CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   boundary layer, very urgent (

nicolas July 18, 2006 03:33

boundary layer, very urgent
Hi. I am a beginner in CFD. I use ICEM CFD 10.0+ cfx 5.7.1

I have a cylinder+ some others parts of a engine. I used blocking + hexa mesh for everything under ICEM. I used O grid generation, and I created a small volume around the wall, to set a fine mesh here. Someone told me that , with hexa mesh, I did'nt have to care about the boundary layer(but i need to have a fine meshin this volume). What i understood, is that I don't care about the position of the first node, and the law mesh in this volume.

Is it right? wrong? I found no explanation on websites, documentations, on "how to" do a boundary layer when using hexa mesh (i found it for prism, tet)... Do I need to set exponential law in the small volume around the wall(and how to do it?)

Does someone can help me to understand how to treat the boundary layer under icem, using hexa mesh (and o grid generation).

If it is explained on doumentation, can you give me the references ?

Regards, Nicolas.

Kramer July 18, 2006 05:46

Re: boundary layer, very urgent
Which kind of turbulence model do you want to use :

k-epsilon, k-omega, SST, or something else?

SST for example needs an y+ value of approx 1 (=>very small first element on the surface). So you will need a fine mesh in the boundary layer and at least 15 hexa elements in the boundary layer.

nicolas July 18, 2006 06:00

Re: boundary layer, very urgent
I use SST.

To know the distance, where i need to set the 1st node(if i choose y+=1),I need to know the Reynolds number? In a certain way, i need to know the solution, before being able to create a good meshing for the boundary layer?

other question: do you you know how to fix the distance between the wall and the 1st node, and, in the same time, set a expansion law (i have found how to set the expansion law, but i can't fix the distance). I use icem

thanks, nicolas

Kramer July 18, 2006 06:36

Re: boundary layer, very urgent
You have to make a good guess for your first node distance, its depending on the flow situation (estimate Reynolds number...)

For example: i have simulated the flow around an airfoil with SST an had to set the first node at 0.01 mm to get y+ <= 1.

Seconde question: there is an overall option to set the distance for the first node generally (settings an so on..., i dont remember exactly where), but independent from that you can use the spacing function (right there where u define expansion law) to set the value

Joe July 18, 2006 08:52

Re: boundary layer, very urgent
Read the section in the turbulence modelling section entitled something like "Advice on near wall meshing".

imad July 18, 2006 09:58

Re: boundary layer, very urgent
Dear Nicolas under blocking you find pre-mesh params select them and use edge params to select the edge near the wall and define the distance for the first and last point and if you want the mesh law

nicolas July 18, 2006 10:23

Re: boundary layer, very urgent
Dear imad, i already try this. but i dont understand how it works. to set the distance from wall to node ->i sould use the values called in the software "spacing 1" and "spacing 2" ?? thanks for your reply. Regards, Nicolas

imad July 18, 2006 13:55

Re: boundary layer, very urgent
DEAR Nicolas when you select the edge An arow appear, his direction define the first and the last point if you put a value and the distribution don't change, you should select copy to parallel edge or update mesh with best regards Imad

imad July 18, 2006 14:00

Re: boundary layer, very urgent
yes spacing 1 is the first distance of edge and spacing 2 is the last but th direction of edge is the direction of arow

Glenn Horrocks July 18, 2006 22:52

Re: boundary layer, very urgent
hi Kramer,

SST does not require y+ approx =1. Using the automatic wall function approach it can switch between full boundary layer modelling (around y+=1) to wall function modelling (y+>11) and blend between.

You should ask yourself whether the boundary layer needs to be modelled directly or if a wall function approach is OK. Then you generate a mesh with y+=1 or >11 based on that decision.

regards, Glenn

All times are GMT -4. The time now is 04:48.