[Loris88]

I have this problem illustrated in figure.


P=600 mm
H= 50 mm
L=3900 mm

The cube has these dimensions: 25x25x25 mm.
It is placed from the inlet at 2600 mm.

The fluid is air at 16.5°C and its velocity at the inlet is 24 m/s.
Reynolds number is 80000.

I don't know how determine the value of the y+ ...
I have read that if there is detachment of vein, y+ will be lesser than 1, for example 0.5.

So, I have opened this link http://www.cfd-online.com/Tools/yplus.php and I have calculated its value.
With my data and after seting up y+=0.5, I have obtained 5.6x10-6 m like "estimated wall distance".... then, in ICEM I have set up the first node to wall to 5.6x10-6 m.
But, after simulation with ANSYS CFX 14.0, I have obtained the max value of y+ circa 3.4689, so I have no convergence.

My question is: what is the real value of y+ that I have to used?

Thanks at everyone who will reply at this post!

[Hamidzoka]

Dear Loris;
y+ is function of velocity and physical properties of the fluid and also the wall-adjacent cell thickness. In CFD calculations, generally, the acceptable range for y+ strictly depends on the turbulence model that have been chosen.
Turbulence models are fallen in two groups: low Re and high Re models.
In low Re models you need to set lower values of y+ for near wall cells (say below 1.0) and therefore the first cell thickness should be quite little. In high Re models, unlike the low Re ones, y+ can be as large as 150-250 and subsequently first cell thickness can be much larger.
On the other hand, existing correlations for calculating the y+ are just initial estimations and needs modifications if the CFD results are not satisfactory. In other words, regarding the y+ you should always trust what CFD software calculates, not the simple existing correlations.
which turbulence model did you use for the simulation?

Regards

[Loris88]

Originally Posted by Hamidzoka

Dear Loris;
y+ is function of velocity and physical properties of the fluid and also the wall-adjacent cell thickness. In CFD calculations, generally, the acceptable range for y+ strictly depends on the turbulence model that have been chosen.
Turbulence models are fallen in two groups: low Re and high Re models.
In low Re models you need to set lower values of y+ for near wall cells (say below 1.0) and therefore the first cell thickness should be quite little. In high Re models, unlike the low Re ones, y+ can be as large as 150-250 and subsequently first cell thickness can be much larger.
On the other hand, existing correlations for calculating the y+ are just initial estimations and needs modifications if the CFD results are not satisfactory. In other words, regarding the y+ you should always trust what CFD software calculates, not the simple existing correlations.
which turbulence model did you use for the simulation?

Regards

Thanks Hamidzoka!
Thanks for your explanation!
I have high turbulence, Re=80000 I think that is an indicator of high turbulence.
Therefore, you say me that I have to use y+=200 for example. Is it correct? The value of circa 0.5 for y+ is used for low turbulece like Re=4000.

I have used SST model (Shear Stress Model) in ANSYS CFX... this model is been that that gave me better results. I also used SSG Reynold Model, but SST is better than SSG.

[Hamidzoka]

Dear Loris;
High or Low Re turbulence models has norhing to do with the Reynolds number of the flow. At each Reynolds number you can use either High or Low Re turbulence models. the word "high" or "low" only indicates the method that each turbulence model uses to resolve the flow at near-wall regions.
For example, in your case your turbulence model is SST. SST is a low Re turbulence model. It means that when you apply this model, whatever is the flow Reynolds number, y+ at first cells should not go beyond 1 to 3.
Therefore you need to adjust first cell thickness so that y+ lies in the range of 1 to 3.
If you use standard k-epsilon turbulence model instead of SST, you can have a y+ of 150 to 250. since this model is a high Re turbulence model.

Regards

[Loris88]

Originally Posted by Hamidzoka

Dear Loris;
High or Low Re turbulence models has norhing to do with the Reynolds number of the flow. At each Reynolds number you can use either High or Low Re turbulence models. the word "high" or "low" only indicates the method that each turbulence model uses to resolve the flow at near-wall regions.
For example, in your case your turbulence model is SST. SST is a low Re turbulence model. It means that when you apply this model, whatever is the flow Reynolds number, y+ at first cells should not go beyond 1 to 3.
Therefore you need to adjust first cell thickness so that y+ lies in the range of 1 to 3.
If you use standard k-epsilon turbulence model instead of SST, you can have a y+ of 150 to 250. since this model is a high Re turbulence model.

Regards

Aaah ok!
Thank you very much!
I did not understand this fact!
I thought that high or low were referred at Reynolds..
This is the first time I use Ansys!
Thanks!

[ferdy]

Originally Posted by Hamidzoka

Dear Loris;
High or Low Re turbulence models has norhing to do with the Reynolds number of the flow. At each Reynolds number you can use either High or Low Re turbulence models. the word "high" or "low" only indicates the method that each turbulence model uses to resolve the flow at near-wall regions.
For example, in your case your turbulence model is SST. SST is a low Re turbulence model. It means that when you apply this model, whatever is the flow Reynolds number, y+ at first cells should not go beyond 1 to 3.
Therefore you need to adjust first cell thickness so that y+ lies in the range of 1 to 3.
If you use standard k-epsilon turbulence model instead of SST, you can have a y+ of 150 to 250. since this model is a high Re turbulence model.

Regards

Hi Hamidzoka!

Reading this topic I have found some useful information for me as well, thank you!
I write here because I think it is easier for me instead of opening a new topic, bacause I have a problem very similar to the problem of Loris.
I am a student using for the first time Ansys, I have a geometry and phisical condition similar to these in this topic, but I am working at a simulation with SSG model (Reynolds Stress Model).
I was wondering about which y+ value I should use, because I don't exactly know if consider this models as low Reynolds turbolence model (y+ between 1 and 3) or high Reynolds turbolence model (y+ between 150 and 250).

I thank you so much in advance for this information.

Ferdy

[Hamidzoka]

Dear Fredy;
As far as I know SSG was first developed as a high Re number turbulence model. But some low Re version of it was proposed later.
I think the high Re version is used in Ansys.
Please note that the y+ range of "150-250" is not exactly applicable to all high Re models. in some models this range can be different.
Please follow the literature of SSG model.

Regards

[Aeronautics El. K.]

Hello all,

Adding to what Hamidzoka said, I would like to suggest before going deep into Computational Fluid Dynamics try to take some time to study some fundamental Fluid Dynamics.
So, regarding the y+ value, try to study about Prandtl's law of the wall or the log law. If you do this you will then be able to understand in which range y+ should be and why.
I hope this helps!

[lehoanganh07]

Hello, Hamidzoka
As you said: High or Low Re turbulence models has nothing to do with the Reynolds number of the flow, Its just model to calculate flow near wall.
So we can use each for even flow with high and low Reynold number?
Because, Book of Wilcox he said that for Low reynold number, we can use Reynold turbulent number (local turbulent or wall damping function) instead of function y+(dont have to find normal distance to wall) which is difficult to calculate in case multi and complex wall in the model.

[borhanalhoseini]

Dear Friends,
I encountered a problem. I have a series of data points (velocity and normal distance u, y) and my free stream velocity is 2.7(m/s), characteristic length of channel 6 inches....I sifted some references on how to find y+ and u+ from these data and unfortunately I do not know whether I can define u*=sqrt(moo/rho*du/dy) or i have to go through some iterations to find u*. I appreciate any help in this respect.