What rules are others using regarding establishing the thickness of the first row of grids adjacent to a turbomachine blade surface? I don't understand Adapco's explaination of the need to keep the value of y+ near the cells centroid (how do i translate from y+ to a physical distance). I am working with an incompressible fluid.

The nature of the problem is that the first row of cells must allow the software's built in log-law wall function to work properly.

Hi Topic,

You probably know that the shearing effects of the no-slip wall boundary has a great influence on the flow-field. However, to accurately capture these effects without using a dense cell mesh near the surface, we use wall functions.

y+ in the turbulence sections of fluid dynamics books is defined as:

y+ = y/nu*sqrt(tau_wall*rho)

where y is the physical distance from the wall

nu is the kinematic viscosity

tau_wall is the shear at the wall

rho is the density of the fluid.

but since we do not want to worry about accurately computing the shear at the wall, the wall function used in the k-epsilon model is defined as (pg 6-3 of the Methodology Manual):

y+ = rho*C_mu^(1/4)*k^(1/2)*y/mu

This is just an empirical approximation.

These 'simple' wall functions assume that the shear stress is constant across the near wall region and the velocity increases logarithmically with distance from the wall to the turbulent region ("log-law of the wall") These wall functions kind of "connect" the wall shear stress to the fully turbulent region using the near-wall-cell. Therefore, we have to place the cell centroid at a "good" place, which is determined by

30 <= y+ <= ~100 (some texts say is is okay to go as high as y+=130-150)

Now, using STAR-CD, you can go to the STAR GUIde, go to Analysis Controls, and then to Output Controls and make sure that you are printing the y+ values to file. After the analysis is done, and after you load your .pst file, you can Get Wall Data to plot the y+. For more information on setting the controls, please refer to 8-2 and for plotting boundary data, please refer to 9-15 of the User Guide.

I hope that this was helpful to you, please let me know if you have any other questions.

Tara

I FAX'ed some sample calculations to Scott Wilinsky at Adapco's NY office on 8/2. Basically, I found that if I assume a free/midstream velocity of 15 m/sec for 200F fluid (ATF), the first cell should be about 0.75 mm thick. I got the fluid speed from a previous "good" run.

I was able to relate Adapco's use of y+ to its use in a turbulence text, which was helpful (Turbulent Flows, by Stephen Pope).

You have inadvertently raised part of the problem: Now that the grid is build and I can see what StarCD thinks the values of y+ are over the blade surface, what can I do with that information?

Does this mean that you understand now how to use the y+ values in the analysis? Unfortunately, like I was trying to explain, you don't really know exactly what your first cell size is until after you do the first analysis...at least a few iterations to get a rough idea. I didn't understand by your previous email whether or not you still had questions. I also work with Scott in the L.I. office, so if you would like to call me, or continue this discussion through the forum...feel free.

Tara

Actually,that is the problem. I currently must hand mesh the models I build, and was hoping for a technique to help with either the first estimate of adjacent cell size or a quick means of correction if I've really blown it (ie: adjacent cell thickness is either way too thick or thin).

Hi,

I understand the problem. When you create your meshes by hand, do you do it using prostar? If you do, have you thought about creating macros with parameters that you can change to create different meshes...sort of automating your task?

Tara