have already tried extending the boundaries further away from the wing body. Also I've tried using the Coupled solution method and decreasing the timestep and even using symmetry side planes but continuity doesnt converge. I'd appreciate any suggestions to resolve this issue. Nick 
Hi Nick you need to explain your case in detail. First I would like to ask a question for myself...you are working with structured or unstructured grid?? in which package you have created the grid?? ICEM or GAMBIT or something else??
Firstly use outflow at the exit with velocity inlet or use pressure inlet with pressure outlet, secondly what's your Reynold No??what's your Mach No?? at what Angle of Attack you are performing your analysis?? do you really need to switch to unsteady solver?? BTW 5*10^5 is not bad at all for the continuity equation..... for how many no. of time steps you have allowed unsteady solver to run before assuming that lift and drag are not converging?? explain these few points then i hope i will be able to help you Regards 
Thanks for your response. My AOA is 4 degrees and the structured hex mesh was created in ICEM. Reynolds is 100,000 (chordbased). The steady solver only goes down to 10^3. The unsteady solver's behavior doesn't change much with the number of time steps, it basically goes down to 5*10^5.
I am comparing two transitional models the SST transitional against KKlw. The SST transitional does better in terms of continuity in the steady solver since it goes down to 10^4 in fluent. The flow is incompressible BTW. Also my yplus is below 1 everywhere on the wing. 
Nick, how are you determining that the lift and drag are not stablized and that the flow is not developed?
Is there any other issue besides continuity residuals? Continuity residuals, or any residuals for that matter are poor estimators of convergence. I would double check the way residuals are defined for each program (scaled vs normalized, and their actual definitions) if you are concerned about residuals in different programs. 
Thanks for your answer. I can't quite follow what you mean by residuals aren't a good criterion for convergence. I monitor lift and drag for judging convergence as well as the residuals. Continuity is the only equation which I am struggling with.
Also I was wondering if anyone has had any experience with the kklw transitional model and come across a similar issue. I'd also appreciate it if you could inform me of the solution method with the highest resolution in Fluent. 
Quote:
how are you determining that the lift and drag are not stabilized and that the flow is not developed? residuals are not a good criterion to judge convergence. especially continuity because of the way it is calculated. monitor solution values. it is obvious that in an unsteady simulation, the lift and drag are also timevarying quantities. so how did you determine that they are not converging? did you compare instantaneous lift and drag or averaged? if averaged, how did you averaged and for how long? also, since it is an unsteady simulation, for which time step is 5e5? the information you are providing is not very clear and it is not even certain if there is a problem at all with your simulation. 
Quote:
I was reading this post and came across this sentence. Could you please argument some more on that? I would be really interested in knowing more. How is mass flow residual calculated? Why it is not reliable? Why generally residuals are not a good criterion to judge convergence? Thanks a lot. Cheers, ROb 
Quote:
Residuals are a measure of how much imbalance is left in each cell volume of the quantities, continuity (mass imbalance), momentum (in x,y,z). If additional models are used, there are more residuals for each equation (k,e or k,w for example, and energy). Usually the raw residuals are not reported. The scaled or normalized residuals are reported so that a relative convergence is reported. For continuity, the unscaled residual is the sum of mass creation. The reported residual by Fluent is a globally scaled residual, the unscaled residual is normalized by the maximum residual of the first five iterations. If the max of the continuity residuals during the first five iterations is very small, the scaled residual for continuity will have trouble reaching very small values. In practice, this is achieved by a very good initial guess. Actually, a perfect initialization of a flow with the actual solution will yield a scaled continuity residual of 1. My simulation is perfect, but if I were to use the reduction in residual as my convergence criteria, my simulation would never converge! Even if it did converge, it would converge to the wrong solution, since I know the scaled residual must be 1! On the other hand, the other scaled (momentum) residuals are calculated differently. The unscaled residuals are calculated the same way but they are normalized by the sum of their convective "speed" of each cell. This actually is not too bad to judge convergence, since if the residual is small then the imbalance is small. But being a large sum, it still does not give too much information about how well converged the solution is at each individual cells. With this method, individual cells can locally have very high imbalances across the cell (even nonphysical) without affecting the reported residual. Hence, although the imbalance is small overall, there is potential for individual cells to just be plain wrong. If this individual cell happens to be a critical cell, it can lead to very poor results. For normalized residuals, the unscaled residuals are normalized by the maximum residual after the first 5 iterations similar to the scaling done by continuity. These are the defaults for Fluent pressure based solver. There are also normalized residuals and the definition of residual is different for the density based solver but still similar. Also different programs use different methods, but similar discussion applies to them also. So far I have discussed global scaling, there is also local scaling whereby the unscaled residuals are normalized by the different in max and min residual of the current iteration. Notice I have not mentioned anything about solution convergence. In other words, there is no guarantee that any of my solution values have converged. Large oscillations in the solution are possible even while the residuals are small and decreasing. Also note that, the continuity equation is normalized differently. This is also the reason for the wellobserved result that, typically, the last residual to converge is the continuity equation / the continuity equation typically has the highest residuals. 
OK. I'm beginning to understand what you mean...so in my case a look at the unscaled residuals would be a better way to judge convergence in addition to the lift coefficient since the initial guess may mess it up for the scaled residuals ..is this correct?
also what i meant before was the flow is supposed to reach a steady state where lift doesnt change (according to experimental results) so perhaps I should only run it in steady mode and monitor the unscaled residuals and lift coefficient 
Quote:
flow will probably never reach steady state in an unsteady simulation! unless you magically hit a stable steady solution, probably only possible for a handful of laminar and trivial flow cases. Also, experimentally the flow is timevarying in nature. The experimental results are just the average of timevarying quantities to result in a timeaveraged and steady state answer. Flows are inherently timevarying, both numerically and experimentally, and physically! for unsteady simulations, you need to turn on data sampling for time variables. this will take running averages of all your quantities and you can then see averaged velocity, pressure, etc. I am not sure if averaged lift and drag are included, I doubt it. that is all the unsteady talk. but I don't see any reason why the problem cannot converge in a steady simulation unless you are specifically trying to extract the unsteady quantities. Running an unsteady simulation on what is supposed to be a steady state simulation will only mask the inherent instabilities, it is a crude workaround and does not actually solve the problem of convergence. 
Firstly i will sorry for not being around as i was very busy. I will fully stand by the facts explained by Lucky tran that residuals are not good criteria to check convergence. I have done many cases in which i got the converged solution for lift and drag while the residuals were still decreasing or oscillating(though small oscillations), so monitoring lift and drag instead of residuals is recommended. regarding steady vs unsteady solution will totally depend on what is the physics of the problem and how much accuracy you need in your results. Some phenomenon are inherently unsteady like flow separation from the wing at higher angle of attacks but in your case i don't think that at 4 deg there will be a significant separation, so steady state is fine enough but again if you are interested in v v accurate results then you have to have unsteady solution for this purpose. that's why i was asking for many time steps you have allowed the unsteady solver to run? what is your time step size?? is it small enough to capture the smallest cell in your grid?? do you have have the concept the residence time? these things are v important for the successful solution of unsteady problem....
kindly tell these and if still you are not satisfied and has any confusion feel free to ask. Regards 
Thank you both for your comprehensive responses. Given your explanation my solution has converged at 4degrees.

