# Uniform Flow around a cylinder

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

 LinkBack Thread Tools Display Modes
 March 6, 2009, 15:52 Dear all, I simulate the th #1 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Sponsored Links Dear all, I simulate the three simple cases with uniform flow around a cylinder(air viscosity): R(mm) U(m/s) Cd 1 0.0002468 102.4368 2 0.0001234 132.8182 4 0.0000617 231.2099 The upstream, downstream and top distances from the cylinder center are the same:100 millimeter. Since the Re numbers are the same in these three cases, I do not know why Cd is different from each other. According to theory, they should be the same when Re is the same. I use simpleFaom, and the residual for U is 10^(-6), for p is 10^(-5). Thank you for your attention. Bin
 Sponsored Links

 March 6, 2009, 18:22 Dear all, I know that I get #2 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Dear all, I know that I get three different answers for the same Reynolds number is disturbing. I would like to give all the detailed information if some of you are interested. Anyway, our purpose is to find a solution to this problem. Best regards, Bin

 March 6, 2009, 18:25 Dear all, I know that I get #3 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Dear all, I know that I get three different answers for the same Reynolds number is disturbing. I would like to give all the detailed information if some of you are interested. Anyway, our purpose is to find a solution to this problem. Best regards, Bin

 March 7, 2009, 02:53 You are scaling the cylinder, #4 New Member   Jon Tegner Join Date: Mar 2009 Posts: 7 Rep Power: 10 You are scaling the cylinder, if you want to solve the same (non dimensional) problem you should also scale the other dimensions of the problem (computational domain, resolution). Regards, /jon

 March 7, 2009, 03:53 Dear Zhoubin im really in #5 Member   Nugroho Adi Join Date: Mar 2009 Location: norway Posts: 79 Rep Power: 10 Dear Zhoubin im really interested with your research and simulation please send me the detailed information now, im working on the condensation process around the cooling tubes need a lot of references my email is : nugroho[dot]adi[dot]s[at]gmail[dot]com xie xie

 March 7, 2009, 08:34 Hi Jon, Thank you for your #6 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi Jon, Thank you for your reply. I will try to do as you suggested and report my results here. BTW, Adi, I will send you my test case to you after I have results from Mr.Joh's advice. Best regards, Bin

 March 8, 2009, 04:08 Hi Jon, You are right, I ha #7 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi Jon, You are right, I have proved your suggestions: even though Re=u*d/miu seems the same in these three cases, if we do not scale the computational domain, Cd will be different (Re is not only influenced by the cylinder features!) Thank you very much for your kindness. Hi Adi, I am sending you the test case I have, if you have any questions, please feel free to email me. Best regards, Bin

 March 8, 2009, 08:55 Hi,zhoubin You mean you sol #8 Senior Member   Hua Zen Join Date: Mar 2009 Posts: 120 Rep Power: 10 Hi,zhoubin You mean you solve the problem after you scale the computational domain? I also consider the problem and wonder if it is caused by the extreme low Re.If you like,you could try experiments with Re around 50-100 and see if it helps. My guess is that at your Re,some other effect may be also important beside Re.

 March 9, 2009, 15:44 Hi Hua Zen, Thank you for y #9 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi Hua Zen, Thank you for your attention and your suggestion. When I use blockMesh and scale my computational domain, Cd is the same. However, this problem is still under study, especially Re is very small, as you said. Since there is no experimental data for Re between 0.01~0.1, I am very interested in this regime. If you know some experiments, welcome to share with me. Best regards, Bin

 March 12, 2009, 18:01 I have proved that when Re: 0. #10 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 I have proved that when Re: 0.5~20, OpenFOAM get very close Cd when compared with analytical results, as well as experiments. Then, what's wrong with Re:0.001~0.1? I ask myself....

 March 12, 2009, 19:12 Hi,Bin Nice to see your res #11 Senior Member   Hua Zen Join Date: Mar 2009 Posts: 120 Rep Power: 10 Hi,Bin Nice to see your results.In fact,I'm doing similiar work now,on the contrary,My interest is in the range of large Re,10^5--10^7. I admire your interest range,at least you are not bothered by the turbulence. For your result,at least for Re 0.1 ,the result is acceptable from my view.The is the lowerest limit of Re in one Cd-Re figure I have ever seen.In the log-log figure,we could not see the difference of the two number. Now my suggestions: Since for your range,you have analytical results.I think it would be better to compare your model formulation with the derivation of the analytical result to check whether there is something different. If they are same,then try change your fvsolution to more stringent values since your velicity and geometry values are both small. Finally,note the assumption used in the analytical derivation. I guess infinite large domain may be used.If this is the case,you would better to keep the computation domain as large as possible. By the way,I have a question,for your interest range,analytical result exist.Then why do you need to model it?Why not just use the analytical formulation.

