Hi all,

I am trying to understand how really affects the mesh in the solution for a well-known problem like the flow past a sphere (D=0.1m) I am performing series of simulations, all at Re=1.4e4 and where the Cd should be 0.4, according to several experimental data also performed at Re=1e4.

The fact is that I am not able to see a logical correlation between the Y+ and the accuracy in the solution depending on the turbulence model deployed in the simulation. Let me show you my little results:

===Simulation 1===

-Velocity inlet: v=1m/s

-Turbulence Int=0.1%

-Hydraulic diam=4m

-Mesh: boundary layer composed of 4 prisms, first row is 3mm thick and the other 3 grow geometrically at a ratio of 1.2

-Solutions:

k-e Realizable, QUICK, Std wall functions -> Cd=0.303

k-w SST, QUICK -> Cd=0.357

Y+ in both cases goes from 2 to 18, which is not suitable for Std. wall functions, as showed in Fluent manuals (well-known recommendation of 30<Y+<300)

===Simulation 2===

-Velocity inlet: v=1m/s

-Turbulence Int=0.1%

-Hydraulic diam=4m

-Mesh: boundary layer composed of 10 prisms, first row is 0.5mm thick and the other 9 grow lineally with a slope of 0.5 up to a thickness of 15mm

-Solutions:

k-e Realizable, QUICK, Std wall functions -> Cd=0.363

k-e Realizable, QUICK, Non-equilibrium wall functions -> Cd=0.392 (convergence is difficult)

k-w SST, QUICK -> Cd=0.51

Y+ in both cases goes from 0.5 to 2.5

I don't really see that following the criteria of 30<Y+<300 the results would be the best. What do you think?

My headache and worry now is to understand and be able to make simulations that are mesh-independent. How can I rely on my mesh? Do you know literature on the internet or book where I can read about this issue of mesh-independency solutions?

Thanks a lot for your opinions in advance!

Is it really important Y+?

It depends on what are you calculating and how are calculating. If you are interested in near wall phenomenas that way you Y+ should be low (<1 even). But the mesh independency is an issue not really coupled with Y+. If your are interested on perform a grid convergence analysis you should first define some important variable (for instance if you are calculating drag coefficient in an airfoil you should chose that variable) and then just calculate severals solutions with different grid sizes until your variable chosen don't change, that way you case would be grid converged.

regards

Hello, Pablo has a good point. The Y+ value can be considered an indication of the size of the first cell height and if wall functions are employed or not.

Basically as you move your grid closer to the cylinder you will be predicting pressure/velocity gradients AWAY from the shape more accurately.

To look at grid independence I would try varying the cell sizes parallel to the surface of the shape. e.g. for an aerofoil use 25, 50 then 100 cell points along the chord length to generate 3 grids. Once you are happy grid independence is achieved then try varying first cell heights.

Also, to truly assess grid independence, the Grid Convergence Index GCI by Roache is a good way of scientifically assessing this important feature of CFD.

Carlos.

Thanks for your info Pablo and Carlos. I am trying to follow now your advices and keep benchmarking Fluent on the problem of the flow past a sphere as I exposed you in the first post.

But what I am really worried about is in the fact that regardless the grid adaptions (with the adapt function available in fluent and adapting by Y+ -trying to keep it between 30 and 300- and also by velocity magnitude), I am not able to get a Cd about 0.4 as literature says, and I keep getting strange Cd values like 0.12 or 0.5, too far from that ideally 0.4.

I want to believe that with this parameters: 1. k-e Realizable (or k-w SST), non-eq wall functions for near wall treatment. 2. 2n order discretization schemes (perhaps for the pressure is not necessary) 3. Keeping Y+ around 30<Y+<300 (because I use non-eq wall functions)

I MUST obtain that Cd=0.4, but it is not the case yet. I will keep simulating, but as I told you I quite worried...

Por cierto, sois españoles ?? Tenéis mucha experiencia en esto del CFD? Mi gran asignatura pendiente es obtener resultados aceptables teniendo un criterio claro para hacer la hacerla malla... por ahora no parece que seguir los criterios de Y+ ayude mucho. Bueno, seguiremos en inglés por respeto a los que estén leyendo esto también.

Un saludo,

Hey guys, I notised another problem: is it not possible to coearsen the grid during a grid Y+ adaption?? I read this in the Fluent manual:

"If you are using the default hanging node adaption, you will not be able to create a grid that is coarser than the original grid. For this, you must use conformal adaption that is conformal coarsening which is only available for 2D or axisymmetric geometries"

And I guess it is true, because when I do a mesh coarsen, Fluent says:

Grid size ( original / adapted / change)

cells ( 311138 / 311138 / 0)

faces ( 691259 / 691259 / 0)

nodes ( 96370 / 96370 / 0)

So there is no change! Does it mean that I have to go back to TGrid and re-mesh again the prisms from the boundary layer in order to obtain values of Y+>30?

Thanks a lot in advance again folks,

Freeman

Is Cd=0.4 for fully turbulent flow? Have you checked your reference values (free stream velocity, density, area)

If you are doing well, you should not have problems.

No soy español, soy de Chile. Saludos, suerte en tus cálculos.

Hola Pablo!

You can see it by yourself:

http://img216.imageshack.us/my.php?i...uentreswi6.jpg

This is one of the simulations (sphere of D=0.2m, vel.inlet=10m/s, hydraul.diam.=4m, turbulence int.at inlet=0.1%, Re=1.37e5, expected Cd=0.4, turbulent regime but still laminar boundary layer)

k-e Realizable, non-equilibrium wall functions, 20<Y+<80, QUICK scheme (2nd order discretization), boundary layer mesh is composed of 4 rows of prisms, being the first of them of a height of 3mm and the others growing geometrically with a ratio of 1.2... and the Cd is around 0.112!!

I think I've failed with this case: any other improvement suggestion before I give up? I will try now with the Ahmed body: I have more literature, not only over the experimentalset up, but also several papers on successful CFD resolutions.

We keep in touch, 1 saludo a Chile. Freeman,

Hola,

How many iterations have you left your simulation running for? Sounds to me like you may be experiencing convergence error whereby your solution is not actually converged.

Try iterating for up to 10,000 iterations with a drag monitor and see what it and the residuals look like. They need to be flat really. I have experienced convergence after 9,500 for complex 3d geometry.

Also, look up convergence error, its very important to understand.

Carlos.

For a flow past a sphere, the drag will be influenced by the recirculation behind the body. And this is very difficult to model, i.e. the turbulence models handle this badly regardless of the Y+. I should think that the Cd would be difficult to calculate correctly using RANS, and if you really want results with better accuracy than 10-20% as you get, you should try LES. If you just want to examine the Y+ influence on a result, you should choose a simple problem, like e.g. a channel flow where the turbulence models do better.

With y+ < 5 you should use Enhanced Wall Treatment for k-epsilon model. For flow past a sphere, y+ > 30 may lead to a coarse mesh that cannot be accurate. It is a complex flow and you may only get good result with y+ < 5 (y+ < 1 is better) and using Enhanced Wall Treatment.

I did a very similar case to yours, but was interested to surface heat transfer. Only very fine grid (y+ < 2) gave result that agree with the literature.

Check if there are not an over production of turbulence energy at the stagnation point (where flow impinge the sphere) since the standard k-epsilon may lead to it.