|
[Sponsors] |
advection/transient scheme-Turbulence numerics |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 21, 2023, 11:38 |
advection/transient scheme-Turbulence numerics
|
#1 |
New Member
Pegah
Join Date: Jun 2022
Posts: 3
Rep Power: 3 |
Hi,
I need some thoughts regarding the simulation of flow over a cylinder. The Reynolds number range is between (3000 to 18000). The Results which I get for Re number over 8000 with an Upwind advection scheme, First order backward Euler transient scheme, and First Order Turbulence numerics (Case 1) show a lot of difference with the high-resolution advection scheme, Second order backward Euler transient scheme, and high-resolution Turbulence numerics (Case 2). Simulations in the first case are closer to the experiment. I am wondering why? and Is it ok if I implement the first case options for the turbulence problem like this? |
|
July 21, 2023, 15:43 |
|
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32 |
Are you comparing different numerical schemes on the same mesh? If so, there is no surprise you notice differences.
Which is better? Difficult to say since I cannot tell which one is closer to mesh-independent convergence. How do you find out? You refine the mesh and compare solutions with the same numerics as you keep refining your mesh. At some point, those solutions will converge. I would expect the solution using First order numerics (Upwind) will converge slower than the Specified Blend Factor/High-Resolution schemes. Making decisions on a single mesh solution w/o verification of mesh-independent behavior, i.e. due diligence, is not a correct use of numerical methods.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 21, 2023, 23:10 |
|
#3 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
Opaque's comments are essential for the numerical side of things.
And there is a physical side as well. In the range of Reynolds number from 3000 to 18000 flow over a cylinder has a laminar boundary layer which goes turbulent in the wake. This means a standard turbulence model is not suitable as the critical part of the flow (the boundary layer) is laminar. This model is in a very tricky part of the Reynolds number regime where the flow is both laminar and turbulent. If you are trying to get lift or drag on the cylinder I would recommend you try a laminar simulation as that will model the boundary layer more accurately. If you are trying to model the wake then a turbulence model is appropriate as that part of the flow is turbulent. If you are trying to model the whole thing accurately you will find this quite challenging. It will require either an LES approach, or maybe a turbulence transition model.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
July 24, 2023, 11:02 |
|
#4 |
New Member
Pegah
Join Date: Jun 2022
Posts: 3
Rep Power: 3 |
Thank you for your help
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Turbulence postprocessing | Mohsin | FLUENT | 2 | October 3, 2016 14:18 |
Troubles Developing Turbulence | fatirishman53 | OpenFOAM Running, Solving & CFD | 1 | September 20, 2015 11:44 |
specify the turbulence intensity and the turbulence length | bennoman75 | Main CFD Forum | 0 | May 15, 2013 05:36 |
K - epsilon VS SST turbulence model | Maicol | Main CFD Forum | 0 | November 30, 2012 16:25 |
Vortex shedding, FSI-analysis, turbulence numerics | tallknuseren | CFX | 3 | May 10, 2010 04:31 |