I have modelled a tube with helically ribbed surface. The Nusselt number at the wall needs to be calculated. The fluid flowing inside is water at Re = 5000, at 328K. The wall is a copper alloy CuZn28 maintained under constant temperature boundary conditions at 283K, with a thickness of 0.7mm. The number of cells are around 120000 with finer cells near the boundary. My problem is that despite the low temperature difference and the fact that all other parameters such as velocity and temperature lying within range, I am obtaining a Nusselt number of the order of 35000. When it should actually lie in the range of few tens. Also by increasing the number of cells to 300000 a significant change in the Nusselt number is not observed. All comments are welcome

Look at the definition of the Nusselt number. By default Fluent uses:

Nu=(q")*(1m)/k/(T-288.15K)

Anywhere along your boundary where the temperature nears 288.15K will give an infinite Nusselt number. This occurs since the wall is at 283K and gas inlet at 328K, thus somewhere the gas is probably near 288.15K. In simple terms, for your problem, the default Nusselt number is a meaningless piece of junk which has lost any usefulness. (Sorry if that was harsh, but all dimensionless numbers have cases where they fail and you must redefine them).

Of course you can always use the heat flux (q") and never have any problems. If you really want a Nusselt number, redefine the reference temperature to something outside your operating temperature (over 328K or under 283K).

Hi Scott Thanks for the answer. I have few more questions. I couldnt find the Nusselt number formula in fluent. The heat flux with above temperature range is also crazy of the order of MW/m2. Does it also depend on a wierd formula?

Chinmay, sorry for taking so long to respond.

I find the formulas in "Fluent 5, Users Guide Volume 4" section 22.4. If you don't have access to the books: open Fluent, click on help, and search for 'field variables'. Both places have a list of every definition that Fluent uses - often including the formulas.

Seems like you have a problem in the heat flux (in addition to the Nusselt number difficulty that you should have as the temperature nears 288K). The formula for heat flux, "Fluent 5, Users Guide Volume 1" section 6.13 gives:

q"=kf*(dT/dn)=kf*(Tw-T)/(dn)

where: kf is the fluid thermal conductivity, dn is the distance from the wall to the center of the first cell, Tw is the wall temperature, and T is the fluid temperature.

If the heat flux is too large, then the problem must be in the fluid conductivity or the temperature gradient at the wall. I'd first check the conductivity (did you use the correct values). Next I'd check the temperature gradient at the wall. Since your temperature differences (between inlet and wall) is small and since you claimed to have a fine mesh at the wall, I wouldn't expect an error to occur with the temperature gradient. That is, unless your soluition was not fully converged. It may be possible that some cells near the wall had diverged in temperature (check if they reach 0K or 5000K, depending on what temperature limits you specified). If neither of those are the problem, I probably cannot help you.

Good luck.

Hi Scott. Thanks for you patience first of all. There is also an important feature which needs attention. The Nusselt number depends on the charecteristic length l_ref. This needs to be inputted under the panel report-reference values which stays by default 1m. Upon changing this value to the charecteristic of my model, the Nusselt number dropped to 1000. This is a great relief. Now I am accurately trying to draw the grid to satisfy the y+ condition.