[zhixin]

Hi all,
I'been modeling using k-omega sst model. But I have some questions about the y+. In help document it says that y+<1, but there will be y+<0.02 in some places when I make sure the max y+<1, is it right?

this is frm CFDwiki

Boundary layer mesh For design iteration type of simulations where, a wall function approach is sufficient, y+ for the first cell should be somewhere between 30 and 300. For more accurate simulations with resolved boundary layers the mesh should have a y+ for the first cell which is below 1. A good rule of thumb is to use a growth ratio in the boundary layer of 1.2 - 1.25.

If you are uncertain of which wall distance to mesh with you can use a y+ estimation tool to estitmate the distance needed to obtain the desired y+.

As a rule of thumb a wall-function mesh typically requires about 10 cells in the boundary layer whereas a resolved low-Re mesh requires about 40 cells in the boundary layer.

it says that 40 cells in the boundary layer, but how can I ensure that? is that means I need to make sure the 40th cell within y+<some value?

Thanks.

[scipy]

ANSYS Fluent Theory Guide chapter 4.16. Near-Wall Treatments for Wall-Bounded Turbulent Flows (page 117 in the V17 version).

The thickness of the prism layer should be designed to ensure that around 15 or more nodes are actually covering the boundary layer. This can be checked after a solution is obtained, by looking at the turbulent viscosity, which has a maximum in the middle of the boundary layer – this maximum gives an indication of the thickness of the boundary layer (twice the location of the maximum gives the boundary layer edge). It is essential that the prism layer is thicker than the boundary layer as otherwise there is a danger that the prism layer confines the growth of the boundary layer.

Same goes for the near-wall model (above is for wall-functions approach). Run your solution and check the turbulent viscosity, zoom in on the near wall region and overlay the mesh display above it. If the max value is at the middle of the prism layer or below, you're all good.

P.S. Don't worry about the y+ of 0.02.. it's just important that it's less than 1, not equal to 1.

[zhixin]

Dear scipy,
I do what you quote but find the turbulent viscosity value seems to be smaller near wall compared to the core zone. By the way, My model is elbow.
Best.

[zhixin]

I may find the reason http://www.computationalfluiddynamic...oundary-layer/

I use structure mesh, and the turbulent viscosity near wall is small and increase ,here is the contour.

[scipy]

You might consider a more appropriate cut plane location and displaying only the local min/max values. You could try and investigate a case of a simple straight pipe (no elbow) first, try to get a fully developed velocity profile and check if the boundary layer is captured appropriately. This is what I usually do (some simple proof of concept case just to check the physics and then move on to the actual problem).

[LuckyTran]

Turbulent viscosity is small directly adjacent to the wall where viscous effects dominate. Turbulent viscosity then increases rapidly, reaching a maximum, and then decreases again as your approach the edge of the boundary layer.

From either your results or a good initial guess, you need to infer the boundary layer thickness and then try to pack 40 cells in there. While this is just a guideline, take the instructions literally. Determine the boundary layer thickness, and the pack 40 cells in there. A lot of people get confused with these guidelines because they try to second guess what the guidelines are. They are simply just take. Find the boundary layer thickness, make sure there are 40 cells.

[zhixin]

Thanks, I'll try.

[zhixin]

Thanks scipy. I'll do it again