
[Sponsors] 
May 16, 2013, 07:07 
a little smaller Strouhal number

#1 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
hi everyone!
I am simulating flow around cylinder at Re=100. But no matter how I tried, the St number I am obtaining remains 1.4, for which an accurater one is 1.6. does someone have any suggestion on how to get the accurate St number? my case setup is like this: D=1, U=1, nu=0.01, no turbulence model. any help is appreciated! 

May 16, 2013, 07:18 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
Hi, what size is your domain, i.e. how many D upstream and downstream of the cylinder?
__________________
The skeleton ran out of shampoo in the shower. 

May 16, 2013, 07:33 

#3 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 

May 16, 2013, 07:36 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
Can you also tell us the density and the viscosity?
__________________
The skeleton ran out of shampoo in the shower. 

May 16, 2013, 08:00 

#5 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
the density rho is set to be 1, and the kinematic viscosity is 0.01. With velocity=1 and Diameter=1, that makes Re =100.
the software I'm using is OpenFoam. I get quite good result in terms of drag and lift coefficients, but for St, it's always smaller. 

May 16, 2013, 08:40 

#6 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
How many time steps per cycle do you have? How much do the residuals go down each time step? How large is the domain perpendicular to the flow?
Maybe you want to have a look at this thread: http://www.cfdonline.com/Forums/mai...rre40a.html
__________________
The skeleton ran out of shampoo in the shower. 

May 16, 2013, 09:40 

#7  
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
Quote:
" the domain perpendicular to the flow", do you mean the height of the Z axis? it is 0.1D, as D=1, it should be 0.1. My case is 2d so I think it does not matter. As for the residuals, in OpenFoam different variables have different residuals, here is my setting for residuals in openfoam Code:
solvers { p { solver GAMG; tolerance 1e06; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } pFinal { solver GAMG; tolerance 1e06; relTol 0; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } "(Ukepsilon)" { solver PBiCG; preconditioner DILU; tolerance 1e05; relTol 0.1; } "(Ukepsilon)Final" { $U; tolerance 1e05; relTol 0; } } I will have a look at that post first. thanks for your help! phillipp you are very kind！ 

May 16, 2013, 09:43 

#8 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
500 time steps is really huge... 50 should be by far enough as far as I know.
No, sorry I don't mean the hight of the cylinder but the "other" dimension of your 2d flow domain. But sorry I just saw that you already wrote "2*20D" in your previous post... What about your grid? Can you post a picture of it? How many cells do you have?
__________________
The skeleton ran out of shampoo in the shower. 

May 16, 2013, 09:49 

#9 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
here is a picture of the domain and mesh.
mesh information: 70900 elements 47488 vertices by the way, do you have a similar mesh file that yields good St number? if you have, could you please send to me so i can test in my own case? 

May 16, 2013, 09:55 

#10 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
No, unfortunately not, and I am currently running computationally expesive simulations, so I can't just give it a try...
Maybe tomorrow. Btw: You mean St=0.16 and not 1.6 in your first post, right?
__________________
The skeleton ran out of shampoo in the shower. 

May 16, 2013, 10:06 

#11 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
yes, that's what i mean. my St number is 1.4, which I think is too low. actually according to the references i found, St should be around 1.65 when Re is 100.
If you have time, please help me with that mesh file, this problem has been haunting me for a week! It's 23pm in japan now and I need to go home. i will let you know if i have any progress. thank you again for you kind help! have a nice evening! 

May 16, 2013, 12:01 
Mesh is available

#12  
Super Moderator

Quote:
http://www.cfdonline.com/Forums/mai...rre40a.html Possible issues are: 1. Mesh 2. Convergence (reduce convergence level to 1e19). Laminar flow should be converged more tightly. 3. Method of determining the strouhal number including the manipulation of transient data 4. Time step size Quote:
Few results from Ansys documentation for similar case: Last edited by Far; May 16, 2013 at 12:15. Reason: adding something more 

May 16, 2013, 13:23 

#13 
Senior Member
cfdnewbie
Join Date: Mar 2010
Posts: 557
Rep Power: 12 
What type of BCs are you applying on the free surfaces? What quantity do you use to measur Str? How do you determine the frequency? By FFT or by eye? Have you validated your code for other cases?


