I know that John (Mr. C. Chien) often put a lot of emphasis on mesh independant solution when dealing with finite volume methods and doesn't put as much emphasis when dealing with FDM or FEM. I remember that John said it was not as important for FEM because the convergence of these schemes is usually proven.

I want to discuss about this subject because recently convergence results were published by Gallouet, Eymard and Herbin in Hanbook of Numerical Analysis. In this book, these authors demonstrated convergence results and error estimates for "classical" FVM methods (cell centered schemes, one DOF per control volume). These results can be compared to those already published for FEM methods.

I know that getting a "mesh independant solution" is important. But it is often realy hard to do so because the conditioning of the system of equations gets worst when nodes (or elements) are added when the mesh is refined. Thus, the final solution is sometimes (not always) harder to get, specialy when solving poisson type equations. As you well know, in the real world, the solution also depends on the solver (even if it shouldn't.

When building a numerical method, I beleive that we should put more emphasis on the repsect of the rules given by the mathematicians. Because if we follow these rules we can say the scheme that we are using should give a better solution when using mesh refinements.

I suggest that It is important to get a mesh independant solution, but it is more important to use a scheme for which the convergence has been proven and error estimates hold.

Comments?

I totally agree with you on the importance of the method over the mesh refinement. In fact in LES, DNS of incompressible flow, it doesn't matter how fine the mesh is to resolve (or model) the turbulence if the method is not fully conservative (Mass, momentum and energy).

sincerely,

frederic Felten

(1). The mesh independent solution is a requirement, because you don't want your solution to change when you re-run the same case with a different mesh one year from now. (2). The convergence property of a numerical scheme definitely is a function of the mesh size used. For example, point S.O.R. will be slower than the line S.O.R. But, it is just a matter of computing time. You have to use a method which will give you converged solution in the first place. (3). Normally, the solution is plotted against the mesh size, so that you can see the trend. This trend will tell you how far you should go in mesh refinement. People have been doing this since 70's, so it is a common practice in CFD. (4). As the mesh is refined, you will also capture more flow features, and this could also affect the rate of convergence. (5). In addition to all of these, it is know that certain form of turbulence models are more difficult to converge during iterations. And sometimes, method to solve the turbulence model equation has to be changed to take care of the nature of the modelled equations. (6). And if you try to use low Reynolds number turbulence model, the convergence rate can be very slow relative to the use of the wall function approach. (7). These issues are common to FD, and FV formulations. In FEM, the approach is different. So, it is hard for me to address the mesh independent solution issue in FEM. (8). The other issue is that FDM will converge to the true solution by truncation error reduction (mesh refinement). For FVM, because of the approximation used in the formulation, it is harder to know whether it will converge to the same true solution or not. (conservation law is only part of the story. The classical control volume method is a good example. The solution satisfies the conservation law, but the result is 0-D.) (9). It is common to see the solution divergence after 10 thousand iterations. I had pretty bad experience with a commercial cfd code, which tends to diverge in a few iterations with a low Re model.

<< (1). The mesh independent solution is a requirement, because you don't want your solution to change when you re-run the same case with a different mesh one year from now. >>

1) It is well known that the solution of low order schemes is more dependant on the mesh than the solution of a higher order scheme. If you use a low order scheme, there is a very strong possibility that the solution will actually change with a new mesh. On the order hand, higher order schemes are often less stable than low order schemes and a realistic solution can be harder to get. And, if the stability are criteria of the higher order scheme are not met with the new mesh, the solution will change. conclusion: There is no perfect solution.....

<< (3). Normally, the solution is plotted against the mesh size,...... >>

3) I kind of agree with that statement. Shouldn't we say that we refine our mesh to see if we were able to get all the relevant physicals behaviors in the last mesh used?

<< (7). These issues are common to FD, and FV formulations. In FEM, the approach is different. So, it is hard for me to address the mesh independent solution issue in FEM. ... For FVM, because of the approximation used in the formulation, it is harder to know whether it will converge to the same true solution or not. >>

7) I must disagree with that statement. As I said earlier, FEM type theoritical results are now available for FVM methods that are properly designed. It was proven that when certain conditions were met (conservativity of the flux, consistency of the approximation of the flux, stability criteria...), a classical FVM method will converge to the unique solution of the problem. (The difference between the true solution and the numerical solution tends to zero when the mesh size (the diameter of the largest element) tends to zero).

