Greetings to all! I have a pretty detailed mesh, quite poor convergence, and the residuals are concentrated in the finest mesh area. Glenn Horrocks mentioned some time ago that too fine mesh may create a problem. Anybody knows why and how? How to predict or determine the critical mesh size at the low end? Thank you.

in cfx post, u can use the mesh calculator to see how good is ur mesh

Yes, Richard, thank you; I did, and it is rather good: min face angle = 0.88-90; max face angle = 52-164; edge length ratio = 1.03-87 (1st inflated layer thickness = 0.04 mm; 20 layers), connectivity = 1-62, element volume ratio = 1-170. 250 knode, 710 kiloelement, 352 ktet, 352 kwedge, 5 kpyramids, 0 hex.

I think you have to improve your face angle to a minimum of probably 20 degrees,

regards Dan

ya. min angle should be >10, and ur connectivity >30

There are a couple of cituations when a "too fine" mesh can create problems. One is when you are using an explicit coupled solver. These often don't work that well in the highly viscous regions close to a wall so if you use a really fine mesh in the wall region they can show really poor convergence. I don't think CFX's implicit pressure based solver suffers from this problem though.

Another occation when a fine mesh can create problems is if you with a fine mesh resolve inherently unsteady flow-features and try to make a steady solution. A typical example is the trailing edge of a turbine blade. With a coarse mesh in the trailing edge region you seldom see any vortex shedding there and you easily get well-converged steady results with quite good predictions on the blade surfaces. If you on the other hand resolve the trailing edge very well you often catch unsteady vortex shedding in the wake. This makes the convergence in your steady solver poor and you can get quite poor results also on the blade.

I'm sure that there are other citations also when a fine mesh can create problems. But I think that these two examples are quite typical - the fine mesh can either create numerical problems or it can reveal new more difficult physics.

Hi,

Jonas has mentioned some important reasons why too fine a mesh can cause problems, and here are a few more.

If the mesh is too fine that can cause problems with single precision numerics. This is especially the case where you have a large range of mesh sizes, such as very fine mesh to resolve near-wall behaviour but coarse mesh in the distance. This is easily fixed by going to double precision numerics in most cases.

Resolution of wall flows in turbulent flows is a big challenge. Traditional codes use wall functions based on the logarithmic section of a standard boundary layer, that is y+>11 up to the start of the defect layer. This works well as long as the first node actually is located in the log-layer, but excessive mesh refinement can cause the y+ to fall below 11 and suddenly you are using a log layer profile in the viscous sublayer where the flow is completely different. This means grid refinement leads to the basic assumption of the boundary conditions not being applicable and your results will probably get worse and worse as you refine the grid.

CFX has helped overcome this y+ issue using the automatic wall function treatment. I won't go into details here (read the manuals) but it allows consistent behaviour and grid independant solutions with fine grids.

Also I am aware that extremely fine grids in the boundary layer (y+<0.01 approx) can lead to problems. I am not exactly sure what the nature of the problems are, whether it is numerical round-off, stabililty or a combination.

Regards, Glenn Horrocks

Yes, dear Richard and Dan, thank you for your advice. In my case, there is a very little percentage of small-angled cells and they are far from the regions of high residuals. High residuals are concentrated in in the area of fine- and high-quality mesh. Generally my mesh is dominated by the elements of connectivity ~ 20 and min. face angle ~ 40 deg.

Dear Jonas and Glenn, thank you very much for sharing your experience and expertise. I will now carefully examine the task at the angles of view you pointed.

Best regards

Steven

All the discussions here are only based on intuitive and practical experience. Did you all take the course of numerical scheme? Did you know the additional effects imposed to N-S equation by numerical difference scheme? Did you know coarser grid can bring more discrete grid viscosity to the numerical simulation? Therefore, more grid viscosity, the flow field more averaged, and easier convergence.

Hi Steven,

I think Jonas and Glenn make good points. Based on my experience and given that your mesh quality is reasonable, the problem is most likely related to either round-off, as Glenn suggested, or local flow instability, as suggested by Jonas.

The former is easily solved by running double precision, and I certainly recommmend this as it is easy to do. In the second case, the instability can be removed by increasing your timestep. Even if you mesh is fine enough to resolve turbulent vortices, you can avoid them by specifying a timestep which is larger than the local turbulent lenght scale. This will effectively "wash out" the local fluctuations. The effect of the local turbulence will then appear in the local turbulent kinetic energy and dissipation.

Finally, while these local effects may prevent convergence, it is sometimes reasonable to ignore the effect if it is away from regions of interest. If the MAX residual is more than one order of magnitude higher than the RMS residual, it usually indicated a local effect. What I often do is write the residuals to my backup file (there is option under Output Control>Backup File in Pre). Suppose the U Momentum is giving you grief, you can then create a new variable in Post equal to the absolute value of the U Momentum residual as:

abs(U Momentum.Residual)

and then create an isovolume of elements with residual values greater than your convergence criteria. This will show you elements where fluctualtions are occurring.

If this regions of fine mesh is far away from anything of interest, it may help in the future not to refine the mesh in that area (if possible).

Best regards, Robin

Robin (and Steven)

you said "you can avoid them by specifying a timestep which is larger than the local turbulent lenght scale"

I would assume you meant "time" scale.

This should be the local mean time scale or possibly one based on shedding frequency.

On another note: sorry, but I think it is going too far to make heuristic arguments about where the "effect of local turbulence will appear"

What the equations are actually simulating is anybody's guess since running a RANS model with internally generated unsteadiness is not the same thing as a proper LES/DES/DNS approach. Formally the RANS averaging process captures all scales of turbulence and the effect of ALL scales shows up as a steady term in the momentum equations: Reynolds stresses. Given the Boussinesq approximation this show up as eddy viscosity in the momentum equations which will dampen internal transient features.

Regards,

Bak_Flow

Yes, I meant time scale, thanks.

If you're going to nitpick, you should also add that the solver is not solving a time accurate simulation while running steady state. The point is that the oscillations may be due to the physics, not the numerics. If the local grid scale and the timestep are small enough, "Turbulence Like" instabilities will develop. Increasing the timestep will may increase the eddy viscosity and damp out these oscillations.

Is that better??

-Robin

[M.Meki]

Hello all,
I have been running a turbulent flow problem. The output velocity profile however, doesn't show zero velocity at walls!.
Dimension D=0.02m, L=10m
I am using an FLT of 1e-7m, 25 layers and 1.24 growthrate.
radial element size is 1e-3m and sweep size is 0.026m.

I have written a matlab m file and produced the correct velocity profile for this problem using viscous boundary layer y+=u+ for y+<5 and a standard log law for the rest of the flow. I found out that the viscous sublayer (y+=5) is about 1.4e-4 m.

The aspect ratio for the thin elements near the wall are 260 K! which is bothering me but not much that I can do about it. I thought I should run double precision, but the U-mom and V-mom solution fail (F).

Please help me.

[Jiricbeng]

How did you obtain the velocity profile in CFD Post? If you plot the contours of velocity on the walls, it should be zero (if you use hybrid values, not conservative).