CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   CFX 12.1: y+ value for SST (http://www.cfd-online.com/Forums/cfx/73259-cfx-12-1-y-value-sst.html)

Aragorn25 March 3, 2010 06:56

CFX 12.1: y+ value for SST
 
Hello

for CFX 11.0 the y+ value has to be set to 1 for SST turbulence model.
is there a change for the new version CFX 12.1 or has y+ still to be set to 1?

Thanks

ghorrocks March 3, 2010 17:56

I assume you are talking about meshing, that is generating a mesh with an estimated y+ of 1? There has been no change there.

Aragorn25 March 10, 2010 16:35

Antwort
 
Das SST-Model in ANSYS CFX benutzt automatische Wandfunktionen, d.h. Sie können sowohl High-Reynolds Netze mit y+ Werten > 11 rechnen als auch Low-Re Netzt mit y+ < 2. Auch im Übergangsbereich arbeitet das Modell konsistent mit den Gleichungen. Diese Implementierung gibt es seit den ersten ANSYS CFX Versionen und hat sich nicht geändert. Die automatische Wandfunktionen gehen mit allen Turbulenzmodellen, die auf der omega-Gelichung beruhen:
SST
BSL
k-omega

Jade M April 5, 2010 14:54

Confused
 
Aragorn25, I'm curious about your response since I see the number 11. I do not understand German.

I thought that the value of y+ should be 1, also. I see this is the 12.1 manuals in a couple of places.

However, in CFX Tutorials, Release 12.1, November 2009, pp. 109-110, there is the statement "At the lower limit, a value of y+ less than or equal to 11 indicates that the first node is within the laminar sublayer of the boundary flow. Values larger than this indicate that an assumed logarithmic shape of the velocity profile is being used to model the boundary layer portion between the wall and the first node.” I am curious abou this value of 11?

Thanks very much for any clarification from anyone out there. Have a great day.

ghorrocks April 5, 2010 18:56

The log layer region and the significance of y+=11 is explained in any turbulence text book, or even most general CFD modelling textbooks. Try "Turbulence Modelling for CFD" by Wilcox, for example.

Jade M April 6, 2010 09:16

I do not have access to these books
 
but thanks for your reference to general resources. Does anyone have an answer to my questions? Thanks in advance for any assistance.

ghorrocks April 6, 2010 18:48

You asked a general turbulence question which is not specific to CFX. I am not going to write a turbulence text book to define where the 11 comes from for you. Your question is answered in any turbulence text book so that is where you should look.

Jade M April 7, 2010 09:16

LOL at ghorrocks
 
I am truly sorry for the inconvenience I have caused you. I appreciate your stating the obvious that I could find the information in books and then following up with antagonism. I do not think I asked you to write a turbulence model or anything for that matter. Good luck though.

Jade M April 7, 2010 09:21

y+=11
 
For those who are interested, 11.06 is the y+ value where the linear velocity profile in the sublayer intersects with the logarithmic velocity profile in the log layer.

For the k-e model you should use y+ < 300. If y+ is below about 11 for the k-e model then it still works fine, but it doesn't make use of the fine near wall mesh, so it's a waste of mesh. Essentially the k-e model always uses the wall function approach. The wall function approach is not valid below y+ ~= 11, so we just ignore the mesh below y+ ~= 11.

If you want accurate boundary layer predictions, such as separation prediction, then you should use the SST model with y+ < 2. In this case the SST model will switch to a low-Re formulation near the wall rather than the wall function formulation. SST will still work fine with 11 < y+ < 300, but the results will be fairly similar to the k-e model since it will be using wall functions. For 2 < y+ < 11 it will be a blend between wall functions and low-Re formulations.

In some situations, such as accurate boundary layer heat transfer predictions or when using the transition model, an even lower y+ of about 1 is recommended with the SST model.

ghorrocks April 7, 2010 18:54

No problem - it looks like you have found the answer to your question.

Your explanation is not quite correct. Here are some points:

There is no real upper limit on the y+ value you can use in the wall function approach. The real upper limit is set by a mesh convergence study - as you coarsen the mesh you will loose boundary layer accuracy and eventually simulation accuracy will suffer. But which y+ value this occurs on will depend on the simulation.

k-e, when using a wall function approach does not "ignore" mesh with y+<11. What it does is to blindly apply the wall function approach to the first node assuming it is in the log layer, but when y+<11 it is not in the log layer but in or near to the laminar sublayer. This means you will be applying the wrong physical model and your boundary layer profile will be wrong.

The wall function approach is accurate providing you are only interested in the log layer and beyond.

