CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   which yplus (SST) (http://www.cfd-online.com/Forums/cfx/71606-yplus-sst.html)

sanchezz January 8, 2010 23:34

which yplus (SST)
 
Hi,

I've read every post on yplus values in this forum, but still I'm not clear what to shoot for.

Are these assumptions correct?
1. yplus needs to be less than 200 (CFX-Help)
2. only for yplus < 1 can SST use it's full potential (however it works also for any higher value)
3. yplus can't be too small

But now what do I go for? If I shoot for yplus = 100 in CFX-Mesh, the mesh I get looks like this:
http://img44.imageshack.us/img44/250/y100.png

If I go for yplus = 10, my mesh looks like this:
http://img189.imageshack.us/img189/3157/y10.png

From a very inexperienced view it seems like the last mesh is not very good as it transitions from very small elements to huge ones. If I would go for yplus = 1, it would be even worse?

So what should I go for? I can't make the mesh around it much smaller, since I have already quite a lot of elements (3 mill). For what it's worth, my object is a car.

Can anyone tell me how I should proceed? Thanks!

zandi January 9, 2010 15:28

yplus
 
hi
it based on the turbulent model that you want to use for problem due to the charactristics that it has.
for example for the most popular flow problems k-epsilon is used and as in cfx help the yplus should be in the range of 20 and 100
so if the problem force you to obtain the parameters in sub layer and ... and you choose k-omega or sst model your yplus limits is different that is in the cfx solver help
i hope it could be useful
good luck

sanchezz January 9, 2010 18:31

thanks, you're right. the cfx help only states that yplus has to be smaller than 200. that's it. but that still leaves me with a huge range of options and I just can't imagine that it doesn't matter which one I take.

zandi January 10, 2010 03:39

ANSYS CFX-Solver Modeling Guide | Turbulence and Near-Wall Modeling | Modeling Flow Near the Wall |
Solver Yplus and Yplus


Guidelines for Mesh Generation




One of the most essential issues for the optimal performance of turbulence models is the proper resolution of the boundary layer. In this section, two criteria are suggested for judging the quality of a mesh:
  • Minimum spacing between nodes in the boundary layer
  • Minimum number of nodes in the boundary layer
These are simple guidelines for the generation of meshes which satisfy the minimal requirements for accurate boundary layer computations.
Minimum Node Spacing




The goal is to determine the required near wall mesh spacing, http://www.cfd-online.com/Forums/mk:...earWall454.jpg, in terms of Reynolds number, running length, and a http://www.cfd-online.com/Forums/mk:...earWall455.jpg target value.
A http://www.cfd-online.com/Forums/mk:...earWall456.jpg < 200 is acceptable if you are using the automatic wall treatment, if not, continue to read the advice below.
After running a solution, the value of http://www.cfd-online.com/Forums/mk:...earWall457.jpg (in particular, the value given by the solver variable Yplus, representing the http://www.cfd-online.com/Forums/mk:...earWall458.jpg value for the first node from the wall) should agree with:
http://www.cfd-online.com/Forums/mk:...earWall459.jpg

Note

Here, y+ refers to the solver variable Yplus (not the solver variable Solver Yplus), which is stored at each node on a wall boundary. For details, see Solver Yplus and Yplus.

Note

Here, low-Re model means using a fine mesh and one of the http://www.cfd-online.com/Forums/mk:...earWall460.jpg models (which include the SST model). The http://www.cfd-online.com/Forums/mk:...earWall461.jpg models do accept coarser meshes, due to the automatic near-wall treatment for these models.


this is from help
you have to choos turbulent model first then you have automatic wall function or standard wall function or wall function then can control the limitations
good luck

sanchezz January 10, 2010 03:49

Hi,

thanks for your answer and posting the help here.
I am using SST with automatic wall functions. I based my assumptions partly on this text. Are they correct?

"The http://www.cfd-online.com/Forums/mk:...earWall461.jpg models do accept coarser meshes, due to the automatic near-wall treatment for these models"
-> SST has automatic wall function, so I can have a coarser mesh.

"yplus http://www.cfd-online.com/Forums/mk:...earWall456.jpg < 200 is acceptable if you are using the
automatic wall treatment"
-> SST has automatic wall function, so yplus needs to be small than 200.

So far so good - but I still don't know, what I'm supposed to go for? I do have yplus < 200 since that is the only obvious regulation, but how small is good for me? I just don't know and I really don't find any advice in the help file on that.

zandi January 10, 2010 04:56

Hi
your welcome
I'm not so experinced in cfd but I know if you choos sst so, y+<2 or 1 not sure
I can't open the link for text you sent.

Attesz January 10, 2010 05:42

Hi,

I recommend you not to use this way to get yplus in CFX-mesher. It's a better way to set the height of the boundary layer, and then set the number of elements in it and its aspect ratio. After a simulation run, you should check the yplus values (which needs to be between 20 or 200, or above 1), and then modify the mesh. The second mesh is not so good quality, because there is a big size different between the last boundary layer cell and the first tetrahedra. The first mesh is better.

Anyway, if you have ICEM CFD, i recommend you to use that, because it's more controlable. This type of mesh you can generate more easier, and can get a better quality.

Regards,
Attesz

sanchezz January 10, 2010 06:04

Thanks for your answer.

So you say that
- I should prefer similar element sizes over certain yplus values (which I take from you statement, that the second mesh is better)
- I should have yplus between 20 and 200

The last point is the most critical to me. With simulation models like k,e-model, I know that yplus has to be in a certain range, e.g. 20 to 200.
But with automatic wall functions (which are part of k,w-models like SST), some people claim that yplus should be below 1.

