I have been trying to simulate the external flow over a cylinder (both laminar and turbulent), but so far I've been unsuccessful. The simulation I'm running involves heat transfer through the cylinder wall. I used the local Nusselt data found in most text books to validate the results; and the values I calculated from the CFX solution are way off.

I've noticed a couple of odd things:

- I set the boundary condition at the cylinder wall to a fixed temperature in CFX-Pre, and after obtaining a solution, I laid a polyline on this wall in CFX-Post, so as to plot the variables. I plotted the temperature and it doesn't remain constant as it should. This can only mean one of two things; either the polyline is not right on the cylinder wall (which it should 'cause I used the boundary intersection method) or the solver is changing this value. - The Reynolds number calculated by the program is not consistent with the geometry and free stream velocity used (actually, it never is, no matter what the simulation).

I don't think it is a mesh problem, the one I generated is pretty refined. If someone has already run this simulation successfully, I'd appreciate some guidelines. I could also send you all the simulation files if you are interested in seeing the results I got. Maybe someone knows of an internet address where I could download a CFX tutorial on this type of flow or something like that. Anyway, I'd really appreciate any help you could give me. Thanks.

Hi,

If you change the variable mode to Hybrid, the Temperature at the cylinder wall shown by CFX-Post will be the same you have precribed in CFX-Pre.If, in Conservative mode the Temperature at the cylinder wall is very different from the one you have prescrbed, this probably means that your mesh near the wall is not fine enough to capture the temperature gradient.

The only CFX tutorials I know are available on the CFX-Community web site.

Regards,

Rui

The conservative temperature is actually the temperature in the near wall control volume. Since the node of this control volume actually lies on the wall, it can be a littel deceptive. Setting the value to hybrid gives you the boundary condition value.

If heat transfer is involved, there will always be a difference between the conservative and hybrid values and this does not necessarily imply that the grid is not fine enough.

Regards, Robin

Yes,

It is the issue with the mesh near the wall. You can find out by looking at the y+ values in Post on the wall.

Regards, test

Hi,

How are you calculating your Nusselt number?:

If you're using the Heat Transfer Coefficient from the solver then be careful about the reference temperature. The solver uses the temperature taken between the 1st and 2nd nodes from the boundary. This is unlikely to be the same reference as one found in a textbook (they will usually use some bulk flow temperature).

Ideally you should calculate the adiabatic surface temperature using the bulk flow temperature and local fluid velocity, then use this as a reference.

It is possible to force the solver to use a different reference temperature by setting the expert parameter "tbulk_for_htc".

Regards

Paul

You should also keep in mind that a heated cylinder will not have a constant surface temperature in this situation, so I wouldn't expect to get exactly the same solution.

-Robin