No problem at all, you are more than welcome at any time and i also want a little help from you regarding the structured hexa meshing on the wing, i know its not the relevant topic to be discussed here but try to tolerate me. I totally know nothing about hexa meshing and blocking strategy in ICEM and looking forward for some help, kindly help me by any means may be through a self made tutorial. thanks in advance
Regards 
The best tutorial I've come across for aerodynamic purposes is on youtube. Just run a search on ICEM airfoil and you'll find Simon's threepart tutorial. It'll teach you how to do 2d hex meshing around a foil. Anything more complex such as a 3d geometry would be variations on the 2d version.

I know how to do 2d hexa meshing on the aerofoil, i learned it fron that Simon's tutorials but i know nothing about the 3d hexa meshing, kindly help me in that

if you know how to do a 2d hex mesh around a foil, the 3d scheme will be easy for you. Instead of creating a 2d block begin by creating a 3d block and associate edges to curves accordingly in three dimensions. there is also another tutorial from ICEM where a wing is meshed in 3d

residual oscillation
Quote:
Could you please explain more about this? Because, in my case, monitor of solution value has gotten constant and the net flux imbalance of total heat transfer rate is also ok. But, the residuals are oscillating although they are decreasing. Thanks. Best, Sagila 
Hi all,
In my case i am making simulation on gas flow in room. it has velocity inlet and pressure outlet as BC , but i have a question my ke doesnt converge but all others converge (gas,velocity,energy) So what is the problem? And please give me some info about solution initialization ..i am quite unaware of it 
Hi all,
I'm modelling a a 3d rotor blade using density based transient solver in Ansys Fluent. I am using pressure far field BC and SpalartAllmaras turbulence model. I have problem with residuals. in fact the continuity residual doesn't go lower than 1e2 and other residuals doesn't go lower than 1e3 and remain constant or oscillate around. I have tried first order and second order implicit formulation, single and double precision. i also tried varying the initial condition since i thought it might be responsible for the problem. none of these didn't help. I have noticed that when i increase yplus on the blade surface (by increasing first cell width) i get better residuals. for example if i increase yplus to 600, continuity residual decrease to 1e3. I thought it might be because of aspect ratio but decreasing aspect ratio didn't solve problem. so what should i do? should i just ignore residual values and monitor lift and drag? what is causing this problem? I'd really appreciate any suggestions to resolve this issue. (I should apologize for my bad english. i hope this doesn't stop you helping me) 
All times are GMT 4. The time now is 08:28. 