y+ and y* issue
 

Hi all!

I am just starting using fluent for my simulations and in many bibliography the y+ and y* appears to be very important to make a right mesh, but the fact is that i still don't understant the meaning of these dimensionless parameters and their implications/utility for meshing?

Can someone explain them to me in plain english please?

Thanxs in advance!

Re: y+ and y* issue
 

Panton book "Incompressible Flow" develops the Law of the wall. In short, we cannot generate a mesh to accuratley capture the flow details inside a boundary layer, instead all CFD programmes represent the boundary layer by a single wall layer. The thickness of this layer is selected so that the law of the wall is valid. This is important because the pressure drop along the flow path depends on the skin friction which is calculaed from the Law of the wall.

Re: y+ and y* issue
 

Thanxs Ahmed. That was really helpfull.

So, from your reply I understand that near the wall CFD soft calculates flow fields following the law of the wall and not only the RANS, don't them?

The only think that I don't know is which is the interval of y+ in what the Yplus Plot must be limited by, depending on the model I use to solve the problem. Can you or anyone highlight me in this? For example, I've read that for the Spallart-Allmaras the Yplus must be grater than 30 or near 1 but not in the 1-30 region? Is that right? And for the other RANS models?

Many thanxs!

Re: y+ and y* issue
 

Once more:

http://university.fluent.com/blog/in...&pb=1#comments

The fourth comment in the above link to be precise.

Re: y+ and y* issue
 

Yes, the shear stress at the wall (Skin friction) is calculated from the Law of the Wall in all CFD programmes that I am familiar with. If you want to gain experience, insight about the acceptable values of Y+ (Y*) It will be helpful if you have the Law of the Wall plotted before you, most CFD/Fluid Mechanics books have that plot, just keep in mind that these published plots are taken from experimental data at zero pressure gradient, and because of this simple fact, CFD vendors advice (Recommend) lower values than those published (if you do not have access to such a plot drop me an email and I will scan the one I have and email it to you). Since you posted your question on this FLUENT Forum, I am going to assume that you are using this software, if so, you have no problem at all, if after carrying your analysis you find the values of Y+ to be high you can adapt the wall layer by going to [Adapt] -> Boundary and follow the instructions(Fluent will break each wall cell that you have selected into four smaller cells). Cheers and good luck with what you are doing.

Re: y+ and y* issue
 

Wow! Nice link pUl|: I didn't notice about this little Fluent forum. Thanxs, that was helpfull!

Ahmed: in point 11.9.1 of Fluent's users guide there's one plot of the law of the wall. And I've also found it in "Prandtl's Essentials of Fluid Mechanics" book. Know in this post I've realized about the importance of Y+ plot. With this, I conclude that I have to avoid the y+ located in the buffer layer, but new questions come to me:

1. In Fluent's users guide, it is said that Fluent makes calculations with the law of the wall for mean velocity when mesh is such that y*>11.225 and when it's lower than this value, it aplies the laminar stress-strain relationship U*=y*. So, this means that although Fluent makes this calculations, they would be not very reliable if I get a mesh with y+ values less than 30?

2. Which is the difference between y* and y+? Does Fluent always use y* for its calculations? In which manner does this affect in the recommended interval of [30,300] of y+?

3. When using Near-wall models (instead of wall functions), is still valid all the methodology done with y+ as we do when using wall functions? I mean, if plotting y+ makes still sense or I have to revise my meshes with other techniques?

I know the above was quite long ;) Thanxs a lot!

Re: y+ and y* issue
 

I can answer the thrid question quickly and so here it is:

When you use Enhanced Wall Treatment (EWT), you're really resolving the flow all the way down to the wall (actually the turbulence models are modified to work that way when you use EWT). Ergo, you need to maintain a very low Y+ value near the wall. The recommended range is (1 to 5) although a value around 1 is usually recommended. Creating a mesh with such resolutions is often tricky as one also needs to ensure that cell aspect ratios (ratio of one edge of a cell to the other) greater than 1:5 are best avoided. So plotting the variation of Y+ along the wall is still useful as you can check if your resolution is within prescribed limits. However, bear in mind that the turbulent reynolds number has to be below 200 or some such for the first 10 odd cells. This is mentioned in the Fluent Users Guide.

Good Luck!

Re: y+ and y* issue
 

Ok pUl|, many thanks. These days I am reading point 11 of fluent's users guide intensively to take care about all these things about the mesh size near walls. I hope I could answer the othr questions for myself in the following days, but those have came to me reading the user's manual xD. Specially the fact that fluent does not work directlly with y+, as he makes calculations with y* and that in some cases,it uses the linear equation U*=y* (I imagine that it is to have a solution "at any cost", knowing that the mesh is not fine enough to use standard wall-equations and the result may be not accurate)

I will keep working on that (and reading/searching the forum for new answers). Thanxs again!

If that is true, why do we still need to know Y+? Y* is already enough to make sure that the first line is inside the subviscous layer.

I know this is an old topic, but in the case anyone has a similar question in the future: The Fluent guide (for version 12.0) says on page 12-6: