Mesh effect on wall shear and velocity
 

Dear foamers,

I am comparing my High Re straight pipe simulations with some experimental data, using RANS turbulence and a wedge geometry in blockMesh. When trying to refine my mesh from 60 cells to 100 radially, I experience that the computed velocity gets better, but wall shear stress gets far worse. Keeping increasing the cell number similarly increases the faulty wall shear stress. This also happens if I still use 60 cells, but adding expanding cell size feature.

May all this be related to having first cell within y+ <5 , or is there something else to this?

Thanks

Hi,

If you are using turbulence models that make use of wall functions, you need to keep your y+ above 30. If you want more resolution, switch to a low Re turbulence model without wall functions, or keep all your nodes at a y+ > 30.

Just to make you more confident with the code, I have obtained an almost perfect experimental vs numerical match for both wall shear stress and mass transfer coefficient using a low Re turbulence model without wall functions (Launder-Sharma) for a wedge geometry.

Regards,
Jose Santos

Thanks for your quick response Jose,

I did use Launder-Sharma for a low Re case, and even with wall functions (that is, using the built-in functions for k, epsilon, and nut) the results were pretty good.

Would you use the zeroGradient condition instead of the built-in wall functions?

Even it is "low Re turbulence model", it is not specific for a flow with low Re values, instead the difference to standard turbulence models is that it solves the fields up to the wall, without wall models. Therefore, you need more cells near the walls to get a proper description of your flow.

If using a low Re turbulence model, I think its better (I read it somewhere in this forum) to use a very small value for k and epsilon, eg 1e-30. Anyway, it will work with zeroGradient as well.

Regards,
Jose Santos

Right, I have heard about using those non-zero conditions ..

Did you ever try this for higher Re? In my case I am in the range 50000 - 300000.

I have tried it for Re = 20000. My friction factor results were 5-10% higher than the Blasius equation, which I suspect was mainly due to the uniform inlet velocity profile I assumed. Just make sure your y+ < 1.

Regards,
Jose Santos

Great. Using a low Re actually works for higher Re .. I wouldn't have guessed ;)

About the nut file, would you set it to ~0, zeroGradient, or delete it and let OF create it by itself?

I dont think you need to have it in your 0 folder, it will be calculated during run-time from k and epsilon.

Regards,
Jose Santos

Right. Well, the reason I'm asking is because nut is created/calculated, but automatically set with condition nutWallFunction for walls. As I have disabled wall functions for epsilon and k, I am not sure whether this also should be turned off (by force by having this file in 0/ initially, set to something apart from the wall function) or just leave it with using the nut file that is automatically created, yielding some sort of quasi wall function setup...

Just to be on the safe side, set nut in 0 in the same way you defined k and epsilon.

Regards,
Jose Santos

I had some mixed experiences now using this method - even the cases still running with wall functions are not that bad. In short, when not using wall functions, the result is pretty much similar to the red graph here. Did you experience results like this?

(I have performed several reruns using different mesh, but I can't really get it as nice and curvy (in the top part) as with the experimental results.)