Dear all, I simulate the th
 

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

Dear all, I know that I get
 

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

Dear all, I know that I get
 

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

You are scaling the cylinder,
 

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

Dear Zhoubin im really in
 

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 http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Hi Jon, Thank you for your
 

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

Hi Jon, You are right, I ha
 

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

Hi,zhoubin You mean you sol
 

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.

Hi Hua Zen, Thank you for y
 

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

I have proved that when Re: 0.
 

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....

Hi,Bin Nice to see your res
 

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.

Hi Bin Just a thought: A
 

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

Hi,Hua Zen, First of all, t
 

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

Hi Niels, Feel excited to s
 

Hi Niels,

Feel excited to see your reply to me http://www.cfd-online.com/OpenFOAM_D...part/happy.gif 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

Dear readers: My conclusion
 

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

Dear OpenFOAM friends: As w
 

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

Dear zhoubin, there is a pape
 

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
_____

Hi David, Thank you for sha
 

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

Hi,bin Since you do not men
 

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.

Hi,Hua Zen, Thank you very
 

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

Hi Bin! Try to use central
 

Hi Bin!

Try to use central differencing (linear) scheme instead of upwind on the convection. I think its more appropriate for your low Reynolds problem.

Regards,
Jose Santos

Hi Santos, Let me try CD sc
 

Hi Santos,

Let me try CD scheme, and report here later.

Thank you.

Bin

Hi,Bin From the first glanc
 

Hi,Bin

From the first glance of your files,I think you are "lazy",you should just copy it from some other place and never change it,just I do. After my searching the forum,I plan my next step is to change something in the two files.One suggestion is as Jose Luis Santos refer,using higher order scheme than upwind.Also if your velocity is small,you should change the tolerance of U,no guarantee to improve the result,but worth to try.


For the third dimension size,I do not see any obvious improvement too,but I read this suggestion in the forum from the developer.Notice that what I mean is not that the third dimension size should be comparable to the size of the cylinder,but the size of the first grid around the cylinder.

If I were you,I will not take the analytical results so serious,because the analytical result is indeed for a different case than what you are trying to simulate,except the Re number.It's not easy to evaluate how the assumptions in the analytical derivation affect Cd.

Hi Bin I would extract some
 

Hi Bin

I would extract some lines along the radial axes and compare these results with the analytical results. Then you will get a feel of the deviation between the simulated and analytical boundary layer.

Especially, you could see if you boundary layer does not resolve the velocity gradient sufficiently good.

Best regards,

Niels

Hi Hua Zen and Niels, Thank
 

Hi Hua Zen and Niels,

Thank you for your suggestions.

As for "using higher order scheme than upwind"and "change the tolerance of U", I have made the following modification in fvSchemes and fvSolution files respectively:
div(phi,U) Gauss linear;
and
p PCG
{
preconditioner DIC;
tolerance 1e-12;
relTol 0.01;
};
U PBiCG
{
preconditioner DILU;
tolerance 1e-12;
relTol 0.1;
};
However, I can not get converged results, pls see the log:
Time = 69997

DILUPBiCG: Solving for Ux, Initial residual = 4.85479001865e-05, Final residual = 1.67447473264e-06, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 5.06896545828e-05, Final residual = 4.71628738443e-06, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.00694162440303, Final residual = 6.92499552004e-05, No Iterations 131
DICPCG: Solving for p, Initial residual = 6.90923506458e-05, Final residual = 5.84082992343e-07, No Iterations 51
DICPCG: Solving for p, Initial residual = 6.61152959367e-07, Final residual = 5.78213683191e-09, No Iterations 139
DICPCG: Solving for p, Initial residual = 2.11009841793e-08, Final residual = 2.04101076342e-10, No Iterations 143
time step continuity errors : sum local = 1.01832061429e-21, global = -1.56519101488e-22, cumulative = 1.18498523108e-20
ExecutionTime = 793.5 s ClockTime = 794 s