<< (9). It is common to see the solution divergence after 10 thousand iterations. I had pretty bad experience with a commercial cfd code, which tends to diverge in a few iterations with a low Re model. >>

9) It also happened to me when my numerical scheme was not properly designed.

P.S. We talked about mesh independant solutions. Shouldn't we also discussed about time independent solutions for transcient and permanent flow? I beleive it is also an issue....

(1). There are two possible approaches to the mesh problem; one is to refine the mesh to reach the mesh independent solution,the other is to look for a better numerical model and algorithm. (2). The former approach is easy as long as the numerical scheme is not mesh size sensitive for large mesh size.(some methods are linear function of mesh size in convergence rate) (3). The latter approach is better if one can control the stability issue. (reduce the sensitivity to mesh size) (4). So, the optimum use of the mesh distribution and the numerical algorithm will provide the practical solution in doing CFD. There are a lot things can be done in these areas. And its impact on the CFD application will be huge. (going parallel computing will sink you deeper into the muddy water. (5). So, the future of CFD depends on two important technology: (a). mesh refinement to achieve mesh independent solution, (b). more accurate and stable solution based on limited mesh size. (RAM required today is not a problem at all, but the convergence and computing time is a critical issue). (6). Once these two problems are solved, one can focus on the turbulence modeling and physical modeling to get more realistic and accurate solutions.

Numerical issues aside, it may still be difficult to achieve grid independence while solving non-linear equations like N-S equations. Turbulent flows and flows transitioning turbulence are a couple of examples. When you refine the grid, you might capture certain spatial (or spatio-temporal) modes that can trigger some instabilities and change the large scale nature of the solution. This aspect is inherent to the discretization process and is solver independent.

Example : Laminar channel flow simulation at Re > Re_critical. If you use 10 grid points in the transverse direction, you can capture the parabolic velocity profile pretty well (what ever the inital profile may be). If you refine and use 20 grid points in the transverse direction, the solution most likely will not change. Does that mean grid independence. Obviously not. If you use 100 (or more) points, then perhaps the flow will transition to turbulence. At Re greater than the critical Re, both a laminar and turbulent solutions are possible but only the turbulent solution is truly stable. One may not know that unless a grid resolution that can capture the transition is provided.

(1). The first thing to learn in fluid mechanics is to know the difference between the laminar flow and the turbulent flow. So, one would not try to deal high Reynolds number flow as laminar flow. (2). I am not familiar with DNS approach, so it is hard for me to know what they are trying to get out of DNS for high Reynolds number flows.

When you can clear judge if the flow is going to be turbulent or laminar, there is no problem. Problem comes when you do not know the critical Re for a given flow geometry. The N-S solver should be able to identify the stable solution (laminar or turbulent) and converge accordingly. This identification may not be possible if the grid is too coarse for predicting transition. You may get a laminar grid independent solution before you reach the level of refinement needed for transition.

Grid independence is largely a steady state issue. In transient simulations of some flows, I doubt if even a RANS solver achieve grid independence. When you start to refine, you begin to capture smaller and smaller scales and these can interact with the large scale solution. Of course, if your scheme is highly dissipative (which was desired and considered a measure of stability at some point), the small scales are immediately dissipated before they can interact with the large scales.

I have a feeling that if you use a conservative, energy conserving (non-dissipative) scheme and a RANS model, you will never be able to get grid independence for certain transient flows unless you reach a near-DNS limit (in terms of grid spacing). Does any one have a different opinion on this.

(1). It is a tough question to answer. (2). So, in most cases, we need test data as a reference. If the test data is not picking up new features, then mesh independent solution should be possible. (3). On the other hand, if the test data keeps showing new features of the same flow with refined measuring technique, then I guess, you will see the same in the numerical solution. (4). High Reynolds number flows can be difficult to solve, because of the stability issue. If the Reynolds averaged equatione also run into the same stability problem, then I guess we are in big trouble. (so far I have not run into such problems for steady-state formulation.)

I think I have a good example of a laminar problem for which it is almost impossible to obtain a mesh independant solution. It is the liddriven cavity flow in 3D. If you keep increasing the Reynold number to certain level (I think it is near 10000), the flow becomes transcient and recirculation moving zones appear. Furthermore, if you keep refining the mesh, you get more and more recirculation zones. This last statement is also true in 2D.

