# Bluff body vortices

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 8, 2008, 15:06 Hello and a Good Evening :-)! #1 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 549 Rep Power: 18 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

 April 8, 2008, 15:22 Yes: you need second order on #2 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,806 Rep Power: 25 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

 April 8, 2008, 17:38 Hello Hrv :-)! And once aga #3 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 549 Rep Power: 18 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

 April 9, 2008, 02:46 Hi Philippose You are askin #4 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,759 Rep Power: 29 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.

 April 10, 2008, 13:18 Hello once again, And ofcou #5 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 549 Rep Power: 18 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

 April 10, 2008, 13:20 One more thing..... I have #6 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 549 Rep Power: 18 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

 April 10, 2008, 13:45 Are you sure the case should e #7 New Member   Steve Collie Join Date: Mar 2009 Location: Valencia, Spain Posts: 5 Rep Power: 10 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

 April 10, 2008, 15:34 Hello Steve, Now thats a ve #8 Senior Member   Philippose Rajan Join Date: Mar 2009 Location: Germany Posts: 549 Rep Power: 18 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

 April 10, 2008, 16:52 Hi Philippose, I'm not an exp #9 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 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

 April 10, 2008, 16:54 ...and another memory coming b #10 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 ...and another memory coming back: the closer to a 2D case is your domain, the larger the coherent structures will be. Dragos

 April 10, 2008, 17:00 ...and another memory coming b #11 Senior Member     Dragos Join Date: Mar 2009 Posts: 649 Rep Power: 13 ...and another memory coming back: the closer to a 2D case is your domain, the larger the coherent structures will be. Dragos

 April 10, 2008, 19:01 "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: 703 Rep Power: 14 "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.

 April 10, 2008, 19:02 Maybe try with the pointed sid #13 New Member   Steve Collie Join Date: Mar 2009 Location: Valencia, Spain Posts: 5 Rep Power: 10 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

 April 11, 2008, 04:53 Hi Interesting discussion, #14 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,759 Rep Power: 29 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.

 April 11, 2008, 08:02 Your problem is almost certain #15 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 14 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post puneshwar verma FLUENT 1 January 1, 2007 14:20 krithiga Siemens 4 November 7, 2006 16:45 justin FLUENT 3 May 4, 2006 20:13 anto FLUENT 2 March 1, 2006 10:39 Anto FLUENT 2 August 3, 2005 05:09

All times are GMT -4. The time now is 16:04.

 Contact Us - CFD Online - Privacy Statement - Top