Time = 69998

DILUPBiCG: Solving for Ux, Initial residual = 2.48311765638e-05, Final residual = 6.84772803551e-07, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 5.02053441742e-05, Final residual = 2.87853528472e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.0157303895822, Final residual = 0.00014742581282, No Iterations 80
DICPCG: Solving for p, Initial residual = 0.000143716280743, Final residual = 1.35346045767e-06, No Iterations 100
DICPCG: Solving for p, Initial residual = 1.35375298735e-06, Final residual = 1.32050674117e-08, No Iterations 147
DICPCG: Solving for p, Initial residual = 1.6946616575e-08, Final residual = 1.56915506155e-10, No Iterations 155
time step continuity errors : sum local = 5.00552481925e-22, global = -9.11982162461e-23, cumulative = 1.17586540945e-20
ExecutionTime = 793.58 s ClockTime = 794 s

Time = 69999

DILUPBiCG: Solving for Ux, Initial residual = 2.38077651352e-05, Final residual = 1.4072658573e-06, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 3.28876452124e-05, Final residual = 4.36425209665e-07, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.00641424933856, Final residual = 5.78238685853e-05, No Iterations 131
DICPCG: Solving for p, Initial residual = 4.82496305812e-05, Final residual = 4.33324957724e-07, No Iterations 43
DICPCG: Solving for p, Initial residual = 5.04520570041e-07, Final residual = 4.57111751424e-09, No Iterations 141
DICPCG: Solving for p, Initial residual = 1.18765927155e-08, Final residual = 1.08764621832e-10, No Iterations 100
time step continuity errors : sum local = 4.75227261696e-22, global = 2.496705833e-23, cumulative = 1.17836211529e-20
ExecutionTime = 793.66 s ClockTime = 794 s

Time = 70000

DILUPBiCG: Solving for Ux, Initial residual = 1.19519643247e-05, Final residual = 4.75905856089e-07, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 3.35627045824e-05, Final residual = 2.95541142512e-06, No Iterations 2
DICPCG: Solving for p, Initial residual = 0.00999944944465, Final residual = 9.12617320076e-05, No Iterations 84
DICPCG: Solving for p, Initial residual = 9.23706787691e-05, Final residual = 8.07128052817e-07, No Iterations 103
DICPCG: Solving for p, Initial residual = 8.16857388457e-07, Final residual = 8.09196470779e-09, No Iterations 136
DICPCG: Solving for p, Initial residual = 1.61059066966e-08, Final residual = 1.36627605826e-10, No Iterations 140
time step continuity errors : sum local = 8.72091539644e-22, global = -8.17798665568e-23, cumulative = 1.17018412863e-20
ExecutionTime = 793.76 s ClockTime = 794 s

I do not know why the simulation cannot converge.

Bin

For the tolerance Take this o
 

For the tolerance
Take this one for example:
tolerance 1e-12;
relTol 0.01;

You change only the "tolerance" ,not "relTol".If you check the user guide,you will know this the solver will stop if one of the two is satisfied. It seems in your log that the first one is never used.

As for the scheme,if you still could not get converged result,I have seen somewhere in the forum that one would better first start some other scheme,and then second order.So you could try the simulation from the result of upwind result as a start.


And in fact I have been considering your case.I do not know for your Re,whether some other physical process will be important.Since for your low Re and Re around 1-100,both flows are laminar.If the model could get good
result for 1-100,then the model should be verified already.(Assume that the round-off error not affect the result)

I guess that the difference between your result and analytical result is because the assumption used in the analytical expression.

Hi Hua Zen, Really apprecia
 

Hi Hua Zen,

Really appreciate that you follow my post and give me some good suggestions.

I will try to play around the "tolerance", "relTol" and "other scheme", in order to get converged results. I find my mesh is too coarse,at far away from the cylinder.

Please follow David's suggestions, to read that paper:
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.
If you could not get it, please let me know.

From now on, I will go back to my micrometer size problem, in order to add my slip boundary code. Welcome to pay attention to my next following post.

Best regards,

Bin

Dear all, Can I ask one que
 

Dear all,

Can I ask one question about simpleFoam solver:

when I set in the file constant/RASProperties:
RASModel laminar
turbulence off;

what will be fvc::div(nuEff()*dev(fvc::grad(U)().T()) in laminar.C file? Is it 0? Why?

Thank you for your attention.

