CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   How to achieve a Cd with k-e in an acceptable range of accuracy (http://www.cfd-online.com/Forums/fluent/117001-how-achieve-cd-k-e-acceptable-range-accuracy.html)

joy2000 April 30, 2013 08:11

How to achieve a Cd with k-e in an acceptable range of accuracy
 
Hello dear everyone,

I'm conducting a 3D wave-structure impact CFD analysis. The goal is to get a favored drag on the structure such as a column, a pile or a beam.

I've found in many literatures that they have achieved a satisfactory drag coefficient with the k-e series turb model in accordance with the experiment result. On the other, many experts proved that the k-e series are not suitable for the external flow, especially with flow separation and large adverse pressure gradient - which is exactly the case of the flow around a cylinder...

The industry may choose the k-e series for the low computional cost. The relatively coarse mesh adjacent to the wall (with y+=30~200) could remarkbly save the scope of the calculation model. I wish to achieve that, but failed again and again.

For that the wave-structure analysis must be conducted with 3D model. If I choose the boundary-layer-computed model such as k-omega SST or LES, the mesh scope will be so large that I could not afford. But till now after many test with cylinder external flow, I could not achieve an acceptable drag with k-e and standard, scalable or non-equilibrium wall functions, though the y+ requirement in the near-wall mesh could be satisfied.

I just wonder that whether there is some method I can obtain a favored drag (maybe only the drag..) in the range acceptable in the engineering sense, say, error in 10~20% for the CFD results. And I still wonder that how the achieved ones succeeded in doing that?

Could anybody give some help?

Many thanks !!

joy2000 April 30, 2013 08:25

In the test calculation, I found that the error anticipation of the separating angle and the pressure in the wake region may be the point. When I attempted to reduce the turbulent viscosity, the result could be a little improved. However, the reduction of the turb viscosity is only an attempt... :confused:

I just only want the drag... with low mesh cost, anyway..

blackmask April 30, 2013 08:49

Why not try the combination of SST kw model along with wall function method?

joy2000 April 30, 2013 12:42

Quote:

Originally Posted by blackmask (Post 424166)
Why not try the combination of SST kw model along with wall function method?

Thank you very much, blackmask. But, I'm using the software Fluent, in which I'm not very clear how to combine the k-w SST with wall functions. I know in fluent the k-omega series would solve the viscous sub-layer in the boundary layer which requires the near wall mesh with y+ around 1.

Er...how I wish I could use that with y+ in >30 !!

And then, another problem is, in using the standard wall function we should guarantee the first inner node with y+>30 and meanwhile there should be at least 10~20 nodes in the whole boudary layer. The former could be easily done, however the latter may be sometimes difficult when the total thickness of the BL is not high, eg. within the max y+ around 100 or a little higher.

Anyway, I would learn and have a try on that. many thanks !! :)

blackmask April 30, 2013 20:40

The y+ requirement is always related to the wall treatment rather than RANS models. You can have a coarse wall grid to use omega-models. In fact, you can also use the epsilon-model for a low-y+ mesh but you have to switch wall treament from the default to EWT (enhanced wall treatment).

Far May 1, 2013 01:13

In newer versions of SST model, the default wall treatment is hybrid wall function aka Enhanced wall treatment W-equation (Fluent theory guide 4.13.6.*Enhanced Wall Treatment ω-Equation (EWT-ω))

1. This is generally known as hybrid wall function in open literature
http://num.math.uni-goettingen.de/ba...ings/knopp.pdf

2. In CFX it is termed as automatic wall treatment

Basic theory is to combine the log law with linear law and give the better treatment of buffer zone using the blending function. For Y+ < 5 Integration to wall approach is used, for Y+ > 30 wall functions is used and for Y = 5-30 blending function is used. Up to 10 the log portion weightage is very low and after Y+ = 20 log law weightage is higher.

So if you get the mesh with Y+ > 30 in most of the wall zones then you are using wall function. Please note that at separation Y -> 0, so linear profile shall be used there hence no worry

For details please refer following threads
http://www.cfd-online.com/Forums/flu...treatment.html

http://www.cfd-online.com/Forums/flu...-function.html

http://www.cfd-online.com/Forums/ans...ys-fluent.html

PS : For skin friction component of drag you need Y + < 1, so if is important component of your study then using wall function would always give you wrong results.

joy2000 May 1, 2013 08:27

Thank you so much, Far and Blackmask and everyone paid attention on this thread. I will have a try on this kind of EWT.

btw, the contrubution brought by the skin friction in the total drag is not significant, especially in my case with rectanglular columns, though, in the case of cylinder external flow, the friction would affect the position of separation.

I'd ever tried the k-omega SST on the circular cylinder which brought me some favored results, e.g. the Cd, Cl and St. This time I really hope it will work on the y+~30 mesh.

Many thanks!! :)


All times are GMT -4. The time now is 02:16.