[ICEM] First layer very small according to y+ calculation

Illmatic · August 17, 2016, 08:05

Hi everyone,

I created a mesh with good quality using ICEM that includes 1 prism layer. Now I wanted to split the layer so that y+ = 1 to use the mesh in a k omega sst simulation. I used the equations here to calculate the thickness of the first layer at the wall using the following parameters:

$\rho = 0.4 kg/m^3$
$U_{fs} = 15 m/s$

$\mu = 4\cdot 10^{-5} Pa s$

This leads to:

$\tau_w = 0.7$
$u_{\star} = 1.32$

That would mean the 1 layer I currently have is actually too small and instead of splitting it I would need to increase its size. Did I do anything wrong? In all examples I see online the layer is splitted into very small parts near the wall and then leads to the main mesh exponentially. However in my case the layer size would actually be larger then the main mesh size. This main mesh base size is needed to follow the geometry properly.

I attached a picture of the layer for better understanding. Thanks for your help in advance!

siw · August 18, 2016, 03:51

It looks like you made one layer and defined its height and probably the growth rate and number of layers. You have some choices: 1) make 1 layer but let it float, e.g. do that by setting 0 for the first and total layer heights, and then split that layer and redistribute, 2) float a few layers, e.g. 5, and then split and redistribute or 3) define the first height and build up the layers as required. See ICEM CFD / Help Manual / Mesh / Global Mesh Setup / Prism Meshing Parameters / Global Prism Settings / Total Height.

Illmatic · August 18, 2016, 03:55

Thanks for your reply!

I think I didn't make my problem clear though. I don't have the problem that I don't know how to split the layer in ICEM technically. My problem is, that the y+ calculation tells me that I should not split it at all, which seems a little strange to me.

bluebase · August 18, 2016, 05:24

Hello Axel,

for the SST model the literature says that y+ should be smaller than 1. So there is no problem with having smaller y+ values.
To know if your boundary mesh is well enough you have to run the simulation. The local boundary layer velocity will define y+ values; Refine according to that initial simulation if neccessary.

So a complete CFD simulation needs multiple proceeding simulations to get good accuracy.

With regards,
Sebastian

Far · August 21, 2016, 12:06

Quote:

Originally Posted by Illmatic

Thanks for your reply!

I think I didn't make my problem clear though. I don't have the problem that I don't know how to split the layer in ICEM technically. My problem is, that the y+ calculation tells me that I should not split it at all, which seems a little strange to me.

how it tells you that you dont need to split your layers?

What about the boundary layer theory? can you define gradient by just one layer?

Illmatic · August 23, 2016, 09:03

Quote:

Originally Posted by Far

how it tells you that you dont need to split your layers?

What about the boundary layer theory? can you define gradient by just one layer?

Hi Far,

my main misunderstanding was that I thought the first layer needs y+=1 instead of y+<1. Thus it seemed to conflict with the other goals a boundary layer should achieve.

cfd seeker · August 23, 2016, 09:23

@ Illmatic Hallo bist du Deutsche? Darf ich fragen wo arbeitest oder studierst du in Deutschland?

Far · August 23, 2016, 10:29

-

Quote:

Originally Posted by Illmatic

Hi Far,

my main misunderstanding was that I thought the first layer needs y+=1 instead of y+<1. Thus it seemed to conflict with the other goals a boundary layer should achieve.

different models requires different y+ values.

k-epsilon type models with low Re models requires y+ < 0.2.

K-omega type models with low Re models requires y+ < 2

New y+ formulation requires y+ < 10

Transitional model requires Y+ <1 + very good stream wise mesh distribution.

Also you need alteast 15-40 nodes inside boundary layer besides the y+ requirements.

siw · August 23, 2016, 14:34

You should not focus too much on the height of the 1st cell (i.e. y+ < 1 or y+ = 1 etc.) as the y+ will varyy depending on the flowfield, geometry etc. Just build a good quality mesh for the turbulence model you will use with sufficient cells for however you are going to handle the boundary layer, as you might not know how the entire boundary layer will form. It is often more important make sure you cover the entire boundary layer with structured cells (prisms or hexas depending on your mesh method) than the first layer height, particularly when you are putting the first cell in the viscous sublayer. Read http://www.computationalfluiddynamic...oundary-layer/ (and their other blogs posts) for useful information.

Illmatic · September 12, 2016, 05:03

Hi siw,

To estimate the boundary layer thickness I tried to use Blasius' solution:

$\frac{\delta}{x}=\frac{5.0}{\sqrt{Re_x}}$

However, actually I am interested in the final layer thickness, right? How can I estimate the final layer thickness, very far from the flow entrance?

siw · September 12, 2016, 09:01

That equation is from laminar boundary layer flow past a flat plate. Is that suitable for your case? In your original post you link the yplus calculator (http://www.cfd-online.com/Tools/yplus.php) which uses equations of turbulent boundary layer flow past a flat plate, next you mention turbulence modelling but the Re is in the laminar region for flat plate flow.

Instead of concerning yourself with calculating meshing parameters you could just run a simulation, see what the are results, modify the mesh accordingly for the boundary layer and re-run the simulation to get (hopefully) what you want.

