

May 25, 2018 at 9:44 amWalaaSubscriber
What is the the difference between near wall treatment options in Ansys workbench 18.2

May 25, 2018 at 6:37 pmraul.raghavSubscriber
Boundary layer:
A wall function is needed to accurately predict the flow in the boundary layer. Boundary layer is the thin region near a wall where the velocity gradient in the direction normal to the wall is high (the velocity goes from zero at the wall to ~ the mainstream velocity at a certain distance away from the wall). The boundary layer exists for all flows, let it be laminar, transitional or turbulent. A laminar flow would have a laminar boundary layer, which is straightforward. On the other hand, a turbulent boundary layer would have a very thin viscous sublayer next to wall, a transition layer (buffer zone) and the turbulent boundary layer (loglayer). The turbulent boundary layer on a flat plate and the velocity profile across a turbulent boundary layer is shown in the image below.
Why do we need a wall function?
From CFD standpoint, it is essential that we create a mesh/grid which can accurately predict the velocity gradient across boundary layer. For turbulent flows, we would ideally want the first cell from the wall to lie within the very thin viscous sublayer. Though this might be possible for certain flow scenarios, this criteria cannot be fulfilled for complex flows in complicated geometries as it would require a very fine mesh resolution near the wall which would extensively increase the time required for solving the problem. To deal with this requirement, a wall function is introduced which allows the use of a "relatively" larger mesh near the vicinity of the wall. Now depending on the region of the boundary layer you want to capture, you would need the appropriate mesh and appropriate wall function. Another important parameter when it comes to wall functions is yplus (y+). y+ is the nondimensional distance from the wall to the first node from the wall. The different regions of the turbulent boundary layer based on y+ would be: laminar sublayer (y+ <5); transition or buffer layer (5 < y+ <30); and turbulent or loglayer (y+ >30). The velocity is linear in the viscous sublayer while its logrithmic for the loglayer (see image below). One important point is that the first cell adjacent to the wall should not lie in the buffer zone, i.e., y+ should not be between 5 and 30 (Not good: 5 > y+ > 30).
Near Wall Treatment for ke turbulence model in Ansys Fluent:
Standard wall function:
If the first cell cannot be placed within the viscous sublayer and it lies in the loglayer region, standard wall functions can be employed. "They provide reasonably accurate predictions for the majority of highReynoldsnumber, wallbounded flows." The y+ value should be between 30 and 300 (valid: 30 > y+ >300).
Nonequilibrium wall function:
Under severe pressure gradient and strong nonequilibrium flows, the standard wall functions do not predict the flow accurately. So the nonequilibrium wall function provides a better prediction. "Because of the capability to partly account for the effects of pressure gradients and departure from equilibrium, the nonequilibrium wall functions are recommended for use in complex flows involving separation, reattachment, and impingement where the mean flow and turbulence are subjected to severe pressure gradients and change rapidly." The y+ value should be between 30 and 300, just like the standard wall function (valid: 30 > y+ >300).
Enhanced wall treatment:
When the viscous sublayer needs to be captured in cases like transitional flow, separation, heat transfer, frictional drag prediction etc., the first cell has to be located within the viscous sublayer and the y+ should be less than 1 (valid: y+ < 1). For complicated geometries, the y+ can go upto 5 (valid: y+ < 5).
Following are some resources which might help you understand more about the topic:
1. A very good blog post explaining the above concepts with respect to the mesh near the wall, turbulence model and the wall function is provided below:
Estimating the First Cell Height for correct Y+
2. LearnCAx: Basics of Y Plus, Boundary layer and wall function in turbulent flows

May 25, 2018 at 10:56 pmWalaaSubscriber
Thanks a bunch Raul.

May 26, 2018 at 3:36 pmJosé MantovaniSubscriber
Very explanatory of your answer Rahul!
Just to complement, the interest in obtaining a mesh with a satisfactory Y + number is due to the fact that in order to calculate the drag coefficient, that in a certain way, the experimental result coincides with the numerical result, this approach is necessary. The calculation is much more accurate (to calculate the wall shear) from a refined cell near the wall than by the cell center value, due to the high gradients. However, in an external flow, for example, around a wing as the angle of attack increases this approach is no longer useful due to the detachment of the boundary layer.
Hugs,
Mantovani.

May 27, 2018 at 11:50 amRaef.KobeissiSubscriber
Also to add, there is an approximative method to calculate the thickness of the inflation layer to achieve a desired Y+ value:
Check this page:
https://www.cfdonline.com/Wiki/Dimensionless_wall_distance_(y_plus)
Also this online calculator:
https://www.raefkobeissi.com/yplus/yplus.aspx

February 9, 2020 at 3:04 pmsalahSubscriber
Hi friends
I am a first year doctoral student at the university. currently I imply CFD modeling in fluent. I spent a year in the mesh, could you help me choose the best mesh for (y plus) and (dy first cell no mesh) for a turbulent simulation with number of Re = 6000 to 100000 to calculate the constant ( of the logarithmic profile of the law of log.
Vx / (V *) = 2.5 Ln (y / k) + B.
with artificial roughness effect
1. Please explain to me how y + was chosen, how the turbulence model was chosen (k epsilon, kw, scalable or improved RNG or standard ...)
2. Can I use the same mesh to calculate the shear stress and the logarithmic profile and the constant B

February 10, 2020 at 6:30 amDrAmineAnsys Employee
1/Better to open a new thread
2/Use a fine mesh with yplus around 1 to 5 if using two equations turbulence models
3/New roughness models requires even finer mesh

March 4, 2020 at 6:39 pmsalahSubscriber

August 6, 2020 at 8:58 pmDiliniSubscriberHello,nIn my case I am using SST model. My first cell height is an extremely small value (around 5*107 m) When I use this I get the floating point error. When I use a coarse mesh and proceed my simulation proceeds without any issue.nSo the problem is with my mesh. But I am not sure how to fix it. I use inflation and make my first cell height the above value.nPlease any help would be highly appreciated. Been stuck for days in this now.nThank you.nRegardsnDilinin

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
Ansys Blog
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.
 Suppress Fluent to open with GUI while performing in journal file
 Heat transfer coefficient
 What are the differences between CFX and Fluent?
 Floating point exception in Fluent
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Getting graph and tabular data from result in workbench mechanical
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error in cfd post

1862

1661

907

650

349
© 2022 Copyright ANSYS, Inc. All rights reserved.