Backward-Facing Step: The Skin Friction Problem

  • Last Post 29 June 2018
José Mantovani posted this 27 June 2018

Hello friends!

So, In the yesterday, I post here in community some doubts about the RANS approach to modeling the turbulent flow through a BFS geometry. But, I make a generally post and my really doubt is around the Skin Coefficient Pressure.

I get the velocity field as in experimental study of Jovic and Driver, with reattach length between 6 +- 0.15 x/h and a acceptable Coeficient Pressure results, as we can see in the image below. 

But the true doubt is, Why the Cf have this behaviour? Since the experimental data and the physical behavior, for this flow have recirculation zone with negative velocity values near wall and the FLUENT just get positive values to Cf. 

Why? Someone Can Help me? 

The Cp numerical result is approaching the experimental result as seen in the images, but the Cf is very different and does not assume negative values as it should be. 

Why it's occur? 

Thanks for opportunity!

Order By: Standard | Newest | Votes
brbell posted this 29 June 2018

It looks like the expression for Cf variable is using "Wall Shear" where it should actually be using "Wall Shear X" (or whatever the streamwise flow direction happens to be).   Each point where the plot hits zero downstream of xH = 0 is where the direction of the shear stress is changing.  

  • Liked by
  • José Mantovani
José Mantovani posted this 29 June 2018

Hello Br Bell, thanks for attention and help. 

I think this and last night I plot the chart again. Now, it's better, the result chart of Cf vs x/h is good compared to experimental. The Cp vs x/h is a little below when compared to the experimental, maybe I should iterate more, I don't know. 

But the problem is, In the experimental study the wind tunnel channel is a complete divergent channel and not just half as I simulated. 

So, instead of being defined as a wall, the upper boundary should have been defined as symmetry. But when I do this I do not get a fully developed velocity profile before the step. I think for this I have to use a UDF inlet, how do I do this? I also saw that in the numerical study of Le et al (1997) that used a DNS approach and unlike my, a 3d simulation, they defined the upper limit as no-stress wall and also use the experimental study of Jovic and Driver for validation . What would be the best way? Because in my point of view, I set the upper limit as the wall the simulation will not be according to Jovic's experiment and Driver.

The reattach length obtained in the simulation presented an acceptable error between 4% ~ 6% (I may have measured wrong there, but the error percentage does not go far beyond this range).

But as I said, I set the simulation with wall in top boundary and in the experimental data (complete channel) this is just half channel, maybe I need set top boundary as symmetry and input a UDF fully developed velocity profile, but I don't now how do this. 



rwoolhou posted this 29 June 2018

There's a boundary profile UDF example in the Customisation manual, but I'd tend to just extend the domain by a few diameters. 

  • Liked by
  • José Mantovani
José Mantovani posted this 29 June 2018

Thank's so much for attention and help rwoolhou. 

I will look for it in the manual. I'll see what I can do, I'll post the results here to compare soon. I simulated yesterday and got a better value for the Cp vs x/h chart, but it is on another computer.