I'm modelling a cylinder in cross-flow using 3d double precision unsteady solver with the geometry that can be found in a paper published by Eckert and Soehngen (1952) [cylinder in a channel]. The Reynolds numbers range from 120 to 600, i.e. laminar and energy equations are being solved. This simple test case gives a 14% Nusselt number error at the front stagnation point and 100% error at the rear of the pin, although the general trends appear reasonable - maximum Nusselt number at the stagnation point reducing to a minimum near the point of separation then recovering in the wake. Grid independence has been proven and the solution is converged. Strouhal numbers are correct.

My question is this - there are no viscous turbulence models being used, the grid is fine enough to resolve the boundary layer so why is difference between experiment and CFD so great? Any views would be much appreciated, Thanks, Mat

Well, Are you sure is you are using bousinesq density model, than you have input the right density and the thermal expansion coefficient.

This greatly changes the result. Also for natural convection problems, your BL mesh size should be generally less than 1 mm. Adapt the grid if it isnt.

Regards

Haroon

Haroon,

Thanks for the reply but I'm not sure the Boussinesq density model is appropriate here where Re=600. This is forced convection, the Grashof number is less than 1 (around 0.12). Bouyancy is negligible.

Any other ideas where the difference may come from?

Mat

One more thing, how big is your computational domain. It should be five hydraulic diameters all around the cylinder. In the wake region it should be 8 hydraulic diameters. Please check this.

Please check if you have scaled the Grid accurately in Fluent. Very important!

Use QUICK scheme. It works well with low Re flows particularly when the quad grid is used.

I had a fluctuating wake when I solved a cylinder problem. This was due to vortex shedding. Try modelling only half the cylinder using symmetry. This solved my problem.

Hope this helps

Thank-you for your sensible suggestions. The cylinder diameter under examination is 12.7mm with a cylinder length of 228mm. The channel is 1000mm long so it meets the entrance/exit length criteria you state.

The grid has been scaled correctly.

The QUICK scheme has been used on the momentum and energy discretisation.

As for the fluctuating wake- this is the only way to physically model this problem correctly so I would prefer not to impose a symmetry condition on the centreline. I'm quite sure that the model is correct but I hoped that someone might be able to suggest reasons for the differences between experiment and CFD other than the usual (iterative convergence error, discretisation error, roundoff).

For example, the flow looks like it is separating too early from the cylinder in the CFD- why might this be? The laminar equations should predict separation from a cylinder accurately shouldn't they?

Any answers would be welcome.

Dont take this as an answer, these are just guesses.

May be the reason of early separation is no slip condition in your CFD model where as in the reported data there might be some slip.

I have solved convection problems but I have always achieved strikingly close results. One case in particular was the flow over flat plate but had high Re number.

If there is a fluctuating wake than try modelling the problem as un-steady. You will see quicker convergence and try to plot the variation of Nu with time. You would probably have a sinosodial curve. Integrating that would give you the final Nu.

Thats all I can think of.

regards

Haroon

Thanks Haroon,

The model is unsteady and the circumferential Nu distribution around the cylinder is time averaged.

I will have a think about the no-slip condition you mentioned, but the scale of the experiment should mean these effects are negligible.

Thanks again, Mat

I am just starting to use FLUENT. can any one help to start generating the geometery for a heat transfer from a cylinder in cross flow in a pipe.

Thank you

Regarding the leading edge stagnation region, you might check the cylinder midspan surface static pressure as a function of circumferential arc length. The satic pressure profile should be parabolic in the stagnation region. Hiemenz flow (see Schlichting) is an exact analytical solution for flow impinging on a plate, and based on your pressure field you can determine the displacement thickness of the stagnation boundary layer, which is constant in Hiemenz flow. In order to resolve the heat transfer in that region, you should have five or so grid cells within that displacement thickness. If you have one or fewer, that may be the problem. For more details, check a paper from IGTI in Montreal 2007, GT2007-28120.