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

Bluff body vortices

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 8, 2008, 15:06
Default Hello and a Good Evening :-)!
  #1
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello and a Good Evening :-)!

Hope everyone is having a great week!!

I have gotten myself stuck with the (fairly strong) wish to try out vortex shedding behind bluff bodies in a liquid medium....

Over the last two days I have tried to simulate this, but for some reason, I just dont seem to get any vortices....The simulation works out fine, but no vortices....

I tried a simple geometry which basically consists of a tube with a triangular body placed diagonally along the entire diameter (perpendicular to the direction of flow). The direction of flow is axial along the tube, and such that it makes contact with the base of the triangle first.

The medium I tried was water, and I used transientSimpleFoam as my top-level solver....

I used the GAMG Solver for pressure, and PBiCG for velocity, k, and epsilon.

The div scheme was upwind, temporal scheme was Euler, and the laplacian scheme was Gauss linear corrected.

The mesh is pure tetrahedral, without any hexahedral cells for boundary layers, etc..etc....

The diameter of the tube at the inlet is 15mm, and I tried it a velocity around 1m/s... which means the reynolds number is around
Re = (1*(15/1000))/(0.95e-06) = ~15800

The question is.... do I need to do anything special to be able to see the vortices? Or do I need to use some special settings on the solver, or use a different solver altogether?

The vortices would be seen as variations in the pressure and velocity fields without any additional post-processing right?

What might I be doing wrong?

Have a great evening!

Philippose
philippose is offline   Reply With Quote

Old   April 8, 2008, 15:22
Default Yes: you need second order on
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Yes: you need second order on momentum convection term at the very least. Second order in time might help, but that depends on how bad your Co number is.

This should work with correct discretisation settings - right now you've got too much numerical diffusion. Do you get a recirculation region behind the body? is it symmetric?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   April 8, 2008, 17:38
Default Hello Hrv :-)! And once aga
  #3
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello Hrv :-)!

And once again.... I deeply appreciate your help, and I profusely thank you for pointing me in the right direction :-)!

I did have recirculation zones on the sloped sides of the triangle, and was wondering why it wasnt detaching itself!

The fvSchemes file has been duly modified... changed the div scheme for div(phi,U) to Gauss linear (which would be a second order bounded scheme right?) and though the transientSimpleFoam Courant number was around 12 odd in my last few trials, I thought I would try out CrankNicholson this time.

Just for completeness... the important parts of the fvSchemes file are:

temporal Scheme: CrankNicholson 1.0

grad Schemes: Gauss linear

div Schemes: Gauss linear for U ; upwind for k, epsilon

laplacian Schemes: Gauss linear corrected

I hope this setup will show up with something....

Thanks again...!

Philippose
philippose is offline   Reply With Quote

Old   April 9, 2008, 02:46
Default Hi Philippose You are askin
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi Philippose

You are asking if you should use another solver. All I have read about the k-epsilon turbulence models have convinced me not ever to use it, if a k-omega model i present.
The short version is that the k-epsilon has a very hard time to handle adverse pressure gradients whereas k-omega model (SST) are significantly better at it. Since your system is strongly influenced by adverse pressure gradients, I would make the switch.

Have fun

- Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   April 10, 2008, 13:18
Default Hello once again, And ofcou
  #5
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello once again,

And ofcourse... a Good Evening to everyone too :-)!

Soo... status update on this issue.... as of now... I have not yet been successful in generating vortex shedding...

I made quite a few screenshots and a couple of animations of how things look, but forgot to bring it back with me... however, here is one I had taken two days ago....:



So far, I have tried with the following setups:

1. Temporal: Crank Nicholson 1.0 ; Crank Nicholson 0.5

2. Div Schemes for U: Gauss linear ; Gauss cubic

3. Interpolation schemes for U: linear ; cubic

And, I have run simulations with a variety of time step sizes (0.0001 to 0.02), a variety of total durations (the longest being 6 seconds), and with meshes of around 110,000 and 300,000 cells

In all the above trials, I maintained all the other settings constant. The inlet is around 10 l/min, and the outlet is around 1 bar (both fixedValue constraints).

One more thing worth mentioning... I have been using transientSimpleFoam all this while. For a check, I tried turbFoam, but even with a time step size of 1e-05, the Courant number kept going up... could the fact that the PISO solver is having trouble point to something?

