Near Wall Turbulence in CFX
Hey guys, just a few quick questions about CFX and turbulence models in general.
I am trying to compare the efficiency of wall functions vs. integration to the wall. I have studied up a fair amount on this but sadly my understanding of the material is low. I am running a simulation of a sharpedged object around mach 6, and so far i have tried running the kw turbulence model, the BSL (which is also based on the komega model  correct? just multiplied by some factors) and the SAS SST model (again, based on the komega model, am I right, except it takes into account the turbulent shear stress). Now these "omegabased" models have an automatic nearwall treatment as opposed to a scalable wall function treatment. This is where I am confused. How do I go about simply integrating to the wall instead of using a wall function? There doesn't seem to be an option for that. The closest thing seems to be an automatic nearwall treatment  which still doesn't allow me to choose whether I want to use a full integration to the wall approach or a wall function approach. Can someone clarify this to me? How do I integrate to the wall using these turbulence models? Thanks very much in advance. 
This is all discussed in the documentation.
When you use automatic wall functions it integrates to the wall if y+<11 or so, and uses wall functions if y+ is above that. There is also a blending between the two so you don't get sharp transitions. 
Quote:
I see, thank you. Perhaps I haven't been careful enough in reading the documentation. So does this mean the that kepsilon turbulence models there is no option to integrate to the wall? If I understand this correctly, any turbulence model should be able to use both a wall function which is just an estimation used at a certain distance from the wall, and integrate to the wall which is pretty much a full out integration to the wall. So what exactly is a scalable wall function? Also are you looking at the documentation in the solver modeling guide or the solver theory guide? Thanks a lot ghorrocks for your response :) 
Quote:
Quote:
Quote:

Hi,
I too am doing a similar study using CFX regarding near wall treatment. I understand that the wall functions can be "disabled" in CFX by changing the mesh so that I have a y+ that is very much greater than 1. However, wouldn't this affect my results as the mesh would be different when I compare my two sets of results in tandem? Is there a way of disabling wall functions without changing the mesh? Does anyone have any good references regarding the effect of mesh densities near the wall? Unfortunately, I do not have much experience with CFD.... I studying the vortex shedding effects off a 2D cylinder and a triangular blunt body. Thanks in advance 
Wall functions are "enabled" by increasing the y+ to larger than 11. So your coarse mesh is using wall functions and the finer mesh is not (it is integrating to the wall).
Do a mesh with y+=1 about and then automatic wall treatment will integrate to the wall. You can select the wall function option to override this and use wall functions. This will allow you to compare wall functions to integration to the wall. 
Thanks Ghorrocks for the response.
I already have a model in CFX with a y+ < 1. However, when I go to the wall functions option for SST turbulence modeling, I only have the option of "automatic" and nothing else. I've tried setting the option through the command editor from "automatic" to "on" but it gave me an error. I have searched through the documentation and found nothing... 
On second thoughts you can't do this as it makes no sense. The wall function approach is only valid above y+>11, so why even let you choose it below 11? Likewise, integrating to the wall is not valid when y+>1 or so, so why let you choose it?
You are trying to compare a valid approach to an invalid approach. This does not seem to make much sense. 
"On second thoughts you can't do this as it makes no sense."
Indeed it doesn't make much sense but I am doing this for a project as a study on how bad wall functions perform. In order to do that, I need to keep a consistent mesh so as to not confound my results with the change in densities at the wall. If CFX is capable of doing this, then my next thought would be how it is actually applying it... 
Well, put it this way:
The ke turbulence model is degenerate at the walls, meaning you have to do something to define it at the walls. So you define wall functions and off you go. The komega model is defined at the walls and so has no need for any special treatment. You can simply integrate it to the wall. So wall functions do not exist. So you can compare a ke model with wall functions to a komega model without. So you are not only comparing wall functions but turbulence models. 
Thanks for the help. I am doing just that =D

