CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   Prism Layer (Boundary Layer) Thickness (http://www.cfd-online.com/Forums/star-ccm/115276-prism-layer-boundary-layer-thickness.html)

Peter-27 March 27, 2013 09:55

Prism Layer (Boundary Layer) Thickness
 
Hi,
i'm using the Star-CCM+ software to model a vehicle and a little confused about the prism layer thickness.

I know that the prism layer is to model the boundary layer, but the equation for boundary layer contains the Reynolds number. The Reynolds number changes at each point along the length of the car which will mean that the boundary layer will change.

Therefore, what should my prism layer thickness be as prism layer thickness can't change along the length of the car ..

Thanks in advance,
Peter.

rwryne March 27, 2013 15:32

Quote:

Originally Posted by Peter-27 (Post 416739)
Hi,
i'm using the Star-CCM+ software to model a vehicle and a little confused about the prism layer thickness.

I know that the prism layer is to model the boundary layer, but the equation for boundary layer contains the Reynolds number. The Reynolds number changes at each point along the length of the car which will mean that the boundary layer will change.

Therefore, what should my prism layer thickness be as prism layer thickness can't change along the length of the car ..

Thanks in advance,
Peter.


Calculate boundary layer for the end of the vehicle, set prism layet to capture that.

i.e. if you were doing a flat plate 1 m long, you would use "1 m" in your boundary layer calculation. Overkill upfront, but it ensures you capture it all.

ggulgulia April 6, 2013 13:37

Hey Peter

I am also very new to Star CCM+ and this question has perplexed me too.. Even I am trying to figure out the logic behind the first prism layer thickness value, however the default values are 33 % of the base value. If your flow is laminar or highly viscous in the region of interest, you can reduce the value to 20% or even lower and use the all y+ wall treatment model with fine mesh around the region of interest. This model blends the viscous and turbulent profiles smoothly.

The finer mesh in the region of interest can be obtained by accessing the following in Star CCM+ Region of interest(Wall Type Boundary)> Mesh Conditions>Custom Boundary Growth Rate> Slow, Medium, Fast options are available you can choose among them depending upon your flow.

I hope this was useful

Alamaas June 18, 2013 06:54

Hi everyone!

If my prism layer has 10 cells (for example) and the overall thickness of the prim layer is equal to the boundary layer thickness, do i still need to worry about y+ wall treatment or is it automatically taken care of?

Thank you!

SailorLiu January 5, 2015 12:49

Hi Alamaas, I know it has been a while since you posted. But I recently have an exact problem as yours. Have you finally figured it out?
As far as I am concerned, there are two parameters defining the boundary: the overall boundary layer thickness and the distance between the first cell and the wall. I read from elsewhere that there should be at least 10 cells inside the boundary layer while in order to use wall functions, you also need to make sure y+ should lie between 30 and 300. Besides, the growth rate should be best set as 1.2-1.25. There are just so many variables to consider. And I doubt all of them can be satisfied at the same time. BTW how do you determine the boundary layer thickness when you generate mesh? Do you use the Blasius solution for flat plates? Cheers,

Best wishes,

Yuanchuan
Quote:

Originally Posted by Alamaas (Post 434621)
Hi everyone!

If my prism layer has 10 cells (for example) and the overall thickness of the prim layer is equal to the boundary layer thickness, do i still need to worry about y+ wall treatment or is it automatically taken care of?

Thank you!


KateEisenhower May 6, 2015 03:55

Quote:

Originally Posted by SailorLiu (Post 526192)
Hi Alamaas, I know it has been a while since you posted. But I recently have an exact problem as yours. Have you finally figured it out?
As far as I am concerned, there are two parameters defining the boundary: the overall boundary layer thickness and the distance between the first cell and the wall. I read from elsewhere that there should be at least 10 cells inside the boundary layer while in order to use wall functions, you also need to make sure y+ should lie between 30 and 300. Besides, the growth rate should be best set as 1.2-1.25. There are just so many variables to consider. And I doubt all of them can be satisfied at the same time. BTW how do you determine the boundary layer thickness when you generate mesh? Do you use the Blasius solution for flat plates? Cheers,

Best wishes,

Yuanchuan

Hi Yuanchuan,

I am just answering to your last question now. Generally, I would use the Blasius solution for laminar flow and the Prandtl solution for a turbulent boundary layer.
Regarding your other question, I have to do some research first. You should at least take into account your choice of turbulence model and whether you are using wall functions or not.

Have a nice day,

Kate

Fiedde1887 May 19, 2015 13:01

Hi, iīm also working at my boundary layer. My scenario is a propeller at open-water conditions. I try to set a boundary-layer which is scientific correct. I used the Prandtl-formula and calculated the over-all thickness of the layer. After that i calculated the closest cell to the wall.
The results gave me an over-all thickness of 2.1mm and a cloesest cell of 0.00456mm for a y+=1. If the closest cell is larger than 0.01mm the solution converge, but if itīs smaler it doesnīt.
Does anyone have a hint for my problem?

Thank you in advance
Nils

Fiedde1887 May 21, 2015 09:59

I solved my problem. I used the Distribution Mode: "Wall Thickness" and the "Hyperbolic Tangent" Stretching Funktion. If the mesh is still bad, i can use "Cell Quality Remediation"...it works fine ;)


All times are GMT -4. The time now is 17:43.