CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Flow around an circular cylinder

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   March 25, 2014, 06:45
Default Flow around an circular cylinder
  #1
Member
 
Chris_321's Avatar
 
Christian
Join Date: Sep 2013
Location: Germany
Posts: 82
Rep Power: 4
Chris_321 is on a distinguished road
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 08:33.
Chris_321 is offline   Reply With Quote

Old   March 25, 2014, 17:47
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is online now   Reply With Quote

Old   March 25, 2014, 17:48
Default
  #3
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 272
Rep Power: 13
brunoc is on a distinguished road
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.
brunoc is offline   Reply With Quote

Old   March 26, 2014, 18:04
Default
  #4
Member
 
Chris_321's Avatar
 
Christian
Join Date: Sep 2013
Location: Germany
Posts: 82
Rep Power: 4
Chris_321 is on a distinguished road


I think this looks better

But there is still the possibillity to improve, maybe behind the cylinder.
Is my y+ ok for SST with auto wall treatment?
Chris_321 is offline   Reply With Quote

Old   March 26, 2014, 20:57
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is online now   Reply With Quote

Old   March 27, 2014, 07:47
Default
  #6
Member
 
Chris_321's Avatar
 
Christian
Join Date: Sep 2013
Location: Germany
Posts: 82
Rep Power: 4
Chris_321 is on a distinguished road
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?
Chris_321 is offline   Reply With Quote

Old   March 27, 2014, 07:57
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is online now   Reply With Quote

Old   March 27, 2014, 08:56
Default
  #8
Member
 
Chris_321's Avatar
 
Christian
Join Date: Sep 2013
Location: Germany
Posts: 82
Rep Power: 4
Chris_321 is on a distinguished road
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!
Chris_321 is offline   Reply With Quote

Old   March 27, 2014, 17:43
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,273
Rep Power: 96
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is online now   Reply With Quote

Old   March 28, 2014, 04:26
Default
  #10
Member
 
Chris_321's Avatar
 
Christian
Join Date: Sep 2013
Location: Germany
Posts: 82
Rep Power: 4
Chris_321 is on a distinguished road
thank you very mutch
Chris_321 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
flow around a circular cylinder with velocity inlet and outflow outlet shuoxue OpenFOAM 1 March 3, 2014 11:42
flow around a circular cylinder with velocity inlet and outflow outlet shuoxue OpenFOAM Running, Solving & CFD 0 November 2, 2013 05:32
2D flow around a circular cylinder case with interFoam solver shuoxue OpenFOAM Running, Solving & CFD 1 August 31, 2013 09:33
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


All times are GMT -4. The time now is 06:00.