Bin

Hello, I know that fvc::div
 

Hello,

I know that fvc::div(nuEff()*dev(fvc::grad(U)().T()) =1/3*nuEff()*grad(div(U)), when it is incompressible flow, it equals to 0.

Now my problem about why it does not converge goes to:
1. mesh quality;
2. div(phi,U), grad(p) and laplacian(nuEff,U) schemes for momentum equation.
3.laplacian((1|A(U)),p), grad(p) schemes for pressure correction equation.

Let me play with different schemes now.

Thank you for your attention.

Bin

Dear Foamers,

This is a very nice platform. OpenFOAM becomes so nice. Thank you, organizers.

As for my uniform flow around a cylinder, the cylinder radius is 1 micrometer, while upstream, downstream and top distance is 1000 micrometer now.

I have tried to use central central difference scheme for the convective term instead of upwind, it works fine when the computational domain is small, however, it does not work for large computational domain like 1000micrometer or more.


Therefore, I learn from some existing posts, use the following schemes for my low Re flow(Re<1):
divSchemes
{
default none;
div(phi,U) Gauss QUICKV cellLimited leastSquares 1.0;
div(phi,k) Gauss QUICK cellLimited leastSquares 1.0;
div(phi,epsilon) Gauss QUICK cellLimited leastSquares 1.0;
div(phi,R) Gauss linear;
div(R) Gauss linear;
div(phi,nuTilda) Gauss QUICK cellLimited leastSquares 1.0;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

What I get:
DILUPBiCG: Solving for Ux, Initial residual = 1.03553200448e-05, Final residual = 2.78983276507e-08, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1.72354405369e-05, Final residual = 1.18743299709e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000573905389101, Final residual = 5.57363086449e-06, No Iterations 120
DICPCG: Solving for p, Initial residual = 5.54622914e-06, Final residual = 5.3858588214e-08, No Iterations 41
DICPCG: Solving for p, Initial residual = 7.90462819447e-08, Final residual = 7.8670023242e-10, No Iterations 75
DICPCG: Solving for p, Initial residual = 1.29586868496e-08, Final residual = 1.1139023921e-10, No Iterations 121
time step continuity errors : sum local = 2.72055609614e-09, global = 4.27382015215e-11, cumulative = 1.32480768615e-06
ExecutionTime = 863.19 s ClockTime = 865 s

Time = 12103

DILUPBiCG: Solving for Ux, Initial residual = 1.01795685162e-05, Final residual = 1.72202544505e-08, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1.62845011413e-05, Final residual = 9.25681206317e-08, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000638536334373, Final residual = 5.94425402805e-06, No Iterations 71
DICPCG: Solving for p, Initial residual = 5.99149129924e-06, Final residual = 5.72198099944e-08, No Iterations 120
DICPCG: Solving for p, Initial residual = 7.1040362187e-08, Final residual = 7.08878632619e-10, No Iterations 130
DICPCG: Solving for p, Initial residual = 1.20902645837e-08, Final residual = 1.11660344159e-10, No Iterations 120
time step continuity errors : sum local = 2.62896976359e-09, global = 6.26439641475e-11, cumulative = 1.32487033011e-06
ExecutionTime = 863.27 s ClockTime = 865 s

Time = 12104

DILUPBiCG: Solving for Ux, Initial residual = 1.01807516553e-05, Final residual = 3.37481036812e-08, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1.60627753132e-05, Final residual = 1.15491299036e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000459795854851, Final residual = 4.52798245098e-06, No Iterations 115
DICPCG: Solving for p, Initial residual = 4.53882529717e-06, Final residual = 4.08024951933e-08, No Iterations 47
DICPCG: Solving for p, Initial residual = 5.52843066809e-08, Final residual = 5.38876565464e-10, No Iterations 120
DICPCG: Solving for p, Initial residual = 1.13196894953e-08, Final residual = 1.08566361529e-10, No Iterations 118
time step continuity errors : sum local = 2.41694994532e-09, global = -2.34079605543e-10, cumulative = 1.32463625051e-06
ExecutionTime = 863.34 s ClockTime = 865 s