Dear Frends
I would like to share something about integration to the wall, automatic wall function and scalable wall functions. 1. Automatic wall treatment AWT(as per discussion with F. Menter) It changes to the integration to wall when y plus is less than 6 and switches to standard wall function when y plus is equal to or greater than 30. In between 6 and 30 it uses the blending function. 2. Integration to wall (ITW) It simply mean that you have mesh with y plus less than 1 and want to solve the viscous sublayer as well. Although the automatic wall treatment is similar to ITW but has many critical differences. a) For ITW you need 3540 points in the boundary layer b) for AWT you only need 1015 points in BL c) AWT will switch to wall function if y plus is equal to or greater than 30. c) scalable wall function In standard wall function you can not refine the mesh as y plus may go to zero at separation or less than 30 due to different velocity scales in domain. This will violate the basic assumption in wall function. Therefore scalable wall function was developed to cure this problem. Now even if you make the mesh with y plus less than 1 and solve it. and Check the y plus and solver y plus contours you will see the y plus contours showing the y plus from 1 or less but the solver y plus will show the y plus 11.06 or greater. That is due to limiter in scalable wall function which does not allow to solver y plus to go to zero. It may be noted that the 11.06 is intersection point of linear law (viscous sub layer) and log law (wall function) The automatic wall treatment is specifically applicable to SA model (Modified eddy viscosity) and K omega based model (omega variable). Scalable wall function is designed for epsilon based models e.g. K epsilon, SSG Reynolds stress mode and LRR Reynolds stress model For more details you may look at the knopp paper Best Regards Far 
I know it is not a good manner to hijack old threads, but this one is quite interesting for me. Especially the last posting. A nice summary about how wall functions are used in Ansys CFX. I still have some questions:
1. It has been said that the quantity of points within the boundary layer (BL) should be 3540 for ITW. This constraint obviously comes from the fact that there have to be enough points to capture the rapid variation in flow variables, right? Is there any reference (literatur?) for that amount of points? 2. Does ITW mean that the tangential wall velocity u(y) is only computed direct from the conservation equations instead of using any physical assumptions? 3. What is the upper limit of y+ for the AWT approach? For example, if the distance y, normal to the wall, is approaching the wall, how does the CFXSolver know where the logarithmic region begins? And anyway, how does CFX know whether the mesh is fine enough for the ITW approach? 4. For the kwSSTModel with AWT I have to put at least 15 points (Ansys even states just 10 nodes) into the BL. The node distribution can be done with total different y+ values and growth ratios and therefore exerts a great influence on the solution of the flow problem. For example, when just a few nodes are located inside the viscous sublayer and y+ is below 6, then CFX switches to ITW. In my humble opinion this is not sufficient for capturing the sublayer. Wouldn't it be better to use a linear assumption instead? 5. There are corresponding wall functions for the thermal boundary layer. Are they usable for heat transfer calculations? Ansys recommends y+ <= 1 for that purpose. 
Quote:
Okay, this is totally off topic. You should not hijack a hijacked thread! :D Please open another topic and I or somebody else will help you. 
1
Quote:
Quote:
Quote:
Quote:
Quote:

Wall functions can work OK for heat transfer  it depends on the application. Do not think that because Far's application requires y+<1 that all means all applications require y+<1. Wall functions are fine for many applications, and I prefer to use them until it is shown that they are unacceptable, rather than assume that y+<1 is required.

Quote:
Quote:
So when you say "It changes to the integration to wall when y plus is less than 6" then you mean it is not ITW in the sense of solving the conservation equations, but more a linear function Approach for the viscous sublayer, right? Quote:
But I thought of the freestream flow. How can CFX know if the nodes are in the vicinity of the wall and that he can switch to wall functions (WF) to save computation time. Is there an criterion that leads to an upper y+ value, so that if y+ <= y+max > Switch from solving the conservation equations in freestream to WF in BL. Quote:
One last question about calculating y+: Somehow it is a "Chicken or the Egg Causality Dilemma" for me. For y+ I need to know the wall shear stress Tw. But Tw is calculated from the y+ value, if I have understood correctly. If it was my task to calculate y+, I would estimate Tw from equations for the friction factor, but this is probably not the way it is done in CFX. Maybe y+ is calculated from the initial flow conditions by means of ITW and then iteratively converges to the physical correct value. 
Quote:
The switch from ITW to wall functions is described in the documentation in the theory manual in the boundray conditions section. In my opinion too many people on this forum are rubbishing wall functions out of hand because they are approximate. But this neglects that getting the integration to the wall approach is an approximation too  and relies on accurate discretisation of the entire boundary layer.... and what is the definition of "discretisation"? It is an approximation. A simulation using wall functions were appropriate will be better than integrating to the wall as it requires a far smaller mesh making the simulation much cheaper and eliminates the need for accurate numerics through the entire boundary layer  the wall function approach just replaces that entire thing with an empirical model. The CFX documentation has a discussion about estimating y+ based on fundamental flow parameters, so you can estimate the mesh required without doing a trial simulation. 
Quote:
For instance, I have got two points inside the viscous sublayer, another one in the buffer layer and the remaining in the logarithmic layer. The first point has y+ = 1 and to be conform with the noslip condition, the velocity is set to zero (virtual shift to y = 0 ?). The second point is y+ < 6 and CFX uses ITW, that means it solves the conservation equations to compute the velocity. The third point is y+ > 6, so CFX uses a function that blends the linear with the log law and for the remaining points CFX simply uses the log law. And that brings me to the question: Where does CFX get the wall shear stress from? Quote:

Quote:
Regarding the ITW, is that kind of large discretization error DNS method that is usually too costly to be used in the real CFD application? For boundary layer separation predictions, will ITW be theoretically much more accurate than AWT? 
All times are GMT 4. The time now is 08:17. 