(1). Well, that's interesting. Sometimes ago, I have seen messages presented here running the square cavity flow problem using various machines. (2). Is it possible for these readers to run a case at Re=10000, with a few cases of fine mesh? Just to see whether it will generate more recirculation bubbles? (3). I am open minded to this problem. Is it possible that certain numerical schemes will tend to promote instability? (4). So, the challenge is "can we obtain mesh independent solution for lid driven square cavity flow at Re=10000?" (laminar flow is assumed)

1) I don't know if you know Michel Fortin from the Universite Laval. Is a very well known researcher in FEM. Once we had a discussion about the liddriven flow. First, from the theoritical study of this problem, we know that the pressure goes to infinity in the right corner (the lid slides from left to right). Therefore, even for low Reynolds number (let say around 1000), the pressure in this corner will keep changing as the mesh is refined. this is not a matter of stability.

2) I know a book where the give a reference to a study of this problem (not Ghia) where mesh refinements was used to study this problem. They found out that the more they refinded the mesh, the more recirculation zones appeared. (Today, I will for this reference).

3) For Reynolds number around 10000 (the regularized liddriven flow with no singularity in the top corners or Reyaroudn 7500 for the true liddriven cavity flow), this not a matter of instabilitites, but the flow really becomes transcient with the appearence of hopf bifurcations. It takes a very accurate solver to get this transcient solution. A more robust scheme (more dissipative...) shouldn't give the appropriate solution to this problem. (Once I read an article about a similar benchmark where most of the commercial codes failed to correctly reproduce the bifurcations....). See the article Hopf Bifurcation of the Unsteady... at this location: http://www.math.psu.edu/shen/publications.html

4) I use a first order scheme, I won't even try to solve this problem. I know I should get a stable solution and not the transcient solution.... Furthurmore, even I get a mesh independent solution, this won't be the true solution (should be transcient...). If I ever succeed in getting a transcient solution, I should consider myself a very lucky researcher...

5) Conclusion: Shouldn't we put more emphasis on the true study of the theoritical properties of the scheme we use. Personaly, I always cross check my solution by solving a problem on three meshes. If the solution keeps behaving in the same manner for the tree meshes, I consider the last solution (the one given by the finer grid) as being the true solution for the limits of my scheme.

Is the Re of 10000 in this problem close to the critical Reynolds number. The appearance of more and more recirculation zones might indicate the periodic doubling type transition to chaos (turbulence). It this Re = 10000 is much lower than the critical Reynolds number, then this problem needs more attention. If the latter is true, could you point me to a reference where this problem and it's numerical solutions are discussed.

(1). There are several issues here: (a). a specific lid driven cavity flow problem, (b). mesh independent solution, (c). transient flow simulation. (2). If we take the unsteady-state, transient flow formulation, then it is really hard to know whether the flow will be transient or steady-state. This issue is hard to resolve, because of the approximate nature of the numerical scheme used, and the true nature of the flow. (3). If we take the steady-state approach to solve the lid driven cavity flow problem, then I am sure that the final mesh independent soltuion can be derived through the step-by-step mesh refinement. (4). If we look at the 3-D flow over the cylinder, we can see the complex structure of flow separation bubbles or vortices in front of the stagnation point. The flow visualization can be performed and test data obtained. (5).For the cavity flow Re=10000 is actually very high, so the boundary layer will be relatively thin, and you will see many features in this corner area (or actually the stagnation point region, if we look at the lid motion as the free stream flow approaching the vertical flat plate. (this is really not necessary, because such cavity flow near the corner can be tested in the lab.) (6). I think, for the steady-state formulation and solution, the mesh independent solution can be obtained through mesh refinement. On the other hand, if we take the transient approach, it is really hard to say whether a steady state solution can be reached. (this is similar to the case of flow over a cylinder at higher Reynolds number, where the oscillating vortex street exists. Steady state approach will always give you the steady state solution. and I don't think this is a problem.) (7). After having said that, now back to the mesh independent solution. I think, in the laminar flow case, the mesh size has to be proportional to the Reynolds number of the problem. So, this make the higher Reynolds number problem more difficult to solve (still laminar by assumption). (8). If we move from the laminar flow case to the Reynolds averaged equations, in most cases, the turbulent Reynolds number will be less than a couple of hundred. So, the Re,t is really very low in the major portion of the flow. (where the effective viscosity is the controlling factor) (9). AS a result, it is much easier to obtain the mesh independent solution in the turbulent flow regime when modelled as steady state Reynolds averaged equations.