So which is it for SST? yplus < 1 or between 20 and 200??

Attesz January 10, 2010 06:22






Here, low-Re model means using a fine mesh and one of the k-omega models (which include the SST model). The http://www.cfd-online.com/common/hel...earWall461.jpg models do accept coarser meshes, due to the automatic near-wall treatment for these models.

Minimum Number of Nodes




Goal




A good mesh should have a minimum number of mesh points inside the boundary layer in order for the turbulence model to work properly. As a general guideline, a boundary layer should be resolved with at least:

Nnormal= 10 for wall function
15 for low-Re model


where Nnormal is the number of nodes in the boundary layer in the direction normal to the wall.




a strict low-Reynolds number implementation of the model would also require a near wall grid resolution of at least y+ < 2. This condition cannot be guaranteed in most applications at all walls. For this reason, a new near wall treatment was developed by ANSYS CFX for the k-omega based models that allows for a smooth shift from a low-Reynolds number form to a wall function formulation. This near wall boundary condition, named automatic near wall treatment in ANSYS CFX, is used as the default in all models based on the omega-equation (standard k.omega, Baseline k-omga, SST, omega-Reynolds Stress).
To take advantage of the reduction in errors offered by the automatic switch to a low-Re near wall formulation, you should attempt to resolve the boundary layer using at least 10 nodes when using these models.



From CFX help, You can see, that both value range is ok, but from the last sentence, it's recommend to use y+<1 or at least yplus<2. But If you have a complex geometry, it's not to easy, to reach it everywhere...


Attesz

sanchezz January 10, 2010 11:07

Thank you, that was very clear and answers my question. There is one more problem though - if I go for yplus < 2 I get even a huger size difference between inflation elements and regular elements.

So would you recommend going for yplus < 2 (while meshing, don't know if I'll achieve them in the end - like in picture 2) or just accept yplus of about 100, but having similar sized cells (like in picture 1)?

Which mesh will be better?

Thanks again for all your help!

Attesz January 10, 2010 11:20

Hi sanchezz,

The huge size difference between inflation elements and regular elements means a big aspect ratio, so the changes in flow will be not resolved there. The recommened aspect ratio is about 1.3-1.5, but maybe you can get bigger. To avoid it, you can set the aspect ratio bigger (1.5-1.6) when generating boundary layer mesh, and set a lower mesh size value near the wall using "Face sizing" or "Edge Sizing". Unfortunately, you have to generate always the mesh, and then modify the values and again and again...thats why I'm not using cfx mesher.

Reading the meshing forum's topics here can be useful
http://www.cfd-online.com/Forums/ansys-meshing/

Good luck,
Attesz

zandi January 10, 2010 15:43

height of boundary layer
 
Quote:

Originally Posted by Attesz (Post 242011)
Hi,

I recommend you not to use this way to get yplus in CFX-mesher. It's a better way to set the height of the boundary layer, and then set the number of elements in it and its aspect ratio. After a simulation run, you should check the yplus values (which needs to be between 20 or 200, or above 1), and then modify the mesh. The second mesh is not so good quality, because there is a big size different between the last boundary layer cell and the first tetrahedra. The first mesh is better.

Anyway, if you have ICEM CFD, i recommend you to use that, because it's more controlable. This type of mesh you can generate more easier, and can get a better quality.

Regards,
Attesz


dear attesz
could you tell me please how I can calculate height of boundary layer
due to the formula from Irving H. Shames book: Integral(1-u/(u max))*dy,o,∞)

Attesz January 10, 2010 16:05

2 Attachment(s)
Hi zandi,

unfortunately I have no exact idea. I'm not so experienced in the theoretical background of CFD. But check these:
Attachment 1942
Attachment 1941

However, you can calculate the boundary layer thickness with this simple form only in simple flows, but it's a good estimate.

Usually I make the b.l.mesh by my own estimate. After simulation I check the yplus values, and then modify the thickness values, or the aspect ratios...it's not easy. But in some work, due the complexity of the problem, you can not reach everywhere yplus<1...

zandi January 10, 2010 16:29

Quote:

Originally Posted by Attesz (Post 242044)
Hi zandi,

unfortunately I have no exact idea. I'm not so experienced in the theoretical background of CFD. But check these:
Attachment 1942
Attachment 1941

However, you can calculate the boundary layer thickness with this simple form only in simple flows, but it's a good estimate.

Usually I make the b.l.mesh by my own estimate. After simulation I check the yplus values, and then modify the thickness values, or the aspect ratios...it's not easy. But in some work, due the complexity of the problem, you can not reach everywhere yplus<1...

hi
thank you very much
but the formula in the first piture is not so clear
could you send me it in the more quality or exact formula please

Attesz January 10, 2010 17:05

2 Attachment(s)
here you are, good luck!
Attachment 1943
Attachment 1944

attesz

sanchezz January 11, 2010 00:29

Hi,

just wanted to let you know that I talked to a ANSYS support guy and he basically confirmed attesz statement:

1. yplus as small as possible (just like any mesh and with automatic wall functions, it can't be too fine)
2. yplus < 1 is good
3. yplus should by no means exceed 200

Thanks for the advice on using different aspect ratios - my mesh looks much better now.

Thanks for your help!

zandi January 11, 2010 03:32

Quote:

Originally Posted by Attesz (Post 242047)
here you are, good luck!
Attachment 1943
Attachment 1944

attesz


thank you very very much

Attesz January 11, 2010 05:45

you're welcome, good work!

Attesz


All times are GMT -4. The time now is 03:13.