June 27, 2018 at 4:44 pmJosé MantovaniSubscriber
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!
June 29, 2018 at 1:26 pmbrbellAnsys Employee
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.
June 29, 2018 at 4:07 pmJosé MantovaniSubscriber
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.
June 29, 2018 at 4:17 pmRobForum Moderator
There's a boundary profile UDF example in the Customisation manual, but I'd tend to just extend the domain by a few diameters.
June 29, 2018 at 4:26 pmJosé MantovaniSubscriber
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.
April 1, 2020 at 6:51 amVijayKumarReddySubscriberHi Jose
Have u got Cf profile correct. If u got please reply how u got it.
December 31, 2020 at 9:14 pmhazem_engSubscriberHi Jose nThe same question of Mr. VijayKumarReddynHave u got Cf profile correct? If u got please reply how u got it.nThank you.n
January 14, 2021 at 7:23 pmhazem_engSubscriberMR. VijayKumarReddy I got the better result just instead of plot skin friction just you have to calculate the skin friction by using wall shear stress X.n
- The topic ‘Backward-Facing Step: The Skin Friction Problem’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- legend min and max
- Ensight hot iron palette from an image
- Streamlines in EnSight using MRI data
- Import MRI data into Ensight
- FLUENT APPLICATIION ERROR
- Total Surface Heat Flux Calculation in Fluent
- Drop Test of a Water-Filled Tube
- Difference between “total pressure” and “absolute pressure”?
- Minimum Orthogonal Quality Less than 0.01 For Transonic Airfoil Flow Analysis
- obtaining pressure distribution by making points in ansys
© 2023 Copyright ANSYS, Inc. All rights reserved.