Time = 12105

DILUPBiCG: Solving for Ux, Initial residual = 1.02192542903e-05, Final residual = 4.30670523412e-09, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 1.62224420005e-05, Final residual = 1.1355526897e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.00062791611302, Final residual = 5.75405936012e-06, No Iterations 118
DICPCG: Solving for p, Initial residual = 5.78040635386e-06, Final residual = 5.73131777609e-08, No Iterations 46
DICPCG: Solving for p, Initial residual = 7.83562369839e-08, Final residual = 7.8192729193e-10, No Iterations 121
DICPCG: Solving for p, Initial residual = 1.25884982906e-08, Final residual = 1.17843703303e-10, No Iterations 126
time step continuity errors : sum local = 2.47922039251e-09, global = -3.53202238733e-10, cumulative = 1.32428304827e-06
ExecutionTime = 863.41 s ClockTime = 865 s

Time = 12106

DILUPBiCG: Solving for Ux, Initial residual = 1.02939664929e-05, Final residual = 4.28857709447e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 1.62688567487e-05, Final residual = 1.36293849551e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000538634222647, Final residual = 5.34445751033e-06, No Iterations 61
DICPCG: Solving for p, Initial residual = 5.38257563201e-06, Final residual = 5.36484980642e-08, No Iterations 122
DICPCG: Solving for p, Initial residual = 8.34912517693e-08, Final residual = 8.2879980719e-10, No Iterations 70
DICPCG: Solving for p, Initial residual = 1.30555418797e-08, Final residual = 1.28991063003e-10, No Iterations 117
time step continuity errors : sum local = 2.37604132027e-09, global = 2.74819423606e-10, cumulative = 1.32455786769e-06
ExecutionTime = 863.48 s ClockTime = 865 s

Time = 12107

DILUPBiCG: Solving for Ux, Initial residual = 1.03387025777e-05, Final residual = 2.75179481283e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 1.66393167178e-05, Final residual = 1.3199226195e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000526005312335, Final residual = 5.24477342292e-06, No Iterations 125
DICPCG: Solving for p, Initial residual = 5.62805031808e-06, Final residual = 5.0483500148e-08, No Iterations 44
DICPCG: Solving for p, Initial residual = 6.41034682407e-08, Final residual = 6.3426681675e-10, No Iterations 119
DICPCG: Solving for p, Initial residual = 1.11918294544e-08, Final residual = 1.08216553477e-10, No Iterations 127
time step continuity errors : sum local = 2.29118741072e-09, global = 4.98494068734e-10, cumulative = 1.32505636176e-06
ExecutionTime = 863.55 s ClockTime = 865 s

Time = 12108

DILUPBiCG: Solving for Ux, Initial residual = 1.02048007513e-05, Final residual = 2.61609759552e-08, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1.66144139216e-05, Final residual = 9.40048099447e-08, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000504044545101, Final residual = 4.16061686449e-06, No Iterations 126
DICPCG: Solving for p, Initial residual = 4.27252809065e-06, Final residual = 4.17187473555e-08, No Iterations 46
DICPCG: Solving for p, Initial residual = 6.56098091566e-08, Final residual = 6.27565825808e-10, No Iterations 120
DICPCG: Solving for p, Initial residual = 1.35910212776e-08, Final residual = 1.25093758127e-10, No Iterations 122
time step continuity errors : sum local = 2.44065654584e-09, global = 5.19977423449e-10, cumulative = 1.32557633919e-06
ExecutionTime = 863.62 s ClockTime = 865 s

Time = 12109

DILUPBiCG: Solving for Ux, Initial residual = 1.0260817769e-05, Final residual = 2.37941701208e-08, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1.67815495455e-05, Final residual = 1.18564614583e-07, No Iterations 3
DICPCG: Solving for p, Initial residual = 0.000596011848656, Final residual = 5.05137334017e-06, No Iterations 120
DICPCG: Solving for p, Initial residual = 5.028472864e-06, Final residual = 4.52981055293e-08, No Iterations 47
DICPCG: Solving for p, Initial residual = 6.27294616621e-08, Final residual = 5.98383839521e-10, No Iterations 122
DICPCG: Solving for p, Initial residual = 1.17453754585e-08, Final residual = 1.16917997412e-10, No Iterations 111
time step continuity errors : sum local = 2.49175931067e-09, global = 2.4882672876e-11, cumulative = 1.32560122186e-06
ExecutionTime = 863.7 s ClockTime = 865 s

As we could see from the above log file, the residual of p fluctuates, but no converge.

