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

Uniform Flow around a cylinder

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 6, 2009, 15:52
Default Dear all, I simulate the th
  #1
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 6, 2009, 18:22
Default Dear all, I know that I get
  #2
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 6, 2009, 18:25
Default Dear all, I know that I get
  #3
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 7, 2009, 02:53
Default You are scaling the cylinder,
  #4
New Member
 
Jon Tegner
Join Date: Mar 2009
Posts: 7
Rep Power: 8
jont is on a distinguished road
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
jont is offline   Reply With Quote

Old   March 7, 2009, 03:53
Default Dear Zhoubin im really in
  #5
Member
 
Nugroho Adi
Join Date: Mar 2009
Location: norway
Posts: 79
Rep Power: 8
mahaputra is on a distinguished road
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
mahaputra is offline   Reply With Quote

Old   March 7, 2009, 08:34
Default Hi Jon, Thank you for your
  #6
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 8, 2009, 04:08
Default Hi Jon, You are right, I ha
  #7
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 8, 2009, 08:55
Default Hi,zhoubin You mean you sol
  #8
lin
Senior Member
 
Hua Zen
Join Date: Mar 2009
Posts: 114
Rep Power: 8
lin is on a distinguished road
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.
lin is offline   Reply With Quote

Old   March 9, 2009, 15:44
Default Hi Hua Zen, Thank you for y
  #9
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 12, 2009, 18:01
Default I have proved that when Re: 0.
  #10
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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....
zhoubinwx is offline   Reply With Quote

Old   March 12, 2009, 19:12
Default Hi,Bin Nice to see your res
  #11
lin
Senior Member
 
Hua Zen
Join Date: Mar 2009
Posts: 114
Rep Power: 8
lin is on a distinguished road
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.
lin is offline   Reply With Quote

Old   March 13, 2009, 02:15
Default Hi Bin Just a thought: A
  #12
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,619
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
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.
ngj is offline   Reply With Quote

Old   March 13, 2009, 02:17
Default Hi,Hua Zen, First of all, t
  #13
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 13, 2009, 02:31
Default Hi Niels, Feel excited to s
  #14
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 13, 2009, 03:36
Default Dear readers: My conclusion
  #15
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 13, 2009, 04:53
Default Dear OpenFOAM friends: As w
  #16
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 13, 2009, 05:20
Default Dear zhoubin, there is a pape
  #17
New Member
 
David Sponiar
Join Date: Mar 2009
Location: Prague, Czech rep.
Posts: 27
Rep Power: 8
sponiar is on a distinguished road
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
_____
sponiar is offline   Reply With Quote

Old   March 13, 2009, 05:29
Default Hi David, Thank you for sha
  #18
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx is offline   Reply With Quote

Old   March 13, 2009, 06:14
Default Hi,bin Since you do not men
  #19
lin
Senior Member
 
Hua Zen
Join Date: Mar 2009
Posts: 114
Rep Power: 8
lin is on a distinguished road
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.
lin is offline   Reply With Quote

Old   March 13, 2009, 06:31
Default Hi,Hua Zen, Thank you very
  #20
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
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
zhoubinwx 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
Air flow over a cylinder momentum_waves Main CFD Forum 1 November 17, 2008 21:54
Flow over a flat plate & Flow over a cylinder cfdxue Main CFD Forum 0 November 27, 2007 00:26
propeller in non-uniform flow ubik Main CFD Forum 0 February 20, 2007 07:28
Is an uniform flow possible for this geometry? Michael Hu FLUENT 1 April 13, 2006 22:11
Cylinder In Jet Flow patrick raj CFX 2 September 24, 2005 02:43


All times are GMT -4. The time now is 11:15.