 March 13, 2009, 02:15 Hi Bin Just a thought: A #12 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,749 Rep Power: 29 Hi Bin Just a thought: As far as I recall the analytical values originates from a potential solution on which a laminar boundary layer is added between the potential flow solution and the cylinder. In your range the drag force should be originating entirely from the shear stress on the cylinder, thus you could try comparing your boundary layers on the cylinder with the analytical expressions and verify, whether or not the development looks reasonable. Have a nice day, Niels __________________ Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.

 March 13, 2009, 02:17 Hi,Hua Zen, First of all, t #13 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi,Hua Zen, First of all, thank you very much for your immediate response. You are right, I am not bothered by the turbulence, and I am lucky at this point. Let me answer for your suggestions: 1.Since for your range,you have analytical results.I think it would be better to compare your model formulation with the derivation of the analytical result to check whether there is something different. Ans: I accept your suggestions, and this is the only way I may find the difference. 2.If they are same,then try change your fvsolution to more stringent values since your velicity and geometry values are both small. Finally,note the assumption used in the analytical derivation. I guess infinite large domain may be used.If this is the case,you would better to keep the computation domain as large as possible. Ans: after I conclude that: when the computational domain is scaled with the cylinder radius, we could get the same Cd when Re is the same. (Thank Mr. Jon) Even though I can not fully understand why computational domain influence Cd? From above conclusion, I use a whole cylinder with radius 1m (not other unit), and the upstream, downstream and top distance to be 100 m (I suppose this is enough, and do you think this could be though as large enough?) 3.By the way,I have a question,for your interest range,analytical result exist.Then why do you need to model it?Why not just use the analytical formulation. Ans: Upon my knowledge, there is no experimental data in this Re range. I have only analytical solution. But my purpose is not verifying OpenFOAM with analytical data for the simple cylinder case. Because I have a very complex model, after I am sure that OF is valid for this simple case, I could use OF to my complex model. Last but not least, appreciate your suggestions. My question for myself now: is there any solver suitable for Re: 0.001~0.1. Now I could conclude: simpleFoam (when trubulence model is off) is not good. Best regards, Bin

 March 13, 2009, 02:31 Hi Niels, Feel excited to s #14 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi Niels, Feel excited to see your reply to me How are you recently? You are right, there is so called Stokes' paradox for this simple cylinder case(when uniform flow is around the cylinder with no-slip wall boundary on it). Until now I have several analytical solutions, one of them is from Davies ( an expert in air filtration), another one is from Prof. Shaw (a mathematician). Davies' expression is validated by Finn's experiment at Reynolds numbers from 0.06 to 0.5. Prof. Shaw get the analytical solution for this problem. This is why I compare their data with OF simulations. As for your suggestions: "you could try comparing your boundary layers on the cylinder with the analytical expressions and verify", could you please tell me how to do? Because I am not so good at CFD. What I have done is that: I have sampled a matrix of points around the cylinder, then I compare the velocity with Prof. Shaw's analytical. They fit quite well. As we know that if velocity field is the same, when we apply Bernoulli's equation,we should get the same pressure field as well as drag coefficient. But why I get different Cd from analytical? Thank you, Mr. Niels. Best regards, Bin

 March 13, 2009, 03:36 Dear readers: My conclusion #15 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Dear readers: My conclusion of my post "Friday, March 13, 2009 - 12:17 am" has a mistake. I could not conclude so rudely. simpleFoam is useful for my extreme low Re case. I will report to you once I get better results. I will show you why. Thank you for your attention. Bin

 March 13, 2009, 04:53 Dear OpenFOAM friends: As w #16 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Dear OpenFOAM friends: As we know, at low Re number flow, the effect of the body extends far away, especially for cylinder. I make a simulation for a cylinder with radius 1m, but with following domain (upstream, downstream, top and down distance L): L (m) 100 500 1000 5000 10000 Cd 5987.933 4269.73 3805.048 3079.464 2756.41 Analytical solution for Re=0.001 is Cd=2821. Should I continue to increase the domain, just for the 1m-radius cylinder? Will Cd decrease further? Best regards, Bin