May 17, 2013, 01:48 

#14 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
For Far:
yes, I made a mistake in the previous post. My St is 0.14 while the accurate one should be 0.16. I'm trying lowering the convergence level to 1e12 because lowering to 1e18 really takes a lot of time. I will post the result when it is finished. As for the two pictures you posted, I think in my case, both timestep per cycle(in my case 500 timesteps per cycle) and number of nodes(in my case 47488 vertices) are fine enough. For cfdnewbie: inlet U: fixed value (1 0 0) p: zeroGradient outlet U: zeroGradient p: fixed value 0 cylinderwall U: fixed value (0 0 0) p: zeroGradient sidewall U: slip p: slip frontandback U，p: empty (indicate 2D) I used the data from Cl(lift force coefficients) to calculate the Str. Both Fourier transform and direct observe from the Cl plot diagram yield the same result. since I am using OpenFoam, I suppose the code itself should be correct, the problem is I have to find the appropriate mesh and settings. Actually what I am trying to solve is a validation case, after this I will perform some simulations with higher Re and more sophisticated geometry. 

May 17, 2013, 01:54 

#15 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
You should have a look at the boundary layer at your cylinder and see how many grid points you use to resolve it.
__________________
The skeleton ran out of shampoo in the shower. 

May 17, 2013, 01:58 

#16 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
The result of convergence level 1e12 has come out. St remains 1.44.
It seems the problem does not come from convergence level. the numerical schemes I'm using is like this: Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss limitedLinearV 0.5; div(phi,k) Gauss limitedLinear 0.5; div(phi,epsilon) Gauss limitedLinear 0.5; div(phi,R) Gauss limitedLinear 0.5; div(R) Gauss linear; div(phi,nuTilda) Gauss limitedLinear 0.5; div((nuEff*dev(T(grad(U))))) Gauss cubic; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(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 ; } 

May 17, 2013, 03:40 

#17 
Super Moderator

You can find mesh here : http://www.cfdonline.com/Forums/ansysmeshing/96191meshinggambitanalysisflowpastcylinders.html.
Try it and see whether you get better results or not?


May 17, 2013, 05:59 

#18 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
Philipp: here is a zoom in look of the mesh near the cylinder. I've tried dividing the perimeter of the cylinder into 128 and 200, but with no luck.
Sijal: here is a picuture of the Cl plot. For FFT, I cut the former part of this plot and used the steady one do calculate frequency. for example, in this case I used 160s~240s to do FFT. I also calculated frequency by manually observe the time difference between two peaks in the steady part. I decide timestep by courant number<0.5, and usually timestep is 0.01 or smaller, depending on the smallest grid size and mesh fineness. One disadvangtage of this is that my timestep is not even. When doing FFT, I used EXCEL to first get a timeuniformly distributed data by linear interpolation, then perform FFT in matlab using this data with a constant timestep. besides, the mesh you provided seems problematic when converting to openfoam mesh, anyway I am working to solve this. 

May 17, 2013, 06:14 

#19 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 19 
Sorry, I mean the actual flow field (e.g. velocity), not the mesh.
You should have a look at the spatial sampling of the velocity, perpendicular to the wall. You need to ensure, that the boundary sheath grid spacing is fine enough to capture the relevant effects...
__________________
The skeleton ran out of shampoo in the shower. 

May 17, 2013, 20:30 

#20 
Senior Member
Join Date: Jan 2013
Posts: 121
Rep Power: 6 
dear all
my problem of getting smaller Str number is now solved. It turns out that my mesh is Ok, the problem lies in the underrelaxation factor I employed in this unsteady cases. It is found out when using under relaxation in unsteady cases, the simulation won't be timeaccurate, so in my case Drag and lift coefficients are OK but vortex shedding frequency becomes bad. I removed the relaxation factors in my settings and then the right results came out. anyway, I really appreciate your help in this thread! 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
compressible flow in turbocharger  riesotto  OpenFOAM  50  May 26, 2014 01:47 
ERROR #001100279 has occurred in subroutine ErrAction.  smnaryal  CFX  7  January 3, 2013 19:09 
error in parallel run  immortality  OpenFOAM Running, Solving & CFD  7  January 1, 2013 14:35 
Problem with decomposePar tool  vinz  OpenFOAM PreProcessing  18  January 26, 2011 03:17 
strouhal number for ellipse  ek  Main CFD Forum  2  December 25, 2008 00:15 