Hello, I am trying to generate a Boundary layer in the floor of my model, but when I turn on the velocity contours in the post-processing analysis, the velocity at the floor remains 20-30 m/s. It does not get any closer to 0 than that… I am using a wall function with a y plus value of 150 to determine the first cell height for the floor in the inflate boundary layer section. I don´t know what I am doing wrong, could you have a look at my project to see how could I capture the boundary layer?
In this image I switched to cell data, to avoid the interpolation into the mesh nodes, which produces nicer plots but is less accurate. To do so, just right click the color bar and select ‘Switch to cell data’.
I do not understand why do I get such a bad range on the y+ on the floor as you mentioned, I chose a y+ of 150 and calculated the first mesh cell height for the floor… Also on the boundary conditions I chose wall function to model turbulence on the floor face. Should I have done something else?
With respect to the velocity not being 0 at the floor, I meant that when I look at it from the side I can not see any boundary layer forming at the bottom, do you know why this could be?
If you have a look at the y+ distribution at the floor, you will find that the bad range is close to the body legs, where there is a mesh refinement. This is why we recommend to use automatic layers, because your manual setup doesn’t take into account the variations in the mesh size.
With respect to the boundary layer, isn’t your second image showing it? What do you expect to see?
With respect to the boundary layer, I was expecting that the velocity at the floor wall would be 0 or very close to 0. Isn´t that how it is supposed to be?
Yes, you are absolutely right, that image does show that the velocity on the floor is 0. But I do not understand why when I look at it from the side, I can´t see a proper BL with 0 velocity at the wall forming…
Could I have modelled something wrong?
Dear @pl00447 , it is not possible to capture the development of the boundary layer using a y+ = 150 for the first cell. I am not completely sure if that is actually what you want.
When you use wall functions, most (if not all) of the development of the boundary layer occurs inside the cell. Therefore, it is not possible to "capture it. Visualization will show you the interpolation from the cell centre to the faces performed by the post-processor, but not the boundary layer. If you want to capture it, you need to use much smaller y+ values and capture the viscous sublayer. Check this link out: What is y+ (yplus)?
There is some interesting materials here: Wall function usage -- CFD Online Discussion Forums
Specially this link is very useful: http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2016/FangqingLiu/openfoamFinal.pdf
