[anno_x]

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]

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.

[ghorrocks]

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.

[anno_x]

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]

I used periodicity in domain interface for front and back planes.
I should wait until the process completes...

[anno_x]

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

[ghorrocks]

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.

[cfdman]

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

[galap]

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.

[anno_x]

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]

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!

[Lance]

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.

[anno_x]

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!

[ojha.mayank485]

Have you validated your results with experiments. May I know which Paper you are looking at for validation ????