[Far]

Originally Posted by Mina_Shahi

Thanks

But can you explain what happens for y+<11 (in standard wall function)? I guess that turbulence equatuion will be integrated untill the wall in th eregion with y+<11, Is that true? or simply for the small y+ it assumes u+=y+ (linear approch and not logaritmic approach)? i am a bit confused with this layers

Ok. for standard wall function, CFX still assumes/enforces the log profile (u+ = A+B logy+), even in the region of u+ = y+ and this is the where standard wall function creates the trouble for you (completely invalid solution)

[Mina_Shahi]

Originally Posted by ghorrocks

If you are using standard wall functions then the wall function equation will be used regardless of y+. Refer to the CFX documentation or a turbulence textbook like Wilcox for details on this. But the key point is that the wall function equation is only applicable from around y+>11. So if you apply standard wall functions with y+<11 then you are simply applying them in a regime where they are not accurate.

So you mean bigger mesh near the wall gives better results? in my model y+ is varying between 0-40, so in the region by y+>11 the standard wall function is working well while in the region by y+<11 is giving us wrong results. on the other hand i read in ansys documentation that at least 10 nodes in boundary layer is needed, so we need bigger mesh for the wall function and smaller mesh for accuracy !!!!!

[ghorrocks]

Yes, ideally you want all nodes to be y+>11 for standard wall functions. And you are correct in that often contradicts the requirement for sufficient nodes in the boundary layer.

The best solution is usually to use the SST turbulence model with automatic wall functions and it can handle just about any y+.

If you still want to stick with standard wall functions then I would do a y+ sensitivity check. You may well find that your simulation is not very sensitive to y+ anyway, and in this case you can run any y+ you like (within reason).

[Far]

I would like to share my work on turbo machinery. In this case, i tried the Yplus 1, 10 and 60 with scalable wall function and Y+ = 10 with standard wall function. Results clearly show the problem with standard wall function.

[Far]

In case of SST y+ greater than 10 does not produce the good results as shown in this pic: Definitely this is the difficult case for any turbulence model and wall treatment. In simpler cases, you might not find any difference at all

[ghorrocks]

Nice dataset Far. Shows the wall boundary condition is important in your turbomachinery case.

But do not make the mistake in assuming therefore it is important in all cases. CFD covers a very wide range of applications, and in quite a few of them the wall boundary condition details does not make much difference. For instance HVAC modelling.

[Mina_Shahi]

Originally Posted by Far

In case of SST y+ greater than 10 does not produce the good results as shown in this pic: Definitely this is the difficult case for any turbulence model and wall treatment. In simpler cases, you might not find any difference at all

Thanks for nice explanation, one basic question, in the model you usualy have a range of Y+ , when you say y+=1, 10, ... you are talking about the maximum y+ in the model, am i right?

[Far]

Originally Posted by ghorrocks

Nice dataset Far. Shows the wall boundary condition is important in your turbomachinery case.

But do not make the mistake in assuming therefore it is important in all cases. CFD covers a very wide range of applications, and in quite a few of them the wall boundary condition details does not make much difference. For instance HVAC modelling.

Very true.

But I want to point-out one important aspect. If you are not solving the equations with integration to the wall approach then you may not be able to predict the quantities accurately e.g. drag on airfoil. So when you are using the wall function you may miss the important flow physics. Obvious fact

On the other side as you have pointed out that if you solve the HVAC problem with intergration to wall approach or wall function apporach, it wont make any difference at all. Very true and I agree again.

But if you are putting the wrong numerics i.e. using the integration to wall mesh for the standard wall function you are forcing the numerical algorithm for the things it was not designed. So we should keep the wrong numrics and wrong physcis into separate boxes.

[Far]

Originally Posted by Mina_Shahi

Thanks for nice explanation, one basic question, in the model you usualy have a range of Y+ , when you say y+=1, 10, ... you are talking about the maximum y+ in the model, am i right?

I am talking about the average values on the blade surface. I have some how higher values at the leading edge and lower values at separation point( Y + = 1-20 for Y+ = 10 case). But that portion is not more than 5-10%.

For example for Y+1 mesh, Maximum Y+ is 5-6.