All the results showed more or less the same results (with varying degrees of recirculation, depending on the length of the simulation), but none of them displayed vortex shedding.

Currently a simulation which uses the k-Omega SST is ongoing. When I checked after a simulation time of around 0.6 seconds, I could see the same behaviour, though the recirculation regions, seem to be much more developed than in the other simulations with the k-epsilon model. So need to see how that looks tomorrow...

To visualise vorticity, I am using the "vorticity" utility in OpenFOAM-1.4.1-dev.

I can post a couple more images of the setup if required, though, it might be easier to mail it due to their size.

Annnny idea what might be going wrong here? I never thought this would be so painful... :-)!

Have a nice day!

Philippose
philippose is offline   Reply With Quote

Old   April 10, 2008, 13:20
Default One more thing..... I have
  #6
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
One more thing.....

I have been wondering... why are the recirculation regions only limited to the top and bottom parts of the body? Shouldn't it be more or less the same down the entire length of the obstruction?

Philippose
philippose is offline   Reply With Quote

Old   April 10, 2008, 13:45
Default Are you sure the case should e
  #7
New Member
 
Steve Collie
Join Date: Mar 2009
Location: Valencia, Spain
Posts: 5
Rep Power: 8
stevecollie is on a distinguished road
Are you sure the case should exhibit vortex shedding? From your image it looks like there are junction vortices at the top and bottom, which are dominating. With such a low aspect ratio the flow is very 3D and there may be no chance for regular vortex shedding to develop. Potentially the mean-flow solution could be steady - or maybe only slightly unsteady with longish time-scales. Your time step size might not be capturing this or your as mentioned earlier numerical diffusion may be damping it out. Is your grid fine enough (y+=1 on the object)?

Also with sharp corners there are defined separation points which reduces the chance of unsteady vortex shedding. Perhaps try a circular cylinder instead of a triangle and with a much bigger aspect ratio.

Steve
stevecollie is offline   Reply With Quote

Old   April 10, 2008, 15:34
Default Hello Steve, Now thats a ve
  #8
Senior Member
 
Philippose Rajan
Join Date: Mar 2009
Location: Germany
Posts: 530
Rep Power: 16
philippose will become famous soon enough
Hello Steve,

Now thats a very interesting picture you have given me :-)!

Maybe its time to put in some background into the whole exercise just to make things more clear....

First... my usual line of work is in Hydraulic valves, so I am extremely new to the whole "simulation of vortex shedding" concept.... (now that the disclaimer is done :-)....!)

The whole thing started out with a discussion that I had with someone who works in a company manufacturing Vortex Flow Meters.

These Vortex flow meters use the concept of vortex shedding, with something like a paddle downstream from the bluff body which detects changes in pressure due to the vortices shed by the bluff body.

Using the frequency of the pressure pulses on either side of the paddle, the flow through the meter can be determined (via the Strouhal Number).

As of now, all the development work in the company occurs via trial and error... for example... the geometry of the bluff body, the distance between the body and the sensor paddle...the frequency to flow relationship...etc...etc...

So I was wondering whether it would be possible to use CFD to help them out by making the development more insightful, since the geometry is very simple, and there are no moving parts, etc...etc... and measuring the frequency on the paddle is also a simple matter in OpenFOAM...

The tube and the triangle in the picture above has the same form as a test model I got of a vortex flow meter they use... the only part I excluded from the test case above, was the paddle located downstream from the triangle...

I am not sure if removing this paddle changed the system... my idea was, that the vortex shedding should be a characteristic of the bluff body, and once I could simulate that, I could include the paddle to measure the forces on it...

After discussing with the person, I found that for a flow of 10 l/min, the pulse frequency should be around 50 - 60 Hz...

Anyway.... I can try with a different aspect ratio, and maybe a triangle with rounded edges...However, I was wondering, would it make more sense to try LES ??

And any other ideas which might bring some more clarity into the situation?

Thanks for all the help :-)!

Philippose
philippose is offline   Reply With Quote

Old   April 10, 2008, 16:52
Default Hi Philippose, I'm not an exp
  #9
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hi Philippose,
I'm not an expert in this area either, but as I remember, vortex shedding is studied usually at Re < 500 so there is no point in having a turbulence model (to model what???). What is your Re number?
Another thing that I remember is the prism oriented in the opposite direction to the flow, not as it is in your case.
Sharp edges will help generating the vortices so don't round them.

