[Haider58]

Hye all..

I am doing 2D analysis on airfoil NACA 0012...
I want to get skin friction drag over the airfoil..It means I need to set y plus value of 1 to get into viscous sublayer...When I calculate Y plus it comes out to be 1.5 e^-5...but when I put this value in fluent, mesh orthognal quality gets disturbed and solution becomes unstable. Once I reduce value to 5 e^-4 in fluent, solution becomes stable but drag values doesn't match standard results.

Need help to adjust y plus value without disturbing orthognal quality of mesh..

Regards

[ghorrocks]

I want to get skin friction drag over the airfoil..It means I need to set y plus value of 1 to get into viscous sublayer.

Why do you say that? When used appropriately wall functions are quite good, and require MUCH less mesh resolution.

Very small values of y+ usually result in round off error causing convergence problems. I would think y+ around 1e-4 and 1e-5 is way lower than you want and will have major problems converging. And that is even the case even if you fix the orthogonality problem.

[Haider58]

[QUOTE=ghorrocks;703135]Why do you say that? When used appropriately wall functions are quite good, and require MUCH less mesh resolution.

Thanks ghorrocks for your quick reply..much appreciated.

I am new to CFD environment and really not much familiar with wall functions. I learnt through tutorials that in order to get good skin friction results, one need to go to sub viscous layer by setting y plus value equal to 1 and use SST turbulence model.

Can you please guide how and where I can make use of wall functions?

2. What is generally y plus value set to get accurate skin friction drag results? I get converged results for 5e^-4 value with orthogonal quality of 0.5..but according to y plus calculator, my y plus value should be 1.5e^-5..

details of my parameters are as follows

rho= 1.225 kg/m^3
L= 0.1524 m
y plus = 1
viscosity= 1.82^e-5
Vel= 20 m/s
Re n No= 200000

First layer thickness calculated by online softwares = 0.000015

Thanks and waiting for an early reply

[ghorrocks]

If you are using SST with automatic wall treatment, then if you coarsen the mesh to y+>11 then it will automatically switch to wall function mode.

Can you confirm your y+ and mesh sizes? y+ is a non-dimensional number, it is not measured in metres, mm, inches or anything. The size of the first mesh element from the wall is a dimensional number, it should be metres, mm, inches or some length unit.

Your calculation says y+=1, first layer thickness = 1.5e-5 but your text says your y+=1.5e-5. This does not look right.

[Haider58]

Sorry about that..it was a typo..

my y+ = 1

by putting y + equal to 1 and other parameters as mentioned earlier in on-line calculators available for calculating , wall spacing comes out to be 1.5e^-5....

Then I use this wall spacing value as First Layer Thickness in Fluent Meshing module..
My mesh size is 37000 nodes

[ghorrocks]

OK, now I know your real question:
You have a NACA0012 airfoil at Re=2e5 and low Mach number. You are using a mesh with y+=1. Your drag values are inaccurate.

A NACA0012 airfoil in the Re number regime will be in transitional flow. The front bit of the airfoil will be laminar, the rear turbulent. At this Re the transition point is likely to be around 25%-50% of chord length, so there is quite a significant amount of laminar flow.

This means you will need to have a turbulence transition model to accurately get drag from this case. Have you included a turbulence transition model? If you have not you will be grossly overestimating the drag as it will be assuming turbulent flow over the entire airfoil. Note that using turbulence transition models is not easy and they require careful validation. It is not a model you simply turn on and it gives you accurate results. You need to check your time step, convergence and mesh sensitivities again.

[Ugee]

while tetra meshing enabling both create prism layer and hexa core option but after mesh completion only tetra mesh is formed . trying two three times but hexa core and prism layer are disable in the resultant mesh .do you have any idea why create prism and hexa core are not working. also applied the delunary option for fluid domain but it is formed in shape like star shaped which is out of the geometry .
I am new to the tetra meshing please help

[karachun]

What help you expect if you even dont tell what program you use to mesh. And this is problem for new topic in meshing forum, nor CFX forum. OK?