In general, integrating to the wall will give more accurate separation predictions then the wall function approach, but not universally. If a separation is off a sharp corner then wall functions work fine.

When integrating to the wall, yes you will need y+<2. But the exact value of y+ required for accuracy is problem dependant and again you need to do a sensitivity study to find out. Generalisations are dangerous.

MuhammadK May 6, 2012 06:25

Hi

I have looked at the Ansys Help document in the wall boundary condition, but still could not find anything with 'Y+'. As a new user, I believe its in the help document, but its just that I could not find it.
Can anyone point clearly where should I look for?

Are there any books/pdf/whatever online of which will help me understand it better?

Thanks :)

Muhammad

ghorrocks May 6, 2012 06:38

You are looking for the CFX theory manual. The section on near wall modelling of turbuelnt flows.

Just about any CFD textbook will describe basic turbulence model application and wall functions. If you want a mode detailed/advanced textbook "Turbulence modelling for CFD" by Wilcox is a good textbook.

evcelica May 8, 2012 21:17

Quote:

Originally Posted by ghorrocks (Post 253674)
when y+<11 it is not in the log layer but in or near to the laminar sublayer. This means you will be applying the wrong physical model and your boundary layer profile will be wrong.


I was under the impression CFX uses scalable wall functions to overcome the problem of too small of a Y+ for the k-e turbulence model.

MuhammadK May 9, 2012 03:54

Quote:

Originally Posted by ghorrocks (Post 359543)
You are looking for the CFX theory manual. The section on near wall modelling of turbuelnt flows.

Just about any CFD textbook will describe basic turbulence model application and wall functions. If you want a mode detailed/advanced textbook "Turbulence modelling for CFD" by Wilcox is a good textbook.

Thanks Glenn. got the book from the library.

Cheers

spl January 23, 2015 05:17

Hi,

Sorry to bring up such an old post but I have a question the statement -

Quote:

The real upper limit is set by a mesh convergence study - as you coarsen the mesh you will loose boundary layer accuracy and eventually simulation accuracy will suffer. But which y+ value this occurs on will depend on the simulation.
Does this mean through your mesh convergence study you would keep a constant initial cell height and overall boundary layer mesh height or change them with mesh density? If you do change these parameters how do you determine if the change in your results is due to the change in boundary layer resolution or the change free stream resolution? Alternately, would you conduct separate boundary layer and free stream refinement studies?

ghorrocks January 23, 2015 06:33

If the boundary layer and free stream are separable then it is easier to do them separately. Often they are not, so you have to do it all together.

More advanced mesh convergence studies (see the references in the FAQ) require a mesh refinement parameter to use for optimisation. It is best if that single parameter controls the entire mesh size. But the technique still works as long as the parameter changes the most significant part of the mesh on the output.

spl January 23, 2015 06:40

Thank you very much Glenn.

Regards

ngoc_tran_bao April 10, 2016 04:29

Quote:

Originally Posted by ghorrocks (Post 253674)
k-e, when using a wall function approach does not "ignore" mesh with y+<11. What it does is to blindly apply the wall function approach to the first node assuming it is in the log layer, but when y+<11 it is not in the log layer but in or near to the laminar sublayer. This means you will be applying the wrong physical model and your boundary layer profile will be wrong.

Hi Ghorrocks, the information you offered is really helpful. As I understand, SST is more accurate in simulating the near-wall flow. However, in a simulation I carry out (for a centrifugal pump), accounting for roughness wall, the outlet Pressure in case of SST model is higher than k-e model. That makes me confuse a lot because it should be lower. Can you give me some advices for this situation? Many thanks. For more BC information: I set static pressure at inlet, mass flow rate at Outlet, Y+=1 for both case.

ghorrocks April 10, 2016 05:56

You cannot generalise with "SST is more accurate in simulating the near-wall flow". It has strengths and weaknesses like all other models. Maybe you found one of its weaknesses.

But really your question is a FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

ngoc_tran_bao April 11, 2016 01:40

Quote:

Originally Posted by ghorrocks (Post 594271)
You cannot generalise with "SST is more accurate in simulating the near-wall flow". It has strengths and weaknesses like all other models. Maybe you found one of its weaknesses.

Thank you, Sir. I know each turbulence model has its own pros and cons. However, as a new user of CFX, I cannot cover all of them. It's the reason why I need advices or experience of senior member like you. In terms of my case, I 'd like to investigate centrifugal pump's efficiency, so I account for hydraulic loss and friction loss within the pump and pipe. Do you have any suggestion above turbulence model I should use when dealing with rough wall surface?:):)


All times are GMT -4. The time now is 14:29.