I shall try to post the pic of Y+ values (Y+ and solver Y+)

[Far]

see Fig. 9 in this reference http://num.math.uni-goettingen.de/ba...ings/knopp.pdf for the definition of average Y+

This is also another reference by same author. http://num.math.uni-goettingen.de/ba...ngs/alrutz.pdf See Fig 4

Note the difference for the SA and SST model for the range of Y+ values. Knopp recommends the Y+ <=10 for SA model for good results for flow with stagnation, separation etc. And higher values for SST model.

[Far]

See Fig 1 & 2 http://www.mscsoftware.com/events/ae...pdf/p10201.pdf

Slide 20 http://www.powershow.com/view/b0e25-...n#.T_FzQxdKol8

Slide 21 http://www.docstoc.com/docs/10845119...mics-Using-CFX

General comments about turbulence model and wall treatment with good data from industry. http://www.ansys.com/staticassets/AN...pabilities.pdf Slide 34 clearly states that the Y+ insensitive treatment is availalbe for all turbulence models in ANSYS CFD (CFX+Fluent+other modules)


https://www.sharcnet.ca/Software/Flu...bModeMath.html

http://www.mathematik.uni-dortmund.de/~kuzmin/IJCSM.pdf

http://nippon.zaidan.info/seikabutsu...okyo_ts059.pdf

http://www.idac.co.uk/products/downl...NSYS%20CFX.pdf

[Mina_Shahi]

Originally Posted by Far

See Fig 1 & 2 http://www.mscsoftware.com/events/ae...pdf/p10201.pdf

Slide 20 http://www.powershow.com/view/b0e25-...n#.T_FzQxdKol8

Slide 21 http://www.docstoc.com/docs/10845119...mics-Using-CFX

General comments about turbulence model and wall treatment with good data from industry. http://www.ansys.com/staticassets/AN...pabilities.pdf Slide 34 clearly states that the Y+ insensitive treatment is availalbe for all turbulence models in ANSYS CFD (CFX+Fluent+other modules)


https://www.sharcnet.ca/Software/Flu...bModeMath.html

http://www.mathematik.uni-dortmund.de/~kuzmin/IJCSM.pdf

http://nippon.zaidan.info/seikabutsu...okyo_ts059.pdf

http://www.idac.co.uk/products/downl...NSYS%20CFX.pdf

Many Thanks Far !

[sam1364]

Hi All,

I was reading your discussion for standard and scalable wall functions. I have a question which may not be related to your discussion, but maybe I can get the answer from you.

I do not know where the boundary conditions for U at first grid point is defined in OpenFoam when using wall functions. I expect to see some values for U at the first grid point based on log law equation, but I can not find this implementation through the code. can you please help me on that?! ( I see some implementation for k, epsilon and nut in their corresponding wall functions but nothing for U)
So, for the first grid point, do we still solve equations to obtain U?!

I will be so appreciated if you can help me with this question.

thanks

[ghorrocks]

This is the CFX forum, try the Openfoam forum for that question.

[MissCFD]

It's not very clear for me, I wonder if below Y+ = 11.06 mesh points are ignored or below Y+ = 11.06 mesh points are set up to y+ =11.06.
But if it's the last option, this means that we associate a y+ of 11.06 on cell initially too small, do you see what I mean ?

Originally Posted by Far

No. Below Y+ = 11.06 mesh points are ignored. If you check the mathematical formulation of scalable wall function you will not find any term for linear profile. Therefore scalable wall function are not built for resolving the viscous sub layer. For that you have to choose the automatic wall treatment which is only available in k-omega based models.

Transition to linear profile is property of hybrid wall functions (aka automatic wall treatment in CFX)

Scalable wall function are designed to avoid the problems

1. With mesh refinement when Y+ goes to 1. In this case standard wall function approach ceases to be valid.
2. At separation when velocity is zero and Y+ is again very low, in this case standard wall function ceases to be valid.

In other words scalable wall function is robust wall function as compared to standard wall function.

Standard wall functions are also valid up to Y+ = 11.06 and it was the default option in Fluent when Y+ is higher than 11.06. See the SA model section of Fluent User guide (I know this is CFX forum )