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

vortex-induced vibration

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 13, 2010, 11:36
Default vortex-induced vibration
  #1
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
Hi, I want to simulate vortex-induced vibration of a free span marine pipeline. if any one have a cfx tutorial, please help me!
anno_x is offline   Reply With Quote

Old   December 13, 2010, 16:49
Default
  #2
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
v~0.8 m/s
d~0.8 m
Re=6.19e-5

So the flow regime would be Super critical. I think I should use 3D modeling.
anno_x is offline   Reply With Quote

Old   December 13, 2010, 17:20
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
There are a few examples of flow over a cylinder shedding vorticies on the web, try google.

If the flow instability causes the pipe to move this will increase the degree of difficulty significantly.
ghorrocks is offline   Reply With Quote

Old   December 27, 2010, 14:07
Default
  #4
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
using 3D model for the pipe in this dimensions is very complicated and time consuming. So I decided to use 2D modeling and analysis.
I used 2D mesh around a circle in box domain in ICEM. as I read in forum, I exported the mesh as fluent (.msh) file type and then opened it in cfx.
I chose the inlet, outlet and wall boundaries in cfx-pre, but when I wanted to cfx-solver, an ERROR occurred concerning that it is a 2D file and instead of using inlet and outlet, symmetry or periodic 1:1 BC should be used!
I don't think these BCs be proper for my case. then what do you suggest?
anno_x is offline   Reply With Quote

Old   December 27, 2010, 14:37
Default
  #5
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
I used periodicity in domain interface for front and back planes.
I should wait until the process completes...

Last edited by anno_x; December 28, 2010 at 08:59.
anno_x is offline   Reply With Quote

Old   December 28, 2010, 08:57
Default
  #6
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
As the first step in modeling VIV, I decided to model vortex shedding behind the cylinder in cfx. I exported the meshing from ICEM and modeled the vortex shedding with following inputs for cfx-pre:
-GEOM: circle (D=0.5m), BOX(8D upstream, 22D downstream, 8D up and 1.5D down for accounting the gap ratio), speed:0.1ms-1 in x direction, Re~3000.
-Analysis Type: Transient, total time 30s, time steps 0.01s,
- Domains: inlet with normal speed=0.1ms-1, outlet with relative pressure=0, circle and top and bottom lines as wall with no slip condition, foward and back faces as domain interface (fluid fluid, transitional periodicity and mesh connection 1:1)
- default domain: water, ref pressure=1 atm, non buoyant, stationary domain and no mesh deformation, NO heat transfer, Turbulence model= SAS SST (as mentioned in cfx help)
- initial condition: u and v=0.1ms-1 and w=0, relative pressure=1, medium intensity and eddy ...
- solver control: advanced scheme: High resolution, Transient Scheme: Second order .., turbulence numerics: High resolution, Max coef loops=3, RMS residual target= 1e-4,

I guess the meshing is fine enough and time steps are small. but I can just see the vortex behind the cylinder and no shedding occurs!!! I am confused a bit
Untitled2.jpg

Untitled.jpg

Last edited by anno_x; December 28, 2010 at 09:36.
anno_x is offline   Reply With Quote

Old   December 28, 2010, 16:44
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
I guess the meshing is fine enough and time steps are small.
There is no guessing here. Either they are small enough or they are not. Do a sensitivity check and find out and stop guessing.

Are you sure you have run the simulation long enough? The flow may still be just starting up based on the images you posted.
ghorrocks is offline   Reply With Quote

Old   December 29, 2010, 04:05
Default
  #8
New Member
 
Arda Ersan
Join Date: Aug 2009
Posts: 13
Rep Power: 7
cfdman is on a distinguished road
Vortex Shedding occurs some range of Re number. See the attached image.
I think you have to choose right range of Re and revise your inlet velocity.
Don't forget timestep must be smaller enough to capture vortex shedding. if f is frequency of vortex, timestep would be smaller than 1 / (2*f)



http://img63.imageshack.us/img63/119/82450048.jpg



Uploaded with ImageShack.us
cfdman is offline   Reply With Quote

Old   December 29, 2010, 05:16
Default
  #9
Member
 
Fabian E.
Join Date: Nov 2009
Posts: 34
Rep Power: 7
galap is on a distinguished road
For the flow around a cylinder you can guess the frequency of the vortex shedding by the Strouhal correlation.

Str = f * D / u

Str ~ 0.2 for Re = 3000

With your given values (d = 0.5 m, u = 0.1 m/s) you get f = 0.04, that is period of 25s. So your total time and your timestep is definitly too small to develop the vortex shedding. As cfdman mentioned I would recommend a smaller Re number for a clearer formation of the vortices. And think about your time settings.
galap is offline   Reply With Quote

Old   December 29, 2010, 09:04
Default
  #10
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
yes friends. you are right! the problem concerned to total time! I extend the total time with time step=0.01 and shedding occurs! I should do sensitivity analysis to ensure the appropriate selection of time steps and meshing quality and to validate the results!
thanks a lot!
anno_x is offline   Reply With Quote

Old   December 29, 2010, 11:46
Default
  #11
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
I have some problems in modeling FSI! I know how to model FSI like Oscillating plate tutorial with Transient Structural and Fluid Flow (cfx) connecting boxes in workbench with their default meshing. now I want to import the ICEM meshing, but I don't know how to import it.
(for my previous post mentioned case, when right clicking on cfx mesh, I could import mesh )
please let me know what do you think about this problem or recommend any useful tutorial.

thank you!
anno_x is offline   Reply With Quote

Old   December 30, 2010, 03:43
Default
  #12
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
It is easy to use ICEM-mesh in CFX, just import it directly inside CFX. To use ICEM-mesh for the structural part you need to import the mesh through the FE-modeler (at least in v12) and then connect it to the structural box.
Lance is offline   Reply With Quote

Old   December 30, 2010, 09:14
Default
  #13
New Member
 
amirhosein h
Join Date: Dec 2010
Posts: 22
Rep Power: 6
anno_x is on a distinguished road
Hi Lance, thanks for you answer. I did what you said. but although I created 2 bodies in ICEM (LIVE and SOLID) but FE MODELER can define 1 body. I don't know what the problem is concerning about


******************************************
PSYMM' answer:

Yes, it is very easy... Block it out as if you were trying to capture the larger region (the fluid in this case). Then instead of deleting the solid blocks (putting them in the VORFN part), right click on the SOLID part and select Add to Part. The last icon in the DEZ is Add Blocking Material. Click that and then select the blocks within the solid region.
*******************************************
Now I have 2 bodies!

Last edited by anno_x; December 30, 2010 at 09:30.
anno_x is offline   Reply With Quote

Old   May 23, 2011, 20:38
Default anno_x
  #14
New Member
 
ojha.mayank485's Avatar
 
Mayank Ojha
Join Date: May 2011
Posts: 22
Rep Power: 6
ojha.mayank485 is on a distinguished road
Have you validated your results with experiments. May I know which Paper you are looking at for validation ????
ojha.mayank485 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
Vortex Induced Vibration (VIV) modelling Kwong FLUENT 1 December 1, 2009 14:08
vortex induced vibration dorin CFX 11 December 1, 2009 14:03
Vortex Induced Vibration modelling Kwong FLUENT 0 March 24, 2007 01:41
"bit" phenomenon in Vortex Induced Vibration? JOEY Main CFD Forum 0 August 4, 2006 08:49
Vortex Induced vibration of subsea pipeline Mobasheri FLUENT 5 February 9, 2006 08:07


All times are GMT -4. The time now is 05:55.