If anyone has some suggestions, welcome.

Best regards,

Bin

More important than the residuals, perhaps, is what your solution looks like. Have you tried monitoring the values for your solution at different points? How does the solution change?

Hi McGlashan,

Thank you for your suggestions. As you said, we should rely on the stability of the parameters (u, or p) at some sampling positions. Also when we increase the deltaT, we can find bigger residual. However, my problem now is:when my computational domain becomes larger and larger, the residual is the order of 10^(-2) and the residual for p just fluctuates.

I can not report my simulated results to my professor with such bad residuals. therefore I need to try suitable discretisation schemes (the mesh is ok through checkMesh utility). BTW, welcome for further advice.

I will post my residual plot, as well as U velocity at some sampling position, if I can not find a suitable way out after several days.

Thank you again, McGlashan.

Bin

Dear all,

Today Mr. Santos pointed out that there maybe something wrong in my mesh, and he is right. Thank you.

Why I made such a mistake using blockMesh?

I follow the equation of U-38, under "2.1.6.2 Changing time and time step", so that I get the expression of the minimum size of the cell.

Here I would like to share with you, after I check very carefully, when R>1, this expression is not correct.


The correct one for R>1 should be: delta_xs=L*(R^(1/(n-1))-1)/(R^(n/(n-1))-1)
Just for your information.


Hi, Santos, thank you again;).
Bin

Dear Foamers,

Would you mind if I attach my test case here, because I still have a problem about convergence.

Best regards,

Bin

One question to myself: is symmetry boundary condition on the top of the computational domain is right? Is it because of this boundary condition that my simulation does not converge?(But if I remember well, when the upstream, downstream and top distances are small, I could get converged results, when they become large and I add more grids correspondingly, no converge...)


:confused:

If I were you.

1. More grid around the cylinder
2. change the residual to smaller value

what is the distance from you first grid to the cylinder?

Hi Lin,

Thank you for your advice.

I am generating and checking again the mesh quality very carefully with blockMesh. Your suggestion of "More grid around the cylinder" is reasonable. although I have already 40 cells on the half cylinder(radius=1micrometer);
As for "change the residual to smaller value", I have set very lower residuals for both p and U. They are of the order 10^12.

Your question: what is the distance from you first grid to the cylinder?
Ans: the distance of my "first grid"(if you mean inlet) to the cylinder is 2000 micrometer; if you mention "first grid" as the grid near the cylinder, then the distance equals to the cell length on the cylinder surface.

I will try my best to eliminate the mesh quality problem....

Thank you agian, Lin.

Bin

I'm quite interested in this, I had similar problems to you but never really had time to sort it out:
See this thread

My drag coefficient would keep increasing. I only get this behaviour for flow around a cylinder. When I did it for a square cylinder I had no such problems.

Hi, Mr. McGlashan,

I have read your post in the above post. I'm lucky we are on the same boat :)

Recently I have tried to use grading mesh around the the cylinder, after I take a look at these mesh, I could see they aspect ratio is quite good near cylinder. Would you please try to calculate the minimum and maximum size of the mesh between your cylinder and out fictious "cylinder"? So that we know R=max/min, and since we know the distance between these two cylinders, we can get how many cells we need from the equation in UserGuide.pdf case.

I can get better converged result, the only problem I have now is as long as time goes on, Cd decreases.

Good luck.

Bin


P.S. you could also send me your test case, so that we may try together.

Hi there!

Allow me to enter your boat, now I am studying creeping flow around a sphere, Reynolds = 0.1. I will be glad to keep up with your progress, and I will keep you up to date with mine as well.

I have run 2 preliminary simulations, the first having the sphere radius 1/10 of the channel height, and the second 1/20. The computed Cd deviates 12% and 8% respectively from Stokes law (24/Re).

Regards,
Jose Santos