Illmatic · September 12, 2016, 09:23

No a flat plate is of course not suitable. What I got is more or less a turbulent pipe flow. So when I run the simulation what are the things I have to look for, besides y+, to tell if the resolution of my prism layers is sufficient?

siw · September 12, 2016, 10:12

Flat plate calcs is a good place to start, but I was more referring to laminar and turbulent aspects.

To tell if you have sufficient prism layers from your results of a turbulent pipe flow look at a section-plane contours of turbulent kinetic energy, boundary layer velocity vectors and the other data detailed in the hyperlink I gave in a previous post. For pipes it is straight forward to make a high quality structured mesh with nicely transitioning hexahedral elements through and above the boundary layer (assuming it is still developing in thickness).

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] sHM layer process keeps getting killed	MBttR	OpenFOAM Meshing & Mesh Conversion	4	August 15, 2016 03:21
Boundary layer thickness calculation	rohit_turbo	CFX	10	February 9, 2016 09:42
[snappyHexMesh] No layers in a small gap	bobburnquist	OpenFOAM Meshing & Mesh Conversion	6	August 26, 2015 09:38
Boundary -Layer thickness calculation	BNLOO	Siemens	0	December 1, 2002 23:12
Boundary Layer thickness calculation in External f	Narsimloo	Siemens	0	January 2, 2001 00:41

August 18, 2016, 03:51		#2
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	It looks like you made one layer and defined its height and probably the growth rate and number of layers. You have some choices: 1) make 1 layer but let it float, e.g. do that by setting 0 for the first and total layer heights, and then split that layer and redistribute, 2) float a few layers, e.g. 5, and then split and redistribute or 3) define the first height and build up the layers as required. See ICEM CFD / Help Manual / Mesh / Global Mesh Setup / Prism Meshing Parameters / Global Prism Settings / Total Height.

August 18, 2016, 03:55		#3
Illmatic Member Axel Join Date: May 2016 Location: Augsburg, Germany Posts: 46 Rep Power: 9	Thanks for your reply! I think I didn't make my problem clear though. I don't have the problem that I don't know how to split the layer in ICEM technically. My problem is, that the y+ calculation tells me that I should not split it at all, which seems a little strange to me.

August 18, 2016, 05:24		#4
bluebase Senior Member Sebastian Engel Join Date: Jun 2011 Location: Germany Posts: 566 Rep Power: 20	Hello Axel, for the SST model the literature says that y+ should be smaller than 1. So there is no problem with having smaller y+ values. To know if your boundary mesh is well enough you have to run the simulation. The local boundary layer velocity will define y+ values; Refine according to that initial simulation if neccessary. So a complete CFD simulation needs multiple proceeding simulations to get good accuracy. With regards, Sebastian

August 23, 2016, 09:23		#7
cfd seeker Senior Member Join Date: Mar 2011 Location: Germany Posts: 552 Rep Power: 20	@ Illmatic Hallo bist du Deutsche? Darf ich fragen wo arbeitest oder studierst du in Deutschland?

August 23, 2016, 14:34		#9
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	You should not focus too much on the height of the 1st cell (i.e. y+ < 1 or y+ = 1 etc.) as the y+ will varyy depending on the flowfield, geometry etc. Just build a good quality mesh for the turbulence model you will use with sufficient cells for however you are going to handle the boundary layer, as you might not know how the entire boundary layer will form. It is often more important make sure you cover the entire boundary layer with structured cells (prisms or hexas depending on your mesh method) than the first layer height, particularly when you are putting the first cell in the viscous sublayer. Read http://www.computationalfluiddynamic...oundary-layer/ (and their other blogs posts) for useful information.

September 12, 2016, 05:03		#10
Illmatic Member Axel Join Date: May 2016 Location: Augsburg, Germany Posts: 46 Rep Power: 9	Hi siw, To estimate the boundary layer thickness I tried to use Blasius' solution: $\frac{\delta}{x}=\frac{5.0}{\sqrt{Re_x}}$ However, actually I am interested in the final layer thickness, right? How can I estimate the final layer thickness, very far from the flow entrance?

September 12, 2016, 09:01		#11
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	That equation is from laminar boundary layer flow past a flat plate. Is that suitable for your case? In your original post you link the yplus calculator (http://www.cfd-online.com/Tools/yplus.php) which uses equations of turbulent boundary layer flow past a flat plate, next you mention turbulence modelling but the Re is in the laminar region for flat plate flow. Instead of concerning yourself with calculating meshing parameters you could just run a simulation, see what the are results, modify the mesh accordingly for the boundary layer and re-run the simulation to get (hopefully) what you want.

September 12, 2016, 09:23		#12
Illmatic Member Axel Join Date: May 2016 Location: Augsburg, Germany Posts: 46 Rep Power: 9	No a flat plate is of course not suitable. What I got is more or less a turbulent pipe flow. So when I run the simulation what are the things I have to look for, besides y+, to tell if the resolution of my prism layers is sufficient?

September 12, 2016, 10:12		#13
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	Flat plate calcs is a good place to start, but I was more referring to laminar and turbulent aspects. To tell if you have sufficient prism layers from your results of a turbulent pipe flow look at a section-plane contours of turbulent kinetic energy, boundary layer velocity vectors and the other data detailed in the hyperlink I gave in a previous post. For pipes it is straight forward to make a high quality structured mesh with nicely transitioning hexahedral elements through and above the boundary layer (assuming it is still developing in thickness).