|
[Sponsors] |
Wall Y+ Simulation Convergence for Various Meshes |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
February 19, 2018, 06:02 |
Wall Y+ Simulation Convergence for Various Meshes
|
#1 |
Member
Hells Blade
Join Date: Nov 2017
Posts: 61
Rep Power: 8 |
I am trying to simulate the flow of air at various pressures and also modifying my no of inlets.
I am simulating the max velocity and mass out flow at my outlet My goal is not to check the pressure and vel gradient losses at the walls however I see that when I change my mesh I get different values of Wall y+ ( from 900 max to 150 max ) the velocity at outlet reduces by 8 m/s In both the sims at diff meshes I have converging monitor residual- ie are weighted avg vell at outlet and mass flow at outlet which converges from 100 to 200 iterations However my question Do I always need to take care of wall y + value (It should be in the range of 30-300 for Standard Wall Function) . I am using K epsilon realizable turbulence model . |
|
February 19, 2018, 10:21 |
|
#2 |
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,675
Rep Power: 66 |
y+ will change with the mesh because it depends on the wall shear stress and the cell size of the wall adjacent cells.
I point you to the work of Salem & Cheah. Generally, the standard wall function likes to either be globally y+<10 or globally y+>30 so that you avoid the buffer region. So it's a good idea to check both the max y+ but also you need to check the min y+ and probably the average y+. I also recommend y+< 300 if you want reasonable wall shear values. |
|
February 19, 2018, 11:40 |
|
#3 |
Member
Hells Blade
Join Date: Nov 2017
Posts: 61
Rep Power: 8 |
Hi thanks for your reply so is wall y+ really an important criteria everytime while using turbulence modelling and do achieve reasonable range of values with increase of pressure and vel i should use a finer mesh and vice versa ?
|
|
February 19, 2018, 12:04 |
|
#4 |
Member
Hells Blade
Join Date: Nov 2017
Posts: 61
Rep Power: 8 |
I am using std wall function my min wall fn is 0.09 and max is 270 area weighted avg is 20
I am getting these results after using a very coarse mesh nw getting a difference of 2 m/s at outlet ie the veloicty now is lesser the mass flow is gone done by 0.004 kg /s The circular dia is my inlet and bottom face of the rectangular domain is my outlet at 1 bar Inlet pressure is 4 bar I am using K epsilon realizable model |
|
February 20, 2018, 09:24 |
|
#6 |
Member
Hells Blade
Join Date: Nov 2017
Posts: 61
Rep Power: 8 |
Thanks for your reply
Yes if wall y+ along the elemental wall is below 30 it means we are underpredicting turbulence What is the difference bettween enhanced and non equilibrium wall treatement |
|
February 20, 2018, 09:26 |
|
#7 |
Member
Hells Blade
Join Date: Nov 2017
Posts: 61
Rep Power: 8 |
Thanks for your reply
Yes if wall y+ along the elemental wall is below 30 it means we are underpredicting turbulence What do you mean that standard wall function is tricky to use ? What is the difference bettween enhanced and non equilibrium wall treatement |
|
February 20, 2018, 10:03 |
|
#8 | |||
Super Moderator
|
Quote:
In fact near the wall, we have no turbulence as there is no velocity We are predicting the shear stress terms incorrectly. Means if the mesh has Y+ = 5 and we are using the standard wall functions, we are providing (input) wrong value of velocity /shear stress to the law of the wall. Coz when we have Y+ below 5 (or 11.06) we should be solving it as the viscous sub-layer not the log layer. Quote:
Quote:
I cannot comment about the non equilibrium wall treatment at the moment. For this I have go back to books |
||||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Natural convection in a closed domain STILL NEEDING help! | Yr0gErG | FLUENT | 4 | December 2, 2019 00:04 |
[Commercial meshers] tmerge utility creates unwanted interface/walls comes in the final mesh | Shoonya | OpenFOAM Meshing & Mesh Conversion | 11 | January 20, 2012 06:23 |
[ICEM] Export ICEM mesh to Gambit / Fluent | romekr | ANSYS Meshing & Geometry | 1 | November 26, 2011 12:11 |
Heat Transfer simulation: No convergence problem | fiqs | CFX | 2 | April 21, 2010 15:47 |
Convergence moving mesh | lr103476 | OpenFOAM Running, Solving & CFD | 30 | November 19, 2007 14:09 |