I am doing simulation of heat transfer of a circular cylinder in crossflow by using Fluent6.1. It is a typical problem. we can get a lot experimental data to check the results.

It seems that in the laminar part before the seperation point the local Nusselt number(time averaged) is predicted well. However after the seperation point(In the wake region) the local nusselt number is a little bit far away from experimental results.

Does anybody has good experience with this kind of simulation and has got very nice result?

Thanks

Is this laminar/turbulent, 2D/3D, i.e. what is the Reynolds number?

If this is an unsteady case (Re>=47):

How well do you predict the unsteady flow, besides heat transfer? Do you get good results on vortex shedding frequency, amplitudes of lift and drag oscillations, mean position and amplitude of oscillation of the separation point... ?

How many cells do you have along the cylinder surface?

What have you tried so far to improve your result? Grid convergence? Temporal resolution?

Thanks Mani,

I am doing 2-D simulation. The Reynolds number is around 5300. The fulid is air.

The Strouhal number at Re = 5300 is around 0.2. My simulation predicted vortex shedding frequency not bad. The deviation is around 10%. The oscillation of drag coefficient is between 1.6 and 1.3. The oscillation of lift coefficient is between 1.2 and -1.2. I don't know how to get the seperation point directly from fluent. By analysing the local nusselt number, the lowest point should be seperation point. so the mean point should be near 90 degree from stagnation point in my result.

The diameter of the circular cylinder is 0.02m. There are 124 nodes along the surface of the cylinder.

I tried to simulate this problem by using different grid density. The solution is almost mesh independent which means when i increased the grid number the average nusselt number keep as a constant.

There is the effect of fluid properties on heat transfer between fluid and the cylinder. In order to eliminate the effect from the fluid properties, the constant properties value at film temperature are configured in the CFD calculation. Actually I tried to simulate with material properties at bulk temperature also. there is almost no changes in average nusselt number and local nusselt number.

This is almost how far I am in this calculation. Any suggestions and ideas will be highly appriciated.

I don't have much experience with heat transfer in this case, but I can give some comments on the flow.

At such a high Reynolds number you are pretty far into the region of turbulent flow. Not upstream, but downstream of the separation point, in the wake, the flow should be turbulent. I am assuming that you are using some turbulence model, since your resolution is by far not high enough for direct numerical simulation. I am not sure what the effect of your turbulence model is on heat transfer, but I would certainly consider turbulence a very important part of your simulation. To get turbulence right is probably essential for getting the heat transfer right.

Furthermore, at that Reynolds number the flow is definitely not two-dimensional. Three-dimensional features start showing at Reynolds numbers above about 180. Again, I can't say for sure that your assumption of 2D flow is not good enough for heat transfer, but I am suspecting it might not be. I would be surprised if you even get the correct vortex shedding mode. A 10 percent inaccuracy in the frequency might hint towards problems in simulating vortex shedding. I would suggest that you read up on the basic behavior of this kind of flow. There are some good papers on experiments over a large range of Re, discussing vortex shedding modes and frequencies, turbulence, and 2D/3D issues. This would help you to see what's wrong with your simulation. For example:

Fey et al., Physics of Fluids, Vol. 10, No. 7, pp. 1547, 1998

About grid resolution, I know of a study by Alonso and Jameson in the mid 90s. They claim that for accurate prediction of the Strouhal number, they needed in the order of 350-400 cells around the cylinder cross-section. This study was done for laminar flow at low Reynolds number! It certainly will depend on the scheme you are using. Since you say your solution is grid converged, I am thinking that you are missing some essential physics, here. This might be related to turbulence or 3D flow, as mentioned above.

Also, you need to make sure that the temporal resolution is adequate. How many time-steps you need to use per period of the oscillation will again depend on the scheme. You may want to also perform a time resolution study on your finest grid.

At the same time you should double-check if there's not something wrong in the way you calculate the Nusselt number. Maybe it's just a mistake in your post-processing. Have you successfully performed simpler studies, e.g. for a flat plate?

Good luck!

Thanks a lot, Mani,

Your ideas help me a lot. I am trying to make more nodes on around the cylinder. Another reason for doing this is that the Drag Coefficient is also not good. The result of Cd is around 1.6(Time averaged). However, as we know at Re = 5000, the drag coefficient should be about 1.2.

Now I have to no time to try 3-D simulation because I have to submit the report. I will do it later. For me It's quite interesting.

Thanks again.

For an interesting look at optimised meshes, take a look at <www.featflow.de>, where they benchmark various schemes for the cylinder example...

This could help you to concentrate your mesh refinement where you can maximise the return...

diaw...

[shreyas9043]

I am currently producing a paper relating to heat transfer due to dynamics of circular cylinder at Re5000 particularly at 350k and 400k. Although I have done the simulations in 3D and steady state. I can confirm that there is negligible influence of temperature on the wake of the cylinder. The data obtained shows that the heat transfer also has a negligible effect on the drag. I hope this helps!