I hope this will be helpful,
Dragos
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 16:54
Default ...and another memory coming b
  #10
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
...and another memory coming back: the closer to a 2D case is your domain, the larger the coherent structures will be.

Dragos
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 17:00
Default ...and another memory coming b
  #11
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
...and another memory coming back: the closer to a 2D case is your domain, the larger the coherent structures will be.

Dragos
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 19:01
Default "I'm not an expert in this are
  #12
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
"I'm not an expert in this area either, but as I remember, vortex shedding is studied usually at Re < 500 so there is no point in having a turbulence model (to model what???)."

I totally agree with Dragos. Also, at higher Re, I have never really understood what the k-epsilon turbulence model is capable of? You might be better off doing a LES instead.
msrinath80 is offline   Reply With Quote

Old   April 10, 2008, 19:02
Default Maybe try with the pointed sid
  #13
New Member
 
Steve Collie
Join Date: Mar 2009
Location: Valencia, Spain
Posts: 5
Rep Power: 8
stevecollie is on a distinguished road
Maybe try with the pointed side of the triangle pointing upstream.

As Dragos said if the flow is at a lower reynolds number than you have been testing at then vortex shedding is much more likely to be apparent. Maybe try without the turbulence model anyway since the turbulent viscosity will definately dampen such features. However if it is RE=15800 as you say then the flow will be turbulent. 2eqn turbulence models should still be able to capture vortex shedding (LES would be overkill), so maybe your grid is just too coarse.

Steve
stevecollie is offline   Reply With Quote

Old   April 11, 2008, 04:53
Default Hi Interesting discussion,
  #14
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,594
Rep Power: 24
ngj will become famous soon enoughngj will become famous soon enough
Hi

Interesting discussion, and very nice way to start the day Though I am not agreeing that vortex shedding is mainly studied for Re < 500 - I am a coastal engineer and we are typically working with Re=O(1E6) and vortex shedding is a significant contribution to such things as mean forces, vortex induced vibrations, etc.

In my old book from a class in vortex shedding (though we mainly worked with cylinders), it is stated that for Re>300 the wake is completely turbulent, thus stick with your turbulence model. Furthermore I have been thinking about the lack of vortex shedding, and believe it is well illustrated by the following analogy:



For the case without a plate, the vortices on either side of the cylinder are free to interact and that results in vortex shedding (which is basically one vortex being large, sucking in the smaller one, which cuts of the source of vorticity to the larger one, thus is becomes a free vortex and it is advected downstream).

In the case with the plate, the vortices are not capable of interacting, thus they are significantly more reluctant to be shed, thus no shedding occurs. In the present case, the vortices are separating at the corners, but if they are not large enough to interact downstream the top of the triangular shaped body, no vortex shedding occur (at least not shedding of the full vortices, smaller parts of either vortex could possibly be shed).

So, if you want to see vortex shedding, try to rotate is a already suggested or just for the fun of it try to put it in a asymmetric way with respect to the center axis.

LES should be last call, I do believe you would be able to get shedding with k-omega SST.

Best regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   April 11, 2008, 08:02
Default Your problem is almost certain
  #15
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Your problem is almost certainly tied to your use of transientSimpleFoam. Please post your fvSolution dictionary.

The main reason turbFoam runs (or any runs for that matter) blow up with steadily increasing Courant numbers is inflow at the outlet. Make sure your velocity boundary at the outlet is of type inletOutlet with zero inletValue. "Gauss linear" for div(phi,U) could also cause the solution to blow up - try "Gauss linearUpwind Gauss linear" instead.

This configuration should shed, no doubt - if it is not doing so, your numerics are simply too damped.
eugene 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
CFD of flow behind bluff body puneshwar verma FLUENT 1 January 1, 2007 14:20
Bluff Body krithiga CD-adapco 4 November 7, 2006 16:45
bluff body and Y+ justin FLUENT 3 May 4, 2006 20:13
RSM+bluff body anto FLUENT 2 March 1, 2006 10:39
BLUFF BODY+ RSM Anto FLUENT 2 August 3, 2005 05:09


All times are GMT -4. The time now is 03:19.