Can´t capture Booundary Layer

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?

Here is the link to my project: SimScale

Please ignore all the simulation runs expect for the ¨Mesh 10 run", this is what I believe its the most accurate simultion.

Thank you very much

Hi, and thanks for using the forum.

First of all, I will suggest you to always verify your y+ value in the post-processor. Look for example what I measured from your floor:

That is not a good range, and you should be concerned about the regions with y+ below 30.

On the other hand, why do you say that the velocity on your floor is not zero? I checked and it actually looks like it is:

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’.

Hello, thank you for your reply!

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?

Thank you very much.

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?

That what I just tried to show you in the post above, don’t you agree?

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?

I think that this is because of the way the coloring and interpolations in the postprocessor work.

Switching to cell data could help, but as you are looking from the side, the cell in the floor is not really visible.

Okay, then I shall assume that there is nothing wrong with the flow in that area.
Thank you very much for your help

1 Like

You are welcome!

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:

I hope this helps,

J.A. Gutiérrez

Thank you for the information! I will definitely have a look at the links you posted.