 March 13, 2009, 05:20 Dear zhoubin, there is a pape #17 New Member   David Sponiar Join Date: Mar 2009 Location: Prague, Czech rep. Posts: 27 Rep Power: 10 Dear zhoubin, there is a paper, which describe the dependece of the Reynolds number to the size of the domain. __________ Title: Momentum and heat transfer from cylinders in laminar crossflow at 10-4 =< Re =< 200 Authors: Bogard D.D.; Garrison D.H.; Lange C.F.; Durst F.; Breuer M. __________ I did not try to simulate laminar flow with so lower Re. I tested spectrum of Re=40 to 180 and I have to prepare domain: Length=200D, Witdth=65 up to 100D. I get results with very good agreement to the experimental data. If you have acces to the paper, you can find the answer to your question. David _____

 March 13, 2009, 05:29 Hi David, Thank you for sha #18 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi David, Thank you for sharing this knowledge. I can not get that pdf paper now, would you mind if I ask you to help me, send that paper to: zhoubinwx at hotmail.com? I will investigate this deeply. Thank you again. Bin

 March 13, 2009, 06:14 Hi,bin Since you do not men #19 Senior Member   Hua Zen Join Date: Mar 2009 Posts: 120 Rep Power: 10 Hi,bin Since you do not mention your fvscheme and fvsolution file.I don't know the detail.Try use higher order discretization method and more stringent tolerance and see if it help. You refer that in the third dimension,you use 100m.That's too large.What is the size of your first grid around the cylinder? Try use the third dimension size that is comparable to the first grid size around the cylinder. Finally,since there is indeed some assumption in the analytical expression.So do not expect perfect agreement with it. Best wishes. BTW,for me,still struggling with the Hi-Re calculations,the only advantage is that ,no matter how large the error is,Cd is still in the range from 0 to 1.since the pressure drag dominate.

 March 13, 2009, 06:31 Hi,Hua Zen, Thank you very #20 Senior Member   ZHOU Bin Join Date: Mar 2009 Location: Nanjing/Torino, Nanjing/Piemente, China/Italy Posts: 164 Rep Power: 10 Hi,Hua Zen, Thank you very much for your input. Now let me answer your questions: 1.Since you do not mention your fvscheme and fvsolution file.I don't know the detail.Try use higher order discretization method and more stringent tolerance and see if it help. Ans: fvScheme file: --------------- ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div(phi,nuTilda) Gauss upwind; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1|A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } fvSolution file: solvers { p PCG { preconditioner DIC; tolerance 1e-06; relTol 0.01; }; U PBiCG { preconditioner DILU; tolerance 1e-05; relTol 0.1; }; k PBiCG { preconditioner DILU; tolerance 1e-05; relTol 0.1; }; epsilon PBiCG { preconditioner DILU; tolerance 1e-05; relTol 0.1; }; R PBiCG { preconditioner DILU; tolerance 1e-05; relTol 0.1; }; nuTilda PBiCG { preconditioner DILU; tolerance 1e-05; relTol 0.1; }; } SIMPLE { nNonOrthogonalCorrectors 3; } relaxationFactors { p 0.3; U 0.7; k 0.7; epsilon 0.7; R 0.7; nuTilda 0.7; } I could see that you suggest me to use : higher order discretization method and more stringent tolerance. Do you have any suggestions for this according to your experience? 2. You refer that in the third dimension,you use 100m.That's too large.What is the size of your first grid around the cylinder? Try use the third dimension size that is comparable to the first grid size around the cylinder. Ans: now in my test case, the third dimension is 1m while the cylinder radius is 1m. BTW, I'm fairly confident to say that z-direction does not have any influence for 2-D simulations. because I've made try with z-width as 1m, 10m and 100m, and I get the same Cd. 3. Finally,since there is indeed some assumption in the analytical expression. So do not expect perfect agreement with it. Ans: I agree with you at this point. The problem is I must get simulated results not far from analytical solution. My acceptable relative error is 2%. 4.I would like to say:good luck to your high-Re simulations. Best regards, Bin

 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 momentum_waves Main CFD Forum 1 November 17, 2008 21:54 cfdxue Main CFD Forum 0 November 27, 2007 00:26 ubik Main CFD Forum 0 February 20, 2007 07:28 Michael Hu FLUENT 1 April 13, 2006 22:11 patrick raj CFX 2 September 24, 2005 02:43

 Sponsored Links

All times are GMT -4. The time now is 05:10.

 Contact Us - CFD Online - Top