|
[Sponsors] |
March 25, 2014, 05:45 |
Flow around an circular cylinder
|
#1 |
Member
Christian
Join Date: Sep 2013
Location: Germany
Posts: 88
Rep Power: 12 |
Hello everbody,
im working in a project at my university. And a part of this project is to simulate a flow around a circular cylinder. My main problem is that i can not reach the values for the drag coefficent that i read in Schlichting. cd(Re=300) = 0.729 | stationary cd(Re=300) = 1.32 | instationary 1. The mesh I Meshed everything in ICEM as octree mesh and put some prism elements around the cylinder. 2. CFX Steady State ref Pressure = 1 bar T.Model = SST Boundarys: Inlet - v = 1,46 m/s Outlet = 0 bar Sides = Symetry Zylinder = Wall no slip Top and Bottom = Wall free slip Transient same as in steady state and i calculated with an Stroudhal number of 0.2 for the transient Setup: Simulation Time 0.01 s Timestep Size 0.0041 s (~25 steps) Now the Problem: For Steady state i get a cd value of 0.83 And for Transient i get an cd value of 1.1 I think both of the simulations are setup wrong because when i take a look at the pressure distribution it doesnt look like something i expect. Where did i make the mistake? Why is there no karman street like in this video http://www.youtube.com/watch?v=BVyu4UEiB1k ? Is maybe just my simulation time not long enougth? Or is my reference Re Value wrong? I calculatet the Re and cd Value with a specific length = (diameter * length) Last edited by Chris_321; March 25, 2014 at 07:33. |
|
March 25, 2014, 16:47 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
||
March 25, 2014, 16:48 |
|
#3 |
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 277
Rep Power: 21 |
A few things:
- Your boundary layer mesh looks very coarse. You should start by checking the Y-plus on the cylinder wall (should be <1-2 for SST). - Regenerate the mesh using a smaller growth ratio for the boundary layers (try 1.1-1.2). - Make sure you have enought layers around the cylinder to cover the whole height of the boundary layer. Cheers. |
|
March 26, 2014, 17:04 |
|
#4 |
Member
Christian
Join Date: Sep 2013
Location: Germany
Posts: 88
Rep Power: 12 |
||
March 26, 2014, 19:57 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
Yes, that looks much better. But you might still be a bit coarse - you will need to do a sensitivity check to find out.
Your y+ means that the automatic wall treatment will be integrating to the wall at all locations. You should be OK here, but again, a sensitivity check is the best way to be sure. |
|
March 27, 2014, 06:47 |
|
#6 |
Member
Christian
Join Date: Sep 2013
Location: Germany
Posts: 88
Rep Power: 12 |
In a tutorial they initilaize the u velocity with (step(y/1[m])+ 0.5)*xvelociy
I Know what the step function do but what means the y and why Do they use this for initilaizing? |
|
March 27, 2014, 06:57 |
|
#7 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
The y/1[m] bit converts y as a value with units of metres to a value with no units. The step function requires an argument which is unitless.
|
|
March 27, 2014, 07:56 |
|
#8 |
Member
Christian
Join Date: Sep 2013
Location: Germany
Posts: 88
Rep Power: 12 |
Is the value of y the max. y value of my domain in meter? They dont specify y in one of their expressions.
Why do they set up the Initial value with a step function? Whats the benefit of it? Is it wrong to initilize just with my x_velocity? - Im confused! |
|
March 27, 2014, 16:43 |
|
#9 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
No, y is a field variable and takes the value of the y coordinate of that point. So it varies at each point of the domain.
I suspect they use this initial condition to give the flow a strong asymmetry to start the vortex street off. This is probably not required and I would start as you have assuming just a constant X velocity. I would only artificially introduce an asymmetry if it is really required. |
|
March 28, 2014, 03:26 |
|
#10 |
Member
Christian
Join Date: Sep 2013
Location: Germany
Posts: 88
Rep Power: 12 |
thank you very mutch
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
2D flow around a circular cylinder case with interFoam solver | shuoxue | OpenFOAM Running, Solving & CFD | 2 | January 14, 2020 13:23 |
flow around a circular cylinder with velocity inlet and outflow outlet | shuoxue | OpenFOAM | 1 | March 3, 2014 10:42 |
flow around a circular cylinder with velocity inlet and outflow outlet | shuoxue | OpenFOAM Running, Solving & CFD | 0 | November 2, 2013 04:32 |
Particle deposition on circular cylinder in turbulent flow | Julian K. | CFX | 1 | October 3, 2011 17:51 |
3D FLOW OVER A CIRCULAR CYLINDER | Srinivas Mettu | FLUENT | 2 | April 4, 2010 22:11 |