CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

interFoam solver for free surface flow past a circular cylinder

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 5, 2011, 00:21
Default interFoam solver for free surface flow past a circular cylinder
  #1
Member
 
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 64
Blog Entries: 1
Rep Power: 5
tfuwa is on a distinguished road
Hi All Foamers,

Thanks for taking time to read on.

As the title indicated, I am simulating the flow around a surface piercing cylinder using interFoam (1.7.1). The Re number and the Froude number based on cylinder diameter D is 27000 and 0.8 (Fr = U/sqrt(g*D). The mesh is generated with Gmsh, for all simulations y+ was kept below 1, and mesh sensitivity study was completed. The mesh looks like as attached (stretching in z-direction ),

The simulations are proceeded with 4-diameters depth of water and 2-diameter depth of air. The LESimulation with oneEqEddy turbulence model is chosen. The results are encouraging but not good enough as simulated in published papers. The lift and drag coefficients are shown below. While the drag is around 1.05 (close to numerical work by others), the lift does not vibrate enough, leading to a Cl rms below 0.1 (should around 0.2). Also, the Strouhal number is away from right.

The average surface elevation is beautiful , but has a space to be improved compared to experimental results, as illustrated below.

In order to improve and get the force coefficient right, I have tried different turbulence models (LES dynOneEqEddy, Standard k-e), and different convection schemes (limitedLinear, filteredLinear, SFCD, upwind and others), but without success.

Can you please enlighten me on how to improve the simulations and point out where I am wrong?

I attached the fvSchemes, fvSolution and LES coefficients files below, but if more information is needed, do not hesitate to ask for.

Cheers,
Albert
Attached Images
File Type: jpg mesh.jpg (74.2 KB, 113 views)
File Type: png forceC.png (12.8 KB, 87 views)
Attached Files
File Type: txt fvSchemes.txt (1.5 KB, 43 views)
File Type: txt fvSolution.txt (3.1 KB, 27 views)
File Type: txt LESProperties.txt (1.7 KB, 35 views)
tfuwa is offline   Reply With Quote

Old   October 5, 2011, 00:23
Default
  #2
Member
 
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 64
Blog Entries: 1
Rep Power: 5
tfuwa is on a distinguished road
Another two attachment.

Albert
Attached Images
File Type: jpg contour4.jpg (89.2 KB, 99 views)
File Type: png ExperimentFromJournalofFluidsandStructures27(2011)122.png (54.0 KB, 57 views)
tfuwa is offline   Reply With Quote

Old   October 5, 2011, 02:12
Default
  #3
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 782
Rep Power: 11
Bernhard is on a distinguished road
How does your mesh compare to the meshes of the results that you are referring to? I can imagine that the high aspect ratio cells at your inlet will be a problem here. Also, what is the inflow condition in your simulation?
Bernhard is offline   Reply With Quote

Old   October 5, 2011, 05:32
Default
  #4
Member
 
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 64
Blog Entries: 1
Rep Power: 5
tfuwa is on a distinguished road
Dear Bernhard,

Thanks a lot for your reply.

The computational domain in my simulation 45D*20D*6D (x*y*z), and I used 60 grids in z-direction. I have two references at hand, and they used 33 grids for 5D (Journal of Fluids Engineering, 2002, Vol. 124, 91-101) and 128 grids for 6D (Journal of Fluids and Structures 27, 2011, 122) in z-direction, respectively. And they got similar results. My cell aspect ratio follow between them, but I will try fine mesh in z-direction later on.

The initial conditions are as follows,

inlet
{
U fixed value; p_rgh buoyantPressure; nuSgs zeroGradient; k fixed value 2.354e-2; alpha1 fixed;
}

atmosphere
{
U pressureInletOutletVelocity; p_rgh zeroGradient; nuSgs zeroGradient; k inletOutlet; alpha1 inletOutlet;
}

outlet
{
U zeroGradient; p_rgh totalPressure; nuSgs zeroGradient; k inletOutlet; alpha1 zeroGradient;
}

cylinder
{
U fixedValue uniform (0 0 0); p_rgh zeroGradient; nuSgs zeroGradient; k fixedValue; alpha1 zeroGradient;
}

bottom and sides
{
type symmetryPlane;
}

I appreciate your comments and would like to receive more to get the problem solved.

Cheers,
Albert
tfuwa is offline   Reply With Quote

Old   October 5, 2011, 05:45
Default
  #5
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 782
Rep Power: 11
Bernhard is on a distinguished road
With a fixedValue BC for U at the inlet, you will not have velocity fluctuations on the scales larger than the grid scale (since you impose a uniform distribution). In other words, you start with u'_rms = 0, which is not true of course.
Please consult Inlet BC for LES for more information. Maybe you want to use the turbulentInlet boundary condition to impose some random fluctuations on the inflow.
Bernhard is offline   Reply With Quote

Old   October 5, 2011, 09:52
Default TurbulentInlet, sure, has the potential to improve the result
  #6
Member
 
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 64
Blog Entries: 1
Rep Power: 5
tfuwa is on a distinguished road
Hi Bernhard,

Thanks for your quick reply. TurbulentInlet, sure, has the potential to improve the result, but it may not be the only reason here. Previously, I simulated one phase flow around a cylinder using pisoFoam combined LES solver with the same inlet and other above mentioned fv conditions, which I should post earlier (sorry for that). That simulation gave a much better prediction on force coefficients, illustrated bellow. This result make me believe there must be other reasons.

Cheers,
Albert
Attached Images
File Type: png pisoFoam-LES.png (11.2 KB, 54 views)
tfuwa is offline   Reply With Quote

Old   June 12, 2013, 08:55
Default exaggerated free surface elevation - interfoam
  #7
Member
 
pedroxramos's Avatar
 
Pedro Ramos
Join Date: Mar 2012
Location: Portugal
Posts: 54
Rep Power: 4
pedroxramos is on a distinguished road
Hi...

I'm doing the open channel flow simulation with interFoam solver and I got a exaggerated elevation upstream the cylinder (http://d.pr/i/Ya1d).



I dont't know why... I use these BC to the atmosphere:

alpha 1
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

U:
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

p_rgh:
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
value uniform 0;
}
k
{
type inletOutlet;
inletValue uniform 0.001;
value uniform 1e-11;
}
nuSgs:
{
type zeroGradient;
}
nuTilda:
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

Help me please!

Best regards!
__________________
Pedro Ramos

FEUP, Portugal
pedroxramos 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
benchmark: flow over a circular cylinder goodegg Main CFD Forum 12 January 22, 2013 11:47
flow around a cylinder pXYZ Main CFD Forum 14 July 25, 2011 10:05
3D FLOW OVER A CIRCULAR CYLINDER Srinivas Mettu FLUENT 2 April 4, 2010 22:11
3D Flow over a circular cylinder Srinivas FLUENT 3 March 15, 2005 19:57
incompressible free surface flow past cylinder vineet FLUENT 2 April 1, 2002 04:56


All times are GMT -4. The time now is 20:03.